User’s Manual CAUTION: This documentation is intended for qualified users who will exercise sound engineering judgment and expertise in the use of the Abaqus Software. The Abaqus Software is inherently complex, and the examples and procedures in this documentation are not intended to be exhaustive or to apply to any particular situation. Users are cautioned to satisfy themselves as to the accuracy and results of their analyses. Dassault Systèmes and its subsidiaries, including Dassault Systèmes Simulia Corp., shall not be responsible for the accuracy or usefulness of any analysis performed using the Abaqus Software or the procedures, examples, or explanations in this documentation. Dassault Systèmes and its subsidiaries shall not be responsible for the consequences of any errors or omissions that may appear in this documentation. The Abaqus Software is available only under license from Dassault Systèmes or its subsidiary and may be used or reproduced only in accordance with the terms of such license. This documentation is subject to the terms and conditions of either the software license agreement signed by the parties, or, absent such an agreement, the then current software license agreement to which the documentation relates. This documentation and the software described in this documentation are subject to change without prior notice. No part of this documentation may be reproduced or distributed in any form without prior written permission of Dassault Systèmes or its subsidiary. The Abaqus Software is a product of Dassault Systèmes Simulia Corp., Providence, RI, USA. © Dassault Systèmes, 2012 Abaqus, the 3DS logo, SIMULIA, CATIA, and Unified FEA are trademarks or registered trademarks of Dassault Systèmes or its subsidiaries in the United States and/or other countries. Other company, product, and service names may be trademarks or service marks of their respective owners. For additional information concerning SIMULIA European Headquarters Fax: +1 401 276 4408, simulia.support@3ds.com, http://www.simulia.com Stationsplein 8-K, 6221 BT Maastricht, The Netherlands, Tel: +31 43 7999 084, Fax: +31 43 7999 306, simulia.europe.info@3ds.com Locations United States Australia Austria Benelux Canada China Finland France Germany India Italy Japan Korea Latin America Scandinavia United Kingdom Argentina Brazil Czech & Slovak Republics Greece Israel Malaysia Mexico New Zealand Poland Russia, Belarus & Ukraine Singapore South Africa Spain & Portugal Dassault Systèmes’ Centers of Simulation Excellence Fremont, CA, Tel: +1 510 794 5891, simulia.west.support@3ds.com West Lafayette, IN, Tel: +1 765 497 1373, simulia.central.support@3ds.com Northville, MI, Tel: +1 248 349 4669, simulia.greatlakes.info@3ds.com Woodbury, MN, Tel: +1 612 424 9044, simulia.central.support@3ds.com Mayfield Heights, OH, Tel: +1 216 378 1070, simulia.erie.info@3ds.com Mason, OH, Tel: +1 513 275 1430, simulia.central.support@3ds.com Warwick, RI, Tel: +1 401 739 3637, simulia.east.support@3ds.com Lewisville, TX, Tel: +1 972 221 6500, simulia.south.info@3ds.com Richmond VIC, Tel: +61 3 9421 2900, simulia.au.support@3ds.com Vienna, Tel: +43 1 22 707 200, simulia.at.info@3ds.com Maarssen, The Netherlands, Tel: +31 346 585 710, simulia.benelux.support@3ds.com Toronto, ON, Tel: +1 416 402 2219, simulia.greatlakes.info@3ds.com Beijing, P. R. China, Tel: +8610 6536 2288, simulia.cn.support@3ds.com Shanghai, P. R. China, Tel: +8621 3856 8000, simulia.cn.support@3ds.com Espoo, Tel: +358 40 902 2973, simulia.nordic.info@3ds.com Velizy Villacoublay Cedex, Tel: +33 1 61 62 72 72, simulia.fr.support@3ds.com Aachen, Tel: +49 241 474 01 0, simulia.de.info@3ds.com Munich, Tel: +49 89 543 48 77 0, simulia.de.info@3ds.com Chennai, Tamil Nadu, Tel: +91 44 43443000, simulia.in.info@3ds.com Lainate MI, Tel: +39 02 3343061, simulia.ity.info@3ds.com Tokyo, Tel: +81 3 5442 6302, simulia.jp.support@3ds.com Osaka, Tel: +81 6 7730 2703, simulia.jp.support@3ds.com Mapo-Gu, Seoul, Tel: +82 2 785 6707/8, simulia.kr.info@3ds.com Puerto Madero, Buenos Aires, Tel: +54 11 4312 8700, Horacio.Burbridge@3ds.com Stockholm, Sweden, Tel: +46 8 68430450, simulia.nordic.info@3ds.com Warrington, Tel: +44 1925 830900, simulia.uk.info@3ds.com Authorized Support Centers SMARTtech Sudamerica SRL, Buenos Aires, Tel: +54 11 4717 2717 KB Engineering, Buenos Aires, Tel: +54 11 4326 7542 Solaer Ingeniería, Buenos Aires, Tel: +54 221 489 1738 SMARTtech Mecânica, Sao Paulo-SP, Tel: +55 11 3168 3388 Synerma s. r. o., Psáry, Prague-West, Tel: +420 603 145 769, abaqus@synerma.cz 3 Dimensional Data Systems, Crete, Tel: +30 2821040012, support@3dds.gr ADCOM, Givataim, Tel: +972 3 7325311, shmulik.keidar@adcomsim.co.il WorleyParsons Services Sdn. Bhd., Kuala Lumpur, Tel: +603 2039 9000, abaqus.my@worleyparsons.com Kimeca.NET SA de CV, Mexico, Tel: +52 55 2459 2635 Matrix Applied Computing Ltd., Auckland, Tel: +64 9 623 1223, abaqus-tech@matrix.co.nz BudSoft Sp. z o.o., Poznań, Tel: +48 61 8508 466, info@budsoft.com.pl TESIS Ltd., Moscow, Tel: +7 495 612 44 22, info@tesis.com.ru WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com Finite Element Analysis Services (Pty) Ltd., Parklands, Tel: +27 21 556 6462, feas@feas.co.za Thailand Turkey Simutech Solution Corporation, Taipei, R.O.C., Tel: +886 2 2507 9550, camilla@simutech.com.tw WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com A-Ztech Ltd., Istanbul, Tel: +90 216 361 8850, info@a-ztech.com.tr Preface Support Both technical engineering support (for problems with creating a model or performing an analysis) and systems support (for installation, licensing, and hardware-related problems) for Abaqus are offered through a network of local support offices. Regional contact information is listed in the front of each Abaqus manual and is accessible from the Locations page at www.simulia.com. Support for SIMULIA products SIMULIA provides a knowledge database of answers and solutions to questions that we have answered, as well as guidelines on how to use Abaqus, SIMULIA Scenario Definition, Isight, and other SIMULIA products. You can also submit new requests for support. All support incidents are tracked. If you contact us by means outside the system to discuss an existing support problem and you know the incident or support request number, please mention it so that we can query the database to see what the latest action has been. Many questions about Abaqus can also be answered by visiting the Products page and the Support page at www.simulia.com. Anonymous ftp site To facilitate data transfer with SIMULIA, an anonymous ftp account is available at ftp.simulia.com. Login as user anonymous, and type your e-mail address as your password. Contact support before placing files on the site. Training All offices and representatives offer regularly scheduled public training classes. The courses are offered in a traditional classroom form and via the Web. We also provide training seminars at customer sites. All training classes and seminars include workshops to provide as much practical experience with Abaqus as possible. For a schedule and descriptions of available classes, see www.simulia.com or call your local office or representative. Feedback We welcome any suggestions for improvements to Abaqus software, the support program, or documentation. We will ensure that any enhancement requests you make are considered for future releases. If you wish to make a suggestion about the service or products, refer to www.simulia.com. Complaints should be made by contacting your local office or through www.simulia.com by visiting the Quality Assurance section of the 1.1.1 1.2.1 1.2.2 1.3.1 1.4.1 2.1.1 2.1.2 2.1.3 2.1.4 2.1.5 2.1.6 2.2.1 2.2.2 2.2.3 2.2.4 2.2.5 2.3.1 2.3.2 2.3.3 2.3.4 Contents Volume I PART I INTRODUCTION, SPATIAL MODELING, AND EXECUTION 1. Introduction Introduction: general Abaqus syntax and conventions Input syntax rules Conventions Abaqus model definition Defining a model in Abaqus Parametric modeling Parametric input 2. Spatial Modeling Node definition Node definition Parametric shape variation Nodal thicknesses Normal definitions at nodes Transformed coordinate systems Adjusting nodal coordinates Element definition Element definition Element foundations Defining reinforcement Defining rebar as an element property Orientations Surface definition Surfaces: overview Element-based surface definition Node-based surface definition Analytical rigid surface definition Eulerian surface definition Operating on surfaces Rigid body definition Rigid body definition Integrated output section definition Integrated output section definition Mass adjustment Adjust and/or redistribute mass of an element set Nonstructural mass definition Nonstructural mass definition Distribution definition Distribution definition Display body definition Display body definition Assembly definition Defining an assembly Matrix definition Defining matrices 3. Job Execution Execution procedures: overview Execution procedure for Abaqus: overview Execution procedures Obtaining information Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution SIMULIA Co-Simulation Engine controller execution Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution Abaqus/CAE execution Abaqus/Viewer execution Python execution Parametric studies Abaqus documentation Licensing utilities ASCII translation of results (.fil) files Joining results (.fil) files Querying the keyword/problem database ii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 2.3.5 2.3.6 2.4.1 2.5.1 2.6.1 2.7.1 2.8.1 2.9.1 2.10.1 2.11.1 3.1.1 3.2.1 3.2.2 3.2.3 3.2.4 3.2.5 3.2.6 3.2.7 3.2.8 3.2.9 3.2.10 Making user-defined executables and subroutines Input file and output database upgrade utility Generating output database reports Joining output database (.odb) files from restarted analyses Combining output from substructures Combining data from multiple output databases Network output database file connector Mapping thermal and magnetic loads Fixed format conversion utility Translating Nastran bulk data files to Abaqus input files Translating Abaqus files to Nastran bulk data files Translating ANSYS input files to Abaqus input files Translating PAM-CRASH input files to partial Abaqus input files Translating RADIOSS input files to partial Abaqus input files Translating Abaqus output database files to Nastran Output2 results files Translating LS-DYNA data files to Abaqus input files Exchanging Abaqus data with ZAERO Encrypting and decrypting Abaqus input data Job execution control Environment file settings Using the Abaqus environment settings Managing memory and disk resources Managing memory and disk use in Abaqus Parallel execution Parallel execution: overview Parallel execution in Abaqus/Standard Parallel execution in Abaqus/Explicit Parallel execution in Abaqus/CFD File extension definitions File extensions used by Abaqus FORTRAN unit numbers FORTRAN unit numbers used by Abaqus CONTENTS 3.2.14 3.2.15 3.2.16 3.2.17 3.2.18 3.2.19 3.2.20 3.2.21 3.2.22 3.2.23 3.2.24 3.2.25 3.2.26 3.2.27 3.2.28 3.2.29 3.2.30 3.2.31 3.2.32 3.2.33 3.3.1 3.4.1 3.5.1 3.5.2 3.5.3 3.5.4 3.6.1 3.7.1 4.1.2 4.1.3 4.1.4 4.2.1 4.2.2 4.2.3 4.3.1 5.1.1 5.1.2 5.1.3 5.1.4 CONTENTS 4. Output PART II OUTPUT Output Output to the data and results files Output to the output database Error indicator output Output variables Abaqus/Standard output variable identifiers Abaqus/Explicit output variable identifiers Abaqus/CFD output variable identifiers The postprocessing calculator The postprocessing calculator 5. File Output Format Accessing the results file Accessing the results file: overview Results file output format Accessing the results file information Utility routines for accessing the results file OI.1 Abaqus/Standard Output Variable Index OI.2 Abaqus/Explicit Output Variable Index OI.3 Abaqus/CFD Output Variable Index 6.1.1 6.1.2 6.1.3 6.1.4 6.1.5 6.1.6 6.2.1 6.2.2 6.2.3 6.2.4 6.2.5 6.2.6 6.2.7 6.3.1 6.3.2 6.3.3 6.3.4 6.3.5 6.3.6 6.3.7 6.3.8 6.3.9 6.3.10 6.3.11 6.4.1 6.5.1 6.5.2 Volume II PART III ANALYSIS PROCEDURES, SOLUTION, AND CONTROL 6. Analysis Procedures Introduction Solving analysis problems: overview Defining an analysis General and linear perturbation procedures Multiple load case analysis Direct linear equation solver Iterative linear equation solver Static stress/displacement analysis Static stress analysis procedures: overview Static stress analysis Eigenvalue buckling prediction Unstable collapse and postbuckling analysis Quasi-static analysis Direct cyclic analysis Low-cycle fatigue analysis using the direct cyclic approach Dynamic stress/displacement analysis Dynamic analysis procedures: overview Implicit dynamic analysis using direct integration Explicit dynamic analysis Direct-solution steady-state dynamic analysis Natural frequency extraction Complex eigenvalue extraction Transient modal dynamic analysis Mode-based steady-state dynamic analysis Subspace-based steady-state dynamic analysis Response spectrum analysis Random response analysis Steady-state transport analysis Steady-state transport analysis Heat transfer and thermal-stress analysis Heat transfer analysis procedures: overview Uncoupled heat transfer analysis 6.5.4 6.6.1 6.6.2 6.7.1 6.7.2 6.7.3 6.7.4 6.7.5 6.7.6 6.8.1 6.8.2 6.9.1 6.10.1 6.11.1 6.12.1 7.1.1 7.2.1 7.2.2 7.2.3 7.2.4 CONTENTS Fully coupled thermal-stress analysis Adiabatic analysis Fluid dynamic analysis Fluid dynamic analysis procedures: overview Incompressible fluid dynamic analysis Electromagnetic analysis Electromagnetic analysis procedures Piezoelectric analysis Coupled thermal-electrical analysis Fully coupled thermal-electrical-structural analysis Eddy current analysis Magnetostatic analysis Coupled pore fluid flow and stress analysis Coupled pore fluid diffusion and stress analysis Geostatic stress state Mass diffusion analysis Mass diffusion analysis Acoustic and shock analysis Acoustic, shock, and coupled acoustic-structural analysis Abaqus/Aqua analysis Abaqus/Aqua analysis Annealing Annealing procedure 7. Analysis Solution and Control Solving nonlinear problems Solving nonlinear problems Analysis convergence controls Convergence and time integration criteria: overview Commonly used control parameters Convergence criteria for nonlinear problems Time integration accuracy in transient problems ANALYSIS TECHNIQUES 8. Analysis Techniques: Introduction Analysis techniques: overview 9. Analysis Continuation Techniques Restarting an analysis Restarting an analysis Importing and transferring results Transferring results between Abaqus analyses: overview Transferring results between Abaqus/Explicit and Abaqus/Standard Transferring results from one Abaqus/Standard analysis to another Transferring results from one Abaqus/Explicit analysis to another 10. Modeling Abstractions Substructuring Using substructures Defining substructures Submodeling Submodeling: overview Node-based submodeling Surface-based submodeling Generating global matrices Generating matrices CONTENTS 8.1.1 9.1.1 9.2.1 9.2.2 9.2.3 9.2.4 10.1.1 10.1.2 10.2.1 10.2.2 10.2.3 10.3.1 Symmetric model generation, results transfer, and analysis of cyclic symmetry models Symmetric model generation Transferring results from a symmetric mesh or a partial three-dimensional mesh to a full three-dimensional mesh Analysis of models that exhibit cyclic symmetry Periodic media analysis Periodic media analysis Meshed beam cross-sections Meshed beam cross-sections vii 10.4.1 10.4.2 10.4.3 10.5.1 Modeling discontinuities as an enriched feature using the extended finite element method Modeling discontinuities as an enriched feature using the extended finite element 10.7.1 11.1.1 11.2.1 11.3.1 11.4.1 11.4.2 11.4.3 11.5.1 11.5.2 11.5.3 11.5.4 11.6.1 11.7.1 11.8.1 12.1.1 12.2.1 12.2.2 12.2.3 12.2.4 method 11. Special-Purpose Techniques Inertia relief Inertia relief Mesh modification or replacement Element and contact pair removal and reactivation Geometric imperfections Introducing a geometric imperfection into a model Fracture mechanics Fracture mechanics: overview Contour integral evaluation Crack propagation analysis Surface-based fluid modeling Surface-based fluid cavities: overview Fluid cavity definition Fluid exchange definition Inflator definition Mass scaling Mass scaling Selective subcycling Selective subcycling Steady-state detection Steady-state detection 12. Adaptivity Techniques Adaptivity techniques: overview Adaptivity techniques ALE adaptive meshing ALE adaptive meshing: overview Defining ALE adaptive mesh domains in Abaqus/Explicit ALE adaptive meshing and remapping in Abaqus/Explicit Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit 12.2.5 12.2.6 12.2.7 12.3.1 12.3.2 12.3.3 12.4.1 13.1.1 13.2.1 13.2.2 13.2.3 14.1.1 14.1.2 14.1.3 14.1.4 15.1.1 15.1.2 16.1.1 16.1.2 16.1.3 17.1.1 17.2.1 Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit Defining ALE adaptive mesh domains in Abaqus/Standard ALE adaptive meshing and remapping in Abaqus/Standard Adaptive remeshing Adaptive remeshing: overview Selection of error indicators influencing adaptive remeshing Solution-based mesh sizing Analysis continuation after mesh replacement Mesh-to-mesh solution mapping 13. Optimization Techniques Structural optimization: overview Structural optimization: overview Optimization models Design responses Objectives and constraints Creating Abaqus optimization models 14. Eulerian Analysis Eulerian analysis Defining Eulerian boundaries Eulerian mesh motion Defining adaptive mesh refinement in the Eulerian domain 15. Particle Methods Smoothed particle hydrodynamic analyses Smoothed particle hydrodynamic analysis Finite element conversion to SPH particles 16. Sequentially Coupled Multiphysics Analyses Predefined fields for sequential coupling Sequentially coupled thermal-stress analysis Predefined loads for sequential coupling 17. Co-simulation Co-simulation: overview Preparing an Abaqus analysis for co-simulation Preparing an Abaqus analysis for co-simulation Co-simulation between Abaqus solvers Abaqus/Standard to Abaqus/Explicit co-simulation Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation 18. Extending Abaqus Analysis Functionality User subroutines and utilities User subroutines: overview Available user subroutines Available utility routines 19. Design Sensitivity Analysis Design sensitivity analysis 20. Parametric Studies Scripting parametric studies Scripting parametric studies Parametric studies: commands aStudy.combine(): Combine parameter samples for parametric studies. aStudy.constrain(): Constrain parameter value combinations in parametric studies. aStudy.define(): Define parameters for parametric studies. aStudy.execute(): Execute the analysis of parametric study designs. aStudy.gather(): Gather the results of a parametric study. aStudy.generate(): Generate the analysis job data for a parametric study. aStudy.output(): Specify the source of parametric study results. aStudy=ParStudy(): Create a parametric study. aStudy.report(): Report parametric study results. aStudy.sample(): Sample parameters for parametric studies. 17.3.1 17.3.2 18.1.1 18.1.2 18.1.3 19.1.1 20.1.1 20.2.1 20.2.2 20.2.3 20.2.4 20.2.5 20.2.6 20.2.7 20.2.8 20.2.9 20.2.10 21.1.1 21.1.2 21.1.3 21.2.1 22.1.1 22.2.1 22.2.2 22.2.3 22.3.1 22.4.1 22.5.1 22.5.2 22.5.3 22.6.1 22.6.2 22.7.1 22.7.2 Volume III PART V MATERIALS 21. Materials: Introduction Introduction Material library: overview Material data definition Combining material behaviors General properties Density 22. Elastic Mechanical Properties Overview Elastic behavior: overview Linear elasticity Linear elastic behavior No compression or no tension Plane stress orthotropic failure measures Porous elasticity Elastic behavior of porous materials Hypoelasticity Hypoelastic behavior Hyperelasticity Hyperelastic behavior of rubberlike materials Hyperelastic behavior in elastomeric foams Anisotropic hyperelastic behavior Stress softening in elastomers Mullins effect Energy dissipation in elastomeric foams Viscoelasticity Time domain viscoelasticity Frequency domain viscoelasticity Nonlinear viscoelasticity Hysteresis in elastomers Parallel network viscoelastic model Rate sensitive elastomeric foams Low-density foams 23. Inelastic Mechanical Properties Overview Inelastic behavior Metal plasticity Classical metal plasticity Models for metals subjected to cyclic loading Rate-dependent yield Rate-dependent plasticity: creep and swelling Annealing or melting Anisotropic yield/creep Johnson-Cook plasticity Dynamic failure models Porous metal plasticity Cast iron plasticity Two-layer viscoplasticity ORNL – Oak Ridge National Laboratory constitutive model Deformation plasticity Other plasticity models Extended Drucker-Prager models Modified Drucker-Prager/Cap model Mohr-Coulomb plasticity Critical state (clay) plasticity model Crushable foam plasticity models Fabric materials Fabric material behavior Jointed materials Jointed material model Concrete Concrete smeared cracking Cracking model for concrete Concrete damaged plasticity xii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 22.8.1 22.8.2 22.9.1 23.1.1 23.2.1 23.2.2 23.2.3 23.2.4 23.2.5 23.2.6 23.2.7 23.2.8 23.2.9 23.2.10 23.2.11 23.2.12 23.2.13 23.3.1 23.3.2 23.3.3 23.3.4 23.3.5 23.4.1 23.5.1 23.7.1 24.1.1 24.2.1 24.2.2 24.2.3 24.3.1 24.3.2 24.3.3 24.4.1 24.4.2 24.4.3 25.1.1 25.2.1 26.1.1 26.1.2 26.1.3 26.1.4 26.2.1 26.2.2 26.2.3 26.2.4 Permanent set in rubberlike materials Permanent set in rubberlike materials 24. Progressive Damage and Failure Progressive damage and failure: overview Progressive damage and failure Damage and failure for ductile metals Damage and failure for ductile metals: overview Damage initiation for ductile metals Damage evolution and element removal for ductile metals Damage and failure for fiber-reinforced composites Damage and failure for fiber-reinforced composites: overview Damage initiation for fiber-reinforced composites Damage evolution and element removal for fiber-reinforced composites Damage and failure for ductile materials in low-cycle fatigue analysis Damage and failure for ductile materials in low-cycle fatigue analysis: overview Damage initiation for ductile materials in low-cycle fatigue Damage evolution for ductile materials in low-cycle fatigue 25. Hydrodynamic Properties Overview Hydrodynamic behavior: overview Equations of state Equation of state 26. Other Material Properties Mechanical properties Material damping Thermal expansion Field expansion Viscosity Heat transfer properties Thermal properties: overview Conductivity Specific heat Latent heat Acoustic properties Acoustic medium Mass diffusion properties Diffusivity Solubility Electromagnetic properties Electrical conductivity Piezoelectric behavior Magnetic permeability Pore fluid flow properties Pore fluid flow properties Permeability Porous bulk moduli Sorption Swelling gel Moisture swelling User materials User-defined mechanical material behavior User-defined thermal material behavior 26.3.1 26.4.1 26.4.2 26.5.1 26.5.2 26.5.3 26.6.1 26.6.2 26.6.3 26.6.4 26.6.5 26.6.6 26.7.1 26.7.2 27.1.1 27.1.2 27.1.3 27.1.4 28.1.1 28.1.2 28.1.3 28.1.4 28.1.5 28.1.6 28.1.7 28.2.1 28.2.2 28.3.1 28.3.2 28.4.1 28.4.2 28.5.1 28.5.2 29.1.1 29.1.2 29.1.3 Volume IV PART VI ELEMENTS 27. Elements: Introduction Element library: overview Choosing the element’s dimensionality Choosing the appropriate element for an analysis type Section controls 28. Continuum Elements General-purpose continuum elements Solid (continuum) elements One-dimensional solid (link) element library Two-dimensional solid element library Three-dimensional solid element library Cylindrical solid element library Axisymmetric solid element library Axisymmetric solid elements with nonlinear, asymmetric deformation Fluid continuum elements Fluid (continuum) elements Fluid element library Infinite elements Infinite elements Infinite element library Warping elements Warping elements Warping element library Particle elements Particle elements Particle element library 29. Structural Elements Membrane elements Membrane elements General membrane element library Cylindrical membrane element library Axisymmetric membrane element library Truss elements Truss elements Truss element library Beam elements Beam modeling: overview Choosing a beam cross-section Choosing a beam element Beam element cross-section orientation Beam section behavior Using a beam section integrated during the analysis to define the section behavior Using a general beam section to define the section behavior Beam element library Beam cross-section library Frame elements Frame elements Frame section behavior Frame element library Elbow elements Pipes and pipebends with deforming cross-sections: elbow elements Elbow element library Shell elements Shell elements: overview Choosing a shell element Defining the initial geometry of conventional shell elements Shell section behavior Using a shell section integrated during the analysis to define the section behavior Using a general shell section to define the section behavior Three-dimensional conventional shell element library Continuum shell element library Axisymmetric shell element library Axisymmetric shell elements with nonlinear, asymmetric deformation 29.1.4 29.2.1 29.2.2 29.3.1 29.3.2 29.3.3 29.3.4 29.3.5 29.3.6 29.3.7 29.3.8 29.3.9 29.4.1 29.4.2 29.4.3 29.5.1 29.5.2 29.6.1 29.6.2 29.6.3 29.6.4 29.6.5 29.6.6 29.6.7 29.6.8 29.6.9 29.6.10 30.1.1 30.1.2 30.2.1 30.2.2 30.3.1 30.3.2 30.4.1 30.4.2 31.1.1 31.1.2 31.1.3 31.1.4 31.1.5 31.2.1 31.2.2 31.2.3 31.2.4 31.2.5 31.2.6 31.2.7 31.2.8 31.2.9 31.2.10 32.1.1 32.1.2 30. Inertial, Rigid, and Capacitance Elements Point mass elements Point masses Mass element library Rotary inertia elements Rotary inertia Rotary inertia element library Rigid elements Rigid elements Rigid element library Capacitance elements Point capacitance Capacitance element library 31. Connector Elements Connector elements Connectors: overview Connector elements Connector actuation Connector element library Connection-type library Connector element behavior Connector behavior Connector elastic behavior Connector damping behavior Connector functions for coupled behavior Connector friction behavior Connector plastic behavior Connector damage behavior Connector stops and locks Connector failure behavior Connector uniaxial behavior 32. Special-Purpose Elements Spring elements Springs Spring element library Dashpot elements Dashpots Dashpot element library Flexible joint elements Flexible joint element Flexible joint element library Distributing coupling elements Distributing coupling elements Distributing coupling element library Cohesive elements Cohesive elements: overview Choosing a cohesive element Modeling with cohesive elements Defining the cohesive element’s initial geometry Defining the constitutive response of cohesive elements using a continuum approach Defining the constitutive response of cohesive elements using a traction-separation description Defining the constitutive response of fluid within the cohesive element gap Two-dimensional cohesive element library Three-dimensional cohesive element library Axisymmetric cohesive element library Gasket elements Gasket elements: overview Choosing a gasket element Including gasket elements in a model Defining the gasket element’s initial geometry Defining the gasket behavior using a material model Defining the gasket behavior directly using a gasket behavior model Two-dimensional gasket element library Three-dimensional gasket element library Axisymmetric gasket element library Surface elements Surface elements General surface element library Cylindrical surface element library Axisymmetric surface element library 32.2.1 32.2.2 32.3.1 32.3.2 32.4.1 32.4.2 32.5.1 32.5.2 32.5.3 32.5.4 32.5.5 32.5.6 32.5.7 32.5.8 32.5.9 32.5.10 32.6.1 32.6.2 32.6.3 32.6.4 32.6.5 32.6.6 32.6.7 32.6.8 32.6.9 32.7.1 32.7.2 32.7.3 32.7.4 32.8.1 32.8.2 32.9.1 32.9.2 32.10.1 32.10.2 32.11.1 32.11.2 32.12.1 32.12.2 32.13.1 32.13.2 32.14.1 32.14.2 32.15.1 32.15.2 Tube support elements Tube support elements Tube support element library Line spring elements Line spring elements for modeling part-through cracks in shells Line spring element library Elastic-plastic joints Elastic-plastic joints Elastic-plastic joint element library Drag chain elements Drag chains Drag chain element library Pipe-soil elements Pipe-soil interaction elements Pipe-soil interaction element library Acoustic interface elements Acoustic interface elements Acoustic interface element library Eulerian elements Eulerian elements Eulerian element library User-defined elements User-defined elements User-defined element library EI.1 Abaqus/Standard Element Index EI.2 Abaqus/Explicit Element Index EI.3 Abaqus/CFD Element Index Volume V PART VII PRESCRIBED CONDITIONS 33. Prescribed Conditions Overview Prescribed conditions: overview Amplitude curves Initial conditions Initial conditions in Abaqus/Standard and Abaqus/Explicit Initial conditions in Abaqus/CFD Boundary conditions Boundary conditions in Abaqus/Standard and Abaqus/Explicit Boundary conditions in Abaqus/CFD Loads Applying loads: overview Concentrated loads Distributed loads Thermal loads Electromagnetic loads Acoustic and shock loads Pore fluid flow Prescribed assembly loads Prescribed assembly loads Predefined fields Predefined fields PART VIII CONSTRAINTS 34. Constraints Overview Kinematic constraints: overview Multi-point constraints Linear constraint equations xx Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 33.1.1 33.1.2 33.2.1 33.2.2 33.3.1 33.3.2 33.4.1 33.4.2 33.4.3 33.4.4 33.4.5 33.4.6 33.4.7 33.5.1 34.2.2 34.2.3 34.3.1 34.3.2 34.3.3 34.3.4 34.4.1 34.5.1 34.6.1 35.1.1 35.2.1 35.2.2 35.2.3 35.2.4 35.2.5 35.2.6 35.3.1 35.3.2 35.3.3 35.3.4 35.3.5 35.3.6 35.3.7 35.3.8 General multi-point constraints Kinematic coupling constraints Surface-based constraints Mesh tie constraints Coupling constraints Shell-to-solid coupling Mesh-independent fasteners Embedded elements Embedded elements Element end release Element end release Overconstraint checks Overconstraint checks PART IX INTERACTIONS 35. Defining Contact Interactions Overview Contact interaction analysis: overview Defining general contact in Abaqus/Standard Defining general contact interactions in Abaqus/Standard Surface properties for general contact in Abaqus/Standard Contact properties for general contact in Abaqus/Standard Controlling initial contact status in Abaqus/Standard Stabilization for general contact in Abaqus/Standard Numerical controls for general contact in Abaqus/Standard Defining contact pairs in Abaqus/Standard Defining contact pairs in Abaqus/Standard Assigning surface properties for contact pairs in Abaqus/Standard Assigning contact properties for contact pairs in Abaqus/Standard Modeling contact interference fits in Abaqus/Standard Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs Adjusting contact controls in Abaqus/Standard Defining tied contact in Abaqus/Standard Extending master surfaces and slide lines Contact modeling if substructures are present Contact modeling if asymmetric-axisymmetric elements are present Defining general contact in Abaqus/Explicit Defining general contact interactions in Abaqus/Explicit Assigning surface properties for general contact in Abaqus/Explicit Assigning contact properties for general contact in Abaqus/Explicit Controlling initial contact status for general contact in Abaqus/Explicit Contact controls for general contact in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit Assigning surface properties for contact pairs in Abaqus/Explicit Assigning contact properties for contact pairs in Abaqus/Explicit Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit Contact controls for contact pairs in Abaqus/Explicit 36. Contact Property Models Mechanical contact properties Mechanical contact properties: overview Contact pressure-overclosure relationships Contact damping Contact blockage Frictional behavior User-defined interfacial constitutive behavior Pressure penetration loading Interaction of debonded surfaces Breakable bonds Surface-based cohesive behavior Thermal contact properties Thermal contact properties Electrical contact properties Electrical contact properties Pore fluid contact properties Pore fluid contact properties 37. Contact Formulations and Numerical Methods Contact formulations and numerical methods in Abaqus/Standard Contact formulations in Abaqus/Standard xxii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 35.3.9 35.3.10 35.4.1 35.4.2 35.4.3 35.4.4 35.4.5 35.5.1 35.5.2 35.5.3 35.5.4 35.5.5 36.1.1 36.1.2 36.1.3 36.1.4 36.1.5 36.1.6 36.1.7 36.1.8 36.1.9 36.1.10 36.2.1 37.1.2 37.1.3 37.2.1 37.2.2 37.2.3 38.1.1 38.1.2 38.2.1 38.2.2 39.1.1 39.2.1 39.2.2 39.3.1 39.3.2 39.4.1 39.4.2 39.5.1 39.5.2 40.1.1 Contact constraint enforcement methods in Abaqus/Standard Smoothing contact surfaces in Abaqus/Standard Contact formulations and numerical methods in Abaqus/Explicit Contact formulation for general contact in Abaqus/Explicit Contact formulations for contact pairs in Abaqus/Explicit Contact constraint enforcement methods in Abaqus/Explicit 38. Contact Difficulties and Diagnostics Resolving contact difficulties in Abaqus/Standard Contact diagnostics in an Abaqus/Standard analysis Common difficulties associated with contact modeling in Abaqus/Standard Resolving contact difficulties in Abaqus/Explicit Contact diagnostics in an Abaqus/Explicit analysis Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit 39. Contact Elements in Abaqus/Standard Contact modeling with elements Contact modeling with elements Gap contact elements Gap contact elements Gap element library Tube-to-tube contact elements Tube-to-tube contact elements Tube-to-tube contact element library Slide line contact elements Slide line contact elements Axisymmetric slide line element library Rigid surface contact elements Rigid surface contact elements Axisymmetric rigid surface contact element library 40. Defining Cavity Radiation in Abaqus/Standard Cavity radiation Printed on: Execution • Chapter 1, “Introduction” • Chapter 2, “Spatial Modeling” Introduction Introduction Abaqus syntax and conventions Abaqus model definition Parametric modeling INTRODUCTION 1.1 1.2 1.3 1.1 Introduction • “Introduction: general,” Section 1.1.1 INTRODUCTION: GENERAL INTRODUCTION Overview of the Abaqus finite element system The Abaqus finite element system includes: • Abaqus/Standard, a general-purpose finite element program; • Abaqus/Explicit, an explicit dynamics finite element program; • Abaqus/CFD, a general-purpose computational fluid dynamics program; • Abaqus/CAE, an interactive environment used to create finite element models, submit Abaqus analyses, monitor and diagnose jobs, and evaluate results; and • Abaqus/Viewer, a subset of Abaqus/CAE that contains only the postprocessing capabilities of the Visualization module. Several add-on options are available to further extend the capabilities of Abaqus/Standard and Abaqus/Explicit. The Abaqus/Aqua option works with Abaqus/Standard and Abaqus/Explicit. The Abaqus/Design and Abaqus/AMS options work with Abaqus/Standard. Abaqus/Aqua contains optional features that are specifically designed for the analysis of beam-like structures installed underwater and subject to loading by water currents and wave action. The Abaqus/Design option enables you to perform design sensitivity analysis (DSA). Abaqus/AMS is an optional eigensolver that works within Abaqus/Standard providing very fast solution of large symmetric eigenvalue problems. The Abaqus co-simulation technique provides several applications, available as separate add-on capabilities, for coupling between Abaqus and third-party analysis programs. Abaqus/Foundation is an optional subset of Abaqus/Standard that provides more cost-efficient access to the linear static and dynamic analysis functionality in Abaqus/Standard. These options are available only if your license includes them. For a comprehensive list of Abaqus products, utilities, and add-on options, see “Abaqus products,” Section 1.2 of the Abaqus Release Notes. Overview of this manual This manual is a reference guide to using Abaqus/Standard (including Abaqus/Aqua, Abaqus/Design, and Abaqus/Foundation), Abaqus/Explicit (including Abaqus/Aqua), and Abaqus/CFD. Abaqus/Standard solves a system of equations implicitly at each solution “increment.” In contrast, Abaqus/Explicit marches a solution forward through time in small time increments without solving a coupled system of equations at each increment (or even forming a global stiffness matrix). Abaqus/CFD provides a computational fluid dynamics capability with extensive support for preprocessing, simulation, and postprocessingin Abaqus/CAE. Throughout the manual the term Abaqus is most commonly used to refer collectively to both Abaqus/Standard and Abaqus/Explicit and, when applicable, Abaqus/CFD; the individual product names are used to indicate when information applies to only that product. Product identifiers appear at the beginning of each section in the manual (excluding overview sections) indicating the products to which the information in the section applies. The manual is divided into several parts: • Part I, “Introduction, Spatial Modeling, and Execution,” discusses basic modeling concepts in Abaqus, such as defining nodes, elements, and surfaces; the conventions and input formats that should be followed when using Abaqus; and the execution procedures for Abaqus/Standard, Abaqus/Explicit, Abaqus/CFD, Abaqus/CAE, and several utilities that are provided with the Abaqus system. • Part II, “Output,” describes how to obtain output from Abaqus and the format of the results (.fil) file. It also describes the output variable identifiers that are available. • Part III, “Analysis Procedures, Solution, and Control,” describes the analysis types (static stress analysis, dynamics, eigenvalue extraction, etc.) that are available. Detailed discussions of the differences between how Abaqus/Standard and Abaqus/Explicit solve finite element analyses are provided in this chapter. • Part IV, “Analysis Techniques,” discusses various analysis techniques available in Abaqus such as submodeling, removing elements or surfaces, and importing results from a previous simulation to define the initial conditions for the current model. • Part V, “Materials,” describes the material modeling options and how to calibrate some of the more advanced material models. • Part VI, “Elements,” describes the elements available in Abaqus. • Part VII, “Prescribed Conditions,” describes the use of prescribed conditions, such as distributed loads and nodal velocities. • Part VIII, “Constraints,” discusses the use of constraints, such as multi-point constraints. • Part IX, “Interactions,” discusses the contact and interaction models available in Abaqus. The manual also includes indexes of all of Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD. the output variables and elements available in Using Abaqus Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD can be run as batch applications or through the interactive Abaqus/CAE environment . The main input to the Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD analysis products is a file containing the options required for the simulation and the data associated with those options. There may also be supplementary files, such as restart or results files from previous analyses, or auxiliary data files, such as a file containing an acceleration record or an earthquake record for dynamic analysis. The input file is usually created by Abaqus/CAE or another preprocessor. Both input file usage and Abaqus/CAE usage information are provided in this manual. As described in “Defining a model in Abaqus,” Section 1.3.1, the main input file consists of two sections: model input and history input. The input is organized around a few natural concepts and conventions, which means that even though input files for complex simulations can be large, they can be managed without difficulty. The basic syntax rules that govern an Abaqus input file are discussed in “Input syntax rules,” Section 1.2.1. The Abaqus Keywords Reference Manual contains a complete description of all the input options available in Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD. For a detailed introduction to using Abaqus for your analyses, it is recommended that you follow the self-paced tutorials in Getting Started with Abaqus: Interactive Edition. Refer to the Abaqus/CAE User’s Manual for detailed information on working with Abaqus/CAE. In addition, many analyses that demonstrate the numerous capabilities of Abaqus are discussed in the Abaqus Example Problems Manual, the Abaqus Benchmarks Manual, and the Abaqus Verification Manual. As a supplement to the Abaqus Analysis User’s Manual, these examples can help you become familiar with the functionality that Abaqus provides and the structure of the Abaqus input file. For example, “Beam impact on cylinder,” Section 1.6.12 of the Abaqus Verification Manual, discusses the various modeling techniques that can be used to analyze the dynamic response of a cantilever beam. Reviewing the results of an Abaqus simulation Information on requesting output from an Abaqus simulation is discussed in “Output,” Section 4.1.1. Requested results from an Abaqus simulation are viewed through the Visualization module in Abaqus/CAE (also licensed separately as Abaqus/Viewer). The output database file is read by the Visualization module in Abaqus/CAE to create contour plots, animations, X–Y plots, and tabular output of Abaqus results. See Part V, “Viewing results,” of the Abaqus/CAE User’s Manual for detailed information on using the Visualization module in Abaqus/CAE. 1.2 Abaqus syntax and conventions • “Input syntax rules,” Section 1.2.1 • “Conventions,” Section 1.2.2 1.2.1 INPUT SYNTAX RULES Products: Abaqus/Standard Abaqus/Explicit Reference • “Defining a model in Abaqus,” Section 1.3.1 Overview This section describes the syntax rules that govern an Abaqus input file. All data definitions in Abaqus are accomplished with option blocks—sets of data describing a part of the problem definition. You choose those options that are relevant for a particular application. Options are defined by lines in the input file. Three types of input lines are used in an Abaqus input file: keyword lines, data lines, and comment lines. Only 7-bit ASCII characters are supported, and a carriage return is required at the end of each line in an input file. • Keyword lines introduce options and often have parameters, which appear as words or phrases separated by commas on the keyword line. Parameters are used to define the behavior of an option. Parameters can stand alone or have a value, and they may be required or optional. • Data lines, which are used to provide numeric or alphanumeric entries, follow most keyword lines. • Any line that begins with stars in columns 1 and 2 (**) is a comment line. Such lines can be placed anywhere in the file. They are ignored by Abaqus, so they will be printed only in the initial listing of the file. There is no restriction on how many or where such lines occur in the file. Relevant parameters and data lines (including the number of entries per data line) are described in the sections of the Abaqus Keywords Reference Manual describing each option. This section describes the general rules that apply to all keyword and data lines. Keyword lines The following rules apply when entering a keyword line: • The first non-blank character of each keyword line must be a star (*). • The keyword must be followed by a comma (,) if any parameters are given. • Parameters must be separated by commas. • Blanks on a keyword line are ignored. • A line can include no more than 256 characters, including blanks. • Keywords and parameters are not case sensitive. • Parameter values usually are not case sensitive. The only exceptions to this rule are those imposed externally to Abaqus, such as file names on case-sensitive operating systems. • Keywords, parameters, and, in most cases, parameter values need not be spelled out completely, but there must be enough characters given to distinguish them from other keywords, parameters, and parameter values that begin in the same way. Abaqus first searches each associated text string for an exact match. If an exact match is not found, Abaqus then searches based upon the minimum number of unique characters in each keyword, parameter, or parameter value, as the case may be. Embedded blanks can be omitted from any item in a keyword line. If a parameter value is used to provide a number or a file name, the complete value should be provided. • If a parameter has a value, the equal sign (=) is used. The value can be an integer, a floating point number, or a character string, depending on the context. For example, *ELASTIC, TYPE=ISOTROPIC, DEPENDENCIES=1 • When the parameter value is a character string that represents the name of an item, you should not use case as a method of distinguishing values unless the values are enclosed within quotation marks. For example, Abaqus does not distinguish between the following definitions: *MATERIAL, NAME=STEEL *MATERIAL, NAME=Steel • The same parameter should not appear more than once on a single keyword line. If a parameter has multiple settings on a single keyword line, Abaqus ignores all but one of the settings. • Continuation of a keyword line is sometimes necessary; for example, because of a large number of parameters. If the last character on a keyword line is a comma, the next line is interpreted as a continuation of the line. For example, the *ELASTIC keyword line above could also be given as *ELASTIC, TYPE=ISOTROPIC, DEPENDENCIES=1 • Certain keywords must be used in conjunction with other keywords; for example, the *ELASTIC and *DENSITY keywords must be used in conjunction with the *MATERIAL keyword. These related keywords must be grouped in a block in the input file; unrelated keywords cannot be specified within this block. • Some options allow the INPUT or FILE parameter to be set equal to the name of an alternate file. Such file names can include a full path name or a relative path name. Relative path names must be with respect to the directory from which the job was submitted. If no path is specified, the file is assumed to be in the directory from which the job was submitted. A substructure library must be in the same directory from which the job was submitted; a full path name cannot be used to specify a substructure library name. For files referenced by the INPUT parameter, the file name must include any extension (e.g., elem.inp). For files referenced by the FILE parameter, the name must be given without an extension in most cases since Abaqus assumes that the file to be read has the correct extension for the file type that is relevant to the option: .res for restart files (“Restarting an analysis,” Section 9.1.1) and .fil for results files (“Output,” Section 4.1.1). However, special rules may apply when a results file (.fil) or an output database file (.odb) is relevant for the option . The file or substructure library name must have the correct case on computers with case- sensitive operating systems. Regardless of whether the user specifies only a file name, a relative path name, or a full path name, the complete name including the path can have a maximum of 80 characters. Data lines Data lines are used to provide data that are more easily given in lists than as parameters on an option. Most options require one or more data lines; if they are required, the data lines must immediately follow the keyword line introducing the option. The following rules apply when entering a data line: • A data line can include no more than 256 characters, including blanks. Trailing blanks are ignored. • All data items must be separated by commas (,). An empty data field is specified by omitting data between commas. Abaqus will use values of zero for any required numeric data that are omitted unless a default value is specified. • A line must contain only the number of items specified. • Empty data fields at the end of a line can be ignored. • Floating point numbers can occupy a maximum of 20 spaces including the sign, decimal point, and any exponential notation. Floating point numbers can be given with or without an exponent. Any exponent, if input, must be preceded by E or D and an optional (−) or (+). The following line shows four acceptable ways of entering the same floating point number: -12.345 -1234.5E-2 -1234.5D-2 -1.2345E1 • Integer data items can occupy a maximum of 9 digits. • Character strings can be up to 80 characters long and are not case sensitive. • Continuation lines are allowed in specific instances . If allowed, such lines are indicated by a comma as the last character of the preceding line. A single data item cannot be entered over multiple lines. In many cases the choice of parameters used with an option determines the type of data lines required. For example, there are five different ways to define a linear elastic material (“Elastic behavior: overview,” Section 22.1.1). The data lines you specify must be consistent with the value of the TYPE parameter given on the *ELASTIC option. Sets One of the most useful features of the Abaqus data definition method is the availability of sets. A set can be a set of nodes or a set of elements. You provide a name (1–80 characters, the first of which must be a letter) for each set. That name then provides a means of referencing all of the members of the set. As an example suppose that, for the structure shown in Figure 1.2.1–1, we wish to apply symmetry boundary conditions at all of the nodes in the set MIDDLE and that the edge SUPPORT is pinned. We assemble the relevant nodes into sets and specify the boundary conditions by *BOUNDARY NSET middle NSET support Figure 1.2.1–1 Example of the use of sets. MIDDLE, ZSYMM SUPPORT, PINNED Sets are the basic reference throughout Abaqus, and the use of sets is recommended. Choosing meaningful set names makes it simple to identify which data belong to which part of the model. Further discussion of sets is provided in “Node definition,” Section 2.1.1, and “Element definition,” Section 2.2.1. Labels Labels such as set names, surface names, and rebar names are case insensitive unless enclosed within quotation marks (except when they are accessed from user subroutines; see “User subroutines: overview,” Section 18.1.1). Labels can be up to 80 characters long. All spaces within a label are ignored unless the label is enclosed in quotation marks, in which case all spaces within the label are maintained. A label that is not enclosed within quotation marks must begin with a letter, may not include a period (.), and should not contain characters such as commas and equal signs. These restrictions do not apply to labels enclosed within quotation marks except if the label is a material name. A material name must always start with a letter, even if the name is enclosed within quotation marks. Labels cannot begin and end with a double underscore (e.g., __STEEL__). This label format is reserved for internal use by Abaqus. The following are examples of labels entered with and without the use of quotation marks: *ELEMENT, TYPE=SPRINGA, ELSET="One element" 1,1,2 *SPRING, ELSET="One element" 1.0E-5, *NSET, ELSET="One element", NSET=NODESET *BOUNDARY nodeset,1,2 Repeating data lines Some options list only a single data line. In cases where only one data line is allowed, this is indicated by the data line title “First (and only) line.” An example of this is the *DYNAMIC option. In many cases the single data line shown can be repeated to define one variable as a function of another; this choice is indicated by a note after the data line. For example, a table of biaxial test data can be given to define a hyperelastic material: *BIAXIAL TEST DATA , , , Etc. There is no limit on the number of data lines allowed, but the data must be given in a certain order, as explained below. Many options require more than one data line; these are indicated by the data line titles “First line:”, “Second line:”, etc. For example, exactly two data lines must be used to define a local orientation for a shell element (*ORIENTATION), and at least three data lines are required to define anisotropic elasticity (*ELASTIC). In many cases the data lines can be repeated, which is indicated by a note after the data lines. As with repetition of a single data line, it is important that sets of data lines be given in the correct order so that Abaqus can interpolate the data properly. Example: Multiple data lines due to field variable dependence Any time an option can be defined as a function of field variables, you must determine the number of data lines required to define the option completely. For example, two data lines are required if stress- based failure criteria (*FAIL STRESS) are defined as a function of two field variables. This pair of data lines is repeated as often as necessary to define the failure criteria completely: first pair ⎭ ⎬ ⎫ ⎭ second ⎬ pair ⎫ ⎭ ⎬ ⎫ third pair *FAIL STRESS, DEPENDENCIES=2 X1, X1, Y1, Y1, S1, , σ1 fv1, fv1 1 2 t c t c biax t c t c biax X2, X2, Y2, Y2, S2, , σ2 fv2, fv2 1 2 t c t c biax X3, X3, Y3, Y3, S3, , σ3 fv3, fv3 1 2 Etc. (In this example the last field on the first data line of each pair was omitted, which means that the stress- based failure criteria are not temperature dependent.) If the stress-based failure criteria were defined as a function of nine field variables, a set of three data lines would be repeated as often as necessary: *FAIL STRESS, DEPENDENCIES=9 X1, X1, Y1, Y1, S1, , σ1 t c t c biax fv1, fv1, fv1, fv1, fv1, fv1, fv1, fv1 1 2 3 4 5 6 7 8 fv1 ⎭ ⎬ ⎫ first set ⎭ second ⎬ set ⎫ X2, X2, Y2, Y2, S2, , σ2 t c t c biax fv2, fv2, fv2, fv2, fv2, fv2, fv2, fv2 1 2 3 4 5 6 7 8 fv2 Etc. Ordering the data lines Whenever one variable is defined as a function of another, the data must be given in the proper order so that Abaqus can interpolate for intermediate values correctly. The variable being defined is assumed to be constant outside the range of independent variables given, except for nonlinear elastic gasket thickness behavior involving damage where the data are extrapolated based on the last slope computed from the user-specified data. If the property being defined is a function of only one variable (such as the *BIAXIAL TEST DATA shown above), the data should be given in the order of increasing value of the independent variable. If the property being defined is a function of multiple independent variables, the variation of the property with respect to the first variable must be given at fixed values of the other variables, in ascending values of the second variable, then of the third variable, and so on. The data lines must always be ordered so that the independent variables are given increasing values. This process ensures that the value of the material property is completely and uniquely defined at any values of the independent variables upon which the property depends. As an example, consider isotropic elasticity defined as a function of three field variables (but not of temperature): *ELASTIC, DEPENDENCIES=3 , , , , , , , , , , , , , , , , , , , , , , , , , , , , 1, 1, 1 , 2, 1, 1 , 1, 2, 1 , 2, 2, 1 , 1, 3, 1 , 2, 3, 1 , 1, 1, 2 , 2, 1, 2 , 1, 2, 2 , , 2, 2, 2 , , 1, 3, 2 , , 2, 3, 2 , , 1, 1, 3 , , 2, 1, 3 , , 1, 2, 3 , , 2, 2, 3 , , 1, 3, 3 , , 2, 3, 3 1.2.2 CONVENTIONS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • Chapter 2, “Spatial Modeling” • Part II, “Output” • “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1 • “Boundary conditions in Abaqus/CFD,” Section 33.3.2 Overview The conventions that are used throughout Abaqus are defined in this section. The following topics are discussed: • Degrees of freedom • Coordinate systems • Self-consistent units • Time measures • Local directions on surfaces in space • Stress and strain conventions • Stress and strain measures in geometrically nonlinear analysis • Conventions for finite rotations • Conventions for tabular data input Degrees of freedom Except for axisymmetric elements, fluid continuum elements, and electromagnetic elements, the degrees of freedom are always referred to as follows: x-displacement y-displacement z-displacement Rotation about the x-axis, in radians Rotation about the y-axis, in radians Rotation about the z-axis, in radians Warping amplitude (for open-section beam elements) Pore pressure, hydrostatic fluid pressure, or acoustic pressure Electric potential 10 11 12 13 14 Connector material flow (units of length) Temperature (or normalized concentration in mass diffusion analysis) Second temperature (for shells or beams) Third temperature (for shells or beams) Etc. Here the x-, y-, and z-directions coincide with the global X-, Y-, and Z-directions, respectively; however, if a local transformation is defined at a node , they coincide with the local directions defined by the transformation. A maximum of 20 temperature values (degrees of freedom 11 through 30) can be defined for shell or beam elements in Abaqus/Standard. Axisymmetric elements The displacement and rotation degrees of freedom in axisymmetric elements are referred to as follows: r-displacement z-displacement Rotation about the z-axis (for axisymmetric elements with twist), in radians Rotation in the r–z plane (for axisymmetric shells), in radians Here the r- and z-directions coincide with the global X- and Y-directions, respectively; however, if a local transformation is defined at a node , they coincide with the local directions defined by the transformation. Fluid continuum elements Fluid continuum elements in Abaqus/CFD are used to define the element shape and to discretize the continuum. Degrees of freedom in a fluid flow analysis are not determined by the element type but by the analysis procedure and options specified (e.g., turbulence models and auxiliary transport equations). Electromagnetic elements Electromagnetic elements in Abaqus/Standard are used to define the element shape and to discretize the continuum. The eddy current and magnetostatic analyses formulations use magnetic vector potential as a degree of freedom . Activation of degrees of freedom Abaqus/Standard and Abaqus/Explicit activate only those degrees of freedom needed at a node. Thus, some of the degrees of freedom listed above may not be used at all nodes in a model, because each element type uses only those degrees of freedom that are relevant. For example, two-dimensional solid (continuum) stress/displacement elements use only degrees of freedom 1 and 2. The degrees of freedom actually used at any node are the envelope of those needed in each element that shares the node. In Abaqus/CFD the active degrees of freedom in a fluid flow analysis are determined by the analysis procedure and the options specified. For example, using the energy equation in conjunction with the incompressible flow procedure activates the velocity, pressure, and temperature degrees of freedom. For more information, see “Active degrees of freedom” in “Boundary conditions in Abaqus/CFD,” Section 33.3.2. Internal variables in Abaqus/Standard In addition to the degrees of freedom listed above, Abaqus/Standard uses internal variables (such as Lagrange multipliers to impose constraints) for some elements. Normally you need not be concerned with these variables, but they may appear in error and warning messages and are checked for satisfaction of nonlinear constraints during iteration. Internal variables are always associated with internal nodes, which have negative numbers to distinguish them from user-defined nodes. Coordinate systems The basic coordinate system in Abaqus is a right-handed, rectangular Cartesian system. You can choose other systems locally for input , for output of nodal variables (displacements, velocities, etc.) and point load or boundary condition specification , and for material or kinematic joint specification . All coordinate systems must be right-handed. Units Abaqus has no units built into it except for rotation and angle measures. Therefore, the units chosen must be self-consistent, which means that derived units of the chosen system can be expressed in terms of the fundamental units without conversion factors. Rotation and angle measures In Abaqus rotational degrees of freedom are expressed in radians, and all other angle measures are expressed in degrees (for example, phase angles). International System of units (SI) The International System of units (SI) is an example of a self-consistent set of units. The fundamental units in the SI system are length in meters (m), mass in kilograms (kg), time in seconds (s), temperature in degrees kelvin (K), and electric current in amperes (A). The units of secondary or derived quantities are based on these fundamental units. An example of a derived unit is the unit of force. A unit of force in the SI system is called a newton (N): Similarly, a unit of electrical charge in the SI system is called a coulomb (C): newton kg m s coulomb A s Another example is the unit of energy, called a joule (J): joule N m A volt s kg m s The unit of electrical potential in the SI system is the volt, which is chosen such that joule volt C volt A s Sometimes the standard units are not convenient to work with. For example, Young’s modulus is frequently specified in terms of megapascals (MPa) (or, equivalently, N/mm2 ), where 1 pascal = 1 N/m2 . In this case the fundamental units could be tonnes (1 tonne = 1000 kilograms), millimeters, and seconds. American or English units American or English units can cause confusion since the naming conventions are not as clear as in the SI system. For example, 1 pound force (lbf) will give 1 pound mass (lbm) an acceleration of g ft/sec2 , where g is the value of acceleration due to gravity. If pounds force, feet (ft), and seconds are taken as fundamental units, the derived unit of mass is lbf sec2 /ft. Since density is commonly given in handbooks as lbm/in3 , it must be converted to lbf sec2/ft4 by lbm in lbf sec ft Frequently it is not made clear in handbooks whether lb stands for lbm or lbf. You need to check that the values used make up a consistent set of units. Two other units that cause difficulty are the slug, defined as the mass that will be accelerated at 1 ft/sec2 by 1 lbf, and the poundal, defined as the force required to accelerate 1 lbm at 1 ft/sec2 . Useful conversions are and slug lbm lbf poundals where g is the magnitude of the acceleration due to gravity in ft/sec2 . Symbols used in Abaqus for units Units are indicated for the value to be given on load and flux types as follows: Dimension Indicator Example (S.I. units) length mass meter kilogram Dimension Indicator Example (S.I. units) time temperature electric current force energy electric charge electric potential mass concentration second degree Celsius ampere newton joule coulomb volt Parts per million Time Abaqus has two measures of time—step time and total time. Except for certain linear perturbation procedures, step time is measured from the beginning of each step. Total time starts at zero and is the total accumulated time over all general analysis steps (including restart steps; see “Restarting an analysis,” Section 9.1.1). Total time does not accumulate during linear perturbation steps. Local directions on surfaces in space Local directions are needed on surfaces in space; for example, to define the tangential slip directions on an element-based contact surface or to define stress and strain components in a shell. The convention used in Abaqus for such directions is as follows. The default local 1-direction is the projection of the global x-axis onto the surface. If the global x-axis is within 0.1° of being normal to the surface, the local 1-direction is the projection of the global z-axis onto the surface. The local 2-direction is then at right angles to the local 1-direction, so that the local 1-direction, local 2-direction, and the positive normal to the surface form a right-handed set . The positive normal direction is defined in an element by the right-hand rotation rule going around the nodes of the element. The local surface directions can be redefined; see “Orientations,” Section 2.2.5. The local 1- and 2-directions become local 2- and 3-directions, respectively, when considering gasket elements or the local systems associated with integrated output sections (“Integrated output section definition,” Section 2.5.1) or user-defined sections (“Section output from Abaqus/Standard” in “Output to the data and results files,” Section 4.1.2). For “line”-type surfaces defined on beam, pipe, or truss elements in space, the default local 1-direction and 2-direction are tangential and transverse to the elements. In this case the local surface directions can also be redefined as described in “Orientations,” Section 2.2.5. surface normal projection of x-axis onto surface surface normal Figure 1.2.2–1 Default local surface directions. Rotation of the local directions For geometrically linear analysis, stress and strain components are given by default in the material directions in the reference (initial) configuration. For geometrically nonlinear analysis, small-strain shell elements in Abaqus/Standard (S4R5, S8R, S8R5, S8RT, S9R5, STRI3, and STRI65) use a total Lagrangian strain, and the stress and strain components are given relative to material directions in the reference configuration. Gasket elements are small-strain small-displacement elements, and the components are output by default in the behavior directions in the reference configuration. For finite-membrane-strain elements (all membrane elements, S3/S3R, S4, S4R, SAX, and SAXA elements) and for small-strain shell elements in Abaqus/Explicit, the material directions rotate with the average rigid body motion of the surface to form the material directions in the current configuration. Stress and strain components in these elements are given relative to these material directions in the current configuration. For a more thorough discussion of the definition of the rotated coordinate directions in membrane elements; S3/S3R, S4, and S4R elements; S3RS, S4RS, and S4RSW elements; and SAXA elements, see: • “Membrane elements,” Section 3.4.1 of the Abaqus Theory Manual, • “Finite-strain shell element formulation,” Section 3.6.5 of the Abaqus Theory Manual, • “Small-strain shell elements in Abaqus/Explicit,” Section 3.6.6 of the Abaqus Theory Manual, and • “Axisymmetric shell element allowing asymmetric loading,” Section 3.6.7 of the Abaqus Theory Manual. You can determine whether the local system associated with a user-defined section is fixed or rotates with the average rigid body motion; see “Section output from Abaqus/Standard” in “Output to the data and results files,” Section 4.1.2, for details. You can determine whether the local system associated with an integrated output section is fixed, translates with average rigid body motion, or translates and rotates with the average rigid body motion; see “Integrated output section definition,” Section 2.5.1, for details. See “Contact formulations in Abaqus/Standard,” Section 37.1.1, for information on how the slip directions evolve during an Abaqus/Standard contact analysis. Convention used for stress and strain components When defining material properties, the convention used for stress and strain components in Abaqus is that they are ordered: Direct stress in the 1-direction Direct stress in the 2-direction Direct stress in the 3-direction Shear stress in the 1–2 plane Shear stress in the 1–3 plane Shear stress in the 2–3 plane For example, a fully anisotropic, linear elasticity matrix is symm. The 1-, 2-, and 3-directions depend on the element type chosen. For solid elements the defaults for these directions are the global spatial directions. For shell and membrane elements the defaults for the 1- and 2-directions are local directions in the surface of the shell or membrane, as defined in Part VI, “Elements.” In both cases the 1-, 2-, and 3-directions can be changed as described in “Orientations,” Section 2.2.5. For geometrically nonlinear analysis with solid elements, the default (global) directions do not rotate with the material. However, user-defined orientations do rotate with the material. , , Abaqus/Explicit stores the stress and strain components internally in a different order: , . For geometrically nonlinear analysis, the internally stored components rotate with the material, regardless of whether or not a user-defined orientation is used. This distinction is important when a user subroutine (such as VUMAT) is used. , , Nonisotropic material behavior When nonisotropic material behavior is defined in continuum elements, a user-defined orientation is necessary for the anisotropic behavior to be associated with material directions. See “State storage,” Section 1.5.4 of the Abaqus Theory Manual, for a description of how material directions rotate. Zero-valued stress components Stress components that are always zero are omitted from storage. For example, in plane stress Abaqus stores only the two direct components and one shear component of stress and strain in the plane where the stress values are nonzero. Shear strains Abaqus always reports shear strain as engineering shear strain, : Stress and strain measures The stress measure used in Abaqus is Cauchy or “true” stress, which corresponds to the force per current area. See “Stress measures,” Section 1.5.2 of the Abaqus Theory Manual, and “Stress rates,” Section 1.5.3 of the Abaqus Theory Manual, for more details on stress measures. For geometrically nonlinear analysis, a large number of different strain measures exist. Unlike “true” stress, there is no clearly preferred “true” strain. For the same physical deformation different strain measures will report different values in large-strain analysis. The optimal choice of strain measure depends on analysis type, material behavior, and (to some degree) personal preference. See “Strain measures,” Section 1.4.2 of the Abaqus Theory Manual, for more details on strain measures. By default, the strain output in Abaqus/Standard is the “integrated” total strain (output variable E). For large-strain shells, membranes, and solid elements in Abaqus/Standard two other measures of total strain can be requested: logarithmic strain (output variable LE) and nominal strain (output variable NE). Logarithmic strain (output variable LE) is the default strain output in Abaqus/Explicit; nominal strain (output variable NE) can be requested as well. The “integrated” total strain is not available in Abaqus/Explicit. Total (integrated) strain The default “integrated” strain measure, E, output by Abaqus/Standard to the data (.dat) and results (.fil) files for all elements that can handle finite strain is obtained by integrating the strain rate numerically in a material frame of reference: are the total strains at increments and n, respectively; is the total strain increment from increment n to 1.2.2–8 is the incremental . For elements that use where rotation tensor; and orientations), the above equation simplifies to CONVENTIONS The strain increment is obtained by integration of the rate of deformation over the time increment: This strain measure is appropriate for elastic-(visco)plastic or elastic-creeping materials, because the plastic strains and creep strains are obtained by the same integration procedure. In such materials the elastic strains are small (because the yield stress is small compared to the elastic modulus), and the total strains can be compared directly with the plastic strains and creep strains. If the principal directions of straining rotate with respect to the material axes, the resulting strain measure cannot be related to the total deformation, regardless whether a spatial or corotational coordinate system is used. If the principal directions remain fixed in the material axes, the strain is the integration of the rate of deformation, which is equivalent to the logarithmic strain discussed later. Green’s strain For small-strain shells and beams in Abaqus/Standard, the default strain measure, E, is Green’s strain: is the deformation gradient and is the identity tensor. This strain measure is appropriate for where the small-strain, large-rotation approximation used in these elements. The components of represent strain along directions in the original configuration. The small-strain shells and beams should not be used in finite-strain analysis with either elastic-plastic or hyperelastic material behavior, since incorrect analysis results may be obtained or program failure may occur. Nominal strain The nominal strain, NE, is is the left stretch tensor, where are the principal stretch directions in the current configuration. The principal values of nominal strain are, therefore, the ratios of change in length to length in the reference configuration in the principal directions, thus giving a direct measure of deformation. are the principal stretches, and Logarithmic strain The logarithmic strain, LE, is where the variables are as defined earlier for nominal strain. This is also the strain output for hyperelastic materials. For a hyper-viscoleastic material, the logarithmic elastic strain EE is computed from the current (relaxed) stress state, and the viscoelastic strain CE is computed as LE EE. Stress invariants Many of the constitutive models in Abaqus are formulated in terms of stress invariants. These invariants are defined as the equivalent pressure stress, the Mises equivalent stress, and the third invariant of deviatoric stress, where is the deviatoric stress, defined as Finite rotations The following convention is used for finite rotations in space: Define global X, Y, and Z-axes (that is, degrees of freedom 4, 5, and 6 at a node). Then define , , as “rotations” about the where The direction according to the right-hand rule . is then the axis of rotation, and is the angular rotation (in radians) about the axis Same vector rotated by ( φ , φ , φ ) y z Initial vector Figure 1.2.2–2 Definition of finite rotation. The value of , any multiple of exceeds for the rotation components. If rotations larger than direction in Abaqus/Standard, the rotation output varies discontinuously between 0 and Abaqus/Explicit the rotation output varies in all cases between is not uniquely determined. In large-rotation problems where the overall rotation can be added or subtracted, which may lead to discontinuous output values about one axis occur in the positive (negative) ). In and ( . This convention provides straightforward input of kinematic boundary conditions and moments in most cases and simple interpretation of the output. The rotations output by Abaqus represent a single rotation from the reference configuration to the current configuration about a fixed axis. The output does not follow the history of rotation at a node. In addition, this convention reduces to the usual convention for small rotations, even in the case of small rotations superposed on an initial finite rotation (such as might be considered in the study of small vibrations about a predeformed state). Compound rotations Because finite rotations are not additive, the way they must be specified is a bit different from the way the increment in rotation specified over a step must be the other boundary conditions are specified: rotation needed to rotate the node from the configuration at the beginning of the step to that desired at the end of the step. It is not enough to rotate the node over this step to a total rotation vector that would have taken the node into its final configuration if applied on the node in some other initial reference configuration. is needed to rotate from the rotation boundary condition at the beginning of the step (and at the end of the previous step) to its final position at the end of the step, the boundary condition must be specified such that the rotation vector is at the end of the step. If the direction of the rotation vector is constant, this method of specifying rotation boundary conditions and the total rotation vector will be the same. If an increment of rotation Example As an example of how to specify compound finite rotations and to interpret finite rotation output, consider the following example of the rotation of a beam. The beam initially lies along the x-axis. We want to perform the compound rotation, where (Step 1) the beam is rotated by 60° about the z-axis, followed by (Step 2) a 90° spin of the beam about itself, followed by (Step 3) a 90° rotation of the beam about an axis perpendicular to the beam in the x–y plane, such that the beam finishes on the z-axis. This compound rotation is achieved in three steps with applied rotation vectors , , and , where , For this example represents the magnitude of each finite rotation about the (unit length) rotation axis. The rotation vectors above are applied in each of the three steps on the configuration at the beginning of that step. It is most straightforward to prescribe these rotations with velocity-type boundary conditions. For convenience, the default amplitude reference in Abaqus for a velocity-type boundary condition is a constant value of one. . Here , and A typical Abaqus step definition for this example, where node 1 is pinned at the origin and the rotation is applied to node 2, is as follows: *STEP, NLGEOM Step 1: Rotate 60 degrees about the z-axis *STATIC *BOUNDARY, TYPE=VELOCITY 2, 4, 5 2, 6, 6, 1.047198 *END STEP ** *STEP, NLGEOM Step 2: Rotate 90 degrees about the beam axis *STATIC *BOUNDARY, TYPE=VELOCITY 2, 4, 4, 0.785398 2, 5, 5, 1.36035 2, 6, 6 *END STEP ** *STEP, NLGEOM Step 3: Rotate beam onto z-axis *STATIC *BOUNDARY, TYPE=VELOCITY 2, 4, 4, 1.36035 2, 5, 5, -0.785398 2, 6, 6 *END STEP The above method for applying finite-rotation boundary conditions (using a velocity-type boundary condition with the default constant amplitude definition) is strongly recommended. However, if the rotation boundary conditions are applied as displacement-type boundary conditions, the input syntax would change. The Abaqus/Standard convention for boundary condition specification within a step is to specify the total or final boundary state. In such a case the specified boundary conditions from all of the previous steps must be added to the incremental rotation vector components. The Abaqus/Standard step definitions from above would change to: *STEP, NLGEOM Step 1: Rotate 60 degrees about the z-axis *STATIC *BOUNDARY 2, 4, 5 2, 6, 6, 1.047198 *END STEP ** *STEP, NLGEOM Step 2: Rotate 90 degrees about the beam axis *STATIC *BOUNDARY 2, 4, 4, 0.785398 2, 5, 5, 1.36035 2, 6, 6, 1.047198 *END STEP ** *STEP, NLGEOM Step 3: Rotate beam onto z-axis *STATIC *BOUNDARY 2, 4, 4, 2.145748 2, 5, 5, 0.574952 2, 6, 6, 1.047198 *END STEP The boundary conditions in Steps 2 and 3 are the sum of the incremental rotation components plus the rotation boundary conditions specified in the previous steps. In Abaqus/Explicit references to amplitude definitions should be used such that there are no jumps in displacement across the steps. It is often convenient to use amplitude definitions given in terms of total time for this purpose. The displacement boundary conditions will be applied incrementally based on the increment in the value of amplitude curve over the time increment. Therefore, any sudden jumps in displacement at the beginning of a step introduced either without the amplitude curves or with two amplitude curves will be ignored . The Abaqus/Explicit step definitions for the above example would change to: *AMPLITUDE, TIME=TOTAL TIME, NAME=RAMPUR1 0., 0., 0.001, 0., 0.002, 0.785398, 0.003, 2.145748 *AMPLITUDE, TIME=TOTAL TIME, NAME=RAMPUR2 0., 0., 0.001, 0., 0.002, 1.36035, 0.003, 0.574952 *AMPLITUDE, TIME=TOTAL TIME, NAME=RAMPUR3 0., 0., 0.001, 1.047198, 0.002, 1.047198, 0.003, 1.047198 *STEP Step 1: Rotate 60 degrees about the z-axis *DYNAMIC, EXPLICIT , 0.001 *BOUNDARY, AMP=RAMPUR1 2, 4, 4, 1.0 *BOUNDARY, AMP=RAMPUR2 2, 5, 5, 1.0 *BOUNDARY, AMP=RAMPUR3 2, 6, 6, 1.0 *END STEP ** *STEP Step 2: Rotate 90 degrees about the beam axis *DYNAMIC, EXPLICIT , 0.001 *END STEP ** *STEP Step 3: Rotate beam onto z-axis *DYNAMIC, EXPLICIT , 0.001 *END STEP The boundary conditions in Steps 2 and 3 are the sum of the incremental rotation components plus the rotation boundary conditions specified in the previous steps. The Abaqus output of the rotation field at the end of Step 3 is We see that none of the individual components of the specified boundary conditions appears in the final rotation output. The final rotation output represents the rotation vector required to obtain the final orientation in a single step. Suppose that in Step 3 of the previous example we want to apply the rotation vector at node 1 instead of at node 2. If the rotation is applied incrementally, the Abaqus/Standard step definition is as follows: *STEP, NLGEOM Step 3: Rotate beam onto z-axis *STATIC *BOUNDARY, TYPE=VELOCITY, OP=NEW 1, 1, 3 1, 4, 4, 1.36035 1, 5, 5, -0.785398 1, 6, 6 *END STEP and the Abaqus/Explicit step definition is similar. conditions that are in effect at node 2. It is necessary to remove the rotation boundary As mentioned previously, using velocity-type boundary conditions is the preferred method for applying finite-rotation boundary conditions. If the rotation boundary condition is to be applied as a displacement-type boundary condition, we must first retrieve the rotation field at node 1 at the end of Step 2. The Abaqus output of this rotation field is These rotation vector components must then be added to the incremental rotation vector components we wish to prescribe in Step 3. The Abaqus/Standard step definition would change to *STEP Step 3: Rotate beam onto z-axis *STATIC *BOUNDARY, OP=NEW 1, 1, 3 1, 4, 4, 2.772 1, 5, 5, 0.0301 1, 6, 6, 0.8155 *END STEP and the Abaqus/Explicit step definition would change to: *STEP Step 3: Rotate beam onto z-axis *DYNAMIC, EXPLICIT , 0.001 *AMPLITUDE, TIME=STEP TIME, NAME=NODE1UR1 0., 1.412, 0.001, 2.772 *AMPLITUDE, TIME=STEP TIME, NAME=NODE1UR2 0., 0.8155, 0.001, 0.0301 *AMPLITUDE, TIME=STEP TIME, NAME=NODE1UR3 0., 0.8155, 0.001, 0.8155 *BOUNDARY, OP=NEW 1, 1, 3 *BOUNDARY, OP=NEW, AMP=NODE1UR1 1, 4, 4, 1. *BOUNDARY, OP=NEW, AMP=NODE1UR2 1, 5, 5, 1. *BOUNDARY, OP=NEW, AMP=NODE1UR3 1, 6, 6, 1. *END STEP The boundary conditions are again specified in the Abaqus/Explicit input using amplitude curves to avoid any sudden jump in their values at the beginning of the step. As stated above and in “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1, any jumps in the displacement values will be ignored and the boundary will be maintained at the previous values. As this last procedure clearly demonstrates, it is simpler to apply finite-rotation boundary conditions as velocity-type boundary conditions rather than as displacement-type boundary conditions. The recommended method of specifying finite-rotation boundary conditions is also described in “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. For further discussion of how finite rotations are accumulated, see “Rotation variables,” Section 1.3.1 of the Abaqus Theory Manual. 1.3 Abaqus model definition • “Defining a model in Abaqus,” Section 1.3.1 1.3.1 DEFINING A MODEL IN Abaqus Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD References • “Input syntax rules,” Section 1.2.1 • Abaqus Keywords Reference Manual • Abaqus/CAE User’s Manual Overview An analysis in Abaqus is defined by an input file, which • contains keyword lines and data lines; and • is divided into model data and history data. The input file An Abaqus input file is an ASCII data file. It can be created by using a text editor or by using a graphical preprocessor such as Abaqus/CAE. The input file consists of a series of lines containing Abaqus options (keyword lines) and data (data lines). The input syntax for keyword and data lines is described in “Input syntax rules,” Section 1.2.1. Most input files have the same basic structure. The following portions of the input file are specified to define a finite element model: 1. An input file often begins with the *HEADING option, which is used to define a title for the analysis. Any number of data lines can be used to give the title; they will appear at the beginning of the output files (“Output,” Section 4.1.1). The first heading line will appear as a heading at the top of each page of the output. While including a title can be helpful for users examining your input file, the *HEADING option is not required. 2. After the heading the input file usually contains a model data section to define nodes, elements, materials, initial conditions, etc. The model data section is explained below. 3. If the model is organized into an assembly of part instances, the model data are further categorized and must fall within the proper level: part, assembly, instance, or model. Models defined in terms of an assembly of part instances are discussed in “Defining an assembly,” Section 2.10.1. 4. Finally, the input file contains history data to define the analysis type, loading, output requests, etc. Step definitions divide the model data from the history data in an input file: everything appearing before the first step definition is model data, and everything appearing within and following the first step definition is history data. The history data section is explained below. The input file is processed by the “analysis input file processor” prior to executing the appropriate analysis product, Abaqus/Standard, Abaqus/Explicit, or Abaqus/CFD. The functions of the analysis input file processor are to interpret the Abaqus options, to perform the necessary consistency checking, and to prepare the data for the analysis products. Most computational mechanics modeling options (element types, loading types, etc.) are available in both Abaqus/Standard and Abaqus/Explicit, although some options are available in only one analysis product or the other. All of the step procedure types used in an input file must be from the same analysis product; however, it is possible to import a solution from Abaqus/Standard into Abaqus/Explicit and vice versa , which allows each analysis product to be used at the various stages of an analysis for which it is best suited (for example, a static preloading in Abaqus/Standard followed by a dynamic analysis in Abaqus/Explicit). Model data Model data define the nodes, elements, materials, initial conditions, etc. Required model data The following model data must be included in an input file to define a finite element model: • Geometry: The geometry of a model is described by elements and their nodes. The rules and methods for defining nodes and elements are described in “Node definition,” Section 2.1.1; “Element definition,” Section 2.2.1; and “Defining an assembly,” Section 2.10.1. Cross-sections for structural elements (such as beams) must be defined. Special features can be defined with special elements such as springs, dashpots, point masses, etc. The element types available for modeling are described in Part VI, “Elements,” along with explanations of how to define the elements. You can view the initial mesh or the configuration after adjustment for initial overclosure in the Visualization module of Abaqus/CAE after a data check run . • Material definitions: A material type must be associated with most portions of the geometry. The material library is described in Part V, “Materials.” Special elements such as springs or dashpots do not have an associated material, but their properties must be defined. Optional model data The following model data can be included as necessary: • Parts and an assembly: The geometry of a model can be defined by organizing it into parts, which are positioned relative to one another in an assembly (“Defining an assembly,” Section 2.10.1). • Initial conditions: Nonzero initial conditions such as initial stresses, temperatures, or velocities can be specified (“Initial conditions,” Section 33.2). • Boundary conditions: Zero-valued boundary conditions (including symmetry conditions) can be imposed on individual solution variables such as displacements or rotations (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). • Kinematic constraints: Equations involving several of the fundamental solution variables in the model (“Linear constraint equations,” Section 34.2.1) or multi-point constraints (“General multi- point constraints,” Section 34.2.2) can be defined. • Interactions: Contact and other interactions between parts can be defined (“Contact interaction analysis: overview,” Section 35.1.1). • Amplitude definitions: Amplitude curves can be defined for later use in specifying time-dependent loading or boundary conditions (“Amplitude curves,” Section 33.1.2). • Output control: You can control model definition output to the data file (“Output,” Section 4.1.1). • Environment properties: Environment properties, such as the attributes of a fluid surrounding the model, may have to be defined. • Analysis continuation: It is possible to write restart data or to use the results from a previous analysis and continue the analysis with new model or history data (“Restarting an analysis,” Section 9.1.1), with a new mesh (“Submodeling: overview,” Section 10.2.1; “Mesh-to-mesh solution mapping,” Section 12.4.1; and “Symmetric model generation,” Section 10.4.1), or with the same or a different Abaqus program (“Transferring results between Abaqus analyses: overview,” Section 9.2.1). History data The purpose of an analysis is to predict the response of a model to some form of external loading or to some nonequilibrium initial conditions. An Abaqus analysis is based on the concept of steps, which are described in the history data portion of the input file. (For more information on steps, see “Defining an analysis,” Section 6.1.2.) The history input data are combined within a step as needed to define the history of the analysis. Multiple steps can be defined in an analysis. Steps can be introduced simply to change the output requests or to change the loads, boundary conditions, analysis procedure, etc. There is no limit on the number of steps in an analysis. There are two kinds of steps in Abaqus: general response analysis steps, which can be linear or nonlinear; and, in Abaqus/Standard, linear perturbation steps . A general analysis step contributes to the response history of the system; a linear perturbation step allows the investigation of the linearized response of the system at any stage during the response history. The state at the end of a general step provides the initial conditions for the next step, making it easy to simulate consecutive loadings of a model, such as a dynamic response following a static preload or the loading of a product during its usage following a simulation of the manufacturing process. The optional history data described below prescribing the loading; boundary conditions; output controls; auxiliary controls; and, in Abaqus/Explicit, contact conditions are continued from one general analysis step to the next general analysis step unless modified. For example, the solution controls prescribed in a general analysis step in Abaqus/Standard will remain in effect for all subsequent general analysis steps until they are modified or reset. For linear perturbation steps only the output controls are continued from one linear perturbation step to the next if there are no intermediate general analysis steps and the output controls are not redefined . Similarly, conditions specified in an Abaqus/CFD analysis are continued from one step to the next unless modified. Input File Usage: Use the following option to begin a step definition: *STEP Use the following option to end a step definition: *END STEP Required history data The following history data must be included in an input file to define an analysis procedure: • Response type: An option to define the analysis procedure type must appear immediately after the beginning of the step definition. Abaqus can perform many types of analyses—linear or nonlinear, static or dynamic, etc. . The type of analysis can be changed from step to step. For example, in Abaqus/Standard a static preload can be analyzed first, then the response type can be changed to transient dynamic. In this way a linear or nonlinear dynamic analysis can be performed based on the conditions at the end of the static solution. Optional history data The following history data can be included as necessary: • Loading: Usually some form of external loading is defined. For example, concentrated or distributed loads can be applied (“Applying loads: overview,” Section 33.4.1), temperature changes leading to thermal expansion can be prescribed (“Thermal expansion,” Section 26.1.2), or contact conditions can be used to apply loads (“Contact interaction analysis: overview,” Section 35.1.1). The loading can be prescribed as a function of time (“Amplitude curves,” Section 33.1.2). This feature can be used to prescribe loadings such as the ground motion during a seismic event, known accelerations, or the temperature and pressure history during a transient in an engine. If an amplitude curve is not defined, Abaqus assumes either that the loading varies linearly over the step or that the load is applied instantaneously at the beginning of the step, depending on the chosen response type . • Boundary conditions: Boundary conditions can be added, modified, or removed during an analysis (“Boundary conditions,” Section 33.3). • Output control: Quantities such as stress, strain, reaction force, temperature, and energy are available as output. The output options are described in “Output to the data and results files,” Section 4.1.2, and “Output to the output database,” Section 4.1.3; and all of the output variables are listed in “Output variables,” Section 4.2. The available output files are described in “Output,” Section 4.1.1. • Contact: Contact surfaces and contact interactions can be added, modified, or removed as step-dependent history data during an Abaqus/Explicit analysis . • Auxiliary controls: You can overwrite the solution controls that are built into Abaqus. In some procedures these values are given in the procedure definition. More generally in Abaqus/Standard they are given by defining solution controls (“Commonly used control parameters,” Section 7.2.2). Solution controls for contact problems (“Adjusting contact controls in Abaqus/Standard,” Section 35.3.6; “Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit,” Section 38.2.2; or “Contact controls for general contact in Abaqus/Explicit,” Section 35.4.5) can also be defined. • Element and surface removal/reactivation: In Abaqus/Standard portions of the model can be removed or reactivated from step to step. See “Element and contact pair removal and reactivation,” Section 11.2.1. • Co-simulation: The steps in the Abaqus model must be defined such that the co-simulation fits entirely within a single Abaqus step. Further, there can be only one co-simulation in the Abaqus job. Including model or history data from an external file You can specify an external file that contains a portion of the Abaqus input file. This file can include model and history definition data, comment lines, and other references to external files. When a reference to an external file is encountered, Abaqus will immediately process the data within the specified file. When the end-of-file is reached, Abaqus will return to processing the original file. A maximum of five levels of nested external file references can be used. UNIX environment variables can be used to specify the file names. Input File Usage: *INCLUDE, INPUT=file_name Including an encrypted data file You can include an encrypted file by reference in an Abaqus input file or in another data file. When you refer to the encrypted file, you must also provide the file’s password. If the password is correct, Abaqus processes the data within the specified file as it would for an unencrypted external file. Material and connector behavior definitions within an encrypted input file are not written to the output database. In addition, all material and connector behavior definitions output to the data file are suppressed if an encrypted file is used as input for any portion of the model. See “Encrypting and decrypting Abaqus input data,” Section 3.2.32, for details about the encryption utility. Some encrypted files are eligible for inclusion only by users with a license for a particular Abaqus feature (such as Abaqus/Explicit) or to users at a particular site. If you attempt to include an encrypted file for which you do not have the proper privileges, Abaqus issues an error message. You cannot include encrypted input files that contain parametric input. Input File Usage: *INCLUDE, INPUT=file_name, PASSWORD=password 1.4 Parametric modeling • “Parametric input,” Section 1.4.1 1.4.1 PARAMETRIC INPUT Products: Abaqus/Standard Abaqus/Explicit References • “Scripting parametric studies,” Section 20.1.1 • “Parametric shape variation,” Section 2.1.2 • *PARAMETER • *PARAMETER DEPENDENCE • *PARAMETER SHAPE VARIATION • Chapter 4, “Introduction to Python,” of the Abaqus Scripting User’s Manual Overview The parametric input capability allows you to create an Abaqus input file in which: • Any number of input parameters is defined by assigning a value to each one of them. • The parameters defined in the input file are used in place of input quantities. • The parameters are evaluated according to their definition and are substituted for the parametrized input quantities before an analysis is run. Parametric input allows greater flexibility in building and manipulating models. The different kinds of parameters and the different ways of parametrizing the Abaqus input quantities are discussed in this section. Introduction You must define all the parameters you wish to use in an analysis by assigning a value to them. The Python language (Lutz, 1999) is used to perform parameter evaluation and substitution; hence, parameter definitions are required to follow the Python syntax rules discussed later in this section. These parameters can then be used in place of input quantities. Input File Usage: Use the following option to define parameters: *PARAMETER Use these parameters in place of input quantities by delimiting them with < >. For example, the following input defines the two parameters width and height, which are then used to define beam section properties: *PARAMETER width = 2.5 height = width*2 *BEAM SECTION, SECTION=RECT, ELSET=name, MATERIAL=name , In this simple example models with beams of different cross-sections can be obtained simply by changing the values of the parameters. Parameters Parameters are user-named variables to which you assign values. When a parameter is used instead of a value, the value of that parameter is substituted. There are two basic types of parameters: independent parameters and dependent parameters. Independent parameters Independent parameters are those that do not depend on any other parameters. The following are examples of independent parameters: thickness = 10.0 area = 5.0**2 length = 3.0*sin(45*pi/180.0) # convert degrees to radians Python expressions using numbers and numerical operations (such as addition, multiplication, and exponentiation) can be used to define independent parameters. Arithmetic support in Python is discussed later in this section. Dependent parameters Dependent parameters are those that depend on other parameters (dependent or independent). Dependent parameters can be defined in one of two ways: using a mathematical expression or using a tabular dependence. Expressional dependence Python parametric expressions involving operations between numbers and parameters are used to define expressionally dependent parameters. In the following example area and mom_inertia are dependent parameters: width = 2.0 height = 5.0 area = width*height mom_inertia = area*height**2/12.0 Tabular dependence Tabular dependence between parameters is defined by specifying the dependent and independent parameters as well as a dependence table. The table that defines the dependence between the parameters must have as many values per line as the number of dependent parameters plus the number of independent parameters for which it is going to be used. The table must contain only real values; dependent parameter values are given first, followed by independent parameter values. Parameter names and character strings cannot be used in a table. The evaluation of tabularly dependent parameters by interpolation between values in a table will result in these parameters being assigned real values. If it is necessary that the tabularly dependent parameters be integer numbers, the real numbers must be converted to integer numbers as described later in the Python language section. When the tabularly dependent parameters are functions of only one independent parameter, the tabular data must be given in order of increasing values of the independent parameter. Abaqus then interpolates linearly for values between those given. The dependent parameters are assumed to be constant outside the range of the independent parameters used in a table. When the tabularly dependent parameters depend on several independent parameters, the variation of the dependent parameters with respect to the first independent parameter must be given at fixed values of the other independent parameters, in ascending values of the second independent parameter, then of the third independent parameter, and so on. The table lines must always be ordered so that the independent parameters are given increasing values. This process ensures that the value of each dependent parameter is completely and uniquely defined for all values of the independent parameters. The fact that the definition of the dependence table is separate from the assignment of the dependence to particular parameters means that the same table can be used for multiple sets of dependent/independent parameters. This is useful when there are different instances of the same kind of input data; for example, multiple material definitions that use the same dependence but different sets of parameters. Because the evaluation of parameters is procedural , a parameter dependence table must always be defined before it is used to specify tabular parameter dependencies. Independent parameters in tabular dependence definitions are treated as independent for the purpose of defining this dependency; however, these “independent” parameters can be defined to depend on other parameters in a preceding parameter definition. Input File Usage: Use the following option to define a parameter dependence table: *PARAMETER DEPENDENCE, TABLE=name, NUMBER VALUES=n table with n values per line Use the following option to define the dependent and independent parameters that are used in the dependence table: *PARAMETER, TABLE=name, DEPENDENT=(parList), INDEPENDENT=(parList) Rules for parameters Some general rules apply to all parameters used in Abaqus input files. These rules are described in the following subsections. Parameter evaluation Parameters are evaluated by ordered execution of the parameter definitions as they appear in the input file. For example, the input *PARAMETER x = 2 y = x + 3 x = 4 gives x=4 and y=5, not x=4 and y=7. The input *PARAMETER y = x + 3 x = 4 is flagged as an error because y cannot be evaluated by ordered execution of the input. In other words, there is no deferred execution of the parameter definitions. It is possible to define parameters anywhere in the input file, even after parameters have been used in place of input quantities, since the parameter definitions are always processed before any other input options are processed. Parameters can also be defined and used in place of input quantities in an input file used for a restart analysis. However, parameters defined in the input file for the original analysis (from which the restart run is continued) are not available in the restart analysis. Parameter substitution When the parameterized data are processed, Abaqus assigns the parameter values as determined at the end of parameter evaluation. An error is reported if a parameter used in place of input quantities has not been assigned a value. Later, the analysis input file processor performs its usual checks on the validity of the parameter values with respect to the options in which they are being used. Data given to define a parameter, a parameter dependence table, or a parameter shape variation cannot be parameterized. For example, the input *PARAMETER SHAPE VARIATION is not valid; however, the analysis input file processor will not report an error for this input. Data types The data type of a parameter is deduced from its definition. An integer parameter results from assigning an integer literal value to the parameter. Similarly, a real parameter arises from assigning a real literal value to the parameter. Integers are promoted to reals if they are used in operations containing reals. A character string parameter results from assigning a character string literal value to the parameter. The input option context in which the parameter is used dictates the data type that the parameter must have. Parameters of real data type should be used in place of real Abaqus input quantities. Parameters of integer (or character string) type should be used in place of integer (or character string) type input quantities, respectively. In some instances, mismatches between the input context and the type of the substituted parameter will cause the analysis input file processor to flag these instances as input errors. For example, the input *PARAMETER int_pts = 5.0 *SHELL SECTION 10.0, will cause the analysis input file processor to report an error because the number of integration points specified for a shell section must be an integer. However, the input *PARAMETER thick = 5/4 *SHELL SECTION , will be accepted by the analysis input file processor without a warning being flagged; as a result of doing integer division, this input gives a shell thickness of 1 (not 1.25). In conclusion, you can rely on the analysis input file processor to catch only some data type errors. Continuous and discrete parameters From the point of view of design activities (sensitivity analysis, parametric studies, etc.) parameters can be continuous valued or discrete valued. A continuous-valued parameter is differentiable and can, thus, be used for design sensitivity analysis purposes. A discrete-valued parameter is not differentiable and can, thus, not be used for design sensitivity analysis purposes; however, it can be used for parametric studies. Examples of continuous-valued parameters may be a shell thickness or a material property. Examples of discrete-valued parameters may be the number of integration points through the thickness of a shell, or an element type. Continuous-valued parameters generally coincide with physical (design) input quantities, while discrete-valued parameters generally coincide with finite element (numerical approximation) input quantities. Auxiliary input files Parameters can be defined in *INCLUDE input files but not in any other auxiliary input files. Names of auxiliary input files can be parameterized, except those used in the *INCLUDE option. Parametrization of input quantities Abaqus treats parametrization of “size” and “shape” quantities somewhat differently. Parametrization of shape input quantities is discussed in a separate section . Size input quantities are understood to include all Abaqus input quantities except those that relate to shape. Size input quantities include section properties, material properties, orientation properties, prescribed conditions, interaction definitions and properties, and analysis procedure data. Parametrizing individual input quantities The following example shows the parametrization of shell section input using three independent parameters of differing data types: *ELSET, ELSET=, GEN 1, 111, 10 *PARAMETER shell_set = 'lining' shell_thick = 1.E2 num_int_pts = 5 *SHELL SECTION, ELSET=, MATERIAL=name , Parametrizing groups of input quantities (expressional dependence) The following example shows the parametrization of a three-layer composite shell section using expressional-dependent parameters. In this example the thickness parameter can be used to change the thickness of the layers of the composite section uniformly. *PARAMETER thickness = 10. layer1_thick = 0.15*thickness layer2_thick = 0.6*thickness layer3_thick = 0.25*thickness *SHELL SECTION, ELSET=, COMPOSITE ,num int pts, material name, orientation ,num int pts, material name, orientation ,num int pts, material name, orientation This parametrization requires that dependent parameters be created for the three input quantities (layer1_thick, layer2_thick, layer3_thick) that each depend on the independent parameter (thickness). Parametrizing groups of input quantities (tabular dependence) The following example shows the parametrization of the section properties of a box beam. The height and wall thicknesses of the beam section are parameters that depend tabularly on the section width. *PARAMETER a = 60. *PARAMETER DEPENDENCE, TABLE=sectprop, NUMBER VALUES=6 25.0, 1.04, 50.0, 4.17, 75.0, 9.38, *PARAMETER, TABLE=sectprop, DEPENDENT=(b, t1, t2, t3, t4), INDEPENDENT=(a) *BEAM SECTION, SECTION=BOX, ELSET=beams, MATERIAL=steel , , , , , 1.04, 1.04, 1.04, 50.0 3.13, 2.08, 2.50, 100.0 6.24, 3.13, 4.90, 150.0 The above parametrization creates dependent parameters (b, t1, t2, t3, t4) that each depend on the independent parameter (a). Usage of tabular dependence allows the definition of the dependencies of input quantities on parameters to be confined to the parameter definitions; i.e., separate from the options where parametrization of input quantities is done. An advantage of this method of parametrization is that the same parameter dependence table can be used for different parameters in different input options. For example, you may wish to use beams of different cross-section dimensions in different parts of the structure being modeled. The parameter dependence table can be reused with new dependent (bb, tt1, tt2, tt3, tt4) and independent (aa) parameters. *PARAMETER aa = 65. *PARAMETER, TABLE=sectprop, DEPENDENT=(bb, tt1, tt2, tt3, tt4), INDEPENDENT=(aa) *BEAM SECTION, SECTION=BOX, ELSET=columns, MATERIAL=steel , , , , , In options where predefined field variable dependence is supported, this method of parametrization provides a clear separation between predefined field variable dependence and parameter dependence; therefore, field variable and parameter dependence can never be confused. Consider, for example, the case of perfect plasticity properties for a metal where the yield stress depends on a field variable and is also parametrized to depend tabularly on the carbon content of the metal alloy. *PARAMETER carbon = 0.01 *PARAMETER DEPENDENCE, TABLE=yield_data, NUMBER=4 ys_fv1 val 1, ys_fv2 val 1, ys_fv3 val 1, carbon val 1 ys_fv1 val 2, ys_fv2 val 2, ys_fv3 val 2, carbon val 2 ys_fv1 val 3, ys_fv2 val 3, ys_fv3 val 3, carbon val 3 ys_fv1 val 4, ys_fv2 val 4, ys_fv3 val 4, carbon val 4 *PARAMETER, TABLE=yield_data, DEPENDENT=(ys_fv1, ys_fv2, ys_fv3), INDEPENDENT=(carbon) *MATERIAL, NAME=alloy *PLASTIC, DEPENDENCIES=1 , , , fv val 1 , , , fv val 2 , , , fv val 3 Consider, for example, the case of metal creep properties where the creep material data are parameters that depend tabularly on the carbon content of the metal alloy. In addition, one of the creep parameters, A, also depends on a predefined field variable. *PARAMETER carbon = 0.01 *PARAMETER DEPENDENCE, TABLE=creepdata, NUMBER=6 A_fv1 val 1, A_fv2 val 1, A_fv3 val 1, n val 1, m val 1, carbon val 1 A_fv1 val 2, A_fv2 val 2, A_fv3 val 2, n val 2, m val 2, carbon val 2 A_fv1 val 3, A_fv2 val 3, A_fv3 val 3, n val 3, m val 3, carbon val 3 A_fv1 val 4, A_fv2 val 4, A_fv3 val 4, n val 4, m val 4, carbon val 4 *PARAMETER, TABLE=creepdata, DEPENDENT=(A_fv1, A_fv2, A_fv3, n, m), INDEPENDENT=(carbon) *MATERIAL, NAME=alloy *CREEP, DEPENDENCIES=1 , , , , fv val 1 , , , , fv val 2 , , , , fv val 3 This example shows that any combination of dependencies on predefined field variables and/or dependent parameters can be defined. Python language Parameter statements in parameter definitions are required to follow the syntax and semantics of the Python language (note that the parameter dependence table and parameter shape variation definitions follow the usual Abaqus input syntax rules). The subset of the Python language that is endorsed is documented here. Statement length and continuation lines Python statements in parameter definitions can be continued over multiple lines by terminating each line with a backslash character (\). The *PARAMETER keyword lines can be continued onto the following line using a trailing comma since they are treated like other Abaqus keyword lines. Comments Comments in a parameter definition start with the number character (#) and continue to the end of the line. However, comments in a parameter dependence table or parameter shape variation definition are indicated by the usual Abaqus input syntax convention (**). Parameter names Parameter names must begin with a letter and can contain the underscore character (_) and numbers. Parameter names are case sensitive. Data types Data types are limited to character strings, integers, and reals. Strings are delimited with single or double quotation marks (’ ’ or ” ”). Backward single quotation marks (‘ ‘) are not permitted. Character strings should not contain the backslash character (\). Integers are created by assignment to integer literals (for example, aInt = 2). Reals are created by assignment to real literals (for example, aReal = 1.0). Real numbers can be given with or without an exponent. Any exponent must be preceded by E or e. The following line shows five acceptable ways of entering the same real number: -12.345, -1234.5E-2, -0.12345E+2, -0.12345E2, -0.12345e2 The syntax -0.12345D+2 (allowed elsewhere in the Abaqus input file) is not valid in Python. Type conversion If integers and reals are mixed in expressions, integers are promoted automatically to reals. Explicit type conversion can be obtained using: int(aReal) float(anInt) str(anIntOrReal) ’anIntOrReal’ aReal converted to integer type anInt converted to real type (float is the same as real) anIntOrReal converted to character string type anIntOrReal converted to character string type Numeric operators Standard support for operators is provided: − x + x x + y x − y x * y x / y x**y Functions x negated x unchanged sum of x and y difference of x and y product of x and y quotient of x and y x to the power y The following utility functions are supported: abs(x) acos(x) asin(x) atan(x) cos(x) log(x) log10(x) pow(x,y) absolute value of x arc cosine of x (result is in radians) arc sine of x (result is in radians) arc tangent of x (result is in radians) cosine of x (x is in radians) natural logarithm of x base 10 logarithm of x x to the power y (equivalent to x**y) sin(x) sqrt(x) tan(x) sine of x (x is in radians) square root of x tangent of x (x is in radians) Character string operators ’abc’ + ’def’ concatenation of character string ’abc’ and character string ’def’ Execution of parametrized input Jobs with parametrized input files are submitted to Abaqus in the usual way; for example, abaqus job=job-name input=input-file where it is assumed that an input file named input-file.inp exists. Abaqus searches input-file.inp and any *INCLUDE input files for parameter, parameter dependence table, and parameter shape variation (“Parametric shape variation,” Section 2.1.2) definitions, as well as parameter names inside < > that may have been used in place of input quantities. If any of the above are found, Abaqus will interpret the parametrized input file and perform the tasks of parameter evaluation and substitution. As a result, a modified input file that is free of parameter and parameter dependence table This file is named job-name.pes and is definitions and instances is produced. subsequently submitted for execution of an analysis. The execution procedure of a parametrized input file, except for the additional processing of parameter shape variation definitions in the analysis input file processor, does not differ from that of a non-parametrized input file. All the files generated by the parametrized input job will be named job-name with the appropriate extension appended to it. Parameter check jobs You can specify an execution mode in which only parameter processing (evaluation and substitution) is carried out. The parameter check execution mode is mutually exclusive of other execution modes, such as complete analysis, data check, continuation of a data check, conversion of results, or recovery . A parameter check run is useful in situations where you have defined complex parametrization in the input. In these cases you may want to study the results of parameter evaluation and substitution before proceeding further. A parameter check run does not permit continuation of the execution in a subsequent run; the job must be rerun from the beginning. Input File Usage: Enter the following input on the command line: abaqus job=job-name input=input-file parametercheck Display of parametric input Display of the results of parameter evaluation and substitution in the data file is described in this section. Visualization of parameter shape variations is described in “Parametric shape variation,” Section 2.1.2. Data file display The data (.dat) file contains information about the model definition generated by the analysis input file processor. You can control the amount of output generated by the analysis input file processor; see “Controlling the amount of analysis input file processor information written to the data file” in “Output,” Section 4.1.1, for details. In particular, you can specify whether or not the original input (.inp) file is echoed to the data file (by default, it is not). In the case of parametric input this file will generally contain a number of parameter, parameter dependence table, and parameter shape variation definitions, as well as a number of instances. To verify the definition of parametric input, you can create a modified version of the original input file showing the parameters and their values (this file is named job-name.par). You can also create the job-name.pes file, which is the modified version of the original input file that is free of parameter and parameter dependence table definitions, as well as instances. Input File Usage: Use the following option to print the contents of the job-name.par file to the data file: *PREPRINT, PARVALUES=YES Use the following option to print the contents of the job-name.pes file to the data file: *PREPRINT, PARSUBSTITUTION=YES Additional reference • Lutz, M., and D. Ascher, Learning Python, O’Reilly & Associates, Inc., 1999. Spatial Modeling Node definition Element definition Surface definition Rigid body definition Integrated output section definition Mass adjustment Nonstructural mass definition Distribution definition Display body definition Assembly definition Matrix definition SPATIAL MODELING 2.1 2.2 2.3 2.4 2.5 2.6 2.7 2.8 2.9 2.10 2.1 Node definition • “Node definition,” Section 2.1.1 • “Parametric shape variation,” Section 2.1.2 • “Nodal thicknesses,” Section 2.1.3 • “Normal definitions at nodes,” Section 2.1.4 • “Transformed coordinate systems,” Section 2.1.5 • “Adjusting nodal coordinates,” Section 2.1.6 2.1.1 NODE DEFINITION Products: Abaqus/Standard Abaqus/Explicit References • *NCOPY • *NFILL • *NGEN • *NMAP • *NODE • *NSET • *SYSTEM Overview This section describes the methods for defining nodes in an Abaqus input file. In a preprocessor such as Abaqus/CAE, you define the model geometry rather than the nodes and elements; when you mesh the geometry, the preprocessor automatically creates the nodes and elements needed for analysis. Although the concepts discussed in this section apply in general to the node definitions in the input file that is created by Abaqus/CAE, the methods and techniques described here apply only if you are creating the input file manually. Node definition consists of: • assigning a node number to the node; • optionally specifying a local coordinate system in which to define nodes; • defining individual nodes by specifying their coordinates; • grouping nodes into node sets; • creating nodes from existing nodes by generating them incrementally, by copying existing nodes, or by filling in nodes between the bounds of a region; and • mapping a set of nodes from one coordinate system to another. If any node is specified more than once, the last specification given is used. Abaqus will eliminate all unnecessary nodes before proceeding with the analysis. This feature is useful because it allows points to be defined as nodes for mesh generation purposes only. Assigning a node number to the node Each individual node must have a numeric label called the node number, which is assigned when the node is defined. The node number must be a positive integer, and the maximum node number allowed is 999999999 (for information on integer input, see “Input syntax rules,” Section 1.2.1). The nodes do not need to be numbered continuously. An Abaqus model can be defined in terms of an assembly of part instances . In such a model all nodes must belong to either a part, part instance, or, in the case of reference nodes, to the assembly. Node numbers must be unique within a part, part instance, or the assembly; but they can be repeated in different parts or part instances. Specifying a local coordinate system in which to define nodes Sometimes it is convenient to define nodal coordinates in a local coordinate system and then transform these coordinates to the global coordinate system. You can define a nodal coordinate system; Abaqus will translate and rotate the local ( ) coordinate values into the global coordinate system. The transformation is done immediately after input and will be applied to all nodal coordinates entered or generated after the nodal coordinate system is defined. The transformation affects only the input of nodal coordinates in node definitions. Nodal coordinate system definitions cannot be used • for applying loads and boundary conditions—see “Transformed coordinate systems,” Section 2.1.5, instead; or • for output of components of stress, strain, and element section forces—see “Orientations,” Section 2.2.5, instead. In addition to defining nodal coordinate systems, you can define individual nodes or node sets in local rectangular, cylindrical, or spherical systems . If a nodal coordinate system is in effect and you specify a local coordinate system for a particular node or node set definition, the input coordinates are first transformed according to the local system specified in the node definition and then according to the nodal coordinate system. Defining the nodal coordinate system You set up the coordinate system specification by specifying the global coordinates of three points in the local system: the origin of the local system (point a in Figure 2.1.1–1), a point on the local -axis (point b in Figure 2.1.1–1), and a point in the plane of the local system on (or near) the local -axis (point c in Figure 2.1.1–1). (global) (local) Figure 2.1.1–1 Nodal coordinate system. If only one point (the origin) is given, Abaqus assumes that you need a translation only. If only two points are given, the direction of the -axis will be projected onto the -axis will be the same as that of the Z-axis; that is, the plane. To change the nodal coordinate system that is in effect, define another nodal coordinate system; to revert to input in the global coordinate system, use a nodal coordinate system definition without any associated data. Input File Usage: Use the following option to define a nodal coordinate system: *SYSTEM , , , , , , , For example, in the following input, nodes 1 through 3 are defined in the first nodal coordinate system, nodes 4 and 5 are defined in the second nodal coordinate system, and nodes 6 and 7 are defined in the global coordinate system: *SYSTEM 0, 0, 0, 5, 5, 5 *NODE 1, 0, 0, 1 2, 0, 0, 2 3, 0, 1, 2 *SYSTEM 2, 3, 4 *NODE 4, 0, 0, 1 5, 1, 4, 0 *SYSTEM *NODE 6, 1, 0, 1 7, 0, 4, 2 Defining a nodal coordinate system within part definitions When you define a nodal coordinate system within a part (or part instance) definition, it is in effect only within that part (or part instance) definition. Nodes defined in other parts are not affected. You specify the local ( ) coordinate values relative to the part coordinate system, which subsequently may be translated and/or rotated according to the positioning data given for the instance . Defining individual nodes by specifying their coordinates You can define individual nodes by specifying the node number and the coordinates that define the node. Abaqus uses a right-handed, rectangular Cartesian coordinate system for all nodes except for axisymmetric models, when the coordinates of the nodes must be given as the radial and axial positions. For more information about direction definitions, see “Conventions,” Section 1.2.2. In a model defined in terms of an assembly of part instances, give nodal coordinates in the local coordinate system of the part (or part instance). See “Defining an assembly,” Section 2.10.1. Input File Usage: *NODE Reading node definitions from a file Node definitions can be read into Abaqus from an alternate file. The syntax of such file names is described in “Input syntax rules,” Section 1.2.1. Input File Usage: *NODE, INPUT=file_name Specifying a local coordinate system for the nodal coordinates You can specify that a local rectangular Cartesian, cylindrical, or spherical coordinate system be used for a particular node definition. These coordinate systems are shown in Figure 2.1.1–2. (X,Y,Z) Rectangular Cartesian (default) (R,θ,Z) (R,θ, φ) Cylindrical (θ and φ are given in degrees) Spherical Figure 2.1.1–2 Coordinate systems. This coordinate system specification is entirely local to the node definition. As the nodal data are read, the coordinates are transformed to rectangular Cartesian coordinates immediately. If a nodal coordinate system is also in effect , these are local rectangular Cartesian coordinates as defined by the nodal coordinate system, which are subsequently transformed to global Cartesian coordinates. Input File Usage: Use the following option to specify the nodal coordinates in a rectangular Cartesian system (this is the default): *NODE, SYSTEM=R Use the following option to specify the nodal coordinates in a cylindrical system: *NODE, SYSTEM=C Use the following option to specify the nodal coordinates in a spherical system: the following lines define node number 1 with coordinates *NODE, SYSTEM=S For example, (10cos20°, 10sin20°, 5.) in a local cylindrical system (R, *NODE, NSET=DISC, SYSTEM=C 1, 10., 20., 5. , Z): If the following lines appeared in the input file before the above node definition, the coordinates of node 1 would be transformed first to rectangular Cartesian coordinates in the nodal coordinate system defined by the *SYSTEM option and then to coordinates in the global system: *SYSTEM 2, 0, 2 Grouping nodes into node sets Node sets are used as convenient cross-references when defining loads, constraints, properties, etc. Node sets are the fundamental references of the model and should be used to assist the input definition. The members of a node set can be individual nodes or other node sets. An individual node can belong to several node sets. Nodes can be grouped into node sets when they are created or after they have already been defined. In either case each node set is assigned a name. Node set names can be up to 80 characters long. The same name can be used for a node set and for an element set. By default, the nodes within a node set will be arranged in ascending order, and duplicate nodes will be removed. Such a set is called a sorted node set. You may choose to create an unsorted node set as described later, which is often useful for features that match two or more node sets. For example, if you define multi-point constraints (“General multi-point constraints,” Section 34.2.2) between two node sets, a constraint will be created between the first node in Set 1 and the first node in Set 2, then between the second node in Set 1 and the second node in Set 2, etc. It is important to ensure that the nodes are combined in the desired way. Therefore, it is sometimes better to specify that a node set be stored in unsorted order. Once nodes are assigned to a node set, additional nodes can be added to the same node set; however, nodes cannot be removed from a node set. Creating an unsorted node set You can choose to assign nodes to a new node set (or to add nodes to an existing node set) in the order in which they are given. The node numbers will not be rearranged, and duplicates will not be removed. This unsorted node set will affect node copies, node fills, linear constraint equations, multi-point constraints, and substructure nodes associated with retained degrees of freedom. An unsorted node set can be created only by directly defining an unsorted node set as described here or by copying an unsorted node set. Any additions or modifications to a node set using other means will result in a sorted node set. Input File Usage: *NSET, NSET=name, UNSORTED Assigning nodes to a node set as they are created There are several ways that nodes can be assigned to node sets as they are created. Input File Usage: Use any of the following options: *NODE, NSET=name *NCOPY, NEW SET=name *NFILL, NSET=name *NGEN, NSET=name *NMAP, NSET=name Assigning previously defined nodes to a node set You can assign nodes that you have defined previously (by specifying their coordinates, by filling in nodes between two bounds, or by generating them incrementally) to a node set by listing the nodes forming the set directly, by generating the node set, or by generating a node set from an element set. Listing the nodes that define the set directly You can list the nodes that form a node set directly. Previously defined node sets, as well as individual nodes, can be assigned to node sets. Input File Usage: *NSET, NSET=name For example, the following lines add nodes 1, 3, 10, 11, and all the nodes in set A11 to set A12: *NSET, NSET=A12 1, 3 10, 11, A11 Node set A11 can be assigned to node set A12 only if the definition of A11 occurs before the definition of A12. All the nodes in node set A12 will be sorted into ascending numerical order. If the UNSORTED parameter were included on the *NSET option, node set A12 would contain the nodes in the order in which they are specified on the data lines. Generating the node set To generate a node set, you must specify a first node, numbers between these nodes, i. All nodes going from set. Therefore, i must be an integer such that is . ; a last node, to ; and the increment in node in increments of i will be added to the is a whole number (not a fraction). The default Input File Usage: *NSET, NSET=name, GENERATE For example, the following lines add all nodes from 100 to 120 in increments of 10 to set A13: *NSET, NSET=A13, GENERATE 100, 120, 10 Generating a node set from an element set You can specify the name of a previously defined element set (“Element definition,” Section 2.2.1), in which case the nodes that define the elements contained in this element set will be assigned to the specified node set. This method can be used only to define sorted node sets. Input File Usage: *NSET, NSET=name, ELSET=name For example, the following lines add all nodes that define elements 50 and 100 (nodes 1, 2, 3, and 4) to node set A14: *ELEMENT, TYPE=B21 50, 1, 2 100, 3, 4 *ELSET, ELSET=B1 50, 100 *NSET, NSET=A14, ELSET=B1 Element set B1 can be assigned to node set A14 since the definition of B1 occurs before the definition of A14. Limitation on updating node sets that are used to define other node sets If a node set is constructed from previously defined node sets, subsequent updates to these sets are not taken into account. Input File Usage: *NSET, NSET=name For example, the following lines add nodes 1 and 2, but not 3, to the set SET-AB while adding nodes 1 and 3 to set SET-A: *NSET, NSET=SET-A 1, *NSET, NSET=SET-B 2, *NSET, NSET=SET-AB SET-A, SET-B *NSET, NSET=SET-A 3, Defining part and assembly sets In a model defined in terms of an assembly of part instances, all node sets must be defined within a part, part instance, or the assembly definition. If a node set is defined within a part (or part instance) definition, you can refer to the node numbers directly. To define an assembly-level node set, you must identify the nodes to be added to the set by prefixing each node number with the part instance name and a “.” (as explained in “Defining an assembly,” Section 2.10.1). An assembly-level node set can have the same name as a part-level node set. Example The following input defines a node set, set1, that belongs to part PartA and will be inherited by every instance of PartA: *PART, NAME=PartA ... *NSET, NSET=set1 1,3,26,500 *END PART A node set with the same name is defined at the assembly level as follows: *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=PartA-1, PART=PartA ... *END INSTANCE *INSTANCE, NAME=PartA-2, PART=PartA ... *END INSTANCE *NSET, NSET=set1 PartA-1.1, PartA-1.3, PartA-1.26, PartA-1.500 PartA-2.1, PartA-2.3, PartA-2.26, PartA-2.500 *END ASSEMBLY Assembly-level node set set1 contains all the nodes from node sets set1 belonging to part instances PartA-1 and PartA-2. Therefore, the nodes are assigned to two separate node sets: one at the part instance level and one at the assembly level. An assembly-level node set called set1 could be created with entirely different nodes than those that belong to the part set; part- and assembly-level node sets assembly-level node sets set1, the assembly-level set could alternatively be defined by NODE DEFINITION *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=PartA-1, PART=PartA ... *END INSTANCE *INSTANCE, NAME=PartA-2, PART=PartA ... *END INSTANCE *NSET, NSET=set1 PartA-1.set1, PartA-2.set1 *END ASSEMBLY This node set definition is equivalent to the previous example, where the nodes are listed individually. Alternate method for defining assembly-level node sets Sometimes it is not convenient to define an assembly-level node set by referring to part-level node sets. In such cases a set definition containing many nodes can get quite lengthy. Therefore, an alternate method is provided. Input File Usage: *NSET, NSET=NsetName, INSTANCE=InstanceName The following example shows two equivalent ways to define an assembly-level node set; once by prefixing each node number with a part instance name (as shown above) and once using the more compact INSTANCE notation: *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=PartA-1, PART=PartA ... *END INSTANCE *INSTANCE, NAME=PartA-2, PART=PartA ... *END INSTANCE *NSET, NSET=set2 PartA-1.11, PartA-1.12, PartA-1.13, PartA-1.14, PartA-2.21, PartA-2.22, PartA-2.23, PartA-2.24 *NSET, NSET=set3, INSTANCE=PartA-1 11, 12, 13, 14 *NSET, NSET=set3, INSTANCE=PartA-2 21, 22, 23, 24 *END ASSEMBLY When the *NSET option is used more than once with the same name, as it is with set3, the nodes in the second use of *NSET are appended to the set created by the first use of *NSET. Internal node sets created by Abaqus/CAE In Abaqus/CAE many modeling operations are performed by picking geometry with the mouse. For example, a concentrated load can be applied by picking a point on a geometric part instance. Since the *CLOAD option refers to a node set, this “picked” geometry must be translated into a node set in the input file. Such sets are assigned a name by Abaqus/CAE and marked as internal. You can view these internal sets using display groups in the Visualization module of Abaqus/CAE . Input File Usage: *NSET, NSET=NsetName, INTERNAL Transferring of node sets If the results of an Abaqus/Explicit analysis are imported into an Abaqus/Standard analysis (or vice versa) or results from an Abaqus/Standard analysis are imported into another Abaqus/Standard analysis , all node set definitions in the original analysis are imported by default. Alternatively, you can import only selected node set definitions; see “Importing element set and node set definitions” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details. If a three-dimensional model is generated from a symmetric model , all node sets in the original model will be used (and expanded) in the generated model. Creating nodes from existing nodes by generating them incrementally You can generate nodes incrementally from existing nodes. All of the nodes along a straight or curved line can be generated by giving the coordinates of the two end nodes and defining the type of curve. The two end nodes must already be defined, usually by specifying their coordinates, but it is also possible to have them defined by an earlier generation. Defining a straight line between the two end nodes To define a straight line between the two end nodes, specify the number of the first end node, number of the last end node, i. Therefore, i must be an integer such that is ; the ; and the increment in node numbers between each node along the line, is a whole number (not a fraction). The default . Input File Usage: *NGEN For example, in the following input node number 1 with coordinates (0., 0., 0.) and node number 6 with coordinates (10., 0., 0.) are defined and nodes 2, 3, 4, and 5 with coordinates (2., 0., 0.), (4., 0., 0.), (6., 0., 0.), and (8., 0., 0.), respectively, are generated automatically: *NODE 1, 0., 0., 0. 6, 10., 0., 0. 1, 6, 1 Defining a circular arc between the two end nodes NODE DEFINITION To define a circular arc between the two end nodes, specify the number of the first end node, number of the last end node, i. Therefore, i must be an integer such that is ; the ; and the increment in node numbers between each node along the arc, is a whole number (not a fraction). The default . In addition, you must specify the coordinates of one extra point, the center of the circle, either by giving the node number of a node that has already been defined or by giving the nodal coordinates directly. If both are supplied, the node number will take precedence over the coordinates. If the coordinates are defined directly, they can be specified in a local coordinate system as described later. The coordinates of the end nodes will be adjusted radially if the circle cannot be passed through both points. An arc of a circle of 180° through 360° will require more extensive definition. For this case you must define the plane of the circular disc by giving the normal to the disc; the nodes will then be numbered according to the right-hand rule about this normal. Input File Usage: *NGEN, LINE=C Defining a parabola between the two end nodes To define a parabola between the two end nodes, specify the number of the first end node, of the last end node, Therefore, i must be an integer such that ; the number ; and the increment in node numbers between each node along the parabola, i. is a whole number (not a fraction). The default is . In addition, you must specify the coordinates of one extra point, the midpoint on the arc between the two end points, either by giving the node number of a node that has already been defined or by giving the nodal coordinates directly. If both are supplied, the node number will take precedence over the coordinates. If the coordinates are defined directly, they can be specified in a local coordinate system as described later. Input File Usage: *NGEN, LINE=P Defining the extra point and the normal direction in a local coordinate system You can specify the coordinates of the extra point that is required for a circle or a parabola in a local rectangular Cartesian system, a cylindrical system, or a spherical system. These coordinate systems are shown in Figure 2.1.1–2. If a nodal coordinate system is in effect , the coordinates and normal direction specified in the node definition are assumed to be in the nodal coordinate system. If a nodal coordinate system is in effect and you specify the extra point for a circle or parabola in a local coordinate system, the input is first transformed according to the local system specified in the node definition and subsequently according to the nodal coordinate system. Input File Usage: Use the following option to specify the extra point in a rectangular Cartesian system (this is the default): *NGEN, SYSTEM=RC Use the following option to specify the extra point in a cylindrical system: *NGEN, SYSTEM=C Use the following option to specify the extra point in a spherical system: *NGEN, SYSTEM=S Creating nodes by copying existing nodes You can create new nodes by copying existing nodes. The coordinates of the new nodes can be translated and rotated, reflected from the nodes being copied, or projected from the nodes being copied by using a polar projection with respect to a pole node. You must identify the existing node set to copy and specify an integer constant, n, that will be added to the node numbers of existing nodes to define node numbers for the nodes being created. You can assign the newly created nodes to a node set. If you do not specify a node set name for the newly created nodes, they are not assigned to a node set. Input File Usage: *NCOPY, OLD SET=name, CHANGE NUMBER=n, NEW SET=new_name Translating and rotating the coordinates of the old nodes You can create new nodes by translating and/or rotating the nodes in the old node set . You specify the value of the translation in the X-, Y-, and Z-directions. In addition, you specify the coordinates of the first point defining the rotation axis (point a in Figure 2.1.1–3), the coordinates of the second point defining the rotation axis (point b in Figure 2.1.1–3), and the angle of rotation (in degrees) about the a–b axis. The rotation can be applied multiple times as described later. If you specify both translation and rotation, the translation is applied once before the rotation. Input File Usage: *NCOPY, OLD SET=name, CHANGE NUMBER=n, SHIFT Applying the rotation multiple times You can specify the number of times the rotation should be applied, m. For example, if nodes are to be created at angles of 30°, 60°, and 90°, set m=3. The identifiers of the nodes created are incremented sequentially by the value of n, as described above. Input File Usage: *NCOPY, OLD SET=name, CHANGE NUMBER=n, SHIFT, MULTIPLE=m Reflecting the coordinates of the old nodes You can create new nodes by reflecting the coordinates of the old nodes through a line, a plane, or a point. Figure 2.1.1–3 Translation and rotation of existing nodes. Reflecting the coordinates through a line To reflect the old nodal coordinates through a line, you specify the coordinates of points a and b . Input File Usage: *NCOPY, OLD SET=name, CHANGE NUMBER=n, REFLECT=LINE Old set New Set a, b define the line Figure 2.1.1–4 Reflection of coordinates through a line. Reflecting the coordinates through a plane To reflect the old nodal coordinates through a plane, you specify the coordinates of points a, b, and c . Input File Usage: *NCOPY, OLD SET=name, CHANGE NUMBER=n, REFLECT=MIRROR New Set Old Set a, b, c define the mirror plane Figure 2.1.1–5 Reflection of coordinates through a plane. Reflecting the coordinates through a point To reflect the old nodal coordinates through a point, you specify the coordinates of point a . Input File Usage: *NCOPY, OLD SET=name, CHANGE NUMBER=n, REFLECT=POINT Projecting the nodes in the old set from a pole node You can create new nodes by projecting the nodes in the old set from a pole node. Each new node will be located such that the corresponding old node is equidistant between the pole node and the new node. The pole node is identified by giving its number or, alternatively, its coordinates. This method is particularly useful for creating nodes that are associated with infinite elements (“Infinite elements,” Section 28.3.1). In this case the pole node should be located at the center of the far-field solution. Input File Usage: *NCOPY, OLD SET=name, CHANGE NUMBER=n, POLE New Set Old set a is the point through which the nodes are reflected Figure 2.1.1–6 Reflection of coordinates through a point. pole node old set new set Figure 2.1.1–7 Projection of existing nodes from a pole node. Creating nodes by filling in nodes between two bounds You can create nodes by filling in nodes between two bounds. In this case you specify the two node sets whose members form the bounds, the number of intervals along each line between the bounding nodes, and the increment in node numbers from the node number at the first bound set end. Let l equal the number of lines of nodes to be created between the two bounding node sets; the number of intervals along each line between the bounding nodes is then given by . node ( must be numbered such that Let n equal the increment in node numbers from the node number at the first bound set end; for each ) in the first bounding node set, the corresponding node in the other bounding node set ( ) is a whole number. The node sets that define the bounds of the region are used as they exist at the time the node fill definition appears in the input file: only those nodes that have been added to the sets prior to the node fill definition are used. Both sorted and unsorted node sets can be used. Nodes that have not yet been given coordinates are assumed to be at the origin, (0.,0.,0.). The nodes created by this method lie on straight lines between corresponding nodes in the two sets. If the sets do not have the same number of nodes, the extra nodes in the longer set are ignored. By default, the spacing between nodes along the lines is uniform. Input File Usage: *NFILL Example For example, Figure 2.1.1–8 shows a simple quarter-cylinder model. OUTSIDE A 6501 OUTSIDE B 6101 INSIDE B 6105 6505 1501 1101 INSIDE A 1105 1505 Figure 2.1.1–8 Filling a three-dimensional region. The quarter circles INSIDEA (nodes 1101–1105), OUTSIDEA (nodes 1501–1505), INSIDEB (nodes 6101–6105), and OUTSIDEB (6501–6505) have already been defined by specifying their coordinates the nodes on those planes into sets A and B and then filling between those sets with the following options: NODE DEFINITION *NFILL, NSET=A INSIDEA, OUTSIDEA, 4, 100 *NFILL, NSET=B INSIDEB, OUTSIDEB, 4, 100 *NFILL A, B, 5, 1000 Concentrating the nodes toward one bound or the other You can concentrate the nodes toward one bound or the other by specifying b, the ratio of adjacent distances between nodes along each line of nodes generated as the nodes go from the first bounding node set to the second. Thus, if b is less than one, the nodes are concentrated toward the first bounding node set; if b is greater than one, the nodes are concentrated toward the second bounding set. The value of b must be positive. The bias intervals along the line from the first bounding node are L, , … (where L is the length of the first interval). In Abaqus/Standard the bias value can be applied at every interval along the line or at every second interval along the line as described later. , , , , Input File Usage: *NFILL, BIAS=b Example For example, suppose the lines of nodes shown in Figure 2.1.1–9 have already been generated by other methods and placed into node sets INSIDE and OUTSIDE. The following option will fill the region as shown in Figure 2.1.1–10: *NFILL, BIAS=0.6 INSIDE, OUTSIDE, 5, 100 Applying the bias value at every second interval along the line In Abaqus/Standard you can apply the bias value at every second interval along the line. In this case the nodes will be positioned along the line correctly for use with second-order elements, so that the midside nodes are at the middle of the interval between the corner nodes of the elements. The bias intervals along the line from the first bounding node are L, L, , … , , , (where L is the length of the first interval). Input File Usage: *NFILL, BIAS=b, TWO STEP Creating quarter-point spacing In Abaqus/Standard you can create quarter-point spacing for fracture mechanics calculations with second-order isoparametric elements (“Fracture mechanics: overview,” Section 11.4.1). This spacing 105 104 103 102 101 605 604 603 602 601 Inside Outside Figure 2.1.1–9 Node sets defining bias example. 5 0 4 105 4 0 4 3 0 4 2 0 4 104 103 3 0 3 2 0 3 4 0 3 5 0 3 202 302 402 502 201 301 401 501 102 101 605 604 603 602 601 Figure 2.1.1–10 Result of bias example. gives a square root singularity in the strain field at the crack tip by placing the first node away from that point at one-quarter of the distance to the second point. The remaining nodes on each line are spaced so that the size of the elements will grow as the square of the distance from the singularity, with the midside nodes exactly at the midsides of the elements. This spacing produces a reasonable mesh gradation for this type of problem; however, better results can be obtained for crude meshes by making the size of the crack element smaller than the quarter-point spacing technique does. Input File Usage: *NFILL, SINGULAR Example Figure 2.1.1–11 shows a simple fracture mechanics example. 507 506 505 504 503 Node set TOP 107 106 105 104 103 Node set MID 108 109 102 101 Nodes 101-109 in node set OUTER Nodes 1-9 at crack tip (node set TIP) Figure 2.1.1–11 Node fill used in a singular problem. (The mesh shown is very coarse, and a finer mesh would probably be used in an actual case.) The nodes on the top edge have been placed in node set TOP, those on the horizontal line at the upper end of the focused region are in node set MID, all of the nodes around the focused region are in node set OUTER, and there are multiple nodes at the crack tip in node set TIP. The following options are used to fill in the region as shown in Figure 2.1.1–12 (note the quarter-point nodes adjacent to the crack tip): *NFILL, BIAS=0.8 MID, TOP, 4, 100 *NFILL, SINGULAR=1 TIP, OUTER, 5, 20 Mapping a set of nodes from one coordinate system to another You can map a set of nodes from one coordinate system to another. You can also rotate, translate, or scale the nodes in a set by using a more direct method instead of coordinate system mapping. These capabilities 503 403 303 203 103 102 101 82 22 62 42 21 41 61 81 Figure 2.1.1–12 Node fill used in a singular problem. are useful for many geometric situations: a mesh can be generated quite easily in a local coordinate system (for example, on the surface of a cylinder) using other methods and then can be mapped into the global (X, Y, Z) system. In other cases some parts of your model need to be translated or rotated along a given axis or scaled with respect to one point. The mapping capability cannot be used in a model defined in terms of an assembly of part instances. The following different mappings are provided: a simple scaling; a simple shift and/or rotation; skewed Cartesian; cylindrical; spherical; toroidal; and, in Abaqus/Standard only, blended quadratic. The first five of these mappings are shown in Figure 2.1.1–13. Blended quadratic mapping is shown in Figure 2.1.1–14. In all cases the coordinates of the nodes in the set are assumed to be defined in the local system: these local coordinates at each node are replaced with the global Cartesian (X, Y, Z) coordinates defined by the mapping. All angular coordinates should be given in degrees. You can use either coordinates or node numbers to define the new coordinate system, the axis of rotation and translation, or the reference point used for scaling. The mapping capability can be used several times in succession on the same nodes, if required. Scaling the local coordinates before they are mapped For all mappings except the blended quadratic mapping, you can specify a scaling factor to be applied to the local coordinates before they are mapped. This facility is useful for “stretching” some of the coordinates that are given. For example, in cases where the local system uses some angular coordinates and some distance coordinates (cylindrical, spherical, etc.), it may be preferable to generate the mesh in a system that uses distance measures in the angular directions and then scale onto the angular coordinate system for the mapping. Two different scaling methods are available. ^ ^ ^ ^ ^ ^ rectangular skewed Cartesian ^ (R, θ, φ) (θ = 0) (φ = 0) ^ (R, θ, Z) (θ = 0) spherical cylindrical (r, θ, φ) b (φ = 0) φ toroidal Figure 2.1.1–13 Coordinate systems; angles are in degrees. 5134 136 138 5126 10134 10136 10138 10130 5138 10001 10126 10124 10122 5122 134 130 126 124 122 ORIGINAL CONFIGURATION 10134 10136 5134 10130 5138 10138 10001 134 136 138 10126 10124 130 126 5126 10122 5122 124 122 MAPPED CONFIGURATION Figure 2.1.1–14 Use of blended quadratic mapping to develop a solid mesh onto a curved block. Specifying the scaling factors directly A first method of scaling the nodes with respect to the origin of the local system is to specify the scale factors directly. In this case the scaling is done at the same time as the mapping from one coordinate system to another. Input File Usage: *NMAP, NSET=name first data line second data line scale factor for first local coord, scale factor for second local coord, scale factor for third local coord Specifying the scaling with respect to a reference point Alternatively, you can scale with respect to a point other than the origin. The reference point with respect to which the scaling is done can be defined by using either its coordinates or the user node number. Input File Usage: Use the following option to define the scaling reference point by using its coordinates (default): *NMAP, TYPE=SCALE, DEFINITION=COORDINATES X-coordinate of reference point, Y-coordinate of reference point, Z-coordinate of reference point scale factor for first local coord, scale factor for second local coord, scale factor for third local coord Use the following option to define the scaling reference point by using its node number: *NMAP, TYPE=SCALE, DEFINITION=NODES Local node number of the reference point scale factor for first local coord, scale factor for second local coord, scale factor for third local coord Introducing a simple shift and/or rotation by mapping from one coordinate system to another In the case of a simple shift and/or rotation, point a in Figure 2.1.1–13 defines the origin of the local rectangular coordinate system defining the map. The local -axis is defined by the line joining points a and b. The local – plane is defined by the plane passing through points a, b, and c. Input File Usage: *NMAP, NSET=name, TYPE=RECTANGULAR Introducing a pure shift by specifying the axis and magnitude of the translation You can define a pure translation (or shift) to move a set of nodes by a prescribed value along a desired axis. You must specify the axis of translation by providing either the coordinates or the two node numbers defining this axis, and you must prescribe the magnitude of the translation. Input File Usage: Use the following option to specify the axis of translation using coordinates (default): *NMAP, NSET=name, TYPE=TRANSLATION, DEFINITION=COORDINATES Use the following option to specify the axis of translation using node numbers: *NMAP, NSET=name, TYPE=TRANSLATION, DEFINITION=NODES Introducing a pure rotation by specifying the axis, origin, and angle of the rotation You can define a rotation of a set of nodes by providing the axis of rotation, the origin of rotation, and the magnitude of the rotation. You must specify the axis of rotation by providing either the coordinates or the two node numbers defining this axis. You must specify the origin of the rotation by providing either the coordinates or the node number at the origin of rotation. Finally, you must specify the angle of the rotation in degrees. Input File Usage: Use the following option to specify the axis of rotation using coordinates (default): *NMAP, NSET=name, TYPE=ROTATION, DEFINITION=COORDINATES Use the following option to specify the axis of rotation using node numbers: *NMAP, NSET=name, TYPE=ROTATION, DEFINITION=NODES Mapping from cylindrical coordinates For mapping from cylindrical coordinates, point a in Figure 2.1.1–13 defines the origin of the local cylindrical coordinate system defining the map. The line going through point a and point b defines the -axis of the local cylindrical coordinate system. The local – plane for is defined by the plane passing through points a, b, and c. Input File Usage: *NMAP, NSET=name, TYPE=CYLINDRICAL Mapping from skewed Cartesian coordinates For mapping from skewed Cartesian coordinates, point a in Figure 2.1.1–13 defines the origin of the local diamond coordinate system defining the map. The line going through point a and point b defines the -axis of the local coordinate system. The line going through point a and point c defines the -axis of the local coordinate system. The line going through point a and point d defines the -axis of the local coordinate system. Input File Usage: *NMAP, NSET=name, TYPE=DIAMOND Mapping from spherical coordinates For mapping from spherical coordinates, point a in Figure 2.1.1–13 defines the origin of the local spherical coordinate system defining the map. The line going through point a and point b defines the polar axis of the local spherical coordinate system. The plane passing through point a and perpendicular to the polar axis defines the plane. The plane passing through points a, b, and c defines the local plane. Input File Usage: *NMAP, NSET=name, TYPE=SPHERICAL Mapping from toroidal coordinates For mapping from toroidal coordinates, point a in Figure 2.1.1–13 defines the origin of the local toroidal coordinate system defining the map. The axis of the local toroidal system lies in the plane defined by points a, b, and c. The R-coordinate of the toroidal system is defined by the distance between points a and b. The line between points a and b defines the the -coordinate is defined in a plane perpendicular to the plane defined by the points a, b, and c and perpendicular to the axis of the toroidal system. lies in the plane defined by the points a, b, and c. position. For every value of Input File Usage: *NMAP, NSET=name, TYPE=TOROIDAL Mapping by means of blended quadratics To map by means of blended quadratics in Abaqus/Standard, you define the new (mapped) coordinates of up to 20 “control nodes”: these are the corner and midedge nodes of the block of nodes being mapped. The mapping in this case is like that of a 20-node brick isoparametric element. Any of the midedge nodes can be omitted, thus allowing linear interpolation along that edge of the block. Abaqus/Standard does not check whether the nodes in the set lie within the physical space of the block defined by the corner and midedge nodes: these control nodes simply define mapping functions that are then applied to all of the nodes in the set. The control nodes should define a “well”-shaped block; for example, midedge nodes should be close to the midpoint of the edge. Otherwise, the mapping can be very distorted. For example, the nodes of a crack-tip 20-node element with midside nodes at the quarter points will not map correctly and, therefore, should not be used as the control nodes. Blended mapping is only available for three-dimensional analyses. Input File Usage: *NMAP, NSET=name, TYPE=BLENDED 2.1.2 PARAMETRIC SHAPE VARIATION Products: Abaqus/Standard Abaqus/Explicit References • “Parametric input,” Section 1.4.1 • *PARAMETER SHAPE VARIATION Overview Shape parametrization can be accomplished in an Abaqus input file by: • parametrizing nodal coordinates; or • relating nodal coordinates to shape parameters using shape variations. The different approaches to shape parametrization are described in this section. Parametrization of nodal coordinates Any individual nodal coordinates can be parametrized directly. This is usually of limited value because it often leads to designs with irregular shape that cannot be manufactured easily. In addition, parametrization of individual nodal coordinates generally requires an excessive number of parameters to define the parametrized shape. Parametrization of nodal coordinates used in conjunction with node generation in Abaqus provides a more practical method of shape parametrization. However, this method is still of somewhat limited practical use because the simple node generation capabilities available in Abaqus cannot describe complex shapes. Direct parametrization of individual nodal coordinates The simplest form of parametrization of nodal coordinates is to define individual parameters and use them in place of the nodal coordinates to be parametrized, as described in “Parametric input,” Section 1.4.1. For example, *PARAMETER x_coord_node_1 = 10. y_coord_node_1 = 20. *NODE 1, , Parametrization of nodal coordinates using node generation Shape parametrization can be accomplished by parametrizing the coordinates of some nodes, then using these nodes to generate other nodes and their coordinates. For example: *PARAMETER x_coord_node_1 = 10. x_coord_node_11 = 20. *NODE 1, , 50. 11, , 50. *NGEN 1, 11, 1 This method of shape parametrization reduces the number of user-defined parameters necessary for shape parametrization by implicitly making the nodal coordinates of the generated nodes dependent on the shape parameters. Shape change by linear combination of shape variations The definition of shape in Abaqus includes a basic shape plus any number of additional shape variations that are added to the basic shape using a linear combination. Mathematically, we can express the nodal coordinates, , as is the basic shape, where shape parameter. shape variation, and This calculation is always done in the global rectangular Cartesian coordinate system. Although it is not necessarily so, it is frequently the case that the input to define a shape variation is simply the gradient of the basic shape taken with respect to the corresponding shape parameter. is the value of the is the You specify the basic shape of a model in the Abaqus input file by providing nodal definitions either directly or through node generation; see “Node definition,” Section 2.1.1. You can specify shape variations and associated shape parameters, as described here. In addition, you can specify perturbations of the shape as a linear combination of other shapes (for example, buckling mode shapes); see “Introducing a geometric imperfection into a model,” Section 11.3.1. The definition of the nodal coordinates for a model in the Abaqus input file is then possible using a combination of four types of methods: • You can directly define individual nodes and their respective coordinates; these coordinates are part of the definition of the basic shape, , and can be parametrized. • Node generation can be used to create nodes and their coordinates according to geometrically simple mappings that rely on existing node definitions; these generated coordinates are also part of the definition of the basic shape, . If necessary, the node generation input can be parametrized. • Parameter shape variations can be used to vary the coordinates of nodes defined using the above methods. • Geometric imperfections can be used to perturb nodal coordinates previously defined using any combination of the above three types of methods. Shape parametrization using shape variations Instead of parametrizing nodal coordinates directly, you can specify shape variations. Each shape variation must be associated with a single shape parameter. The names of the parameters associated with the shape variations must be chosen such that the names remain unique when interpreted in a case-insensitive manner. The values of the shape parameters are assigned using parameter definitions. A parameter shape variation can be defined more than once for the same parameter so that different parts of a shape variation can be specified separately. In these cases if the same node is specified in multiple parameter shape variation definitions, the last definition for the node prevails. A node that is specified under a parameter shape variation definition that has not also been defined directly or through node generation will be ignored. You can specify shape variations using a combination of three possibilities: directly specifying them, reading them from an alternate input file, and reading them from the results files of auxiliary analyses. These methods are described in the following sections. Defining shape variations directly or reading them from an alternate input file You can define the shape variation data directly by specifying the node number and corresponding variations of coordinate components. Alternatively, the data can be given in an ASCII file. Input File Usage: Use the following option to specify the shape variation data directly: *PARAMETER SHAPE VARIATION, PARAMETER=name Use the following option to specify the shape variation data in an alternate input file: *PARAMETER SHAPE VARIATION, PARAMETER=name, INPUT=input file Defining shape variations in alternative coordinate systems By default, the shape variation data are interpreted in the global rectangular Cartesian coordinate system. You can specify the shape variation data (either directly or in an alternate input file) in cylindrical or spherical coordinate systems. In such cases the computation of the shape variation is done as follows. The nodal coordinate components that define the basic shape are first transformed from the global rectangular Cartesian coordinate system in which they are stored to the specified coordinate system. The shape variation coordinate components are then added to give updated coordinate components, which are transformed back to the global rectangular Cartesian coordinate system. Finally, the shape variation is taken as the difference between the updated coordinate components and the original coordinate components, using the components expressed in the global rectangular Cartesian coordinate system. The value of the shape parameter associated with the shape variation is not used at any point in the calculation of the shape variation. Input File Usage: Use the following option to specify the shape variation data in a rectangular coordinate system (the default): *PARAMETER SHAPE VARIATION, PARAMETER=name, SYSTEM=R Use the following option to specify the shape variation data in a cylindrical coordinate system: *PARAMETER SHAPE VARIATION, PARAMETER=name, SYSTEM=C Use the following option to specify the shape variation data in a spherical coordinate system: *PARAMETER SHAPE VARIATION, PARAMETER=name, SYSTEM=S Using auxiliary analyses to generate shape variations Auxiliary models are additional finite element models that are used to generate shape variations for a primary model. Rather than defining shape variations directly on a node-by-node basis, auxiliary models can be used to simplify this process. Auxiliary analyses are finite element analyses of these auxiliary models. An auxiliary model usually has the same geometry, element connectivity, and material type as the primary model. However, the boundary conditions are usually different. Applying loading to an auxiliary model results in sets of displacements that we may interpret as shape variations. For example, we may be interested in studying the sensitivity of the nonlinear buckling behavior of a structure with respect to imperfections in the structure. In this case we could perform an auxiliary eigenvalue linear buckling analysis and then use the resulting mode shapes as shape variations to be added to the basic geometry of the primary model. (This particular problem could also be addressed by using a geometric imperfection.) Abaqus reads the shape variation data from auxiliary analyses through the user node labels. Abaqus does not check model compatibility between both analysis runs. Shape variation data cannot be read from the results file for models defined in terms of an assembly of part instances (“Defining an assembly,” Section 2.10.1). Reading shape variations from a static analysis results file To define a shape variation based on the deformed geometry of a previous static analysis, specify the results file and step from a previous static analysis. Optionally, you can specify the increment number from which displacement data are read. (By default, Abaqus will read data from the last increment available for the specified step on the results file.) In addition, you can read shape variation data for a specified node set. Input File Usage: *PARAMETER SHAPE VARIATION, PARAMETER=name, FILE=results file, STEP=step, INC=inc, NSET=name Reading shape variations from an eigenvalue analysis results file To define a shape variation based on a mode shape from a previous eigenvalue analysis, specify the results file and step from a previous eigenfrequency extraction or eigenvalue buckling prediction analysis. Optionally, you can specify the mode number from which eigenvector data are read. (By default, Abaqus will read data from the first eigenvector available for the specified step on the results file.) In addition, you can read eigenmode data for a specified node set. Input File Usage: *PARAMETER SHAPE VARIATION, PARAMETER=name, FILE=results file, STEP=step, MODE=mode, NSET=name Shape parametrization and design sensitivity analysis For the purpose of design sensitivity analysis with Abaqus/Design (“Design sensitivity analysis,” Section 19.1.1) if the parameter specified for a parameter shape variation is also specified as a design parameter, the shape variation is used to define the design gradient of the nodal coordinates and nodal normals with respect to the design parameter. If you wish to perform design sensitivity analysis for the basic shape, all shape parameters must be given a value of zero. In addition, if any parameter specified in a parameter shape variation definition is also specified as a design parameter, the parameters of all parameter shape variations must be specified as design parameters. In DSA calculations for shell and beam elements Abaqus always computes the design gradients of nodal normals using the design gradients of nodal coordinates. To overwrite the gradients computed by Abaqus, you must provide the nodal normal as part of the node definition and design gradients of the normals using a parameter shape variation. To prescribe a design-independent normal, you must provide a zero design gradient explicitly. For shape variations read from the results file, Abaqus computes the gradients of the normals based on the displacements and ignores the nodal rotations. For beam elements Abaqus computes the design gradients for the -direction of the beam cross- section using the gradients of the node coordinates and the gradients for the -direction specified using a parameter shape variation. You cannot provide the shape variation for the -direction. Abaqus ignores any such design gradients implicitly provided in either the beam section definition or as an extra node in the beam element connectivity. In cases where the data defining a shape variation are given in a cylindrical or spherical coordinate system it is important that you understand how the shape variation is calculated from the data. This calculation is described in the previous section. Visualization of shape variations Shape variations can be visualized only after the parametrized input file has been processed by the analysis input file processor. Therefore, at least a data check run must be executed before parameter shape variations can be visualized using Abaqus/CAE. The shape variations associated with each individual shape parameter can be visualized as displaced shape plots at step zero of the analysis. The basic shape is interpreted as the undeformed shape, and the shape generated by adding the displaced shape. shape variation to the basic shape is interpreted as the The combination of all shape variations added to the basic shape represents the true undeformed shape of the analysis. Using Abaqus/CAE to compute shape variations A capability for computing shape variations is provided by the Abaqus Scripting Interface command _computeShapeVariations( ). Using the command requires some familiarity with the Abaqus Scripting Interface and the execution of scripts in Abaqus/CAE. The procedure that must be followed is described and illustrated in “Design sensitivity analysis: overview,” Section 13.1.1 of the Abaqus Example Problems Manual. 2.1.3 NODAL THICKNESSES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Membrane elements,” Section 29.1.1 • “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5 • “Using a general shell section to define the section behavior,” Section 29.6.6 • *NODAL THICKNESS • *MEMBRANE SECTION • *RIGID BODY • *SHELL GENERAL SECTION • *SHELL SECTION Overview Nodal thicknesses are used to define continuously varying thicknesses for: • shell structures; • membrane structures; or • in Abaqus/Explicit rigid elements. Defining nodal thicknesses You can specify the thickness of a shell, membrane, or rigid element at a particular node or node set. Input File Usage: *NODAL THICKNESS node_number or node_set_name, thickness Abaqus/CAE Usage: Use the following option for a conventional shell composite layup: Property module: composite layup editor: Shell Parameters: Nodal distribution: select an analytical field or a node-based discrete field Use the following option for a homogeneous shell section: Property module: shell section editor: Basic: Nodal distribution: select an analytical field or a node-based discrete field Use the following option for a composite shell section: Property module: shell section editor: Advanced: Nodal distribution: select an analytical field or a node-based discrete field Reading nodal thicknesses from an alternate file The nodal thickness data can be stored in a separate file and read from there at the start of the analysis. For details on the syntax of such file names, see “Input syntax rules,” Section 1.2.1. Input File Usage: Abaqus/CAE Usage: *NODAL THICKNESS, INPUT=file_name Reading nodal Abaqus/CAE. thicknesses from an alternate file is not supported in Generating continuously varying thicknesses between two nodes or node sets Abaqus can linearly interpolate the thickness between two bounding nodes or node sets. The thicknesses at the bounding nodes must first be defined. Input File Usage: Use the following options: *NODAL THICKNESS first bounding node or node set, thickness second bounding node or node set, thickness *NODAL THICKNESS, GENERATE first bounding node or node set, second bounding node or node set, number of intervals, increment in node numbers Abaqus/CAE Usage: Generating thicknesses between bounding nodes or node sets is not supported in Abaqus/CAE. Specifying a continuously varying thickness for shell, membrane, and rigid elements You must specify that a shell or membrane element is going to have a continuously varying thickness rather than a homogeneous thickness when you define the element section. See “Membrane elements,” Section 29.1.1; “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5; and “Using a general shell section to define the section behavior,” Section 29.6.6, for details. In Abaqus/Explicit you must specify that a rigid element is going to have a continuously varying thickness when you define the rigid body to which the element belongs; see “Rigid elements,” Section 30.3.1. In Abaqus/Standard rigid elements cannot have a continuously varying thickness. Every node that is part of a shell, membrane, or rigid element using a continuously varying thickness must have a nodal thickness defined. Abaqus will issue an error message if there is a node with no nodal thickness in an element that is using a continuously varying thickness. Specifying a continuously varying thickness for a composite shell When a composite shell structure has a continuously varying thickness, the total thickness of the shell at any node is defined by the nodal thickness value. The total thickness at an integration point is interpolated from the nodal thicknesses. The layer thicknesses given in the shell section definition are used as relative thicknesses and are scaled proportionally such that the sum of the layer thicknesses equals the total thickness at the integration point. Example For example, if a composite shell section were defined with the following input: *SHELL SECTION, COMPOSITE, NODAL THICKNESS, ELSET=name 1.5, 3, STEEL 2.5, 3, FOAM 1.0, 3, STEEL and the total thickness at a point was only 1.0, the thicknesses of the individual layers at the point would be 0.3 for the first steel layer, 0.5 for the foam layer, and 0.2 for the second steel layer. Creating a discontinuity in the shell, membrane, or rigid element thicknesses You can specify only a single thickness at each node. Therefore, use separate nodes along the interface on shell, membrane, or rigid elements where there is a discontinuity in the thickness and assign the appropriate thickness to each group of nodes. For elements that are not part of a rigid body, multi-point constraints must be used to make the displacements (and rotations, for shells) the same at corresponding nodes. 2.1.4 NORMAL DEFINITIONS AT NODES Products: Abaqus/Standard Abaqus/Explicit References • *NORMAL • *NODE Overview Normals can be defined at nodes: • with a user-specified normal definition; • following the nodal coordinates as part of the node definition for beam and shell elements; • on rigid master surfaces used in contact pairs in Abaqus/Standard; • in beam and shell elements; • for line spring elements to give the direction normal to the flaw in the structure; • for gasket elements to give the thickness direction of the elements; and • for contour integral evaluation. The normals defined at nodes do not affect the element face normals, which are defined by the element connectivity. They need not be of unit length. Contact surfaces in Abaqus/Standard User-specified surface normals for contact surfaces in Abaqus/Standard are relevant only when the small- sliding contact approach is used or when the finite-sliding contact approach is used with rigid elements that make up the master surface. User-specified surface normals defined on deformable master surfaces in contact pairs are ignored when finite sliding is used. The small-sliding contact formulation uses the surface normals at each node along the master surface to define a normal vector that varies smoothly from point to point on the surface. For a detailed discussion on how the “master plane” is constructed for each slave node using the surface normals, see “Contact formulations in Abaqus/Standard,” Section 37.1.1. For master surfaces composed of rigid elements Abaqus/Standard smooths any discontinuous surface normal transitions between the rigid elements. The surface normals at the nodes are used to control the surface normal interpolation. For a detailed discussion on the smoothing of such master surfaces, see “Analytical rigid surface definition,” Section 2.3.4. To define the normal, specify the components of the normal in the global coordinate system. Input File Usage: *NORMAL, TYPE=CONTACT SURFACE Elements User-specified normals may be necessary for beam and shell elements, line spring elements, gasket elements, or elements involved in contour integral evaluations. In such cases specify the components of the normal in the global coordinate system. Input File Usage: *NORMAL, TYPE=ELEMENT Beam and shell elements User-specified normals may be needed to define the desired normal directions at shell surface intersections or at beam intersections where the automatically determined normals may be inappropriate for the model . The nodal normals can also be defined as part of the node definition. While you can define a single normal for all elements connected to a node as part of the node definition, a user-specified normal definition defines a normal for a particular element at a node, thus allowing you to define separate normals for each element connected to a node. User-specified normal definitions supersede normals defined as part of a node definition. Input File Usage: *NODE Specify the normals in the fifth, sixth, and seventh positions on the data line. For example, the following lines define some normals as part of node definitions; the normal to be used at node 7 in element 2 is then redefined using a user-specified normal definition: *NODE 6, 5., 5., , -0.5, .8 7, 10., 8., , -0.5, .8 9, 14., 4., , .6, .6 *NORMAL 2, 7, .6, .6 Line spring elements For line spring elements user-specified normals can be used to give the direction normal to the flaw in the structure. See “Line spring elements for modeling part-through cracks in shells,” Section 32.9.1, for a description of these elements. Gasket elements For gasket elements user-specified normals can be used to specify the thickness direction of the elements. The nodal thickness directions can also be defined as part of the gasket section definition. Thickness directions defined by user-specified normals supersede thickness directions defined as part of the gasket section definition. See “Defining the gasket element’s initial geometry,” Section 32.6.4, for a description of the definition of the thickness direction for these elements. Contour integral evaluation For contour integral evaluations (“Contour integral evaluation,” Section 11.4.2) surface normals should be specified at all surface nodes lying within the bounds of the requested contours. These nodes are printed out under the “Contour Integral” information in the data (.dat) file. For accurate contour integral evaluation it is important that the virtual crack extension direction is in the plane of the surface for the following cases: when a crack front intersects the external surface of a three-dimensional solid, when the crack front intersects a surface of material discontinuity, or when the crack is in a curved shell. If no normals are specified, Abaqus will calculate the normals automatically. The nodal normal data specified as part of a node definition will not be activated for solid elements unless a user-specified normal definition is used in the model; it suffices to include a user-specified normal definition for only one node to activate the utilization of the nodal normal data specified as part of a node definition. The coordinate system in which normals are defined Abaqus models can be defined in terms of an assembly of part instances . Normals at nodes defined within a part (or part instance) are defined relative to the part coordinate system. These normals are rotated according to the positioning data given for each instance of the part. Normals can be defined at reference nodes at the assembly level if necessary. Normals defined at the assembly level are defined in the global coordinate system. For models that are not defined in terms of an assembly of part instances, normals are defined in the global coordinate system. 2.1.5 TRANSFORMED COORDINATE SYSTEMS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Prescribed conditions: overview,” Section 33.1.1 • *TRANSFORM • “Transforming results into a new coordinate system,” Section 42.6.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “An overview of the methods for creating a datum coordinate system,” Section 62.5.4 of the Abaqus/CAE User’s Manual Overview A nodal transformation is used to define a local coordinate system for: • the definition of concentrated forces and moments; • the definition of displacement and rotation boundary conditions; • the definition of linear constraint equations; and • the output of vector-valued quantities. A nodal transformation cannot be used to specify a local coordinate system for defining: • nodal coordinates—see “Specifying a local coordinate system in which to define nodes” in “Node definition,” Section 2.1.1, or “Specifying a local coordinate system for the nodal coordinates” in “Node definition,” Section 2.1.1, instead; or • material properties or rebars—see “Orientations,” Section 2.2.5, instead. Defining a local coordinate system Normally displacement and rotation components are associated with the global, rectangular Cartesian axis system. When a transformed coordinate system is associated with a node, all input data for concentrated forces and moments and for displacement and rotation boundary conditions at the node are given in the local system. The following transformations are available: • Rectangular Cartesian • Cylindrical • Spherical The coordinate transformation defined at a node must be consistent with the degrees of freedom that exist at the node. For example, a transformed coordinate system should not be defined at a node that is connected only to a SPRING1 or SPRING2 element, since these elements have only one active degree of freedom per node. Input File Usage: You must identify the node set for which the local transformed system is defined. Abaqus/CAE Usage: *TRANSFORM, NSET=name In Abaqus/CAE you define a local coordinate system independent of its use and then refer to it when you apply a load or boundary condition at a node. Any module: Tools→Datum: Type: CSYS Interaction module: load or boundary condition editor: CSYS: Edit: select local coordinate system Defining a local coordinate system in a model that contains an assembly of part instances In a model defined in terms of an assembly of part instances, you can define a nodal transformation at the part, part instance, or assembly level. A nodal transformation defined at the part or part instance level will be rotated according to the positioning data given for each instance of that part (or for the part instance). See “Defining an assembly,” Section 2.10.1. Multiple transformation definitions are not allowed at a node, even if one of them is at the part level and another is at the assembly level. Large-displacement analysis The transformed coordinate system is always a set of fixed Cartesian axes at a node (even for cylindrical or spherical transforms). These transformed directions are fixed in space; the directions do not rotate as the node moves. Therefore, even in large-displacement analysis, the displacement components must always be given with respect to these fixed directions in space. Defining a rectangular Cartesian coordinate transformation In a rectangular Cartesian transformation the transformed directions are parallel at all nodes of the set. The coordinates of two points must be given, as shown in Figure 2.1.5–1. Z1 Y1 a X1 (global) Figure 2.1.5–1 Cartesian transformation. The first point, a, must be on a line through the global origin; this point defines the transformed -direction. The second point, b, must be in the plane containing the global origin and the transformed - and -axis. -directions. This second point should be on or near the positive *TRANSFORM, NSET=name, TYPE=R (default) Any module: Tools→Datum: Type: CSYS: select any method, and click OK: Rectangular Abaqus/CAE Usage: Input File Usage: Defining a cylindrical coordinate transformation The radial, tangential, and axial directions must be defined based on the original coordinates of each node in the node set for which the transformation is invoked. The global ( ) coordinates of the two points defining the axis of the cylindrical system (points a and b as shown in Figure 2.1.5–2) must be given. (radial) (axial) (tangential) (global) Figure 2.1.5–2 Cylindrical transformation. The origin of the local coordinate system is at the node of interest. The local line through the node, perpendicular to the line through points a and b. The local line that is parallel to the line through points a and b. The local system with -axis is defined by a -axis is defined by a -axis forms a right-handed coordinate and . A cylindrical coordinate system cannot be defined for a node that lies along the line joining points a and b. Input File Usage: Abaqus/CAE Usage: *TRANSFORM, NSET=name, TYPE=C Any module: Tools→Datum: Type: CSYS: select any method, and click OK: Cylindrical Defining a spherical coordinate transformation The radial, circumferential, and meridional directions must be defined based on the original coordinates of each node in the node set for which the transformation is invoked. The global ( ) coordinates of the center of the spherical system, a, and of a point on the polar axis, b, must be given as shown in Figure 2.1.5–3. (meridional) (circumferential) 1 (radial) (global) Figure 2.1.5–3 Spherical transformation. The origin of the local coordinate system is at the node of interest. The local -axis is defined by -axis lies in a plane containing the polar axis (the line -axis forms a right-handed -axis. The local a line through the node and point a. The local between points a and b) and is perpendicular to the local coordinate system with and . A spherical coordinate system cannot be defined for a node that lies along the line joining points a and b. Input File Usage: Abaqus/CAE Usage: *TRANSFORM, NSET=name, TYPE=S Any module: Tools→Datum: Type: CSYS: select any method, and click OK: Spherical Output at a node associated with a coordinate transformation Printed and file output of vector-valued quantities from Abaqus/Standard at transformed nodes can be in the local or global system . By default, the values are written to the data file in the local system, whereas the values are written to the results file in the global system (since this is more convenient for postprocessing). Consequently, reaction forces printed using the default will not appear to equilibrate loads applied in the global system. However, these reaction forces and loads should equilibrate if you output them to the data file in the global system. File output from Abaqus/Explicit is always in the global system. Output database output of field vector-valued quantities at transformed nodes is in the global system. The local transformations are also written to the output database. You can apply these transformations to the results in the Visualization module of Abaqus/CAE to view the vector components in the transformed systems. Output database output of history vector-valued quantities at transformed nodes can be in the local or global system . By default, the values are written in the global system (since this is more convenient for postprocessing). 2.1.6 ADJUSTING NODAL COORDINATES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • *ADJUST • “Defining adjust points constraints,” Section 15.15.5 of the Abaqus/CAE User’s Manual Overview Nodal adjustment is used for: • adjusting user-specified nodal coordinates so that the nodes lie on a given surface; and • specifying the direction along which the nodes are moved. Adjusting nodal coordinates In general, user-specified nodal coordinates are not modified during input file processing. However, there are some situations where mesh coordinates are known only in a generic way and it is inconvenient to determine their coordinates for their actual usage. For example, when using fasteners the specified reference node should be positioned at its projection point on the associated surface. Since that location may be known only approximately, you can use nodal adjustment to move the reference node to that location automatically. For typical usage of the nodal adjustment feature, refer to “About assembled fasteners,” Section 29.1.3 of the Abaqus/CAE User’s Manual. When using this feature, the nodes are adjusted to lie on the specified surface without regard for shell thickness or shell offsets. Therefore, it is not advisable to use this feature as a way of correcting initial overclosures for contact or for tie constraints. In addition, care should be taken when choosing the nodes to be adjusted because the feature does not respect any constraints relating the relative position of the adjusted node with other nodes (e.g., rigid body definitions). Input File Usage: Use the following option to identify the nodes to be moved and the surface onto which the nodes are to be moved: Abaqus/CAE Usage: *ADJUST, NODE SET=name, SURFACE=name Use the following option to move the control point of a coupling constraint onto the coupling surface: Interaction module: Constraint→Create: Coupling; Adjust control point to lie on surface Use the following option to move any point or points onto any surface: Interaction module: Constraint→Create: Adjust points Specifying the nodal adjustment direction A node can be moved to the surface using a normal adjustment or a directed adjustment. By default, the node is adjusted to the closest point on the specified surface along the normal to the surface. You can specify an orientation to move the node to the surface along a given direction rather than along the normal to the surface. The vector along the local Z-direction from the orientation definition is used to move the node to the surface . If no projection can be found, the nodal coordinates are left unmodified. Input File Usage: Abaqus/CAE Usage: *ADJUST, ORIENTATION=name The orientation projection option is not supported in Abaqus/CAE. 2.2 Element definition • “Element definition,” Section 2.2.1 • “Element foundations,” Section 2.2.2 • “Defining reinforcement,” Section 2.2.3 • “Defining rebar as an element property,” Section 2.2.4 • “Orientations,” Section 2.2.5 2.2.1 ELEMENT DEFINITION Products: Abaqus/Standard Abaqus/Explicit References • *ELCOPY • *ELEMENT • *ELGEN • *ELSET Overview This section describes the methods for defining elements in an Abaqus input file. In a preprocessor such as Abaqus/CAE, you define the model geometry rather than the nodes and elements; when you mesh the geometry, the preprocessor automatically creates the nodes and elements needed for analysis. Although the concepts discussed in this section apply in general to the element definitions in the input file that is created by Abaqus/CAE, the methods and techniques described here apply only if you are creating the input file manually. Element definition consists of: • assigning an element number to the element; • defining individual elements by specifying their nodes; • grouping elements into element sets; and • creating elements from existing elements by generating them incrementally or by copying existing elements. If any element is specified more than once, the last specification given is used. Assigning an element number to the element Each individual element must have a numeric label called the element number, which is assigned when the element is defined. The element number must be a positive integer, and the maximum element number allowed is 999999999 (for information on integer input, see “Input syntax rules,” Section 1.2.1). The elements do not need to be numbered continuously. An Abaqus model can be defined in terms of an assembly of part instances . In such a model almost all elements must belong to a part or part instance. The only exceptions are mass, rotary inertia, capacitance, connector, spring, and dashpot elements, which can belong to a part or to the assembly. Element numbers must be unique within a part, part instance, or the assembly; but they can be repeated in different parts or part instances. Defining individual elements by specifying their nodes You can define individual elements by specifying the element number and the nodes that define the element. In addition, you must specify the element type. The element must be chosen from one of the element types specified in Part VI, “Elements”; or, in Abaqus/Standard, it can be a user-defined element (“User-defined elements,” Section 32.15.1) or a substructure (“Using substructures,” Section 10.1.1). Input File Usage: *ELEMENT, TYPE=name For example, the following lines create element number 11, which is of type C3D8R, by defining its nodes (2, 3, 9, 7, 5, 8, 12, 16): *ELEMENT, TYPE=C3D8R 11, 2, 3, 9, 7, 5, 8, 12, 16 Using large node numbers with elements that use many nodes The following rules apply when defining elements: • The connectivity for each element is considered a logical record, and any number of input lines can be used to specify it. Abaqus will read the first line for an element and consider the next line a continuation line if a comma ends the line and the element definition is not complete. • Any number of continuation lines can be used. • For elements such as C3D27 with a variable number of nodes elements,” Section 28.1.1), the last line should not end with a comma or Abaqus will interpret the next element definition as a continuation of the current element. For example, *ELEMENT, TYPE=C3D20 100001, 100001, 100002, 100003, 100004, 100005, 100006, 100007, 100008, 100009, 100010, 100011, 100012, 100013, 100014, 100015, 100016, 100017, 100018, 100019, 100020 Reading element definitions from a file Element definitions can be read into Abaqus from an alternate file. The syntax of such file names is described in “Input syntax rules,” Section 1.2.1. Input File Usage: *ELEMENT, INPUT=file_name Reading substructure definitions from a substructure library Substructure definitions can be read from the substructure library in which the substructure resides (“Using substructures,” Section 10.1.1). Input File Usage: *ELEMENT, FILE=substructure_library_name If the FILE parameter is used without a value, the default substructure library name is used. Defining axisymmetric elements with asymmetric deformation You can define a positive offset number that will be used to specify nodes for axisymmetric elements with asymmetric deformation . The default offset is 100000. Input File Usage: *ELEMENT, OFFSET=number Defining gasket elements There are several methods for defining gasket elements. overview,” Section 32.6.1; “Including gasket elements in a model,” Section 32.6.3; and “Defining the gasket element’s initial geometry,” Section 32.6.4, for more information on gasket elements; they are available only in Abaqus/Standard.) face of the solid element coincides with the first (SNEG) face of the gasket element. If the equivalent solid element is oriented differently, specify the face number on the solid element that corresponds to the first face of the gasket element. The solid element must have the same number of nodes on each face as the corresponding gasket element; If both any nodes between the faces will be ignored. The 18-node gasket element is an exception. element faces are part of contact surfaces, the connectivity of a 20-node brick element can be used, and Abaqus/Standard will generate the node numbers and coordinates of the midface nodes automatically. Abaqus/Standard will transform the solid element connectivity to the normal gasket element connectivity immediately upon reading the data. Hence, all output to the data (.dat), results (.fil), and output database (.odb) files will use the normal gasket element connectivity. Input File Usage: Use the following option to specify solid element connectivity for a gasket element in which the first face of the solid element corresponds to the first face of the gasket element: *ELEMENT, TYPE=name, SOLID ELEMENT NUMBERING Use the following option to specify solid element connectivity for a gasket element and the face of the solid element that corresponds to the first face of the gasket element: *ELEMENT, TYPE=name, SOLID ELEMENT NUMBERING=face number Examples The following lines create GK3D12M element number 11 that has node numbers 1, 2, 3, 4, 5, 6, 1001, 1002, 1003, 1004, 1005, and 1006: *ELEMENT, TYPE=GK3D12M 11, 1, 2, 3, 4, 5, 6, 1001, 1002, 1003, 1004, 1005, 1006 The same element connectivity is also created by the following lines: *ELEMENT, TYPE=GK3D12M, OFFSET=1000 11, 1, 2, 3, 4, 5, 6 The equivalent solid element would be C3D15, with the following input: *ELEMENT, TYPE=GK3D12M, SOLID ELEMENT NUMBERING 11, 1, 2, 3, 1001, 1002, 1003, 4, 5, 6, 1004, 1005, 1006, 501, 502, 503 where nodes 501, 502, and 503 would not be used. Defining cohesive elements • In the first method you specify the element number and all of the nodes that define the element. • In the second method you specify only the nodes on the bottom face of the cohesive element and Abaqus will create the remaining nodes, numbering them according to an offset number that you specify. • In the third method, which is applicable only to pore pressure cohesive elements, you specify the nodes on the bottom and top faces. Abaqus will create the remaining middle-face nodes according to an offset number that you specify. Defining a cohesive element by specifying all nodes With this method you specify all nodes that define the cohesive element. See “Two-dimensional cohesive element library,” Section 32.5.8; “Three-dimensional cohesive element library,” Section 32.5.9; and “Axisymmetric cohesive element library,” Section 32.5.10, for the element node numbering definition. Input File Usage: Use the following option to specify the element number and the nodes that define the element: *ELEMENT, TYPE=name For example, the following lines create COH3D8 element number 11 that has node numbers 1, 2, 3, 4, 1001, 1002, 1003, and 1004: *ELEMENT, TYPE=COH3D8 11, 1, 2, 3, 4, 1001, 1002, 1003, 1004 Defining a cohesive element by specifying only the bottom face nodes With this method you specify only the nodes on the bottom face of the cohesive element and a positive offset number. With displacement cohesive elements, the offset number is added to the bottom face node numbers to create the corresponding nodes on the top face. With pore pressure cohesive elements, the offset number first is added to the bottom face node numbers to create the corresponding nodes on the top face, then the offset number is added to the top face node numbers to create the corresponding nodes on the middle face. Input File Usage: Use the following option to specify the nodes on the bottom face of the element and a positive offset number for nodes on the remaining face or faces: *ELEMENT, TYPE=name, OFFSET=offset number For example, the following lines create COH3D8 element number 11 that has node numbers 1, 2, 3, 4, 1001, 1002, 1003, and 1004: *ELEMENT, TYPE=COH3D8, OFFSET=1000 11, 1, 2, 3, 4 and the following lines create pore pressure cohesive element COH3D8P element number 11 that has node numbers 1, 2, 3, 4, 1001, 1002, 1003, 1004, 2001, 2002, 2003, and 2004 (nodes 1, 2, 3, and 4 define the bottom face; nodes 1001, 1002, 1003, and 1004 define the top face; and nodes 2001, 2002, 2003, and 2004 define the middle face): *ELEMENT, TYPE=COH3D8P, OFFSET=1000 11, 1, 2, 3, 4 Defining a pore pressure cohesive element by specifying only the bottom and top face nodes With this method you specify only the nodes on the bottom and top faces of the pore pressure cohesive element and a positive offset number. The offset number is added to the bottom face node numbers to create the corresponding nodes on the middle face. Input File Usage: Use the following option to specify the nodes on the bottom and top faces of the pore pressure cohesive element and a positive offset number for the remaining middle-face nodes: *ELEMENT, TYPE=name, OFFSET=offset number For example, the following lines create a pore pressure cohesive element COH3D8P element number 11 that has node numbers 1, 2, 3, 4, 1001, 1002, 1003, 1004, 2001, 2002, 2003, and 2004 (nodes 1, 2, 3, and 4 define the bottom face; nodes 1001, 1002, 1003, and 1004 define the top face; and nodes 2001, 2002, 2003, and 2004 define the middle face): *ELEMENT, TYPE=COH3D8P, OFFSET=2000 11, 1, 2, 3, 4, 1001, 1002, 1003, 1004 Grouping elements into element sets Element sets are used as convenient cross-references for defining loads, properties, etc. Element sets are the fundamental references of the model and should be used to assist the input definition. The members of an element set can be individual elements or other element sets. An individual element can belong to several element sets. Elements can be grouped into element sets when they are created or after they have already been defined. In either case each element set is assigned a name. Element set names can be up to 80 characters long. The same name can be used for a node set and for an element set. All elements within an element set will be arranged in ascending order of their element number, and duplicates will be removed. Once elements are assigned to an element set, additional elements can be added to the same element set; however, elements cannot be removed from an element set. Assigning elements to an element set as they are created There are several ways that elements can be assigned to element sets as they are created. Input File Usage: Use any one of the following options: *ELEMENT, ELSET=name *ELGEN, ELSET=name *ELCOPY, NEW SET=name Assigning previously defined elements to an element set You can assign elements that you have defined previously (by specifying their nodes, by generating them incrementally, or by copying existing elements) to an element set by listing the elements forming the set directly or by generating the element set. Listing the elements that form the set directly You can list the elements that form the element set directly. Previously defined element sets, as well as individual elements, can be assigned to element sets. Input File Usage: *ELSET, ELSET=name For example, the following lines add elements 3, 13, and 20 to set LEFT: *ELSET, ELSET=LEFT 20 3, 13 The following lines add elements 5 and 16 to the existing set LEFT: *ELSET, ELSET=LEFT 5, 16 ** The above data line is equivalent to specifying 5, 16, LEFT The following lines add elements 22, 14, and all elements in set LEFT to set B: *ELSET, ELSET=B 22, 14, LEFT Thus, element set B contains the following elements: 3, 5, 13, 14, 16, 20, and 22. Element set LEFT can be assigned to element set B since the definition of LEFT occurs before the definition of B. Generating the element set To generate an element set, you must specify a first element, element numbers between these elements, i. All elements going from to to the set. Therefore, i must be an integer such that default is ; a last element, ; and the increment in in steps of i will be added is a whole number (not a fraction). The . Input File Usage: *ELSET, ELSET=name, GENERATE For example, the following lines add elements 1, 3, 5, …, 19, 21 and elements 39, 49, 59, …, 129, 139 to set UP: *ELSET, ELSET=UP, GENERATE 1, 21, 2 39, 139, 10 Limitation on updating element sets that are used to define other element sets If an element set is constructed from previously defined element sets, subsequent updates to these sets are not taken into account. Input File Usage: *ELSET, ELSET=name For example, the following lines add elements 1 and 2, but not 3, to the set SET-AB while adding elements 1 and 3 to set SET-A: *ELSET, ELSET=SET-A 1, *ELSET, ELSET=SET-B 2, *ELSET, ELSET=SET-AB SET-A, SET-B *ELSET, ELSET=SET-A 3, Defining part and assembly sets In a model defined in terms of an assembly of part instances, all element sets must be defined within a part, part instance, or the assembly definition. If an element set is defined within a part (or part instance), you can refer to the element numbers directly. To define an assembly-level element set, you must identify the elements to be added to the set by prefixing each element number with the part instance name and a “.” (as explained in “Defining an assembly,” Section 2.10.1). An assembly-level element set can have the same name as a part-level element set. Example The following input defines an element set, set1, that belongs to part PartA and will be inherited by every instance of PartA: *PART, NAME=PartA ... *ELSET, ELSET=set1 1,3,26,500 *END PART An element set with the same name is defined at the assembly level as follows: *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=PartA-1, PART=PartA ... *END INSTANCE *INSTANCE, NAME=PartA-2, PART=PartA ... *END INSTANCE *ELSET, ELSET=set1 PartA-1.1, PartA-1.3, PartA-1.26, PartA-1.500 PartA-2.1, PartA-2.3, PartA-2.26, PartA-2.500 *END ASSEMBLY Assembly-level element set set1 contains all the elements from element sets set1 belonging to part instances PartA-1 and PartA-2. Therefore, the elements are assigned to two separate element sets: one at the part instance level and one at the assembly level. An assembly-level element set called set1 could be created with entirely different elements than those that belong to the part set; part- and assembly- level element sets are independent. However, since in this example the same elements are assigned to both the part- and assembly-level element sets set1, the assembly-level set could alternatively be defined by *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=PartA-1, PART=PartA ... *END INSTANCE *INSTANCE, NAME=PartA-2, PART=PartA ... *END INSTANCE *ELSET, ELSET=set1 PartA-1.set1, PartA-2.set1 *END ASSEMBLY This element set definition is equivalent to the previous example, where the elements are listed individually. Alternate method for defining assembly-level element sets Sometimes it is not convenient to define an assembly-level element set by referring to part-level element sets. In such cases a set definition containing many elements can get quite lengthy. Therefore, an alternate method is provided. Input File Usage: *ELSET, ELSET=ElsetName, INSTANCE=InstanceName The following example shows two equivalent ways to define an assembly-level element set; once by prefixing each element number with a part instance name (as shown above) and once using the more compact INSTANCE notation: *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=PartA-1, PART=PartA ... *END INSTANCE *INSTANCE, NAME=PartA-2, PART=PartA ... *END INSTANCE *ELSET, ELSET=set2 PartA-1.11, PartA-1.12, PartA-1.13, PartA-1.14, PartA-2.21, PartA-2.22, PartA-2.23, PartA-2.24 *ELSET, ELSET=set3, INSTANCE=PartA-1 11, 12, 13, 14 *ELSET, ELSET=set3, INSTANCE=PartA-2 21, 22, 23, 24 *END ASSEMBLY When the *ELSET option is used more than once with the same name, as it is with set3, the elements in the second use of *ELSET are appended to the set created by the first use of *ELSET. Internal element sets created by Abaqus/CAE In Abaqus/CAE many modeling operations are performed by picking geometry with the mouse. For example, a surface can be created by picking a face on a geometric part instance. Since the *SURFACE option refers to an element set, this “picked” geometry must be translated into an element set in the input file. Such sets are assigned a name by Abaqus/CAE and marked as internal. You can view these internal sets using display groups in the Visualization module of Abaqus/CAE . Input File Usage: *ELSET, ELSET=ElsetName, INTERNAL Transferring of element sets If the results of an Abaqus/Explicit analysis are imported into an Abaqus/Standard analysis (or vice versa) or results from an Abaqus/Standard analysis are imported into another Abaqus/Standard analysis , all element set definitions in the original analysis are imported by default. Alternatively, you can import only selected element set definitions; see “Importing element set and node set definitions” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details. If a three-dimensional model is generated from a symmetric model , all element sets in the original model will be used (and expanded) in the generated model. Creating elements from existing elements by generating them incrementally You can generate elements incrementally from existing elements. The newly created elements are always the same element type as that of the master element. Abaqus first generates a row of elements by copying the node pattern of a given element with prescribed increments in the node and element numbers. This row can then be repeated to form a layer, which can also be repeated to form a block. To generate a row of elements, you must specify the following information: • The master element number. The master element must exist at the time that the generation is specified, although it can be an element that has just been defined in this same element generation. • The number of elements to be defined in the first row generated, including the master element. • The increment in node numbers of corresponding nodes from element to element in the row. The default is 1. All element node numbers (except special-purpose nodes, discussed later) will increase by the same value. • The increment in element numbers in the row. The default is 1. To copy this newly created master row to create a layer of elements, you must specify the following additional information: • The number of rows to be defined, including the master row. • The increment in node numbers of corresponding nodes from row to row. • The increment in element numbers of corresponding elements from row to row. To copy this newly created master layer to create a block of elements, you must specify the following additional information: • The number of layers to be defined, including the master layer. • The increment in node numbers of corresponding nodes from layer to layer. • The increment in element numbers of corresponding elements from layer to layer. Input File Usage: *ELGEN For example, the elements forming the quarter cylinder shown in Figure 2.2.1–1 can be generated by the following lines: *ELGEN 1, 3, 1, 1, 5, 10, 10, 6, 100, 100 Incrementing special-purpose nodes By default, the following nodes are not incremented: • rigid body reference nodes for IRS-type and drag chain elements; and • nodes used to define the direction of the first cross-section axis for beams or frames in space. You can specify that all nodes should be incremented. You define the increment between node numbers as described above. Usually the incrementation of all nodes is needed only for nodes used to define the direction of the first cross-section axis for beams in space. Input File Usage: *ELGEN, ALL NODES Creating elements by copying existing elements You can create new elements by copying existing elements. You must identify the existing element set to copy and specify an integer constant that will be added to the node numbers of the existing elements to define the node numbers of the new elements. Likewise, you must specify an integer constant that will be added to the element numbers of existing elements to define element numbers for the elements being created. 301 211 201 111 501 411 401 311 321 221 511 521 421 121 431 331 231 441 341 131 141 241 531 541 101 11 22 21 31 32 13 12 23 33 43 42 41 a. Element numbers (Only visible elements shown). 501 411 601 511 421 401 301 311 211 321 221 201 101 111 11 611 621 521 12 121 21 13 22 23 14 24 33 32 131 31 42 41 43 34 44 54 431 441 331 231 341 241 141 451 351 251 53 52 51 151 631 531 641 541 651 551 b. Node numbers (Only visible nodes shown). Figure 2.2.1–1 Element generation example. You can assign the newly created elements to an element set. If you do not specify an element set name for the newly created elements, they are not assigned to an element set. Input File Usage: *ELCOPY, OLD SET=name, NEW SET=new_name, SHIFT NODES=number, ELEMENT SHIFT=number For example, the following data lines will generate new elements in set B that are copies of all elements in set A at the time this option is processed, with 1000 added to each element number and to each node number in the definitions of the new elements. The members of set A at the time the line is processed are those elements defined to be in set A by all element generation and element set definition lines that appear in the input file prior to this *ELCOPY option. *ELCOPY, OLD SET=A, NEW SET=B, ELEMENT SHIFT=1000, SHIFT NODES=1000 Special considerations for continuum elements When copying existing elements, you can choose to modify the node numbering sequence for the elements being created to avoid creating continuum elements that violate the Abaqus convention for counterclockwise element numbering. This modification is normally required when the nodes have been generated by copying existing nodes (“Creating nodes by copying existing nodes” in “Node definition,” Section 2.1.1). Input File Usage: *ELCOPY, REFLECT For example, assume element 1 is in element set A and is defined by nodes 1, 2, 3, 4. The following data line will generate element number 11, also in set A, with nodes 11, 14, 13, and 12: *ELCOPY, OLD SET=A, NEW SET=A, ELEMENT SHIFT=10, SHIFT NODES=10, REFLECT If the REFLECT parameter is not used, the new element will be defined by the node sequence 11, 12, 13, 14 and will violate the counterclockwise element numbering convention used with continuum elements . 13 12 14 11 Figure 2.2.1–2 Example of modification of node numbering sequence. 2.2.2 ELEMENT FOUNDATIONS Products: Abaqus/Standard Abaqus/CAE References • *FOUNDATION • “Defining foundations,” Section 15.13.20 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Elastic element foundations: • can be defined for stress/displacement elements in Abaqus/Standard according to the load identifiers described in Part VI, “Elements”; • act like springs to ground; and • are a simple way of including the stiffness effects of a support (such as the soil under a building) without modeling the details of the support. Defining element foundation behavior Foundation pressures act normal to the element faces on which they are applied. In large-displacement analysis the direction of action of the foundation is based on the deformed configuration; foundations rotate with the element sides. Convergence difficulties may arise with large-deformation problems since no corresponding foundation load stiffness terms are included in the element stiffness matrices. To define the foundation behavior, you specify the foundation stiffness per unit area (per unit length for beams). Input File Usage: Use the following option in the model definition portion of the input file: Abaqus/CAE Usage: *FOUNDATION Interaction module: Create Interaction: Step: Initial, Elastic foundation 2.2.3 DEFINING REINFORCEMENT Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • *EMBEDDED ELEMENT • *MEMBRANE SECTION • *PRESTRESS HOLD • *REBAR • *REBAR LAYER • *SHELL SECTION • *SURFACE SECTION • “Defining rebar layers,” Section 12.13.19 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Rebar: • are used to define layers of uniaxial reinforcement in membrane, shell, and surface elements (such layers are treated as a smeared layer with a constant thickness equal to the area of each reinforcing bar divided by the reinforcing bar spacing); • can be used to add layers of reinforcement in a solid by embedding reinforced surface or membrane elements in the “host” solid elements as described in “Embedded elements,” Section 34.4.1; • can be used to add additional stiffness, volume, and mass to the model; • can be used to add discrete axial reinforcement in beam elements in Abaqus/Standard; • can be used in coupled temperature-displacement analysis but do not contribute to the thermal conductivity and specific heat; • can be used in coupled thermal-electrical-structural analysis but do not contribute to the electrical conductivity, thermal conductivity and specific heat; • cannot be used in heat transfer or mass diffusion analysis; and • have material properties that are distinct from those of the underlying or host element. • do not include the mass or volume of the underlying elements. Defining a rebar layer You can specify one or multiple layers of reinforcement in membrane, shell, or surface elements. For each layer you specify the rebar properties including the rebar layer name; the cross-sectional area of each rebar; the rebar spacing in the plane of the membrane, shell, or surface element; the position of the rebars in the thickness direction (for shell elements only), measured from the midsurface of the shell (positive in the direction of the positive normal to the shell); the rebar material name; the initial angular orientation, in degrees, measured relative to the local 1-direction; and the isoparametric direction from which the rebar angle output will be measured. You can model rebar layers in solid (continuum) elements by embedding a set of surface or membrane elements with rebar layers defined as discussed above in a set of host continuum elements. Input File Usage: Use the following options to define one or more rebar layers in membrane elements: *MEMBRANE SECTION, ELSET=memb_set_name *REBAR LAYER Use the following options to define one or more rebar layers in shell elements: *SHELL SECTION, ELSET=shell_set_name *REBAR LAYER Use the following options to define one or more rebar layers in surface elements: *SURFACE SECTION, ELSET=surf_set_name *REBAR LAYER Use the following option to model rebar layers in solid (continuum) elements: *EMBEDDED ELEMENT, HOST ELSET=solid_set_name memb_set_name or surf_set_name Abaqus/CAE Usage: Property module: membrane, shell, or surface section editor: Rebar Layers Interaction module: Create Constraint: Embedded region Assigning a name to the rebar layer You must assign each layer of rebar in a particular element or element set a separate name. This name can be used in defining rebar prestress and output requests. Input File Usage: *REBAR LAYER rebar layer name Abaqus/CAE Usage: Property module: membrane, shell, or surface section editor: Rebar Layers: Layer Name rebar layer name Specifying rebar geometry The rebar geometry is always defined with respect to a local coordinate system. Defining an appropriate local system is described in the next section. The rebar geometry can be constant, vary as a function of radial position in a cylindrical coordinate system, or vary according to the tire “lift” equation. In each case you must specify the spacing, s, and the area, A, which are used to determine the thickness of the equivalent rebar layer, , of the rebar with respect to this local system. , as well as the angular orientation, In addition, for shell elements you must specify the position of the rebars in the shell thickness direction measured from the midsurface of the shell (positive in the direction of the positive normal to the shell). If the shell’s thickness is defined by nodal thicknesses (“Nodal thicknesses,” Section 2.1.3), this distance will be scaled by the ratio of the thickness defined by the nodal thickness to the thickness defined by the section definition. If the shell’s thickness is defined with a distribution (“Distribution definition,” Section 2.8.1), this distance is scaled by the ratio of the element thickness defined by the distribution to the default thickness. Defining rebar with constant spacing You can specify the geometry to be constant in the local rebar coordinate system. In this case the spacing, s, is specified as a length measure. Input File Usage: Abaqus/CAE Usage: *REBAR LAYER, GEOMETRY=CONSTANT Property module: membrane, shell, or surface section editor: Rebar Layers: Rebar geometry: Constant Defining rebar spacing as a function of radial position You can specify the spacing, s, in terms of angular spacing in degrees as shown in Figure 2.2.3–1. middle surface of shell position in shell thickness direction rebar angular spacing in degrees radial rebar (orientation angle 0o) Figure 2.2.3–1 Example of radial rebars in axisymmetric shell elements. Angular spacing values can also be used for non-radial rebars as well as for rebars having nonzero orientation angles from the meridional plane. In these cases the orientation angles of the rebars do not change. The angular spacing option is used only to compute the spacing between rebars in units of length by multiplying the angular spacing by the radial distance of the concerned point on the rebar from the axis of axisymmetry. A local cylindrical coordinate system must be defined for the rebar if the rebar is associated with three-dimensional elements. Input File Usage: Abaqus/CAE Usage: *REBAR LAYER, GEOMETRY=ANGULAR Property module: membrane, shell, or surface section editor: Rebar Layers: Rebar geometry: Angular Defining rebar using the tire “lift” equation Structural tire analysis is often performed using the cured tire geometry as the reference configuration for the finite element model. However, the cord geometry is more conveniently specified with respect to the “green,” or uncured, tire configuration. The tire lift equation provides mapping from the uncured geometry to the cured geometry . αο αο revolution axis rο rd a) uncured geometry rd revolution axis b) cured geometry Figure 2.2.3–2 Mapping between uncured and cured tire rebar geometry. You can specify the spacing and orientation of the rebar cords with respect to the uncured configuration and let Abaqus map these properties to the reference configuration of the cured tire. Using a cylindrical coordinate system, the spacing, s, and angular orientation, , in the cured tire are obtained from and where r is the position of the rebar along the radial direction in the cured geometry, the rebar in the uncured geometry, is the spacing in the uncured geometry, is the position of is the angle measured with respect to the projected local 1-direction in the uncured geometry, and e is the cord extension ratio. In a tire e represents the pre-strain that occurs during the curing process; e =1 means a 100% extension. When is equal to 90°, the rebar is assumed to have a constant spacing of . A local cylindrical coordinate system must be defined for the rebar if the rebar is associated with three-dimensional elements. Input File Usage: Abaqus/CAE Usage: *REBAR LAYER, GEOMETRY=LIFT EQUATION Property module: membrane, shell, or surface section editor: Rebar Layers: Rebar geometry: Lift equation–based Local rebar orientation system The rebar geometry, such as rebar orientation and spacing, is defined with respect to a local orientation system. This local rebar orientation system is entirely independent from the local orientation system used for the underlying assignment. The rebar angle is always defined with respect to the local 1-direction as shown in Figure 2.2.3–3. Default projected local surface directions or user-defined local surface directions Initial rebar angle, α Figure 2.2.3–3 Rebar in a three-dimensional shell, membrane, or surface element. Rebar defined with either angular spacing or spacing defined by the tire lift equation is specified with respect to a cylindrical orientation system. For axisymmetric analysis the global coordinate system is used as the cylindrical system. For three-dimensional analysis you must provide a user-defined cylindrical orientation definition. Local orientation system for three-dimensional elements You can define the local system by referring to a user-defined local coordinate system. See “Orientations,” Section 2.2.5, for a description of how the local coordinate system is calculated from the user-defined directions for definition of rebar in shell, membrane, and surface elements. If you do not specify a user-defined orientation, the local 1-direction is based on the default projected local coordinate system. See “Conventions,” Section 1.2.2, for a definition of the default projected local directions on a surface in space. A positive angle defines a rotation from local direction 1 to local direction 2 around the element’s normal direction or the user-defined normal direction. If the shell, membrane, or surface element is curved in space, the local 1-direction will vary across the element and the initial rebar angular orientation will also vary accordingly. The orientation definition that can optionally be associated with a shell or membrane section definition has no influence on the rebar angular orientation definitions. For example, in a membrane section, shell section, or surface section, the following data would result in the rebar layer definition shown in Figure 2.2.3–4: A=0.01; s=0.1; distance of rebar from the shell midsurface=0.0; =30.; and the rebar definition refers to a local rectangular orientation defined to have its X-axis go plane include the point (−0.7071, −0.7071, 0.0), and through the point (−0.7071, 0.7071, 0.0), its an additional rotation of 0.0 degrees about the 3-direction. OR1 OR2 ORn = user-defined local directions 1, 2 = default local directions Figure 2.2.3–4 Rebar defined relative to user-defined local coordinate directions. The following data would result in the rebar layer definition shown in Figure 2.2.3–5: A=0.01, s=0.1, distance of rebar from the shell midsurface=0.0, and =45. Input File Usage: Abaqus/CAE Usage: Use the following options to define the local 1-direction for a rebar layer: *ORIENTATION, NAME=name *REBAR LAYER, ORIENTATION=name Property module: Tools→Datum: Type: CSYS Assign→Rebar Reference Orientation Local orientation system for axisymmetric elements Rebars in an axisymmetric membrane element or an axisymmetric surface element must lie in the element reference surface, whereas rebars in an axisymmetric shell can lie in the shell reference surface or can be offset from the midsurface. Rebars in axisymmetric membrane, shell, and surface elements can be local directions α = 45° Figure 2.2.3–5 Rebar defined relative to default local coordinate directions. defined to have any angular orientation with respect to the r–z plane. See Figure 2.2.3–6 for an example of circumferential rebars and Figure 2.2.3–1 for an example of radial rebars in axisymmetric shells. CL 10 circumferential rebar (90o orientation) middle surface of shell spacing of rebar position in shell thickness direction 20 Figure 2.2.3–6 Example of circumferential rebars in axisymmetric shell elements. You cannot specify a user-defined orientation for rebar layers in axisymmetric membrane, shell, and surface elements. Instead, in the rebar layer definition you specify the angular orientation of the rebar layer, in degrees, with respect to the r–z plane; this orientation is measured positive about the positive normal to the membrane, shell, or surface element. If you specify an orientation angle other than 0° or 90° for rebar in an axisymmetric membrane without twist, axisymmetric shell, or axisymmetric surface without twist, Abaqus assumes that the rebars are balanced (i.e., half the rebar lie at the specified angle and the other half at an angle of ) and internal calculations are handled accordingly. Such a rebar definition should not be used with the symmetric model generation capability (“Symmetric model generation,” Section 10.4.1). The recommended modeling technique is to define unbalanced rebar in axisymmetric elements with twist. Balanced rebar, on the other hand, can be defined in regular axisymmetric elements or in axisymmetric elements with twist and should be defined by specifying half the rebar at the specified angle and the other half at an angle of . Large-displacement considerations In geometrically nonlinear analyses as the rebar-reinforced element deforms, the initially defined geometric properties and orientation of the rebar layer can change as a result of finite-strain effects. The deformation of the rebar layer is determined from the deformation gradient of the underlying shell, membrane, or surface element. Rebars rotate with the actual deformation and not with the average rigid body rotation of the material point in the underlying element. See “Rebar modeling in shell, membrane, and surface elements,” Section 3.7.3 of the Abaqus Theory Manual, for details. For example, consider a plate modeled with a first-order element under large pure shear deformation as shown in Figure 2.2.3–7, where rebars are initially aligned with the element isoparametric directions. Figure 2.2.3–7 Rebar orientation evolves in a geometrically nonlinear analysis. As a result of finite-strain effects, rebars rotate but remain aligned with the element isoparametric directions. If the same problem is modeled using anisotropic material properties rather than rebars and the material directions (1 and 2) are initially aligned with the element isoparametric directions, under such large shear deformation the material directions rotate and are no longer aligned with the element isoparametric directions. The material directions in this case are determined based on the average rigid body rotation of the material point. Hence, if the material is not truly a continuum, the anisotropic behavior is better modeled with rebars. Defining rebar in Abaqus/Standard beam elements You must use element-based rebar, described in “Defining rebar as an element property,” Section 2.2.4, to model discrete rebar in beam elements in Abaqus/Standard. You specify the elements that contain the rebar, the cross-sectional area of each rebar, and the location of each rebar with respect to the local beam section axis . Rebar Local beam section axes Figure 2.2.3–8 Rebar location in a beam section. Each individual rebar must be assigned a separate name in a particular element or element set. This name can be used in defining rebar prestress and output requests. Input File Usage: Abaqus/CAE Usage: *REBAR, ELEMENT=BEAM, MATERIAL=mat, NAME=name Rebar in Abaqus/Standard beam elements are not supported in Abaqus/CAE. Defining the rebar material The material properties of the rebars are distinct from those of the underlying element and are defined by a separate material definition (“Material data definition,” Section 21.1.2). You must associate each rebar layer (or, for beam elements in Abaqus/Standard, each rebar definition) with a set of material properties. The following material behavior cannot be used in Abaqus/Standard to define rebar materials: • “Porous metal plasticity,” Section 23.2.9. The following material behaviors cannot be used in Abaqus/Explicit to define rebar materials: • “Defining fully anisotropic elasticity” in “Linear elastic behavior,” Section 22.2.1; • “Defining orthotropic elasticity by specifying the terms in the elastic stiffness matrix” in “Linear elastic behavior,” Section 22.2.1; • “Equation of state,” Section 25.2.1; • “Anisotropic yield/creep,” Section 23.2.6; • “Porous metal plasticity,” Section 23.2.9; • “Extended Drucker-Prager models,” Section 23.3.1; • “Modified Drucker-Prager/Cap model,” Section 23.3.2; • “Crushable foam plasticity models,” Section 23.3.5; or • “Cracking model for concrete,” Section 23.6.2. Although Abaqus/Standard will allow for a rebar material to be defined with orthotropic elasticity (“Defining orthotropic elasticity by specifying the terms in the elastic stiffness matrix” in “Linear elastic behavior,” Section 22.2.1) or anisotropic elasticity (“Defining fully anisotropic elasticity” in “Linear elastic behavior,” Section 22.2.1), is the only meaningful material constant in these definitions. , using the corresponding stress component, , as discussed in “Linear elastic behavior,” Section 22.2.1; no other strain or stress components exist is used to compute the strain in the rebar direction, in rebars. If a nonzero density is specified for the material in a rebar layer, the mass of the rebar is taken into account for dynamic analysis as well as for gravity, centrifugal, and rotary acceleration distributed loads. The mass is not taken into account for rebar in beam elements (available only in Abaqus/Standard); you should adapt the density of the beam material to account for the rebar mass. Input File Usage: Abaqus/CAE Usage: *REBAR LAYER rebar layer name, A, s, distance of rebar from shell midsurface, rebar material name Property module: membrane, shell, or surface section editor: Rebar Layers: Material rebar material name Initial conditions Initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) can be used to define prestress or solution-dependent values for rebars. Defining prestress in rebar For structures in which reinforcing is defined (such as reinforced concrete structures), you can use initial conditions to define the prestress in the rebars. In such cases in Abaqus/Standard the structure must be brought to a state of equilibrium before it is actively loaded by means of an initial static analysis step (“Static stress analysis,” Section 6.2.2) with no external loads applied (or, perhaps, with the “dead” loads only)—see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. Input File Usage: *INITIAL CONDITIONS, TYPE=STRESS, REBAR element number or element set name, rebar name, prestress value Abaqus/CAE Usage: Rebar prestress is not supported in Abaqus/CAE. Holding prestress in rebar in Abaqus/Standard If prestress is defined in the rebars and unless the prestress is held fixed, it will be allowed to change during an equilibrating static analysis step; this is a result of the straining of the structure as the self- equilibrating stress state establishes itself. An example is the pretension type of concrete prestressing in which reinforcing tendons are initially stretched to a desired tension before being covered by concrete. After the concrete cures and bonds to the rebar, release of the initial rebar tension transfers load to the concrete, introducing compressive stresses in the concrete. The resulting deformation in the concrete reduces the stress in the rebar. Alternatively, you can keep the initial stress defined in some or all of the rebars constant during this initial equilibrium solution. An example is the post-tension type of concrete prestressing; the rebars are allowed to slide through the concrete (normally they are in conduits), and the prestress loading is maintained by some external source (prestressing jacks). The magnitude of the prestress in the rebar is normally part of the design requirements and must not be reduced as the concrete compresses under the loading of the prestressing. Normally, the prestress is held constant only in the first step of an analysis. This is generally the more common assumption for prestressing. If the prestress is not held constant in analysis steps following the step in which it is held constant, the stress in the rebar will change due to additional deformation in the concrete. If there is no additional deformation, the stress in the rebar will remain at the level set by the initial conditions. If the loading history is such that no plastic deformation is induced in the concrete or rebar in steps subsequent to the steps in which the prestress is held constant, the stress in the rebar will return to the level set by the initial conditions upon removal of the loading applied in those steps. Input File Usage: Abaqus/CAE Usage: *PRESTRESS HOLD Rebar prestress is not supported in Abaqus/CAE. Defining the initial values of solution-dependent state variables for rebars You can define the initial values of solution-dependent state variables for rebars within elements. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, for details. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=SOLUTION, REBAR Initial solution-dependent state variables are not supported in Abaqus/CAE. Output Rebar force output is available at the rebar integration locations with output variable RBFOR. The rebar force is equal to the rebar stress times the current rebar cross-sectional area. The current cross-sectional area of the rebar is calculated by assuming the rebar is made of an incompressible material, regardless of the actual material definition. For rebars in membrane, shell, or surface elements output variables RBANG and RBROT identify the current orientation of rebar within the element and the relative rotation of the rebar as a result of finite deformation, respectively. These quantities are measured with respect to the user-specified isoparametric direction in the element, not the default local element system or the orientation-defined system. See “Rebar modeling in shell, membrane, and surface elements,” Section 3.7.3 of the Abaqus Theory Manual. See “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2, for information on additional output quantities such as stress and strain. For rebars in membrane, shell, or surface elements with multiple integration points, output quantities are available at the integration points and at the centroid of the element. Specifying the direction for rebar angle output The output quantities RBANG and RBROT can be measured from either of the isoparametric directions in the plane of the membrane, shell, or surface elements. You can specify the desired isoparametric direction from which the rebar angle will be measured (1 or 2). The rebar angle is measured from the isoparametric direction to the rebar with a positive angle defined as a counterclockwise rotation around the element’s normal direction. The default direction is the first isoparametric direction. In axisymmetric shell, surface, and membrane elements the first isoparametric direction coincides with the meridional direction, and the second isoparametric direction coincides with the hoop direction. In triangular elements Abaqus defines the isoparametric directions as follows: for a 3-node triangle the first isoparametric direction is a straight line going from node 1 to the midpoint of the second element edge, and the second isoparametric direction is a straight line going from the midpoint of the first element edge to the midpoint of the third element edge; for a 6-node triangle the first isoparametric direction is a straight line going from node 1 to node 5, and the second isoparametric direction is a straight line going from node 4 to node 6 . Input File Usage: *REBAR LAYER rebar layer name, A, s, distance of rebar from shell midsurface, rebar material name, angular orientation of rebar, isoparametric direction Abaqus/CAE Usage: You cannot specify the direction for rebar angle output in Abaqus/CAE; the first isoparametric direction is always used. Example As an example, a user-defined local coordinate system is used to define rebar in a shell element ( = and the output value of RBANG is 75°, as illustrated in Figure 2.2.3–9: ), *REBAR LAYER, ORIENTATION=ORIENT Rbname, 0.01, 0.1, 0.0, Rbmat, 30., 2 *ORIENTATION, SYSTEM=RECTANGULAR, NAME=ORIENT -0.7071, 0.7071, 0.0, -0.7071, -0.7071, 0.0 3, 0.0 The rebars are located at the midsurface of the shell. Output variable RBANG is measured from the second isoparametric direction to the rebar. If the first isoparametric direction were chosen instead, output variable RBANG would report an angle of 165°. Visualizing rebar orientation and results in rebar Abaqus/CAE supports visualization of rebar direction and results in rebar layers. Plots of rebar orientation are available only if you request element output for rebars . Element variables for rebar can be contoured as field output or plotted as history output in the Visualization module. Each rebar layer will have a unique name and represents one additional section point in a membrane, shell, or surface element. You can select a RBANG = 75 2, ISO2 OR1 OR2 ISOn = isoparametric directions ORn = user-defined local directions 1, 2 = default local directions 1, ISO1 Figure 2.2.3–9 RBANG measurement for rebar defined relative to user-defined local coordinate directions. named rebar layer in a membrane, shell, or surface element to display its results in the Visualization module. Abaqus/CAE does not yet support rebar in beams. 2.2.4 DEFINING REBAR AS AN ELEMENT PROPERTY Products: Abaqus/Standard Abaqus/Explicit References • *PRESTRESS HOLD • *REBAR Overview The preferred method for defining rebar in shell and membrane elements is defining layers of reinforcement as part of the element section definition (documented in “Defining reinforcement,” Section 2.2.3). The preferred method for defining rebar in solids is embedding reinforced surface or membrane elements in “host” solid elements as described in “Embedded elements,” Section 34.4.1. This section describes an alternative method of defining rebar in shell, membrane, and continuum elements as an element property. This method is more cumbersome than the method described in “Defining reinforcement,” Section 2.2.3, and does not allow visualization of the rebar and rebar results in Abaqus/CAE. Element-based rebars: • are used to define uniaxial reinforcement in solid, membrane, and shell elements; • can be defined as individual reinforcing bars in solid elements; • can be defined as layers of uniformly spaced reinforcing bars in shell, membrane, and solid elements (such layers are treated as a smeared layer with a constant thickness equal to the area of each reinforcing bar divided by the reinforcing bar spacing); • can be used with coupled temperature-displacement elements but do not contribute to the thermal conductivity and specific heat; • can be used with coupled thermal-electrical-structural elements but do not contribute to the electrical conductivity, thermal conductivity and specific heat; • do not contribute to the mass of the model in Abaqus/Standard; • cannot be used in elements intended for heat transfer or mass diffusion analysis; • cannot be used with triangular shell and membrane elements or with triangular, triangular prism, and tetrahedral solid elements; and • have material properties that are distinct from those of the underlying element. Assigning a name to the rebar set You must assign a name to the rebar set. This name can be used in defining rebar prestress and output requests. Each layer of rebar must be assigned a separate name in a particular element or element set. Input File Usage: *REBAR, ELEMENT=elem, MATERIAL=mat, NAME=name Defining rebars in three-dimensional shell and membrane elements Both isoparametric and skew rebars can be defined in three-dimensional shell and membrane elements. Rebars cannot be used with triangular shells or membranes. If triangular-shaped shells or membranes are needed, collapsed quadrilateral shells or membranes can be used. The resulting rebar directions will depend on the type of rebar (isoparametric or skew) used. The rebar must be defined carefully since the element is distorted. This technique should be used only in regions of the mesh where results are not critical and stress gradients are not high. The stiffness calculations for the rebars use the same integration points as the calculations for the underlying shell or membrane elements. See “Shell elements: overview,” Section 29.6.1, and “Membrane elements,” Section 29.1.1, for more information about shell and membrane elements. Defining isoparametric rebars in three-dimensional shell and membrane elements Isoparametric rebars are aligned along the mapping of constant isoparametric lines in the element . Similar to edge 1 or 3 (cid:0)(cid:0) (cid:0)(cid:0) (cid:0)(cid:0) (cid:0)(cid:0) (cid:0)(cid:0) (cid:0)(cid:0) (cid:0)(cid:0) Similar to edge 2 or 4 physical space (cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0) (cid:0)(cid:0) (cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0) (cid:0)(cid:0) (cid:0)(cid:0) isoparametric space Edge Corner nodes 1 1-2 2 2-3 3 3-4 4 4-1 Figure 2.2.4–1 “Isoparametric” rebar in an undistorted three-dimensional shell or membrane element. If opposite edges of the element containing the rebar are not parallel, the rebar directions will be different at each of the integration points within an element . The spacing of the rebar will be fixed in physical space. The spacing, s, and the area of the rebar, A, are used to determine the thickness of the equivalent smeared layer, . If the edges of the element containing the rebar are not parallel, the number of actual rebar with this spacing passing through one edge will be different than the number passing through the opposite edge (opposite in isoparametric space). You specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; the rebar spacing in the plane of the shell, s; and the edge number to which the rebars are parallel when plotted in isoparametric space . In addition, for shell elements you specify the position of the rebars in the shell thickness direction measured from the midsurface of the shell (positive in the direction of the positive normal to the shell). If the shell’s thickness is defined by nodal thicknesses Figure 2.2.4–2 “Isoparametric” rebar directions in a distorted three-dimensional shell or membrane element (dashed lines indicate rebar directions). (“Nodal thicknesses,” Section 2.1.3), this distance is scaled by the ratio of the thickness defined by the nodal thickness to the thickness defined by the section definition. If the shell’s thickness is defined with a distribution (“Distribution definition,” Section 2.8.1), this distance is scaled by the ratio of the element thickness defined by the distribution to the default thickness. If the shell has a composite section whose layer thicknesses are defined with distributions (“Distribution definition,” Section 2.8.1), this distance is scaled by the ratio of the sum of the element layer thicknesses defined by the distributions to the sum of the default layer thicknesses. Input File Usage: Use the following option to define isoparametric rebars in three-dimensional shell elements: *REBAR, ELEMENT=SHELL, MATERIAL=mat, GEOMETRY=ISOPARAMETRIC Use the following option to define isoparametric rebars in general membrane elements: *REBAR, ELEMENT=MEMBRANE, MATERIAL=mat, GEOMETRY=ISOPARAMETRIC Defining skew rebars in three-dimensional shell and membrane elements Skew rebars need not be similar to an element edge; they can lie at any prescribed angle from the local 1-axis. The direction of the rebars must be defined in one of two ways, as indicated in Figure 2.2.4–3: 1. The rebars can be defined relative to the default projected local coordinate system . 2. The rebars can be defined relative to a user-defined local coordinate system . Projected local surface directions or user-defined local surface directions Skew angle, α Figure 2.2.4–3 “Skew” rebar in a three-dimensional shell or membrane. The orientation definition that can optionally be associated with a shell or membrane section definition has no influence on the rebar angular orientation definitions. If the shell or membrane is curved in space, the local 1-direction will vary across the element and the skew rebar will also vary accordingly. For shell elements the definition of a local coordinate system using distributions (“Distribution definition,” Section 2.8.1) has no influence on the rebar angular orientation definitions. If the rebar cross-sectional area is A, the rebar spacing, s, should be given so that the thickness of the equivalent “smeared” layer of reinforcing is . Defining skew rebars relative to the default projected local coordinate system To define skew rebars relative to the default projected local coordinate system, you specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; the rebar spacing in the plane of the shell, s; the position of the rebars in the thickness direction (for shell elements only), measured from the midsurface of the shell (positive in the direction of the positive normal to the shell); and the angle , in degrees, between the default local 1-direction and the rebars. See “Conventions,” Section 1.2.2, for a definition of the default projected local directions on a surface in space. If the shell’s thickness is defined by nodal thicknesses (“Nodal thicknesses,” Section 2.1.3), the rebar position in the thickness direction will be scaled by the ratio of the thickness defined by the nodal thickness to the thickness defined by the section definition. If the shell’s thickness is defined with a distribution (“Distribution definition,” Section 2.8.1), the rebar position in the thickness direction is scaled by the ratio of the element thickness defined by the distribution to the default thickness. A positive angle defines a rotation from local direction 1 to local direction 2 around the element’s normal direction. For example, in a membrane the following data would result in the rebar definition shown in Figure 2.2.4–4: A=0.05, s=0.1, and =45. When a user-defined local orientation definition is not used to define the angular orientation of the rebar and the normal to the shell is nearly parallel to the global 1-axis, the local 1-axis may change significantly within an element or from one element to the next . local directions α = 45° Figure 2.2.4–4 Skew rebar defined relative to default local coordinate directions. Input File Usage: Use the following option to define skew rebars relative to the default projected local coordinate system in three-dimensional shell elements: *REBAR, ELEMENT=SHELL, MATERIAL=mat, GEOMETRY=SKEW Use the following option to define skew rebars relative to the default projected local coordinate system in general membrane elements: *REBAR, ELEMENT=MEMBRANE, MATERIAL=mat, GEOMETRY=SKEW Defining skew rebars relative to a user-defined local coordinate system To define skew rebars relative to a user-defined local coordinate system, you specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; the rebar spacing in the plane, s; the position of the rebars in the thickness direction (for shell elements only), measured from the midsurface of the shell (positive in the direction of the positive normal to the shell); and the angle, , in degrees, between the user-defined 1-direction and the rebars. See “Orientations,” Section 2.2.5, for a description of how the local coordinate system is calculated from the user-defined directions for definition of rebar in shells and membranes. A positive angle defines a rotation from local direction 1 to local direction 2 around the user-defined normal direction. For example, in a shell the following data would result in the skew rebar definition shown in Figure 2.2.4–5: A=0.01; s=0.1; distance of rebar from the shell midsurface=0.0; =30.; and the rebar definition refers to a local rectangular orientation defined to have its X-axis go through the point (−0.7071, 0.7071, 0.0), its X–Y plane include the point (−0.7071, −0.7071, 0.0), and an additional rotation of 0.0 degrees about the 3-direction. Input File Usage: Use the following option to define skew rebars relative to a user-defined local coordinate system in three-dimensional shell elements: *REBAR, ELEMENT=SHELL, MATERIAL=mat, GEOMETRY=SKEW, ORIENTATION=name OR1 OR2 ORn = user-defined local directions 1, 2 = default local directions Figure 2.2.4–5 Skew rebar defined relative to user-defined local coordinate directions. Use the following option to define skew rebars relative to a user-defined local coordinate system in general membrane elements: *REBAR, ELEMENT=MEMBRANE, MATERIAL=mat, GEOMETRY=SKEW, ORIENTATION=name Defining rebars in axisymmetric shell and membrane elements Rebars in an axisymmetric membrane must lie in the membrane reference surface, whereas rebars in an axisymmetric shell can lie in the shell reference surface or can be offset from the midsurface. Rebars in axisymmetric shells and membranes can be defined to have any orientation with respect to the r–z plane. See Figure 2.2.4–6 for an example of circumferential rebars and Figure 2.2.4–7 for an example of radial rebars in axisymmetric shells. You specify the cross-sectional area, A, of each rebar; the rebar spacing, s; for shell elements the position of the rebars in the shell thickness direction, measured from the midsurface of the shell (positive in the direction of the positive normal to the shell); the angular orientation with respect to the r–z plane, , measured in degrees; and the radial position at which the rebar spacing is measured. The angular orientation is measured positive about the positive normal to the shell or membrane element. If the shell’s thickness is defined by nodal thicknesses (“Nodal thicknesses,” Section 2.1.3), the distance from the midsurface will be scaled by the ratio of the thickness defined by the nodal thickness to the thickness defined by the section definition. If the shell’s thickness is defined with a distribution (“Distribution definition,” Section 2.8.1) the distance from the midsurface will be scaled by the ratio of the element thickness defined by the distribution to the default thickness. If an orientation angle other than 0 or 90° is specified for rebar in an axisymmetric shell or membrane without twist, Abaqus assumes that the rebars are balanced (i.e., half the rebar lie at the specified angle ) and internal calculations are handled accordingly. and the other half at an angle of 10 circumferential rebar (90o orientation) middle surface of shell spacing of rebar position in shell thickness direction 20 CL Figure 2.2.4–6 Example of circumferential rebars in axisymmetric shell elements. radial position where rebar spacing is given middle surface of shell position in shell thickness direction rebar spacing radial rebar (orientation angle 0o) Figure 2.2.4–7 Example of radial rebars in axisymmetric shell elements. See “Rebar modeling in two dimensions,” Section 3.7.1 of the Abaqus Theory Manual, for details. If the symmetric model generation capability (“Symmetric model generation,” Section 10.4.1) is used to create a three-dimensional model from an axisymmetric shell or membrane model, only balanced rebars will be translated appropriately. The definition of balanced rebars in the axisymmetric model will result in balanced rebars in the three-dimensional model; such a translation with unbalanced rebars is not available. Unbalanced rebars in generalized axisymmetric membranes with twist will be translated properly. If the radial position for the rebar spacing is given, the total cross-sectional area of rebar will remain constant as the radial position changes; this behavior corresponds to the number of rebar in the circumferential direction remaining constant and implies that the thickness of the smeared layer of rebar decreases and that the spacing of the rebars increases as r increases . If the radial position for the rebar spacing is omitted (or is set to zero), Abaqus assumes that the spacing of the rebar remains constant; the thickness of the corresponding smeared layer is held fixed such that . Input File Usage: Use the following option to define rebars in an axisymmetric shell element: *REBAR, ELEMENT=AXISHELL, MATERIAL=mat Use the following option to define rebars in an axisymmetric membrane element: *REBAR, ELEMENT=AXIMEMBRANE, MATERIAL=mat Defining rebars in continuum elements Two- or three-dimensional continuum (solid) elements can contain rebars; rebars cannot be defined in triangular, prism, tetrahedral, or infinite elements. If triangular or wedge-shaped elements are needed, collapsed quadrilateral or brick elements can be used. Be careful when collapsing elements that contain rebar. It is important to check that the location and orientation of the rebar are correct. Rebars are defined as single bars or in layers. In the latter case the layer is a surface in each element; you provide the rebar orientation in the surface. Defining layers of rebars in planar and axisymmetric continuum elements By default, the rebars form a layer that lies in a surface that is at right angles to the plane of the model. You define the line where this rebar surface intersects the plane of the model, as described below. The orientation of the rebars within the rebar surface is defined by giving an angle, in degrees, between the line of intersection in the plane of the model and the rebars. This angle is measured in physical three-dimensional space, not in isoparametric space. See “Rebar modeling in two dimensions,” Section 3.7.1 of the Abaqus Theory Manual, for details. The positive direction along the line of intersection is from the lower to the higher numbered element edge that is intersected, and a positive angle indicates rebars oriented down into the plane of the model (where the plane is parallel to the z-axis in plane strain analysis or the -axis for axisymmetric analysis), as shown in Figure 2.2.4–8. If an orientation angle other than 0 or 90° is specified for rebar in an axisymmetric element without twist, it is assumed that the rebar in the element are balanced (i.e., half the rebar lie at the specified angle and the other half at the angle ). Defining isoparametric rebars For isoparametric rebars the intersection of the rebar layer with the plane of the model will lie along the mapping of a constant isoparametric line in the element. You specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; the rebar spacing, s; the rebar orientation, (as described gle n a n t a tio O rie edge 4 Rebar Positive direction from lower to higher numbered edge. edge 1 rebar spacing edge 2 edge 3 Figure 2.2.4–8 Orientation of rebars in plane and axisymmetric solid elements. above); the fractional distance from the edge, f (the ratio of the distance between the edge and the rebar to the distance across the element); and the edge number from which the rebars are defined. In addition, for axisymmetric elements you specify the radial position at which the rebar spacing is measured. If the radial position for the rebar spacing is given for rebar in axisymmetric elements, the total cross-sectional area of rebar will remain constant as the radial position changes; this behavior corresponds to the number of rebar remaining constant as r increases; that is, the thickness of the smeared layer If the radial position for the rebar spacing is omitted (or is set to of rebar decreases as r increases. zero), Abaqus assumes that the spacing of the rebar remains constant; the thickness of the corresponding smeared layer is held fixed such that . Figure 2.2.4–9 shows an example of isoparametric rebar. In the isoparametric mapping of the element, the line of rebars is parallel to one of the edges of the element. In this figure the line for rebar layer A can be defined using edges 1 or 3 and rebar layer B can be defined by edges 2 or 4. The fractional distance from edge 1 for rebar layer A is the ratio ; alternatively, layer A can be defined from edge 3, so that . Input File Usage: Use the following option to define layers of isoparametric rebars in planar and axisymmetric continuum elements: *REBAR, ELEMENT=CONTINUUM, MATERIAL=mat, GEOMETRY=ISOPARAMETRIC rebar layer B, defined with edge 2 or 4 4L A4L rebar layer A, defined with edge 1 and f = = A2L L2 A4L L4 Actual element Edge Corner nodes 1 1-2 2 2-3 3 3-4 4 4-1 L2 LA2 rebar layer B rebar layer A Isoparametric mapping of element with rebar Figure 2.2.4–9 Isoparametric rebar layer definition in solid elements. Defining skew rebars For skew rebars the intersection of the rebar layer with the plane of the model can intersect any two edges of an element. You specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; the rebar spacing, s; and the rebar orientation, (as described above). In addition, for axisymmetric elements you specify the radial position at which the rebar spacing is measured. You also specify the fractional distance along the element edge, from the first node of the edge (as listed in Figure 2.2.4–10) to where the rebar layer intersects the edge, for all edges. Only the two values corresponding to the two edges that the rebar intersects can be nonzero. Figure 2.2.4–10 shows an example of skew rebar. In the isoparametric mapping of the element, the line of rebars intersects two of the element edges. The intersection points are located by defining a fractional distance along each intersected edge. In this figure rebar layer A is defined by the ratio along edge 2. Rebar layer B is defined by the along edge 1 and the ratio ratio along edge 3 and the ratio along edge 4. Defining skew rebars in continuum elements can increase the run time for an Abaqus/Explicit analysis significantly. The element’s stable time increment will, in most cases, be determined by the stable time increment of the rebar, which is proportional to the rebar length. The rebar length is determined by factors including the rebar surface position in the element, the rebar spacing, the rebar area, and the rebar orientation within the rebar surface. If a skew rebar in a continuum element is defined Edge Corner nodes 1 1-2 2 2-3 3 3-4 4 4-1 rebar layer A defined with A2L L2 f1 = , f2 = , f3 = 0 and f4 = 0 A1L L1 B3L rebar layer B L2 A2 rebar layer A Isoparametric mapping of element with rebar rebar layer B defined with f1 = 0, f2 = 0, f3 = and f4 = B3L L3 B4L L4 3L 4L B4L A1L 1L Actual element Figure 2.2.4–10 Skew rebar layer definition in solid elements. such that it intersects two adjacent element edges, the resulting rebar length could be considerably less than the average element edge length, thus resulting in a very small element stable time increment. Input File Usage: Use the following option to define layers of skew rebars in planar and axisymmetric continuum elements: *REBAR, ELEMENT=CONTINUUM, MATERIAL=mat, GEOMETRY=SKEW Defining single rebars in two-dimensional axisymmetric and generalized plane strain continuum elements You can define single rebars in axisymmetric and generalized plane strain continuum elements. In this case the rebar is assumed to be at right angles with the plane of the model—in the thickness direction for generalized plane strain elements or the hoop direction for axisymmetric elements. The intersection of the rebar with the plane of the model is defined by the fractional distances along edges 1 and 2 of the intersections of constant isoparametric lines that pass through the rebar location . The fractional distances are measured from the first edge node listed in Figure 2.2.4–11. Edge Corner nodes 1 1-2 2 2-3 single rebar defined with 2l f1 = and f2 = L2 1l L1 1l L2 2l 1L Actual element single rebar Isoparametric mapping of element with rebar Figure 2.2.4–11 Single rebar in a solid element. You specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; and the fractional distances locating the rebar’s position in the element, and . Input File Usage: Use the following option to define single rebars in axisymmetric and generalized plane strain continuum elements: *REBAR, ELEMENT=CONTINUUM, MATERIAL=mat, SINGLE Defining layers of rebars in three-dimensional continuum elements By default, the rebars in three-dimensional continuum elements are defined as layers lying in surfaces. The surfaces are most easily defined with respect to the isoparametric mapped cube of the element. Therefore, you must consider how the rebar will be defined before generating the mesh; if the rebar surfaces are not taken into account in designing the mesh, the rebar definition can be very inefficient. In the isoparametric mapped cube the rebar surface always has two edges (opposite to one another) that are parallel to an isoparametric direction. The isoparametric directions are defined in Figure 2.2.4–12. You specify this isoparametric direction (1, 2, or 3). actual element ⇒ isoparametric mapping Isoparametric direction: 1 (parallel to the 1-2 edge of the element and intersecting face 1-4-8-5) Edge Corner nodes 1 1-4 2 4-8 3 8-5 4 5-1 Isoparametric direction: 2 (parallel to the 1-4 edge of the element and intersecting face 1-5-6-2) Edge Corner nodes 1 1-5 2 5-6 3 6-2 4 2-1 Isoparametric direction: 3 (parallel to the 1-5 edge of the element and intersecting face 1-2-3-4) Edge Corner nodes 1 1-2 2 2-3 3 3-4 4 4-1 Figure 2.2.4–12 Isoparametric direction and edge definitions for three-dimensional elements. A particular face of the element, which is perpendicular to this isoparametric direction in the isoparametric mapped cube, is used to define the position of the other two edges of the surface; the faces are defined in Figure 2.2.4–12, where the edges of the faces are also defined. If isoparametric rebars are defined, the two edges of the rebar surface that are not parallel to the user-specified isoparametric direction will be parallel to one of the other two isoparametric directions; in the isoparametric-mapped cube one isoparametric coordinate is constant on the rebar surface. Figure 2.2.4–13 illustrates this concept with an element containing two layers of isoparametric rebars. The position of each surface is given by the fractional distance f from an edge of the face defined in Figure 2.2.4–12 for the isoparametric direction chosen; you must specify the edge from which the fractional distance is measured. If skew rebars are defined, the two edges of the rebar surface, which are not parallel to the user- specified isoparametric direction, are generally not parallel to one of the other isoparametric directions. The positions of these two edges of the rebar surface are specified by the intersection of the rebar surface with edges of the intersecting face, defined in Figure 2.2.4–12, for the isoparametric direction chosen; the intersections are given by the fractional distance f along each edge of the face. (Note that the fractional distance is along the edge for skew rebars; for isoparametric rebars the fractional distances are measured from an edge.) The fractional distance along an edge is measured from the first node of the edge. All four fractional distances must be given, but only two can be nonzero. The orientation angle, , of the rebars within the rebar layer is defined in the isoparametric-mapped cube; it is measured in degrees and is the angle between the line of intersection of the rebar surface with the face for the isoparametric direction chosen and the rebar. The positive direction of the line of intersection is from the lower numbered edge to the higher numbered edge; the positive direction for the rebars points into the elements. An example is shown in Figure 2.2.4–14. The orientation angle is defined in the rebar layer in the isoparametric-mapped cube; therefore, the definition is the same for isoparametric and skew rebar. If the rebar layer is not flat in physical space, the orientation angle at each integration point may be different. Since it is possible to define only one orientation angle per element, an average value orientation angle for the element must be used; for reasonable meshes this approximation should not affect the results significantly. Defining isoparametric rebars You specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; the rebar spacing, s; the rebar orientation, (as described above); the fractional distance, f, from the edge; the number of the edge from which the fractional distance is measured; and the isoparametric direction of the rebar surface. Input File Usage: Use the following option to define layers of three-dimensional continuum elements: isoparametric rebars in *REBAR, ELEMENT=CONTINUUM, MATERIAL=mat, GEOMETRY=ISOPARAMETRIC 30o REBAR AS ELEMENT PROPERTY L3 WA f4L3 layer b element in physical space layer a 45o L1 120o f4L1 LA 135o f3L4 L4 layer b 2.0 corresponding isoparametric-mapped cube 63.4o layer a 139.3o 153.4o 49.3o 2.0 2.0 0.5 Figure 2.2.4–13 Element with two layers of isoparametric rebar. Edge Corner nodes 1 1-5 2 5-6 3 6-2 4 2-1 edge 2 f3L3 edge 1 Orientation angle, α L3 L1 f1L1 edge 3 Positive direction along line of intersection edge 4 positive direction of rebar Figure 2.2.4–14 Orientation example for three-dimensional skew rebar modeling, isoparametric direction 2. Shown in the mapped isoparametric element. Example: isoparametric rebar For example, the following input defines the isoparametric rebar shown in Figure 2.2.4–13: *HEADING ISOPARAMETRIC REBAR *NODE 0., 1, 2, 10., 3, 10., 4, 0., 0., 5, 6, 10., 7, 10., 0., 8, 0. 0. 5. 5. 7.5 0., 0., 12.5 5., 12.5 5., 7.5 *ELEMENT, TYPE=C3D8R, ELSET=ONE 1,1,2,3,4,5,6,7,8 *REBAR, ELEMENT=CONTINUUM, MATERIAL=STEEL, GEOMETRY=ISOPARAMETRIC, NAME=LAYER_A ONE,.04,2.5,49.32628,0.25,4,2 *REBAR, ELEMENT=CONTINUUM, MATERIAL=STEEL, GEOMETRY=ISOPARAMETRIC, NAME=LAYER_B ONE,.04,1.,63.43494,0.5,3,2 *MATERIAL, NAME=STEEL *ELASTIC 30.E6, … Rebar layers A and B are defined using isoparametric direction 2. From Figure 2.2.4–12 the position of the layers must be given with respect to the face with nodes 1-5-6-2. . It could also be given from edge 2 (edge with nodes 5–6), so that The fractional distance defining the position of intersection of layer A with this face can be measured from edge 4 (edge with nodes 2–1) along edge 3 (edge with nodes 6–2), as shown in Figure 2.2.4–13. For layer A, . , equal to 30° for layer A. This angle must be transformed into the corresponding angle in the isoparametric-mapped cube. This transformation can be done as follows: consider a single rebar that intersects the intersecting line (described above) and an adjacent edge . The orientation of rebar for layer A in physical space is defined by an angle, β = 120o β = 30o rebar layer A in physical space α = 139.3o α = 49.3o rebar layer A in isoparametric-mapped cube Figure 2.2.4–15 Example defining isoparametric rebar. . The length of the rebar layer along the intersecting line is L, and the From the figure length of the opposite edge is W. Consider the same rebar in the rebar layer in the isoparametric-mapped cube. The orientation angle, . (The 2 is included because the isoparametric-mapped cube is a 2 × 2 × 2 cube.) This expression can be simplified to give , is given by , where and For layer A, must be specified. , , , and , where is the orientation angle that The fractional distance defining the position of the intersection of layer B with this face can be . It could also be measured from edge 1 (edge . The orientation angle for layer B in the rebar layer is 45°. In measured from edge 3 (edge with nodes 6–2); with nodes 1–5), such that the isoparametric-mapped cube , , and . , Since an isoparametric rebar layer always lies in two of the isoparametric directions, an alternative but equivalent definition can be given. For example, layer A also lies in isoparametric direction 1, with the intersecting face having nodes 1-4-8-5. The fractional distance for layer A, measured from edge 1 (edge with nodes 1–4), is . The positive sense of the line of intersection is from edge 2 (edge with nodes 4–8) to edge 4 (edge with nodes 5–1); therefore, , and , , . Layer B also lies in isoparametric direction 3, with the intersecting face having nodes 1-2-3-4. The fractional distance for layer B, measured from edge 2 (edge with nodes 2–3), is . The positive sense of the intersecting line is from edge 1 (edge with nodes 1–2) to edge 3 (edge with nodes 3–4); therefore, the orientation angle of the rebar in physical space is , and in the isoparametric-mapped cube , , . Defining skew rebars You specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; the rebar spacing, s; the rebar orientation, (as described above); and the isoparametric direction. In addition, you specify the fractional distance f along the element edge for each edge of the intersecting face defined in Figure 2.2.4–12. Only the values corresponding to the two edges that the rebar intersects can be nonzero. Input File Usage: Use the following option to define layers of skew rebars in three-dimensional continuum elements: *REBAR, ELEMENT=CONTINUUM, MATERIAL=mat, GEOMETRY=SKEW Example: skew rebar For example, the following input defines the skew rebar shown in Figure 2.2.4–16: *HEADING *NODE 0., 1, 2, 10., 3, 10., 4, 0., 0., 5, 6, 10., 7, 10., 0., 8, 0. 0. 5. 5. 7.5 0., 0., 12.5 5., 12.5 5., 7.5 L1 30o f1L1 f3L3 L3 Figure 2.2.4–16 Example defining skew rebar. *ELEMENT, TYPE=C3D8R, ELSET=ONE 1,1,2,3,4,5,6,7,8 *REBAR, ELEMENT=CONTINUUM, MATERIAL=STEEL, GEOMETRY=SKEW, NAME=LAYER_A ONE, .04, 2.5, 55.28, , 2 .2, 0., .4, .0 *MATERIAL, NAME=STEEL *ELASTIC 30.E6, … The rebar layer is defined using isoparametric direction 2. The intersecting face is defined in Figure 2.2.4–12 and has nodes 1-5-6-2. The position of the rebar layer is given by its intersection with the edges of this face; the fractional distances, , are shown in Figure 2.2.4–16. The orientation angle of the rebar in physical space is 30°. Following the same procedure for calculating , and the orientation angle in the as was described for isoparametric rebar, and , isoparametric-mapped cube is 55.28°. Defining single rebars in three-dimensional continuum elements You can define single rebars in three-dimensional continuum elements; in this case the rebar is assumed to be placed along one of the element’s isoparametric directions. The rebar is then located by its intersection with the intersecting face (defined in Figure 2.2.4–12). The intersections of constant isoparametric lines with edges 1 and 2 of the intersecting face are given by fractional distances along edges 1 and 2, measured from the first node of each edge, as shown in Figure 2.2.4–11. You specify the elements that contain the rebars; the cross-sectional area, A, of each rebar; the fractional distances locating the rebar’s position in the element, ; and the isoparametric direction. Give the fractional distances with respect to edge 1 and edge 2 for the isoparametric direction chosen, as defined in Figure 2.2.4–12. and Input File Usage: Use the following option to define single rebars in three-dimensional continuum elements: *REBAR, ELEMENT=CONTINUUM, MATERIAL=mat, SINGLE Defining the rebar material The material properties of the rebars are distinct from those of the underlying element and are defined by a separate material definition (“Material data definition,” Section 21.1.2). You must associate each rebar definition with a set of material properties. The following material behavior cannot be used in Abaqus/Standard to define rebar materials: • “Porous metal plasticity,” Section 23.2.9. The following material behaviors cannot be used in Abaqus/Explicit to define rebar materials: • “Defining fully anisotropic elasticity” in “Linear elastic behavior,” Section 22.2.1; • “Defining orthotropic elasticity by specifying the terms in the elastic stiffness matrix” in “Linear elastic behavior,” Section 22.2.1; • “Equation of state,” Section 25.2.1; • “Anisotropic yield/creep,” Section 23.2.6; • “Porous metal plasticity,” Section 23.2.9; • “Extended Drucker-Prager models,” Section 23.3.1; • “Modified Drucker-Prager/Cap model,” Section 23.3.2; • “Crushable foam plasticity models,” Section 23.3.5; or • “Cracking model for concrete,” Section 23.6.2. Although Abaqus/Standard will allow for a rebar material to be defined with orthotropic elasticity (“Defining orthotropic elasticity by specifying the terms in the elastic stiffness matrix” in “Linear elastic behavior,” Section 22.2.1) or anisotropic elasticity (“Defining fully anisotropic elasticity” in “Linear elastic behavior,” Section 22.2.1), is the only meaningful material constant in these definitions. , using the corresponding stress component, , as discussed in “Linear elastic behavior,” Section 22.2.1; no other strain or stress components exist is used to compute the strain in the rebar direction, in rebars. In Abaqus/Standard density is ignored for the rebar material properties. Hence, the mass of the rebar is neglected in eigenvalue extraction and implicit dynamic procedures and for gravity, centrifugal, and rotary acceleration distributed loads. Input File Usage: Use the following option to associate a material definition with a rebar definition: *REBAR, ELEMENT=elem, MATERIAL=mat Initial conditions Initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) can be used to define rebar prestress or solution-dependent values for rebars. Defining prestress in rebar For structures in which reinforcing is defined (such as reinforced concrete structures), you can use initial conditions to define the prestress in the rebars. In such cases in Abaqus/Standard the structure must be brought to a state of equilibrium before it is actively loaded by means of an initial static analysis step (“Static stress analysis,” Section 6.2.2) with no external loads applied (or, perhaps, with the “dead” loads only)—see “Defining initial stresses” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. Input File Usage: *INITIAL CONDITIONS, TYPE=STRESS, REBAR element number or element set name, rebar name, prestress value Holding prestress in rebar in Abaqus/Standard If prestress is defined in the rebars and unless the prestress is held fixed, it will be allowed to change during an equilibrating static analysis step; this is a result of the straining of the structure as the self- equilibrating stress state establishes itself. An example is the pretension type of concrete prestressing in which reinforcing tendons are initially stretched to a desired tension before being covered by concrete. After the concrete cures and bonds to the rebar, release of the initial rebar tension transfers load to the concrete, introducing compressive stresses in the concrete. The resulting deformation in the concrete reduces the stress in the rebar. Alternatively, you can keep the initial stress defined in some or all of the rebars constant during this initial equilibrium solution. An example is the post-tension type of concrete prestressing; the rebars are allowed to slide through the concrete (normally they are in conduits), and the prestress loading is maintained by some external source (prestressing jacks). The magnitude of the prestress in the rebar is normally part of the design requirements and must not be reduced as the concrete compresses under the loading of the prestressing. Normally, the prestress is held constant only in the first step of an analysis. This is generally the more common assumption for prestressing. If the prestress is not held constant in analysis steps following the step in which it is held constant, the stress in the rebar will change due to additional deformation in the concrete. If there is no additional deformation, the stress in the rebar will remain at the level set by the initial conditions. If the loading history is such that no plastic deformation is induced in the concrete or rebar in steps subsequent to the steps in which the prestress is held constant, the stress in the rebar will return to the level set by the initial conditions upon removal of the loading applied in those steps. Input File Usage: *PRESTRESS HOLD Defining the initial values of solution-dependent state variables for rebars You can define the initial values of solution-dependent state variables for rebars within elements. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, for details. Input File Usage: *INITIAL CONDITIONS, TYPE=SOLUTION, REBAR Output Rebar force output is available at the rebar integration locations with output variable RBFOR. The rebar force is equal to the rebar stress times the current rebar cross-sectional area. The current cross-sectional area of the rebar is calculated by assuming the rebar is made of an incompressible material, regardless of the actual material definition. For rebars in membrane or shell elements output variables RBANG and RBROT identify the current orientation of isoparametric or skew rebar within the element and the relative rotation of the rebar as a result of finite deformation, respectively. These quantities are measured with respect to the user-specified isoparametric direction in the element, not the default local element system or the orientation-defined system. See “Rebar modeling in shell, membrane, and surface elements,” Section 3.7.3 of the Abaqus Theory Manual. See “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2, for information on additional output quantities such as stress and strain. For rebars in membrane or shell elements with multiple integration points, output quantities are available at the integration points and at the centroid of the element. Specifying the direction for rebar angle output in shell and membrane elements The output quantities RBANG and RBROT can be measured from either of the isoparametric directions in the plane of the shell or the membrane. You can specify the desired isoparametric direction from which the rebar angle will be measured (1 or 2). In axisymmetric shells and membranes the first isoparametric direction coincides with the meridional direction, and the second isoparametric direction coincides with the hoop direction. The rebar angle is measured from the isoparametric direction to the rebar with a positive angle defined as a counterclockwise rotation around the element’s normal direction. The default direction is the first isoparametric direction. Input File Usage: Use any of the following options: *REBAR, ELEMENT=SHELL, MATERIAL=mat, ISODIRECTION=n *REBAR, ELEMENT=AXISHELL, MATERIAL=mat, ISODIRECTION=n *REBAR, ELEMENT=MEMBRANE, MATERIAL=mat, ISODIRECTION=n *REBAR, ELEMENT=AXIMEMBRANE, MATERIAL=mat, ISODIRECTION=n Example As an example, a user-defined local coordinate system is used to define skewed rebar in a shell element (skew angle ), and the output value of RBANG is 75°, as illustrated in Figure 2.2.4–17: *REBAR, ELEMENT=SHELL, MATERIAL=MAT1, NAME=REBARB, RBANG = 75 2, ISO2 OR1 OR2 ISOn = isoparametric directions ORn = user-defined local directions 1, 2 = default local directions 1, ISO1 Figure 2.2.4–17 RBANG measurement for skew rebar defined relative to user-defined local coordinate directions. GEOMETRY=SKEW, ORIENTATION=ORIENT, ISODIRECTION=2 ELSET1, 0.01, 0.1, 0.0, 30. *ORIENTATION, SYSTEM=RECTANGULAR, NAME=ORIENT -0.7071, 0.7071, 0.0, -0.7071, -0.7071, 0.0 3, 0.0 The rebars are located at the midsurface of the shell. Output variable RBANG is measured from the second isoparametric direction to the rebar. If the first isoparametric direction were chosen instead, output variable RBANG would report an angle of 165°. Visualizing rebar orientation and results in rebar Abaqus/CAE does not support visualization of element-based rebar or rebar results. Abaqus/CAE does support visualization of rebar defined as described in “Defining reinforcement,” Section 2.2.3. 2.2.5 ORIENTATIONS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Distribution definition,” Section 2.8.1 • “Material library: overview,” Section 21.1.1 • “Material data definition,” Section 21.1.2 • “Fabric material behavior,” Section 23.4.1 • “Distributed loads,” Section 33.4.3 • “Kinematic coupling constraints,” Section 34.2.3 • “Coupling constraints,” Section 34.3.2 • “Inertia relief,” Section 11.1.1 • *ORIENTATION • “Creating datum coordinate systems,” Section 62.9 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A user-defined orientation is used to define a local coordinate system for: • definition of material properties—for example, anisotropic materials or jointed materials (a local coordinate system must be defined if anisotropic material properties are defined for solid elements); • definition of local material directions, such as the in-plane fill and warp yarn directions of a fabric material or the fiber directions of anisotropic hyperelastic materials; • definition of rebars in shell, membrane, and surface elements; • definition of rotary inertia and connector elements; • definition of coupling constraints; • definition of loading directions for distributed general tractions, shear tractions, and general edge loads; • definition of slip directions for contact in Abaqus/Standard; • material calculations at integration points; • output of components of stress, strain, and element section force; and • definition of a local system of rigid body motion directions for inertia relief in Abaqus/Standard. A user-defined orientation cannot be used: • at points where the smeared crack concrete material behavior (“Concrete smeared cracking,” Section 23.6.1) is also used in Abaqus/Standard; • to specify a local coordinate system for defining nodal coordinates—see “Specifying a local coordinate system in which to define nodes” in “Node definition,” Section 2.1.1, or “Specifying a local coordinate system for the nodal coordinates” in “Node definition,” Section 2.1.1, instead; or • to specify a local coordinate system for applying loads and boundary conditions—see “Transformed coordinate systems,” Section 2.1.5, instead. Considerable generality is provided in the way the local system can be defined, since this system must often change from point to point because of the shape and construction of the structure being modeled. You can define the local orientation directly. The direct data methods provided in Abaqus are intended to give sufficient generality to model most cases easily: they are particularly useful for regular geometry. Distributions (“Distribution definition,” Section 2.8.1) can be used to define spatially varying local coordinate systems for solid continuum, shell, and membrane (in Abaqus/Standard) elements directly for arbitrary geometries. In Abaqus/Standard you can alternatively define the local orientation in user subroutine ORIENT. Assigning a name to an orientation You must assign a name to each orientation definition. This name is used by various features to refer to the orientation definition. Input File Usage: Abaqus/CAE Usage: *ORIENTATION, NAME=name Any module: Tools→Datum: Type: CSYS: select any method, and click OK: Name: name Defining a local coordinate system in a model that contains an assembly of part instances In a model defined in terms of an assembly of part instances, you can define a local orientation at the part, part instance, or assembly level. An orientation defined at the part or part instance level is rotated according to the positioning data given for each instance of that part (or for the part instance). This includes the case when an orientation is defined using a distribution. See “Defining an assembly,” Section 2.10.1, and “Distribution definition,” Section 2.8.1. Defining a local coordinate system directly A two-stage process is used to define the local system directly. 1. You define the local coordinate system at the particular location at which it is required. You can select a rectangular, cylindrical, or spherical coordinate system. The coordinate system is defined in terms of points a, b, and c, as shown in Figure 2.2.5–1. You can select the method for defining points a, b, and c, as described below. , or 2. Optionally, you can specify an additional rotation by identifying one of these local directions ( , ) as a rotation axis and giving a rotation, in degrees, about that axis. The local system is then rotated through this angle about the specified axis. This method of defining a local system is required for contact surfaces in Abaqus/Standard, shells, membranes, gasket elements, and when the orientation is associated with a composite solid section. The additional rotation is illustrated in Figure 2.2.5–2. Rectangular system (a on X'-axis) Cylindrical system Spherical system Rectangular system (a on Z'-axis) Y b a X X (radial) Y (tangential) Z (meridional) X (global) X (global) Y (circumferential) X (radial) X (global) Y X b a Z c X (global) Figure 2.2.5–1 Orientation systems. a. 1-direction specified. b. 2-direction specified. c. 3-direction specified. 2 (3) 1 (2) 1 (2) 2 (3) 2 (3) 1 (2) Figure 2.2.5–2 Specifying rotation about a local axis for shell elements, membrane elements, gasket elements (in parentheses), composite solids (in parentheses), and contact surfaces in Abaqus/Standard. . The local The local coordinate system for composite solids is indicated by coordinate system for other element types is indicated by 1, 2, and 3; the axis labels in parentheses are oriented for gasket elements. , and , Available coordinate systems Rectangular, cylindrical, and spherical coordinate systems are available. Defining a rectangular coordinate system A rectangular Cartesian coordinate system is shown in Figure 2.2.5–1(a). The rectangular coordinate system is the default. Alternatively, you can define a rectangular Cartesian coordinate system as shown in Figure 2.2.5–1(d). Input File Usage: Abaqus/CAE Usage: *ORIENTATION, NAME=name, SYSTEM=RECTANGULAR *ORIENTATION, NAME=name, SYSTEM=Z RECTANGULAR Any module: Tools→Datum: Type: CSYS: select any method, and click OK: Rectangular Defining a cylindrical coordinate system A cylindrical coordinate system is shown in Figure 2.2.5–1(b). The local axes are =radial, =tangential, =axial. Input File Usage: Abaqus/CAE Usage: *ORIENTATION, NAME=name, SYSTEM=CYLINDRICAL Any module: Tools→Datum: Type: CSYS: select any method, and click OK: Cylindrical Defining a spherical coordinate system A spherical coordinate system is shown in Figure 2.2.5–1(c). The local axes are =radial, =circumferential, =meridional. Input File Usage: Abaqus/CAE Usage: *ORIENTATION, NAME=name, SYSTEM=SPHERICAL Any module: Tools→Datum: Type: CSYS: select any method, and click OK: Spherical Methods for defining a coordinate system You can define a coordinate system by specifying the locations of points a, b, and c directly; by specifying the locations of points a, b, and c relative to global node numbers; by specifying the locations of points a, b, and c relative to local node numbers; by specifying an offset from another coordinate system; or by specifying two lines in the coordinate system. Defining a coordinate system by specifying the locations of points a, b, and c directly You can specify the coordinates of points a, b, and c directly. These coordinates should be appropriate to the system chosen. This method is the default. You can define a rectangular Cartesian coordinate system (a, b, and c) that lie on the point a must lie on the -axis, and point b must lie on the intuitive to select point b such that it is on or near the local - - -axis. by specifying three points plane, as shown in Figure 2.2.5–1(a). Point c is the origin of the system, plane. Although not necessary, it is by specifying three points (a, b, and c) that lie on the Alternatively in Abaqus/Standard you can define a rectangular Cartesian coordinate system plane, as shown in -axis, and point b must plane. Although not necessary, it is intuitive to select point b such that it is on or near Figure 2.2.5–1(d). Point c is the origin of the system, point a must lie on the lie on the the local - -axis. - For rectangular coordinate systems the default location of the origin (point c) is the global origin. You define a cylindrical coordinate system by giving the two points, a and b, on the polar axis of the cylindrical system, as shown in Figure 2.2.5–1(b). You define a spherical coordinate system by giving the center of the sphere, a, and point b on the polar axis, as shown in Figure 2.2.5–1(c). To define a spatially varying local coordinate system directly on solid continuum and shell elements, you can specify the coordinates of points a and b on an element-by-element basis using a distribution. Using a distribution to define the coordinates of the optional point c is not currently supported. See “Distribution definition,” Section 2.8.1. Input File Usage: Abaqus/CAE Usage: *ORIENTATION, NAME=name, DEFINITION=COORDINATES Any module: Tools→Datum: Type: CSYS, Method: 3 points Defining a coordinate system by giving global node numbers for points a, b, and c You can locate points a, b, and c at nodes by specifying three global node numbers. For a rectangular coordinate system the default location of the origin (point c) is the global origin. Input File Usage: Abaqus/CAE Usage: *ORIENTATION, NAME=name, DEFINITION=NODES You cannot define a coordinate system by giving global node numbers in Abaqus/CAE. Defining a coordinate system by giving local node numbers for points a, b, and c You can locate points a, b, and c by specifying the local node numbers of an element. Local node numbers refer to the order in which nodes are specified in the element connectivity. For example, local node number 2 corresponds to the second node specified for the element definition. This definition method allows for variation of the local coordinate system on an element-by-element basis with a single orientation definition. For example, if local node number 2 is given as the location of point c and local node number 3 is given as the location of point a, the local -direction is defined to be parallel to the (2, 3) side of the element. By default, the origin (point c) of the local coordinate system is the first node of the element (local node number 1). Input File Usage: Abaqus/CAE Usage: *ORIENTATION, NAME=name, DEFINITION=OFFSET TO NODES You cannot define a coordinate system by giving local node numbers in Abaqus/CAE. Defining a coordinate system by giving an offset from another coordinate system You can define a coordinate system by specifying an offset from an existing coordinate system. Input File Usage: You cannot define a coordinate system by giving an offset from another coordinate system in the input file. Abaqus/CAE Usage: Any module: Tools→Datum: Type: CSYS: Offset from CSYS Defining a coordinate system by giving two edges You can define a coordinate system by specifying two edges. The first edge defines the X- or R-axis, and the X–Y or plane passes through the second. Input File Usage: You cannot define a coordinate system by giving two edges in the input file. Abaqus/CAE Usage: Any module: Tools→Datum: Type: CSYS: 2 lines Defining local material directions for anisotropic hyperelastic materials When modeling anisotropic hyperelastic materials with an invariant-based formulation (“Invariant-based formulation” in “Anisotropic hyperelastic behavior,” Section 22.5.3) you must define the local directions that characterize each family of fibers. These directions need not be orthogonal in the initial configuration. You can specify these local directions with respect to an orthogonal orientation system at a material point. Up to three local directions can be specified as part of the definition of a local orientation system. The local directions can be output as field variables to the output database . Input File Usage: Use the following option to define an orthogonal system and N local directions with respect to that system to identify the preferred directions of an anisotropic hyperelastic material: Abaqus/CAE Usage: *ORIENTATION, LOCAL DIRECTIONS=N Local material directions cannot be defined in Abaqus/CAE. Defining yarn directions in the reference configuration for a fabric material In general, the yarn directions in a fabric material may not be orthogonal to each other in the reference configuration . You can specify these local directions with respect to the in-plane axes of an orthogonal orientation system at a material point. Both the local directions and the orthogonal system are defined together as a single orientation definition. If the local directions are not specified, these directions are assumed to match the in-plane axes of the orthogonal system defined. The local direction may not remain orthogonal with deformation. Abaqus updates the local directions with deformation and computes the nominal strains along these directions and the angle between them (the fabric shear strain). The constitutive behavior for the fabric defines the nominal stresses in the local system in terms of the fabric strain. The local directions can be output as field variables to the output database . Input File Usage: Use the following option to define an orthogonal system and the local directions with respect to that system to identify the yarn directions in the reference configuration: Abaqus/CAE Usage: *ORIENTATION, LOCAL DIRECTIONS=2 Yarn directions for fabric materials cannot be defined in Abaqus/CAE. Defining a local coordinate system in Abaqus/Standard using a user subroutine In some cases the simplest way to specify a local system is by means of a user subroutine. User subroutine ORIENT is provided in Abaqus/Standard. In this case the user subroutine is called each time that an orientation definition is needed. In a model defined in terms of an assembly of part instances, the local directions defined by user subroutine ORIENT must be defined relative to the coordinate system of the assembly. Input File Usage: *ORIENTATION, NAME=name, SYSTEM=USER Abaqus/CAE Usage: You can enter the name of an orientation defined in user subroutine ORIENT whenever a user-defined orientation is allowed. Multiple references to an orientation definition Because the orientation is independent of the material definition and they can both be referenced in any element property definition, the ability to describe complex structural components (such as laminated composite shells) is quite general and straightforward to use. An orientation definition can be used as often as needed and with different material or element type definitions; for example, it can be used for different layers of a shell where the orientation is the same. Large-displacement considerations In large-displacement analysis a user-defined orientation rotates with the average rigid body motion of the material point, the rigid body when the orientation is used with ROTARYI elements, the first node of the joint in JOINTC elements, the pipeline edge for pipe-soil interaction elements, the appropriate surface for contact in Abaqus/Standard, or the reference node when the orientation is used with coupling constraints. However, when an orientation is defined for spring, dashpot, or gasket elements in Abaqus/Standard, the local directions always remain fixed in space. Because the material directions rotate with the average rigid body motion at a material point, using anisotropic elasticity to model a material that is not truly a continuum can give significant errors if shear deformation is large. For example, an individual fiber in a reinforcing belt of a tire can shear relatively easily with respect to fibers in other directions. The fibers rotate with the actual deformation of the material point and not with the average rigid body motion. In this case the anisotropic behavior is better modeled with rebars or as a fabric material. The fabric material model in Abaqus/Explicit tracks the current yarn directions as local directions with respect to the orthogonal coordinate system. Use with two-dimensional solid elements When a user-defined orientation is used with two-dimensional solid elements such as plane stress, plane strain, or torsionless axisymmetric elements, the orientation must redefine only the X- and Y-directions: the third direction must remain unchanged (Z-direction for plane strain and plane stress elements, -direction for axisymmetric elements). When a user-defined orientation is used with axisymmetric elements with twist, all three directions can be redefined. For axisymmetric elements, including the CGAX and CAXA families of elements, the global 1-, 2-, and 3-directions are the radial, axial, and hoop directions, respectively. Cylindrical or spherical orientations may be appropriate for axisymmetric elements only if the local -direction is in the global 3-, or hoop, direction. Use with shell, membrane, or gasket elements or contact surfaces When a user-defined orientation is used with shell, membrane, or gasket elements or with contact surfaces, Abaqus first rotates and then projects the orientation system onto the element or contact surface using the algorithm described in this section. Abaqus first rotates (through the additional rotation angle) the user-defined local coordinate system about the specified rotation axis. If you do not specify a rotation axis or an additional angle, Abaqus will by default use the local 1-axis and a rotation of 0°. After the rotation, Abaqus follows a cyclic permutation (1, 2, 3) of the axes and projects the axis following the axis for additional rotation onto the contact surface or onto the surface of the element to form the local material 1-direction (or the local material 2-direction for gaskets). The remaining material direction is then defined by the cross product of the element normal and the projected direction. Thus, for example: 1. If you choose the user-defined 1-axis as the axis for additional rotation, Abaqus projects the 2-axis onto the element or contact surface. This will be local direction 1 for contact surfaces, shells, and membranes and local direction 2 for gaskets. 2. Abaqus takes the positive element or contact surface normal as the local 3-direction for contact surfaces, shells, and membranes and the local 1-direction for gaskets. 3. Abaqus computes the local 2-direction (3-direction for gaskets) by taking the cross product of the element or contact surface normal and the local 1-direction (2-direction for gaskets), such that the three local axes form an orthonormal, right-handed local coordinate system. When the axis for additional rotation points in a direction that is opposite to the element or contact surface normal, the local 2-direction (3-direction for gaskets) is reversed with respect to the corresponding user- defined axis; see Figure 2.2.5–3. This does not apply in the case of an orientation used to define rebars; see below. S1 S2 S1 normal defined by local orientation definition is opposite to element normal S2 orientation used by Abaqus S = user-defined directions Figure 2.2.5–3 The local 3-direction (1-direction for gaskets) will be in the same direction as the element or contact surface normal. As an example, the orientation of the spiral-wound layer of the cylindrical shell shown in Figure 2.2.5–4 would be given by defining a cylindrical coordinate system and then specifying the (in degrees). The local 1- and 2-directions for rotation axis as the 1-axis and giving the rotation angle material property specification and material calculations are then those indicated in the figure. Figure 2.2.5–4 Spiral-wound cylindrical shell layer: material orientation example. The projected directions are most easily understood when the axis for additional rotation is approximately perpendicular to the element or contact surface. To define a spatially varying local coordinate system directly on solid continuum and shell elements, as well as membrane elements in Abaqus/Standard, you can specify the additional angle of rotation on an element-by-element basis using a distribution. See “Distribution definition,” Section 2.8.1. Defining rebars in shell, membrane, and surface elements The orientation of skew rebars in shell, membrane, and surface elements can be defined relative to a user-defined orientation . In this case the local coordinate system is calculated as follows: 1. The local 1-direction follows a cyclic permutation of the additional rotation direction; for example, if you choose the user-defined 1-axis as the axis for additional rotation, Abaqus projects the 2-axis onto the element. This will be the local 1-direction. 2. The axis for additional rotation is made orthogonal to the element to create the local 3-direction. This local 3-direction need not be in the same direction as the element normal; in fact it will be in the opposite direction when the dot product of the axis for additional rotation and the element normal is negative. 3. Abaqus computes the local 2-direction by taking the cross product of the local 3-direction and the local 1-direction, such that the three local axes form an orthonormal, right-handed local coordinate system. Since the local 3-direction may be opposite to the element normal, the definition of rebars is independent of the element connectivity. Special considerations when defining orientations on contact surfaces in Abaqus/Standard When a user-defined orientation is used to define the tangential slip directions on a surface of a three-dimensional contact pair in Abaqus/Standard , you cannot define points a and b by giving local node numbers . For geometrically nonlinear analysis the tangential slip directions of a contact pair rotate with the surface on which the directions were defined initially. These rotated tangential slip directions are further rotated to ensure that the normal vector, computed using the cross product of the rotated tangential slip directions, corresponds to the normal vector on the master surface when the slave node comes into contact. Arbitrary slip directions can be defined for a “line”-type slave surface defined on three-dimensional beam, truss, or pipe elements. When this surface comes into contact with the master surface during a large-displacement analysis, the slip directions are projected onto the master surface. Use with laminated shells There are two ways in which a user-defined orientation can be used in the section definition of a laminated shell. In each case the name referenced in the shell section definition is the name of the user-defined orientation. The first is to associate the user-defined orientation with the entire composite shell section definition. Then each layer’s orientation angle can be given relative to this section orientation (or the default shell coordinate directions if no section orientation is used). The angle is given as an additional rotation about the shell normal after the orientation directions have been projected onto the shell surface. Section forces (available only from Abaqus/Standard) are given in the local system specified for the section. The second is to specify the name of each layer’s orientation separately; this method allows different orientation definitions to be referenced for the different layers. Section forces and strains are still reported in the local orientation defined for the entire section (or the default shell coordinate directions if no section orientation is used). The individual layer orientations are used for material calculations and for output of stress and strain. See “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, and “Using a general shell section to define the section behavior,” Section 29.6.6, for more information. Use with laminated three-dimensional solid elements When a user-defined orientation is used with composite solid elements (available only in Abaqus/Standard), one of the local directions must be identified as the axis for additional rotation. There are two ways in which this orientation can be used with a composite solid section definition to specify the material orientation for individual layers. In each case the name referenced in the solid section definition is the name of the user-defined orientation. The first is to associate the user-defined orientation with the entire composite solid section definition. Then each layer’s orientation angle can be given relative to this section orientation. The angle is given as an additional rotation about the local direction defined as the axis for additional rotation. The second is to specify the name of each layer’s orientation separately; this method allows different orientation definitions to be referenced for the different layers. (In this case any user-defined orientation associated with the entire solid section will be ignored.) See “Defining the element’s section properties” in “Solid (continuum) elements,” Section 28.1.1, for more information. Use with pipe-soil interaction elements An arbitrary user-defined orientation can be defined for pipe-soil interaction elements (available only in Abaqus/Standard). In a large-displacement analysis the local orientation system rotates with the rigid body motion of the underlying pipeline. In a small-displacement analysis the local system is defined by the initial geometry of the PSI element and remains fixed in space during the analysis. Use with beam, frame, and truss elements See “Beam element cross-section orientation,” Section 29.3.4, for information on defining local material directions for beams, frames, or trusses. Use with the fabric material model The fill and the warp yarn directions in the fabric plane are allowed to rotate with respect to each other under shear deformations (“Fabric material behavior,” Section 23.4.1). The current yarn directions are tracked with respect to the orthogonal coordinate system that also rotates with the material. Use with the jointed material model When a user-defined orientation is used to define a joint system orientation for the jointed material model available in Abaqus/Standard (“Jointed material model,” Section 23.5.1), only the local coordinate system need be defined. It is assumed that the first direction is the direction normal to the plane of the joint and the other directions are in the plane of the joint. An additional axis of rotation cannot be used. Use with rotary inertia and connector elements A user-defined orientation must be used to define the local directions for certain connection types used to define connector elements . A user-defined orientation can be used with SPRING1, SPRING2, DASHPOT1, DASHPOT2, JOINTC, JOINT2D, JOINT3D, and ROTARYI elements to provide a local system for defining the direction of action of such elements. Points a, b, and c cannot be defined by giving local node numbers when the orientation is used for these elements. If you do not specify an axis for additional rotation, the local 1-direction with no additional rotation will be chosen as the default. Use with the kinematic coupling constraint User-defined orientations can be used in Abaqus/Standard to define the local coordinate systems in which constraint directions are specified for a kinematic coupling constraint (see “Kinematic coupling constraints,” Section 34.2.3). In this case you cannot define points a, b, and c by giving local node numbers . Use with surface-based coupling constraints User-defined orientations can be used to define the local coordinate systems in which surface-based coupling constraint directions are specified . In this case you cannot define points a, b, and c by giving local node numbers . Use with inertia relief A user-defined orientation can be used in Abaqus/Standard to define a local system of directions along which the inertia relief loads are computed . In this case you cannot define points a, b, and c by giving local node numbers . Use with distributed general traction, shear traction, and general edge loads User-defined orientations can be used in Abaqus to define the local coordinate systems in which the loading directions for distributed general tractions, shear tractions, and general edge loads are specified. See “Distributed loads,” Section 33.4.3. Orientations defined with distributions Spatially varying local coordinate systems (for material definitions, material calculations, and output) defined with a distribution can be applied only to solid continuum, membrane (in Abaqus/Standard), and shell elements. See “Solid (continuum) elements,” Section 28.1.1; “Membrane elements,” Section 29.1.1; “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5; and “Using a general shell section to define the section behavior,” Section 29.6.6. Output When a user-defined orientation is used in an element section definition, the stress, the strain, and the element section force components are output in the local system. For a fabric material the output of the regular material point tensors such as stress and strain are given in an orthogonal coordinate system even when the local yarn directions are non-orthogonal. However, the nominal fabric stress SFABRIC and the nominal fabric strain EFABRIC are also available for output . This use of a local system is indicated by a footnote in the printed output Abaqus/Standard. An orientation used with the jointed material model does not affect the output. tables from When a user-defined orientation is used in Abaqus/Standard with kinematic or distributing coupling constraints, the local system is indicated in the analysis input file processor output tables. Local coordinate systems are written automatically to the output database with the exception of systems defined by specifying points a and b relative to local or global node numbers or systems defined through a user subroutine. Any additional rotations specified are ignored. Material directions are written automatically to the output database. They can also be written to the Abaqus/Standard results file (with at least one output variable specified; see “Output of local directions to the results file” in “Output to the data and results files,” Section 4.1.2). The material directions can be visualized in Abaqus/CAE by selecting Plot→Material Orientations in the Visualization module. 2.3 Surface definition • “Surfaces: overview,” Section 2.3.1 • “Element-based surface definition,” Section 2.3.2 • “Node-based surface definition,” Section 2.3.3 • “Analytical rigid surface definition,” Section 2.3.4 • “Eulerian surface definition,” Section 2.3.5 • “Operating on surfaces,” Section 2.3.6 2.3.1 SURFACES: OVERVIEW Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Element-based surface definition,” Section 2.3.2 • “Node-based surface definition,” Section 2.3.3 • “Analytical rigid surface definition,” Section 2.3.4 • “Eulerian surface definition,” Section 2.3.5 • “Operating on surfaces,” Section 2.3.6 • “Integrated output section definition,” Section 2.5.1 • “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1 • “Distributed loads,” Section 33.4.3 • “Prescribed assembly loads,” Section 33.5.1 • “Mesh tie constraints,” Section 34.3.1 • “Coupling constraints,” Section 34.3.2 • “Shell-to-solid coupling,” Section 34.3.3 • “Contact interaction analysis: overview,” Section 35.1.1 • “Defining tied contact in Abaqus/Standard,” Section 35.3.7 • “Cavity radiation,” Section 40.1.1 Overview In Abaqus surfaces: • can be used to define contact and interactions, including acoustic-structural interactions; • can define regions used to prescribe distributed surface loads; • can be used to tie dissimilar meshes together; • can define cavities used for a cavity radiation analysis in Abaqus/Standard; • can define pre-tensioned sections used in prescribing assembly loads in Abaqus/Standard; • can define sections used for tracking the average motion of a surface in Abaqus/Explicit; • can define sections for output quantities such as the total force transmitted through a surface; • are geometric entities that have an area associated with them but have zero volume; • have an identifiable orientation defined by their normals; • are defined by specifying nodes or node sets, an analytic curve or surface, an Eulerian material instance, or element faces, edges, or ends; and • can be deformable, rigid, or partially deformable and partially rigid. This section describes the general rules that apply when creating surfaces in Abaqus. Why use surfaces? Surfaces can be used to model the interaction of two or more distinct bodies in a mechanical, acoustic, coupled acoustic-structural, coupled thermal-mechanical, coupled thermal-electrical-structural, thermal, coupled thermal-electrical, or cavity radiation analysis. A rigid surface can be used to represent a body that is much stiffer than the rest of the model in a mechanical or coupled thermal-mechanical analysis, with the limitation that no heat can be transferred to the rigid body. In acoustic-structural analysis, surfaces can be used to define impedance boundary conditions, including first-order conditions for modeling acoustic radiation. Surfaces can be used to define a region on which a distributed surface load is prescribed; this can facilitate user input of distributed surface loads for complex models. In addition, surfaces can be used to define multi-point or coupling constraints. Surfaces can also define pre-tension sections used in prescribing assembly loads in Abaqus/Standard. Finally, surfaces can be used to define sections to obtain output of accumulated quantities; this provides a “free body diagram” output, allowing analyses of “force-flow” through a statically indeterminate structure. The following types of surfaces can be defined in Abaqus: • Element-based surfaces are defined on the faces, edges, or ends of elements. The elements can be deformable or rigid, leading to a surface that is deformable or rigid. When some of the deformable elements underlying a surface are part of a rigid body, the surface will become partially deformable and partially rigid. In Abaqus/Explicit a default element-based surface that includes all bodies in the model is provided for use with the general contact algorithm. • Node-based surfaces are defined on nodes and, hence, are by definition discontinuous. A user- defined area can be associated with each node on the surface. • Analytical surfaces are defined directly in geometric terms and are always rigid. • Eulerian material surfaces are defined on material instances in an Eulerian section. These surfaces are available in Abaqus/Explicit for use with the general contact algorithm. Element-based surfaces contain more intrinsic information than either node-based surfaces or analytical rigid surfaces. When an element-based surface is used in a mechanical contact analysis, Abaqus can associate a surface area with each node and can calculate the contact stress acting on the surface. In contrast, Abaqus may not be able to calculate accurate contact stresses when a node-based surface (“Node-based surface definition,” Section 2.3.3) is used because the actual area associated with each node may not be correct. In addition, when a surface formed by shell, membrane, or rigid elements is used, Abaqus can consider the thickness and possibly the offset of the reference surface of these elements in some applications that refer to surfaces. For example, these thicknesses are accounted for by all contact algorithms available in Abaqus/Explicit and by the surface-to-surface, small-sliding contact formulation in Abaqus/Standard. Contact between two node-based surfaces or a node-based surface with itself is not allowed; contact between two analytical rigid surfaces is not allowed. Contact between two rigid surfaces defined using rigid elements is not allowed in Abaqus/Standard and is allowed only with penalty contact in Abaqus/Explicit. Surface definitions cannot change from step to step; however, new surfaces can be defined upon restart. Internal surfaces created by Abaqus/CAE In Abaqus/CAE many modeling operations are performed by picking geometry with the mouse. For example, a contact pair can be defined by picking faces on geometric part instances. Each such face must be translated into a surface in the input file. Such a surface is assigned a name by Abaqus/CAE and is marked as internal. These internal surfaces can be viewed using display groups in the Visualization module of Abaqus/CAE . Input File Usage: *SURFACE, NAME=surface_name, INTERNAL Restrictions on surfaces Refer to the subsequent sections on the different surface types available in Abaqus for details on the In addition, some features general restrictions that apply to all surface definitions of a given type. in Abaqus that use surfaces impose other restrictions on surface characteristics. These limitations are discussed in the following sections: • “Integrated output section definition,” Section 2.5.1 • “Distributed loads,” Section 33.4.3 • “Mesh tie constraints,” Section 34.3.1 • “Coupling constraints,” Section 34.3.2 • “Shell-to-solid coupling,” Section 34.3.3 • “Contact interaction analysis: overview,” Section 35.1.1 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1 • “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1 In models that are defined in terms of an assembly of part instances, all surfaces must belong to a part, part instance, or the assembly. All of the general restrictions on surfaces still apply in such models. Additional rules are given in “Defining an assembly,” Section 2.10.1. 2.3.2 ELEMENT-BASED SURFACE DEFINITION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Surfaces: overview,” Section 2.3.1 • “Integrated output section definition,” Section 2.5.1 • “Distributed loads,” Section 33.4.3 • “Prescribed assembly loads,” Section 33.5.1 • “Mesh tie constraints,” Section 34.3.1 • “Coupling constraints,” Section 34.3.2 • “Shell-to-solid coupling,” Section 34.3.3 • “Contact interaction analysis: overview,” Section 35.1.1 • “Cavity radiation,” Section 40.1.1 • *SURFACE • “What is a surface?,” Section 73.2.3 of the Abaqus/CAE User’s Manual Overview An element-based surface: • can be defined on solid, structural, rigid, surface, gasket, or acoustic elements; • can be deformable or rigid; • can be defined on any combination of elements in many cases; • can be defined on the exterior of any body; and • can be defined on the interior of any body that is modeled with continuum, shell, membrane, surface, beam, pipe, truss, or rigid elements (e.g., to define a cross-section through a body) either by simply cutting the body with a plane or by identifying the elements and the corresponding interior facets. For details about defining node-based surfaces, see “Node-based surface definition,” Section 2.3.3. For details about defining analytical rigid surface definition,” Section 2.3.4. For details about defining surfaces using Boolean combinations of existing surfaces, see “Operating on surfaces,” Section 2.3.6. rigid surfaces, see “Analytical Defining element-based surfaces You must assign a name to all element-based surfaces; this name can be used with various features to define a contact model, a surface-based load, or a surface-based constraint. In addition, you must specify the region of your model on which the surface is defined. In an input file you can define element-based surfaces on element faces, edges, or ends. In Abaqus/CAE you can define element-based surfaces on geometric or element faces, edges, or ends. The methods for defining surfaces depend on the underlying element type and are discussed later in this section. In an input file you need only specify an element number or element set name and all exposed element faces of these elements (or “contact edges” of beam, pipe, and truss elements) will be included in the surface. Optionally(and the only available method in Abaqus/CAE), you can specify individual faces, edges, or ends, which allows you direct control over which faces, edges, or ends are to be included in the surface. For general contact in Abaqus/Explicit the surface perimeter edges are generated automatically from the surface facets for use in edge-to-edge contact constraints; you can specify that geometric feature edges should be included as well . Input File Usage: *SURFACE, NAME=surface_name, TYPE=ELEMENT (default) An element number or element set name is specified as the first entry of each data line. Optionally, an element face, edge, or end identifier can be specified as the second entry on a data line. The face and edge identifiers used in Abaqus are discussed later in this section. Multiple data lines can be used to define a surface. For example, SURF_1 can be specified by the following input: *SURFACE, NAME=SURF_1, TYPE=ELEMENT ELSET_1, ELSET_2, S2 Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name General restrictions on element-based surfaces Elements defining a single surface must satisfy the following rules, regardless of how the surface is used in Abaqus: • Two-dimensional, axisymmetric, and three-dimensional elements cannot be mixed in the same surface definition. • In Abaqus/Standard deformable elements cannot be combined with rigid elements to define a single surface, but can be combined with other deformable elements that are part of a rigid body . • The following element types cannot be mixed with other element types in the same surface definition: – Coupled thermal-electrical-structural elements – Coupled temperature-displacement elements – Heat transfer elements – Pore pressure elements – Coupled thermal-electrical elements – Acoustic finite or infinite elements • The axisymmetric solid Fourier elements with nonlinear, asymmetric deformation (CAXA elements) cannot form element-based surfaces. Surface discretization For element-based surfaces Abaqus uses a faceted geometry defined by the finite element mesh as the surface definition. The surface in a coarse finite element model may not be a very good approximation for contact modeling if the physical surface is curved. Therefore, sufficient mesh refinement must be used to ensure that the faceted surface is a reasonable approximation of the curved physical surface. Alternatively, some curved surface geometries may be more effectively modeled with analytical rigid surfaces . Creating surfaces on solid, continuum shell, and cohesive elements There are three ways to define the facets of an element-based surface on solid, continuum shell, and cohesive elements: 1. by instructing Abaqus to generate the “free surface” from the exposed faces of elements, 2. by specifying the particular faces for each element, and 3. in Abaqus/Explicit by instructing Abaqus to generate an interior surface from element faces that are not exposed (i.e., not part of the “free surface” of the model). The automatic free surface generation approach is the simplest method of defining exterior surfaces on solid elements. Specifying the element faces gives you exact control over which element faces (any combination of exterior and interior faces) form the surface. Automatic generation of an interior surface is the simplest method of defining interior surfaces on solid elements (interior surfaces can be useful for modeling surface erosion due to element failure). It is possible to use all three approaches in the same surface definition when creating a single surface. Generating the free surface automatically You can define the facets of a surface by specifying a series of elements. The faces of these elements that are on the exterior (free) surface of the model are included in the surface definition. When the free surface generation method is used to define surfaces, the specified elements can be a mixture of continuum and structural elements. Multi-point constraints (“General multi-point constraints,” Section 34.2.2) involving nodes on exposed surfaces are not taken into account during free surface generation, which can result in faces that are not on the exterior of a body being included in surface definitions. For example, the nodes of the elements in element set REFINED shown in Figure 2.3.2–1 are used in linear, mesh-refinement constraints. The surfaces generated with and without multi-point constraints are shown in Figure 2.3.2–1. with MPCs: Surface SURF generated by specifying element set REFINED ⇒ element set "REFINED" resulting surface "SURF" without MPCs: ⇒ element set "REFINED" resulting surface "SURF" Figure 2.3.2–1 Effect of multi-point constraints on automatic surface generation. Input File Usage: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, For example, if the name of the shaded element set in Figure 2.3.2–2 is ESETA, the surface named ASURF is specified by *SURFACE, NAME=ASURF, TYPE=ELEMENT ESETA, Abaqus/CAE Usage: The automatic free surface generation method is not supported in Abaqus/CAE. Special treatment of cohesive elements for automatic free surface generation The definition of exposed faces of elements for the purpose of automatic free surface generation has the following unique aspects regarding cohesive elements: • Faces of non-cohesive elements along an interface of shared nodes with cohesive elements are considered exposed. • The top and bottom faces of all cohesive elements are considered exposed; side faces of cohesive elements are never considered exposed. See “Modeling with cohesive elements,” Section 32.5.3, for examples of surfaces on or near cohesive elements. FEM model perimeter ⇒ user-specified element set automatically generated surface Figure 2.3.2–2 Automatic free surface generation. Creating surface facets by specifying solid, continuum shell, and cohesive element faces You can define the facets of a surface by identifying the element faces that should be included in the surface definition. Input File Usage: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or set, face identifier Element face numbers are defined in Part VI, “Elements.” Table 2.3.2–1 contains a list of valid face identifiers for all solid, continuum shell, and cohesive elements. The face identifier can refer to individual elements or to entire element sets. When you specify the element faces to define surfaces, the specified elements cannot be a mixture of continuum and structural elements; however, each data line of the surface definition can refer to different element types. Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick faces in viewport Generating an interior surface automatically In Abaqus/Explicit you can define the facets of a surface on the interior of a solid element mesh. The faces of the specified elements that are not on the exterior (free) surface of the model will be included in the surface definition. For example, interior surfaces are used with the general contact algorithm in Abaqus/Explicit for modeling surface erosion due to element failure . Table 2.3.2–1 Surface definition face identifier labels for solid, continuum shell, and cohesive elements. Face Labels SPOS, SNEG S1, S2, S3 S1, S2, S3, S4 S1, S2, S3, S4, S5 S1, S2, S3, S4, S5, S6 Elements DCCAX2(D) CPEG3(H)(T) CPS3(T) CPE3(H)(T) CAX3(H)(T) CGAX3(H) AC2D3 ACAX3 DC2D3(E) DCAX3(E) CGAX4(R)(H)(T) CPEG4(H)(I)(R)(T) CPS4(I)(R)(T) CPE4(H)(I)(R)(T)(P) CAX4(H)(I)(R)(T)(P) C3D4(H)(T) AC2D4(R) ACAX4(R) AC3D4 DC2D4(E) DCAX4(E) DC3D4(E) DCC2D4(D) COH2D4 C3D6(H)(T) AC3D6 CCL9(H) DC3D6(E) SC6R C3D8(H)(I)(R)(T)(P) C3D27(R)(H) AC3D8(R) CCL12(H) DC3D8(E) DCC3D8(D) SC8R CPEG6(M)(H)(T) CPS6M(T) CPE6(M)(H)(T) CAX6(M)(H)(T) CGAX6(M)(H)(T) AC2D6 ACAX6 DC2D6(E) DCAX6(E) CGAX8(R)(H) CPEG8(R)(H)(T) CPS8(R)(T) CPE8(H)(R)(T)(P) CAX8(R)(H)(T)(P) C3D10(M)(H)(I)(T) AC2D8 ACAX8 AC3D10 DC2D8(E) DCAX8(E) DC3D10(E) DCCAX4(D) COHAX4 C3D15(H)(V) AC3D15 CCL18(H) DC3D15(E) COH3D6 C3D20(H)(R)(T)(P) AC3D20 CCL24(R)(H) DC3D20(E) COH3D8 The automatic generation of an interior surface is equivalent to constructing a surface consisting of all faces of the elements and then subtracting the free surfaces of those elements. Shell elements, beam elements, pipe elements, membrane elements, etc. are ignored since they do not have any interior faces by definition. Multi-point constraints are not taken into account when generating interior surfaces. This can result in faces that are on the interior of a body being excluded from the surface definition. Input File Usage: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, INTERIOR For example, if the name of the shaded element set in Figure 2.3.2–3 is ESETA, the surface named ASURFINTR (the elements in the figure have been reduced in size to differentiate faces that share the same nodes) is specified by *SURFACE, NAME=ASURFINTR, TYPE=ELEMENT ESETA, INTERIOR Abaqus/CAE Usage: The generation of interior surfaces is not supported in Abaqus/CAE. FEM model ⇒ user-specified element set surface ASURFINTR drawn with solid lines Figure 2.3.2–3 Automatic interior surface generation. Creating surfaces on structural, surface, and rigid elements There are five ways to define surfaces on structural, surface, and rigid elements: 1. You can create a single-sided surface with a well-defined orientation by indicating either the top or bottom surface of each specified element. 2. You can create a double-sided surface by specifying only the elements and letting Abaqus generate the “free surface” from the exposed faces. 3. You can create an edge-based surface. 4. You can create a cross-section surface on the ends of beam, pipe, and truss elements. 5. You can create a three-dimensional curve-type surface along the length of beam, pipe, and truss elements by specifying only the elements and letting Abaqus generate the “free surface.” It is possible to use any or all of the above approaches in the same surface definition as long as it makes sense in the use of that surface with other features in Abaqus. Table 2.3.2–2 contains a list of valid face and edge identifiers for structural, surface, and rigid elements. Table 2.3.2–2 Surface definition face and edge identifier labels for structural, surface, and rigid elements. Face and Edge Labels SPOS, SNEG Elements SAX2(T) MAX2 MGAX2 M3D8(R) MCL6 DS4 DSAX1 SFMAX1 SFMGAX1 SFM3D3 SFM3D6 SFMCL9 RAX2 B22(H) (Abaqus/Standard) PIPE22(H) T2D3(H)(T) END1, END2 SAX1 MAX1 MGAX1 M3D6 M3D9(R) MCL9 DS8 DSAX2 SFMAX2 SFMGAX2 SFM3D4(R) SFM3D8(R) SFMCL6 B21(H) B23(H) PIPE21(H) T2D2(H)(T) B22 (Abaqus/Explicit) B32(H)(OS) ELBOW31(B)(C) PIPE31(H) T3D2(H)(T) STRI3 S3(R)(S) M3D3 B31(H)(OS) B33(H) ELBOW32 PIPE32(H) T3D3(H)(T) STRI65 R3D3 END1, END2; must use node-based surfaces with the contact pair algorithm in Abaqus/Explicit. SPOS, SNEG, E1, E2, E3 ACIN2D2 ACINAX2 S4(R)(S)(W)(5) S9R5 M3D4(R) ACIN3D3 Elements ACIN2D3 ACINAX3 S8R5(T) R3D4 ACIN3D6 ACIN3D4 ACIN3D8 Face and Edge Labels SPOS E1, E2 SPOS, SNEG, E1, E2, E3, E4 SPOS E1, E2, E3 SPOS E1, E2, E3, E4 Defining single-sided surfaces You can define a single-sided surface on the positive or negative face of structural, surface, or rigid elements. The positive face is defined as the one in the direction of the positive element normal, and the negative face is defined as the one in the direction opposite to the element normal. The definition of the element normal for all elements is given in Part VI, “Elements.” You must ensure that all of the specified elements have their normals oriented consistently. If they are oriented as shown in Figure 2.3.2–4, the surface normals will reverse direction as the surface is traversed and improper results may occur when the surface is used with features requiring an orientation such as distributed surface loads. Further, an error message will be issued and the analysis will terminate if this condition is detected for surfaces used with mesh tie constraints in Abaqus/Standard or with contact pairs. To correct the surface orientations in this figure, two separate element sets with different face identifiers should be used. Input File Usage: Use the following option to define a surface on the positive face of a structural, surface, or rigid element: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, SPOS Use the following option to define a surface on the negative face of a structural, surface, or rigid element: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, SNEG For example, single-sided surfaces on the positive faces of the elements in element set SHELL can be defined using input similar to *SURFACE, NAME=BSURF, TYPE=ELEMENT SHELL, SPOS element set SHELL element normals Figure 2.3.2–4 Inconsistent orientation of structural element normals can result in an invalid surface. Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick face in viewport, click mouse button 2, and specify the side of the selected face Defining double-sided surfaces You can create double-sided surface facets on three-dimensional shell, membrane, surface, and rigid elements using the automatic surface facet generation approach (i.e., specifying only the element numbers or sets). Some applications that refer to surfaces do not allow the use of double-sided surfaces: examples include contact pairs in Abaqus/Standard and features requiring an oriented surface such as distributed surface loads. When double-sided surfaces can be used, they are often preferred to single-sided surfaces. In some applications, such as when defining the contact domain for general contact, it does not matter whether single- or double-sided surfaces are used. When double-sided surfaces are used with contact pairs in Abaqus/Explicit, the normals of all the underlying elements do not need to have a consistent positive orientation: Abaqus/Explicit will define the contact surface such that its facets have consistent normals, even if the underlying elements do not have consistent normals. The facet normals will be the same as the element normals if the element normals are all consistent; otherwise, an arbitrary positive orientation is chosen for the surface. The positive orientation is significant only with respect to the sign of the contact pressure output variable for the contact pair algorithm, CPRESS . Although contact is enforced unconditionally on both sides of a surface when self-contact is used with contact pairs, contact is enforced on both sides of a surface used in two-body contact only when that surface is double-sided (if allowed). The use of single-sided surfaces with contact pairs is sometimes desirable: the resolution of large initial overclosures in contact pairs is more robust with single-sided surfaces than with double-sided surfaces . However, single-sided contact is generally more limiting than double-sided contact; it may cause an analysis to fail due to excessive element distortion or not enforce the contact conditions realistically if a slave node unexpectedly moves behind a master surface. This condition can occur, for example, when large deformations or rigid-body motions are present or due to complex tool shapes in a forming analysis. Input File Usage: Use the following option to define a double-sided surface on three-dimensional shell, membrane, surface, or rigid elements in Abaqus/Explicit: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, For example, double-sided surfaces on the elements in element set SHELL can be defined using input similar to *SURFACE, NAME=BSURF, TYPE=ELEMENT SHELL, Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick face in viewport, click mouse button 2, and choose Both sides Defining edge-based surfaces You can define an edge-based surface on three-dimensional shell, membrane, surface, or rigid elements by specifying the individual edges. Alternatively, you can specify that all the edges of the elements that are on the exterior (free) surface of the model are used to form the surface; this method cannot be used to define edge-based surfaces that are in the interior of the model. It is possible to use both methods in the same surface definition when creating a single surface. Input File Usage: Use the following option to specify the individual edges that form the surface: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, edge identifier The individual edge identifiers used in Abaqus are listed in Table 2.3.2–2. Use the following option to specify that all the edges of the elements that are on the exterior (free) surface of the model are used to form the surface: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, EDGE For example, if the shaded element set in Figure 2.3.2–2 is composed of three- dimensional shell elements and is named ESETA, the surface named ESURF could be specified by the following input: *SURFACE, NAME=ESURF, TYPE=ELEMENT ESETA, EDGE Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick edges in viewport In Abaqus/CAE you can specify that all the edges of the elements that are on the exterior (free) surface of the model are used to form the surface by directly picking all the free edges in the viewport. Defining a surface over the cross-section at the ends of beam, pipe, and truss elements To define a surface over the cross-section of beam, pipe, or truss elements, you must specify the end on which the surface is defined. Surfaces created on the ends of these elements can be used only for integrated output request and integrated output section definitions. Input File Usage: Use the following option to define a surface over the cross-section of a beam, pipe, or truss element: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, END1 or END2 Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick three-dimensional wire region in viewport, click mouse button 2, and choose End (Magenta) or End (Yellow) Defining a surface along the length of three-dimensional beam, pipe, and truss elements You cannot specify the faces to define a surface along the length of three-dimensional beams, pipes, or trusses because their element connectivity cannot define a unique element or surface normal. Instead, you must specify that Abaqus should generate a surface for these elements. Therefore, the use of surfaces along the length of these elements is restricted. In Abaqus/Standard element-based surfaces created along the length of three-dimensional beam, pipe, or truss elements can be used in tie constraints but can be used only as slave surfaces in contact interactions. However, there are several advantages to using an element-based surface rather than a node-based surface when modeling contact in Abaqus/Standard with three-dimensional beams, pipes, or trusses: 1. The default slip directions are parallel and orthogonal to the element axis. 2. Abaqus/Standard calculates the contact results as contact forces per unit length rather than just contact forces. 3. It can be easier to define an element-based surface than a node-based surface. In Abaqus/Standard a surface definition is not allowed for cases where three or more three-dimensional beams, pipes, or trusses are joined at a common node because of the lack of uniquely defined element tangents. In Abaqus/Explicit element-based surfaces created along the length of three-dimensional beam, pipe, or truss elements can be used only with the general contact algorithm or tie constraints. To define contact for these elements using the contact pair algorithm, the nodes forming the beam, pipe, or truss elements can be included in a node-based surface definition (“Node-based surface definition,” Section 2.3.3) and a contact pair can be defined for this node-based surface and a non-node-based surface. Surfaces along the length of three-dimensional beam, pipe, or truss elements cannot be used to prescribe a distributed surface load since the loading direction is not unique. Input File Usage: Use the following option to define a surface along the length of a three-dimensional beam, pipe, or truss element: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick three-dimensional wire region in viewport, click mouse button 2, and choose Circumferential Surfaces along the length of two-dimensional beam, pipe, and truss elements Surfaces created along the length of two-dimensional beam, pipe, and truss elements can be used as master surfaces in a contact pair simulation because the underlying elements have unique element normals that lie in the plane of the model. These surfaces can also be used to prescribe distributed surface loads. Shell, membrane, or rigid element thickness and shell offset Some applications that refer to surfaces will account for underlying element thicknesses and any offset of the midsurface relative to the reference surface for surfaces based on shell, membrane, or rigid elements. For example, all of the contact algorithms available in Abaqus/Explicit can account for these effects. Of the contact algorithms available in Abaqus/Standard, only the surface-to-surface small-sliding contact formulation can account for these effects. See the following sections for additional details on applications that can account for surface thickness and offset: • “Mesh tie constraints,” Section 34.3.1 • “Contact formulations in Abaqus/Standard,” Section 37.1.1 • “Assigning surface properties for general contact in Abaqus/Explicit,” Section 35.4.2 • “Assigning surface properties for contact pairs in Abaqus/Explicit,” Section 35.5.2 Creating surfaces on gasket elements When surfaces are defined on gasket elements, automatic surface facet generation cannot be used because only the top and bottom element faces can be used to create surfaces . Abaqus/Standard cannot create surfaces on gasket link elements since the top and bottom surfaces are each reduced to a single node. For other gasket elements you must specify the top and bottom surfaces directly. The positive face of the element is in the thickness direction of the element. The definition of the thickness direction of all gasket elements is given in “Defining the gasket element’s initial geometry,” Section 32.6.4. The negative face is defined as the face in the direction opposite to the thickness direction of the element. Input File Usage: Use the following option to define a surface on the positive face of a gasket element: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, SPOS Use the following option to define a surface on the negative face of a gasket element: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, SNEG For example, single-sided surfaces on the positive faces of the elements in element set GASKET can be defined using input similar to *SURFACE, NAME=BSURF, TYPE=ELEMENT GASKET, SPOS Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: surface_name, pick top or bottom faces in viewport Surfaces on three-dimensional gasket line elements There are several advantages to using an element-based surface rather than a node-based surface when modeling contact in Abaqus/Standard with three-dimensional gasket line elements: 1. The slip directions are parallel and orthogonal to the gasket line element, which is useful for output purposes and for anisotropic friction definition. 2. Abaqus/Standard calculates the contact results as contact forces per unit length rather than just contact forces. Surfaces created on three-dimensional gasket line elements can be used only as slave surfaces because Abaqus/Standard cannot form unique normals for these surfaces. Creating interior cross-section surfaces To study the “force-flow” through various paths in a model, you must create interior surfaces that cut through one or more components (similar to a cross-section) so that you can request integrated output of the total force transmitted across these surfaces . Abaqus provides a simple method to create such an interior surface over the element facets, edges, or ends by cutting through a region of the model with a plane. The region can be identified using one or more element sets. If no element sets are specified, the region consists of the whole model. The cutting plane is defined by specifying the coordinates of a point on the plane and a vector normal to the plane. Alternatively, the cutting plane can be defined by specifying the global node numbers of point a on the plane and point b that lies off the cutting plane with the normal determined as the vector from point a to point b. Abaqus then automatically forms a surface close to the specified cutting plane by selecting the element facets, edges, or ends of the continuum solid, shell, membrane, surface, beam, pipe, truss, or rigid elements in the selected region. The surface generated in this manner is an approximation for the cutting plane. Multi-point mesh constraints are ignored while generating the interior surface based on the cutting plane; therefore, the result may be a surface that is not continuous if these constraints stitch disjointed meshes together in a region that is cut by the cutting plane. When the cutting plane intersects a beam, pipe, or truss element, the entire element is shown in the Visualization module of Abaqus/CAE as being part of the surface. However, if this surface is used for integrated output, only the element nodal forces from the element end that lies on the positive side as defined by the normal to the cutting plane are included in the integrated output. Point mass and rotary elements, connector elements, spot welds, and spring elements will not be part of the generated surface even if they are cut by the cutting plane. Input File Usage: Use the following option to define the cutting surface by specifying coordinates of a point on the plane and a vector normal to the plane: *SURFACE, NAME=surface_name, TYPE=CUTTING SURFACE, DEFINITION=COORDINATES Use the following option to define the cutting surface by specifying global node numbers of points a and b: *SURFACE, NAME=surface_name, TYPE=CUTTING SURFACE, DEFINITION=NODES Abaqus/CAE Usage: Interior cross-section surfaces are not supported in Abaqus/CAE. Whole-model free surface in an Abaqus/Explicit input file In an Abaqus/Explicit input file you can create a surface containing the exposed faces of all elements (and “contact edges” of beam, pipe, and truss elements) in the model except cohesive elements by specifying a blank element set name and a blank face identifier. This “free” surface of the model can be used as the base surface for the cropping and combining operations; without modifications this surface is similar to the default all-inclusive surface commonly used in general contact . Input File Usage: Abaqus/CAE Usage: *SURFACE, NAME=surface_name, TYPE=ELEMENT , The whole-model automatic free surface generation method is not supported in Abaqus/CAE. Trimming the perimeter of an open surface An “open” surface is one that has ends in two dimensions or an outside edge in three dimensions. The ends of a two-dimensional surface and the edge of a three-dimensional surface are called the surface’s “perimeter.” Since Abaqus allows a surface to be defined as only a part of the surface of a body, it may have a perimeter even though it is defined on a closed body. Abaqus automatically performs surface “trimming” on solid element meshes. You can change the default setting when a surface is created, providing some basic control over the extent of surfaces. Surface trimming: • is a recursive procedure that removes undesirable convex corners near the perimeter of an open surface ; • has no effect on closed surfaces (ones with no ends or edges); • is performed automatically, unless the surface is used as a master surface in a finite-sliding simulation in Abaqus/Standard or the surface is used with the contact pair algorithm in Abaqus/Explicit; • can be used only for external surfaces on solid element meshes (either specified surfaces or automatically generated free surfaces); and • has no effect on surfaces used with the contact pair algorithm in Abaqus/Explicit. Input File Usage: Use the following option to suppress automatic surface trimming: Abaqus/CAE Usage: *SURFACE, TYPE=ELEMENT, NAME=surface_name, TRIM=NO Automatic surface trimming cannot be suppressed in Abaqus/CAE. The effect of surface trimming The effect of surface trimming is best explained by means of an example. Figure 2.3.2–5 illustrates the effect of trimming for two different surfaces defined on the same simple two-dimensional mesh. In Case I the surface definition consists of a single layer of elements on the perimeter of the model. Using automatic surface facet generation, the resulting default surface (curve) includes the vertical element faces A and B since these faces lie on the perimeter of the model. Trimming the default surface created in Case I eliminates faces A and B since their presence results in the two spurious corners near the perimeter of the curve. Abaqus uses a special criterion in deciding to remove faces A and B from the original open curve. A face is removed if one of its end nodes is an endpoint and either of the following is true: another face node is a node on an element corner belonging to the curve or the face normal differs by more than 30° from the normal of an adjacent face also belonging to the curve. To be a node on an element corner belonging to the curve means to be a node on two different faces of the same element, both of which are part of the curve. The face removal criterion is applied recursively to the curve definition until all corners on or near the perimeter of the curve have been removed. This procedure is generalized for three-dimensional surface definitions. In Case II in Figure 2.3.2–5 trimming would not result in the elimination of faces A and B because neither of the endpoints of these two faces meets the criterion described above. Why Abaqus will, by default, trim most surfaces Trimming of surfaces used for application of distributed loads is usually desired since loads are normally applied to specific sides of a body. Any surface that is used for application of a distributed load will, by default, be trimmed. In Abaqus/Standard trimming the slave surface in contact or interaction simulations results in more accurate estimates of the contact pressures, heat fluxes, and electrical current densities along the perimeter of the surface. Any surface that is used as a slave surface in a contact or interaction simulation will, by default, be trimmed. If the slave surface is left untrimmed, the nodes at the corners of the surface will be assigned additional contact area from the element faces around the corners that may never be involved in the interaction between the surfaces. This additional contact area introduces errors into the estimates of the contact output variables at those nodes. Master surfaces in small-sliding simulations will, by DEFINING ELEMENT-BASED SURFACES user-specified element set automatically generated surface trim ⇒ Case I trim ⇒ Case II automatically generated surface Figure 2.3.2–5 Case I: Faces A and B are removed when trimming is done since one node of each of the faces is an end node and the other is a corner node. Case II: Faces A and B are not removed when trimming is done since one node of each of the faces is an end node but the other is not a corner node. default, be trimmed; Abaqus/Standard will normally form a better approximate surface. However, master surfaces in finite-sliding contact simulations will, by default, be left untrimmed, and they should extend far enough away from all expected regions of contact. This practice protects against the possibility of the slave surface nodes sliding off the master surface . 2.3.3 NODE-BASED SURFACE DEFINITION Products: Abaqus/Standard Abaqus/Explicit References • “Surfaces: overview,” Section 2.3.1 • “Mesh tie constraints,” Section 34.3.1 • “Contact interaction analysis: overview,” Section 35.1.1 • *SURFACE Overview A node-based “surface”: • can be used only as a “slave surface” in contact calculations; • can be used as a “slave” or “master surface” in a surface-based tie constraint; • is convenient in three-dimensional cases where Abaqus cannot construct a unique physical surface on the elements, such as a pipe modeled with pipe elements contacting the ocean floor or cables modeled with trusses contacting the ground after they break; • should be used with caution or not at all if accurate contact stresses are needed or if heat will be exchanged between the two surfaces; • can be assigned a nonzero thickness for use with the general contact algorithm in Abaqus/Explicit; • should not be used to model a shell or membrane surface if the thickness and midsurface offset need to be considered in the problem; • must either contain nodes that are all part of the same rigid body or not contain any nodes that are part of a rigid body if the node-based surface is to be used in a penalty contact pair in Abaqus/Explicit; • in Abaqus/Standard does not provide heat conduction between surfaces in fully coupled temperature-displacement analysis or pore fluid flow between surfaces in coupled pore pressure–displacement analysis; • in Abaqus/Standard does not provide heat conduction and electrical conduction between surfaces in a fully coupled thermal-electrical-structural analysis; and • does not include circumferential friction when used with axisymmetric elements with twist (CGAX, MGAX elements). Alternatives to node-based surfaces are element-based surfaces and, in the case of rigid surfaces, analytical rigid surfaces . See “Operating on surfaces,” Section 2.3.6, for information on defining surfaces using Boolean combinations of existing surfaces. Creating a node-based surface You create a node-based surface by specifying the nodes or node sets that form the surface. You must assign a name to the node-based surface; this name will be used when defining contact interactions that involve the surface. An optional associated area can be defined for each node. If no area is defined for a node and the surface is defined in a contact pair, the area specified as part of the contact property definition is used. If no area is specified as part of the contact property definition, a unit area is used. In Abaqus/Explicit the area used in contact pair calculations for a node in a node-based surface is always 1.0, regardless of the user-specified value. Therefore, the contact pressure output variable in Abaqus/CAE should be interpreted as the contact force when a node-based surface is used for contact pairs in Abaqus/Explicit. In models that are defined in terms of an assembly of part instances, all surfaces must belong to a part, part instance, or the assembly. Additional rules are given in “Defining an assembly,” Section 2.10.1. When the nodes of shell and membrane elements are used in a node-based surface, the thickness and midsurface offset of the shell or membrane at each node are not considered. However, a nonzero thickness can be assigned to node-based surfaces when used with the general contact algorithm in Abaqus/Explicit,” in Abaqus/Explicit . Input File Usage: *SURFACE, NAME=name, TYPE=NODE node number or node set, area 2.3.4 ANALYTICAL RIGID SURFACE DEFINITION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Surfaces: overview,” Section 2.3.1 • “Contact interaction analysis: overview,” Section 35.1.1 • “RSURFU,” Section 1.1.16 of the Abaqus User Subroutines Reference Manual • *RIGID BODY • *SURFACE Overview An analytical rigid surface: • can be two-dimensional or three-dimensional; • must be defined as model data; • can be used with the infinitesimal-sliding, small-sliding, or finite-sliding mechanical contact formulations; • should be oriented such that the analytical rigid surface’s outward normal points toward any body it may contact; and • is associated with a node, known as the rigid body reference node, whose motion governs the motion of the surface. What are analytical rigid surfaces and why use them? Analytical rigid surfaces are geometric surfaces with profiles that can be described with straight and curved line segments. These profiles can be swept along a generator vector or rotated about an axis to form a three-dimensional surface. An analytical rigid surface is associated with a rigid body reference node, whose motion governs the motion of the surface. An analytical rigid surface does not contribute to the rigid body’s mass or inertia properties . The degrees of freedom of the rigid body reference node become active only when the analytical surface is used in a contact interaction or when an element (such as a spring element or a mass element) is connected to the rigid body reference node. Analytical rigid surfaces are always single-sided with their orientation specified through their definition. Therefore, contact interaction is recognized only on the outer boundary of an analytical rigid surface. To model contact on both sides of a thin structure, use an analytical rigid surface that wraps around the boundary of the thin structure. Advantages Using analytical rigid surfaces instead of defining element-based rigid surfaces provides two important advantages in contact modeling. • Many curved geometries can be modeled exactly with analytical rigid surfaces because of the ability to parameterize the surface with curved line segments. The result is a smoother surface description, which can reduce contact noise and provide a better approximation to the physical contact constraint. • Using analytical rigid surfaces instead of rigid surfaces formed by element faces may result in decreased computational cost incurred by the contact algorithm. The use of curved line segments instead of many linear facets will decrease the time spent in contact tracking operations. Additional computational savings may be realized in three dimensions because of the intrinsic two-dimensional descriptions of the analytical surfaces. Disadvantages There are also some disadvantages to using analytical rigid surfaces for contact modeling. • An analytical rigid surface must always act as a master surface in a contact interaction. Therefore, contact cannot be modeled between two analytical rigid surfaces. • Contact forces and pressures cannot be contoured on an analytical rigid surface. However, contact forces and pressures can be plotted on the slave surface. • The use of a very large number (thousands) of segments to define an analytical rigid surface can degrade performance. In most cases it is not necessary to use a large number of segments to define an analytical rigid surface, because curved segment types are allowed. In rare cases in which a very large number of segments would be necessary, the analysis may be more efficient if an element- based rigid surface is used instead . • An analytical rigid surface does not contribute to the mass and rotary inertia properties of the rigid body with which it is associated. Therefore, if the mass distribution on an analytical rigid surface needs to be accounted for, equivalent mass and rotary inertia properties must be defined for the rigid body by using MASS and ROTARYI elements, or a finite element discretization of the surface should be used instead of an analytical rigid surface . • In Abaqus/Explicit reaction force output for a rigid body containing an analytical rigid surface is calculated only for constraints that are active at the reference node (e.g., constraints specified as boundary conditions). If the net contact force on the rigid body corresponding to an unconstrained degree of freedom is desired, it must be calculated from the rigid body’s acceleration and mass. Creating an analytical rigid surface You can define the following types of simple, two- or three-dimensional, geometric analytical surfaces: • planar (two-dimensional) surfaces, • three-dimensional cylindrical (swept) surfaces, and • three-dimensional surfaces of revolution. In Abaqus/Standard if none of these surfaces is adequate, you can define a more general analytical surface with user subroutine RSURFU. Analytical rigid surfaces are useful when the cross-sections of the surfaces can be represented by straight and curved line segments. The curved segments can be either circular or parabolic arcs. In two- dimensional simulations the line segments are defined in the global coordinate system of the deformable model. In three-dimensional simulations a local, two-dimensional coordinate system must be created, and the line segments are then defined in that system. The two standard types of three-dimensional analytical rigid surfaces available are shown in Figure 2.3.4–1. surface of revolution cylindrical surface Figure 2.3.4–1 Examples of three-dimensional rigid surfaces. You must indicate which type of analytical surface (planar, cylindrical, or revolution) is being created and assign a name to the surface. In addition, you must define the analytical surface as part of a rigid body by specifying the name of the analytical surface and the rigid body reference node that will control the motion of the surface in a rigid body definition. An Abaqus model can be defined in terms of an assembly of part instances . A part can contain only one analytical surface. A part containing an analytical surface definition cannot also contain elements. Input File Usage: Use both of the following options to create an analytical rigid surface: Abaqus/CAE Usage: *SURFACE, TYPE=analytical_surface_type, NAME=name *RIGID BODY, ANALYTICAL SURFACE=name, REF NODE=n Part module: Create Part: Name: analytical_rigid_part: select Analytical rigid as the Type Then do one of the following: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: select analytical_rigid_part Interaction module: Create Constraint: Rigid body: Analytical Surface: Edit: select analytical_rigid_part Interaction module: Create Interaction: any valid type: select analytical_rigid_part as one of the regions involved in contact Defining a surface profile The surface profile is the collection of line segments defining the cross-section of the surface. The surface type determines whether the profile is swept (cylindrical surfaces), revolved (surfaces of revolution), or, in the two-dimensional case, used as is (planar surfaces). You construct a profile by providing the endpoint of each line segment in the profile; the starting point is always the endpoint of the previous segment, or, in the case of the first segment, the point specified as the starting point. The center points of circular arcs must be given. Abaqus can define only arcs that are less than 179.74°; thus, it will use the shorter arc defined by the data provided (use two adjacent arcs to define a longer arc). For parabolic arcs you must give a third point that lies on the parabola and within the arc. Two-dimensional rigid surfaces To define a planar rigid surface, specify the line segments forming the rigid surface’s profile in the global coordinate system. If the analytical surface is being defined inside a part, specify the line segments in the local part coordinate system. Input File Usage: *SURFACE, TYPE=SEGMENTS, NAME=name data lines to define the line segments forming the surface For example, the definition of the two-dimensional rigid surface depicted in Figure 2.3.4–2 is *SURFACE, TYPE=SEGMENTS, NAME=BSURF START, CIRCL, LINE, CIRCL, *RIGID BODY, ANALYTICAL SURFACE=BSURF, REF NODE=101 where are the global coordinates of the points shown in Figure 2.3.4–2. , , and , , , , , , Abaqus/CAE Usage: Part module: Create Part: Name: analytical_rigid_part: select 2D Planar or Axisymmetric as the Modeling Space and Analytical rigid as the Type Three-dimensional cylindrical rigid surfaces To define a cylindrical rigid surface in a model that is not defined in terms of an assembly of part instances, specify the points a, b, and c shown in Figure 2.3.4–3 that define the local coordinate system. Give the coordinates of these points—( )—in the default global ), ( coordinate system. As shown in Figure 2.3.4–3, point a defines the origin of the local system; point b defines the local x-axis; and point c defines the generator vector, which is the negative local z-axis. If the segment , Abaqus will automatically adjust point c within the plane defined by points a, b, and c, such that they become perpendicular. The line segments forming the profile of the rigid surface are defined in the local x–y plane. The three-dimensional surface is formed by sweeping this profile along the generator vector. The resulting surface extends to infinity in both the positive and negative directions of the generator vector. is not perpendicular to ), and ( rigid reference node 101 BSURF ASURF Figure 2.3.4–2 Two-dimensional analytical rigid surface contacting a deformable body. Start Line segment Outward normal Circular arc segment Local y-axis Generator direction b Local x-axis Local z-axis Figure 2.3.4–3 Cylindrical rigid surface. To define a cylindrical rigid surface within a part, specify the line segments forming the profile of the rigid surface in the part coordinate system. For an analytical surface defined within a part (or part instance), point a is located at the origin of the part coordinate system, point b is located on the part x-axis, and point c is located on the negative part z-axis. If the segment , Abaqus will automatically adjust point c within the plane defined by points a, b, and c, such that they become perpendicular. You cannot redefine this analytical surface coordinate system; instead, you can position the surface in the model by giving positioning data when you instance the part . is not perpendicular to Input File Usage: *SURFACE, TYPE=CYLINDER, NAME=name data lines to define the line segments forming the surface , , and are points in the local For example, the following input, where coordinate system, would define the rigid surface shown in Figure 2.3.4–3 in a model that is not defined in terms of an assembly of part instances (the reference node is not shown in the figure): *SURFACE, TYPE=CYLINDER, NAME=CSURF , , , , , START, LINE, CIRCL, … … *RIGID BODY, ANALYTICAL SURFACE=CSURF, REF NODE=n Leave the first two data lines blank to define a cylindrical rigid surface within a part. , , Abaqus/CAE Usage: Part module: Create Part: Name: analytical_rigid_part: select 3D as the Modeling Space, Analytical rigid as the Type, and Extruded shell as the Base Feature Three-dimensional surfaces of revolution To define a rigid surface of revolution in a model that is not defined in terms of an assembly of part instances, specify the two points a and b shown in Figure 2.3.4–4 that define the local coordinate system. Give the coordinates of these points—( )—in the default global coordinate system. As shown in Figure 2.3.4–4, point a defines the origin of the local system, and the vector from a to b defines the local z-axis, which is the axis of a cylindrical coordinate system. The line segments forming the profile of the surface of revolution are defined in the local r–z plane, where the local r-axis aligns with the radial axis of the cylindrical coordinate system. The three-dimensional surface is formed by revolving this profile about the axis of the cylindrical system, the local z-axis. ) and ( To define a rigid surface of revolution within a part, specify the line segments forming the cross- section of the rigid surface in the local part coordinate system. For an analytical surface defined within a local z Start line segment local r circular arc segment Figure 2.3.4–4 Rigid surface of revolution. part (or part instance), point a is located at the origin of the part coordinate system, the part x-axis aligns with the radial axis of the cylindrical coordinate system, and point b is located on the part y-axis. You cannot redefine this local axis; instead, you can position the surface in the model by giving positioning data when you instance the part . *SURFACE, TYPE=REVOLUTION, NAME=name Input File Usage: data lines to define the line segments forming the surface For example, the following input would define the rigid surface shown in Figure 2.3.4–4 (the reference node is not shown in the figure): *SURFACE, TYPE=REVOLUTION, NAME=REVSURF , , , , , , START, LINE, … CIRCL, … … *RIGID BODY, ANALYTICAL SURFACE=REVSURF, REF NODE=999 Leave the first data line blank to define a rigid surface of revolution within a part. Abaqus/CAE Usage: Part module: Create Part: Name: analytical_rigid_part: select 3D as the Modeling Space, Analytical rigid as the Type, and Revolved shell as the Base Feature Defining the surface normals The outward surface normal for analytical rigid surfaces is determined by the direction of the line segments forming the profile of the surface. The sequence of line segments defines a vector along the rigid surface from the starting point of the first segment to the ending point of the last segment. The outward surface normal is created by taking the cross product of the vector , the unit normal to the plane in which the surface is defined, and the vector . Figure 2.3.4–5 shows the vector in the definition plane of an analytical rigid surface. , the tangent to the surface: Line segment Start e2 e3 e1 Circular segments Line segment Figure 2.3.4–5 Orientation of surface normals for a rigid surface. , and is defined such that and The unit vector , form a right-handed orthonormal coordinate system. In-plane coordinate directions depend on the type of analytical rigid surface being defined. For two-dimensional analytical rigid surfaces they correspond to the global X- and Y-axes in planar models and the r- and z-axes in axisymmetric models. For cylindrical rigid surfaces they correspond to the local x- and y-axes, and for rigid surfaces of revolution they correspond to the local r- and z-axes. The outward normals for a cylindrical rigid surface and rigid surface of revolution are shown in Figure 2.3.4–3 and Figure 2.3.4–4, respectively. If the line segments are specified in the wrong order, the surface normals of a rigid surface will appear in exactly the opposite direction to what was intended. Such a mistake can be corrected only by specifying the line segments in the opposite sequence. Smoothing analytical rigid surfaces In many cases it can be beneficial to smooth surfaces to more accurately represent the surface geometry. In particular, it can be very difficult to obtain a converged solution in a finite-sliding Abaqus/Standard simulation if the master surface does not have continuous normal and surface tangent vectors ; therefore, it is important to smooth any sharp corners on the master surface so that discontinuities in these vectors are eliminated. By default, Abaqus does not smooth master surfaces that are analytical rigid surfaces. Smooth transitions between adjacent line segments can always be created by manually inserting additional curved line segments. Alternatively, smooth surfaces can be generated automatically by Abaqus. You specify the radius of curvature, r, in the units of length used in the model, that Abaqus will use to construct a smooth transition between any discontinuous line segments forming the rigid surface. The default value of zero provides no smoothing of the surface. The effect of a fillet radius on adjoining line segments and on adjoining line and circular arc segments is illustrated in Figure 2.3.4–6. END START fillet radius Y-local X-local OUTWARD NORMAL Figure 2.3.4–6 Effect of fillet radius on an analytical rigid surface. The sharp corners have been smoothed using the fillet radius so that the normal and tangent surface vectors are continuous along the entire master surface. Any value r can be used in a model. However, if r is greater than the length of either of the two adjacent segments, no smoothing will occur. Therefore, a practical limit on the size of r is the length of the smallest line segment forming the surface. Input File Usage: *SURFACE, TYPE=analytical_surface_type, NAME=name, FILLET RADIUS=r Abaqus/CAE Usage: When you create an analytical rigid part in Abaqus/CAE, you can create a fillet radius between segments or join the segments using arcs. See “Sketching simple objects,” Section 20.10 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual. Surface tangent conventions , is always along the direction Abaqus forms analytical rigid surfaces such that the first surface tangent, of the line segments forming the surface . The second surface tangent, , is defined such that the outward surface normal and the two surface tangents form a right-handed orthonormal system, as shown in Figure 2.3.4–7. a. Two-dimensional cases b. Three-dimensional cases t1 t2 t1 Figure 2.3.4–7 Surface tangent and outward normal definitions for analytical rigid surfaces. Creating an analytical rigid surface in a user subroutine More complicated analytical rigid surfaces can be defined in Abaqus/Standard by user subroutine RSURFU. Writing subroutine RSURFU to create a smooth surface is usually difficult, and convergence problems are often caused by inadequate surface definition in this subroutine. When using RSURFU, ensure that the outward surface normal and the two surface tangents form a right-handed orthonormal system. In two-dimensional cases the second surface tangent is always (0, 0, −1). You must also ensure that the surface is smooth in finite-sliding simulations and that the orientation of the rigid surface relative to the deformable surface is reasonable (i.e., the rigid surface cannot be inside the deformable surface). Input File Usage: Abaqus/CAE Usage: *SURFACE, TYPE=USER, NAME=name User subroutine RSURFU is not supported in Abaqus/CAE. Defining analytical rigid surfaces when drag chain or rigid surface elements are used An alternative method of defining analytical rigid surfaces must be used to define the surface of the seabed when three-dimensional drag chain elements (available only in Abaqus/Standard) are used. This alternative method must also be used when rigid surface elements are used; these elements are required only when CAXA or SAXA elements contact a rigid surface. For this method the rigid surface must be flat and parallel to the x–y plane. In a model defined in terms of an assembly of part instances, the rigid surface definition must appear inside the same part definition as the drag chain or rigid surface elements. You must indicate which type of analytical surface (planar, cylindrical, or user-defined) is being created. Cylindrical rigid surfaces are not valid for use with CAXA or SAXA elements. In addition, you must assign a name to the surface and identify the rigid body reference node that will control the motion of the surface. Input File Usage: Abaqus/CAE Usage: *RIGID SURFACE, TYPE=surface_type, NAME=name, REF NODE=n Drag chain and rigid surface elements are not supported in Abaqus/CAE. Two-dimensional rigid surfaces To define a planar rigid surface, define the line segments forming the rigid surface’s cross-section in the global coordinate system. You must provide the endpoint of each line segment; the starting point is always the endpoint of the previous segment, or, in the case of the first segment, the point specified as the starting point. The centers of the circular arcs, points c and f in Figure 2.3.4–2, must be given. Abaqus can define only arcs that are less than, but not equal to, 179.74°; thus, it will use the shorter arc defined by the data provided (use two adjacent arcs to define a longer arc). For parabolic arcs you must give a third point that lies on the parabola and within the arc. Input File Usage: *RIGID SURFACE, TYPE=SEGMENTS, NAME=name, REF NODE=n START, starting point X- or r-coordinate, starting point Y- or z-coordinate data lines to define the endpoints of the line segments forming the surface, beginning with the word LINE (for straight line segments), CIRCL (for circular arc segments), or PARAB (for parabolic arc segments) Abaqus/CAE Usage: Drag chain and rigid surface elements are not supported in Abaqus/CAE. Three-dimensional cylindrical rigid surfaces To define a cylindrical rigid surface, specify the points a, b, and c shown in Figure 2.3.4–3 that define the local coordinate system. Give the coordinates of these points—( ), and ( )—in the default global coordinate system. As shown in Figure 2.3.4–3, point a defines the origin of the local system; point b defines the local x-axis; and point c defines the generator vector, which is the negative local z-axis. The line segments forming the cross-section of the rigid surface are defined in the local x–y plane. The three-dimensional surface is formed by sweeping this cross-section along the generator vector. The resulting surface extends to infinity in both the positive and negative directions of the generator vector. ), ( Input File Usage: *RIGID SURFACE, TYPE=CYLINDER, NAME=name, REF NODE=n START, starting point x-coordinate, starting point y-coordinate data lines to define the endpoints of the line segments forming the surface, beginning with the word LINE (for straight line segments), CIRCL (for circular arc segments), or PARAB (for parabolic arc segments) Abaqus/CAE Usage: Drag chain and rigid surface elements are not supported in Abaqus/CAE. 2.3.5 EULERIAN SURFACE DEFINITION Product: Abaqus/Explicit References • “Surfaces: overview,” Section 2.3.1 • “Eulerian analysis,” Section 14.1.1 • “Contact interaction analysis: overview,” Section 35.1.1 • *EULERIAN SECTION • *SURFACE Overview An Eulerian surface: • must be three-dimensional; • must be defined as model data; • can be used with the general contact algorithm in Abaqus/Explicit; and • is created by specifying the name of an Eulerian material instance. What are Eulerian surfaces and why use them? An Eulerian surface represents the exterior surface of a particular Eulerian material instance in an Abaqus/Explicit analysis. Since Eulerian materials flow through the Eulerian mesh, their surfaces cannot be defined by a simple list of element faces. Instead, these surfaces often lie within Eulerian elements and must be computed in each time increment using element volume fraction data. You can use Eulerian surfaces to define specific interactions with Lagrangian surfaces in Abaqus/Explicit’s general contact algorithm. Once defined, you can reference Eulerian surfaces in inclusions, exclusions, and interaction definitions. You cannot combine or crop Eulerian surfaces. Eulerian surface definitions are not required for the use of Eulerian-Lagrangian contact. If you specify “automatic” contact for the entire model, the exterior surface of all Eulerian materials will automatically be considered for contact. Advantages of creating Eulerian surfaces You can use Eulerian surfaces to: • Assign contact properties for contact interactions involving a particular Eulerian material instance. • Exclude interactions between Eulerian materials and Lagrangian bodies that are unlikely to make contact, simplifying the contact problem and reducing computational cost. Creating an Eulerian surface To create an Eulerian surface, you must specify the name of a material instance that is present in the model. The material instance names are defined as part of the Eulerian section . Abaqus/Explicit calculates the exterior boundary of the specified material instance and defines a surface corresponding to that boundary. The surface is recalculated in each time increment as the material deforms. Input File Usage: *SURFACE, TYPE=EULERIAN MATERIAL, NAME=name material instance name, 2.3.6 OPERATING ON SURFACES Products: Abaqus/Standard Abaqus/Explicit References • “Surfaces: overview,” Section 2.3.1 • “Coupling constraints,” Section 34.3.2 • “Mesh-independent fasteners,” Section 34.3.4 • “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1 • *SURFACE Overview Combined surfaces: • are created by performing a Boolean operation (union, intersection, or difference) on existing surfaces; • can be formed from element-based or node-based surfaces; • cannot be formed from Eulerian surfaces; • can be used in the same way as other element-based or mode-based surfaces in Abaqus/Standard; and • cannot be used with contact pairs in Abaqus/Explicit (but can be used with general contact in Abaqus/Explicit). Cropped surfaces: • are created by cropping an existing surface and keeping only that part of the surface that is enclosed in a specified rectangular box; • can be formed from element-based or node-based surfaces; • cannot be formed from Eulerian surfaces; • can be used in the same way as other element-based or mode-based surfaces in Abaqus/Standard; and • cannot be used with contact pairs in Abaqus/Explicit (but can be used with general contact in Abaqus/Explicit). Creating a combined surface You must assign a name to the combined surface; this name can be used with other features that refer to surfaces. In models that are defined in terms of an assembly of part instances, all surfaces must belong to a part, part instance, or the assembly. Surfaces can be created at the part level and combined at the assembly level. Additional rules are given in “Defining an assembly,” Section 2.10.1. The surfaces being combined must be the same type; i.e., an element-based surface can be combined with another element-based surface but not with a node-based surface. Combined surfaces can be used to create another combined surface. Union of existing surfaces Any number of existing surfaces can be combined to create a new surface. If the surfaces being combined are element-based surfaces, the new surface will also be an element-based surface and any overlap among the surfaces will be merged. Similarly, if the surfaces being combined are node-based surfaces, the new surface will be a node-based surface and any overlap among the surfaces will be merged. Input File Usage: *SURFACE, NAME=name, COMBINE=UNION list of surface names Intersection or difference of existing surfaces The intersection or difference of two existing surfaces can be used to create a new surface. The difference operation subtracts the second surface from the first surface. When the intersection or difference operations are performed on element-based surfaces, they act only on the facets. A warning message is issued if the intersection operation results in an empty surface. Input File Usage: Use the following option to create a new surface based on the intersection of two existing surfaces: *SURFACE, NAME=name, COMBINE=INTERSECTION first surface name, second surface name Use the following option to create a new surface based on the difference of two existing surfaces: *SURFACE, NAME=name, COMBINE=DIFFERENCE first surface name, second surface name Creating a cropped surface You can create a new surface that will contain only those faces of an existing surface that have nodes inside a specified cropping box. For a node-based surface the new surface will contain only those nodes that are enclosed inside the cropping box. If the face has at least one node inside the box, the entire face is accepted as valid. You must assign a name to the new surface and specify the name of the existing surface from which the new surface is to be generated. Only one surface can be specified. To define the location of the box, specify the coordinates of the lower corner of the box ( , , ). The cutting box can be rotated about the lower corner ( ) if an optional rotation is defined. The coordinates of the two points, a and b, that define the rotation are given in the unrotated system. ) and the coordinates of the opposite (upper) corner of the box ( , , , , These points should be defined such that point a lies on the rotated X-axis and point b lies on the X–Y plane and close to the Y-axis. Input File Usage: *SURFACE, NAME=name, CROP old_surface_name , , , , , , , , , , For example, to crop the surface that contains all exposed faces in the model, use the following input: *SURFACE, TYPE=ELEMENT, NAME=entire_surface , *SURFACE, NAME=name, CROP entire_surface , , , , , , , , 2.3.6–3 , 2.4 Rigid body definition • “Rigid body definition,” Section 2.4.1 2.4.1 RIGID BODY DEFINITION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Surfaces: overview,” Section 2.3.1 • “Element-based surface definition,” Section 2.3.2 • “Analytical rigid surface definition,” Section 2.3.4 • “Rigid elements,” Section 30.3.1 • *RIGID BODY • “Defining rigid body constraints,” Section 15.15.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A rigid body: • can be two-dimensional planar, axisymmetric, or three-dimensional; • is associated with a node, called the rigid body reference node, whose motion governs the motion of the entire rigid body; • can consist of nodes, elements, and surfaces; • can act as a method of constraint; • can be used with connector elements in multibody dynamic simulations; • can be used to prescribe the motion of a rigid surface for contact modeling; • can be computationally efficient and, in Abaqus/Explicit, does not affect the global time increment; and • can have temperature gradients or be isothermal in a fully coupled temperature-displacement analysis where thermal interactions are considered. What is a rigid body? A rigid body is a collection of nodes, elements, and/or surfaces whose motion is governed by the motion of a single node, called the rigid body reference node. The relative positions of the nodes and elements that are part of the rigid body remain constant throughout a simulation. Therefore, the constituent elements do not deform but can undergo large rigid body motions. The mass and inertia of a rigid body can be calculated based on contributions from its elements or can be assigned specifically. Analytical surfaces can also be made part of the rigid body, whereas any surfaces based on the nodes or elements of a rigid body are associated automatically with the rigid body. The motion of a rigid body can be prescribed by applying boundary conditions at the rigid body reference node. Loads on a rigid body are generated from concentrated loads applied to nodes and from distributed loads applied to elements that are part of the rigid body. Rigid bodies interact with the remainder of the model in several ways. Rigid bodies can connect at the nodes to deformable elements, and surfaces defined on rigid bodies can continue on these deformable elements, provided that compatible element types are used. Rigid bodies can also be connected to other rigid bodies by connector elements . Surfaces defined on rigid bodies can contact surfaces defined on other bodies in the model. Determining when to use a rigid body Rigid bodies can be used to model very stiff components, either fixed or undergoing large motions. For example, rigid bodies are ideally suited for modeling tooling (i.e., punch, die, drawbead, blank holder, roller, etc.). They can also be used to model constraints between deformable components, and they provide a convenient method of specifying certain contact interactions. Rigid bodies can be used with connector elements to model a wide variety of multibody dynamic problems. It may be useful to make parts of a model rigid for model verification purposes. For example, in complex models elements far away from the particular region of interest could be included as part of a rigid body, resulting in faster run times at the model development stage. When you are satisfied with the model, you can remove the rigid body definitions and incorporate an accurate deformable finite element representation throughout. In multibody dynamic simulations rigid bodies are useful for many reasons. Although the motion of the rigid body is governed by the six degrees of freedom at the reference node, rigid bodies allow accurate representation of the geometry, mass, and rotary inertia of the rigid body. Furthermore, rigid bodies provide accurate visualization and postprocessing of the model. The principal advantage to representing portions of a model with rigid bodies rather than deformable finite elements is computational efficiency. Element-level calculations are not performed for elements that are part of a rigid body. Although some computational effort is required to update the motion of the nodes of the rigid body and to assemble concentrated and distributed loads, the motion of the rigid body is determined completely by a maximum of six degrees of freedom at the reference node. Rigid bodies are particularly effective for modeling relatively stiff parts of a model in Abaqus/Explicit for which tracking waves and stress distributions are not important. Element stable time increment estimates in the stiff region can result in a very small global time increment. Since rigid bodies and elements that are part of a rigid body do not affect the global time increment, using a rigid body instead of a deformable finite element representation in a stiff region can result in a much larger global time increment, without significantly affecting the overall accuracy of the solution. Creating a rigid body You must assign a rigid body reference node to the rigid body. Input File Usage: Abaqus/CAE Usage: *RIGID BODY, REF NODE=n Interaction module: Tools→Reference Point: select a point to act as a reference point Create Constraint: Rigid body: Point: Edit: select reference point region The rigid body reference node A rigid body reference node has both translational and rotational degrees of freedom and must be defined for every rigid body. If the reference node has not been assigned coordinates, Abaqus will assign it the coordinates of the global origin by default. Alternatively, you can specify that the reference node should be placed at the center of mass of the rigid body. In fully coupled temperature-displacement analysis where a rigid body is considered as isothermal, a single temperature degree of freedom describing the temperature of the rigid body exists at the rigid body reference node. The rigid body reference node: • can be connected to mass, rotary inertia, capacitance, or deformable elements; • cannot be a rigid body reference node for another rigid body; and • can have a temperature degree of freedom if the body is an isothermal rigid body. Positioning the reference node at the center of mass The specific location of the rigid body reference node relative to the rest of the rigid body or to its center of mass is important if nonzero boundary conditions are to be applied to the rigid body or concentrated loads are to be applied at the reference node. In many problems of rigid body dynamics, it may be desirable to apply loads and boundary conditions to the rigid body at its center of mass. In addition, it may be useful to monitor the configuration of the rigid body at its center of mass for output purposes. However, it may be difficult to locate the center of mass a priori when the rigid body mass and inertia properties (discussed below) contain contributions from a finite element discretization or a complex arrangement of MASS and ROTARYI elements. By default, the rigid body reference node will not be repositioned. You can specify that it should be repositioned at the calculated center of mass. In this case if a MASS element is defined at the rigid body reference node, the calculated center of mass used for repositioning includes all mass contributions except the mass at the reference node. The MASS element is then repositioned at the center of mass and included in the mass properties of the rigid body. If the only mass contribution to the rigid body is from a MASS element defined at the rigid body reference node, the reference node will not be repositioned. Input File Usage: Abaqus/CAE Usage: Use the following option to indicate that the reference node should not be repositioned (the default): *RIGID BODY, REF NODE=n, POSITION=INPUT Use the following option to specify that the rigid body reference node should be repositioned at the calculated center of mass: *RIGID BODY, REF NODE=n, POSITION=CENTER OF MASS Interaction module: Create Constraint: Rigid body: toggle Adjust point to center of mass at start of analysis The collection of nodes that constitute the rigid body In addition to the rigid body reference node, rigid bodies consist of a collection of nodes that is generated by assigning elements and nodes to the rigid body. These nodes provide a connection to other elements. Nodes that are part of a rigid body are one of two types: • pin nodes, which have only translational degrees of freedom associated with the rigid body, or • tie nodes, which have both translational and rotational degrees of freedom associated with the rigid body. The rigid body node type is determined by the type of elements on the rigid body to which the node is attached. You can also specify the node type when you assign nodes directly to a rigid body. For pin nodes only the translational degrees of freedom are part of the rigid body, and the motion of these degrees of freedom is constrained by the motion of the rigid body reference node. For tie nodes both the translational and rotational degrees of freedom are part of the rigid body and are constrained by the motion of the rigid body reference node. The node type has important implications when the node is connected to rotary inertia elements, deformable structural elements, or connector elements or when the node has concentrated moments or follower loads applied to it. Rotary inertia elements and applied concentrated moments affect the rigid body only when associated with a tie node. Rigid body connections to deformable elements always involve the translational degrees of freedom; rigid body connections to deformable shell, beam, pipe, and connector elements also involve the rotational degrees of freedom if the connection is at a tie node. The behavior of the two types of connections is illustrated in Figure 2.4.1–1, which shows an octagonal rigid body connected to two deformable shell elements through nodes at opposite ends subjected to an applied rotational velocity. tie node pin node initial configuration Final configuration after counterclockwise rotation through 45 Figure 2.4.1–1 Rigid body with tie node and pin node connections. The shell elements are assumed to be stiff (negligible bending is shown in the figure). When the nodes common to the rigid body and the shell elements are tie nodes, the rotation applied to the rigid body is transmitted directly to the shell elements. When the common nodes are pin nodes, the rigid body rotation is not transmitted directly to the shell elements, which can result in large relative motions between the rigid body and the adjacent shell structure. Assigning elements to a rigid body To include elements in the rigid body definition, you specify the region of your model containing all of the elements that are part of the rigid body. Elements in this region or nodes connected to the elements in this region cannot be part of any other rigid body. Table 2.4.1–1 lists the continuum, structural, and rigid element types that can be included in a rigid body and the respective node types generated in the rigid body. Table 2.4.1–1 List of valid elements that can be included in a rigid body (* indicates all elements beginning with the preceding label). Elements Generate Pin Nodes Generate Tie Nodes Nodal Degrees of Freedom Pin Nodes Tie Nodes B21*, B22*, B23*, FRAME2D, PIPE2*, RB2D2 CGAX*, MGAX*, SAX1, SAX2* B31*, B32*, B33*, FRAME3D, PIPE*, RB3D2, S3*, S4*, S8*, S9* CPE3*, CPE4*, CPE6*, CPE8*, CPS3, CPS4*, CPS6*, CPS8*, GK2D2, GKPS*, GKPE*, R2D2, T2D2* CAX3, CAX4*, CAX6*, CAX8*, GKAX*, MAX*, RAX2 C3D4*, C3D6*, C3D8*, C3D10*, C3D15*, C3D20*, C3D27*, GK3D*, M3D3, M3D4*, M3D6, M3D8*, M3D9*, SFM3D*, SFMAX*, SFMGAX*, R3D3, R3D4, T3D2*, CCL*, MCL*, SFMCL* 2.4.1–5 Rigid Body Geometry Planar Axisymmetric Three- When connector elements are included in the rigid body, the type of generated nodes depends on whether the rotational degrees of freedom are active for their connection type. If connector elements that activate material flow degree of freedom at nodes are included in the rigid body, the material and flow through the rigid body as that degree of freedom is constrained to the motion of the rigid body. The following elements cannot be declared as rigid: • Acoustic elements • Axisymmetric-asymmetric continuum and shell elements • Coupled thermal-electrical elements • Diffusive heat transfer/mass diffusion elements and forced convection/diffusion elements • Eulerian elements • Generalized plane strain elements • Gasket elements with thickness-direction behavior • Heat capacitance elements • Inertial elements (mass and rotary inertia) • Infinite elements • Piezoelectric elements • Special-purpose elements • Substructures • Thermal-electrical-structural elements • User-defined elements If elements of more than one type or section definition are part of a rigid body, the specified region will contain elements with different section definitions. When continuum or structural elements are assigned to a rigid body, they are no longer deformable and their motion is governed by the motion of the rigid body reference node. Element stiffness calculations are not performed for these elements, and they do not affect the global time increment in Abaqus/Explicit. However, the mass and inertia of the rigid body includes contributions from these elements as calculated from their section and material density definitions . Mass and rotary inertia elements, as well as point heat capacitance elements, should not be included in the specified region. Contributions to a rigid body from mass, rotary inertia, and heat capacitance elements are accounted for automatically when these elements are connected to nodes that are part of the rigid body. A list of nodes that are part of a rigid body is generated automatically when you assign elements to a rigid body. The node list is constructed as a unique list including all the nodes that are connected to elements in the specified region. Nodes in this list cannot be part of any other rigid body. The type of each node, pin or tie, is determined by the type of elements on the rigid body to which it is connected. Shell, beam, pipe, and rigid beam elements generate tie nodes; solid, membrane, truss, and rigid (other than beam) elements generate pin nodes . For nodes that are connected to both elements that generate pin nodes and elements that generate tie nodes, the common node is defined as the tie type. All elements that are part of a rigid body must be of like geometry. Therefore, elements contained in the specified region must be either planar, axisymmetric, or three-dimensional. The geometry of the elements determines the geometry of the rigid body as shown in Table 2.4.1–1. Input File Usage: Use the following option to assign elements to a rigid body: Abaqus/CAE Usage: *RIGID BODY, REF NODE=n, ELSET=name Interaction module: Create Constraint: Rigid body: Body (elements): Edit: select body regions Assigning nodes to a rigid body To assign nodes directly to a rigid body, you specify all the desired pin nodes and all the tie nodes separately. These nodes become part of the rigid body in addition to any nodes that have been generated from elements assigned to the rigid body. The following rules apply when assigning nodes directly to a rigid body: • The rigid body reference node cannot be contained in either the set of pin nodes or the set of tie nodes. • Nodes that are part of the set of pin nodes cannot also be contained in the set of tie nodes. • Nodes that are contained in the set of pin nodes or the set of tie nodes cannot be part of any other rigid body definition. • Nodes that are generated automatically from elements assigned to the rigid body that are also contained in the set of pin nodes are classified as pin nodes, regardless of their element connections. • Nodes that are generated automatically from elements assigned to the rigid body that are also contained in the set of tie nodes are classified as tie nodes, regardless of their element connections. The types of nodes generated by elements included in a rigid body can, therefore, be overridden by assigning the nodes directly to the rigid body, thereby allowing you greater flexibility to define a constraint with a rigid body by easily specifying the type of connection the rigid body makes with its attached deformable finite elements. Input File Usage: Use the following option to assign nodes to a rigid body: Abaqus/CAE Usage: *RIGID BODY, REF NODE=n, PIN NSET=name, TIE NSET=name Interaction module: Create Constraint: Rigid body: Pin (nodes): Edit: select pin regions, and Tie (nodes): Edit: select tie regions Assigning analytical surfaces to a rigid body You can assign an analytical surface to a rigid body. The procedure for creating and naming an analytical rigid surface is described in “Analytical rigid surface definition,” Section 2.3.4. Only one analytical surface can be defined as part of the rigid body definition. Input File Usage: Use the following option to assign an analytical rigid surface to a rigid body: *RIGID BODY, REF NODE=n or name, ANALYTICAL SURFACE=name Abaqus/CAE Usage: Interaction module: Create Constraint: Rigid body: Analytical Surface: Edit: select analytical surface regions Defining a rigid body in a model that is defined in terms of an assembly of part instances An Abaqus model can be defined in terms of an assembly of part instances . A rigid body in such a model can be created from deformable elements at either the part level or the assembly level. In either case all node and element definitions must belong to one or more parts. If all nodes making up the rigid body belong to the same part, create a rigid part by defining the rigid body at the part level. Multiple deformable part instances can be combined into a single rigid body by creating an assembly-level node or element set that spans the part instances, then defining the rigid body at the assembly level to refer to that set. The rigid body reference node can also be defined at the assembly level, if necessary. Rigid body mass and inertial properties When a rigid body is not constrained fully, the mass and inertia properties of the rigid body are important to its dynamic response. In Abaqus/Explicit an error message will be issued if there is no mass (or rotary inertia) corresponding to an unconstrained degree of freedom. Abaqus automatically calculates the mass, center of mass, and rotary inertia of each rigid body and prints the results to the data (.dat) file if model definition data are requested . The following rules are used to determine the mass and inertia of a rigid body: • The mass of each continuum, structural, and rigid element that is part of the rigid body contributes to the rigid body’s mass, center of mass, and rotary inertia properties. • Point mass elements that are connected to any node that is part of a rigid body or to the rigid body reference node contribute to the rigid body’s mass, center of mass, and rotary inertia properties. • Rotary inertia elements that are connected to any tie node or to the rigid body reference node contribute to the rigid body’s rotary inertia properties. Since the rotational degrees of freedom at a pin node are not part of a rigid body, rotary inertia elements connected to a pin node do not contribute to the rigid body inertia but are rather associated with the independent rotation of the node. Defining mass and inertia properties by discretization In many cases it is desirable to model rigid components for which the mass, center of mass, and rotary inertia are not readily available. In Abaqus it is not necessary to define the mass and inertia properties of the rigid body directly. Instead, a finite element discretization can be used to model the rigid components, and Abaqus will automatically calculate the properties from the discretization. Rigid structures with one-dimensional rod or beam geometries can be modeled with beam or truss elements, structures containing two-dimensional surface geometries can be modeled with shell or membrane elements, and solid geometries can be modeled with solid elements. The mass contributions to the rigid body for each of these elements are based on that element’s section properties and the material density . Although both shell and membrane elements in a rigid body can yield similar mass contributions given similar section and density definitions, they will generate different node types (tie nodes for shells and pin nodes for membranes), which may affect the overall results. The same holds true for beam and truss elements. In situations where one portion of a rigid component can be modeled with a finite element discretization but it is not convenient to do so for other portions, point mass and rotary inertia elements can be used to represent the mass distribution of these other portions. The mass, center of mass, and rotary inertia for the rigid body will then include the contributions from both the finite elements and the point mass and rotary inertia elements. Abaqus uses the lumped mass formulation for low-order elements. As a consequence, the second mass moments of inertia can deviate from the theoretical values, especially for coarse meshes. This inaccuracy can be circumvented by adding point mass and rotary inertia elements with the correct inertia properties and eliminating the mass contribution from the solid elements. Alternatively, second-order elements could be used in Abaqus/Standard. Defining mass and inertia properties directly When the mass, center of mass, and rotary inertia properties of the actual rigid component are known or can be approximated, it is not necessary to use a finite element discretization or to use an array of point masses to generate the rigid body properties. You can assign these properties directly by locating the rigid body reference node at the center of mass and by specifying the rigid body mass and rotary inertia at the reference node . It may also be desirable to input mass properties directly at the center of mass but to specify boundary In this case you should place the rigid body conditions at a location other than the center of mass. reference node at the desired boundary condition location. In addition, you must define a tie node at the center of mass of the rigid body by correctly specifying its coordinates to coincide with the coordinates of the center of mass of the rigid body and then assigning it to a tie node set in the rigid body definition. You can then define the rigid body mass and rotary inertia at the tie node. For most applications where mass properties are input directly, it may be necessary to assign additional elements or nodes to a rigid body so that the rigid body can interact with the rest of the model. For example, contact pair definitions could require rigid surfaces formed with element faces on the rigid body and additional pin or tie nodes may be necessary to provide the desired constraints with deformable elements attached to the rigid body. Abaqus will account for the mass and rotary inertia contributions from all elements on a rigid body; therefore, if you want to assign the rigid body mass properties directly, you should take care to ensure that contributions from other element types that are part of the rigid body do not affect the desired input mass properties. If rigid elements are part of the rigid body definition, you can set their mass contribution to zero by not specifying a density for these elements in the rigid body definition. If other element types are used to define the rigid body, you should set their density to zero. Kinematics of a rigid body The motion of a rigid body is defined entirely by the motion of its reference node. The active degrees of freedom at the reference node depend on the geometry of the rigid body . The geometry of a rigid body is planar, axisymmetric, or three-dimensional and is determined by the type of elements that are assigned to the rigid body. In the case where no elements are assigned to a rigid body, the geometry of the rigid body is assumed to be three-dimensional. The calculated mass and rotary inertia properties for each of the active degrees of freedom for all rigid bodies are printed to the data (.dat) file if model definition data are requested . These properties include the contributions from elements that are part of the rigid body, as well as point mass and rotary inertia elements at the nodes of the rigid body. Although this calculated mass represents the true mass of the rigid body, Abaqus/Explicit actually uses an augmented mass in the integration of the equation of motion, which is conceptually similar to an added mass formulation. Essentially, the calculated mass and rotary inertia of the rigid body is augmented with the mass contributions of all of its attached deformable elements to create a larger, augmented mass and rotary inertia. Rotary inertia contributions from adjacent deformable elements are also included in the augmented rotary inertia if the nodal connection is at a tie node. Rigid body motions A rigid body can undergo free rigid body motion in each of its active translational degrees of freedom, as well as each of its active rotational degrees of freedom. Boundary conditions Boundary conditions for rigid bodies should be defined as described in “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1, at the rigid body reference node. Reaction forces and moments can be recovered for all degrees of freedom that are constrained at the reference node. If a nodal transformation is defined at the rigid body reference node, boundary conditions are applied in the local system . In Abaqus/Standard, if boundary conditions are applied to any nodes on a rigid body other than the rigid body reference node, Abaqus will attempt to transfer these boundary conditions to the reference node. If successful, you are warned that this transfer has taken place. Otherwise, an error message is produced . In Abaqus/Explicit, if boundary conditions are applied to any nodes on a rigid body other than the rigid body reference node, these boundary conditions are ignored with the exception of the symmetry-type boundary conditions that can affect the contact logic at the perimeter of a surface in the Abaqus/Explicit contact pair algorithm . Constraints In Abaqus/Standard nodes on a rigid body, excluding the rigid body reference node, cannot be used in a multi-point constraint or linear constraint equation definition. In Abaqus/Explicit a multi-point constraint or linear constraint equation can be defined for any node on a rigid body, including the reference node. Connector elements Connector elements can be used at any node of a rigid body, including the reference node, to define a connection between rigid bodies, between a rigid body and a deformable body, or from a rigid body to ground. Connector elements are convenient for providing multiple points of attachment on rigid bodies; modeling complex nonlinear kinematic constraints; specifying zero or nonzero boundary conditions at a point on a rigid body that is not the rigid body reference node; applying force actuation; and modeling discrete interactions, such as spring, dashpot, node-to-node contact, friction, locking mechanisms, and failure joints. Unlike multi-point constraints or linear constraint equations, connector elements retain degrees of freedom in the connection, thereby allowing output of information related to the connection (such as constraint forces and moments, relative displacements, velocities, accelerations, etc.). See “Connector elements,” Section 31.1.2, for a detailed description of connector elements. Planar rigid body A rigid body with a planar geometry has three active degrees of freedom: 1, 2, and 6 ( , and ). Here, the x- and y-directions coincide with the global X- and Y-directions, respectively. If a nodal transformation is defined at the rigid body reference node, the x- and y-directions coincide with the user- defined local directions. The coordinate transformation defined at the reference node must be consistent with the geometry; the local directions must remain in the global X–Y plane. All nodes and elements that are part of a planar rigid body should lie in the global X–Y plane. , Planar rigid bodies should be connected only to planar deformable elements. To model the connection of a rigid component with a planar geometry to three-dimensional deformable elements, model the planar rigid component as a three-dimensional rigid body consisting of the appropriate three-dimensional elements. Axisymmetric rigid body , A rigid body with an axisymmetric geometry has three active degrees of freedom in Abaqus: 1, 2, and 6 ( ). Classical axisymmetric theory admits only one rigid body mode, which is displacement in the z-direction. To maximize the flexibility of using rigid bodies for axisymmetric analysis, Abaqus allows for three active degrees of freedom, although only the axial displacement is a rigid body mode. , The r- and z-directions coincide with the global X- and Y-directions, respectively. If a nodal transformation is defined at the rigid body reference node, the r- and z-directions coincide with the user-defined local directions. The coordinate transformation defined at the reference node must be consistent with the geometry; the local directions must remain in the global X–Y plane. All nodes and elements that are part of an axisymmetric rigid body should lie in the global X–Y plane. Translation in the r-direction is associated with a radial mode, and rotation in the r–z plane is associated with a rotary mode . For an axisymmetric rigid body in Abaqus each of these modes develop no hoop stress, but mass and inertia computed for these degrees of freedom represent the modal mass associated with their modal motion. The mass properties for an axisymmetric rigid body are, therefore, calculated based on the initial configuration assuming the following: • Point masses defined on nodes of the rigid body are assumed to account for the entire mass around the circumference of the body. • Mass contributions from axisymmetric elements assigned to the rigid body include the integrated value around the circumference. • The center of mass of the rigid body is located at the center of mass of the circumferential slice, as shown in Figure 2.4.1–2. If the rigid body reference node is positioned at the center of mass, the reference node for an axisymmetric rigid body will, thus, be repositioned at the center of mass of the circumferential slice. These assumptions are consistent with the manner in which Abaqus handles other axisymmetric features but are noted here because of the deviation from classical rigid body theory. Axisymmetric rigid bodies should be connected only to axisymmetric deformable elements. To model the connection of a rigid component with an axisymmetric geometry to three-dimensional deformable elements, model the axisymmetric rigid component as a three-dimensional rigid body consisting of the appropriate three-dimensional elements. Three-dimensional rigid body , A rigid body with a three-dimensional geometry has six active degrees of freedom: 1, 2, 3, 4, 5, and 6 ( ). Here, the x-, y-, and z-directions coincide with the global X-, Y- and Z- directions, respectively. If a nodal transformation is defined at the rigid body reference node, the x-, y-, and z-directions coincide with the user-defined local directions. , , , , In general, three-dimensional rigid bodies will possess a full, nonisotropic inertia tensor and can behave in a nonintuitive manner when they are spun about an axis that is not one of the principal inertia axes. Classical phenomena of rigid body dynamics (e.g., precession, gyroscopic moments, etc.) can be simulated using three-dimensional rigid bodies in Abaqus. In most cases three-dimensional rigid bodies should be connected only to three-dimensional deformable elements. If it is physically relevant, a three-dimensional rigid body can be connected to two-dimensional plane stress, plane strain, or axisymmetric elements; however, you should always constrain the z-displacement, x-axis rotation, and y-axis rotation of the rigid body. The above procedure is useful when incorporating a two-dimensional plane strain approximation in one region of a model and a three-dimensional discretization in another. Rigid bodies can be used to constrain the two finite element geometries at their interface as shown in Figure 2.4.1–3. A unique rigid body should be used at each node in the plane along the interface to handle the constraint properly. Defining loads on rigid bodies Loads on a rigid body are assembled from contributions of all of the loads on nodes and elements that are part of the rigid body. Loads are defined on nodes and elements that are part of a rigid body in the original configuration rigid body center of mass radial mode rotary mode Figure 2.4.1–2 Axisymmetric rigid body modes. same manner that they are specified if the nodes and elements are not part of a rigid body. Contributions include: • applied concentrated forces on pin nodes, tie nodes, and the rigid body reference node; • applied concentrated moments on tie nodes and the rigid body reference node; and • applied distributed loads on all elements and surfaces that are part of the rigid body. rigid body 3D mesh 2D mesh rigid body Figure 2.4.1–3 Rigid body nodes used to connect a two-dimensional and three-dimensional mesh. Unless the point of action is through the rigid body center of mass, each of these loads will create both a force at and a torque about the center of mass, which will tend to rotate an unconstrained rigid body. If a nodal transformation is defined at any rigid body nodes, concentrated loads defined at these nodes are interpreted in the local system. The local system defined by the nodal transformation does not rotate with the rigid body. Concentrated moments defined on rigid body pin nodes do not contribute load to the rigid body but are rather associated with the independent rotation of that node. Independent rotation of a pin node exists only if it is connected to a deformable element with rotational degrees of freedom or a rotary inertia element. Follower forces can be defined at pin nodes if the independent rotation exists. However, the results may be nonintuitive since the direction of the force is determined by the independent rotation even though the follower force acts on the rigid body. Rigid bodies with temperature degrees of freedom Only rigid bodies that contain coupled temperature-displacement elements have temperature degrees of freedom. If it is reasonable to assume that a rigid body used in a fully coupled temperature-displacement analysis has a uniform temperature, you can define the rigid body as isothermal. A transient heat transfer process involving an isothermal rigid body assumes that the internal resistance of the body to heat is negligible in comparison with the external resistance. Thus, the body temperature can be a function of time but cannot be a function of position. The temperature degree of freedom that is created at the rigid body reference node describes the temperature of the body. Thermal interactions for rigid bodies with analytical rigid surfaces are available only in Abaqus/Explicit and are activated by specifying that the rigid body is isothermal. By default, rigid bodies are not considered isothermal and all nodes on a rigid body connected to coupled temperature-displacement elements will have independent temperature degrees of freedom. The fact that the nodes are part of a rigid body does not affect the ability of the coupled elements to conduct heat within the rigid body. However, the mechanical response will be rigid. The lumped heat capacitance associated with the rigid body reference node of an isothermal body is calculated automatically if the rigid body is composed of coupled temperature-displacement elements for which a specific heat and a density property are defined. Otherwise, you should specify a point heat capacitance for the rigid body . An error message will be issued in Abaqus/Explicit if no heat capacitance is associated with an isothermal rigid body for which temperature is not prescribed at the reference node. • The capacitance of each coupled temperature-displacement element that is part of the rigid body contributes to the isothermal rigid body’s capacitance. For an axisymmetric isothermal rigid body, capacitance contributions from axisymmetric elements assigned to the rigid body include the integrated value around the circumference. • HEATCAP elements that are connected to any node that is part of a rigid body or the rigid body reference node contribute to the isothermal rigid body’s capacitance. For an axisymmetric isothermal rigid body the point capacitances defined on nodes of the rigid body are assumed to account for the capacitance integrated around the circumference of the body. Thermal loads acting on the reference node of an isothermal body are assembled from contributions of all the thermal loads on nodes and elements that are part of the rigid body. Heat transfer between a deformable body and an isothermal rigid body can occur during contact, as well as when the bodies are not in contact if gap conductance and gap radiation are defined . Heat transfer between two isothermal rigid bodies can occur only via gap conduction and gap radiation. Input File Usage: Abaqus/CAE Usage: *RIGID BODY, ISOTHERMAL=YES Interaction module: Create Constraint: Rigid body: toggle on Constrain selected regions to be isothermal Modeling contact with a rigid body Contact with a rigid body is modeled by specifying a contact interaction formed with a rigid surface and with a surface defined on another body . A rigid surface can be formed by nodes, element faces, or an analytical surface . Contact modeling can be a primary factor when choosing the appropriate rigid body geometry. Contact interactions should be formed with surfaces of like geometry. For example, a planar rigid body should be used to model contact either with deformable surfaces formed by two-dimensional plane stress or plane strain elements or via node-based surfaces with two-dimensional beam, pipe, or truss elements. Similarly, an axisymmetric rigid body should be used to model contact with surfaces formed by axisymmetric elements, and a three-dimensional rigid body should be used to model contact either with surfaces formed by three-dimensional element faces or via node-based surfaces with three-dimensional beam, pipe, or truss elements. A rigid body must contain only two-dimensional or only three-dimensional elements. Nodes cannot be shared between two rigid bodies. Contact between two analytical rigid surfaces or between an analytical rigid surface and itself cannot be modeled. Limitations in Abaqus/Standard Contact between rigid bodies is allowed if the slave surface belongs to an elastic body that has been declared as rigid. In this case softened contact should be prescribed to avoid possible overconstraints. Contact between two rigid surfaces defined using rigid elements is not allowed. Rigid beams and trusses cannot be included in a contact pair definition because surfaces from beams and trusses can be node-based surfaces only. A node-based surface must be a slave surface, and elements that are part of a rigid body should be part of the master surface in a contact pair. Limitations in Abaqus/Explicit Contact between two rigid surfaces can be modeled in Abaqus/Explicit only if the penalty contact pair algorithm or the general contact algorithm is used; kinematic contact pairs cannot be used for rigid- to-rigid contact. Therefore, when converting two deformable regions of a model to two distinct rigid bodies for the purpose of model development, any contact interaction definitions between these rigid bodies must use penalty contact pairs or general contact. For rigid-to-rigid contact involving analytical rigid surfaces, at least one of the rigid surfaces must be formed by element faces since contact between two analytical rigid surfaces cannot be modeled in Abaqus. The penalty contact pair algorithm, which introduces numerical softening to the contact enforcement through the use of penalty springs, or the general contact algorithm must be used for all contact interactions involving a rigid body if an equation constraint, a multi-point constraint, a tie constraint, or a connector element is defined for a node on the rigid body. Rigid beams and trusses cannot be included in a kinematic contact pair definition because surfaces from beams and trusses can be node-based surfaces only. A node-based surface must be a slave surface, and elements that are part of a rigid body must be part of the master surface in a kinematic contact pair. When a rigid surface acts as a slave surface in a penalty contact pair or in general contact, initial penetrations of the rigid slave nodes into the master surface will not be corrected with strain-free corrections . For contact pairs any initial penetrations of this type may cause artificially large contact forces in the initial increments. For general contact these initial penetrations are stored as contact offsets. Using rigid bodies in geometrically linear Abaqus/Standard analysis If rigid bodies are used in a geometrically linear Abaqus/Standard analysis , the rigid body constraints are linearized. Consequently, except for analytical rigid surfaces, the distance between any two nodes belonging to the rigid body may not remain constant during the analysis if the magnitudes of the rotations are not small. 2.5 Integrated output section definition • “Integrated output section definition,” Section 2.5.1 2.5.1 INTEGRATED OUTPUT SECTION DEFINITION Products: Abaqus/Explicit Abaqus/CAE References • “Output to the output database,” Section 4.1.3 • *INTEGRATED OUTPUT SECTION • *INTEGRATED OUTPUT • *SURFACE • “Defining integrated output sections,” Section 14.13.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview An integrated output section: • can be two-dimensional or three-dimensional; • can be used to track the average motion of a surface; • can be used in association with integrated output requests to study the “force-flow” in the model; and • does not impose any constraint on the motion of the surface. Introduction An integrated output section is a way to associate a surface with a coordinate system and/or a reference node for one or both of the following purposes: • tracking the average motion of the surface; and/or • expressing the force and the moment transmitted through the surface in a local coordinate system, with the moment taken about a point that moves with the surface. The average motion of a surface can be obtained as the displacement and/or rotation history at the reference node on an integrated output section definition. You must define a reference node that is not connected to any other part of the finite element model and select whether the reference node follows only the average translation of the surface or both the translation and the rotation. Since the reference node is not connected to the rest of the model, an integrated output section definition used to track the average surface motion does not form a constraint on the motion of any nodes in the model. The “force-flow” in a complicated model can be studied using integrated output sections defined over a number of interior cross-section-like surfaces cutting through various parts of the model. It can be equally useful to sum forces over an exterior surface in contact or to sum forces transmitted through a tie constraint between surfaces, which is done by associating an integrated output section definition with an integrated output request. The vector output quantities can be expressed in a coordinate system of choice by specifying an orientation on an integrated output section definition. This coordinate system can rotate by an amount given by the rotational degrees of freedom at the reference node. In addition, the output of the integrated moment across the surface can be taken about a location that can translate by an amount given by the translational degrees of freedom at the reference node. Integrated output over a given surface can be requested with different coordinate systems and reference nodes by employing multiple integrated output section definitions over the same surface. Creating an integrated output section You must assign a name to each integrated output section. This name is used to associate the section with an integrated output request. In addition, you must identify the surface over which the section is being defined . Input File Usage: *INTEGRATED OUTPUT SECTION, NAME=section_name, SURFACE=surface_name Abaqus/CAE Usage: Step module: Output→Integrated Output Sections→Create: Name: section_name: select surface region Creating interior cross-section surfaces To study the “force-flow” through various paths in a model, you must create interior surfaces that cut through one or more regions (similar to a cross-section) so that you can request integrated output of the total force and moment transmitted across these surfaces. You can create such interior surfaces over the element facets, edges, or ends by simply cutting through one or more regions of the model with a plane; see “Creating interior cross-section surfaces” in “Element-based surface definition,” Section 2.3.2, for more information. The integrated output section reference node A reference node can be associated with an integrated output section for one or both of the following purposes: • tracking the average motion of the surface; and/or • computing the variables from an integrated output request in a coordinate system that moves with the motion of the reference node. If the average surface motion must be tracked, you must define a reference node that is not connected to any other part of the finite element model and select whether the reference node follows only the average translation of the surface or both the translation and the rotation. The rotational degrees of freedom will be activated in addition to the translational degrees of freedom at the reference node if it is selected to follow the average rotation of the surface. Further, the initial position of the reference node may be adjusted to lie at the center of the surface automatically. When an integrated output section with a reference node is associated with an integrated output request, the total moment transmitted through the section is computed with respect to the current location of the reference node. If the reference node has active rotational degrees of freedom, the coordinate system used to express the integrated output variables rotates with the rotation of the reference node. Positioning the reference node at the center of the surface The reference node can be repositioned automatically at the center of the surface in the initial configuration when the reference node is not connected to the rest of the model. The default is to leave the reference node in its specified position. Input File Usage: Abaqus/CAE Usage: Use the following option to position the reference node at the center of the surface: *INTEGRATED OUTPUT SECTION, REF NODE=n, POSITION=CENTER Step module: integrated output section editor: Anchor at reference point: Edit: select reference point: Move point to center of surface Setting the reference node to track the average motion of the surface It is often meaningful to obtain integrated output over a surface using a coordinate system and a point that moves with the average surface motion. When the reference node is not connected to the rest of the model, it can be specified to translate with the average translation of the surface without any rotation or to both translate and rotate with the average motion of the surface. The average motion is based on the mass weighted motion of the individual nodes that are on the surface and are not part of any rigid body. By default, the reference node does not track the average motion of the surface. Input File Usage: Abaqus/CAE Usage: Use the following option if the reference node must translate with the average translation of the surface: *INTEGRATED OUTPUT SECTION, REF NODE=n, REF NODE MOTION=AVERAGE TRANSLATION Use the following option if the reference node must both translate and rotate with the average translation of the surface: *INTEGRATED OUTPUT SECTION, REF NODE=n, REF NODE MOTION=AVERAGE Step module: integrated output section editor: Anchor at reference point: Edit: select reference point: Point motion: Average translation and rotation or Average translation The integrated output section local coordinate system You can define a local coordinate system on an integrated output section and associate the section with an integrated output request to express the integrated output variables in the local coordinate system. You can specify an orientation as the local coordinate system and, possibly, further project it onto the surface. Alternatively, you can form a local coordinate system by projecting the global coordinate system onto the surface following the Abaqus conventions . If a local system is not defined explicitly, the local system is initialized to the global coordinate system. The initial coordinate system, whether explicitly defined or initialized to the global coordinate system, will rotate with the deformation if a reference node is specified and that reference node has active rotational degrees of freedom. If the reference node is not connected to the rest of the model and its motion is based on both the average translation and rotation of the surface, the rotational and translational degrees of freedom are activated at the reference node. Input File Usage: Use the following option to define the initial coordinate system for the section: Abaqus/CAE Usage: *INTEGRATED OUTPUT SECTION, ORIENTATION=orientation_name Step module: integrated output section editor: CSYS: Edit: select orientation Projecting the coordinate system onto the section surface Either the coordinate system defined by the specified orientation or the global coordinate system can be projected onto the section surface to obtain a local coordinate system. Projection onto the surface is based on the average normal of the surface; the local 1-direction is formed perpendicular to the surface . Input File Usage: Use the following option to project the coordinate system onto the section surface: Abaqus/CAE Usage: *INTEGRATED OUTPUT SECTION, PROJECT ORIENTATION=YES Step module: integrated output section editor: Project orientation onto surface defined section anchor point anchor point elements used to define the section defined section 2-D and axisymmetric 3-D Figure 2.5.1–1 User-defined local coordinate system. Associating an integrated output section with an integrated output request An integrated output request is used to obtain history output of variables such as total force transmitted across a surface . Such a request may refer to an integrated output section definition to identify the surface where output is needed and to provide a local coordinate system and/or a reference node as a point about which the total moment across the surface is computed. Input File Usage: Use both of the following options to associate an integrated output section with an integrated output request: Abaqus/CAE Usage: *INTEGRATED OUTPUT SECTION, NAME=section_name *INTEGRATED OUTPUT, SECTION=section_name Step module: Output→Integrated Output Sections→Create: Name: section_name History output request editor: Domain: Integrated output section: section_name Limitations Integrated output sections are subject to the following limitations: • The surface associated with an integrated output section cannot be an analytical rigid surface. • The surface associated with an integrated output section can contain facets over rigid or axisymmetric elements. However, such an integrated output section cannot be associated with an integrated output request . 2.6 Mass adjustment • “Adjust and/or redistribute mass of an element set,” Section 2.6.1 ADJUST AND/OR REDISTRIBUTE MASS OF AN ELEMENT SET MASS ADJUST Product: Abaqus/Explicit References • “Density,” Section 21.2.1 • “Point masses,” Section 30.1.1 • “Nonstructural mass definition,” Section 2.7.1 • “Mass scaling,” Section 11.6.1 • *MASS ADJUST Overview Mass adjustment: • is useful to set the net mass of one or more components in the model to a known value; • is useful to account for any errors in mass due to modeling approximations; • is useful to account for mass from nonstructural features otherwise omitted from the model, such as paint; • can be applied over all element types that have mass; • adjusts the mass of the individual elements in an element set in proportion to their pre-adjusted mass including any nonstructural mass, so as to meet the specified target value for the set; • can be used to redistribute mass among elements in the set to raise the minimum stable time increment to a target value; • can be specified only once in an Abaqus/Explicit analysis during the model definition; and • can be applied in a hierarchical fashion to adjust the mass for individual parts first and then for an assembly of these parts. Adjusting the total mass of an element set to a known value The mass of a component in a numerical model may differ from its actual value for a number of reasons including modeling approximations and omission of minor features from the model. You can specify mass adjustment in the numerical model for such components by identifying the element sets defining these components and their respective total mass values. For a given element set, the mass is adjusted at the start of the analysis such that the adjustment in each element in that set is in proportion to the pre- adjusted mass of that element, thus preserving the center of mass and the principal directions of the rotary inertia. The pre-adjusted mass of an element includes the mass due to any associated material density; any mass directly specified on the section definition as in the case of beam, pipe, shell, membrane, rigid, and surface elements; and any nonstructural mass applied directly to that element. “Knee bolster impact with general contact,” Section 2.1.9 of the Abaqus Example Problems Manual, is an example of setting the total mass of an element set using mass adjustment. When mass is adjusted for an element with active rotational degrees of freedom, the rotary inertia contribution from that element is also modified proportionally to correspond with the scaling in the element mass from mass adjustment, thus preserving the principal directions of the rotary inertia. The adjusted mass value is considered when calculating the stable time increment of an element. Loads such as mass proportional damping and gravity take the adjusted mass into account. Mass adjustment can be applied in a hierarchical fashion to adjust the mass for individual parts first and then for an assembly of these parts. In this scenario, the mass adjustment defined over the assembly may further modify the adjusted mass of the individual parts. You must associate all of the mass-adjusted element sets in the desired order with a single mass adjustment definition. Abaqus/Explicit automatically calculates the mass, center of mass, and rotary inertia of each element set and prints the results to the data (.dat) file if model definition data are requested . The contributions from mass adjustment are also listed in these tables. Redistribution of mass to raise the minimum stable time increment to a target value You can increase the minimum stable time increment in the initial configuration for an element set to a specified target value by redistributing mass among the elements in that set. The redistribution of mass to affect the stable time increment and adjustment of mass to achieve a target total mass can be requested independently of each other. If both options are requested for a given element set, the mass is first adjusted to meet the target total mass for the set and then redistributed among the elements to achieve the target time increment. You can set a default target time increment that is applicable for all of the mass-adjusted element sets as well as specific targets for any of the individual element sets. Within each set, the mass is transferred to the elements with time increments below the target value from the remaining elements. Abaqus/Explicit prints the amount of mass available for redistribution along with the percentage of this amount that is redistributed to the data (.dat) file if model definition data are requested . If a sufficient amount of mass is not available to meet the specified target time increment, the analysis terminates with an error message. “Impact of a water-filled bottle,” Section 2.3.2 of the Abaqus Example Problems Manual, is an example of maintaining the target stable time increment of an element set using mass adjustment. When compared to the fixed mass scaling functionality, the redistribution feature above does not alter the total mass of the set. However, both features affect the center of mass and the principal directions of rotary inertia. The redistribution feature is performed only in the initial configuration at the start of the analysis; whereas the fixed mass scaling is performed in the configuration at the start of the step requesting that mass scaling. When you specify mass adjustment and mass scaling, the mass scaling adds mass as necessary on top of the adjusted mass. Defining mass adjustment To adjust the total mass of one or more components in the model, you first identify the corresponding element sets. If you specify multiple elements sets, the mass is adjusted in the order in which the element sets are specified. For element sets that share elements, you must determine the order in which to specify the element sets to obtain the desired results. Defining total mass for an element set without altering its center of mass You must specify the total mass for each mass-adjusted element set. *MASS ADJUST element_set_name, element_set_mass Input File Usage: Defining mass redistribution to raise the time increment You can redistribute the mass of an element set to achieve a target time increment and specify the total mass for each mass-adjusted element set, or you can redistribute the mass without changing the existing total mass of the element set. You can set a default target time increment that is applicable for all of the mass-adjusted sets as well as specific targets for any of the individual sets. When both a default target and a specific target are specified, the specific target is used for that set. Input File Usage: Use the following option to raise the time increment and specify the total mass: *MASS ADJUST, TARGET DT=min_stable_time_increment element_set_name, element_set_mass, element_set_min_stable_time_increment Use the following option to raise the time increment without altering the total mass: *MASS ADJUST, TARGET DT=min_stable_time_increment element_set_name, CURRENT, element_set_min_stable_time_increment 2.7 Nonstructural mass definition • “Nonstructural mass definition,” Section 2.7.1 2.7.1 NONSTRUCTURAL MASS DEFINITION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Point masses,” Section 30.1.1 • “Density,” Section 21.2.1 • “Adjust and/or redistribute mass of an element set,” Section 2.6.1 • *NONSTRUCTURAL MASS • “Defining nonstructural mass,” Section 33.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A nonstructural mass: • is a contribution to the model mass from features that have negligible structural stiffness (such as paint on sheet metal panels in a car); • can be used to bring the net mass of one or more components in the model up to a known value; • can be positive to add mass to the model and negative to remove mass from the model, with the corresponding increase or decrease in the element stable time increment in an Abaqus/Explicit analysis; • can be specified in the form of a total mass of the nonstructural features to be distributed over one or more components in the model; • can be specified in the form of an increase in density over the smeared region; • can be specified in the form of mass per unit area to be applied over a smeared region consisting of shells, membranes, and/or surface elements; and • can be specified in the form of mass per unit length to be applied over a smeared region consisting of beam, pipe, and/or truss elements. Nonstructural mass The mass contribution from nonstructural features can be included in the model even if the features themselves are omitted. The nonstructural mass is smeared over an element set that is typically adjacent to the nonstructural feature. This element set can contain solid, shell, membrane, surface, beam, pipe, or truss elements. The nonstructural mass can be specified in the following forms: • a total mass value, • a mass per unit volume, • a mass per unit area (for element sets that contain conventional shell, membrane, and/or surface elements), or • a mass per unit length (for element sets that contain beam, pipe, and/or truss elements). When a total mass is spread over an element set region, it can be distributed either in proportion to the underlying element “structural” mass or in proportion to the element volume in the initial configuration. A “structural” mass is defined as the sum of all the mass contributions to an element outside of the nonstructural features. This may include the mass due to any material definitions associated with the element; any “mass per unit area” given on the section definition for shell, membrane, and surface elements; mass from any rebars included in shell, membrane, and surface elements; and any additional inertia given on the section definition of beam/pipe elements. A nonstructural mass contribution to an element is not allowed if that element has no structural mass. A given element in the model can have contributions from multiple nonstructural mass specifications. The nonstructural mass in a given element will participate in any mass proportional distributed loads, such as gravity loading, defined on that element. When a nonstructural mass is added to a shell, beam, or pipe element with active rotational degrees of freedom, the nonstructural contribution affects both the element mass and the element rotary inertia. The element stable time increment increases with a positive nonstructural mass and decreases with a negative nonstructural mass. In general, it is easier to use a nonstructural mass definition to bring an additional mass into the model than to do the same with a group of point masses. It is also more beneficial in an Abaqus/Explicit analysis due to a possibly higher time increment. Any mass proportional damping specified as part of the material definition will also apply to the nonstructural mass contribution assigned to the element or element set using that material definition. Defining nonstructural mass To define a nonstructural mass contribution to the model mass, you must first identify the region over which the contribution must be added. You then specify the value of the nonstructural mass using the appropriate units and, if the total mass from the nonstructural features is known, determine how the nonstructural mass is distributed over the region. Input File Usage: Abaqus/CAE Usage: *NONSTRUCTURAL MASS, ELSET=element_set_name Property or Interaction module: Special→Inertia→Create: Nonstructural mass: select region Specifying the units of the nonstructural mass The nonstructural mass can be specified in different types of units, depending on the types of elements contained in the specified region. Specifying units of mass A total nonstructural mass with units of “mass” can be spread over a region containing solid, shell, membrane, beam, pipe, and/or truss elements. Input File Usage: *NONSTRUCTURAL MASS, UNITS=TOTAL MASS total mass of the nonstructural feature Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Nonstructural mass: select region: Units: Total Mass: Magnitude: total mass of the nonstructural feature Specifying units of mass per unit volume A nonstructural mass with units of “mass per unit volume” can be spread over a region containing solid, shell, membrane, beam, pipe, and/or truss elements. Input File Usage: *NONSTRUCTURAL MASS, UNITS=MASS PER VOLUME added density due to the nonstructural feature Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Nonstructural mass: select region: Units: Mass per Volume: Magnitude: added density due to the nonstructural feature Specifying units of mass per unit area A nonstructural mass with units of “mass per unit area” can be spread over a region containing conventional shells, membranes, and/or surface elements. Input File Usage: *NONSTRUCTURAL MASS, UNITS=MASS PER AREA added mass per unit area due to the nonstructural feature Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Nonstructural mass: select region: Units: Mass per Area: Magnitude: added mass per unit area due to the nonstructural feature Specifying units of mass per unit length A nonstructural mass with units of “mass per unit length” can be spread over a region containing beam, pipe, and/or truss elements. Input File Usage: *NONSTRUCTURAL MASS, UNITS=MASS PER LENGTH added mass per unit length due to the nonstructural feature Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Nonstructural mass: select region: Units: Mass per Length: Magnitude: added mass per unit length due to the nonstructural feature Controlling the distribution of the total mass from nonstructural features There are two methods available for distributing the nonstructural mass over the region when the total mass from the nonstructural features is known. Distributing the nonstructural mass in proportion to the element structural mass If you do not want to change the center of mass for the region, distribute the nonstructural mass in proportion to the element structural mass. This method results in a uniform scaling of the structural density of the region. Abaqus uses mass proportional distribution by default. The element structural mass in shell, membrane, and surface elements includes any mass the rebar are defined as a rebar layer . Input File Usage: *NONSTRUCTURAL MASS, UNITS=TOTAL MASS, DISTRIBUTION=MASS PROPORTIONAL total mass of the nonstructural feature Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Nonstructural mass: select region: Units: Total Mass: Magnitude: total mass of the nonstructural feature: Distribution: Mass Proportional Distributing the nonstructural mass in proportion to the element volume Alternatively, you can distribute the nonstructural mass in proportion to the element volume in the initial configuration. This method results in a uniform value added to the underlying structural density over the region. Therefore, the center of mass for the region may be altered if the region has nonuniform structural density. Input File Usage: *NONSTRUCTURAL MASS, UNITS=TOTAL MASS, DISTRIBUTION=VOLUME PROPORTIONAL total mass of the nonstructural feature Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Nonstructural mass: select region: Units: Total Mass: Magnitude: total mass of the nonstructural feature: Distribution: Volume Proportional 2.8 Distribution definition • “Distribution definition,” Section 2.8.1 2.8.1 DISTRIBUTION DEFINITION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Orientations,” Section 2.2.5 • “Material library: overview,” Section 21.1.1 • “Material data definition,” Section 21.1.2 • “Combining material behaviors,” Section 21.1.3 • “Density,” Section 21.2.1 • “Linear elastic behavior,” Section 22.2.1 • “Thermal expansion,” Section 26.1.2 • “Solid (continuum) elements,” Section 28.1.1 • “Membrane elements,” Section 29.1.1 • “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5 • “Using a general shell section to define the section behavior,” Section 29.6.6 • “Connectors: overview,” Section 31.1.1 • “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 35.4.4 • “Boundary conditions in Abaqus/CFD,” Section 33.3.2 • *DISTRIBUTION • *DISTRIBUTION TABLE • Chapter 63, “The Discrete Field toolset,” of the Abaqus/CAE User’s Manual Overview A distribution: • is a spatially varying field defined over elements or nodes in an Abaqus model; • can be used to define shell thicknesses on an element-by-element basis; • can be used to define shell stiffness on an element-by-element basis; • can be used to define local coordinate systems on solid continuum and shell elements on an element- by-element basis; • can be used to define orientation angles on the layers of composite shell elements; • can be used to define orientation angles for connector elements; • can be used to define thicknesses on the layers of conventional composite shell elements; • can be used to specify initial contact clearances; • can be used to specify pressure that varies with the total volume of fluid crossing a surface in an Abaqus/CFD analysis; and • in an Abaqus/Standard analysis can be used to define mass density, linear elastic material behavior, and thermal expansion for solid continuum elements; shell offsets; orientation angles on the layers of composite solid continuum elements; local coordinate systems on membrane elements; and membrane thickness on an element-by-element basis. Distributions A distribution is a spatial analogy of an amplitude definition . Amplitude definitions are used to provide arbitrary time variations of loads, displacements, and other prescribed variables. Distributions are used to specify arbitrary spatial variations of selected element properties, material properties, local coordinate systems, and spatial variations of initial contact clearances. The two main components of a distribution are its location and field data. The location identifies where the distribution is defined, either on elements or nodes. Field data are a specified number of floating point values defined for each element or node in the distribution. To define a distribution, you must assign it a unique name. You must also specify the number and physical dimension of each data value in the distribution by referring to a distribution table. Input File Usage: Abaqus/CAE Usage: *DISTRIBUTION, NAME=name, TABLE=distribution table name Abaqus/CAE supports distributions using discrete fields. Property, Interaction, or Load module: Tools→Discrete Field→Create Specifying the location of a distribution You can define a distribution on elements or nodes. Currently distributions on nodes are supported only for defining initial contact clearances as described in “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 35.4.4. For a distribution used with fluid boundary definitions in Abaqus/CFD, you specify that no location is required. All other applications of distributions require distributions defined on elements. There is no limit on the number of distributions to which a given element or node may belong. Elements and nodes cannot be combined within the same distribution definition. Defining a distribution on elements Defining a distribution on elements requires you to specify field data for each element or element set included in the distribution definition. All distributions on elements require that default data be defined. Default data are used for all elements that are not specifically assigned a value in the distribution. *DISTRIBUTION, LOCATION=ELEMENT blank space, field data element set or element number, field data Input File Usage: Default data are defined by using a blank space instead of an element number or element set for the first data item on the first data line of a distribution definition. Only one set of default data can be defined for a distribution. If you specify only default data, all elements that reference that distribution use the default values. If an element is specified more than once in a given distribution definition, the last specification given is used. Abaqus/CAE Usage: Property, Interaction, or Load module: Tools→Discrete Field→Create: Definition: Elements Defining a distribution on nodes Defining a distribution on nodes requires you to specify field data for each node or node set included in the distribution definition. Input File Usage: *DISTRIBUTION, LOCATION=NODE node set or node number, field data If a node is specified more than once in a given distribution definition, the last specification given is used. Abaqus/CAE Usage: Defining a distribution on nodes for initial contact clearances is not supported in Abaqus/CAE. Defining a distribution used in Abaqus/CFD For a distribution used to define fluid boundary conditions for pressure that varies with the total volume of fluid crossing a surface, you specify field data and that no location is required. Input File Usage: *DISTRIBUTION, LOCATION=NONE field data, field data Abaqus/CAE Usage: Defining a distribution used in Abaqus/CFD is not supported in Abaqus/CAE. Defining a distribution table Every distribution definition must refer to a distribution table. A distribution table defines the number of field data items needed for each element or node in a distribution. The distribution table also defines the physical dimension of each data value in a distribution. A distribution table can be referred to as many times as needed by different distributions. The distribution table consists of a list of predefined labels shown in Table 2.8.1–1 and Table 2.8.1–2. The combination of labels needed for a given distribution is determined by how the distribution is applied. Input File Usage: Use the following option to define a distribution table: *DISTRIBUTION TABLE, NAME=distribution table name list of distribution table labels Abaqus/CAE Usage: Abaqus/CAE creates a distribution table when you specify a distribution by selecting a discrete field. Defining a distribution table used in Abaqus/CFD is not supported in Abaqus/CAE. Table 2.8.1–1 Distribution table labels—Abaqus/Standard and Abaqus/Explicit. Data label Physical dimension Number of data items per label ANGLE COORD3D DENSITY EXPANSION LENGTH MODULUS RATIO SHELLSTIFF1 SHELLSTIFF2 SHELLSTIFF3 angle in degrees (L, L, L) ML−3 −1 FL−2 dimensionless FL-1 FL Table 2.8.1–2 Distribution table labels—Abaqus/CFD. Data label Physical dimension PRESSURE VOLUME FL−2 L3 Number of data items per label Applying distributions The data defined in a distribution are not used in an Abaqus analysis unless the distribution is referred to by name by a feature that supports distributions, and the distribution is applied only to the elements or nodes that are associated with the referenced feature. In addition, a distribution definition can be referenced more than one time in a given model. These points are illustrated in the examples below. Examples The simple examples below illustrate how distributions are defined. A large number of illustrative example problems using distributions can be found in “Spatially varying element properties,” Section 5.1.4 of the Abaqus Verification Manual. Example 1 A distribution for shell thickness is defined and applied to two different shell section definitions through the SHELL THICKNESS parameter—as noted above the distribution dist0 would not be used if it is not referred to by a feature that supports distributions. See “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, for more details. The distribution table defines both the number of data values (one) and the physical dimension (LENGTH) of the thickness data. The thicknesses defined in distribution dist0 are assigned only to shell elements that belong to the element set elset1 or elset2. The default thickness (t0 ) defined in the first data line of dist0 will be assigned to all elements in elset1 and elset2 that are not explicitly assigned a thickness in dist0. *DISTRIBUTION TABLE, NAME=tab0 LENGTH *DISTRIBUTION, NAME=dist0, LOCATION=element, TABLE=tab0 , t0 element set or number, t1 element set or number, t2 … *SHELL SECTION, ELSET=elset1, SHELL THICKNESS=dist0 *SHELL SECTION, ELSET=elset2, SHELL THICKNESS=dist0 Example 2 A distribution for spatially varying isotropic elastic material behavior is defined and applied to a material definition (“Linear elastic behavior,” Section 22.2.1). This material is then referred to by a solid section definition. This is important because like any material definition, a material defined by a distribution is not used unless it is referred to by a section definition, and then it is applied only to the elements associated with the section definition. The distribution table defines both the number of data values (two) and the physical dimensions (MODULUS and RATIO) of the isotropic elastic data. Other material behaviors (in this case plasticity) can also be included in the material definition. The default elastic constants (E0 , 0 ) in distribution dist1 will be assigned to all elements in elset3 that are not explicitly assigned elastic constants in dist1. *DISTRIBUTION TABLE, NAME=tab1 MODULUS, RATIO *DISTRIBUTION, NAME=dist1, LOCATION=element, TABLE=tab1 , E0, 0 element set or number, E1, 1 element set or number, E2, 2 … *MATERIAL, NAME=MAT *ELASTIC dist1 *PLASTIC … *SOLID SECTION, ELSET=elset3, MATERIAL=MAT Example 3 A spatially varying local coordinate system ( “Orientations,” Section 2.2.5) is defined by specifying both spatially varying coordinates for points a and b as well as a spatially varying additional rotation angle. This orientation is then referred to by a general shell section definition. This is important because like any orientation definition, an orientation defined by a distribution is not used unless it is referred to by a section definition, and then it is applied only to the elements associated with the section definition. The distribution table for the coordinates specifies COORD3D twice to indicate that data for two three- dimensional coordinates points must be specified for each element in the distribution. *DISTRIBUTION TABLE, NAME=tab2 COORD3D, COORD3D *DISTRIBUTION, NAME=dist2, LOCATION=element, TABLE=tab2 , aX0,aY0 ,aZ0 ,bX0,bY0 ,bZ0 element set or number, aX1,aY1 ,aZ1 ,bX1,bY1 ,bZ1 element set or number, aX2,aY2 ,aZ2 ,bX2,bY2 ,bZ2 … *DISTRIBUTION TABLE, NAME=tab3 ANGLE *DISTRIBUTION, NAME=dist3, LOCATION=element, TABLE=tab3 , 0 element set or number, 1 element set or number, 2 … *ORIENTATION, NAME=ORI, DEFINITION=COORDINATES dist2 3, dist3 *SHELL GENERAL SECTION, ELSET=elset4, ORIENTATION=ORI Example 4 Spatially varying thicknesses and orientation angles are defined on the layers of a composite shell element. The distribution table for the thicknesses specifies LENGTH, and the distribution table for the orientation angles specifies ANGLE. A distribution of thicknesses is used on layers 1 and 3, while a distribution of angles is used on layers 2 and 3. *DISTRIBUTION TABLE, NAME=tableThick LENGTH *DISTRIBUTION, NAME=thickPly1, LOCATION=element, TABLE=tableThick , t0 element set or number, t1 element set or number, t2 … *DISTRIBUTION, NAME=thickPly3, LOCATION=element, TABLE=tableThick , t0 element set or number, t1 element set or number, t2 … *DISTRIBUTION TABLE, NAME=tableOriAngle ANGLE *DISTRIBUTION, NAME=oriAnglePly2, LOCATION=element, TABLE=tableOriAngle , element set or number, element set or number, … *DISTRIBUTION, NAME=oriAnglePly3, LOCATION=element, TABLE=tableOriAngle , element set or number, element set or number, … *SHELL SECTION, ELSET=elset1, COMPOSITE thickPly1, 3, mat1, 0. 1., 3, mat2, oriAnglePly2 thickPly3, 3, mat3, oriAnglePly3 2.9 Display body definition • “Display body definition,” Section 2.9.1 2.9.1 DISPLAY BODY DEFINITION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • *DISPLAY BODY • “Defining display body constraints,” Section 15.15.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A display body: • can be two-dimensional planar, axisymmetric, or three-dimensional; • is associated with a part instance and up to three reference nodes, such that the motion of the part instance is governed by the motion of the reference nodes; • is used for display purposes only and does not take part in the analysis; • can be used to make the analysis more efficient while improving visualization of analysis results; and • is especially useful for mechanism or multibody dynamic analyses. What is a display body? A display body is a part instance that is used for display only. None of the nodes or elements of the instance take part in the analysis, but they are still available during postprocessing. The motion of the display body is governed by the motion of the associated reference nodes, if any. It behaves like a rigid body since the relative positions of the nodes and elements of the part instance remain constant throughout a simulation. The nodes and elements of the part instance cannot be used to define prescribed conditions, interactions, constraints, etc. Section properties do not have to be assigned to the elements. A display body is useful in cases where the physical model is different from the idealized model used for the analysis. An idealized model may be difficult to visualize; it may help to include more details in the model for realistic postprocessing purposes. Display bodies allow this without increasing the analysis time. Display bodies are especially useful in mechanism or multibody dynamics problems where rigid parts interact with each other via connectors. In such cases a part can be represented by a very simple rigid body and a more complex display body. In this case, the rigid body can be as simple as just a node, along with mass and rotary inertia elements attached to that node. Display bodies can also be used to model stationary objects that are not involved in the analysis but aid in visualization. Creating a display body You must specify the part instance to be made a display body. Input File Usage: Abaqus/CAE Usage: *DISPLAY BODY, INSTANCE=name Interaction module: Create Constraint: Display body: select part instance The reference nodes If the display body is not associated with any reference nodes, it will remain fixed in space during the analysis. However, you can specify that the motion of the display body should be governed by the motion of selected reference nodes. These nodes must belong to another part instance in the assembly. They cannot belong to another display body definition. If you specify only one reference node, the display body will translate and rotate based on the translations and rotations of that node during the analysis. If the reference node has no rotational degrees of freedom, the display body will not rotate during the analysis. If you specify three reference nodes, the display body will translate and rotate based on the translations of all three nodes. The new position of the part instance at any time will be calculated from the new position and orientation of the coordinate system defined by the three reference nodes: the first node will be the origin, the second will be a point in the x-direction, and the third node will be a point in the X–Y plane. Care should be taken when specifying the three nodes so that they do not become colinear at any stage of the analysis. If this occurs, the position of the part instance may change abruptly through that increment. Input File Usage: Abaqus/CAE Usage: *DISPLAY BODY, INSTANCE=name first reference node number, second reference node number, third reference node number Interaction module: Create Constraint: Display body: select part instance, choose Follow single point or Follow three points, click Edit, and select the reference points Using display bodies with connectors Display bodies can be used effectively in models containing rigid part instances that interact with each other using connector elements. Such models need both rigid bodies and display bodies. The rigid body should contain any nodes used by connectors, used to define mass and inertia properties, and used to apply loads or boundary conditions. The display body should contain the nodes and elements representing the physical part. Care should be taken to ensure that the nodes in the rigid body are not part of the display body. The reference node of the display body will typically be the same as the rigid body reference node. Figure 2.9.1–1(a) illustrates a model containing rigid bodies and a display body. Part instance A is included in a display body definition. Figure 2.9.1–1(b) shows the same model without the display body. This model will actually be involved in the analysis. The connector node and reference node form a rigid body that represents the analysis version of part instance A. Both these nodes are assembly-level nodes and are not included in the display body. Connector node Connector Reference node Reference node Connector node Connector (a) (b) Figure 2.9.1–1 Example of a display body. Input file template The following input shows how display bodies can be used in a model with rigid part instances and connectors: *ASSEMBLY ... *INSTANCE, NAME=INST1 ... *END INSTANCE *NODE, NSET=INST1-REFNODE 1001, -10, 0, 0 *NODE, NSET=INST1-CONNECTOR-NODE 1002, -5, -5, 0 *RIGID BODY, TIE NSET=INST1-CONNECTOR-NODE, REF NODE=INST1-REFNODE *DISPLAY BODY, INSTANCE=INST1 1001 ... *END ASSEMBLY 2.10 Assembly definition • “Defining an assembly,” Section 2.10.1 2.10.1 DEFINING AN ASSEMBLY Products: Abaqus/Standard Abaqus/Explicit References • *ASSEMBLY • *INSTANCE • *PART Overview A finite element model in Abaqus can be defined as an assembly of part instances. The organization of such a model: • is consistent with models generated by Abaqus/CAE and displayed in the Visualization module (Abaqus/Viewer); and • allows reuse of part definitions, which is valuable for creating large, complex models. allows reuse of part definitions, which is valuable for creating large, complex models. By default, input files written by Abaqus/CAE are written in terms of an assembly of part instances. For input files not written by Abaqus/CAE, the use of part and assembly definitions in the input file is currently optional. However, since the Visualization module displays results in terms of an assembly of part instances, an assembly and at least one part instance will be created automatically by the analysis input file processor if they are not defined in the input file. Introduction A physical model is typically created by assembling various components. The assembly interface in Abaqus allows analysts to create a finite element mesh using an organizational scheme that parallels the physical assembly. In Abaqus the components that are assembled together are called part instances. This section explains how to organize an Abaqus finite element model in terms of an assembly of part instances. The mesh is created by defining parts, then assembling instances of each part. Each part can be used (instanced) one or more times, and each part instance has its own position within the assembly. This organization of the model definition matches the way models are created in Abaqus/CAE, where the assembly can be created interactively or imported from an input file . Terminology Assembly An assembly is a collection of positioned part instances. An analysis is conducted by defining boundary conditions, constraints, interactions, and a loading history for the assembly. Part A part is a finite element idealization of an object. Parts are the building blocks of an assembly and can be either rigid or deformable. Parts are reusable; they can be instanced multiple times in the assembly. Parts are not analyzed directly; a part is like a blueprint for its instances. Part instance A part instance is a usage of a part within the assembly. All characteristics (such as mesh and section definitions) defined for a part become characteristics for each instance of that part—they are inherited by the part instances. Each part instance is positioned independently within the assembly. Example A hinge can be modeled using two flanges and a pin, as shown in Figure 2.10.1–1. The flange geometry is defined by creating a part, which is instanced twice inside the hinge assembly. Another part, the pin, is created and instanced once. The pin is modeled as a rigid body created from an analytical surface . The Hinge Assembly Part instance Flange-2 Part instance Flange-1 Ref Pt Ref Part instance Pin-1 Figure 2.10.1–1 The hinge assembly. This hinge example is used throughout this section to illustrate the keyword interface for parts and assemblies. This example is also used to illustrate the interactive assembly process . Defining parts, part instances, and the assembly Everything defined within a part, instance, or the assembly is local to that part, instance, or the assembly. This means that node/element identifiers and names (like set and surface names) need not be unique throughout a model; they need only be unique within the part, instance, or assembly where they are being defined . Names should not use an underscore to join part instance names to element set, node set, orientation names, or distribution names because the names may conflict with internal names used by Abaqus. For example, consider Figure 2.10.1–2. In this model the assembly (Hinge) contains three part instances (Flange-1, Flange-2, and Pin-1). Multiple sets named top can be defined: in this case one is defined within the assembly and one is defined within each of the Flange part instances. The set name top can be reused, and each set named top is independent from the others. assembly part instance set: top Hinge Flange-1 Pin-1 Flange-2 set: top set: top Figure 2.10.1–2 The organization of the Hinge assembly. Input File Usage: Use the following options to begin and end each part, instance, and assembly definition: *PART/*END PART *INSTANCE/*END INSTANCE *ASSEMBLY/*END ASSEMBLY If any one of these options appears in an input file, they must all appear except when you import a part instance from a previous analysis; in this case *PART and *END PART are not required. The model must be consistently defined as an assembly of part instances. Defining a part A part definition must appear outside the assembly definition. Multiple parts can be defined in a model; each part must have a unique name. Input File Usage: Use the following options to define a part: *PART, NAME=PartName Node, element, section, set, and surface definitions *END PART Defining part instances A part instance definition must appear within the assembly definition. If the part instance is not imported from a previous analysis, each part instance must have a unique name and refer to a part name. A part instance name of Assembly is not allowed. In addition, you can specify data that are used to position the instance within the assembly. Give a translation and rotation for the part instance relative to the origin of the assembly (global) coordinate system. If the part instance is to be imported from a previous analysis, each part instance must specify the name of the instance to be imported. For more information on defining part instances for use with the import capability, see “Transferring results between Abaqus analyses: overview,” Section 9.2.1. Additional sets and surfaces can be defined at the instance level, as explained later in this section. Input File Usage: Use the following options to instance a part that is not imported from a previous analysis: *INSTANCE, NAME=InstanceName, PART=PartName Additional set and surface definitions (optional) *END INSTANCE Repeat these options, each time referring to the same part name, to instance a part multiple times. Use the following options to import a part instance from a previous analysis: *INSTANCE, INSTANCE=instance-name Additional set and surface definitions (optional) *IMPORT *END INSTANCE Defining the assembly Only one assembly can be defined in a model. All part instance definitions must appear within the assembly definition. Sets and surfaces can be defined at the assembly level by including the appropriate definitions within the assembly definition. Input File Usage: Use the following options to create an assembly: *ASSEMBLY, NAME=name Part instance definitions Set and surface definitions Connector and constraint definitions Rigid body definitions *END ASSEMBLY Example The hinge assembly shown in Figure 2.10.1–1 can be defined using the following syntax in the input file: *PART, NAME=Flange *NODE, NSET=Flange 1, ... 2, ... ... 360, ... *ELEMENT, ELSET=Flange 1, ... 2, ... ... 200, ... *SOLID SECTION, ELSET=Flange, MATERIAL=Steel *ELSET, ELSET=Flat, GENERATE 176, 200, 1 *SURFACE, NAME=Flat Flat, S1 *END PART *PART, NAME=Pin *NODE, NSET=RefPt 1, ... *SURFACE, TYPE=REVOLUTION, NAME=Pin ... *RIGID BODY, REF NODE=1, ANALYTICAL SURFACE=Pin *END PART *ASSEMBLY, NAME=Hinge *INSTANCE, NAME=Flange-1, PART=Flange *END INSTANCE *INSTANCE, NAME=Flange-2, PART=Flange *END INSTANCE *INSTANCE, NAME=Pin-1, PART=Pin *END INSTANCE *ELSET, ELSET=Top ... *NSET, NSET=Output ... *END ASSEMBLY *MATERIAL, NAME=Steel ... Notes • All of the nodes and elements that describe the Flange part are defined between the *PART and *END PART options. The section definition (*SOLID SECTION) must also appear within the part definition. • At least one element set must be defined within the Flange part so that the section definition can refer to it. Additional node and element sets can also be defined in the part. • The Flange part is instanced twice in the Hinge assembly. Therefore, the model contains two element sets named Flat: one belongs to part instance Flange-1, and the other belongs to part instance Flange-2. • When a meshed part is instanced, the node and element numbers are repeated in each part instance. • The Pin part is instanced once. It is a rigid body created from an analytical surface . • Keywords can be indented to help clarify the definition of each part, part instance, and assembly. Organizing the model definition In a traditional Abaqus model without an assembly definition, the components of the model fall into one of two categories: model data (step independent) and history data (step dependent). In an Abaqus model that is organized into an assembly of part instances, all components are further categorized and must fall within the proper level: part, assembly, instance, step, or model. Step-level components correspond to history data; all step-dependent component definitions must appear within a step definition . Model-level data include everything that does not fall into part-, assembly-, instance-, or step-level data (for example, material definitions; see Figure 2.10.1–3). The proper level within which a keyword option must appear in the input file is indicated at the top of each section in the Abaqus Keywords Reference Manual. Rules for defining an assembly The organization shown in Figure 2.10.1–3 is achieved by following a few basic rules. Referring to items between levels When creating a model, it is often necessary to refer to something outside of the current level; for example, a section definition within a part must refer to a material, which is defined at the model level. Loads defined within a step must refer to sets within the assembly. But some references between levels are not allowed; for example, a set in one part instance cannot refer to nodes in another part instance. The following references are allowed: An Abaqus model Part Assembly Mesh Node Set Element Set Surface Local Coordinate System Section Definition Constraint Reference Point Part level Model data Node Set Element Set Surface Section Definition Constraint Reference Point Local Coordinate System Part Instance Mesh Node Set Element Set Surface Local Coordinate System Section Definition Constraint Reference Point Part instance level Assembly level Material Amplitude Physical Constants Interaction Property Interaction Initial Condition Boundary Condition Model level Analysis Step Output Database Request Restart Output Request Diagnostic Output Request Load Boundary Condition Predefined Fields Interaction Property Interaction Step level History data Figure 2.10.1–3 Organization of a model defined in terms of an assembly of part instances. A definition within: Can refer to items within: the assembly an instance an instance a part a step the model the model the model the assembly an instance the model These rules are illustrated in Figure 2.10.1–4. Naming conventions The Abaqus naming conventions allow for a model that contains an assembly. When something is defined within a part, instance, or the assembly and is referred to from outside its level, the complete name must be used to identify it (set Flat of instance Flange-2 in assembly Hinge, for example). A complete Part instance Part instance Model Step Assembly Part Allowable reference between levels Figure 2.10.1–4 Allowable references between levels. name is given in the input file using “dot” notation: each name in the hierarchy is separated by a “.” (period). For example, some complete names in the Hinge assembly are Hinge.Flange-2.Flat Hinge.Output An element set that belongs to part instance Flange-2. A node set that belongs to assembly Hinge. Such names would be used to refer to the sets from outside the assembly. The same syntax is used to refer to individual nodes or elements. Hinge.Flange-1.3 Hinge.Flange-2.11 A node or element that belongs to part instance Flange-1. A node or element that belongs to part instance Flange-2. As always, the context determines whether a node or element is being referred to. The “.” has special meaning; it is used to separate the individual names in a complete name. Therefore, the “.” cannot be used in labels such as set and surface names. For example, *ELSET, ELSET=Set.1 *ELSET, ELSET=Set1 Error OK Complete names are limited to 80 characters, including the periods. However, when referring to a name in an input file that is not defined in terms of an assembly of part instances, the “.” in the name should be replaced by underscores. Such a situation can occur, for example, when an element set from a previous analysis is referred to by the current analysis but the current input file is not defined in terms of an assembly of part instances. Quoted labels Labels for set and surface names can be defined by enclosing the label in quotation marks . Any subsequent use of the label in a complete name must be enclosed in quotation marks as well. For example, *PART, NAME=Flange ... *ELSET, ELSET="Set 1" ... *END PART ... *ELEMENT OUTPUT, ELSET=Hinge.Flange-1."Set 1" Example An assembly node set Top can be defined by the following syntax: *ASSEMBLY, NAME=Hinge ... *NSET, NSET=Top Flange-1.2, Flange-1.5, ... Flange-2.1, Flange-2.4, ... *END ASSEMBLY Since the node set is defined within the assembly level, Hinge. is not part of the complete names given on the data lines. However, the prefix Hinge. would be required to request output for this node set, since the output request exists within the step definition, which is outside the assembly level. *STEP ... *NODE OUTPUT, NSET=Hinge.Top *END STEP Similarly, a boundary condition could be applied to a set defined for part instance Flange-2. *STEP ... *BOUNDARY Hinge.Flange-2.FixedEnd, 1, 3 *END STEP The mesh (nodes and elements) • The mesh can be defined either on a part or on an instance of that part (not both). Typically, parts are meshed and instances inherit that mesh, but it is not required. If, for example, you want to use fully integrated elements for one part instance and reduced-integration elements for another, or if you want to define a more refined mesh on one part instance than on another, you must mesh the instances separately. – If the mesh is defined on a part, it is inherited by every instance of that part. – If the mesh is defined on a part, it cannot be redefined (overridden) on an instance of that part. In other words, if the node and element definitions appear within the part definition, they cannot appear within the instance definition for that part. – If a mesh is not defined on a part, it must be defined on every instance of that part. • A part definition is required even if no mesh is defined on it. In such cases the empty part definition is used only to relate various instances to each other via the instance definitions. This allows the Visualization module to group information by part. • Rebar must be defined within a part along with the elements that are being reinforced. • Reference nodes can be created at the assembly level. • Only mass, rotary inertia, capacitance, connector, spring, and dashpot elements can be created at the part or the assembly level. All other element types must be defined within a part (or part instance). To define assembly-level elements that refer to part-level nodes, include the part instance name when defining the element connectivity. For example: *ELEMENT, TYPE=MASS 1, Instance-1.10 Section definitions • Sections must be assigned where the mesh is defined (either within a part definition or within each instance of the part). • If a part is meshed, all instances of that part have the same element types and are made of the same materials. • The set referred to by a section definition must be created at the same level as the mesh and section definition. • If the part is meshed, the section assignment cannot be overridden at the instance level. Sets and surfaces • Sets and surfaces (rigid or deformable) can be created within a part, part instance, or the assembly. – Sets and surfaces can be created on a part if a mesh is defined on the part. – Sets and surfaces defined on a part are inherited by each instance of that part. – Assembly-level sets and, in Abaqus/Standard, slave surfaces can span part instances. • If an element set or node set definition with the same name appears more than once at the same level, the new members are appended to the set. • A surface definition cannot appear more than once with the same surface name within the same level. • New sets and surfaces can be created on a part instance. If a set or surface is defined on a part instance and a set or surface with that name was not defined on the part, the set or surface is added to the instance. • Sets and surfaces cannot be redefined on a part instance. If a set or surface is defined on a part instance and a set or surface with that name was also defined on the part, an error will be generated. • Sets and surfaces are not step dependent. All sets and surfaces must be defined within a part, part instance, or the assembly. Defining assembly-level sets You can refer to a part instance from an element set or node set definition as a shortcut to using the complete name when defining assembly-level sets. Specify the name of the instance that contains the specified elements or nodes. To add elements or nodes from more than one instance to the set, repeat the element set or node set definition . Input File Usage: Use the following options to define assembly-level sets: *NSET, NSET=NsetName, INSTANCE=InstanceName *ELSET, ELSET=ElsetName, INSTANCE=InstanceName Adding sets and surfaces on restart • Existing sets and surfaces cannot be redefined on restart. • Analytical surfaces cannot be created on restart. • New sets and surfaces (excluding analytical surfaces) can be added to part instances or the assembly on restart. To add a set or surface, give the complete name. As in the original analysis, you can refer to the part instance name from the element set or node set definition to define an assembly-level set in the restart analysis. For example, *HEADING *RESTART, READ, STEP=1 ** Add element set "Bottom" to assembly "Hinge": *ELSET, ELSET=Hinge.Bottom Flange-1.40, Flange-2.99 ** Add node set "Top" to assembly "Hinge": *NSET, NSET=Hinge.Top, Instance=Flange-1 21, 22, 23, 24, 26, 28, 31 *NSET, NSET=Hinge.Top, Instance=Flange-2 21, 22, 23, 24, 26, 28, 31 ** ** Add element set "Right" to part instance "Flange-2": *ELSET, ELSET=Hinge.Flange-2.Right 16, 18, 20, 29 ** ** Add surface "surfR" to part instance "Flange-2": *SURFACE, TYPE=ELEMENT, NAME=Hinge.Flange-2.surfR Right, S1 ** *STEP ... *END STEP Rigid bodies Rigid bodies can be defined at the part or assembly level. • To define a rigid body at the part level, include the rigid body and rigid body reference node definitions within the part definition. – Rigid elements, deformable elements, and analytical surfaces cannot be combined within a part. – If a rigid body is defined within a part, all deformable, rigid, or connector elements in the part must belong to the rigid body. – Mass, rotary inertia, spring, dashpot, and heat capacitance elements can be included in a part that contains a rigid body definition, but these elements cannot belong to the rigid body. – To create a part-level rigid body from an analytical surface, include the surface definition within the part definition. Only one analytical surface is allowed per part. • To define a rigid body at the assembly level, include the rigid body and reference node definitions within the assembly definition. – A rigid body can be created at the assembly level from any combination of rigid elements, deformable elements, and up to one analytical surface. – The rigid body definition can refer to assembly-level or part-level sets. – A part that contains a rigid body definition cannot be included in an assembly-level rigid body. • You can define a discrete surface at the part or assembly level independent from the rigid body definition. • An analytical surface definition can appear only within a part definition, even if the rigid body is defined at the assembly level. Materials • Materials are defined at the model level so that they can be reused. The material definition cannot appear within a part, part instance, or the assembly. • All materials in a model must have unique names. Interactions An interaction is a relationship between surfaces or between a surface and its environment. Interactions in Abaqus include contact, radiation, film conditions, and element foundations. • Interactions are defined at the model level in Abaqus/Standard and at the model level or within steps in Abaqus/Explicit; they cannot be defined within a part, assembly, or instance. Constraints Constraints are inflexible coupling mechanisms such as MPCs and equations . • Constraints can be defined within a part or the assembly. They can be defined within a part instance if the mesh is defined within the part instance. Constraints should be defined at the assembly level if they constrain the motion of one part instance relative to another. • Constraints are translated and rotated according to the positioning data given for a part instance. Distributions Distributions are used to specify arbitrary spatial variations of selected element properties, material properties, local coordinate systems, and spatial variations of initial contact clearances . • Distributions should be defined at the level at which they are used. For example, if a distribution is used to define shell thicknesses, the distribution should be defined at the same level as the section definition that refers to it. If a distribution is used to define a material property, it should be defined at the model level with the material definition. Examples In the following examples most parameters and data lines are omitted for clarity. Example 1 *PART, NAME=PartA *NODE ... *ELEMENT ... *SOLID SECTION, ELSET=setA, MATERIAL=Mat1 *SURFACE, NAME=surf1 setB, ... *ELSET, ELSET=setA *NSET, NSET=setA *SURFACE, NAME=surf2 setA, ... Notes The mesh is defined on the part. error Section assignment must appear within the part level if the mesh is defined on the part. Element set setB is not defined at the part level. Sets and surfaces can be defined on the part since the mesh is defined on the part. Example 1 Notes *END PART *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=I1, PART=PartA *NODE *ELEMENT *SOLID SECTION *ELSET, ELSET=setA *NSET, NSET=setA *SURFACE, NAME=surf2 *ELSET, ELSET=setB *NSET, NSET=setB *SURFACE, NAME=surf3 setA, ... *END INSTANCE *END ASSEMBLY error error error error error error Mesh and section assignment cannot be defined on the instance if they are defined on the part. Sets and surfaces cannot be redefined on the instance. New sets and surfaces can be defined on the instance. Set and surface definitions can refer to inherited sets. In the second example the instances are meshed. Example 2 Notes *PART, NAME=PartB *END PART *PART, NAME=PartC *SOLID SECTION, ... *END PART *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=I1, PART=PartB *NODE ... *ELEMENT ... *SOLID SECTION, ELSET=setA, MATERIAL=Mat1 *ELSET, ELSET=setA *NSET, NSET=setA *SURFACE, NAME=surf2 setA, ... *END INSTANCE The *PART and *END PART options are required, even when the instance is meshed. Section cannot be defined on the part if mesh is not defined on the part. error The mesh is defined on the part instance. Section assignment must appear within the same level as the mesh definition. Sets and surfaces are defined on the instance since the mesh is defined on the instance. Example 2 Notes *INSTANCE, NAME=I3, PART=PartC *END INSTANCE *END ASSEMBLY Coordinate system definitions error The mesh and section must be defined for each instance since the part is not meshed. Abaqus provides several methods for defining local coordinate systems. Nodal coordinate systems You can define nodal coordinates in a local coordinate system . The coordinate system can be defined within a part definition to define the nodes in that part. The nodal coordinate system definition remains in effect until another nodal coordinate system is defined within the same level or until the level ends. Nodal transformations A nodal transformation is used for applying loads and boundary conditions . It can be defined at the part or assembly level to define a local coordinate system for application of loads and boundary conditions or for the definition of linear constraint equations. User-defined orientations A user-defined orientation is used for defining material properties, coupling, connectors, and rebar . It can be defined at the part level for reference from a section, connector, rebar, or coupling definition. An orientation definition can also be used at the assembly level for reference from a connector or coupling definition. Distributions Distributions can be used to specify arbitrary spatial variations of local coordinate systems for continuum and shell elements . A distribution used by an orientation should be defined at the level in which the orientation is defined. Normal definitions at nodes Normals can be defined at nodes as part of the node definition for beam, pipe, and shell elements or with a user-specified normal definition . These normals can be defined at the part or assembly level. A local coordinate system defined for a part using any of these methods is inherited by all instances of the part. Translating and rotating a part instance The assembly’s coordinate system is the global coordinate system. You can position part instances within the assembly by giving a translation and/or rotation relative to the global origin. Specify a translation by giving a translation vector. Specify a rotation by giving two points, a and b, to define a rotation axis plus a right-handed angular rotation around that axis. Local coordinate systems defined within a part or part instance will be translated and rotated according to the specified positioning data, as shown in Figure 2.10.1–5. (In this figure details such as element and section definitions are omitted for clarity.) Results given in a local coordinate system are output in the transformed local system. Equations will also be translated and rotated according to the positioning data for an instance. All data within a part (or part instance) definition are defined relative to the part’s local coordinate system; positioning data are applied to a part instance after everything within that instance is defined. Limitations The following capabilities are not supported in a model defined in terms of an assembly of part instances: • “Mapping a set of nodes from one coordinate system to another” in “Node definition,” Section 2.1.1 • “Using auxiliary analyses to generate shape variations” in “Parametric shape variation,” Section 2.1.2 • “Symmetric model generation,” Section 10.4.1 • “Transferring results from a symmetric mesh or a partial three-dimensional mesh to a full three- dimensional mesh,” Section 10.4.2 • “Reading the element matrices from an Abaqus/Standard results file” in “User-defined elements,” Section 32.15.1 The substructure library is not organized in terms of an assembly of part instances, so substructures cannot be generated from models that have an assembly defined. None of the substructure options are supported in models that have an assembly defined. Input file template This template shows an input file that is written in terms of parts and assemblies with the part instances defined in this analysis. For templates that show how to import a part instance from a previous analysis to transfer model data and results, see “Transferring results between Abaqus/Explicit and Abaqus/Standard,” Section 9.2.2, and “Transferring results from one Abaqus/Standard analysis to another,” Section 9.2.3. *HEADING *PART, NAME=Part-1 Node, element, section, set, and surface definitions Connector and constraint definitions *END PART *PART, NAME=Part-2 *Part, Name=P *System *Node *End part *Part, Name=Q *Node *End part Local coordinate system defined relative to part coordinate system Nodes defined in local coordinate system Local coordinate system only applies within this part definition Nodes defined in part coordinate system *Assembly, Name=Assembly-1 *Instance, Name=Instance-1, Part=Q *End Instance *Instance, Name=Instance-2, Part=P *End Instance *Instance, Name=Instance-3, Part=P *End Instance *End assembly Instances positioned relative to global coordinate system Instance-2 Instance-1 Instance-3 Assembly-1 coordinate system Position given relative to the assembly (global) coordinate system (defined by ∗INSTANCE) Part-local coordinate system (defined by ∗NORMAL, ∗ORIENTATION, ∗SYSTEM, or ∗TRANSFORM) Figure 2.10.1–5 Defining local coordinate systems. **The instance is meshed, so the part definition is empty *END PART *MATERIAL, NAME=mat1 Suboptions and data lines to define this material *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=i1, PART=Part-1 Additional set and surface definitions (optional) *END INSTANCE *INSTANCE, NAME=i2, PART=Part-2 Node, element, section, set, and surface definitions Connector and constraint definitions *END INSTANCE Assembly-level set and surface definitions Assembly-level connectors and constraints Assembly-level reference node definitions Assembly-level rigid body definitions *END ASSEMBLY *MATERIAL, NAME=mat2 Suboptions and data lines to define this material *AMPLITUDE *INITIAL CONDITIONS *BOUNDARY Zero-valued boundary conditions *PHYSICAL CONSTANTS *CONNECTOR BEHAVIOR Suboptions and data lines to define this connector behavior Interaction and interaction property definitions in Abaqus/Standard or Abaqus/Explicit *STEP Loads and boundary conditions Predefined field definitions Output requests Contact interaction definitions in Abaqus/Explicit *END STEP 2.11 Matrix definition • “Defining matrices,” Section 2.11.1 2.11.1 DEFINING MATRICES Product: Abaqus/Standard References • “Generating matrices,” Section 10.3.1 • *MATRIX ASSEMBLE • *MATRIX GENERATE • *MATRIX INPUT • *MATRIX OUTPUT Overview A matrix: • can be used to represent stiffness, mass, viscous damping, or structural damping for a part of the model or for the entire model; • is defined by giving it a unique name and by specifying matrix data, which may be scaled; • can be symmetric or unsymmetric; • can be given in text format in lower triangular, upper triangular, or square form or read from binary .sim files generated by the matrix generation procedure; • can be used to provide linear elastic response with large translations but not large rotations; • can be used in static and natural frequency extraction procedures; • can be used in matrix generation and substructure generation procedures; • can be used in transient modal dynamics, mode-based steady-state dynamics, subspace-based steady-state dynamics, random response, response spectrum, and complex eigenvalue extraction procedures that use the SIM architecture; • can have loads, boundary conditions, and constraints applied directly to any matrix nodal degrees of freedom; • can be used in submodeling analysis; and • cannot be used in direct steady-state dynamic or mode-based analyses that do not use the SIM architecture. What is a matrix in Abaqus/Standard? Designing complex models of structures like automobiles typically involves subcontracting the work on various parts. When the entire model has to be put together, information about the parts needs to be exchanged between different vendors. Often, to avoid the exchange of proprietary information, this information is exchanged in terms of matrices representing the stiffness, mass, and damping for each part. During an analysis these matrices are added to the corresponding global finite element matrices to complete the assembly of the entire model. Abaqus/Standard provides the capability to input stiffness, mass, viscous damping, and structural damping matrices directly. You can define as many different matrices as are necessary to build the model. Including matrices in a model You must assign a name to the matrix to include it in the matrix usage model. Input File Usage: *MATRIX INPUT, NAME=name Specifying a matrix type For matrices given in text format, you can specify the matrix type as symmetric (default) or unsymmetric. If symmetric, it can be entered as a lower triangular, upper triangular, or square matrix. For matrices read from a .sim file, the matrix type is automatically set according to the matrix data stored on the SIM database. Input File Usage: Use one of the following options to specify the type for matrices given in text format: *MATRIX INPUT, NAME=name, TYPE=SYMMETRIC *MATRIX INPUT, NAME=name, TYPE=UNSYMMETRIC Scaling the matrix data You can define a multiplication scale factor for all matrix entries. Input File Usage: *MATRIX INPUT, NAME=name, SCALE FACTOR=sval Providing matrix data directly You can specify data directly to define a symmetric matrix in lower triangular, upper triangular, or square format. For a square matrix to be symmetric, corresponding entries above and below the diagonal must have exactly the same values. You can specify data directly to define an unsymmetric matrix by providing data for each matrix entry. Input File Usage: *MATRIX INPUT row node label, degree of freedom for row node, column node label, degree of freedom for column node, matrix entry Repeat this data line to specify data for each matrix entry. Reading the matrix data in text format from an alternate file Matrix data in text format can be contained in an alternate file. Typically, an alternate file is used for large matrices. To ensure acceptable performance, the data lines in the alternate file are read without extensive checking for data format. You should make sure that the data entries are specified in the proper format without any comments or blank lines. Matrix data output in text format can be generated in the matrix generation procedure . Input File Usage: *MATRIX INPUT, NAME=name, INPUT=input_file_name Reading the matrix data from the SIM database Matrix data in binary format can be read from the .sim file generated by the matrix generation procedure . The .sim file can contain stiffness, mass, viscous damping, and structural damping matrices. You specify each matrix to be read from the .sim file. Input File Usage: Use the following options: *MATRIX INPUT, NAME=stif_name, INPUT=sim_file_name, MATRIX=STIFFNESS *MATRIX INPUT, NAME=mass_name, INPUT=sim_file_name, MATRIX=MASS *MATRIX INPUT, NAME=dmpv_name, INPUT=sim_file_name, MATRIX=VISCOUS DAMPING *MATRIX INPUT, NAME=dmps_name, INPUT=sim_file_name, MATRIX=STRUCTURAL DAMPING Defining the stiffness, mass, and damping with matrices included in a model You can assemble the stiffness, mass, viscous damping, and structural damping matrices that you have specified into the corresponding global finite element matrices for the model. Many matrices with different names can be defined and assembled. Input File Usage: Use the following option to assemble matrices generated from the same original model: *MATRIX ASSEMBLE, STIFFNESS=stif_name, MASS=mass_name, VISCOUS DAMPING=dmpv_name, STRUCTURAL DAMPING=dmps_name To assemble matrices generated from different original models, repeat the *MATRIX ASSEMBLE option for each model. Connecting a part of a model represented by matrices A part of the model represented by user-defined matrices is connected to other parts and finite elements through shared nodes. You must define these nodes directly in the model . In addition, there may be nodes that are used only by matrices but that are not shared. You do not need to define nodes that are not shared and have no loads, boundary conditions, or constraints associated with them; these nodes will be defined for you and placed at the origin of the global coordinate system. Input File Usage: Use the following option to define the shared nodes directly: *NODE Remapping user-defined nodes in assembled matrices The nodes defined in the assembled matrices can be remapped (renamed) to different node labels in the matrix usage model. You must define all the new node labels in the matrix usage model, create a node set from them, and specify this node set when assembling the matrices. The size of the node set and the order of the nodes in the set must fully correspond to the combined set of nodes of all the matrices that are assembled. The matrix nodes are assumed to be sorted in ascending order of their original labels that were defined at generation or specified in the matrix data. Input File Usage: Use the following option to create a node set for the matrix nodes: *NSET, NSET=nset_name, UNSORTED Use the following option to assemble matrices with node remapping: *MATRIX ASSEMBLE, STIFFNESS=stif_name, MASS=mass_name, VISCOUS DAMPING=dmpv_name, STRUCTURAL DAMPING=dmps_name, NSET=nset_name Multiple instantiation of matrices With the node remapping feature, the same matrix can be used multiple times in the matrix usage model. You define the matrix once and assemble it several times, specifying the relevant node sets for remapping. Input File Usage: *MATRIX INPUT, NAME=name *MATRIX ASSEMBLE, STIFFNESS=name *MATRIX ASSEMBLE, STIFFNESS=name, NSET=nset1_name *MATRIX ASSEMBLE, STIFFNESS=name, NSET=nset2_name Internal nodes in matrix data Internal nodes are nodes with internal degrees of freedom associated with them (for example, Lagrange multipliers and generalized displacements) that are created internally by Abaqus/Standard. By definition, user-defined nodes have positive node labels, and internal nodes have negative node labels. You can use the matrix generation procedure to designate some of the user-defined nodes as internal nodes to hide them in the matrix usage model . When using matrix data that contains internal nodes, these nodes are remapped automatically to unique internal node labels in the matrix usage model. For assembled matrices that originate from the same model, the internal nodes are shared. For assembled matrices that originate from different models, the internal nodes are mapped to different internal nodes in the matrix usage model, even if they have the same negative node labels. Using matrices in nonlinear analyses When you use matrices in a nonlinear analysis procedure, nonlinearities are not accounted for. Since the matrix data remain unchanged during the analysis, only linear elastic material behavior can be represented and only large translations can be modeled correctly in a geometrically nonlinear analysis. Changes to the matrix due to large rotations or load stiffness are not computed in a geometrically nonlinear analysis. Using matrices in linear perturbation analyses Matrices can be used in a static perturbation analysis as well as in a natural frequency extraction analysis using the Lanczos or AMS eigensolver. For certain quantities (such as participation factors and global inertia properties) to be computed properly, the coordinates of the nodes associated with the matrices should be defined in the model using matrices. Matrices can also be used in modal analysis procedures using the high-performance SIM architecture; namely, steady-state dynamic, modal dynamic, random response, response spectrum, and complex frequency extraction analyses. Matrices can be used in the substructure generation and matrix generation procedures as well. Matrices cannot be used in the direct-solution steady-state dynamic analysis procedure and in modal procedures that are not based on the high-performance SIM architecture. Constraints and transformations Kinematic constraints (for example, coupling constraints, linear constraint equations, multi-point constraints, or surface-based tie constraints) can be applied to any nodes in a model containing matrices. Since kinematic constraints in Abaqus/Standard are usually imposed by eliminating degrees of freedom at the dependent nodes, matrix nodes should not be used as dependent nodes. To apply contact constraints on matrix nodes, a node-based surface must be defined on these nodes and this surface should be used as the slave surface in the contact pair definition. Nodal transformations defined at nodes that appear in the matrix do not affect the matrix. The matrix entries corresponding to these nodes are assumed to be in the local coordinates defined by the nodal transformations. Initial conditions Initial conditions can be specified as usual; however, only node-based initial conditions can be applied to nodes that appear in matrices. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. Boundary conditions Boundary conditions can be specified as usual. See “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Matrix nodes can be defined as driven nodes in a submodel analysis ; they cannot be defined as driving nodes in a global model. For shell-to-solid submodeling, matrix nodes that are defined as driven nodes are treated as lying within the center zone no matter how far they are from the shell reference surface. Loads Concentrated nodal forces can be applied at displacement degrees of freedom (1–6) of any node as usual. Distributed pressure forces can be applied to surface elements defined over matrix nodes (see “Surface elements,” Section 32.7.1). Body forces cannot be applied to parts of the model represented by matrices. User-defined loads can be applied with the same restrictions as above for distributed pressure forces and body forces. Predefined fields can be applied at any nodes as usual ; however, matrix data are not affected by predefined fields. For example, if temperatures are specified as a predefined field on nodes that appear on a matrix, only the elements that share these nodes with the matrix experience thermal strains if thermal expansion is specified for those elements. The matrix does not experience any thermal strains, but it may experience linear elastic forces due to displacements at shared nodes. Elements All elements that can be used in static stress analysis are available . Output All nodal output variables that apply to static analysis are available . Limitations The following are known limitations to using matrices: • An analysis that contains matrices cannot be restarted. In addition, matrices cannot be introduced in a restart analysis. • Matrices cannot be used in a model containing parts and assemblies. • Matrices containing acoustic pressure and mechanical degrees of freedom will disable the coupled acoustic structural eigenvalue extraction. • Matrices containing Lagrange multiplier degrees of freedom can produce inaccurate results in Abaqus/Standard analysis procedures that use the direct sparse solver, except for analysis procedures based on the AMS eigensolver or using the eigenmodes extracted with the AMS eigensolver. To address this limitation, you can set the constraint optimization solver control for the analysis procedure. Setting this solver control is helpful if the matrix data contain up to several hundred Lagrange multipliers. However, for matrices with a larger number of Lagrange multipliers, using the constraint optimization solver control can significantly affect performance or the analysis may fail due to insufficient memory. Setting this solver control does not help for matrices generated from models using hybrid elements. • In an Abaqus/Standard analysis using matrix input data for the mass matrix, inertia quantities for the global model that are reported in the data (.dat) file, including coordinates of the center of mass and moments of inertia, may be calculated incorrectly. • Matrices cannot be used in analyses with inertia relief loads. DEFINING MATRICES *HEADING … *NODE Data lines to specify nodes *NSET, NSET=NSET1, UNSORTED Data lines to specify a node set with the nodes in a particular order … *BOUNDARY Data lines to specify zero-valued boundary conditions *MATRIX INPUT, NAME=MAT1, SCALE FACTOR=sval Data lines to specify a stiffness matrix *MATRIX INPUT, NAME=MAT2, SCALE FACTOR=sval Data lines to specify a mass matrix *MATRIX INPUT, NAME=MAT3, SCALE FACTOR=sval Data lines to specify a viscous damping matrix *MATRIX INPUT, NAME=MAT4, INPUT=input_file_name *MATRIX INPUT, NAME=MAT5, INPUT=input_file_name *MATRIX INPUT, NAME=MAT6, INPUT=sim_file_name, MATRIX=STIFFNESS *MATRIX ASSEMBLE, STIFFNESS=MAT1, MASS=MAT2, VISCOUS DAMPING=MAT3, STRUCTURAL DAMPING=MAT4 *MATRIX ASSEMBLE, STIFFNESS=MAT6, MASS=MAT5 *MATRIX ASSEMBLE, STIFFNESS=MAT6, MASS=MAT5, NSET=NSET1 *STEP(,NLGEOM)(,PERTURBATION) Use NLGEOM to include nonlinear geometric effects; it will remain active in all subsequent steps. *STATIC *BOUNDARY Data lines to prescribe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD Data lines to specify loads *END STEP *STEP *FREQUENCY *BOUNDARY Data lines to prescribe zero-valued or nonzero boundary conditions *END STEP *STEP *STEADY STATE DYNAMICS *CLOAD and/or *DLOAD Data lines to specify loads *END STEP Job Execution Execution procedures: overview Execution procedures Environment file settings Managing memory and disk resources Parallel execution File extension definitions FORTRAN unit numbers JOB EXECUTION 3.1 3.2 3.3 3.4 3.5 3.6 3.1 Execution procedures: overview • “Execution procedure for Abaqus: overview,” Section 3.1.1 EXECUTION PROCEDURE FOR Abaqus: OVERVIEW EXECUTION PROCEDURE: OVERVIEW Overview Abaqus is executed by using the Abaqus execution procedure. In the following discussion the command to run the execution procedure is assumed to be abaqus. However, you can customize the execution procedure to run Abaqus using any alias you choose. The abaqus command is described in “Execution procedures,” Section 3.2. The following sections contain further information about running Abaqus jobs: • “Using the Abaqus environment settings,” Section 3.3.1 • “Managing memory and disk use in Abaqus,” Section 3.4.1 • “Parallel execution,” Section 3.5 • “File extensions used by Abaqus,” Section 3.6.1 • “FORTRAN unit numbers used by Abaqus,” Section 3.7.1 Conventions The following conventions are used in these sections: • Each discussion includes a “Command summary” section that provides the syntax for the command in the left column and the syntax for its options in the right column. The full command must appear first, followed by the options. In some cases the command has multiple words, such as abaqus cae; you must enter all words of the command before issuing any option statements. • Options are presented in boldface. They can appear in any order and can be abbreviated. • Default options are underlined ( __ ). • Items enclosed in square brackets ([ ]) are optional. • Items appearing in a list separated by bars ( | ) are mutually exclusive. • One value must be selected from a list of values enclosed by curly brackets ({ }). • You must supply values in italics. • Blanks are used as separators between options and must not precede nor follow an equal sign. • An alternate syntax of -option value can be used instead of the option=value format. The abaqus procedure will prompt for any information required that is not provided on the command line. If abaqus is typed with no options, prompts are issued for all options. Environment settings The Abaqus execution procedure uses “environment” settings to customize the execution of a job. These settings can be changed using the Abaqus environment file, abaqus_v6.env. The execution procedure looks for this file in two places other than the installation location when running a job. The first place it looks is in your home directory. If it exists, the settings in this file will be applied to all jobs that you run. The second place the execution procedure looks is in the current directory. If the file exists, the settings defined there will be applied to all jobs run from that directory. If the same job parameter is defined in more than one environment file or is defined more than once within the same environment file, the last definition encountered will be used. Some exceptions to this rule are noted in “Using the Abaqus environment settings,” Section 3.3.1. These environment files can be used to customize the behavior of Abaqus, including modification of the default options. See “Using the Abaqus environment settings,” Section 3.3.1, for further information on the environment files. Selecting TCP/UDP port numbers Several of the execution procedure command line options, such as port and listenerport, require that you specify a port number. TCP/UDP port numbers can range from 0 to 65535. Port numbers 0 to 1023 are well-known ports used by system processes (such as FTP, SSH, SMTP, etc.) and should never be used. Port numbers 1024 to 49151 are registered ports with the Internet Assigned Number Authority (IANA) by software vendors. These ports can be used, but you should be careful that you are not conflicting with any software installed on your system that may be using this port. Port numbers 49152 to 65535 are unreserved and can be used freely, as long as no other application uses them. Ports may be blocked by a firewall. Contact your system administrator to ensure that the ports that you want to specify are not blocked. You can use the netstat command to obtain information on TCP/UDP network connections. 3.2 Execution procedures • “Obtaining information,” Section 3.2.1 • “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2 • “SIMULIA Co-Simulation Engine controller execution,” Section 3.2.3 • “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution,” Section 3.2.4 • “Abaqus/CAE execution,” Section 3.2.5 • “Abaqus/Viewer execution,” Section 3.2.6 • “Python execution,” Section 3.2.7 • “Parametric studies,” Section 3.2.8 • “Abaqus documentation,” Section 3.2.9 • “Licensing utilities,” Section 3.2.10 • “ASCII translation of results (.fil) files,” Section 3.2.11 • “Joining results (.fil) files,” Section 3.2.12 • “Querying the keyword/problem database,” Section 3.2.13 • “Fetching sample input files,” Section 3.2.14 • “Making user-defined executables and subroutines,” Section 3.2.15 • “Input file and output database upgrade utility,” Section 3.2.16 • “Generating output database reports,” Section 3.2.17 • “Joining output database (.odb) files from restarted analyses,” Section 3.2.18 • “Combining output from substructures,” Section 3.2.19 • “Combining data from multiple output databases,” Section 3.2.20 • “Network output database file connector,” Section 3.2.21 • “Mapping thermal and magnetic loads,” Section 3.2.22 • “Fixed format conversion utility,” Section 3.2.23 • “Translating Nastran bulk data files to Abaqus input files,” Section 3.2.24 • “Translating Abaqus files to Nastran bulk data files,” Section 3.2.25 • “Translating ANSYS input files to Abaqus input files,” Section 3.2.26 • “Translating PAM-CRASH input files to partial Abaqus input files,” Section 3.2.27 • “Translating RADIOSS input files to partial Abaqus input files,” Section 3.2.28 • “Translating Abaqus output database files to Nastran Output2 results files,” Section 3.2.29 • “Translating LS-DYNA data files to Abaqus input files,” Section 3.2.30 • “Exchanging Abaqus data with ZAERO,” Section 3.2.31 • “Encrypting and decrypting Abaqus input data,” Section 3.2.32 • “Job execution control,” Section 3.2.33 3.2.1 OBTAINING INFORMATION Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The Abaqus execution procedure can be used to obtain help regarding command syntax or information about the installation and computing environment. Command summary abaqus Command line options help {help | information={environment | local | memory | release | support | system | all} [job=job-name] | whereami} This option prints a summary of the abaqus command syntax. information This option writes information about the installation and the environment that is in effect to the screen. The following information is output for all information requests: the current release, the directory in which Abaqus is located, and the directory in which the information files are located. If information=environment, the current settings of the environment file options are displayed. If information=local, the local installation notes are output. If information=memory, some suggestions for setting memory parameters for analysis jobs are output. If information=release, information is provided about where to locate the current release notes. If information=support, information on diagnosing hardware-related issues is provided. Please send this information to systems support when requesting assistance. If information=system, information is provided about system software and hardware resources (operating system level, compiler levels, processor type, graphics board, memory, etc). If information=all, information on all of the above information topics is output. job If a job-name is specified, the information text is written to the file job-name.log. whereami This option prints the location of the Abaqus release directory. Examples Use the following command to display the local installation notes: abaqus information=local The following command will write the local installation notes to the file support.log: abaqus information=local job=support Abaqus/Standard, Abaqus/Explicit, AND Abaqus/CFD EXECUTION ANALYSIS EXECUTION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD are executed by running the Abaqus execution procedure. Several parameters can be set either on the command line or in the environment file . Alternatively, you can use the convenient Abaqus/CAE user interface to submit an Abaqus analysis from an input file and set the analysis parameters; see “Understanding analysis jobs,” Section 19.2 of the Abaqus/CAE User’s Manual. Abaqus enforces a character limit on file names. For any command line reference to a file, the total length of the file name, including the path description, cannot exceed 256 characters. job=job-name [analysis | datacheck | parametercheck | continue | convert={select | odb | state | all} | recover | syntaxcheck | information={environment | local | memory | release | support | system | all}] [input=input-file] [user={source-file | object-file}] [oldjob=oldjob-name] [fil={append | new}] [globalmodel={results file-name | output database file-name}] [cpus=number-of-cpus] [parallel={domain | loop}] [domains=number-of-domains] [dynamic_load_balancing] [mp_mode={mpi | threads}] [standard_parallel={all | solver}] [gpus=number-of-gpgpus] [memory=memory-size] [interactive | background | queue=[queue-name] [after=time] ] [double={explicit | both | off | constraint}] [scratch=scratch-dir] [output_precision={single | full} ] [field={odb | exodus | nemesis} ] [history={odb | csv} ] [madymo=MADYMO-input-file] 3.2.2–1 Command summary Command line options Required option job [host=co-simulation hostname] [port=co-simulation port-number] [listenerport=Co-Simulation Engine listener port-number] [remoteconnections=Co-Simulation remote job host:port-number] [timeout=co-simulation timeout value in seconds] [unconnected_regions={yes | no}] Engine host:port-number, The value of this option specifies the name of all files generated during the run and the name of files that are read in the continue, convert, and recover phases. If this option is omitted from the command line, you will be prompted for its value (except when only the informational options described in “Obtaining information,” Section 3.2.1, are used). If the input option is not supplied, the procedure will look for an input file called job-name.inp in the current directory. Mutually exclusive options that determine which phases of an analysis are performed All options are order independent. If none of these options is present, the analysis option is assumed. The convert option is an exception to the mutual exclusion rule: convert can appear with any option except datacheck, parametercheck, syntaxcheck, and information. The convert and parametercheck options are not available for Abaqus/CFD. analysis This option indicates that a complete Abaqus analysis (or a restart of an Abaqus analysis) is to be performed. datacheck This option indicates that the run is for data checking only. No analysis will be performed. If this option is used, all files necessary to continue the analysis are saved. parametercheck This option indicates that the run is for input parameter checking only (parameter definitions must have been used; see “Parametric input,” Section 1.4.1). No analysis or data checking will be performed. This option is not applicable for Abaqus/CFD. continue This option indicates that the run is to begin at the point at which a previous data check run ended. convert The value of this parameter indicates which files will be postprocessed. This option is not applicable for Abaqus/CFD. Results can be converted either immediately following an analysis run, as a separate run subsequent to an analysis run, or while an analysis is running as follows: 1. To run an analysis including a subsequent conversion of the results, use the convert option in conjunction with the job and analysis options. 2. To convert the results of a previously run analysis, use the convert option in conjunction with the job option. 3. To convert results from a job that is currently running, use the convert option in conjunction with the oldjob option (to name the running job) and the job option (to supply a new name for the files generated by the convert option). If convert=select, the Abaqus/Explicit selected results file (job-name.sel) will be converted into a standard Abaqus results file (job-name.fil). If the analysis is run in parallel with parallel=domain, the separate selected results files (job-name.sel.n) will be converted into a single selected results file (job-name.sel) prior to being converted into a standard Abaqus results file. If convert=odb, the output database (job-name.odb) will be converted using the postprocessing calculator . This conversion is necessary only if the types of output listed in “The postprocessing calculator,” Section 4.3.1, are requested. If convert=state, the separate Abaqus/Explicit state files (job-name.abq.n) will be converted into a single Abaqus/Explicit state file (job-name.abq) if the analysis is run in parallel with parallel=domain. If convert=all, all of the applicable convert options will be executed. recover This option applies only to Abaqus/Explicit. It indicates that an analysis is to be restarted at the last available step and increment in the state file. This capability is available to restart after a catastrophic failure, such as exceeding a CPU limit or a disk quota ( see “Restarting an analysis,” Section 9.1.1). If the original analysis was run in parallel with parallel=domain, it must be restarted with parallel=domain and the same number of processors. syntaxcheck This option indicates that the run is for checking the syntax of the input file only. This option does not use any license tokens. No analysis will be performed, and the continue option cannot be used to continue with an analysis. Only the data (.dat) and output database (.odb) files are generated for viewing. In an Abaqus/Explicit analysis, the model data in the output database may not be complete. information This option writes information about the installation and the environment that is in effect to the screen or to the file job-name.log. For output information for each value of this option, see “Obtaining information,” Section 3.2.1. If the information option is used in conjunction with the analysis option, the job must be run in the background to write the information text to the log file. Additional options available for the analysis module input This option is used to specify the input file name, which may be given with or without the .inp extension (if the extension is not supplied, Abaqus will append it automatically). If this option is not supplied, the procedure will look for an input file called job-name.inp in the current directory. If job-name.inp cannot be found, the procedure will prompt for the input file name. user This option specifies the name of a source or object file that contains any user subroutines to be used in the analysis. The name of the user routine may contain a path name and may be given with or without a file extension. Abaqus/Standard and Abaqus/Explicit only accept user subroutines written in FORTRAN. Abaqus/CFD accepts user subroutines written in C or C++. If an extension is given, the program will take the appropriate action based on the file type. If the file name has no extension, the program will search for a FORTRAN, C, or C++ source file depending on the analysis type. If the source file does not exist, an object file will be searched for instead. The execution procedure creates a shared library using the user subroutine file that is used by the analysis during execution. If the same user subroutine will be needed often, consider setting the usub_lib_dir environment file parameter and using the abaqus make execution procedure to create a shared library containing the user subroutine. This will avoid the need to recompile and/or relink the user subroutine each time it is needed. The user option is not required if the user subroutine called by the analysis is contained in the user library. User libraries contained in the directory given by the usub_lib_dir environment file parameter will not be used if the user option is specified. The user option cannot be used to specify an object file when the double option is used to run an Abaqus/Explicit analysis because Abaqus/Explicit double precision runs need both single precision and double precision objects. In this case you must set the usub_lib_dir environment file parameter and place the single and double precision object files in the specified directory; alternatively, you can supply the user subroutine source. oldjob This option specifies the name of the files from a previous run from which a restart or postprocessing (Abaqus/Standard only; see “Recovering additional results output from restart data in Abaqus/Standard” in “Output,” Section 4.1.1) run is to be started or from which results are to be imported. A path or file extension is not allowed. This option is required when a restart, postprocessing, symmetric model generation, or import analysis reads data from the restart or the results file. The oldjob-name must be different from the current job-name. fil This option specifies whether the data from the old results file specified in a restart run are included at the beginning of the new results file (default). If fil=new is used, the new results file will contain only the data from the point in the analysis where the restart occurred. This feature is used for Abaqus/Standard runs to join the output from restarted analyses into a single, continuous results file. Non-restart jobs cannot use this feature to append results file output to an old results file; the abaqus append execution procedure must be used for this purpose. Setting fil=new is not allowed for Abaqus/Explicit runs. This option is not applicable for Abaqus/CFD. globalmodel This option specifies the name of the global model’s results file or output database file from which the results are to be interpolated to drive a submodel analysis. This option is required whenever a submodel analysis or submodel boundary condition reads data from the global model’s results. The file extension is optional. If both a results file and an output database file exist for the global model and no extension is given, the results file will be used. This option is not applicable for Abaqus/CFD. cpus This option specifies the number of processors to use during an analysis run if parallel processing is available. The default value for this parameter is 1 and can be changed in the environment file . parallel This option specifies the method to use for thread-based parallel processing in Abaqus/Explicit. The possible values are domain and loop. If parallel=domain, the domain-level method is used to break the model into geometric domains. If parallel=loop, the loop-level method is used to parallelize low- level loops. See “Parallel execution in Abaqus/Explicit,” Section 3.5.3, for more information on these methods. The default value is domain, which can be changed in the environment file . domains This option specifies the number of parallel domains in Abaqus/Explicit. If the value is greater than 1, the domain decomposition will be performed regardless of the values of the parallel and cpus options. However, if parallel=domain, the value of cpus must be evenly divisible into the value of domains. The default value is set equal to the number of processors used during the analysis run if parallel=domain and 1 if parallel=loop. The default value can be changed in the environment file (see“Using the Abaqus environment settings,” Section 3.3.1). A restart analysis uses the same number of parallel domains as the original analysis, and the value specified with this option will be ignored. dynamic_load_balancing For domain-parallel execution in Abaqus/Explicit (parallel=domain) where the number of domains is larger than the number of cpus, this option activates the dynamic load balancing scheme. Abaqus/Explicit will attempt to improve computational efficiency by periodically reassigning domains to processors in a way that minimizes load imbalance . mp_mode If this option is set equal to mpi, the MPI-based parallelization method will be used when applicable. Set mp_mode=threads to use the thread-based parallelization method. The default value is mpi on Windows platforms if MPI components are installed; otherwise, thread-based parallel execution is the default behavior. On all other platforms, the default value is mpi. The default setting can be changed in the environment file . For Abaqus/CFD only mp_mode=mpi can be used. standard_parallel This option specifies the parallel execution mode in Abaqus/Standard. The possible values are all If standard_parallel=all, both the element operations and the solver will run in and solver. If standard_parallel=solver, only the solver will run in parallel. The default value is parallel. standard_parallel=all on platforms where MPI-based parallelization is supported. The parallel execution mode can also be set in the environment file . gpus This option specifies acceleration of the Abaqus/Standard direct solver. This option is meaningful only on computers equipped with appropriate GPGPU hardware. By default, GPGPU solver acceleration is not activated. The value of this parameter is the number of GPGPUs to use in an Abaqus/Standard analysis. GPGPU-based solver acceleration can also be set in the environment file . memory Maximum amount of memory or maximum percentage of the physical memory that can be allocated during the input file preprocessing and during the Abaqus/Standard analysis phase . The default values can be changed in the environment file . This option is not applicable for Abaqus/CFD. interactive This option will cause the job to run interactively. For Abaqus/Standard and Abaqus/CFD the log file will be output to the screen; for Abaqus/Explicit the status file and the log file will be output to the screen. The default run_mode can be set in the environment file . background This option will submit the job to run in the background, which is the default. Log file output will be saved in the file job-name.log in the current directory. The default method for submitting the job can be set in the environment file by using the run_mode parameter . queue This option will submit the job to a batch queue. If the option appears with no value, the job will be submitted to the system default queue. Quoted strings are allowed. The available queues are site specific. Contact your site administrator to find out more about local queuing capabilities. Use information=local to see what local queuing capabilities have been installed. The default method for submitting the job can be set in the environment file by using the run_mode parameter . after This option is used in conjunction with the queue option to specify the time at which the job will start in the selected batch queue. This capability is supported for each individual site through the Abaqus environment file. double This option is used to specify that the double precision executable is to be used for Abaqus/Explicit. The possible values are both, constraint, explicit, and off. This capability is also supported through the Abaqus environment file with the environment variable double_precision . If double=both, both the Abaqus/Explicit packager and analysis will run in double precision. If double=constraint, the constraint packaging and constraint solver in Abaqus/Explicit will run in double precision, while the Abaqus/Explicit packager and Abaqus/Explicit analysis continue to run in single precision. If double=explicit, the Abaqus/Explicit analysis will run in double precision, while the packager will still run in single precision. The default value is explicit. If double=off, the environment file setting is overridden if necessary to invoke both the Abaqus/Explicit packager and Abaqus/Explicit analysis in single precision. For a discussion of when to use the double precision executable, see “Defining an analysis,” Section 6.1.2. scratch This option is used to specify the name of the directory used for scratch files. On UNIX platforms the default value is the value of the $TMPDIR environment variable or /tmp if $TMPDIR is not defined. On Windows platforms the default value is the value of the %TEMP% environment variable or \TEMP if this variable is not defined. During the analysis a subdirectory will be created under this directory to hold the analysis scratch files. The default value for this parameter can be set in the environment file . output_precision This option specifies the precision of the nodal field output written to the output database file (job-name.odb). Using output_precision=full results in double precision field output for Abaqus/Standard analyses. To obtain double precision field output for Abaqus/Explicit analyses, use the double option in addition to using output_precision=full. Nodal history output is available only in single precision. This option cannot be used with the recover option. field This option specifies the format of field output for Abaqus/CFD. If field=odb, field output is written to the output database file. If field=exodus, the field output is written to files in EXODUS-II format, one file per processor. To obtain a single file for parallel execution, use field=nemesis; the file is written in EXODUS-II format using the NEMESIS library. The default value is odb. For more information, see “Alternate output formats in Abaqus/CFD” in “Output,” Section 4.1.1. history This option specifies the format of history output for Abaqus/CFD. If history=odb, history output is written to the output database file. If history=csv, history output is written to a file in comma- separated values format. The default value depends on the setting for the field option. When field=odb, the default is history=odb. When field=exodus or nemesis, the default is history=csv. For more information, see “Alternate output formats in Abaqus/CFD” in “Output,” Section 4.1.1. madymo This option is used to specify the MADYMO input file name for a co-simulation analysis that couples Abaqus/Explicit and MADYMO. The MADYMO input file name must be given with the .saf extension. For more information, see the Abaqus User’s Guide for Crash Safety Simulation Using Abaqus/Explicit and MADYMO. port host This option is used to specify the TCP/UDP port number for co-simulation between solvers using the direct coupling interface, which includes co-simulation between Abaqus and certain third-party analysis programs. Set port equal to the port number used for the connection. The default value is 48000. The default port number that Abaqus uses to initiate communication can be set with the cosimulation_port parameter in the environment file . This option is used in conjunction with the host option. For more information, see “Selecting TCP/UDP port numbers” in “Execution procedure for Abaqus: overview,” Section 3.1.1. This option is used to specify the host name for co-simulation between solvers using the direct coupling interface, which includes co-simulation between Abaqus and certain third-party analysis programs. This option specifies the name of the machine that is hosting the connection. Refer to the third-party program documentation to determine if the host option is required. This option is used in conjunction with the port option. listenerport This option is used to specify the TCP/UDP port number for co-simulation between Abaqus solvers and between Abaqus and certain third-party analysis programs using the SIMULIA Co-Simulation Engine. Set listenerport equal to the port number used for the connection. Refer to the third-party program documentation to determine if the listenerport option is required. This option is used in conjunction with the remoteconnections option. For more information, see “Selecting TCP/UDP port numbers” in “Execution procedure for Abaqus: overview,” Section 3.1.1. remoteconnections for co-simulation between This option is used to specify the remote socket connections Abaqus solvers and between Abaqus and certain third-party analysis programs using the SIMULIA Co-Simulation Engine. The remote connections list consists of a pair of entries; the first entry identifies the host name and the listener TCP/UDP port number for the SIMULIA Co-Simulation Engine controller, and the second entry identifies the host name and the listener TCP/UDP port number for the remote job. The host name and port number for the controller must be the first entry. Each entry is separated by a comma, and the host (machine) name and port number within an entry are separated by a colon (e.g., enter discovery:20000,atlantis:30000 for an analysis where the co-simulation controller is running on machine “discovery” using a listener port of “20000” and the remote job is running on machine “atlantis” using a listener port of “30000”). Refer to the third-party program documentation to determine if the remoteconnections option is required. This option is used in conjunction with the listenerport option. For more information, see “Selecting TCP/UDP port numbers” in “Execution procedure for Abaqus: overview,” Section 3.1.1. timeout This option is used to specify a timeout value in seconds for the co-simulation connection using the direct coupling interface or the SIMULIA Co-Simulation Engine. Abaqus terminates if it does not receive any communication from the coupled analysis program during the time specified. The default value is 3600 seconds. The default timeout value that Abaqus uses can be set with the cosimulation_timeout parameter in the environment file . Additional option available for the datacheck module unconnected_regions This option is used to request that Abaqus/Standard create element and node sets for unconnected regions in the analysis output database. Set unconnected_regions=yes to create element and node sets that are named MESH COMPONENT N, where N is the component number. Examples The following examples illustrate the different functions and capabilities of the abaqus execution procedure. Running analyses in Abaqus/Standard Use the following command to run a heat transfer analysis called “c8” in the background: abaqus analysis job=c8 background The following command will run the job c8 in the background and output the current environment settings to the log file: abaqus analysis job=c8 information=environment background The follow-up analysis to the heat transfer analysis c8 is “c10,” which is a static analysis that uses temperature data from c8 as input. The temperature data are read in from the c8 results file as predefined fields. The execution procedure scans the Abaqus/Standard input file for file dependencies of this sort. In this example the procedure will look for the c8 results file in the current directory with the extension .fil. The results file identifier can include a path name , and the execution procedure will then look in the directory specified. In either case an error message will be issued if the file does not exist. The following command is used to run the job c10 in the “long” queue: abaqus analysis job=c10 queue=long This job is next restarted as “c11,” using the final results from c10 as the starting point for a creep analysis. The following command is used to run this job in the default queue: abaqus analysis job=c11 oldjob=c10 queue= The following command is used to run an Abaqus/Standard analysis called “draw_imp” that imports the results from a previously run Abaqus/Explicit analysis called “draw_exp”: abaqus analysis job=draw_imp oldjob=draw_exp Running analyses in Abaqus/Explicit Use the following command to submit an Abaqus/Explicit analysis called “beam” to the default queue: abaqus analysis job=beam convert=all queue= Equivalent results would be obtained from the following series of commands: abaqus datacheck job=beam interactive abaqus continue job=beam queue= abaqus convert=all job=beam interactive Note that the CPU-intensive analysis option is run in batch, while the other options are run interactively. Running analyses in Abaqus/CFD Use the following command to submit an Abaqus/CFD analysis called “cylinder” using 128 cores in parallel: abaqus analysis job=cylinder cpus=128 Running different phases of an analysis Use the following command to perform a parameter check run on an input file called “parmodel”: abaqus job=parmodel parametercheck Use the following command to perform a data check run on an input file called “parmodel” (the parameter check is done again if this job is run after the previous one): abaqus job=parmodel datacheck The following command will continue the previous datacheck job to execute the analysis: abaqus job=parmodel continue Running an Abaqus/Standard to Abaqus/Explicit, Abaqus/Standard to Abaqus/CFD, or Abaqus/Explicit to Abaqus/CFD co-simulation This example illustrates submitting the co-simulation analyses (“Job1” and “Job2”) separately, which also involves invoking the SIMULIA Co-Simulation Engine (CSE) controller, as described in “SIMULIA Co-Simulation Engine controller execution,” Section 3.2.3. You can submit these jobs using the co-simulation procedure, where the port assignments described below, as well as the launching of the CSE controller, are performed automatically . Use the following command for the first Abaqus analysis, running on “einstein”, to initiate listening communication via port 55555 and to connect to the SIMULIA Co-Simulation Engine listening on port 66666 on machine “godel” and to the other Abaqus analysis listening on port 77777 on machine “feynman”: abaqus job=Job1 listenerport=55555 remoteconnections=godel:66666,feynman:77777 Use the following command for the second Abaqus analysis, running on machine “feynman”, to initiate listening communication via port 77777 and to connect to the SIMULIA Co-Simulation Engine listening on port 66666 on machine “godel” and to the other Abaqus analysis listening on port 66666 on machine “einstein”: abaqus job=Job2 listenerport=77777 remoteconnections=godel:66666,einstein:55555 Use the following command for the SIMULIA Co-Simulation Engine, running on machine “godel” and listening on port 66666 to connect to the Abaqus analyses described above: abaqus cse job=csecontrol listenerport=66666 remoteconnections=feynman:77777,einstein:55555 Running a co-simulation using Abaqus/Explicit and MADYMO Use the following command to launch an Abaqus/Explicit analysis called “vehicle” for co-simulation with a MADYMO model called “dummy”: abaqus job=vehicle madymo=dummy.saf 3.2.3 SIMULIA Co-Simulation Engine CONTROLLER EXECUTION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview Co-simulation between Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD is governed by an additional process called the SIMULIA Co-Simulation Engine (CSE) controller. Typically, you are not required to invoke the CSE controller process; it is invoked automatically when you run the Abaqus co-simulation procedure (“Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution,” Section 3.2.4). If you are unable to use the Abaqus co-simulation procedure and are required to submit the co-simulation analyses separately using the Abaqus execution procedure (“Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2), you must invoke the CSE controller as described in this section. Command summary abaqus cse Command line options job job=cosim-job-name listenerport=listener port-number remoteconnections=comma-separated list of remote connection hosts: port-numbers [interactive] [timeout=timeout value in seconds] The value of this option specifies the name of the co-simulation summary log file generated during the run. If this option is omitted from the command line, you will be prompted for its value. listenerport This option is used to specify the TCP/UDP port number for co-simulation inbound messages to the controller. Set listenerport equal to the port number used for the connection. remoteconnections This option is used to specify the remote connections for co-simulation outbound messages between the controller and the participating processes. One entry for each process is required, and the entries are separated by commas. The remote connection entry consists of a host name and the listener TCP/UDP port number separated by a colon (e.g., earth:30000,mars:40000 indicates that one process is running on machine “earth” and using a listener port of “30000”, and another process is running on machine “mars” and using a listener port of “40000”). interactive This option causes the controller to run interactively. timeout This option is used to specify a timeout value in seconds for the co-simulation controller connection. The controller terminates if it does not receive any communication from the coupled analysis program during the time specified. The default value is 3600 seconds. Example The following example illustrates the different functions and capabilities of the co-simulation controller execution procedure when you are required to submit the co-simulation analyses separately. Running an Abaqus/Standard to Abaqus/Explicit co-simulation Use the following command for the first Abaqus analysis, running on machine “earth,” to receive communication via port 55555: abaqus job=explicit listenerport=55555 remoteconnections=mercury:44444,venus:66666 Use the following command for the second Abaqus analysis, running on machine “venus,” to receive communication via port 66666: abaqus job=standard listenerport=66666 remoteconnections=mercury:44444,earth:55555 Use the following command for the co-simulation controller running on machine “mercury,” to receive communication via port 44444: abaqus cse job=cosim listenerport=44444 remoteconnections=venus:66666,earth:55555 Abaqus/Standard, Abaqus/Explicit, AND Abaqus/CFD CO-SIMULATION EXECUTION CO-SIMULATION EXECUTION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview Co-simulation between Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD can be executed by running the Abaqus co-simulation procedure. Several parameters can be set either on the command line or in the environment file . A co-simulation analysis executes two “child” analyses and directs the communication of the two processes. The co-simulation execution procedure allows you to enter a single command to run the co-simulation and should be used whenever possible . If you are unable to use the Abaqus co-simulation procedure, you are required to submit the co-simulation analyses separately using the Abaqus execution procedure (“Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2) and to invoke the SIMULIA Co-Simulation Engine (CSE) controller (“SIMULIA Co-Simulation Engine controller execution,” Section 3.2.3). The co-simulation execution procedure supports a subset of the options that are available for the Abaqus execution procedure; these options are included in the command summary below. Allocating CPUs for parallel processing Three methods are available for allocating CPUs to child analysis jobs for parallel processing: specifying the number of CPUs for each job, distributing CPUs between analysis jobs, and distributing CPUs between analysis products. Specifying the number of CPUs for each job The most direct method of allocating CPUs is to specify the number of CPUs to be used for each child analysis. You provide a comma-separated pair of values using the cpus parameter. Distributing CPUs between analysis jobs You can specify the total number of CPUs to be used for your co-simulation analysis and weighting factors that determine the distribution of the CPUs between the two child analyses. This method enables you to specify a CPU count that relates directly to your resource limits and to describe the relative computational needs of the two child analyses. You provide one value for the number of CPUs to allocate for the co-simulation using the cpus parameter, and you define weight factors using the cpuratio parameter. Weight factors are floating point numbers and are considered in a normalized sense. For example, if you wish to specify that the CPU allocation for the first child job is four times that of the second job, you can provide any of the following pairings: cpuratio=4.0,1.0 cpuratio=16,4 cpuratio=0.8,0.2 Distributing CPUs between analysis products You can specify the total number of CPUs to be used for your co-simulation analysis and weighting factors that determine the distribution of the CPUs between the analysis products involved in the co-simulation. This method enables you to specify a CPU count that relates directly to your resource limits and to describe the relative computational needs of the two child analyses based on the analysis product used (Abaqus/Standard, Abaqus/Explicit, or Abaqus/CFD). You provide one value for the number of CPUs to allocate for the co-simulation using the cpus parameter, and you define weight factors in the environment file using the cpus_weight_std, cpus_weight_xpl, and cpus_weight_cfd environment variable parameters . Weight factors are interpreted in a normalized sense. For example, if you wish to specify that the CPU allocation for the Abaqus/CFD analysis is twice that of the Abaqus/Explicit analysis, you define the parameters in the environment file as follows: cpus_weight_xpl=1 cpus_weight_cfd=2 Rounding considerations for distributing CPUs In cases where the distribution of the CPUs between analysis jobs or analysis products does not result in whole numbers, Abaqus rounds down the CPU allocation for the first job listed in the job parameter and rounds up the allocation for the second job listed. For example, if 8 CPUs are allocated and the CPU allocation for the Abaqus/CFD analysis is twice that of the Abaqus/Explicit analysis, the distribution between Abaqus/Explicit and Abaqus/CFD is 2/6 if the Abaqus/Explicit job is listed first and is 3/5 if the Abaqus/CFD job is listed first. Specifying options for child analyses Command line options that pertain to the child analyses require you to enter a comma-separated pair of values. The order of entries in the pairing must be consistent for all child analysis options to obtain the desired co-simulation execution behavior. For example, in an Abaqus/Standard to Abaqus/Explicit co-simulation, if you specify the job name for the Abaqus/Standard analysis as the first entry for the job parameter, the first entry for the remainder of the child analysis options will apply to the Abaqus/Standard analysis. If an option is relevant for only one of the child analyses, you can enter a value of NONE for the analysis in which the option is not relevant. In cases where you wish to use the default settings for an option for both child analyses or wish to use environment settings to control the behavior, you need not provide that option in the command line. Limitations The following limitations apply to the co-simulation execution procedure: • Only co-simulation between two analyses is supported. • The analyses can be run only on a single machine or a compute cluster where the head node can be shared by both child analysis jobs. • Co-simulation with third-party applications is not supported with this execution procedure; for information on Abaqus job execution for co-simulation with third-party applications, consult the third-party program documentation. Command summary abaqus cosimulation cosimjob=cosim-job-name job=comma-separated pair of job names [cpus={number-of-cpus | comma-separated pair of number-of-cpus}] [cpuratio=comma-separated pair of weight factors specifying cpu allocation to child analyses] [interactive | background | queue=[queue-name] [after=time] ] [timeout=co-simulation timeout value in seconds] [portpool=colon-separated pair of socket port numbers] [input=comma-separated pair of input-file names] [user=comma-separated pair of {source-file | object-file} names] [globalmodel=comma-separated pair of {results file | output database file} names] [memory=comma-separated pair of memory-sizes] [oldjob=comma-separated pair of oldjob-names] [double=comma-separated pair of double precision executable settings] [scratch=comma-separated pair of scratch-dir names] [output_precision=comma-separated pair of {single | full}] [field=comma-separated pair of field output format settings] [history=comma-separated pair of history output format settings] Command line options Required global option cosimjob This option specifies the name of the co-simulation summary log file generated during the run. If this option is omitted from the command line, you will be prompted for its value. Required option for child analyses job The comma-separated values of this option specify the names of all child analysis files generated during the run. If this option is omitted from the command line, you will be prompted for its value. Parallel processing options cpus This option is used to specify how CPUs are allocated for the co-simulation during parallel processing. The default value for this parameter is 2 and can be changed to a value greater than 2 in the environment file . If this option is set equal to a single value, that value specifies the total number of processors allocated for the co-simulation, which can be distributed between child analyses or between analysis products. The distribution of the CPUs between child analyses is split evenly by default and may be further controlled either by using the cpuratio parameter or by defining the distribution of the CPUs between analysis products by setting the cpus_weight_std, cpus_weight_xpl, and cpus_weight_cfd environment file parameters . If this option is set equal to a comma-separated pair of values, these values specify the number of processors to be used for each child analysis. cpuratio The comma-separated values of this option specify the relative weighting of the distribution of processors allocated to each child analysis. This option is valid only when the cpus option is set to a single value. Additional global options available interactive This option causes the co-simulation job to run interactively. A summary log file will be output to the screen, and the child analysis summary output will be written to their separate log files. background This option submits the co-simulation job to run in the background, which is the default. Log file output is saved for the co-simulation job in the file cosim-job-name.log and in the child analysis files job- name.log in the current directory. queue This option submits the co-simulation job to a batch queue. If the option appears with no value, the job is submitted to the system default queue. Quoted strings are allowed. The available queues are site specific. Contact your site administrator to find out more about local queuing capabilities. after This option is used in conjunction with the queue option to specify the time at which the job will start in the selected batch queue. This capability is supported for each individual site through the Abaqus environment file. timeout This option is used to specify a timeout value in seconds for the co-simulation connection. Abaqus terminates if it does not receive any communication between the child analysis processes during the time specified. The default value is 3600 seconds. The default timeout value that Abaqus uses can be set with the cosimulation_timeout parameter in the environment file . portpool This option is used to specify a colon-separated pair of TCP/UDP port numbers that represent the start and end value of port numbers to be used when establishing connections between the child processes. The default range is 51000:52000. The default range that Abaqus uses can be set with the portpool parameter in the environment file . Additional options for child analyses input The comma-separated values of this option specify the child analysis input file names, which may be given with or without the .inp extension (if the extension is not supplied, Abaqus appends it automatically). For each child analysis, if this option is not supplied, the procedure looks for an input file called job-name.inp in the current directory. If job-name.inp cannot be found, the procedure prompts for the input file name. user The comma-separated values of this option specify the names of FORTRAN source or object files that contain any user subroutines to be used in the analysis. The names of the user routines may contain a path name and may be given with or without a file extension. This option is not applicable for Abaqus/CFD. globalmodel The comma-separated values of this option specify the names of the global model’s results (.fil) file or output database (.odb) file from which the results are to be interpolated to drive a submodel analysis. This option is required whenever a submodel analysis or submodel boundary condition reads data from the global model’s results. The file extension is optional. If both a results file and an output database file exist for the global model and no extension is given, the results file is used. This option is not applicable for Abaqus/CFD. memory The comma-separated values of this option specify the maximum amount of memory or maximum percentage of the physical memory that can be allocated during the input file preprocessing and during the Abaqus/Standard analysis phase . This option is not applicable for Abaqus/CFD. oldjob The comma-separated values of this option specify the names of the files from a previous run from which a restart run is to be started or from which results are to be imported. A path or file extension is not allowed. This option is required when a restart or import analysis reads data from the restart file. The oldjob-names must be different from the current job-names. double This option is applicable only for an Abaqus/Explicit analysis. The comma-separated values of this option specify the double precision executable settings to be used; the value for the Abaqus/Standard or Abaqus/CFD analysis is always NONE. The possible values for the Abaqus/Explicit analysis are both, constraint, explicit, and off. This capability is also supported through the Abaqus environment file with the environment variable double_precision . If the double option is omitted for an Abaqus/Standard to Abaqus/Explicit co-simulation, the Abaqus/Explicit packager and analysis will be run in double precision. If the double option is omitted for an Abaqus/CFD to Abaqus/Explicit co-simulation, the Abaqus/Explicit packager and analysis will be run in single precision. If double=both, both the Abaqus/Explicit packager and analysis will run in double precision. If double=constraint, the constraint packaging and constraint solver in Abaqus/Explicit will run in double precision, while the Abaqus/Explicit packager and Abaqus/Explicit analysis continue to run in single precision. If double=explicit or the double option is specified without a value, the Abaqus/Explicit analysis will run in double precision, while the packager will still run in single precision. If double=off, the environment file setting is overridden if necessary to invoke both the Abaqus/Explicit packager and Abaqus/Explicit analysis in single precision. For a discussion of when to use the double precision executable, see “Defining an analysis,” Section 6.1.2. scratch The comma-separated values of this option specify the names of the directories used for scratch files. On UNIX platforms the default value is the value of the $TMPDIR environment variable or /tmp if $TMPDIR is not defined. On Windows platforms the default value is the value of the %TEMP% environment variable or \TEMP if this variable is not defined. During the analysis a subdirectory will be created under this directory to hold the analysis scratch files. output_precision The comma-separated values of this option specify the precision of the nodal field output written to the output database files (job-name.odb). Using output_precision=full results in double precision field output for Abaqus/Standard analyses. To obtain double precision field output for Abaqus/Explicit analyses, use the double option in addition to using output_precision=full. Nodal history output is available only in single precision. This option is not applicable for Abaqus/CFD. field This option is applicable only for an Abaqus/CFD analysis. The comma-separated values of this option specify the format of the field output; the value for the Abaqus/Standard or Abaqus/Explicit analysis is always NONE. The possible values for the Abaqus/CFD analysis are odb, exodus, and nemesis. If field=odb, field output is written to the output database file. If field=exodus, the field output is written to files in EXODUS-II format, one file per processor. To obtain a single file for parallel execution, use field=nemesis; the file is written in EXODUS-II format using the NEMESIS library. The default value is odb. For more information, see “Alternate output formats in Abaqus/CFD” in “Output,” Section 4.1.1. history This option is applicable only for an Abaqus/CFD analysis. The comma-separated values of this option specify the format of the history output; the value for the Abaqus/Standard or Abaqus/Explicit analysis is always NONE. The possible values for the Abaqus/CFD analysis are odb and csv. If history=odb, history output is written to the output database file. If history=csv, history output is written to a file in comma-separated values format. The default value depends on the setting for the field option. When field=odb, the default is history=odb. When field=exodus or nemesis, the default is history=csv. For more information, see “Alternate output formats in Abaqus/CFD” in “Output,” Section 4.1.1. Examples The following examples illustrate the different functions and capabilities of the abaqus cosimulation execution procedure. Running an Abaqus/Standard to Abaqus/CFD co-simulation interactively Use the following command to run a co-simulation between a heat transfer analysis called “solid_heat” and a fluids analysis called “fluid”, interactively: abaqus cosimulation cosimjob=cosim_cht job=solid_heat,fluid interactive Allocating CPUs in an Abaqus/Explicit to Abaqus/CFD co-simulation Use the following command to run a co-simulation between an Abaqus/Explicit analysis called “beam” and an Abaqus/CFD analysis called “fluid” and to allocate 8 cores to the Abaqus/Explicit job and 16 cores to the Abaqus/CFD job: abaqus cosimulation cosimjob=beam_fluid job=beam,fluid cpus=8,16 Equivalent results would be obtained using the following command: abaqus cosimulation cosimjob=beam_fluid job=beam,fluid cpus=24 cpuratio=1,2 Alternatively, you can specify settings for co-simulation environment variable parameters in the environment file and run the co-simulation execution procedure. Use the following combination of environment file settings: ask_delete=OFF # The following parameters set the CPU # allocation by analysis product cpus_weight_xpl=1 cpus_weight_std=1 cpus_weight_cfd=2 Use the following command: abaqus cosimulation cosimjob=beam_fluid job=beam,fluid cpus=24 Submitting an Abaqus/Standard to Abaqus/Explicit co-simulation to a batch queue Use the following command to submit a co-simulation for an Abaqus/Explicit analysis called “beam” and an Abaqus/Standard analysis called “beam2” to a batch queue named “long” and to allocate 8 cores to the Abaqus/Explicit analysis and 4 cores to the Abaqus/Standard analysis: abaqus cosimulation cosimjob=beam job=beam,beam2 cpus=8,4 queue=long 3.2.5 Abaqus/CAE EXECUTION Product: Abaqus/CAE Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview Abaqus/CAE, an interactive environment for creating, submitting, monitoring, and evaluating results from Abaqus simulations, is executed by running the Abaqus execution procedure and specifying the cae parameter. Command summary abaqus cae Command line options database [database=database-file] [replay=replay-file] [recover=journal-file] [startup=startup-file] [script=script-file] [noGUI=[noGUI-file] ] [noenvstartup] [noSavedOptions] [noSavedGuiOptions] [noStartupDialog] [custom=script-file] [guiTester=[GUI-script] ] [guiRecord] [guiNoRecord] This option specifies the name of the model database file or output database file to open. To specify a model database file, include either the .cae file extension or no file extension in the file name. To specify an output database file, include the .odb file extension in the file name. replay This option specifies the name of the file from which Abaqus/CAE commands are to be replayed. The commands in replay-file will execute immediately upon startup of Abaqus/CAE. If no file extension is given, the default extension is .rpy. You cannot use the replay option to execute a script with control flow statements. recover This option specifies the name of the file from which a model database is to be rebuilt. The commands in journal-file will execute immediately upon startup of Abaqus/CAE. If no file extension is given, the default extension is .jnl. startup This option specifies the name of the file containing Python configuration commands to be run at application startup. Commands in this file are run after any configuration commands that have been set in the environment file. Abaqus/CAE does not echo the commands to the replay file when they are executed. script This option specifies the name of the file containing Python configuration commands to be run at application startup. Commands in this file are run after any configuration commands that have been set in the environment file. Arguments can be passed into the file by entering -- on the command line, followed by the arguments separated by one or more spaces. These arguments will be ignored by the Abaqus/CAE execution procedure, but they will be accessible within the script. noGUI This option specifies that Abaqus/CAE is to be run without the graphical user interface (GUI). If no file name is specified, an Abaqus/CAE license is checked out and the Python interpreter is initialized to allow interactive entry of Python or Abaqus Scripting Interface commands. If a file name is specified, Abaqus/CAE runs the commands in the file and exits upon their If no file extension is given, the default extension is .py. This option is useful for completion. automating pre- or post-analysis processing tasks without the added expense of running a display. Since no interface is provided, the scripts cannot include any user interaction. If you use the noGUI option, Abaqus/CAE ignores any other command line options that you provide. Arguments can be passed into the file by entering -- on the command line, followed by the arguments separated by one or more spaces. These arguments will be ignored by the Abaqus/CAE execution procedure, but they will be accessible within the Python script. If you are using the noGUI option, you can use an argument to pass in a variable that would otherwise be provided by a command line option. For example, you can pass in the name of a file that would otherwise be specified by the script option. noenvstartup This option specifies that all configuration commands in the environment files should not be run at application startup. This option can be used in conjunction with the script command to suppress all configuration commands except those in the script file. noSavedOptions This option specifies that Abaqus/CAE should not apply the display options settings stored in abaqus_v6.12.gpr (for example, the render style and the display of datum planes). For more information, see “Saving your display options settings,” Section 76.16 of the Abaqus/CAE User’s Manual. noSavedGuiOptions This option specifies stored in abaqus_v6.12.gpr (for example, the size and location of the Abaqus/CAE main window or its dialog boxes). that Abaqus/CAE should not apply the GUI settings noStartupDialog This option specifies that the Start Session dialog box for Abaqus/CAE should not be displayed. custom This option specifies the name of the file containing Abaqus GUI Toolkit commands. This option executes an application that is a customized version of Abaqus/CAE. For more information, see Chapter 1, “Introduction,” of the Abaqus GUI Toolkit User’s Manual. guiTester This option starts a separate user interface containing the Abaqus Python development environment along with Abaqus/CAE. The Abaqus Python development environment allows you to create, edit, step through, and debug Python scripts. For more information, see Part III, “The Abaqus Python development environment,” of the Abaqus Scripting User’s Manual. You can specify a script as the argument for this option, which prompts Abaqus/CAE to run a GUI script. Abaqus/CAE closes when the end of the script is reached. guiRecord This option enables you to record your actions in the Abaqus/CAE user interface in a file named abaqus.guiLog. You can also set this option at startup by using the environment variable ABQ_CAE_GUIRECORD. The guiRecord option cannot be used with the guiTester option. guiNoRecord This option enables you to disable user ABQ_CAE_GUIRECORD is set. Examples interface recording when the environment variable The following examples illustrate the command line options of the cae execution procedure and how arguments are passed to Abaqus/CAE. Opening a model database The following command will execute Abaqus/CAE and load the model database file called “beam”: abaqus cae database=beam Passing arguments to a script The following command will run the Python script in a file named “try.py” at application startup and pass “argument1” to the script: abaqus cae script=try.py -- argument1 The above command will print argument1 if “try.py” is defined as import sys print sys.argv[-1] Running Abaqus/CAE without the graphical user interface The following command will run the Python script in a file named “checkPartValidity.py” and pass arguments to the script specifying the model database, the model, and the part. The script is executed by Abaqus/CAE; however, the graphical user interface is never displayed. abaqus cae noGui=checkPartValidity.py -- test.cae Model-1 Part-1 The above command will print Part-1 is valid if “checkPartValidity.py” is defined as import sys import os myMdb= sys.argv[-3] myModel = sys.argv[-2] myPart = sys.argv[-1] mdb = openMdb(myMdb) model = mdb.models[myModel] part = model.parts[myPart] if part.geometryValidity: sys.__stderr__.write('%s is valid\n' % myPart) else: sys.__stderr__.write('%s is invalid\n' % myPart) 3.2.5 Abaqus/CAE EXECUTION This Abaqus functionality is not applicable to V6. 3.2.6 Abaqus/Viewer EXECUTION Product: Abaqus/Viewer Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview Abaqus/Viewer, a subset of Abaqus/CAE that contains only the postprocessing capabilities of the Visualization module, is executed by running the Abaqus execution procedure and specifying the viewer parameter. Command summary abaqus viewer Command line options database [replay=replay-file] [database=database-file] [script=script-file] [noGUI=[noGUI-file] ] [noenvstartup] [noSavedOptions] [noSavedGuiOptions] [noStartupDialog] [custom=script-file] [guiTester=[GUI-script] ] [guiRecord] [guiNoRecord] [startup=startup-file] This option specifies the name of the output database file to use if it is different from job-name. The procedure searches for database-file as entered on the command line with the .odb file extension. replay This option specifies the name of the file from which Abaqus/Viewer commands are read. The commands in replay-file will execute immediately upon startup of Abaqus/Viewer. If no file extension is given, the default extension is .rpy. You cannot use the replay option to execute a script with control flow statements. startup This option specifies the name of the file containing the Python configuration commands to be run at application startup. Commands in this file are run after any configuration commands that have been set in the environment file. Abaqus/Viewer does not echo the commands to the replay file when they are executed. script This option specifies the name of the file containing Python configuration commands to be run at application startup. Commands in this file are run after any configuration commands that have been set in the environment file. noGUI This option specifies that Abaqus/Viewer is to be run without the graphical user interface (GUI). If no file name is specified, an Abaqus/Viewer license is checked out and the Python interpreter is initialized to allow interactive entry of Python or Abaqus Scripting Interface commands. If a file name is specified, Abaqus/Viewer runs the commands in the file and exits upon their If no file extension is given, the default extension is .py. This option is useful for completion. automating post-analysis processing tasks without the added expense of running a display. Since no interface is provided, the scripts cannot include any user interaction. noenvstartup This option specifies that all configuration commands in the environment files should not be run at application startup. This option can be used in conjunction with the script command to suppress all configuration commands except those in the script file. noSavedOptions This option specifies that Abaqus/Viewer should not apply the display options settings stored in abaqus_v6.12.gpr (for example, the render style and the display of boundary conditions). For more information, see “Saving your display options settings,” Section 76.16 of the Abaqus/CAE User’s Manual. noSavedGuiOptions stored in This option specifies abaqus_v6.12.gpr (for example, the size and location of the Abaqus/CAE main window or its dialog boxes). should not apply the GUI that Abaqus/Viewer settings noStartupDialog This option specifies that the Start Session dialog box for Abaqus/Viewer should not be displayed. custom This option specifies the name of the file containing Abaqus GUI Toolkit commands. This option executes an application that is a customized version of Abaqus/Viewer. For more information, see Chapter 1, “Introduction,” of the Abaqus GUI Toolkit User’s Manual. guiTester This option starts a separate user interface containing the Python development environment along with Abaqus/Viewer. The Python development environment allows you to create, edit, step through, and debug Python scripts. For more information, see Part III, “The Abaqus Python development environment,” of the Abaqus Scripting User’s Manual. You can specify a script as the argument for this option, which prompts Abaqus/Viewer to run a GUI script. Abaqus/Viewer closes when the end of the script is reached. guiRecord This option enables you to record your actions in the Abaqus/Viewer user interface in a file named abaqus.guiLog. You can also set this option at startup by using the environment variable ABQ_CAE_GUIRECORD. The guiRecord option cannot be used with the guiTester option. guiNoRecord This option enables you to disable user ABQ_CAE_GUIRECORD is set. interface recording when the environment variable 3.2.6 Abaqus/Viewer EXECUTION This Abaqus functionality is not applicable to V6. 3.2.7 Python EXECUTION Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The Python language is used throughout Abaqus: in the Abaqus Scripting Interface, in the Abaqus environment file (abaqus_v6.env), and to perform parametric studies. The abaqus python facility is used to access the Python interpreter. Command summary abaqus python [script-file] Command line option script-file The Python interpreter executes the instructions in the specified script-file. If this option is omitted from the command line, the Python interpreter is started in interactive mode. 3.2.8 PARAMETRIC STUDIES Products: Abaqus/Standard Abaqus/Explicit References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2 Overview The abaqus script facility indicates that a parametric study is to be done . Each analysis involved in the design can be executed using the execute command . You can add any necessary Abaqus execution options (refer to “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2) to the execution command for each of the analyses by specifying them on the execOptions option of the execute command. If the script file contains references to other input files, these files must be located in the same directory as the script file. The files created by the execution of the script file are placed in the directory from which the Abaqus execution procedure is run. Command summary abaqus script Command line options script-file [=script-file] [startup=startup file-name ] [noenvstartup] When a script file name is specified, the parametric study module is imported and the instructions in the parametric study script file are executed. If the script file name is omitted from the command line, the Python interpreter is initialized by importing the parametric study module. startup This option specifies the name of the file containing Python configuration commands to be run at application startup. Commands in this file are run after any configuration commands that have been set in the environment file. noenvstartup This option specifies that all configuration commands in the environment files should not be run at application startup. This option can be used in conjunction with the startup command to suppress all configuration commands except those in the startup file. Examples Use the following command to execute the Python script in a file named “parstudy.psf”: abaqus script=parstudy The following command will initiate a Python scripting session: abaqus script In a Python scripting session the following command will execute the Python script in a file named “scriptfile”: script("scriptfile") 3.2.9 Abaqus DOCUMENTATION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Getting help,” Section 2.6 of the Abaqus/CAE User’s Manual Overview Abaqus documentation is installed separately from the product and is viewed through a web browser or PDF reader. See Chapter 2, “Installing Abaqus,” of the Abaqus Installation and Licensing Guide, for information on installing the Abaqus documentation. The documentation consists of the following books: • Abaqus Analysis User’s Manual • Abaqus/CAE User’s Manual • Abaqus Keywords Reference Manual • Abaqus Theory Manual • Abaqus User Subroutines Reference Manual • Abaqus Glossary • Abaqus Example Problems Manual • Abaqus Benchmarks Manual • Abaqus Verification Manual • Abaqus Release Notes • Abaqus Installation and Licensing Guide • Getting Started with Abaqus: Interactive Edition • Getting Started with Abaqus: Keywords Edition • Abaqus Scripting User’s Manual • Abaqus Scripting Reference Manual • Abaqus GUI Toolkit User’s Manual • Abaqus GUI Toolkit Reference Manual • Abaqus Interface for MSC.ADAMS User’s Manual • Abaqus Interface for Moldflow User’s Manual • Using Abaqus Online Documentation Using Abaqus documentation To view the documentation: 1. Type abaqus doc. The documentation collection page (index.html or index.pdf file) opens in either a web browser or Adobe Acrobat Reader, depending on which formats of documentation were installed and configured by your system administrator. See “Information to enter during product installation,” Section 2.4.2 of the Abaqus Installation and Licensing Guide, and “Configuration of documentation application” below. The documentation collection page lists the book titles grouped by category. 2. Click the title of a book to display it. In the HTML documentation, each book opens in a new browser window or tab. The book window contains four HTML frames: the navigation frame (top frame), the expand/collapse frame (upper left frame), the table of contents frame (lower left frame), and the text frame (right frame). 3. Navigate and search the book’s content. • In the HTML documentation, use any of the following methods: – Use the buttons in the expand/collapse frame to vary the level of detail displayed in the table of contents frame. – Use the back and forward arrows in the text frame to navigate sequentially through the text. You can also use the web browser functions to return to recently viewed pages. – Expand the topic headings in the table of contents by clicking the book icon to the left of the heading. To jump directly to a section whose title is displayed in the table of contents, click that title. – Use the search panel located in the navigation frame to search for specific words or phrases. • In the PDF documentation, use the standard controls in Adobe Acrobat Reader to navigate and search the books. For more detailed information on viewing and searching the HTML or PDF documentation, refer to Using Abaqus Online Documentation. Configuration of documentation application The abaqus doc command locates a web browser executable or the Adobe Acrobat Reader executable depending on which documentation format was installed and configured by your system administrator. Configuration of web browser If the HTML documentation was installed and configured by your system administrator, the abaqus doc command will locate a web browser executable as follows: • Windows platforms: The abaqus doc command uses your default web browser. • UNIX and Linux platforms: The abaqus doc command searches the system path for Firefox. If the help system cannot find Firefox, an error is displayed. The browser_type and browser_path variables can be set in the Abaqus environment file to modify the behavior of this command. For more information, see “System customization parameters,” Section 4.1.4 of the Abaqus Installation and Licensing Guide. Configuration of PDF reader executable If the PDF documentation was installed and configured by your system administrator, the abaqus doc command will locate the Adobe Acrobat Reader executable as follows: • Windows platforms: The abaqus doc command uses the default installed Acrobat Reader. • UNIX and Linux platforms: The abaqus doc command searches the system path for the acroread executable. You can also set the doc_resource variable (in the Abaqus environment file) to the path of the acroread executable. For more information, see “System customization parameters,” Section 4.1.4 of the Abaqus Installation and Licensing Guide. Command summary abaqus doc 3.2.10 LICENSING UTILITIES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The abaqus licensing utilities provide management and monitoring tools for both types of Abaqus licensing: FLEXnet and Dassault Systèmes licensing. Executing the abaqus licensing command without additional arguments displays a command usage summary of all available utilities. For a detailed description of all of the FLEXnet Licensing utilities, refer to the FLEXnet Licensing End User Guide Version 11.6.1. You can download this document from the Licensing section of the Support page at www.simulia.com. Several of the most useful licensing utilities are listed in the command summary below. For more information, see Chapter 3, “Abaqus licensing,” of the Abaqus Installation and Licensing Guide. Command summary abaqus licensing [lmstat | lmdiag | lmpath | lmtools | dslsstat] Command line options lmstat This option displays information about the location and features served by the FLEXnet Licensing servers used to serve the Abaqus license. Additional arguments may be used with this command to generate more license usage information. lmdiag This option displays information relating to the various FLEXnet Licensing features and indicates whether or not the feature may be checked out. lmpath This option can be used to control where Abaqus looks for licenses. Additional arguments are used to print, set, or add license location information. Running the command without arguments will display the command summary for each action. lmtools This option starts the FLEXnet Licensing toolchest on Windows platforms. This application can be used to invoke most FLEXnet Licensing administration tool functions. dslsstat This option displays information about the location and features served by the Dassault Systèmes license server (DSLS). See “Using the dslsstat utility for the Dassault Systèmes license server,” Section 3.9 of the Abaqus Installation and Licensing Guide, for more information. 3.2.11 ASCII TRANSLATION OF RESULTS (.FIL) FILES Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The abaqus ascfil translation facility: • is provided to convert results (.fil) files (produced by an Abaqus analysis) to ASCII format for porting between dissimilar operating systems; • permits the movement of results data to a different system for postprocessing; and • can also be used to convert a results file in ASCII format to binary format to save disk space. Command summary abaqus ascfil Command line options job job=job-name [input=input-file] This option specifies the input and output file names to use during results file translation. The job-name value is used as the default input file name. The translated output file will have the name job-name.fin. If the input file is in binary format (default), this utility will create the job-name.fin file in ASCII format. To transfer the results file back to binary format after porting to a dissimilar operating system, rename the job-name.fin file to job-name.fil, and use this utility again; the resulting job-name.fin file will be in binary format. If this option is omitted from the command line, you will be prompted for this value. input This option specifies the name of the input file if it is different from job-name. Example To convert the results file c4.fil from binary to ASCII format, use the following command: abaqus ascfil job=c4 The translated file will have the name c4.fin. 3.2.12 JOINING RESULTS (.FIL) FILES Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The abaqus append postprocessing facility: • is provided to join results (.fil) files into a single file; • permits two results files that may be either ASCII or binary files, or a combination of ASCII and binary, to be joined for further postprocessing; and • will write a results file in the same format as the file specified with the oldjob option. A similar utility, abaqus restartjoin, is used to join output database (.odb) files. See “Joining output database (.odb) files from restarted analyses,” Section 3.2.18, for details. Command summary abaqus append Command line options job job=job-name oldjob=oldjob-name input=input-file This option specifies the output file name to use during execution. The job-name value is used as the output file name. The joined output file will have the name job-name.fil. If this option is omitted from the command line, you will be prompted for this value. oldjob This option specifies the name of the first results file to use during execution. The oldjob-name value is used as the results file name. If this option is omitted from the command line, you will be prompted for this value. input This option specifies the name of the second results file to use during execution. The input-file results file will be appended to the oldjob-name results file. If this option is omitted from the command line, you will be prompted for this value. Example The following command will append the history contents of the fjoin003.fil results file to the end of the fjoin002.fil results file and create the file fjoin001.fil: abaqus append job=fjoin001 oldjob=fjoin002 input=fjoin003 3.2.13 QUERYING THE KEYWORD/PROBLEM DATABASE Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The abaqus findkeyword utility queries a keyword/problem database that contains information on Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD example problems, verification problems, problems used in training seminars, problems shown in the Abaqus technology briefs, benchmark timing problems, and those in the tutorial book Getting Started with Abaqus: Keywords Edition. You specify which keywords, parameters, and values are of interest; and this utility will list the input files that contain those keywords, parameters, and values. You can specify multiple keywords, which causes the findkeyword utility to list those input files that contain all of the specified keywords. You can then use the abaqus fetch utility to fetch the input files . The output is grouped into problem sets; e.g., Abaqus Example Problems or Abaqus/Standard Technology Brief Problems. Command summary abaqus findkeyword keyword data lines Command line options job [job=job-name] [maximum=maximum-output] This option is used to specify the output file name for the output listing. If this option is omitted from the command line, the output will be printed to the standard output device. maximum This option is used to limit the number of sample problems that are listed for each set. If this option is omitted, a maximum of 100 sample problems are listed for each set. keyword data lines The keyword data lines specify which Abaqus keywords, parameters, and values are of interest to the user. The names of sample problems that contain the specified keywords, parameters, and values are printed to the standard output device or to the file indicated by the job command line parameter. The keyword is required, but parameters and values are optional. If a keyword is specified without a parameter or a value, all sample problems that use that keyword (with or without parameters and values) will be listed. If a parameter is specified without a value, all sample problems that use that parameter with any value will be listed. Parameter values that are user-specified data (e.g., numeric data, set names, orientation names, etc.) are ignored. The end of the keyword data lines is indicated by an empty line or an end of file. Examples The following examples illustrate the different types of search criteria utilized by the findkeyword execution procedure. Querying for keywords and parameters To list the sample problems that use the *RESTART option with the WRITE parameter, type the following command and data lines: abaqus findkeyword *RESTART,WRITE To generate a list of sample problems that contain two keyword lines in the same file, both keywords are included as data lines. For example, abaqus findkeyword *RESTART,WRITE *NGEN To list all sample problems that use a keyword and parameter with a value, the value must be included on the data line. For example, abaqus findkeyword job=beam *BEAM SECTION,SECTION=ARBITRARY The output is written to the file beam.dat. Querying for user-specified parameter values User-specified parameter values (e.g., numeric data, set names, orientation names, etc.) are ignored. The following two examples are equivalent because the value MYSET is an element set name. abaqus findkeyword *ELSET,ELSET=MYSET abaqus findkeyword *ELSET,ELSET 3.2.14 FETCHING SAMPLE INPUT FILES Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The abaqus fetch utility is used to extract sample Abaqus input files, user subroutine files, journal files, parametric study script files, or postprocessing programs from the compressed archive files provided with the release (for problems in the Abaqus Example Problems Manual, the Abaqus Benchmarks Manual, and the Abaqus Verification Manual). File names are specified in the manuals. If no file extension is specified, all files corresponding to the name given will be extracted. Wildcard expressions can be used when specifying the file names and include the following: • An asterisk (*) matches a sequence of zero or more characters. • A question mark (?) matches exactly one character. • A bracketed item [...] matches any single character found inside the brackets; ranges are specified by a beginning character, a hyphen, and an ending character. If an exclamation point (!) or a caret (^) follow the left bracket, the range of characters within the brackets is complemented; that is, anything except the characters inside the brackets is considered a match. Any character that might otherwise be interpreted or modified by the operating system, particularly on UNIX platforms, should be placed inside quotation marks. If no matches are found using the wildcard expressions, the abaqus fetch utility attempts to extract a file with the name specified. Command summary abaqus fetch Command line options job job=job-name [input=input-file] This option is used to specify the output file name for the fetched input file or files. It is also the default name of the input file to fetch. If this option is omitted from the command line, you will be prompted for this value. input This option is used to specify the name of the input file or files to fetch if it is different from the job-name. Examples To fetch the example input file c2.inp from the archive files, use the following command: abaqus fetch job=c2.inp To fetch all files associated with job c8 from the archive files, do not specify a file extension. The following command will extract both the input file (c8.inp) and the user subroutine file (c8.f): abaqus fetch job=c8 To fetch the sample parametric study scripting file parstudy.psf from the archive files, use the following command: abaqus fetch job=parstudy.psf 3.2.15 MAKING USER-DEFINED EXECUTABLES AND SUBROUTINES Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The abaqus make utility is used to create user postprocessing executables and user-defined libraries of Abaqus user subroutines. The commands used to compile and link a user-supplied program or user subroutine source file can be changed using the appropriate Abaqus environment file parameters; i.e., compile_cpp, compile_fortran, link_exe, and link_sl. You can skip the compilation step by providing a precompiled object as input for postprocessing programs. Postprocessing executables created using this procedure must be run using the Abaqus execution procedure. This is necessary to set the operating system environment variables for finding the Abaqus utility libraries. To run a user postprocessing program, use the following command: abaqus job-name User subroutine shared libraries created using this procedure are used by specifying the usub_lib_dir variable in the Abaqus environment file. The advantage of doing this is that an analysis using user subroutines can execute without having to compile or link the user subroutine. Command summary abaqus make Command line options job {job=job-name | library=source-file} [user={source-file | object-file}] [directory=library-dir] [object_type={fortran | c | cpp}] This option is used to create a user-supplied postprocessing program. The value of the option specifies the name of the executable created by this procedure. It is also used as the default source file name. If no option is given on the command line, you will be prompted for this value. library This option is used to create user subroutine object files and shared libraries. The value of the option specifies the name of the user subroutine source file to be compiled and linked. The resulting object and shared library files are placed in the directory given by the command line directory option. If the directory option is not used, the files are placed in the current working directory. The object file or files created have a suffix indicating if the user subroutine is for Abaqus/Standard or Abaqus/Explicit. The Abaqus/Standard object file suffix is —std. Abaqus/Explicit has single and double precision object files; the object file suffixes are —xpl and —xplD. The Abaqus/Standard user subroutine shared library that is created is called standardU, and the Abaqus/Explicit shared libraries are called explicitU and explicitU-D. If the directory option is used and it contains object files with the appropriate suffix for the shared library that is being created, those files are linked to the shared library. user This option is valid only when used in conjunction with the job option. It is used to specify the name of the source or object file containing your program if it is different from job-name. If a file extension is not provided, the option value with a FORTRAN source file extension is sought. If a file by this name is not found, the option value with an object file extension is sought. directory This option is valid only when used in conjunction with the library option. It is used to specify the destination of the user subroutine object and shared library files that will be created by the procedure. It is also used to specify the location of additional object files that are to be linked to the shared library or libraries being created. If the option is omitted, the files created by the procedure are placed in the current working directory. object_type This option is valid only when used in conjunction with the job option. It is used to specify the type of object file, either FORTRAN, C, or C++, given by the job or user option. Example To create an executable called “pprocess” given a FORTRAN source file of the same name, use the following command: abaqus make job=pprocess This program can then be run using the command abaqus pprocess INPUT FILE AND OUTPUT DATABASE UPGRADE UTILITY UPGRADE UTILITY Products: Abaqus/Standard Abaqus/Explicit References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Fixed format conversion utility,” Section 3.2.23 Overview The abaqus upgrade utility will convert an input file or output database file from earlier releases of Abaqus to the current release. Input files based on the syntax of Abaqus 5.8 or later can be upgraded; output database files from Abaqus 6.1 or later can be upgraded. The abaqus upgrade utility will generate a log file (job-name.log) that contains error, warning, diagnostic, and informational messages. You should carefully review the conversion log file to ensure that changes made to the older release input file or output database file are appropriate. If no conversions are necessary, a message will be issued to the log file as well as to the screen. Abaqus does not allow the use of dots (".") in set, surface, or rebar names in an input file except as delimiters between a part instance name and a set, surface, or rebar name. The abaqus upgrade utility will change dots to underscores ("_") for dots not used as delimiters. Manual conversion of dots to underscores will improve performance for very large input or include files. The abaqus upgrade utility expects input files to be in free format; you can use the abaqus free utility to convert fixed format data to free format. See “Fixed format conversion utility,” Section 3.2.23. job=job-name [input=old-input-file-name | odb=old-odb-file-name] [fromversion=release] [previousdefaults] Command summary abaqus upgrade Command line options Required option job This option is used to specify the name of the upgraded input file or output database file to be output by the utility. Mutually exclusive options input This option is used to specify the name of the input file to be upgraded. odb This option is used to specify the name of the output database file to be upgraded. Additional options fromversion This option is relevant for input file upgrades only. By default, the upgrade utility converts the input file from Abaqus 6.11 to the current release. This option is used to upgrade an input file from an earlier release. For the release number, specify the general release number (two numbers separated by a period, such as 6.8). previousdefaults This option is relevant for input file upgrades only. This option is used to minimize modeling differences between the old input file and the upgraded input file. 3.2.17 GENERATING OUTPUT DATABASE REPORTS Products: Abaqus/Standard Abaqus/Explicit References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Object model for the output database,” Section 10.5 of the Abaqus Scripting User’s Manual Overview The output database report utility prints information from an Abaqus output database (.odb) file to a formatted report. By default, the report is printed in plain text format; however, you can also create reports in HTML and CSV (comma-separated values) formats. Output database structure Every output database consists of two main sections: model data and results data. The database is further broken down into a hierarchical structure of containers, as indicated in Figure 3.2.17–1. odb mesh sets Model Data steps frames fieldOutputs historyRegions invariants components orientation historyOutputs Results Data Figure 3.2.17–1 Structure of an output database The data that can appear in a report reside in the containers at the far right of each branch. These containers can be used to classify the four main branches of the output database: • The mesh branch terminates in a container holding nodal coordinates and element connectivity information for the model. • The sets branch terminates in a container holding the names and node or element labels of the sets and surfaces in the model. • The fieldOutputs branch terminates in a container holding the values of field output variables from the analysis. These values are further broken down into their vector or tensor attributes: invariants, components, and orientation. • The historyOutputs branch terminates in a container holding the values of history output variables from the analysis. The containers in the model data section of the tree are singular containers: each model has one container for mesh information and one container for sets information. The containers in the results section of the tree, however, represent aggregates of multiple containers. For a multistep analysis, the output database will have a separate step container for each step of the analysis. Within each step container will be multiple frames and historyRegions containers. Within each individual frames container will be multiple fieldOutputs containers, and so on. The output database assigns names or values to these individual containers to help distinguish and identify them. For a more detailed discussion of the output database structure, see “Object model for the output database,” Section 10.5 of the Abaqus Scripting User’s Manual. Generating summary reports If you generate a report using only the required and file formatting command line options, the report will be a brief summary of the output database. This summary contains a listing of the following information: • Part instance names • Number of nodes and elements in the model • Names of sets and surfaces • Names of steps and load cases • Numbers of frames in the steps • Names of field and history output variables The information contained in this summary can help you determine the names and values of containers in the output database. Adding information to a report You can create more comprehensive reports using additional command line options. Most of these options correspond to a container in the output database structure outlined in Figure 3.2.17–1. Using these options to specify the name or value of a container instructs the utility to extract the data found in that container and to add it to the generated report. Container names and values are not always unique, and may appear more than once in an output database. For example, a container corresponding to frame 1 will likely appear in every individual step container for a multistep analysis; similarly, a container holding a specific field output variable usually appears inside every frame of the step. The utility will add all instances of these containers to the report. To refine the container selection, you can combine options. When more than one container from the same branch is indicated on the command line, the utility only reports the data that are common to both containers. For example, if two options specify the container for Step 1 and the container for frame 3, the utility will add results data only from the third frame of the first step to the report. If you specify containers from different branches, the data from each container are added to the report. For example, if the two options specify the sets container and a history region container, both sets data and history output data are added to the report. You identify specific containers by setting the associated option equal to the name or value of that container. To include multiple containers of the same type, set the option equal to a comma-separated list. The names are case-sensitive. If the names include spaces, you must enclose the entire value in double quotation marks ("container name"). Additional options The output database report utility offers some additional options for controlling the organization and details of a report. These options will have no effect unless they are invoked in conjunction with other “container” options. Command summary abaqus odbreport Command line options Required options [job=job-name] [odb=output-database-file] [mode={HTML | CSV}] [all] [mesh] [sets] [results] [step={step-name | _LAST_}] [frame={number | load-case-name | description | _LAST_}] [framevalue={time | mode | frequency}] [field=[field-variable] ] [components] [invariants] [orientation] [histregion=region-name] [history=[history-variable] ] [instance={instance-name | _NONE_}] [blocked] [extrema] You must include at least one of the following options when executing abaqus odbreport. They tell the utility where to find the output database and where to print the report. Use both options together to make the report’s file name unique from the output database name. job This option is used to specify the file name of the generated report. If you omit this option, the utility prints the report to the standard output device. odb This option is used to specify the output database (.odb) file from which the report is generated. If you omit this option, the utility looks for an output database called job-name.odb in the current directory. File formatting option mode This option specifies the file format of the generated report. If you omit this option, the report is in plain text format with the file extension .rep. If mode=HTML, the report is in HTML format with the file extension .htm. If mode=CSV, the report is in comma-separated values format with the file extension .csv. Option to generate a full output database report all This option is used to report all available model information and results information from every step in the analysis; data from the base state of each step (frame zero) is not included in the report. The report will be very long for large output databases. Options to report model data The following options extract information from the model data section of the output database. mesh This option is used to report the nodal coordinates and element connectivity associated with the model’s mesh. sets This option is used to report the names and contents of all sets and surfaces associated with the model. Options to report results data The following options extract information from the results data section of the output database. results This option is used to report all field and history output variable values from the output database. If you include any other options corresponding to specific results containers, this option is ignored. step This option is used to report the field and history output variable values for the specified steps. When invoking this option, you must set it equal to at least one step name. If step=_LAST_, the report includes results from only the last step of the analysis. The steps container is common to both the fieldOutputs and historyOutputs branches of the output database. If you combine the step option with a field output variable option, only field output variable data appear in the report. Similarly, if you combine the step option with a history output variable option, only history output variable data appear in the report. If you combine the step option with both field and history output variable options, both types of variable data appear in the report. Options to report field output variables The following options extract information from containers in the fieldOutputs branch of the output database. frame This option is used to report field output variable values for the specified frames. When invoking this option, you must set it equal to at least one frame number, load case name, or frame description. The initial (or “zero increment”) frame can be identified only by setting frame=0. If frame=_LAST_, the report includes results from only the last frame of each included step. framevalue This option is used to report field output variable values for the specified frame values. Each frame can be identified by a frame value that may be unique from the frame number. The frame value is either the time, eigenmode number, or frequency point associated with a frame. This option can be used as an alternative or complement to the frame option. When invoking this option, you must set it equal to at least one frame value. The values you provide do not need to be exact; the utility will find the frame with the closest frame value. field This option is used to report the specified field output variable values. If you invoke this option without setting it equal to any variable names, all field variable containers are included in the report. Options to report different field variable attributes If none of the following options is invoked, the utility automatically reports components and (if applicable) orientations for each field variable. Otherwise, the utility reports only the attributes specified by these options. These options will have an effect only if used in conjunction with other field output variable options. Invariants and orientations are not available for all field variables. components This option is used to report components for all field output variables. invariants This option is used to report invariant values for all field output variables. orientation This option is used to report the local coordinate system for each field output variable. Options to report history output variables The following options extract information from containers in the historyOutputs branch of the output database. histregion This option is used to report history output variable values for the specified history region. When invoking this option, you must set it equal to at least one history region name. history This option is used to report the specified history output variable values. If you invoke this option without setting it equal to any variable names, all history variable containers are included in the report. Additional options The following options add an additional level of control and detail to a report. They are not associated directly with the output database structure and will not add database information to a report. They must be used in conjunction with the previously described options. instance This option is used to limit reported model and results data to a specific part or assembly instance in the model. It is not directly associated with any output database containers and will not add any data to a report. When invoking this option, you must set it equal to at least one instance name. If instance=_NONE_, the report includes data for the whole assembly and model. blocked This option is used to subdivide tables of field output variables into blocks according to part instance, element type, and section point. It is useful if you are interested in separating output from different areas of a large model. By default, the tables are organized according to variable name and frame. This option instructs the report utility to access the output database using the field bulk data API. For details about how the field bulk data API operates, see “Using bulk data access to an output database,” Section 10.10.7 of the Abaqus Scripting User’s Manual. An additional benefit of this option is enhanced performance of the utility when dealing with large volumes of field variables, leading to faster report generation. The option has no effect if there are no field output variables in a report, or when the invariants option is also specified. extrema This option is used to report maximum and minimum values at the end of each table of nodal coordinates and field output variables. By default, these extrema do not appear in a report. The option will have no effect if there are no nodal coordinates or field output variables in a report. Examples The following examples illustrate the capabilities of the odbreport execution procedure and the effects of different option combinations. File naming and formatting The following command generates a brief summary of the output database beam.odb in a plain text file named beam.rep: abaqus odbreport job=beam To create the same report in HTML format and with the name beamreport.htm, execute the following command: abaqus odbreport job=beamreport odb=beam mode=html Adding information to a report Use additional command line options to add data from specified containers to a report. The following command creates a report listing nodal coordinates and element connectivity from the model and all output variable values associated with the step named Apply weight: abaqus odbreport job=beam mesh step="Apply weight" You can refine the results data listed by using combinations of options. In the following example, the utility reports only history output variable values that were output from the history region named Node350 in the Apply weight step: abaqus odbreport job=beam step="Apply weight" histregion=Node350 If a container is identified by a name or value that is not unique, the generated report will include all occurrences of that container. The following command creates a report listing the values for field variable RF that were output in the third frame of every individual step: abaqus odbreport job=beam frame=3 field=RF To report the magnitude of RF instead of its components, use the invariants option: abaqus odbreport job=beam frame=3 field=RF invariants To add multiple containers of the same type to a report, you can set an option equal to a comma-separated list. The following command reports all values of field output variables U and S that were output during the steps Apply weight and Side load: abaqus odbreport job=beam step="Apply weight","Side load" field=U,S Additional options Use the instance option to limit reported information to a particular section of your model. The following command reports set names and nodes, and values of S in the last frame of every step from the database motor.odb. However, only information related to part instance pistonA appears in the report: abaqus odbreport job=motor sets frame=_LAST_ field=S instance=pistonA Selecting frames The frame and framevalue options can accept a wide variety of value types, making them powerful report-building options. Because of this variety, it is sometimes necessary to invoke both options to specify a particular frame. For example, consider the output database plate.odb, the results of a steady-state dynamic analysis. The analysis investigated the response of a plate over a range of 20 different frequencies under three different load cases. The output database, therefore, includes results for the three different load cases at each frequency. You are interested in the response at 45 Hz under the load case named lc2. Setting frame=lc2 will report field variables for load case lc2 at every frequency (a total of 20 frames). Setting framevalue=45 will report field variables for every load case associated with the 45 Hz frequency (a total of three frames). To limit the report to the single frame of interest, you must invoke both options together: abaqus odbreport job=plate frame=lc2 framevalue=45 3.2.18 JOINING OUTPUT DATABASE (.ODB) FILES FROM RESTARTED ANALYSES Products: Abaqus/Standard Abaqus/Explicit References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Continuation of output upon restart” in “Restarting an analysis,” Section 9.1.1 Overview The abaqus restartjoin utility appends an output database (.odb) file produced by a restart analysis of a model to the output database produced by the original analysis of that model. Combining the original and restart output database files into a single file enables you to examine all of the output data for the analysis in Abaqus/CAE. A similar utility, abaqus append, is used to join results (.fil) files. See “Joining results (.fil) files,” Section 3.2.12, for details. Appending data when the analysis restarts between steps versus midstep You can append output database files from analyses that restart between steps and from analyses that restart in the middle of a step. While the required syntax is the same for these two types of analyses, Abaqus appends data differently, as follows: • For an analysis that stops and restarts between steps, Abaqus simply appends the output from the new steps to the output from the existing steps of the original analysis. • For an analysis that stops and restarts in the middle of a step, the original and restart analyses overlap because the restart analysis resumes at the beginning of the interrupted step. In this case the abaqus restartjoin utility retains the results for any completed steps in the original analysis but replaces the results for the interrupted step with the output data produced by the restart analysis. Customizing the combined output database file By default, Abaqus appends the output data produced by the restart analysis directly to the original output database file. If you prefer to retain the original output database file, you can create a copy of it and append the restart analysis output data to the copy instead. Abaqus names this copy using the format Restart_original-odb-filename; for example, a copy of the original output database file job–1.odb would be named Restart_job-1.odb. Abaqus omits history data when you combine original and restart output databases; however, you can override this default. You can also control whether Abaqus compresses the combined output database file. Command summary abaqus restartjoin Command line options originalodb originalodb=odb-file-name restartodb=odb-file-name [copyoriginal] [history] [compressresult] This option specifies the output database file produced by the original analysis. If you omit the copyoriginal option, Abaqus appends the output data from the restart output database file directly to the original output database file. If you omit this option from the command line, Abaqus will prompt you for its value. restartodb This option specifies the output database file produced by the restart analysis. You can specify only one restart analysis output database file at a time. If you omit this option from the command line, Abaqus will prompt you for its value. copyoriginal If this option is specified, Abaqus creates a copy of the output database file specified by the originalodb option and appends the contents of the restartodb output database file to that copy instead of to the original file. When this option is omitted, Abaqus appends the output data from the restart analysis directly to the original output database file. Abaqus names the copied output database file by adding the prefix Restart_ to the name of the original output database file; for example, a copy of the original output database file original.odb would be named Restart_original.odb. history If this option is specified, Abaqus copies history data from the restart output database to the original output database or its copy. Abaqus omits history data in the joined output database file unless you specify this option. compressresult If this option is specified, Abaqus compresses the resulting output database file. Examples If your model produced an initial output database file named Job-1.odb and a restart output database file named Job-1_res.odb, issue the following command to append the contents of the restart database to the initial output database file: abaqus restartjoin originalodb=Job-1.odb restartodb=Job-1_res.odb If you prefer to retain the original output database file, you can create a copy of this original file and append the contents of the restart output database file to the copy instead. Abaqus creates the name of the copied output database file by adding the prefix Restart_ to the name of the original file; in the preceding example the copy of the original file Job-1.odb would be named Restart_Job-1.odb. To perform the restart join operation using a copy of the original file, issue the following command: abaqus restartjoin originalodb=Job-1.odb restartodb=Job-1_res.odb copyoriginal By default, Abaqus does not copy history data to the combined output database. To include history data, issue the following command: abaqus restartjoin originalodb=Job-1.odb restartodb=Job-1_res.odb history 3.2.19 COMBINING OUTPUT FROM SUBSTRUCTURES Products: Abaqus/Standard Abaqus/Explicit References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Obtaining output of results within a substructure” in “Using substructures,” Section 10.1.1 Overview The abaqus substructurecombine utility combines the model and results data produced by two of a model’s substructures into a single output database (.odb) file. By combining all of a model’s substructure analysis output database files, you can display all of the data produced by a substructure analysis in Abaqus/CAE. Abaqus combines output data by adding the contents of the second file you specify (the copy output database) directly into the first file you specify (the base output database). Because this process changes the base output database, consider backing up your data before using this utility. Combining data for models with more than two substructures Because the abaqus substructurecombine utility combines data from only two output databases at a time, you must run the utility multiple times to create a single output database from an analysis with more than two substructures. Combine data from two of the substructures first, then repeat the operation to combine the resulting output database file with data from each remaining substructure. Customizing the combined output database You can customize the substructure combine operation by adding only a subset of the data from the copy output database into the base output database. Abaqus enables you to add output data to the base output database from a single step or frame in the copy output database. You can also include only output data from the copy output database that relates to a particular variable; for example, you can copy output data related to Mises stress. Command summary abaqus substructurecombine baseodb=odb-file-name copyodb=odb-file-name [all] [step=step-name] [frame=frame-number] [variable=variable-key] Command line options baseodb This option specifies the name of the base output database, to which Abaqus adds the contents of the copy output database. If you omit this option from the command line, Abaqus will prompt you for its value. copyodb This option specifies the name of the copy output database, which Abaqus adds to the contents of the base output database. You can specify only one file at a time for this option. If you omit this option from the command line, Abaqus will prompt you for its value. all step This option indicates that data for all variables within all steps and frames of output should be copied to the combined output database. When you specify this option, Abaqus ignores the step, frame, and variable options. This option indicates the name of the step from which Abaqus will copy results data. You can specify only one step; if you omit this option, Abaqus copies data from the last step in the output database. Abaqus ignores this option if you specify the all option. frame This option indicates the number of the frame from which Abaqus will copy results data. You can specify only one frame; if you omit this option, Abaqus uses the last frame in the step specified by the step option. Abaqus ignores this option if you specify the all option. variable This option indicates the variable key for the variable from which Abaqus will copy results data. If you omit this option, Abaqus copies data for all variables in the output database. Abaqus ignores this option if you specify the all option. Only output variable keys that are valid for output database file output are available for use with abaqus substructurecombine. In general, if a key corresponds to a collective output variable, rather than an individual component, it can be used with this execution procedure. The collective output variable keys are distinguished from their individual components by the fact that they have a bullet ( ) in one of the .odb columns in the tables in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Examples The following examples illustrate different methods of combining substructures using the abaqus substructurecombine execution procedure. Combining two substructures If your model contains two substructures that produce output database files named subst1.odb and subst2.odb, issue the following command to overwrite subst1.odb with the combined contents of the two files: abaqus substructureCombine baseodb=subst1.odb copyodb=subst2.odb Combining more than two substructures If your model contains more than two substructures, you must first combine the output database files from two of the substructures, then combine the combined output database with each of the other substructures’ output databases in turn. In this example the substructure analysis produces four output database files named subst1.odb, subst2.odb, subst3.odb and subst4.odb, so you must issue the abaqus substructure command a total of three times to combine all four files into a single output database, as shown in the following example: abaqus substructureCombine baseodb=subst1.odb copyodb=subst2.odb abaqus substructureCombine baseodb=subst1.odb copyodb=subst3.odb abaqus substructureCombine baseodb=subst1.odb copyodb=subst4.odb Combining specific elements of the substructures If you want to include only the output data from the step Step-1 in the combined output database, issue the following command: abaqus substructureCombine baseodb=subst1.odb copyodb=subst2.odb step="Step-1" If you want to include only the output data from the Mises variable in the combined output database, issue the following command: abaqus substructureCombine baseodb=subst1.odb copyodb=subst2.odb variable="Mises" COMBINING DATA FROM MULTIPLE OUTPUT DATABASES COMBINING OUTPUT DATABASES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Joining output database (.odb) files from restarted analyses,” Section 3.2.18 • “Combining data from multiple output databases,” Section 82.13 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The abaqus odbcombine utility combines the results data in two or more Abaqus output database files (.odb) into a single output database (.odb) file. The abaqus odbcombine utility is intended for the combination of output databases containing different results. If you want to combine output databases from the same analysis before and after a restart, use the abaqus restartjoin execution procedure instead. For more information, see “Joining output database (.odb) files from restarted analyses,” Section 3.2.18. Abaqus includes all model data from the selected output databases in the combined output database; however, for results data you can choose to include a subset of the data from the output databases that you specify. Abaqus/CAE determines which results data are included in the combined output database based on two factors: the filtering options you specify and your selection of master output database. Filters You can filter the data that the utility includes in the combined output database to include results only from selected steps or frames, from selected output variables, or from a combination of these options. For example, a filter can enable you to include results data only from the last step and the last frame of the specified output databases, and the same filter can dictate that only Mises stress results are included in the combined output database. You can also establish multiple filters if you want to set up different filtering conditions for the first step than in the second step. The abaqus odbcombine utility also provides two levels of filtering: output database–specific filters, which filter results from only a single output database; and default filters, which apply to the entire job. The output database–specific filters take precedence over the default filters, so Abaqus/CAE employs the settings in the default filters only when the default filter you define does not conflict with filters for one of the individual output databases. The filtering syntax is flexible enough to allow you to specify multiple steps, frame, or output variable values. You can specify multiple step names in a comma-separated list, such as Step-1, Step-2, Step-4. For frames you can include ranges or individual values; for example, entering 1, 3, 5, 7:9 returns frames 1, 3, 5, 7, 8, and 9 to the combined output database. You can also use the symbolic constants ’ALL’, ’FIRST’, and ’LAST’ as shortcuts to specify the data you want to include. These options enable you to include results data from all steps or frames and data from all output variables rather than one or more selected variables. Master output database One output database in every combine operation is designated as the master output database. The utility first transfers all field output data, subject to filtering selections, from the master output database to the combined output database. The utility then locates results data from matching steps and frames in the subsequent output databases and copies only those data into the combined output database. This strategy provides a more coherent structure for the combined results data. Configuration file usage The abaqus odbcombine utility uses data in configuration files to determine which output databases to combine, the file to designate as the master output database, and the filtering options to enforce by default and for each output database. The configuration file must be in .xml format, and it can have three types of elements in the following order: • The element specifies one or more default filtering definitions. This section is optional, but you must include it if you want to set up default filtering for your combine operation. • The element specifies the location of the master output database and, if desired, one or more filtering definitions for the data in that output database. This section is required. • One element is required for each additional output database that you want to include in the combine operation. You can then specify default filters for output database–specific filters by embedding elements within the element or within one of the output database elements. Configuration file template The following example illustrates the structure of the configuration file for the abaqus odbcombine utility. Your XML file declaration may differ from this one. The default filtering element is optional. If you include this element in the configuration file, you must include at least one element within this section. Filter elements can use the Steps or Frames attributes to refer to symbolic constants or the StepName or FrameIndex attributes to refer to individual steps or frames, as shown in the following examples: Filtering elements for the master output database are optional. If you want to filter the data from this output database, include a element within this section for each filtering option you want to define. Filtering elements for the output database are optional. If you want to filter the data from this output database, include a element within this section for each filtering option you want to define. Append an element for each additional output database you want to include. Data not included in combined output databases The following types of output data are not included when you combine output database files: • History output. • Surface data. • Data from analytical rigid part instances. • Local coordinate systems associated with field output data. Command summary abaqus odbcombine Command line options job {job=job-name} [input=configuration-file-name] [verbose=level] This option specifies the name of the resulting combined output database and the name of the log file. Abaqus also searches for a configuration file by this name. If you omit this option from the command line, Abaqus will prompt you for its value. input This option specifies the name of the configuration file that specifies the output databases you want to combine and the steps, frames, and output variables to be included in the combination. The configuration file must be in .xml format. verbose This option specifies the level of detail for the messages that Abaqus writes to the log file. Possible values are 1 or 2. If you specify 1, Abaqus writes only errors and warnings to the log file; if you specify 2, Abaqus also records the filtering options you select and lists the model data and field output data that were successfully copied to the combined output database. 3.2.21 NETWORK OUTPUT DATABASE FILE CONNECTOR Products: Abaqus/CAE Abaqus/Viewer References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Accessing an output database on a remote computer,” Section 9.3 of the Abaqus/CAE User’s Manual Overview A network ODB connector creates a connection to a network ODB server that can be used to access a remote output database. The abaqus networkDBConnector command is used to start the network ODB server. A network ODB connector can be created from any platform—Windows, UNIX, or Linux; however, the network ODB server must reside on a UNIX or Linux platform. Abaqus uses password files to authenticate the connection between the client and the server. The password on the network ODB server must be stored in a file called .abaqus_net_passwd in your home directory on the remote system. You must update this file after 30 days, and the password must be at least 8 characters long. In addition, your home directory on the local client machine can contain either of the following: • A file called .abaqus_hostname_passwd. This file allows you to connect to the remote server on the machine called hostname. • A file called .abaqus_net_passwd. This file allows you to connect to the network ODB server on any machine. The contents of the password file on both the server and the client must be identical. In addition, Abaqus checks that you are the only user with permission to read from or to write to the password files. If neither file exists, Abaqus tries to use remote and secure shell commands to read the password from the network ODB server. However, the security configuration at your site may prevent Abaqus from reading the password. Command summary abaqus networkDBConnector port={serverPortNumber | auto_assigned} [timeout=time out value in seconds] [host=hostname] [stop] [ping] Command line options port This option specifies the port number on the network ODB server. If port=auto_assigned, Abaqus automatically assigns the port number. timeout This option specifies the timeout period in seconds for the network ODB server. The server exits if it does not receive any communication from the client during the time specified. A timeout value of zero indicates that the server will run until it is terminated explicitly using the stop option. host stop ping This option specifies the name of the machine that is hosting the network ODB server. This option is used with the stop and ping options. If this option is not provided, Abaqus uses the name of the machine from which the execution procedure was issued. This option specifies that Abaqus should stop the network ODB server that was established using the specified host name and port number. This option queries the network ODB file server that was established using the specified host name and port number. Use this option to confirm that the network ODB server exists and that communications have been established. 3.2.22 MAPPING THERMAL AND MAGNETIC LOADS Product: Abaqus/Standard References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Eddy current analysis,” Section 6.7.5 • “Predefined loads for sequential coupling,” Section 16.1.3 • *CFLUX • *CLOAD Overview The abaqus emloads utility converts results output from a time-harmonic eddy current analysis for use as loads in a subsequent heat transfer, coupled temperature-displacement, or stress/displacement analysis. For example, magnetic body force intensity output is converted to point loads. You specify the names of the time-harmonic eddy current analysis results output database (.odb) file and the input file for the subsequent analysis on the command line. The utility creates an output database file containing a mesh that matches the mesh in your subsequent analysis and steady-state concentrated nodal fields consistent with the time-harmonic eddy current analysis results. Your time-harmonic eddy current and subsequent analysis meshes can be dissimilar, and results transfer ensures global conservation of the flux quantities when your model domains match; i.e., the model boundaries are the same. You can then use this new output database file to apply concentrated loads and concentrated heat fluxes in the subsequent analysis. Results conversion The utility converts whole element output quantities from a time-harmonic eddy current analysis to nodal results. You use the options listed in Table 3.2.22–1 in the subsequent analysis to specify the output database file (and optionally the step and increment) from which the data are to be read. Utility execution The utility executes in two phases. Abaqus writes progress information and, if appropriate, error messages to the screen during each phase. In the first phase a datacheck analysis is performed on your subsequent analysis input file to create an output database representation of a “target” mesh. This phase requires that your input file be sufficiently complete to successfully run abaqus datacheck, with the exception that you can have *CFLUX and *CLOAD options that include the FILE parameter to refer to files that are not available. If this phase is successful, the utility proceeds to the second phase; otherwise, an error message is issued. In the second phase time-harmonic eddy current analysis load data are mapped from the source to the target output database. In this phase all steps and increments found in the original analysis are defined Electromagnetic analysis output variable Rate of Joule heat dissipation EMJH Magnetic body force intensity EMBF Table 3.2.22–1 Supported results conversion. Converted output variable Input file option Concentrated heat flux CFL11 Point load components CF *CFLUX, FILE=odb-name, STEP=step-number, INC=inc *CLOAD, FILE=odb-name, STEP=step-number, INC=inc in the target output database. This phase requires that your target model domain lie within the source model domain. If it does not, an appropriate error message is issued. Command summary abaqus emloads Command line options job job=target-odb-name input=subsequent analysis input-file-name sourceodb=time-harmonic eddy current analysis odb-file-name This option specifies the name of the resulting “target” output database file. input This option specifies the name of the subsequent analysis Abaqus input file. This file must be sufficiently complete to successfully run, as described above. sourceodb This option specifies the name of the time-harmonic eddy current analysis output database file. 3.2.23 FIXED FORMAT CONVERSION UTILITY Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The abaqus free utility will convert the fixed format input files used with Abaqus 5.8 to the free format input files used with subsequent Abaqus releases. Command summary abaqus free Command line options job job=job-name input=input-file This option is used to specify the name of the free format input file to be output by the utility. input This option is used to specify the name of the fixed format input file to be converted. 3.2.24 TRANSLATING NASTRAN BULK DATA FILES TO Abaqus INPUT FILES Products: Abaqus/Standard Abaqus/Explicit References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Translating Abaqus files to Nastran bulk data files,” Section 3.2.25 • “Importing a model from a Nastran input file,” Section 10.5.4 of the Abaqus/CAE User’s Manual Overview The translator from Nastran to Abaqus converts certain entities in a Nastran input file into their equivalent in Abaqus. Using the translator The Nastran data must be in a file with the extension .bdf, .dat, .nas, .nastran, .blk, or .bulk. The Nastran data entries that are translated are listed in the tables below. Other valid Nastran data are skipped over and noted in the log file. The translator is designed to translate a complete Nastran input file. If only bulk data are present, the first two lines in the file should be the terminators for the executive control and case control sections, namely: CEND BEGIN BULK For normal termination, end the Nastran input data with the line ENDDATA Nastran solution sequences are translated to the Abaqus procedures listed in Table 3.2.24–1. The translator attempts to create a history section based on the contents of the case control data in the Nastran file. Summary of Nastran entities translated Table 3.2.24–1 Executive control data. Nastran Statement Abaqus Equivalent SOL Nastran Statement Abaqus Equivalent (STATICS1) *STATIC 24 (STATICS) 101 (SESTATIC) 106 (NLSTATIC) (MODES) *FREQUENCY 25 (OLDMODES) 103 (SEMODES) (BUCKLING) *BUCKLE 105 (SEBUCKL) 26 (DFREQ) *STEADY STATE DYNAMICS, DIRECT 108 (SEDFREQ) 27 (DTRAN) *DYNAMIC 109 (SEDTRAN) 107 (SEDCEIG) *COMPLEX FREQUENCY 110 (SEMCEIG) 30 (DFREQ) 111 (SEMFREQ) *FREQUENCY and *STEADY STATE DYNAMICS 31 (MTRAN) *FREQUENCY and *MODAL DYNAMIC 112 (SEMTRAN) Table 3.2.24–2 Case control data. Nastran Command Comment SPC LOAD METHOD SUBCASE Selects SPC sets alone or in combinations Selects individual loads and load combinations Selects EIGRL, EIGR, or EIGB from bulk data for eigenfrequency extraction and eigenvalue buckling prediction procedures Delimiter for steps or load cases; optional if there is only one step Nastran Command Comment TITLE SUBTITLE LABEL DLOAD LOADSET FREQUENCY MPC Echoed as comment at top of input file and for each step Echoed as comment for the step to which it applies Used as text following the *STEP option Selects dynamic loads from bulk data Selects forcing frequencies from bulk data Selects MPCADD and MPC from bulk data if referenced in the first SUBCASE SUPORT1 Selects SUPORT1 from bulk data Selects TSTEP from bulk data Selects DMIG from bulk data using the matrix name from the first SUBCASE TSTEP K2GG K2PP M2GG M2PP B2GG B2PP K42GG TEMPERATURE Selects nodal temperatures from bulk data SET Selects nodal quantities for output DISPLACEMENT VELOCITY ACCELERATION SPCFORCES PRESSURE Table 3.2.24–3 Bulk data. Nastran Data Entry Comment PARAM CDAMP1 CDAMP2 PDAMP PDAMPT CELAS1 CELAS2 PELAS PELAST CMASS2 CBUSH PBUSH PBUSHT CWELD PWELD CONM1 CONM2 Ignored except for: 1. WTMASS, which can be used to modify density, mass, and rotary inertia values if the wtmass_fixup command line parameter is used 2. INREL, which if equal to −1 or −2 will create inertia relief loads 3. G, which is translated to *GLOBAL DAMPING, STRUCTURAL, FIELD=MECHANICAL 4. GFL, which is translated to *GLOBAL DAMPING, STRUCTURAL, FIELD=ACOUSTIC DASHPOT1/DASHPOT2 and *DASHPOT SPRING1/SPRING2 and *SPRING (CELAS2 at SPOINTs are translated to *MATRIX INPUT, stiffness, and/or structural damping terms.) *MATRIX INPUT mass terms CONN3D2 and *CONNECTOR SECTION *FASTENER and *FASTENER PROPERTY MASS and/or ROTARY INERTIA and/or UEL MASS and/or ROTARY INERTIA Nastran Data Entry Comment CHEXA CPENTA CTETRA PSOLID PLSOLID CQUAD4 CTRIA3 CQUAD8 CTRIA6 CQUADR CTRIAR PSHELL PCOMP PCOMPG CSHEAR PSHEAR CBAR CBEAM PBAR PBARL PBEAM PBEAML CROD CONROD PROD CGAP PGAP RBAR C3D8I/C3D20R/C3D6/C3D15/C3D4/C3D10 and *SOLID SECTION S4/S3R/S8R/STRI65, and *SHELL SECTION, *SHELL GENERAL SECTION, or *MEMBRANE SECTION. M3D4 and *MEMBRANE SECTION; T3D2 and *SOLID SECTION B31 and *BEAM SECTION or *BEAM GENERAL SECTION T3D2 and *SOLID SECTION GAPUNI and *GAP *COUPLING or *MPC, type BEAM Nastran Data Entry Comment MAT1 MAT2 MAT8 MAT9 MAT10 ACMODL NSM NSM1 NSML NSML1 NSMADD GRID *ELASTIC, TYPE=ISO; *EXPANSION, TYPE=ISO; *DENSITY; and *DAMPING (G is used only for *BEAM GENERAL SECTION) When used alone in a PSHELL, MAT2 is translated to *ELASTIC, TYPE=LAMINA or *ELASTIC, TYPE=ANISOTROPIC. When used in combination with other materials, the coefficients relating midsurface strains and curvatures to section forces and moments are computed and entered following the *SHELL GENERAL SECTION option. *ELASTIC, TYPE=LAMINA; *EXPANSION, TYPE=ORTHO; *DENSITY; and *DAMPING *ELASTIC, TYPE=ANISOTROPIC unless the data are found to be orthotropic, in which case the data are analyzed to create *ELASTIC, TYPE=ENGINEERING CONSTANTS. Also *DENSITY; *EXPANSION, TYPE=ANISO or ORTHO; and *DAMPING. *ACOUSTIC MEDIUM and *DENSITY *TIE between a *SURFACE, TYPE=ELEMENT defining the exterior surfaces of all acoustic solid elements and a *SURFACE, TYPE=NODE defined by the SET1 referenced by the SSID. *NONSTRUCTURAL MASS *NODE and *SYSTEM Nastran Data Entry Comment *SYSTEM for nodes; *TRANSFORM if referred to on GRID; *ORIENTATION for some elements *COUPLING and *KINEMATIC; or *KINEMATIC COUPLING (If the RBE2 has only two nodes and neither node has rotational stiffness, the RBE2 is translated to *MPC, type LINK) *COUPLING and *DISTRIBUTING; or DCOUP3D and *DISTRIBUTING COUPLING Used to combine SPC/SPC1/SPCD data into a new set *BOUNDARY Used to combine FORCE, MOMENT, etc. data into a new set *CLOAD *DLOAD 3.2.24–7 CORD1R CORD1C CORD1S CORD2R CORD2C CORD2S RBE2 RBE3 SPCADD SPC SPC1 SPCD LOAD FORCE FORCE1 FORCE2 MOMENT MOMENT1 MOMENT2 PLOAD PLOAD1 PLOAD2 PLOAD4 Nastran Data Entry Comment DLOAD DAREA LSEQ RLOAD1 RLOAD2 TLOAD1 TABLED1 TABLED2 TABLED4 DELAY DPHASE TEMP TEMPD TSTEP EIGB EIGR EIGRL EIGC TABDMP1 FREQ FREQ1 FREQ2 FREQ3 FREQ4 FREQ5 MPCADD MPC Dynamic loads as functions of time or frequency *INITIAL CONDITIONS, TYPE=TEMPERATURE and *TEMPERATURE Time step size for dynamic and modal dynamic procedures *BUCKLE *FREQUENCY *COMPLEX FREQUENCY *MODAL DAMPING Forcing frequencies for steady-state dynamic procedures *EQUATION Nastran Data Entry Comment SUPORT SUPORT1 DMIG GENEL *INERTIA RELIEF and *BOUNDARY *MATRIX INPUT and *MATRIX ASSEMBLE *USER ELEMENT, LINEAR and *MATRIX, TYPE=STIFFNESS PLOTEL Ignored unless the command line option plotel=ON. Command summary abaqus fromnastran Command line options job job=job-name [input=input-file] [wtmass_fixup={OFF | ON}] [loadcases={OFF | ON}] [pbar_zero_reset=[small-real-number] ] [distribution={OFF | preservePID | ON}] [surface_based_coupling={OFF | ON}] [beam_offset_coupling={OFF | ON}] [beam_orientation_vector={OFF | ON}] [cbar=2-node-beam-element] [cquad4=4-node-shell-element] [chexa=8-node-brick-element] [ctetra=10-node-tetrahedron-element] [plotel={OFF | ON}] [cdh_weld={OFF | RIGID | COMPLIANT}] This option is used to specify the name of the Abaqus input file to be output by the translator. It is also the default name of the file containing the Nastran data. Diagnostics created by the translator will be written to a file named job-name.log. input This option is used to specify the name of the file containing the Nastran data if it is different from job-name. wtmass_fixup If wtmass_fixup=ON, the value on the Nastran data line PARAM, WTMASS, value is used as a multiplier for all density, mass, and rotary inertia values created in the Abaqus input file. This option can be defined in the Abaqus environment file as follows: fromnastran_wtmass_fixup={OFF | ON} loadcases By default, each SUBCASE is translated to a *STEP option in Abaqus. If loadcases=ON, this behavior is altered for linear static analyses: each SUBCASE is translated to a *LOAD CASE option, and all such *LOAD CASE options are grouped in a single *STEP option. This option can be defined in the Abaqus environment file as follows: fromnastran_loadcases={OFF | ON} pbar_zero_reset Nastran allows beams to have zero values for cross-sectional area or moments of inertia; Abaqus does not. Set this option equal to a small real number to reset any zero values for A, , or J to the specified small real number. If this option is omitted or present without a value, the default value of 1.0 × 10−20 is used in place of the zeros. To retain the zeros in the translated Abaqus input file, set pbar_zero_reset=0. , This option can be defined in the Abaqus environment file as follows: fromnastran_pbar_zero_reset=small-real-number distribution This option determines how shell and membrane sections in Nastran data are translated to Abaqus. If distribution=OFF, a separate section is created for each combination of orientation, material offset, and/or thickness. If distribution=preservePID or ON, element orientations and offsets are written If distribution=preservePID, an Abaqus section is created using the *DISTRIBUTION option. corresponding to each PSHELL or PCOMP property ID. If distribution=ON, a single Abaqus section is created for all homogeneous elements referencing the same material. This option can be defined in the Abaqus environment file as follows: fromnastran_distribution={OFF | preservePID | ON} surface_based_coupling rigid If Certain Nastran one elements surface_based_coupling=ON, RBE2 and RBE3 elements to *COUPLING with the appropriate parameters. Otherwise, RBE2 elements translate to *KINEMATIC COUPLING and RBE3 elements translate to *DISTRIBUTING COUPLING. This translation behavior also applies to “implied” RBE2-type rigid elements used for offsets on CBAR, CBEAM, and CONM2 elements. equivalent translate in Abaqus. have more than For input files created with surface_based_coupling=ON, the translated elements can be visualized and manipulated in Abaqus/CAE. However, large numbers of these elements may cause slower performance. This option can be defined in the Abaqus environment file as follows: fromnastran_surface_based_coupling={OFF | ON} beam_offset_coupling If beam_offset_coupling=ON, beam element offsets are translated by creating new nodes at the offset locations, changing the beam connectivity to the new nodes, and rigidly coupling the new and original nodes. If beam_offset_coupling=OFF, beam element offsets are translated to the *CENTROID and *SHEAR CENTER options, which are suboptions of the *BEAM GENERAL SECTION option. The setting for this parameter is ignored if the beam element references a PBARL or PBEAML property or if the beam offset has a significant component in the direction of the beam axis. In these situations the beam offsets are always translated as if beam_offset_coupling=ON. This option can be defined in the Abaqus environment file as follows: fromnastran_beam_offset_coupling={OFF | ON} beam_orientation_vector If beam_orientation_vector=OFF, beam cross-section orientations are translated by creating new nodes at the tips of vectors defining the first principal direction of the cross-section and changing the beam connectivity to the new nodes. If beam_orientation_vector=ON, beam cross-sections are translated by defining vectors on the *BEAM SECTION and *BEAM GENERAL SECTION options. This option can be defined in the Abaqus environment file as follows: fromnastran_beam_orientation_vector={OFF | ON} cbar This option is used to define the 2-node beam that is created from CBAR and CBEAM elements. The default is B31. This option can be defined in the Abaqus environment file as follows: fromnastran_cbar=2-node-beam-element cquad4 This option is used to define the 4-node shell that is created from CQUAD4 elements. The default is S4R. If a reduced-integration element is chosen, the enhanced hourglass formulation is applied automatically. This option can be defined in the Abaqus environment file as follows: fromnastran_cquad4=4-node-shell-element chexa This option is used to define the 8-node brick that is created from CHEXA elements. The default is C3D8I. If a reduced-integration element is chosen, the enhanced hourglass formulation is applied automatically. This option can be defined in the Abaqus environment file as follows: fromnastran_chexa=8-node-brick-element ctetra This option is used to define the 10-node tetrahedron that is created from CTETRA elements. The default is C3D10. This option can be defined in the Abaqus environment file as follows: fromnastran_ctetra=10-node-tetrahedron-element plotel By default, PLOTEL elements are not translated. If plotel=ON, PLOTEL elements are translated to T3D2 truss elements in an element set named PLOTEL_TRUSSES. The cross-sectional area of the trusses is the value entered for pbar_zero_reset, and the material has a Young’s modulus, E, equal to 1.0. cdh_weld By default, CHEXA elements with RBE3 elements at all eight corner nodes are translated to the type of 8-node element specified in the chexa parameter. If cdh_weld=RIGID, CHEXA elements with RBE3 elements at all eight corner nodes are translated to rigid fasteners in Abaqus. If cdh_weld=COMPLIANT, CHEXA elements with RBE3 elements at all eight corner nodes are translated to compliant fasteners in Abaqus. 3.2.25 TRANSLATING Abaqus FILES TO NASTRAN BULK DATA FILES Products: Abaqus/Standard Abaqus/Explicit References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Translating Nastran bulk data files to Abaqus input files,” Section 3.2.24 Overview The translator from Abaqus to Nastran converts certain entities in an Abaqus file into equivalent entities in Nastran. Only “flat” Abaqus files can be translated; i.e., the Abaqus file cannot contain parts and assemblies. Using the translator The Abaqus input data must be in a file with the extension .inp or .sim. If you specify an .inp file, the execution procedure translates selected keywords and creates a Nastran bulk data file with the extension .bdf. If you use the substructure option and specify a .sim file, the execution procedure translates the substructure data and creates a Nastran bulk data file with the extension .bdf. Summary of Abaqus keywords translated In the *ELEMENT usages listed below, an italicized x indicates that all Abaqus elements beginning with the preceding label will be mapped to the Nastran entity shown. For example, the statement *ELEMENT, C3D4x indicates that the selected Abaqus-to-Nastran translation applies to the Abaqus elements C3D4, C3D4H, and C3D4T. Table 3.2.25–1 Abaqus keyword–to–Nastran mapping. Abaqus Keyword Nastran Complement *BEAM GENERAL SECTION, SECTION=GENERAL *BOUNDARY *CLOAD *COUPLING, DISTRIBUTING *COUPLING, KINEMATIC *ELEMENT, B31 PBAR SPC FORCE RBE3 RBE2 CBAR (for *BEAM GENERAL SECTION, SECTION=GENERAL) Abaqus Keyword *ELEMENT, B33 Nastran Complement CBAR (for *BEAM GENERAL SECTION, SECTION=GENERAL) CQUAD4 CQUAD8 CTETRA CTETRA CPENTA CPENTA CHEXA CHEXA CONM2 CONM2 CTRIA3 *ELEMENT, C3D4x *ELEMENT, C3D10x *ELEMENT, C3D6x *ELEMENT, C3D15x *ELEMENT, C3D8x *ELEMENT, C3D20x *ELEMENT, MASS *ELEMENT, ROTARYI *ELEMENT, S3x *ELEMENT, S4x *ELEMENT, S8x *ELEMENT, SPRING1 or SPRING2 *ELEMENT, SPRINGA *ELEMENT, STRI65 *ELEMENT, T3D2 *FREQUENCY *HEADING *MATERIAL, DENSITY *MATERIAL, ELASTIC, TYPE=ISO *MATERIAL, ELASTIC, TYPE=LAMINA *MATERIAL, EXPANSION, TYPE=ISO *MATERIAL, EXPANSION, TYPE=ORTHO MAT8 *NODE GRID *ORIENTATION, DEFINITION=COORDINATES MAT1 MAT1 MAT8 MAT1 CELAS CROD CTRIA6 CROD SOL 103 TITLE CORD2R, CORD2C, or CORD2S Abaqus Keyword Nastran Complement *SHELL GENERAL SECTION (Non-composite) *SHELL SECTION (Non-composite) *SHELL SECTION (Composite) *SHELL GENERAL SECTION (Composite) *SOLID SECTION *SOLID SECTION (Trusses) *STATIC *SYSTEM *TRANSFORM PSHELL PCOMP PSOLID PROD SOL 101 CORD2R, CORD2C, or CORD2S Command summary abaqus tonastran job=job-name [input=input-file] [substructure] Command line options job This option is used to specify the name of the Nastran bulk data file to be output by the translator. It is also the default name of the Abaqus file. Diagnostics created by the translator are written to a file named job-name.log. input This option is used to specify the name of the file containing the Abaqus data if it is different from job-name. substructure This option is used to translate a substructure within an Abaqus .sim file into Nastran bulk data file (.bdf) format. 3.2.26 TRANSLATING ANSYS INPUT FILES TO Abaqus INPUT FILES Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The translator from ANSYS to Abaqus converts certain entities in an ANSYS blocked coded database file into their equivalent in an Abaqus input file. Using the translator The abaqus fromansys translator can convert ANSYS blocked coded database files (.cdb) into a “flat” Abaqus input file; that is, an Abaqus input file that is not written in terms of parts and assemblies. The .cdb file must be created in ANSYS using the following command: CDWRITE , , , cdb The second field of the CDWRITE command may contain ALL or DB. The eighth field may contain BLOCKED. Any other use of the CDWRITE command will create problems for the translator. Summary of ANSYS entities translated The translator from ANSYS to Abaqus supports the mappings shown in the tables below. Table 3.2.26–1 Nodal data mapping for ANSYS commands. ANSYS command NBLOCK Abaqus equivalent *NODE *TRANSFORM Table 3.2.26–2 Element data mapping for ANSYS structural lines. ANSYS command LINK1 LINK8 LINK10 Abaqus equivalent *ELEMENT, TYPE=T2D2 *ELEMENT, TYPE=T3D2 *ELEMENT, TYPE=T3D2 ANSYS command LINK11 LINK180 Abaqus equivalent *ELEMENT, TYPE=T3D2 *ELEMENT, TYPE=T3D2 Table 3.2.26–3 Element data mapping for ANSYS structural beams. ANSYS command BEAM3 BEAM4 BEAM23 BEAM24 BEAM188 BEAM189 Abaqus equivalent *ELEMENT, TYPE=B21 *ELEMENT, TYPE=B31 *ELEMENT, TYPE=B21 *ELEMENT, TYPE=B31 *ELEMENT, TYPE=B31 or B32 *ELEMENT, TYPE=B32 Table 3.2.26–4 Element data mapping for ANSYS structural shells. ANSYS command SHELL43 SHELL63 SHELL93 SHELL181 Abaqus equivalent *ELEMENT, TYPE=S4 or S3 *ELEMENT, TYPE=S4, S3, M3D4, or M3D3 *ELEMENT, TYPE=S8R or STRI65 *ELEMENT, TYPE=S4R or S3R Table 3.2.26–5 Element data mapping for ANSYS structural pipes. ANSYS command PIPE16 PIPE20 PIPE59 Abaqus equivalent *ELEMENT, TYPE=PIPE32 *ELEMENT, TYPE=PIPE31 *ELEMENT, TYPE=PIPE31 Table 3.2.26–6 Element data mapping for ANSYS planar elements. Abaqus equivalent *ELEMENT, TYPE=CPSn, CAXn, or CPEn ANSYS command PLANE42 PLANE82 PLANE182 PLANE183 Table 3.2.26–7 Element data mapping for ANSYS solid elements. ANSYS command SOLID45 SOLID65 SOLID92 SOLID95 SOLID147 SOLID148 SOLID185 SOLID186 SOLID187 Abaqus equivalent *ELEMENT, TYPE=C3D8I, C3D4, or C3D6 *ELEMENT, TYPE=C3D8I, C3D4, or C3D6 *ELEMENT, TYPE=C3D10 *ELEMENT, TYPE=C3D20, C3D10, or C3D15 *ELEMENT, TYPE=C3D20, C3D10, or C3D15 *ELEMENT, TYPE=C3D10 *ELEMENT, TYPE=C3D8, C3D4, or C3D6 *ELEMENT, TYPE=C3D20R, C3D10, or C3D15 *ELEMENT, TYPE=C3D10 Table 3.2.26–8 Load and boundary condition data mapping. ANSYS command SFE, ELEM, LKEY, PRES, KVAL, VAL1, VAL2, VAL3, VAL4, where VAL1=VAL2=VAL3=VAL4=n SFE, ELEM, LKEY, HFLU, KVAL, VAL1, VAL2, VAL3, VAL4, where VAL1=VAL2=VAL3=VAL4=n BF, NODE, TEMP, VAL1, VAL2, VAL3, VAL4 Abaqus equivalent *SURFACE and *DSLOAD *SURFACE and *DSFLUX *TEMPERATURE and *CFLUX ANSYS command Abaqus equivalent BFE, NODE, HGEN, STLOCVAL1, VAL2, VAL3, VAL4 ACEL, 1-component, 2-component, 3-component F, NODE, Lab, VALUE, VALUE2, NEND, NINC, where Lab=FX, FY, or FZ *DFLUX *DLOAD *CLOAD D, NODE, Lab, VALUE, VALUE2, NEND, NINC, where Lab=UX ,UY, UZ, ROTX, ROTY, or ROTZ *BOUNDARY Table 3.2.26–9 Material data mapping. ANSYS command Abaqus equivalent MPTEMP, … MPDATA, … , EX MPDATA, … , NUXY or PRXY MPTEMP, …. MPDATA, … , EX MPDATA, … , EY MPDATA, … , EZ MPDATA, … , NUXY or PRXY MPDATA, … , NUXZ or PRXZ MPDATA, … , NUYZ or PRYZ MPDATA, … , GXY MPDATA, … , GXZ MPDATA, … , GYZ MPTEMP, … MPDATA, … , KXX MPTEMP, … MPDATA, … , DENS MPTEMP, … MPDATA, … , C *MATERIAL and *ELASTIC Minor Poisson’s ratios (such as NUXY), if present, are automatically converted to major Poisson’s ratios (such as PRXY). *MATERIAL and *ELASTIC, TYPE=ENGINEERING CONSTANTS Minor Poisson’s ratios (such as NUXY), if present, are automatically converted to major Poisson’s ratios (such as PRXY). *MATERIAL and *CONDUCTIVITY *DENSITY *SPECIFIC HEAT MPTEMP, … MPDATA, … , CTEX or ALPX *EXPANSION Command summary abaqus fromansys job=job-name [input=input-file] Command line options job This option is used to specify the name of the Abaqus input file to be output by the translator. It is also the default name of the input file containing the ANSYS data. Diagnostics created by the translator will be written to a file named job-name.log. input This option is used to specify the name of the file containing the ANSYS data if it is different from job-name. TRANSLATING PAM-CRASH INPUT FILES TO PARTIAL Abaqus INPUT FILES TRANSLATION FROM PAM-CRASH Product: Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The translator from PAM-CRASH to Abaqus converts certain keywords in a PAM-CRASH input file into their equivalent in Abaqus/Explicit. Using the translator The translator requires an input file created by PAM-CRASH Version 2002 or later. The input file can have any name and extension. The PAM-CRASH data entries that are translated are listed in the tables below. Other PAM-CRASH keywords and data are skipped over and noted in the log file. The translator creates a partial Abaqus input file that contains only the model data. You must provide history data (including output data) to complete the input. Element numbering and grouping All elements must have unique element numbers. Elements that are assigned the same PART identification number are grouped together in an element set. Except for connector elements that result from the translation of SPRING and KJOIN, section properties need to be entered in the PART section rather than individually in the element section. Elements that have different material or section properties should be given different PART identification numbers; that is, the same material and section properties must be applicable to all elements grouped in the same element set. If elements that result from the translation of SPRING and KJOIN have different element data (such as frame numbers used to define local directions), and they are assigned the same PART identification number, the translator automatically separates them into different element sets. Material models The translator supports only the material models shown in Table 3.2.27–3. All unsupported material models between Types 1 and 99 are translated as bilinear elastic-plastic, and all other material types are translated as linear elastic if a stress-strain law definition is required. In these cases the translator provides nominal values for the material properties. History section data The translator creates a history section based partially on keywords (except TITLE) from the control section of the PAM-CRASH file as shown in Table 3.2.27–1. Other control data are unsupported. Summary of PAM-CRASH entities translated Table 3.2.27–1 Control section data. PAM-CRASH keyword Abaqus equivalent TITLE RUNEND TCTRL / DYNA_MASS_SCALE ECTRL / RATEFILTER *HEADING *DYNAMIC, EXPLICIT time period *VARIABLE MASS SCALING *MATERIAL, SRATE FACTOR Table 3.2.27–2 Part section data. PAM-CRASH keyword Abaqus equivalent PART / BAR PART / BEAM PART / SPRING PART / KJOIN PART / SOLID PART / SHELL PART / MEMBR PART / TIED PART / PLINK Truss element properties and grouping data Beam element properties and grouping data Connector behavior and grouping data Connector type, behavior, and grouping data Solid element properties and grouping data Shell element properties and grouping data Membrane element properties and grouping data Mesh tie constraint data and parameters Mesh-independent fastener data and parameters Table 3.2.27–3 Material section data. PAM-CRASH keyword Abaqus equivalent MATER / Types 1, 16, 41, 99 C3D4/C3D6/C3D8R; solid material model data MATER / Types 100, 101, 102, 103, 105 S3RS/S4RS; shell material model data MATER / Types 150, 151 MATER / Types 200, 201, 202 M3D3/M3D4/M3D4R and *USER MATERIAL T3D2/B31; beam and truss material model data PAM-CRASH keyword Abaqus equivalent MATER / Types 203, 204, 205, 230 CONN3D2; connector behavior data MATER / Types 212, 213 B31; beam material model data MATER / Type 3021 CONN3D2; connector behavior data 1 Material type 302 supports the use of a rupture model . Table 3.2.27–4 Node section data. PAM-CRASH keyword Abaqus equivalent FRAME NODE MASS NSMAS INVEL BOUNC DIS3D VEL3D DAMP TRSFM *ORIENTATION and *TRANSFORM *NODE *MASS and *ROTARY INERTIA *NONSTRUCTURAL MASS *INITIAL CONDITIONS, TYPE=VELOCITY or ROTATING VELOCITY *BOUNDARY *BOUNDARY and *AMPLITUDE *BOUNDARY and *AMPLITUDE *DLOAD and *AMPLITUDE *NODE with transformed coordinates Table 3.2.27–5 Element section data. PAM-CRASH keyword Abaqus equivalent C3D4/C3D6/C3D8R and *SOLID SECTION C3D4 and *SOLID SECTION S3RS/S4RS and *SHELL SECTION M3D3/M3D4R and *MEMBRANE SECTION B31 and *BEAM SECTION, SECTION=CIRC For MATER / Types 203 and 204: CONN3D2 and *CONNECTOR SECTION [AXIAL] For all other MATER / Types: T3D2 and *SOLID SECTION 3.2.27–3 SOLID TETR4 SHELL MEMBR BEAM PAM-CRASH keyword Abaqus equivalent SPRING KJOIN PLINK CONN3D2 and *CONNECTOR SECTION [CARTESIAN + CARDAN] CONN3D2 and *CONNECTOR SECTION *FASTENER and *FASTENER PROPERTY; CONN3D2 and *CONNECTOR SECTION Table 3.2.27–6 Constraint section data. PAM-CRASH keyword Abaqus equivalent RWALL (Stationary, segmented finite rigid wall) Velocity flag=0 Wall description=20 *RIGID BODY and *CONTACT RBODY Types 0, 3 RBODY Type 1 CNTAC Sliding interface types: 33, 34, 36, 37, 46 *RIGID BODY and/or *MPC (type BEAM) To define a group of elements as a rigid body, enter the part identification number of that element group as the PART entity1. To define an element as a rigid body, enter the element number as the ELE entity or enter all the element node numbers as the NOD entity2 . CONN3D2, *CONNECTOR SECTION [PROJECTION CARTESIAN + PROJECTION FLEXION-TORSION], *CONNECTOR DAMAGE INITIATION, and *CONNECTOR DAMAGE EVOLUTION *CONTACT, *CONTACT INCLUSIONS, *CONTACT EXCLUSIONS, *CONTACT PROPERTY ASSIGNMENT, *CONTACT FORMULATION, *SURFACE INTERACTION, and *SURFACE PROPERTY ASSIGNMENT TIED *TIE 1 If PART entities are used to define a rigid body, RBODY is translated as *RIGID BODY. 2 If the ELE and NOD entities constitute all elements in a part, RBODY is translated as *RIGID BODY. If the ELE and NOD entities do not constitute all elements in a part (i.e., if the part consists of both rigid and deformable elements), RBODY is translated as *MPC (MPC type BEAM), a beam-type multi-point constraint for the set of nodes that consists of all input NOD entities and nodes extracted from all ELE entities. Table 3.2.27–7 Nodes/faces/elements entity selection data. PAM-CRASH keyword Abaqus equivalent ELE PART NOD ELE>NOD PART>NOD DELELE DELPART DELNOD GRP *ELSET; data for elements to be grouped in a set using *ELSET Data for selecting element sets (*ELSET) already defined Data for nodes to be grouped in a set using *NSET Same procedure as ELE Same procedure as PART *ELSET and *NSET *ELSET and *NSET *ELSET and *NSET Named set of entities defined in GROUP Table 3.2.27–8 Airbag data. PAM-CRASH keyword Abaqus equivalent *FLUID BEHAVIOR, *MOLECULAR WEIGHT, and *CAPACITY *PHYSICAL CONSTANTS and *FLUID CAVITY *INITIAL CONDITIONS *FLUID CAVITY, BEHAVIOR or MIXTURE *NODE, NSET=ref_node_name; *SURFACE, TYPE=ELEMENT; and *FLUID CAVITY M3D3/M3D4 and *SURFACE, TYPE=ELEMENT *FLUID EXCHANGE, *FLUID EXCHANGE ACTIVATION, and *FLUID EXCHANGE PROPERTY *FLUID EXCHANGE, *FLUID EXCHANGE ACTIVATION, and *FLUID EXCHANGE PROPERTY *FLUID EXCHANGE, *FLUID EXCHANGE ACTIVATION, and *FLUID EXCHANGE PROPERTY 3.2.27–5 GASPEC BAGIN GEN_INI_COND GAS CHAMBER EXT_SKIN WALL_OPENING WALL_FABRIC PAM-CRASH keyword Abaqus equivalent INI_COND INFLATOR *INITIAL CONDITIONS *FLUID INFLATOR, *FLUID INFLATOR ACTIVATION, *FLUID INFLATOR MIXTURE, and *FLUID INFLATOR PROPERTY Table 3.2.27–9 Seat belt data. PAM-CRASH keyword Abaqus equivalent SLIPR RETRA *ELEMENT, TYPE=CONN3D2; *CONNECTOR SECTION; and *BOUNDARY *ELEMENT, TYPE=CONN3D2; *CONNECTOR SECTION; and *BOUNDARY Table 3.2.27–10 Miscellaneous data. PAM-CRASH keyword Abaqus equivalent GROUP METRIC SENSOR FUNCT RUPMO THELE THNOD Convert entities to Abaqus equivalents *INITIAL CONDITIONS, TYPE=REF COORDINATE Type-1: use activation time in *AMPLITUDE Type-4: use belt feed rate in *CONNECTOR LOCK Data for material properties and time-dependent parameters, such as *AMPLITUDE, *CONNECTOR ELASTICITY, *PLASTIC, and *FLUID EXCHANGE PROPERTY Data for connector behavior, such as *CONNECTOR DAMAGE INITIATION, *CONNECTOR DAMAGE EVOLUTION, *CONNECTOR POTENTIAL, and *CONNECTOR HARDENING Element sets defined as *ELSET; output quantities are not specified for the element set Node sets defined as *NSET; output quantities are not specified for the node set Command summary abaqus frompamcrash Command line options job job=job-name input=input-file [pLinkConnectors={OFF | ON}] [splitAirbagElements={OFF | ON}] [autoKJoinStops={OFF | ON}] This option is used to specify the name of the Abaqus input file to be output by the translator. The name of the Abaqus input file must be given without the .inp extension. Diagnostics created by the translator are written to a file named job-name_frompam.log. input This option is used to specify the name of the file containing the PAM-CRASH data. The name of the file must be given with the file extension. pLinkConnectors This option is used to specify the inclusion of connector elements in the PLINK translation. The default value is ON. splitAirbagElements This option is used to specify the splitting of 4-node airbag membrane elements into two 3-node airbag membrane elements. The default value is ON. Airbag membrane elements result from the translation of MEMBR and MATER / Types 150 and 151. This option is valid only if the keyword BAGIN is specified in the PAM-CRASH input file. autoKJoinStops This option is used to add connector stops to the behavior of all KJOIN connector elements. If the stiffness interpolated at an endpoint on the force-displacement curve exceeds the stiffness interpolated at an adjacent point by a factor of 10, a connector stop is defined at the point adjacent to the endpoint. The default value is OFF. TRANSLATING RADIOSS INPUT FILES TO PARTIAL Abaqus INPUT FILES TRANSLATION FROM RADIOSS Product: Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The translator from RADIOSS to Abaqus converts certain keywords in a RADIOSS input file into their equivalent in Abaqus/Explicit. Using the translator The translator requires an input file in block format created by RADIOSS Version 4.4 or 5.1. The input file can have any name and an optional extension. The RADIOSS data entries that are translated are listed in the tables below. Other RADIOSS keywords and data are skipped over and noted in the log file. The translator creates a partial Abaqus input file that contains only the model data and time history output data. You can provide additional output data to complete the input. Element numbering and grouping All elements in the generated Abaqus input file will have unique element numbers. New element numbers will be assigned automatically to elements with non-unique element numbers in the RADIOSS input. Elements that are assigned the same PART identification number are grouped together in an element set. Elements that have different material or properties must be given different PART identification numbers; that is, the same material and properties must be applicable to all elements grouped in the same element set. If elements that result from the translation of SPRING have different element properties (such as skew systems used to define local directions) and are assigned the same PART identification number, the translator automatically separates them into different element sets. Material models The translator supports only the material models shown in Table 3.2.28–1. All unsupported material models are translated as linear elastic if a stress-strain law definition is required. In these cases the translator provides nominal values for the material properties. Summary of RADIOSS entities translated RADIOSS keyword MAT / LAW01 (ELAST) MAT / LAW02 (PLAS_JOHN) MAT / LAW03 (HYDPLA) MAT / LAW19 (FABRI) MAT / LAW22 (DAMA) MAT / LAW35 (FOAM_VISC) MAT / LAW36 (PLAS_TAB) Table 3.2.28–1 Material data. Abaqus equivalent *ELASTIC *PLASTIC, HARDENING=JOHNSON COOK *EOS, *TENSILE FAILURE, *DAMAGE INITIATION, and *DAMAGE EVOLUTION *USER MATERIAL *PLASTIC, HARDENING=JOHNSON COOK; *RATE DEPENDENT, TYPE=JOHNSON COOK; *DAMAGE INITIATION; and *DAMAGE EVOLUTION *HYPERFOAM and *VISCOELASTIC *PLASTIC, HARDENING=ISOTROPIC Table 3.2.28–2 Property data. RADIOSS keyword Abaqus equivalent PROP / TRUS PROP / BEAM PROP / SPRING PROP / SPR_BEAM PROP / SPR_GENE PROP / SOLID PROP / SOL_ORTH PROP / SHELL PROP / SH_ORTH Truss element properties and grouping data Beam element properties and grouping data Connector behavior and grouping data Connector behavior and grouping data Connector behavior and grouping data Solid element properties and grouping data Solid element properties and grouping data Shell element properties and grouping data Shell element properties and grouping data Table 3.2.28–3 Nodal data. RADIOSS keyword Abaqus equivalent NODE ADMAS *NODE *MASS and *ROTARY INERTIA Abaqus equivalent TRANSLATION FROM RADIOSS BCS IMPDISP IMPVEL INIVEL CLOAD GRAV SKEW FRAME *BOUNDARY *BOUNDARY and *AMPLITUDE *BOUNDARY and *AMPLITUDE *INITIAL CONDITIONS, TYPE=VELOCITY or ROTATING VELOCITY *CLOAD and *AMPLITUDE *DLOAD and *AMPLITUDE *ORIENTATION and *TRANSFORM *ORIENTATION and *TRANSFORM Table 3.2.28–4 Element data. RADIOSS keyword Abaqus equivalent BRICK SHELL1 SH3N1 BEAM TRUSS SPRING C3D4/C3D6/C3D8R and *SOLID SECTION S3RS/S4RS and *SHELL SECTION; or M3D3/M3D4/M3D4R and *MEMBRANE SECTION S3RS and *SHELL SECTION; or M3D3 and *MEMBRANE SECTION B31 and *BEAM SECTION, SECTION=CIRC T3D2 and *SOLID SECTION CONN3D2 and *CONNECTOR SECTION 1 Shell elements with one integration point through the thickness are translated as membrane elements. Table 3.2.28–5 Constraint data. RADIOSS keyword Abaqus equivalent *RIGID BODY and *CONTACT *RIGID BODY and/or *MPC (type BEAM) To define an element as a rigid body, enter all the element node numbers in the node group associated with the rigid body. 3.2.28–3 RWALL RADIOSS keyword INTER / Type 2 INTER / Types 7, 10, 11 CYL_JOINT Abaqus equivalent *TIE and *FASTENER *CONTACT, *CONTACT CONTROLS ASSIGNMENT, *CONTACT FORMULATION, *CONTACT INCLUSIONS, *CONTACT EXCLUSIONS, *CONTACT PROPERTY ASSIGNMENT, *SURFACE INTERACTION, and *SURFACE PROPERTY ASSIGNMENT CONN3D2 and *CONNECTOR SECTION Table 3.2.28–6 Group data. RADIOSS keyword Abaqus equivalent *ELSET; data for elements to be grouped in a set using *ELSET *ELSET; data for elements to be grouped in a set using *ELSET *ELSET; data for elements to be grouped in a set using *ELSET *ELSET; data for elements to be grouped in a set using *ELSET *NSET; data for elements to be grouped in a set using *NSET *ELSET; data for elements to be grouped in a set using *ELSET *ELSET; data for elements to be grouped in a set using *ELSET *NSET; data for elements to be grouped in a set using *NSET *ELSET; data for elements to be grouped in a set using *ELSET *ELSET; data for elements to be grouped in a set using *ELSET *ELSET; data for elements to be grouped in a set using *ELSET *NSET; data for elements to be grouped in a set using *NSET 3.2.28–4 SUBSET PART MAT PROP NODE SH3N SHEL GRNOD GRSH3N GRSHEL GRSPRI Abaqus equivalent TRANSLATION FROM RADIOSS *ELSET; data for elements to be grouped in a set using *ELSET *ELSET and *NSET Table 3.2.28–7 Monitored volume and seat belt data. SEG SURF RADIOSS keyword MONVOL / GAS MONVOL / AIRBAG Abaqus equivalent *FLUID BEHAVIOR, *FLUID CAVITY, *FLUID EXCHANGE, *FLUID EXCHANGE ACTIVATION, *FLUID EXCHANGE PROPERTY, *FLUID INFLATOR, *FLUID INFLATOR ACTIVATION, *FLUID INFLATOR MIXTURE, *FLUID INFLATOR PROPERTY, *MOLECULAR WEIGHT, *CAPACITY, and *PHYSICAL CONSTANTS *ELEMENT, TYPE=CONN3D2; *CONNECTOR SECTION; and *BOUNDARY SPRING with property SPR_PUL Table 3.2.28–8 Miscellaneous data. RADIOSS keyword Abaqus equivalent *HEADING CONN3D2 and connector type ACCELEROMETER Data for material properties and time-dependent parameters, such as *AMPLITUDE, *CONNECTOR ELASTICITY, *PLASTIC, and *FLUID EXCHANGE PROPERTY *INTEGRATED OUTPUT SECTION Use activation time in *AMPLITUDE Data for time history output, such as *OUTPUT, HISTORY; *NODE OUTPUT; *ELEMENT OUTPUT; and *ENERGY OUTPUT job=job-name input=input-file [splitAirbagElements={OFF | ON}] [readAbaqusDat=data-file] [userDefaultMass=real-number] [userDefaultInertia=real-number] [userHistoryTime=real-number] 3.2.28–5 TITLE ACCEL FUNCT SECT SENSOR / Type 0 TH Command summary Command line options job This option is used to specify the name of the Abaqus input file to be output by the translator. The name of the Abaqus input file must be given without the .inp extension. Diagnostics created by the translator are written to a file named job-name_fromradioss.log. input This option is used to specify the name of the file containing the RADIOSS data. The file extension is optional. splitAirbagElements This option is used to specify the splitting of 4-node airbag membrane elements into two 3-node airbag membrane elements. The default value is ON. Airbag membrane elements result from the translation of SHELL or SH3N with one integration point through the thickness. This option is valid only if the keyword MONVOL/AIRBAG is specified in the RADIOSS input file. readAbaqusDat This option enables the use of an Abaqus data (.dat) file from a previous Abaqus analysis to reformulate spot weld definitions. The data file should identify spot welds that could not be formed. Using this option, the attachment points for the identified spot welds are translated using distributed coupling constraints. userDefaultMass This option is used to specify the nodal mass that is assigned to additional nodes generated during the translation that require nonzero mass. This value should be small (typically 10−6 times the mass for the entire model). If this option is omitted, the default mass is set to 10−4. userDefaultInertia This option is used to specify the rotary inertia that is assigned to additional nodes generated during the translation that require nonzero rotary inertia. This value should be small (typically 10−6 times the inertia for the entire model). If this option is omitted, the default rotary inertia is set to 10−3. userHistoryTime This option is used to specify the time interval used for time history output. If this option is omitted, the time history interval is set to 10−5 . 3.2.29 TRANSLATING Abaqus OUTPUT DATABASE FILES TO NASTRAN OUTPUT2 RESULTS FILES Product: Abaqus/Standard Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The translator converts certain results from an Abaqus output database (.odb) file to the Nastran Output2 file format. Using the translator The toOutput2 translator can only be used to translate Abaqus output database of a *STATIC or *FREQUENCY procedure. Results from an Abaqus analysis are written to the Abaqus output database by using the *OUTPUT option. The following options should be included in the Abaqus input file to ensure that the results to be translated are available in the Abaqus output database: *OUTPUT, FIELD *NODE OUTPUT U, RF, CF, *ELEMENT OUTPUT S, E, SF, NFORC, Results in the Abaqus output database other than those specified above are skipped during translation. Only results from spring elements and three-dimensional continuum, shell, membrane, beam, and truss elements are translated. For shell elements, the translator treats stresses and strains at the lowest numbered section point as being at the bottom surface and stresses and strains at the highest numbered section point as being at the top surface. Midsurface stresses and strains translated to the Output2 file are computed as the averages of the stresses and strains at the bottom and top surfaces. Nodal results are always in global coordinates. Element tensor results are in the Abaqus element coordinate system. Model data from the output database (nodal coordinates, element topology, material properties, and element properties) are written to the Output2 file when applicable records exist. Command summary abaqus toOutput2 Command line options job=job-name [odb=odb-name] [step=step-number] [increment=increment-number] [slim] [quad4corner] job odb step This option specifies the name of the Nastran Output2 file to be created by the translator. It is also the default name for the Abaqus output database. This option specifies the name of the Abaqus output database if it is different from job-name. This option specifies the step number of the Abaqus output database for the translator to translate. If the specified step contains multiple load cases, all of the load cases are translated. The default value is the last step of the analysis. increment This option is valid only when used in conjunction with the step option. It is used to specify the increment number of the step in the Abaqus output database for the translator to translate. The default value is the last increment of the specified step. slim This option is used to include data blocks required for postprocessing in the SLIM/VISION software (available from Third Millennium Productions, Inc.) in the Output2 file. quad4corner This option is used to request shell output at corner nodes instead of at the centroid. This option is relevant for stress, strain, and section force output. TRANSLATING LS-DYNA DATA FILES TO Abaqus INPUT FILES TRANSLATION FROM LS-DYNA Product: Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The translator from LS-DYNA to Abaqus converts a set of supported keywords in an LS-DYNA input file into their equivalent in Abaqus. Using the translator The translator supports translation of input files created by LS-DYNA Version 971 Rev 5 or earlier. The input file can have any name and an optional extension. The LS-DYNA keywords that are supported are listed in the tables below. Other LS-DYNA keywords and data are skipped over and noted in the log file. The translator creates an Abaqus input file that contains both the model data and history data. However, the translator does not create exact Abaqus equivalents for specific output quantities for nodal output, element output, and contact output; it uses preselected variables instead. You can provide additional output entities to complete the requests. Element numbering and grouping All elements in the generated Abaqus input file have unique element numbers. New element numbers are assigned automatically to elements with non-unique element numbers in the LS-DYNA input; all element number reassignments are noted in the log file. Elements that are assigned the same PART identification number are grouped together in an element set. Elements that have different material or properties must be given different PART identification numbers; that is, the same material and properties must be applicable to all elements grouped in the same element set. When a PART references a rigid material, the part is considered rigid. The element set that corresponds to the part is used in the rigid body definition. Material models The translator supports only the material models shown in Table 3.2.30–1. All unsupported material models are translated as linear elastic if a stress-strain law definition is required. In these cases the translator provides nominal values for the material properties. Mapping LS-DYNA elements that end in _ID or _TITLE Many LS-DYNA keywords include the options _ID, _TITLE, or both of these options. Unless the LS-DYNA keyword with _ID or _TITLE is specified in the mapping tables in this document, the translator maps data from these options to the same Abaqus keywords specified for the main LS-DYNA keyword. Summary of LS-DYNA entities translated The translator from LS-DYNA to Abaqus supports the mappings shown in the tables below. Table 3.2.30–1 Material data. LS-DYNA Keyword Abaqus Equivalent *MAT_BLATZ-KO_RUBBER *MAT_CABLE_DISCRETE_BEAM *MAT_DAMPER_NONLINEAR _VISCOUS *MAT_DAMPER_VISCOUS *MAT_ELASTIC *MAT_ELASTIC_PLASTIC _THERMAL *MAT_FU_CHANG_FOAM *MAT_HONEYCOMB *MAT_JOHNSON_COOK *MAT_LINEAR_ELASTIC _DISCRETE_BEAM *MAT_LOW_DENSITY_FOAM *HYPERELASTIC, NEO HOOKE *ELASTIC *CONNECTOR DAMPING, NONLINEAR *CONNECTOR DAMPING *ELASTIC *ELASTIC *PLASTIC *EXPANSION *LOW DENSITY FOAM and *UNIAXIAL TEST DATA Built-in VUMAT user material model ABQ_HONEYCOMB1 *PLASTIC, HARDENING=JOHNSON COOK *RATE DEPENDENT, TYPE=JOHNSON COOK *SHEAR FAILURE, TYPE=JOHNSON COOK *TENSILE FAILURE, TYPE=JOHNSON COOK *CONNECTOR ELASTICITY and *CONNECTOR DAMPING *HYPERFOAM and *UNIAXIAL TEST DATA LS-DYNA Keyword Abaqus Equivalent *MAT_NULL *MAT_OGDEN_RUBBER *MAT_PIECEWISE_LINEAR _PLASTICITY *MAT_PLASTIC_KINEMATIC *MAT_RIGID *MAT_SEATBELT *MAT_SPOTWELD *MAT_SPRING_ELASTIC *MAT_SPRING_NONLINEAR _ELASTIC *ELASTIC Shell elements that reference a null material are translated as surface elements *HYPERELASTIC, OGDEN *PLASTIC *PLASTIC, HARDENING=KINEMATIC *ELASTIC *RIGID BODY (for LS-DYNA parts that refer to a rigid material) *CONNECTOR ELASTICITY, NONLINEAR *CONNECTOR ELASTICITY, RIGID *CONNECTOR ELASTICITY *CONNECTOR ELASTICITY, NONLINEAR *MAT_VISCOELASTIC *VISCOELASTIC, TIME=PRONY 1 For more information about using ABQ_HONEYCOMB, refer to “Abaqus/Explicit honeycomb material model,” which is available in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com. Table 3.2.30–2 Part data. LS-DYNA Keyword Abaqus Equivalent *PART *PART_PRINT *PART_CONTACT *PART_INERTIA *ELSET and the corresponding type of element section *SURFACE INTERACTION properties *ELEMENT, TYPE=MASS *ELEMENT, TYPE=ROTARYI Table 3.2.30–3 Auxiliary data. LS-DYNA Keyword Abaqus Equivalent *DEFINE_COORDINATE_NODES *DEFINE_COORDINATE _SYSTEM *DEFINE_COORDINATE _VECTOR *DEFINE_CURVE *DEFINE_SD_ORIENTATION *DEFINE_TABLE *ORIENTATION, DEFINITION=NODES *ORIENTATION, DEFINITION=COORDINATES *ORIENTATION, DEFINITION=COORDINATES Data from a single curve used in the following keywords: *AMPLITUDE *CONNECTOR DAMPING (nonlinear) *CONNECTOR ELASTICITY (nonlinear) *SURFACE BEHAVIOR *UNIAXIAL TEST DATA *ORIENTATION Multi-curve data used in conjunction with *PLASTIC and *LOW DENSITY FOAM in which the stress-strain relationship is defined for various strain rates LS-DYNA Keyword *SECTION_BEAM *SECTION_DISCRETE *SECTION_SEATBELT *SECTION_SHELL Table 3.2.30–4 Section data. Abaqus Equivalent Beam elements: *BEAM SECTION or *BEAM GENERAL SECTION Truss elements: *SOLID SECTION *CONNECTOR SECTION *CONNECTOR SECTION Shell elements: *SHELL SECTION Membrane elements: *MEMBRANE SECTION Surface elements: *SURFACE SECTION LS-DYNA Keyword *SECTION_SOLID *SECTION_TSHELL Abaqus Equivalent *SOLID SECTION *SHELL SECTION Table 3.2.30–5 Nodal data. LS-DYNA Keyword Abaqus Equivalent *NODE *NODE Table 3.2.30–6 Output options data. LS-DYNA Keyword Abaqus Equivalent *DATABASE_BINARY_D3PLOT *DATABASE_BINARY_D3THDT *DATABASE_DEFORC *DATABASE_ELOUT *DATABASE_NODOUT *DATABASE_HISTORY_BEAM *DATABASE_HISTORY_BEAM_ID *DATABASE_HISTORY_BEAM_SET *DATABASE_HISTORY_NODE *DATABASE_HISTORY_NODE_ID *DATABASE_HISTORY_NODE_SET *DATABASE_HISTORY_SHELL *DATABASE_HISTORY_SHELL_ID *DATABASE_HISTORY_SHELL_SET *DATABASE_HISTORY_SOLID *DATABASE_HISTORY_SOLID_ID *DATABASE_HISTORY_SOLID_SET *OUTPUT, FIELD and *ELEMENT OUTPUT *OUTPUT, FIELD and *ELEMENT OUTPUT *OUTPUT, FIELD and *ELEMENT OUTPUT *OUTPUT, FIELD and *ELEMENT OUTPUT *OUTPUT, FIELD and *NODE OUTPUT *OUTPUT, HISTORY and *ENERGY OUTPUT *OUTPUT, HISTORY and *ENERGY OUTPUT *OUTPUT, HISTORY and *ENERGY OUTPUT *OUTPUT, HISTORY and *ENERGY OUTPUT Table 3.2.30–7 Element data. LS-DYNA Keyword Abaqus Equivalent *ELEMENT_BEAM *ELEMENT_BEAM_PID *ELEMENT_DISCRETE *ELEMENT_MASS *ELEMENT_SEATBELT *ELEMENT_SHELL Beam elements: *ELEMENT, TYPE=B31 Truss elements: *ELEMENT, TYPE=T3D2 *ELEMENT, TYPE=CONN3D2 and *FASTENER *ELEMENT, TYPE=CONN3D2 *ELEMENT, TYPE=MASS and *MASS *ELEMENT, TYPE=CONN3D2 Shell elements: *ELEMENT, TYPE=S3R or S4R Membrane elements: *ELEMENT, TYPE=M3D3 or M3D4R Surface elements (with *MAT_NULL): *ELEMENT, TYPE=SFM3D3 or SFM3D4R *ELEMENT_SOLID *ELEMENT, TYPE=C3D4, C3D6, C3D8R, or C3D10M *ELEMENT_TSHELL *ELEMENT, TYPE=SC6R or SC8R Table 3.2.30–8 Prescribed conditions data. LS-DYNA Keyword Abaqus Equivalent *BOUNDARY_PRESCRIBED _MOTION_NODE *BOUNDARY_PRESCRIBED _MOTION_SET *BOUNDARY, TYPE=DISPLACEMENT, VELOCITY, or ACCELERATION *BOUNDARY, TYPE=DISPLACEMENT, VELOCITY, or ACCELERATION *BOUNDARY_PRESCRIBED _MOTION_RIGID *BOUNDARY for reference node of rigid body *BOUNDARY_PRESCRIBED _MOTION_RIGID_LOCAL *BOUNDARY for reference node of rigid body *BOUNDARY_SPC_NODE *BOUNDARY_SPC_SET *BOUNDARY *BOUNDARY LS-DYNA Keyword Abaqus Equivalent *INITIAL_VELOCITY _GENERATION *INITIAL_VELOCITY_NODE *INITIAL CONDITIONS, TYPE=ROTATING VELOCITY *INITIAL CONDITIONS, TYPE=VELOCITY Table 3.2.30–9 Miscellaneous constraints data. LS-DYNA Keyword Abaqus Equivalent *CONSTRAINED_NODE_SET *CONSTRAINED_NODAL_RIGID _BODY *CONSTRAINED_EXTRA_NODES _NODE *CONSTRAINED_EXTRA_NODES _SET *CONSTRAINED_JOINT _CYLINDRICAL *CONSTRAINED_JOINT _REVOLUTE *CONSTRAINED_JOINT _SPHERICAL *CONSTRAINED_JOINT _STIFFNESS_GENERALIZED *CONSTRAINED_JOINT _TRANSLATIONAL *CONSTRAINED_JOINT _UNIVERSAL *EQUATION *MPC type BEAM Node set used as TIE NSET in the definition of *RIGID BODY Node set used as TIE NSET in the definition of *RIGID BODY *ELEMENT, TYPE=CONN3D2 *ELEMENT, TYPE=CONN3D2 *ELEMENT, TYPE=CONN3D2 *ELEMENT, TYPE=CONN3D2 *CONNECTOR SECTION, BEHAVIOR *ELEMENT, TYPE=CONN3D2 *ELEMENT, TYPE=CONN3D2 *CONSTRAINED_RIGID_BODIES *CONSTRAINED_SPOTWELD Merged element set used in the definition of *RIGID BODY *MPC type BEAM Table 3.2.30–10 Load data. LS-DYNA Keyword Abaqus Equivalent *LOAD_BODY_PARTS *ELSET for *DLOAD *LOAD_BODY_X *LOAD_BODY_Y *LOAD_BODY_Z *DLOAD *DLOAD *DLOAD *LOAD_NODE_POINT *CLOAD with node data *LOAD_NODE_SET *CLOAD with node set data Table 3.2.30–11 Set data. LS-DYNA Keyword *SET_NODE_LIST *SET_NODE_LIST_GENERATE *SET_PART *SET_PART_LIST *SET_PART_LIST_GENERATE *SET_SEGMENT *SET_SHELL_LIST *SET_SHELL_LIST_GENERATE *SET_SOLID_LIST Abaqus Equivalent *NSET with node data *NSET with node data *ELSET with element set data *ELSET with element set data *ELSET with element set data *ELSET with element data *ELSET with element data *ELSET with element data *ELSET with element data Table 3.2.30–12 Contact data. LS-DYNA Keyword Abaqus Equivalent *CONTACT_AUTOMATIC_GENERAL *CONTACT *CONTACT INCLUSION *CONTACT PROPERTY ASSIGNMENT *SURFACE INTERACTION *SURFACE PROPERTY ASSIGNMENT Abaqus Equivalent TRANSLATION FROM LS-DYNA *CONTACT_AUTOMATIC _NODES_TO_SURFACE *CONTACT_AUTOMATIC _SINGLE_SURFACE *CONTACT_AUTOMATIC _SURFACE_TO_SURFACE *CONTACT_NODES_TO_SURFACE *CONTACT_RIGID_NODES_TO _RIGID_BODY *CONTACT_SINGLE_SURFACE *CONTACT *CONTACT INCLUSION *CONTACT PROPERTY ASSIGNMENT *SURFACE INTERACTION *SURFACE PROPERTY ASSIGNMENT *CONTACT *CONTACT INCLUSION *CONTACT PROPERTY ASSIGNMENT *SURFACE INTERACTION *SURFACE PROPERTY ASSIGNMENT *CONTACT *CONTACT INCLUSION *CONTACT PROPERTY ASSIGNMENT *SURFACE INTERACTION *SURFACE PROPERTY ASSIGNMENT *CONTACT *CONTACT INCLUSION *CONTACT PROPERTY ASSIGNMENT *SURFACE INTERACTION *SURFACE PROPERTY ASSIGNMENT *CONTACT *CONTACT INCLUSION *CONTACT PROPERTY ASSIGNMENT *SURFACE INTERACTION *SURFACE PROPERTY ASSIGNMENT *CONTACT *CONTACT INCLUSION *CONTACT PROPERTY ASSIGNMENT *SURFACE INTERACTION *SURFACE PROPERTY ASSIGNMENT LS-DYNA Keyword Abaqus Equivalent *CONTACT_SURFACE_TO_SURFACE *CONTACT_TIED_NODES _TO_SURFACE *CONTACT_TIED_SURFACE _TO_SURFACE *CONTACT *CONTACT INCLUSION *CONTACT PROPERTY ASSIGNMENT *SURFACE INTERACTION *SURFACE PROPERTY ASSIGNMENT *TIE *TIE Table 3.2.30–13 Miscellaneous data. LS-DYNA Keyword Abaqus Equivalent *CONTROL _TERMINATION *END *KEYWORD *TITLE *INCLUDE Time period entered in *DYNAMIC, EXPLICIT *END None *HEADING Process multiple LS-DYNA files Command summary abaqus fromdyna Command line options job job=job-name input=dyna-input-file [splitFile={OFF | ON}] This option is used to specify the name of the Abaqus input file to be output by the translator. The name of the Abaqus input file must be given without the .inp extension. Diagnostics created by the translator are written to a file named job-name.log. input This option is used to specify the name of the file containing the LS-DYNA keyword data. The LS-DYNA input file can have an extension. splitFile This option specifies whether the Abaqus input file is to be split into multiple files. If splitFile=ON, the following files are output: • job-name_nodes.inc: include file that contains the nodal data • job-name_elements.inc: include file that contains the element data • job-name_model.inc: include file that contains the remaining model data • job-name.inp: Abaqus input file that includes all of the above include files and the history data 3.2.31 EXCHANGING Abaqus DATA WITH ZAERO Product: Abaqus/Standard Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The abaqus tozaero interface enables you to exchange aeroelastic data between the Abaqus and ZAERO analysis products. By using this interface between the applications, you can perform structural modal analysis on a model in Abaqus, transfer the model to ZAERO for aeroelastic analysis, then transfer it back to Abaqus for stress analysis. Universal file The universal file is the means of data exchange between Abaqus and ZAERO. It consists of four data sets: 2411, which describes node and coordinate data; 2414, which describes mass-normalized mode shapes; 2420, which describes the global coordinate system; and 2453, which describes the mass matrix in text format, or 2453b, which describes the mass matrix in binary format. You can specify the universal file’s output format by using the mode parameter. Choosing text format enables you to modify the universal file in a text editor but increases the file size to over twice that of similar files in binary format. Text is the default format and the only format supported by ZAERO. Table 3.2.31–1 and Table 3.2.31–2 describe the mass matrix data set text format and binary format, respectively. Table 3.2.31–1 Format for data set 2453 (text). Record Field Format (I10) Description Matrix Identifier 1: DOF 131: Mass 139: Stiffness 147: Back-expansion Record Field Format (6I10) Description Matrix Data Type 1: Integer 2: Real 4: Double Precision 5: Complex 6: Complex Double Precision Matrix Form 3: General Rectangular Number of rows Number of columns Storage Key 1: Row 2: Column 11: Sparse (not supported for IMAT=1) Matrix Size Parameter For IMAT=1 this is the number of dynamic modes. For sparse this is the number of matrix entries. Otherwise, 0. 3 for storage keys 1 and 2 N/A Matrix Data For data type 1: (8 I10) For data type 2: (4 E20.12) For data type 4: (4 D20.12) For data type 5: (2 (2 E20.12)) For data type 6: (2 (2 D20.12)) Field Description Format TRANSLATION TO ZAERO 3 for storage key 11 Row Column Value at cell For data type 1: (2 (2I10 1I10)) For data type 2: (2 (2I10 1E20.12)) For data type 4: (2 (2I10 1D20.12)) For data type 5: (1 (2I10 2E20.12)) For data type 6: (1 (2I10 2D20.12)) Table 3.2.31–2 Format for data set 2453b (binary). Field Description Format Record Header 2453 Lowercase b Byte Ordering Method 1: Little Endian (Windows and DOS) 2: Big Endian (most UNIX) Floating Point Format 1: DEC VMS 2: IEEE 754 (UNIX) 3: IBM 5/370 Number of ASCII lines following 2 for data set 2453b (I6) (IA1) (I6) (I6) (I12) Number of bytes following ASCII lines (I12) Not used (fill with zeros) (I10) Matrix Identifier 1: DOF 131: Mass 139: Stiffness 147: Back-expansion 3.2.31–3 7–10 Record Field Format (6I10) Description Matrix Data Type 1: Integer 2: Real 4: Double Precision 5: Complex 6: Complex Double Precision Matrix Form 3: General Rectangular Number of rows Number of columns Storage Key 1: Row 2: Column 11: Sparse (not supported for IMAT=1) Matrix Size Parameter For IMAT=1 this is the number of dynamic modes. For sparse this is the number of matrix entries. Otherwise, 0. 3 (Binary Matrix Data) 1 (4 bytes) Row 2 (4 bytes) Column Value at cell For data type 1: (2 Int32 1 Int32) For data type 2: (2 Int32 1 Flt32) For data type 4: (2 Int32 1 Dbl64) For data type 5: (2 Int32 2 Flt32) For data type 6: (2 Int32 2 Dbl64) Preparing the Abaqus analysis input file Before the interface can create the universal file, you must make the following additions to your Abaqus input (.inp) file, then run Abaqus: • Normalize the eigenvectors in the eigenfrequency extraction analysis with respect to the structure’s mass matrix. This normalization is necessary because the translator assumes the mode shapes are mass normalized; if you skip this step before the Abaqus run, the modes translated will be incorrect and will give incorrect results with no warnings or errors. For more information, see “Natural frequency extraction,” Section 6.3.5. • Include the following line in the analysis step: *ELEMENT MATRIX OUTPUT, ELSET=allelements, MASS=YES, OUTPUT FILE=USER DEFINED, FILE NAME=mtx-file-name where allelements is a defined element set containing all the elements that should be included in the global mass matrix. The matrix output will be placed into the file mtx-file-name.mtx; you should not specify the .mtx extension since Abaqus adds it automatically. Workflow This section describes the input and output of the three main steps in the workflow between Abaqus and ZAERO. Modal analysis in Abaqus The Abaqus modal analysis uses an Abaqus input file and outputs the following data to an output database (.odb) file and matrix (.mtx) file: structural model nodes, coordinate systems, mode frequencies, generalized mass, mode shapes, and the mass matrix. Aeroelastic analysis in ZAERO Aeroelastic analysis requires a ZAERO input file and the universal file created by toZAERO. ZAERO outputs force and moment data on structural nodes due to aeroelastic forces to the universal file. Stress analysis in Abaqus The forces and moments output from ZAERO can then be used in a static (linear or nonlinear) Abaqus analysis to calculate deflections, stresses, and loads. job=job-name [unvfile=unv-file-name] [odbfile=odb-file-name] [mtxfile=mtx-file-name] [step=step-number] [mode={text | binary}] 3.2.31–5 Command summary Command line options job This option is used to specify the name of the Abaqus input file. It is also the default name for the universal output database and mass matrix files. unvfile This option is used to specify the name of the universal file if it is different from job-name. If the .unv extension is not supplied, Abaqus adds it automatically. odbname This option is used to specify the name of the Abaqus output database file if it is different from job-name. If the .odb extension is not supplied, Abaqus adds it automatically. mtxfile This option is used to specify the file containing the element mass matrices generated by Abaqus. If the .mtx extension is not supplied, Abaqus adds it automatically. step This option specifies the step number containing the eigenfrequency extraction results from Abaqus. The default value is 1. Note: You must normalize the eigenvectors in the eigenfrequency extraction analysis with respect to the structure’s mass matrix. For more information, see “Natural frequency extraction,” Section 6.3.5. mode This option specifies the output format of the universal file. If this option is set equal to binary, Abaqus writes a portion of the universal file in binary format to save space. If this option is set equal to text, Abaqus writes the entire file in all text format. The default value is text, which is the only mode currently supported by ZAERO. 3.2.32 ENCRYPTING AND DECRYPTING Abaqus INPUT DATA Products: Abaqus/Standard Abaqus/Explicit References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Including an encrypted data file” in “Defining a model in Abaqus,” Section 1.3.1 • *INCLUDE Overview You can use the abaqus encrypt utility to prevent the unauthorized use of Abaqus input data. The utility converts a data file into an encrypted, password-protected format that only authorized Abaqus input parties can access. The utility is intended for the encryption of data that you include by reference in input (.inp) files or in other data files. For example, you could encrypt a file that contains all of the proprietary material data for your model, then include the encrypted data file by reference in an unencrypted Abaqus input file. See “Including an encrypted data file” in “Defining a model in Abaqus,” Section 1.3.1, for information on how to include an encrypted data file in an Abaqus input file. You can encrypt any input file. However, Abaqus cannot run an encrypted Abaqus input file directly; the encrypted file must be included in an unencrypted file. Specifying additional access levels and controls You can customize your encryption so that only users with a license for a particular Abaqus feature or from a particular site can include or decrypt the file. For example, you can specify that only Abaqus/Standard users can access the file. You can also prevent decryption of an encrypted file by any user, regardless of their license and site; end users can still use the encrypted data in an analysis by including it by reference in an unencrypted Abaqus input file, provided that the users know the encrypted file’s password. Security and support considerations The primary intent of the Abaqus encryption implementation is to prevent unauthorized use of encrypted input data, not to prevent disclosure of encrypted data to authorized users. Running an Abaqus analysis input using encrypted data may produce output files that are not encrypted. Only material and connector behavior information contained within an encrypted input file is prevented from being visible in the output. This approach means that recipients of encrypted data who satisfy the access criteria, such as the password, license feature, or SiteID, will be able to reconstruct some input in an unencrypted form. Providers of encrypted data should consider establishing contractual agreements to protect proprietary data. Users of encrypted data must accept responsibility for security of files produced from encrypted input and should consider restricting access to resulting analysis files. Abaqus technical support cannot retrieve lost passwords for encrypted data files. Users receiving encrypted data should contact the data provider for any technical support issues. Adding comments to the header of an encrypted file When you encrypt a file, Abaqus adds the following unencrypted comment line to the beginning of the file: ** encrypted input Do not modify or delete this header comment. You can, however, insert additional comment lines between this header comment and the first line of encrypted data. These post-encryption comment lines can describe the encrypted file’s contents, provide release numbers, or display copyright and legal information about the encrypted data. For more information about comment line syntax, see “Input syntax rules,” Section 1.2.1. You should not, however, add post-encryption comment lines within the lines of encrypted data. If you want to edit or amend the comment lines within the data itself, you must first decrypt the data. Command summary abaqus {encrypt | decrypt} Command line options input input=input-file-name output=output-file-name password=password [license=feature_list] [expiration=expiration_date] [siteid=site-id_list] [include_only] This option specifies the name of the data file that you want to encrypt or decrypt. If you omit this option from the command line, Abaqus will prompt you for its value. output This option specifies the name of the data file after encryption or decryption. If you omit this option from the command line, Abaqus will prompt you for its value. password This option specifies the password for this encryption or decryption. Passwords are case-sensitive. If you omit this option from the command line while encrypting data, Abaqus will prompt you for its value. If you enter the password incorrectly or omit it from the command line while decrypting data, Abaqus reports that the input file is either corrupted or the password is incorrect. license This option applies only to file encryption. This option specifies the Abaqus feature or features for which end users must be licensed if they want to include or decrypt this encrypted data file. You can use a comma-separated list to allow access to the file by licensees of any one of a series of Abaqus features. Any feature name that appears in an Abaqus license file is valid. These might include the following features: foundation, standard, explicit, design, aqua, ams, cae, viewer, cae_nogui, adams, cmold, moldflow, safe, cadporter_catia, cadporter_catiav5, cadporter_ideas, cadporter_parasolid, cadporter_proe, afcv5_structural, and afcv5_thermal. siteid This option applies only to file encryption. This option specifies the Abaqus Site ID or IDs where end users can include or decrypt this encrypted data file. You can use a comma-separated list to allow multiple sites access to the file. You can use this option only when you also use the license option. To determine your Abaqus Site ID, run abaqus whereami from a command prompt. include_only This option applies only to file encryption. This option specifies that encrypted input data cannot be decrypted using the abaqus decrypt execution procedure; such data can only be included in an Abaqus input file. If you attempt to decrypt a file that was encrypted with the include_only option, Abaqus issues an error message stating that the input file can be included in an analysis but is not eligible for decryption. expiration This option applies only to file encryption. This option specifies the date after which the end users can no longer decrypt or include the encrypted data file. The date must be provided in the formYYYY-MM-DD. Examples The following examples illustrate the different encryption methods that are possible using the encrypt execution procedure. Creating encrypted files In the simplest encryption scenario an Abaqus user creates an encrypted copy of a file named material_data.inp, which contains all of the material data for a model, before sending the encrypted version to an authorized end user. Encryption prevents unauthorized users from accessing the encrypted file during its transmission. To create an encrypted copy of material_data.inp named material_data_enc.inp, issue the following command: abaqus encrypt input=material_data.inp output=material_data_enc.inp password=e1No9c2z Upon receiving the file, the end user can run the abaqus decrypt execution procedure to create a copy of the original, non-encrypted material data file. Because of the encryption options selected in this example, the end user requires only the encrypted file’s password to decrypt it. To decrypt the encrypted data file material_data_enc.inp, producing the non-encrypted file material_data.inp, issue the following command: abaqus decrypt input=material_data_enc.inp output=material_data.inp password=e1No9c2z Alternatively, the end user can skip the decryption and run an analysis that includes the encrypted data by reference. To include the encrypted file by reference in an Abaqus input file, add the following statement to the input file: *INCLUDE, INPUT=material_data_enc.inp, PASSWORD=e1No9c2z Limiting access to decrypted files by license feature or site ID You can specify that end users cannot access the file unless they have a valid license for a particular Abaqus feature, run Abaqus at a particular site, or satisfy both of these criteria. To encrypt a data file that can be accessed only by users who have an Abaqus/Explicit license and who run the software at site 09YYY, issue the following command: abaqus encrypt input=material_data.inp output=material_data_enc.inp password=e1No9c2z license=explicit siteid=09YYY An end user can attempt to access the file material_data_enc.inp using the same decryption or inclusion syntax specified in the previous example. For this encrypted file, Abaqus would validate that the end user has an Abaqus/Explicit license and is running Abaqus at site 09YYY before providing access to the file. If the end user’s license or site settings do not match those specified during encryption, Abaqus issues an error message that lists the licenses or sites that are required to access the file. Creating encrypted files that must be included to be used by Abaqus You can use the include_only option to prevent end users from decrypting the file directly using abaqus decrypt. Authorized users can access a file encrypted with the include_only option by including the file by reference in an Abaqus input file. Material and connector behavior definitions within an encrypted input file are not written to the output database. In addition, all material and connector behavior definitions output to the data file are suppressed if an encrypted file is used as input for any portion of the model. To create an encrypted file that is available only for inclusion by reference in other input files, issue the following command: abaqus encrypt input=material_data.inp output=material_data_enc.inp password=e1No9c2z include_only The resulting encrypted file can be included by reference in an Abaqus input file using the same syntax as in the previous example. If you attempt to decrypt a file that was encrypted with the include_only option, Abaqus returns an error message. 3.2.33 JOB EXECUTION CONTROL Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The execution procedures for job execution control include abaqus suspend, abaqus resume, and abaqus terminate. These utilities are used to suspend, resume, and terminate Abaqus analysis jobs. Suspending an analysis job will stop its execution and release its license tokens to the free-token pool. Resuming an analysis will reactivate a suspended job and check out license tokens for that job if they are available. The job will be placed in the license queue if license tokens are not available. Terminating an analysis job will stop the executable for the analysis and release its license tokens. A terminated analysis job cannot be resumed. Command summary abaqus {suspend | resume | terminate} job=job-name Command line options Required option job This option is used to specify the name of the analysis job to suspend, resume, or terminate. 3.3 Environment file settings • “Using the Abaqus environment settings,” Section 3.3.1 3.3.1 USING THE Abaqus ENVIRONMENT SETTINGS Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The Abaqus environment settings allow you to control various aspects of an Abaqus job’s execution. For example, you can • “Tune” Abaqus to improve its performance by changing memory-related parameters. • Control where and how scratch files are written. • Provide default values for job parameters that would otherwise have to be given on the command line. Many other aspects of a job’s execution can be configured through the environment settings. Some of these are discussed in this section; others, which are mainly of interest to the Abaqus site manager, are discussed in detail in the Abaqus Installation and Licensing Guide. Environment settings hierarchy Abaqus environment settings are processed in the following order: 1. The host-level environment settings. These settings are applied to all Abaqus jobs run on the designated computer. 2. The user-level environment settings. These settings are applied to all Abaqus jobs run in your account. For Abaqus to locate the environment file in your home directory on Windows platforms, the full path to your home directory must be specified using the HOME environment variable or a combination of the HOMEDRIVE and HOMEPATH environment variables. 3. The job-level environment settings. These settings are applied to only the designated Abaqus job. Environment settings can be specified more than once. The last value processed will be the one used for the setting if it is defined at more than one level or if it is given twice at the same level. Abaqus environment settings are set using special files in specific directories. The host-level settings are set in the site directory in the abaqus account directory. You can change these settings by creating an environment file, abaqus_v6.env, in your home directory and/or the current directory. Settings in the home directory file will be applied to all jobs that you run. Settings in the current directory file will be applied only to jobs run from the current directory. Syntax The entries given in the environment file must be given using Python language syntax. Entries take the form: parameter=value The following is a brief overview of the Python syntax rules: • The parameter must always have a value. The value can be any valid Python constant or expression. • A string value must be enclosed in a pair of double or single quotes. • Comments are preceded by a number sign (#). All characters following a number sign on a line are ignored. Number signs within a quoted string are part of the string, not the beginning of a comment. • Blank lines are ignored. • Embedded single quotes do not require special handling if they are placed within a double quoted string. For example, "my value’s" is translated as my value’s. The same holds true for double quotes embedded in a single quoted string. Quotes of the same type as the enclosing quotes can be embedded if they are prefixed by the backslash (\) character. • Triple quoted (""") strings can span more than one line, and no special treatment of quotes within the string is necessary. Entries take the form: parameter=""" multi-line value """ • Lists must be enclosed in parentheses (( )) or square brackets ([ ]). Individual items in the list are separated by commas. If the list is enclosed in parentheses and contains only one value, a comma has to follow the value. String list items must be enclosed in quotes. Entries take the form: parameter=(value1, value2, value3) Troubleshooting Problems caused by faulty environment settings can be diagnosed by using the command abaqus information=environment This command prints all of the current environment settings. Command line default parameters The following parameters provide default values for various settings that would otherwise have to be specified on the command line . Values given on the command line override values specified in the environment files. cpus Number of processors to use if parallel processing is available. The default is 2 for the co-simulation execution procedure; otherwise, the default is 1. domains If the value is greater than 1, the domain The number of parallel domains in Abaqus/Explicit. decomposition will be performed regardless of the values of the parallel and cpus parameters. However, if parallel=domain, the value of cpus must be evenly divisible into the value of domains. If this parameter is not set, the number of domains defaults to the number of processors used during the analysis run if parallel=domain or to 1 if parallel=loop. double_precision The default precision version of Abaqus/Explicit to run if you do not specify the precision version on the abaqus command line. Possible values are EXPLICIT (only the Abaqus/Explicit analysis is run in double precision), BOTH (both the Abaqus/Explicit packager and analysis are run in double precision), CONSTRAINT (the constraint packager and constraint solver in Abaqus/Explicit are run in double precision, while the Abaqus/Explicit packager and analysis continue to run in single precision), or OFF (both the Abaqus/Explicit packager and analysis are run in single precision). The default is OFF. parallel The default parallel method in Abaqus/Explicit if you do not specify the parallel method on the abaqus command line. Possible values are DOMAIN or LOOP; the default value is DOMAIN. run_mode Default run mode (interactive, background, or batch) if you do not specify the run mode on the abaqus command line. The default for abaqus analysis is "background", while the default for abaqus viewer is "interactive". scratch Directory to be used for scratch files. This directory must exist (i.e., it will not be created by Abaqus) and must have write permission assigned. On UNIX platforms the default value is the value of the $TMPDIR environment variable or /tmp if $TMPDIR is not defined. On Windows platforms the default value is the value of the %TEMP% environment variable or \TEMP if this variable is not defined. During the analysis a subdirectory will be created under this directory to hold the analysis scratch files. The name of the subdirectory is constructed from your user name, the job id, and the job’s process identifier. The subdirectory and its contents are deleted upon completion of the analysis. standard_parallel The default parallel execution mode in Abaqus/Standard if you do not specify the parallel mode on the abaqus command line. If this parameter is set equal to ALL, both the element operations and the solver will run in parallel. If this parameter is set equal to SOLVER, only the solver will run in parallel. The default parallel execution mode is ALL. gpus The GPGPU direct solver acceleration setting in Abaqus/Standard if you do not specify the GPGPU solver acceleration option on the abaqus command line. By default, GPGPU solver acceleration is not activated. The value of this parameter is the number of GPGPUs to be used in an Abaqus/Standard analysis. In an MPI-based analysis, this is the number of GPGPUs to be used on each host. unconnected_regions If this variable is set to ON, Abaqus/Standard will create element and node sets in the output database for unconnected regions in the model during a datacheck analysis. Element and node sets created with this option are named MESH COMPONENT N, where N is the component number. The default value is OFF. order_parallel The ordering mode for the direct sparse solver in Abaqus/Standard if you do not specify the ordering mode on the abaqus command line. If this parameter is set equal to OFF, the ordering procedure will not run in parallel. If this parameter is set equal to ON, the ordering procedure will run in parallel. The default ordering mode is ON. System resource parameters The following environment file variable can be set after the code has been installed to change the resources used by Abaqus and, therefore, to improve system performance. By default, Abaqus detects the physical memory on a machine (or on each compute node in a cluster) and allocates a percentage of the available memory based on the machine platform (for details, refer to the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com). You can override the default percentage by specifying a number followed by the percentage sign. The variable can also be defined as the number of megabytes or the number of gigabytes. More detailed information about changing the system resources used by Abaqus is given in “Managing memory and disk use in Abaqus,” Section 3.4.1. memory Maximum amount of memory or maximum percentage of the physical memory that can be allocated during the input file preprocessing and during the Abaqus/Standard analysis phase. For parallel execution on computer clusters, this memory limit specifies the maximum amount of memory that can be allocated on each process. System customization parameters The following is a discussion of some additional environment file parameters that are commonly used. A complete listing of parameters can be found in the Abaqus Installation and Licensing Guide. ask_delete If this parameter is set equal to OFF, you will not be asked whether old job files of the same file name should be deleted; the files will be deleted automatically. The default value is ON. auto_calculate If this parameter is set equal to ON, the postprocessing calculator will be launched automatically at the end of an analysis if the execution procedure detects that output database file conversion is necessary. If this parameter is set to OFF, the postprocessing calculator will not run at the end of an analysis even if the execution procedure detects that it is necessary. The default value is ON. auto_convert If this parameter is set equal to ON and an Abaqus/Explicit analysis is run in parallel with parallel=domain, the convert=select, convert=state, and convert=odb options will be run automatically at the end of the analysis. The default value is ON. average_by_section If this parameter is set equal to This parameter is used only for an Abaqus/Standard analysis. OFF, the averaging regions for output written to the data (.dat) file and results (.fil) file are based on the structure of the elements. If this parameter is set equal to ON, the averaging regions also take into account underlying values of element properties and material constants. In problems with many section and/or material definitions the default value of OFF will, in general, give much better performance than the nondefault value of ON. See “Output to the data and results files,” Section 4.1.2, for further details on the averaging scheme. mp_host_list List of host machine names to be used for an MPI-based parallel Abaqus analysis, including the number of processors to be used on each machine; for example, mp_host_list=[['maple',1],['pine',1],['oak',2]] indicates that, if the number of cpus specified for the analysis is 4, the analysis will use one processor on a machine called maple, one processor on a machine called pine, and two processors on a machine called oak. The total number of processors defined in the host list has to be greater than or equal to the number of cpus specified for the analysis. If the host list is not defined, Abaqus will run on the local system. When using a supported queuing system, this parameter does not need to be defined. If it is defined, it will get overridden by the queuing environment. mp_mode Set this variable equal to MPI to indicate that the MPI components are available on the system. Set mp_mode=THREADS to use the thread-based parallelization method. The default value is MPI where applicable. odb_output_by_default If this parameter is set equal to ON, output database output will be generated automatically. If this parameter is set equal to OFF, output database request keywords must be placed in an input file to obtain output database output. The default value is ON. onCaeStartup Optional function to be executed before Abaqus/CAE begins. See “Customizing Abaqus/CAE startup,” Section 4.3.3 of the Abaqus Installation and Licensing Guide, for examples of this function. Co-simulation parameters The following environment file variables provide default settings for co-simulation between solvers using the direct coupling interface. This includes Abaqus/Standard to Abaqus/Explicit co-simulation and co-simulation between Abaqus and certain third-party analysis programs. cosimulation_port Set cosimulation_port equal to the port number used for the connection. The default value is 48000. cosimulation_timeout Set cosimulation_timeout equal to the timeout period in seconds. Abaqus terminates if it does not receive any communication from the coupled analysis program during the time specified. The default value is 3600 seconds. The following environment file variables provide settings that allow you to allocate CPUs This includes and Abaqus/CFD and Abaqus/CFD for co-simulation jobs submitted using the co-simulation execution procedure. Abaqus/Standard to Abaqus/Explicit, Abaqus/Standard to Abaqus/CFD, to Abaqus/Explicit co-simulation . cpus_weight_std This option controls the allocation of CPUs to Abaqus/Standard analyses. The actual CPU allocation for Abaqus/Standard analyses is made in proportion to this value and considering the settings of cpus_weight_xpl, cpus_weight_cfd, and cpus. cpus_weight_xpl This option controls the allocation of CPUs to Abaqus/Explicit analyses. The actual CPU allocation for Abaqus/Explicit analyses is made in proportion to this value and considering the settings of cpus_weight_std, cpus_weight_cfd, and cpus. cpus_weight_cfd This option controls the allocation of CPUs to Abaqus/CFD analyses. The actual CPU allocation for Abaqus/CFD analyses is made in proportion to this value and considering the settings of cpus_weight_std, cpus_weight_xpl, and cpus. portpool Set this variable equal to a colon-separated pair of TCP/UDP port numbers that represents the start and end value of port numbers to be used by the co-simulation execution procedure when establishing connections between the child processes. Environment file examples Example environment files that use some of the previously discussed parameters are shown below. A sample environment file, named abaqusinc.env, is included in the site subdirectory of the release to show the options used at SIMULIA. UNIX environment file: ask_delete=OFF # The following parameter causes the scratch files to # be written to /tmp. scratch="/tmp" Windows environment file: ask_delete=OFF # The following parameter causes the scratch files to # be written to the tmp directory on c:. scratch="c:/tmp" 3.4 Managing memory and disk resources • “Managing memory and disk use in Abaqus,” Section 3.4.1 3.4.1 MANAGING MEMORY AND DISK USE IN Abaqus Products: Abaqus/Standard Abaqus/Explicit References • “Execution procedure for Abaqus: overview,” Section 3.1.1 • “Using the Abaqus environment settings,” Section 3.3.1 Overview For small analyses management of computer resources is generally of secondary concern, but with large models intelligent use of disk and memory resources is a critical part of the analysis process. For moderate to large analyses you will find it necessary to modify resource management settings. Understanding resource use For Abaqus disk and memory are effectively two similar means of storing data. Data that will be required after an analysis completes must eventually be written to disk; but during an analysis, disk and memory provide functionally equivalent storage mechanisms. Typically disk is a more abundant resource, while memory provides faster access to stored data. Management of Abaqus resources hinges on this simple trade-off. Abaqus data There are effectively two types of data generated by an Abaqus analysis. The first is “output” data that must persist after an analysis is complete. Output data are typically either results that you require for postprocessing or data that are necessary to restart an analysis. As mentioned above, these data must be stored on disk before an analysis completes. In addition, an analysis generates a considerable amount of “scratch” or temporary data. These are data that are needed only while an analysis is running. The scratch data can be subdivided into two groups: performance-critical data and generic data. The performance-critical data are always stored in memory, while the generic data can be stored either in memory or on disk. Requirements and considerations To run an analysis, the following requirements must be satisfied: • There must be sufficient disk space available to hold the requested output data. • There must be sufficient memory available to hold all performance-critical data. • There must be sufficient disk space or memory resource available to hold all generic scratch data. If the above requirements are satisfied, an analysis can be completed; however, for Abaqus/Standard you may find that allowing Abaqus to use additional memory will often improve performance. With the increased availability of computer clusters, dedicated shared memory computers, and most importantly job queuing systems that allocate processors and memory for analyses, it makes most sense to be able to use all the memory resources to improve performance. Typically Abaqus/Standard allocates a large portion of the available system memory on a machine during the analysis phase, but you can manually specify a limit for memory usage with the memory parameter . No scratch data are written to disk during the Abaqus/Explicit analysis phase, since the majority of scratch data are performance critical. Resource management parameters into two classes: memory management and disk Abaqus resource management parameters fall management. Each can be adjusted through one environment file parameter. The following sections explain how to best make use of this parameter. For information about the environment file, see “Using the Abaqus environment settings,” Section 3.3.1. Memory management parameters The memory parameter is used to limit the amount of memory that can be used during the analysis phase of Abaqus/Standard and during the input file processing phase, which is executed before both Abaqus/Standard and Abaqus/Explicit analyses. If you do not define the memory parameter, Abaqus automatically detects the physical memory on the machine and allocates a percentage of this available memory. The default percentages are platform specific, but they typically represent a large portion of the available physical memory. For details on the default memory allocation settings, refer to the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com. You can override the default memory allocation by specifying the percent of physical memory or by specifying an absolute limit in units of megabytes or gigabytes. Percentages are indicated by a “%” sign following the specified limit. Units of megabytes and gigabytes are indicated by “mb” or “gb” following the specified limit. If no units are specified, megabytes are assumed. For example, with any of the following settings: memory="2048 mb" memory="2 gb" memory="25 %" Abaqus uses up to 2 gigabytes of memory on a machine with 8 gigabytes physical memory. The memory setting value must be surrounded by quotes. The values specified for memory must be reasonable for the machine being used. Abaqus/Standard does not check the validity of the numerical values. To be consistent with operating system memory measurement tools, a megabyte is defined by Abaqus to be 1,048,576 bytes, not 1,000,000 bytes. A similar rule applies to the unit of gigabyte. There are no memory management parameters for the Abaqus/Explicit analysis phase, since no scratch data are written to disk during this phase. Environment file parameters can be set for a host, for a user, or for a particular job . Because a default memory setting that works well for one machine with a large amount of memory may not be ideal for another machine that has less memory, it may be useful to vary the default memory settings by machine. Disk management parameters Management of output data is discussed in detail in “Output,” Section 4.1.1. Output data are written to files in the directory from which you launched the job. Abaqus/Standard scratch files are written to a separate scratch directory. You can control the directory used to hold the scratch files with the scratch environment file parameter. Due to the frequent access of the scratch data throughout the analysis phase, ensuring high I/O speed of the scratch disks is essential to the analysis performance. As explained above, no scratch data are written to disk for Abaqus/Explicit, so you have to be concerned only with proper management of output data. Input file processing and data check In general, the amount of memory required during input file processing is not large. The amount of memory and disk space needed for the analysis phase of a job is more likely to be a concern. It is not possible for Abaqus to estimate the amount of memory that will be required to complete input file processing. A data check run can be performed by using the datacheck parameter in the command for running Abaqus to obtain an estimate of the required memory for completing the analysis phase. General guidelines for setting the memory parameter for performing the data check (which includes the input file processing phase) are given below. Guidelines for memory settings You will usually not have to change the default memory setting. If a job fails as a result of insufficient memory with the default setting, you will need to find a machine with more memory to run the job. If you need to override the default behavior by specifying a value for the memory environment file parameter, Table 3.4.1–1 lists some typical data check memory settings for problems of various sizes. The actual values required for memory may vary considerably from problem to problem depending on the features used in a model. Table 3.4.1–1 Typical memory settings for performing the data check analysis. Degrees of freedom Memory 250,000 1 million 2.5 million 5 million 250 megabytes 750 megabytes 1200 megabytes 2000 megabytes Abaqus/Standard analysis Depending on the execution environment and typical job sizes run on the machine, memory can be set by machine or by job. More detailed guidelines are provided in the following section. When setting memory by job is needed, you are advised to run a data check analysis and set memory based on the memory estimates. These estimates are written to the printed output (.dat) file in a table under the heading “MEMORY ESTIMATE.” Two columns in this table are relevant to memory use. The first relevant column is labeled “MINIMUM MEMORY REQUIRED” and specifies the memory setting that is needed to hold critical scratch data in memory. An attempt to run the analysis with memory set below this value will result in a warning, and the job is not likely to run to completion due to the insufficient memory. The second relevant column is labeled “MEMORY TO MINIMIZE I/O” and specifies the memory that is required to hold all scratch data, both critical and generic, in memory. If the memory specified by memory is larger than the “MINIMUM MEMORY REQUIRED,” Abaqus/Standard automatically uses the additional memory up to the memory limit to improve speed of access to generic scratch data that would otherwise be written to disk. When the memory is not enough to hold all the generic scratch data in memory, Abaqus/Standard decides which data should be written to disk and which should be kept in memory based on their relative importance with respect to their effect on the analysis performance. Therefore, the actual disk space used by the scratch data can vary from very close to zero to the “MEMORY TO MINIMIZE I/O” depending on the memory setting. The memory setting can be changed in an analysis continued from a data check without the need of rerunning the analysis input file processor. Guidelines for memory settings The memory parameter allows you to specify the memory limit that can be used by Abaqus during the input file processing and analysis phases. You can specify the setting that should generally be available to Abaqus on a particular machine in the host environment file. Settings can be modified as necessary for individual jobs in job-specific environment files. Reasonable settings for a particular machine depend on the size of the problems being run and how the machine is being used in addition to the physical memory available on the machine. You should be aware of the difference between physical and virtual memory. When virtual memory is used, a machine’s operating system simply uses disk for additional memory. While this can be useful, memory access may require I/O operations that add a considerable performance penalty. Therefore, the guidelines below for managing memory in Abaqus/Standard are always given relative to the physical memory on a machine. Virtual memory should be used only when necessary and with awareness of the associated performance penalty. Setting memory on single-user machines For a single-user machine that is dedicated to running Abaqus/Standard, using the default setting of memory is sensible. If the estimates indicate that the job requires more than this value, the job is too large to run efficiently on this machine. At this point you are urged to move the analysis to another machine with more memory resources. For a single-user machine that is used to run both Abaqus/Standard and other applications If an analysis requires more than the simultaneously, setting a lower memory limit makes sense. specified value, you can decide to increase memory and continue the job. However, Abaqus/Standard will have to contend with the other applications for memory, which will impair the efficiency of both Abaqus/Standard and the other applications. If the other applications are interactive, the performance degradation could be problematic. In such a case you might decide to delay continuing the analysis until the machine can be dedicated to running Abaqus/Standard alone. Setting memory on multi-user machines The guidelines for setting memory on a multi-user machine are very similar to those for single-user machines, except that a judgement must be made as to the amount of memory that each user on the machine can expect to have for a single analysis. A reasonable approach might be to divide the machine’s physical memory by the number of expected simultaneous jobs. Another sensible approach is to divide the machine’s physical memory by the total number of CPUs and then multiply by the number of CPUs used for the current job. If the memory requirement among the simultaneous jobs is not even, you might want to divide the machine’s physical memory in an uneven way accordingly. In general, to ensure acceptable performance, users on multi-user machines need to coordinate with each other to properly set the memory limit. Setting memory when using queues Often queues have an associated memory limit, and determining the appropriate queue for a job requires some judgement. You are advised to run a data check analysis and select a queue based on the estimates provided in the printed output file. However, for large analyses even a data check analysis can require a large amount of memory. Choosing an appropriate queue for a data check analysis requires some experience with particular classes of problems. You may want to submit data check runs initially to queues with very large memory limits to get the necessary estimates. An appropriate queue can then be chosen to actually run the job. If the jobs are to be submitted to shared memory machines, it makes sense to set memory to about 90% of the memory limit for the queue. If the jobs are to be submitted to computer clusters, it is reasonable to use the default memory setting. 3.5 Parallel execution • “Parallel execution: overview,” Section 3.5.1 • “Parallel execution in Abaqus/Standard,” Section 3.5.2 • “Parallel execution in Abaqus/Explicit,” Section 3.5.3 • “Parallel execution in Abaqus/CFD,” Section 3.5.4 3.5.1 PARALLEL EXECUTION: OVERVIEW Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD References • “Obtaining information,” Section 3.2.1 • “Using the Abaqus environment settings,” Section 3.3.1 • “Parallel execution in Abaqus/Standard,” Section 3.5.2 • “Parallel execution in Abaqus/Explicit,” Section 3.5.3 • “Parallel execution in Abaqus/CFD,” Section 3.5.4 Overview Parallel execution of Abaqus is implemented using two different schemes: threads and message passing. Threads are lightweight processes that can perform different tasks simultaneously within the same application. Threads can communicate relatively easily by sharing the same memory pool. Thread-based parallelization is readily available on all shared memory platforms. Parallelization with message passing uses multiple analysis processes that communicate with each other via the Message Passing Interface (MPI). This requires MPI components to be installed. On the command line you can set mp_mode=mpi to indicate that MPI components are available on the system. Alternatively, set mp_mode=MPI in the environment file . The MPI-based implementation is the default on all platforms where it is supported. Abaqus/CFD is implemented using only the MPI mode and does not support threads. The parallel linear solvers used in Abaqus/CFD require that MPI components be installed even for single-processor calculations. Output the local installation notes for your system to learn about local multiprocessing capabilities . From the Support page at www.simulia.com, refer to the System Information page for the current release of Abaqus for complete information about parallel processing support on various platforms, including information about MPI requirements and availability. Parallel processing support for Abaqus features The following Abaqus/Standard features can be executed in parallel: the direct sparse solver, the iterative solver, and element operations. The analysis input preprocessing is not executed in parallel. For Abaqus/Explicit all of the computations other than those involving the analysis input preprocessor and the packager can be executed in parallel. Each of the features that are available for parallel execution has certain limitations, which are documented in detail; see “Parallel execution in Abaqus/Standard,” Section 3.5.2, and “Parallel execution in Abaqus/Explicit,” Section 3.5.3. All features in Abaqus/CFD are available for parallel execution without restrictions. Parallel execution on shared memory computers Abaqus/Standard and Abaqus/Explicit can be executed in parallel on shared memory computers by using threads or the MPI. When the MPI is available, Abaqus runs all available parallel features with MPI- based parallelization and activates thread-based parallel implementations for cases where an equivalent MPI-based implementation does not exist (e.g., direct sparse solver). Abaqus/CFD can also be executed on shared memory computers but only with the MPI. Parallel execution on computer clusters Abaqus can be executed in parallel on computer clusters by using MPI-based parallelization. For parallel execution on computer clusters, the list of machines or hosts is given with the mp_host_list environment file parameter. This parameter also defines the number of processors to be used on each host. Parallel execution using GPGPU hardware The direct solver in Abaqus/Standard can be executed in parallel on computers equipped with compute- capable GPGPU cards. Use with user subroutines User subroutines can be used when running jobs in parallel. However, user subroutines and any subroutines called by them must be thread safe. This precludes the use of common blocks, data statements, and save statements. Calling subroutines that are not thread safe will result in unpredictable behavior of the executable. 3.5.2 PARALLEL EXECUTION IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Obtaining information,” Section 3.2.1 • “Using the Abaqus environment settings,” Section 3.3.1 • “Controlling job parallel execution,” Section 19.8.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Parallel execution in Abaqus/Standard: • reduces run time for large analyses; • is available for shared memory computers and computer clusters for the element operations, direct sparse solver, and iterative linear equation solver; and • can use compute-capable GPGPU hardware on shared memory computers for the direct sparse solver. Parallel equation solution with the default direct sparse solver The direct sparse solver (“Direct linear equation solver,” Section 6.1.5) supports both shared memory computers and computer clusters for parallelization. On shared memory computers or a single node of a computer cluster, thread-based parallelization is used for the direct sparse solver, and high-end graphics cards that support general processing (GPGPUs) can be used to accelerate the solution. On multiple compute nodes of a computer cluster, a hybrid MPI and thread-based parallelization is used. The direct sparse solver cannot be used on multiple compute nodes of a computer cluster if: • the analysis also includes an eigenvalue extraction procedure, or • the analysis requires features for which MPI-based parallel execution of element operations is not supported. In addition, the direct sparse solver cannot be used on multiple nodes of a computer cluster for analyses that include any of the following: • multiple load cases with changing boundary conditions (“Multiple load case analysis,” Section 6.1.4), and • the quasi-Newton nonlinear solution technique (“Convergence criteria for nonlinear problems,” Section 7.2.3). To execute the parallel direct sparse solver on computer clusters, the environment variable mp_host_list must be set to a list of host machines . MPI-based parallelization is used between the machines in the host list. Thread-based parallelization is used within a host machine if more than one processor is available on that machine in the host list and if the model does not contain cavity radiation using parallel decomposition . For example, if the environment file has the following: cpus=8 mp_host_list=[['maple',4],['pine',4]] Abaqus/Standard will use four processors on each host through thread-based parallelization. A total of two MPI processes (equal to the number of hosts) will be run across the host machines so that all eight processors are used by the parallel direct sparse solver. Models containing parallel cavity decomposition use only MPI-based parallelization. Therefore, MPI is used on both shared memory parallel computers and distributed memory compute clusters. The number of processes is equal to the number of CPUs requested during job submission. Element operations are executed in parallel using MPI-based parallelization when parallel cavity decomposition is enabled. Input File Usage: Use the following option in conjunction with the command line input to execute the parallel direct sparse solver: *STEP Enter the following input on the command line: abaqus job=job-name cpus=n For example, the following input will run the job “beam” on two processors: abaqus job=beam cpus=2 Abaqus/CAE Usage: Step module: step editor: Other: Method: Direct Job module: job editor: Parallelization: toggle on Use multiple processors, and specify the number of processors, n GPGPU acceleration of the direct sparse solver The direct sparse solver supports GPGPU acceleration for the symmetric solver; GPGPU acceleration cannot be used with the unsymmetric solver. Input File Usage: Enter the following input on the command line to activate GPGPU direct sparse solver acceleration: Abaqus/CAE Usage: Step module: step editor: Other: Method: Direct abaqus job=job-name gpus=n Job module: job editor: Parallelization: toggle on Use GPGPU acceleration, and specify the number GPGPUs Memory requirements for the parallel direct sparse solver The parallel direct sparse solver processes multiple fronts in parallel in addition to parallelizing the solution of individual fronts. Therefore, the direct parallel solver requires more memory than the serial solver. The memory requirements are not predictable exactly in advance since it is not determined a priori which fronts will actually be processed simultaneously. Equation ordering for minimum solve time Direct sparse solvers require the system of equations to be ordered for minimum floating point operation count. The ordering procedure is performed in parallel when multiple host machines are used on a computer cluster. In a shared memory configuration the ordering procedure is not performed in parallel. The parallel ordering procedure will compute different orders when run on different number of host machines, which will affect the floating point operation count for the direct solver. Parallel ordering can offer performance improvements, particularly for large models using many host machines by significantly reducing the time to compute the order. Parallel ordering may cause performance degradation if the order determined results in a higher floating point operation count for the direct solver. The serial ordering procedure can be used in cases where the variability in the ordering inherent in the parallel ordering procedure is not acceptable. You can deactivate parallel solver ordering from the command line or by using the order_parallel environment file parameter . Input File Usage: Abaqus/CAE Usage: Enter the following input on the command line to deactivate parallel solver ordering: abaqus job=job-name order_parallel=OFF Deactivation of parallel solver ordering is not supported in Abaqus/CAE. Parallel equation solution with the iterative solver The iterative solver (“Iterative linear equation solver,” Section 6.1.6) uses only MPI-based parallelization. Therefore, MPI is used on both shared memory parallel computers and distributed memory compute clusters. To execute the parallel iterative solver, specify the number of CPUs for the job. The number of processes is equal to the number of CPUs requested during job submission. Element operations are executed in parallel using MPI-based parallelization when the parallel iterative solver is used. Input File Usage: Use the following option in conjunction with the command line input to execute the parallel iterative solver: *STEP, SOLVER=ITERATIVE Enter the following input on the command line: abaqus job=job-name cpus=n For example, the following input will run the job “cube” on four processors with the iterative solver: abaqus job=cube cpus=4 Abaqus/CAE Usage: Step module: step editor: Other: Method: Iterative Job module: job editor: Parallelization: toggle on Use multiple processors, and specify the number of processors, n Parallel execution of the element operations in Abaqus/Standard Parallel execution of the element operations is the default on all supported platforms. The command line and environment variable standard_parallel can be used to control the parallel execution of the element operations . operations is used, the solvers also run in parallel automatically. For analysis using the direct sparse solver and not containing parallel cavity decomposition, thread-based parallelization of the element operations is used on shared memory computers and a hybrid MPI and thread parallel scheme is used on computer clusters. For analyses using the iterative solver or if parallel cavity decomposition is enabled, only MPI-based parallelization of element operations is supported. When MPI-based parallelization of element operations is used, element sets are created for each domain and can be inspected in Abaqus/CAE. The sets are named STD_PARTITION_n, where n is the domain number. Parallel execution of the element operations (thread or MPI-based parallelization) is not supported for the following procedures: • eigenvalue buckling prediction (“Eigenvalue buckling prediction,” Section 6.2.3), • natural frequency extraction (“Natural frequency extraction,” Section 6.3.5) that does not use the SIM architecture, • response spectrum analysis (“Response spectrum analysis,” Section 6.3.10), • random response analysis (“Random response analysis,” Section 6.3.11), and • mode-based linear dynamics (“Transient modal dynamic analysis,” Section 6.3.7; “Mode-based steady-state dynamic analysis,” Section 6.3.8; “Subspace-based steady-state dynamic analysis,” Section 6.3.9; and “Complex eigenvalue extraction,” Section 6.3.6) that do not use the SIM architecture. Parallel execution of element operations is available only through MPI-based parallelization for analyses that include any of the following: • static linear perturbation (“General and linear perturbation procedures,” Section 6.1.3), • direct cyclic analysis (“Direct cyclic analysis,” Section 6.2.6), • direct-solution Section 6.3.4), (“Direct-solution steady-state steady-state dynamics dynamic analysis,” • steady-state transport (“Steady-state transport analysis,” Section 6.4.1), • coupled temperature-displacement (“Fully coupled thermal-stress analysis,” Section 6.5.3), • coupled thermal-electrical-structural (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4), • coupled pore fluid diffusion and stress (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1), • crack propagation analysis (“Crack propagation analysis,” Section 11.4.3), and • pressure penetration loading (“Pressure penetration loading,” Section 36.1.7). Analyses using the direct sparse solver and any of the procedures above that support only MPI-based parallelization of element operations can be run on computer clusters. However, only one processor per compute node is used for the element operations since thread-based parallelization is not supported. Parallel execution of element operations is available only through thread-based parallelization for: • cavity radiation analyses where parallel decomposition of the cavity is not allowed and writing of restart data is requested (“Cavity radiation,” Section 40.1.1), and • heat transfer analyses where average-temperature radiation conditions are specified (“Thermal loads,” Section 33.4.4). Finally, parallel execution of the element operations is not supported for analyses that include any of the following: • element matrix output requests (“Element matrix output Section 4.1.1), in Abaqus/Standard” in “Output,” • alternative solution techniques (“Approximate quasi-Newton method except implementation” in “Fully coupled thermal-stress analysis,” Section 6.5.3; “Approximate implementation” in “Coupled thermal-electrical analysis,” Section 6.7.3; and “Specifying the separated method” in “Convergence criteria for nonlinear problems,” Section 7.2.3), the for • continuation of output upon restart (“Continuation of output upon restart” in “Restarting an analysis,” Section 9.1.1), • import from Abaqus/Explicit (“Transferring results between Abaqus analyses: Section 9.2.1), overview,” • substructures (“Substructuring,” Section 10.1), and • adaptive meshing (“Defining ALE adaptive mesh domains in Abaqus/Standard,” Section 12.2.6). Input File Usage: Enter the following input on the command line: Abaqus/CAE Usage: abaqus job=job-name standard_parallel=all cpus=n Control of the parallel execution of the element operations is not supported in Abaqus/CAE. Memory management with parallel execution of the element operations When running parallel execution of the element operations in Abaqus/Standard, specifying the upper limit of the memory that can be used specifies the maximum amount of memory that can be allocated by each process. Transverse shear stress output for stacked continuum shells The output variables CTSHR13 and CTSHR23 are currently not available when running parallel execution of the element operations in Abaqus/Standard. See “Continuum shell element library,” Section 29.6.8. Consistency of results Some physical systems (systems that, for example, undergo buckling, material failure, or delamination) can be highly sensitive to small perturbations. For example, it is well known that the experimentally measured buckling loads and final configurations of a set of seemingly identical cylindrical shells can show significant scatter due to small differences in boundary conditions, loads, initial geometries, etc. When simulating such systems, the physical sensitivities seen in an experiment can be manifested as sensitivities to small numerical differences caused by finite precision effects. Finite precision effects can lead to small numerical differences when running jobs on different numbers of processors. Therefore, when simulating physically sensitive systems, you may see differences in the numerical results (reflecting the differences seen in experiments) between jobs run on different numbers of processors. To obtain consistent simulation results from run to run, the number of processors should be constant. 3.5.3 PARALLEL EXECUTION IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Obtaining information,” Section 3.2.1 • “Using the Abaqus environment settings,” Section 3.3.1 • “Controlling job parallel execution,” Section 19.8.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Parallel execution in Abaqus/Explicit: • reduces run time for analyses that require a large number of increments; • reduces run time for analyses that contain a large number of nodes and elements; • produces analysis results that are independent of the number of processors used for the analysis; • is available for shared memory computers using a thread-based loop level or thread-based domain decomposition implementation; and • is available for both shared memory computers and computer clusters using an MPI-based domain decomposition parallel implementation. Invoking parallel processing Parallelization in Abaqus/Explicit is implemented in two ways: domain level and loop level. The domain-level method breaks the model up into topological domains and assigns each domain to a processor. The domain-level method is the default. The loop-level method parallelizes low-level loops that are responsible for most of the computational cost. The element, node, and contact pair operations account for the majority of the low-level parallelized routines. Parallelization can be invoked by specifying the number of processors to be used. Input File Usage: Enter the following input on the command line: abaqus job=job-name cpus=n For example, the following input will run the job “beam” on two processors: abaqus job=beam cpus=2 Abaqus/CAE Usage: Job module: job editor: Parallelization: toggle on Use multiple processors, and specify the number of processors, n Domain-level parallelization The domain-level method splits the model into a number of topological domains. These domains are referred to as parallel domains to distinguish them from other domains associated with the analysis. The domains are distributed evenly among the available processors. The analysis is then carried out independently in each domain. However, information must be passed between the domains in each increment because the domains share common boundaries. Both MPI and thread-based parallelization modes are supported with the domain-level method. During initialization, the domain-level method divides the model so that the resulting domains take approximately the same amount of computational expense. The load balance is defined as the ratio of the computational expense of all domains in the most expensive process to that of all domains in the least expensive process. For cases exhibiting significant load imbalance, either because the initial load balancing is not adequate (static imbalance) or because imbalance develops over time (dynamic imbalance), the dynamic load balancing technique may be applied . Dynamic load balancing is based on over-decomposition: the user selects a number of domains that is a multiple of the number of processors. During the calculation, Abaqus/Explicit will regularly measure the computational expense and redistribute the domains over the processors so as to minimize the load imbalance. The following functionality is not supported with dynamic load balancing: • Selective subcycling (“Selective subcycling,” Section 11.7.1) • Co-simulation (“Co-simulation,” Section 17.1) • Predefined fields using a results file (“Predefined fields,” Section 33.6.1) The efficiency of the dynamic load balancing scheme depends on the load imbalance inherent to the problem, on the degree of overdecomposition, and on the efficiency of the hardware. Most imbalanced problems will see optimal performance improvement when the number of domains is two to four times the number of processors. The efficiency may be significantly reduced on systems with a slow interconnect, such as Gigabit Ethernet clusters. Best results are obtained when an external interconnect is not needed, such as within a multicore node of a cluster, or on a shared-memory system. Applications most likely to benefit from dynamic load balancing are problems with a strongly time-dependent and/or spatially varying computational load. Examples are models containing airbags, where contact-impact activity is highly localized and time dependent; and coupled Lagrangean-Eulerian problems, where constitutive activity follows the material as it moves through empty space. Element and node sets are created for each domain and can be inspected in Abaqus/CAE. The sets are named domain_n, where n is the domain number. During the analysis, separate state (job-name.abq) and selected results (job-name.sel) files are created. There will be one state and one selected results file for each processor. The naming convention is to append the processor number to the file name. For example, the state files are named job-name.abq.n, where n is the processor number. At the completion of the analysis the individual files are merged automatically into a single file (for example, job-name.abq), and the individual files are deleted. Input File Usage: Enter the following input on the command line: abaqus job=job-name dynamic_load_balancing cpus=n parallel=domain domains=m For example, the following input will run the job “beam” on two processors with the domain-level parallelization method: abaqus job=beam cpus=2 parallel=domain domains=2 The domain-level parallelization method can also be set in the environment file using the environment file parameters parallel=DOMAIN and domains. Job module: job editor: Parallelization: toggle on Use multiple processors and specify the number of processors, n; Number of domains: m; toggle on Activate dynamic load balancing; Parallelization method: Domain You can activate dynamic load balancing when the number of domains is a multiple of the number of processors. Abaqus/CAE Usage: Consistency of results The analysis results are independent of the number of processors used for the analysis. However, the results do depend on the number of parallel domains used during the domain decomposition. Except for cases in which the single- and multiple-domain models are different due to features that are not yet available with multiple parallel domains (discussed below), these differences should be triggered only by finite precision effects. For example, the order of the nodal force assembly may depend on the number of parallel domains, which can result in differences in trailing digits in the computed force. Some physical systems are highly sensitive to small perturbations, so a tiny difference in the force applied in one increment can result in noticeable differences in results in subsequent increments. Simulations involving buckling and other bifurcations tend to be sensitive to small perturbations. To obtain consistent analysis results from run to run, the number of domains used in the domain decomposition should be constant. Increasing the number of domains increases the computational cost slightly; therefore, unless dynamic load balancing is being applied, it is recommended that the number of domains be set equal to the maximum number of processors used for analysis execution for optimal performance. If you do not specify the number of domains, the number defaults to the number of processors. Features that do not allow domain-level parallelization The use of the domain-level parallelization method is not allowed with the following features: • Extreme value output. • Steady-state detection. If these features are included, an error message will be issued. Features that cannot be split across domains Certain features cannot be split across domains. The domain decomposition algorithm automatically takes this into account and forces these features to be contained entirely within one domain. If fewer domains than requested processors are created, Abaqus/Explicit issues an error message. Even if the algorithm succeeds in creating the requested number of domains, the load may be balanced unevenly. If this behavior is not acceptable, the job should be run with the loop-level parallelization method. Adaptive smoothing domains cannot span parallel domain boundaries. The nodes on the boundary between an adaptive smoothing domain and a nonadaptive domain as well as the adaptive nodes on the surface of the adaptive smoothing domain cannot be shared with another parallel domain. To enforce this in a consistent manner when parallel domains are specified, all nodes shared by adjacent adaptive smoothing domains will be set as nonadaptive. In this case the analysis results may be significantly different from that of a serial run with no parallel domains. Set the number of parallel domains to 1, and switch to the loop-level parallelization method if this behavior is undesirable. See “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2, for details. A contact pair cannot be split across parallel domains, but separate contact pairs are not restricted to be in the same parallel domain. A contact pair that uses the kinematic contact algorithm requires that all of the nodes associated with the involved surfaces be within a single parallel domain and not be shared with any other parallel domains. A contact pair that uses the penalty contact algorithm requires that the associated nodes be part of a single parallel domain, but these nodes may also be part of other parallel domains. Analyses in which a large percentage of nodes are involved in contact may not scale well if contact pairs are used, especially with kinematic enforcement of contact constraints. General contact does not limit the domain decomposition boundaries. Nodes involved in kinematic constraints (“Kinematic constraints: overview,” Section 34.1.1) will be within a single parallel domain, and they will not be shared with another parallel domain. However, two kinematic constraints that do not share nodes can be placed within different parallel domains. In some cases beam elements that share a node may be forced into the same parallel domain. This happens only for beams whose center of mass does not coincide with the location of the beam node or for beams with additional inertia . Restart There are certain restrictions for restart when using domain-level parallelization. To ensure that optimal parallel speedup is achieved, the number of processors used for the restart analysis must be chosen so that the number of parallel domains used during the original analysis can be distributed evenly among the processors. Because the domain decomposition is based only on the features specified in the original analysis and steps defined therein, features that affect domain decomposition are restricted from being defined in restart steps only if they would invalidate the original domain decomposition. Because the newly added features will be added to existing domains, there is a potential for load imbalance and a corresponding degradation of parallel performance. The restart analysis requires that the separate state and selected results files created during the original analysis be converted into single files, as described in “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2. This should be done automatically at the conclusion of the original analysis. If the original analysis fails to complete successfully, you must convert the state and selected results files prior to restart. An Abaqus/Explicit analysis packaged to run with a domain-level parallelization technique cannot be restarted or continued with a loop-level parallelization technique. Co-simulation The co-simulation technique (“Co-simulation: overview,” Section 17.1.1) for run-time coupling of Abaqus/Explicit to Abaqus/Standard or to third-party analysis programs can be used with Abaqus/Explicit running either in serial or parallel. Loop-level parallelization The loop-level method parallelizes low-level loops in the code that are responsible for most of the computational cost. The speedup factor using loop-level parallelization may be significantly less than what can be achieved with domain-level parallelization. The speedup factor will vary depending on the features included in the analysis since not all features utilize parallel loops. Examples are the general contact algorithm and kinematic constraints. The loop-level method may scale poorly for more than four processors depending on the analysis. Using multiple parallel domains with this method will degrade parallel performance and, hence, is not recommended. The loop-level method is not supported on the Windows platform. Analysis results for this method do not depend on the number of processors used. Input File Usage: Enter the following input on the command line: abaqus job=job-name cpus=n parallel=loop The loop-level parallelization method can also be set in the environment file using the environment file parameter parallel=LOOP. Job module: job editor: Parallelization: toggle on Use multiple processors, and specify the number of processors, n; Parallelization method: Loop Abaqus/CAE Usage: Restart There are no restrictions on features that can be included in steps defined in a restart analysis when using loop-level parallelization. For performance reasons the number of processors used when restarting must be a factor of the number of processors used in the original analysis. The most common case would be restarting with the same number of processors as used in the original analysis. An Abaqus/Explicit analysis packaged to run with a loop-level parallelization technique cannot be restarted or continued with a domain-level parallelization technique. Measuring parallel performance Parallel performance is measured by comparing the total time required to run on a single processor (serial run) to the total time required to run on multiple processors (parallel run). This ratio is referred to as the speedup factor. The speedup factor will equal the number of processors used for the parallel run in the case of perfect parallelization. Scaling refers to the behavior of the speedup factor as the number of processors is increased. Perfect scaling indicates that the speedup factor increases linearly with the number of processors. For both parallelization methods the speedup factors and scaling behavior are heavily problem dependent. In general, the domain-level method will scale to a larger number of processors and offer the higher speedup factor. Output There are no output restrictions. 3.5.4 PARALLEL EXECUTION IN Abaqus/CFD Products: Abaqus/CFD Abaqus/CAE References • “Obtaining information,” Section 3.2.1 • “Using the Abaqus environment settings,” Section 3.3.1 • “Controlling job parallel execution,” Section 19.8.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Parallel execution in Abaqus/CFD: • reduces run time for analyses that require a large number of increments; • reduces run time for analyses that contain a large number of nodes and elements; • produces analysis results that are independent of the number of processors used for the analysis; and • is available for both shared memory computers and computer clusters using an MPI-based domain decomposition parallel implementation. Invoking parallel processing Abaqus/CFD uses domain-based parallelism implemented with explicit message passing for both shared memory and distributed memory computers. All procedures provided by Abaqus/CFD and their associated features are fully parallel (“Parallel execution: overview,” Section 3.5.1). Parallel execution is invoked by specifying the number of processors to be used. Input File Usage: Enter the following input on the command line: abaqus job=job-name cpus=n For example, the following input will run the job “manifold” on two processors: abaqus job=manifold cpus=2 Abaqus/CAE Usage: Job module: job editor: Parallelization: toggle on Use multiple processors, and specify the number of processors, n Domain-based parallelism Abaqus/CFD uses a domain-decomposition message passing paradigm for its parallel implementation. An element-based decomposition strategy is used that minimizes the number of communications required between subdomains while providing a nearly uniform computational work distribution among the processors. The number of domains maps exactly to the number of user-specified processors for a given calculation. The load-balancing procedures are implemented in parallel as well, so that you can avoid time consuming serial load-balancing procedures at the start of a calculation. Every attempt has been made to ensure that Abaqus/CFD provides scalable parallel solutions for a broad range of applications. All procedures and features in Abaqus/CFD are provided with a fully parallel implementation. All output is serialized automatically for the user so that there is no translation between parallel domains and the original user input. In addition, this permits Abaqus/CFD to restart seamlessly on any number of processors, regardless of how many were used for the original computation. Co-simulation The co-simulation technique (“Co-simulation: overview,” Section 17.1.1) for run-time coupling of Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit can be used with Abaqus/CFD running either in serial or parallel. Restart There are no restrictions on features that can be included in steps defined in a restart analysis. The number of processors used for the restart analysis is not required to be the same as the number of processors used in the original analysis. Output There are no output restrictions. 3.6 File extension definitions • “File extensions used by Abaqus,” Section 3.6.1 3.6.1 FILE EXTENSIONS USED BY Abaqus Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview The abaqus procedure generates several files. Some of these files contain analysis, postprocessing, and translation results and are retained for use by other analysis options, restarting, or postprocessing. This section describes the files that are created and retained by Abaqus. Other files exist only while Abaqus is executing and are deleted when a run completes. These temporary files are generated in the scratch directory. The number and types of temporary files generated depend on the analysis procedures, memory management parameters, and environment settings. Certain file extensions used by Abaqus are also used by other software applications. You must handle any file extension conflicts with other applications. File extensions abq axi bsp c++ cpp State file, only used by Abaqus/Explicit. It is written by the analysis, continue, and recover options. It is read by the convert and recover options. This file is required for restart. Symmetric model data file, only used by Abaqus/Standard. It is written during symmetric model generation by the datacheck and analysis options. Text file containing beam cross-section properties for meshed section profiles. Abaqus/Standard during meshed beam cross-section generation. It is written by User subroutine or other special-purpose C file. User subroutine or other special-purpose C++ file. User subroutine or other special-purpose C++ file. cid com dat fil fin inp ipm lck log Auto-release file, which contains information needed for license recovery and suspension. Command file, created by the Abaqus execution procedure. Printed output file. options. Abaqus/Explicit and Abaqus/CFD do not write analysis results to this file. It is written by the analysis, datacheck, parametercheck, and continue User subroutine or other special-purpose FORTRAN file. Results file. convert=select and convert=all options in Abaqus/Explicit. It is written by the analysis and continue options in Abaqus/Standard and by the Results file created when changing the format of the .fil file using the abaqus ascfil command. files,” It can be in either ASCII or binary format. Section 3.2.11.) The ASCII format is convenient for data transfer between machines that do not have compatible binary data formats. Analysis input file. selected. It is read when the analysis, datacheck, and parametercheck options are Interprocess message file. It is written when an analysis is run from Abaqus/CAE, and it contains a log of all messages sent from Abaqus/Standard, Abaqus/Explicit, or Abaqus/CFD to Abaqus/CAE. Lock file for the output database. This file is written whenever an output database file is opened with write access; it prevents you from having simultaneous write permission to the output database from multiple sources. It is deleted automatically when the output database file is closed or when the analysis that creates it ends. The ask_delete environment file parameter setting will not affect the lock file. Log file, which contains start and end times for modules run by the current Abaqus execution procedure. mdl msg nck odb pac par pes pmg prt Model file, used by Abaqus/Standard and Abaqus/Explicit. It is written by the datacheck option. It is read and can be written by the analysis and continue options in Abaqus/Standard. It is read by the analysis and continue options in Abaqus/Explicit. Multiple model files may exist if the element operations are executed in parallel in an Abaqus/Standard analysis. In such a case a process identifier is attached to the file name. This file is required for restart. Message file. It is written by the analysis, datacheck, and continue options in Abaqus/Standard and Abaqus/Explicit. Multiple message files may exist if the element operations are executed in parallel in an Abaqus/Standard analysis. In such a case a process identifier is attached to the file name. Nickname file used by Abaqus/Standard. It stores a set of internal identifiers for the degrees of freedom in a model. Output database. Abaqus/Explicit, and Abaqus/CFD. (Abaqus/Viewer) and by the convert=odb option. This file is required for restart. It is written by the analysis and continue options in Abaqus/Standard, It is read by the Visualization module in Abaqus/CAE Package file, which contains model information and is used by Abaqus/Explicit only. It is written by the analysis and datacheck options. It is read by the analysis, continue, and recover options. This file is required for restart. Modified version of original parametrized input file showing input parameters and their values. Modified version of original parametrized input file showing input free of parameter information (after input parameter evaluation and substitution has been performed). Parameter evaluation and substitution message file. It is written when the input file is parametrized. Part file, used by Abaqus/Standard and Abaqus/Explicit. This file is used to store part and assembly information and is created even if the input file does not contain an assembly definition. The part file is required for restart, import, sequentially coupled thermal-stress analysis, symmetric model generation, and underwater shock analysis, even if the model is not defined in terms of an assembly of part instances. This file may also be needed for submodeling analysis. psf res sel sim sta stt sup var 023 Python scripting file. You must create this type of file to define a parametric study. Restart file, which contains information necessary to continue a previous analysis and is used by Abaqus/Standard and Abaqus/Explicit. The restart file is written by the analysis, datacheck, and continue options. It is read by any restarted analysis. Selected results file, used by Abaqus/Explicit. It is written by the analysis, continue, and recover options and is read by the convert=select option. This file is required for restart. Linear dynamics data file, used by Abaqus/Standard. It is written during the frequency extraction procedure in SIM-based linear dynamics analyses and is used to store eigenvectors, substructure matrices, and other modal system information. This file is required for restart. Model file, used by Abaqus/CFD. It is written by the datacheck option. It is read and can be written by the analysis and continue options. This file is required for restart. Status file. Abaqus writes increment summaries to this file in the analysis, continue, and recover options. State file. It is written by the datacheck option in Abaqus/Standard and Abaqus/Explicit. It is read and can be written by the analysis and continue options in Abaqus/Standard. It is read by the analysis and continue options in Abaqus/Explicit. Multiple state files may exist if the element operations are executed in parallel in an Abaqus/Standard analysis. In such a case a process identifier is attached to the file name. This file is required for restart. Substructure file, used by Abaqus/Standard. File containing information about the input file variations generated by a parametric study. Communications file, used by Abaqus/Standard and Abaqus/Explicit. It is written by the analysis and datacheck options and is read by the analysis and continue options. 3.7 FORTRAN unit numbers • “FORTRAN unit numbers used by Abaqus,” Section 3.7.1 3.7.1 FORTRAN UNIT NUMBERS USED BY Abaqus Products: Abaqus/Standard Abaqus/Explicit Reference • “Execution procedure for Abaqus: overview,” Section 3.1.1 Overview Abaqus uses the FORTRAN unit numbers outlined in the table below. Unless noted otherwise, you should not try to write to these FORTRAN units from user subroutines. For Abaqus/Standard, you should specify unit numbers 15–18 or unit numbers greater than 100 . For Abaqus/Explicit, specify units 16–18 or unit numbers greater than 100 ending in 5 to 9, e.g. 105, 268, etc. You cannot write to the.sta file. FORTRAN unit numbers Code Unit Number Description Abaqus/Standard 10 12 19–30 73 Internal database Solver file Printed output (.dat) file (You can write output to this file.) Message (.msg) file (You can write output to this file.) Results (.fil) file Internal database Restart (.res) file Internal databases (scratch files). Unit numbers 21 and 22 are always written to disk. Text file containing meshed beam cross-section properties (.bsp) Code Unit Number Description Abaqus/Explicit If domain-parallel 12 13 15 23 60 61 62 63 64 65 67 68 69 70 71 73 80 81 83 ... Printed output (.log) . Restart (.res) file Old restart (.res) file, if applicable Analysis Preprocessor (.dat or .pre) file Communications (.023) file Global package (.pac) file Global state (.abq) file Temporary file Global selected results (.sel) file Message (.msg) file Output database (.odb) file Old package (.pac) file, if import from Abaqus/Explicit Old state (.abq) file, if import from Abaqus/Explicit Internal database; temporary file Local package (.pac.1) file for CPU #1 Local state (.abq.1) file for CPU #1 Local selected results (.sel.1) file for CPU #1 Local package (.pac.2) file for CPU #2 Local state (.abq.2) file for CPU #2 Local selected results (.sel.2) file for CPU #2 Add three files, incrementing units by 10, for each additional CPU • Chapter 4, “Output” Output Output Output variables The postprocessing calculator OUTPUT 4.1 4.2 4.1 Output • “Output,” Section 4.1.1 • “Output to the data and results files,” Section 4.1.2 • “Output to the output database,” Section 4.1.3 • “Error indicator output,” Section 4.1.4 4.1.1 OUTPUT Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Output to the data and results files,” Section 4.1.2 • “Output to the output database,” Section 4.1.3 • “Abaqus/Standard output variable identifiers,” Section 4.2.1 • “Abaqus/Explicit output variable identifiers,” Section 4.2.2 • “Abaqus/CFD output variable identifiers,” Section 4.2.3 • “Diagnostic printing,” Section 14.5.3 of the Abaqus/CAE User’s Manual • “Degree of freedom monitor requests,” Section 14.5.4 of the Abaqus/CAE User’s Manual Overview Abaqus can create the following output files during an analysis: • a data file containing printed output of the model and history definition generated by the analysis input file processor and, in Abaqus/Standard, printed output of results written during the analysis run; • an output database file containing results for postprocessing with the Visualization module of Abaqus/CAE (Abaqus/Viewer) and, in Abaqus/Standard, diagnostic information; • a selected results file in Abaqus/Explicit; • a results file containing results for postprocessing with external software in Abaqus/Standard and Abaqus/Explicit (in Abaqus/Explicit this file is generated by converting the selected results file); • a message file containing diagnostic messages about Abaqus/Explicit; the solution in Abaqus/Standard and • a status file containing information about the status of the analysis and, in Abaqus/Explicit, diagnostic messages and information about the stable time increment; and • output files in Abaqus/CFD using alternate file formats. In Abaqus can create files for restarting an analysis—see “Restarting an analysis,” Section 9.1.1. Abaqus/Standard these files can also be used to extract results output not requested during an analysis. The data file The data file (job-name.dat) is a text file that contains information about the model definition (generated by the analysis input file processor) and, in Abaqus/Standard, tabular output of results. The analysis input file processor information includes the model definition, the history definition, and messages identifying any error and warning conditions that were detected while processing the input data. Controlling the amount of analysis input file processor information written to the data file You can control the amount of information written to the data file by the analysis input file processor in Abaqus/Standard and Abaqus/Explicit. Input File Usage: Use the following option in the model definition section of the input file: Abaqus/CAE Usage: *PREPRINT Job module: job editor: General: Preprocessor Printout Input file echo By default, the input file will not be echoed to the data file. You can choose to activate this printout. If the input file is defined in terms of an assembly of part instances, the echo to the data file will be that of the flattened input file (i.e., one that does not use parts and assemblies). Input File Usage: Abaqus/CAE Usage: *PREPRINT, ECHO=YES or NO Job module: job editor: General: Preprocessor Printout: Print an echo of the input data Input parameter information For parametrized input files, information about input parameters and their values can be printed in the data file. By default, the modified version of the original input file showing this information will not be printed in the data file. You can choose to activate this printout. Input File Usage: Abaqus/CAE Usage: *PREPRINT, PARVALUES=YES or NO Parametrized input files are not supported in Abaqus/CAE. Parameter-free input file information For parametrized input files, a parameter-free version (after parameter evaluation and substitution) of the original input file can be printed in the data file. By default, this modified version of the input file will not be printed in the data file. You can choose to activate this printout. Input File Usage: Abaqus/CAE Usage: *PREPRINT, PARSUBSTITUTION=YES or NO Parametrized input files are not supported in Abaqus/CAE. Model and history definition summaries By default, the options defining the model and history data will not be summarized in the data file. You can choose to activate this printout. For an Abaqus/Explicit analysis the model summary data, when requested, includes the mass, center of mass, and the rotary inertia information for the element sets in the model and for the whole model. However, for two-dimensional models the reported rotary inertia includes the component corresponding to the only active rotation degree of freedom; the remaining components are not included. Input File Usage: *PREPRINT, MODEL=YES or NO, HISTORY=YES or NO Abaqus/CAE Usage: Job module: job editor: General: Preprocessor Printout: Print model definition data and Print history data Contact constraint information In Abaqus/Standard you can choose to activate printout of detailed information about the contact constraints generated by the contact pair definition data. Input File Usage: Abaqus/CAE Usage: *PREPRINT, CONTACT=YES or NO Job module: job editor: General: Preprocessor Printout: Print contact constraint data Mass information In Abaqus/Explicit you can choose to activate printout of detailed information about the mass property of each user-defined element set. Input File Usage: Abaqus/CAE Usage: *PREPRINT, MASS PROPERTY=YES or NO This parameter is not supported by Abaqus/CAE. Requesting printed results In Abaqus/Standard the values of output variables can be printed to the data file in tabular format throughout the analysis. You can control the following types of printed output during the analysis run: element output, node output, contact surface output, energy output, fastener interaction output, modal output, section output, and radiation output—see “Output to the data and results files,” Section 4.1.2, and “Cavity radiation,” Section 40.1.1. You specify the variables to be printed in each output table and, for element variables, the locations at which they are to be printed (at the integration points, at the element centroid, at the nodes, or averaged at the nodes). Nodal variables at nodes with transformations can be written in either the global or the local coordinate system . The list of available variables is given in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Output of results to the data file is requested as part of a step definition. Viewing part and assembly information in the data file An Abaqus model can be defined in terms of an assembly of part instances . In such a model node and element numbers can be repeated within the definitions of different parts. These local numbers are converted internally by Abaqus to unique global numbers, and the output written to the data file is given in terms of those internal numbers. A map between user-defined numbers and internal numbers is printed to the data file (after the step data) if any output that includes node and element numbers is requested in the data file. Set and surface names that appear in the data file are prefixed by the assembly and part instance names, separated by underscores (Assembly_Part1–1_setname, for example). Local coordinate systems defined within a part or part instance are translated and rotated according to the positioning data given in the part instance definition. The output database The Abaqus output database (job-name.odb) is a neutral binary file used to store model information and analysis results in terms of an assembly of part instances. The Visualization module of Abaqus/CAE (Abaqus/Viewer) uses the output database for postprocessing analysis results and viewing diagnostic information. Requesting output to the output database You choose the variables to be written to the output database from the lists in “Abaqus/Standard output variable identifiers,” Section 4.2.1, “Abaqus/Explicit output variable identifiers,” Section 4.2.2, and “Abaqus/CFD output variable identifiers,” Section 4.2.3. The following types of output are available: element output, node output, contact surface output, energy output, integrated output, time incrementation output, fastener interaction output, modal output, and radiation output. In addition, a subset of the diagnostic information that is written to the message file in Abaqus/Standard and Abaqus/Explicit and to the Abaqus/Explicit status file is included in the output database. See “Output to the output database,” Section 4.1.3, for a detailed explanation of how to generate output database requests. Three types of information are stored in the output database: “field” output, “history” output, and diagnostic information. Field output is intended to be relatively infrequent output for a large portion of the model. Abaqus/CAE uses field output to generate contour plots, displaced shape plots, symbol plots, and X–Y plots in the Visualization module. History output is intended to be output for a small portion of the model requested at a fairly high frequency. Abaqus/CAE uses history output to generate X–Y plots in the Visualization module. See “Output to the output database,” Section 4.1.3, for detailed descriptions of field and history output. Diagnostic information is intended to provide convergence information for use in Abaqus/CAE; for more information, see Chapter 41, “Viewing diagnostic output,” of the Abaqus/CAE User’s Manual. Format of the output database The output database is a neutral binary, platform-independent file. Unlike the restart or binary results files, it can be copied directly from one computing platform to another without translation. By default, floating point data are written to the output database file in single precision. You can choose to write floating point nodal field output data to the output database file in double precision; see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2, for details. You can open an output database file from an older release of Abaqus in Abaqus/CAE, with the exception that Abaqus 5.8 output database files cannot be opened in Version 6. Output database files from previous releases of Abaqus must be converted to the current release when they are opened. If you are using an older release of Abaqus/CAE, you cannot open an output database file created from a newer release of Abaqus. The selected results file The Abaqus/Explicit selected results file (job-name.sel) stores user-selected results, which are converted into the results file (job-name.fil) for postprocessing by other commercial postprocessing packages. Element output, node output, and energy output can be requested ; the variables available for output are listed in “Abaqus/Explicit output variable identifiers,” Section 4.2.2. You can write a user-selected subset of the results for a given node set or element set at more frequent intervals than the restart intervals. You specify the output requests within a step definition, which allows you to be selective about the amount of data written to the selected results file to avoid using excessive disk storage. For example, when dealing with a very large model, you may choose to write only the current displacements and the equivalent plastic strain for the entire model 20 times in the step and to write the acceleration history at one node 200 times in the step. The results file The Abaqus results file in Abaqus/Standard and Abaqus/Explicit (job-name.fil) can be read by external postprocessors to produce X–Y plots or printed tabular output. Most commercial finite element results-display packages provide translators that use the Abaqus results file as their input. The results file can also be used as a convenient medium for importing analysis results into your own postprocessing program. “Accessing the results file information,” Section 5.1.3, provides details on how to read this file. Results file output of temperature from a heat transfer, thermal-electrical, or thermal-electrical- structural analysis can be used as input to a stress analysis of the same mesh . Obtaining results file output in Abaqus/Standard In Abaqus/Standard you choose the variables to be written to the results file from the lists in “Abaqus/Standard output variable identifiers,” Section 4.2.1, in a manner similar to that for output printed to the data file. You must specifically request that values be written to the results file or none will be provided. Element output, node output, contact surface output, energy output, modal output, and radiation output are available—see “Output to the data and results files,” Section 4.1.2, and “Cavity radiation,” Section 40.1.1, for details. Obtaining results at the beginning of a step You can request that the solution state at the beginning of a step (the zero increment) be written to the Abaqus/Standard results file. Zero-increment file output is available only for steps in which the concept of time governs the incrementation scheme of the selected procedure and, hence, the following procedures are excluded: • Linear static perturbation analysis (“Static stress analysis,” Section 6.2.2) • “Eigenvalue buckling prediction,” Section 6.2.3 • “Natural frequency extraction,” Section 6.3.5 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 • “Response spectrum analysis,” Section 6.3.10 • “Random response analysis,” Section 6.3.11 If you request zero-increment results file output, it will be generated for all valid procedures in a given analysis. You must request zero-increment results file output to generate a zero-increment results file in a data check analysis . It is strongly recommended that you request zero-increment results file output if the results file is used to drive a submodel; see “Node-based submodeling,” Section 10.2.2, for further discussion. *FILE FORMAT, ZERO INCREMENT Input File Usage: The *FILE FORMAT option can be given as model data or as history data, but it can appear only once in the input file. Abaqus/CAE Usage: Results file output cannot be requested in Abaqus/CAE. Obtaining results file output in Abaqus/Explicit The Abaqus/Explicit results file is a sequential access file generated from the selected results file . The results file contains the requested results in the format described in “Results file output format,” Section 5.1.2. Input File Usage: Use either of the following command line options to convert a selected results file to a results file: abaqus job=job-name convert=select Abaqus/CAE Usage: abaqus job=job-name convert=all The selected results file cannot be converted in Abaqus/CAE. Part and assembly information An Abaqus model can be defined in terms of an assembly of part instances . However, the results file does not contain part and assembly records. In a model defined in terms of an assembly of part instances, node and element numbers can be repeated within the definitions of different parts. These local numbers are converted internally by Abaqus to unique global numbers, and the output written to the results file is given in terms of the global (internal) numbers. A map between user-defined numbers and internal numbers is printed to the data file if any results file output that includes node and element numbers is requested. Set and surface names that appear in the results file are prefixed by the assembly and part instance names, separated by underscores (Assembly_Part1–1_setname, for example). Local coordinate systems defined within a part or part instance are translated and rotated according to the positioning data given in the part instance definition. Format of the results file The Abaqus results file in Abaqus/Standard or Abaqus/Explicit is organized as a sequential file, in binary or in ASCII format. ASCII format is necessary if the file is to be read on a computer system that is different from the one on which the file was written. ASCII format allows the results file to be transferred between different computer systems without having to translate binary data. ASCII format is not needed if the file will always be used on the same system or on systems that use the same binary format. If the results file output will always reside on the same computer, the default binary format is usually the most efficient way of storing the file. For large problems a file in ASCII format will be significantly larger than the same file in binary format. Controlling the format of the results file in Abaqus/Standard Abaqus/Standard can write the results file in either binary or ASCII format. The default format is binary. The results file output must be written in the same format for the entire analysis. The format cannot be changed upon restarting the problem. The format of the Abaqus/Standard results file can also be controlled in the Abaqus/Standard environment file . The format specified in an analysis supersedes the value defined in the enviroment file. In addition, the ascfil facility in the Abaqus execution procedure (“ASCII translation of results (.fil) files,” Section 3.2.11) can be used to convert a binary Abaqus/Standard results file (job-name.fil) to ASCII format (job-name.fin) after the analysis completes. Input File Usage: *FILE FORMAT, ASCII The *FILE FORMAT option can be given as model data or as history data, but it can appear only once in the input file. Abaqus/CAE Usage: Results file output cannot be requested in Abaqus/CAE. Controlling the format of the results file in Abaqus/Explicit Abaqus/Explicit always writes the results file output in binary format during file conversion, but the binary Abaqus/Explicit results file can be converted to ASCII format using the ascfil facility (“ASCII translation of results (.fil) files,” Section 3.2.11). ASCII format “Results file output format,” Section 5.1.2, defines the contents of the records that are written to the results file; these descriptions also hold if the results file is written in ASCII format. All the data items in these files are either integers, floating point numbers, or character strings. When ASCII format is requested, each data item is translated into an equivalent character string before it is written to the file. These strings are written in 80-character logical records in the order described in the record definitions. Each 80-character logical record is completely filled before the next one is started, so that any data item can be split, with some of the characters that define the item in one logical record and the remainder in the next. Each data item usually follows immediately behind its predecessor. The exception is that for results file record key 2001 Abaqus will fill out the logical record with blank characters, so that the record can be written immediately to the physical storage medium. Abaqus then inserts a logical record consisting of 80 blanks, which allows the end-of-file to be handled correctly. The beginning of each “record” is indicated by an asterisk (*). Each floating point number begins with the character D, followed by the number in the format E22.15 or D22.15, depending on whether the release of Abaqus that wrote the results file used single precision or double precision. Each character string begins with the character A, followed by eight characters (if the character string has fewer than eight characters, the right part of the string is blank; character strings longer than eight characters are written eight characters at a time). Each integer begins with the character I, followed by a two digit integer giving the number of decimal digits in the integer, followed by the integer itself (written as decimal digits). For example, record key 1900 for an S4R element with element number 5 and nodes 195, 198, 205, and 204 would be written *I 18I 41900I 15AS4R I 3195I 3198I 3205I 3204 and record key 101 for node 135 and 6 degrees of freedom would be written *I 19I 3101I 3135D1.280271914214298E-10D1.500000000000036E+00 D-1.074629835784448E-46D 6.983222716550941E-12 D-4.084928798492785E-13D-1.072688441364597E-10 Precision of floating point data in the results file The precision of floating point data written to the results file depends on the precision of the executable thus, floating point data that generates the data. Abaqus/Standard always uses double precision; are always written to the Abaqus/Standard results file in double precision. Abaqus/Explicit can be run in single or double precision on most machines; see “Defining an analysis,” Section 6.1.2, for details on the precision level of the Abaqus/Explicit executable. If the double precision executable for Abaqus/Explicit is used, floating point data are written to the Abaqus/Explicit results file in double precision; likewise, if the single precision executable for Abaqus/Explicit is used, floating point data are written to the Abaqus/Explicit results file in single precision. Maximizing the efficiency of the results file In Abaqus/Standard each element output request (a collection of identifying keys entered on a single line) is preceded by an “element header” record . Hence, the size of the results file can be minimized by entering all element output variables of the same “type” (element integration point variable, element section variable, whole element variable, etc.) on a single line. Consolidating output variable entries is encouraged, since it will reduce the size of the results file. Example For example, the following output requests can be used to request output of element variables in the results file in a stress/displacement analysis: *EL FILE S, SINV, E, PE, CE, EE, ENER, TEMP, FV, COORD SF, SE LOADS, ELEN, EVOL *EL FILE, REBAR S, SINV, E, PE, CE, EE, RBFOR, RBANG SF, SE LOADS, ELEN (The output requests for rebar quantities need not be the same as the underlying element output requests.) The message file in Abaqus/Standard and Abaqus/Explicit The message file (job-name.msg) is a text file that contains diagnostic messages about the progress of the solution. The Abaqus/Standard message file In Abaqus/Standard the message file contains diagnostic or informative messages about the progress If any of these messages describe errors or warnings, the number of such errors or of the solution. warnings is also given at the end of the data file. The message file is written automatically during an Abaqus/Standard analysis. The Abaqus/Standard message file contains information about the increment number, step time, fraction of a step completed, equilibrium iterations, severe discontinuity (contact) iterations, plasticity algorithms, adaptive mesh smoothing, the load proportionality factor in a Riks analysis, etc. A portion of the diagnostic information in the message file is also written to the output database for use in Abaqus/CAE (for more information, see “Requesting diagnostic information in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3). You can control the amount of information written to the message file for each step. This feature is sometimes helpful in difficult analyses since it allows detailed diagnostic information to be written about certain events (such as contact) during a nonlinear solution; this information can often be useful in developing a strategy for the solution of highly nonlinear problems. Input File Usage: *PRINT The *PRINT option can appear only once within a step definition. Abaqus/CAE Usage: Step module: Output→Diagnostic Print Controlling the frequency of output to the message file You can control the frequency at which information is printed to the message file by specifying the desired output frequency in increments. The default output frequency is 1 (or 10 in a direct cyclic or a low-cycle fatigue analysis). The output will always be printed at the last increment of each step unless you specify a frequency of zero to suppress the output. Input File Usage: Abaqus/CAE Usage: *PRINT, FREQUENCY=N Step module: Output→Diagnostic Print: Frequency N Requesting detailed contact printout You can obtain a detailed printout of contact conditions during iteration. This information about which points are contacting or separating in interface and gap problems is useful in tracking the development of the solution in difficult contact problems. The details are written for every severe discontinuity iteration. By default, the detailed contact output is suppressed. Input File Usage: Abaqus/CAE Usage: *PRINT, CONTACT=YES or NO Step module: Output→Diagnostic Print: toggle on Contact Requesting detailed model change printout You can obtain a detailed printout of model change operations (removal and reactivation) at the start of a step. This information includes the new original coordinates and normals of elements being reactivated strain free in a large-displacement analysis. By default, the detailed model change output is suppressed. See “Element and contact pair removal and reactivation,” Section 11.2.1, for details on model change operations. Input File Usage: Abaqus/CAE Usage: *PRINT, MODEL CHANGE=YES or NO Step module: Output→Diagnostic Print: toggle on Model Change Requesting detailed printout of problems with the plasticity algorithms You can activate printout of element and integration point numbers for which the plasticity algorithms have failed to converge during an iteration. This information is useful for finding the place in the mesh and/or the plasticity model at which Abaqus is encountering material model difficulties. Modeling problems and material parameter specification problems can be identified using this detailed printout. By default, this printout is suppressed. Input File Usage: Abaqus/CAE Usage: *PRINT, PLASTICITY=YES or NO Step module: Output→Diagnostic Print: toggle on Plasticity Requesting output of equilibrium residuals By default, equilibrium residuals during equilibrium iterations are output. You can choose to suppress this output entirely, but it is not recommended; without the output of equilibrium residuals, you cannot see the accuracy of the iteration process. Input File Usage: Abaqus/CAE Usage: *PRINT, RESIDUAL=YES or NO Step module: Output→Diagnostic Print: toggle on Residual Requesting solver information By default, information about the number of equations being solved and the required memory for each iteration is output. You can request that output be suppressed. Input File Usage: Abaqus/CAE Usage: *PRINT, SOLVE=YES or NO Step module: Output→Diagnostic Print: toggle on Solve Requesting detailed adaptive mesh smoothing printout You can activate detailed printout of adaptive mesh smoothing in Abaqus/Standard. The output includes information about the magnitude of the maximum displacement and the node and degree of freedom where the maximum displacement increment occurs during each mesh sweep. It also provides the node numbers at which geometric feature changes occur. By default, only a summary is output. Input File Usage: Abaqus/CAE Usage: *PRINT, ADAPTIVE MESH=YES or NO Adaptive mesh output to the message file is not supported in Abaqus/CAE. Monitoring a degree of freedom in the message file You can write the current value of a specified point and degree of freedom to the message file. This information can be used to monitor the progress of the solution. The information will also be written in the status file . You can control the frequency at which the value is printed in the message file. The default frequency is 1 (or 10 in a direct cyclic analysis). Degree of freedom monitoring does not apply to eigenvalue buckling prediction, eigenfrequency extraction, or response spectrum procedures. For other linear perturbation procedures output for the monitored degree of freedom is the base state value. Input File Usage: *MONITOR, NODE=node_number, DOF=dof, FREQUENCY=N Abaqus/CAE Usage: The node and degree of freedom being monitored can be changed from step to step by repeating the *MONITOR option. The node and degree of freedom specified in the last occurrence of this option in a step will be used for that step. Step module: Output→DOF Monitor: Monitor a degree of freedom throughout the analysis, click Edit to select the point, Degree of freedom: dof, Print to the message file every N increments In Abaqus/CAE only one point and degree of freedom can be monitored for an analysis; you cannot change the monitor request from step to step. The Abaqus/Explicit message file In Abaqus/Explicit the message file contains messages if potential problems are detected during an analysis. You can control the output of diagnostic messages for each step . A portion of the diagnostic information in the message file is also written to the output database for use in Abaqus/CAE (for more information, see “Requesting diagnostic information in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3). The status file The status file (job-name.sta) is a text file that contains information about the progress of an analysis. The Abaqus/Standard or Abaqus/CFD status file The Abaqus/Standard or Abaqus/CFD status file contains a single 80-character record for each increment and is updated upon completion of each increment of an analysis. This record is written directly to secondary storage immediately at the completion of the increment. Therefore, the status file can be examined as the analysis job is executing, thus providing a monitor of the progress of the analysis. Other than specifying that a degree-of-freedom variable be monitored in the status file in Abaqus/Standard (as described below), the information written to the Abaqus/Standard or Abaqus/CFD status file cannot be controlled. The Abaqus/Explicit status file In Abaqus/Explicit the status file (job-name.sta) contains, by default, mass and inertial properties for the model, initial stable time increment information, a synopsis of the progress of the analysis including total accumulated CPU usage and the current time increment size, and an estimate of the memory required to process each step. You can control additional output including the total kinetic energy, the energy balance, the identifiers of the elements with the smallest stable time increments, and the percent change in total mass of the model due to mass scaling. The frequency at which summary increments are written to the Abaqus/Explicit status file depends on the duration of the analysis in CPU minutes and the amount of output specified in the analysis. The following list provides general guidelines for when a summary increment will be written to the status file. Summary information will generally be written: • Each time restart information, field output to the output database, or results file output is written. • Once per increment if the problem requires fewer than 20 increments. • 20 times during the step for a short analysis (less than 40 CPU minutes). • Every 2 CPU minutes for an analysis longer than 40 CPU minutes. A degree-of-freedom variable can be monitored in the status file while the analysis is running. You can also write additional diagnostic information to the status file . A portion of the diagnostic information in the status file, including information for each summary increment, is also written to the output database for use in Abaqus/CAE (for more information, see “Requesting diagnostic information in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3). Errors that can be detected only while packaging the data for Abaqus/Explicit or during analysis are also written to the status file. Input File Usage: *PRINT Abaqus/CAE Usage: The *PRINT option can appear only once within a step definition. Step module: Output→Diagnostic Print Requesting kinetic energy output By default, the kinetic energy for the model is written to the status file. This output is written periodically throughout the step. You can choose to include or exclude the kinetic energy output for each step. Input File Usage: Abaqus/CAE Usage: *PRINT, ALLKE=YES or NO Step module: Output→Diagnostic Print: toggle on Allke Requesting total energy output By default, the energy balance is written periodically throughout the step. You can choose to include or exclude the energy balance output for each step. Input File Usage: Abaqus/CAE Usage: *PRINT, ETOTAL=YES or NO Step module: Output→Diagnostic Print: toggle on Etotal Requesting output of the critical element By default, the number of the element with the current minimum stable time increment and its value are output to the status file. This output is written periodically throughout the step. You can choose to include or exclude the critical element output for each step. Input File Usage: Abaqus/CAE Usage: *PRINT, CRITICAL ELEMENT=YES or NO Step module: Output→Diagnostic Print: toggle on Crit. Elem. Requesting output of the change in the total mass You can write the percent change in total mass of the model due to mass scaling to the status file for each step. This output is written periodically throughout the step. The percent change in total mass is printed by default only if mass scaling is present in the model. Input File Usage: Abaqus/CAE Usage: *PRINT, DMASS=YES or NO Step module: Output→Diagnostic Print: toggle on Dmass Monitoring a degree of freedom in the status file You can write the current value of a specified point and degree of freedom to the Abaqus/Standard status file. The value of the point and degree of freedom being monitored will appear in the status file for every increment written during the analysis. When a degree of freedom is monitored in the Abaqus/Standard status file, the same information is written to the message file , but the specified frequency has no effect on the output to the status file. Degree of freedom monitoring does not apply to eigenvalue buckling prediction, eigenfrequency extraction, or response spectrum procedures. For other linear perturbation procedures output for the monitored degree of freedom is the base state value. Input File Usage: *MONITOR, NODE=node_number, DOF=dof The node and degree of freedom being monitored can be changed from step to step by repeating the *MONITOR option. The node and degree of freedom specified in the last occurrence of this option in a step will be used for that step. Abaqus/CAE Usage: Step module: Output→DOF Monitor: Monitor a degree of freedom throughout the analysis, click Edit to select the point, Degree of freedom: dof In Abaqus/CAE only one point and degree of freedom can be monitored for an analysis; you cannot change the monitor request from step to step. Alternate output formats in Abaqus/CFD By default, when you request output in Abaqus/CFD, the output is sent to the output database file. However, you have the option of selecting alternate file formats for field and history output. Field output can be sent to files in EXODUS-II format; history output can be sent to files in comma-separated values (CSV) format. You request the field and history output in the same manner as described in “Requesting output to the output database.” To select an alternate output format, you set the field and history options on the command line when you run an Abaqus/CFD analysis. For more information, see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2. Field output in EXODUS-II format The EXODUS-II format is widely supported by third-party postprocessors for both computational solid mechanics and computational fluid dynamics. This format is binary, machine independent, and well suited for transient simulation results on unstructured grids. The EXODUS-II format and associated EXODUS-II/NEMESIS programming API for reading and writing were developed at Sandia National Laboratories. This open source software is available under the BSD License. The source code and documentation can be found at http://sourceforge.net/projects/exodusii. The EXODUS-II format cannot natively represent all of the Abaqus/CFD output features. The features listed in Table 4.1.1–1 cannot be represented directly and are either omitted or modified. Table 4.1.1–1 Abaqus/CFD output feature representation in EXODUS-II format. Feature Comment Parts and assemblies Element sets Amplitudes Node and element numbers do not include the part instance name and are numbered sequentially General element sets are not supported and are omitted Not supported The EXODUS-II format uses file extension exo. For parallel processing of an analysis run, EXODUS-II output is directed to multiple files (one file per processor is created), which is useful for some third-party postprocessors. The files are named job.exo.rank, where rank is a number ranging from 0 to one less than the number of CPUs. In contrast, you can write field output for parallel execution to a single file (job.exo); the file is written in EXODUS-II format using the NEMESIS library. Input File Usage: Abaqus/CAE Usage: Use the following command line option in Abaqus/CFD to write field output in EXODUS-II format to one file per processor: abaqus job=job-name field=exodus Use the following command line option in Abaqus/CFD to write field output in EXODUS-II format to a single file for parallel execution: abaqus job=job-name field=nemesis You cannot select an alternate format for field output in Abaqus/CAE. History output in CSV format The comma-separated values (CSV) format is a text-based output format. The format of the CSV text file consists of one or more comment lines followed by one line of comma-separated data per history output frame. Comments in the CSV file begin with the character #. Each column in the CSV file has a comment that describes the mesh location, the part instance, and the output request label. Possible values for mesh locations are node, element, or surface. Vector output requests also include the component; i.e., 1, 2, or 3. This format uses file extension csv. History output in the CSV format creates one file per output request label per step. Additional files are created if the job is run in parallel and the set associated with the history output request is split between processors due to the domain decomposition. In this case there will be one file per processor on which the set is present. The files are named job_output- request_rank_step-number.csv, where rank is a number ranging from 0 to one less than the number of CPUs. Input File Usage: Abaqus/CAE Usage: Use the following command line option to write history output to an alternate file format in Abaqus/CFD: abaqus job=job-name history=csv You cannot select an alternate format for history output in Abaqus/CAE. Requesting output in multiple steps In general, output requests apply to the step in which they are given and to all subsequent steps until they are respecified. However, output specifications for linear perturbation steps (available only in Abaqus/Standard; see below and “General and linear perturbation procedures,” Section 6.1.3) are treated independently of output requests for general analysis steps and apply only to a continuous sequence of linear perturbation steps. Database output, printed output, and results file output are independent output modes in Abaqus; therefore, changing the specification for one form of output does not affect the other forms. General analysis steps The default output requests are used in the first general analysis step of an analysis unless you redefine them. For subsequent general analysis steps, the definition of each form of output from the previous general step is maintained unless you redefine it. Linear perturbation steps The default output requests are used in the first of any sequence of linear perturbation steps unless they are redefined in that step. If a subsequent linear perturbation step is defined without an intermediate general analysis step, the definition of each mode of output from the previous perturbation step is maintained unless you redefine it. If an intermediate general step is defined, the default output requests are again used in the linear perturbation step unless they are redefined in that step. Element matrix output in Abaqus/Standard In Abaqus/Standard you can write element stiffness matrices and, if available, mass matrices for each step to a file. For heat transfer elements the operator matrices are written if stiffness matrix output is requested. Element matrix output is available only for elements without internal nodes (unless those nodes have no active degrees of freedom) and with no acoustic or internal degrees of freedom. Examples of elements for which element matrix output is prohibited include acoustic, pipe, elbow, frame, gap, and interface elements as well as axisymmetric elements with Fourier modes. Element matrix output is not available for elements with coupled fields such as coupled temperature-displacement elements and pore pressure elements. For incompatible mode and hybrid elements, stiffness matrix output is prohibited while mass matrix output is available. A substructure matrix output request is used to write a substructure’s reduced stiffness matrix, mass matrix, and load case vectors to a file . Element matrix output cannot be requested in a mode-based dynamic analysis (response spectrum, steady-state dynamic, modal dynamic, or random response). However, it can be requested in the eigenfrequency extraction analysis that precedes the mode-based dynamic analysis to output the mass and stiffness matrices. The element matrices are written without the effects of nodal conditions; therefore, boundary conditions, concentrated loads, and the effects of multi-point constraints are not included in this output. The degrees of freedom are always in the global directions, even if a local coordinate system (“Transformed coordinate systems,” Section 2.1.5) has been defined at nodes associated with the element. You must select the element set for which output is requested. For models defined in terms of an assembly of part instances (“Defining an assembly,” Section 2.10.1), element numbers written with element matrix output are internal numbers generated by Abaqus/Standard. A map between internal numbers and the original element numbers and part instance names is provided in the data file. Writing the element matrices to the results file By default, element matrix output records are written to the Abaqus/Standard results file. The record formats for the results file are described in “Results file output format,” Section 5.1.2. The file can be written in binary or ASCII format based on the file format you specify . Input File Usage: Abaqus/CAE Usage: *ELEMENT MATRIX OUTPUT, ELSET=element_set, OUTPUT FILE=RESULTS FILE Element matrix output is not supported in Abaqus/CAE. Writing the element matrices to a user-defined file You can write the element matrices to a user-defined file. The file name should not include an extension; the extension .mtx will be added. The format of the output file is compatible with the linear user element . Input File Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, OUTPUT FILE=USER DEFINED, FILE NAME=output_file_name Abaqus/CAE Usage: Element matrix output is not supported in Abaqus/CAE. Writing the element matrices to the data file You can write the element matrix records to the Abaqus/Standard data file. *ELEMENT MATRIX OUTPUT, ELSET=elset, OUTPUT FILE=USER DEFINED Input File Usage: Abaqus/CAE Usage: Element matrix output is not supported in Abaqus/CAE. Including distributed loads You can choose to write the load vector from distributed loads on the elements. By default, the load vector is not written. Input File Usage: Abaqus/CAE Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, DLOAD=YES or NO Element matrix output is not supported in Abaqus/CAE. Controlling the frequency of element matrix output You can control the frequency at which element matrix output will be written by specifying an output frequency in increments. By default, the element matrices will be output every increment (equivalent to an output frequency of 1). Specify an output frequency of 0 to suppress output of the element matrices. Unless the output is suppressed, the matrices will always be written at the last increment of a step. Input File Usage: Abaqus/CAE Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, FREQUENCY=N Element matrix output is not supported in Abaqus/CAE. Writing the stiffness or operator matrix You can choose to output the stiffness matrix (or operator matrix in heat transfer elements). By default, the stiffness (operator) matrix is not output. Input File Usage: Abaqus/CAE Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, STIFFNESS=YES or NO Element matrix output is not supported in Abaqus/CAE. Writing the mass matrix You can choose to output the mass matrix. By default, element mass matrices are not output. Input File Usage: Abaqus/CAE Usage: *ELEMENT MATRIX OUTPUT, ELSET=elset, MASS=YES or NO Element matrix output is not supported in Abaqus/CAE. User-defined output variables in Abaqus/Standard In Abaqus/Standard output quantities can be defined as functions of any element integration point variable listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, by using user subroutine UVARM. Then, output variable UVARMn can be requested for output to the data file, the results file, or the output database. User-defined state variables in Abaqus/Standard In Abaqus/Standard you can allocate solution-dependent state variables and define them in user subroutines defining material behavior, as well as user subroutines FRIC, UEL, and UINTER . Output variable SDVn can be requested for output of these state variables to the data file, the results file, or the output database. For user-defined elements output variable SDVn cannot be requested for output to the output database. Postprocessing with Abaqus/CAE Abaqus/CAE provides interactive graphical postprocessing from the Abaqus output database file in the Visualization module (also licensed separately as Abaqus/Viewer). Capabilities include model and deformed shape plotting, contour plotting, vector plotting, X–Y plotting, and animation. Recovering additional results output from restart data in Abaqus/Standard Data needed for restart in Abaqus/Standard are contained in several files that are generated when you request that restart data be written for an analysis: the restart (.res), analysis database (.mdl and .stt), part (.prt), and output database (.odb) files. “Restarting an analysis,” Section 9.1.1, describes the writing of restart data in more detail. In Abaqus/Standard you can extract output from the restart data and write it to new data (.dat), results (.fil), and output database (.odb) files using a postprocessing analysis procedure. If the original analysis included user subroutines, the postprocessing analysis procedure requires the specification of the user subroutines. The data, results, and output database file output requests are defined as described in “Output to the data and results files,” Section 4.1.2, and “Output to the output database,” Section 4.1.3. The output requests should be defined exactly as they would be in an analysis, except that: 1. The output frequency specification has no meaning and is, therefore, ignored (unless you are recovering additional output from a previous direct cyclic or low-cycle fatigue analysis). Instead, you specify each increment at which output is to be generated in the postprocessing procedure definition. 2. No default output is provided to the output database. Furthermore, model information, such as boundary conditions, is not written to the output database. 3. Element set energy information cannot be recovered since it is not written to the restart file. 4. Output is not available for procedures that do not support restart; for example, linear perturbation procedures. The element sets and node sets that are defined for the analysis can be used for defining output sets during the postprocessing procedure. Additional sets can also be defined for the postprocessing procedure. You specify the step number in the restart file from which output is required. You cannot obtain results at the beginning of a step . Input File Usage: *POST OUTPUT, STEP=step_number When the *POST OUTPUT option is used, it must appear as the first option in the input file. No data lines from the analysis input file are required. This option can be repeated as often as necessary to obtain further output. Since *POST OUTPUT is a purely postprocessing procedure, analysis options must not appear in the input file. Abaqus/CAE Usage: Postprocessing of restart data is not supported in Abaqus/CAE. Recovering additional output from a direct cyclic analysis If you use this postprocessing technique to recover additional output from a previous direct cyclic analysis , you must specify the iteration number in the restart file from which output is required instead of the increment. If temperatures (or predefined field variables) are read from a results (.fil) file in the original direct cyclic analysis, the same temperatures (or predefined field variables) must be read into the postprocessing analysis. This specification is needed to recover thermal strains at each time increment in the original direct cyclic analysis since the results file is not stored in the restart analysis database. Input File Usage: *POST OUTPUT, STEP=step_number, ITERATION=iteration_number There are no data lines associated with this option if the ITERATION parameter is specified. Abaqus/CAE Usage: Postprocessing of restart data is not supported in Abaqus/CAE. Recovering additional output from a low-cycle fatigue analysis If you use this postprocessing technique to recover additional output from a previous low-cycle fatigue analysis , you must specify the cycle number in the restart file from which output is required instead of the increment. If temperatures (or predefined field variables) are read from a results (.fil) file in the original low-cycle fatigue analysis, the same temperatures (or predefined field variables) must be read into the postprocessing analysis. This specification is needed to recover thermal strains at each time increment in the original low-cycle fatigue analysis since the results file is not stored in the restart analysis database. Input File Usage: *POST OUTPUT, STEP=step_number, CYCLE=cycle_number There are no data lines associated with this option if the CYCLE parameter is specified. Abaqus/CAE Usage: Postprocessing of restart data is not supported in Abaqus/CAE. Example A job can be submitted using the following input file. The analysis for which restart data were written must be specified when you submit the job (using the oldjob parameter of the Abaqus execution procedure). This example creates a new data (.dat) file containing tabular data. The first two tables will contain data from increments 5 and 10 of Step 1 and will give the reaction forces of the nodes in the set CLAMP, which was defined when the analysis was run. The next table will contain data from increment 3 of Step 2 and will give displacements from the new node set TIP that is defined in this postprocessing analysis. *HEADING *POST OUTPUT, STEP=1 5, 10 *NODE PRINT, NSET=CLAMP RF, *POST OUTPUT, STEP=2 3, *NSET, NSET=TIP 1200, 1203, 1205 *NODE PRINT, NSET=TIP U, The following example input file recovers additional output from a previous direct cyclic analysis and creates a new output database (.odb) file, which contains the stress and strain for the elements in the set ELIST from each increment in Iteration 5 of Step 1, followed by data from each increment in Iteration 10 of Step 1: *HEADING *POST OUTPUT, STEP=1, ITERATION=5 *OUTPUT, HISTORY *ELEMENT OUTPUT, ELSET=ELIST S,E *POST OUTPUT, STEP=1, ITERATION=10 *OUTPUT, HISTORY *ELEMENT OUTPUT, ELSET=ELIST S,E The following example input file recovers additional output from a previous low-cycle fatigue analysis and creates a new output database (.odb) file, which contains the stress and strain for the elements in the set ELIST from each increment in Cycle 5 of Step 1, followed by data from each increment in Cycle 10 of Step 1: *HEADING *POST OUTPUT, STEP=1, CYCLE=5 *OUTPUT, HISTORY *ELEMENT OUTPUT, ELSET=ELIST S,E *POST OUTPUT, STEP=1, CYCLE=10 *OUTPUT, HISTORY *ELEMENT OUTPUT, ELSET=ELIST S,E 4.1.2 OUTPUT TO THE DATA AND RESULTS FILES Products: Abaqus/Standard Abaqus/Explicit References • “Output,” Section 4.1.1 • *CONTACT FILE • *CONTACT PRINT • *EL FILE • *EL PRINT • *ENERGY FILE • *ENERGY PRINT • *FILE OUTPUT • *MODAL FILE • *MODAL PRINT • *NODE FILE • *NODE PRINT • *RADIATION FILE • *RADIATION PRINT • *SECTION PRINT • *SECTION FILE Overview Output variables are available for: • element integration points, element section points, whole elements, and element sets; • nodes; • the whole model; • modes in mode-based dynamics procedures; • surfaces in Abaqus/Standard; and • sections in Abaqus/Standard. All of the output variables are defined in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. Output quantities from the elements, nodes, and whole model can be written to the data and results files in Abaqus/Standard and to the selected results file in Abaqus/Explicit. In Abaqus/Standard output quantities from eigenmodes, surfaces, and sections can also be written to the data and results files. For Abaqus models defined in terms of an assembly of part instances , output in the data and results files is given in terms of node, element, set, and surface labels generated internally by Abaqus. See “Output,” Section 4.1.1, for details on how to relate the internally generated numbers and names to those you specified. Requesting output to the data and results files The following sections discuss the input file syntax for requesting output to the data and results files. Abaqus/CAE automatically requests that a data file containing the default printed output for the current analysis procedure at the end of each step be generated; you cannot control the contents of the data file from within Abaqus/CAE. An analysis from Abaqus/CAE does not create a results file. Output to the Abaqus/Standard data file Abaqus/Standard analysis results can be written to the data (.dat) file. Element output, nodal output, contact surface output, energy output, modal output, and section output are available. Input File Usage: Use any of the following options to request output to the Abaqus/Standard data file: *CONTACT PRINT *EL PRINT *ENERGY PRINT *MODAL PRINT *NODE PRINT *SECTION PRINT These options are discussed in detail below. Output to the Abaqus/Standard results file Abaqus/Standard analysis results can be written to the results (.fil) file. Element output, nodal output, contact surface output, energy output, modal output, and section output are available. Input File Usage: Use any of the following options to request output to the Abaqus/Standard results file: *CONTACT FILE *EL FILE *ENERGY FILE *MODAL FILE *NODE FILE *SECTION FILE These options are discussed in detail below. Output to the Abaqus/Explicit results file You can write Abaqus/Explicit analysis results to the selected results (.sel) file by specifying a results file output request in conjunction with element output, nodal output, and/or energy output requests, as explained below. A results file output request can appear only once per step but remains in effect in subsequent steps unless it is redefined. You can convert the selected results file (job-name.sel) into the results (job-name.fil) file using the convert utility described in “Obtaining results file output in Abaqus/Explicit” in “Output,” Section 4.1.1, and “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2. Input File Usage: Use the first option in conjunction with one or more of the subsequent options to request output to the Abaqus/Explicit selected results file: *FILE OUTPUT *EL FILE *ENERGY FILE *NODE FILE Output frequency You can control the frequency of all Abaqus/Explicit results file output for a particular step by specifying the number of intervals during the step at which file output will be written, n. The data are always written at the start and end of each step in which a results file output request is active. The times at which the results are written are referred to as time marks. If the specified number of intervals is 10, Abaqus/Explicit will write results 11 times: the values at the beginning of the step and at the end of 10 equal time intervals throughout the step. The specified number of intervals must be a positive integer. By default, results will be written at the increment ending immediately after each time mark. Alternatively, you can choose to have the time increment size adjusted so that an increment will end exactly at each of the time marks calculated by dividing the step into n equal intervals. Input File Usage: Use the following option to request immediately after each time interval: results at the increments ending *FILE OUTPUT, NUMBER INTERVAL=n, TIME MARKS=NO Use the following option to request results at the exact time intervals: *FILE OUTPUT, NUMBER INTERVAL=n, TIME MARKS=YES Requesting output in multiple steps Output requests apply to the step in which they are defined and to all subsequent steps until they are respecified. One exception occurs when the step type changes from general to linear perturbation (available only in Abaqus/Standard). Output requests defined in general steps apply only to subsequent general steps; output requests defined in linear perturbation steps apply only to subsequent consecutive linear perturbation steps. In other words, output defined in a general step is independent of output defined in a linear perturbation step. Propagation between linear perturbation steps occurs only for consecutive linear perturbation steps. If a general analysis step occurs between perturbation steps, output defined in the first perturbation step will not propagate to the next perturbation step. In addition, section output requests are not propagated among linear perturbation steps in Abaqus/Standard. Element output You can output element variables (stresses, strains, section forces, element energies, etc.) for a particular step to the Abaqus/Standard data (.dat) file, the Abaqus/Standard results (.fil) file, or the Abaqus/Explicit selected results (.sel) file. The output requests can be repeated as often as necessary within a step to define output for different types of element variables, different element sets, etc. The same element (or element set) can appear in several output requests. In general, element output requests remain in effect for subsequent steps unless they are redefined; the appearance of a single element output request in a step removes all element output requests from a previous step. See “Output,” Section 4.1.1, for a discussion of requesting output in multiple general analysis steps or linear perturbation steps. In Abaqus/Explicit the element output is written to the selected results (.sel) file, which must be converted to the results (.fil) file as explained above. Input File Usage: Use the following option to output element variables to the Abaqus/Standard data file: *EL PRINT Use the following option to output element variables to the Abaqus/Standard results file or the Abaqus/Explicit selected results file: *EL FILE Selecting the element output variables The following types of element variables are recognized for the purpose of defining output: • “Element integration point” variables are associated with the integration points at which the material calculations are performed (for example, components of stress and strain). For beams and pipes defined in Abaqus/Standard with a general beam section, integration point variables are available only if the output section points were specified for the section . For first-order heat transfer elements the integration points are located at the corners of the element in heat capacitance calculations. • “Element section point” variables are associated with the cross-section of a beam, pipe, or a shell (for example, bending moments and membrane forces on the section). • “Whole element” variables are attributes of an entire element (for example, the total energy content of the element). • “Whole element set” variables are attributes of an entire element set (for example, the current coordinates of the center of mass); these variables are available only in Abaqus/Standard. The element variables that can be written to the data and results files are defined in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. Abaqus/Standard allows only complete sets of basic variables (for example, all of the stress or strain components) to be written to the results file. Individual variables (such as a particular stress component) cannot be selected and must be obtained by postprocessing. Abaqus/Standard element variables can be written to the data and results files at the integration points, at the centroid, averaged at the nodes, or extrapolated to the nodes. In Abaqus/Explicit the complete stress or strain tensors can be written to the selected results file, or individual scalar variables such as equivalent plastic strain can be written. Abaqus/Explicit writes element variables to the results file only at the integration points where they are calculated. Selecting the elements for which output is required You can specify the element set for which output is being requested. If you do not specify an element set, the output will be printed for all elements and, in Abaqus/Explicit, for all rebars in the model. In Abaqus/Standard output requests for rebars are governed separately, as discussed below. Input File Usage: Use either of the following options: *EL PRINT, ELSET=element_set_name *EL FILE, ELSET=element_set_name Specifying the section point in beams, pipes, shells, and layered solid elements For beams, pipes, shells, or layered solid elements in Abaqus/Standard output is provided at the default section points listed in Part VI, “Elements.” You can specify nondefault output points. In Abaqus/Explicit output is always provided at all section points for beam, pipe, and shell element output requests. Input File Usage: Use either of the following options in Abaqus/Standard: *EL PRINT list of output points *EL FILE list of output points Requesting output for rebars in a reinforced model In Abaqus/Standard you can request output for rebars (“Defining reinforcement,” Section 2.2.3). If you do not explicitly request rebar output in an Abaqus/Standard model with rebars, the element output requests govern the output for the matrix material only (except for section forces, where the forces in the rebar are included in the force calculation). You can request output for a particular rebar. If you do not specify the name of a rebar, output will be given for all rebars in the specified element set (or in the whole model, if you have not specified an element set). In beam and continuum elements in Abaqus/Standard rebar output can be obtained at the integration points only. In shell, membrane, and surface elements rebar output is available at the integration points and at the element’s centroid. In Abaqus/Explicit output for the rebars in the specified element set (or the whole model, if you have not specified an element set) is always included for element output requests. Input File Usage: Use either of the following options in Abaqus/Standard: *EL PRINT, REBAR=rebar_name *EL FILE, REBAR=rebar_name Selecting the position of element integration and section point output in Abaqus/Standard In Abaqus/Standard integration point variables and section variables can be written to the data and results files in four different positions. By default, output is provided at the integration points. Obtaining element output at the integration points By default, the variables are output at the integration points where they are calculated. (You can obtain the position of the integration points by using output variable COORD—see “Abaqus/Standard output variable identifiers,” Section 4.2.1.) Input File Usage: Use either of the following options: *EL PRINT, POSITION=INTEGRATION POINTS *EL FILE, POSITION=INTEGRATION POINTS Obtaining element output at the centroid of each element You can choose to output the variables at the centroid of each element (the centroid of the reference surface of a shell element or the midpoint between the end nodes of a beam or a pipe element). Centroidal values are obtained by interpolation of the integration point values if the integration scheme for the element does not include a centroidal integration point. Input File Usage: Use either of the following options: *EL PRINT, POSITION=CENTROIDAL *EL FILE, POSITION=CENTROIDAL Obtaining element output averaged at the nodes You can choose to extrapolate the variables to the nodes, then average them over all of the elements in the set that contribute to each node. For derived variables, such as the principal stress, Abaqus/Standard will first average the extrapolated tensor components over all of the elements connected to the node to obtain unique components at each node, then calculate the derived value based on the averaged components. By default, Abaqus/Standard partitions the elements in the model into averaging regions. The partitioning is based upon the structure of the elements: element type, number of section points, type of material, single layer or composite, etc. Partitioning is not based upon the values of element properties (such as thickness), material orientations, or material constants. Averaging will occur only over elements that contribute to a node and belong to the same averaging region. In some situations you may want the averaging regions to take into account the values of element properties. For example, since variables may be discontinuous between elements with different material constants, you may not want elements with different property definitions included in the same averaging region. In such cases you can force Abaqus/Standard to take into account values of element properties by setting the Abaqus environment parameter average_by_section to ON. However, in problems with many section and/or material definitions the default value of OFF will, in general, give much better performance than the nondefault value of ON. Input File Usage: Use either of the following options: *EL PRINT, POSITION=AVERAGED AT NODES *EL FILE, POSITION=AVERAGED AT NODES Obtaining element output extrapolated to the nodes You can choose to extrapolate the element integration point variables to the nodes of each element independently, without averaging the results from adjoining elements. Input File Usage: Use either of the following options: *EL PRINT, POSITION=NODES *EL FILE, POSITION=NODES Extrapolation and interpolation of element output variables The shape functions of the element are used for purposes of extrapolation and interpolation of output variables. Extrapolated values are generally not as accurate as the values calculated at the integration points in the areas of high stress gradients, particularly in the case of modified triangles and tetrahedra. Therefore, adequately detailed meshing is necessary around nodes where accurate nodal values of such element results are needed. If a cylindrical or spherical coordinate system is defined for the element , the orientation at each integration point may be different. When the values at the integration points are extrapolated to the nodes, the difference in the orientation is not taken into account; therefore, if the orientation varies significantly over the elements connected to a node, the extrapolated values will not be very accurate. If the material orientation undergoes significant spatial variation in a region of the model where the material behavior is truly anisotropic, a finer mesh is required to obtain accurate results even at the integration points. In that situation once the overall solution has converged with respect to the mesh density, the interpolation or extrapolation away from the integration points can also be assumed to be reasonably accurate. Element output for second-order elements with one collapsed side in two dimensions or one collapsed face in three dimensions should not be extrapolated to the nodes. In a coupled temperature-displacement and a coupled thermal-electrical-structural analysis nodal temperatures (variable NT11) are more accurate than temperatures at the integration point (variable TEMP) extrapolated to the nodes. For derived variables, such as the Mises equivalent stress, the components are first extrapolated or interpolated, then the derived value is calculated from the extrapolated or interpolated components. However, in linear mode-based dynamic analysis procedures where values are obtained as nonlinear combinations of modal response magnitudes (“Random response analysis,” Section 6.3.11, and “Response spectrum analysis,” Section 6.3.10), the nonlinear combinations are first calculated at the integration points. These derived values are extrapolated to the nodes or interpolated to the centroid. Requesting summaries in the Abaqus/Standard data file By default in Abaqus/Standard, summaries of element variables are printed in the data file. A summary of the maximum and minimum values is printed at the end of each column in an output table. The locations of the maximum and minimum values are also printed. You can choose to suppress this summary. Input File Usage: *EL PRINT, SUMMARY=YES or NO Requesting totals in the Abaqus/Standard data file In Abaqus/Standard you can print the sum (total) of each column in an output table to the data file. Totals can be used, for example, to obtain a sum of all the energies in a set of elements. By default, these totals are suppressed. Input File Usage: *EL PRINT, TOTALS=YES or NO Controlling the frequency of output In Abaqus/Standard you can control the frequency of element output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step. In Abaqus/Explicit the frequency of element output is controlled as described in “Output frequency” above. Input File Usage: Use either of the following options in Abaqus/Standard: *EL PRINT, FREQUENCY=n *EL FILE, FREQUENCY=n Specifying the directions for element output For components of stress, strain, and similar material variables, 1, 2, and 3 refer to the directions in an orthogonal coordinate system. If a local orientation is not defined for the element, the stress/strain components are in the default directions defined by the convention given in “Conventions,” Section 1.2.2: global directions for solid elements; surface directions for shell, membrane, and gasket elements; and axial and transverse directions for beam and pipe elements. If a local orientation is associated with the element, the element output variable components are in the local directions defined by the orientation . In Abaqus/Standard you can request that the local directions be written to the results file if component output is requested for any variable . In Abaqus/Explicit the local directions will always be written to the results file when tensor output is requested for any element variable. The local directions are written automatically to the output database file from both Abaqus/Standard and Abaqus/Explicit. In large-displacement problems the local directions defined in the reference configuration are rotated into the current configuration by the average material rotation. See “State storage,” Section 1.5.4 of the Abaqus Theory Manual, for details. Controlling the output during eigenvalue extraction You can control element output during natural frequency extraction (“Natural frequency extraction,” Section 6.3.5), complex eigenvalue extraction (“Complex eigenvalue extraction,” Section 6.3.6), and eigenvalue buckling analysis (“Eigenvalue buckling prediction,” Section 6.2.3) by specifying the first and last mode numbers for which output is required. By default, the first mode number is 1 and the last mode number is N, where N is the number of modes extracted. If you specify the first mode number, the default value for the last mode number is M, where M is the value specified for the first mode number. Input File Usage: Use either of the following options: *EL PRINT, MODE=m, LAST MODE=n *EL FILE, MODE=m, LAST MODE=n Abaqus/Standard data file format In Abaqus/Standard the printed output of variables is arranged in tables in the data file. For element variables, each row of a table corresponds to a particular location: an element, a node, a section point within an element, or an integration point. The rows that will appear in a particular table are defined by choosing an element set and, possibly, locations within each element in the set. Each table is defined by a data line of the element output request, which specifies the variables to appear in that table. There is no limit to the number of tables that can be defined. The first columns of a table define the location—the element or node number, integration point number, etc. You choose which data will appear in the remaining columns; up to 9 variables (columns) can appear in a table. For example, output variables S and E cannot be requested on the same data line in a three-dimensional analysis because that would produce 12 columns of output. If all of the entries in a row are zero, the row is not printed. Each table can contain only one type of output variable (whole element, section, or integration point); one type of element; and only one type of section definition. If an element output request to the data file includes more than one type of output variable, element, or section definition, Abaqus/Standard will split the output automatically into the necessary number of individual tables. All of the tables defined by the first data line of the output request will be printed, then all of the tables defined by the second data line, etc. Results file format An element header record (the type 1 record described in “Results file output format,” Section 5.1.2) is created for each line of requests for each integration point and section point in an element. In addition to the element header record, a direction record (record type 85) can be written in Abaqus/Standard when complete stress or strain tensor output is requested . In Abaqus/Explicit a direction record is always written when complete stress or strain tensor output is requested. For Abaqus/Standard file output requests with multiple variables, it is advantageous to specify as many variables as possible on each data line of the element output request (up to 16). By keeping the number of lines of requests to a minimum, extra type 1 and type 85 records are avoided and the size of the results file may be reduced substantially. This is not an issue in Abaqus/Explicit. Element variables must be of the same “type” (element integration point variable; element section variable; whole element variable; etc.) to be entered on a single line—see “Output,” Section 4.1.1. In Abaqus/Standard if all results in a file output record are zero, the record is not written to the results file. Output of local directions to the results file By default, in Abaqus/Standard the local coordinate directions are not written to the results file. If component output is requested, you can write the local coordinate directions to the results file. A direction record of type 85 will be written following the type 1 record. In Abaqus/Explicit the local coordinate directions are always written to the selected results file as a direction record of type 85 when complete stress or strain tensor output is requested. Tensor component output is given in the local coordinate system, which may be inherent to the element (as is the case in shells and membranes) or user-defined (“Orientations,” Section 2.2.5). For shell elements a direction record is written for every material point in the section for which component output is requested, and a separate direction record is written for section forces and section strains. For geometrically nonlinear analysis in Abaqus/Standard the record contains the current, updated directions, except for small-strain shells and gasket elements, for which the original directions are given. For three-dimensional beams, direction output is written only if section output has been requested. Direction output is not provided for trusses, two-dimensional beams, two-dimensional gasket elements, axisymmetric shells, axisymmetric membranes, axisymmetric gasket elements, or for values averaged at nodes. In addition, it is not provided for GKxxN-type gasket elements, which have no membrane or transverse shear deformation. Input File Usage: Use the following option in Abaqus/Standard: *EL FILE, DIRECTIONS=YES Default element output If you do not specify an element output request to the results file in a step (or in any previous step of the analysis), no element output will be written to the results file; similarly, if you do not specify an element output request to the data file (available only in Abaqus/Standard) in a step (or in any previous step of the analysis), no element output will be written to the data file. Node output You can output nodal variables (displacements, reaction forces, etc.) for a particular step to the Abaqus/Standard data (.dat) file, the Abaqus/Standard results (.fil) file, or the Abaqus/Explicit selected results (.sel) file. The output requests can be repeated as often as necessary within a step to define output for different node sets. The same node (or node set) can appear in several output requests. In general, nodal output requests remain in effect for subsequent steps unless they are redefined; the appearance of a single nodal output request in a step removes all nodal output requests from a previous step. See “Output,” Section 4.1.1, for a discussion of requesting output in multiple general analysis steps or linear perturbation steps. In Abaqus/Explicit the nodal output is written to the selected results (.sel) file, which must be converted to the results (.fil) file as explained above. Input File Usage: Use the following option to output nodal variables to the Abaqus/Standard data file: *NODE PRINT Use the following option to output nodal variables to the Abaqus/Standard results file or the Abaqus/Explicit selected results file: *NODE FILE Selecting the nodal output variables The nodal variables that can be written to the data and results files are defined in the “Nodal variables” portion of “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. Abaqus allows only complete sets of basic variables (for example, all of the displacement components) to be written to the results file. Individual variables (such as a particular displacement component) cannot be selected and must be obtained by postprocessing. Selecting the nodes for which output is required You can specify the node set for which output is being requested. If you do not specify a node set, the output will be printed for all nodes in the model. Input File Usage: Use either of the following options: *NODE PRINT, NSET=node_set_name *NODE FILE, NSET=node_set_name Requesting summaries in the Abaqus/Standard data file By default in Abaqus/Standard, summaries of nodal variables are printed in the data file. A summary of the maximum and minimum values is printed at the end of each column in an output table. The locations of the maximum and minimum values are also printed. You can choose to suppress this summary. *NODE PRINT, SUMMARY=YES or NO Input File Usage: Requesting totals in the Abaqus/Standard data file In Abaqus/Standard you can print the sum (total) of each column in an output table to the data file. Totals can be used, for example, to sum reaction forces at the nodes. By default, these totals are suppressed. Input File Usage: *NODE PRINT, TOTALS=YES or NO Controlling the frequency of output In Abaqus/Standard you can control the frequency of nodal output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step. In Abaqus/Explicit the frequency of nodal output is controlled as described in “Output frequency” above. Input File Usage: Use either of the following options in Abaqus/Standard: *NODE PRINT, FREQUENCY=n *NODE FILE, FREQUENCY=n Specifying the directions for nodal output For nodal variables 1, 2, and 3 refer to the global directions X, Y, and Z, respectively. For axisymmetric elements 1 and 2 refer to the global directions r and z. In Abaqus/Standard components of nodal variables such as reaction forces are output in the global directions unless a local coordinate system has been defined at a node . In this case you can specify whether output is desired in global or local directions. The local directions defined by the nodal transformation cannot be written to the results file. The data in the Abaqus/Explicit selected results file are always output in the global directions, even if a local coordinate system has been defined at a node. Obtaining nodal output in the global directions In Abaqus/Standard you can request vector-valued nodal variables in the global directions, which is the default for nodal output requests to the results file since most postprocessors assume that components are given in the global system. Input File Usage: Use either of the following options: *NODE PRINT, GLOBAL=YES *NODE FILE, GLOBAL=YES Obtaining nodal output in the local directions defined by nodal transformations In Abaqus/Standard you can request vector-valued nodal variables in the local directions defined by nodal transformations, which is the default for nodal output requests to the data file. Input File Usage: Use either of the following options: *NODE PRINT, GLOBAL=NO *NODE FILE, GLOBAL=NO Controlling the output during eigenvalue extraction You can control nodal output during natural frequency extraction, complex eigenvalue extraction, and eigenvalue buckling analysis by specifying the first and last mode numbers for which output is required, as described above for element output. Input File Usage: Use either of the following options: *NODE PRINT, MODE=m, LAST MODE=n *NODE FILE, MODE=m, LAST MODE=n Abaqus/Standard data file format In Abaqus/Standard the printed output of variables is arranged in tables by node set in the data file. For nodal variables each row of a table corresponds to an individual node. Each table is defined by a data line of the nodal output request, which specifies the variables to appear in that table. There is no limit to the number of tables that can be defined. The first column of each table is the node number. You choose the variables to appear in the remaining columns; up to nine variables (columns) can appear in a table. If all of the entries in a row are zero, the row is not printed. Displacement, velocity, and acceleration components less than a relative tolerance (equal to 100 times the machine precision times the current maximum value in the model) are treated as zero. Results file format There is no header or direction record for nodes, so it makes little difference whether items are requested on a single line or multiple lines. In Abaqus/Standard if all results in a record are zero, the record is not written to the results file. Default nodal output If you do not specify a nodal output request to the results file in a step (or in any previous step of the analysis), no nodal output will be written to the results file; similarly if you do not specify a nodal output request to the data file (available only in Abaqus/Standard) in a step (or in any previous step of the analysis), no nodal output will be written to the data file. Total energy output You can output summaries of the energy content of the model to the Abaqus/Standard data (.dat) file, the Abaqus/Standard results (.fil) file, or the Abaqus/Explicit selected results (.sel) file. Energy output requests are not available for the following procedures: • “Eigenvalue buckling prediction,” Section 6.2.3 • “Natural frequency extraction,” Section 6.3.5 • “Complex eigenvalue extraction,” Section 6.3.6 Energy output requests remain in effect for subsequent steps. Detailed energy density output is available by using element output requests . In Abaqus/Explicit the energy output is written to the selected results (.sel) file, which must be converted to the results (.fil) file as explained above. Input File Usage: Use the following option to output summaries of the energy content to the Abaqus/Standard data file: *ENERGY PRINT Use the following option to output summaries of the energy content to the Abaqus/Standard results file or the Abaqus/Explicit selected results file: *ENERGY FILE External work calculation due to concentrated follower forces Abaqus/Standard may generate inaccurate external work (ALLWK) in the presence of a concentrated follower load that rotates with time . This problem may occur in both static and implicit dynamic analyses and may result in an inaccurate total energy (ETOTAL) history output. Other results (displacements, stresses, strains, etc.) are not affected. The inaccuracy is due to the fact that the increment of work is calculated using the direction of the concentrated load at the end of the increment instead of using an average load over the increment. Selecting the energy output variables When energy output is requested, all of the total energy quantities listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, or “Abaqus/Explicit output variable identifiers,” Section 4.2.2, are output; the variables cannot be selected individually. Selecting the element set for which total energy output is required In Abaqus/Standard you can specify the element set for which total energy output is being requested. In this case the energies are summed for all the elements in the specified set. You cannot specify an element set for the following procedures: • “Transient modal dynamic analysis,” Section 6.3.7 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 • “Response spectrum analysis,” Section 6.3.10 • “Random response analysis,” Section 6.3.11 If you do not specify an element set, the total energies for the whole model will be output. If total energy output for both the whole model and for different element sets is desired, the energy output requests must be repeated; once without a specified element set to request energy output for the whole model and once for each specified element set. In Abaqus/Explicit you cannot specify selected element sets for an energy output request; the total energies for the whole model will always be output. Input File Usage: Use one of the following options in Abaqus/Standard: *ENERGY PRINT, ELSET=element_set_name *ENERGY FILE, ELSET=element_set_name Controlling the frequency of output In Abaqus/Standard you can control the frequency of energy output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step. In Abaqus/Explicit the frequency of energy output is controlled as described in “Output frequency” above. Input File Usage: Use either of the following options in Abaqus/Standard: *ENERGY PRINT, FREQUENCY=n *ENERGY FILE, FREQUENCY=n Default energy output Energy output requests must be included for total energy output to be written to the data and results files; no default output is provided. Modal output from Abaqus/Standard You can output generalized coordinate (modal amplitude and phase) values during modal dynamic procedures to the data (.dat) file or results (.fil) file. You can also request that eigenvalues be written to the results file during “Eigenvalue buckling prediction,” Section 6.2.3, or “Natural frequency extraction,” Section 6.3.5. The eigenvalues are always written to the results file when element or nodal output to the results file is requested; however, modal output requests allow you to write the eigenvalues to the results file without requesting any additional output. Input File Usage: Use the following option to output modal variables to the Abaqus/Standard data file: *MODAL PRINT Use the following option to output modal variables to the Abaqus/Standard results file: *MODAL FILE Selecting the modal output variables The modal variables that can be written to the data and results files are defined in the “Modal variables” portion of “Abaqus/Standard output variable identifiers,” Section 4.2.1. Controlling the frequency of output You can control the frequency of modal output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step. Input File Usage: Use either of the following options: *MODAL PRINT, FREQUENCY=n *MODAL FILE, FREQUENCY=n Default modal output Modal output requests must be included for modal results to be written to the data and results files; no default output is provided. Surface output from Abaqus/Standard In Abaqus/Standard you can write variables associated with surfaces in contact, coupled temperature- displacement, coupled thermal-electrical-structural, coupled thermal-electrical, and crack propagation problems to the data and results files. The output requests can be repeated as often as necessary within a step to define output for different contact pairs and different types of surface variables. See “Cavity radiation,” Section 40.1.1, for information on requesting output of surface variables associated with cavity radiation. Use element output requests to obtain data and results file output for contact elements (such as slide line elements; see “Slide line contact elements,” Section 39.4.1). Selecting the surface output variables The following types of surface variables are recognized for the purpose of defining output: • “Slave node” variables are associated with the integration points at which the material calculations are performed (for example, the contact stress). • “Whole surface” variables are attributes of an entire slave surface (for example, the total force due to contact pressure). The surface variables that can be written to the data and results files are listed in the “Surface variables” portion of “Abaqus/Standard output variable identifiers,” Section 4.2.1. Selecting the contact pairs for which output is required You can select the master and slave surfaces for which output is required, and you can specify a subset of slave nodes for output in addition to the master and slave surfaces or independently. If no surfaces or slave nodes are specified, surface variables are written for all the contact pairs in the model. If you specify the slave surface but not the master surface, output is given for all contact pairs that involve the specified slave surface. Input File Usage: Use either of the following options: *CONTACT PRINT, MASTER=master, SLAVE=slave, NSET=node_set *CONTACT FILE, MASTER=master, SLAVE=slave, NSET=node_set Requesting summaries in the data file By default, summaries of surface variables are printed in the data file. A summary of the maximum and minimum values is printed at the end of each column in an output table. The locations of the maximum and minimum values are also printed. You can choose to suppress this summary. Input File Usage: *CONTACT PRINT, SUMMARY=YES or NO Requesting totals in the data file You can print the sum (total) of each column in an output table to the data file. By default, these totals are suppressed. Input File Usage: *CONTACT PRINT, TOTALS=YES or NO Controlling the frequency of output You can control the frequency of surface output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step. Input File Usage: Use either of the following options: *CONTACT PRINT, FREQUENCY=n *CONTACT FILE, FREQUENCY=n Default surface output Surface output requests must be included for surface variables associated with contact pairs to be written to the data and results files; no default output is provided. If a surface output request is defined without any specified output variables, the following variables will be written to the data and results files by default: • For contact analysis, contact pressure (CPRESS), frictional shear stresses (CSHEAR), contact opening (COPEN), and relative tangential motions (CSLIP); see “Defining contact pairs in Abaqus/Standard,” Section 35.3.1. • For heat transfer analysis, heat flux per unit area (HFL), heat flux (HFLA), time integrated HFL (HTL), and time integrated HFLA (HTLA); see “Thermal contact properties,” Section 36.2.1. • For coupled thermal-electrical analysis, HFL, HFLA, HTL, HTLA, electrical current per unit area (ECD), electrical current (ECDA), time integrated ECD (ECDT), and time integrated ECDA (ECDTA); see “Electrical contact properties,” Section 36.3.1. • For coupled pore fluid-mechanical analysis, CPRESS, CSHEAR, COPEN, CSLIP, pore fluid volume flux per unit area (PFL), pore fluid volume flux (PFLA), time integrated PFL (PTL), and time integrated PFLA (PTLA); see “Pore fluid contact properties,” Section 36.4.1. • For crack propagation analysis, there are no default output quantities; bond failure quantities must be requested explicitly; see “Crack propagation analysis,” Section 11.4.3. Data file format Printed output of variables is arranged in tables. Each table is defined by a data line of the surface output request, which specifies the variables to appear in that table. Each table can contain only one type of output variable (slave node or whole surface). For example, output variables CSTRESS and CFN cannot be requested on the same data line. For the slave node type of output, each row of a table corresponds to a node on the slave surface. The rows that will appear in a particular table will be limited to the node set specified in the output request. The first column of each table defines the location (the node number). The remaining columns contain variables such as contact pressure, frictional shear stresses, contact opening, and relative tangential (slip) motions. For the whole surface type of output, each row of a table corresponds to an entire slave surface. If all of the variables in a row of a table are zero, the row is not printed. If a contact output request refers to more than one contact pair, a separate table will be generated for each contact pair. All of the tables defined by the first data line of the output request will be printed, then all of the tables defined by the second line, etc. Results file format A contact output request record (the type 1503 record described in “Results file output format,” Section 5.1.2) is created for each output request. For the slave node type of output, this record is followed by several node header records, each of which contains a node on the slave surface. Each node header record is followed by records that contain output variables. The output will be limited to the node set specified in the output request. For the whole surface type of output, the type 1503 record is followed by only one type 1504 node header record with a node number zero. The node header record is followed by records containing the requested output variables. If a contact output request refers to more than one contact pair, a separate contact output request record is generated for each contact pair. Section output from Abaqus/Standard In Abaqus/Standard you can output accumulated quantities associated with user-defined sections for a particular step to the data or results file. This facility provides “free body diagram” output, allowing analyses of force flow through a redundant structure. The output requests can be repeated as often as necessary within a step to define output for different sections and different section output variables. You can assign a label to each output request that will be used to identify the output for the section. Section output is not available for eigenfrequency extraction, eigenvalue buckling prediction, complex eigenfrequency extraction, or linear dynamics procedures or in procedures using multiple load cases. Defining the surface section Section output requests are available only for sections defined using element-based surfaces . Consequently, the sections must be defined using faces of continuum elements although other types of elements (beams, membranes, shells, springs, dashpots, etc.) can be attached to the section. Calculation of accumulated quantities on the section (such as the total force) involves nodal quantities associated with elements on one side of the section only. Therefore, the surface definition should use elements only from one side of the section (the “base elements,” as defined in “Prescribed assembly loads,” Section 33.5.1), thus precisely identifying the side from which accumulated quantities are computed. Since the section usually cuts through the mesh in a typical section output request, automatic generation of the surface cannot be used. Specifying the element faces gives exact control over which element faces form the surface, which is essential when defining a cross-section through a solid body. You must specify the name of the surface for which output is being requested. Surfaces that are defined in a restart analysis can be used only for section output requests. The newly defined surface cannot be used for any other purpose (such as a contact pair or pre-tension section definition). Input File Usage: Use either of the following options: *SECTION PRINT, NAME=section_name, SURFACE=surface_name *SECTION FILE, NAME=section_name, SURFACE=surface_name Example For example, the following input illustrates a typical section output request to the data file: *HEADING Section print example … *SURFACE, NAME=surface_name Data lines that specify the elements and their associated faces to define the surface section … *STEP … *SECTION PRINT, NAME=section_name, SURFACE=surface_name, … … *END STEP Alternatively, if additional section output requests are needed after the analysis is completed, a restart analysis can be performed to request more output as shown in the following input: *RESTART, READ, … … *SURFACE, NAME=surface_name Data lines that specify the elements and their associated faces to define the surface section … *STEP … *SECTION PRINT, NAME=section_name, SURFACE=surface_name, … … *END STEP Selecting the coordinate system in which output is desired You can specify the choice of coordinate system in which the section output is desired. By default, the components of vector quantities associated with the section are obtained with respect to the global system of coordinates. Alternatively, you can specify that output is desired in a local system as defined below. Input File Usage: Use either of the following options: *SECTION PRINT, NAME=section_name, SURFACE=surface_name, AXES=GLOBAL or LOCAL *SECTION FILE, NAME=section_name, SURFACE=surface_name, AXES=GLOBAL or LOCAL Defining a coordinate system local to the surface section You can allow Abaqus/Standard to define the local system, or you can specify it directly. Default local system The default local system is particularly useful when the section is flat or almost flat. While it can also be used in the case when the defined surface is curved, the default local system may be irrelevant for such problems. The default system is defined by a straight line in two-dimensional and axisymmetric cases or by a plane in three-dimensional cases, fitted (in a least square sense) through the nodes belonging to the section. The anchor point (origin) of the local system is the centroid of the projection of the surface on the fitted line or plane. The local directions are given by the normal (1-direction) and the tangent direction (the 2-direction in two-dimensional and axisymmetric cases) or the tangent directions (the 2- and 3-directions in three-dimensional cases) to the fitted line or plane. When several straight lines or planes can be fit equally well between the nodes defining the section (for example, a closed circular or spherical surface), the original local directions will be parallel to the global axes. The positive local 1-direction is selected such that it will form an acute angle with the average normal direction to the section, computed by averaging the positive normals to the element faces defining the section. If the average normal direction is zero (a closed surface), the 1-direction will form an acute angle with the global x-axis. If in two-dimensional or axisymmetric cases the 1-direction is within 0.1° of being normal to the global x-axis, it will form an acute angle with the global y-axis. In three-dimensional cases if the 1-direction is within 0.1° of being normal to the global X–Y plane, it will form an acute angle with the global z-axis. In two-dimensional and axisymmetric cases the local 2-direction is obtained by rotating the local 1-direction counterclockwise by 90° about the anchor point. For three-dimensional situations the tangent directions of the surface are defined using the Abaqus conventions for local directions on surfaces in space . Input File Usage: Use either of the following options to use the default local coordinate system: *SECTION PRINT, NAME=section_name, SURFACE=surface_name, AXES=LOCAL *SECTION FILE, NAME=section_name, SURFACE=surface_name, AXES=LOCAL User-specified local system A user-specified local system is defined by specifying the origin and the directions of the axes. You can specify the origin (anchor point) by giving a node number or by specifying the coordinates of the anchor point. In two-dimensional and axisymmetric cases the local 2-direction is defined by specifying either a predefined node number or the coordinates of a point (point a) on the local 2-direction. The local 1-direction is then obtained by rotating the local 2-axis clockwise by 90° about the anchor point . If node numbers are used to define the anchor point or the local directions, they must be connected to the mesh. In three-dimensional cases either two predefined nodes or the coordinates of two points can be used to specify the local directions. A rectangular Cartesian coordinate system is then defined by its origin (the anchor point) and these two points. The first point (point a) must lie on the local 2-direction, and anchor point .DAT AND .FIL OUTPUT anchor point elements used to define the section defined section 2-D and axisymmetric 3-D Figure 4.1.2–1 User-defined local coordinate system. the second (point b) must be in the local 2–3 plane on the side of the local 3-direction. Although it is not necessary, it is intuitive to select the second point such that it is on or near the local 3-direction . If you do not specify the anchor point of the local system, it is taken to be the centroid of the projection of the surface on the fitted line or plane. If you do not specify the directions of the axes, the local system will be anchored at the specified anchor point and its axes will be parallel to the default axes of the projected surface. If neither the anchor point nor the directions are defined, the default local system will be used. In large-deformation analyses the surface section may rotate significantly during the deformation. By default, when output is requested in a local coordinate system, the system rotates with the average rigid body motion of the elements used to define the surface section (i.e., the local system and the output are updated during the analysis). The anchor point and local directions must then be specified relative to the undeformed configuration. You can choose to obtain vector output in the original local coordinate system instead. This choice is irrelevant in steps in which geometric nonlinearities are not considered. Input File Usage: Use either of the following options to specify the local coordinate system directly: *SECTION PRINT, NAME=section_name, SURFACE=surface_name, AXES=LOCAL, UPDATE=YES or NO anchor point definition axes definition *SECTION FILE, NAME=section_name, SURFACE=surface_name, AXES=LOCAL, UPDATE=YES or NO anchor point definition axes definition Controlling the frequency of output You can control the frequency of section output by specifying the output frequency in increments. Unless a frequency of zero is specified to suppress output, the variables will always be output at the last increment of the step. Input File Usage: Use either of the following options: *SECTION PRINT, NAME=section_name, SURFACE=surface_name, FREQUENCY=n *SECTION FILE, NAME=section_name, SURFACE=surface_name, FREQUENCY=n Data file format Printed output is arranged in tables. The first line of the table contains the name of the requested output variable , and the second line contains the corresponding value. If a section output request is defined without any specified output variables, all appropriate variables associated with the current analysis type are output. If several section output requests to the data file are encountered in one particular step, separate tables will be created for each request. Each table has a header denoting the name of the section and the name of the surface used. In addition, if the output is requested in a local coordinate system, the global coordinates of the anchor point and the cosine directions of the local axes are output. Results file format Several section output records (record numbers 1580–1591 in “Results file output format,” Section 5.1.2) are output for each section output request to the results file. The actual collection of records to be written to the results file depends on the number of valid output requests. If a section output request is defined without any specified output variables, all records relevant to the current analysis type are stored in the results file. Vector output in the section Vector output associated with section output requests consists of the total force (SOF), the total moment (SOM), and the center of forces (SOCF). Output variable SOF is computed as a vector sum of the stress- based (internal) nodal forces of the nodes in the surface. Output variable SOM is computed with respect to the origin of the coordinate system considered. Thus, if the output is requested in the global coordinate system, the total moment is computed about the global origin; if the output is requested in a local coordinate system, the moment is computed about the current anchor point of the local system. The coordinates of the current anchor point may change during the analysis if the local coordinate system is updated. Output variables SOF and SOM are both reported in the coordinate system considered. The center of forces SOCF is computed as the closest point to the centroid of the section through which the total force SOF acts. SOCF is always reported in the global coordinate system. If the total force vector is equal to zero, the centroid of the section is reported as the center of forces SOCF. The total moment vector, SOM, will not necessarily equal the cross product of the center of force vector, SOCF, and total force vector, SOF. Forces acting on two different points of the section may have components acting in opposite directions, such that these force components generate a net moment but not a net force; therefore, the total moment may not arise entirely from the resultant force. Scalar output in the section Scalar output associated with a section output request consists of the area of the defined section (SOAREA), the total heat flux (SOH) in heat transfer analysis, the total current (SOE) in electrical analysis, the total mass flow (SOD) in mass diffusion analysis, and the total pore fluid volume flux (SOP) in couple pore fluid diffusion-stress analysis. These output variables are computed as the algebraic sum of the scalar internal nodal fluxes (work-conjugate to the associated primary solution variables) of the nodes in the surface. For example, in heat transfer analysis the total heat flux (SOH) is the sum of the NFLUX values at the nodes on the surfaces. Limitations when using section output requests Section output requests are subject to the following limitations: • Section output requests are available only for sections defined by an element-based surface. Thus, they can be used only for sections along faces of continuum elements. • When defining the section, elements on only one side of the section must be used. Abaqus/Standard identifies all elements attached to the surface on this side and computes the section output variables as in a free-body diagram. • The defined section must cut completely through the mesh, form a closed surface, or be on the exterior of the body. Figure 4.1.2–2 presents some typical cases of valid surfaces. If the section cuts only partially through the mesh, a valid free-body diagram cannot be isolated and incorrect answers may be computed. Abaqus/Standard will attempt to identify the invalid cases and will issue error or warning messages. • Elements attached to the section can be on either side of the surface but must not cross the defined section. Figure 4.1.2–3 presents a few invalid cases. In most cases Abaqus/Standard will successfully identify elements that cross the surface, and warning messages will be issued. The elements will then not be considered in the calculation of the section variables. • For section output purposes, Abaqus/Standard will ignore the elements attached to the section for which it cannot establish whether they belong to one side or the other of the section (e.g., SPRING1 elements). • Section output requests cannot be specified within a substructure. • Section output requests cannot be specified in random response analyses. • The total force and the total moment in the section are computed based only on the stresses (internal forces) in the identified elements. Thus, inaccurate results may be obtained if distributed body spring A pressure load beam spring A defined section elements used to define the section Figure 4.1.2–2 Valid section definitions. beam incomplete cut defining elements on both sides beam crossing the section defined section elements used to define the section Figure 4.1.2–3 Invalid section definitions. loads are present in these elements since their effect on the total force in the section is not included. Common examples are the inertial loading in dynamic analyses, gravity loads, distributed body forces, and centrifugal loads. In these cases the total force in the section may depend on the choice of elements used to define the section as illustrated in Figure 4.1.2–4(a). Assuming that gravity loading is the only active load, the element stresses will be different in the two elements. Hence, if the same section is defined first using element 1 and then using element 2, different answers for the total force will be obtained. In a similar way the effects of any distributed body fluxes (heat, electrical, etc.) prescribed in the identified elements are not included. surface defined using element 1 concentrated loads distributed body loads (a) surface defined using element 2 (b) Figure 4.1.2–4 Total force in the section. • Depending on which side of the surface is used to define the section, different answers will be obtained in analyses similar to the case illustrated in Figure 4.1.2–4(b). Assuming a static analysis with the concentrated loads shown in the figure being the only active loads, a zero total force is reported if the section is defined using element 1 and a nonzero force equal to the sum of the concentrated loads is obtained if the section is defined using element 2. 4.1.3 OUTPUT TO THE OUTPUT DATABASE Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Element-based surface definition,” Section 2.3.2 • “Integrated output section definition,” Section 2.5.1 • “Output,” Section 4.1.1 • “The postprocessing calculator,” Section 4.3.1 • *OUTPUT • *FILTER • *CONTACT OUTPUT • *ELEMENT OUTPUT • *ENERGY OUTPUT • *INTEGRATED OUTPUT • *INCREMENTATION OUTPUT • *MODAL OUTPUT • *NODE OUTPUT • *RADIATION OUTPUT • *SURFACE OUTPUT • “Understanding output requests,” Section 14.4 of the Abaqus/CAE User’s Manual Overview Output variables are available for: • element integration points, element section points, whole elements, and element sets; • surfaces in Abaqus/Explicit and Abaqus/CFD; • integrated output sections in Abaqus/Explicit; • nodes; and • the whole model. All the output variables are defined in “Abaqus/Standard output variable identifiers,” Section 4.2.1, “Abaqus/Explicit output variable identifiers,” Section 4.2.2, and “Abaqus/CFD output variable identifiers,” Section 4.2.3. Model information and analysis results are stored in terms of an assembly of part instances . See the Abaqus Scripting User’s Manual for a description of how to use the Abaqus Scripting Interface or C++ to access an output database. Requesting output to the output database Three types of information are stored in the output database in Abaqus/Standard and Abaqus/Explicit: “field” output, “history” output, and diagnostic information. In Abaqus/CFD four types of information are stored in the output database: nodal field output, surface field output, element history output, and surface history output. Field output and history output are controlled by output database requests as described in this section. A subset of the diagnostic information that is written to the message file for Abaqus/Standard analyses and to the status and message files for Abaqus/Explicit analyses is included in the output database. • Field output is intended for infrequent requests for a large portion of the model and can be used to generate contour plots, animations, symbol plots, X–Y plots, and displaced shape plots in Abaqus/CAE. Only complete sets of basic variables (for example, all the stress or strain components) can be requested as field output. • History output is intended for relatively frequent output requests for small portions of the model and is displayed in X–Y data plots in Abaqus/CAE. Individual variables (such as a particular stress component) can be requested. • Diagnostic information in Abaqus/Standard and Abaqus/Explicit is intended to provide analysis warning and/or error information as well as convergence information for use in Abaqus/CAE. Output database requests can be repeated as often as necessary within a step to produce both field and history output at multiple frequencies. Requesting field output Contact surface output, element output, nodal output, and radiation output are available as field output in Abaqus/Standard and Abaqus/Explicit. Nodal, element, and surface output are available as field output in Abaqus/CFD. Input File Usage: Use the first option in conjunction with one or more of the subsequent options to request field output to the output database: *OUTPUT, FIELD *CONTACT OUTPUT *ELEMENT OUTPUT *NODE OUTPUT *RADIATION OUTPUT *SURFACE OUTPUT These options are discussed in detail below. Abaqus/CAE Usage: Step module: field output request editor Requesting history output Contact surface output, element output, energy output, integrated output, time incrementation output, modal output, nodal output, and radiation output are available as history output in Abaqus/Standard and Abaqus/Explicit. Both element output and surface output are available as history output in Abaqus/CFD. Requesting large amounts of history output (more than 1000 output requests) may cause performance to degrade in Abaqus/Standard and will cause performance to degrade in Abaqus/Explicit and Abaqus/CFD. For vector- or tensor-valued output variables each component is considered to be a single request. In the case of element variables history output will be generated at each integration point. For example, requesting history output of the tensor variable S (stress) for a C3D10M element will generate 24 history output requests: (6 components) × (4 integration points). When requesting history output of vector- and tensor-valued variables, it is recommended that individual components be selected where available. Input File Usage: Use the first option in conjunction with one or more of the subsequent options to request history output to the output database: *OUTPUT, HISTORY *CONTACT OUTPUT *ELEMENT OUTPUT *ENERGY OUTPUT *INTEGRATED OUTPUT *INCREMENTATION OUTPUT *MODAL OUTPUT *NODE OUTPUT *RADIATION OUTPUT *SURFACE OUTPUT These options are discussed in detail below. Abaqus/CAE Usage: Step module: history output request editor Requesting diagnostic information in Abaqus/Standard and Abaqus/Explicit By default, a subset of the diagnostic information that is written to the message file for Abaqus/Standard analyses and to the status and message files for Abaqus/Explicit analyses is also written to the output database. You can use the Visualization module of Abaqus/CAE to view this diagnostic information interactively, highlighting problematic areas on a view of the model and using them to resolve errors and warnings in the analysis. For more information, see “The message file in Abaqus/Standard and Abaqus/Explicit” in “Output,” Section 4.1.1, and Chapter 41, “Viewing diagnostic output,” of the Abaqus/CAE User’s Manual. Input File Usage: Use the following option to write diagnostic information to the output database: Abaqus/CAE Usage: *OUTPUT, DIAGNOSTICS=YES Use the following option to exclude diagnostic information: *OUTPUT, DIAGNOSTICS=NO You cannot exclude diagnostic information from the output database from within Abaqus/CAE. Use the following option to view the saved diagnostic information: Visualization module: Tools→Job Diagnostics Controlling the output frequency The frequency of output to the output database is controlled differently in Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD. Control of the output frequency in Abaqus/Explicit depends upon whether field or history output was selected. Controlling the output frequency in Abaqus/Standard Abaqus/Standard provides several options for controlling the output frequency, depending on whether the analysis is in the time domain (e.g., general statics), frequency domain (e.g., steady state dynamics), or mode domain (e.g., natural frequency extraction). These options can be used to reduce the amount of output written and hence improve performance and disk space use as compared to the default output. History output in Abaqus/Standard is buffered and is written to disk only after every 10 increments of history data output or when a step has completed. Therefore, history results may not be available immediately for postprocessing. Default output frequency If you do not specify the output frequency, field and history output will be written at every increment of the analysis for all procedure types except dynamic and modal dynamic analyses for which output will be written every 10 increments. Controlling output frequency in a frequency domain analysis In frequency domain procedures, you only can control the frequency of output by specifying the frequency of output in increments. The data will be written at this frequency as well as at the end of each step of the analysis. Specify an output frequency of zero to suppress output. *OUTPUT, FREQUENCY=n Input File Usage: Abaqus/CAE Usage: Step module: field or history output request editor: Frequency: Every n increments: n Controlling output frequency in a mode domain analysis In an eigenvalue extraction or eigenvalue buckling analysis, you can select the modes at which output is desired. If you do not specify a list of modes, output is produced for all of the modes. *OUTPUT, FIELD, MODE LIST Step module: field output request editor: Frequency: Specify modes: list of modes Abaqus/CAE Usage: Input File Usage: Controlling output frequency in a time domain analysis In time domain analyses, you can control the frequency of output by specifying the output frequency in terms of increments, the number of intervals during the step, the size of regular time intervals throughout the step, or time points throughout the step. The different options are described in more detail below. Whichever option is chosen, the output will always be written at the zero-increment and last increment of the analysis and, for a low-cycle fatigue analysis, at the end of each cycle. The zero-increment output represents the initial conditions for the current analysis step and is essential for sequential thermal-stress analyses and analyses involving submodeling, for which a complete solution history (including the solution state at the beginning of the step) is needed to ensure proper interpolation in time. The zero-increment state is written at the beginning of the step, before the solution of the incremental nonlinear finite-element equations for the step commences, and is therefore in general not an equilibrium solution. Particular examples where the solution is not in equilibrium include the first step of an analysis in which an initial stress state is defined and when loads or boundary condition changes are discontinuous between steps. Usually, the zero-increment output in any step corresponds to the base state, which is the state of the model at the end of the last general step. The exception to this is modal transient dynamic analysis, where the zero-increment output represents the linear perturbation response at time zero. Time domain analysis: specifying output frequency in increments You can specify how frequently you want output in terms of increments. Specify an output frequency of zero to suppress output. Input File Usage: Abaqus/CAE Usage: *OUTPUT, FREQUENCY=n Step module: field or history output request editor: Frequency: Every n increments: n Time domain analysis: specifying output frequency in number of intervals You can specify the output frequency in number of intervals, n. The specified number of intervals must be a positive integer. By default, Abaqus/Standard adjusts the time increment (in some cases Abaqus/Standard might violate the minimum time increment specified) to ensure that data are written at the exact times calculated by dividing the step into n equal intervals. Alternatively, you can specify that the data be written immediately after each time mark. In this case no adjustment of the time increment is necessary. Input File Usage: Use the following option to request results at the exact time intervals: *OUTPUT, NUMBER INTERVAL=n, TIME MARKS=YES Use the following option to request immediately after each time interval: results at the increments ending Abaqus/CAE Usage: *OUTPUT, NUMBER INTERVAL=n, TIME MARKS=NO Use the following option to request results at the exact time intervals: Step module: field or history output request editor: Frequency: Evenly spaced time intervals, Interval: n, Timing: Output at exact times Use the following option to request immediately after each time interval: results at the increments ending Step module: field or history output request editor: Frequency: Evenly spaced time intervals, Interval: n, Timing: Output at approximate times Time domain analysis: specifying output frequency in regular time interval size You can write the results at specified regular intervals throughout the step as well as at the end of the step. By default, Abaqus/Standard will adjust the time increment (in some cases Abaqus/Standard might violate the minimum time increment specified) to ensure that data will be written at the exact times, as defined by multiples of the time interval, t. Alternatively, the data can be written immediately after each time mark. In this case no adjustment of the time increment is necessary. Input File Usage: Use the following option to request results at the exact time intervals: *OUTPUT, TIME INTERVAL=t , TIME MARKS=YES Use the following option to request immediately after each time interval: results at the increments ending Abaqus/CAE Usage: *OUTPUT, TIME INTERVAL=t , TIME MARKS=NO Use the following option to request results at the exact time intervals: Step module: field or history output request editor: Frequency: Every x units of time: t, Timing: Output at exact times Use the following option to request immediately after each time interval: results at the increments ending Step module: field or history output request editor: Frequency: Every x units of time: t, Timing: Output at approximate times Time domain analysis: specifying output frequency in time points You can write the results at specified time points throughout the step. By default, Abaqus/Standard adjusts the time increment (in some cases Abaqus/Standard might violate the minimum time increment specified) to ensure that data are written at the exact time points specified. Alternatively, you can specify that the data be written immediately after each time point. In this case no adjustment of the time increment is necessary. Input File Usage: Use the following options to request results at the exact time points: *TIME POINTS, NAME=time points name *OUTPUT, TIME POINTS=time points name, TIME MARKS=YES Use the following options to request results at immediately after each time point: the increments ending *TIME POINTS, NAME=time points name *OUTPUT, TIME POINTS=time points name, TIME MARKS=NO Use the following option to request results at the exact time points: Step module: field or history output request editor: From time points, Name: time points name, Timing: Output at exact times Abaqus/CAE Usage: Use the following option to request immediately after each time point: results at the increments ending Step module: field or history output request editor: From time points, Name: time points name, Timing: Output at approximate times Time domain analysis: time incrementation If the output frequency is specified at exact times and in terms of the number of intervals, in regular time intervals, or in time points, Abaqus/Standard adjusts the time increments to ensure that data are written at the exact time points. In some cases Abaqus may use a time increment smaller than the minimum time increment allowed in the step in the increment directly before a time point. However, Abaqus will not violate the minimum time increment allowed for consolidation, transient mass diffusion, transient heat transfer, transient couple thermal-electrical, transient coupled temperature-displacement, and transient coupled thermal-electrical-structural analyses. For these procedures if a time increment smaller than the minimum time increment is required, Abaqus will use the minimum time increment allowed in the step and will write output data at the first increment after the time point. When the output frequency is specified at exact times and in terms of the number of intervals, in regular time intervals, or in time points, the number of increments necessary to complete the analysis might increase, which might adversely affect performance. Controlling the output frequency for field output in Abaqus/Explicit Field output data are always written at the start and end of each step in which the output request is active. In addition, you can specify the output frequency in terms of the number of intervals during the step, the size of regular time intervals throughout the step, or time points throughout the step. The times at which the results are written are referred to as time marks. Specifying field output frequency in number of intervals You can specify the output frequency in number of intervals, n. The specified number of intervals must be a positive integer. For example, if the specified number of intervals is 10, Abaqus/Explicit will write field data 11 times: the values at the beginning of the step and at the end of 10 equal time intervals throughout the step. By default, field data will be written at the increment ending immediately after each time mark. Alternatively, when you specify the output frequency in number of intervals, you can choose to have the time increment size adjusted so that an increment will end exactly at each of the time marks calculated by dividing the step into n equal intervals. Input File Usage: Use the following option to request immediately after each time interval: results at the increments ending *OUTPUT, FIELD, NUMBER INTERVAL=n, TIME MARKS=NO Use the following option to request results at the exact time intervals: *OUTPUT, FIELD, NUMBER INTERVAL=n, TIME MARKS=YES Abaqus/CAE Usage: Use the following option to request immediately after each time interval: results at the increments ending Step module: field output request editor: Frequency: Evenly spaced time intervals, Interval: n, Timing: Output at approximate times Use the following option to request results at the exact time intervals: Step module: field output request editor: Frequency: Evenly spaced time intervals, Interval: n, Timing: Output at exact times Specifying field output frequency in regular time interval size Alternatively, you can write the results at specified regular intervals throughout the step as well as at the beginning and end of the step. The time increment size will not be adjusted to meet the specified time marks; results will be written at the increment ending immediately after each time mark, as defined by multiples of the time interval, t. Input File Usage: Abaqus/CAE Usage: *OUTPUT, FIELD, TIME INTERVAL=t Step module: field output request editor: Frequency: Every x units of time: t Specifying field output frequency in time points You can write the results at specified time points throughout the step. Regular time intervals between time points are not required; you can specify any desired time points at which the field output is to be written. Input File Usage: Abaqus/CAE Usage: Use the following option to request results at the exact time points: *TIME POINTS, NAME=time points name *OUTPUT, FIELD, TIME POINTS=time points name, TIME MARKS=YES the increments ending Use the following option to request immediately after each time point: *TIME POINTS, NAME=time points name *OUTPUT, FIELD, TIME POINTS=time points name, TIME MARKS=NO Use the following option to request results at the exact time points: results at Step module: field output request editor: Frequency: From time points, Name: time points name, Timing: Output at exact times Use the following option to request immediately after each time point: results at the increments ending Step module: field output request editor: Frequency: From time points, Name: time points name, Timing: Output at approximate times Default field output If you do not specify the output frequency (in either number of intervals, time interval size, or time points), field output will be written at 20 equally spaced intervals throughout the step. Controlling the output frequency for history output in Abaqus/Explicit If history output is selected, you can specify the output frequency in terms of either increments or regular intervals throughout the step. Specifying history output frequency in increments You can specify the output frequency in increments. The data will be written at this frequency as well as at the end of each step of the analysis. Input File Usage: Abaqus/CAE Usage: *OUTPUT, HISTORY, FREQUENCY=n Step module: history output request editor: Frequency: Every n time increments: n Specifying history output frequency in regular time interval size Alternatively, you can write the results at specified regular intervals throughout the step as well as at the end of the step. The time increment size will not be adjusted to meet the specified time marks; results will be written at the increment ending immediately after each time mark, as defined by multiples of the time interval, t. Input File Usage: Abaqus/CAE Usage: *OUTPUT, HISTORY, TIME INTERVAL=t Step module: history output request editor: Frequency: Every x units of time: t Default history output If you do not specify the output frequency (in either increments or time interval size), history output will be written at 200 equally spaced intervals throughout the step. Controlling the output frequency for field output in Abaqus/CFD Field output data are always written at the start and end of each step in which the output request is active. In addition, you can specify the output frequency in terms of increments, the number of intervals during the step, or the size of regular time intervals throughout the step. By default, field output will be written at 20 equally spaced intervals throughout the step. Specifying field output frequency in increments You can specify the output frequency in increments. The data will be written at this frequency as well as at the beginning and end of each step of the analysis. Input File Usage: Abaqus/CAE Usage: *OUTPUT, FIELD, FREQUENCY=n Step module: field output request editor: Frequency: Every n time increments: n Specifying field output frequency in number of intervals You can specify the output frequency in number of intervals, n. The specified number of intervals must be a positive integer. For example, if the specified number of intervals is 10, Abaqus/CFD will write field data 11 times: the values at the beginning of the step and at the end of 10 equal time intervals throughout the step. Input File Usage: Abaqus/CAE Usage: *OUTPUT, FIELD, NUMBER INTERVAL=n Step module: field output request editor: Frequency: Evenly spaced time intervals, Interval: n Specifying field output frequency in regular time interval size Alternatively, you can write the results at specified regular intervals throughout the step as well as at the beginning and end of the step. The time increment size will not be adjusted to meet the specified time marks; results will be written at the increment ending immediately after each time mark, as defined by multiples of the time interval, t. Input File Usage: Abaqus/CAE Usage: *OUTPUT, FIELD, TIME INTERVAL=t Step module: field output request editor: Frequency: Every x units of time: t Controlling the output frequency for history output in Abaqus/CFD You can specify the output frequency in terms of increments, the number of intervals during the step, or regular intervals throughout the step. By default, no history output is automatically written to the output database. Specifying history output frequency in increments You can specify the output frequency in increments. The data will be written at this frequency as well as at the beginning and end of each step of the analysis. Input File Usage: Abaqus/CAE Usage: *OUTPUT, HISTORY, FREQUENCY=n Step module: history output request editor: Frequency: Every n time increments: n Specifying history output frequency in number of intervals You can specify the output frequency in number of intervals, n. The specified number of intervals must be a positive integer. For example, if the specified number of intervals is 10, Abaqus/CFD will write history data 11 times: the values at the beginning of the step and at the end of 10 equal time intervals throughout the step. Input File Usage: Abaqus/CAE Usage: *OUTPUT, HISTORY, NUMBER INTERVAL=n Step module: history output request editor: Frequency: Evenly spaced time intervals, Interval: n Specifying history output frequency in regular time interval size Alternatively, you can write the results at specified regular intervals throughout the step as well as at the end of the step. The time increment size will not be adjusted to meet the specified time marks; results will be written at the increment ending immediately after each time mark, as defined by multiples of the time interval, t. Input File Usage: Abaqus/CAE Usage: *OUTPUT, HISTORY, TIME INTERVAL=n Step module: history output request editor: Frequency: Every x units of time: t Requesting output in multiple steps Output requests apply to the step in which they are defined and to all subsequent steps until they are respecified. The only exception occurs when the step type changes from general to linear perturbation (available only in Abaqus/Standard). Output requests defined in general steps apply only to subsequent general steps; output requests defined in linear perturbation steps apply only to subsequent consecutive linear perturbation steps. In other words, output defined in a general step is independent of output defined in a linear perturbation step. Propagation between linear perturbation steps occurs only for consecutive linear perturbation steps. If a general analysis step occurs between perturbation steps, output defined in the first perturbation step will not propagate to the next perturbation step. In any given step you can add or selectively replace the output requests that are continued from previous steps. Alternatively, you can discontinue all requests from previous steps and request a completely new set of output. The preselected field variables and preselected history output variables are requested by default for the first step of an analysis; you can modify this request as in any other step. Specifying new output requests By default, all output requests defined in previous steps are removed when new requests are defined, regardless of the type of output request being defined. In other words, a new field output request in a step removes all field and history output requests defined in previous steps. Because all existing output requests are removed when a new request is defined in a step, all output requests within the same step are treated as new (i.e., additional output requests or replacement output requests are treated as equivalent to new output requests). Input File Usage: Use one of the following options to remove all existing output requests and to specify new requests: Abaqus/CAE Usage: *OUTPUT, FIELD, OP=NEW *OUTPUT, HISTORY, OP=NEW Step module: Create Field Output Request or Create History Output Request Abaqus/CAE automatically respecifies all previously defined output requests when you create a new request. Specifying additional output requests Alternatively, you can specify additional output requests without removing all default and previously defined output requests. Input File Usage: Use one of the following options to specify additional output requests without removing all default and previously defined output requests: Abaqus/CAE Usage: *OUTPUT, FIELD, OP=ADD *OUTPUT, HISTORY, OP=ADD Step module: Create Field Output Request or Create History Output Request Abaqus/CAE automatically respecifies all previously defined output requests when you create a new request. Replacing or removing an output request You can replace an output request of the same type (e.g., field or history) and frequency with a new request. No other previously defined requests will be affected. You cannot replace an output request to change its frequency. If no matching request is found, the request specified is simply added to the step. To remove a previously defined request, you can replace the output request without specifying any new output variables. Input File Usage: Abaqus/CAE Usage: Use one of the following options to replace an output request with a new request: *OUTPUT, FIELD, OP=REPLACE *OUTPUT, HISTORY, OP=REPLACE Step module: Field Output Requests Manager or History Output Requests Manager: Edit or Delete Suppressing output requests defined in previous steps To suppress completely all output requests that have been defined in previous steps, you can specify an output frequency of 0. Preselected output requests There are two ways to define output variable requests quickly and easily. Both methods are available for field and history output requests and for the individual output requests used for requesting specific variable types (e.g., nodal, element). There are no preselected output variables for surface output requests in Abaqus/CFD. The use of these methods with individual output requests for specific variable types is explained in detail later in this section. Requesting procedure-specific preselected output requests You can activate a procedure-specific set of commonly requested output variables. See Table 4.1.3–1 for a list of procedure types and their accompanying preselected variables. The variables written to the output database may change if the procedure type changes between steps. If you request preselected field or history output and request additional output variables using individual output requests for specific variable types, the variables requested will be appended to the variables contained in the preselected list. For geometrically nonlinear analysis in Abaqus/Standard, E is not available for output and LE is output by default. For linear perturbation analyses and geometrically linear analyses in Abaqus/Standard, LE and NE strain output requests yield the same output as E. For geometrically linear analysis in Abaqus/Explicit, LE is output. Abaqus may omit some preselected variables from the analysis results. Abaqus omits preselected output variables if they are not applicable for the element type used to mesh the model or if other factors make the variables unsuitable for the analysis. No preselected variables are available for surface output in an Abaqus/CFD analysis. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *OUTPUT, FIELD, VARIABLE=PRESELECT *OUTPUT, HISTORY, VARIABLE=PRESELECT Step module: field or history output request editor: Preselected defaults Table 4.1.3–1 List of preselected variables for various procedure types. Procedure type Preselected element variables (field; history for Abaqus/CFD) Preselected nodal and surface variables (field) Preselected energy variables (history) Annealing Complex frequency extraction Coupled pore fluid diffusion/stress none none none none none S, E, VOIDR, SAT, POR U, RF, CF, PFL, PFLA, PTL, PTLA, TPFL, TPTL ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL Procedure type Preselected element variables (field; history for Abaqus/CFD) Preselected nodal and surface variables (field) Preselected energy variables (history) Coupled thermal-electric HFL, EPG NT, RFL, EPOT Direct cyclic S, E, PE, PEEQ, PEMAG U, RF, CF Direct-integration implicit dynamic (with an output frequency of 10) S, E, PE, PEEQ, PEMAG U, V, A, RF, CF, CSTRESS, CDISP Direct-solution steady-state dynamic Eigenfrequency extraction Eigenvalue buckling prediction S, E none none U, V, A, RF, CF ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL ALLKE, ALLSE, ALLVD, ALLWK none none Procedure type Explicit dynamic Preselected element variables (field; history for Abaqus/CFD) S, LE, PE, PEEQ, EVF, SVAVG, PEVAVG, PEEQVAVG Preselected nodal and surface variables (field) Preselected energy variables (history) U, V, A, RF, CSTRESS ALLKE, ALLSE, ALLWK, ALLPD, ALLCD, ALLVD, ALLDMD, ALLAE, ALLIE, ALLFD, ETOTAL Fully coupled thermal- electrical-structural in Abaqus/Standard S, E, PE, PEEQ, PEMAG, HFL, EPG U, RF, CF, NT, RFL, CSTRESS, CDISP, EPOT Fully coupled thermal-stress in Abaqus/Standard S, E, PE, PEEQ, PEMAG, HFL U, RF, CF, NT, RFL, CSTRESS, CDISP Fully coupled thermal-stress in Abaqus/Explicit S, LE, PE, PEEQ, HFL U, V, A, RF, CSTRESS, NT, RFL ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL ALLKE, ALLSE, ALLWK, ALLPD, ALLCD, ALLVD, ALLDMD, ALLAE, ALLIE, ALLFD, ALLIHE, ALLHF, ETOTAL Procedure type Preselected element variables (field; history for Abaqus/CFD) Preselected nodal and surface variables (field) Preselected energy variables (history) Geostatic stress field S, E, POR, SAT, VOIDR U, RF, CF, CSTRESS, CDISP Heat transfer HFL NT, RFL Incompressible fluid dynamics in Abaqus/CFD V, PRESSURE, TEMP, TURBNU U, V, PRESSURE, TEMP, TURBNU Linear static perturbation S, E U, RF, CF ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL none none ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL Mass diffusion CONC, MFL NNC, RFL none Modal dynamic (with an output frequency of 10) S, E U, V, A, RF, CF ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL SIM-based modal dynamic none none none Quasi-static Preselected element variables (field; history for Abaqus/CFD) S, E, PE, PEEQ, PEMAG, CE, CEEQ, CEMAG .ODB OUTPUT Preselected nodal and surface variables (field) Preselected energy variables (history) U, RF, CF, CSTRESS, CDISP ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL none ALLKE, ALLSE, ALLWK ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL ALLKE, ALLSE, ALLWK ALLAE, ALLCD, ALLFD, ALLIE, ALLKE, ALLPD, ALLSE, ALLVD, ALLDMD, ALLWK, ALLKL, ALLQB, ALLEE, ALLJD, ALLSD, ETOTAL ALLKE, ALLSE, ALLVD, ALLWK Random response Response spectrum S, E S, E U, V, A U, RF, CF Static S, E, PE, PEEQ, PEMAG U, RF, CF, CSTRESS, CDISP Steady-state dynamic S, E U, V, A, RF, CF SIM-based steady-state dynamic none Steady-state transport S, E none none U, RF, CF, CSTRESS, CDISP Subspace-based steady-state dynamic S, E U, V, A, RF, CF Requesting all variables applicable to the current procedure and material type in Abaqus/Standard and Abaqus/Explicit You can request all variables applicable to the current procedure and material type. Any individual output requests for specific variable types are ignored in this case. Input File Usage: Use one of the following options: *OUTPUT, FIELD, VARIABLE=ALL *OUTPUT, HISTORY, VARIABLE=ALL Step module: field or history output request editor: All Abaqus/CAE Usage: Default output In Abaqus/Standard and Abaqus/Explicit, if no output database requests are specified, the preselected field and history output variables are written automatically to the output database. In Abaqus/Standard the default variables are written at every increment for both field and history output for all procedure types except dynamic and modal dynamic analyses; the default frequency for field and history output for these procedure types is every 10 increments. In Abaqus/Explicit the default variables are written at 20 intervals for field output and 200 intervals for history output. In Abaqus/CFD the default variables are written at 20 intervals for field output. You can turn these defaults off for an analysis in Abaqus/Standard and Abaqus/Explicit by using the odb_output_by_default environment file parameter; see “Using the Abaqus environment settings,” Section 3.3.1, for details. Furthermore, specifying new output database requests in a step overrides the default field and history output requests for that step. For large models the default output to the output database may increase the solution time and required disk space considerably. In such cases you are encouraged to review carefully the relevance of the default output variables for the proposed analysis. A C++ program is available that creates a smaller copy of a large output database by copying data from only selected frames; for more information, see “Decreasing the amount of data in an output database by retaining data at specific frames,” Section 10.15.4 of the Abaqus Scripting User’s Manual. The odb_output_by_default environment file parameter is ignored in a restart analysis. If no output requests are defined in a restart analysis, the output requests are those that propagate from the original analysis. Abaqus/Explicit output as a result of analysis termination When an Abaqus/Explicit analysis encounters a fatal error in an increment, the preselected variables applicable to the current procedure are written automatically to the output database as field data. The analysis will go through an additional increment with a zero time increment size before writing these data. Element output You can request that element variables (stresses, strains, section forces, element energies, etc.) be written to the output database. The output request can be repeated as often as necessary to define output for different types of element variables, different element sets, etc. The same element (or element set) can appear in several output requests. Element output to the output database is not supported for user elements. Selecting the element output variables The following types of element variables are recognized for the purpose of defining output: • “Element integration point” variables are associated with the integration points at which material calculations are performed (for example, components of stress and strain). • “Element section point” variables are associated with the cross-section of a beam, pipe, or a shell (for example, bending moments and membrane forces on the section); these variables are not available in Abaqus/CFD. • “Element face” variables are associated with the faces of a shell or a solid (for example, uniformly distributed pressure load on the face). • “Whole element” variables are attributes of an entire element (for example, the total energy content of the element). • “Whole element set” variables are attributes of an entire element set (for example, the current these variables are available in Abaqus/Standard and coordinates of the center of mass); Abaqus/Explicit. The element variables that can be written to the output database are defined in “Abaqus/Standard output variable identifiers,” Section 4.2.1, “Abaqus/Explicit output variable identifiers,” Section 4.2.2, and “Abaqus/CFD output variable identifiers,” Section 4.2.3. Input File Usage: *ELEMENT OUTPUT list of output variables Abaqus/CAE Usage: Step module: field or history output request editor: Select from list below Selecting elements for which output is required For history output you must specify the element set (or, in Abaqus/Explicit, the tracer set) for which output is being requested. For field output specifying the element set or tracer set is optional; if you do not specify an element set or tracer set, the output will be written for all the elements in the model. Input File Usage: Abaqus/CAE Usage: *ELEMENT OUTPUT, ELSET=element_set_name Step module: field or history output request editor: Domain: Set: set_name Requesting field output for the exterior elements in the model in Abaqus/Standard and Abaqus/Explicit You can select output on the element set consisting of all the exterior three-dimensional elements in the model. This element set is generated internally by Abaqus. Input File Usage: Abaqus/CAE Usage: *ELEMENT OUTPUT, EXTERIOR Step module: field output request editor: Domain: Whole model; toggle on Exterior only Specifying the section point in beam, pipe, shell, and layered solid elements in Abaqus/Standard and Abaqus/Explicit For beams, pipes, shells, or layered solids output is provided at the default section points. You can specify nondefault output points. Input File Usage: *ELEMENT OUTPUT list of output points list of output variables Abaqus/CAE Usage: Step module: field or history output request editor: Output at shell, beam, and layered section points: Specify: list of output points Requesting output for rebars in a reinforced model in Abaqus/Standard and Abaqus/Explicit You can request output for rebars (“Defining reinforcement,” Section 2.2.3). If you do not explicitly request rebar output in a model with rebars, the element output requests govern the output for the matrix material only (except for section forces, where the forces in the rebar are included in the force calculation). You can request output for a particular rebar. If you do not specify the name of a rebar, output will be given for all rebars in the specified element set (or in the whole model, if you have not specified an element set). Rebar output is available only in membrane, shell, or surface elements at the integration points and at the centroid of the element. Input File Usage: Use the following options: Abaqus/CAE Usage: *OUTPUT, FIELD *ELEMENT OUTPUT, REBAR=rebar_name, ELSET=element_set_name *OUTPUT, HISTORY *ELEMENT OUTPUT, REBAR=rebar_name, ELSET=element_set_name Use the following option to request output for rebar in addition to output for the matrix material: Step module: field or history output request editor: Output for rebar: Include Use the following option to request output only for rebar: Step module: field or history output request editor: Output for rebar: Only You cannot request output for a particular rebar in Abaqus/CAE; if you request rebar output, it is given for all rebars in the specified output domain. Selecting the position of element integration point and section point output Integration point variables and section variables in Abaqus/Standard and Abaqus/Explicit can be written as field output to the output database in three different positions: the integration points, the centroid, or the nodes. By default, output is provided at the integration points. In most cases Abaqus writes only integration point data to the output database. Transferring of results from the integration points to the user-specified position in Abaqus/Standard and Abaqus/Explicit is done by the postprocessing calculator. See “The postprocessing calculator,” Section 4.3.1, for details. In Abaqus/Standard an alternative procedure is available for three commonly requested output variables: stress components, Mises equivalent stress, and equivalent pressure stress. To activate this alternate procedure for Mises equivalent stress and equivalent pressure stress, output variables MISESONLY and PRESSONLY, respectively, must be requested. If output variables, MISES and PRESS, are used instead, the old procedure is invoked. If output at the nodes or at the centroid is requested for any of these variables, the interpolation and extrapolation are performed during the analysis as soon as stresses are available at the integration points. This eliminates the need to store stress components at the integration points and reduces the size of the output database. This procedure is invoked automatically when output is requested for any of the supported variables. Element history output to the output database is always provided at the integration points. Obtaining output at the integration points in Abaqus/Standard and Abaqus/Explicit the variables are output at By default, In Abaqus/Standard you can obtain the position of the integration points by using output variable COORD . the integration points where they are calculated. Input File Usage: Abaqus/CAE Usage: *ELEMENT OUTPUT, POSITION=INTEGRATION POINTS You cannot select the position of element output in Abaqus/CAE; it is always given at the integration points. Obtaining output at the centroid of each element in Abaqus/Standard and Abaqus/Explicit You can choose to output the variables at the centroid of each element (the midpoint between the end nodes of a beam or a pipe element). Centroidal values are obtained through the postprocessing calculator by interpolation of the integration point values if the integration scheme for the element does not include a centroidal integration point. Element output of the element centroidal values is not available for recovering results within substructures; for more information, see “Using substructures,” Section 10.1.1. Input File Usage: Abaqus/CAE Usage: *ELEMENT OUTPUT, POSITION=CENTROIDAL You cannot select the position of element output in Abaqus/CAE; it is always given at the integration points. Obtaining element output extrapolated to the nodes in Abaqus/Standard and Abaqus/Explicit You can choose to extrapolate the element integration point variables to the nodes of each element independently, without averaging the results from adjoining elements. Element output at the element nodes is not available for recovering results within substructures; for more information, see “Using substructures,” Section 10.1.1. Input File Usage: Abaqus/CAE Usage: *ELEMENT OUTPUT, POSITION=NODES You cannot select the position of element output in Abaqus/CAE; it is always given at the integration points. Extrapolation and interpolation of element output variables in Abaqus/Standard and Abaqus/Explicit The shape functions of the element are used by the postprocessing calculator for purposes of extrapolation and interpolation of output variables. Extrapolated values are generally not as accurate as the values calculated at the integration points in the areas of high stress gradients, particularly in the case of modified triangles and tetrahedra. Therefore, adequately detailed meshing is necessary around nodes where accurate nodal values of such element results are needed. If a cylindrical or spherical coordinate system is defined for the element , the orientation at each integration point may be different. When the values at the integration points are extrapolated to the nodes, the difference in the orientation is not taken into account; therefore, if the orientation varies significantly over the elements connected to a node, the extrapolated values are not very accurate. If the material orientation undergoes significant spatial variation in a region of the model where the material behavior is truly anisotropic, a finer mesh is required to obtain accurate results even at the integration points. In that situation once the overall solution has converged with respect to the mesh density, the interpolation or extrapolation away from the integration points can also be assumed to be reasonably accurate. You should also be particularly careful when interpreting output variables extrapolated to the nodes for second-order elements with midside nodes outside the quarter-point region, such as when one edge is collapsed in two dimensions or one face is collapsed in three dimensions. For derived variables, such as Mises equivalent stress, the components are first extrapolated or interpolated. The derived value is then calculated from the extrapolated or interpolated components. However, in linear mode-based dynamic analysis procedures where derived values are obtained as nonlinear combinations of modal response magnitudes (“Random response analysis,” Section 6.3.11, and “Response spectrum analysis,” Section 6.3.10), the nonlinear combinations are first calculated at the integration points. These derived values are then extrapolated to the nodes or interpolated to the centroid. Controlling the output frequency The frequency of element output is controlled as described above in “Controlling the output frequency.” Requesting preselected output You can request the preselected, procedure-specific element output variables described in Table 4.1.3–1. In this case you can specify additional variables as part of the output request. Alternatively, you can request all element variables applicable to the current procedure and material type. In this case any additional variables you specify are ignored. Input File Usage: Use the following option to request the preselected element output variables: *ELEMENT OUTPUT, VARIABLE=PRESELECT Use the following option to request all applicable element output variables: Abaqus/CAE Usage: *ELEMENT OUTPUT, VARIABLE=ALL Step module: field or history output request editor: Preselected defaults or All Specifying the directions for element output in Abaqus/Standard and Abaqus/Explicit For components of stress, strain, and similar material variables 1, 2, and 3 refer to the directions for an orthogonal coordinate system. If a local orientation is not defined for the element, the stress/strain components are in the default directions defined by the convention given in “Orientations,” Section 2.2.5: global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam and pipe elements. By default, the element material directions for element field output are written to the output database. If a local orientation is associated with the element, by default the results displayed in Abaqus/CAE are in the directions defined by the local orientation. These directions can be visualized in Abaqus/CAE by selecting Plot→Material Orientations in the Visualization module. You can choose to suppress the direction output to the output database. Input File Usage: Use the following option to indicate that the element material directions should not be written to the output database: Abaqus/CAE Usage: *ELEMENT OUTPUT, DIRECTIONS=NO Step module: field output request editor: toggle off Include local coordinate directions when available Node output You can output nodal variables (displacements, reaction forces, etc.) to the output database. The output request can be repeated as often as necessary to define output for different node sets. The same node (or node set) can appear in several output requests. Selecting the nodal output variables The nodal variables that can be written to the output database are defined in the “Nodal variables” section of “Abaqus/Standard output variable identifiers,” Section 4.2.1, “Abaqus/Explicit output variable identifiers,” Section 4.2.2, and “Abaqus/CFD output variable identifiers,” Section 4.2.3. Input File Usage: *NODE OUTPUT list of output variables Abaqus/CAE Usage: Step module: field or history output request editor: Select from list below Selecting the nodes for which output is required For history output you must specify the node set (or, in Abaqus/Explicit, the tracer set) for which output is being requested. For field output the specification of the node set or tracer set is optional; if you do not specify a node set or tracer set, the output will be written for all the nodes in the model. Input File Usage: Abaqus/CAE Usage: *NODE OUTPUT, NSET=node_set_name Step module: field or history output request editor: Domain: Set: set_name Requesting field output for the exterior nodes in the model in Abaqus/Standard and Abaqus/Explicit You can select output on the node set consisting of all the exterior nodes in the model. This node set is generated internally by Abaqus and includes all the nodes that belong to the exterior three-dimensional elements. Input File Usage: Abaqus/CAE Usage: *NODE OUTPUT, EXTERIOR Step module: field output request editor: Domain: Whole model; toggle on Exterior only Controlling the output frequency The frequency of nodal output is controlled as described above in “Controlling the output frequency.” Controlling the precision in Abaqus/Standard and Abaqus/Explicit You can control the precision of nodal output for an analysis. Input File Usage: Use the following command line option to request single-precision nodal output: abaqus job=job-name output_precision=single Use the following command line option to request double-precision nodal output: Abaqus/CAE Usage: abaqus job=job-name output_precision=full Job module: job editor: Precision: Nodal output precision: Single or Full Requesting preselected output You can request the preselected, procedure-specific nodal output variables described in Table 4.1.3–1. In this case you can specify additional variables as part of the output request. Alternatively, you can request all nodal variables applicable to the current procedure type. In this case any additional variables you specify are ignored. Input File Usage: Use the following option to request the preselected nodal output variables: *NODE OUTPUT, VARIABLE=PRESELECT Use the following option to request all applicable nodal output variables: Abaqus/CAE Usage: *NODE OUTPUT, VARIABLE=ALL Step module: field or history output request editor: Preselected defaults or All Specifying the directions for nodal field output in Abaqus/Standard and Abaqus/Explicit For nodal variables 1, 2, and 3 refer to the global directions X, Y, and Z, respectively. For axisymmetric elements 1 and 2 refer to the global directions r and z. Nodal field results are written to the output database in the global directions. If a local coordinate system is defined at a node , the local nodal transformations are written to the output database as well. You can apply these transformations to the results in the Visualization module of Abaqus/CAE to view components in the local systems. Specifying the directions for nodal history output in Abaqus/Standard and Abaqus/Explicit For nodal variables 1, 2, and 3 refer to the global directions X, Y, and Z, respectively. For axisymmetric elements 1 and 2 refer to the global directions r and z. Nodal history results are written to the output database in the global directions unless a local coordinate system has been defined at a node . desired in global or local directions. Obtaining nodal history output in the global directions You can request vector-valued nodal variables in the global directions, which is the default for nodal history output requests to the output database since most postprocessors assume that components are given in the global system. Input File Usage: Abaqus/CAE Usage: *NODE OUTPUT, GLOBAL=YES Step module: history output request editor: Domain: Set: global directions for vector-valued output toggle on Use Obtaining nodal history output in the local directions defined by nodal transformations You can request vector-valued nodal variables in the local directions defined by nodal transformations. Input File Usage: Abaqus/CAE Usage: *NODE OUTPUT, GLOBAL=NO Step module: history output request editor: Domain: Set: global directions for vector-valued output toggle off Use Visualizing boundary conditions Boundary conditions can be visualized in the Visualization module of Abaqus/CAE by selecting View→ODB Display Options. Click the Entity Display tab in the dialog box that appears. In an Abaqus/Standard analysis boundary condition information is written to the output database only when some nodal output variables are requested as field output. Tracer particle output from Abaqus/Explicit In Abaqus/Explicit tracer particles can be used to obtain output at specific material points that may not correspond to a fixed location in the mesh if adaptive meshing is used. Tracer particles follow the material motion throughout an analysis regardless of the mesh motion, which makes them ideal for use with adaptive meshing . Both nodal and element output can be obtained at tracer particles. Defining tracer particles You define the initial location of each tracer particle to be coincident with a node, called the “parent node.” These parent nodes are grouped into a tracer set; you must assign a name to the tracer set when you define the tracer particles. Input File Usage: *TRACER PARTICLE, TRACER SET=tracer_set_name list of parent nodes (either node numbers or node set labels) Abaqus/CAE Usage: Tracer particles are not supported in Abaqus/CAE. Particle birth stages Sets of tracer particles can be released from the current locations of the parent nodes at multiple times during a step. Each release of tracer particles is referred to as a “particle birth.” After particle birth the tracer particles follow the motion of the associated material regardless of the motion of the mesh. You can indicate the number of particle birth stages in a step, n. One particle birth will occur at the beginning of the step, and the rest of the stages will be evenly spaced throughout the step. If you do not specify a number of particle birth stages, a single particle birth will occur at the beginning of the step. Input File Usage: *TRACER PARTICLE, TRACER SET=tracer_set_name, PARTICLE BIRTH STAGES=n Abaqus/CAE Usage: Tracer particles are not supported in Abaqus/CAE. Tracer particles in the output database Tracer sets will appear as both node and element sets in the output database. If a tracer set has multiple birth stages, additional node and element sets will be created that group all the tracer particles associated with a given birth stage. These subsets are named by appending the birth stage number to the tracer set name. For example, if a tracer set with the name INLET is defined with two particle birth stages, three node sets and three element sets will be created in the output database: INLET Stage 1, INLET Stage 2, and INLET (which contains all the nodes/elements from both INLET Stage 1 and INLET Stage 2). Internal field output requests are generated automatically for the requested output variables for all the elements or nodes in the domain that completely defines the space of possible tracer particle locations. This region is determined by Abaqus/Explicit and typically corresponds to the elements attached to the parent nodes and any intersecting adaptive mesh domains. The postprocessing calculator will compute the value of any requested output quantity at a tracer particle by interpolating the results from the element that encompasses the particle at the time of output. Requesting output at tracer particles You can request element or nodal output for a particular tracer set. Output will be given for all tracer particles that are associated with the specified tracer set name. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *NODE OUTPUT, TRACER SET=tracer_set_name *ELEMENT OUTPUT, TRACER SET=tracer_set_name Tracer particle output is not supported in Abaqus/CAE. Field output at tracer particles Displacement is the only valid field request for tracer particles. You can obtain the positions of the tracer particles in a specific tracer set by requesting displacements as nodal field output. Tracer particle displacements are output automatically if displacement output is requested for the entire model. You can use the node and element sets created for tracer particles in the output database to control the display of tracer particles in the Visualization module of Abaqus/CAE. Input File Usage: Use both of the following options: *OUTPUT, FIELD *NODE OUTPUT, TRACER SET=tracer_set_name Abaqus/CAE Usage: Tracer particle output is not supported in Abaqus/CAE. History output at tracer particles Requesting history output for tracer particles is similar to requesting history output for elements and nodes. Any valid element integration point variable can be requested. U, V, A, and COORD are the only valid nodal requests. Whole element variables and element section variables cannot be requested. History data are available for a tracer particle only after its birth. A tracer particle history output request triggers an internal field output request for the desired variables for all the elements or nodes in the domain that completely defines the space of possible tracer particle locations. Input File Usage: Use the following options: *OUTPUT, HISTORY *NODE OUTPUT, TRACER SET=tracer_set_name *ELEMENT OUTPUT, TRACER SET=tracer_set_name Tracer particle output is not supported in Abaqus/CAE. Abaqus/CAE Usage: Tracer particle propagation in multiple steps Once defined, all tracer particles remain active in subsequent steps. However, no further particle births occur in the steps that follow the tracer set definition. You can define new tracer particles in subsequent steps by specifying a new tracer set name. The same tracer set name cannot be used more than once within an analysis. Tracer particle deactivation Individual tracer particles are deactivated if they flow out of the mesh across an Eulerian boundary or are currently tracking material points inside a failed element that has been deleted from the mesh. History data for tracer particles are zero at all times after deactivation. Controlling the output frequency at tracer particles The frequency of tracer particle output is controlled as described above in “Controlling the output frequency.” WARNING: Requesting tracer set history output at a high frequency may cause the output database (.odb) to become large. The disk space required to store the field data is directly proportional to the size of the adaptive mesh domain and the number of tracer sets. The disk space usage is independent of the number of tracer particles in a tracer set. The output database file size is reduced after the postanalysis calculation is performed. Integrated output in Abaqus/Explicit Integrated output can be requested either over a surface or over an element set. An integrated output request is used to write the time history of variables such as the total force transmitted across a surface, the total mass of an element set, or the percentage change of the total mass of an element set. Selecting the integrated output variables The integrated variables that can be written to the output database are defined in the “Integrated variables” section of “Abaqus/Explicit output variable identifiers,” Section 4.2.2. Input File Usage: *INTEGRATED OUTPUT list of output variables Abaqus/CAE Usage: Step module: history output request editor: Select from list below Selecting the surface over which integrated output is required You can specify the surface directly for an integrated output request. Alternatively, you can associate an integrated output section that identifies the surface with the integrated output request. Integrated output can be requested for a surface that includes facets, edges, or ends of various types of deformable elements. The surface can include facets of three-dimensional solid elements and continuum shell elements; edges of two-dimensional solid elements, membrane elements, conventional shell, and surface elements; and ends of beam elements, pipe elements, and truss elements. Specifying the surface for integrated output directly If you specify the surface for an integrated output request directly, any vector output variables are given with respect to a fixed global coordinate system and the total moment transmitted across the surface, SOM, is computed about the fixed global origin. See “Element-based surface definition,” Section 2.3.2, for information on defining element-based surfaces. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *SURFACE, NAME=surface_name, TYPE=ELEMENT *INTEGRATED OUTPUT, SURFACE=surface_name You cannot specify the surface for an integrated output request directly in Abaqus/CAE; you must create an integrated output section as described below. Specifying the surface through an integrated output section definition If you associate an integrated output section definition with an integrated output request, the integrated output variables can be obtained in a local coordinate system that can translate and/or rotate with the deformation . In addition, the total moment transmitted across the surface, SOM, can be computed about a moving location. defined section anchor point anchor point elements used to define the section defined section 2-D 3-D Figure 4.1.3–1 A user-defined local coordinate system. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *INTEGRATED OUTPUT SECTION, NAME=section_name, SURFACE=surface_name *INTEGRATED OUTPUT, SECTION=section_name Step module: Output→Integrated Output Sections→Create: Name: section_name: select regions for the surface History output request editor: Domain: Integrated output section: section_name Requesting integrated output for “force-flow” studies To study the “force-flow” through various paths in a model, you must create interior surfaces that cut through one or more regions (similar to a cross-section) so that you can request integrated output of the total force transmitted across these surfaces. You can create such interior surfaces over the element facets, edges, or ends by simply cutting through one or more regions of the model with a plane; see “Creating interior cross-section surfaces” in “Element-based surface definition,” Section 2.3.2, for more information. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *SURFACE, NAME=surface_name, TYPE=CUTTING SURFACE *INTEGRATED OUTPUT, SURFACE=surface_name You cannot specify the surface for an integrated output request directly in Abaqus/CAE; you must create an integrated output section as described above. Requesting integrated output over an element set You can request integrated output over an element set to output its total mass, the percentage change of its total mass, its average rigid body motion or any combination of these variables. The element set must have been defined previously, and it can include any type of elements. Input File Usage: Use the following option to request integrated output over an element set: Abaqus/CAE Usage: *INTEGRATED OUTPUT, ELSET=element set name Requesting integrated output over an element set Abaqus/CAE. is not supported in Controlling the output frequency The frequency of integrated output is controlled as described above in “Controlling the output frequency for history output in Abaqus/Explicit.” Requesting preselected output Preselected output variables are available only when the integrated output is requested over a surface. If integrated output is requested over an element set, you must specify the variables on the data line. If the integrated output is requested over a surface, you can request the preselected integrated output variables SOF and SOM. In this case you can also specify additional variables as part of the output request. Alternatively, you can request all integrated variables applicable to the current procedure type. In this case any additional variables that you specify are ignored. If you do not request the preselected variables or all variables, you must specify the variables individually. Input File Usage: Use the following option to request the preselected integrated output variables: *INTEGRATED OUTPUT, VARIABLE=PRESELECT optional additional variables Use the following option to request all integrated output variables relevant to the current procedure type: *INTEGRATED OUTPUT, VARIABLE=ALL Use the following option to specify individual integrated output variables: *INTEGRATED OUTPUT individual variables Abaqus/CAE Usage: Step module: history output request editor: Preselected defaults or All Limitations when using integrated output requests Integrated output requests over a surface are subject to the following limitations: • Integrated output can be requested over a surface that includes facets, edges, or ends of various types of deformable elements. The surface can include facets of three-dimensional solid elements and continuum shell elements; edges of two-dimensional solid elements, membrane elements, conventional shell, and surface elements; and ends of beam elements, pipe elements, and truss elements. The surface should not contain facets of axisymmetric elements or facets of rigid elements. • When defining the surface, elements on only one side of the surface must be used. Abaqus/Explicit computes the integrated output variables using the stresses and hourglass-mode forces in elements underlying the surface as in a free-body diagram. • The defined surface must cut completely through the mesh, form a closed surface, or be on the exterior of the body. Figure 4.1.3–2 presents some typical cases of valid surfaces. If the surface cuts only partially through the mesh, a valid free-body diagram cannot be isolated and incorrect answers may be computed. spring A pressure load beam spring A defined section elements used to define the section Figure 4.1.3–2 Valid section definitions. beam incomplete cut defining elements on both sides beam crossing the section defined section elements used to define the section Figure 4.1.3–3 Invalid section definitions. • Elements attached to the surface can be on either side of the surface but must not cross the defined surface. Figure 4.1.3–3 presents a few invalid cases. • The total force and the total moment in the section are computed based only on the stresses (internal forces) in the identified elements. Thus, inaccurate results may be obtained if distributed body loads are present in these elements since their effect on the total force in the section is not included. Common examples are the inertial loading in dynamic analyses, gravity loads, distributed body forces, and centrifugal loads. In these cases the total force in the section may depend on the choice of elements used to define the section as illustrated in Figure 4.1.3–4(a). Assuming that gravity loading is the only active load, the element stresses will be different in the two elements. Hence, if the same surface is defined first using element 1 and then using element 2, different answers for the total force will be obtained. In a similar way the effects of any distributed body fluxes (heat, electrical, etc.) prescribed in the identified elements are not included. • Depending on which side of the surface is used to define the section, different answers will be obtained in analyses similar to the case illustrated in Figure 4.1.3–4(b). Assuming a quasi-static analysis with the concentrated loads shown in the figure being the only active loads, a zero total force is reported if the surface is defined using element 1 and a nonzero force equal to the sum of the concentrated loads is obtained if the surface is defined using element 2. Total energy output You can output the total energy of the model or of a specific element set to the output database. Energy output is available only as history output. Energy output requests are not available for the following procedures: • “Eigenvalue buckling prediction,” Section 6.2.3 surface defined using element 1 concentrated loads distributed body loads (a) surface defined using element 2 (b) Figure 4.1.3–4 Total force in the section. • “Natural frequency extraction,” Section 6.3.5 • “Complex eigenvalue extraction,” Section 6.3.6 Selecting the energy output variables The energy variables that can be written to the output database are defined in the “Total energy output quantities” section of “Abaqus/Standard output variable identifiers,” Section 4.2.1; “Abaqus/Explicit output variable identifiers,” Section 4.2.2; and “Abaqus/CFD output variable identifiers,” Section 4.2.3. Input File Usage: *ENERGY OUTPUT list of output variables Abaqus/CAE Usage: Step module: history output request editor: Select from list below Selecting the element set for which total energy output is required You can specify the element set for which total energy output is being requested. In this case the energies are summed for all the elements in the specified set. You cannot specify an element set for the following procedures: • “Transient modal dynamic analysis,” Section 6.3.7 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 • “Response spectrum analysis,” Section 6.3.10 • “Random response analysis,” Section 6.3.11 The following energies are not available as element set quantities: ALLWK, ALLFD, ALLQB, ALLKL, ALLFC, and ETOTAL. If If you do not specify an element set, the total energies for the whole model will be output. total energy output for both the whole model and for different element sets is desired, the energy output requests must be repeated: once without a specified element set to request energy output for the whole model and once for each specified element set. Input File Usage: Abaqus/CAE Usage: *ENERGY OUTPUT, ELSET=element_set_name Step module: history output request editor: Domain: Set: set_name Controlling the output frequency The frequency of energy output is controlled as described above in “Controlling the output frequency.” Requesting preselected output You can request the preselected, procedure-specific energy output variables described in Table 4.1.3–1. In this case you can specify additional variables as part of the output request. Alternatively, you can request all energy variables applicable to the current procedure and material type. In this case any additional variables you specify are ignored. Input File Usage: Use the following option to request the preselected energy output variables: *ENERGY OUTPUT, VARIABLE=PRESELECT Use the following option to request all applicable energy output variables: Abaqus/CAE Usage: *ENERGY OUTPUT, VARIABLE=ALL Step module: history output request editor: Preselected defaults or All Sensor definition in Abaqus/Standard and Abaqus/Explicit For nodal and connector element output variables, history output requests can be used to define sensors. Sensors are named entities that are intended to be used to model physical sensors such as the total force or displacement of a hydraulic piston, the motion of a given point on a structure, or the acceleration as measured by an accelerometer. Sensor values can be fed back into the model to produce actuation that is a function of the sensed quantity thus allowing for modeling of control engineering aspects of your system. You can use sensors in user subroutine UAMP or VUAMP to define a customized amplitude that is a function of sensor values at the end of the previous increment as shown in “VUAMP,” Section 1.2.7 of the Abaqus User Subroutines Reference Manual, and illustrated in the example in “Crank mechanism,” Section 4.1.2 of the Abaqus Example Problems Manual. The amplitude function can be used to actuate any Abaqus feature that can reference an amplitude, such as concentrated loads, boundary conditions, connector motion/load, distributed pressure, and material properties via field variables. A sensor must be uniquely associated with a particular scalar output variable (U1, CTF3, etc.) and can be defined using history output requests by following some simple rules. The sensor name is specified in the history output definition, and one and only one nodal output or element output request can be specified for each sensor definition. Since the named sensor must point to a unique real number at a given time, the node set or element set used in the definition must contain only one member. Moreover, regardless of the user-specified output frequency, sensors are computed at every increment during the analysis. However, they are written to the output database according to the user-specified frequency. Input File Usage: Use the following options to specify a sensor definition using element output: *OUTPUT, HISTORY, SENSOR, NAME=name *ELEMENT OUTPUT element output variable Use the following options to specify a sensor definition using nodal output: *OUTPUT, HISTORY, SENSOR, NAME=name *NODE OUTPUT nodal output variable Abaqus/CAE Usage: Step module: history output request editor: Domain: Set: name, toggle on Include sensor when available Filtering output and operating on output in Abaqus/Explicit You can pre-filter element and nodal field output and element, nodal, contact, integrated, and fastener interaction history output before it is written to the output database. You can also operate on filtered or unfiltered (raw) output data to extract the maximum, minimum, or absolute maximum of the output variables over time. In addition, you can set a limit value for the output variables, and you can stop the analysis at the time this limit is reached. For field output the time at which the maximum, minimum, and absolute maximum were reached or the time when the limit was reached is output by default for each output variable. If you filter a field output request that includes many output variables and applies to the entire model, the memory requirements and the running time will both increase. For common output requests consisting of a few element output variables and a few nodal output variables the memory requirements and the running time will not increase substantially. Defining a low-pass Infinite Impulse Response digital filter You can define three types of low-pass Infinite Impulse Response filters as part of the model definition. Typical magnitude curves for analog type filters are presented in Figure 4.1.3–5, where represents the normalized cutoff frequency, which is the ratio of the cutoff frequency to the sampling frequency (the sampling frequency is the inverse of the time increment). The Butterworth filter is very common; its response in the pass band is known as maximally flat. The Type I Chebyshev filter has a sharper transition between the pass band and the stop band, but it has a ripple in the pass band. The Type II Chebyshev filter also has a sharper transition between the pass band and the stop band than a Butterworth filter of the same order, but it has a ripple in the stop band. The higher the order of the filter, the narrower the transition band. However, the computational cost increases as the order increases. In addition, for high-order filters the phase lag, which is the time delay between the filtered and unfiltered signal, may become significant. For most applications filter orders of two or four are sufficiently accurate. To define a Butterworth filter, you must specify the cutoff frequency, , and the filter order, N. Since the implementation of the filters is done using cascades of second-order sections, Abaqus expects an even number for the filter order. If you specify an odd number for the order, the order will be increased internally to the next even number. The default value for the order is two, and the highest order that can be prescribed is twenty. For the Chebyshev filters you must also specify an additional parameter, the ripple factor. The ripple factor is equal to for a Type I Chebyshev filter and is equal to for a Type II Chebyshev filter .  ⏐ ⏐ (magnitude gain) Butterworth Type I Chebyshev Type II Chebyshev passband stopband 1+ε2  c transition band (frequency) Figure 4.1.3–5 Typical magnitude curves for low-pass filters. No checks are performed to ensure that the cutoff frequency is appropriate; for example, Abaqus does not check that only the noise of the signal is eliminated. You need to know the range of the physical frequencies that are expected in the solution, and you must prescribe a cutoff frequency greater than these frequencies. In addition, the cutoff frequency should be less than half the sampling frequency; otherwise, no filtering is performed. Abaqus internally remaps (using a quadratic interpolation) the output raw data so that the filtering can satisfy the constant time-increment (sampling) requirement. You must assign each filter definition a name that can be used to refer to the filter from an output request. Input File Usage: Abaqus/CAE Usage: Use one of the following options to define a filter: *FILTER, NAME=filter_name, TYPE=BUTTERWORTH *FILTER, NAME=filter_name, TYPE=CHEBYS1 *FILTER, NAME=filter_name, TYPE=CHEBYS2 Step module: Tools→Filter→Create: Name: filter_name; Butterworth, Type I Chebyshev, or Type II Chebyshev Start-up conditions for the filter By default, the values of the variables at time zero (zero increment) are used as the initial conditions (or start-up conditions); however, you can change this initial value. Input File Usage: Use the following option to use the default initial conditions: *FILTER, NAME=filter_name, TYPE=filter_type, START CONDITION=DC Use the following option to specify the initial variable values: *FILTER, NAME=filter_name, TYPE=filter_type, START CONDITION=USER DEFINED Abaqus/CAE Usage: You cannot specify the initial variable values in Abaqus/CAE. Filtering using the low-pass Infinite Impulse Response filters To pre-filter element, nodal, contact, or integrated history output or element and nodal field output based on one of the low-pass Infinite Impulse Response filters that you defined, you refer to this filter by name from the output request. Input File Usage: Use the following option to apply a filter to an output request: Abaqus/CAE Usage: *OUTPUT, FILTER=filter_name Step module: field or history output request editor: Apply filter: filter_name Filtering the output based on the time interval For history output you can request that Abaqus/Explicit create an anti-aliasing filter that is internally based on the time interval specified in the output request. The cutoff frequency is set internally to one- sixth of the time frequency (the time frequency is the inverse of the time interval, t, used for history output). If no time intervals are specified, the default number of history output intervals is used to create the cutoff frequency of the filter. You can also use anti-aliasing filters for a field output request, but in this case the cutoff frequency is set to one-sixth of a time frequency corresponding to two hundred time intervals per step if less than two hundred field frames are requested. If more than two hundred field frames are requested, the cutoff frequency is set to one-sixth of the requested time frequency. The anti-aliasing filter is a second-order Butterworth type and a filter definition is not required. Abaqus/Explicit does not check whether the specified time interval for history output provides an appropriate cutoff frequency to build the internal filter. You should know approximately how many data points are required to describe your history curve (or signal) accurately, and Abaqus/Explicit will give you the most physical (un-aliased) representation of the signal for that number of points. Similarly for field output Abaqus/Explicit does not check whether the cutoff corresponding to two hundred sampling intervals or more (if you request more than two hundred frames) is appropriate for your analysis. If a lower (or higher) cutoff frequency is needed, you should define the filter in the model data. Filtering field output or history output written at time intervals You can apply a filter to a field output request or a history output request written at intervals of time in your analysis. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *OUTPUT, FIELD, FILTER=ANTIALIASING, TIME INTERVAL=t *OUTPUT, HISTORY, FILTER=ANTIALIASING, TIME INTERVAL=t Step module: field or history output request editor: Frequency: Every x units of time: t, Apply filter: Antialiasing Filtering field output written at evenly spaced intervals of time Input File Usage: You can apply a filter to a field output request written at evenly spaced time intervals in your analysis. *OUTPUT, FIELD, FILTER=ANTIALIASING, NUMBER INTERVAL=n Step module: field output request editor: Frequency: Evenly spaced time intervals, Interval: n, Apply filter: Antialiasing Abaqus/CAE Usage: Requesting maximum, minimum, or absolute maximum values for an output request You can apply a filter to a field output request or a history output request to obtain the maximum, minimum, or absolute maximum values for each variable in the output request. The absolute maximum option enables you to obtain the largest absolute value, negative or positive, for each variable in the output request. Abaqus evaluates maximum, minimum, or absolute maximum values at every increment during the analysis and reports these values at the time given by the output interval specified in the output request. For field output requests the last output frame will contain the maximum (or absolute maximum) value and minimum value over the entire step; the intermediate frames will show the maximum, minimum, or absolute maximum value up to the frame time. An additional output variable containing the time when the maximum, minimum, or absolute maximum occurred is output automatically for each output variable requested. This time output is written by default (and it cannot be suppressed). For field output requests Abaqus filters by default each component of tensor and vector quantities of output variable independently and provides separate maximum, minimum, or absolute maximum values for each component of the variable. You can, however, request the maximum or minimum value or apply a limit value to an invariant such as Mises stress for element output or magnitude for nodal output . Requesting maximum, minimum, or absolute maximum values for filtered output You can define a low-pass digital filter that returns the maximum, minimum, or absolute maximum value for output requests to which it is applied. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *FILTER, TYPE=filter_type, OPERATOR=MAX *FILTER, TYPE=filter_type, OPERATOR=MIN *FILTER, TYPE=filter_type, OPERATOR=ABSMAX Step module: Tools→Filter→Create: Butterworth, Type I Chebyshev, or Type II Chebyshev: Determine bounding value: Maximum, Minimum, or Absolute maximum Requesting maximum, minimum, or absolute maximum values for unfiltered output You can define a filter that returns the maximum, minimum, or absolute maximum value for output requests to which it is applied without performing any digital filtering of the data. Input File Usage: Use one of the following options: *FILTER, OPERATOR=MAX Abaqus/CAE Usage: *FILTER, OPERATOR=MIN *FILTER, OPERATOR=ABSMAX Step module: Tools→Filter→Create: Type: Operator: Determine bounding value: Maximum, Minimum, or Absolute maximum Setting an upper or lower limit on variables in an output request You can apply a filter to a field output request or a history output request to prescribe a bounding value for the variables in the output request. If any of the variables in the output request reach a value higher than the maximum limit, lower than the minimum limit, or greater than the absolute maximum limit, Abaqus returns the limiting value. The time at which the limit was reached is output separately for each requested variable. This time output is written by default (and it cannot be suppressed). Setting an upper limit or a lower limit for filtered output You can define a low-pass digital filter that enforces an upper or lower bound for the variables in the output requests to which it is applied. Input File Usage: Abaqus/CAE Usage: *FILTER, TYPE=filter_type, OPERATOR=operator_type, LIMIT=value Type: Butterworth, Type I Step module: Chebyshev, or Type II Chebyshev: Determine bounding value: Maximum, Minimum, or Absolute maximum: toggle on Bounding value limit: value Tools→Filter→Create: Setting an upper limit or a lower limit for unfiltered output You can define a filter that enforces an upper or lower bound for the variables in the output requests to which it is applied but that does not perform any Butterworth or Chebyshev filtering of the data. Input File Usage: Abaqus/CAE Usage: *FILTER, OPERATOR=operator_type, LIMIT=value Step module: Tools→Filter→Create: Type: Operator: Determine bounding value: Maximum, Minimum, or Absolute maximum: toggle on Bounding value limit: value Stopping an analysis when an output variable reaches a prescribed limit You can apply a filter to a field output request or a history output request that stops the analysis when the value of any variable in the output request reaches a specified upper bound or lower bound. Stopping an analysis of filtered output when a variable reaches a prescribed limit You can define a low-pass digital filter that stops the analysis if any of the variables in the output requests to which it is applied reach a prescribed limit. Input File Usage: *FILTER, TYPE=filter_type, OPERATOR=operator_type, LIMIT=value, HALT Abaqus/CAE Usage: Step module: Tools→Filter→Create: Butterworth, Type I Chebyshev, or Type II Chebyshev: Determine bounding value: Maximum, Minimum, or Absolute maximum: toggle on Bounding value limit: value: toggle on Stop analysis upon reaching limit Stopping an analysis of unfiltered output when a variable reaches a prescribed limit You can define a filter that does not perform any Butterworth or Chebyshev filtering of your output data and stops the analysis if any of the variables in the output requests to which it is applied reach a prescribed limit. Input File Usage: Abaqus/CAE Usage: *FILTER, OPERATOR=operator_type, LIMIT=value, HALT Step module: Tools→Filter→Create: Type: Operator: Determine bounding value: Maximum, Minimum, or Absolute maximum: toggle on Bounding value limit: value: toggle on Stop analysis upon reaching limit Applying bounding values to invariants By default, each component of a tensor or vector quantity is filtered individually and the maximum, minimum, or absolute maximum value and the limiting values are reported separately for each component. You can, however, apply a filter directly to an invariant. In this case Abaqus internally monitors the invariant you specified. Abaqus still writes the components to the output database, but these components correspond to the maximum, minimum, or limiting values of the invariant. Table 4.1.3–2 shows which invariants are available for output variable categories. Table 4.1.3–2 Invariants available for output variable categories. Category First invariant Second invariant All nodal vector output Magnitude Stress element output Mises – Press Applying bounding values to invariants of filtered output You can define a low-pass digital filter that filters the invariant. Input File Usage: *FILTER, TYPE=filter_type, OPERATOR=operator_type, LIMIT=value, INVARIANT=FIRST or SECOND Abaqus/CAE Usage: Tools→Filter→Create: Step module: Chebyshev, or Type II Chebyshev; value: Invariant: First or Second Type: Butterworth, Type I toggle on Bounding value limit: Applying bounding values to invariants of unfiltered output You can define a filter that does not perform any Butterworth or Chebyshev filtering of your output data and filters the invariant. Input File Usage: *FILTER, OPERATOR=operator_type, LIMIT=value, INVARIANT= FIRST or SECOND Abaqus/CAE Usage: Step module: Tools→Filter→Create: Bounding value limit: value: Invariant: First or Second Type: Operator; toggle on Output variables available for filtering Low-pass Infinite Impulse Response filters such as Butterworth and Chebyshev filters are intended for filtering of output variables susceptible to noise, such as accelerations and reaction forces or, to a lesser degree, stress and strain. However, digital filtering is allowed for most element and nodal output variables, and you can apply bounding values on unfiltered data for nearly all element and nodal output variables. Table 4.1.3–3 shows the set of output variables that cannot be digitally filtered but to which you can apply bounding values, and Table 4.1.3–4 shows the set of output variables for which neither digital filtering nor application of bounding values are allowed. Table 4.1.3–3 Output variables to which bounding values can be applied but digital filtering cannot be applied. Category Output variables Tensors and invariants PEEQ State and field variables TEMP, FV Energy densities ENER, SENER, PENER, CENER, VENER, DMENER Additional plasticity quantities PEQC Cracking model quantities CKSTAT Whole element variables EDT, EMSF, ELEDEN, ESEDEN, EPDDEN, ECDDEN, EVDDEN, EASEDEN, EIHEDEN, EDMDDEN, ECDDEN, ELEN, ELSE, ELCD, ELPD, ELVD, ELASE, ELIHE, ELDMD, ELDC, STATUS Nodal output variables NT, COORD Table 4.1.3–4 Output variables that cannot be digitally filtered or modified with bounding values. Category Output variables Cracking model quantities CRACK Element face variables STAGP, TRNOR, TRSHR Whole element variables GRAV, BF, SBF, P Nodal output variables CF Modal output from Abaqus/Standard You can output generalized coordinate (modal amplitude and phase) values during modal dynamic procedures to the output database. Modal output is available only as history output. Controlling the frequency of output The frequency of modal output is controlled as described above in “Controlling the output frequency in Abaqus/Standard.” Requesting output You can choose to request all modal variables applicable to the current procedure and material type. In this case any additional variables you specify are ignored. Input File Usage: Abaqus/CAE Usage: *MODAL OUTPUT, VARIABLE=ALL Step module: history output request editor: All Surface output in Abaqus/Standard and Abaqus/Explicit You can write variables associated with surfaces in contact, coupled thermal-electrical-structural (Abaqus/Standard only), coupled thermal-electrical, and crack propagation problems to the output database. Multiple output requests can be used to customize requests among interactions, surfaces, or node sets. For surface variables associated with cavity radiation, coupled temperature-displacement see “Cavity radiation output (Abaqus/Standard only), in Abaqus/Standard” below. Use element output requests to obtain database output for contact elements (such as gap elements; see “Gap contact elements,” Section 39.2.1). In Abaqus/Standard contact history output cannot be saved in a linear perturbation step with frequency extraction. Displacement nodal output is generated automatically in Abaqus/Explicit when requesting surface output. Selecting the surface output variables The surface variables that can be written to the output database are listed in the “Surface variables” section of “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. Input File Usage: *CONTACT OUTPUT list of output variables Abaqus/CAE Usage: Step module: field or history output request editor: Select from list below Limiting the extent of a surface output request in Abaqus/Standard Output requests apply to general contact and all contact pair interactions in a model by default in Abaqus/Standard. Options to limit an output request to certain interactions are discussed below. Limiting output to a node set in Abaqus/Standard You can limit a surface output request to apply to a subset of surface nodes involved in contact pairs or general contact in Abaqus/Standard. Input File Usage: Abaqus/CAE Usage: *CONTACT OUTPUT, NSET=node_set_name Step module: field or history output request editor: Domain: Interaction: contact_interaction_name Limiting output for contact pairs based on slave and master surface names in Abaqus/Standard You can limit output to certain contact pairs based on surface names. If you specify both the slave and master surface names, the output request is limited to a specific contact pair. If you specify the slave surface but not the master surface, output is written for all contact pairs that involve the specified slave surface. If you also specify a node set, the applicability of an output request is further limited (i.e., the output request will generate output only for certain nodes of a certain contact pair (or pairs). Output requests with a specific slave and/or master surface role specified will not generate output for general contact. Input File Usage: *CONTACT OUTPUT, MASTER=master, SLAVE=slave, NSET=node_set_name Abaqus/CAE Usage: Step module: field or history output request editor: Domain: Interaction: contact_interaction_name Limiting the extent of a surface field output request in Abaqus/Explicit Field output requests apply to general contact and all contact pair interactions in a model by default in Abaqus/Explicit. Options to limit a surface field output request to certain interactions are discussed below. Limiting surface field output to a contact pair set in Abaqus/Explicit In Abaqus/Explicit you can select the contact pairs for which surface field output is desired. Surface output is contact pair-specific, so that contact output for a particular surface involved in a selected contact pair will include only the contributions from that contact pair if the surface is involved in multiple contact pairs. Surface output is available only for discrete (node-based or element-based) surfaces; it is not available for any analytical surfaces within a contact pair. Input File Usage: Use the following option to request surface field output for a particular contact pair set: *CONTACT OUTPUT, CPSET=contact_pair_set_name Abaqus/CAE Usage: Step module: field output request editor: Domain: Interaction: contact_interaction_name Limiting surface field output to general contact in Abaqus/Explicit You can limit surface field output requests to apply only to general contact in Abaqus/Explicit, but you cannot further limit this output to a subset of the general contact domain. *CONTACT OUTPUT, GENERAL CONTACT You cannot limit surface field output to general contact in Abaqus/CAE. Abaqus/CAE Usage: Input File Usage: Limiting surface field output to a single surface in Abaqus/Explicit You can limit surface field output requests to a single surface in the general contact domain in Abaqus/Explicit. The contact output for the specified surface will include all the contributions from other contact surfaces interacting with the surface. Input File Usage: Abaqus/CAE Usage: *CONTACT OUTPUT, SURFACE=surface_name You cannot limit a single surface output to general contact in Abaqus/CAE. Limiting surface field output to pairwise surfaces in Abaqus/Explicit You can specify a pair of surfaces in the general contact domain in Abaqus/Explicit for which the interactions on one surface due to the contact with another surface will be output. This type of output cannot be used for surfaces involving Eulerian regions. Input File Usage: *CONTACT OUTPUT, SURFACE=first_surface_name, SECOND SURFACE=second_surface_name Abaqus/CAE Usage: You cannot limit pairwise surface output to general contact in Abaqus/CAE. Specifying surface history output regions in Abaqus/Explicit You must specify an interaction to which a surface history output request applies with one of the methods discussed below. Specifying surface history output by contact pair set in Abaqus/Explicit In Abaqus/Explicit you can select the contact pairs for which surface history output is desired. Surface output is contact pair-specific, so that contact output for a particular surface involved in a selected contact pair will include only the contributions from that contact pair if the surface is involved in multiple contact pairs. Surface output is available only for discrete (node-based or element-based) surfaces; it is not available for any analytical surfaces within a contact pair. Input File Usage: Abaqus/CAE Usage: Use the following option to request surface history output for a particular contact pair: *CONTACT OUTPUT, CPSET=contact_pair_set_name Step module: history output request editor: Domain: Interaction: contact_interaction_name Specifying whole surface history output in Abaqus/Explicit You can specify a surface in the general contact domain for which whole surface contact force resultants will be output. Whole surface contact force resultants for a surface in the general contact domain are available only as history output. Input File Usage: Abaqus/CAE Usage: *CONTACT OUTPUT, SURFACE=surface_name Step module: history output request editor: Domain: General contact surface: surface_name Specifying pairwise surface history output in Abaqus/Explicit You can specify a pair of surfaces in the general contact domain for which the resultant contact forces on one surface due to the contact with another surface will be output. The contact force resultants in this case consider only the contact interactions between the two specified surfaces. This type of output cannot be requested for surfaces involving Eulerian regions. Input File Usage: *CONTACT OUTPUT, SURFACE=first_surface_name, SECOND SURFACE=second_surface_name Abaqus/CAE Usage: You cannot request surface history output for a pair of surfaces in Abaqus/CAE. Specifying surface history output by fastened node set in Abaqus/Explicit You can select a fastened node set for which bond history output is desired: Input File Usage: Use the following option to request surface history output for a particular fastened node set: Abaqus/CAE Usage: *CONTACT OUTPUT, NSET=node_set_name You cannot request surface history output for a particular fastened node set in Abaqus/CAE. Controlling the output frequency The frequency of surface output is controlled as described above in “Controlling the output frequency.” Requesting preselected output You can request the preselected, procedure-specific surface output variables described in Table 4.1.3–1. In this case you can specify additional variables as part of the output request. Alternatively, you can request all surface variables applicable to the current procedure. In this case any additional variables you specify are ignored. Input File Usage: Use the following option to request the preselected surface output variables: *CONTACT OUTPUT, VARIABLE=PRESELECT Use the following option to request all applicable surface output variables: *CONTACT OUTPUT, VARIABLE=ALL Abaqus/CAE Usage: Step module: field or history output request editor: Preselected defaults or All Surface output in Abaqus/CFD You can write field and history output variables associated with surfaces in an Abaqus/CFD analysis to the output database. Selecting the surface output variables The surface variables that can be written to the output database are listed in the “Surface variables” section of “Abaqus/CFD output variable identifiers,” Section 4.2.3. Input File Usage: *SURFACE OUTPUT, SURFACE=surface_set_name list of output variables Abaqus/CAE Usage: You cannot request surface output in Abaqus/CAE. Controlling the output frequency The frequency of surface output is controlled as described above in “Controlling the output frequency.” Time incrementation output in Abaqus/Explicit You can output incrementation variables for an Abaqus/Explicit analysis to the output database. Incrementation output is available only as history output. Selecting the incrementation output variables The available incrementation output variables are the Abaqus/Explicit time increment size, DT; the percent change in mass of the model due to mass scaling, DMASS; and the steady-state detection variables SSPEEQ, SSSPRD, SSFORC, and SSTORQ. Input File Usage: *INCREMENTATION OUTPUT list of output variables Abaqus/CAE Usage: Step module: history output request editor: Select from list below Controlling the output frequency The frequency of incrementation output is controlled as described above in “Controlling the output frequency for history output in Abaqus/Explicit.” Requesting preselected output You can request the preselected, procedure-specific incrementation output variables. In this case you can specify additional variables as part of the output request. Alternatively, you can request all incrementation variables applicable to the current procedure type. In this case any additional variables you specify are ignored. Input File Usage: Abaqus/CAE Usage: Use the following option to request the preselected incrementation output variables: *INCREMENTATION OUTPUT, VARIABLE=PRESELECT Use the following option to request all applicable incrementation output variables: *INCREMENTATION OUTPUT, VARIABLE=ALL Step module: history output request editor: Preselected defaults or All Cavity radiation output in Abaqus/Standard You can request that cavity-, element-, or surface-based output such as radiation fluxes, viewfactor totals for a facet, and facet temperatures from an Abaqus/Standard analysis be written to the output database. The output request can be repeated as often as necessary to define output for different variables, different cavities, different element sets, different surfaces, etc. Selecting the radiation output variables The radiation output variables that can be written to the output database are listed in the “Cavity radiation variables” section of “Abaqus/Standard output variable identifiers,” Section 4.2.1. Input File Usage: *RADIATION OUTPUT list of output variables Abaqus/CAE Usage: Cavity radiation output requests are not supported in Abaqus/CAE. Selecting the region of the model for which radiation output is required You can specify the cavity, element set, or surface for which radiation output is required. Each radiation output request can apply to only one type of region. If you do not specify a region of the model, radiation variables are output for all the cavities in the model. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *RADIATION OUTPUT, CAVITY=cavity_name *RADIATION OUTPUT, ELSET=element_set_name *RADIATION OUTPUT, SURFACE=surface_name Cavity radiation output requests are not supported in Abaqus/CAE. Controlling the output frequency The frequency of radiation output is controlled as described above in “Controlling the output frequency.” Requesting output You can request all radiation variables applicable to the current procedure. In this case any additional variables you specify are ignored. Input File Usage: Abaqus/CAE Usage: *RADIATION OUTPUT, VARIABLE=ALL Cavity radiation output requests are not supported in Abaqus/CAE. Examples The examples that follow illustrate how to request multiple types of output over multiple steps in both Abaqus/Standard and Abaqus/Explicit. Abaqus/Standard example The input listing below will produce both field and history output for Step 1. Field output will be written every 2 increments. This field output request consists of preselected element variables for the whole model, as well as the variable PEQC. In addition, plastic strains will be written out for element set SMALL, and the nodal variables U and RF will be written to the output database for node set NSMALL. History output will be written every increment. The variables ALLKE, ALLSE, and ALLWK will be written for the whole model. In addition, ALLPD will be written for element set SMALL. In Step 2 the history output request defined in Step 1 is replaced by a request for the energy variables ALLKE, ALLPD, and ALLSE for element set SMALL. The history output request defined in Step 1 is removed. The field output request defined in Step 1 is passed into Step 2 unchanged, but another field output request for element energies at every increment is added. *STEP *STATIC ... ... *OUTPUT, FIELD, FREQUENCY=2 *ELEMENT OUTPUT, VARIABLE=PRESELECT PEQC, *ELEMENT OUTPUT, ELSET=SMALL PE, *NODE OUTPUT, NSET=NSMALL U, RF *OUTPUT, HISTORY, FREQUENCY=1 *ENERGY OUTPUT ALLKE, ALLSE, ALLWK *ENERGY OUTPUT, ELSET=SMALL ALLPD *END STEP *STEP *STATIC ... ... *OUTPUT, HISTORY, OP=REPLACE, FREQUENCY=1 *ENERGY OUTPUT, ELSET=SMALL ALLKE, ALLPD, ALLSE *OUTPUT, FIELD, OP=ADD, FREQUENCY=1 *ELEMENT OUTPUT ELEN *END STEP Abaqus/Explicit example The input listing below will produce both field and history output for Step 1. Field output will be written at 5 equally spaced intervals, and the time marks will be hit exactly. This field output request consists of preselected element variables for the whole model, as well as the variable PEQC. In addition, plastic strains will be written out for element set SMALL, and the nodal variables U and RF will be written to the output database for node set NSMALL. History output will be written at a time interval of 0.005. The Abaqus/Explicit time step, DT, will be written, along with the variables ALLKE, ALLSE, and ALLWK for the whole model. The output variables SOAREA and SOF integrated over the surface CROSS_SECTION1 will be written. The preselected variables SOF and SOM integrated over the surface CROSS_SECTION2 defined by the integrated output section SECTION1 will be written in the local coordinate system LOCALSYSTEM. In addition, ALLPD will be written for element set SMALL. In Step 2 the history output request defined in Step 1 is replaced by a request for the energy variables ALLKE, ALLPD, and ALLSE for element set SMALL. The history output request defined in Step 1 is removed. The field output request defined in Step 1 is passed into Step 2 unchanged, but another field output request for element energies at 10 equally spaced intervals is added. *STEP *DYNAMIC, EXPLICIT,.1... ... *OUTPUT, FIELD, NUMBER INTERVAL=5, TIME MARKS=YES *ELEMENT OUTPUT, VARIABLE=PRESELECT PEQC, *ELEMENT OUTPUT, ELSET=SMALL PE, *NODE OUTPUT, NSET=NSMALL U, RF *OUTPUT, HISTORY, TIME INTERVAL=0.005 *INCREMENTATION OUTPUT DT *ENERGY OUTPUT ALLKE, ALLSE, ALLWK *ENERGY OUTPUT, ELSET=SMALL ALLPD *INTEGRATED OUTPUT, SURFACE=CROSS_SECTION1 SOF, SOAREA *INTEGRATED OUTPUT SECTION, NAME=SECTION1, SURFACE=CROSS_SECTION2, ORIENTATION=LOCALSYSTEM *INTEGRATED OUTPUT, SECTION=SECTION1, VARIABLE=PRESELECT *END STEP *STEP *DYNAMIC, EXPLICIT,.1... ... *OUTPUT, HISTORY, OP=REPLACE, TIME INTERVAL=0.005 *ENERGY OUTPUT, ELSET=SMALL ALLKE, ALLPD, ALLSE *OUTPUT, FIELD, OP=ADD, NUMBER INTERVAL=10 *ELEMENT OUTPUT ELEN *END STEP 4.1.4 ERROR INDICATOR OUTPUT Products: Abaqus/Standard Abaqus/CAE WARNING: Error indicator output variables are approximate and do not represent an accurate or conservative estimate of your solution error. The quality of an error indicator can be particularly poor if your mesh is coarse. The error indicator quality improves as you refine the mesh; however, you should never interpret these variables as indicating what the value of a solution variable would be upon further refinement of the mesh. References • “Abaqus/Standard output variable identifiers,” Section 4.2.1 • “Adaptive remeshing: overview,” Section 12.3.1 • “Selection of error indicators influencing adaptive remeshing,” Section 12.3.2 • *CONTACT OUTPUT • *ELEMENT OUTPUT Overview Error indicator output variables: • indicate discretization error in a solution quantity (the base solution) and have units of the base solution; • can be requested with element output or contact output options or as part of an adaptive remeshing rule; • can be normalized by forms of the base solution to obtain nondimensional, such as percentage, indicators of error; • can increase your analysis solution time significantly in some cases; and • are available in Abaqus/Standard but not Abaqus/Explicit. Solution accuracy The ability of a finite element analysis to make useful predictions of physical behavior depends on many factors, including: • representation of geometry, material behavior, load history, and various other modeling aspects associated with describing the problem posed; • spatial and temporal discretization (mesh refinement and incrementation); and • convergence tolerances. The primary focus of this section is spacial discretization error. Discussion to help understand and control other potential sources of error appears in “Convergence criteria for nonlinear problems,” Section 7.2.3, “Time integration accuracy in transient problems,” Section 7.2.4, “Evaluating hyperelastic and viscoelastic material behavior,” Section 12.4.7 of the Abaqus/CAE User’s Manual, and other portions of the Abaqus documentation. You should perform a detailed study of your analysis methods and assumptions as part of any error assessment. Spatial discretization error The finite element discretization of a model domain results in an approximation to the exact solution for all but trivial analyses. To aid you in understanding the extent and spatial distribution of the discretization error in a finite element solution, Abaqus/Standard provides a set of error indicator output variables. Ideally, error indicator output variables should be supplemented by other techniques, such as a mesh refinement study, to gain confidence that discretization error is not significantly degrading the ability of the finite element analysis to make useful predictions. In fact, error indicators can help automate a mesh refinement study through the adaptive remeshing functionality of Abaqus/CAE; error indicators variables are used by this functionality to determine where to refine or coarsen a mesh . Error indicator and base solution variables available in Abaqus/Standard Abaqus error indicator variables provide a measure of the local error resulting from mesh discretization. Each error indicator, . For example, the Mises stress error indicator, MISESERI, provides an indicator of error in the Mises stress variable MISESAVG. Table 4.1.4–1 shows the available error indicator variables and the corresponding base solution variables. , provides an indication of error in a particular base solution variable, Table 4.1.4–1 Error indicator variables and their corresponding base solution variables. Solution Quantity Error indicator Element energy density Mises stress Contact pressure Contact shear stress Equivalent plastic strain Plastic strain Creep strain Heat flux Electric flux Electric potential gradient variable ( ) ENDENERI MISESERI CPRESSERI CSHEARERI PEEQERI PEERI CEERI HFLERI EFLERI EPGERI 4.1.4–2 Base solution variable ( ) ENDEN MISESAVG CPRESS CSHEAR PEEQAVG PEAVG CEAVG HFLAVG EFLAVG The algorithms used by Abaqus/CAE to modify mesh seed sizes for the adaptive remeshing capability consider error indicator values and corresponding base solution values together. When you create a remeshing rule and request a particular error indicator, Abaqus automatically writes the error indicator and corresponding base solution variable to the output database. Input File Usage: Abaqus/CAE Usage: *OUTPUT, FIELD, ELSET=ElsetName *ELEMENT OUTPUT *CONTACT OUTPUT Step module: Output→Field Output Request Or, if you use the following option to specify an adaptive remeshing rule, the associated error indicator and base solution output will occur by default: Mesh module: Create Remeshing Rule: Step and Indicator Effect of error indicator output requests on solution time Abaqus/Standard determines error indicator variables based on the difference between a smoothed and unsmoothed distribution of the base solution, using a smoothing technique such as the patch recovery technique of Zienkiewicz and Zhu, (1987). The smoothing calculations occasionally noticeably increase analysis time. If you find that adding an error indicator output request significantly increases analysis time, strategies for reducing this effect include reducing the output frequency and limiting the output request to a particular region of interest. Computations for most error indicator variables only occur just prior to writing the error indicator variable to the output database, so reducing the output frequency will tend to reduce the computation time; however this is not the case for the element energy density error indicator, because contributions to this error indicator are accumulated each increment regardless of whether this error indicator is output for a given increment. Additional considerations for extent of output requests for element error indicator variables When you request element error indicator output, the request should only apply to elements supported for error indicator output. The patch recovery technique used to compute element error indicator variables assumes that the solution should be continuous over the element set specified. Abaqus/Standard confirms that your error indicator output specification is consistent with this assumption by checking section property references within the error indicator domain and issues a warning message if the elements in the provided element set refer to distinct section definitions. You can safely ignore this warning if the sections are identical in their properties. Interpreting error indicator output When interpreting error indicator output, you should remember that the error indicators are approximate measures of the local error in the base solution and are, themselves, subject to discretization error. The accuracy of the error estimates tends to improve as the mesh is refined. Each error indicator variable has the same units has the corresponding base solution variable, which facilitates comparison of local estimates of the error magnitude with local estimates of the base solution. Regions of interest of a base solution and corresponding error indicator Viewing contour plots of a base solution variable and corresponding error indicator variable side-by-side can provide a useful perspective on the solution accuracy. For example, if the base solution is expressed in units of stress, the corresponding error indicator is also expressed in units of stress. Figure 4.1.4–1 shows contour plots of CPRESS and CPRESSERI for an analysis of a sphere pressed into a rigid plate. These plots can be interpreted as follows: • The contact pressure solution is quite accurate near the center of the active contact region, where the contact pressure is largest, because the error indicator is a small fraction of the base solution in that region. • The contact pressure solution is less accurate near the perimeter of the active contact region, where local variations in the contact pressure solution are largest (but the contact pressure is significantly less than the maximum value), because the error indicator is quite large compared to the base solution in that region. The analyst may judge that the level of mesh refinement is adequate if the maximum contact pressure is of primary interest in such a case. Local mesh refinement would be needed to accurately predict the maximum contact pressure if the active contact region was significantly smaller than that shown in Figure 4.1.4–1. CPRESS CPRESSERI +6.1e+04 +5.4e+04 +4.8e+04 +4.2e+04 +3.6e+04 +3.0e+04 +2.4e+04 +1.8e+04 +1.2e+04 +6.1e+03 +0.0e+00 +1.6e+04 +1.4e+04 +1.3e+04 +1.1e+04 +9.7e+03 +8.0e+03 +6.4e+03 +4.8e+03 +3.2e+03 +1.6e+03 +0.0e+00 Figure 4.1.4–1 Contour plots of CPRESS and CPRESSERI for contact between a deformable sphere and a rigid plate. An error indicator tends to give a crude, non-conservative approximation of the deviation from the exact solution if the mesh is coarse relative to local solution variations or the exact solution to the problem posed involves a stress singularity. The following qualitative interpretations of error indicator results exceeding approximately 10% of base solution results are often appropriate: • “Significant potential for solution inaccuracy exists in this region.” • “The mesh may be too coarse to give a good estimate of solution error in this region.” • “Perhaps a stress singularity exists at this corner.” Calculating normalized measures of solution error You can use corresponding error indicator and base solution variables, a field of local, normalized error indicators: and , respectively, to compute where is a normalized error measure. For example, provides a percentage form of the Mises stress-based error indicator; however this normalized error measure may not be particularly useful, because it: • will tend to draw attention to regions where base solution values are small, which typically are not critical regions of a design; and • will have divide-by-zero issues where the base solution value is zero. Other normalization approaches, such as normalizing based on a global norm of the base solution variable or a constant value that you choose (such as the maximum value of the base solution allowed in a design), may be more effective. Normalized forms of an error indicator are not available directly through the error indicator output variables; however, you can calculate normalized measures using the Visualization module of Abaqus/CAE (Abaqus/Viewer) to operate on field output data. For more information, see “Building valid field output expressions,” Section 42.7.1 of the Abaqus/CAE User’s Manual. Alternatively, you can use the Abaqus Scripting Interface to read the error indicator and the base solution from the output database and calculate normalized forms. For more information, see Chapter 9, “Using the Abaqus Scripting Interface to access an output database,” of the Abaqus Scripting User’s Manual. Limitations Only the following element types are supported for error indicator computations: • Planar continuum triangles and quadrilaterals • Shell triangles and quadrilaterals • Tetrahedrals • Hexahedrals Elements with variable nodes are not supported. Additional reference • Zienkiewicz, O. C., and J. Z. Zhu, “A Simple Error Estimator and Adaptive Procedure for Practical Engineering Analysis,” International Journal for Numerical Methods in Engineering, vol. 24, pp. 337–357, 1987. 4.2 Output variables • “Abaqus/Standard output variable identifiers,” Section 4.2.1 • “Abaqus/Explicit output variable identifiers,” Section 4.2.2 • “Abaqus/CFD output variable identifiers,” Section 4.2.3 4.2.1 Abaqus/Standard OUTPUT VARIABLE IDENTIFIERS Product: Abaqus/Standard References • “Output,” Section 4.1.1 • “Output to the data and results files,” Section 4.1.2 • “Output to the output database,” Section 4.1.3 Overview The tables in this section list all of the output variables that are available in Abaqus/Standard. These output variables can be requested for output to the data (.dat) and results (.fil) files or as either field- or history-type output to the output database (.odb) file . As noted specifically in the tables, a few of the output variables are written only to the output database and restart (.res) files (they are not available for output to the data or results files). These variables can be accessed only in the Visualization module of Abaqus/CAE (Abaqus/Viewer). Each table contains one variable type: • Element integration point variables • Element centroidal variables • Element section variables • Whole element variables • Whole element energy density variables • Nodal variables • Modal variables • Surface variables • Cavity radiation variables • Section variables • Whole and partial model variables • Solution-dependent amplitude variables • Structural optimization variables Symbols used in the tables The availability of the various output variable identifiers is defined by a under the following headings: in the columns of the table, .dat means that the identifier can be used as a data file output selection. .fil means that the identifier can be used as a results file output selection. .odb Field means that the identifier can be used as a field-type output selection to the output database. .odb History means that the identifier can be used as a history-type output selection to the output database. The appearance of a in the .dat, .fil, or .odb columns indicates that the variable cannot be requested by name but that it will be written to the data, results, or output database file according to the conditions specified in the table for that particular variable type. Requesting output of components Variable identifiers of the form ABCn can be used with highest value of n is determined by the type of variable. Similarly, variable identifiers of the form DEF can be used for the ranges of i and j indicated (DEF11, DEF12, (ABC1, ABC2, …), where the ). Individual components cannot be requested in the results (.fil) file. For postprocessing of a particular component of a variable, request file output for all components of the variable. Output for individual variables can be requested during postprocessing. Individual components of variables can be requested as history-type output in the output database for X–Y plotting in Abaqus/CAE. Individual component requests to the output database are not available for field-type output, with the exception of state, field, and user-defined variables (SDVn, FVn, and UVARMn). If a particular component is desired for contouring in Abaqus/CAE, request field output of the generic variable (e.g., S for stress). Output for individual components of field output can be requested within the Visualization module of Abaqus/CAE. Direction definitions The direction definitions depend on the variable type. Direction definitions for element variables For components of stress, strain, and other tensor quantities 1, 2, and 3 refer to the directions in an orthogonal coordinate system. These directions are global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam elements. For finite-membrane-strain shell elements, membrane elements, and continuum elements associated with a local orientation , the local output directions rotate with the average rotation of the element (integral with respect to time of the spin—see “Stress rates,” Section 1.5.3 of the Abaqus Theory Manual). Tensor components in these cases are output in the rotating local directions. In some cases the local output directions may differ from one integration point to the next within an element. Abaqus/Standard does not take this variation into account when extrapolating output variables to the nodes, which affects output such as element quantities averaged at the nodes or contour plots of individual tensor components. Invariant quantities at the integration points will not be influenced by the local output directions. You can control writing the local directions to the output database file or to the results file . By default, the local directions are written to the output database for all frames that include element field output. The local (material) directions (averaged at the nodes) can be visualized in Abaqus/CAE by selecting Plot→Material Orientations in the Visualization module. The directions can be printed to the data file by using user subroutine UVARM. Direction definitions for equivalent rigid body variables For all equivalent rigid body variables 1, 2, and 3 refer to global directions. Direction definitions for nodal variables For nodal variables 1, 2, and 3 are global directions (1=X, 2=Y, and 3=Z; or for axisymmetric elements, 1=r and 2=z). If a local coordinate system is defined at a node , you can specify whether output to the data or results file of vector-valued quantities at these nodes is in the local or global system . By default, nodal output is written to the data file in the local system, whereas it is written to the results file in the global system (since this is more convenient for postprocessing). If nodal field output is requested for a node that has a local coordinate system defined, a quaternion representing the rotation from the global directions is written to the output database. Abaqus/CAE automatically uses this quaternion to transform the nodal results into the local directions. Nodal history data written to the output database are always stored in the global directions. Direction definitions for integrated variables For components of total force, total moment, and similar variables obtained through integration over a surface, the directions 1, 2, and 3 refer to directions in an orthogonal coordinate system. A fixed global coordinate system is used if the surface is specified directly for the integrated output request. If the surface is identified by an integrated output section definition that is associated with the integrated output request, a local coordinate system in the initial configuration can be specified and can translate or rotate with the deformation. Distributed load output You need to be aware of limitations that may be encountered when distributed load output is requested. Distributed load output and user subroutines Output can be requested for many of the distributed loads discussed in “Loads,” Section 33.4. However, contributions to these loads defined through user subroutines (see “Abaqus/Standard subroutines,” Section 1.1 of the Abaqus User Subroutines Reference Manual) are not displayed, except for the variables FILMCOEF and SINKTEMP. Distributed load output with modal procedures For modal procedures only the magnitude of the load is written to the output database. Strain output The total strain E is composed of the elastic strain EE, the inelastic strain IE, and the thermal strain THE. The inelastic strain IE consists of the plastic strain PE and the creep strain CE. For geometrically nonlinear analysis Abaqus/Standard makes it possible to output different strain measures as well as elastic and various inelastic strains. The various total strain measures (integrated strain measure E, nominal strain measure NE, and logarithmic strain measure LE) are described in “Conventions,” Section 1.2.2. The default strain measure for output to the data (.dat) and results (.fil) files is E. However, for geometrically nonlinear analysis using element formulations that support finite strains, E is not available for output to the output database (.odb) file, and LE is the default strain measure. Temperature output In Abaqus temperature can either be a field variable (stress analysis, mass diffusion, …) or a degree of freedom (heat transfer analysis, fully coupled temperature-displacement analysis, …). For any analysis that involves temperature, you can request the temperature either at nodes (variable NT) or in elements (variable TEMP). If element temperature output is requested at the nodes, the integration point values are extrapolated and, if requested, averaged. These extrapolated values are generally not as accurate as the nodal temperatures themselves. An exception to this is adiabatic analysis, in which the element temperatures change due to plastic heat generation but the nodal temperatures are not updated. In that case the current nodal temperatures are obtained only if element temperature output is requested at the nodes. For continuum elements there is only one temperature value per node (NT11). For shells and beams more than one temperature is available for each node (NT11, NT12, …) since a temperature gradient can exist through the thickness of a shell or across the cross-section of a beam. In general, variables NT12, NT13, etc. contain temperature values. However, when temperature is defined by specifying temperature gradients, nodal temperatures for a given section point can be obtained only by using the variable TEMP. See “Specifying temperature and field variables” in “Using a beam section integrated during the analysis to define the section behavior,” Section 29.3.6, and “Specifying temperature and field variables” in “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, for discussions on specifying temperatures in beams and shells. Principal value output Output of the principal values can be requested for stresses, strains, and other material tensors. Either all principal values or the minimum, maximum, or intermediate values can be obtained. All principal values of tensor ABC are obtained with the request ABCP. The minimum, intermediate, and maximum principal values are obtained with the requests ABCP1, ABCP2, and ABCP3. For three-dimensional, (generalized) plane strain, and axisymmetric elements all three principal values are obtained. For plane stress, membrane, and shell elements, the out-of-plane principal value cannot be requested for history-type output. For field-type output, Abaqus/CAE always reports the out- of-plane principal value as zero. Principal values cannot be obtained for truss elements or for any beam elements other than the three-dimensional beam elements with torsional shear stresses. If a principal value or an invariant is requested for field-type output, the output request is replaced with an output request for the components of the corresponding tensor. Abaqus/CAE calculates all principal values and invariants from these components. If a principal value is desired as history-type output, it must be explicitly requested since Abaqus/CAE does no calculations on history data. Tensor output Tensor variables that are written to the output database as field-type output are written as components in either the default directions defined by the convention given in “Orientations,” Section 2.2.5 (global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam elements), or the user-defined local system. Abaqus/CAE calculates all principal values and invariants from these components. See “Writing field output data,” Section 9.6.4 of the Abaqus Scripting User’s Manual, for a description of the different types of tensor variables. For plane stress, membrane, and shell elements, only the in-plane tensor components (11, 22, and 12 components) are stored by Abaqus/Standard. The out-of-plane direct component for stress (S33) is reported as zero to the output database as expected, and the out-of-plane component of strain (E33) is reported as zero even though it is not. This is because the thickness direction is computed based on section properties rather than at the material level. The out-of-plane components can be requested for field-type output and cannot be requested for history-type output. The out-of-plane stress components are not reported to the data (.dat) file or to the results (.fil) file. For three-dimensional beam elements with torsional shear stresses, only the axial and the torsional components (the 11 and 12 components) are stored by Abaqus/Standard. The other direct component (the 22 component) is reported as zero for field-type output and cannot be requested for history-type output. The components for tensor variables are written to the output database in single precision. Therefore, a small amount of precision roundoff error may occur when calculating the variables’ principal values. Such roundoff error may be observed, for example, when analytically zero values are calculated as relatively small nonzero values. Element integration point variables You can request element integration point variable output to the data, results, or output database file . Identifier .dat .fil .odb Field History Description Tensors and associated principal values and invariants • • All stress components. • • • • • • Sij SP SPn SINV MISES MISESMAX MISESONLY • • • • • • • • • • -component of stress ( ). All principal stresses. Minimum, stresses (SP1 SP2 SP3). intermediate, and maximum principal • • All stress invariant components (MISES, TRESC, PRESS, INV3). For field output SINV is converted to a request for the generic variable S. Mises equivalent stress, defined as where is the deviatoric stress tensor, defined as where is the stress, p is the equivalent pressure stress (defined below), and is a unit matrix. In index notation where Kronecker delta. , , and is the Maximum Mises stress among all of the section points. For a shell element it represents the maximum Mises value among all the section points in the layer, for a beam element it is the maximum Mises stress among all the section points in the cross-section, and for a solid element it represents the Mises stress at the integration points. Mises equivalent stress. When MISESONLY is used the stress components are not instead of MISES, written to the output database; consequently, the size of the database is reduced. Identifier .dat .fil .odb Field History Description Tresca equivalent stress, defined as the maximum difference between principal stresses. Equivalent pressure stress, defined as Equivalent pressure stress. When PRESSONLY is used instead of PRESS, the stress components are not written to the output database; consequently, the size of the database is reduced. Third stress invariant, defined as where of Mises equivalent stress, above. is the deviatoric stress defined in the context Stress triaxiality, All total kinematic hardening shift tensor components. . -component of the total shift tensor ( ). All ( kinematic hardening shift tensor components ). kinematic hardening shift -component of the and ). tensor ( All tensor components of all the kinematic hardening shift tensors, except the total shift tensor, ALPHA. All principal values of the total shift tensor. Minimum, values of ALPHAP2 ALPHAP3). All strain components. For geometrically nonlinear analysis using element formulations that support finite strains, E is not available for output to the output database (.odb) file. intermediate, and maximum principal tensor the total (ALPHAP1 shift -component of strain ( ). All principal strains. Minimum, strains (EP1 All nominal strain components. EP3). EP2 intermediate, and maximum principal -component of nominal strain ( ). 4.2.1–7 TRESC PRESS PRESSONLY INV3 TRIAX ALPHA ALPHAij ALPHAk ALPHAk_ij ALPHAN ALPHAP ALPHAPn Eij EP EPn NE NEij • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Identifier .dat .fil .odb Field History Description intermediate, and maximum principal All principal nominal strains. Minimum, nominal strains (NEP1 NEP2 NEP3). All logarithmic strain components. For geometrically nonlinear analysis using element formulations that support finite strains, LE is the default strain measure for output to the output database (.odb) file. -component of logarithmic strain ( ). All principal logarithmic strains. Minimum, logarithmic strains (LEP1 All mechanical strain rate components. LEP2 LEP3). intermediate, and maximum principal -component of strain rate ( ). ERP2 ERP3). intermediate, and maximum principal All principal mechanical strain rates. Minimum, mechanical strain rates (ERP1 All components of the total deformation gradient. hyperfoam, Available and material models defined in user subroutine UMAT. For fully integrated first-order quadrilaterals and hexahedra, the selectively reduced integration technique is used. A modified deformation gradient is output for these elements. hyperelasticity, only for -component of the total deformation gradient ( ). Principal stretches. Minimum, principal stretches (DGP1 DGP2 DGP3). All elastic strain components. intermediate, and maximum values of -component of elastic strain ( ). All principal elastic strains. Minimum, elastic strains (EEP1 All inelastic strain components. EEP2 EEP3). intermediate, and maximum principal -component of inelastic strain ( ). All principal inelastic strains. 4.2.1–8 NEP NEPn LE LEij LEP LEPn ER ERij ERP ERPn DG DGij DGP DGPn EE EEij EEP EEPn IE IEij IEP • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Identifier .dat .fil .odb Field History Description Minimum, inelastic strains (IEP1 IEP2 IEP3). intermediate, and maximum principal All thermal strain components. -component of thermal strain ( ). All principal thermal strains. Minimum, thermal strains (THEP1 intermediate, and maximum principal THEP2 THEP3). All plastic strain components. This identifier also provides PEEQ, a yes/no flag telling if the material is currently yielding or not (AC YIELD: “actively yielding”; that is, the plastic strain changed during the increment), and PEMAG when PE is requested for the data or results files. When PE is requested for field output to the output database, PEEQ is also provided. -component of plastic strain ( ). Equivalent plastic strain. This identifier also provides a yes/no flag (1/0 on the output database) telling if the material is currently yielding or not (AC YIELD: “actively yielding”; that is, the plastic strain changed during the increment). The equivalent plastic strain is defined as , where is the initial equivalent plastic strain. The definition of model. For classical metal depends on the material (Mises) plasticity . For other plasticity models, see the appropriate section in Part V, “Materials.” When plasticity occurs in the thickness direction to a gasket element whose plastic behavior is specified as part of a gasket behavior definition, PEEQ is PE11. Maximum equivalent plastic strain, PEEQ, among all of the section points. For a shell element it represents the maximumPEEQ value among all the section points in the layer, for a beam element it is the maximum PEEQ among all the section points in the cross-section, 4.2.1–9 • • • • • • • • • • • • • IEPn THE THEij THEP THEPn PE PEij PEEQ • • • • • • • • • • • Identifier .dat .fil .odb Field History Description • • • • • • • • • • • • • • • and for a solid element it represents thePEEQ at the integration points. Equivalent plastic strain in uniaxial tension for cast iron, Mohr-Coulomb tension cutoff, and concrete damaged plasticity, which is defined as . This identifier also provides a yes/no flag (1/0 on the output database) telling if the material is currently yielding or not (AC YIELDT: “actively yielding”; that is, the plastic strain changed during the increment). Plastic strain magnitude, defined as . For most materials, PEEQ and PEMAG are equal only for proportional loading. When plasticity occurs in the thickness direction to a gasket element whose plastic behavior is specified as part of a gasket behavior definition, PEMAG is PE11. All principal plastic strains. Minimum, plastic strains (PEP1 PEP2 PEP3). intermediate, and maximum principal All creep strain components. This identifier also provides CEEQ, CESW, and CEMAG when CE is requested for the data or results files. -component of creep strain ( Equivalent creep strain, defined as ). . The definition of depends on the material model. For classical metal (Mises) creep . For other creep models, see the appropriate section in Part V, “Materials.” When creep occurs in the thickness direction to a gasket element whose creep behavior is specified as part of a gasket behavior definition, CEEQ is CE11. • • Magnitude of swelling strain. For cap creep CESW gives the equivalent creep strain produced by the consolidation creep mechanism, is the equivalent creep defined as pressure, , where 4.2.1–10 PEEQT PEMAG PEP PEPn CE CEij CEEQ CESW • • • • • • • Identifier .dat .fil .odb Field History Description • • • • • • • • • • • • • • • Magnitude of creep strain (defined by the same formula given above for PEMAG, applied to the creep strains). All principal creep strains. Minimum, creep strains (CEP1 CEP2 CEP3). intermediate, and maximum principal for contact pressure Average link and three- dimensional line gasket elements. Available only if the gasket contact area is specified; see “Defining the contact area for average contact pressure output” in “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6. All transverse shear stress components. Available only for thick shell elements such as S3R, S4R, S8R, and S8RT. Contouring of this variable is supported in the Visualization module of Abaqus/CAE. -component of transverse shear stress ( ). Available only for thick shell elements such as S3R, S4R, S8R, and S8RT. stress components stacked for Transverse shear Available only for continuum shell elements. SC6R and SC8R elements. Contouring of this variable is supported in the Visualization module of Abaqus/CAE. -component of transverse shear stress ( Available only for SC6R and SC8R elements. ). All substresses. Available only for ITS elements. nth substress ( elements. ). Available only for ITS Vibration intensity. Available only for the steady-state dynamics procedure. real-only steady-state For dynamics analyses, the intensity is a pure imaginary vector, but it is stored as real on the output database. 4.2.1–11 CEMAG CEP CEPn • • • • Additional element stresses • CS11 • TSHR TSHRi3 CTSHR CTSHRi3 SS SSn • • • • • • • • Vibration and acoustic quantities Identifier .dat .fil .odb Field History Description Available for structural, solid, and acoustic elements and for rebar. Acoustic particle velocity. Available only if the steady-state dynamic procedure is used, and available only for acoustic finite elements. Component n of the acoustic particle velocity vector (n = 1, 2, 3). Available only if the steady-state dynamic procedure is used, and available only for acoustic finite elements. Acoustic pressure gradient. Available only if the steady-state dynamic procedure is used, and available only for acoustic finite elements. All energy densities. None of the energy densities are available in mode-based procedures; a limited number of them are available for direct-solution steady-state dynamic and subspace-based steady-state dynamic analyses. In steady-state dynamics all energy quantities are net per-cycle values, unless otherwise noted . Elastic strain energy density (with respect to current volume). When the Mullins effect is modeled with hyperelastic materials, this quantity represents only the recoverable part of energy per unit volume. This is the only energy density available in the data file for eigenvalue extraction procedures; to obtain this quantity for eigenvalue extraction procedures in the results file or as field output in the output database, request ENER. In steady-state dynamic analysis this is the cyclic mean value. Energy dissipated by rate-independent and rate- dependent plasticity, per unit volume. Not available for steady-state dynamic analysis. dissipated Energy and viscoelasticity, per unit volume. Not available for steady-state dynamic analysis. swelling, creep, by 4.2.1–12 • • • • • • • • • • • • • ACV ACVn GRADP Energy densities ENER • • SENER PENER CENER • • Identifier .dat .fil .odb Field History Description VENER EENER JENER DMENER • • • • • • • • • • • • Energy dissipated by viscous effects (except those from viscoelasticity and static dissipation), per unit volume. Electrostatic energy density. Not available for steady- state dynamic analysis. Electrical energy dissipated as a result of the flow of current, per unit volume. Not available for steady-state dynamic analysis. Energy dissipated by damage, per unit volume. Not available for steady-state dynamic analysis. State, field, and user-defined output variables • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Solution-dependent state variables. Solution-dependent state variable n. Temperature. Predefined field variables, including those imported using the FVi co-simulation field ID. Predefined field variable n. Predefined mass flow rates. Component ( User-defined output variables. User-defined output variable n. predefined mass flow rate of ). All failure measure components. Maximum stress theory failure measure. Tsai-Hill theory failure measure. Tsai-Wu theory failure measure. Azzi-Tsai-Hill theory failure measure. Maximum strain theory failure measure. Current value of the mass flow rate. Current value of the total mass flow. 4.2.1–13 SDV SDVn TEMP FV FVn MFR MFRn UVARM UVARMn • • • • • • • • • • • • • • Composite failure measures • CFAILURE MSTRS TSAIH TSAIW AZZIT MSTRN • • • • • • Fluid link quantities • • MFL MFLT • Identifier .dat .fil .odb Field History Description Fracture mechanics quantities JK • • • • J-integral, stress intensity factors. Available only for line spring elements. Output is in the following order for LS3S elements: J, K, . Output is in the following order for LS6 elements: J, , , and , , , and . Concrete cracking and additional plasticity CRACK CONF PEQC PEQCn • • • • • • • Unit normal to cracks in concrete. Number of cracks at a concrete material point. • • • All equivalent plastic strains when the model has more than one yield/failure surface. nth equivalent plastic strain ( ). For jointed materials: PEQC provides equivalent plastic strains for all four possible systems (three joints - PEQC1, PEQC2, PEQC3, and bulk material - PEQC4). This identifier also provides a yes/no flag (1/0 on the output database) telling if each individual system is currently yielding or not (AC YIELD: “actively yielding”; that is, the plastic strain changed during the increment). For cap plasticity: PEQC provides equivalent plastic three possible yield/failure surfaces strains for all (Drucker-Prager failure surface - PEQC1, cap surface - PEQC2, and transition surface - PEQC3) and the total volumetric inelastic strain (PEQC4). All identifiers also provide a yes/no flag (1/0 on the output database) telling whether the yield surface is currently active or not (AC YIELD: “actively yielding”, that is, the plastic strain changed during the increment). When PEQC is requested as output to the output database, the active yield flags for each component are named AC YIELD1, AC YIELD2, etc. and take the value 1 or 0. Identifier .dat .fil .odb Field History Description Concrete damaged plasticity DAMAGEC DAMAGET SDEG PEEQ Rebar quantities RBFOR RBANG RBROT • • • • • • • Heat transfer analysis HFL HFLM HFLn • • • Mass diffusion analysis CONC ISOL MFL MFLM • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • . . Compressive damage variable, Tensile damage variable, Scalar stiffness degradation variable, d. Equivalent plastic strain in uniaxial compression, This identifier also which is defined as provides a yes/no flag (1/0 on the output database) telling if is currently undergoing compressive failure or not (AC YIELD: “actively yielding”; that is, the plastic strain changed during the increment). the material . Force in rebar. Angle in degrees between rebar and the user-specified isoparametric direction. Available only for shell, membrane, and surface elements. Change in angle in degrees between rebar and the user- specified isoparametric direction. Available only for shell, membrane, and surface elements. Current magnitude and components of the heat flux per unit area vector. The integration points for these values are located at the Gauss points. Current magnitude of heat flux per unit area vector. Component n of the heat flux vector ( ). Mass concentration. Amount of solute at an integration point, calculated as the product of the mass concentration (CONC) and the integration point volume (IVOL). Current magnitude concentration flux vector. Current magnitude of the concentration flux vector. components and the of Identifier .dat .fil MFLn • .odb Field History • Description Component n of the concentration flux vector ( ). Elements with electrical potential degrees of freedom • EPG • • • Current magnitude and components of the electrical potential gradient vector. Current magnitude of the electrical potential gradient vector. Component n of the electrical potential gradient vector ( ). Current magnitude and components of the electrical flux vector. Current magnitude of the electrical flux vector. Component n of the electrical flux vector ( ). Current magnitude and components of the electrical current density. Current magnitude of the electrical current density. Component n of the electrical current density vector ( ). Maximum nominal stress damage initiation criterion. Maximum nominal strain damage initiation criterion. Quadratic nominal stress damage initiation criterion. Quadratic nominal strain damage initiation criterion. All active components of the damage initiation criteria. Overall scalar stiffness degradation. Status of the element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). Number of cycles to initialize the damage at material point. the 4.2.1–16 • • • • • • • • • • • • • • • • EPGM EPGn • • Piezoelectric analysis EFLX EFLXM EFLXn • • • • • Coupled thermal-electrical elements • ECD • • ECDM ECDn • • Cohesive elements • MAXSCRT • MAXECRT • QUADSCRT QUADECRT • • DMICRT • SDEG • STATUS • • • Low-cycle fatigue analysis CYCLEINI • • • • • • • Identifier .dat .fil .odb Field History Description • • • • • • • • • • • • • • • • SDEG STATUS • • Pore pressure analysis VOIDR POR SAT GELVR FLUVR FLVEL FLVELM FLVELn • • • • • • • • Pore pressure cohesive elements • • • • • • • GFVR • PFOPEN • LEAKVRT • LEAKVRB • ALEAKVRT ALEAKVRB • • • • • • • Porous metal plasticity quantities • • • • RD VVF VVFG VVFN • • • • • • • • Two-layer viscoplasticity quantities • • VS VSij • • • • • • • • • • • • • • • • • • • • • • • • Overall scalar stiffness degradation. Status of the element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). Void ratio. Pore pressure. Saturation. Gel volume ratio. Total fluid volume ratio. Current magnitude and components of the pore fluid effective velocity vector. Current magnitude of the pore fluid effective velocity vector. Component n of the pore fluid effective velocity vector ( ). Gap flow volume rate. Pore pressure fracture opening. Leak-off flow rate at the top of the element. Leak-off flow rate at the bottom of the element. Accumulated leak-off volume at the top of the element. Accumulated leak-off volume at the bottom of the element. Relative density. Void volume fraction. Void volume fraction due to void growth. Void volume fraction due to void nucleation. Stress in the elastic-viscous network. -component of stress in the elastic-viscous network ( ). Identifier .dat .fil .odb Field History Description PS PSij VE VEij PE PEij VEEQ PEEQ • • • • • • • • Geometric quantities • COORD IVOL • • • • • • • • • • • • • • • • • • • • • • • LOCALDIRn Accuracy indicators • SJP • Random response analysis Stress in the elastic-plastic network. -component of stress in the elastic-plastic network ( Viscous strain in the elastic-viscous network. ). -component of viscous strain in the elastic-viscous network ( ). Plastic strain in the elastic-plastic network. -component of plastic strain in the elastic-plastic ). network ( Equivalent viscous network, defined as Equivalent plastic strain in the elastic-plastic network, defined as strain in the elastic-viscous . . Coordinates of the integration point for solid elements and rebar. These are the current coordinates if the large-displacement formulation is being used. Section point volume Integration point volume. in the case of beams and shells. (Not available for eigenfrequency extraction, eigenvalue buckling prediction, complex eigenfrequency extraction, or linear dynamics procedures. Available only for continuum and structural elements not using general beam or shell section definitions.) Direction cosines of the local material directions for an anisotropic hyperelastic material model. This variable is output automatically if any other element field output is requested for an anisotropic hyperelastic material . Strain jumps at nodes. The following variables (beginning with R) are available only for random response dynamic analysis: Identifier .dat .fil .odb Field History Description • • • RS RSij RMISES RE REij RCTF RCTFn RCTMn RCEF RCEFn RCEMn RCVF RCVFn RCVMn RCRF RCRFn RCRMn RCSF RCSFn • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Root mean square of all stress components. Root mean square of -component of stress ( ). Root mean square of Mises equivalent stress. Root mean square of all strain components. Root mean square of -component of strain ( ). RMS values of all components of connector total forces and moments. RMS value of connector total force component n ( ). RMS value of connector total moment component n ( ). RMS values of all components of connector elastic forces and moments. RMS value of connector elastic force component n ( ). RMS value of connector elastic moment component n ( ). RMS values of all components of connector viscous forces and moments. RMS value of connector viscous force component n ( ). RMS value of connector viscous moment component n ( ). RMS values of all components of connector reaction forces and moments. RMS value of connector reaction force component n ( ). RMS value of connector reaction moment component n ( ). RMS values of all components of connector friction forces and moments. RMS value of connector friction force component n ( ). Identifier .dat .fil .odb Field History Description RCSMn RCSFC RCU RCUn RCURn RCCU RCCUn RCCURn RCNF RCNFn RCNMn RCNFC • • • • • • • • • • • • • • • • • • • • • • • • • • • ). ). ). all RMS value of connector friction moment component n ( RMS value of connector friction force in the direction of the instantaneous slip direction. Available only if friction is defined in the slip direction. RMS values of all components of connector relative displacements and rotations. RMS value of connector relative displacement in the n-direction ( RMS value of connector relative rotation in the n-direction ( RMS values of components of constitutive displacements and rotations. RMS value of connector constitutive displacement in the n-direction ( ). RMS value of connector constitutive rotation in the n-direction ( RMS values of all components of connector friction- generating contact forces and moments. RMS value of connector friction-generating contact force component n ( RMS value of connector friction-generating contact moment component n ( RMS values of connector friction-generating contact force components in the instantaneous slip direction. Available only if friction is defined in the slip direction. connector ). ). ). Steady-state dynamic analysis The following variables (beginning with P) are available only for steady-state (frequency domain) dynamic analysis. These variables include both the magnitude and phase angle for all components. Phase angles are given in degrees. In the data file there are two lines of output for each request. The first line contains the magnitude, and the second line (indicated by the SSD footnote) contains the phase angle. In the results file the magnitudes of all components are first, followed by the phase angles of all components. PHS PHSij • • • Magnitude and phase angle of all stress components. Magnitude and phase angle of -component of stress ( ). Identifier .dat .fil .odb Field History Description PHE PHEij PHEPG PHEPGn PHEFL PHEFLn PHMFL PHMFT PHCTF PHCTFn PHCTMn PHCEF PHCEFn PHCEMn PHCVF PHCVFn PHCVMn PHCRF PHCRFn • • • • • • • • • • • • • • • • • • • • • • • • • • • • ). ). ). total mass flow. Magnitude and phase angle of all strain components. Magnitude and phase angle of -component of strain ( Magnitude and phase angles of the electrical potential gradient vector. Magnitude and phase angle of component n of the electrical potential gradient ( Magnitude and phase angles of the electrical flux vector. Magnitude and phase angle of component n of the electrical flux vector ( Magnitude and phase angle of mass flow rate. Available only for fluid link elements. Magnitude and phase angle of Available only for fluid link elements. Magnitude and phase of all components of connector total forces and moments. Magnitude and phase of connector component n ( ). Magnitude and phase of connector total moment component n ( ). Magnitude and phase of all components of connector elastic forces and moments. Magnitude and phase of connector elastic force component n ( ). Magnitude and phase of connector elastic moment component n ( ). Magnitude and phase of all components of connector viscous forces and moments. Magnitude and phase of connector viscous force component n ( ). Magnitude and phase of connector viscous moment component n ( ). Magnitude and phase of all components of connector reaction forces and moments. Magnitude and phase of connector reaction force component n ( ). force total Identifier .dat .fil .odb Field History Description PHCRMn PHCSF PHCSFn PHCSMn PHCSFC PHCU PHCUn PHCURn PHCCU PHCCUn PHCCURn PHCV PHCVn PHCVRn PHCA PHCAn PHCARn PHCNF • • • • • • • • • • • • • • • • • • • • • • • • ). of phase relative connector Magnitude and phase of connector reaction moment component n ( ). Magnitude and phase of all components of connector friction forces and moments. Magnitude and phase of connector friction force component n ( ). Magnitude and phase of connector friction moment component n ( ). Magnitude and phase of connector friction force in the direction of the instantaneous slip direction. Available only if friction is defined in the slip direction. Magnitude and phase of all components of connector relative displacements and rotations. Magnitude and displacement in the n-direction ( Magnitude and phase of connector relative rotation in the n-direction ( ). Magnitude and phase of all components of connector constitutive displacements and rotations. Magnitude and phase of connector constitutive displacement in the n-direction ( Magnitude and phase of connector constitutive rotation in the n-direction ( Magnitude and phase of all components of connector relative velocities. Magnitude and phase of connector relative velocity in the n-direction ( ). Magnitude and phase of connector relative angular velocity in the n-direction ( Magnitude and phase of all components of connector relative accelerations. Magnitude of and acceleration in the n-direction ( Magnitude and phase of connector relative angular acceleration in the n-direction ( Magnitude and phase of all components of connector friction-generating contact forces and moments. connector ). relative phase ). ). ). ). Identifier .dat .fil .odb Field History Description ). Magnitude and phase of connector friction-generating contact force component n ( Magnitude and phase of connector friction-generating contact moment component n ( Magnitude and phase of connector friction-generating contact force in the instantaneous slip direction. Available only if friction is defined in the slip direction. Magnitude and phase of connector instantaneous velocity in the slip direction. Available only if friction is defined in the slip direction. ). Scalar stiffness degradation variable. All active components of the damage initiation criteria. Ductile damage initiation criterion. Shear damage initiation criterion. Forming limit diagram (FLD) damage initiation criterion. Forming limit initiation criterion. Müschenborn-Sonne forming limit stress diagram (MSFLD) damage initiation criterion. Ratio of principal strain rates, damage initiation criterion. Shear stress ratio, shear damage initiation criterion. stress diagram (FLSD) damage , used for the MSFLD , used for the Hashin’s fiber tensile damage initiation criterion. Hashin’s fiber compressive damage initiation criterion. Hashin’s matrix tensile damage initiation criterion. Hashin’s matrix compressive damage criterion. All active components of the damage initiation criteria. Fiber tensile damage variable. Fiber compressive damage variable. initiation 4.2.1–23 PHCNFn PHCNMn PHCNFC PHCIVC • • • • • Failure with progressive damage SDEG DMICRT DUCTCRT SHRCRT FLDCRT FLSDCRT MSFLDCRT ERPRATIO SHRRATIO • • • • Fiber-reinforced materials damage • • • • • HSNFTCRT • HSNFCCRT HSNMTCRT • HSNMCCRT • • DMICRT DAMAGEFT • DAMAGEFC • • • • • • • • • • • • • • • • • • • • • • Identifier .dat .fil .odb Field History Description DAMAGEMT • DAMAGEMC • DAMAGESHR • • STATUS • • • • • • • • • • • • Matrix tensile damage variable. Matrix compressive damage variable. Shear damage variable. Status of the element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). Element centroidal variables For electromagnetic elements, the element output is at the centroid of the element instead of at the integration points. These variables are defined for electromagnetic elements in the element descriptions in Part VI, “Elements,” and “Eddy current analysis,” Section 6.7.5. Identifier .dat .fil .odb Field History Description EMB EMH EME EMCD EMJH EMBF EMBFC • • • • • • • • • • • • • • All components of the magnetic flux density vector. All components of the magnetic field vector. All components of the electric field vector. All components of conducting regions. the eddy current vector in Rate of Joule heat dissipation (amount of heat dissipated per unit volume per unit time) in conductor regions. Magnetic body force intensity (force per unit volume) vector in conductor regions. Complex magnetic body force intensity (force per unit volume) vector in conductor regions in a time-harmonic eddy current analysis. Element section variables You can request element section variable output to the data, results, or output database file . These variables are available only for beam and shell elements with the exception of STH, which is also available for membrane elements. They are defined for particular elements in the element descriptions in Part VI, “Elements.” Identifier .dat .fil .odb Field History Description SF SFn SMn BIMOM ESF1 SSAVG SSAVGn SE SEn SKn BICURV MAXSS COORD STH • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • for for continuum All section force and moment components. Section force component n ( conventional shells; shells; for beams). Section moment component n ( Bimoment of beam cross-section. Available only for open-section beam elements. Effective axial force for beams and pipes subjected to pressure loading. Available for all stress/displacement procedure types except response spectrum and random response. All average shell section stress components. Average shell section stress component n ( ). ). ). for stress on the section. All section strain, curvature change, and twist components. Section strain component n ( shells; for beams). Section curvature change or twist n ( Bicurvature of beam cross-section. Available only for open-section beam elements. (This Maximum axial variable can be used with the following types of general beam section definitions: standard library cross-sections, linear generalized cross-sections, or meshed cross-sections with specified output section points. If the output section points are specified, the MAXSS output will be the maximum of the stresses at the user-specified points.) Coordinates of the section point. These are the current coordinates if the large-displacement formulation is being used. Section thickness (current thickness for SAX1, SAX2, SAX2T, S3/S3R, S4, S4R, SAXA1N, SAXA2N, and all membrane elements if the large-displacement formulation is used; initial thickness for all other cases). Identifier .dat .fil .odb Field History Description SVOL SPE SPEn SEPE SEPEn Frame elements SEE SEE1 SKEn SEP • • • • • • • • • • • • • • • • • • • • • • • • • • • • (Not available for Integrated section volume. eigenfrequency buckling extraction, prediction, complex eigenfrequency extraction, or Available only for linear dynamics procedures. continuum and structural elements not using general beam or shell section definitions.) eigenvalue All generalized plastic strain components. Available only for inelastic nonlinear response in a general beam section. Generalized plastic strain component n ( ). Representing axial plastic strain, curvature change about the local 1-axis, curvature change about the local 2-axis, and twist of the beam. Available only for inelastic nonlinear response in a general beam section. All equivalent plastic strains. Available only for inelastic nonlinear response in a general beam section. Equivalent plastic strain component n ( ). Representing axial plastic strain, curvature change about the local 1-axis, curvature change about the local 2-axis, and twist of the beam. Available only for inelastic nonlinear response in a general beam section. All elastic section axial, curvature, and twist strain components. Elastic axial strain component. Elastic section curvature or twist strain component ( ). All plastic axial displacements and rotations at the element’s ends. This identifier also provides a yes/no flag telling if the frame element’s end section is currently yielding or not (AC YIELD: “actively yielding”; that is, the plastic strain changed during the increment) and a yes/no/na flag telling if buckling occurred in the strut response (AC BUCKL) or is not applicable. AC YIELD and AC BUCKL are not available in the output database. Identifier .dat .fil .odb Field History Description SEP1 SKPn SALPHA SALPHAn • • • • • • • • • • Plastic axial displacement at the element’s ends. Plastic rotations, either bending or twisting, at the element’s ends ( ). All generalized backstress element’s ends. ends Generalized ( is the axial section backstress, followed by two bending backstress components and the twist backstress component. element’s The first component backstress ). components the the at at Whole element variables You can request whole element variable output to the data, results, or output database file . Identifier .dat .fil .odb Field History Description LOADS FOUND FLUXS CHRGS ECURS ELEN ELKE ELSE • • • • • • • • • • • • • • • • • • • • • Current values of distributed loads (not available for nonuniform loads). Current values of foundation pressures. Current values of distributed (heat or concentration) fluxes (not available for nonuniform fluxes), including those imported using the HFL co-simulation field ID. Current values of distributed electrical charges. Current values of distributed electrical currents. None All energy magnitudes in the element. of in mode-based are procedures; a limited number of them are available and for subspace-based steady-state dynamic analyses. In steady-state dynamics all energy quantities are net per-cycle values, unless otherwise noted. Total kinetic energy in the element. dynamic analysis this is the cyclic mean value. Total elastic strain energy in the element. When the Mullins effect is modeled with hyperelastic materials, In steady-state direct-solution steady-state available dynamic energies the Identifier .dat .fil .odb Field History Description ELPD ELCD ELVD ELSD ELCTE ELJD ELASE ELDMD NFORC • • • • • • • • • • • • • • • • • • • • • • • • • • • • in the output database, this quantity represents only the recoverable part of energy in the element. This is the only energy request available in the data file for eigenvalue extraction to obtain this quantity for eigenvalue procedures; extraction procedures in the results file or as field output request ELEN. In steady-state dynamic analysis this is the cyclic mean value. Total energy dissipated in the element by rate- independent and rate-dependent plastic deformation. Not available for steady-state dynamic analysis. Total energy dissipated in the element by creep, swelling, and viscoelasticity. Not available for steady-state dynamic analysis. Total energy dissipated in the element by viscous effects, not including energy dissipated by static stabilization or viscoelasticity. Total energy dissipated in the element resulting from automatic static stabilization. Not available for steady- state dynamic analysis. Total electrostatic energy in the element. Not available for steady-state dynamic analysis. Total electrical energy dissipated due to flow of current. Not available for steady-state dynamic analysis. Total “artificial” strain energy in the element (energy associated with constraints used to remove singular modes, such as hourglass control, and with constraints used to make the drill rotation follow the in-plane rotation of the shell element). Not available for steady-state dynamic analysis. Total energy dissipated in the element by damage. Not available for steady-state dynamic analysis. Forces at the nodes of an element from both the hourglass and the regular deformation modes of that element (internal forces in the global coordinate system). The specified position in data and results file requests is ignored. Identifier .dat .fil .odb Field History Description Forces at the nodes of a beam element caused by the stress resultants in the element (internal forces in the beam section orientation coordinate system). Uniformly distributed gravity load. Uniformly distributed body force. Magnitude of Coriolis load. Magnitude of rotary acceleration load. is the mass density per unit volume and load (measured as Magnitude of centrifugal where the angular velocity). , is Magnitude of centrifugal load (measured as , where is the angular velocity). Heat body flux. Fluxes at the nodes of the element caused by the heat conduction or mass diffusion in the element (internal fluxes). (The specified position for data and output database file requests is ignored.) Flux n at the nodes of the element ( ) caused by the heat conduction or mass diffusion in the element (internal fluxes). (The specified position for data and output database file requests is ignored.) Electrical current at conduction in the element. the nodes due to electrical Current values of film conditions (not available for nonuniform films). Current values of radiation conditions. (Not available for Current element volume. buckling extraction, eigenfrequency prediction, complex eigenfrequency extraction, or linear dynamics procedures. Available only for continuum and structural elements not using general beam or shell section definitions.) eigenvalue Amount of solute in an element, calculated as the sum of ISOL (amount of solute at an integration point) over all the integration points in the element. 4.2.1–29 NFORCSO GRAV BF CORIOMAG ROTAMAG CENTMAG CENTRIFMAG HBF NFLUX NFLn NCURS FILM RAD EVOL ESOL • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Identifier .dat .fil .odb Field History Description Enriched elements STATUSXFEM • • Status of the enriched element. (The status of an enriched element is 1.0 if the element is completely cracked; 0.0 if the element is not. If the element is partially cracked, the value lies between 1.0 and 0.0.) Enriched elements when the XFEM-based LEFM approach is used • ENRRTXFEM • All components of strain energy release rate. Enriched elements in low-cycle fatigue analysis • • • • • • • • • • CYCLEINIXFEM Connector elements • CTF CTFn CTMn CEF CEFn CEMn CUE CUEn CUREn CUP CUPn CURPn CUPEQ CUPEQn CURPEQn • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Number of cycles to initialize the crack at the enriched element. ). ). total forces and All components of connector moments. Connector total force component n ( Connector total moment component n ( All components of connector elastic forces and moments. Connector elastic force component n ( Connector elastic moment component n ( Elastic displacements and rotations in all directions. Elastic displacement in the n-direction ( ). Elastic rotation in the n-direction ( Plastic relative displacements and rotations in all directions. Plastic relative displacement in the n-direction ( ). ). ). ). Plastic relative rotation in the n-direction ( ). Equivalent plastic relative displacements and rotations in all directions. Equivalent plastic relative displacement n-direction ( Equivalent plastic relative rotation in the n-direction ( in the ). ). Identifier .dat .fil .odb Field History Description Equivalent plastic relative motion for a coupled plasticity definition. All components of connector kinematic hardening shift forces and moments. Connector kinematic hardening shift force component n ( ). Connector component n ( kinematic hardening ). shift moment All components of connector viscous forces and moments. Connector viscous force component n ( Connector viscous moment component n ( ). ). All components of connector friction forces and moments. Connector friction force component n ( Connector friction moment component n ( ). ). Connector friction force in the instantaneous slip direction. Available only if friction is defined in the slip direction. All components of connector contact forces and moments. friction-generating Connector component n ( Connector component n ( friction-generating friction-generating contact force contact moment ). ). Connector friction-generating contact force in the instantaneous slip direction. Available only if friction is defined in the slip direction. All components of the overall damage variable. Overall damage variable component n ( Overall damage variable component n ( Components initiation criterion in all directions. connector of force-based ). ). damage Connector force-based damage initiation criterion in the n-translation direction ( ). 4.2.1–31 • • • • • • • • • • • • • • • • • • • • CUPEQC CALPHAF CALPHAFn CALPHAMn CVF CVFn CVMn CSF CSFn CSMn CSFC CNF CNFn CNMn CNFC CDMG CDMGn CDMGRn CDIF CDIFn • • • • • • • • • • • • • • • • • • • • • • • • • Identifier .dat .fil .odb Field History Description CDIFRn CDIFC CDIM CDIMn CDIMRn CDIMC CDIP CDIPn CDIPRn CDIPC CSLST CSLSTi CASU CASUn CASURn CASUC CIVC CRF CRFn • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • ). ). ). Connector force-based damage initiation criterion in the n-rotation direction ( Connector force-based damage initiation criterion in the instantaneous slip direction. Components of connector motion-based damage initiation criterion in all directions. Connector motion-based damage initiation criterion in the n-translation direction ( Connector motion-based damage initiation criterion in the n-rotation direction ( Connector motion-based damage initiation criterion in the instantaneous slip direction. Components of damage initiation criterion in all directions. Connector plastic motion-based damage initiation criterion in the n-translation direction ( Connector plastic motion-based damage initiation criterion in the n-rotation direction ( Connector plastic motion-based damage initiation criterion in the instantaneous slip direction. All flags for connector stop and connector lock status. Flag for connector stop and connector lock status in the i-direction ( ). Components of accumulated slip in all directions. Connector accumulated slip in the n-direction ( connector plastic motion-based ). ). ). ). Connector angular accumulated slip in the n-direction ( Connector accumulated slip in the instantaneous slip direction. Available only if friction is defined in the slip direction. Connector instantaneous velocity in the slip direction. Available only if friction is defined in the slip direction. All components of connector reaction forces and moments. Connector reaction force component n ( ). Identifier .dat .fil .odb Field History Description • CRMn CCF CCFn CCMn CP CPn CPRn CU CUn CURn CCU CCUn CCURn CV CVn CVRn CA CAn CARn CFAILST CFAILSTi • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Connector reaction moment component n ( ). All components of connector concentrated forces and moments. Connector concentrated force component n ( ). Connector concentrated moment component n ( ). in the position angular ). ). in all ). n-direction Relative positions in all directions. Relative position in the n-direction ( Relative ( Relative displacements and rotations in all directions. ). Relative displacement in the n-direction ( Relative rotation in the n-direction ( Constitutive displacements and rotations directions. Constitutive ( Constitutive rotation in the n-direction ( Relative velocities in all directions. Relative velocity in the n-direction ( Relative ( Relative accelerations in all directions. Relative acceleration in the n-direction ( Relative angular acceleration in the n-direction ( ). n-direction angular ). displacement n-direction velocity the the in in ). ). ). ). All flags for connector failure status. Flag for connector failure status in the i-direction ( ). Element face variables You can request element face variable output to the output database . These variables are available only for shell, membrane, and solid elements. Identifier .dat .fil .odb Field History Description HP TRNOR TRSHR FLUXS FILMCOEF SINKTEMP • • • • • • • Uniformly distributed pressure load on element faces, including those imported using the PRESS co-simulation field ID. When the pressure is defined using *DLOAD, the variable name is changed automatically to PDLOAD. When the pressure is defined using *DLOAD on shell or membrane elements, Abaqus changes the sign of its value to make it consistent with the pressure defined using *DSLOAD. Hydrostatic pressure load on element faces. When the pressure is defined using *DLOAD, the variable name is changed automatically to HPDLOAD. When the pressure is defined using *DLOAD on shell or membrane elements, Abaqus changes the sign of its value to make it consistent with the pressure defined using *DSLOAD. Normal component (component along face normal) of traction load on element faces. Shear component (component along face tangent) of traction load on element faces. Uniformly distributed heat fluxes on element faces. Reference film coefficient value on element faces. Reference sink temperature on element faces. Whole element energy density variables The following energy density output variables are written to the restart (.res) file and the output database (.odb) file : Identifier .dat .fil ELEDEN .odb Field History • Description All energy density components. None of the energies are available in mode-based procedures; a limited number of them are available for direct-solution steady-state dynamic and subspace-based steady-state dynamic analyses. In steady-state dynamics all energy quantities are net per-cycle values, unless otherwise noted. Identifier .dat .fil .odb Field History Description EKEDEN ESEDEN EPDDEN ECDDEN EVDDEN ESDDEN ECTEDEN EASEDEN EDMDDEN • • • • • • • • • • • • • • • • • • Kinetic energy density in the element. In steady-state dynamic analysis this is the cyclic mean value. Total elastic strain energy density in the element. When the Mullins effect is modeled with hyperelastic materials, this quantity represents only the recoverable part of energy density in the element. This variable is not available in eigenvalue extraction procedures. In steady-state dynamic analysis this is the cyclic mean value. Total energy dissipated per unit volume in the element by rate-independent and rate-dependent plastic deformation. Not available for steady-state dynamic analysis. Total energy dissipated per unit volume in the element by creep, swelling, and viscoelasticity. Not available for steady-state dynamic analysis. Total energy dissipated per unit volume in the element by viscous effects, not inclusive of energy dissipated through static stabilization or viscoelasticity. Total energy dissipated per unit volume in the element resulting from static stabilization. Not available for steady-state dynamic analysis. Total electrostatic energy density in the element. Not available for steady-state dynamic analysis. Total “artificial” strain energy density in the element (energy associated with constraints used to remove singular modes, such as hourglass control, and with constraints used to make the drill rotation follow the in-plane rotation of the shell element). Not available for steady-state dynamic analysis. Total energy dissipated per unit volume in the element by damage. Not available for steady-state dynamic analysis. Whole element error indicator variables You can request that the following error indicator variables and element average variables be output only to the output database (.odb) file . Identifier .dat .fil .odb Field History Description ENDEN ENDENERI MISESAVG MISESERI PEEQAVG PEEQERI PEAVG PEERI CEAVG CEERI HFLAVG HFLERI EFLAVG EFLERI EPGAVG EPGERI Nodal variables • • • • • • • • • • • • • • • • Element energy density, including plastic dissipation and creep dissipation if present. including Element energy density error indicator, plastic dissipation error and creep dissipation error if present. Element average Mises equivalent stress. Element Mises equivalent stress error indicator. Element average equivalent plastic strain. Element equivalent plastic strain error indicator. Element average plastic strain. Element plastic strain error indicator. Element average creep strain. Element creep strain error indicator. Element average heat flux. Element heat flux error indicator. Element average electric flux. Element electric flux error indicator. Element average electric potential gradient. Element electric potential gradient error indicator. You can request nodal variable output to the data, results, or output database file . Identifier .dat .fil .odb Field History Description UT UR Un URn • • • • • • • • • • • • including All physical displacement components, rotations at nodes with rotational degrees of freedom (for output to the output database, only field-type output includes the rotations). All translational displacement components. All rotational displacement components. displacement component ( rotation component ( ). ). Identifier .dat .fil .odb Field History Description WARP VT VR Vn VRn AT AR An ARn POR CFF NT NTn EPOT NNC NNCn RF • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • velocity components, Warping magnitude. Available only for open-section beam elements. rotational All velocities at nodes with rotational degrees of freedom (for output to the output database, only field-type output includes the rotational velocities). All translational velocity components. All rotational velocity components. including velocity component ( rotational velocity component ( ). ). including rotational All acceleration components, accelerations at nodes with rotational degrees of freedom (for output to the output database, only field-type output includes the rotational accelerations). All translational acceleration components. All rotational acceleration components. acceleration component ( rotational acceleration component ( ). ). Pore or acoustic pressure at a node. Concentrated fluid flow at a node, including those imported using the CFLOW co-simulation field ID. including those All temperature values at a node, imported using the TEMP co-simulation field ID. These will be the temperatures defined as degrees of freedom if heat transfer elements are connected to the node, or predefined temperatures if the node is connected only to stress or mass diffusion elements without temperature degrees of freedom. Temperature degree of ( All electrical potential degrees of freedom at a node. All normalized concentration values at a node. Normalized concentration degree of freedom n at a node ( including All components of reaction moments at nodes with rotational degrees of freedom (conjugate to prescribed ). components of freedom n at a node reaction forces, ). Identifier .dat .fil .odb Field History Description ) ). For output ) (conjugate loads and concentrated including loads imported using the CF displacements and rotations). to the output database, only the field-type output includes the components of reaction moments at nodes with rotational degrees of freedom. All reaction force components. All reaction moment components. Reaction force component n ( to prescribed displacement Reaction moment component n ( (conjugate to prescribed rotation ). Reaction bimoment in degree of freedom 7, conjugate to prescribed warping amplitude. Available only for open-section beam elements. All components of point moments, co-simulation field ID. Point load component n ( Point moment component n ( Load component in degree of freedom 7. Available only for open-section beam elements. All components of total forces, including components of total moments at nodes with rotational degrees of freedom. Total force is the sum of the reaction force and point loads. For output to the output database, only the field-type output includes the components of total moments at nodes with rotational degrees of freedom. Total force component n ( Total moment component n ( All components of viscous forces and moments due to static stabilization. Stabilization viscous force component n ( Stabilization viscous moment component n ( ). ). ). ). ). ). These are the current Coordinates of the node. coordinates if the large-displacement formulation is being used. Coordinate n ( ). 4.2.1–38 • • • • • • • • • • RT RM RFn RMn RWM CF CFn CMn CW TF TFn TMn VF VFn VMn COORD COORn • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Identifier .dat .fil .odb Field History Description Strain-free adjustments to initial nodal positions (adjusted position minus unadjusted position; only written to the output database (.odb) file for the original field output frame at zero time). Reactive prescribed electrical potential). electrical nodal charge Concentrated electrical nodal charge. Reactive electrical nodal current prescribed electrical potential). Concentrated electrical nodal current. (conjugate to (conjugate to Hydrostatic fluid gauge pressure (total pressure = ambient pressure + hydrostatic fluid gauge pressure). Hydrostatic fluid cavity volume. All components of motion in cavity radiation heat transfer analysis. motion component ( ) in cavity radiation heat transfer analysis. Acoustic pressure. Acoustic infinite element “radius,” used in the coordinate map for these elements. Available only if the steady-state dynamic procedure is used, and available only for nodes attached to acoustic infinite elements. Acoustic infinite element “cosine,” used in the coordinate map for these elements. Available only if the steady-state dynamic procedure is used, and available only for nodes attached to acoustic infinite elements. Acoustic infinite element normal vector. Available only if the steady-state dynamic procedure is used, and available only for nodes attached to acoustic infinite elements. Acoustic pressure coefficients for the higher-order basis functions in acoustic infinite elements. Available 4.2.1–39 STRAINFREE RCHG CECHG RECUR CECUR PCAV CVOL MOT MOTn • • • • • • • • Acoustic quantities • POR INFR • • • • • • • • INFC INFN PINF • • • • • • • • • • • • • • • • • • • Identifier .dat .fil .odb Field History Description SPL Enriched element quantities PHILSM PSILSM • • • • • • Heat or mass flux only if the steady-state dynamic procedure is used, and available only for acoustic infinite elements. Acoustic sound pressure level at a node. Signed distance function to describe the crack surface. Signed distance function to describe the initial crack front. The following variables correspond to heat flux in temperature analyses or concentration volumetric flux in mass diffusion analysis: • RFL • • • • • • • RFLn CFL CFLn RFLE RFLEn • • • • • • • • • • All reaction flux values (conjugate to prescribed temperature or normalized concentration). Reaction flux value n at a node ( ) (conjugate to prescribed temperature or normalized concentration). All concentrated flux values, including those imported using the CFL co-simulation field ID. Concentrated flux values n at a node ( ). The total flux at the node (including flux convected through the node in convection elements), excluding external fluxes (due to concentrated fluxes, distributed fluxes, film conditions, radiation conditions, and radiation viewfactors). The value of RFLE is, thus, equal and opposite to the sum of all applied fluxes. Flux value n excluding externally applied flux loads at a node ( ). Steady-state dynamic analysis The following variables are available only for steady-state (frequency domain) dynamic analyses (modal and direct). These variables include both magnitude and phase angle for all components. Phase angles are given in degrees. In the data file there are two lines of output for each request. The first line contains the magnitude, and the second line (indicated by the SSD footnote) contains the phase angle. In the results file, the magnitudes of all components are first, followed by the phase angles of all components. PU • • Magnitude and phase angle of all displacement components at the node and magnitude and phase Identifier .dat .fil .odb Field History Description PUn PURn PPOR PHPOT PRF PRFn PRMn PHCHG • • • • • • • • • • • • ). angle of the rotations at nodes with rotational degrees of freedom. Magnitude and phase angle of component n of the displacement ( ). Magnitude and phase angle of component n of the rotation ( Magnitude and phase angle of the fluid, pore, or acoustic pressure at the node. Magnitude and phase angle of the electrical potential at the node. Magnitude and phase angle of the reaction forces at the node and of the reaction moments at nodes with rotational degrees of freedom. Magnitude and phase angle of component n of the reaction force ( ). Magnitude and phase angle of component n of the reaction moment ( Magnitude and phase angle of the reactive charge at the node. ). Modal dynamic, steady-state, and random response analysis The following variables are available only for modal dynamic, steady-state (frequency domain), and random response analyses. “Relative” values are measured relative to the motion of the primary base and are obtained with the identifiers U, V, and A; “Total” values include the motion of the primary base. For steady-state dynamic output printed to the data file, there are two lines printed for each request; the first line contains the real part of the variable, and the second line (indicated by the SSD footnote) contains the imaginary part. • • • • TU TUn TURn TV TVn TVRn • • • • • • • • • • • • All components of the total displacements at the node and of the total rotations at nodes with rotational degrees of freedom. Component n of the total displacement ( Component n of the total rotation ( All components of the total velocity at the node, including rotational velocities at nodes with rotational degrees of freedom. Component n of the total velocity ( Component n of the total rate of rotation ( ). ). ). ). Identifier .dat .fil .odb Field History Description • • TA TAn TARn • • • • • • All components of the total acceleration at the node, including rotational accelerations at nodes with rotational degrees of freedom. Component n of the total acceleration ( Component n of the total rotational acceleration ( ). ). Mode-based steady-state dynamic analysis The following variables are available only for steady-state (frequency domain) dynamic analysis based on modal superposition. “Total” values include the base motion. PTU PTUn PTURn • • • • Pore pressure analysis Magnitude and phase angle of the total displacement components at the node and magnitude and phase angle of the total rotations at nodes with rotational degrees of freedom. Magnitude and phase angle of component n of the total displacement ( ). Magnitude and phase angle of component n of the total rotation ( ). The following variables correspond to fluid volume flux in pore pressure analyses. • RVF • • • Reaction fluid volume flux due to prescribed pressure. This flux is the rate at which fluid volume is entering or leaving the model through the node to maintain the prescribed pressure boundary condition. A positive value of RVF indicates fluid is entering the model. Reaction total fluid volume (computed only in a transient coupled pore fluid diffusion/stress analysis). This value is the time integrated value of RVF. RVT • • • • Random response analysis The following variables are available only for random response dynamic analysis. “Relative” values are measured relative to the base motion; “Total” values include the base motion. RU • • • • Root mean square values of all components of the relative displacement at the node and of the components of rotation at nodes with rotational degrees of freedom. Identifier .dat .fil .odb Field History Description RUn RURn RTU RTUn RTURn RV RVn RVRn RTV RTVn RTVRn RA RAn RARn RTA • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • ). ). ). Root mean square value of component n of the relative displacement ( ). Root mean square value of component n of the relative rotation ( Root mean square values of all components of the total displacement at the node and of the components of total rotation at nodes with rotational degrees of freedom. Root mean square value of component n of the total displacement ( ). Root mean square value of component n of the total rotation ( Root mean square values of all components of the relative velocity at the node and of the components of the rate of rotation at nodes with rotational degrees of freedom. Root mean square value of component n of the relative velocity ( Root mean square value of component n of the relative rate of rotation ( Root mean square values of all components of the total velocity at the node and of the components of total rotation at nodes with rotational degrees of freedom. Root mean square value of component n of the total velocity ( Root mean square value of component n of the total rate of rotation ( Root mean square values of all components of the relative acceleration at the node and of the components of rotational acceleration at nodes with rotational degrees of freedom. Root mean square value of component n of the relative acceleration ( Root mean square value of component n of the relative rotational acceleration ( Root mean square values of all components of the total acceleration at the node and of the components of ). ). ). ). ). Identifier .dat .fil .odb Field History Description • • RTAn RTARn RRF RRFn RRMn • • • • • Modal variables rotational acceleration at nodes with rotational degrees of freedom. Root mean square value of component n of the total value of acceleration ( ). Root mean square value of component n of the total rotational acceleration ( ). Root mean square values of all components of the reaction forces and of reaction moments at nodes with rotational degrees of freedom. Root mean square value of component n of the reaction force ( ). Root mean square value of component n of the reaction moment ( ). • • • • • You can request modal variable output to the data, results, or output database file . etc. provide the amplitude of the mode. Identifier .dat .fil .odb Field History Description GU GUn GV GVn GA GAn GPU GPUn GPV GPVn GPA GPAn • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Generalized displacements for all modes. Generalized displacement for mode n. Generalized velocities for all modes. Generalized velocity for mode n. Generalized acceleration for all modes. Generalized acceleration for mode n. Phase angle of generalized displacements for all modes. Phase angle of generalized displacement for mode n. Phase angle of generalized velocities for all modes. Phase angle of generalized velocity for mode n. Phase angle of generalized acceleration for all modes. Phase angle of generalized acceleration for mode n. Identifier .dat .fil .odb Field History Description SNE SNEn KE KEn Tn BM • • • • • • • • • • • Surface variables • • • • • • • Elastic strain energy for the entire model per each mode (not available for random response analysis). Elastic strain energy for the entire model for mode n (not available for random response analysis). Kinetic energy for the entire model per each mode (not available for random response analysis). Kinetic energy for the entire model for mode n (not available for random response analysis). External work for the entire model per each mode (not available for random response analysis). External work for the entire model for mode n (not available for random response analysis). Base motion (not available for random response or response spectrum analyses). You can request surface variable output to the data, results, or output database file . Additional information on these variables is provided in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1, and Chapter 36, “Contact Property Models.” The letter “M” at the end of an output variable identifier designates the magnitude of the variable. Those variables that are output on both master and slave surfaces in a single master-slave contact pair are designated below. For exceptions to output on the master surface, see “Defining contact pairs in Abaqus/Standard,” Section 35.3.1. Identifier .dat .fil .odb Field History Description • Contact pressure (CPRESS) and frictional shear stresses (CSHEAR). Output is also available on the master surface to the .odb file in a single master-slave setting. Contact pressure (CPRESSETOS) and frictional shear stresses (CSHEARETOS) due to edge-to-surface contact constraints. Output is also available on the 4.2.1–45 Mechanical analysis–nodal quantities • CSTRESS • • CSTRESSETOS Identifier .dat .fil .odb Field History Description master surface to the .odb file in a single master-slave setting. Error indicators for the contact pressure (CPRESSERI) and frictional shear stresses (CSHEARERI). Output is also available on the master surface to the .odb file in a single master-slave setting. Viscous pressure (CDPRESS) and viscous shear stresses (CDSHEAR). Output is also available on the master surface to the .odb file in a single master-slave setting. Contact opening (COPEN) and relative tangential motions (CSLIP). opening Contact relative tangential motions (CSLIPETOS) for edge-to-surface contact constraints. (COPENETOS) and Contact normal force (CNORMF) and frictional shear force (CSHEARF). Output is also available on the master surface to the .odb file in a single master-slave setting. Contact nodal area. Output is also available on the master surface to the .odb file in a single master-slave setting. Contact status. Output is also available on the master surface to the .odb file in a single master-slave setting. Maximum stress-based damage initiation criterion for cohesive surfaces. Quadratic stress-based damage initiation criterion for cohesive surfaces. Maximum separation-based criterion for cohesive surfaces. damage initiation Quadratic separation-based damage initiation criterion for cohesive surfaces. Damage variable for cohesive surfaces. Fluid pressure for pressure penetration analysis. Solution-dependent state variables. 4.2.1–46 • • • • CSTRESSERI CDSTRESS CDISP CDISPETOS CFORCE CNAREA CSTATUS CSMAXSCRT CSQUADSCRT CSMAXUCRT CSQUADUCRT CSDMG PPRESS SDV • • • • • • • • • • • • • • • • • • • • • • • • • • Identifier .dat .fil .odb Field History Description Mechanical analysis–whole surface quantities • • • • • • • • • • • • • • • • • • • Total force due to contact pressure (CFNn, n = 1, 2, 3). Magnitude of total force due to contact pressure. Total force due to frictional stress (CFSn, n = 1, 2, 3). Magnitude of total force due to frictional stress. Total force due to contact pressure and frictional stress (CFTn, n = 1, 2, 3). Magnitude of total force due to contact pressure and frictional stress. Total moment about the origin due to contact pressure (CMNn, n = 1, 2, 3). Magnitude of total moment about origin due to contact pressure. Total moment about the origin due to frictional stress (CMSn, n = 1, 2, 3). Magnitude of total moment about the origin due to frictional stress. Total moment about the origin due to contact pressure and frictional stress (CMTn, n = 1, 2, 3). Magnitude of total moment about the origin due to contact pressure and frictional stress. Total area in contact. Maximum torque that can be transmitted about the z-axis by a contact surface in an axisymmetric analysis with a friction coefficient of unity. Center of the total force due to contact pressure (XNn, n = 1, 2, 3). Center of the total force due to frictional stress (XSn, n = 1, 2, 3). Center of the total force due to contact pressure and frictional stress (XTn, n = 1, 2, 3). Heat flux per unit area leaving the slave surface. HFL multiplied by the nodal area. 4.2.1–47 • • • • • • • • • • • • • • • CFN CFNM CFS CFSM CFT CFTM CMN CMNM CMS CMSM CMT CMTM CAREA CTRQ XN XS XT • • • • • • • • • • • Heat transfer analysis HFL HFLA • Identifier .dat .fil .odb Field History Description HTL HTLA • • • • • • Coupled thermal-electrical analysis • • • • • • • • • • • • • ECD ECDA ECDT ECDTA HFL HFLA HTL HTLA SJD SJDA SJDT SJDTA WEIGHT • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Time integrated HFL. Time integrated HFLA. Electrical current per unit area. ECD multiplied by the nodal area. Time integrated ECD. Time integrated ECDA. Heat flux per unit area leaving the slave surface. HFL multiplied by the nodal area. Time integrated HFL. Time integrated HFLA. Heat flux per unit area due to electrical current. SJD multiplied by the nodal area. Time integrated SJD. Time integrated SJDA. Weighting factor for heat distribution between the interface surfaces. Fully coupled temperature-displacement analysis HFL HFLA HTL HTLA SFDR SFDRA SFDRT SFDRTA WEIGHT • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Heat flux per unit area leaving the slave surface. HFL multiplied by the nodal area. Time integrated HFL. Time integrated HFLA. Heat flux per unit area due to frictional dissipation. SFDR multiplied by the nodal area. Time integrated SFDR. Time integrated SFDRA. Weighting factor for heat distribution between the interface surfaces. Fully coupled thermal-electrical-structural analysis • • • ECD ECDA ECDT • • • • • • • • • Electrical current per unit area. ECD multiplied by the nodal area. Time integrated ECD. Identifier .dat .fil .odb Field History Description ECDTA HFL HFLA HTL HTLA SFDR SFDRA SFDRT SFDRTA SJD SJDA SJDT SJDTA WEIGHT • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Time integrated ECDA. Heat flux per unit area leaving the slave surface. HFL multiplied by the nodal area. Time integrated HFL. Time integrated HFLA. Heat flux per unit area due to frictional dissipation. SFDR multiplied by the nodal area. Time integrated SFDR. Time integrated SFDRA. Heat flux per unit area due to electrical current. SJD multiplied by the nodal area. Time integrated SJD. Time integrated SJDA. Weighting factor for heat distribution between the interface surfaces. Coupled pore fluid-mechanical analysis–nodal quantities PFL PFLA PTL PTLA • • • • • • • • • • • • • • • • Pore fluid volume flux per unit area leaving the slave surface. PFL multiplied by the nodal area. Time integrated PFL. Time integrated PFLA. Coupled pore fluid-mechanical analysis–whole surface quantities TPFL TPTL • • Bond failure quantities DBT DBS DBSF BDSTAT CSDMG OPENBC • • • • • • • • • • • • • • Total pore fluid volume flux leaving the slave surface. Time integrated TPFL. • • • • • • • • • • • • Time when bond failure occurs. All components of remaining stress in the failed bond. Fraction of stress that remains at bond failure. Bond state (varies from 1.0 to 0.0). Damage variable. Relative displacement behind crack when fracture criterion is met. Identifier .dat .fil .odb Field History Description CRSTS ENRRT EFENRRTR • • • • • • • • • • • • All components of critical stress at failure. All components of strain energy release rate. Effective energy release rate ratio. Cavity radiation variables The following variables are associated with facets (sides of elements) composing cavities in radiation heat transfer and include contributions due to exchanges with the ambient. You can request cavity radiation variable output to the data, results, or output database file . Identifier .dat .fil .odb Field History Description RADFL RADFLA RADTL RADTLA VFTOT FTEMP • • • • • • • • • • • • • • • • • • • • • • • • Radiation flux per unit area. Radiation flux over the facet. Time integrated radiation per unit area. Time integrated radiation over the facet. Total viewfactor for the facet (sum of viewfactor values in the row of viewfactor matrix corresponding to the facet). Facet temperature. Section variables You can request section variable output to the data or results file . By default, all components of forces and moments are given with respect to the global system. If a local coordinate system is defined for the section output request, all components are given with respect to the local system. Different output variables are available depending on the type of analysis. For coupled analyses the appropriate combination of variables can be requested. For example, in a coupled thermal-electrical analysis both SOH and SOE are valid output requests. Section output variables are not available for random response analysis. Identifier .dat .fil .odb Field History Description All analysis types SOAREA • • Area of the defined section. Identifier .dat .fil .odb Field History Description Stress/displacement analysis SOF SOM SOCF • • • Heat transfer analysis SOH Electrical analysis SOE • • Mass diffusion analysis SOD • • • • • • • Total force in the section. Total moment in the section. Center of the total force in the section. Total heat flux associated with the section. Total current associated with the section. Total mass flow associated with the section. Coupled pore fluid diffusion-stress analysis SOP • • Whole and partial model variables Total pore fluid volume flux associated with the section. The output variables listed below are available for part of the model as well as the whole model. Identifier .dat .fil .odb Field History Description Adaptive mesh domains The following variable is available only for adaptive domains . • VOLC Change in area or change in volume of an element set solely due to adaptive meshing. • • Equivalent rigid body motion variables You can request equivalent rigid body motion whole element set variable output to the data, results, or output database file . The variables listed are available only for implicit dynamic analyses using direct integration except where indicated. Identifier .dat .fil .odb Field History Description XC XCn UC UCn URCn VC VCn VRCn HC HCn HO HOn RI • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • ). extraction, eigenvalue Current coordinates of the center of mass for the entire set or the entire model. Not available for buckling eigenfrequency prediction, complex eigenfrequency extraction, or linear dynamics procedures. Available also for static analyses but only from the output database. Coordinate n of the center of mass for the entire set or the entire model ( Current displacement of the center of mass for the entire set or the entire model. Available also for static analyses but only from the output database. Displacement component n of the center of mass for the entire set or the entire model ( Rotation component n of the center of mass for the entire set or the entire model ( Equivalent rigid body velocity components summed over the entire set or the entire model. Component n of the equivalent rigid body velocity summed over the entire set or the entire model ( ). ). ). ). ). Component n of the equivalent rigid body angular velocity summed over the entire set or the entire model ( Current angular momentum about the center of mass for the entire set or the entire model. Component n of the angular momentum about the center of mass for the entire set or the entire model ( Current angular momentum about the origin for the entire set or the entire model. Component n of the angular momentum about the origin for the entire set or the entire model ( Current rotary inertia about the origin of the entire set or the entire model. Not available for eigenfrequency extraction, eigenvalue buckling prediction, complex dynamics eigenfrequency extraction, linear or ). Identifier .dat .fil .odb Field History Description RIij MASS VOL • • • • • • • • procedures. Available also for static analyses but only from the output database. -component of the rotary inertia about the origin of the entire set or the entire model ( ). Current mass of the entire set or the entire model. Available also for static analyses but only from the output database. Current volume of the entire set or the entire model. Available also for static analyses but only from the output database. (Available only for continuum and structural elements that do not use general beam or shell section definitions.) Inertia relief output variables You can request inertia relief whole model variable output to the data or output database file . Since these variables have unique values for the entire model, the variable output is independent of the specified region. The variables listed are available only for those analyses that include inertia relief loading . Current coordinates of the reference point. Coordinate n of the reference point ( ). Equivalent rigid body acceleration components. Component n of the equivalent rigid body acceleration ( ). Component n of the equivalent rigid body angular to the reference point acceleration with respect ( ). Inertia relief load corresponding to the equivalent rigid body acceleration. Component n of the inertia relief load corresponding to the equivalent rigid body acceleration ( ). of the Component relief moment corresponding to the equivalent rigid body angular acceleration with respect to the reference point ( ). inertia Rotary inertia about the reference point. 4.2.1–53 • • • • • • • • • IRX IRXn IRA IRAn IRARn IRF IRFn IRMn IRRI • • • • • • • • Identifier .dat .fil .odb Field History Description IRRIij IRMASS • • Mass diffusion analysis • • -component of the rotary inertia about the reference point ( ). Whole model mass. You can request variable output from a mass diffusion analysis (“Mass diffusion analysis,” Section 6.9.1) to the data, results, or output database file . If you specify an output region, the variable is calculated over the user-specified region. If you do not specify an output region, the variable is calculated as the total over the entire model. SOL • • • Amount of solute in an element set, calculated as the sum of ESOL (amount of solute in each element) over all the elements in the set. Analyses with time-dependent material behavior CRPTIME • Creep time, which is equal time in procedures with time-dependent material behavior . to the total Eigenvalue extraction The following variables are output automatically during a frequency extraction analysis (“Natural frequency extraction,” Section 6.3.5). EIGVAL EIGFREQ GM CD PFn EMn Eigenvalues. Eigenfrequencies. Generalized masses. Composite damping factors. Modal participation factors 1–7 ( corresponding to displacements, the rotations, and Modal effective masses 1–7 ( corresponding to displacements, for the rotations, and for acoustic pressure). for for acoustic pressure). Complex eigenvalue extraction The following variables are output automatically during a complex frequency extraction analysis (“Complex eigenvalue extraction,” Section 6.3.6). Identifier .dat .fil .odb Field History Description EIGREAL EIGIMAG EIGFREQ DAMPRATIO Total energy output quantities Real parts of the eigenvalues. Imaginary parts of the eigenvalues. Eigenfrequencies. Damping ratios. If the following whole model variables are relevant for a particular analysis, you can request them as output to the data, results, or output database file . If you do not specify an output region, whole model variables are calculated. When you specify an output region, the relevant energy totals are calculated over the user-specified region. These variables are not available for eigenvalue buckling prediction, eigenfrequency extraction, or complex frequency extraction analysis. You cannot specify an output region for modal dynamic, random response, response spectrum, or steady-state dynamic analysis. See “Energy balance,” Section 1.5.5 of the Abaqus Theory Manual, for details of the energy definitions. ALLAE ALLCD ALLEE ALLFD ALLIE ALLJD ALLKE ALLKL ALLPD ALLQB • • • • • • • • • • by and creep, swelling, dissipated “Artificial” strain energy associated with constraints used to remove singular modes (such as hourglass control), and with constraints used to make the drill rotation follow the in-plane rotation of the shell elements. Energy viscoelasticity. Electrostatic energy. Total energy dissipated through frictional effects. (Available only for the whole model.) Total strain energy. (ALLIE = ALLSE + ALLPD + ALLCD + ALLAE + ALLQB + ALLEE + ALLDMD.) Electrical energy dissipated due to flow of electrical current. Kinetic energy. Loss of kinetic energy at impact. (Available only for the whole model.) Energy dissipated by rate-independent and rate- dependent plastic deformation. Energy dissipated through quiet boundaries (infinite elements). (Available only for the whole model.) Identifier .dat .fil .odb Field History Description ALLSD ALLSE ALLVD ALLDMD ALLWK ETOTAL • • • • • • Energy dissipated by automatic stabilization. This includes both volumetric static stabilization and automatic approach of contact pairs (the latter part included only for the whole model). Recoverable strain energy. Energy dissipated by viscous effects including viscous regularization, not inclusive of energy dissipated by automatic stabilization and viscoelasticity. Energy dissipated by damage. External work. (Available only for the whole model.) Total energy balance (available only for the whole model). (ETOTAL = ALLKE + ALLIE + ALLVD + ALLSD + ALLKL + ALLFD + ALLJD − ALLWK.) Solution-dependent amplitude variables Solution-dependent amplitude variables are given automatically with any file output or output database request. Identifier .dat .fil .odb Field History Description LPF AMPCU RATIO Load proportionality factor in a static Riks analysis. Current value of the solution-dependent amplitude. Current maximum ratio of creep strain rate and target creep strain rate. Structural optimization variables Structural optimization output variables are requested by the Abaqus Topology Optimization Module during each design cycle. For more information, see Chapter 13, “Optimization Techniques.” Identifier .dat .fil .odb Field History Description Toplogy optimization The following variable is output automatically during topology optimization . MAT_PROP_NORMALIZED Element-based normalized material value. Identifier .dat .fil .odb Field History Description Shape optimization The following variables are output automatically during shape optimization . CTRL_INPUT(OPT) DISP_OPT_VAL DISP_OPT Material scaling coefficient. The value of the optimization displacement. A vector representing the optimization displacement. 4.2.2 Abaqus/Explicit OUTPUT VARIABLE IDENTIFIERS Product: Abaqus/Explicit References • “Output,” Section 4.1.1 • “Output to the data and results files,” Section 4.1.2 • “Output to the output database,” Section 4.1.3 Overview Except for the information in the status file, results can be obtained from Abaqus/Explicit only by postprocessing. The tables in this section list all of the output variables that are available in Abaqus/Explicit. These output variables can be requested for output to the results (.fil) file or as either field- or history-type output to the output database (.odb) file . When the output variables are requested for output to the results file, Abaqus/Explicit will first output these variables to the selected results (.sel) file and will then convert the selected results file to the results file after the analysis completes. Symbols used in the tables The availability of the various output variable identifiers is defined by a under the following headings: in the columns of the table, .fil means that the identifier can be used as a results file output selection. .odb Field means that the identifier can be used as a field-type output selection to the output database. .odb History means that the identifier can be used as a history-type output selection to the output database. Direction definitions The direction definitions depend on the variable type. Direction definitions for element variables For components of stress, strain, and similar material variables, 1, 2, and 3 refer to the directions in an orthogonal coordinate system. These are global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam and pipe elements. However, if a local orientation (“Orientations,” Section 2.2.5) is associated with the elements for which output is being requested, 1, 2, and 3 are local directions. Direction definitions for nodal variables For nodal variables, 1, 2, and 3 refer to the global directions (1=X, 2=Y, 3=Z except for axisymmetric elements, in which case 1=R, 2=Z). Even if a local coordinate system has been defined at a node (“Transformed coordinate systems,” Section 2.1.5), the data in the results file and the selected results file are still output in the global directions. If nodal field output is requested for a node that has a local coordinate system defined, a quaternion representing the rotation from the global directions is written to the output database. Abaqus/CAE automatically uses this quaternion to transform the nodal results into the local directions. Nodal history data written to the output database are always stored in the global directions. Direction definitions for integrated variables For components of total force, total moment, and similar variables obtained through integration over a surface, the directions 1, 2, and 3 refer to directions in an orthogonal coordinate system. A fixed global coordinate system is used if the surface is specified directly for the integrated output request. If the surface is identified by an integrated output section definition that is associated with the integrated output request, a local coordinate system in the initial configuration can be specified and can translate or rotate with the deformation. Distributed load output and user subroutines Output can be requested for many of the distributed loads discussed in “Loads,” Section 33.4. However, contributions to these loads defined through user subroutines are not displayed. Principal value output Output of the principal values can be requested for stresses, logarithmic strains, and nominal strains. Either all principal values or the minimum, intermediate, or maximum values can be obtained. All principal values of tensor ABC are obtained with the request ABCP, and the minimum, intermediate, and maximum principal values are obtained with the requests ABCP1, ABCP2, and ABCP3, respectively. For three-dimensional, plane strain, and axisymmetric elements all three principal values are obtained. For plane stress, membrane, and shell elements only the in-plane principal values are obtained for history- type output, and the out-of-plane principal value cannot be requested. For field-type output, all three principal values are obtained through Abaqus/CAE. Principal values cannot be obtained for beam, pipe, and truss elements, and principal values of plastic strains cannot be requested. If a principal value or an invariant is requested for field-type output, the output request is replaced with an output request for the components of the corresponding tensor. Abaqus/CAE calculates all principal values and invariants from these components. If a principal value is desired as history-type output, it must be requested explicitly since Abaqus/CAE does no calculations on history data. Tensor output Tensor variables that are written to the output database as field-type output are written as components in either the default directions defined by the convention given in “Orientations,” Section 2.2.5 (global directions for solid elements, surface directions for shell and membrane elements, and axial and transverse directions for beam and pipe elements), or the user-defined local system. Abaqus/CAE calculates all principal values and invariants from these components. See “Writing field output data,” Section 9.6.4 of the Abaqus Scripting User’s Manual, for a description of the different types of tensor variables. The components for tensor variables are written to the output database in single precision. Therefore, a small amount of precision roundoff error may occur when calculating the variables’ principal values. Such roundoff error may be observed, for example, when analytically zero values are calculated as relatively small yet nonzero values. Requesting output of components Individual components of variables can be requested as history-type output in the output database for X–Y plotting in Abaqus/CAE. Individual component requests are not available for field-type output. If a particular component is desired for contouring in Abaqus/CAE, request field output of the generic variable (e.g., S for stress). Output for individual components of this field output can be requested within the Visualization module of Abaqus/CAE. Element integration point variables You can request element integration point variable output to the results or output database file . Identifier .fil .odb Field History Description Tensors and invariants MISESMAX • • • Sij SP • • • • • All stress components. Maximum Mises stress among all of the section points. For a shell element it represents the maximum Mises value among all the section points in the layer, for a beam or pipe element it is the maximum Mises stress among all the section points in the cross-section, and for a solid element it represents the Mises stress at the integration points. -component of stress ( ). All principal stress components. Identifier .fil .odb Field History Description intermediate, and maximum principal Minimum, stress components (SP1 All infinitesimal strain components for geometrically linear analysis. SP3). SP2 -component of infinitesimal strain ( All logarithmic strain components. -component of logarithmic strain ( ). ). intermediate, and maximum principal All principal logarithmic strain components. Minimum, logarithmic strain components (LEP1 LEP3). All logarithmic strain rate components. -component of logarithmic strain rate( LEP2 ). All principal logarithmic strain rate components. Minimum, strain rate components (ERP1 All nominal strain components. intermediate, and maximum principal ERP3). ERP2 -component of nominal strain ( ). All principal nominal strain components. Minimum, intermediate, and maximum principal nominal strain components (NEP1 NEP2 NEP3). All plastic strain components. -component of plastic strain ( ). All principal plastic strains. Minimum, plastic strains. Volumetric strain rate. intermediate, and maximum principal Mises equivalent stress, defined as where is the deviatoric stress tensor, defined as , where is the stress and , is the equivalent pressure stress. Equivalent pressure stress, Stress triaxiality, All total kinematic hardening shift tensor components. . . -component of the total shift tensor ( ). 4.2.2–4 SPn Eij LE LEij LEP LEPn ER ERij ERP ERPn NE NEij NEP NEPn PE PEij PEP PEPn ERV MISES PRESS TRIAX ALPHA ALPHAij • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Identifier .fil .odb Field History Description All ( kinematic hardening shift tensor components ). -component of the and tensor ( kinematic hardening shift ). All tensor components of all the kinematic hardening shift tensors, except the total shift tensor, ALPHA. All principal values of the total shift tensor. Minimum, values of ALPHAP2 ALPHAP3). intermediate, and maximum principal tensor the total (ALPHAP1 shift Equivalent plastic strain. For porous metal plasticity PEEQ is the equivalent plastic strain in the matrix material defined as . For cap plasticity PEEQ gives (the cap position). crushable For foam plasticity with volumetric hardening PEEQ gives the volumetric compacting plastic strain defined as . For crushable foam plasticity with isotropic hardening PEEQ gives the equivalent plastic strain defined as is the uniaxial compression yield , where stress. Equivalent plastic strain in uniaxial tension for cast iron, Mohr-Coulomb tension cutoff, and concrete damaged plasticity, which is defined as . Maximum equivalent plastic strain, PEEQ, among all of the section points. For a shell element it represents the maximum PEEQ value among all the section points in the layer, for a beam or a pipe element it is the maximum PEEQ among all the section points in the cross-section, and for a solid element it represents the PEEQ at the integration points. 4.2.2–5 ALPHAk ALPHAk_ij ALPHAN ALPHAP ALPHAPn PEEQ • • PEEQT PEEQMAX • • • • • • • • • • • • Identifier .fil .odb Field History DMICRTMAX • Description Maximum damage initiation among all of the section points and all of the damage initiation criteria. This output variable generates three output quantities as follows: DMICRTMAXVAL outputs the maximum damage initiation value. DMICRTPOS outputs the section point in the layer in which the maximum damage initiation value occurred. For solid elements, the output value is one. DMICRTTYPE outputs a value that represents the damage initiation criteria type that reached the maximum value in the element as follows: For elements that have failure with progressive 1-DUCTCRT, 2-SHRCRT, 3-JCCRT, damage: 4-FLDCRT, and 7-MKCRT. 5-MSFLDCRT, 6-FLSDCRT, For elements that have fiber-reinforced material damage: 11-HSNFTCRT, 12-HSNFCCRT, 13- HSNMTCRT, and 14-HSNMCCRT. cohesive For behavior: QUADSCRT, and 24-QUADECRT. elements with traction-separation 23- 22-MAXECRT, 21-MAXSCRT, Geometric quantities COORD • • The maximum damage initiation output values are retained across the requested output frames until a higher maximum damage initiation value is computed. solid Coordinates of elements. These are the current coordinates if the large-displacement formulation is being used. the integration point for Identifier .fil .odb Field History Description Direction cosines of the local material directions for an anisotropic hyperelastic material model, or yarn direction cosines for a fabric material model. This variable is output automatically if any other element field output is requested for anisotropic hyperelastic or fabric material . transverse shear stress components for three- All dimensional conventional shell elements. -component of transverse shear stress. -component of transverse shear stress. All energy densities. Elastic strain energy density, per unit volume. Energy dissipated by rate-independent and rate- dependent plasticity, per unit volume. Energy dissipated by viscoelasticity, per unit volume (not supported for hyperelastic and hyperfoam material models). Energy dissipated by viscous effects, per unit volume. Energy dissipated by damage, per unit volume. Solution-dependent state variables. Solution-dependent state variable n. Temperature. Material density. Field variables. Field variable n. All failure measure components. Maximum stress theory failure measure. 4.2.2–7 • • • • • • • • • • • • • • • LOCALDIRn Additional element stresses • TSHR • • • TSHR13 TSHR23 Energy densities ENER SENER PENER CENER VENER DMENER State and field variables SDV SDVn TEMP DENSITY FV FVn • • • • • • • Composite failure measures • CFAILURE Identifier .fil .odb Field History Description TSAIH TSAIW AZZIT MSTRN Tsai-Hill theory failure measure. Tsai-Wu theory failure measure. Azzi-Tsai-Hill theory failure measure. Maximum strain theory failure measure. All equivalent plastic strains, when the model has more than one yield/failure surface. nth equivalent plastic strain ( ). For cap plasticity: PEQC provides equivalent plastic strains for all three possible yield/failure surfaces (Drucker-Prager failure surface - PEQC1, cap surface - PEQC2, and transition surface - PEQC3) and the total volumetric plastic strain (PEQC4). All identifiers also provide a yes/no flag (1/0 in the output database), telling whether the yield surface is currently active or not (AC YIELD: “actively yielding”). When PEQC is requested as output to the output database, the active yield flags for each component are named AC YIELD1, AC YIELD2, etc. Void volume fraction (porous metal plasticity). Void volume fraction due to growth (porous metal plasticity). Void volume fraction due to nucleation (porous metal plasticity). Compressive damage variable, . Tensile damage variable, . Scalar stiffness degradation variable, d. Equivalent plastic strain in uniaxial compression, . which is defined as 4.2.2–8 Additional plasticity quantities PEQC PEQCn • • • • Porous metal plasticity quantities • • VVFG VVF • • • • VVFN • • DAMAGEC Concrete damaged plasticity • • • • DAMAGET SDEG PEEQ • • • • Identifier .fil .odb Field History Description Cracking model quantities All cracking strain components. -component of cracking strain. All cracking strain components in local crack axes. -component of cracking strain in local crack axes. Cracking strain magnitude, defined as . All stress components in local crack axes. -component of stress in local crack axes. Crack orientations. Crack status of each crack. CKSTAT can have the following values for each crack: 0.0=uncracked, 1.0=closed crack, 2.0=actively cracking, 3.0=crack closing/reopening. stress diagram (FLSD) damage All active components of the damage initiation criteria. Ductile damage initiation criterion. Johnson-Cook damage initiation criterion. Shear damage initiation criterion. Forming limit diagram (FLD) damage initiation criterion. Forming limit initiation criterion. Müschenborn-Sonne forming limit stress diagram (MSFLD) damage initiation criterion. Marciniak-Kuczynski criterion. Overall scalar stiffness degradation. Ratio of principal strain rates, damage initiation criterion. Shear stress ratio, shear damage initiation criterion. , used for the MSFLD , used for the initiation damage (M-K) All active components of the damage initiation criteria. 4.2.2–9 CKE CKEij CKLE CKLEij CKEMAG CKLS CKLSij CRACK CKSTAT • • • • • • Failure with progressive damage DMICRT DUCTCRT JCCRT SHRCRT FLDCRT FLSDCRT MSFLDCRT MKCRT SDEG ERPRATIO SHRRATIO • • • • • • • • • • • • • • • Fiber-reinforced materials damage • DMICRT Identifier .fil .odb Field History Description HSNFTCRT HSNFCCRT HSNMTCRT HSNMCCRT DAMAGEFT DAMAGEFC DAMAGEMT DAMAGEMC DAMAGESHR Fabric material • • • • • • • • • • • • • • Hashin’s fiber tensile damage initiation criterion. Hashin’s fiber compressive damage initiation criterion. Hashin’s matrix tensile damage initiation criterion. Hashin’s matrix compressive damage criterion. Fiber tensile damage variable. Fiber compressive damage variable. Matrix tensile damage variable. Matrix compressive damage variable. Shear damage variable. initiation Output variable LOCALDIR (described above) is output automatically for fabric materials. All fabric stress components. All fabric strain components. -component of fabric stress ( -component of fabric strain ( ). ). Burn fraction of the ignition and growth material. Reaction rate of the ignition and growth material. Density of the unreacted explosive in the ignition and growth material. Density of the reacted gas product in the ignition and growth material. Distension, Minimum value, during plastic compaction of the material. , of the distension attained porous porous material. , of the Force in rebar. Angle, in degrees, between rebar and the user- specified isoparametric direction. Available only for shell and membrane elements. 4.2.2–10 SFABRIC EFABRIC SFABRICij EFABRICij Equation of state BURNF DBURNF RHOE RHOP PALPH PALPHMIN Rebar quantities RBFOR RBANG • • • • • • • • • • • • • • • • • • • • • • • Identifier .fil .odb Field History Description Change in angle, in degrees, between rebar and the user-specified isoparametric direction. Available only for shell and membrane elements. Coordinates of element integration point. Current magnitude and components of the heat flux per unit area vector. Current magnitude of the heat flux per unit area vector. Component n of the heat flux vector ( ). Maximum nominal stress damage initiation criterion. Maximum nominal strain damage initiation criterion. Quadratic nominal stress damage initiation criterion. Quadratic nominal strain damage initiation criterion. All active components of the damage initiation criteria. Overall scalar stiffness degradation. Status of the element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). Eulerian volume fraction. Output includes volume fraction data for each material defined in the Eulerian section, plus the volume fraction of void. Density, computed as a volume fraction weighted average of all materials in the element. Mises stress, computed as a volume fraction weighted average of all materials in the element. Plastic strain components, computed as a volume fraction weighted average of all materials in the element. Equivalent plastic strain, computed as a volume fraction weighted average of all materials in the element. 4.2.2–11 • • • • • • • • • • • • • RBROT • • Integration point coordinates COORD • Coupled thermal-stress elements • • HFL HFLM HFLn Cohesive elements MAXSCRT MAXECRT QUADSCRT QUADECRT DMICRT SDEG STATUS Eulerian elements EVF DENSITYVAVG MISESVAVG PEVAVG PEEQVAVG • • • • • • • Identifier .fil .odb Field History Description PRESSVAVG SVAVG TEMPMAVG • • • Element section variables Equivalent pressure stress, computed as a volume fraction weighted average of all materials in the element. Stress components, computed as a volume fraction weighted average of all materials in the element. Temperature, computed as a mass fraction weighted average of all materials in the element. You can request element section variable output to the results or output database file . These variables are available only for beam, pipe, and shell elements with the exception of STH, which is also available for membrane elements. They are defined for particular elements in the element descriptions in Part VI, “Elements.” .odb Field History • • • • • • • • • • • • Description Section thickness (shell and membrane elements only). All section resultant components, both translational (forces) and rotational (moments). Section force component n, conventional shells; shells; for beams and pipes. for for continuum Section moment component n, . All section nominal strains, both translational and rotational (e.g., midplane strain and curvature in shells). Section nominal strain for shells; component n, for beams and pipes. Section curvature change or twist n, . All average membrane and transverse shear stress components (shell elements only). transverse shear stress (shell elements Average membrane or component n, only). 4.2.2–12 Identifier .fil • • • • STH SF SFn SMn SE SEn SKn SSAVG Whole element variables You can request whole element variable output to the results or output database file . .odb Field History • • • • • • • • • • • • • • • • • • • • • • • • • Description All energy magnitudes in the element. Total elastic strain energy in the element (includes energy in transverse shear deformation in shells). Total energy dissipated in the element by viscoelastic (Not supported for hyperelastic and deformation. hyperfoam material models.) Total energy dissipated in the element by rate- independent and rate-dependent plastic deformation. Total energy dissipated in the element by viscous effects. This includes bulk viscosity and material damping. Total “artificial” strain energy in the element. This includes hourglass energy and drilling stiffness energy in shells. Internal heat energy in the element. Total energy dissipated in the element by damage. Total energy dissipated in the element by distortion control. All element energy density components. Total elastic strain energy density in the element. Total energy dissipated per unit volume in the element by rate-independent and rate-dependent plastic deformation. Total energy dissipated per unit volume in the element by viscoelasticity. Total energy dissipated per unit volume in the element by viscous effects. Total “artificial” strain energy density in the element (energy associated with constraints used to remove singular modes, such as hourglass control). Internal heat energy density in the element. 4.2.2–13 Identifier .fil • ELEN ELSE ELCD ELPD ELVD ELASE ELIHE ELDMD ELDC ELEDEN ESEDEN EPDDEN ECDDEN EVDDEN EASEDEN Identifier .fil .odb Field History Description EDMDDEN EDCDEN EDT EMSF STATUS • • • EVOL NFORC GRAV SBF BF EDMICRTMAX • • • • • • • • • • • • • • • Total energy dissipated per unit volume in the element by damage. Total energy dissipated per unit volume in the element by distortion control. Element stable time increment. Element mass scaling factor. Status of element (material failure with progressive damage, shear failure model, tensile failure model, porous failure criterion, brittle failure model, Johnson- Cook plasticity model, and VUMAT). The status of an element is 1.0 if the element is active, 0.0 if the element is not. Current element volume. (Only available for continuum and structural elements not using general beam or shell section definitions.) Forces at the nodes of an element from both the hourglass and the regular deformation modes of that element (internal forces in the global coordinate system). Uniformly distributed gravity load. Stagnation body force. Uniformly distributed body force, including viscous body force. Whole shell element maximum damage initiation output among all of the layers, all of the damage initiation criteria, and for fully integrated elements across all of the integration points. This output variable is the same as DMICRTMAX output for solid and beam elements but complements the DMICRTMAX output variable for composite shell elements because it extracts the maximum damage initiation across all of the layers. This output variable generates four element output quantities as follows: Identifier .fil .odb Field History Description EDMICRTMAXVAL outputs the maximum damage initiation value in the entire element. EDMICRTLAYER outputs the layer number in which the maximum damage initiation value occurred. EDMICRTTYPE outputs a value that represents the damage initiation criteria type that reached the maximum value in the element, as described in the DMICRTMAX output variable description. EDMICRTINTP outputs the integration point number for which the maximum damage value occurred. For reduced-integration elements, the output value is one. The maximum damage initiation output values are retained across the requested output frames until a higher maximum damage initiation value is computed. ). ). total forces and All components of connector moments. Connector total force component n ( Connector total moment component n ( All components of connector elastic forces and moments. Connector elastic force component n ( Connector elastic moment component n ( Elastic displacements and rotations in all directions. Elastic displacement in the n-direction ( ). Elastic rotation in the n-direction ( Plastic relative displacements and rotations in all directions. Plastic relative displacement in the n-direction ( ). ). ). ). ). Plastic relative rotation in the n-direction ( Equivalent plastic relative displacements and rotations in all directions, and equivalent plastic relative motion for a coupled plasticity definition. 4.2.2–15 Connector elements • CTF CTFn CTMn CEF CEFn CEMn CUE CUEn CUREn CUP CUPn CURPn CUPEQ • • • • • • • • • • • • • • • • • • • • • Identifier .fil .odb Field History Description CUPEQn CURPEQn CUPEQC CALPHAF CALPHAFn CALPHAMn CVF CVFn CVMn CUF CUFn CUMn CSF CSFn CSMn CSFC CNF CNFn CNMn • • • • • • • • • • • • • • • • • • • • • • • • • Equivalent plastic relative displacement n-direction ( ). in the Equivalent plastic relative rotation in the n-direction ( ). Equivalent plastic relative motion for a coupled plasticity definition. All components of connector kinematic hardening shift forces and moments. Connector kinematic hardening shift force component n ( ). Connector component n ( kinematic hardening ). shift moment All components of connector viscous forces and moments. Connector viscous force component n ( Connector viscous moment component n ( ). ). All components of connector uniaxial forces and moments. Connector uniaxial force component n ( ). Connector uniaxial moment component n ( ). All components of connector friction forces and moments. Connector friction force component n ( Connector friction moment component n ( ). ). Connector friction force in the instantaneous slip direction. Available only if friction is defined in the slip direction. All components of connector contact forces and moments. Connector component n (n = 1, 2, 3). friction-generating Connector component n (n = 1, 2, 3). friction-generating friction-generating contact force contact moment Identifier .fil .odb Field History Description Connector friction-generating contact force in the instantaneous slip direction. Available only if friction is defined in the slip direction. All components of the overall damage variable. Overall damage variable component n ( Overall damage variable component n ( Components initiation criterion in all directions. connector of force-based ). ). damage Connector force-based damage initiation criterion in the n-translation direction ( ). Connector force-based damage initiation criterion in the n-rotation direction ( ). Connector force-based damage initiation criterion in the instantaneous slip direction. Components of connector motion-based damage initiation criterion in all directions. Connector motion-based damage initiation criterion in the n-translation direction ( ). Connector motion-based damage initiation criterion in the n-rotation direction ( ). Connector motion-based damage initiation criterion in the instantaneous slip direction. Components of connector plastic motion-based damage initiation criterion in all directions (including the instantaneous slip direction). Connector plastic motion-based damage initiation criterion in the n-translation direction ( ). Connector plastic motion-based damage initiation criterion in the n-rotation direction ( ). Connector plastic motion-based damage initiation criterion in the instantaneous slip direction. All flags for connector stop and connector lock status. Flag for connector stop and connector lock status in the i-direction ( ). Components of accumulated slip in all directions. 4.2.2–17 CNFC CDMG CDMGn CDMGRn CDIF CDIFn CDIFRn CDIFC CDIM CDIMn CDIMRn CDIMC CDIP CDIPn CDIPRn CDIPC CSLST CSLSTi CASU • • • • • • • • • • • • • • • • • • • • • • • • • • Identifier .fil .odb Field History Description CASUn CASURn CASUC CIVC CRF CRFn CRMn CCF CCFn CCMn CP CPn CPRn CU CUn CURn CCU CCUn CCURn CV CVn CVRn • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Connector accumulated slip in the n-direction (n = 1, 2, 3). Connector angular accumulated slip in the n-direction (n = 1, 2, 3). Connector accumulated slip in the instantaneous slip direction. Available only if friction is defined in the slip direction. Connector instantaneous velocity in the slip direction. Available only if friction is defined in the slip direction. All components of connector reaction forces and moments. Connector reaction force component n ( Connector reaction moment component n ( ). ). All components of connector concentrated forces and moments. Connector concentrated force component n ( ). Connector concentrated moment component n ( ). in the position angular ). ). n-direction Relative positions in all directions. Relative position in the n-direction ( Relative ( Relative displacements and rotations in all directions. ). Relative displacement in the n-direction ( Relative rotation in the n-direction ( Constitutive displacements and rotations directions. Constitutive ( Constitutive rotation in the n-direction ( Relative velocities in all directions. Relative velocity in the n-direction ( Relative ( ). n-direction ). in all angular ). displacement n-direction velocity the the in in ). ). Identifier .fil .odb Field History Description • • CA CAn CARn CFAILST CFAILSTi CDERU CDERF • • • • • • • • • • • Element face variables Relative accelerations in all directions. Relative acceleration in the n-direction ( ). Relative angular acceleration in the n-direction ( ). All flags for connector failure status. Flag for connector failure status in the i-direction ( ). Connector derived displacement. Connector derived force. You can request element face variable output to the output database file . These variables are available only for shell, membrane, and solid elements. Identifier .fil .odb Field History • • • • • • STAGP VP IWCONWEP TRNOR TRSHR Nodal variables Description Uniformly distributed pressure load on element faces. When the pressure is defined using *DLOAD, the variable name is changed automatically to PDLOAD. Stagnation pressure load on element faces. Viscous pressure load on element faces. Air blast pressure load from the CONWEP model on element faces. Normal component (component along face normal) of traction load on element faces. Shear component (component along face tangent) of traction load on element faces. You can request nodal variable output to the results or output database file . .odb Field History • • • • • • • • • • • • • • • • • • • • • • • • • • • • • Description Coordinates of the node. These are the current coordinates if the large-displacement formulation is being used. Coordinate n ( ). Displacement components. Results file and field-type output: both translation and rotation. History-type output: translation only. Rotation results should be requested by components. Translational displacement components. Rotational displacement components. displacement component ( rotation component ( ). ). Velocity components (both translation and rotation). Results file and field-type output: both translation and rotation. History-type output: translation only. Rotation results should be requested by components. Translational velocity components. Rotational velocity components. velocity component ( rotational velocity component ( ). ). Acceleration components rotation). (both translation and Results file and field-type output: both translation and rotation. History-type output: translation only. Rotation results should be requested by components. Translational acceleration components. Rotational acceleration components. acceleration component ( rotational acceleration component ( ). ). Acoustic pressure at a node. 4.2.2–20 Identifier .fil COORD COORn UT UR Un URn VT VR Vn VRn AT AR An ARn POR • • • • Identifier .fil .odb Field History Description Acoustic absolute pressure at a node. All temperature values at a node. Available only for coupled thermal-stress analysis. Temperature degree of freedom n at a node ( Available only for coupled thermal-stress analysis. Reaction force and moment components. ). Results file and field-type output: both translation and rotation. History-type output: translation only. Rotation results should be requested by components. ). ) (conjugate ). Available Reaction force components. Reaction moment components. Reaction force component n ( to prescribed displacement All reaction flux values. Available only for coupled thermal-stress analysis. Reaction flux value n at a node ( only for coupled thermal-stress analysis. Reaction moment component n ( (conjugate to prescribed rotation ). All components of point moments. Point load component n ( Point moment component n ( Nodal volume fraction. Status of the tied slave nodes (the status of a slave node is 2 if the slave node is not tied, 1 if the slave node is tied, and 0 for nodes that do not participate in a tie constraint). Position adjustment vector components of the tied slave nodes. loads and concentrated ). ). ) Fluid cavity gauge pressure. Fluid cavity volume. 4.2.2–21 • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • PABS NT NTn RF RT RM RFn RFL RFLn RMn CF CFn CMn NVF TIEDSTATUS TIEADJUST Fluid cavity variables • • PCAV Identifier .fil .odb Field History Description CTEMP CSAREA CLAREA CBLARAT CMASS APCAV TCVOL ACTEMP TCSAREA TCMASS CMF CMFL CMFLT CEFL CEFLT MINFL MINFLT TINFL • • • • • • • • • • • • • • • • • • Fluid cavity temperature for an ideal gas model used under adiabatic conditions. Fluid cavity surface area. Fluid cavity unblocked leakage area. Ratio of the blocked leakage area to the unblocked leakage area. Mass of the fluid contained in a fluid cavity. Average gauge pressures for multiple fluid cavities. Total volume of multiple fluid cavities. Average fluid cavity temperature for an ideal gas model used under adiabatic conditions for multiple fluid cavities. Total surface area of multiple fluid cavities. Total mass of the fluid contained in the multiple fluid cavities. Molecular mass fraction of fluid species contained in a fluid cavity. Mass flow rate out of a fluid cavity. Accumulated mass flow out of a fluid cavity. Heat energy flow rate out of a fluid cavity. Accumulated heat energy flow out of a fluid cavity. Inflator mass flow rate into a fluid cavity. Accumulated inflator mass flow into a fluid cavity. Inflator temperature. Surface variables You can request surface variable output in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3); additional information on these variables is provided in “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1; “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1; and “Thermal contact properties,” Section 36.2.1. to the output database file (see “Surface output Identifier .fil .odb Field History Description Mechanical analysis–nodal quantities damage initiation Contact normal force (CNORMF) and frictional shear force (CSHEARF). Contact pressure (CPRESS) and frictional shear stress (CSHEAR). CSHEAR is not available for general contact analyses. Contact thickness in general contact or contact pairs. Maximum stress-based damage initiation criterion for cohesive surfaces in general contact. Quadratic stress-based damage initiation criterion for cohesive surfaces in general contact. Maximum separation-based criterion for cohesive surfaces in general contact. Quadratic separation-based damage initiation criterion for cohesive surfaces in general contact. Damage variable for cohesive surfaces in general contact. Length of contact slip path at slave nodes during contact (FSLIPEQ) and in some cases tangent components of net contact slip in local directions (FSLIP1 and FSLIP2). These variables remain constant while a slave node is not in contact. Magnitude of contact slip rate at slave nodes during contact (FSLIPR) and in some cases components of contact slip rate in local tangent directions (FSLIPR1 and FSLIPR2). These variables are set to zero while a slave node is not in contact. Spot weld bond status. Spot weld bond load. Time when bond failure occurs. All components of remaining stress in the failed bond. Fraction of stress that remains at bond failure. 4.2.2–23 CFORCE CSTRESS CTHICK CSMAXSCRT CSQUADSCRT CSMAXUCRT CSQUADUCRT CSDMG FSLIP FSLIPR • • • • • • • • • • BONDSTAT BONDLOAD • • Crack bond failure quantities DBT DBS DBSF • • Identifier .fil .odb Field History Description BDSTAT OPENBC CRSTS ENRRT EFENRRTR • • • • • Mechanical analysis–whole surface quantities CFN CFNM CFS CFSM CFT CFTM CMN CMNM CMS CMSM CMT CMTM CAREA XN XS XT • • • • • • • • • • • • • • • • Bond state (the state is 1.0 if bonded, 0.0 if unbonded). Relative displacement behind crack when fracture criterion is met. All components of critical stress at failure. All components of strain energy release rate. Effective energy release rate ratio. Total force due to contact pressure (CFNn, n = 1, 2, 3). Magnitude of total force due to contact pressure. Total force due to frictional stress (CFSn, n = 1, 2, 3). Magnitude of total force due to frictional stress. Total force due to contact pressure and frictional stress (CFTn, n = 1, 2, 3). Magnitude of total force due to contact pressure and frictional stress. Total moment about the origin due to contact pressure (CMNn, n = 1, 2, 3). Magnitude of total moment about the origin due to contact pressure. Total moment about the origin due to frictional stress (CMSn, n = 1, 2, 3). Magnitude of total moment about the origin due to frictional stress. Total moment about the origin due to contact pressure and frictional stress (CMTn, n = 1, 2, 3). Magnitude of total moment about the origin due to contact pressure and frictional stress. Total area in contact. Center of the total force due to contact pressure (XNn, n = 1, 2, 3). Center of the total force due to frictional stress (XSn, n = 1, 2, 3). Center of the total force due to contact pressure and frictional stress (XTn, n = 1, 2, 3). Identifier .fil .odb Field History Description Fully coupled temperature-displacement analysis HFL HFLA HTL HTLA SFDR SFDRA SFDRT SFDRTA Integrated variables • • • • • • • • Heat flux per unit area leaving the surface. HFL multiplied by the nodal area. Time integrated HFL. HTL multiplied by the nodal area. Heat flux per unit area due to frictional dissipation. SFDR multiplied by the nodal area. Time integrated SFDR. SFDRT multiplied by the nodal area. integrated variable output You can request in Abaqus/Explicit” in “Output to the output database,” Section 4.1.3). The output quantity is computed by integration over a surface or an element set that is specified either directly in the integrated output request or by associating an integrated output section definition or an element set definition with the integrated output request. to the output database (see “Integrated output The components of the vector output variables are given with respect to a global coordinate system when no integrated output section definition is associated with the integrated output request. When an integrated output section is associated with the integrated output request and a local coordinate system is defined for the integrated output section, the components are given in the local system. The local system will rotate with the deformation if a reference node with rotation degrees of freedom is associated with the section definition. Identifier .fil SOAREA SOF SOM .odb Field History • • • Description Area of the surface as projected onto a plane normal to the average surface normal. Total force transmitted through the surface. Total moment transmitted through the surface. The moment of the forces transmitted through the surface is taken about the current location of the reference node if one is specified on an integrated output section and is associated with the integrated output request. The moment is taken about the global origin either if no section definition is associated with the integrated output request or if there is no reference node defined in the associated section definition. Identifier .fil .odb Field History Description MASS DMASS UCOM VCOM ACOM COORDCOM MASSEUL VOLEUL Total energy output • • • • • • • • Total mass of the element set. Total mass change in percentage of the element set due to mass scaling. Equivalent rigid-body translational displacement of the element set. Equivalent rigid-body translational velocity of the element set. Equivalent rigid-body translational acceleration of the element set. Coordinates of the center of mass of the element set. Total mass of each Eulerian material instance in the element set. Total volume of each Eulerian material instance in the element set. You can request total energy variable output to the results or output database file . All of these variables are written when total energy output is requested. Energy history totals can be requested to the output database for part of the model as well as the whole model. Identifier .fil ALLAE ALLCD ALLFD ALLIE ALLKE • • • • • .odb Field History • • • • • Description “Artificial” strain energy associated with constraints used to remove singular modes (such as hourglass control) and with constraints used to make the drill rotation follow the in-plane rotation of the shell elements. Energy dissipated by viscoelasticity. (Not supported for hyperelastic and hyperfoam material models). Total energy dissipated through frictional effects. (Available only for the whole model). Total strain energy. (ALLIE=ALLSE + ALLPD + ALLCD + ALLAE + ALLDMD+ ALLDC+ ALLFC.) Kinetic energy. Identifier .fil .odb Field History Description • • • • • • • • ALLPD ALLSE ALLVD ALLWK ALLIHE ALLHF ALLDMD ALLDC ALLFC ALLPW ALLCW ALLMW ETOTAL • • • • • • • • • • • • • • Energy dissipated by rate-independent and rate- dependent plastic deformation. Recoverable strain energy. Energy dissipated by viscous effects. External work. (Available only for the whole model). Internal heat energy. External heat energy through external fluxes. Energy dissipated by damage. Energy dissipated by distortion control. Fluid cavity energy, defined as the negative of the work done by all fluid cavities. (Available only for the whole model.) Work done by contact penalties, penalty/kinematic contact (Available only for the whole model.) Work done by constraint penalties. (Available only for the whole model.) Work done in propelling mass added in mass scaling. (Available only for the whole model.) Energy balance defined as: ALLKE + ALLIE + ALLVD + ALLFD + ALLIHE − ALLWK − ALLPW − ALLCW − ALLMW − ALLHF. (Available only for the whole model.) including general pairs. contact and Time increment and mass output The DT and DMASS variables are always written when any results file output is requested . You can request output of the time increment and the steady-state detection variables SSPEEQ, SSSPRD, SSFORC, and SSTORQ to the output database . Identifier .fil • • DT DMASS SSPEEQ .odb Field History • • • Description Time increment. Percent change in mass of the model due to mass scaling. Steady-state equivalent plastic strain norms. Identifier .fil .odb Field History Description SSPEEQn SSSPRD SSSPRDn SSFORC SSFORCn SSTORQ SSTORQn • • • • • • • Steady-state equivalent plastic strain norm n. Steady-state spread strain norms. Steady-state spread norm n. Steady-state force norms. Steady-state force norm n. Steady-state torque norms. Steady-state torque norm n. 4.2.3 Abaqus/CFD OUTPUT VARIABLE IDENTIFIERS Products: Abaqus/CFD Abaqus/CAE References • “Output,” Section 4.1.1 • “Output to the data and results files,” Section 4.1.2 • “Output to the output database,” Section 4.1.3 Overview Results can be obtained from Abaqus/CFD only by postprocessing. The tables in this section list all of the output variables that are available in Abaqus/CFD. The output variables can be requested for either field- or history-type output to the output database (.odb) file . The field type variables can be requested at the nodes, elements, or element faces attached to a surface. Symbols used in the tables The availability of the various output variable identifiers is defined by a under the following headings: in the columns of the table, .odb Field means that the identifier can be used as a field-type output selection to the output database. .odb History means that the identifier can be used as a history-type output selection to the output database. Direction definitions The direction definitions depend on the variable type. Direction definitions for element variables For element variables, 1, 2, and 3 refer to the global directions (1=X, 2=Y, and 3=Z). Even if a local coordinate system has been defined at a node (“Transformed coordinate systems,” Section 2.1.5), the data are still output in the global directions. Direction definitions for nodal variables For nodal variables, 1, 2, and 3 refer to the global directions (1=X, 2=Y, and 3=Z). Even if a local coordinate system has been defined at a node (“Transformed coordinate systems,” Section 2.1.5), the data are still output in the global directions. Requesting output of components Individual components of variables can be requested as history-type output in the output database for X–Y plotting in Abaqus/CAE. Individual component requests are not available for field-type output. If a particular component is desired for contouring in Abaqus/CAE, request field output of the generic variable (e.g., V for velocity). Output for individual components of this field output can then be requested within the Visualization module of Abaqus/CAE. Element variables You can request element variable output to the output database file . Identifier .odb Description Field History Coordinates of the element centroid for solid elements. These are the current coordinates if the mesh has moved. Element volume. Fluid density. Divergence of the fluid velocity. Enstrophy per unit mass. Dot product of vorticity and velocity. Fluid pressure. Fluid temperature. Fluid velocity. Second (symmetric part of the velocity gradient tensor). Curl of the velocity vector. Element molecular viscosity. Shear rate computed using the second invariant of the rate-of-strain tensor. rate-of-strain invariant tensor the of Wall-normal distance. Energy dissipation rate. 4.2.3–2 Geometric quantities COORD EVOL State and field variables DENSITY DIV ENSTROPHY HELICITY PRESSURE TEMP VGINV2 VORTICITY VISCOSITY SHEARRATE Turbulence variables DIST TURBEPS • • • • • • • • • • • • • • • • • • • • • • • • • • Identifier .odb Description TURBKE TURBNU Nodal variables Field History • • • • Turbulent kinetic energy. Turbulent eddy viscosity. You can request nodal variable output to the output database file . Identifier .odb Description Field History Coordinates of the node. coordinates if the mesh has moved. Coordinate n ( ). These are the current Fluid density at a node. Divergence of the fluid velocity at a node. Enstrophy per unit mass at a node. Helicity at a node. Fluid pressure at a node. Fluid temperature at a node. Fluid displacement components at a node. fluid displacement component ( Fluid velocity components at a node. fluid velocity component ( the invariant of tensor rate-of-strain Second (symmetric part of the velocity gradient tensor). Vorticity components at a node. Vorticity vorticity component ( Shear rate at the nodes computed using the second invariant of the rate-of-strain tensor. ). ). ). Wall-normal distance. Energy dissipation rate. 4.2.3–3 Geometric quantities COORD COORn State and field variables DENSITY DIV ENSTROPHY HELICITY PRESSURE TEMP Un Vn VGINV2 VORTICITY VORTICITYn SHEARRATE Turbulence variables DIST TURBEPS • • • • • • • • • • • • • • • • • Identifier .odb Description Field History TURBKE TURBNU • • Surface variables Turbulent kinetic energy. Turbulent eddy viscosity at a node. You can request surface variable output to the output database file . The field output corresponds to the element faces attached to a surface. Identifier .odb Description Field History Area of a surface. For deforming meshes, it is the surface area in the current configuration. Area-averaged surface pressure. Area-averaged surface temperature. Area-averaged surface velocity vector. Total fluid force components on the surface. Integrated normal heat flux on a given surface. Heat flow is considered positive if heat is added to the system and negative otherwise. Heat flux vector on a surface. Normal heat flux on a surface. Integrated mass flow rate across a given surface. Fluid normal traction on a surface. Fluid pressure force on a given surface. Fluid surface (or shear) traction on a surface. Fluid total traction on a surface. This is equal to the sum of the normal traction (NTRACTION) and the shear traction (STRACTION). Fluid viscous force on a given surface. Integrated volume flow rate across a given surface. Fluid shear stress magnitude on a surface. It is the magnitude of the shear traction (STRACTION) vector. 4.2.3–4 Geometric quantities SURFAREA State and field variables AVGPRESS AVGTEMP AVGVEL FORCE HEATFLOW HFL HFLN MASSFLOW NTRACTION PRESSFORCE STRACTION TRACTION VISCFORCE VOLFLOW WALLSHEAR • • • • • • • • • • • • • • • Identifier .odb Description Field History Turbulence variables YPLUS YSTAR • • Wall-normal distance measured in viscous lengths or wall units. A default value of 0 is output for surfaces that are not attached to a wall boundary. Wall-normal distance scaled using turbulent kinetic energy and viscosity. YSTAR output is available only when TYPE=RNG KEPSILON is specified. A default value of 0 is output for surfaces that are not attached to a wall boundary. Whole and partial model variables The output variables listed below are available for part of the model as well as the whole model. Identifier .odb Description Field History Geometric quantities VOL • Total energy output quantities Current volume of the entire set or the entire model. If the following whole model variables are relevant for a particular analysis, you can request them as output to the output database file . If you do not specify an output region, whole model variables are calculated. When you specify an output region, the relevant energy totals are calculated over the user-specified region. ALLKE • Kinetic energy. 4.3 The postprocessing calculator • “The postprocessing calculator,” Section 4.3.1 4.3.1 THE POSTPROCESSING CALCULATOR Products: Abaqus/Standard Abaqus/Explicit References • “Output to the output database,” Section 4.1.3 • “Abaqus/Standard output variable identifiers,” Section 4.2.1 • “Abaqus/Explicit output variable identifiers,” Section 4.2.2 • “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2 Overview The postprocessing calculator can perform operations on output quantities written to the output database (job-name.odb) by Abaqus. It then expands the output database by writing these new output quantities to the output database. Once this expansion is done, it is not possible to convert the output database back to its original form. The postprocessing calculator is for use only with the Visualization module of Abaqus/CAE (Abaqus/Viewer). Functionality of the calculator The postprocessing calculator performs the following calculations on data written to the output database: • Extrapolation of integration point quantities to the nodes or interpolation of integration point quantities to the centroid of an element, according to the user-specified position for element output; see “Selecting the position of element integration point and section point output” in “Output to the output database,” Section 4.1.3, for details. • Calculation of history output at tracer particles; see “Tracer particle output from Abaqus/Explicit” in “Output to the output database,” Section 4.1.3. Running the calculator By default, the postprocessing calculator will run automatically upon the completion of an analysis. During the execution of the analysis, Abaqus will determine if there are keywords in the input file that require the use of the calculator and will initiate the calculator upon completion if it is required. You can override this default behavior by using the environment variable auto_calculate in the Abaqus environment file. See “Using the Abaqus environment settings,” Section 3.3.1, for details. You can run the postprocessing calculator manually by using the convert=odb option on the abaqus execution procedure. To see the postprocessed results before an analysis is complete, you can run the postprocessing calculator manually while the analysis is still running, using the oldjob option in conjunction with the convert=odb option on the abaqus execution procedure. The postprocessing calculator will write a new output database using the value of the job parameter as the file name. Due to the fact that the analysis is writing to the output database at the same time the postprocessing calculator is attempting to read it, the output database may be in an inconsistent state that makes reading it impossible. If this problem occurs, the postprocessing calculator will stop attempting to read the output database and exit. A warning message explaining what has happened will be output to the screen. You can then attempt to run the postprocessing calculator again. If the inconsistent state has cleared, the postprocessing calculator will run normally. If the postprocessing calculator is run during an analysis without the oldjob option, Abaqus will ask you to confirm that the existing output database can be overwritten. You should make sure the analysis is complete before running the postprocessing calculator manually without the oldjob option. If the analysis is still running when the postprocessing calculator is run without using the oldjob option, the output database will be corrupted. For a detailed description of the procedure for running the postprocessing calculator manually, see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2. If an analysis aborts because available CPU time has expired and you restart the analysis, the postprocessing calculator will not automatically expand the output database from the original, aborted run. You must manually run the postprocessing calculator to expand the original output database using the procedure outlined above. 5. File Output Format Accessing the results file 5.1 Accessing the results file • “Accessing the results file: overview,” Section 5.1.1 • “Results file output format,” Section 5.1.2 • “Accessing the results file information,” Section 5.1.3 • “Utility routines for accessing the results file,” Section 5.1.4 5.1.1 ACCESSING THE RESULTS FILE: OVERVIEW Writing information to the results file The Abaqus results file is the medium through which analysis results can be carried over into other software, such as postprocessing programs. The following types of output can be written to the results file: • element output, nodal output, energy output, modal output, contact surface output, and section output • element matrix output • substructure matrix output • cavity radiation viewfactor matrices “Output,” Section 4.1.1, describes the general format of the results file. An Abaqus model can be defined in terms of an assembly of part instances . However, the results file is not organized by part; it contains internal node and element numbers . A map between the original numbers and part instance names and the internal numbers is written to the data file. Accessing information in the results file This chapter contains technical descriptions of the results file and is intended to be read by users or programmers who need to write programs that use the results file. • “Results file output format,” Section 5.1.2, describes the format of the individual records in the results file. • “Accessing the results file information,” Section 5.1.3, describes the subroutine calls required to read the file output, contains an example of a program written to use the Abaqus results file, and shows how you can write (or modify) a results file using the Abaqus file format. • “Utility routines for accessing the results file,” Section 5.1.4, describes the utility subroutines that can be used to access the results file. 5.1.2 RESULTS FILE OUTPUT FORMAT Products: Abaqus/Standard Abaqus/Explicit References • “Accessing the results file: overview,” Section 5.1.1 • “Abaqus/Standard output variable identifiers,” Section 4.2.1 • “Abaqus/Explicit output variable identifiers,” Section 4.2.2 Overview This section describes the format of the individual records in the Abaqus results file. Where applicable, the output variable identifier used in writing a given value to the file is printed below the corresponding record type description. Records that are available only in Abaqus/Standard are designated with an (S) ; records that are available only in Abaqus/Explicit are designated with an (E) . The record key for a particular record may differ between Abaqus/Standard and Abaqus/Explicit. Record format The results file is written as a sequential file. Each record has the following format: Location Length Description 3, 4... ( ) ) Record length ( Record type key Attributes All words in the results file are of the same length, whether they contain integer, floating point number, or character string data. The word length is that of a double precision floating point number (8 bytes). The attributes in a given record may depend on the element type being considered. For example, (in local , and the stress components associated with three-dimensional shell elements are directions), while those associated with three-dimensional solids are (in global directions if no local orientation is specified). Thus, care must be used in interpreting the data when postprocessing the file output. Refer to Part VI, “Elements,” for a definition of the ordering of element-dependent attributes. , and , , , , , In steady-state dynamic analyses, complex values are stored as the real components followed by the imaginary components. For example, the stress components associated with three-dimensional shell elements are followed by , and , and , . , In models that are defined in terms of an assembly of part instances, the results file contains internal (global) node and element numbers, as explained in “Output,” Section 4.1.1. Part and assembly records are not included in the results file. Local coordinate system If the components of an element quantity are in local directions, a record of type 85 defining these directions is generated for each point at which component output is requested if the local coordinate directions were requested in Abaqus/Standard and automatically in Abaqus/Explicit. The local coordinate system may be inherent to the element, as is the case in shells and membranes, or may have been defined by a local orientation . For shell elements a direction record is written for every material point in the section for which component output is requested, and a separate direction record is written for section forces and section strains. For geometrically nonlinear analysis in Abaqus/Standard the record contains the current, updated directions, except for small-strain shells, in which case the original directions are given. Direction output is not provided for trusses, two-dimensional beams, axisymmetric shells or membranes, or for values averaged at nodes. Label record Some record types include labels, such as element and node set names, written in A8 format. If a label exceeds 8 characters, an integer identifier will be written instead. This identifier can then be used to cross-reference the actual label stored in 10A8 format on record type 1940. Records written for any file output request Record Record type key 1900 Element definitions 1990(S) Element definition continuation Attributes 1. Element number. 2. Element justified). type (characters, A8 format, left 3. First node on the element. 4. Second node on the element. 5. Etc. 1. Node on the element in the previous 1900 record. 2. Etc. In Abaqus/Explicit quadrilateral/brick elements that are degenerate (i.e., possessing identical nodes) are written out in record 1900 as corresponding triangular/tetrahedral/wedge elements. For example, a CPE4R element with two identical nodes is written as a CPE3 element, and a C3D8R element with identical third and fourth nodes and identical seventh and eighth nodes is written as a C3D6 element. 1901 Node definitions 1. Node number. 2. First coordinate. 3. Second coordinate. 4. Etc. Record Record type key Attributes Record key 1902 (below) defines the location of each active degree of freedom. For example, if the model contains only two-dimensional beam elements, the only active degrees of freedom are 1, 2, and 6. Therefore, this record would have the attributes (1, 2, 0, 0, 0, 3), meaning that degree of freedom 1 ( ) is the first active variable at each node; degree of freedom 2 ( ) is the second active variable at each node; degrees of freedom 3, 4, and 5 are not active in the model; and degree of freedom 6 is the third active variable at each node. 1902 Active degrees of freedom 1. Location in nodal arrays of degree of freedom 1 (0 if dof 1 is not active in the model). 2. Location in nodal arrays of degree of freedom 2 (0 if dof 2 is not active in the model). 3. Etc. 1910(S) Substructure path 1. 0 substructure enter record; 1 substructure leave record. 2. Element number on usage level. 3. Substructure type identifier (Zn). 4. Element number at the previous level if it is not the usage level. 5. Etc. 1. Flag for element-based output (0), nodal output (1), modal output (2), or element set energy output (3). 2. Set name (node or element set) used in the request (A8 format). This attribute is blank if no set was specified. 3. Element format). type (only for element output, A8 1. Abaqus release number (A8 format). 2. Date (2A8 format). 3. Date cont’d. 4. Time (A8 format). 5. Number of elements in the model. 6. Number of nodes in the model. 7. Typical element length in the model. 1. Attributes 1–10. The heading entered as the first data line of the *HEADING option (A8 format). Equivalent to the job description in Abaqus/CAE. 5.1.2–3 1911 Output request definition 1921 Abaqus release, etc. 1922 Record Record type key 1931 Node set Attributes 1. Node set name (A8 format). In Abaqus/Explicit only node sets defined as part of the model definition are written. 2. First node in the node set. 3. Second node in the node set. 4. Etc. 1932 Node set continuation 1. Node number in the node set of the previous 1931 1933 Element set 1. Element set name (A8 record. 2. Etc. Abaqus/Explicit only element as part of the model definition are written. format). In sets defined 2. First element in the element set. 3. Second element in the element set. 4. Etc. 1934 Element set continuation 1. Element number in the element set of the previous 1940 Label cross-reference 1933 record. 2. Etc. 1. Integer reference. 2. Label (10A8 format). Record written once per eigenvalue in natural frequency extraction Record Record type key 1980(S) Modal Attributes 1. Eigenvalue number. 2. Eigenvalue. 3. Generalized mass. 4. Composite damping. 5. Participation factor for degree of freedom 1. 6. Effective mass for degree of freedom 1. 7. Participation factor for degree of freedom 2. 8. Effective mass for degree of freedom 2. 9. Etc. Any nodal or element data after this record refer to the eigenvector, until a new record key 1980 or a record key 2001 is encountered. Eigenvalue output for substructures also uses these records to divide up elemental and nodal results. This record is written if Record Record type key Attributes there are any results file output requests for an eigenvalue buckling prediction or eigenfrequency extraction step. The generalized mass, etc. are not written for an eigenvalue buckling prediction step. This record is not written for a complex eigenfrequency extraction step. Records written once per increment Record Record type key 2000 Increment start record Attributes 1. Total time. 2. Step time. 3. Maximum creep strain-rate ratio (control of solution-dependent amplitude) in Abaqus/Standard; currently not used in Abaqus/Explicit. 4. Solution-dependent amplitude in Abaqus/Standard; currently not used in Abaqus/Explicit. 5. Procedure type: gives a key to the step type. See Table 5.1.2–1 at the end of this section. 6. Step number. 7. Increment number. 8. Linear perturbation flag in Abaqus/Standard: 0 if general step, 1 if linear perturbation step; currently not used in Abaqus/Explicit. 9. Load proportionality factor: nonzero only in static Riks steps; currently not used in Abaqus/Explicit. 10. Frequency (cycles/time) in a steady-state dynamic response analysis or steady-state transport angular velocity (rad/time) in a steady-state transport analysis; currently not used in Abaqus/Explicit. 11. Time increment. 12. Attributes 12–21. The step subheading entered as the first data line of the *STEP option (A8 format). Equivalent to the step description in Abaqus/CAE. The following record is written once per increment, after all data records have been written for that increment. 2001 Increment end record 1. No attributes. Record Record type key Attributes Note: When binary format is used, the results file is written in blocks of 512 words for each increment. If there are fewer than 512 words in the last block of the current increment, record 2001 has zeros appended to it so that the total length of the block is 512. Hence, the length of record 2001 is 2 + the number of zeros appended. For an ASCII format results file record 2001 is extended to complete an 80 character logical record, and a logical record of 80 blank characters is added after this record. See “Accessing the results file information,” Section 5.1.3. Records written for any element file output request These records contain data about element variables at integration points within the elements, at the centroid of elements, or at the nodes of an element. Attributes 1. Element number or the node number if the averaged contain nodal records subsequent element values. 2. Integration point number if the subsequent records contain integration point data. Node number the if the subsequent records contain data at nodes of the element. Integration plane number if records contain centroidal values for CAXA and SAXA elements. 0 if the subsequent records contain centroidal values or nodal averaged values. the subsequent 3. Section point number if this is a shell, beam, or layered solid element and the subsequent records contain data at a section point through the thickness. 0 for continuum elements and for section values in beams and shell elements. 4. Location identification. 0 if the subsequent records contain data at an integration point; 1 if the subsequent records contain values at the centroid of the element; 2 if the subsequent records contain data at the nodes of the element; 3 if the subsequent records contain data associated with rebar within an element; 4 if the subsequent records contain nodal averaged values; 5 if the subsequent records contain values associated with the whole element. 5.1.2–6 Record Record type key key Attributes FILE OUTPUT FORMAT 5. Rebar name if the subsequent records contain values associated with a named rebar. 6. Number of direct stresses at a point (NDI). 7. Number of shear stresses at a point (NSHR). 8. 0, currently not used in Abaqus/Standard; number of directions in which displacement or temperature gradients are computed in the element (NDIR) in Abaqus/Explicit. 9. Number of section force or section strain components (NSFC). 1. Temperature. 1. Load type. 2. Magnitude. 1. Flux type. 2. Magnitude. 1. State variable 1. 2. State variable 2. 3. Etc. The record can have up to 80 words in ASCII format or 512 words in binary format. Repeat this record as often as necessary to output all active state variables in the model. Temperature Output variable: TEMP Distributed load Output variable: LOADS Distributed flux Output variable: FLUXS Solution-dependent state variables Output variable: SDV Void ratio Output variable: VOIDR Foundation pressure Output variable: FOUND Coordinates Output variable: COORD Field variables Output variable: FV Nodal flux caused by heat Output variable: NFLUX 1. Void ratio. 1. Foundation type. 2. Magnitude. 1. First coordinate. 2. Etc. 1. First field variable. 2. Etc. 1. Node number. 2. First flux component. 3. Etc. Stresses Output variable: S 1. First stress component. 2. Second stress component. 5.1.2–7 3(S) 4(S) 6(S) 7(S) 8(S) 9(S) 10(S) Record Record type key Attributes 3. Etc. 1. Magnitude (available only when the gasket contact area is specified; see “Defining the contact area for average contact pressure output” in “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6). 1. Mises stress. 2. Tresca stress. 3. Hydrostatic pressure. 4. Currently not used. 5. Currently not used. 6. Currently not used. 7. Third stress invariant. 1. First section force. 2. Second section force. 3. Etc. 1. Effective axial section force for beams and pipes subjected to pressure loading. 1. Strain energy. Elastic strain energy is the only energy density request available in eigenvalue extractions. None of the energy densities are available in modal procedures or direct-solution steady-state dynamics analyses. 2. Plastic dissipation. 3. Creep dissipation. 4. Viscous dissipation. 5. Electrostatic energy. 6. Energy dissipated due to electrical conduction. 7. Damage dissipation. 1. Elastic strain energy. 2. Plastic dissipation. 3. Viscoelastic dissipation (not supported for hyperelastic and hyperfoam material models). 5.1.2–8 475(S) Average contact pressure (for link and three-dimensional line gasket elements) Output variable: CS11 12(S) Stress invariants Output variable: SINV 13 Section forces and moments Output variable: SF 449(S) 14(S) Effective axial section force Output variable: ESF1 Energy densities Output variable: ENER 14(E) Energy densities Record Record type key Attributes 15(S) Nodal forces caused by stress Output variable: NFORC 4. Viscous dissipation. 5. Currently not used. 6. Currently not used. 7. Damage dissipation. 1. Node number. 2. First force component. 3. Etc. 16(S) Maximum section stresses 1. Maximum stress on section. The order of the data and the number of data items for record 17 depends on the element type. For LS3S elements: 17(S) Js, K for LS3S line springs Output variable: JK For LS6 elements: 17(S) Js, Ks for LS6 line springs Output variable: JK 18(S) 19(S) Pore or acoustic pressure Output variable: POR Energy summed over element Output variable: ELEN 1. J (J-integral). 2. K (stress intensity). 3. 4. (elastic part of J-integral). (plastic part of J-integral). 1. J (J-integral). 2. 3. 4. 5. 6. (elastic part of J-integral). (plastic part of J-integral). (Mode I stress intensity factor). (Mode II stress intensity factor). (Mode III stress intensity factor). 1. Liquid pressure. 1. Kinetic energy. 2. Strain energy. Elastic strain energy is the only whole element energy request available in eigenvalue extractions. None of the element energies are available in modal procedures or direct-solution steady-state dynamics analyses. 3. Plastic dissipation. 4. Creep dissipation. 5. Viscous dissipation, not including dissipation due to stabilization. 6. Static dissipation (due to stabilization). 7. Artificial strain energy. Record Record type key Attributes 19(E) Energy summed over element Output variable: ELEN 21 22 Total strain in Abaqus/Standard; infinitesimal strain in Abaqus/Explicit Output variable: E Plastic strains Output variable: PE 8. Electrostatic energy. 9. Electrical energy dissipated in a conductor. 10. Damage dissipation. 1. Currently not used. 2. Strain energy. 3. Plastic dissipation. 4. Viscoelastic dissipation (not supported for hyperelastic and hyperfoam material models). 5. Viscous dissipation. 6. Artificial strain energy. 7. Distortion control dissipation. 8. Currently not used. 9. Internal heat energy. 10. Damage dissipation. 1. First strain component. 2. Second strain component. 3. Etc. 1. First plastic strain component. 2. Second plastic strain component. 3. Etc; by followed equivalent plastic the strain, actively yielding flag (yes or no, A8 format), and magnitude of plastic strain in Abaqus/Standard; followed by “0.0, UNUSED, 0.0” in Abaqus/Explicit for consistency with the length of the Abaqus/Standard record. 23(S) Creep strains (including swelling) Output variable: CE 24(S) Total inelastic strains Output variable: IE 1. First creep strain component. 2. Second creep strain component. 3. Etc; followed by the equivalent creep strain, volumetric swelling strain, and magnitude of creep strain. 1. First inelastic strain component. 2. Second inelastic strain component. 3. Etc. key 25(S) Total elastic strains Output variable: EE 26 Unit normal to crack in concrete Output variable: CRACK 27 28 29 Section thickness Output variable: STH Heat flux vector Output variable: HFL Section strains and curvatures Output variable: SE 30(S) Deformation gradient Output variable: DG FILE OUTPUT FORMAT Attributes 1. First elastic strain component. 2. Second elastic strain component. 3. Etc. 1. 11-component (if a 1-D, 2-D, or 3-D analysis). 2. 12-component (if a 2-D or 3-D analysis). 3. 13-component (if a 3-D analysis). 4. 21-component (if a 2-D or 3-D analysis). 5. 22-component (if a 2-D or 3-D analysis). 6. 23-component (if a 3-D analysis). 7. 31-component (if a 3-D analysis). 8. 32-component (if a 3-D analysis). 9. 33-component (if a 3-D analysis). 1. Current section thickness for membranes and finite-strain shells in Abaqus/Standard and for membranes and all shells in Abaqus/Explicit. 1. Magnitude. 2. First component. 3. Second component. 4. Etc. 1. First section strain. 2. Second section strain. 3. Etc. 1. . 2. Etc. , , , The record will have NDI diagonal then NSHR above diagonal components of ), then NSHR below components ( ), where NDI diagonal components ( and NSHR are given in the element header record (record key 1). Available only for hyperelasticity, hyperfoam, and material models defined in user subroutine UMAT. , , Record Record type key Attributes 31(S) 32(S) 33(S) 34(S) 35(S) 36(S) 38(S) 446(S) 447(S) 448(S) Concrete failure Output variable: CONF Strain jumps at nodes Output variable: SJP Film Output variable: FILM Radiation Output variable: RAD Saturation (pore pressure analysis) Output variable: SAT Substresses (for ITT elements) Output variable: SS Mass concentration (mass diffusion analysis) Output variable: CONC Amount of solute at the integration point (mass diffusion analysis) Output variable: ISOL Amount of solute in the current element (mass diffusion analysis) Output variable: ESOL Amount of solute in the element set or model (mass diffusion analysis) Output variable: SOL 1. Summary of the state of a concrete material point. This is the number of cracks or −1 if the concrete has crushed. 1. First strain jump component. 2. Second strain jump component. 3. Etc. 1. Type. 2. Sink temperature. 3. Film coefficient. 1. Type. 2. Sink temperature. 3. Radiation constant. 1. Saturation. 1. First substress. 2. Second substress. 1. Concentration. 1. Amount of solute. 1. Amount of solute. 1. Amount of solute. The number of data items for record 39 depends on the element type. For pore pressure elements and mass diffusion analysis: 39(S) Mass concentration flux vector Output variable: MFL 1. Magnitude. 2. First component. Attributes 3. Second component. 4. Etc. 1. Current flow rate. 1. Gel volume ratio. 1. Total fluid volume ratio. 1. Status of element (shear failure model, tensile failure model, porous failure criterion, brittle failure model, Johnson-Cook plasticity model, and VUMAT). The status of an element is 1.0 if the element is active, 0.0 if the element is not. 1. Equivalent plastic strain. For crushable foam plasticity with volumetric hardening, it is the volumetric compacting plastic strain. For cap plasticity it is (the cap position). 1. Mean pressure stress. 1. Mises stress. 1. Current maximum ratio of creep strain rate and target creep strain rate. 1. Volumetric strain rate. 1. Current value of the solution-dependent amplitude. 1. First section stress. 2. Second section stress. 3. Etc. 5.1.2–13 Record Record type key For fluid link elements: 39(S) 40(S) 43(S) 61(E) 73(E) 74(E) 75(E) 79(S) 79(E) 80(S) 83(S) Mass flow rate Output variable: MFL Gel (pore pressure analysis) Output variable: GELVR Total fluid volume ratio Output variable: FLUVR Element status Output variable: STATUS Equivalent plastic strain Output variable: PEEQ Mean pressure stress Output variable: PRESS Mises equivalent stress Output variable: MISES Creep strain rate ratio Output variable: RATIO Volumetric strain rate Output variable: ERV Solution-dependent amplitude value Output variable: AMPCU Average shell section stresses Record Record type key Attributes The following record is generated in Abaqus/Standard when the local coordinate directions are requested, component output is requested for a material or section point, and the components are given in a local coordinate system ; it is generated automatically in Abaqus/Explicit when component output is requested for a material or a section point and the components are given in a local coordinate system. Only the first two directions are given; if needed, the third direction can be obtained as the cross product of the first two. The direction record is not generated for trusses, two-dimensional beams, axisymmetric shells or membranes, or for values averaged at nodes. 85 Local coordinate directions 1. First component of the first direction. 2. Second component of the first direction. 3. Third component of the first direction. 4. First component of the second direction. 5. Second component of the second direction. 6. Third component of the second direction. 86 87(S) 88(S) 89 90 Backstress for kinematic hardening plasticity Output variable: ALPHA component. component. 1. First 2. Second 3. Etc. (The number of components is equal to the number of stress components; see the element description in Part VI, “Elements.”) User-defined output variables Output variable: UVARM 1. Output variable 1. 2. Output variable 2. 3. Etc. Thermal strains Output variable: THE Logarithmic strains Output variable: LE 1. First thermal strain component. 2. Second thermal strain component. 3. Etc. 1. First logarithmic strain component. 2. Second logarithmic strain component. 3. Etc. Nominal strains Output variable: NE 1. First nominal strain component. 2. Second nominal strain component. key Attributes FILE OUTPUT FORMAT 91(S) Mechanical strain rates Output variable: ER 96(S) 97(S) 476(E) 477(E) Total mass flow through fluid link Output variable: MFLT Pore fluid effective velocity vector Output variable: FLVEL Scaling factor Output variable: EMSF Element time increment Output variable: EDT Principal value records 3. Etc. 1. First strain rate component. 2. Second strain rate component. 3. Etc. 1. Magnitude. 1. Magnitude. 2. First component. 3. Second component. 4. Etc. 1. Element mass scaling factor. 1. Element stable time increment. For all principal values, the number of components equals NDI unless NDI equals 1, in which case the number of components equals NDI plus NSHR, where NDI and NSHR are given on the element header record. In the cases where NDI equals 2, only the in-plane values are given. 401 402 403 404 405 Principal stresses Output variable: SP Principal values of backstress tensor for kinematic hardening plasticity Output variable: ALPHAP 1. Minimum principal stress. 2. Etc. 1. Minimum principal value. 2. Etc. Principal strains Output variable: EP 1. Minimum principal strain. 2. Etc. Principal nominal strains Output variable: NEP Principal logarithmic strains Output variable: LEP 1. Minimum principal nominal strain. 2. Etc. 1. Minimum principal logarithmic strain. 2. Etc. Record Record type key Attributes 406(S) 407(S) 408(S) 409(S) 410(S) 411(S) 412(S) Principal mechanical strain rates Output variable: ERP 1. Minimum principal strain rate. 2. Etc. Principal values of deformation gradient Output variable: DGP 1. Minimum principal value. 2. Etc. Principal elastic strains Output variable: EEP Principal inelastic strains Output variable: IEP Principal thermal strains Output variable: THEP Principal plastic strains Output variable: PEP Principal creep strains Output variable: CEP 1. Minimum principal elastic strain. 2. Etc. 1. Minimum principal inelastic strain. 2. Etc. 1. Minimum principal thermal strain. 2. Etc. 1. Minimum principal plastic strain. 2. Etc. 1. Minimum principal creep strain. 2. Etc. 1. f. 1. 1. 1. . . 1. First cracking strain component. 2. Second cracking strain component. 3. Etc. 1. First strain component in local crack directions. 2. Second strain component in local crack directions. 5.1.2–16 Records for porous metal plasticity 413 414 415 Void volume fraction Output variable: VVF Void volume fraction (growth) Output variable: VVFG Void volume fraction (nucleation) Output variable: VVFN 416(S) Relative density Output variable: RD Records for brittle cracking 421(E) Cracking strains Output variable: CKE 422(E) Local cracking strains key Attributes FILE OUTPUT FORMAT 423(E) Local cracking stresses Output variable: CKLS 424(E) Status of cracks Output variable: CKSTAT 3. Etc. 1. First stress component in local crack directions. 2. Second stress component in local crack directions. 3. Etc. 1. Status of first crack (if a 1-D, 2-D, or CKSTAT can have the 0.0=uncracked, 1.0=closed 3.0=crack 3-D analysis). following values: crack, closing/reopening. 2.0=actively cracking, 441(E) Cracking strain magnitude Output variable: CKEMAG 2. Status of second crack (if a 2-D or 3-D analysis). 3. Status of third crack (if a 3-D analysis). 1. Magnitude of cracking strain. Records for inelastic nonlinear response in a beam general section 42(S) Plastic strain components Output variable: SPE 47(S) Equivalent plastic strains Output variable: SEPE 1. Axial plastic strain. 2. Curvature change about the local 1-axis. 3. Curvature change about the local 2-axis (available only for 3-D beams). 4. Twist of the beam (available only for 3-D beams). 1. Axial equivalent plastic strain. 2. Curvature change about the local 1-axis. 3. Curvature change about the local 2-axis (available only for 3-D beams). 4. Twist of the beam (available only for 3-D beams). Records for elastic-plastic response in frame elements 462(S) Elastic section strain components Output variable: SEE 1. Elastic axial strain. 2. Elastic curvature change about the local 1-axis. 3. Elastic curvature change about the local 2-axis (available only for 3-D frame elements). 4. Elastic twist of the beam (available only for 3-D frame elements). Record Record type key Attributes 1. Plastic axial displacement. 2. Plastic rotation about the local 1-axis. 3. Plastic rotation about the local 2-axis (available only for 3-D frame elements). 4. Plastic rotation about the element axis (available only for 3-D frame elements). 5. Actively yielding flag (yes or no, A8 format) for frame element’s end sections. 6. Buckling flag (yes, no, or na; A8 format) for frame element’s end sections. 1. Axial backstress component. 2. Bending backstress about the local 1-axis. 3. Bending backstress about the local 2-axis (available only for 3-D frame elements). 4. Twist backstress of the beam (available only for 3-D frame elements). 1. First component of total force. 2. Second component of total force. 3. Etc. 1. First component of elastic force. 2. Second component of elastic force. 3. Etc. 1. First component of viscous force. 2. Second component of viscous force. 3. Etc. 1. First component of friction force. 2. Second component of friction force. 3. Etc. 1. Flag in the 1-direction. 2. Flag in the 2-direction. 3. Etc. 1. First component of reaction force. 2. Second component of reaction force. 3. Etc. 5.1.2–18 463(S) Plastic displacements at frame element’s ends Output variable: SEP 464(S) Generalized backstress components Output variable: SALPHA Records for connector elements 495 496 497 498 499 500 Connector total force Output variable: CTF Connector elastic force Output variable: CEF Connector viscous force Output variable: CVF Connector friction force Output variable: CSF Connector lock and connector stop status flags Output variable: CSLST Connector reaction force Record Record type key Attributes 501 502 503 504 505 506 Connector concentrated force Output variable: CCF Connector relative position Output variable: CP Connector relative displacement Output variable: CU Connector constitutive displacement Output variable: CCU Connector relative velocity Output variable: CV Connector relative acceleration Output variable: CA 1. First component of concentrated force. 2. Second component of concentrated force. 3. Etc. 1. First component of relative position. 2. Second component of relative position. 3. Etc. 1. First component of relative displacement. 2. Second component of relative displacement. 3. Etc. 1. First component of constitutive displacement. 2. Second component of constitutive displacement. 3. Etc. 1. First component of relative velocity. 2. Second component of relative velocity. 3. Etc. 1. First component of relative acceleration. 2. Second component of relative acceleration. 3. Etc. 507(E) Connector failure status flags Output variable: CFAILST 1. Flag in the 1-direction. 2. Flag in the 2-direction. 3. Etc. 1. First component of friction-generating force. 2. Second component of friction-generating force. 3. Etc. 1. Relative velocity in the direction of instantaneous slip. 1. First component of accumulated frictional slip. 2. Second component of accumulated frictional slip. 3. Etc. 1. First component of elastic displacement. 2. Second component of elastic displacement. 3. Etc. 1. First component of plastic relative displacement. relative 2. Second component plastic of displacement. 5.1.2–19 542 546 548 556 557 Connector friction-generating contact force Output variable: CNF Connector relative velocity in the direction of instantaneous slip Output variable: CIVC Accumulated frictional slip Output variable: CASU Connector elastic displacement Output variable: CUE Connector plastic relative displacement Record Record type key Attributes 3. Etc. 558 Connector equivalent plastic relative displacement Output variable: CUPEQ 1. First component of equivalent plastic relative displacement. 2. Second component of equivalent plastic relative displacement. 3. Etc. Connector overall damage variable Output variable: CDMG 1. First component of overall damage variable. 2. Second component of overall damage variable. 3. Etc. Connector force-based damage initiation criterion Output variable: CDIF 1. First component of connector force-based damage initiation criterion. 2. Second component of connector force-based damage initiation criterion. 3. Etc. Connector motion-based damage initiation criterion Output variable: CDIM 1. First component of connector motion-based damage initiation criterion. 2. Second component of connector motion-based 559(E) 560(E) 561(E) 562(E) Connector plastic motion-based damage initiation criterion Output variable: CDIP 563 Connector kinematic hardening shift force Output variable: CALPHAF damage initiation criterion. 3. Etc. 1. First component of connector plastic motion- based damage initiation criterion. 2. Second component of connector plastic motion- based damage initiation criterion. 3. Etc. 1. First component of connector kinematic hardening shift force. 2. Second component of hardening shift force. 3. Etc. connector kinematic Record for plane stress orthotropic failure measures 44(S) Failure measures Output variable: CFAILURE 1. Maximum stress theory. 2. Tsai-Hill theory. 3. Tsai-Wu theory. 4. Azzi-Tsai-Hill theory. 5. Maximum strain theory. Record for equivalent plastic strain components for cap plasticity key 45 Equivalent plastic strain components Output variable: PEQC FILE OUTPUT FORMAT Attributes 1. Equivalent plastic strain for Drucker-Prager failure surface. 2. Actively yielding flag (yes or no, A8 format) for Drucker-Prager failure surface. 3. Equivalent plastic strain for cap surface. 4. Actively yielding flag (yes or no, A8 format) for cap surface. 5. Equivalent plastic strain for transition surface. 6. Actively yielding flag (yes or no, A8 format) for transition surface. 7. Total volumetric inelastic strain. 8. Actively yielding flag (yes or no, A8 format). Record for equivalent plastic strain components for jointed materials 45(S) Equivalent plastic strain components Output variable: PEQC 1. Equivalent plastic strain for joint 1. 2. Actively yielding flag (yes or no, A8 format) for joint 1. 3. Equivalent plastic strain for joint 2. 4. Actively yielding flag (yes or no, A8 format) for joint 2. 5. Equivalent plastic strain for joint 3. 6. Actively yielding flag (yes or no, A8 format) for joint 3. 7. Equivalent plastic strain for bulk material. 8. Actively yielding flag (yes or no, A8 format) for bulk material. Record for equivalent plastic strain in uniaxial tension for cast iron plasticity 473(S) Equivalent plastic strain in uniaxial tension Output variable: PEEQT Records for two-layer viscoplasticity 22(S) Plastic strains in the elastic- plastic network Output variable: PE 1. Equivalent plastic strain in uniaxial tension for cast iron plasticity model. 2. Actively yielding flag (yes or no, A8 format). 1. First plastic strain component. 2. Second plastic strain component. 3. Etc.; followed by the equivalent plastic strain, actively yielding flag (yes or no, A8 format), and magnitude of plastic strain. Record Record type key Attributes 524(S) 525(S) 526(S) Stresses in the elastic-viscous network Output variable: VS Stresses in the elastic-plastic network Output variable: PS 1. First stress component. 2. Second stress component. 3. Etc. 1. First stress component. 2. Second stress component. 3. Etc. Viscous strains in the elastic- viscous network Output variable: VE 1. First viscous strain component. 2. Second viscous strain component. 3. Etc.; followed by the equivalent viscous strain. Record for elements with electric potential degrees of freedom 50(S) Electrical potential gradients Output variable: EPG Records for rebar quantities 442 443 444 Force in rebar Output variable: RBFOR Rebar angle Output variable: RBANG Change in rebar angle Output variable: RBROT 1. Magnitude. 2. First potential gradient. 3. Etc. 1. Magnitude. 1. Angle in degrees between the reinforcing and the user-specified isoparametric direction. Available only for membrane, shell, and surface elements. 1. Change in angle in degrees between the reinforcing and the user-specified isoparametric direction. Available only for membrane, shell, and surface elements. Record for forced convection/diffusion heat transfer elements 445(S) Mass flow rates Output variable: MFR 1. First mass flow rate. 2. Etc. Records for piezoelectric materials key Attributes FILE OUTPUT FORMAT 46(S) Magnitudes and phases of potential gradients (linear dynamics only) Output variable: PHEPG 49(S) Magnitudes and phases of electrical charge fluxes (linear dynamics only) Output variable: PHEFL 51(S) Electrical charge fluxes Output variable: EFLX 1. Magnitude of first electrical potential gradient. 2. Magnitude of second electrical potential gradient. 4. Phase angle of first electrical potential gradient. 5. Phase second electrical potential angle of gradient. 6. Etc. 1. Magnitude of first charge flux. 2. Magnitude of second charge flux. 3. Etc. 4. Phase angle of first charge flux. 5. Phase angle of second charge flux. 6. Etc. 1. Magnitude. 2. First charge flux. 3. Etc. 60(S) Distributed electrical charges Output variable: CHRGS 1. Charge type. 2. Magnitude. Records for coupled thermal-electric elements 425(S) Electrical current density Output variable: ECD 1. Magnitude. 2. First current density. 3. Etc. 426(S) 427(S) Distributed electrical current density Output variable: ECURS Nodal current due to electric conduction Output variable: NCURS 1. Electrical current type. 2. Magnitude. 1. Node number. 2. Magnitude. Record Record type key Records for cohesive elements 252(S) All active components of the damage initiation criteria Output variable: DMICRT 235(S) 61(S) Overall scalar stiffness degradation Output variable: SDEG Element status Output variable: STATUS Attributes 1. MAXSCRT, maximum nominal stress damage initiation criterion. 2. MAXECRT, maximum nominal strain damage initiation criterion. 3. QUADSCRT, quadratic nominal stress damage initiation criterion. 4. QUADECRT, quadratic nominal strain damage initiation criterion. 1. Magnitude. 1. Status of the element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). Records for equivalent rigid body variables in direct-integration implicit dynamic analyses Records 52–59 provide values summed over an element set. These variables are available only in direct- integration implicit dynamic analyses . 52(S) 53(S) 54(S) 55(S) 56(S) Current coordinates of center of mass Output variable: XC Displacement of the center of mass Output variable: UC Equivalent rigid body velocity Output variable: VC Angular momentum about center of mass Output variable: HC 1. Coordinate 1. 2. Coordinate 2. 3. Etc. (The number of components depends upon the overall dimensionality of the element set.) 1. Displacement 1. 2. Displacement 2. 3. Etc. (The number of components depends upon the overall dimensionality of the element set.) 1. Component 1. 2. Component 2. 3. Etc. (The number of components depends upon the overall dimensionality of the element set.) 1. Component 1. 2. Component 2. 3. Etc. (The number of components depends upon the overall dimensionality of the element set.) Angular momentum about origin Output variable: HO 1. Component 1. 2. Component 2. Record Record type key Attributes 57(S) 58(S) 59(S) Rotary inertia about the origin Output variable: RI Current mass of element set Output variable: MASS Current volume of element set Output variable: VOL 3. Etc. (The number of components depends upon the overall dimensionality of the element set.) 1. Component 11. 2. Component 22. 3. Etc. (The number of components depends upon the overall dimensionality of the element set.) 1. Mass. 1. Volume. (Only available for continuum and structural elements not using general beam or shell section definitions.) Record for transverse shear stress in thick shell elements such as S3R, S4R, S8R, and S8RT 48 Transverse shear stresses in 13 and 23 planes Output variable: TSHR Records for linear dynamics 1. Component 13. 2. Component 23. Magnitude and phase angle of stress components Output variable: PHS 1. Magnitude of first stress component. 2. Magnutude of second stress component. 3. Etc. 4. Phase angle of first stress component. 5. Phase angle of second stress component. 6. Etc. RMS values of stress components Output variable: RS 1. First component of stress. 2. Second component of stress. 3. Etc. 62(S) 63(S) 65(S) Magnitude and phase angle of strain components Output variable: PHE 1. Magnitude of first strain component. 2. Magnitude of second strain component. 3. Etc. 4. Phase angle of first strain component. 5. Phase angle of second strain component. 6. Etc. 1. First component of strain. 2. Second component of strain. 3. Etc. 66(S) RMS values of strain components Output variable: RE Records for connector elements (available only for linear dynamics) Record Record type key Attributes 508(S) Magnitude and phase angle of connector total forces Output variable: PHCTF 509(S) Magnitude and phase angle of connector elastic forces Output variable: PHCEF 510(S) Magnitude and phase angle of connector viscous forces Output variable: PHCVF 511(S) Magnitude and phase angle of connector reaction forces Output variable: PHCRF 520(S) Magnitude and phase angle of connector friction forces Output variable: PHCSF 512(S) Magnitude and phase angle of connector relative displacements Output variable: PHCU 1. Magnitude of the first component. 2. Magnitude of the second component. 3. Etc. 4. Phase angle of the first component. 5. Phase angle of the second component. 6. Etc. 1. Magnitude of the first component. 2. Magnitude of the second component. 3. Etc. 4. Phase angle of the first component. 5. Phase angle of the second component. 6. Etc. 1. Magnitude of the first component. 2. Magnitude of the second component. 3. Etc. 4. Phase angle of the first component. 5. Phase angle of the second component. 6. Etc. 1. Magnitude of the first component. 2. Magnitude of the second component. 3. Etc. 4. Phase angle of the first component. 5. Phase angle of the second component. 6. Etc. 1. Magnitude of the first component. 2. Magnitude of the second component. 3. Etc. 4. Phase angle of the first component. 5. Phase angle of the second component. 6. Etc. 1. Magnitude of the first component. 2. Magnitude of the second component. 3. Etc. 4. Phase angle of the first component. 5. Phase angle of the second component. 6. Etc. key 513(S) Magnitude and phase angle of connector constitutive displacements Output variable: PHCCU 522(S) Magnitude and phase angle of connector relative velocities Output variable: PHCV 523(S) Magnitude and phase angle of connector relative accelerations Output variable: PHCA 543(S) Magnitude and phase angle of friction-generating connector force Output variable: PHCNF FILE OUTPUT FORMAT Attributes 1. Magnitude of the first component. 2. Magnitude of the second component. 3. Etc. 4. Phase angle of the first component. 5. Phase angle of the second component. 6. Etc. 1. Magnitude of the first component. 2. Magnitude of the second component. 3. Etc. 4. Phase angle of the first component. 5. Phase angle of the second component. 6. Etc. 1. Magnitude of the first component. 2. Magnitude of the second component. 3. Etc. 4. Phase angle of the first component. 5. Phase angle of the second component. 6. Etc. 1. Magnitude of the first component of friction- generating connector force. 2. Magnitude of the second component of friction- generating connector force. 3. Etc. 4. Phase angle of the first component of friction- generating connector force. 5. Phase angle of the second component of friction- generating connector force. 6. Etc. 547(S) 514(S) Magnitude and phase angle of connector relative velocity in the direction of instantaneous slip Output variable: PHCIVSL 1. Magnitude of connector relative velocity in the direction of instantaneous slip. 2. Phase angle of connector relative velocity in the direction of instantaneous slip. RMS values of connector total forces Output variable: RCTF 1. First component of force. 2. Second component of force. 3. Etc. Record Record type key Attributes 515(S) 516(S) 517(S) 521(S) 518(S) 519(S) 544(S) RMS values of connector elastic forces Output variable: RCEF RMS values of connector viscous forces Output variable: RCVF RMS values of connector reaction forces Output variable: RCRF RMS values of connector friction forces Output variable: RCSF 1. First component of force. 2. Second component of force. 3. Etc. 1. First component of force. 2. Second component of force. 3. Etc. 1. First component of force. 2. Second component of force. 3. Etc. 1. First component of force. 2. Second component of force. 3. Etc. RMS values of connector relative displacements Output variable: RCU 1. First component of relative displacements. 2. Second component of relative displacements. 3. Etc. RMS values of connector constitutive displacements Output variable: RCCU 1. First component of constitutive displacements. 2. Second component of constitutive displacements. 3. Etc. RMS values of connector force generating friction Output variable: RCNF 1. RMS values of first component of friction- generating connector force. 2. RMS values of second component of friction- generating connector force. 3. Etc. Records for fluid link elements (available only for linear dynamics) 94(S) 95(S) Magnitude and phase angle of mass flow rate Output variable: PHMFL Magnitude and phase angle of total mass flow Output variable: PHMFT Records for output of element volumes 1. Magnitude. 2. Phase angle. 1. Magnitude. 2. Phase angle. The following three variables are not available for eigenfrequency extraction, complex eigenfrequency extraction, eigenvalue buckling prediction, or linear dynamics procedures. They are available only for continuum and structural elements not using general beam or shell section definitions. key 76(S) 77(S) 78(S) Integration point volume Output variable: IVOL Section volume Output variable: SVOL Whole element volume Output variable: EVOL FILE OUTPUT FORMAT Attributes 1. Current integration point volume. Section point volume in the case of beams and shells. 1. Current section volume. 1. Current element volume. Record for solid elements in an adaptive mesh domain in Abaqus/Standard 264(S) Change in volume. Output variable: VOLC 1. Change in area or volume of an element set solely due to adaptive meshing. Records written for any node file output request Record Record type key Attributes 101 102 103 104 Displacements Output variable: U Velocities Output variable: V Accelerations Output variable: A Reaction forces Output variable: RF 105(S) 106(S) Electrical potential Output variable: EPOT Point loads, moments, fluxes Output variable: CF 1. Node number. 2. First component of displacement. 3. Second component of displacement. 4. Etc. 1. Node number. 2. First component of velocity. 3. Second component of velocity. 4. Etc. 1. Node number. 2. First component of acceleration. 3. Second component of acceleration. 4. Etc. 1. Node number. 2. First component of reaction force. 3. Second component of reaction force. 4. Etc. 1. Node number. 2. Magnitude. 1. Node number. 2. First component of load or flux. 3. Second component of load or flux. 4. Etc. Record Record type key 107 Coordinates Output variable: COORD 108 109(S) 110(S) 119(S) 120(S) 136 137 138(S) 139(S) 145(S) Pore or acoustic pressure Output variable: POR Reactive fluid volume flux Output variable: RVF Reactive fluid total volume Output variable: RVT Electrical reaction charges Output variable: RCHG Concentrated electrical nodal charges Output variable: CECHG Fluid cavity pressure Output variable: PCAV Fluid cavity volume Output variable: CVOL Electrical reaction current Output variable: RECUR Concentrated electrical nodal current Output variable: CECUR Viscous forces due to static stabilization Output variable: VF 146(S) Total forces Output variable: TF Attributes 1. Node number. 2. First coordinate. 3. Second coordinate. 4. Etc. 1. Node number. 2. Pressure. 1. Node number. 2. Reaction fluid volume flux. 1. Node number. 2. Reaction fluid total volume. 1. Node number. 2. Charge scalar value. 1. Node number. 2. Current scalar value. 1. Fluid cavity reference node number. 2. Pressure. 1. Fluid cavity reference node number. 2. Volume. 1. Node number. 2. Electrical current. 1. Node number. 2. Electrical current. 1. Node number. 2. First component of viscous force. 3. Second component of viscous force. 4. Etc. 1. Node number. 2. First component of total force. 3. Second component of total force. 4. Etc. 151(E) Acoustic absolute pressure Output variable: PABS 1. Node number. 2. Absolute pressure. Record Record type key 201 Temperatures Output variable: NT 204(S) 204(E) 206(S) 214(S) 221(S) 237(S) Residual fluxes Output variable: RFL Reaction fluxes Output variable: RFL Concentrated fluxes Output variable: CFL Internal fluxes Output variable: RFLE Normalized concentration (mass diffusion analysis) Output variable: NNC Motions (in cavity radiation analysis) Output variable: MOT Attributes 1. Node number. 2. Temperature. 3. Etc. (for heat shells) 1. Node number. 2. Residual flux. 3. Etc. (for heat shells) 1. Node number. 2. First component of reaction flux. 3. Second component of reaction flux. 4. Etc. 1. Node number. 2. Concentrated flux. 3. Etc. (for heat shells) 1. Node number. 2. Flux, excluding external flux. 3. Etc. (for heat shells) 1. Node number. 2. Concentration. 1. Node number. 2. First component of motion. 3. Second component of motion. 4. Etc. 320(S) Concentrated fluid flow Output variable: CFF 1. Node number. 2. Magnitude of fluid flow. Records for linear dynamics 111(S) Magnitude and phase angle of relative displacement Output variable: PU 1. Node number. 2. Magnitude of first displacement component. 3. Magnitude of second displacement component. 4. Etc. 5. Phase angle of first displacement component. 6. Phase angle of second displacement component. 7. Etc. Record Record type key Attributes 112(S) Magnitude and phase angle of total displacement Output variable: PTU 113(S) Total displacement Output variable: TU 114(S) Total velocity Output variable: TV 115(S) Total acceleration Output variable: TA 116(S) 117(S) 118(S) 123(S) Magnitude and phase angle of acoustic or fluid cavity pressure Output variable: PPOR Magnitude and phase angle of electrical potential Output variable: PHPOT Magnitude and phase angle of reactive charge (piezoelectric analysis) Output variable: PHCHG RMS values of relative displacement Output variable: RU 124(S) RMS values of total displacement Output variable: RTU 1. Node number. 2. Magnitude of first displacement component. 3. Magnitude of second displacement component. 4. Etc. 5. Phase angle of first displacement component. 6. Phase angle of second displacement component. 7. Etc. 1. Node number. 2. First component of displacement. 3. Second component of displacement. 4. Etc. 1. Node number. 2. First component of velocity. 3. Second component of velocity. 4. Etc. 1. Node number. 2. First component of acceleration. 3. Second component of acceleration. 4. Etc. 1. Node number. 2. Magnitude of pressure. 3. Phase angle of pressure. 1. Node number. 2. Magnitude of potential. 3. Phase angle of potential. 1. Node number. 2. Magnitude of charge. 3. Phase angle of charge. 1. Node number. 2. First component of displacement. 3. Second component of displacement. 4. Etc. 1. Node number. 2. First component of displacement. 3. Second component of displacement. key 127(S) RMS values of relative velocity Output variable: RV 128(S) RMS values of total velocity Output variable: RTV 131(S) RMS values of relative acceleration Output variable: RA 132(S) RMS values of total acceleration Output variable: RTA 134(S) RMS values of reaction forces Output variable: RRF 135(S) Magnitude and phase angle of reaction force Output variable: PRF FILE OUTPUT FORMAT Attributes 4. Etc. 1. Node number. 2. First component of velocity. 3. Second component of velocity. 4. Etc. 1. Node number. 2. First component of velocity. 3. Second component of velocity. 4. Etc. 1. Node number. 2. First component of acceleration. 3. Second component of acceleration. 4. Etc. 1. Node number. 2. First component of acceleration. 3. Second component of acceleration. 4. Etc. 1. Node number. 2. First component of reaction force. 3. Second component of reaction force. 4. Etc. 1. Node number. 2. Magnitude of first component of reaction force. 3. Magnitude of second component of reaction force. 4. Etc. 5. Phase angle of first component of reaction force. 6. Phase angle of second component of reaction force. 7. Etc. Records written for any modal file output request during mode-based dynamic analysis Record Record type key Attributes 301(S) Generalized displacements Output variable: GU 1. First generalized displacement. 2. Second generalized displacement. Record Record type key Generalized velocities Output variable: GV Generalized accelerations Output variable: GA Base motions Output variable: BM Attributes 3. Etc. 1. First generalized velocity. 2. Second generalized velocity. 3. Etc. 1. First generalized acceleration. 2. Second generalized acceleration. 3. Etc. 1. 1 if displacement, 2 if velocity, 3 if acceleration. 2. x-direction component. 3. y-direction component. 4. z-direction component. 5. x-rotation component. 6. y-rotation component. 7. z-rotation component. 8. Base name. Phase angle of generalized displacement Output variable: GPU 1. Phase angle of generalized displacement for first mode. 2. Phase angle of generalized displacement for second mode. 3. Etc. Phase angle of generalized velocity Output variable: GPV 1. Phase angle of generalized velocity for first mode. 2. Phase angle of generalized velocity for second mode. 3. Etc. Phase angle of generalized acceleration Output variable: GPA 1. Phase angle of generalized acceleration for first mode. 2. Phase angle of generalized acceleration for second Strain energy per mode Output variable: SNE Kinetic energy per mode Output variable: KE mode. 3. Etc. 1. Strain energy for first mode. 2. Strain energy for second mode. 3. Etc. 1. Kinetic energy for first mode. 2. Kinetic energy for second mode. 3. Etc. 5.1.2–34 302(S) 303(S) 304(S) 305(S) 306(S) 307(S) 308(S) Record Record type key 310(S) External work per mode Output variable: T Attributes 1. External work for first mode. 2. External work for second mode. 3. Etc. Records written for any element matrix or substructure matrix file output request The ordering of variables on element matrices is the same as that used for user elements : first the variables at the element’s first node, then those at its second node, etc. Abaqus allows elements to have repeated nodes. Record Record type key 1001(S) Element matrix header record 1002(S) Element or substructure recovery matrix nodal dof 1003(S) Element or substructure recovery matrix nodal dof change 1004(S) Element matrix record size Attributes 1. Element number (zero if this is a substructure). 2. Element or substructure type in A8 format. 3. Number of nodes on the element. 4. Node number of the element’s first node. 5. Node number of the element’s second node. 6. Etc. 1. First dof at the element’s or at the recovery matrix’s first retained node. 2. Second dof at the element’s or at the recovery matrix’s first retained node. 3. Etc. 1. Node where the dof’s change. 2. First dof at this node. 3. Second dof at this node. 4. Etc. 1. Maximum record length (including the record length and record key words) for element matrix and load vector records that follow. The matrix or load vector records will be subdivided into multiple records as needed to fit within this maximum length. The record key for any continuation record will be the same as for the first record. 1005(S) Element matrix header (continued) 1. Element node number continued from record 1001 (if necessary). Record Record type key 1011(S) Symmetric element stiffness matrix Attributes 2. Etc. 1. (1, 1) stiffness. 2. (1, 2) stiffness. 3. (2, 2) stiffness. 4. Etc., stored in columns, from the first row to the diagonal term of each column. 1012(S) Nonsymmetric element stiffness matrix 1. (1, 1) stiffness. 2. (2, 1) stiffness. 3. (3, 1) stiffness. 4. Etc., stored in columns. 1021(S) Symmetric element mass matrix 1. (1, 1) mass. 2. (1, 2) mass. 3. (2, 2) mass. 4. Etc., stored in columns, from the first row to the diagonal term of each column. 1022(S) Nonsymmetric element mass matrix 1031(S) Load vector 1032(S) Substructure load case vector 1041(S) Substructure recovery matrix header record 1. (1, 1) mass. 2. (2, 1) mass. 3. (3, 1) mass. 4. Etc., stored in columns. 1. Load case. 2. Load on first dof. 3. Load on second dof. 4. Etc. 1. Load case name (A8 format). 2. Load on first dof. 3. Load on second dof. 4. Etc. 1. Zero. 2. Element or substructure type in A8 format. 3. Number of eliminated nodes. 4. Node number of the first eliminated node. 5. Node number of the second eliminated node. 6. Etc. Record Record type key Attributes 1042(S) Substructure recovery matrix 1. Column number corresponding to the retained 1043(S) Substructure recovery matrix header (continued) dofs list. 2. Coefficient of first eliminated dof. 3. Coefficient of second eliminated dof. 4. Etc. 1. Node number continued from record 1041 (if necessary). 2. Etc. Record written for any energy file output request When you do not specify an element set for which energy output is being requested in Abaqus/Standard, record 1999 provides values summed over the entire model; when you specify an element set for energy output, record 1999 provides values summed over all the elements in the specified element set. You can distinguish between a whole model 1999 energy record and an element set 1999 energy record by searching for a 1911 output request definition record containing the element set name; this 1911 record will be written just before the element set 1999 energy record. This 1911 record also has the first attribute set to 3 to indicate element set output. In Abaqus/Explicit you cannot specify selected element sets for an energy output request; record 1999 provides the total energies for the whole model. Record Record type key 1999(S) Total energies record Attributes 1. Total kinetic energy (ALLKE). 2. Total recoverable (elastic) strain energy (ALLSE). 3. Total external work (ALLWK, available only for the whole model.) 4. Total plastic dissipation (ALLPD). 5. Total creep dissipation (ALLCD). 6. Total dissipation, viscous not including dissipation due to stabilization (ALLVD). 7. Total loss of kinetic energy at impacts (ALLKL, available only for the whole model). 8. Total artificial strain energy (ALLAE). 9. Total energy dissipated through quiet boundaries (ALLQB, available only for the whole model). 10. Total electrostatic energy (ALLEE). 11. Total strain energy (ALLIE). 12. Total energy balance (ETOTAL, available only for the whole model). Record Record type key Attributes 1999(E) Total energies record 13. Total energy dissipated through frictional effects (ALLFD, available only for the whole model). 14. Total electrical energy dissipated in conductors (ALLJD). 15. Total static dissipation (due to stabilization, ALLSD). 16. Total damage dissipation (ALLDMD). 17. Currently not used. 18. Currently not used. 1. Total kinetic energy (ALLKE). 2. Total recoverable (elastic) strain energy (ALLSE). 3. Total external work (ALLWK). 4. Total plastic dissipation (ALLPD). 5. Total viscoelastic dissipation (ALLCD). 6. Total viscous dissipation (ALLVD, not supported for hyperelastic and hyperfoam material models). 7. Currently not used. 8. Total artificial strain energy (ALLAE). dissipation 9. Total distortion control energy (ALLDC). 10. Currently not used. 11. Total strain energy (ALLIE). 12. Total energy balance (ETOTAL). 13. Total energy dissipated through frictional effects (ALLFD). 14. Currently not used. 15. Percent change in mass (DMASS). 16. Total damage dissipation (ALLDMD). 17. Internal heat energy (ALLIHE). 18. External heat energy (ALLHF). Records written for contour integrals Calculations of the J-integral and the C -integral, the stress intensity factors, the crack propagation direction, and the T-stress can be requested. The record is written for each crack, one record per crack front location. See record key 17 for J-integral values for line spring elements. key 1991(S) J-integral values 1992(S) C -integral values 1995(S) Stress intensity factors FILE OUTPUT FORMAT Attributes 1. Crack number. 2. Node set (A8 format). 3. Number of contours. 4. J-integral value estimated by first contour. 5. J-integral value estimated by second contour. 6. Etc. 1. Crack number. 2. Node set (A8 format). 3. Number of contours. 4. C -integral value estimated by first contour. 5. C -integral value estimated by second contour. 6. Etc. 1. Crack number. 2. Node set (A8 format). 3. Number of contours. 4. (Mode I stress intensity factor) estimated by 5. 6. first contour. (Mode II stress intensity factor) estimated by first contour. 7. Crack (Mode III stress intensity factor) estimated by first contour (available only for 3-D elements). degrees) estimated by first contour (available only for homogeneous, isotropic elastic materials). propagation direction (in 8. J-integral value estimated from stress intensity factors of first contour. 9. (Mode I stress intensity factor) estimated by second contour. 10. 11. (Mode II stress intensity factor) estimated by second contour. (Mode III stress intensity factor) estimated (available only for 3-D by second contour elements). 12. Crack direction propagation estimated by second contour for homogeneous, isotropic elastic materials). 13. J-integral value estimated from stress intensity degrees) (available only (in factors of second contour. 14. Etc. Record Record type key 1996(S) T-stress values Attributes 1. Crack number. 2. Node set (A8 format). 3. Number of contours. 4. T-stress value estimated by first contour. 5. T-stress value estimated by second contour. 6. Etc. Record written for crack propagation analysis The following record is written for each crack that is identified in the crack propagation analysis: Record Record type key 1993(S) Crack tip location and associated quantities Attributes 1. Crack number. 2. Slave surface (A8 format). 3. Master surface (A8 format). 4. Initial crack-tip node number. 5. Current crack-tip node number. 6. Flag to indicate crack propagation criterion. 1 for crack length criterion. 2 for critical stress criterion. 3 for crack opening displacement criterion. 5 for VCCT criterion. 7. Cumulative incremental crack length. 8. Value of stress criterion is used. Current value of critical crack opening displacement if crack opening displacement criterion is used. if critical Records written once for any file output request when surfaces are defined in Abaqus/Standard The number of data items for the following record depends on the type of surface being defined. 9. Value of if critical stress criterion is used. Record Record type key Rigid surfaces 1501(S) Surface definition header Attributes 1. Surface name. 2. Dimension key (1-1D, 2-2D, 3-3D, 4-Axisymmetric). 3. Type key (1-Deformable, 2-Rigid). key Attributes FILE OUTPUT FORMAT Deformable surfaces 1501(S) Surface definition header 1502(S) Surface facet 4. Number of facets making up the surface. 5. Reference node label. 1. Surface name. 2. Dimension key (1-1D, 2-2D, 3-3D, 4-Axisymmetric). 3. Type key (1-Deformable, 2-Rigid). 4. Number of facets making up the surface. 5. Number of contact master surfaces associated with this surface through contact pairing (0 if this surface is a master surface). 6. First master surface name. 7. Second master surface name. 8. Etc. 1. Underlying element number. 2. Element face key (1–S1, 2–S2, 3–S3, 4–S4, 5–S5, 6–S6, 7–SPOS, 8–SNEG). 3. Number of nodes in facet. 4. Node number of the facet’s first node. 5. Node number of the facet’s second node. 6. Etc. Records written for any contact surface file output request Record Record type key Attributes 5(S) Solution-dependent state variables Output variable: SDV 1503(S) Output request definition 1. State variable 1. 2. State variable 2. 3. Etc. The record can have up to 80 words in ASCII format or 512 words in binary format. Repeat this record as often as necessary to output all active state variables in the model. 1. Contact file output (0). 2. Slave surface name. 3. Master surface name. 4. Node set containing a subset of the nodes making up the slave surface. Record Record type key 1504(S) Node header 1511(S) Contact tractions Output variable: CSTRESS 1512(S) Viscous tractions Output variable: CDSTRESS 1521(S) Contact clearances Output variable: CDISP 1522(S) Total force due to contact pressure Output variable: CFN 1523(S) Total force due to frictional stress Output variable: CFS 1575(S) Total force due to contact pressure and frictional stress Output variable: CFT Attributes 1. Node number. 2. Number of traction components (2 for 2-D or axisymmetric cases, 3 for 3-D cases). 1. Contact pressure between the node on the slave surface and the master surface with which it interacts. 2. Frictional shear traction component in the local 1-direction on the master surface. 3. Frictional shear traction component in the local 2-direction on the master surface for 3-D. 1. Viscous pressure between the node on the slave surface and the master surface with which it interacts. 2. Viscous shear traction component in the local 1- direction on the master surface. 3. Viscous shear traction component in the local 2- direction on the master surface for 3-D. 1. Separation of the surfaces in the direction of the normal to the master surface. 2. Accumulated relative tangential displacement of the surfaces in the local 1-direction on the master surface. 3. Accumulated relative tangential displacement of the surfaces in the local 2-direction on the master surface for 3-D. 1. Magnitude. 2. Force component in the global 1-direction. 3. Force component in the global 2-direction. 4. Force component in the global 3-direction. 1. Magnitude. 2. Force component in the global 1-direction. 3. Force component in the global 2-direction. 4. Force component in the global 3-direction. 1. Magnitude. 2. Force component in the global 1-direction. 3. Force component in the global 2-direction. 4. Force component in the global 3-direction. Attributes 1. Magnitude. 1. Magnitude. 2. Moment component about the global 1-axis. 3. Moment component about the global 2-axis. 4. Moment component about the global 3-axis. 1. Magnitude. 2. Moment component about the global 1-axis. 3. Moment component about the global 2-axis. 4. Moment component about the global 3-axis. 1. Magnitude. 2. Moment component about the global 1-axis. 3. Moment component about the global 2-axis. 4. Moment component about the global 3-axis. 1. Magnitude. 1. Coordinate in the global 1-direction. 2. Coordinate in the global 2-direction. 3. Coordinate in the global 3-direction. 1. Coordinate in the global 1-direction. 2. Coordinate in the global 2-direction. 3. Coordinate in the global 3-direction. 1. Coordinate in the global 1-direction. 2. Coordinate in the global 2-direction. 3. Coordinate in the global 3-direction. 1. Magnitude. 1. Magnitude. 5.1.2–43 Record Record type key 1524(S) 1526(S) 1527(S) 1576(S) Total area in contact Output variable: CAREA Total moment about the origin due to contact pressure Output variable: CMN Total moment about the origin due to frictional stress Output variable: CMS Total moment about the origin due to contact pressure and frictional stress Output variable: CMT 1578(S) Maximum torque that can be transmitted about the z-axis by a contact surface in an axisymmetric analysis with a friction coefficient of unity Output variable: CTRQ 1573(S) 1574(S) 1577(S) 1528(S) 1529(S) Coordinates of the center of the force due to contact pressure Output variable: XN Coordinates of the center of the force due to frictional stress Output variable: XS Coordinates of the center of the force due to contact pressure and frictional stress Output variable: XT Heat flux density Output variable: HFL HFL multiplied by the nodal area Record Record type key Attributes 1530(S) 1531(S) 1532(S) 1533(S) 1534(S) 1535(S) Time integrated HFL Output variable: HTL Time integrated HFLA Output variable: HTLA Heat flux density due to frictional dissipation Output variable: SFDR SFDR multiplied by the nodal area Output variable: SFDRA Time integrated SFDR Output variable: SFDRT Time integrated SFDRA Output variable: SFDRTA 1536(S) Weighting factor Output variable: WEIGHT 1537(S) 1538(S) 1539(S) 1540(S) 1541(S) 1542(S) 1543(S) 1544(S) Heat flux density due to electrical current Output variable: SJD SJD multiplied by the nodal area Output variable: SJDA Time integrated SJD Output variable: SJDT Time integrated SJDA Output variable: SJDTA Electrical current density Output variable: ECD ECD multiplied by area Output variable: ECDA Time integrated ECD Output variable: ECDT Time integrated ECDA Output variable: ECDTA 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. Record Record type key Attributes 1545(S) 1546(S) 1547(S) 1548(S) 1549(S) Pore fluid volume flux per unit area Output variable: PFL PFL multiplied by the nodal area Output variable: PFLA Time integrated PFL Output variable: PTL Time integrated PFLA Output variable: PTLA Total pore fluid volume flux leaving the slave surface Output variable: TPFL 1550(S) Time integrated TPFL Output variable: TPTL 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. Records for bond failure quantities from crack propagation analysis 1570(S) 1571(S) 1572(S) 290(S) 293(S) 294(S) 235(S) 295(S) Time when bond failure occurs Output variable: DBT Fraction of stress that remains at bond failure Output variable: DBSF 1. Magnitude. 1. Magnitude. Remaining stress in the failed bond Output variable: DBS 1. 11-component of debond stress. 2. 12-component of debond stress. Relative displacement behind crack when fracture criterion is met Output variable: OPENBC Effective energy release rate ratio Output variable: EFENRRTR Bond state (varies from 1.0 to 0.0) Output variable: BDSTAT Damage variable Output variable: CSDMG Critical stress at failure Output variable: CRSTS 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. 11-component of critical stress. 2. 12-component of critical stress. Record Record type key Attributes 296(S) Strain energy release rate Output variable: ENRRT 3. 13-component of critical stress (only available to three-dimensional models). 1. 11-component of strain energy release rate. 2. 12-component of strain energy release rate. 3. 13-component of strain energy release rate (only available to three-dimensional models). Record for surface-based pressure penetration analysis 1592(S) Fluid pressure for surface-based pressure penetration analysis Output variable: PPRESS 1. Magnitude. Records for surface-based cohesive behavior with damage 253(S) 345(S) 346(S) 347(S) 348(S) Overall value of the scalar damage variable Output variable: CSDMG Maximum contact stress damage initiation criterion Output variable: CSMAXSCRT Maximum separation damage initiation criterion Output variable: CSMAXUCRT Quadratic contact stress damage initiation criterion Output variable: CSQUADSCRT Quadratic separation damage initiation criterion Output variable: CSQUADUCRT 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. Records written once for any file output request when cavities are defined Record Record type key 1601(S) Cavity definition header Attributes 1. Number of surfaces making up the cavity. 2. Cavity name. 3. Name of cavity’s first surface. 4. Name of cavity’s second surface. 5. Etc. key 1610(S) Facet order record size 1602(S) Cavity facet order FILE OUTPUT FORMAT Attributes 1. Maximum record length (including the record length and record key words) for cavity facet order records that follow. The cavity facet order data will be subdivided into multiple records as needed to fit within this maximum length. The record key for any continuation record will be the same as for the first record. 1. Number of facets making up the cavity. 2. Cavity name. 3. Cavity’s first (underlying) element number. 4. First element face key (1-S1, 2–S2, 3–S3, 4–S4, 5–S5, 6–S6, 7–SPOS, 8–SNEG) 5. Cavity’s second (underlying) element number. 6. Second element face key (1–S1, 2–S2, 3–S3, 4–S4, 5–S5, 6–S6, 7–SPOS, 8–SNEG) 7. Etc. Records written for any viewfactor matrix output request The ordering of the facets (each facet corresponds to one row of the viewfactor matrix) is that appearing in the cavity facet order record 1602. Record Record type key 1608(S) Output request definition 1605(S) Viewfactor matrix header 1609(S) Viewfactor matrix record size 1606(S) Nonsymmetric viewfactor matrix Attributes 1. Viewfactor output (0). 2. Cavity name. 1. Number of facets in the cavity. 2. Cavity name. 1. Maximum record length (including the record length and record key words) for viewfactor matrix and facet area records that follow. The matrix or facet area records will be subdivided into multiple records as needed to fit within this maximum length. The record key for any continuation record will be the same as for the first record. 1. (1, 1) dimensionless viewfactor. 2. (1, 2) dimensionless viewfactor. Record Record type key Attributes 1607(S) Facet areas 3. (1, 3) dimensionless viewfactor. 4. Etc., stored in rows. 1. Area of first facet. 2. Area of second facet. 3. Area of third facet. 4. Etc. Records written for any radiation file output request Record Record type key 1603(S) Output request definition Attributes 1. Radiation file output (1). 2. Cavity name. 3. Surface name. 4. Element set name. 1604(S) Facet header record 1. (Underlying) user element number. 2. Element face key (1–S1, 2–S2, 3–S3, 4–S4, 5–S5, 6–S6, 7–SPOS, 8–SNEG) 231(S) 232(S) 233(S) 234(S) 235(S) Radiation flux density Radiation flux Time integrated radiation flux density Time integrated radiation flux Total viewfactor (sum of viewfactor matrix row) 3. Facet area. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 1. Magnitude. 236(S) Facet temperature 1. Magnitude. Records written for any section file output request The output variables described below are not available for random response analysis. Record Record type key 1580(S) Output request definition Attributes 1. Surface section output (1). 2. Section name. key 1581(S) Section output header record FILE OUTPUT FORMAT Attributes 1. Surface name. 2. System of coordinates used for output (1–Global, 2–Local). 3. Flag to indicate whether or not the local coordinate system and the output are updated during the analysis (1–Yes, 2–No). For all analysis types The following two records are generated only when section output is requested in a local coordinate system. In that case all components of forces and moments are given with respect to the local system. Only the first two directions of the local coordinate system are given; if needed, the third direction can be calculated as the cross product of the first two. 1582(S) 1583(S) Global coordinates of the anchor point Direction cosines of the local coordinate system 1584(S) Area of the defined section Output variable: SOAREA For stress/displacement analyses 1585(S) 1586(S) 1587(S) Total force in the section in the selected system Output variable: SOF Total moment in the section about the origin of the selected system Output variable: SOM Global coordinates of the center of the total force in the section Output variable: SOCF For heat transfer analyses 1. First coordinate. 2. Etc. 1. First component of the first direction. 2. Second component of the first direction. 3. Third component of the first direction. 4. First component of the second direction. 5. Second component of the second direction. 6. Third component of the second direction. 1. Magnitude. 1. Magnitude. 2. First force component. 3. Etc. 1. Magnitude. 2. First moment component. 3. Etc. 1. First coordinate. 2. Etc. 1588(S) Total heat flux across the section Output variable: SOH 1. Magnitude. Record Record type key For electrical analyses Attributes 1589(S) Total current across the section Output variable: SOE 1. Magnitude. For mass diffusion analyses 1590(S) Total mass flow across the section Output variable: SOD 1. Magnitude. For coupled pore fluid diffusion-stress analyses 1591(S) Total pore fluid volume flux across the section Output variable: SOP 1. Magnitude. For coupled analyses the appropriate combination of records is available. For example, in a thermal-electrical analysis both SOH and SOE are valid output requests. Procedure type keys Key Description Table 5.1.2–1 Keys to procedure types. 11 12 13 17 21 22 31 32 33 Static, automatic incrementation Static, direct incrementation Direct cyclic, automatic time incrementation Direct cyclic, fixed time incrementation Implicit dynamic, half-increment residual tolerance given Implicit dynamic, fixed time increments Implicit dynamic, subspace projection Explicit dynamic Quasi-static, explicit time integration Quasi-static, implicit integration Heat transfer, steady-state Heat transfer, transient, fixed time increments Heat transfer, transient, maximum allowable nodal temperature change given Description FILE OUTPUT FORMAT 34 35 36 41 42 51 61 62 63 64 65 71 72 73 74 75 76 77 85 86 91 92 93 94 95 98 Mass diffusion, steady-state Mass diffusion, transient, fixed time increments Mass diffusion, transient, maximum allowable normalized concentration change given Eigenvalue frequency extraction Eigenvalue buckling prediction Substructure generation Geostatic stress field Coupled pore fluid diffusion/stress, steady-state, fixed time incrementation Coupled pore fluid diffusion/stress, steady-state, automatic time incrementation Coupled pore fluid diffusion/stress, transient, fixed time incrementation Coupled pore fluid diffusion/stress, transient, automatic time incrementation Coupled thermal-stress, steady-state Coupled thermal-stress, transient, fixed time increments Coupled thermal-stress, transient, maximum allowable nodal temperature change and/or accuracy tolerance parameter given Explicit dynamic coupled thermal-stress Coupled thermal-electrical, steady-state Coupled thermal-electrical, transient analysis, fixed time increments Coupled thermal-electrical, transient analysis, maximum allowable nodal temperature change given Steady-state transport, automatic incrementation Steady-state transport, direct incrementation Response spectrum Modal dynamic Steady-state dynamic Random response Direct-solution steady-state dynamic Annealing 5.1.3 ACCESSING THE RESULTS FILE INFORMATION Products: Abaqus/Standard Abaqus/Explicit References • “Accessing the results file: overview,” Section 5.1.1 • “Results file output format,” Section 5.1.2 • “Utility routines for accessing the results file,” Section 5.1.4 Overview The Abaqus results (.fil) file is written using internal data management routines to minimize I/O cost. A postprocessing program must use these same Abaqus data management routines to read the results file. The following utility routines must be called to obtain data from the Abaqus results file: • INITPF • DBRNU • DBFILE • POSFIL You can also write a file in the format of the Abaqus results file by using the following utility subroutines: • INITPF • DBFILW The syntax of these utility subroutines is described in “Utility routines for accessing the results file,” Section 5.1.4. Reading floating point and integer variables To read both floating point and integer variables in the records, the following coding can be used in the postprocessing program: INCLUDE 'aba_param.inc' DIMENSION ARRAY(513), JRRAY(NPRECD,513) EQUIVALENCE (ARRAY(1),JRRAY(1,1)) With this technique, for example, the record key is available after each call to DBFILE with LOP=0 as KEY = JRRAY (1,2) The use of aba_param.inc eliminates the need to have different versions of the code for single and double precision. The file aba_param.inc defines an appropriate IMPLICIT REAL statement and sets the value of NPRECD to 1 or 2, depending upon whether the machine uses single or double precision. The file aba_param.inc is referenced from the site subdirectory of the Abaqus installation when the postprocessing program is compiled and linked using the abaqus make utility (explained below). Linking the postprocessing program The postprocessing program must be linked using the make parameter when running the Abaqus execution procedure . To link properly, the postprocessing program cannot contain a FORTRAN PROGRAM statement. Instead, the program must begin with a FORTRAN SUBROUTINE with the name ABQMAIN. Compiling, linking, and running a postprocessing program consists of two steps. For example, if the name of the postprocessing program is postproc.f, use the following command to compile and link postproc.f: abaqus make job=postproc The program must then be run using the command: abaqus postproc Calling the utility subroutines for reading the results file Subroutine INITPF must be called before any results file is accessed. This subroutine contains FORTRAN OPEN statements for all FORTRAN units assigned to results files through the call to INITPF; therefore, your code must not contain any OPEN statements for these units. Abaqus constructs a file name for a given unit based on information supplied as LRUNIT(1,K1) and FNAME, as discussed in “Utility routines for accessing the results file,” Section 5.1.4. Subroutine DBRNU must also be called before reading the first results file and then again each time you need to change to reading another results file. This subroutine simply establishes the FORTRAN unit number of the results file being read; no information is returned. DBRNU can be called before or after INITPF but must be called before DBFILE. Subroutine DBFILE is used to read each record from the results file. This subroutine will return one record at a time in the format described in “Results file output format,” Section 5.1.2. Example The following program reads all the von Mises stresses in the results file and obtains the maximum value. Then, it prints this value along with the element, section point, and integration point numbers where it occurred. In this example FORTRAN unit 8 is used to read the results file, and the name of the results file is assumed to be TEST.fil. The results file is assumed to be a binary file, and only one results file will be read. Thus, LRUNIT is dimensioned as LRUNIT(2,1); and in the call to the INITPF routine NRU is set to 1, LRUNIT(1,1) is set to 8, and LRUNIT(2,1) is set to 2. A new results file will not be written, so LOUTF is set to zero. ACCESSING THE FILE INFORMATION SUBROUTINE ABQMAIN Calculate the maximum von Mises stress and its location INCLUDE 'aba_param.inc' CHARACTER*80 FNAME DIMENSION ARRAY(513),JRRAY(NPRECD,513),LRUNIT(2,1) EQUIVALENCE (ARRAY(1),JRRAY(1,1)) File initialization FNAME='TEST' NRU=1 LRUNIT(1,1)=8 LRUNIT(2,1)=2 LOUTF=0 CALL INITPF(FNAME,NRU,LRUNIT,LOUTF) JUNIT=8 CALL DBRNU(JUNIT) Loop on all records in results file STRESS=0. DO 100 K1=1,99999 CALL DBFILE(0,ARRAY,JRCD) IF(JRCD.NE.0)GO TO 110 KEY=JRRAY(1,2) IF(KEY.EQ.1) THEN Element header record: extract element, sec pt, int pt numbers JEL=JRRAY(1,3) JPNT=JRRAY(1,4) JSPNT=JRRAY(1,5) Stress invariant record for Abaqus/Standard ELSE IF(KEY.EQ.12)THEN Stress invariant record for Abaqus/Explicit ELSE IF(KEY.EQ.75)THEN Extract von Mises stress IF(ARRAY(3).GT.STRESS)THEN STRESS=ARRAY(3) KEL=JEL KPNT=JPNT KSPNT=JSPNT END IF END IF 100 110 CONTINUE CONTINUE WRITE(6,120) KEL,KPNT,KSPNT,STRESS FORMAT(5X,'ELEMENT',I5,5X,'POINT',I4,5X,'SECTION POINT', 120 1 I4,5X,'STRESS',1PG12.3) STOP END See Chapter 14, “Postprocessing of Abaqus Results Files,” of the Abaqus Example Problems Manual for additional examples. Writing a file in the results file format Subroutine DBFILW can be used to write a file in the format of the Abaqus results file to modify the file information or to add additional information before postprocessing. Subroutine INITPF must be called before DBFILW. The file will be written to FORTRAN unit 9 with the extension .fin. Unit 9 is opened by Abaqus when DBFILW is first called; your coding must not open or redefine unit 9, but you must ensure that FORTRAN unit 9 is saved following the job. “Joining data from multiple results files and converting file format: FJOIN,” Section 14.1.2 of the Abaqus Example Problems Manual, contains an example of the use of subroutine DBFILW to merge specific records of discontinuous results files. Continuous results files are required for postprocessing purposes; if you have written a results file during an analysis and a new results file on the restart of the analysis without making the files continuous, they must be made continuous before postprocessing. “Analysis of a cantilever subject to earthquake motion,” Section 1.4.13 of the Abaqus Benchmarks Manual, also shows the use of DBFILW for merging results files. Alternatively, results files can be merged using the abaqus append utility as described in “Joining results (.fil) files,” Section 3.2.12. The DBFILW subroutine can also be used to convert the Abaqus results file from binary to ASCII format to transfer it from one computer system to another. Alternatively, this conversion can be done automatically by using the abaqus ascfil execution procedure, as described in “ASCII translation of results (.fil) files,” Section 3.2.11. 5.1.4 UTILITY ROUTINES FOR ACCESSING THE RESULTS FILE Products: Abaqus/Standard Abaqus/Explicit References • “Accessing the results file information,” Section 5.1.3 • “URDFIL,” Section 1.1.48 of the Abaqus User Subroutines Reference Manual • “Joining data from multiple results files and converting file format: FJOIN,” Section 14.1.2 of the Abaqus Example Problems Manual • “Calculation of principal stresses and strains and their directions: FPRIN,” Section 14.1.3 of the Abaqus Example Problems Manual • “Creation of a perturbed mesh from original coordinate data and eigenvectors: FPERT,” Section 14.1.4 of the Abaqus Example Problems Manual Overview The Abaqus results (.fil) file can be accessed with the utility routines described in this section. Access is subsequent to an analysis by a user-written postprocessing program or, in Abaqus/Standard, from within an analysis by user subroutine URDFIL. The following utility subroutines are available: • DBFILE (read from a file) • DBFILW (write to a file) • DBRNU (set a unit number for a file) • INITPF (initialize a file) • POSFIL (determine position in a file; available only in Abaqus/Standard) These utility subroutines are described below in alphabetical order. Only the subroutines DBFILE and POSFIL can be called from user subroutine URDFIL. DBFILE (read from a file) Interface CALL DBFILE(LOP,ARRAY,JRCD) Variable to be provided to the utility routine LOP A flag, which you must set before calling DBFILE, indicating the operation. Set LOP=0 to read the next record in the file; set LOP=2 to rewind the file currently being read (for example, if it is necessary to read the file more than once, it must be rewound since it is a sequential file). If LOP=2 is used, the file must first be read to the end, and it should be rewound only when the end-of-file is reached. Variables returned from the utility routine ARRAY The array containing one record from the file, in the format described in “Results file output format,” Section 5.1.2. When LOP=0, this array will be filled by the data management routines with the contents of the next record in the file as each call to DBFILE is executed. ARRAY must be dimensioned adequately in your routines to contain the largest record in the file. For almost all cases 500 words is sufficient. The exceptions arise if the problem definition includes user elements or user materials that use more than this many state variables or if substructures with a large number of retained degrees of freedom are used . When the results file has been written on a system on which Abaqus runs in double precision, ARRAY must be declared double precision in your routine. JRCD Returned as nonzero if an end-of-file marker is read when DBFILE is called with LOP=0. DBFILW (write to a file) Interface CALL DBFILW(LOP,ARRAY,JRCD) Variables to be provided to the utility routine ARRAY The array containing one record to be written to the file, in the format described in “Results file output format,” Section 5.1.2. JRCD LOP Return code (0 – record written successfully, 1 – record not written). Not currently used. DBRNU (set a unit number for a file) Interface CALL DBRNU(JUNIT) Variable to be provided to the utility routine JUNIT The FORTRAN unit number of the results file to be read. Valid unit numbers are 8 to read the .fil file, 15–18, or numbers greater than 100. INITPF (initialize a file) Interface CALL INITPF(FNAME,NRU,LRUNIT,LOUTF) Variables to be provided to the utility routine FNAME A character string defining the root file name (that is, the name without an extension) of the files being read or written. FNAME must be declared as CHARACTER*80 and can include the directory specification as well as the root file name. The extension of each individual file is defined by the LRUNIT array below. See the discussion below for file naming conventions. NRU An integer giving the number of results files that the postprocessing program will read. Normally only one results file is read, but sometimes it is necessary to read several results files—for example, to merge them into a single file. LRUNIT An integer array that must be dimensioned LRUNIT(2,NRU) in the postprocessing program and must contain the following data before INITPF is called: LRUNIT(1,K1) is the FORTRAN unit number on which the K1th results file will be read. Valid unit numbers are 8 to read the .fil file, 15–18, or numbers greater than 100. All other units are reserved by Abaqus. See below for naming conventions based on the unit numbers. LRUNIT(2,K1) is an integer that must be set to 2 if the K1th results file was written as a binary file or set to 1 if the K1th results file was written in ASCII format. LOUTF Needs to be defined only if the program that is making the call to INITPF will also write an output file in the Abaqus results file format (for example, if results files are being merged into a single results file or if a results file is being converted from binary to ASCII format). In that case LOUTF should be set to 2 if the output file is to be written as a binary file or set to 1 if the output file is to be written as an ASCII file. This results file will be written with the file name extension .fin. See “Accessing the results file information,” Section 5.1.3, for a discussion of writing results files; see below for information on the naming of this file. File naming conventions The file extension is derived from the value of LRUNIT(1,K1). If LRUNIT(1,K1) is 8, the file name will be constructed with the extension fil. Any other unit number will result in a file extension of 0nn, where nn is the number assigned to LRUNIT(1,K1). For example, if LRUNIT(1,K1) is 15, the file extension is .015. If an output file has been indicated by a nonzero value of LOUTF, its extension will be .fin. For example, to read a file xxxx.fil, set LRUNIT(1,K1) to 8 and the character variable FNAME to xxxx using assignment or data statements. If desired, FNAME can include a directory specification, device name, or path. Operating system environment and shell variables will not be translated properly and, therefore, should not be used. All error messages generated by Abaqus are written to FORTRAN unit 6. On most machines error messages will be printed by default directly to the screen if the program is run interactively. You can include an open statement for unit 6 in the main program to redirect messages to a file. If you wish to read or write to units other than those units specified in LRUNIT, OPEN statements for those units may have to be included in the program (depending upon the computer being used). Unit numbers of such auxiliary files should be greater than 100 to avoid any conflict with Abaqus internal files. POSFIL (determine position in a file) The POSFIL utility routine is available only in Abaqus/Standard. Interface CALL POSFIL(NSTEP,NINC,ARRAY,JRCD) Variables to be provided to the utility routine NSTEP Desired step. If this variable is set to 0, the first available step will be read. NINC Desired increment. If this variable is set to 0, the first available increment of the specified step will be read. Variables returned from the utility routine ARRAY Real array containing the values of record 2000 from the results file for the requested step and increment. JRCD Return code (0 – specified increment found, 1 – specified increment not found). If the step and increment requested are not found in the results file, POSFIL will return an error and leave you positioned at the end of the results file. Positioning with POSFIL You may find it convenient to call POSFIL with both NSTEP and NINC set to 0 to skip over the information that is written to the results file at the beginning of an analysis and, thus, start reading from the first increment written to the file. POSFIL cannot be used to move backward in the results file: you cannot use POSFIL to find a given increment in the file and then make a second call to POSFIL later to read an increment earlier than the first one found. If this is attempted, POSFIL will return an error indicating that the requested increment was not found. OI.1 Abaqus/Standard OUTPUT VARIABLE INDEX This index provides a reference to all of the output variables that are available in Abaqus/Standard. Output variables are listed in alphabetical order. Variable Page Variable Page Variable Page BF . . . . . . . . . . . 4.2.1–29 BICURV . . . . . . . 4.2.1–25 BIMOM . . . . . . . 4.2.1–25 BM. . . . . . . . . . . 4.2.1–45 CA . . . . . . . . . . . 4.2.1–33 CALPHAF . . . . . 4.2.1–31 CALPHAFn. . . . . 4.2.1–31 CALPHAMn . . . . 4.2.1–31 CAn . . . . . . . . . . 4.2.1–33 CAREA . . . . . . . 4.2.1–47 CARn . . . . . . . . . 4.2.1–33 CASU. . . . . . . . . 4.2.1–32 CASUC . . . . . . . 4.2.1–32 CASUn . . . . . . . . 4.2.1–32 CASURn. . . . . . . 4.2.1–32 CCF . . . . . . . . . . 4.2.1–33 CCFn . . . . . . . . . 4.2.1–33 CCMn. . . . . . . . . 4.2.1–33 CCU . . . . . . . . . . 4.2.1–33 CCUn . . . . . . . . . 4.2.1–33 CCURn . . . . . . . . 4.2.1–33 CD . . . . . . . . . . . 4.2.1–54 CDIF . . . . . . . . . 4.2.1–31 CDIFC . . . . . . . . 4.2.1–32 CDIFn . . . . . . . . 4.2.1–31 CDIFRn . . . . . . . 4.2.1–32 CDIM . . . . . . . . . 4.2.1–32 CDIMC. . . . . . . . 4.2.1–32 CDIMn . . . . . . . . 4.2.1–32 CDIMRn . . . . . . . 4.2.1–32 CDIP . . . . . . . . . 4.2.1–32 CDIPC . . . . . . . . 4.2.1–32 CDIPn . . . . . . . . 4.2.1–32 CDIPRn . . . . . . . 4.2.1–32 OI.1–1 CDISP . . . . . . . . 4.2.1–46 CDISPETOS . . . . 4.2.1–46 CDMG . . . . . . . . 4.2.1–31 CDMGn . . . . . . . 4.2.1–31 CDMGRn . . . . . . 4.2.1–31 CDSTRESS . . . . . 4.2.1–46 CE . . . . . . . . . . . 4.2.1–10 CEAVG. . . . . . . . 4.2.1–36 CECHG . . . . . . . 4.2.1–39 CECUR . . . . . . . 4.2.1–39 CEEQ . . . . . . . . . 4.2.1–10 CEERI . . . . . . . . 4.2.1–36 CEF . . . . . . . . . . 4.2.1–30 CEFn . . . . . . . . . 4.2.1–30 CEij . . . . . . . . . . 4.2.1–10 CEMAG . . . . . . . 4.2.1–11 CEMn. . . . . . . . . 4.2.1–30 CENER. . . . . . . . 4.2.1–12 CENTMAG . . . . . 4.2.1–29 CENTRIFMAG . . 4.2.1–29 CEP . . . . . . . . . . 4.2.1–11 CEPn . . . . . . . . . 4.2.1–11 CESW . . . . . . . . 4.2.1–10 CF . . . . . . . . . . . 4.2.1–38 CFAILST . . . . . . 4.2.1–33 CFAILSTi . . . . . . 4.2.1–33 CFAILURE . . . . . 4.2.1–13 CFF . . . . . . . . . . 4.2.1–37 CFL . . . . . . . . . . 4.2.1–40 CFLn . . . . . . . . . 4.2.1–40 CFn . . . . . . . . . . 4.2.1–38 CFN . . . . . . . . . . 4.2.1–47 CFNM . . . . . . . . 4.2.1–47 CFORCE. . . . . . . 4.2.1–46 A . . . . . . . . . . . . 4.2.1–37 ACV. . . . . . . . . . 4.2.1–12 ACVn . . . . . . . . . 4.2.1–12 ALEAKVRB . . . . 4.2.1–17 ALEAKVRT . . . . 4.2.1–17 ALLAE. . . . . . . . 4.2.1–55 ALLCD. . . . . . . . 4.2.1–55 ALLDMD . . . . . . 4.2.1–56 ALLEE . . . . . . . . 4.2.1–55 ALLFD . . . . . . . . 4.2.1–55 ALLIE . . . . . . . . 4.2.1–55 ALLJD . . . . . . . . 4.2.1–55 ALLKE. . . . . . . . 4.2.1–55 ALLKL. . . . . . . . 4.2.1–55 ALLPD . . . . . . . . 4.2.1–55 ALLQB. . . . . . . . 4.2.1–55 ALLSD . . . . . . . . 4.2.1–56 ALLSE . . . . . . . . 4.2.1–56 ALLVD. . . . . . . . 4.2.1–56 ALLWK . . . . . . . 4.2.1–56 ALPHA. . . . . . . . 4.2.1–7 ALPHAij. . . . . . . 4.2.1–7 ALPHAk . . . . . . . 4.2.1–7 ALPHAk_ij . . . . . 4.2.1–7 ALPHAN . . . . . . 4.2.1–7 ALPHAP. . . . . . . 4.2.1–7 ALPHAPn . . . . . . 4.2.1–7 AMPCU . . . . . . . 4.2.1–56 An . . . . . . . . . . . 4.2.1–37 AR . . . . . . . . . . . 4.2.1–37 ARn . . . . . . . . . . 4.2.1–37 AT . . . . . . . . . . . 4.2.1–37 AZZIT . . . . . . . . 4.2.1–13 Variable Page Variable Page Variable Page CSFn . . . . . . . . . 4.2.1–31 CSLST . . . . . . . . 4.2.1–32 CSLSTi. . . . . . . . 4.2.1–32 CSMAXSCRT . . . 4.2.1–46 CSMAXUCRT. . . 4.2.1–46 CSMn . . . . . . . . . 4.2.1–31 CSQUADSCRT . . 4.2.1–46 CSQUADUCRT . . 4.2.1–46 CSTATUS . . . . . . 4.2.1–46 CSTRESS . . . . . . 4.2.1–45 CSTRESSERI . . . 4.2.1–46 CSTRESSETOS . . 4.2.1–45 CTF . . . . . . . . . . 4.2.1–30 CTFn . . . . . . . . . 4.2.1–30 CTMn. . . . . . . . . 4.2.1–30 CTRL_INPUT(OPT) 4.2.1–57 CTRQ. . . . . . . . . 4.2.1–47 CTSHR . . . . . . . . 4.2.1–11 CTSHRi3 . . . . . . 4.2.1–11 CU . . . . . . . . . . . 4.2.1–33 CUE . . . . . . . . . . 4.2.1–30 CUEn . . . . . . . . . 4.2.1–30 CUn . . . . . . . . . . 4.2.1–33 CUP . . . . . . . . . . 4.2.1–30 CUPEQ. . . . . . . . 4.2.1–30 CUPEQC . . . . . . 4.2.1–31 CUPEQn . . . . . . . 4.2.1–30 CUPn . . . . . . . . . 4.2.1–30 CUREn . . . . . . . . 4.2.1–30 CURn . . . . . . . . . 4.2.1–33 CURPEQn. . . . . . 4.2.1–30 CURPn . . . . . . . . 4.2.1–30 CV . . . . . . . . . . . 4.2.1–33 CVF . . . . . . . . . . 4.2.1–31 CVFn . . . . . . . . . 4.2.1–31 CVMn . . . . . . . . 4.2.1–31 CVn . . . . . . . . . . 4.2.1–33 CVOL. . . . . . . . . 4.2.1–39 CVRn . . . . . . . . . 4.2.1–33 OI.1–2 CW . . . . . . . . . . 4.2.1–38 CYCLEINI . . . . . 4.2.1–16 CYCLEINIXFEM 4.2.1–30 DAMAGEC. . . . . 4.2.1–15 DAMAGEFC. . . . 4.2.1–23 DAMAGEFT . . . . 4.2.1–23 DAMAGEMC . . . 4.2.1–24 DAMAGEMT . . . 4.2.1–24 DAMAGESHR . . 4.2.1–24 DAMAGET. . . . . 4.2.1–15 DAMPRATIO . . . 4.2.1–55 DBS . . . . . . . . . . 4.2.1–49 DBSF . . . . . . . . . 4.2.1–49 DBT . . . . . . . . . . 4.2.1–49 DG . . . . . . . . . . . 4.2.1–8 DGij . . . . . . . . . . 4.2.1–8 DGP . . . . . . . . . . 4.2.1–8 DGPn . . . . . . . . . 4.2.1–8 DISP_OPT . . . . . 4.2.1–57 DISP_OPT_VAL . 4.2.1–57 DMENER . . . . . . 4.2.1–13 DMICRT. . . . . . . 4.2.1–16 4.2.1–23 DUCTCRT . . . . . 4.2.1–23 E . . . . . . . . . . . . 4.2.1–7 EASEDEN . . . . . 4.2.1–35 ECD . . . . . . . . . . 4.2.1–16 4.2.1–48 ECDA. . . . . . . . . 4.2.1–48 ECDDEN . . . . . . 4.2.1–35 ECDM . . . . . . . . 4.2.1–16 ECDn . . . . . . . . . 4.2.1–16 ECDT . . . . . . . . . 4.2.1–48 ECDTA. . . . . . . . 4.2.1–48 4.2.1–49 ECTEDEN . . . . . 4.2.1–35 ECURS . . . . . . . . 4.2.1–27 EDMDDEN. . . . . 4.2.1–35 EE . . . . . . . . . . . 4.2.1–8 CFS . . . . . . . . . . 4.2.1–47 CFSM. . . . . . . . . 4.2.1–47 CFT . . . . . . . . . . 4.2.1–47 CFTM. . . . . . . . . 4.2.1–47 CHRGS . . . . . . . 4.2.1–27 CIVC . . . . . . . . . 4.2.1–32 CMn . . . . . . . . . . 4.2.1–38 CMN . . . . . . . . . 4.2.1–47 CMNM . . . . . . . . 4.2.1–47 CMS. . . . . . . . . . 4.2.1–47 CMSM . . . . . . . . 4.2.1–47 CMT . . . . . . . . . 4.2.1–47 CMTM . . . . . . . . 4.2.1–47 CNAREA . . . . . . 4.2.1–46 CNF . . . . . . . . . . 4.2.1–31 CNFC . . . . . . . . . 4.2.1–31 CNFn . . . . . . . . . 4.2.1–31 CNMn . . . . . . . . 4.2.1–31 CONC . . . . . . . . 4.2.1–15 CONF. . . . . . . . . 4.2.1–14 COORD . . . . . . . 4.2.1–18 4.2.1–25 4.2.1–38 COORn. . . . . . . . 4.2.1–38 CORIOMAG . . . . 4.2.1–29 CP . . . . . . . . . . . 4.2.1–33 CPn . . . . . . . . . . 4.2.1–33 CPRn . . . . . . . . . 4.2.1–33 CRACK . . . . . . . 4.2.1–14 CRF . . . . . . . . . . 4.2.1–32 CRFn . . . . . . . . . 4.2.1–32 CRMn. . . . . . . . . 4.2.1–33 CRPTIME . . . . . . 4.2.1–54 CRSTS . . . . . . . . 4.2.1–50 CS11 . . . . . . . . . 4.2.1–11 CSDMG . . . . . . . 4.2.1–46 4.2.1–49 CSF . . . . . . . . . . 4.2.1–31 Variable Page Variable Page Variable Page ENER . . . . . . . . . 4.2.1–12 ENRRT . . . . . . . . 4.2.1–50 ENRRTXFEM . . . 4.2.1–30 EP . . . . . . . . . . . 4.2.1–7 EPDDEN . . . . . . 4.2.1–35 EPG . . . . . . . . . . 4.2.1–16 EPGAVG . . . . . . 4.2.1–36 EPGERI . . . . . . . 4.2.1–36 EPGM . . . . . . . . 4.2.1–16 EPGn . . . . . . . . . 4.2.1–16 EPn . . . . . . . . . . 4.2.1–7 EPOT . . . . . . . . . 4.2.1–37 ER . . . . . . . . . . . 4.2.1–8 ERij . . . . . . . . . . 4.2.1–8 ERP . . . . . . . . . . 4.2.1–8 ERPn . . . . . . . . . 4.2.1–8 ERPRATIO . . . . . 4.2.1–23 ESDDEN . . . . . . 4.2.1–35 ESEDEN. . . . . . . 4.2.1–35 ESF1 . . . . . . . . . 4.2.1–25 ESOL . . . . . . . . . 4.2.1–29 ETOTAL . . . . . . . 4.2.1–56 EVDDEN . . . . . . 4.2.1–35 EVOL. . . . . . . . . 4.2.1–29 FILM . . . . . . . . . 4.2.1–29 FILMCOEF . . . . . 4.2.1–34 FLDCRT . . . . . . . 4.2.1–23 FLSDCRT . . . . . . 4.2.1–23 FLUVR. . . . . . . . 4.2.1–17 FLUXS . . . . . . . . 4.2.1–27 4.2.1–34 FLVEL . . . . . . . . 4.2.1–17 FLVELM. . . . . . . 4.2.1–17 FLVELn . . . . . . . 4.2.1–17 FOUND . . . . . . . 4.2.1–27 FTEMP . . . . . . . . 4.2.1–50 FV . . . . . . . . . . . 4.2.1–13 FVn . . . . . . . . . . 4.2.1–13 GA . . . . . . . . . . . 4.2.1–44 OI.1–3 GAn . . . . . . . . . . 4.2.1–44 GELVR. . . . . . . . 4.2.1–17 GFVR. . . . . . . . . 4.2.1–17 GM . . . . . . . . . . 4.2.1–54 GPA . . . . . . . . . . 4.2.1–44 GPAn . . . . . . . . . 4.2.1–44 GPU . . . . . . . . . . 4.2.1–44 GPUn . . . . . . . . . 4.2.1–44 GPV . . . . . . . . . . 4.2.1–44 GPVn . . . . . . . . . 4.2.1–44 GRADP . . . . . . . 4.2.1–12 GRAV. . . . . . . . . 4.2.1–29 GU . . . . . . . . . . . 4.2.1–44 GUn . . . . . . . . . . 4.2.1–44 GV . . . . . . . . . . . 4.2.1–44 GVn . . . . . . . . . . 4.2.1–44 HBF . . . . . . . . . . 4.2.1–29 HC . . . . . . . . . . . 4.2.1–52 HCn . . . . . . . . . . 4.2.1–52 HFL . . . . . . . . . . 4.2.1–15 4.2.1–47 4.2.1–48 4.2.1–49 HFLA . . . . . . . . . 4.2.1–47 4.2.1–48 4.2.1–49 HFLAVG . . . . . . 4.2.1–36 HFLERI . . . . . . . 4.2.1–36 HFLM . . . . . . . . 4.2.1–15 HFLn . . . . . . . . . 4.2.1–15 HO . . . . . . . . . . . 4.2.1–52 HOn . . . . . . . . . . 4.2.1–52 HP . . . . . . . . . . . 4.2.1–34 HSNFCCRT . . . . 4.2.1–23 HSNFTCRT. . . . . 4.2.1–23 HSNMCCRT . . . . 4.2.1–23 HSNMTCRT . . . . 4.2.1–23 HTL . . . . . . . . . . 4.2.1–48 4.2.1–49 EEij . . . . . . . . . . 4.2.1–8 EENER . . . . . . . . 4.2.1–13 EEP . . . . . . . . . . 4.2.1–8 EEPn . . . . . . . . . 4.2.1–8 EFENRRTR. . . . . 4.2.1–50 EFLAVG . . . . . . . 4.2.1–36 EFLERI . . . . . . . 4.2.1–36 EFLX . . . . . . . . . 4.2.1–16 EFLXM . . . . . . . 4.2.1–16 EFLXn . . . . . . . . 4.2.1–16 EIGFREQ . . . . . . 4.2.1–54 4.2.1–55 EIGIMAG . . . . . . 4.2.1–55 EIGREAL . . . . . . 4.2.1–55 EIGVAL . . . . . . . 4.2.1–54 Eij . . . . . . . . . . . 4.2.1–7 EKEDEN . . . . . . 4.2.1–35 ELASE . . . . . . . . 4.2.1–28 ELCD . . . . . . . . . 4.2.1–28 ELCTE . . . . . . . . 4.2.1–28 ELDMD . . . . . . . 4.2.1–28 ELEDEN. . . . . . . 4.2.1–34 ELEN . . . . . . . . . 4.2.1–27 ELJD . . . . . . . . . 4.2.1–28 ELKE . . . . . . . . . 4.2.1–27 ELPD . . . . . . . . . 4.2.1–28 ELSD . . . . . . . . . 4.2.1–28 ELSE . . . . . . . . . 4.2.1–27 ELVD . . . . . . . . . 4.2.1–28 EMB . . . . . . . . . 4.2.1–24 EMBF. . . . . . . . . 4.2.1–24 EMBFC . . . . . . . 4.2.1–24 EMCD . . . . . . . . 4.2.1–24 EME. . . . . . . . . . 4.2.1–24 EMH . . . . . . . . . 4.2.1–24 EMJH . . . . . . . . . 4.2.1–24 EMn . . . . . . . . . . 4.2.1–54 ENDEN . . . . . . . 4.2.1–36 Variable Page Variable Page Variable Page PEEQ . . . . . . . . . 4.2.1–9 4.2.1–15 4.2.1–18 PEEQAVG . . . . . 4.2.1–36 PEEQERI . . . . . . 4.2.1–36 PEEQMAX . . . . . 4.2.1–9 PEEQT . . . . . . . . 4.2.1–10 PEERI . . . . . . . . 4.2.1–36 PEij . . . . . . . . . . 4.2.1–9 4.2.1–18 PEMAG . . . . . . . 4.2.1–10 PENER . . . . . . . . 4.2.1–12 PEP . . . . . . . . . . 4.2.1–10 PEPn . . . . . . . . . 4.2.1–10 PEQC . . . . . . . . . 4.2.1–14 PEQCn . . . . . . . . 4.2.1–14 PFL . . . . . . . . . . 4.2.1–49 PFLA . . . . . . . . . 4.2.1–49 PFn . . . . . . . . . . 4.2.1–54 PFOPEN . . . . . . . 4.2.1–17 PHCA. . . . . . . . . 4.2.1–22 PHCAn . . . . . . . . 4.2.1–22 PHCARn. . . . . . . 4.2.1–22 PHCCU . . . . . . . 4.2.1–22 PHCCUn. . . . . . . 4.2.1–22 PHCCURn . . . . . 4.2.1–22 PHCEF . . . . . . . . 4.2.1–21 PHCEFn . . . . . . . 4.2.1–21 PHCEMn . . . . . . 4.2.1–21 PHCHG . . . . . . . 4.2.1–41 PHCIVC . . . . . . . 4.2.1–23 PHCNF . . . . . . . . 4.2.1–22 PHCNFC. . . . . . . 4.2.1–23 PHCNFn . . . . . . . 4.2.1–23 PHCNMn . . . . . . 4.2.1–23 PHCRF . . . . . . . . 4.2.1–21 PHCRFn . . . . . . . 4.2.1–21 PHCRMn . . . . . . 4.2.1–22 PHCSF . . . . . . . . 4.2.1–22 HTLA. . . . . . . . . 4.2.1–48 4.2.1–49 IE. . . . . . . . . . . . 4.2.1–8 IEij. . . . . . . . . . . 4.2.1–8 IEP. . . . . . . . . . . 4.2.1–8 IEPn . . . . . . . . . . 4.2.1–9 INFC . . . . . . . . . 4.2.1–39 INFN . . . . . . . . . 4.2.1–39 INFR . . . . . . . . . 4.2.1–39 INTEN . . . . . . . . 4.2.1–11 INV3 . . . . . . . . . 4.2.1–7 IRA . . . . . . . . . . 4.2.1–53 IRAn . . . . . . . . . 4.2.1–53 IRARn . . . . . . . . 4.2.1–53 IRF. . . . . . . . . . . 4.2.1–53 IRFn . . . . . . . . . . 4.2.1–53 IRMASS . . . . . . . 4.2.1–54 IRMn . . . . . . . . . 4.2.1–53 IRRI . . . . . . . . . . 4.2.1–53 IRRIij . . . . . . . . . 4.2.1–54 IRX . . . . . . . . . . 4.2.1–53 IRXn . . . . . . . . . 4.2.1–53 ISOL . . . . . . . . . 4.2.1–15 IVOL . . . . . . . . . 4.2.1–18 JENER . . . . . . . . 4.2.1–13 JK . . . . . . . . . . . 4.2.1–14 KE . . . . . . . . . . . 4.2.1–45 KEn . . . . . . . . . . 4.2.1–45 LE . . . . . . . . . . . 4.2.1–8 LEAKVRB . . . . . 4.2.1–17 LEAKVRT . . . . . 4.2.1–17 LEij . . . . . . . . . . 4.2.1–8 LEP . . . . . . . . . . 4.2.1–8 LEPn . . . . . . . . . 4.2.1–8 LOADS. . . . . . . . 4.2.1–27 LOCALDIRn . . . . 4.2.1–18 LPF . . . . . . . . . . 4.2.1–56 MASS. . . . . . . . . 4.2.1–53 MAT_PROP_NORMALIZED 4.2.1–56 MAXECRT . . . . . 4.2.1–16 MAXSCRT . . . . . 4.2.1–16 MAXSS . . . . . . . 4.2.1–25 MFL . . . . . . . . . . 4.2.1–13 4.2.1–15 MFLM . . . . . . . . 4.2.1–15 MFLn . . . . . . . . . 4.2.1–16 MFLT . . . . . . . . . 4.2.1–13 MFR. . . . . . . . . . 4.2.1–13 MFRn . . . . . . . . . 4.2.1–13 MISES . . . . . . . . 4.2.1–6 MISESAVG . . . . . 4.2.1–36 MISESERI . . . . . 4.2.1–36 MISESMAX . . . . 4.2.1–6 MISESONLY. . . . 4.2.1–6 MOT . . . . . . . . . 4.2.1–39 MOTn. . . . . . . . . 4.2.1–39 MSFLDCRT . . . . 4.2.1–23 MSTRN . . . . . . . 4.2.1–13 MSTRS. . . . . . . . 4.2.1–13 NCURS . . . . . . . 4.2.1–29 NE . . . . . . . . . . . 4.2.1–7 NEij . . . . . . . . . . 4.2.1–7 NEP . . . . . . . . . . 4.2.1–8 NEPn . . . . . . . . . 4.2.1–8 NFLn . . . . . . . . . 4.2.1–29 NFLUX. . . . . . . . 4.2.1–29 NFORC . . . . . . . 4.2.1–28 NFORCSO . . . . . 4.2.1–29 NNC. . . . . . . . . . 4.2.1–37 NNCn . . . . . . . . . 4.2.1–37 NT . . . . . . . . . . . 4.2.1–37 NTn . . . . . . . . . . 4.2.1–37 OPENBC . . . . . . 4.2.1–49 P . . . . . . . . . . . . 4.2.1–34 PCAV . . . . . . . . . 4.2.1–39 PE . . . . . . . . . . . 4.2.1–9 4.2.1–18 PEAVG . . . . . . . . 4.2.1–36 Variable Page Variable Page Variable Page PSij . . . . . . . . . . 4.2.1–18 PSILSM . . . . . . . 4.2.1–40 PTL . . . . . . . . . . 4.2.1–49 PTLA . . . . . . . . . 4.2.1–49 PTU . . . . . . . . . . 4.2.1–42 PTUn . . . . . . . . . 4.2.1–42 PTURn . . . . . . . . 4.2.1–42 PU . . . . . . . . . . . 4.2.1–40 PUn . . . . . . . . . . 4.2.1–41 PURn . . . . . . . . . 4.2.1–41 QUADECRT . . . . 4.2.1–16 QUADSCRT . . . . 4.2.1–16 RA . . . . . . . . . . . 4.2.1–43 RAD. . . . . . . . . . 4.2.1–29 RADFL. . . . . . . . 4.2.1–50 RADFLA . . . . . . 4.2.1–50 RADTL. . . . . . . . 4.2.1–50 RADTLA . . . . . . 4.2.1–50 RAn . . . . . . . . . . 4.2.1–43 RARn . . . . . . . . . 4.2.1–43 RATIO . . . . . . . . 4.2.1–56 RBANG . . . . . . . 4.2.1–15 RBFOR. . . . . . . . 4.2.1–15 RBROT . . . . . . . 4.2.1–15 RCCU. . . . . . . . . 4.2.1–20 RCCUn . . . . . . . . 4.2.1–20 RCCURn. . . . . . . 4.2.1–20 RCEF . . . . . . . . . 4.2.1–19 RCEFn . . . . . . . . 4.2.1–19 RCEMn . . . . . . . 4.2.1–19 RCHG . . . . . . . . 4.2.1–39 RCNF . . . . . . . . . 4.2.1–20 RCNFC. . . . . . . . 4.2.1–20 RCNFn . . . . . . . . 4.2.1–20 RCNMn . . . . . . . 4.2.1–20 RCRF . . . . . . . . . 4.2.1–19 RCRFn . . . . . . . . 4.2.1–19 RCRMn . . . . . . . 4.2.1–19 RCSF . . . . . . . . . 4.2.1–19 OI.1–5 RCSFC . . . . . . . . 4.2.1–20 RCSFn . . . . . . . . 4.2.1–19 RCSMn. . . . . . . . 4.2.1–20 RCTF . . . . . . . . . 4.2.1–19 RCTFn . . . . . . . . 4.2.1–19 RCTMn . . . . . . . 4.2.1–19 RCU . . . . . . . . . . 4.2.1–20 RCUn . . . . . . . . . 4.2.1–20 RCURn . . . . . . . . 4.2.1–20 RCVF . . . . . . . . . 4.2.1–19 RCVFn . . . . . . . . 4.2.1–19 RCVMn . . . . . . . 4.2.1–19 RD . . . . . . . . . . . 4.2.1–17 RE . . . . . . . . . . . 4.2.1–19 RECUR . . . . . . . 4.2.1–39 REij . . . . . . . . . . 4.2.1–19 RF . . . . . . . . . . . 4.2.1–37 RFL . . . . . . . . . . 4.2.1–40 RFLE . . . . . . . . . 4.2.1–40 RFLEn . . . . . . . . 4.2.1–40 RFLn . . . . . . . . . 4.2.1–40 RFn . . . . . . . . . . 4.2.1–38 RI. . . . . . . . . . . . 4.2.1–52 RIij. . . . . . . . . . . 4.2.1–53 RM. . . . . . . . . . . 4.2.1–38 RMISES . . . . . . . 4.2.1–19 RMn . . . . . . . . . . 4.2.1–38 ROTAMAG . . . . . 4.2.1–29 RRF . . . . . . . . . . 4.2.1–44 RRFn . . . . . . . . . 4.2.1–44 RRMn. . . . . . . . . 4.2.1–44 RS . . . . . . . . . . . 4.2.1–19 RSij . . . . . . . . . . 4.2.1–19 RT . . . . . . . . . . . 4.2.1–38 RTA . . . . . . . . . . 4.2.1–43 RTAn . . . . . . . . . 4.2.1–44 RTARn . . . . . . . . 4.2.1–44 RTU . . . . . . . . . . 4.2.1–43 RTUn . . . . . . . . . 4.2.1–43 PHCSFC . . . . . . . 4.2.1–22 PHCSFn . . . . . . . 4.2.1–22 PHCSMn. . . . . . . 4.2.1–22 PHCTF . . . . . . . . 4.2.1–21 PHCTFn . . . . . . . 4.2.1–21 PHCTMn . . . . . . 4.2.1–21 PHCU. . . . . . . . . 4.2.1–22 PHCUn . . . . . . . . 4.2.1–22 PHCURn. . . . . . . 4.2.1–22 PHCV. . . . . . . . . 4.2.1–22 PHCVF . . . . . . . . 4.2.1–21 PHCVFn . . . . . . . 4.2.1–21 PHCVMn . . . . . . 4.2.1–21 PHCVn . . . . . . . . 4.2.1–22 PHCVRn. . . . . . . 4.2.1–22 PHE . . . . . . . . . . 4.2.1–21 PHEFL . . . . . . . . 4.2.1–21 PHEFLn . . . . . . . 4.2.1–21 PHEij . . . . . . . . . 4.2.1–21 PHEPG . . . . . . . . 4.2.1–21 PHEPGn . . . . . . . 4.2.1–21 PHILSM . . . . . . . 4.2.1–40 PHMFL . . . . . . . 4.2.1–21 PHMFT . . . . . . . 4.2.1–21 PHPOT . . . . . . . . 4.2.1–41 PHS . . . . . . . . . . 4.2.1–20 PHSij . . . . . . . . . 4.2.1–20 PINF . . . . . . . . . 4.2.1–39 POR . . . . . . . . . . 4.2.1–17 4.2.1–37 4.2.1–39 PPOR . . . . . . . . . 4.2.1–41 PPRESS . . . . . . . 4.2.1–46 PRESS . . . . . . . . 4.2.1–7 PRESSONLY. . . . 4.2.1–7 PRF . . . . . . . . . . 4.2.1–41 PRFn . . . . . . . . . 4.2.1–41 PRMn . . . . . . . . . 4.2.1–41 Variable Page Variable Page Variable Page SFDRT . . . . . . . . 4.2.1–48 4.2.1–49 SFDRTA . . . . . . . 4.2.1–48 4.2.1–49 SFn . . . . . . . . . . 4.2.1–25 SHRCRT. . . . . . . 4.2.1–23 SHRRATIO . . . . . 4.2.1–23 Sij . . . . . . . . . . . 4.2.1–6 SINKTEMP. . . . . 4.2.1–34 SINV . . . . . . . . . 4.2.1–6 SJD . . . . . . . . . . 4.2.1–48 4.2.1–49 SJDA . . . . . . . . . 4.2.1–48 4.2.1–49 SJDT . . . . . . . . . 4.2.1–48 4.2.1–49 SJDTA . . . . . . . . 4.2.1–48 4.2.1–49 SJP. . . . . . . . . . . 4.2.1–18 SKEn . . . . . . . . . 4.2.1–26 SKn . . . . . . . . . . 4.2.1–25 SKPn . . . . . . . . . 4.2.1–27 SMn . . . . . . . . . . 4.2.1–25 SNE . . . . . . . . . . 4.2.1–45 SNEn . . . . . . . . . 4.2.1–45 SOAREA . . . . . . 4.2.1–50 SOCF . . . . . . . . . 4.2.1–51 SOD . . . . . . . . . . 4.2.1–51 SOE . . . . . . . . . . 4.2.1–51 SOF . . . . . . . . . . 4.2.1–51 SOH . . . . . . . . . . 4.2.1–51 SOL . . . . . . . . . . 4.2.1–54 SOM . . . . . . . . . 4.2.1–51 SOP . . . . . . . . . . 4.2.1–51 SP . . . . . . . . . . . 4.2.1–6 SPE . . . . . . . . . . 4.2.1–26 SPEn . . . . . . . . . 4.2.1–26 SPL . . . . . . . . . . 4.2.1–40 SPn . . . . . . . . . . 4.2.1–6 OI.1–6 SS . . . . . . . . . . . 4.2.1–11 SSAVG . . . . . . . . 4.2.1–25 SSAVGn . . . . . . . 4.2.1–25 SSn . . . . . . . . . . 4.2.1–11 STATUS . . . . . . . 4.2.1–16 4.2.1–17 4.2.1–24 STATUSXFEM . . 4.2.1–30 STH . . . . . . . . . . 4.2.1–25 STRAINFREE . . . 4.2.1–39 SVOL . . . . . . . . . 4.2.1–26 T . . . . . . . . . . . . 4.2.1–45 TA . . . . . . . . . . . 4.2.1–42 TAn . . . . . . . . . . 4.2.1–42 TARn . . . . . . . . . 4.2.1–42 TEMP. . . . . . . . . 4.2.1–13 TF . . . . . . . . . . . 4.2.1–38 TFn . . . . . . . . . . 4.2.1–38 THE . . . . . . . . . . 4.2.1–9 THEij . . . . . . . . . 4.2.1–9 THEP . . . . . . . . . 4.2.1–9 THEPn . . . . . . . . 4.2.1–9 TMn . . . . . . . . . . 4.2.1–38 Tn . . . . . . . . . . . 4.2.1–45 TPFL . . . . . . . . . 4.2.1–49 TPTL . . . . . . . . . 4.2.1–49 TRESC . . . . . . . . 4.2.1–7 TRIAX . . . . . . . . 4.2.1–7 TRNOR . . . . . . . 4.2.1–34 TRSHR . . . . . . . . 4.2.1–34 TSAIH . . . . . . . . 4.2.1–13 TSAIW . . . . . . . . 4.2.1–13 TSHR . . . . . . . . . 4.2.1–11 TSHRi3 . . . . . . . 4.2.1–11 TU . . . . . . . . . . . 4.2.1–41 TUn . . . . . . . . . . 4.2.1–41 TURn . . . . . . . . . 4.2.1–41 TV . . . . . . . . . . . 4.2.1–41 TVn . . . . . . . . . . 4.2.1–41 RTURn . . . . . . . . 4.2.1–43 RTV . . . . . . . . . . 4.2.1–43 RTVn . . . . . . . . . 4.2.1–43 RTVRn . . . . . . . . 4.2.1–43 RU . . . . . . . . . . . 4.2.1–42 RUn . . . . . . . . . . 4.2.1–43 RURn . . . . . . . . . 4.2.1–43 RV . . . . . . . . . . . 4.2.1–43 RVF . . . . . . . . . . 4.2.1–42 RVn . . . . . . . . . . 4.2.1–43 RVRn . . . . . . . . . 4.2.1–43 RVT . . . . . . . . . . 4.2.1–42 RWM . . . . . . . . . 4.2.1–38 S . . . . . . . . . . . . 4.2.1–6 SALPHA. . . . . . . 4.2.1–27 SALPHAn . . . . . . 4.2.1–27 SAT . . . . . . . . . . 4.2.1–17 SDEG . . . . . . . . . 4.2.1–15 4.2.1–16 4.2.1–17 4.2.1–23 SDV . . . . . . . . . . 4.2.1–13 4.2.1–46 SDVn . . . . . . . . . 4.2.1–13 SE . . . . . . . . . . . 4.2.1–25 SEE . . . . . . . . . . 4.2.1–26 SEE1 . . . . . . . . . 4.2.1–26 SEn . . . . . . . . . . 4.2.1–25 SENER . . . . . . . . 4.2.1–12 SEP . . . . . . . . . . 4.2.1–26 SEP1 . . . . . . . . . 4.2.1–27 SEPE . . . . . . . . . 4.2.1–26 SEPEn . . . . . . . . 4.2.1–26 SF . . . . . . . . . . . 4.2.1–25 SFDR . . . . . . . . . 4.2.1–48 4.2.1–49 SFDRA . . . . . . . . 4.2.1–48 Variable Page Variable Page Variable Page TVRn . . . . . . . . . 4.2.1–41 U . . . . . . . . . . . . 4.2.1–36 UC . . . . . . . . . . . 4.2.1–52 UCn . . . . . . . . . . 4.2.1–52 Un . . . . . . . . . . . 4.2.1–36 UR . . . . . . . . . . . 4.2.1–36 URCn . . . . . . . . . 4.2.1–52 URn . . . . . . . . . . 4.2.1–36 UT . . . . . . . . . . . 4.2.1–36 UVARM . . . . . . . 4.2.1–13 UVARMn . . . . . . 4.2.1–13 V . . . . . . . . . . . . 4.2.1–37 VC . . . . . . . . . . . 4.2.1–52 VCn . . . . . . . . . . 4.2.1–52 VE . . . . . . . . . . . 4.2.1–18 VEEQ. . . . . . . . . 4.2.1–18 VEij . . . . . . . . . . 4.2.1–18 VENER. . . . . . . . 4.2.1–13 VF . . . . . . . . . . . 4.2.1–38 VFn . . . . . . . . . . 4.2.1–38 VFTOT . . . . . . . . 4.2.1–50 VMn. . . . . . . . . . 4.2.1–38 Vn . . . . . . . . . . . 4.2.1–37 VOIDR . . . . . . . . 4.2.1–17 VOL . . . . . . . . . . 4.2.1–53 VOLC. . . . . . . . . 4.2.1–51 VR . . . . . . . . . . . 4.2.1–37 VRCn . . . . . . . . . 4.2.1–52 VRn . . . . . . . . . . 4.2.1–37 VS . . . . . . . . . . . 4.2.1–17 VSij . . . . . . . . . . 4.2.1–17 VT . . . . . . . . . . . 4.2.1–37 VVF . . . . . . . . . . 4.2.1–17 VVFG. . . . . . . . . 4.2.1–17 VVFN. . . . . . . . . 4.2.1–17 WARP . . . . . . . . 4.2.1–37 WEIGHT . . . . . . 4.2.1–48 4.2.1–49 XC . . . . . . . . . . . 4.2.1–52 XCn . . . . . . . . . . 4.2.1–52 XN . . . . . . . . . . . 4.2.1–47 XS . . . . . . . . . . . 4.2.1–47 XT . . . . . . . . . . . 4.2.1–47 OI.2 Abaqus/Explicit OUTPUT VARIABLE INDEX This index provides a reference to all of the output variables that are available in Abaqus/Explicit. Output variables are listed in alphabetical order. Variable Page Variable Page Variable Page BF . . . . . . . . . . . 4.2.2–14 BONDLOAD. . . . 4.2.2–23 BONDSTAT . . . . 4.2.2–23 BURNF . . . . . . . 4.2.2–10 CA . . . . . . . . . . . 4.2.2–19 CALPHAF . . . . . 4.2.2–16 CALPHAFn. . . . . 4.2.2–16 CALPHAMn . . . . 4.2.2–16 CAn . . . . . . . . . . 4.2.2–19 CAREA . . . . . . . 4.2.2–24 CARn . . . . . . . . . 4.2.2–19 CASU. . . . . . . . . 4.2.2–17 CASUC . . . . . . . 4.2.2–18 CASUn . . . . . . . . 4.2.2–18 CASURn. . . . . . . 4.2.2–18 CBLARAT . . . . . 4.2.2–22 CCF . . . . . . . . . . 4.2.2–18 CCFn . . . . . . . . . 4.2.2–18 CCMn. . . . . . . . . 4.2.2–18 CCU . . . . . . . . . . 4.2.2–18 CCUn . . . . . . . . . 4.2.2–18 CCURn . . . . . . . . 4.2.2–18 CDERF . . . . . . . . 4.2.2–19 CDERU . . . . . . . 4.2.2–19 CDIF . . . . . . . . . 4.2.2–17 CDIFC . . . . . . . . 4.2.2–17 CDIFn . . . . . . . . 4.2.2–17 CDIFRn . . . . . . . 4.2.2–17 CDIM . . . . . . . . . 4.2.2–17 CDIMC. . . . . . . . 4.2.2–17 CDIMn . . . . . . . . 4.2.2–17 CDIMRn . . . . . . . 4.2.2–17 CDIP . . . . . . . . . 4.2.2–17 CDIPC . . . . . . . . 4.2.2–17 OI.2–1 CDIPn . . . . . . . . 4.2.2–17 CDIPRn . . . . . . . 4.2.2–17 CDMG . . . . . . . . 4.2.2–17 CDMGn . . . . . . . 4.2.2–17 CDMGRn . . . . . . 4.2.2–17 CEF . . . . . . . . . . 4.2.2–15 CEFL . . . . . . . . . 4.2.2–22 CEFLT . . . . . . . . 4.2.2–22 CEFn . . . . . . . . . 4.2.2–15 CEMn. . . . . . . . . 4.2.2–15 CENER. . . . . . . . 4.2.2–7 CF . . . . . . . . . . . 4.2.2–21 CFAILST . . . . . . 4.2.2–19 CFAILSTi . . . . . . 4.2.2–19 CFAILURE . . . . . 4.2.2–7 CFn . . . . . . . . . . 4.2.2–21 CFN . . . . . . . . . . 4.2.2–24 CFNM . . . . . . . . 4.2.2–24 CFORCE. . . . . . . 4.2.2–23 CFS . . . . . . . . . . 4.2.2–24 CFSM. . . . . . . . . 4.2.2–24 CFT . . . . . . . . . . 4.2.2–24 CFTM. . . . . . . . . 4.2.2–24 CIVC . . . . . . . . . 4.2.2–18 CKE . . . . . . . . . . 4.2.2–9 CKEij . . . . . . . . . 4.2.2–9 CKEMAG . . . . . . 4.2.2–9 CKLE . . . . . . . . . 4.2.2–9 CKLEij . . . . . . . . 4.2.2–9 CKLS . . . . . . . . . 4.2.2–9 CKLSij . . . . . . . . 4.2.2–9 CKSTAT . . . . . . . 4.2.2–9 CLAREA . . . . . . 4.2.2–22 CMASS . . . . . . . 4.2.2–22 A . . . . . . . . . . . . 4.2.2–20 ACOM . . . . . . . . 4.2.2–26 ACTEMP . . . . . . 4.2.2–22 ALLAE. . . . . . . . 4.2.2–26 ALLCD. . . . . . . . 4.2.2–26 ALLCW . . . . . . . 4.2.2–27 ALLDC. . . . . . . . 4.2.2–27 ALLDMD . . . . . . 4.2.2–27 ALLFC . . . . . . . . 4.2.2–27 ALLFD . . . . . . . . 4.2.2–26 ALLHF . . . . . . . . 4.2.2–27 ALLIE . . . . . . . . 4.2.2–26 ALLIHE . . . . . . . 4.2.2–27 ALLKE. . . . . . . . 4.2.2–26 ALLMW . . . . . . . 4.2.2–27 ALLPD . . . . . . . . 4.2.2–27 ALLPW . . . . . . . 4.2.2–27 ALLSE . . . . . . . . 4.2.2–27 ALLVD. . . . . . . . 4.2.2–27 ALLWK . . . . . . . 4.2.2–27 ALPHA. . . . . . . . 4.2.2–4 ALPHAij. . . . . . . 4.2.2–4 ALPHAk . . . . . . . 4.2.2–5 ALPHAk_ij . . . . . 4.2.2–5 ALPHAN . . . . . . 4.2.2–5 ALPHAP. . . . . . . 4.2.2–5 ALPHAPn . . . . . . 4.2.2–5 An . . . . . . . . . . . 4.2.2–20 APCAV. . . . . . . . 4.2.2–22 AR . . . . . . . . . . . 4.2.2–20 ARn . . . . . . . . . . 4.2.2–20 AT . . . . . . . . . . . 4.2.2–20 AZZIT . . . . . . . . 4.2.2–8 Variable Page Variable Page Variable Page CSTRESS . . . . . . 4.2.2–23 CTEMP . . . . . . . 4.2.2–22 CTF . . . . . . . . . . 4.2.2–15 CTFn . . . . . . . . . 4.2.2–15 CTHICK . . . . . . . 4.2.2–23 CTMn. . . . . . . . . 4.2.2–15 CU . . . . . . . . . . . 4.2.2–18 CUE . . . . . . . . . . 4.2.2–15 CUEn . . . . . . . . . 4.2.2–15 CUF . . . . . . . . . . 4.2.2–16 CUFn . . . . . . . . . 4.2.2–16 CUMn . . . . . . . . 4.2.2–16 CUn . . . . . . . . . . 4.2.2–18 CUP . . . . . . . . . . 4.2.2–15 CUPEQ. . . . . . . . 4.2.2–15 CUPEQC . . . . . . 4.2.2–16 CUPEQn . . . . . . . 4.2.2–16 CUPn . . . . . . . . . 4.2.2–15 CUREn . . . . . . . . 4.2.2–15 CURn . . . . . . . . . 4.2.2–18 CURPEQn. . . . . . 4.2.2–16 CURPn . . . . . . . . 4.2.2–15 CV . . . . . . . . . . . 4.2.2–18 CVF . . . . . . . . . . 4.2.2–16 CVFn . . . . . . . . . 4.2.2–16 CVMn . . . . . . . . 4.2.2–16 CVn . . . . . . . . . . 4.2.2–18 CVOL. . . . . . . . . 4.2.2–21 CVRn . . . . . . . . . 4.2.2–18 DAMAGEC. . . . . 4.2.2–8 DAMAGEFC. . . . 4.2.2–10 DAMAGEFT . . . . 4.2.2–10 DAMAGEMC . . . 4.2.2–10 DAMAGEMT . . . 4.2.2–10 DAMAGESHR . . 4.2.2–10 DAMAGET. . . . . 4.2.2–8 DBS . . . . . . . . . . 4.2.2–23 DBSF . . . . . . . . . 4.2.2–23 DBT . . . . . . . . . . 4.2.2–23 OI.2–2 DBURNF . . . . . . 4.2.2–10 DENSITY . . . . . . 4.2.2–7 DENSITYVAVG . 4.2.2–11 DMASS . . . . . . . 4.2.2–26 4.2.2–27 DMENER . . . . . . 4.2.2–7 DMICRT. . . . . . . 4.2.2–9 4.2.2–11 DMICRTMAX. . . 4.2.2–6 DT . . . . . . . . . . . 4.2.2–27 DUCTCRT . . . . . 4.2.2–9 E . . . . . . . . . . . . 4.2.2–4 EASEDEN . . . . . 4.2.2–13 ECDDEN . . . . . . 4.2.2–13 EDCDEN . . . . . . 4.2.2–14 EDMDDEN. . . . . 4.2.2–14 EDMICRTMAX. . 4.2.2–14 EDT . . . . . . . . . . 4.2.2–14 EFABRIC . . . . . . 4.2.2–10 EFABRICij . . . . . 4.2.2–10 EFENRRTR. . . . . 4.2.2–24 EIHEDEN . . . . . . 4.2.2–13 Eij . . . . . . . . . . . 4.2.2–4 ELASE . . . . . . . . 4.2.2–13 ELCD . . . . . . . . . 4.2.2–13 ELDC . . . . . . . . . 4.2.2–13 ELDMD . . . . . . . 4.2.2–13 ELEDEN. . . . . . . 4.2.2–13 ELEN . . . . . . . . . 4.2.2–13 ELIHE . . . . . . . . 4.2.2–13 ELPD . . . . . . . . . 4.2.2–13 ELSE . . . . . . . . . 4.2.2–13 ELVD . . . . . . . . . 4.2.2–13 EMSF . . . . . . . . . 4.2.2–14 ENER . . . . . . . . . 4.2.2–7 ENRRT . . . . . . . . 4.2.2–24 EPDDEN . . . . . . 4.2.2–13 ER . . . . . . . . . . . 4.2.2–4 ERij . . . . . . . . . . 4.2.2–4 CMF. . . . . . . . . . 4.2.2–22 CMFL. . . . . . . . . 4.2.2–22 CMFLT. . . . . . . . 4.2.2–22 CMn . . . . . . . . . . 4.2.2–21 CMN . . . . . . . . . 4.2.2–24 CMNM . . . . . . . . 4.2.2–24 CMS. . . . . . . . . . 4.2.2–24 CMSM . . . . . . . . 4.2.2–24 CMT . . . . . . . . . 4.2.2–24 CMTM . . . . . . . . 4.2.2–24 CNF . . . . . . . . . . 4.2.2–16 CNFC . . . . . . . . . 4.2.2–17 CNFn . . . . . . . . . 4.2.2–16 CNMn . . . . . . . . 4.2.2–16 COORD . . . . . . . 4.2.2–6 4.2.2–11 4.2.2–20 COORDCOM . . . 4.2.2–26 COORn. . . . . . . . 4.2.2–20 CP . . . . . . . . . . . 4.2.2–18 CPn . . . . . . . . . . 4.2.2–18 CPRn . . . . . . . . . 4.2.2–18 CRACK . . . . . . . 4.2.2–9 CRF . . . . . . . . . . 4.2.2–18 CRFn . . . . . . . . . 4.2.2–18 CRMn. . . . . . . . . 4.2.2–18 CRSTS . . . . . . . . 4.2.2–24 CSAREA . . . . . . 4.2.2–22 CSDMG . . . . . . . 4.2.2–23 CSF . . . . . . . . . . 4.2.2–16 CSFC . . . . . . . . . 4.2.2–16 CSFn . . . . . . . . . 4.2.2–16 CSLST . . . . . . . . 4.2.2–17 CSLSTi. . . . . . . . 4.2.2–17 CSMAXSCRT . . . 4.2.2–23 CSMAXUCRT. . . 4.2.2–23 CSMn . . . . . . . . . 4.2.2–16 CSQUADSCRT . . 4.2.2–23 Variable Page Variable Page Variable Page MINFLT . . . . . . . 4.2.2–22 MISES . . . . . . . . 4.2.2–4 MISESMAX . . . . 4.2.2–3 MISESVAVG. . . . 4.2.2–11 MKCRT . . . . . . . 4.2.2–9 MSFLDCRT . . . . 4.2.2–9 MSTRN . . . . . . . 4.2.2–8 MSTRS. . . . . . . . 4.2.2–7 NE . . . . . . . . . . . 4.2.2–4 NEij . . . . . . . . . . 4.2.2–4 NEP . . . . . . . . . . 4.2.2–4 NEPn . . . . . . . . . 4.2.2–4 NFORC . . . . . . . 4.2.2–14 NT . . . . . . . . . . . 4.2.2–21 NTn . . . . . . . . . . 4.2.2–21 NVF . . . . . . . . . . 4.2.2–21 OPENBC . . . . . . 4.2.2–24 P . . . . . . . . . . . . 4.2.2–19 PABS . . . . . . . . . 4.2.2–21 PALPH . . . . . . . . 4.2.2–10 PALPHMIN. . . . . 4.2.2–10 PCAV . . . . . . . . . 4.2.2–21 PE . . . . . . . . . . . 4.2.2–4 PEEQ . . . . . . . . . 4.2.2–5 4.2.2–8 PEEQMAX . . . . . 4.2.2–5 PEEQT . . . . . . . . 4.2.2–5 PEEQVAVG . . . . 4.2.2–11 PEij . . . . . . . . . . 4.2.2–4 PENER . . . . . . . . 4.2.2–7 PEP . . . . . . . . . . 4.2.2–4 PEPn . . . . . . . . . 4.2.2–4 PEQC . . . . . . . . . 4.2.2–8 PEQCn . . . . . . . . 4.2.2–8 PEVAVG . . . . . . . 4.2.2–11 POR . . . . . . . . . . 4.2.2–20 PRESS . . . . . . . . 4.2.2–4 PRESSVAVG. . . . 4.2.2–12 QUADECRT . . . . 4.2.2–11 OI.2–3 QUADSCRT . . . . 4.2.2–11 RBANG . . . . . . . 4.2.2–10 RBFOR. . . . . . . . 4.2.2–10 RBROT . . . . . . . 4.2.2–11 RF . . . . . . . . . . . 4.2.2–21 RFL . . . . . . . . . . 4.2.2–21 RFLn . . . . . . . . . 4.2.2–21 RFn . . . . . . . . . . 4.2.2–21 RHOE. . . . . . . . . 4.2.2–10 RHOP. . . . . . . . . 4.2.2–10 RM. . . . . . . . . . . 4.2.2–21 RMn . . . . . . . . . . 4.2.2–21 RT . . . . . . . . . . . 4.2.2–21 S . . . . . . . . . . . . 4.2.2–3 SBF . . . . . . . . . . 4.2.2–14 SDEG . . . . . . . . . 4.2.2–8 4.2.2–9 4.2.2–11 SDV . . . . . . . . . . 4.2.2–7 SDVn . . . . . . . . . 4.2.2–7 SE . . . . . . . . . . . 4.2.2–12 SEn . . . . . . . . . . 4.2.2–12 SENER . . . . . . . . 4.2.2–7 SF . . . . . . . . . . . 4.2.2–12 SFABRIC . . . . . . 4.2.2–10 SFABRICij . . . . . 4.2.2–10 SFDR . . . . . . . . . 4.2.2–25 SFDRA . . . . . . . . 4.2.2–25 SFDRT . . . . . . . . 4.2.2–25 SFDRTA . . . . . . . 4.2.2–25 SFn . . . . . . . . . . 4.2.2–12 SHRCRT. . . . . . . 4.2.2–9 SHRRATIO . . . . . 4.2.2–9 Sij . . . . . . . . . . . 4.2.2–3 SKn . . . . . . . . . . 4.2.2–12 SMn . . . . . . . . . . 4.2.2–12 SOAREA . . . . . . 4.2.2–25 SOF . . . . . . . . . . 4.2.2–25 SOM . . . . . . . . . 4.2.2–25 ERP . . . . . . . . . . 4.2.2–4 ERPn . . . . . . . . . 4.2.2–4 ERPRATIO . . . . . 4.2.2–9 ERV . . . . . . . . . . 4.2.2–4 ESEDEN. . . . . . . 4.2.2–13 ETOTAL . . . . . . . 4.2.2–27 EVDDEN . . . . . . 4.2.2–13 EVF . . . . . . . . . . 4.2.2–11 EVOL. . . . . . . . . 4.2.2–14 FLDCRT . . . . . . . 4.2.2–9 FLSDCRT . . . . . . 4.2.2–9 FSLIP . . . . . . . . . 4.2.2–23 FSLIPR. . . . . . . . 4.2.2–23 FV . . . . . . . . . . . 4.2.2–7 FVn . . . . . . . . . . 4.2.2–7 GRAV. . . . . . . . . 4.2.2–14 HFL . . . . . . . . . . 4.2.2–11 4.2.2–25 HFLA . . . . . . . . . 4.2.2–25 HFLM . . . . . . . . 4.2.2–11 HFLn . . . . . . . . . 4.2.2–11 HSNFCCRT . . . . 4.2.2–10 HSNFTCRT. . . . . 4.2.2–10 HSNMCCRT . . . . 4.2.2–10 HSNMTCRT . . . . 4.2.2–10 HTL . . . . . . . . . . 4.2.2–25 HTLA. . . . . . . . . 4.2.2–25 IWCONWEP . . . . 4.2.2–19 JCCRT . . . . . . . . 4.2.2–9 LE . . . . . . . . . . . 4.2.2–4 LEij . . . . . . . . . . 4.2.2–4 LEP . . . . . . . . . . 4.2.2–4 LEPn . . . . . . . . . 4.2.2–4 LOCALDIRn . . . . 4.2.2–7 MASS. . . . . . . . . 4.2.2–26 MASSEUL . . . . . 4.2.2–26 MAXECRT . . . . . 4.2.2–11 MAXSCRT . . . . . 4.2.2–11 Variable Page Variable Page Variable Page SP . . . . . . . . . . . 4.2.2–3 SPn . . . . . . . . . . 4.2.2–4 SSAVG . . . . . . . . 4.2.2–12 SSAVGn . . . . . . . 4.2.2–12 SSFORC . . . . . . . 4.2.2–28 SSFORCn . . . . . . 4.2.2–28 SSPEEQ . . . . . . . 4.2.2–27 SSPEEQn . . . . . . 4.2.2–28 SSSPRD . . . . . . . 4.2.2–28 SSSPRDn . . . . . . 4.2.2–28 SSTORQ . . . . . . . 4.2.2–28 SSTORQn . . . . . . 4.2.2–28 STAGP . . . . . . . . 4.2.2–19 STATUS . . . . . . . 4.2.2–11 4.2.2–14 STH . . . . . . . . . . 4.2.2–12 SVAVG . . . . . . . . 4.2.2–12 TCMASS . . . . . . 4.2.2–22 TCSAREA . . . . . 4.2.2–22 TCVOL. . . . . . . . 4.2.2–22 TEMP. . . . . . . . . 4.2.2–7 TEMPMAVG. . . . 4.2.2–12 TIEADJUST . . . . 4.2.2–21 TIEDSTATUS . . . 4.2.2–21 TINFL . . . . . . . . 4.2.2–22 TRIAX . . . . . . . . 4.2.2–4 TRNOR . . . . . . . 4.2.2–19 TRSHR . . . . . . . . 4.2.2–19 TSAIH . . . . . . . . 4.2.2–8 TSAIW . . . . . . . . 4.2.2–8 TSHR . . . . . . . . . 4.2.2–7 TSHR13 . . . . . . . 4.2.2–7 TSHR23 . . . . . . . 4.2.2–7 U . . . . . . . . . . . . 4.2.2–20 UCOM . . . . . . . . 4.2.2–26 Un . . . . . . . . . . . 4.2.2–20 UR . . . . . . . . . . . 4.2.2–20 URn . . . . . . . . . . 4.2.2–20 UT . . . . . . . . . . . 4.2.2–20 V . . . . . . . . . . . . 4.2.2–20 VCOM . . . . . . . . 4.2.2–26 VENER. . . . . . . . 4.2.2–7 Vn . . . . . . . . . . . 4.2.2–20 VOLEUL . . . . . . 4.2.2–26 VP . . . . . . . . . . . 4.2.2–19 VR . . . . . . . . . . . 4.2.2–20 VRn . . . . . . . . . . 4.2.2–20 VT . . . . . . . . . . . 4.2.2–20 VVF . . . . . . . . . . 4.2.2–8 VVFG. . . . . . . . . 4.2.2–8 VVFN. . . . . . . . . 4.2.2–8 XN . . . . . . . . . . . 4.2.2–24 XS . . . . . . . . . . . 4.2.2–24 XT . . . . . . . . . . . 4.2.2–24 OI.3 Abaqus/CFD OUTPUT VARIABLE INDEX This index provides a reference to all of the output variables that are available in Abaqus/CFD. Output variables are listed in alphabetical order. Variable Page Variable Page Variable Page ALLKE. . . . . . . . 4.2.3–5 AVGPRESS . . . . . 4.2.3–4 AVGTEMP . . . . . 4.2.3–4 AVGVEL . . . . . . 4.2.3–4 COORD . . . . . . . 4.2.3–2 4.2.3–3 COORn. . . . . . . . 4.2.3–3 DENSITY . . . . . . 4.2.3–2 4.2.3–3 DIST . . . . . . . . . 4.2.3–2 4.2.3–3 DIV . . . . . . . . . . 4.2.3–2 4.2.3–3 ENSTROPHY . . . 4.2.3–2 4.2.3–3 EVOL. . . . . . . . . 4.2.3–2 FORCE . . . . . . . . 4.2.3–4 HEATFLOW . . . . 4.2.3–4 HELICITY . . . . . 4.2.3–2 4.2.3–3 HFL . . . . . . . . . . 4.2.3–4 HFLN . . . . . . . . . 4.2.3–4 MASSFLOW . . . . 4.2.3–4 NTRACTION . . . 4.2.3–4 PRESSFORCE. . . 4.2.3–4 PRESSURE . . . . . 4.2.3–2 4.2.3–3 SHEARRATE . . . 4.2.3–2 4.2.3–3 STRACTION. . . . 4.2.3–4 SURFAREA . . . . 4.2.3–4 TEMP. . . . . . . . . 4.2.3–2 4.2.3–3 TRACTION. . . . . 4.2.3–4 TURBEPS . . . . . . 4.2.3–2 4.2.3–3 TURBKE . . . . . . 4.2.3–3 4.2.3–4 TURBNU . . . . . . 4.2.3–3 4.2.3–4 U . . . . . . . . . . . . 4.2.3–3 Un . . . . . . . . . . . 4.2.3–3 V . . . . . . . . . . . . 4.2.3–2 4.2.3–3 VGINV2 . . . . . . . 4.2.3–2 4.2.3–3 VISCFORCE . . . . 4.2.3–4 VISCOSITY . . . . 4.2.3–2 Vn . . . . . . . . . . . 4.2.3–3 VOL . . . . . . . . . . 4.2.3–5 VOLFLOW . . . . . 4.2.3–4 VORTICITY . . . . 4.2.3–2 4.2.3–3 VORTICITYn . . . 4.2.3–3 WALLSHEAR . . . 4.2.3–4 YPLUS . . . . . . . . 4.2.3–5 YSTAR . . . . . . . . 4.2.3–5 SIMULIA is the Dassault Systèmes brand that delivers a scalable portfolio of Realistic Simulation solutions including the Abaqus product suite for Unified Finite Element Analysis; multiphysics solutions for insight into challenging engineering problems; and lifecycle management solutions for managing simulation data, processes, and intellectual property. By building on established technology, respected quality, and superior customer service, SIMULIA makes realistic simulation an integral business practice that improves product performance, reduces physical prototypes, and drives innovation. Headquartered in Providence, RI, USA, with R&D centers in Providence and in Vélizy, France, SIMULIA provides sales, services, and support through a global network of regional offices and distributors. For more information, visit www.simulia.com. About Dassault Systèmes As a world leader in 3D and Product Lifecycle Management (PLM) solutions, Dassault Systèmes brings value to more than 100,000 customers in 80 countries. A pioneer in the 3D software market since 1981, Dassault Systèmes develops and markets PLM application software and services that support industrial processes and provide a 3D vision of the entire lifecycle of products from conception to maintenance to recycling. The Dassault Systèmes portfolio consists of CATIA for designing the virtual product, SolidWorks for 3D mechanical design, DELMIA for virtual production, SIMULIA for virtual testing, ENOVIA for global collaborative lifecycle management, and 3DVIA for online 3D lifelike experiences. Dassault Systèmes’ shares are listed on Euronext Paris (#13065, DSY.PA), and Dassault Systèmes’ ADRs may be traded on the US Over-The-Counter (OTC) market (DASTY). For more information, visit www.3ds.com. fi , , , , , , , , . . , © . , , . / User’s Manual CAUTION: This documentation is intended for qualified users who will exercise sound engineering judgment and expertise in the use of the Abaqus Software. The Abaqus Software is inherently complex, and the examples and procedures in this documentation are not intended to be exhaustive or to apply to any particular situation. Users are cautioned to satisfy themselves as to the accuracy and results of their analyses. Dassault Systèmes and its subsidiaries, including Dassault Systèmes Simulia Corp., shall not be responsible for the accuracy or usefulness of any analysis performed using the Abaqus Software or the procedures, examples, or explanations in this documentation. Dassault Systèmes and its subsidiaries shall not be responsible for the consequences of any errors or omissions that may appear in this documentation. The Abaqus Software is available only under license from Dassault Systèmes or its subsidiary and may be used or reproduced only in accordance with the terms of such license. This documentation is subject to the terms and conditions of either the software license agreement signed by the parties, or, absent such an agreement, the then current software license agreement to which the documentation relates. This documentation and the software described in this documentation are subject to change without prior notice. No part of this documentation may be reproduced or distributed in any form without prior written permission of Dassault Systèmes or its subsidiary. The Abaqus Software is a product of Dassault Systèmes Simulia Corp., Providence, RI, USA. © Dassault Systèmes, 2012 Abaqus, the 3DS logo, SIMULIA, CATIA, and Unified FEA are trademarks or registered trademarks of Dassault Systèmes or its subsidiaries in the United States and/or other countries. Other company, product, and service names may be trademarks or service marks of their respective owners. For additional information concerning SIMULIA European Headquarters Fax: +1 401 276 4408, simulia.support@3ds.com, http://www.simulia.com Stationsplein 8-K, 6221 BT Maastricht, The Netherlands, Tel: +31 43 7999 084, Fax: +31 43 7999 306, simulia.europe.info@3ds.com Locations United States Australia Austria Benelux Canada China Finland France Germany India Italy Japan Korea Latin America Scandinavia United Kingdom Argentina Brazil Czech & Slovak Republics Greece Israel Malaysia Mexico New Zealand Poland Russia, Belarus & Ukraine Singapore South Africa Spain & Portugal Dassault Systèmes’ Centers of Simulation Excellence Fremont, CA, Tel: +1 510 794 5891, simulia.west.support@3ds.com West Lafayette, IN, Tel: +1 765 497 1373, simulia.central.support@3ds.com Northville, MI, Tel: +1 248 349 4669, simulia.greatlakes.info@3ds.com Woodbury, MN, Tel: +1 612 424 9044, simulia.central.support@3ds.com Mayfield Heights, OH, Tel: +1 216 378 1070, simulia.erie.info@3ds.com Mason, OH, Tel: +1 513 275 1430, simulia.central.support@3ds.com Warwick, RI, Tel: +1 401 739 3637, simulia.east.support@3ds.com Lewisville, TX, Tel: +1 972 221 6500, simulia.south.info@3ds.com Richmond VIC, Tel: +61 3 9421 2900, simulia.au.support@3ds.com Vienna, Tel: +43 1 22 707 200, simulia.at.info@3ds.com Maarssen, The Netherlands, Tel: +31 346 585 710, simulia.benelux.support@3ds.com Toronto, ON, Tel: +1 416 402 2219, simulia.greatlakes.info@3ds.com Beijing, P. R. China, Tel: +8610 6536 2288, simulia.cn.support@3ds.com Shanghai, P. R. China, Tel: +8621 3856 8000, simulia.cn.support@3ds.com Espoo, Tel: +358 40 902 2973, simulia.nordic.info@3ds.com Velizy Villacoublay Cedex, Tel: +33 1 61 62 72 72, simulia.fr.support@3ds.com Aachen, Tel: +49 241 474 01 0, simulia.de.info@3ds.com Munich, Tel: +49 89 543 48 77 0, simulia.de.info@3ds.com Chennai, Tamil Nadu, Tel: +91 44 43443000, simulia.in.info@3ds.com Lainate MI, Tel: +39 02 3343061, simulia.ity.info@3ds.com Tokyo, Tel: +81 3 5442 6302, simulia.jp.support@3ds.com Osaka, Tel: +81 6 7730 2703, simulia.jp.support@3ds.com Mapo-Gu, Seoul, Tel: +82 2 785 6707/8, simulia.kr.info@3ds.com Puerto Madero, Buenos Aires, Tel: +54 11 4312 8700, Horacio.Burbridge@3ds.com Stockholm, Sweden, Tel: +46 8 68430450, simulia.nordic.info@3ds.com Warrington, Tel: +44 1925 830900, simulia.uk.info@3ds.com Authorized Support Centers SMARTtech Sudamerica SRL, Buenos Aires, Tel: +54 11 4717 2717 KB Engineering, Buenos Aires, Tel: +54 11 4326 7542 Solaer Ingeniería, Buenos Aires, Tel: +54 221 489 1738 SMARTtech Mecânica, Sao Paulo-SP, Tel: +55 11 3168 3388 Synerma s. r. o., Psáry, Prague-West, Tel: +420 603 145 769, abaqus@synerma.cz 3 Dimensional Data Systems, Crete, Tel: +30 2821040012, support@3dds.gr ADCOM, Givataim, Tel: +972 3 7325311, shmulik.keidar@adcomsim.co.il WorleyParsons Services Sdn. Bhd., Kuala Lumpur, Tel: +603 2039 9000, abaqus.my@worleyparsons.com Kimeca.NET SA de CV, Mexico, Tel: +52 55 2459 2635 Matrix Applied Computing Ltd., Auckland, Tel: +64 9 623 1223, abaqus-tech@matrix.co.nz BudSoft Sp. z o.o., Poznań, Tel: +48 61 8508 466, info@budsoft.com.pl TESIS Ltd., Moscow, Tel: +7 495 612 44 22, info@tesis.com.ru WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com Finite Element Analysis Services (Pty) Ltd., Parklands, Tel: +27 21 556 6462, feas@feas.co.za Thailand Turkey Simutech Solution Corporation, Taipei, R.O.C., Tel: +886 2 2507 9550, camilla@simutech.com.tw WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com A-Ztech Ltd., Istanbul, Tel: +90 216 361 8850, info@a-ztech.com.tr Preface Support Both technical engineering support (for problems with creating a model or performing an analysis) and systems support (for installation, licensing, and hardware-related problems) for Abaqus are offered through a network of local support offices. Regional contact information is listed in the front of each Abaqus manual and is accessible from the Locations page at www.simulia.com. Support for SIMULIA products SIMULIA provides a knowledge database of answers and solutions to questions that we have answered, as well as guidelines on how to use Abaqus, SIMULIA Scenario Definition, Isight, and other SIMULIA products. You can also submit new requests for support. All support incidents are tracked. If you contact us by means outside the system to discuss an existing support problem and you know the incident or support request number, please mention it so that we can query the database to see what the latest action has been. Many questions about Abaqus can also be answered by visiting the Products page and the Support page at www.simulia.com. Anonymous ftp site To facilitate data transfer with SIMULIA, an anonymous ftp account is available at ftp.simulia.com. Login as user anonymous, and type your e-mail address as your password. Contact support before placing files on the site. Training All offices and representatives offer regularly scheduled public training classes. The courses are offered in a traditional classroom form and via the Web. We also provide training seminars at customer sites. All training classes and seminars include workshops to provide as much practical experience with Abaqus as possible. For a schedule and descriptions of available classes, see www.simulia.com or call your local office or representative. Feedback We welcome any suggestions for improvements to Abaqus software, the support program, or documentation. We will ensure that any enhancement requests you make are considered for future releases. If you wish to make a suggestion about the service or products, refer to www.simulia.com. Complaints should be made by contacting your local office or through www.simulia.com by visiting the Quality Assurance section of the 1.1.1 1.2.1 1.2.2 1.3.1 1.4.1 2.1.1 2.1.2 2.1.3 2.1.4 2.1.5 2.1.6 2.2.1 2.2.2 2.2.3 2.2.4 2.2.5 2.3.1 2.3.2 2.3.3 2.3.4 Contents Volume I PART I INTRODUCTION, SPATIAL MODELING, AND EXECUTION 1. Introduction Introduction: general Abaqus syntax and conventions Input syntax rules Conventions Abaqus model definition Defining a model in Abaqus Parametric modeling Parametric input 2. Spatial Modeling Node definition Node definition Parametric shape variation Nodal thicknesses Normal definitions at nodes Transformed coordinate systems Adjusting nodal coordinates Element definition Element definition Element foundations Defining reinforcement Defining rebar as an element property Orientations Surface definition Surfaces: overview Element-based surface definition Node-based surface definition Analytical rigid surface definition Eulerian surface definition Operating on surfaces Rigid body definition Rigid body definition Integrated output section definition Integrated output section definition Mass adjustment Adjust and/or redistribute mass of an element set Nonstructural mass definition Nonstructural mass definition Distribution definition Distribution definition Display body definition Display body definition Assembly definition Defining an assembly Matrix definition Defining matrices 3. Job Execution Execution procedures: overview Execution procedure for Abaqus: overview Execution procedures Obtaining information Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution SIMULIA Co-Simulation Engine controller execution Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution Abaqus/CAE execution Abaqus/Viewer execution Python execution Parametric studies Abaqus documentation Licensing utilities ASCII translation of results (.fil) files Joining results (.fil) files Querying the keyword/problem database ii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 2.3.5 2.3.6 2.4.1 2.5.1 2.6.1 2.7.1 2.8.1 2.9.1 2.10.1 2.11.1 3.1.1 3.2.1 3.2.2 3.2.3 3.2.4 3.2.5 3.2.6 3.2.7 3.2.8 3.2.9 3.2.10 Making user-defined executables and subroutines Input file and output database upgrade utility Generating output database reports Joining output database (.odb) files from restarted analyses Combining output from substructures Combining data from multiple output databases Network output database file connector Mapping thermal and magnetic loads Fixed format conversion utility Translating Nastran bulk data files to Abaqus input files Translating Abaqus files to Nastran bulk data files Translating ANSYS input files to Abaqus input files Translating PAM-CRASH input files to partial Abaqus input files Translating RADIOSS input files to partial Abaqus input files Translating Abaqus output database files to Nastran Output2 results files Translating LS-DYNA data files to Abaqus input files Exchanging Abaqus data with ZAERO Encrypting and decrypting Abaqus input data Job execution control Environment file settings Using the Abaqus environment settings Managing memory and disk resources Managing memory and disk use in Abaqus Parallel execution Parallel execution: overview Parallel execution in Abaqus/Standard Parallel execution in Abaqus/Explicit Parallel execution in Abaqus/CFD File extension definitions File extensions used by Abaqus FORTRAN unit numbers FORTRAN unit numbers used by Abaqus CONTENTS 3.2.14 3.2.15 3.2.16 3.2.17 3.2.18 3.2.19 3.2.20 3.2.21 3.2.22 3.2.23 3.2.24 3.2.25 3.2.26 3.2.27 3.2.28 3.2.29 3.2.30 3.2.31 3.2.32 3.2.33 3.3.1 3.4.1 3.5.1 3.5.2 3.5.3 3.5.4 3.6.1 3.7.1 4.1.2 4.1.3 4.1.4 4.2.1 4.2.2 4.2.3 4.3.1 5.1.1 5.1.2 5.1.3 5.1.4 CONTENTS 4. Output PART II OUTPUT Output Output to the data and results files Output to the output database Error indicator output Output variables Abaqus/Standard output variable identifiers Abaqus/Explicit output variable identifiers Abaqus/CFD output variable identifiers The postprocessing calculator The postprocessing calculator 5. File Output Format Accessing the results file Accessing the results file: overview Results file output format Accessing the results file information Utility routines for accessing the results file OI.1 Abaqus/Standard Output Variable Index OI.2 Abaqus/Explicit Output Variable Index OI.3 Abaqus/CFD Output Variable Index 6.1.1 6.1.2 6.1.3 6.1.4 6.1.5 6.1.6 6.2.1 6.2.2 6.2.3 6.2.4 6.2.5 6.2.6 6.2.7 6.3.1 6.3.2 6.3.3 6.3.4 6.3.5 6.3.6 6.3.7 6.3.8 6.3.9 6.3.10 6.3.11 6.4.1 6.5.1 6.5.2 Volume II PART III ANALYSIS PROCEDURES, SOLUTION, AND CONTROL 6. Analysis Procedures Introduction Solving analysis problems: overview Defining an analysis General and linear perturbation procedures Multiple load case analysis Direct linear equation solver Iterative linear equation solver Static stress/displacement analysis Static stress analysis procedures: overview Static stress analysis Eigenvalue buckling prediction Unstable collapse and postbuckling analysis Quasi-static analysis Direct cyclic analysis Low-cycle fatigue analysis using the direct cyclic approach Dynamic stress/displacement analysis Dynamic analysis procedures: overview Implicit dynamic analysis using direct integration Explicit dynamic analysis Direct-solution steady-state dynamic analysis Natural frequency extraction Complex eigenvalue extraction Transient modal dynamic analysis Mode-based steady-state dynamic analysis Subspace-based steady-state dynamic analysis Response spectrum analysis Random response analysis Steady-state transport analysis Steady-state transport analysis Heat transfer and thermal-stress analysis Heat transfer analysis procedures: overview Uncoupled heat transfer analysis 6.5.4 6.6.1 6.6.2 6.7.1 6.7.2 6.7.3 6.7.4 6.7.5 6.7.6 6.8.1 6.8.2 6.9.1 6.10.1 6.11.1 6.12.1 7.1.1 7.2.1 7.2.2 7.2.3 7.2.4 CONTENTS Fully coupled thermal-stress analysis Adiabatic analysis Fluid dynamic analysis Fluid dynamic analysis procedures: overview Incompressible fluid dynamic analysis Electromagnetic analysis Electromagnetic analysis procedures Piezoelectric analysis Coupled thermal-electrical analysis Fully coupled thermal-electrical-structural analysis Eddy current analysis Magnetostatic analysis Coupled pore fluid flow and stress analysis Coupled pore fluid diffusion and stress analysis Geostatic stress state Mass diffusion analysis Mass diffusion analysis Acoustic and shock analysis Acoustic, shock, and coupled acoustic-structural analysis Abaqus/Aqua analysis Abaqus/Aqua analysis Annealing Annealing procedure 7. Analysis Solution and Control Solving nonlinear problems Solving nonlinear problems Analysis convergence controls Convergence and time integration criteria: overview Commonly used control parameters Convergence criteria for nonlinear problems Time integration accuracy in transient problems ANALYSIS TECHNIQUES 8. Analysis Techniques: Introduction Analysis techniques: overview 9. Analysis Continuation Techniques Restarting an analysis Restarting an analysis Importing and transferring results Transferring results between Abaqus analyses: overview Transferring results between Abaqus/Explicit and Abaqus/Standard Transferring results from one Abaqus/Standard analysis to another Transferring results from one Abaqus/Explicit analysis to another 10. Modeling Abstractions Substructuring Using substructures Defining substructures Submodeling Submodeling: overview Node-based submodeling Surface-based submodeling Generating global matrices Generating matrices CONTENTS 8.1.1 9.1.1 9.2.1 9.2.2 9.2.3 9.2.4 10.1.1 10.1.2 10.2.1 10.2.2 10.2.3 10.3.1 Symmetric model generation, results transfer, and analysis of cyclic symmetry models Symmetric model generation Transferring results from a symmetric mesh or a partial three-dimensional mesh to a full three-dimensional mesh Analysis of models that exhibit cyclic symmetry Periodic media analysis Periodic media analysis Meshed beam cross-sections Meshed beam cross-sections vii 10.4.1 10.4.2 10.4.3 10.5.1 Modeling discontinuities as an enriched feature using the extended finite element method Modeling discontinuities as an enriched feature using the extended finite element 10.7.1 11.1.1 11.2.1 11.3.1 11.4.1 11.4.2 11.4.3 11.5.1 11.5.2 11.5.3 11.5.4 11.6.1 11.7.1 11.8.1 12.1.1 12.2.1 12.2.2 12.2.3 12.2.4 method 11. Special-Purpose Techniques Inertia relief Inertia relief Mesh modification or replacement Element and contact pair removal and reactivation Geometric imperfections Introducing a geometric imperfection into a model Fracture mechanics Fracture mechanics: overview Contour integral evaluation Crack propagation analysis Surface-based fluid modeling Surface-based fluid cavities: overview Fluid cavity definition Fluid exchange definition Inflator definition Mass scaling Mass scaling Selective subcycling Selective subcycling Steady-state detection Steady-state detection 12. Adaptivity Techniques Adaptivity techniques: overview Adaptivity techniques ALE adaptive meshing ALE adaptive meshing: overview Defining ALE adaptive mesh domains in Abaqus/Explicit ALE adaptive meshing and remapping in Abaqus/Explicit Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit 12.2.5 12.2.6 12.2.7 12.3.1 12.3.2 12.3.3 12.4.1 13.1.1 13.2.1 13.2.2 13.2.3 14.1.1 14.1.2 14.1.3 14.1.4 15.1.1 15.1.2 16.1.1 16.1.2 16.1.3 17.1.1 17.2.1 Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit Defining ALE adaptive mesh domains in Abaqus/Standard ALE adaptive meshing and remapping in Abaqus/Standard Adaptive remeshing Adaptive remeshing: overview Selection of error indicators influencing adaptive remeshing Solution-based mesh sizing Analysis continuation after mesh replacement Mesh-to-mesh solution mapping 13. Optimization Techniques Structural optimization: overview Structural optimization: overview Optimization models Design responses Objectives and constraints Creating Abaqus optimization models 14. Eulerian Analysis Eulerian analysis Defining Eulerian boundaries Eulerian mesh motion Defining adaptive mesh refinement in the Eulerian domain 15. Particle Methods Smoothed particle hydrodynamic analyses Smoothed particle hydrodynamic analysis Finite element conversion to SPH particles 16. Sequentially Coupled Multiphysics Analyses Predefined fields for sequential coupling Sequentially coupled thermal-stress analysis Predefined loads for sequential coupling 17. Co-simulation Co-simulation: overview Preparing an Abaqus analysis for co-simulation Preparing an Abaqus analysis for co-simulation Co-simulation between Abaqus solvers Abaqus/Standard to Abaqus/Explicit co-simulation Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation 18. Extending Abaqus Analysis Functionality User subroutines and utilities User subroutines: overview Available user subroutines Available utility routines 19. Design Sensitivity Analysis Design sensitivity analysis 20. Parametric Studies Scripting parametric studies Scripting parametric studies Parametric studies: commands aStudy.combine(): Combine parameter samples for parametric studies. aStudy.constrain(): Constrain parameter value combinations in parametric studies. aStudy.define(): Define parameters for parametric studies. aStudy.execute(): Execute the analysis of parametric study designs. aStudy.gather(): Gather the results of a parametric study. aStudy.generate(): Generate the analysis job data for a parametric study. aStudy.output(): Specify the source of parametric study results. aStudy=ParStudy(): Create a parametric study. aStudy.report(): Report parametric study results. aStudy.sample(): Sample parameters for parametric studies. 17.3.1 17.3.2 18.1.1 18.1.2 18.1.3 19.1.1 20.1.1 20.2.1 20.2.2 20.2.3 20.2.4 20.2.5 20.2.6 20.2.7 20.2.8 20.2.9 20.2.10 21.1.1 21.1.2 21.1.3 21.2.1 22.1.1 22.2.1 22.2.2 22.2.3 22.3.1 22.4.1 22.5.1 22.5.2 22.5.3 22.6.1 22.6.2 22.7.1 22.7.2 Volume III PART V MATERIALS 21. Materials: Introduction Introduction Material library: overview Material data definition Combining material behaviors General properties Density 22. Elastic Mechanical Properties Overview Elastic behavior: overview Linear elasticity Linear elastic behavior No compression or no tension Plane stress orthotropic failure measures Porous elasticity Elastic behavior of porous materials Hypoelasticity Hypoelastic behavior Hyperelasticity Hyperelastic behavior of rubberlike materials Hyperelastic behavior in elastomeric foams Anisotropic hyperelastic behavior Stress softening in elastomers Mullins effect Energy dissipation in elastomeric foams Viscoelasticity Time domain viscoelasticity Frequency domain viscoelasticity Nonlinear viscoelasticity Hysteresis in elastomers Parallel network viscoelastic model Rate sensitive elastomeric foams Low-density foams 23. Inelastic Mechanical Properties Overview Inelastic behavior Metal plasticity Classical metal plasticity Models for metals subjected to cyclic loading Rate-dependent yield Rate-dependent plasticity: creep and swelling Annealing or melting Anisotropic yield/creep Johnson-Cook plasticity Dynamic failure models Porous metal plasticity Cast iron plasticity Two-layer viscoplasticity ORNL – Oak Ridge National Laboratory constitutive model Deformation plasticity Other plasticity models Extended Drucker-Prager models Modified Drucker-Prager/Cap model Mohr-Coulomb plasticity Critical state (clay) plasticity model Crushable foam plasticity models Fabric materials Fabric material behavior Jointed materials Jointed material model Concrete Concrete smeared cracking Cracking model for concrete Concrete damaged plasticity xii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 22.8.1 22.8.2 22.9.1 23.1.1 23.2.1 23.2.2 23.2.3 23.2.4 23.2.5 23.2.6 23.2.7 23.2.8 23.2.9 23.2.10 23.2.11 23.2.12 23.2.13 23.3.1 23.3.2 23.3.3 23.3.4 23.3.5 23.4.1 23.5.1 23.7.1 24.1.1 24.2.1 24.2.2 24.2.3 24.3.1 24.3.2 24.3.3 24.4.1 24.4.2 24.4.3 25.1.1 25.2.1 26.1.1 26.1.2 26.1.3 26.1.4 26.2.1 26.2.2 26.2.3 26.2.4 Permanent set in rubberlike materials Permanent set in rubberlike materials 24. Progressive Damage and Failure Progressive damage and failure: overview Progressive damage and failure Damage and failure for ductile metals Damage and failure for ductile metals: overview Damage initiation for ductile metals Damage evolution and element removal for ductile metals Damage and failure for fiber-reinforced composites Damage and failure for fiber-reinforced composites: overview Damage initiation for fiber-reinforced composites Damage evolution and element removal for fiber-reinforced composites Damage and failure for ductile materials in low-cycle fatigue analysis Damage and failure for ductile materials in low-cycle fatigue analysis: overview Damage initiation for ductile materials in low-cycle fatigue Damage evolution for ductile materials in low-cycle fatigue 25. Hydrodynamic Properties Overview Hydrodynamic behavior: overview Equations of state Equation of state 26. Other Material Properties Mechanical properties Material damping Thermal expansion Field expansion Viscosity Heat transfer properties Thermal properties: overview Conductivity Specific heat Latent heat Acoustic properties Acoustic medium Mass diffusion properties Diffusivity Solubility Electromagnetic properties Electrical conductivity Piezoelectric behavior Magnetic permeability Pore fluid flow properties Pore fluid flow properties Permeability Porous bulk moduli Sorption Swelling gel Moisture swelling User materials User-defined mechanical material behavior User-defined thermal material behavior 26.3.1 26.4.1 26.4.2 26.5.1 26.5.2 26.5.3 26.6.1 26.6.2 26.6.3 26.6.4 26.6.5 26.6.6 26.7.1 26.7.2 27.1.1 27.1.2 27.1.3 27.1.4 28.1.1 28.1.2 28.1.3 28.1.4 28.1.5 28.1.6 28.1.7 28.2.1 28.2.2 28.3.1 28.3.2 28.4.1 28.4.2 28.5.1 28.5.2 29.1.1 29.1.2 29.1.3 Volume IV PART VI ELEMENTS 27. Elements: Introduction Element library: overview Choosing the element’s dimensionality Choosing the appropriate element for an analysis type Section controls 28. Continuum Elements General-purpose continuum elements Solid (continuum) elements One-dimensional solid (link) element library Two-dimensional solid element library Three-dimensional solid element library Cylindrical solid element library Axisymmetric solid element library Axisymmetric solid elements with nonlinear, asymmetric deformation Fluid continuum elements Fluid (continuum) elements Fluid element library Infinite elements Infinite elements Infinite element library Warping elements Warping elements Warping element library Particle elements Particle elements Particle element library 29. Structural Elements Membrane elements Membrane elements General membrane element library Cylindrical membrane element library Axisymmetric membrane element library Truss elements Truss elements Truss element library Beam elements Beam modeling: overview Choosing a beam cross-section Choosing a beam element Beam element cross-section orientation Beam section behavior Using a beam section integrated during the analysis to define the section behavior Using a general beam section to define the section behavior Beam element library Beam cross-section library Frame elements Frame elements Frame section behavior Frame element library Elbow elements Pipes and pipebends with deforming cross-sections: elbow elements Elbow element library Shell elements Shell elements: overview Choosing a shell element Defining the initial geometry of conventional shell elements Shell section behavior Using a shell section integrated during the analysis to define the section behavior Using a general shell section to define the section behavior Three-dimensional conventional shell element library Continuum shell element library Axisymmetric shell element library Axisymmetric shell elements with nonlinear, asymmetric deformation 29.1.4 29.2.1 29.2.2 29.3.1 29.3.2 29.3.3 29.3.4 29.3.5 29.3.6 29.3.7 29.3.8 29.3.9 29.4.1 29.4.2 29.4.3 29.5.1 29.5.2 29.6.1 29.6.2 29.6.3 29.6.4 29.6.5 29.6.6 29.6.7 29.6.8 29.6.9 29.6.10 30.1.1 30.1.2 30.2.1 30.2.2 30.3.1 30.3.2 30.4.1 30.4.2 31.1.1 31.1.2 31.1.3 31.1.4 31.1.5 31.2.1 31.2.2 31.2.3 31.2.4 31.2.5 31.2.6 31.2.7 31.2.8 31.2.9 31.2.10 32.1.1 32.1.2 30. Inertial, Rigid, and Capacitance Elements Point mass elements Point masses Mass element library Rotary inertia elements Rotary inertia Rotary inertia element library Rigid elements Rigid elements Rigid element library Capacitance elements Point capacitance Capacitance element library 31. Connector Elements Connector elements Connectors: overview Connector elements Connector actuation Connector element library Connection-type library Connector element behavior Connector behavior Connector elastic behavior Connector damping behavior Connector functions for coupled behavior Connector friction behavior Connector plastic behavior Connector damage behavior Connector stops and locks Connector failure behavior Connector uniaxial behavior 32. Special-Purpose Elements Spring elements Springs Spring element library Dashpot elements Dashpots Dashpot element library Flexible joint elements Flexible joint element Flexible joint element library Distributing coupling elements Distributing coupling elements Distributing coupling element library Cohesive elements Cohesive elements: overview Choosing a cohesive element Modeling with cohesive elements Defining the cohesive element’s initial geometry Defining the constitutive response of cohesive elements using a continuum approach Defining the constitutive response of cohesive elements using a traction-separation description Defining the constitutive response of fluid within the cohesive element gap Two-dimensional cohesive element library Three-dimensional cohesive element library Axisymmetric cohesive element library Gasket elements Gasket elements: overview Choosing a gasket element Including gasket elements in a model Defining the gasket element’s initial geometry Defining the gasket behavior using a material model Defining the gasket behavior directly using a gasket behavior model Two-dimensional gasket element library Three-dimensional gasket element library Axisymmetric gasket element library Surface elements Surface elements General surface element library Cylindrical surface element library Axisymmetric surface element library 32.2.1 32.2.2 32.3.1 32.3.2 32.4.1 32.4.2 32.5.1 32.5.2 32.5.3 32.5.4 32.5.5 32.5.6 32.5.7 32.5.8 32.5.9 32.5.10 32.6.1 32.6.2 32.6.3 32.6.4 32.6.5 32.6.6 32.6.7 32.6.8 32.6.9 32.7.1 32.7.2 32.7.3 32.7.4 32.8.1 32.8.2 32.9.1 32.9.2 32.10.1 32.10.2 32.11.1 32.11.2 32.12.1 32.12.2 32.13.1 32.13.2 32.14.1 32.14.2 32.15.1 32.15.2 Tube support elements Tube support elements Tube support element library Line spring elements Line spring elements for modeling part-through cracks in shells Line spring element library Elastic-plastic joints Elastic-plastic joints Elastic-plastic joint element library Drag chain elements Drag chains Drag chain element library Pipe-soil elements Pipe-soil interaction elements Pipe-soil interaction element library Acoustic interface elements Acoustic interface elements Acoustic interface element library Eulerian elements Eulerian elements Eulerian element library User-defined elements User-defined elements User-defined element library EI.1 Abaqus/Standard Element Index EI.2 Abaqus/Explicit Element Index EI.3 Abaqus/CFD Element Index Volume V PART VII PRESCRIBED CONDITIONS 33. Prescribed Conditions Overview Prescribed conditions: overview Amplitude curves Initial conditions Initial conditions in Abaqus/Standard and Abaqus/Explicit Initial conditions in Abaqus/CFD Boundary conditions Boundary conditions in Abaqus/Standard and Abaqus/Explicit Boundary conditions in Abaqus/CFD Loads Applying loads: overview Concentrated loads Distributed loads Thermal loads Electromagnetic loads Acoustic and shock loads Pore fluid flow Prescribed assembly loads Prescribed assembly loads Predefined fields Predefined fields PART VIII CONSTRAINTS 34. Constraints Overview Kinematic constraints: overview Multi-point constraints Linear constraint equations xx Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 33.1.1 33.1.2 33.2.1 33.2.2 33.3.1 33.3.2 33.4.1 33.4.2 33.4.3 33.4.4 33.4.5 33.4.6 33.4.7 33.5.1 34.2.2 34.2.3 34.3.1 34.3.2 34.3.3 34.3.4 34.4.1 34.5.1 34.6.1 35.1.1 35.2.1 35.2.2 35.2.3 35.2.4 35.2.5 35.2.6 35.3.1 35.3.2 35.3.3 35.3.4 35.3.5 35.3.6 35.3.7 35.3.8 General multi-point constraints Kinematic coupling constraints Surface-based constraints Mesh tie constraints Coupling constraints Shell-to-solid coupling Mesh-independent fasteners Embedded elements Embedded elements Element end release Element end release Overconstraint checks Overconstraint checks PART IX INTERACTIONS 35. Defining Contact Interactions Overview Contact interaction analysis: overview Defining general contact in Abaqus/Standard Defining general contact interactions in Abaqus/Standard Surface properties for general contact in Abaqus/Standard Contact properties for general contact in Abaqus/Standard Controlling initial contact status in Abaqus/Standard Stabilization for general contact in Abaqus/Standard Numerical controls for general contact in Abaqus/Standard Defining contact pairs in Abaqus/Standard Defining contact pairs in Abaqus/Standard Assigning surface properties for contact pairs in Abaqus/Standard Assigning contact properties for contact pairs in Abaqus/Standard Modeling contact interference fits in Abaqus/Standard Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs Adjusting contact controls in Abaqus/Standard Defining tied contact in Abaqus/Standard Extending master surfaces and slide lines Contact modeling if substructures are present Contact modeling if asymmetric-axisymmetric elements are present Defining general contact in Abaqus/Explicit Defining general contact interactions in Abaqus/Explicit Assigning surface properties for general contact in Abaqus/Explicit Assigning contact properties for general contact in Abaqus/Explicit Controlling initial contact status for general contact in Abaqus/Explicit Contact controls for general contact in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit Assigning surface properties for contact pairs in Abaqus/Explicit Assigning contact properties for contact pairs in Abaqus/Explicit Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit Contact controls for contact pairs in Abaqus/Explicit 36. Contact Property Models Mechanical contact properties Mechanical contact properties: overview Contact pressure-overclosure relationships Contact damping Contact blockage Frictional behavior User-defined interfacial constitutive behavior Pressure penetration loading Interaction of debonded surfaces Breakable bonds Surface-based cohesive behavior Thermal contact properties Thermal contact properties Electrical contact properties Electrical contact properties Pore fluid contact properties Pore fluid contact properties 37. Contact Formulations and Numerical Methods Contact formulations and numerical methods in Abaqus/Standard Contact formulations in Abaqus/Standard xxii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 35.3.9 35.3.10 35.4.1 35.4.2 35.4.3 35.4.4 35.4.5 35.5.1 35.5.2 35.5.3 35.5.4 35.5.5 36.1.1 36.1.2 36.1.3 36.1.4 36.1.5 36.1.6 36.1.7 36.1.8 36.1.9 36.1.10 36.2.1 37.1.2 37.1.3 37.2.1 37.2.2 37.2.3 38.1.1 38.1.2 38.2.1 38.2.2 39.1.1 39.2.1 39.2.2 39.3.1 39.3.2 39.4.1 39.4.2 39.5.1 39.5.2 40.1.1 Contact constraint enforcement methods in Abaqus/Standard Smoothing contact surfaces in Abaqus/Standard Contact formulations and numerical methods in Abaqus/Explicit Contact formulation for general contact in Abaqus/Explicit Contact formulations for contact pairs in Abaqus/Explicit Contact constraint enforcement methods in Abaqus/Explicit 38. Contact Difficulties and Diagnostics Resolving contact difficulties in Abaqus/Standard Contact diagnostics in an Abaqus/Standard analysis Common difficulties associated with contact modeling in Abaqus/Standard Resolving contact difficulties in Abaqus/Explicit Contact diagnostics in an Abaqus/Explicit analysis Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit 39. Contact Elements in Abaqus/Standard Contact modeling with elements Contact modeling with elements Gap contact elements Gap contact elements Gap element library Tube-to-tube contact elements Tube-to-tube contact elements Tube-to-tube contact element library Slide line contact elements Slide line contact elements Axisymmetric slide line element library Rigid surface contact elements Rigid surface contact elements Axisymmetric rigid surface contact element library 40. Defining Cavity Radiation in Abaqus/Standard Cavity radiation Printed on: Prescribed Conditions Overview Initial conditions Boundary conditions Loads Prescribed assembly loads Predefined fields PRESCRIBED CONDITIONS 33.1 33.2 33.3 33.4 33.5 33.1 Overview • “Prescribed conditions: overview,” Section 33.1.1 • “Amplitude curves,” Section 33.1.2 33.1.1 PRESCRIBED CONDITIONS: OVERVIEW The following types of external conditions can be prescribed in an Abaqus model: • Initial conditions: Nonzero initial conditions can be defined for many variables, as described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, and “Initial conditions in Abaqus/CFD,” Section 33.2.2. • Boundary conditions: Boundary conditions are used to prescribe values of basic solution variables: displacements and rotations in stress/displacement analysis, temperature in heat transfer or coupled thermal-stress analysis, electrical potential in coupled thermal-electrical analysis, pore pressure in soils analysis, acoustic pressure in acoustic analysis, etc. Boundary conditions can be defined as described in “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1, and “Boundary conditions in Abaqus/CFD,” Section 33.3.2. • Loads: Many types of loading are available, depending on the analysis procedure. “Applying loads: overview,” Section 33.4.1, gives an overview of loading in Abaqus. Load types specific to one analysis procedure are described in the appropriate procedure section in Part III, “Analysis Procedures, Solution, and Control.” General loads, which can be applied in multiple analysis types, are described in: – “Concentrated loads,” Section 33.4.2 – “Distributed loads,” Section 33.4.3 – “Thermal loads,” Section 33.4.4 – “Electromagnetic loads,” Section 33.4.5 – “Acoustic and shock loads,” Section 33.4.6 – “Pore fluid flow,” Section 33.4.7 • Prescribed assembly loads: Pre-tension sections can be defined in Abaqus/Standard to prescribe assembly loads in bolts or any other type of fastener. Pre-tension sections are described in “Prescribed assembly loads,” Section 33.5.1. • Connector loads and motions: Connector elements can be used to define complex mechanical connections between parts, including actuation with prescribed loads or motions. Connector elements are described in “Connectors: overview,” Section 31.1.1. • Predefined fields: Predefined fields are time-dependent, non-solution-dependent fields that exist over the spatial domain of the model. Temperature is the most commonly defined field. Predefined fields are described in “Predefined fields,” Section 33.6.1. Amplitude variations Complex time- or frequency-dependent boundary conditions, loads, and predefined fields can be specified by referring to an amplitude curve in the prescribed condition definition. Amplitude curves are explained in “Amplitude curves,” Section 33.1.2. In Abaqus/Standard if no amplitude is referenced from the boundary condition, loading, or predefined field definition, the total magnitude can be applied instantaneously at the start of the step and remain constant throughout the step (a “step” variation) or it can vary linearly over the step from the value at the end of the previous step (or from zero at the start of the analysis) to the magnitude given (a “ramp” variation). You choose the type of variation when you define the step; the default variation depends on the procedure chosen, as shown in “Defining an analysis,” Section 6.1.2. In Abaqus/Standard the variation of many prescribed conditions can be defined in user subroutines. In this case the magnitude of the variable can vary in any way with position and time. The magnitude variation for prescribing and removing conditions must be specified in the subroutine . In Abaqus/Explicit if no amplitude is referenced from the boundary condition or loading definition, the total value will be applied instantaneously at the start of the step and will remain constant throughout the step (a “step” variation), although Abaqus/Explicit does not admit jumps in displacement . If no amplitude is referenced from a predefined field definition, the total magnitude will vary linearly over the step from the value at the end of the previous step (or from zero at the start of the analysis) to the magnitude given (a “ramp” variation). When boundary conditions are removed , in stress/displacement analysis) is converted to an applied conjugate flux (force or moment in stress/displacement analysis) at the beginning of the step. This flux magnitude is set to zero with a “step” or “ramp” variation depending on the procedure chosen, as discussed in “Defining an analysis,” Section 6.1.2. Similarly, when loads and predefined fields are removed, the load is set to zero and the predefined field is set to its initial value. In Abaqus/CFD if no amplitude is referenced from the boundary or loading condition, the total value is applied instantaneously at the start of the step and remains constant throughout the step. Abaqus/CFD does admit jumps in the velocity, temperature, etc. from the end value of the previous step to the magnitude given in the current step. However, jumps in velocity boundary conditions may result in a divergence-free projection that adjusts the initial velocities to be consistent with the prescribed boundary conditions in order to define a well-posed incompressible flow problem. Applying boundary conditions and loads in a local coordinate system You can define a local coordinate system at a node as described in “Transformed coordinate systems,” Section 2.1.5. Then, all input data for concentrated force and moment loading and for displacement and rotation boundary conditions are given in the local system. Loads and predefined fields available for various procedures Table 33.1.1–1 Available loads and predefined fields. Loads and predefined fields Procedures Added mass (concentrated and distributed) Abaqus/Aqua eigenfrequency extraction analysis (“Natural frequency extraction,” Section 6.3.5) Base motion Procedures based on eigenmodes: “Transient modal dynamic analysis,” Section 6.3.7 “Mode-based steady-state dynamic analysis,” Section 6.3.8 “Response spectrum analysis,” Section 6.3.10 “Random response analysis,” Section 6.3.11 All procedures except those based on eigenmodes All relevant procedures except modal extraction, buckling, those based on eigenmodes, and direct steady-state dynamics Boundary condition with a nonzero prescribed boundary Connector motion Connector load Cross-correlation property “Random response analysis,” Section 6.3.11 Current density (concentrated and distributed) “Coupled thermal-electrical analysis,” Section 6.7.3 “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4 Current density vector “Eddy current analysis,” Section 6.7.5 Electric charge (concentrated and distributed) “Piezoelectric analysis,” Section 6.7.2 Equivalent pressure stress “Mass diffusion analysis,” Section 6.9.1 Film coefficient and associated sink temperature All procedures involving temperature degrees of freedom Fluid flux Analysis involving hydrostatic fluid elements Fluid mass flow rate Analysis involving convective heat transfer elements Flux (concentrated and distributed) All procedures involving temperature degrees of freedom “Mass diffusion analysis,” Section 6.9.1 Force and moment (concentrated and distributed) All procedures with displacement degrees of freedom except response spectrum Loads and predefined fields Procedures Incident wave loading Direct-integration dynamic analysis (“Implicit dynamic analysis using direct integration,” Section 6.3.2) involving solid and/or fluid elements undergoing shock loading Predefined field variable All procedures except those based on eigenmodes Seepage coefficient and associated sink pore pressure Distributed seepage flow “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 Substructure load All procedures involving the use of substructures Temperature as a predefined field All procedures except adiabatic analysis, mode-based procedures, and procedures involving temperature degrees of freedom With the exception of concentrated added mass and distributed added mass, no loads can be applied in eigenfrequency extraction analysis. 33.1.2 AMPLITUDE CURVES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Prescribed conditions: overview,” Section 33.1.1 • *AMPLITUDE • Chapter 57, “The Amplitude toolset,” of the Abaqus/CAE User’s Manual Overview An amplitude curve: • allows arbitrary time (or frequency) variations of load, displacement, and other prescribed variables to be given throughout a step (using step time) or throughout the analysis (using total time); • can be defined as a mathematical function (such as a sinusoidal variation), as a series of values at points in time (such as a digitized acceleration-time record from an earthquake), as a user-customized definition via user subroutines, or, in Abaqus/Standard, as values calculated based on a solution-dependent variable (such as the maximum creep strain rate in a superplastic forming problem); and • can be referred to by name by any number of boundary conditions, loads, and predefined fields. Amplitude curves By default, the values of loads, boundary conditions, and predefined fields either change linearly with time throughout the step (ramp function) or they are applied immediately and remain constant throughout the step (step function)—see “Defining an analysis,” Section 6.1.2. Many problems require a more elaborate definition, however. For example, different amplitude curves can be used to specify time variations for different loadings. One common example is the combination of thermal and mechanical load transients: usually the temperatures and mechanical loads have different time variations during the step. Different amplitude curves can be used to specify each of these time variations. Other examples include dynamic analysis under earthquake loading, where an amplitude curve can be used to specify the variation of acceleration with time, and underwater shock analysis, where an amplitude curve is used to specify the incident pressure profile. Amplitudes are defined as model data (i.e., they are not step dependent). Each amplitude curve must be named; this name is then referred to from the load, boundary condition, or predefined field definition . *AMPLITUDE, NAME=name Load or Interaction module: Create Amplitude: Name: name Abaqus/CAE Usage: Input File Usage: Defining the time period Each amplitude curve is a function of time or frequency. Amplitudes defined as functions of frequency are used in “Direct-solution steady-state dynamic analysis,” Section 6.3.4, “Mode-based steady-state dynamic analysis,” Section 6.3.8, and “Eddy current analysis,” Section 6.7.5. Amplitudes defined as functions of time can be given in terms of step time (default) or in terms of total time. These time measures are defined in “Conventions,” Section 1.2.2. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *AMPLITUDE, NAME=name, TIME=STEP TIME (default) *AMPLITUDE, NAME=name, TIME=TOTAL TIME Load or Interaction module: Create Amplitude: any type: Time span: Step time or Total time Continuation of an amplitude reference in subsequent steps If a boundary condition, load, or predefined field refers to an amplitude curve and the prescribed condition is not redefined in subsequent steps, the following rules apply: • If the associated amplitude was given in terms of total time, the prescribed condition continues to follow the amplitude definition. • If no associated amplitude was given or if the amplitude was given in terms of step time, the prescribed condition remains constant at the magnitude associated with the end of the previous step. Specifying relative or absolute data You can choose between specifying relative or absolute magnitudes for an amplitude curve. Relative data By default, you give the amplitude magnitude as a multiple (fraction) of the reference magnitude given in the prescribed condition definition. This method is especially useful when the same variation applies to different load types. Input File Usage: Abaqus/CAE Usage: *AMPLITUDE, NAME=name, VALUE=RELATIVE Amplitude magnitudes are always relative in Abaqus/CAE. Absolute data Alternatively, you can give absolute magnitudes directly. When this method is used, the values given in the prescribed condition definitions will be ignored. Absolute amplitude values should generally not be used to define temperatures or predefined field variables for nodes attached to beam or shell elements as values at the reference surface together with the gradient or gradients across the section (default cross-section definition; see “Using a beam section integrated during the analysis to define the section behavior,” Section 29.3.6, and “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5). Because the values given in temperature fields and predefined fields are ignored, the absolute amplitude value will be used to define both the temperature and the gradient and field and gradient, respectively. Input File Usage: Abaqus/CAE Usage: *AMPLITUDE, NAME=name, VALUE=ABSOLUTE Absolute amplitude magnitudes are not supported in Abaqus/CAE. Defining the amplitude data The variation of an amplitude with time can be specified in several ways. The variation of an amplitude with frequency can be given only in tabular or equally spaced form. Defining tabular data Choose the tabular definition method (default) to define the amplitude curve as a table of values at convenient points on the time scale. Abaqus interpolates linearly between these values, as needed. By default in Abaqus/Standard, if the time derivatives of the function must be computed, some smoothing is applied at the time points where the time derivatives are discontinuous. In contrast, in Abaqus/Explicit no default smoothing is applied (other than the inherent smoothing associated with a finite time increment). You can modify the default smoothing values (smoothing is discussed in more detail below, under the heading “Using an amplitude definition with boundary conditions”); alternatively, a smooth step amplitude curve can be defined . If the amplitude varies rapidly—as with the ground acceleration in an earthquake, for example—you must ensure that the time increment used in the analysis is small enough to pick up the amplitude variation accurately since Abaqus will sample the amplitude definition only at the times corresponding to the increments being used. If the analysis time in a step is less than the earliest time for which data exist in the table, Abaqus applies the earliest value in the table for all step times less than the earliest tabulated time. Similarly, if the analysis continues for step times past the last time for which data are defined in the table, the last value in the table is applied for all subsequent time. Several examples of tabular input are shown in Figure 33.1.2–1. Input File Usage: Abaqus/CAE Usage: *AMPLITUDE, NAME=name, DEFINITION=TABULAR Load or Interaction module: Create Amplitude: Tabular Defining equally spaced data Choose the equally spaced definition method to give a list of amplitude values at fixed time intervals beginning at a specified value of time. Abaqus interpolates linearly between each time interval. You must specify the fixed time (or frequency) interval at which the amplitude data will be given, . You can also specify the time (or lowest frequency) at which the first amplitude is given, ; the default is =0.0. If the analysis time in a step is less than the earliest time for which data exist in the table, Abaqus applies the earliest value in the table for all step times less than the earliest tabulated time. Similarly, a. Uniformly increasing load 1.0 Relative load magnitude 0.0 Time period 1.0 b. Uniformly decreasing load 1.0 Relative load magnitude 0.0 Time period 1.0 c. Variable load 1.0 Relative load magnitude Amplitude Table: Time Relative load 0.0 1.0 0.0 1.0 0.0 0.4 0.6 0.8 1.0 0.0 1.0 1.0 0.0 0.0 1.2 0.5 0.5 0.0 0.0 Time period 1.0 Figure 33.1.2–1 Tabular amplitude definition examples. if the analysis continues for step times past the last time for which data are defined in the table, the last value in the table is applied for all subsequent time. Input File Usage: Abaqus/CAE Usage: *AMPLITUDE, NAME=name, DEFINITION=EQUALLY SPACED, FIXED INTERVAL= , BEGIN= Load or Interaction module: Create Amplitude: Equally spaced: Fixed interval: The time (or lowest frequency) at which the first amplitude is given, indicated in the first table cell. , is Defining periodic data Choose the periodic definition method to define the amplitude, a, as a Fourier series: for for , N, where input is shown in Figure 33.1.2–2. , and , , , , are user-defined constants. An example of this form of Input File Usage: Abaqus/CAE Usage: *AMPLITUDE, NAME=name, DEFINITION=PERIODIC Load or Interaction module: Create Amplitude: Periodic 0.60 0.40 0.20 0.00 − 0.20 − 0.40 0.00 0.10 0.20 0.30 0.40 0.50 Time p = 0.2s a = A0 + Σ [An cos nω(t−t0) + Bn sin nω(t−t0)] for t ≥ t0 n=1 a = A0 for t < t0 with N = 2, ω = 31.416 rad/s, t0 = −0.1614 s A0= 0, A1 = 0.227, B1 = 0.0, A2 = 0.413, B2 = 0.0 Figure 33.1.2–2 Periodic amplitude definition example. Defining modulated data Choose the modulated definition method to define the amplitude, a, as for for , and are user-defined constants. An example of this form of input is shown in *AMPLITUDE, NAME=name, DEFINITION=MODULATED Load or Interaction module: Create Amplitude: Modulated where , Figure 33.1.2–3. , A, Input File Usage: Abaqus/CAE Usage: -1 Time 10 ( x 10-1) a = A0 + A sin ω 1 (t−t0) sin ω 2 (t−t0) for t > t0 a = A0 with for t ≤ t0 A0= 1.0, A = 2.0, ω 1 = 10π, ω 2 = 20π, t0 = .2 Figure 33.1.2–3 Modulated amplitude definition example. Defining exponential decay Choose the exponential decay definition method to define the amplitude, a, as for for where Figure 33.1.2–4. , A, , and are user-defined constants. An example of this form of input is shown in Input File Usage: Abaqus/CAE Usage: *AMPLITUDE, NAME=name, DEFINITION=DECAY Load or Interaction module: Create Amplitude: Decay Time ( x 10-1) 10 a = A0 + A exp [−(t−t0) / td] for t ≥ t0 a = A0 for t < t0 with A0 = 0.0, A = 5.0, t0 = 0.2, td = 0.2 Figure 33.1.2–4 Exponential decay amplitude definition example. Defining smooth step data Abaqus/Standard and Abaqus/Explicit can calculate amplitudes based on smooth step data. Choose the smooth step definition method to define the amplitude, a, between two consecutive data points and as for where first and second derivatives of a are zero at smoothly from one amplitude value to another. The amplitude, a, is defined such that . The above function is such that and , and the . This definition is intended to ramp up or down at at , for for where and are the first and last data points, respectively. Examples of this form of input are shown in Figure 33.1.2–5 and Figure 33.1.2–6. This definition cannot be used to interpolate smoothly between a set of data points; i.e., this definition cannot be used to do curve fitting. Input File Usage: Abaqus/CAE Usage: *AMPLITUDE, NAME=name, DEFINITION=SMOOTH STEP Load or Interaction module: Create Amplitude: Smooth step Defining a solution-dependent amplitude for superplastic forming analysis Abaqus/Standard can calculate amplitude values based on a solution-dependent variable. Choose the solution-dependent definition method to create a solution-dependent amplitude curve. The data consist of an initial value, a minimum value, and a maximum value. The amplitude starts with the initial value and is then modified based on the progress of the solution, subject to the minimum and maximum values. The maximum value is typically the controlling mechanism used to end the analysis. This method is used with creep strain rate control for superplastic forming analysis . Input File Usage: Abaqus/CAE Usage: *AMPLITUDE, NAME=name, DEFINITION=SOLUTION DEPENDENT Load or Interaction module: Create Amplitude: Solution dependent Defining the bubble load amplitude for an underwater explosion Two interfaces are available in Abaqus for applying incident wave loads . For either interface bubble dynamics can be described using a model internal to Abaqus. A description of this built-in mechanical model and the parameters that define the bubble behavior are discussed in “Defining bubble loading for spherical incident wave loading” in “Acoustic and shock loads,” Section 33.4.6. The related theoretical details are described in “Loading due to an incident dilatational wave field,” Section 6.3.1 of the Abaqus Theory Manual. 1.0 0.1 Time t0 = 0.0 A0 = 0.0 t1 = 0.1 A1 = 1.0 a = A0 for t ≤ t0 = A0 + (A1 − A0) ξ3 (10 − 15 ξ + 6 ξ2) for t0 < t < t1 = A1 for t ≥ t1 where ξ = t − t0 t1 − t0 Figure 33.1.2–5 Smooth step amplitude definition example with two data points. The preferred interface for incident wave loading due to an underwater explosion specifies bubble dynamics using the UNDEX charge property definition . The alternative interface for incident wave loading uses the bubble definition described in this section to define bubble load amplitude curves. An example of the bubble amplitude definition with the following input data is shown in Figure 33.1.2–7. (t3, A3) (t4, A4) (t2, A2) (t0, A0) (t1, A1) Time (t5, A5) (t6, A6) t0 = 0.0 A0 = 0.1 t1 = 0.1 A1 = 0.1 t2 = 0.2 A2 = 0.3 t3 = 0.3 A3 = 0.5 t4 = 0.4 A4 = 0.5 t5 = 0.5 A5 = 0.2 t6 = 0.8 A6 = 0.2 a = A0 for t ≤ t0 = A6 for t ≥ t6 Amplitude, a, between any two consecutive data points (ti, Ai) and (ti+1, Ai+1) is a = Ai + (Ai+1 − Ai) ξ3 (10 − 15ξ + 6 ξ2) where ξ = t − ti ti+1 − ti Figure 33.1.2–6 Smooth step amplitude definition example with multiple data points. Input File Usage: Abaqus/CAE Usage: *AMPLITUDE, NAME=name, DEFINITION=BUBBLE Bubble amplitudes are not supported in Abaqus/CAE. However, bubble loading for an underwater explosion is supported in the Interaction module using the UNDEX charge property definition. (a) (b) Figure 33.1.2–7 Bubble amplitude definition example: (a) radius of bubble and (b) depth of bubble center under fluid surface. Defining an amplitude via a user subroutine Choose the user definition method to define the amplitude curve via coding in user subroutine UAMP (Abaqus/Standard) or VUAMP (Abaqus/Explicit). You define the value of the amplitude function in time and, optionally, the values of the derivatives and integrals for the function sought to be implemented as outlined in “UAMP,” Section 1.1.19 of the Abaqus User Subroutines Reference Manual, and “VUAMP,” Section 1.2.7 of the Abaqus User Subroutines Reference Manual. You can use an arbitrary number of properties to calculate the amplitude, and you can use an arbitrary number of state variables that can be updated independently for each amplitude definition. In Abaqus/Standard user-defined amplitudes are not supported for complex eigenvalue extraction and for linear dynamic procedures, except for steady-state dynamic analysis with the response computed directly in terms of the physical degrees of freedom. Moreover, solution-dependent sensors can be used to define the user-customized amplitude. The sensors can be identified via their name, and two utilities allow for the extraction of the current sensor value inside the user subroutine . Simple control/logical models can be implemented using this feature as illustrated in “Crank mechanism,” Section 4.1.2 of the Abaqus Example Problems Manual. Input File Usage: *AMPLITUDE, NAME=name, DEFINITION=USER, PROPERTIES=m, VARIABLES=n Abaqus/CAE Usage: Load or Interaction module: Create Amplitude: User: Number of variables: n User-defined amplitude properties are not supported in Abaqus/CAE. Using an amplitude definition with boundary conditions When an amplitude curve is used to prescribe a variable of the model as a boundary condition (by referring to the amplitude from the boundary condition definition), the first and second time derivatives of the variable may also be needed. For example, the time history of a displacement can be defined for a direct integration dynamic analysis step by an amplitude variation; in this case Abaqus must compute the corresponding velocity and acceleration. When the displacement time history is defined by a piecewise linear amplitude variation (tabular or equally spaced amplitude definition), the corresponding velocity is piecewise constant and the acceleration may be infinite at the end of each time interval given in the amplitude definition table, as shown in Figure 33.1.2–8(a). This behavior is unreasonable. (In Abaqus/Explicit time derivatives of amplitude curves are typically based on finite differences, such as , so there is some inherent smoothing associated with the time discretization.) You can modify the piecewise linear displacement variation into a combination of piecewise linear and piecewise quadratic variations through smoothing. Smoothing ensures that the velocity varies continuously during the time period of the amplitude definition and that the acceleration no longer has singularity points, as illustrated in Figure 33.1.2–8(b). the When the velocity time history is defined by a piecewise linear amplitude variation, corresponding acceleration is piecewise constant. Smoothing can be used to modify the piecewise linear velocity variation into a combination of piecewise linear and piecewise quadratic variations. Smoothing ensures that the acceleration varies continuously during the time period of the amplitude definition. You specify t, the fraction of the time interval before and after each time point during which the piecewise linear time variation is to be replaced by a smooth quadratic time variation. The default in Abaqus/Standard is t=0.25; the default in Abaqus/Explicit is t=0.0. The allowable range is 0.0 0.5. A value of 0.05 is suggested for amplitude definitions that contain large time intervals to avoid severe deviation from the specified definition. In Abaqus/Explicit if a displacement jump is specified using an amplitude curve (i.e., the beginning displacement defined using the amplitude function does not correspond to the displacement at that time), this displacement jump will be ignored. Displacement boundary conditions are enforced in Abaqus/Explicit in an incremental manner using the slope of the amplitude curve. To avoid the “noisy” solution that may result in Abaqus/Explicit when smoothing is not used, it is better to specify the velocity history of a node rather than the displacement history . When an amplitude definition is used with prescribed conditions that do not require the evaluation of time derivatives (for example, concentrated loads, distributed loads, temperature fields, etc., or a static analysis), the use of smoothing is ignored. When the displacement time history is defined using a smooth-step amplitude curve, the velocity and acceleration will be zero at every data point specified, although the average velocity and acceleration τ = Smooth Value x Minimum (t1 ,t2) t1 t2 time time time time time time (a) without smoothing (b) with smoothing Figure 33.1.2–8 Piecewise linear displacement definitions. may well be nonzero. Hence, this amplitude definition should be used only to define a (smooth) step function. Input File Usage: Use either of the following options: *AMPLITUDE, NAME=name, DEFINITION=TABULAR, SMOOTH=t *AMPLITUDE, NAME=name, DEFINITION=EQUALLY SPACED, SMOOTH=t Abaqus/CAE Usage: Load or Interaction module: Create Amplitude: choose Tabular or Equally spaced: Smoothing: Specify: t Using an amplitude definition with secondary base motion in modal dynamics When an amplitude curve is used to prescribe a variable of the model as a secondary base motion in a modal dynamics procedure (by referring to the amplitude from the base motion definition during a modal dynamic procedure), the first or second time derivatives of the variable may also be needed. For example, the time history of a displacement can be defined for secondary base motion in a modal dynamics procedure. In this case Abaqus must compute the corresponding acceleration. The modal dynamics procedure uses an exact solution for the response to a piecewise linear force. Accordingly, secondary base motion definitions are applied as piecewise linear acceleration histories. When displacement-type or velocity-type base motions are used to define displacement or velocity time histories and an amplitude variation using the tabular, equally spaced, periodic, modulated, or exponential decay definitions is used, an algorithmic acceleration is computed based on the tabular data (the amplitude data evaluated at the time values used in the modal dynamics procedure). At the end of any time increment where the amplitude curve is linear over that increment, linear over the previous increment, and the slopes of the amplitude variations over the two increments are equal, this algorithmic acceleration reproduces the exact displacement and velocity for displacement time histories or the exact velocity for velocity time histories. When the displacement time history is defined using a smooth-step amplitude curve, the velocity and acceleration will be zero at every data point specified, although the average velocity and acceleration may well be nonzero. Hence, this amplitude definition should be used only to define a (smooth) step function. Defining multiple amplitude curves You can define any number of amplitude curves and refer to them from any load, boundary condition, or predefined field definition. For example, one amplitude curve can be used to specify the velocity of a set of nodes, while another amplitude curve can be used to specify the magnitude of a pressure load on the body. If the velocity and the pressure both follow the same time history, however, they can both refer to the same amplitude curve. There is one exception in Abaqus/Standard: only one solution-dependent amplitude (used for superplastic forming) can be active during each step. Scaling and shifting amplitude curves You can scale and shift both time and magnitude when defining an amplitude. This can be helpful for example when your amplitude data need to be converted to a different unit system or when you reuse existing amplitude data to define similar amplitude curves. If both scaling and shifting are applied at the same time, the amplitude values are first scaled and then shifted. The amplitude shifting and scaling can be applied to all amplitude definition types except for solution dependent, bubble, and user. Input File Usage: *AMPLITUDE, NAME=name, SHIFTX=shiftx_value, SHIFTY=shifty_value, SCALEX=scalex_value, SCALEY=scaley_value Abaqus/CAE Usage: The scaling and shifting of amplitude curves is not supported in Abaqus/CAE. Reading the data from an alternate file The data for an amplitude curve can be contained in a separate file. Input File Usage: *AMPLITUDE, NAME=name, INPUT=file_name If the INPUT parameter is omitted, it is assumed that the data lines follow the keyword line. Abaqus/CAE Usage: Load or Interaction module: Create Amplitude: any type: click mouse button 3 while holding the cursor over the data table, and select Read from File Baseline correction in Abaqus/Standard When an amplitude definition is used to define an acceleration history in the time domain (a seismic record of an earthquake, for example), the integration of the acceleration record through time may result in a relatively large displacement at the end of the event. This behavior typically occurs because of instrumentation errors or a sampling frequency that is not sufficient to capture the actual acceleration history. In Abaqus/Standard it is possible to compensate for it by using “baseline correction.” The baseline correction method allows an acceleration history to be modified to minimize the overall drift of the displacement obtained from the time integration of the given acceleration. It is relevant only with tabular or equally spaced amplitude definitions. Baseline correction can be defined only when the amplitude is referenced as an acceleration boundary condition during a direct-integration dynamic analysis or as an acceleration base motion in modal dynamics. Input File Usage: Use both of the following options to include baseline correction: *AMPLITUDE, DEFINITION=TABULAR or EQUALLY SPACED *BASELINE CORRECTION The *BASELINE CORRECTION option must appear immediately following the data lines of the *AMPLITUDE option. Load or Interaction module: Create Amplitude: choose Tabular or Equally spaced: Baseline Correction Abaqus/CAE Usage: Effects of baseline correction The acceleration is modified by adding a quadratic variation of acceleration in time to the acceleration definition. The quadratic variation is chosen to minimize the mean squared velocity during each correction interval. Separate quadratic variations can be added for different correction intervals within the amplitude definition by defining the correction intervals. Alternatively, the entire amplitude history can be used as a single correction interval. The use of more correction intervals provides tighter control over any “drift” in the displacement at the expense of more modification of the given acceleration trace. In either case, the modification begins with the start of the amplitude variation and with the assumption that the initial velocity at that time is zero. The baseline correction technique is described in detail in “Baseline correction of accelerograms,” Section 6.1.2 of the Abaqus Theory Manual. 33.2 Initial conditions • “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1 • “Initial conditions in Abaqus/CFD,” Section 33.2.2 33.2.1 INITIAL CONDITIONS IN Abaqus/Standard AND Abaqus/Explicit Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Prescribed conditions: overview,” Section 33.1.1 • *INITIAL CONDITIONS • “Using the predefined field editors,” Section 16.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Initial conditions are specified for particular nodes or elements, as appropriate. The data can be provided directly; in an external input file; or, in some cases, by a user subroutine or by the results or output database file from a previous Abaqus analysis. If initial conditions are not specified, all initial conditions are zero except relative density in the porous metal plasticity model, which will have the value 1.0. Specifying the type of initial condition being defined Various types of initial conditions can be specified, depending on the analysis to be performed. Each type of initial condition is explained below, in alphabetical order. Defining initial acoustic static pressure In Abaqus/Explicit you can define initial acoustic static pressure values at the acoustic nodes. These values should correspond to static equilibrium and cannot be changed during the analysis. You can specify the initial acoustic static pressure at two reference locations in the model, and Abaqus/Explicit interpolates these data linearly to the acoustic nodes in the specified node set. The linear interpolation is based upon the projected position of each node onto the line defined by the two reference nodes. If the value at only one reference location is given, the initial acoustic static pressure is assumed to be uniform. The initial acoustic static pressure is used only in the evaluation of the cavitation condition when the acoustic medium is capable of undergoing cavitation. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=ACOUSTIC STATIC PRESSURE Initial acoustic static pressure is not supported in Abaqus/CAE. Defining initial normalized concentration In Abaqus/Standard you can define initial normalized concentration values for use with diffusion elements in mass diffusion analysis . *INITIAL CONDITIONS, TYPE=CONCENTRATION Initial normalized concentration is not supported in Abaqus/CAE. Abaqus/CAE Usage: Input File Usage: Defining initially bonded contact surfaces In Abaqus/Standard you can define initially bonded or partially bonded contact surfaces. This type of initial condition is intended for use with the crack propagation capability . The surfaces specified have to be different; this type of initial condition cannot be used with self-contact. If the crack propagation capability is not activated, the bonded portion of the surfaces will not separate. In this case defining initially bonded contact surfaces would have the same effect as defining tied contact, which generates a permanent bond between two surfaces during the entire analysis (“Defining tied contact in Abaqus/Standard,” Section 35.3.7). Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=CONTACT Initially bonded surfaces are not supported in Abaqus/CAE. Define the initial location of an enriched feature You can specify the initial location of an enriched feature, such as a crack, in an Abaqus/Standard analysis . Two signed distance functions per node are generally required to describe the crack location, including the location of crack tips, in a cracked geometry. The first signed distance function describes the crack surface, while the second is used to construct an orthogonal surface such that the intersection of the two surfaces defines the crack front. The first signed distance function is assigned only to nodes of elements intersected by the crack, while the second is assigned only to nodes of elements containing the crack tips. No explicit representation of the crack is needed because the crack is entirely described by the nodal data. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=ENRICHMENT Interaction module: crack editor: Crack location: Specify: select region Defining initial values of predefined field variables You can define initial values of predefined field variables. The values can be changed during an analysis . You must specify the field variable number being defined, n. Any number of field variables can be used; each must be numbered consecutively (1, 2, 3, etc.). Repeat the initial conditions definition, with a different field variable number, to define initial conditions for multiple field variables. The default is n=1. The definition of initial field variable values must be compatible with the section definition and with adjacent elements, as explained in “Predefined fields,” Section 33.6.1. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n Initial predefined field variables are not supported in Abaqus/CAE. Initializing predefined field variables with nodal temperature records from a user-specified results file You can define initial values of predefined field variables using nodal temperature records from a particular step and increment of a results file from a previous Abaqus analysis or from a results file you create . The previous analysis is most commonly an Abaqus/Standard heat transfer analysis. The use of the .fil file extension is optional. The part (.prt) file from the previous analysis is required to read the initial values of predefined field variables from the results file (“Defining an assembly,” Section 2.10.1). Both the previous model and the current model must be consistently defined in terms of an assembly of part instances. Input File Usage: *INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n, FILE=file, STEP=step, INC=inc Abaqus/CAE Usage: Initial predefined field variables are not supported in Abaqus/CAE. Defining initial predefined field variables using scalar nodal output from a user-specified output database file You can define initial values of predefined field variables using scalar nodal output variables from a particular step and increment in the output database file of a previous Abaqus/Standard analysis. For a list of scalar nodal output variables that can be used to initialize a predefined field, see “Predefined fields,” Section 33.6.1. The part (.prt) file from the previous analysis is required to read initial values from the output database file . Both the previous model and the current model must be defined consistently in terms of an assembly of part instances; node numbering must be the same, and part instance naming must be the same. The file extension is optional; however, only the output database file can be used for this option. Input File Usage: *INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n, FILE=file, OUTPUT VARIABLE=scalar nodal output variable, STEP=step, INC=inc Abaqus/CAE Usage: Initial predefined field variables are not supported in Abaqus/CAE. Defining initial predefined field variables by interpolating scalar nodal output variables for dissimilar meshes from a user-specified output database file When the mesh for one analysis is different from the mesh for the subsequent analysis, Abaqus can interpolate scalar nodal output variables (using the undeformed mesh of the original analysis) to predefined field variables that you choose. For a list of supported scalar nodal output variables that can be used to define predefined field variables, see “Predefined fields,” Section 33.6.1. This technique can also be used in cases where the meshes match but the node number or part instance naming differs between the analyses. Abaqus looks for the .odb extension automatically. The part (.prt) file from the previous analysis is required if that analysis model is defined in terms of an assembly of part instances . Input File Usage: *INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n, OUTPUT VARIABLE=scalar nodal output variable, INTERPOLATE, FILE=file, STEP=step, INC=inc Abaqus/CAE Usage: Initial predefined field variables are not supported in Abaqus/CAE. Defining initial fluid pressure in fluid-filled structures You can prescribe initial pressure for fluid-filled structures . Do not use this type of initial condition to define initial conditions in porous media in Abaqus/Standard; use initial pore fluid pressures instead . Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=FLUID PRESSURE Load module: Create Predefined Field: Step: Initial, choose Other for the Category and Fluid cavity pressure for the Types for Selected Step; select a fluid cavity interaction; Fluid cavity pressure: pressure Defining initial values of state variables for plastic hardening You can prescribe initial equivalent plastic strain and, if relevant, the initial backstress tensor for elements that use one of the metal plasticity (“Inelastic behavior,” Section 23.1.1) or Drucker-Prager (“Extended Drucker-Prager models,” Section 23.3.1) material models. These initial quantities are intended for materials in a work hardened state; they can be defined directly or by user subroutine HARDINI. You can also prescribe initial values for the volumetric compacting plastic strain, , for elements that use the crushable foam material model with volumetric hardening (“Crushable foam plasticity models,” Section 23.3.5). You can also specify multiple backstresses for the nonlinear kinematic hardening model. Optionally, you can specify the kinematic shift tensor (backstress) using the full tensor format, regardless of the element type to which the initial conditions are applied. Input File Usage: *INITIAL CONDITIONS, TYPE=HARDENING, NUMBER BACKSTRESSES=n, FULL TENSOR Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; select region; Number of backstresses: n Defining hardening parameters for rebars The hardening parameters can also be defined for rebars within elements. Rebars are discussed in “Defining rebar as an element property,” Section 2.2.4. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING, REBAR Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; select region; Definition: Rebar Defining hardening parameters in user subroutine HARDINI For complicated cases in Abaqus/Standard user subroutine HARDINI can be used to define the initial work hardening. In this case Abaqus/Standard will call the subroutine at the start of the analysis for each material point in the model. You can then define the initial conditions at each point as a function of coordinates, element number, etc. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING, USER Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; select region; Definition: User-defined Defining elements initially open for tangential fluid flow You can specify the pore pressure cohesive elements that are initially open for tangential fluid flow . Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=INITIAL GAP Initial gap is not supported in Abaqus/CAE. Defining initial mass flow rates in forced convection heat transfer elements In Abaqus/Standard you can define the initial mass flow rate through forced convection heat transfer elements. You can specify a predefined mass flow rate field to vary the value of the mass flow rate within the analysis step . Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=MASS FLOW RATE Initial mass flow rate is not supported in Abaqus/CAE. Defining initial values of plastic strain You can define an initial plastic strain field on elements that use one of the metal plasticity (“Inelastic behavior,” Section 23.1.1) or Drucker-Prager (“Extended Drucker-Prager models,” Section 23.3.1) material models. The specified plastic strain values will be applied uniformly over the element unless they are defined at each section point through the thickness in shell elements. If a local coordinate system was defined , the plastic strain components must be given in the local system. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=PLASTIC STRAIN Initial plastic strain conditions are not supported in Abaqus/CAE. Defining initial plastic strains for rebars Initial values of stress can also be defined for rebars within elements ( see “Defining rebar as an element property,” Section 2.2.4). Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=PLASTIC STRAIN, REBAR Initial plastic strain conditions are not supported in Abaqus/CAE. Defining initial pore fluid pressures in a porous medium In Abaqus/Standard you can define the initial pore pressure, , for nodes in a coupled pore fluid diffusion/stress analysis . The initial pore pressure can be defined either directly as an elevation-dependent function or by user subroutine UPOREP. Elevation-dependent initial pore pressures When an elevation-dependent pore pressure is prescribed for a particular node set, the pore pressure in the vertical direction (assumed to be the z-direction in three-dimensional and axisymmetric models and the y-direction in two-dimensional models) is assumed to vary linearly with this vertical coordinate. You must give two pairs of pore pressure and elevation values to define the pore pressure distribution throughout the node set. Enter only the first pore pressure value (omit the second pore pressure value and the elevation values) to define a constant pore pressure distribution. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=PORE PRESSURE Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Pore pressure for the Types for Selected Step; select region; Point 1 distribution: Uniform or select an analytical field Defining initial pore pressures in user subroutine UPOREP For complicated cases initial pore pressure values can be defined by user subroutine UPOREP. In this case Abaqus/Standard will make a call to subroutine UPOREP at the start of the analysis for all nodes in the model. You can define the initial pore pressure at each node as a function of coordinates, node number, etc. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=PORE PRESSURE, USER Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Pore pressure for the Types for Selected Step; select region; Point 1 distribution: User-defined Defining initial pore pressure values using nodal pore pressure output from a user-specified output database file You can define initial pore pressure values using nodal pore pressure output variables from a particular step and increment in the output database (.odb) file of a previous Abaqus/Standard analysis. The file extension is optional; however, only the output database file can be used. For the same mesh pore pressure mapping, both the previous model and the current model must be defined consistently, including node numbering, which must be the same in both models. If the models are defined in terms of an assembly of part instances, the part instance naming must be the same. Input File Usage: *INITIAL CONDITIONS, TYPE=PORE PRESSURE, FILE=file, STEP=step, INC=inc Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Pore pressure for the Types for Selected Step; select region; Point 1 distribution: From output database file Interpolating initial pore pressure values for dissimilar pore pressure mapping values in a user-specified output database file For dissimilar mesh pore pressure mapping, interpolation is required. You can also limit the interpolation region by specifying the source region in the form of an element set from which pore pressure is to be interpolated and the target region in the form of a node set onto which the pore pressure is mapped. Input File Usage: *INITIAL CONDITIONS, TYPE=PORE PRESSURE, FILE=file, INTERPOLATE, STEP=step, INC=inc *INITIAL CONDITIONS, TYPE=PORE PRESSURE, FILE=file, INTERPOLATE, STEP=step, INC=inc, DRIVING ELSETS Abaqus/CAE Usage: You cannot specify the regions where pore pressure values are to be interpolated in Abaqus/CAE. Defining initial pressure stress in a mass diffusion analysis In Abaqus/Standard you can specify the initial pressure stress, diffusion analysis . , at the nodes in a mass Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=PRESSURE STRESS Initial pressure stress is not supported in Abaqus/CAE. Defining initial pressure stress from a user-specified results file You can define initial values of pressure stress as those values existing at a particular step and increment in the results file of a previous Abaqus/Standard stress/displacement analysis . The use of the .fil file extension is optional. The initial values of pressure stress cannot be read from the results file when the previous model or the current model is defined in terms of an assembly of part instances (“Defining an assembly,” Section 2.10.1). Input File Usage: *INITIAL CONDITIONS, TYPE=PRESSURE STRESS, FILE=file, STEP=step, INC=inc Abaqus/CAE Usage: Initial pressure stress is not supported in Abaqus/CAE. Defining initial void ratios in a porous medium In Abaqus/Standard you can specify the initial values of the void ratio, e, at the nodes of a porous medium . The initial void ratio can be defined either directly as an elevation-dependent function, by interpolation from a previous output database file, or by user subroutine VOIDRI. Elevation-dependent initial void ratio When an elevation-dependent void ratio is prescribed for a particular node set, the void ratio in the vertical direction (assumed to be the z-direction in three-dimensional and axisymmetric models and the y-direction in two-dimensional models) is assumed to vary linearly with this vertical coordinate. When the void ratio is specified for a region meshed with fully integrated first-order elements, the nodal values of void ratio are interpolated to the centroid of the element and are assumed to be constant through the element. You must provide two pairs of void ratio and elevation values to define the void ratio throughout the node set. Enter only the first void ratio value (omit the second void ratio value and the elevation values) to define a constant void ratio distribution. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=RATIO Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step; select region; Point 1 distribution: Uniform or select an analytical field Defining void ratio from a user-specified output database You can define initial void ratios from the output database (.odb) file of a previous Abaqus/Standard soil analysis in which the void ratio is requested as output. Input File Usage: *INITIAL CONDITIONS, TYPE=RATIO, FILE=file, STEP=step, INC=inc Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step; select region; Point 1 distribution: From output database file Interpolating initial void ratios from values in a user-specified output database When you define initial void ratios from the output database (.odb) file of a previous Abaqus/Standard soil analysis, you can also limit the interpolation region by specifying the source region in the form of an element set from which void ratios are to be interpolated and the target region in the form of a node set onto which the void ratios are mapped. Input File Usage: *INITIAL CONDITIONS, TYPE=RATIO, INTERPOLATE, FILE=file, STEP=step, INC=inc, DRIVING ELSETS Abaqus/CAE Usage: You cannot specify the regions where void ratios are to be interpolated in Abaqus/CAE. Defining void ratios in user subroutine VOIDRI For complicated cases initial values of the void ratios can be defined by user subroutine VOIDRI. In this case Abaqus/Standard will make a call to subroutine VOIDRI at the start of the analysis for each material integration point in the model. You can then define the initial void ratio at each point as a function of coordinates, element number, etc. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=RATIO, USER Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step; select region; Point 1 distribution: User-defined Defining a reference mesh for membrane elements In Abaqus/Explicit you can specify a reference mesh (initial metric) for membrane elements. This is typically useful in finite element airbag simulations to model the wrinkles that arise from the airbag folding process. A flat mesh may be suitable for the unstressed reference configuration, but the initial state may require a corresponding folded mesh defining the folded state. Defining a reference configuration that is different from the initial configuration may result in nonzero stresses and strains in the initial configuration based on the material definition. If a reference mesh is specified for an element, any initial stress or strain conditions specified for the same element are ignored. If rebar layers are defined in membrane elements, the angular orientation defined in the reference configuration is updated to obtain the same orientation in the initial configuration. You can define the reference mesh using either the element numbers and the coordinates of the nodes in each element or the node numbers and the coordinates of the nodes. The coordinates of all of the nodes in the element have to be specified for both methods to have a valid initial condition for that element. The two alternatives are mutually exclusive. Input File Usage: Specifying the reference mesh using element numbers and coordinates of all of the element’s nodes: *INITIAL CONDITIONS, TYPE=REF COORDINATE Specifying the reference mesh using node numbers and the coordinates of the nodes: *INITIAL CONDITIONS, TYPE=NODE REF COORDINATE The specification of a reference mesh for membrane elements is not supported in Abaqus/CAE. Abaqus/CAE Usage: Defining initial relative density You can specify the initial values of the relative density field for a porous metal plasticity material model or equations of state . Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=RELATIVE DENSITY Initial relative density is not supported in Abaqus/CAE. Defining initial angular and translational velocity You can prescribe initial velocities in terms of an angular velocity and a translational velocity. This type of initial condition is typically used to define the initial velocity of a component of a rotating machine, such as a jet engine. The initial velocities are specified by giving the angular velocity, ; the axis of rotation, defined from a point a at . The initial ; and a translational velocity, velocity of node N at is then to a point b at Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=ROTATING VELOCITY Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Velocity for the Types for Selected Step Defining initial saturation for a porous medium In Abaqus/Standard you can define the initial saturation, s, for elements in a coupled pore fluid diffusion/stress analysis . Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=SATURATION Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Saturation for the Types for Selected Step Defining the initial values of solution-dependent state variables You can define initial values of solution-dependent state variables . The initial values can be defined directly or, in Abaqus/Standard, by user subroutine SDVINI. Values given directly will be applied uniformly over the element. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=SOLUTION Initial solution-dependent variables are not supported in Abaqus/CAE. Defining the initial values of solution-dependent state variables for rebars The initial values of solution-dependent variables can also be defined for rebars within elements. Rebars are discussed in “Defining rebar as an element property,” Section 2.2.4. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=SOLUTION, REBAR Initial solution-dependent state variables are not supported in Abaqus/CAE. Defining the initial values of solution-dependent state variables in user subroutine SDVINI For complicated cases in Abaqus/Standard user subroutine SDVINI can be used to define the initial values of solution-dependent state variables. In this case Abaqus/Standard will make a call to subroutine SDVINI at the start of the analysis for each material integration point in the model. You can then define all solution-dependent state variables at each point as functions of coordinates, element number, etc. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=SOLUTION, USER User subroutine SDVINI is not supported in Abaqus/CAE. Defining initial specific energy for equations of state In Abaqus/Explicit you can specify the initial values of the specific energy for equations of state . Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY Initial specific energy is not supported in Abaqus/CAE. Defining spud can embedment or spud can preload In Abaqus/Standard you can define an initial embedment of a spud can. Alternatively, you can define an initial vertical preload of a spud can . Input File Usage: Use one of the following options: *INITIAL CONDITIONS, TYPE=SPUD EMBEDMENT *INITIAL CONDITIONS, TYPE=SPUD PRELOAD Initial spud can embedment and preload are not supported in Abaqus/CAE. Abaqus/CAE Usage: Defining initial stresses You can define an initial stress field. Initial stresses can be defined directly or, in Abaqus/Standard, by user subroutine SIGINI. Stress values given directly will be applied uniformly over the element unless they are defined at each section point through the thickness in shell elements. If a local coordinate system was defined , stresses must be given in the local system. In soils (porous medium) problems the initial effective stress should be given; see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1, for a discussion of defining initial conditions in porous media. If the section properties of beam elements or shell elements are defined by a general section, the initial stress values are applied as initial section forces and moments. In the case of beams initial conditions can be specified only for the axial force, the bending moments, and the twisting moment. In the case of shells initial conditions can be specified only for the membrane forces, the bending moments, and the twisting moment. In both shells and beams initial conditions cannot be prescribed for the transverse shear forces. Initial stress fields cannot be defined for spring elements. See “Springs,” Section 32.1.1, for a discussion of defining initial forces in spring elements. Initial stress fields cannot be defined for elements using a fabric material. However, an initial stress and strain state can be introduced in a fabric material made of membrane elements by defining a reference mesh . Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=STRESS Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step Defining initial stresses for rebars Initial values of stress can also be defined for rebars within elements . Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=STRESS, REBAR Initial stress for rebars is not supported in Abaqus/CAE. Defining initial stresses that vary through the thickness of shell elements Initial values of stress can be defined at each section point through the thickness of shell elements. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=STRESS, SECTION POINTS Definition of initial stress that varies through the thickness of shell elements is not supported in Abaqus/CAE. Defining initial stresses in user subroutine SIGINI For complicated cases (such as elbow elements) in Abaqus/Standard the initial stress field can be defined by user subroutine SIGINI. In this case Abaqus/Standard will make a call to subroutine SIGINI at the start of the analysis for each material calculation point in the model. You can then define all active stress components at each point as functions of coordinates, element number, etc. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=STRESS, USER User subroutine SIGINI is not supported in Abaqus/CAE. Defining initial stresses using stress output from a user-specified output database file You can define initial stresses using stress output variables from a particular step and increment in the output database (.odb) file of a previous Abaqus/Standard analysis. In this case both the previous model and the current model must be defined consistently. The element numbering and element types must be the same in both models. If the models are defined in terms of an assembly of part instances, part instance naming must be the same. The file extension is optional; however, only the output database file can be used. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=STRESS, FILE=file, STEP=step, INC=inc Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step; select region; Specification: From output database file Establishing equilibrium in Abaqus/Standard When initial stresses are given in Abaqus/Standard (including prestressing in reinforced concrete or interpolation of an old solution onto a new mesh), the initial stress state may not be an exact equilibrium state for the finite element model. Therefore, an initial step should be included to allow Abaqus/Standard to check for equilibrium and iterate, if necessary, to achieve equilibrium. In a soils analysis (that is, for models containing elements that include pore fluid pressure as a variable) the geostatic stress field procedure (“Geostatic stress state,” Section 6.8.2) should be used for the equilibrating step. Any initial loading (such as geostatic gravity loads) that contributes to the initial equilibrium should be included in this step definition. The initial time increment and the total time specified in this step should be the same. The initial stresses are applied in full at time zero; and if equilibrium can be achieved, this step will converge in one increment. Therefore, there is no benefit to incrementing. To achieve equilibrium for all other analyses, a first step using the static procedure (“Static stress analysis,” Section 6.2.2) should be used. It is recommended that you specify the initial time increment to be equal to the total time specified in this step so that Abaqus/Standard will attempt to find equilibrium in one increment. By default, Abaqus/Standard ramps down the unbalanced stress over the first step. This allows Abaqus/Standard to use automatic incrementation if equilibrium cannot be found in one increment. This ramping is achieved in the following manner: 1. An additional set of artificial stresses is defined at each material point. These stresses are equal in magnitude to the initial stresses but are of opposite sign. The sum of the material point stresses and these artificial stresses creates zero internal forces at the beginning of the step. 2. The internal artificial stresses are ramped off linearly in time during the first step. Thus, at the end of the step the artificial stresses have been removed completely and the remaining stresses in the material will be the stress state in equilibrium. You can force Abaqus/Standard to achieve equilibrium in one increment by using a step variation on the initial condition to resolve the unbalanced stress instead of ramping the stress down over the entire step. If Abaqus/Standard cannot achieve equilibrium in one increment, the analysis will terminate. If the equilibrating step does not converge, it indicates that the initial stress state is so far from equilibrium with the applied loads that significantly large deformations would be generated. This is generally not the intention of an initial stress state; therefore, it suggests that you should recheck the specified initial stresses and loads. Input File Usage: Use one of the following options to specify how the unbalanced stress should be resolved: *INITIAL CONDITIONS, TYPE=STRESS, UNBALANCED STRESS=RAMP (default) *INITIAL CONDITIONS, TYPE=STRESS, UNBALANCED STRESS=STEP Abaqus/CAE Usage: Initial equilibrium stress is not supported in Abaqus/CAE. Establishing equilibrium in Abaqus/Explicit Abaqus/Explicit computes the initial acceleration at nodes taking into account the initial stresses, the loads, and the boundary conditions in the initial configuration. For an initially static problem, the specified boundary conditions, the initial stresses, and the initial loading should be consistent with a static equilibrium. Otherwise, the solution is likely to be noisy. The noise may be reduced by introducing a dummy step with a temporary viscous loading to attempt to reestablish a static equilibrium. Alternatively, you can introduce an initial short step in which all degrees of freedom are fixed with boundary conditions (all initial loads should be included in this initial step); in a second step, release all but the actual boundary conditions. Defining elevation-dependent (geostatic) initial stresses You can define elevation-dependent initial stresses. When a geostatic stress state is prescribed for a particular element set, the stress in the vertical direction (assumed to be the z-direction in three-dimensional and axisymmetric models and the y-direction in two-dimensional models) is assumed to vary (piecewise) linearly with this vertical coordinate. For the vertical stress component, you must give two pairs of stress and elevation values to define the stress throughout the element set. For material points lying between the two elevations given, Abaqus will use linear interpolation to determine the initial stress; for points lying outside the two elevations given, Abaqus will use linear extrapolation. In addition, horizontal (lateral) stress components are given by entering one or two “coefficients of lateral stress,” which define the lateral direct stress components as the vertical stress at the point multiplied by the value of the coefficient. In axisymmetric cases only one value of the coefficient of lateral stress is used and, therefore, only one value need be entered. Geostatic initial stresses are for use with continuum elements only. In Abaqus/Standard elevation-dependent initial stresses should be specified for beams and shells in user subroutine SIGINI, as explained earlier. In Abaqus/Explicit elevation-dependent initial stresses cannot be specified for beams and shells. The geostatic stress state specified initially should be in equilibrium with the applied loads (such as gravity) and boundary conditions. An initial step should be included to allow Abaqus to check for equilibrium after this interpolation has been done; see the discussion above on establishing equilibrium when an initial stress field is applied. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Geostatic stress for the Types for Selected Step Defining initial temperatures You can define initial temperatures at the nodes of either heat transfer or stress/displacement elements. The temperatures of stress/displacement elements can be changed during an analysis . The definition of initial temperature values must be compatible with the section definition of the element and with adjacent elements, as explained in “Predefined fields,” Section 33.6.1. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=TEMPERATURE Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step Defining initial temperatures from a user-specified results or output database file You can define initial temperatures as those values existing as nodal temperatures at a particular step and increment in the results or output database file of a previous Abaqus/Standard heat transfer analysis . The part (.prt) file from the previous analysis is required to read initial temperatures from the results or output database file . Both the previous model and the current model must be consistently defined in terms of an assembly of part instances; node numbering must be the same, and part instance naming must be the same. The file extension is optional; however, if both results and output database files exist, the results file will be used. Input File Usage: *INITIAL CONDITIONS, TYPE=TEMPERATURE, FILE=file, STEP=step, INC=inc Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file, Step: step, and Increment: inc Interpolating initial temperatures for dissimilar meshes from a user-specified results or output database file When the mesh for the heat transfer analysis is different from the mesh for the subsequent stress/displacement analysis, Abaqus can interpolate the temperature values from the nodes in the undeformed heat transfer model to the current nodal temperatures. This technique can also be used in cases where the meshes match but the node number or part instance naming differs between the analyses. Only temperatures from an output database file can be used for the interpolation; Abaqus will look for the .odb extension automatically. The part (.prt) file from the previous analysis is required if that analysis model is defined in terms of an assembly of part instances . Input File Usage: *INITIAL CONDITIONS, TYPE=TEMPERATURE, INTERPOLATE, FILE=file, STEP=step, INC=inc Abaqus/CAE Usage: Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file, Mesh compatibility: Incompatible Interpolating initial temperatures for dissimilar meshes with user-specified regions When regions of elements in the heat transfer analysis are close or touching, the dissimilar mesh interpolation capability can result in an ambiguous temperature association. For example, consider a node in the current model that lies on or close to a boundary between two adjacent parts in the heat transfer model, and consider a case where temperatures in these parts are different. When interpolating, Abaqus will identify a corresponding parent element at the boundary for this node from the heat transfer analysis. This parent element identification is done using a tolerance-based search method. Hence, in this example the parent element might be found in either of the adjacent parts, resulting in an ambiguous temperature definition at the node. You can eliminate this ambiguity by specifying the source regions from which temperatures are to be interpolated. The source region refers to the heat transfer analysis and is specified by an element set. The target region refers to the current analysis and is specified by a node set. Input File Usage: *INITIAL CONDITIONS, TYPE=TEMPERATURE, INTERPOLATE, FILE=file, STEP=step, INC=inc, DRIVING ELSETS Abaqus/CAE Usage: You cannot specify the regions where temperatures are to be interpolated in Abaqus/CAE. Interpolating initial temperatures for meshes that differ only in element order from a user-specified results or output database file If the only difference in the meshes is the element order (first-order elements in the heat transfer model and second-order elements in the stress/displacement model), in Abaqus/Standard you can indicate that midside node temperatures in second-order elements are to be interpolated from corner node temperatures read from the results or output database file of the previous heat transfer analysis using first-order elements. You must ensure that the corner node temperatures are not defined using a mixture of direct data input and reading from the results or output database file, since midside node temperatures that give unrealistic temperature fields may result. In practice, the capability for calculating midside node temperatures is most useful when temperatures generated by a heat transfer analysis are read from the results or output database file for the whole mesh during the stress analysis. Once the midside node capability is activated, the capability will remain active for the rest of the analysis, including for any predefined temperature fields defined to change temperatures during the analysis. The general interpolation and midside node capabilities are mutually exclusive. Input File Usage: *INITIAL CONDITIONS, TYPE=TEMPERATURE, MIDSIDE, FILE=file, STEP=step, INC=inc Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file, Step: step, Increment: inc, Mesh compatibility: Compatible, and toggle on Interpolate midside nodes Defining initial velocities for specified degrees of freedom You can define initial velocities for specified degrees of freedom. When initial velocities are given for dynamic analysis, they should be consistent with all of the constraints on the model, especially time- dependent boundary conditions. Abaqus will ensure that they are consistent with boundary conditions and with multi-point and equation constraints but will not check for consistency with internal constraints such as incompressibility of the material. In case of conflict, boundary conditions take precedence over initial conditions. Initial velocities must be defined in global directions, regardless of the use of local transformations (“Transformed coordinate systems,” Section 2.1.5). Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=VELOCITY Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Velocity for the Types for Selected Step Defining initial volume fractions for Eulerian elements You can define initial volume fractions to create material within Eulerian elements in Abaqus/Explicit. By default, these elements are filled with void. See “Initial conditions” in “Eulerian analysis,” Section 14.1.1, for a description of strategies for initializing Eulerian materials. Input File Usage: *INITIAL CONDITIONS, TYPE=VOLUME FRACTION Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Material Assignment for the Types for Selected Step Reading the input data from an external file The input data for an initial conditions definition can be contained in a separate file. See “Input syntax rules,” Section 1.2.1, for the syntax of such file names. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, INPUT=file_name Initial conditions cannot be read from a separate file in Abaqus/CAE. Consistency with kinematic constraints Abaqus does not ensure that initial conditions are consistent with multi-point or equation constraints for nodal quantities other than velocity . Initial conditions on nodal quantities such as temperature in heat transfer analysis, pore pressure in soils analysis, or acoustic pressure in acoustic analysis must be prescribed to be consistent with any multi-point constraint or equation constraint governing these quantities. Spatial interpolation method When you define initial conditions using a method that interpolates between dissimilar meshes, Abaqus operates by interpolating results from nodes in the old mesh to nodes in the new mesh. For each node: 1. The element (in the old mesh) in which the node lies is found, and the node’s location in that element is obtained. (This procedure assumes that all nodes in the new mesh lie within the bounds of the old mesh: warning messages are issued if this is not so.) 2. The initial condition values are then interpolated from the nodes of the element (in the old mesh) to the new node. 33.2.2 INITIAL CONDITIONS IN Abaqus/CFD Products: Abaqus/CFD Abaqus/CAE References • “Prescribed conditions: overview,” Section 33.1.1 • “Using the predefined field editors,” Section 16.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview In Abaqus/CFD initial conditions for fluid flow simulation are specified using element sets. Defining initial velocities You can define the initial fluid flow velocity in elements; however, if such conditions are omitted, a default value of zero is assumed. Initial velocities must be defined in global directions, regardless of the use of local transformations . For incompressible flow Abaqus/CFD automatically uses the user-defined boundary conditions and tests the specified initial velocity to be sure that the initial velocity field is divergence-free and that the velocity boundary conditions are compatible with the initial velocity field. If they are not, the initial velocity is projected onto a divergence-free subspace, yielding initial conditions that define a well-posed incompressible Navier-Stokes problem. Therefore, in some circumstances, the user-specified initial velocity may be overridden with a velocity that is divergence-free and matches the velocity boundary conditions. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=VELOCITY, ELEMENT AVERAGE Load module: Create Predefined Field: Step: Initial: Category: Fluid: Fluid velocity Defining initial density You can define the initial fluid density in elements. However, if the initial condition is omitted, the material density definition is assumed as default . Similarly, if the initial density is specified on an element set that does not include all fluid elements, the material density is assumed as the default for those elements not contained in the element set. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=DENSITY, ELEMENT AVERAGE Load module: Create Predefined Field: Step: Initial: Category: Fluid: Fluid density Initial pressure for incompressible fluid flow For incompressible flows it is not necessary to prescribe the initial pressure condition since the initial pressure field is computed automatically from the initial velocity field and boundary conditions. This is done to ensure proper starting conditions for incompressible flows. Defining initial temperature If the energy equation is solved, the initial fluid temperature in elements must be defined. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=TEMPERATURE, ELEMENT AVERAGE Load module: Create Predefined Field: Step: Initial: Category: Fluid: Fluid thermal energy Defining initial Spalart-Allmaras turbulent eddy viscosity for fluid flow If the Spalart-Allmaras turbulence model is active, you must prescribe an initial value for the Spalart- Allmaras turbulent eddy viscosity that is greater than zero and roughly three to five times the kinematic viscosity. The kinematic viscosity is the ratio of the fluid viscosity and density ( ). For more information, see “Viscosity,” Section 26.1.4. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=TURBNU, ELEMENT AVERAGE Load module: Create Predefined Field: Step: Initial: Category: Fluid: Fluid turbulence; Eddy viscosity: Defining initial k and for fluid flow If the RNG k– turbulence model is active, initial conditions need to be specified for both k and . The k and values must be greater than zero. A simple procedure to approximate the initial conditions can be obtained from values of the turbulence intensity and an approximate initial turbulent eddy viscosity as described below. The turbulent kinetic energy is defined as where characteristic velocity scale of the flow ( is the characteristic velocity scale or root mean square velocity that is usually related to the ) through the turbulence intensity, Therefore, an estimation for the initial conditions for the turbulent kinetic energy, k, can be expressed in terms of the characteristic velocity and turbulence intensity as The initial value for the turbulent kinetic energy dissipation, , can be obtained from a known/proposed level of the turbulent eddy viscosity, , as where is the k– turbulent viscosity model coefficient and is the fluid kinematic viscosity. Input File Usage: Use the following option to specify the initial turbulent kinetic energy: *INITIAL CONDITIONS, TYPE=TURBKE, ELEMENT AVERAGE Use the following option to specify the initial dissipation rate: turbulent kinetic energy *INITIAL CONDITIONS, TYPE=TURBEPS, ELEMENT AVERAGE Load module: Create Predefined Field: Step: Initial: Category: Fluid: Fluid turbulence; Turbulent kinetic energy: k, Dissipation rate: Abaqus/CAE Usage: 33.3 Boundary conditions • “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1 • “Boundary conditions in Abaqus/CFD,” Section 33.3.2 33.3.1 BOUNDARY CONDITIONS IN Abaqus/Standard AND Abaqus/Explicit Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Defining a model in Abaqus,” Section 1.3.1 • “Prescribed conditions: overview,” Section 33.1.1 • “VDISP,” Section 1.2.1 of the Abaqus User Subroutines Reference Manual • “DISP,” Section 1.1.4 of the Abaqus User Subroutines Reference Manual • *BOUNDARY • “Using the boundary condition editors,” Section 16.10 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Boundary conditions: • can be used to specify the values of all basic solution variables (displacements, rotations, warping amplitude, fluid pressures, pore pressures, temperatures, electrical potentials, normalized concentrations, acoustic pressures, or connector material flow) at nodes; • can be given as “model” input data (within the initial step in Abaqus/CAE) to define zero-valued boundary conditions; • can be given as “history” input data (within an analysis step) to add, modify, or remove zero-valued or nonzero boundary conditions; and • can be defined by the user through subroutines DISP for Abaqus/Standard and VDISP for Abaqus/Explicit. Relative motions in connector elements can be prescribed similar to boundary conditions. “Connector actuation,” Section 31.1.3, for more detailed information. See Prescribing boundary conditions as model data Only zero-valued boundary conditions can be prescribed as model data (i.e., in the initial step in Abaqus/CAE). You can specify the data using either “direct” or “type” format. As described below, the “type” format is a way of conveniently specifying common types of boundary conditions in stress/displacement analyses. “Direct” format must be used in all other analysis types. For both “direct” and “type” format you specify the region of the model to which the boundary conditions apply and the degrees of freedom to be restrained. Boundary conditions prescribed as model data can be modified or removed during analysis steps. Input File Usage: Abaqus/CAE Usage: Using the direct format *BOUNDARY Any number of data lines can be used to specify boundary conditions, and in stress/displacement analyses both “direct” and “type” format can be specified with a single use of the *BOUNDARY option. Load module: Create Boundary Condition: Step: Initial You can choose to enter the degrees of freedom to be constrained directly. Input File Usage: Either a single degree of freedom or the first and last of a range of degrees of freedom can be specified. *BOUNDARY node or node set, degree of freedom *BOUNDARY node or node set, first degree of freedom, last degree of freedom For example, *BOUNDARY EDGE, 1 indicates that all nodes in node set EDGE are constrained in degree of freedom 1 ( ), while the data line EDGE, 1, 4 indicates that all nodes in node set EDGE are constrained in degrees of freedom 1–4 ( ). , , , Abaqus/CAE Usage: Load module: Create Boundary Condition: Step: Initial Use one of the following options: Category: Mechanical; Displacement/Rotation, Velocity/Angular velocity, or Acceleration/Angular acceleration; select regions and toggle on the degree or degrees of freedom Category: Electrical/Magnetic; Electric potential; select regions Category: Other; Temperature, Pore pressure, Mass concentration, Acoustic pressure, or Connector material flow; select regions If you are specifying a temperature boundary condition for a shell region, you can enter multiple degrees of freedom, from 11 to 31, inclusive. Using the “type” format in stress/displacement analyses The type of boundary condition can be specified instead of degrees of freedom. The following boundary condition “types” are available in both Abaqus/Standard and Abaqus/Explicit: XSYMM Symmetry about a plane (degrees of freedom ). YSYMM ZSYMM ENCASTRE PINNED Symmetry about a plane Symmetry about a plane Fully built-in (degrees of freedom Pinned (degrees of freedom (degrees of freedom (degrees of freedom ). ). ). ). The following boundary condition types are available only in Abaqus/Standard: XASYMM YASYMM ZASYMM Antisymmetry about a plane with Antisymmetry about a plane with Antisymmetry about a plane with (degrees of freedom 2, 3, 4 (degrees of freedom 1, 3, 5 (degrees of freedom 1, 2, 6 ). ). ). Caution: When boundary conditions are prescribed at a node in an analysis involving finite rotations, at least two rotation degrees of freedom should be constrained. Otherwise, the prescribed rotation at the node may not be what you expect. Therefore, antisymmetry boundary conditions should generally not be used in problems involving finite rotations. NOWARP NOOVAL NODEFORM Prevent warping of an elbow section at a node. Prevent ovalization of an elbow section at a node. Prevent all cross-sectional deformation (warping, ovalization, and uniform radial expansion) at a node. The NOWARP, NOOVAL, and NODEFORM types apply only to elbow elements (“Pipes and pipebends with deforming cross-sections: elbow elements,” Section 29.5.1). For example, applying a boundary condition of type XSYMM to node set EDGE indicates that the node set lies on a plane of symmetry that is normal to the X-axis (which will be the global X-axis or the local X-axis if a nodal transformation has been applied at these nodes). This boundary condition is identical to applying a boundary condition using the direct format to degrees of freedom 1, 5, and 6 in node set EDGE since symmetry about a plane X=constant implies , and . , Once a degree of freedom has been constrained using a “type” boundary condition as model data, the constraint cannot be modified by using a boundary condition in “direct” format as model data; modifying a constraint in such a way will only produce an error message in the data (.dat) file indicating that conflicting boundary conditions exist in the model data. Input File Usage: *BOUNDARY node or node set, boundary condition type Abaqus/CAE Usage: Load module: Create Boundary Condition: Step: Initial: Symmetry/Antisymmetry/Encastre: select regions and toggle on the boundary condition type Prescribing boundary conditions at phantom nodes for enriched elements For an enriched element , you can specify the boundary conditions at a phantom node that is originally located coincident with the specified real node. Input File Usage: Use the following option to specify boundary conditions at a phantom node originally located coincident with the specified real node: *BOUNDARY, PHANTOM=NODE node number, first degree of freedom, last degree of freedom Abaqus/CAE Usage: Prescribing boundary conditions at phantom nodes for enriched elements is not supported in Abaqus/CAE. Prescribing boundary conditions as history data Boundary conditions can be prescribed within an analysis step using either “direct” or “type” format. As with model data boundary conditions, the “type” format can be used only in stress/displacement analyses; whereas, the “direct” format can be used in analysis types. When using the “direct” format, boundary conditions can be defined as the total value of a variable or, in a stress/displacement analysis, as the value of a variable’s velocity or acceleration. As many boundary conditions as necessary can be defined in a step. Input File Usage: Abaqus/CAE Usage: *BOUNDARY Load module: Create Boundary Condition: Step: analysis_step Using the direct format Specify the region of the model to which the boundary conditions apply, the degree or degrees of freedom to be specified , and the magnitude of the boundary condition. If the magnitude is omitted, it is the same as specifying a zero magnitude. In stress/displacement analysis you can specify a velocity history or an acceleration history. The default is a displacement history. Input File Usage: Use either of the following options to prescribe a displacement history: *BOUNDARY or *BOUNDARY, TYPE=DISPLACEMENT node or node set, degree of freedom, magnitude node or node set, first degree of freedom, last degree of freedom, magnitude Use the following option to prescribe a velocity history (the data lines are the same as above): *BOUNDARY, TYPE=VELOCITY Use the following option to prescribe an acceleration history (the data lines are the same as above): *BOUNDARY, TYPE=ACCELERATION For example, *BOUNDARY, TYPE=VELOCITY EDGE, 1, 1, 0.5 indicates that all nodes in node set EDGE have a prescribed velocity magnitude of 0.5 in degree of freedom 1 ( ). Abaqus/CAE Usage: Load module: Create Boundary Condition: Step: analysis_step: Select one of the following categories and types: Category: Mechanical; Displacement/Rotation; select regions; Distribution: Uniform or select an analytical field or a discrete field; toggle on the degree or degrees of freedom; magnitude Category: Mechanical; Velocity/Angular velocity or Acceleration/Angular acceleration; select regions; Distribution: Uniform or select an analytical field; toggle on the degree or degrees of freedom; magnitude Category: Electrical/Magnetic; Electric potential; select regions; Distribution: Uniform or select an analytical field; Method: Specify magnitude; magnitude Category: Other; Temperature, Pore pressure, Mass concentration, Acoustic pressure, or Connector material flow; select regions; Distribution: Uniform or select an analytical field; Method: Specify magnitude; magnitude If you are specifying a temperature boundary condition for a shell region, you can enter multiple degrees of freedom, from 11 to 31, inclusive. Prescribed displacement In Abaqus/Standard you can prescribe jumps in displacements. For example, a displacement-type boundary condition is used to apply a prescribed displacement magnitude of 0.5 in degree of freedom 1 ) to the nodes in node set EDGE. In a second step these nodes can be moved by another 0.5 length ( units (to a total displacement of 1.0) by applying a prescribed displacement magnitude of 1.0 in degree of freedom 1 to node set EDGE. Specifying a prescribed displacement magnitude of 0 (or omitting the magnitude) in degree of freedom 1 in the next step would return the nodes in node set EDGE to their original locations. In contrast, Abaqus/Explicit does not admit jumps in displacements and rotations. Displacement boundary conditions in displacement and rotation degrees of freedom are enforced in an incremental manner using the slope of the amplitude curve . If no amplitude is specified, Abaqus/Explicit will ignore the user-supplied displacement value and enforce a zero velocity boundary condition. The displacement must remain continuous across steps. If amplitude curves are specified, it is possible, but not valid, to specify a jump in the displacement across a step boundary when using step time for the amplitude definition. Abaqus/Explicit will ignore such jumps in displacement if they are specified. Using the “type” format in stress/displacement analyses The type of boundary condition can be specified (as history data) instead of degrees of freedom in the same manner as discussed above for model data. The boundary condition “types” that are available as history data are the same as those available as model data. Once a degree of freedom has been constrained using a “type” boundary condition as history data, the constraint cannot be modified by using a boundary condition in “direct” format. The constraint can be redefined only by using a boundary condition in “direct” format after all previously applied boundary conditions specified using “type” format are removed. Input File Usage: *BOUNDARY node or node set, boundary condition type Abaqus/CAE Usage: Load module: Create Boundary Condition: Step: analysis_step: Symmetry/Antisymmetry/Encastre: select regions and toggle on the boundary condition type Prescribing boundary conditions at phantom nodes for enriched elements You can specify boundary conditions at phantom nodes as history data in the same manner as discussed above for model data . To specify nonzero boundary conditions, enter the actual magnitude. Input File Usage: Use the following option to specify boundary conditions at a phantom node originally located coincident with the specified real node: *BOUNDARY, PHANTOM=NODE node number, first degree of freedom, last degree of freedom, magnitude Abaqus/CAE Usage: Prescribing boundary conditions at phantom nodes for enriched elements is not supported in Abaqus/CAE. Defining boundary conditions that vary with time The prescribed magnitude of a basic solution variable, a velocity, or an acceleration can vary with time during a step according to an amplitude definition (“Amplitude curves,” Section 33.1.2). When an amplitude definition is used with a boundary condition in a dynamic or modal dynamic analysis, the first and second time derivatives of the constrained variable may be discontinuous. For example, Abaqus will compute the corresponding velocity and acceleration from a given displacement boundary condition. By default, Abaqus/Standard will smooth the amplitude curve so that the derivatives of the specified boundary condition will be finite. You must ensure that the applied values are correct after smoothing. Abaqus/Explicit does not apply default smoothing to discontinuous amplitude curves. To avoid the “noisy” solution that may result from discontinuities in Abaqus/Explicit, it is better to specify the velocity history of a node. See “Amplitude curves,” Section 33.1.2. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *AMPLITUDE, NAME=name *BOUNDARY, AMPLITUDE=name Load or Interaction module: Create Amplitude: Name: amplitude_name Load module: Create Boundary Condition: Step: analysis_step: boundary condition; Amplitude: amplitude_name Defining boundary condition through user subroutines If an amplitude based evolution of a boundary condition is not sufficient, you can define it yourself For this purpose, Abaqus/Standard provides the routine DISP; whereas, in a user subroutine. Abaqus/Explicit provides the routine VDISP. The region to which the boundary conditions apply and the constrained degrees of freedom are specified as part of the boundary condition definition. The actual boundary condition is set within the user routine based on a number of variables made available in those routines ( see “DISP,” Section 1.1.4 of the Abaqus User Subroutines Reference Manual for DISP and “VDISP,” Section 1.2.1 of the Abaqus User Subroutines Reference Manual for VDISP ). Abaqus/Standard allows for an amplitude and a reference magnitude definition for a user defined boundary condition and you may overwrite the amplitude based boundary value within the DISP routine. Whereas, Abaqus/Explicit ignores the reference magnitude, but passes in the amplitude value as an argument to the user routine VDISP and you may define the boundary condition to a non-zero value. Input File Usage: Abaqus/CAE Usage: *BOUNDARY, USER Load module: Create Boundary Condition: Step: analysis_step; boundary condition; Distribution: User-defined Boundary condition propagation By default, all boundary conditions defined in the previous general analysis step remain unchanged in the subsequent general step or in subsequent consecutive linear perturbation steps. Boundary conditions do not propagate between linear perturbation steps. You define the boundary conditions in effect for a given step relative to the preexisting boundary conditions. At each new step the existing boundary conditions can be modified and additional boundary conditions can be specified. Alternatively, you can release all previously applied boundary conditions in a step and specify new ones. In this case any boundary conditions that are to be retained must be respecified. Modifying boundary conditions When you modify an existing boundary condition, the node or node set must be specified in exactly the same way as previously. For example, if a boundary condition is specified for a node set in one step and for an individual node contained in the set in another step, Abaqus issues an error. You must remove the boundary condition and respecify it to change the way the node or node set is specified. Input File Usage: Use either of the following options to modify an existing boundary condition or to specify an additional boundary condition: Abaqus/CAE Usage: *BOUNDARY *BOUNDARY, OP=MOD Load module: Create Boundary Condition or Boundary Condition Manager: Edit Removing boundary conditions If you choose to remove any boundary condition in a step, no boundary conditions will be propagated from the previous general step. Therefore, all boundary conditions that are in effect during this step must be respecified. The only exception to this rule is during an eigenvalue buckling prediction procedure, as described in “Eigenvalue buckling prediction,” Section 6.2.3. Setting a boundary condition to zero is not the same as removing it. Input File Usage: Use the following option to release all previously applied boundary conditions and to specify new boundary conditions: Abaqus/CAE Usage: *BOUNDARY, OP=NEW If the OP=NEW parameter is used on any *BOUNDARY option within a step, it must be used on all *BOUNDARY options in the step. Use the following option to remove a boundary condition within a step: Load module: Boundary Condition Manager: Deactivate Abaqus/CAE automatically respecifies any boundary conditions that should remain in effect during this step. Fixing degrees of freedom at a point in an Abaqus/Standard analysis In Abaqus/Standard you can “freeze” specified degrees of freedom at their final values from the last general analysis step. Specifying a zero velocity or zero acceleration boundary condition will have the same effect as fixing the degrees of freedom for displacement or velocity, respectively. Input File Usage: Abaqus/CAE Usage: *BOUNDARY, FIXED The OP=NEW parameter must be used with the FIXED parameter if there are any other *BOUNDARY options in the same step that have the OP=NEW parameter. Any magnitudes given for the boundary condition are ignored. Load module; Create Boundary Condition; Step: analysis_step; boundary condition; Method: Fixed at Current Position (available only if a previous general analysis step exists) Prescribing boundary conditions in linear perturbation steps In a linear perturbation step (“General and linear perturbation procedures,” Section 6.1.3) the magnitudes of prescribed boundary conditions should be given as the magnitudes of the perturbations about the base state. Boundary conditions given within the model definition are always regarded as part of the base state, even if the first analysis step is a linear perturbation step. The boundary conditions given in a linear perturbation step will not affect subsequent steps. If a perturbation step does not contain a boundary condition definition, degrees of freedom that are restrained/prescribed in the base state will be restrained in the perturbation step and will have perturbation magnitudes of zero. To prescribe nonzero perturbation magnitudes, you have to modify the existing boundary conditions. You can also fix and prescribe perturbation magnitudes of degrees of freedom that are unrestrained in the base state. If degrees of freedom that are restrained/prescribed in the base state are released, all restraints that are to remain must be respecified, remembering that all magnitudes will be interpreted as perturbations. Fixing the degrees of freedom at their final values from the last general analysis step has the same effect as modifying the existing boundary conditions to have zero perturbation magnitudes for all specified degrees of freedom. The antisymmetric buckling modes of a symmetric structure can be found in an eigenvalue buckling prediction analysis by specifying the proper boundary conditions . Prescribing real and imaginary values in boundary conditions In steady-state dynamic and matrix generation procedures, a boundary condition can be prescribed using either a real or an imaginary value . If the real value is prescribed for a degree of freedom (and the imaginary value is not explicitly prescribed), the imaginary value is considered to be zero. Similarly, if the imaginary value is prescribed (and the real value is not explicitly prescribed), the real value is considered to be zero. Prescribed motion in modal superposition procedures In modal superposition procedures (“Dynamic analysis procedures: overview,” Section 6.3.1) prescribed displacements cannot be defined directly using a boundary condition. Instead, the boundary conditions are grouped into bases in a frequency extraction step. Then, the motion of each base is prescribed in the modal superposition step. See “Natural frequency extraction,” Section 6.3.5, and “Transient modal dynamic analysis,” Section 6.3.7, for details on this method. Input File Usage: Abaqus/CAE Usage: *BOUNDARY, BASE NAME *BASE MOTION Load module; Create Boundary Condition; Step: modal_dynamic_step, steady-state_dynamic_step, or random_response_step; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion Submodeling When using the submodeling technique, the magnitudes of the boundary conditions in the submodel can be defined by interpolating the values of the prescribed degrees of freedom from the file output results of the global model. See “Node-based submodeling,” Section 10.2.2, for details. Prescribing large rotations Sequential finite rotations about different axes of rotation are not additive, which can make direct It is much simpler to apply finite-rotation boundary specification of such rotations challenging. conditions by specifying the rotational velocity versus time. For a discussion of the rotation degrees of freedom and a multiple step finite rotation example that demonstrates why velocity-type boundary conditions are preferred for specifying finite-rotation boundary conditions, see “Conventions,” Section 1.2.2. When velocity-type boundary conditions are used to prescribe rotations, the definition is given in If the angular velocity is associated with terms of the angular velocity instead of the total rotation. a nondefault amplitude, Abaqus calculates the prescribed increment of rotation as the average of the prescribed angular velocities at the beginning and the end of each increment, multiplied by the time increment. In Abaqus/Explicit displacement-type boundary conditions that refer to an amplitude curve are effectively enforced as velocity boundary conditions using average velocities over time increments as computed by finite differences of values from the amplitude curve. As with prescribed displacements , Abaqus/Explicit does not admit jumps in rotations. Displacement-type boundary conditions in Abaqus/Standard that constrain just one component of rotation can have essentially no effect on the solution because the two unconstrained rotational degrees of freedom can combine to override the constraint. Example: Using velocity-type boundary conditions to prescribe rotations For example, if a rotation of about the z-axis is required in a static step, with no rotation about the x- and y-axes, use a step time (specified as part of the static step definition) of 1.0, and define a velocity- type boundary condition to specify zero velocity for degrees of freedom 4 and 5 and a constant angular velocity of for degree of freedom 6. Since the default variation for a velocity-type boundary condition in a static procedure is a step, the velocity will be constant over the step. Alternatively, an amplitude reference could be used to specify the desired variation over the step. *BOUNDARY, TYPE=VELOCITY NODE, 4 NODE, 5 NODE, 6, 6, 18.84955592 If, in the next step, the same node should have an additional rotation of radians about the global x-axis, use another static step with a step time of 1.0 and again define a velocity-type boundary condition to prescribe zero velocity for degrees of freedom 5 and 6 and a constant angular velocity of for degree of freedom 4. *BOUNDARY, TYPE=VELOCITY NODE, 4, 4, 1.570796327 NODE, 5 NODE, 6 Prescribing radial motion on an axisymmetric model The radial coordinate for any node in an axisymmetric model must be positive. Therefore, you must make sure that any specified boundary condition does not violate this condition. 33.3.2 BOUNDARY CONDITIONS IN Abaqus/CFD Products: Abaqus/CFD Abaqus/CAE References • “Distribution definition,” Section 2.8.1 • “Prescribed conditions: overview,” Section 33.1.1 • “Conventions,” Section 1.2.2 • *BOUNDARY • *DISTRIBUTION • *FLUID BOUNDARY • “Using the boundary condition editors,” Section 16.10 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Boundary conditions: • are used to prescribe the values of all primitive variables involved in a fluid dynamics calculation (e.g., velocities, temperatures, turbulence variables, wall-normal distance, etc.); • can be given as “history” input data (within an analysis step) to add, modify, or remove zero-valued or nonzero boundary conditions; and • can be prescribed through the use of a co-simulation region for multiphysics problems. Computational fluid dynamics problems typically require the prescription of multiple variables such as pressure, temperature, and velocity for boundary conditions. In practice, boundary conditions tend to appear together to collectively define a physical behavior; e.g., no-slip/no-penetration conditions at a wall. In contrast, Neumann conditions (e.g., prescribed heat flux) are specified as loads . In the absence of a prescribed boundary condition or load, the default behavior for Abaqus/CFD is to enforce a homogeneous (zero) Neumann condition. For example, if the temperature is not specified at a wall, the default behavior is to automatically specify a perfectly insulated boundary; i.e., zero normal heat flux. Similarly, if the velocity is not prescribed, the normal derivative of the velocity is set to zero. In Abaqus/CAE combinations of boundary conditions that represent an inflow, outflow, or wall behavior are grouped collectively for ease of use (for more information, see “Using the boundary condition editors,” Section 16.10 of the Abaqus/CAE User’s Manual). Active degrees of freedom In Abaqus/CFD the active fields (degrees of freedom) are determined by the analysis procedure and the options specified, such as turbulence models and auxiliary transport equations. You specify a boundary condition type to identify the degree of freedom for a fluid boundary condition. Element-based and node-based degrees of freedom and the analysis procedure and additional options required for activation, if any, are listed in Table 33.3.2–1 and Table 33.3.2–2, respectively. Table 33.3.2–1 Element-based degrees of freedom and activation options for fluid boundary conditions. Boundary condition type Description Incompressible flow TEMP TEMPn TURBEPS TURBEPSn TURBKE TURBKEn TURBNU TURBNUn VELX VELXn VELY VELYn VELZ VELZn VELXNU VELYNU Energy equation Energy equation RNG - model RNG - model RNG - model RNG - model Spalart-Allmaras model Spalart-Allmaras model — — — — — — — — Fluid temperature Fluid temperature on face n Turbulent energy dissipation rate ( ) Turbulent energy dissipation rate ( ) on face n Turbulent kinetic energy ( ) Turbulent kinetic energy ( ) on face n Turbulent kinematic eddy viscosity Turbulent kinematic eddy viscosity on face n x-velocity x-velocity on face n y-velocity y-velocity on face n z-velocity z-velocity on face n x-velocity defined via user subroutine y-velocity defined via user subroutine Description Incompressible flow Boundary condition type VELZNU z-velocity defined via user subroutine PASSIVEOUTFLOW Passive outflow PNU Fluid pressure Fluid pressure defined via user subroutine — — — — Table 33.3.2–2 Node-based degrees of freedom and activation options for fluid boundary conditions. Boundary condition type Description Incompressible flow PVDEP DIST Fluid pressure Fluid pressure that varies with the total volume of fluid crossing the boundary Wall-distance normal function — — — Prescribing inflow and outflow boundary conditions You can specify boundary conditions to describe the flow behavior where fluid enters the analysis domain and where the fluid leaves the analysis domain. Input File Usage: Use the following option to define inflow and outflow boundary conditions at surfaces: *FLUID BOUNDARY, TYPE=SURFACE surface name, boundary condition type label, magnitude where boundary condition type label is VELX, VELY, VELZ, VELXNU, VELYNU, VELZNU, TEMP, TURBKE, TURBEPS, TURBNU, P, PNU, or PASSIVEOUTFLOW. The value of magnitude is ignored for PASSIVEOUTFLOW. Use the following option to define distributed inflow and outflow boundary conditions at element faces: *FLUID BOUNDARY, TYPE=ELEMENT element set label, boundary condition type label, magnitude where boundary condition type label is VELXn, VELYn, VELZn, TEMPn, TURBKEn, TURBEPSn, or TURBNUn. Use the following option to define distributed inflow and outflow boundary conditions at nodes: *FLUID BOUNDARY, TYPE=NODE node set label, P, magnitude Abaqus/CAE Usage: Use the following option to define the inflow and outflow boundary conditions at surfaces: Load module: Create Boundary Condition: Step: flow_step: Category: Fluid: Fluid inlet/outlet: select inlet regions or outlet regions; and specify momentum (pressure or velocity), thermal energy (temperature), and turbulence conditions at the inlet or outlet Defining distributed inflow and outflow boundary conditions at element faces is supported in Abaqus/CAE only for velocity boundary conditions. Use the following option: Load module: Create Boundary Condition: Step: flow_step: Category: Fluid: Fluid inlet/outlet: select inlet regions or outlet regions; Momentum: toggle on Specify, and choose Velocity; Distribution: select an analytical field Defining distributed inflow and outflow boundary conditions at nodes is not supported in Abaqus/CAE. Inflow boundary conditions An inflow boundary condition is used to describe the flow behavior at a surface where fluid enters the analysis domain. For incompressible flows, inflow conditions can be prescribed for velocity or pressure, temperature, and turbulence variables. If boundary conditions are not specified explicitly for a variable, a homogeneous Neumann condition is assumed automatically. This corresponds to permitting the variable (e.g., temperature) to vary at the inflow and the incoming fluid to correspond to that local variable. Similarly, if pressure is not specified, its normal derivative at the inflow surface is automatically set to zero. The velocity components can be prescribed independently. Outflow boundary conditions An outflow boundary corresponds to a surface where the fluid flow leaves the analysis domain. In Abaqus/CFD outflow conditions are most frequently associated with a specified pressure. However, all other flow variables can be prescribed at an outflow boundary as well. Similar to an inflow boundary, when a variable is not specified, its normal derivative is assumed to be zero. As such, convective outflows carry their quantities out of the domain at a fixed level, resulting in essentially nonreflecting boundaries. Prescribing wall boundary conditions Wall boundary conditions are typically associated with the no-slip/no-penetration behavior at a solid surface. However, the behavior at a solid wall may also require the prescription of temperature and, optionally, turbulence variables depending on the flow conditions. In situations where a wall heat flux is required, a heat flux loading must be prescribed in addition to the wall boundary conditions. Depending on the physical properties of the wall, the wall boundary conditions can be modified to achieve a variety of physical behaviors that include slip, no-slip, infiltration, symmetry, etc. Input File Usage: Use the following option to define wall boundary conditions at surfaces: *FLUID BOUNDARY, TYPE=SURFACE surface name, boundary condition type label, magnitude where boundary condition type label is VELX, VELY, VELZ, VELXNU, VELYNU, VELZNU, TEMP, TURBKE, TURBEPS, TURBNU, P, PNU or DIST. Use the following option to define distributed wall boundary conditions at element faces: *FLUID BOUNDARY, TYPE=ELEMENT element set label, boundary condition type label, magnitude where boundary condition type label is VELXn, VELYn, VELZn, TEMPn, TURBKEn, TURBEPSn, or TURBNUn. Use the following option to define distributed wall boundary conditions at nodes: *FLUID BOUNDARY, TYPE=NODE node set label, P, magnitude For example, use the following settings for a no-slip/no-penetration wall that is not moving and with the Spalart-Allmaras turbulence model active (wall- normal distance boundary condition and turbulent eddy viscosity set to zero at the wall): *FLUID BOUNDARY, TYPE=SURFACE surface name, DIST, 0 surface name, VELX, 0 surface name, VELY, 0 surface name, VELZ, 0 surface name, TURBNU, 0 Abaqus/CAE Usage: Use the following option to define wall boundary conditions at surfaces: Load module: Create Boundary Condition: Step: flow_step: Category: Fluid: Fluid wall condition: select regions; select Condition: No slip, Shear, or Infiltration; and specify velocity, thermal energy (temperature), and turbulence conditions at the wall Defining distributed wall boundary conditions at elements is supported in Abaqus/CAE only for velocity boundary conditions at a slip wall or infiltration wall. Use the following option to define distributed wall boundary conditions at elements: Load module: Create Boundary Condition: Step: flow_step: Category: Fluid: Fluid wall condition: select regions; Velocity: Distribution: select an analytical field Defining distributed wall boundary conditions at nodes is not supported in Abaqus/CAE. No-slip/no-penetration wall A no-slip (and no-penetration) wall is a surface where the fluid adheres to the wall without penetrating it. No-slip/no-penetration conditions are prescribed by setting all velocity components equal to the wall velocity (zero if the wall is not moving). If a turbulence model is specified, the wall-normal distance boundary condition must be set to zero at the wall. The boundary conditions for the different turbulence variables depend on the model selected. For the Spalart-Allmaras model, the turbulent eddy viscosity, , is set to zero at the wall. For the RNG k– model, the wall boundary conditions are automatically are required implemented by the solver using the wall-function approach; no user settings for k or because they are prescribed automatically. Slip wall A slip wall is a surface where the fluid does not adhere to the wall but cannot penetrate it. This wall condition is modeled by specifying the wall-normal fluid velocity equal to the wall velocity (zero if the wall is not moving). This situation also represents a symmetry condition for fluid flow since the in-plane velocities can vary, but the out-of-plane velocity is zero. In cases where a moving boundary is being considered, an associated set of mesh displacement boundary conditions must be prescribed in conjunction with the surface fluid velocity to achieve the proper behavior. If a turbulence model is specified, the wall-normal distance boundary condition must be set to zero at the wall. Infiltration wall Infiltration at a surface permits the fluid to penetrate the surface while maintaining the no-slip condition. This wall condition is modeled by specifying the wall-normal velocity equal to the velocity representing the infiltration velocity, while the wall-tangent fluid velocity is equal to the wall velocity (zero if the wall is not moving). In the special case when a turbulence model is implemented, the wall-normal distance boundary condition must be set to zero at the wall. If the Spalart-Allmaras turbulence model is enabled, you can specify the value of the Spalart-Allmaras turbulent eddy viscosity, , that is allowed at the wall due to infiltration. If the RNG k– model is implemented, you can prescribe values at the wall for the turbulent kinetic energy, k, and the dissipation rate, . Prescribed temperature Temperatures can be prescribed at a wall. By default, if no temperature is prescribed at a wall, a perfectly insulated boundary is specified automatically. For multiphysics applications such as conjugate heat transfer, a variable temperature condition is imposed automatically using a co-simulation region (for more information, see “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1). Prescribed displacement Abaqus/CFD provides the capability to perform both deforming-mesh and fluid-structure interaction (FSI) simulations using an arbitrary Lagrangian-Eulerian (ALE) methodology for the fluid flow. For FSI and deforming-mesh problems, typically some portion of the fluid domain is deformed consistent with a boundary motion. To manage the mesh motion, you must prescribe displacement boundary conditions on the mesh. For FSI problems, displacement boundary conditions are not permitted at the co-simulation region because these conditions are prescribed automatically. Input File Usage: *BOUNDARY node or node set, first degree of freedom, last degree of freedom, magnitude Abaqus/CAE Usage: freedom is 1 for the x-displacement, 2 for the where first degree of y-displacement, or 3 for the z-displacement. Load module: Create Boundary Condition: Step: flow_step: Category: Mechanical: Displacement/Rotation: select regions and toggle on the degree or degrees of freedom Defining pressure boundary conditions that vary with the total volume of fluid crossing a surface Abaqus/CFD provides the capability to define pressure boundary conditions that vary with the total volume of fluid crossing a surface. The total volume of fluid crossing the surface is automatically calculated and used to determine the current amplitude of the applied pressure. Input File Usage: Use the following options: *DISTRIBUTION TABLE, NAME=table name *DISTRIBUTION, LOCATION=NONE, TABLE=table name, NAME=distribution name *FLUID BOUNDARY, TYPE=SURFACE, DISTRIBUTION=distribution name surface name, PVDEP, initial volume Abaqus/CAE Usage: Defining pressure boundary conditions that vary with the total volume of fluid crossing a surface is not supported in Abaqus/CAE. Defining boundary conditions that vary with time The prescribed magnitude of the boundary conditions can vary with time during a step according to an amplitude definition (“Amplitude curves,” Section 33.1.2). Input File Usage: Use both of the following options to define the prescribed displacement at a moving boundary: *AMPLITUDE, NAME=name *BOUNDARY, AMPLITUDE=name Use both of the following options to define inflow and outflow boundary conditions and wall boundary conditions that vary with time: *AMPLITUDE, NAME=name *FLUID BOUNDARY, AMPLITUDE=name Load or Interaction module: Create Amplitude: Name: amplitude_name Load module: Create Boundary Condition: Step: flow_step: boundary condition; Amplitude: amplitude_name Abaqus/CAE Usage: Boundary condition propagation By default, all boundary conditions defined in the previous general analysis step remain unchanged in the subsequent general step. You define the boundary conditions in effect for a given step relative to the preexisting boundary conditions. At each new step the existing boundary conditions can be modified and additional boundary conditions can be specified. Alternatively, you can release all previously applied boundary conditions in a step and specify new ones. In this case any boundary conditions that are to be retained must be respecified. Modifying boundary conditions When you modify an existing boundary condition, the node or node set must be specified in exactly the same way as previously. For example, if a boundary condition is specified for a node set in one step and for an individual node contained in the set in another step, Abaqus issues an error. You must remove the boundary condition and respecify it to change the way the node or node set is specified. Input File Usage: Use one of the following options to modify an existing boundary condition or to specify an additional boundary condition: *BOUNDARY *BOUNDARY, OP=MOD *FLUID BOUNDARY *FLUID BOUNDARY, OP=MOD Load module: Create Boundary Condition or Boundary Condition Manager: Edit Abaqus/CAE Usage: Removing boundary conditions If you choose to remove any boundary condition in a step, no boundary conditions will be propagated from the previous general step. Therefore, all boundary conditions that are in effect during this step must be respecified. Setting a boundary condition to zero is not the same as removing it. Input File Usage: Use one of the following options to release all previously applied boundary conditions and to specify new boundary conditions: *BOUNDARY, OP=NEW If the OP=NEW parameter is used on any *BOUNDARY option within a step, it must be used on all *BOUNDARY options in the step. *FLUID BOUNDARY, OP=NEW If the OP=NEW parameter is used on any *FLUID BOUNDARY option within a step, it must be used on all *FLUID BOUNDARY options in the step. Use the following option to remove a boundary condition within a step: Load module: Boundary Condition Manager: Deactivate Abaqus/CAE automatically respecifies any boundary conditions that should remain in effect during this step. Abaqus/CAE Usage: 33.4 Loads • “Applying loads: overview,” Section 33.4.1 • “Concentrated loads,” Section 33.4.2 • “Distributed loads,” Section 33.4.3 • “Thermal loads,” Section 33.4.4 • “Electromagnetic loads,” Section 33.4.5 • “Acoustic and shock loads,” Section 33.4.6 • “Pore fluid flow,” Section 33.4.7 33.4.1 APPLYING LOADS: OVERVIEW Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “General and linear perturbation procedures,” Section 6.1.3 • “Prescribed conditions: overview,” Section 33.1.1 • “Concentrated loads,” Section 33.4.2 • “Distributed loads,” Section 33.4.3 • “Thermal loads,” Section 33.4.4 • “Electromagnetic loads,” Section 33.4.5 • “Acoustic and shock loads,” Section 33.4.6 • “Pore fluid flow,” Section 33.4.7 • “Creating and modifying prescribed conditions,” Section 16.4 of the Abaqus/CAE User’s Manual • “Using the load editors,” Section 16.9 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview External loading can be applied in the following forms: • Concentrated or distributed tractions. • Concentrated or distributed fluxes. • Incident wave loads. Many types of distributed loads are provided; they depend on the element type and are described in Part VI, “Elements.” This section discusses general concepts that apply to all types of loading; see “Prescribed conditions: overview,” Section 33.1.1, for general information that applies to all types of prescribed conditions. Concentrated and distributed tractions are discussed in “Concentrated loads,” Section 33.4.2, and “Distributed loads,” Section 33.4.3, respectively. Thermal loading (heat flux) is discussed in “Thermal loads,” Section 33.4.4. Electromagnetic loads are discussed in “Electromagnetic loads,” Section 33.4.5. Loads due to incident wave fields such as due to sound sources or an underwater explosion are discussed in “Acoustic and shock loads,” Section 33.4.6. Pore fluid flow is discussed in “Pore fluid flow,” Section 33.4.7. All other load types, which are applicable to only a single type of analysis, are discussed in the appropriate sections in Part III, “Analysis Procedures, Solution, and Control.” In some situations, concentrated loads and some commonly used distributed loads (such as pressure applied on a surface) may rotate during a geometrically nonlinear analysis. Such loads are known as follower loads; further details on follower loads can be found in “Follower loads in large-displacement analysis;” “Specifying concentrated follower forces” in “Concentrated loads,” Section 33.4.2; “Follower surface loads” in “Distributed loads,” Section 33.4.3; and “Follower edge and line loads” in “Distributed loads,” Section 33.4.3. Follower loads may also lead to an unsymmetric contribution to the stiffness matrix, which is generally referred to as the load stiffness; some issues related to the load stiffness contribution are discussed in “Improving the rate of convergence in large-displacement implicit analysis” in “Concentrated loads,” Section 33.4.2, and “Improving the rate of convergence in large-displacement implicit analysis” in “Distributed loads,” Section 33.4.3. Element-based versus surface-based distributed loads There are two ways of specifying distributed loads in Abaqus: element-based distributed loads and surface-based distributed loads. Element-based distributed loads can be prescribed on element bodies, element surfaces, or element edges. Surface-based distributed loads can be prescribed on geometric surfaces or geometric edges. In Abaqus/CAE distributed surface and edge loads can be element-based or surface-based, while distributed body loads are prescribed on geometric bodies or element bodies. Element-based loads Use element-based loads to define distributed loads on element surfaces, element edges, and element bodies. With element-based loads you must provide the element number (or an element set name) and the distributed load type label. The load type label identifies the type of load and the element face or edge on which the load is prescribed . This method of specifying distributed loads is very general and can be used for all distributed load types and elements. Surface-based loads Use surface-based loads to prescribe a distributed load on a geometric surface or geometric edge. With surface-based loads you must specify the surface or edge name and the distributed load type. The surface or edge, which contains the element and face information, is defined as described in “Element-based surface definition,” Section 2.3.2. In Abaqus/CAE surfaces can be defined as collections of geometric faces and edges or collections of element faces and edges.This method of prescribing a distributed load facilitates user input for complex models. It can be used with most element types for which a valid surface can be defined. You can specify in the surface definition how the distributed load is applied to the boundary of an adaptive mesh domain in Abaqus/Explicit . Varying the magnitude of a load The magnitude of a load is usually defined by the input data. The variation of the load magnitude during a step can be defined by the default amplitude variation for the step ; by a user-defined amplitude curve ; or, in some cases, by user subroutine DLOAD, UDECURRENT, UDSECURRENT, UTRACLOAD, or VDLOAD. Loading during general analysis steps If the analysis consists of one step only, the loads are defined in that step. If there are several analysis steps, the definition of loading in each analysis step depends on whether that step and the previous steps are general analysis steps or linear perturbation steps. Loading during linear perturbation steps is discussed below. In general analysis steps, load magnitudes must always be given as total values, not as changes in magnitude. Multiple definitions of the same load condition in the same step are applied additively. Element-based and surface-based distributed loads are considered independently. For example, element- based and surface-based pressures applied to an element face in the same step are added. A single redefinition of that same load condition in a subsequent step, however, replaces all the like definitions (same load option, same load type) given in previous steps according to the rules described in “Removing loads” below. Any combination of loads can be applied together during a step. For a linear step it is possible to analyze several load cases based on the same stiffness. Modifying loads At each new step the loading can be either modified or completely redefined. To redefine a load, the node, element, node set, element set, or surface name must be specified in exactly the same way and the load type must be identical. For example, if a node is part of a loaded node set in one step and is loaded as an individual node (by listing its node number) in another step, the loads will be added. All loads defined in previous steps remain unchanged unless they are redefined. When a load is left unchanged, the following rules apply: • If the associated amplitude was specified in terms of total time, the load continues to follow the amplitude definition. • If no amplitude was associated with the load or if the amplitude was given in terms of step time, the load remains constant at the magnitude associated with the end of the previous step. Input File Usage: Use either of the following options to modify an existing load or to specify an additional load (*LOADING OPTION represents any load type): *LOADING OPTION *LOADING OPTION, OP=MOD Abaqus/CAE Usage: Load module: Create Load or Load Manager: Edit Removing loads If you choose to remove any load of a particular type (concentrated load, element-based distributed load, surface-based distributed load, etc.) in a step, no loads of that type will be propagated from the previous general step. All loads of that type that are in effect during this step must be respecified. To redefine a load, the node, element, node set, element set, or surface name must be specified in exactly the same way and the load type must be identical. Refer to “Prescribed conditions: overview,” Section 33.1.1, for a discussion of amplitude variations when removing loads. Input File Usage: Use the following option to release all previously applied loads of a given type and to specify new loads (*LOADING OPTION represents any load type): *LOADING OPTION, OP=NEW For example, *CLOAD, OP=NEW with no data lines will remove all concentrated forces and moments from the model. If the OP=NEW parameter is used on any loading option in a step, it must be used on all loading options of the same type within the step. Abaqus/CAE Usage: Use the following option to remove a load within a step: Load module: Load Manager: Deactivate Abaqus/CAE automatically respecifies any loads that should remain in effect during this step. Example In the history definition input file section shown below, the distributed load (type BX) applied to element set A2 has a magnitude of 20.0 in the first step, which is changed to 50.0 in the second step. Both the set identifier (or element or node number) and the load type must be identical in both steps for Abaqus to identify a load for redefinition. In Step 1 a concentrated load of magnitude 10.0 is applied to degree of freedom 3 of all nodes in node set NLEFT. In Step 2 a concentrated load of magnitude 5.0 is applied to degree of freedom 3 of node 1. If node 1 is in node set NLEFT, the total load applied in Step 2 at this node is 15.0: the loads add. The two distributed loads of type P1 acting on element set E1 in Step 1 will be added to give a total distributed load of 43.0. The pressure loads on element sets B3 and E1 are active during both steps. *STEP Step 1 *STATIC *CLOAD NLEFT, 3, 10. *DLOAD A2, BX, 20. B3, P1, 5. E1, P1, 21. *DLOAD E1, P1, 22. *END STEP ** *STEP Step 2 *STATIC *CLOAD 1, 3, 5. *DLOAD, OP=MOD A2, BX, 50. *END STEP Follower loads in large-displacement analysis In large-displacement analysis distributed loads will be treated as follower forces when appropriate. For beam and shell elements point (concentrated) loads may be fixed in direction or they may rotate with the structure depending on whether you specify follower forces for the load . Follower loads defined at a rigid body tie node rotate with the rigid body in Abaqus/Explicit. Loading during linear perturbation steps In a linear perturbation step (available only in Abaqus/Standard) the state at the end of the previous general analysis step is considered as the “base state.” If the linear perturbation step is the first step of the analysis, the initial conditions of the model form the base state. Loading during a linear perturbation step must be defined as the change in load from the base state (the perturbation of load), not the total of the base state load plus the perturbation load. In consecutive linear perturbation steps, the perturbation of load that applies to each step must be defined completely within that step—the analysis within each such step always starts from the base state (except when you specify that a modal dynamic step should use the initial conditions from the immediately preceding step—see “Transient modal dynamic analysis,” Section 6.3.7). In nonlinear steps that follow linear perturbation analysis steps, the analysis is continued from the base state as if the intermediate linear perturbation steps did not exist. Loading during linear (mode-based) dynamics procedures If a user subroutine is used to define loading in a mode-based linear dynamics analysis, the subroutine will be called only at the beginning of the step to obtain the magnitude of the load. The load magnitude then remains constant in the step unless it is modified by an amplitude curve. CONCENTRATED LOADS CONCENTRATED LOADS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Applying loads: overview,” Section 33.4.1 • *CLOAD • “Defining a concentrated force,” Section 16.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a moment,” Section 16.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a generalized plane strain load,” Section 16.9.10 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a fluid reference pressure,” Section 16.9.23 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Concentrated loads: • apply concentrated forces and moments to nodal degrees of freedom; and • can be fixed in direction; or • can rotate as the node rotates (referred to as follower forces), resulting in an additional, and possibly unsymmetric, contribution to the load stiffness In steady-state dynamic analysis both real and imaginary concentrated loads can be applied . Multiple concentrated load cases can be defined in random response analysis . Concentrated loads are also used to apply the pressure-conjugate at nodes with pressure degree of freedom in acoustic analysis and to specify a fluid reference pressure for incompressible flow . Actuation loads in connector elements can be defined as connector loads, applied similarly to concentrated loads. See “Connector actuation,” Section 31.1.3, for more detailed information. The procedures in which these loads can be used are outlined in “Prescribed conditions: overview,” Section 33.1.1. See “Applying loads: overview,” Section 33.4.1, for general information that applies to all types of loading. Concentrated loads In Abaqus/Standard and Abaqus/Explicit analyses concentrated forces or moments can be applied at any nodal degree of freedom. You should not apply a moment load at the origin of a cylindrical coordinate system; doing so would make the radial and tangential loads indeterminate. Input File Usage: *CLOAD node number or node set, degree of freedom, magnitude Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Concentrated force, Moment, or Generalized plane strain for the Types for Selected Step Specifying concentrated follower forces You can specify that the direction of a concentrated force should rotate with the node to which it is applied. This specification should be used only in large-displacement analysis and can be used only at nodes with active rotational degrees of freedom (such as the nodes of beam and shell elements or, in Abaqus/Explicit, tie nodes on a rigid body), excluding the reference node of generalized plane strain elements. If you specify follower forces, the components of the concentrated force must be specified with respect to the reference configuration. Follower loads lead to an unsymmetric contribution to the stiffness matrix that is generally referred to as the load stiffness. Some issues associated with the load stiffness contribution are discussed in “Improving the rate of convergence in large-displacement implicit analysis.” *CLOAD, FOLLOWER Load module: Create Load: choose Mechanical for the Category and Concentrated force or Moment for the Types for Selected Step: Follow nodal rotation Abaqus/CAE Usage: Input File Usage: Defining the values of concentrated nodal force from a user-specified file You can define nodal force using nodal force output from a particular step and increment in the output database (.odb) file of a previous Abaqus analysis. The part (.prt) file from the original analysis is also required when reading data from the output database file. In this case both the previous model and the current model must be defined consistently, including node numbering, which must be the same in both models. If the models are defined in terms of an assembly of part instances, part instance naming must be the same. Input File Usage: *CLOAD, FILE=file, STEP=step, INC=inc Abaqus/CAE Usage: Defining the values of concentrated nodal force from a user-specified file is not supported in Abaqus/CAE. Specifying a fluid reference pressure For incompressible fluid dynamic analyses in Abaqus/CFD, when no other pressure condition is prescribed, you must specify a fluid reference pressure at one node to set the hydrostatic pressure level. Multiple reference pressures can be specified, but only the last specified hydrostatic pressure load is applied. For more information, see “Incompressible fluid dynamic analysis,” Section 6.6.2, and “Boundary conditions in Abaqus/CFD,” Section 33.3.2. Input File Usage: *CLOAD node number or node set, HP, magnitude Abaqus/CAE Usage: Load module: Create Load: choose Fluid for the Category and Fluid reference pressure for the Types for Selected Step Defining time-dependent concentrated loads The prescribed magnitude of a concentrated load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 33.1.1. If different variations are needed for different loads, each load can refer to its own amplitude. Modifying concentrated loads Concentrated loads can be added, modified, or removed as described in “Applying loads: overview,” Section 33.4.1. Improving the rate of convergence in large-displacement implicit analysis When concentrated follower forces are specified in a geometrically nonlinear static and dynamic analysis, the unsymmetric matrix storage and solution scheme should normally be used. See “Defining an analysis,” Section 6.1.2, for more information on the unsymmetric matrix storage and solution scheme. 33.4.3 DISTRIBUTED LOADS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Applying loads: overview,” Section 33.4.1 • *DLOAD • *DSLOAD • “Defining a pressure load,” Section 16.9.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a shell edge load,” Section 16.9.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a surface traction load,” Section 16.9.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a pipe pressure load,” Section 16.9.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a body force,” Section 16.9.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a line load,” Section 16.9.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a gravity load,” Section 16.9.9 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a rotational body force,” Section 16.9.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a porous drag body force,” Section 16.9.24 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Distributed loads: • can be prescribed on element faces, element bodies, or element edges; • can be prescribed over geometric surfaces or geometric edges; • require that an appropriate distributed load type be specified—see Part VI, “Elements,” for definitions of the distributed load types available for particular elements; and • may be of follower type, which can rotate during a geometrically nonlinear analysis and result in an additional (often unsymmetric) contribution to the stiffness matrix that is generally referred to as the load stiffness. The procedures in which these loads can be used are outlined in “Prescribed conditions: overview,” Section 33.1.1. See “Applying loads: overview,” Section 33.4.1, for general information that applies to all types of loading. Follower loads are discussed further in “Follower surface loads” and “Follower edge and line loads.” The contribution of follower loads to load stiffness is discussed in “Improving the rate of convergence in large-displacement implicit analysis.” In steady-state dynamic analysis both real and imaginary distributed loads can be applied . Incident wave loading is used to apply distributed loads for the special case of loads associated with a wave traveling through an acoustic medium. Inertia relief is used to apply inertia-based loading in Abaqus/Standard. These load types are discussed in “Acoustic and shock loads,” Section 33.4.6, and “Inertia relief,” Section 11.1.1, respectively. Abaqus/Aqua load types are discussed in “Abaqus/Aqua analysis,” Section 6.11.1. Defining time-dependent distributed loads The prescribed magnitude of a distributed load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 33.1.1. If different variations are needed for different loads, each load can refer to its own amplitude definition. Modifying distributed loads Distributed loads can be added, modified, or removed as described in “Applying loads: overview,” Section 33.4.1. Improving the rate of convergence in large-displacement implicit analysis In large-displacement analyses in Abaqus/Standard some distributed load types introduce unsymmetric load stiffness matrix terms. Examples are hydrostatic pressure, pressure applied to surfaces with free edges, Coriolis force, rotary acceleration force, and distributed edge loads and surface tractions modeled In such cases using the unsymmetric matrix storage and solution scheme for the as follower loads. analysis step may improve the convergence rate of the equilibrium iterations. See “Defining an analysis,” Section 6.1.2, for more information on the unsymmetric matrix storage and solution scheme. Defining distributed loads in a user subroutine Nonuniform distributed loads such as a nonuniform body force in the X-direction can be defined by means of user subroutine DLOAD in Abaqus/Standard or VDLOAD in Abaqus/Explicit. When an amplitude reference is used with a nonuniform load defined in user subroutine VDLOAD, the current value of the amplitude function is passed to the user subroutine at each time increment in the analysis. DLOAD and VDLOAD are not available for surface tractions, edge tractions, or edge moments. In Abaqus/Standard nonuniform distributed surface tractions, edge tractions, and edge moments can be defined by means of user subroutine UTRACLOAD. User subroutine UTRACLOAD allows you to define a nonuniform magnitude for surface tractions, edge tractions, and edge moments, as well as nonuniform loading directions for general surface tractions, shear tractions, and general edge tractions. Nonuniform distributed surface tractions, edge tractions, and edge moments are not currently supported in Abaqus/Explicit. When the user subroutine is used, the external work is calculated based only on the current magnitude of the distributed load since the incremental value for the distributed load is not defined. Specifying the region to which a distributed load is applied As discussed in “Applying loads: overview,” Section 33.4.1, distributed loads can be defined as element- based or surface-based. Element-based distributed loads can be prescribed on element bodies, element surfaces, or element edges. Surface-based distributed loads can be prescribed directly on geometric surfaces or geometric edges. Three types of distributed loads can be defined: body loads, surface loads, and edge loads. Distributed body loads are always element-based. Distributed surface loads and distributed edge loads can be element-based or surface-based. Table 33.4.3–1 summarizes the regions on which each load type can be prescribed. In Abaqus/CAE distributed loads are specified by selecting the region in the viewport or from a list of surfaces.In the Abaqus input file different options are used depending on the type of region to which the load is applied, as illustrated in the following sections. Table 33.4.3–1 Regions on which the different load types can be prescribed. Load type Load definition Input file region Abaqus/CAE region Body loads Element-based Element bodies Volumetric bodies Surface loads Element-based Element surfaces Edge loads (including beam line loads) Surface-based Geometric element- based surfaces Element-based Element edges Surface-based Geometric edge-based surfaces Surfaces defined as collections of geometric faces or element faces (excluding analytical rigid surfaces) Surfaces defined as collections of geometric edges or element edges Body forces Body loads, such as gravity, centrifugal, Coriolis, and rotary acceleration loads, are applied as element- based loads. The units of a body force are force per unit volume. Table 33.4.3–2 lists all of the distributed body load types that are available in Abaqus, along with the corresponding load type labels. Table 33.4.3–2 Distributed body load types. Load description Body force in global X-, Y-, and Z-directions Nonuniform body force in global X-, Y-, and Z-directions Body force in radial and axial directions (only for axisymmetric elements) Nonuniform body force in radial and axial directions (only for axisymmetric elements) Viscous body force in global X-, Y-, and Z-directions (available only in Abaqus/Explicit) Stagnation body force in global X-, Y-, and Z-directions (available only in Abaqus/Explicit) Gravity loading Centrifugal load (magnitude is input as is the mass density , where per unit volume and is the angular velocity) Centrifugal load (magnitude is input as , where velocity) is the angular Coriolis force Rotary acceleration load Rotordynamic load Porous drag load (input is porosity of the medium) Load type label for element-based loads Abaqus/CAE load type BX, BY, BZ Body force BXNU, BYNU, BZNU Body force BR, BZ BRNU, BZNU VBF SBF GRAV CENT CENTRIF CORIO ROTA ROTDYNF PDBF 33.4.3–4 Not supported Gravity Not supported Rotational body force Coriolis force Rotational body force Not supported Porous drag body Specifying general body forces You can specify body forces on any elements in the global X-, Y-, or Z-direction. You can specify body forces on axisymmetric elements in the radial or axial direction. Input File Usage: Use the following option to define a body force in the global X-, Y-, or Z- direction: *DLOAD element number or element set, load type label, magnitude where load type label is BX, BY, BZ, BXNU, BYNU, or BZNU. Use the following option to define a body force in the radial or axial direction on axisymmetric elements: *DLOAD element number or element set, load type label, magnitude where load type label is BR, BZ, BRNU, or BZNU. Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Body force for the Types for Selected Step Specifying viscous body force loads in Abaqus/Explicit Viscous body force loads are defined by where is the viscous force applied to the body; is the velocity of the point on the body where the force is being applied; is the viscosity, given as the magnitude of the load; is the velocity of the reference node; and is the element volume. Viscous body force loading can be thought of as mass-proportional damping in the sense that it gives a damping contribution proportional to the mass for an element if the coefficient is chosen to be a small value multiplied by the material density . Viscous body force loading provides an alternative way to define mass-proportional damping as a function of relative velocities and a step-dependent damping coefficient. Input File Usage: Use the following option to define a viscous body force load: *DLOAD, REF NODE=reference_node element number or element set, VBF, magnitude Abaqus/CAE Usage: Viscous body force loads are not supported in Abaqus/CAE. Specifying stagnation body force loads in Abaqus/Explicit Stagnation body force loads are defined by is the velocity of the point on the body where the body force is being applied; is the stagnation body force applied to the body; where load; of the reference node; and is the element volume. The coefficient excessive damping and a dramatic drop in the stable time increment. is the factor, given as the magnitude of the is the velocity should be very small to avoid Input File Usage: Use the following option to define a stagnation body force load: *DLOAD, REF NODE=reference_node element number or element set, SBF, magnitude Abaqus/CAE Usage: Stagnation body force loads are not supported in Abaqus/CAE. Specifying gravity loading Gravity loading (uniform acceleration in a fixed direction) is specified by using the gravity distributed load type and giving the gravity constant as the magnitude of the load. The direction of the gravity field is specified by giving the components of the gravity vector in the distributed load definition. Abaqus uses the user-specified material density , together with the magnitude and direction, to calculate the loading. The magnitude of the gravity load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 33.1.1. However, the direction of the gravity field is always applied at the beginning of the step and remains fixed during the step. You need not specify an element or an element set as is customary for the specification of other distributed loads. Abaqus/Standard and Abaqus/Explicit automatically collect all elements in the model that have mass contributions (including point mass elements but excluding rigid elements) in an element set called _Whole_Model_Gravity_Elset and apply the gravity loads to the elements in this element set. Abaqus/CFD applies the gravity loading to all user-defined elements. In Abaqus/CFD gravity loading defines the gravity vector used with a Boussinesq-type body force in buoyancy driven flow. You must activate the energy equation for incompressible flow and define thermal expansion to specify the thermal expansion coefficient . Gravity loading can be used only in conjunction with the energy equation and will be ignored if used without the energy equation; general body forces can be defined for incompressible flow without the energy equation. When gravity loading is used with substructures, the density must be defined and unit gravity load vectors must be calculated when the substructure is created . Input File Usage: Use the following option to define a gravity load: *DLOAD element number or element set, GRAV, gravity constant, comp1, comp2, comp3 Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Gravity for the Types for Selected Step Specifying loads due to rotation of the model in Abaqus/Standard Centrifugal loads, Coriolis forces, rotary acceleration, and rotordynamic loads can be applied in Abaqus/Standard by specifying the appropriate distributed load type in an element-based distributed load definition. These loading options are primarily intended for replicating dynamic loads while performing analyses other than implicit dynamics using direct integration (“Dynamic stress/displacement analysis,” Section 6.3). In an implicit dynamic procedure inertia loads due to rotations come about naturally due to the equations of motion. Applying distributed centrifugal, Coriolis, rotary acceleration, and rotordynamic loads in an implicit dynamic analysis may lead to non-physical loads and should be used carefully. Centrifugal loads , where , where Centrifugal load magnitudes can be specified as is the angular velocity in radians per time. Abaqus/Standard uses the specified material density , together with the load magnitude and the axis of rotation, to calculate the loading. Alternatively, a centrifugal load magnitude can be given as is the material density (mass per unit volume) for solid or shell elements or the mass per unit length for beam elements and is the angular velocity in radians per time. This type of centrifugal load formulation does not account for large volume changes. The two centrifugal load types will produce slightly different local results for first-order elements; uses a consistent mass matrix, and uses a lumped mass matrix in calculating the load forces and load stiffnesses. The magnitude of the centrifugal load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 33.1.1. However, the position and orientation of the axis around which the structure rotates, which is defined by giving a point on the axis and the axis direction, are always applied at the beginning of the step and remain fixed during the step. Input File Usage: Use either of the following options to define a centrifugal load: *DLOAD element number or element set, CENTRIF, comp2, comp3 *DLOAD element number or element set, CENT, comp2, comp3 , coord1, coord2, coord3, comp1, , coord1, coord2, coord3, comp1, Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Rotational body force for the Types for Selected Step: Load effect: Centrifugal Coriolis forces , where Coriolis force is defined by specifying the Coriolis distributed load type and giving the load magnitude as is the material density (mass per unit volume) for solid and shell elements or the mass per unit length for beam elements and is the angular velocity in radians per time. The magnitude of the Coriolis load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 33.1.1. However, the position and orientation of the axis around which the structure rotates, which is defined by giving a point on the axis and the axis direction, are always applied at the beginning of the step and remain fixed during the step. In a static analysis Abaqus computes the translational velocity term in the Coriolis loading by dividing the incremental displacement by the current time increment. The Coriolis load formulation does not account for large volume changes. Input File Usage: Use the following option to define a Coriolis load: *DLOAD element number or element set, CORIO, comp1, comp2, comp3 , coord1, coord2, coord3, Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Coriolis force for the Types for Selected Step Rotary acceleration loads Rotary acceleration loads are defined by specifying the rotary acceleration distributed load type and , in radians/time2, which includes any precessional motion giving the rotary acceleration magnitude, effects. The axis of rotary acceleration must be defined by giving a point on the axis and the axis direction. Abaqus/Standard uses the specified material density , together with the rotary acceleration magnitude and axis of rotary acceleration, to calculate the loading. The magnitude of the load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 33.1.1. However, the position and orientation of the axis around which the structure rotates are always applied at the beginning of the step and remain fixed during the step. Rotary acceleration loads are not applicable to axisymmetric elements. Input File Usage: Use the following option to define a rotary acceleration load: *DLOAD element number or element set, ROTA, comp1, comp2, comp3 , coord1, coord2, coord3, Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Rotational body force for the Types for Selected Step: Load effect: Rotary acceleration Specifying general rigid-body acceleration loading in Abaqus/Standard General rigid-body acceleration loading can be specified in Abaqus/Standard by using a combination of the gravity, centrifugal ( ), and rotary acceleration load types. Rotordynamic loads in a fixed reference frame Rotordynamic loads can be used to study the vibrational response of three-dimensional models of axisymmetric structures, such as a flywheel in a hybrid energy storage system, that are spinning about their axes of symmetry in a fixed reference frame . This is in contrast to the centrifugal loads, Coriolis forces, and rotary acceleration loads discussed above, which are formulated in a rotating frame. Rotordynamic loads are, therefore, not intended to be used in conjunction with these other dynamic load types. The intended workflow for rotordynamic loads is to define the load in a nonlinear static step to establish the centrifugal load effects and load stiffness terms associated with a spinning body. The nonlinear static step can then be followed by a sequence of linear dynamic analyses such as complex eigenvalue extraction and/or a subspace or direct-solution steady-state dynamic analysis to study complex dynamic behaviors (induced by gyroscopic moments) such as critical speeds, unbalanced responses, and whirling phenomena in rotating structures. You do not need to redefine the rotordynamic load in the linear dynamic analyses—the load definition is carried over from the nonlinear static step. The contribution of the gyroscopic matrices in the linear dynamic steps is unsymmetric; therefore, you must use unsymmetric matrix storage as described in “Defining an analysis,” Section 6.1.2, during these steps. Rotordynamic loads are intended only for three-dimensional models of axisymmetric bodies; you must ensure that this modeling assumption is met. Rotordynamic loads are supported for all three-dimensional continuum and cylindrical elements, shell elements, membrane elements, cylindrical membrane elements, beam elements, and rotary inertia elements. The spinning axis defined as part of the load must be the axis of symmetry for the structure. Therefore, beam elements must be aligned with the symmetry axis. In addition, one of the principal directions of each loaded rotary inertia element must be aligned with the symmetry axis, and the inertia components of the rotary inertia elements must be symmetric about this axis. Multiple spinning structures spinning about different axes can be modeled in the same step. The spinning structures can also be connected to non-axisymmetric, non-rotating structures (such as bearings or support structures). Rotordynamic loads are defined by specifying the angular velocity, , in radians per time. The magnitude of the rotordynamic load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 33.1.1. However, the position and orientation of the axis around which the structure rotates, which is defined by giving a point on the axis and the axis direction, are always applied at the beginning of the step and remain fixed during the step. Input File Usage: Use the following option to define a rotordynamic load: *DLOAD element number or element set, ROTDYNF, comp1, comp2, comp3 , coord1, coord2, coord3, Abaqus/CAE Usage: Element-based rotordynamic loads are not supported in Abaqus/CAE. Specifying porous drag body force load in Abaqus/CFD In Abaqus/CFD porous drag loading defines the porous drag body forces (Darcy and inertial drag forces) in flow through porous media . If the porous drag body forces are activated, permeability of the medium must be defined . flow problems involving heat transfer, the properties of both the solid and fluid phases of the porous medium must be defined using a fluid section definition. Porous drag loads are defined by specifying the dimensionless porosity, (ratio of the fluid to the total volume of the porous medium). Input File Usage: Use the following option to define a porous drag body force load: *DLOAD element number or element set, PDBF, porosity Abaqus/CAE Usage: Load module: Create Load: choose Fluid for the Category and Porous drag body force for the Types for Selected Step Surface tractions and pressure loads General or shear surface tractions and pressure loads can be applied in Abaqus as element-based or surface-based distributed loads. The units of these loads are force per unit area. Table 33.4.3–3 lists all of the distributed surface load types that are available in Abaqus, along with the corresponding load type labels. Part VI, “Elements,” lists the distributed surface load types that are available for particular elements and the Abaqus/CAE load support for each load type. For some element-based loads you must identify the face of the element upon which the load is prescribed in the load type label (for example, Pn or PnNU for continuum elements). Follower surface loads With the exception of general surface tractions, all By definition, the line of action of a follower surface load rotates with the surface in a geometrically nonlinear analysis. This is in contrast to a non-follower load, which always acts in a fixed global direction. the distributed surface loads listed in Table 33.4.3–3 are modeled as follower loads. The hydrostatic and viscous pressures listed in Table 33.4.3–3 always act normal to the surface in the current configuration, the shear tractions always act tangent to the surface in the current configuration, and the internal and external pipe pressures follow the motion of the pipe elements. General surface tractions can be specified to be follower or non-follower loads. There is no difference between a follower and a non-follower load in a geometrically linear analysis since the configuration of the body remains fixed. The difference between a follower and non-follower general surface traction is illustrated in the next section through an example. Input File Usage: Use one of the following options to define general surface tractions as follower loads (the default): *DLOAD, FOLLOWER=YES *DSLOAD, FOLLOWER=YES Use one of the following options to define general surface tractions as non- follower loads: *DLOAD, FOLLOWER=NO *DSLOAD, FOLLOWER=NO Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: Traction: General, toggle on or off Follow rotation Abaqus/CAE Usage: Table 33.4.3–3 Distributed surface load types. Load description Load type label for element-based loads Load type label for surface-based loads Abaqus/CAE load type General surface traction TRVECn, TRVEC TRVEC Surface traction Shear surface traction TRSHRn, TRSHR TRSHR Nonuniform general surface traction Nonuniform shear surface traction Pressure Nonuniform pressure Hydrostatic pressure (available only in Abaqus/Standard) Viscous pressure (available only in Abaqus/Explicit) Stagnation pressure (available only in Abaqus/Explicit) Hydrostatic internal and external pressure (only for PIPE and ELBOW elements ) Uniform internal and external pressure (only for PIPE and ELBOW elements ) Nonuniform internal and external pressure (only for PIPE and ELBOW elements ) TRVECnNU, TRVECNU TRSHRnNU, TRSHRNU Pn, P PnNU, PNU HPn, HP VPn, VP SPn, SP HPI, HPE PI, PE TRVECNU TRSHRNU Surface traction (surface-based loads only) Pressure Pressure (surface-based loads only) Pipe pressure PNU HP VP SP N/A N/A PINU, PENU N/A Specifying general surface tractions General surface tractions allow you to specify a surface traction, load, , is computed by integrating over S: , acting on a surface S. The resultant where specify both a load magnitude, is the magnitude and is the direction of the load. To define a general surface traction, you must , and the direction of the load with respect to the reference configuration, . The magnitude and direction can also be specified in user subroutine UTRACLOAD. The specified traction directions are normalized by Abaqus and, thus, do not contribute to the magnitude of the load: Input File Usage: Use one of the following options to define a general surface traction: *DLOAD element number or element set, load type label, magnitude, direction components where load type label is TRVECn, TRVEC, TRVECnNU, or TRVECNU. *DSLOAD surface name, TRVEC or TRVECNU, magnitude, direction components Abaqus/CAE Usage: Use the following input to define an element-based general surface traction: Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: Traction: General, Distribution: select an analytical field Use the following input to define a surface-based general surface traction: Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: Traction: General, Distribution: Uniform or User-defined Nonuniform element-based general surface traction is not supported in Abaqus/CAE. Defining the direction vector with respect to a local coordinate system By default, the components of the traction vector are specified with respect to the global directions. You can also refer to a local coordinate system for the direction components of these tractions. See “Examples: using a local coordinate system to define shear directions” below for an example of a traction load defined with respect to a local coordinate system. Input File Usage: Use one of the following options to specify a local coordinate system: Abaqus/CAE Usage: *DLOAD, ORIENTATION=name *DSLOAD, ORIENTATION=name Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: select CSYS: Picked and click Edit to pick a local coordinate system, or select CSYS: User-defined to enter the name of a user subroutine that defines a local coordinate system Rotation of the traction vector direction The traction load acts in the fixed direction in a geometrically linear analysis or if a non-follower load is specified in a geometrically nonlinear analysis (which includes a perturbation step about a geometrically nonlinear base state). If a follower load is specified in a geometrically nonlinear analysis, the traction load rotates rigidly , with the surface using the following algorithm. The reference configuration traction vector, is decomposed by Abaqus into two components: a normal component, and a tangential component, where The applied traction in the current configuration is then computed as is the unit reference surface normal and is the unit projection of onto the reference surface. where the current surface; i.e., decomposition of the local two-dimensional surface deformation gradient is the normal to the surface in the current configuration and , where rotated onto is the standard rotation tensor obtained from the polar is the image of . Examples: follower and non-follower tractions The following two examples illustrate the difference between applying follower and non-follower tractions in a geometrically nonlinear analysis. Both examples refer to a single 4-node plane strain element (element 1). In Step 1 of the first example a follower traction load is applied to face 1 of element 1, and a non-follower traction load is applied to face 2 of element 1. The element is rotated rigidly 90° counterclockwise in Step 1 and then another 90° in Step 2. As illustrated in Figure 33.4.3–1, the follower traction rotates with face 1, while the non-follower traction on face 2 always acts in the global x-direction. *STEP, NLGEOM Step 1 - Rotate square 90 degrees ... *DLOAD, FOLLOWER=YES 1, TRVEC1, 1., 0., -1., 0. *DLOAD, FOLLOWER=NO 1, TRVEC2, 1., 1., 0., 0. *END STEP *STEP, NLGEOM (a) (b) (c) follower traction non-follower traction Figure 33.4.3–1 Follower and non-follower traction loads in a geometrically nonlinear analysis, load applied in Step 1: (a) beginning of Step 1; (b) end of Step 1, beginning of Step 2; (c) end of Step 2. Step 2 - Rotate square another 90 degrees ... *END STEP In the second example the element is rotated 90° counterclockwise with no load applied in Step 1. In Step 2 a follower traction load is applied to face 1, and a non-follower traction load is applied to face 2. The element is then rotated rigidly by another 90°. The direction of the follower load is specified with respect to the original configuration. As illustrated in Figure 33.4.3–2, the follower traction rotates with face 1, while the non-follower traction on face 2 always acts in the global x-direction. *STEP, NLGEOM Step 1 - Rotate square 90 degrees ... *END STEP *STEP, NLGEOM Step 2 - Rotate square another 90 degrees *DLOAD, FOLLOWER=YES 1, TRVEC1, 1., 0., -1., 0. *DLOAD, FOLLOWER=NO 1, TRVEC2, 1., 1., 0., 0. ... *END STEP (a) (b) (c) follower traction non-follower traction Figure 33.4.3–2 Follower and non-follower traction loads in a geometrically nonlinear analysis, load applied in Step 2: (a) beginning of Step 1; (b) end of Step 1, beginning of Step 2; (c) end of Step 2. Specifying shear surface tractions Shear surface tractions allow you to specify a surface force per unit area, S. The resultant load, , is computed by integrating over S: , that acts tangent to a surface is the magnitude and where traction, you must provide both the magnitude, and direction vector can also be specified in user subroutine UTRACLOAD. is a unit vector along the direction of the load. To define a shear surface , for the load. The magnitude , and a direction, Abaqus modifies the traction direction by first projecting the user-specified vector, , onto the surface in the reference configuration, where direction is the reference surface normal. The specified traction is applied along the computed traction tangential to the surface: Consequently, a shear traction load is not applied at any point where surface. is normal to the reference The shear traction load acts in the fixed direction in a geometrically linear analysis. In a geometrically nonlinear analysis (which includes a perturbation step about a geometrically nonlinear base state), the shear traction vector will rotate rigidly; i.e., is the standard rotation tensor obtained from the polar decomposition of the local two-dimensional surface deformation gradient , where . Input File Usage: Use one of the following options to define a shear surface traction: *DLOAD element number or element set, load type label, magnitude, direction components where load type label is TRSHRn, TRSHR, TRSHRnNU, or TRSHRNU. *DSLOAD surface name, TRSHR or TRSHRNU, magnitude, direction components Abaqus/CAE Usage: Use the following input to define an element-based shear surface traction: Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: Traction: Shear, Distribution: select an analytical field Use the following input to define a surface-based general surface traction: Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: Traction: Shear, Distribution: Uniform or User-defined Nonuniform element-based shear surface traction is not supported in Abaqus/CAE. Defining the direction vector with respect to a local coordinate system By default, the components of the shear traction vector are specified with respect to the global directions. You can also refer to a local coordinate system for the direction components of these tractions. Input File Usage: Abaqus/CAE Usage: Use one of the following options to specify a local coordinate system: *DLOAD, ORIENTATION=name *DSLOAD, ORIENTATION=name Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: select CSYS: Picked and click Edit to pick a local coordinate system, or select CSYS: User-defined to enter the name of a user subroutine that defines a local coordinate system Examples: using a local coordinate system to define shear directions It is sometimes convenient to give shear and general traction directions with respect to a local coordinate system. The following two examples illustrate the specification of the direction of a shear traction on a cylinder using global coordinates in one case and a local cylindrical coordinate system in the other case. defined on the outside of the cylinder. DISTRIBUTED LOADS In the first example the direction of the shear traction, , is given in global The sense of the resulting shear tractions using global coordinates is shown in coordinates. Figure 33.4.3–3(a). (a) (b) Figure 33.4.3–3 Shear tractions specified using global coordinates (a) and a local cylindrical coordinate system (b). *STEP Step 1 - Specify shear directions in global coordinates ... *DSLOAD SURFA, TRSHR, 1., 0., 1., 0. ... *END STEP In the second example the direction of the shear traction, , is given with respect to a local cylindrical coordinate system whose axis coincides with the axis of the cylinder. The sense of the resulting shear tractions using the local cylindrical coordinate system is shown in Figure 33.4.3–3(b). *ORIENTATION, NAME=CYLIN, SYSTEM=CYLINDRICAL 0., 0., 0., 0., 0., 1. ... *STEP Step 1 - Specify shear directions in local cylindrical coordinates ... *DSLOAD, ORIENTATION=CYLIN SURFA, TRSHR, 1., 0., 1., 0. ... *END STEP Resultant loads due to surface tractions You can choose to integrate surface tractions over the current or the reference configuration by specifying whether or not a constant resultant should be maintained. In general, the constant resultant method is best suited for cases where the magnitude of the resultant load should not vary with changes in the surface area. However, it is up to you to decide which approach is best for your analysis. An example of an analysis using a constant resultant can be found in “Distributed traction and edge loads,” Section 1.4.18 of the Abaqus Verification Manual. Choosing not to have a constant resultant If you choose not to have a constant resultant, the traction vector is integrated over the surface in the current configuration, a surface that in general deforms in a geometrically nonlinear analysis. By default, all surface tractions are integrated over the surface in the current configuration. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *DLOAD, CONSTANT RESULTANT=NO *DSLOAD, CONSTANT RESULTANT=NO Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: Traction is defined per unit deformed area Maintaining a constant resultant If you choose to have a constant resultant, the traction vector is integrated over the surface in the reference configuration and then held constant. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *DLOAD, CONSTANT RESULTANT=YES *DSLOAD, CONSTANT RESULTANT=YES Load module: Create Load: choose Mechanical for the Category and Surface traction for the Types for Selected Step: Traction is defined per unit undeformed area Example The constant resultant method has certain advantages when a traction is used to model a distributed load with a known constant resultant. Consider the case of modeling a uniform dead load, magnitude p, acting on a flat plate whose normal is in the -direction in a geometrically nonlinear analysis (Figure 33.4.3–4). e 2 e 1 deformed configuration Figure 33.4.3–4 Dead load on a flat plate. Such a model might be used to simulate a snow load on a flat roof. The snow load could be modeled as a distributed dead traction load and S denote the total surface area of the plate in the reference and current configurations, respectively. With no constant resultant, the total integrated load on the plate, . Let , is In this case a uniform traction leads to a resultant load that increases as the surface area of the plate increases, which is not consistent with a fixed snow load. With the constant resultant method, the total integrated load on the plate is In this case a uniform traction leads to a resultant that is equal to the pressure times the surface area in the reference configuration, which is more consistent with the problem at hand. Specifying pressure loads Distributed pressure loads can be specified on any two-dimensional, three-dimensional, or axisymmetric elements. Hydrostatic pressure loads can be specified in Abaqus/Standard on two-dimensional, three- dimensional, and axisymmetric elements. Viscous and stagnation pressure loads can be specified in Abaqus/Explicit on any elements. Distributed pressure loads Distributed pressure loads can be specified on any elements. For beam elements, a positive applied pressure results in a force vector acting along the particular local direction of the section or a global direction, whichever is specified. For conventional shell elements, the force vector points along the element SPOS normal. For continuum solid or a continuum shell elements with the distributed load on an explicitly identified facet, the force vector acts against the outward normal of that facet. Distributed pressure loads are not supported for pipe and elbow elements. Distributed pressure loads can be specified on a surface formed over elements; a positive applied pressure results in a force vector acting against the local surface normal. Input File Usage: Use one of the following options to define a pressure load: *DLOAD element number or element set, load type label, magnitude where load type label is Pn, P, PnNU, or PNU. *DSLOAD surface name, P or PNU, magnitude Abaqus/CAE Usage: Use the following input to define an element-based pressure load: Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: select an analytical field or a discrete field Use the following input to define a surface-based pressure load: Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Uniform or User-defined Nonuniform element-based pressure loads are not supported in Abaqus/CAE. Hydrostatic pressure loads on two-dimensional, three-dimensional, and axisymmetric elements in Abaqus/Standard To define hydrostatic pressure in Abaqus/Standard, give the Z-coordinates of the zero pressure level (point a in Figure 33.4.3–5) and the level at which the hydrostatic pressure is defined (point b in Figure 33.4.3–5) in an element-based or surface-based distributed load definition. For levels above the zero pressure level, the hydrostatic pressure is zero. Figure 33.4.3–5 Hydrostatic pressure distribution. In planar elements the hydrostatic head is in the Y-direction; for axisymmetric elements the Z-direction is the second coordinate. Input File Usage: Use one of the following options to define a hydrostatic pressure load: *DLOAD element number or element set, HPn or HP, magnitude, Z-coordinate of point a, Z-coordinate of point b *DSLOAD surface name, HP, magnitude, Z-coordinate of point a, Z-coordinate of point b Abaqus/CAE Usage: Use the following input to define a surface-based hydrostatic pressure load: Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: Hydrostatic Element-based hydrostatic pressure loads are not supported in Abaqus/CAE. Viscous pressure loads in Abaqus/Explicit Viscous pressure loads are defined by where p is the pressure applied to the body; the velocity of the point on the surface where the pressure is being applied; reference node; and is the unit outward normal to the element at the same point. is the viscosity, given as the magnitude of the load; is is the velocity of the Viscous pressure loading is most commonly applied in structural problems when you want to damp out dynamic effects and, thus, reach static equilibrium in a minimal number of increments. A common example is the determination of springback in a sheet metal product after forming, in which case a viscous pressure would be applied to the faces of shell elements defining the sheet metal. An appropriate choice for the value of is important for using this technique effectively. To compute , consider the infinite continuum elements described in “Infinite elements,” Section 28.3.1. In explicit dynamics those elements achieve an infinite boundary condition by applying a viscous normal pressure where the coefficient is the density of the material at the surface, and is the value of the dilatational wave speed in the material (the infinite continuum elements also apply a viscous shear traction). For an isotropic, linear elastic material is given by ; and are Lamé’s constants, E is Young’s modulus, and where is Poisson’s ratio. This choice of the viscous pressure coefficient represents a level of damping in which pressure waves crossing the free surface are absorbed with no reflection of energy back into the interior of the finite element mesh. For typical structural problems it is not desirable to absorb all of the energy (as is the case in the as an coefficient should have a positive value. infinite elements). Typically effective way of minimizing ongoing dynamic effects. The is set equal to a small percentage (perhaps 1 or 2 percent) of Input File Usage: Use one of the following options to define a viscous pressure load: *DLOAD, REF NODE=reference_node element number or element set, VPn or VP, magnitude *DSLOAD, REF NODE=reference_node surface name, VP, magnitude Abaqus/CAE Usage: Use the following input to define a surface-based viscous pressure load: Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: Viscous, toggle on or off Determine velocity from reference point Element-based viscous pressure loads are not supported in Abaqus/CAE. Stagnation pressure loads in Abaqus/Explicit Stagnation pressure loads are defined by is the stagnation pressure applied to the body; where load; normal to the element at the same point; and is the factor, given as the magnitude of the is the unit outward is the velocity of the reference node. The coefficient is the velocity of the point on the surface where the pressure is being applied; should be very small to avoid excessive damping and a dramatic drop in the stable time increment. Input File Usage: Use one of the following options to define a stagnation pressure load: *DLOAD, REF NODE=reference_node element number or element set, SPn or SP, magnitude *DSLOAD, REF NODE=reference_node element number or element set, SP, magnitude Abaqus/CAE Usage: Use the following input to define a surface-based stagnation pressure load: Load module: Create Load: choose Mechanical for the Category and Pressure for the Types for Selected Step: Distribution: Stagnation, toggle on or off Determine velocity from reference point Element-based stagnation pressure loads are not supported in Abaqus/CAE. Pressure on pipe and elbow elements You can specify external pressure, internal pressure, external hydrostatic pressure, or internal hydrostatic pressure on pipe or elbow elements. When pressure loads are applied, the effective outer or inner diameter must be specified in the element-based distributed load definition. The loads resulting from the pressure on the ends of the element are included: Abaqus assumes a closed-end condition. Closed-end conditions correctly model the loading at pipe intersections, tight bends, corners, and cross-section changes; in straight sections and smooth bends the end loads of adjacent elements cancel each other precisely. If an open-end condition is to be modeled, a compensating point load should be added at the open end. A case where such an end load must be applied occurs if a pressurized pipe is modeled with a mixture of pipe and beam elements. In that case closed-end conditions generate a physically non-existing force at the transition between pipe and beam elements. Such mixed modeling of a pipe is not recommended. For pipe elements subjected to pressure loading, the effective axial force due to the pressure loads can be obtained by requesting output variable ESF1 . DISTRIBUTED LOADS Use the following option to define an external pressure load on pipe or elbow elements: *DLOAD element number or element set, PE or PENU, magnitude, effective outer diameter Use the following option to define an internal pressure load on pipe or elbow elements: *DLOAD element number or element set, PI or PINU, magnitude, effective inner diameter Use the following option to define an external hydrostatic pressure load on pipe or elbow elements: *DLOAD element number or element set, HPE, magnitude, effective outer diameter Use the following option to define an internal hydrostatic pressure load on pipe or elbow elements: *DLOAD element number or element set, HPI, magnitude, effective inner diameter Abaqus/CAE Usage: Use the following input to define an external or internal pressure load on pipe or elbow elements: Load module: Create Load: choose Mechanical for the Category and Pipe pressure for the Types for Selected Step: Side: External or Internal, Distribution: Uniform, User-defined, or select an analytical field Use the following input to define an external or internal hydrostatic pressure load on pipe or elbow elements: Load module: Create Load: choose Mechanical for the Category and Pipe pressure for the Types for Selected Step: Side: External or Internal, Distribution: Hydrostatic Defining distributed surface loads on plane stress elements Plane stress theory assumes that the volume of a plane stress element remains constant in a large-strain analysis. When a distributed surface load is applied to an edge of plane stress elements, the current length and orientation of the edge are considered in the load distribution, but the current thickness is not; the original thickness is used. This limitation can be circumvented only by using three-dimensional elements at the edge so that a change in thickness upon loading is recognized; suitable equation constraints (“Linear constraint equations,” Section 34.2.1) would be required to make the in-plane displacements on the two faces of these elements equal. Three-dimensional elements along an edge can be connected to interior shell elements by using a shell-to-solid coupling constraint . Edge tractions and moments on shell elements and line loads on beam elements Distributed edge tractions (general, shear, normal, or transverse) and edge moments can be applied to shell elements in Abaqus as element-based or surface-based distributed loads. The units of an edge traction are force per unit length. The units of an edge moment are torque per unit length. References to local coordinate systems are ignored for all edge tractions and moments except general edge tractions. Distributed line loads can be applied to beam elements in Abaqus as element-based distributed loads. The units of a line load are force per unit length. Table 33.4.3–4 lists all of the distributed edge and line load types that are available in Abaqus, along with the corresponding load type labels. Part VI, “Elements,” lists the distributed edge and line load types that are available for particular elements and the Abaqus/CAE load support for each load type. For element-based loads applied to shell elements, you must identify the edge of the element upon which the load is prescribed in the load type label (for example, EDLDn or EDLDnNU). Follower edge and line loads By definition, the line of action of a follower edge or line load rotates with the edge or line in a geometrically nonlinear analysis. This is in contrast to a non-follower load, which always acts in a fixed global direction. With the exception of general edge tractions on shell elements and the forces per unit length in the global directions on beam elements, all the edge and line loads listed in Table 33.4.3–4 are modeled as follower loads. The normal, shear, and transverse edge loads listed in Table 33.4.3–4 act in the normal, shear, and transverse directions, respectively, in the current configuration . The edge moment always acts about the shell edge in the current configuration. The forces per unit length in the local beam directions rotate with the beam elements. Table 33.4.3–4 Distributed edge load types. Load description General edge traction Normal edge traction Shear edge traction Transverse edge traction Edge moment Load type label for element-based loads Load type label for surface-based loads Abaqus/CAE load type Shell edge load EDLDn EDNORn EDSHRn EDTRAn EDMOMn EDLD EDNOR EDSHR EDTRA EDMOM Load description Load type label for element-based loads Load type label for surface-based loads Abaqus/CAE load type Nonuniform general edge traction EDLDnNU Nonuniform normal edge traction EDNORnNU Nonuniform shear edge traction EDSHRnNU Nonuniform transverse edge traction EDTRAnNU EDLDNU EDNORNU EDSHRNU EDTRANU Nonuniform edge moment EDMOMnNU EDMOMNU Shell edge load (surface-based loads only) PX, PY, PZ N/A Line load Force per unit length in global X-, Y-, and Z-directions (only for beam elements) Nonuniform force per unit length in global X-, Y-, and Z-directions (only for beam elements) Force per unit length in beam local 1- and 2-directions (only for beam elements) P1, P2 PXNU, PYNU, PZNU N/A N/A Nonuniform force per unit length in beam local 1- and 2-directions (only for beam elements) P1NU, P2NU N/A The forces per unit length in the global directions on beam elements are always non-follower loads. General edge tractions can be specified to be follower or non-follower loads. There is no difference between a follower and a non-follower load in a geometrically linear analysis since the configuration of the body remains fixed. Input File Usage: Abaqus/CAE Usage: Use one of the following options to define general edge tractions as follower loads (the default): *DLOAD, FOLLOWER=YES *DSLOAD, FOLLOWER=YES Use one of the following options to define general edge tractions as non-follower loads: *DLOAD, FOLLOWER=NO *DSLOAD, FOLLOWER=NO Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction: General, toggle on or off Follow rotation EDTRA EDTRA EDSHR EDNOR EDTRA EDNOR EDTRA EDNOR EDSHR EDNOR EDSHR EDSHR EDTRA EDTRA EDSHR EDNOR EDSHR EDTRA EDNOR EDNOR EDSHR Figure 33.4.3–6 Positive edge loads. Specifying general edge tractions General edge tractions allow you to specify an edge load, , is computed by integrating over L: , acting on a shell edge, L. The resultant load, To define a general edge traction, you must provide both a magnitude, , for the load. The specified load directions are normalized by Abaqus; thus, they do not contribute to the magnitude of the load. , and direction, If a nonuniform general edge traction is specified, the magnitude, , and direction, , must be specified in user subroutine UTRACLOAD. Input File Usage: Use one of the following options to define a general edge traction: *DLOAD element number or element set, EDLDn or EDLDnNU, magnitude, direction components *DSLOAD surface name, EDLD or EDLDNU, magnitude, direction components Abaqus/CAE Usage: Use the following input to define an element-based general edge traction: Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction: General, Distribution: select an analytical field Use the following input to define a surface-based general edge traction: Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction: General, Distribution: Uniform or User-defined Nonuniform element-based general edge traction is not supported in Abaqus/CAE. Rotation of the load vector In a geometrically linear analysis the edge load, , acts in the fixed direction defined by If a non-follower load is specified in a geometrically nonlinear analysis (which includes a , acts in the fixed direction perturbation step about a geometrically nonlinear base state), the edge load, defined by If a follower load is specified in a geometrically nonlinear analysis (which includes a perturbation step about a geometrically nonlinear base state), the components must be defined with respect to the reference configuration. The reference edge traction is defined as The applied edge traction, , is computed by rigidly rotating onto the current edge. Defining the direction vector with respect to a local coordinate system By default, the components of the edge traction vector are specified with respect to the global directions. You can also refer to a local coordinate system for the direction components of these tractions. Input File Usage: Use one of the following options to specify a local coordinate system: Abaqus/CAE Usage: *DLOAD, ORIENTATION=name *DSLOAD, ORIENTATION=name Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: select CSYS: Picked and click Edit to pick a local coordinate system, or select CSYS: User-defined to enter the name of a user subroutine that defines a local coordinate system Specifying shear, normal, and transverse edge tractions The loading directions of shear, normal, and transverse edge tractions are determined by the underlying elements. A positive shear edge traction acts in the positive direction of the shell edge as determined by the element connectivity. A positive normal edge traction acts in the plane of the shell in the inward direction. A positive transverse edge traction acts in a sense opposite to the facet normal. The directions of positive shear, normal, and transverse edge tractions are shown in Figure 33.4.3–6. To define a shear, normal, or transverse edge traction, you must provide a magnitude, If a nonuniform shear, normal, or transverse edge traction is specified, the magnitude, for the load. , must be specified in user subroutine UTRACLOAD. In a geometrically linear step, the shear, normal, and transverse edge tractions act in the tangential, normal, and transverse directions of the shell, as shown in Figure 33.4.3–6. In a geometrically nonlinear analysis the shear, normal, and transverse edge tractions rotate with the shell edge so they always act in the tangential, normal, and transverse directions of the shell, as shown in Figure 33.4.3–6. Input File Usage: Use one of the following options to define a directed edge traction: *DLOAD element number or element set, directed edge traction label, magnitude *DSLOAD surface name, directed edge traction label, magnitude For element-based loads the directed edge traction label can be EDSHRn or EDSHRnNU for shear edge tractions, EDNORn or EDNORnNU for normal edge tractions, or EDTRAn or EDTRAnNU for transverse edge tractions. For surface-based loads the directed edge traction label can be EDSHR or EDSHRNU for shear edge tractions, EDNOR or EDNORNU for normal edge tractions, or EDTRA or EDTRANU for transverse edge tractions. Abaqus/CAE Usage: Use the following input to define an element-based directed edge traction: Load module: Create Load; choose Mechanical for the Category and Shell edge load for the Types for Selected Step; Traction: Normal, Transverse, or Shear; Distribution: select an analytical field Use the following input to define a surface-based directed edge traction: Load module: Create Load; choose Mechanical for the Category and Shell edge load for the Types for Selected Step; Traction: Normal, Transverse, or Shear; Distribution: Uniform or User-defined Nonuniform element-based directed edge traction is not supported in Abaqus/CAE. Specifying edge moments An edge moment acts about the shell edge with the positive direction determined by the element connectivity. The directions of positive edge moments are shown in Figure 33.4.3–7. Figure 33.4.3–7 Positive edge moments. To define a distributed edge moment, you must provide a magnitude, If a nonuniform edge moment is specified, the magnitude, , for the load. , must be specified in user subroutine UTRACLOAD. An edge moment always acts about the current shell edge in both geometrically linear and nonlinear analyses. In a geometrically linear step an edge moment acts about the shell edge as shown in Figure 33.4.3–7. In a geometrically nonlinear analysis an edge moment always acts about the shell edge as shown in Figure 33.4.3–7. Input File Usage: Use one of the following options to define an edge moment: *DLOAD element number or element set, EDMOMn or EDMOMnNU, magnitude *DSLOAD surface name, EDMOM or EDMOMNU, magnitude Abaqus/CAE Usage: Use the following input to define an element-based edge moment: Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction: Moment, Distribution: select an analytical field Use the following input to define a surface-based edge moment: Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction: General, Distribution: Uniform or User-defined Nonuniform element-based edge moments are not supported in Abaqus/CAE. Resultant loads due to edge tractions and moments You can choose to integrate edge tractions and moments over the current or the reference configuration by specifying whether or not a constant resultant should be maintained. In general, the constant resultant method is best suited for cases where the magnitude of the resultant load should not vary with changes in the edge length. However, it is up to you to decide which approach is best for your analysis. Choosing not to have a constant resultant If you choose not to have a constant resultant, an edge traction or moment is integrated over the edge in the current configuration, an edge whose length changes during a geometrically nonlinear analysis. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *DLOAD, CONSTANT RESULTANT=NO *DSLOAD, CONSTANT RESULTANT=NO Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction is defined per unit deformed area Maintaining a constant resultant If you choose to have a constant resultant, an edge traction or moment is integrated over the edge in the reference configuration, whose length is constant. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *DLOAD, CONSTANT RESULTANT=YES *DSLOAD, CONSTANT RESULTANT=YES Load module: Create Load: choose Mechanical for the Category and Shell edge load for the Types for Selected Step: Traction is defined per unit undeformed area Specifying line loads on beam elements You can specify line loads on beam elements in the global X-, Y-, or Z-direction. In addition, you can specify line loads on beam elements in the beam local 1- or 2-direction. Input File Usage: Use the following option to define a force per unit length in the global X-, Y-, or Z-direction on beam elements: *DLOAD element number or element set, load type label, magnitude where load type label is PX, PY, PZ, PXNU, PYNU, or PZNU. Use the following option to define a force per unit length in the beam local 1- or 2-direction: *DLOAD element number or element set, load type label, magnitude where load type label is P1, P2, P1NU, or P2NU. Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Line load for the Types for Selected Step Additional references • Genta, G., Dynamics of Rotating Systems, Springer, 2005. 33.4.4 THERMAL LOADS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Applying loads: overview,” Section 33.4.1 • *CFLUX • *DFLUX • *DSFLUX • *CFILM • *FILM • *SFILM • *FILM PROPERTY • *CRADIATE • *RADIATE • *SRADIATE • “Defining a concentrated heat flux,” Section 16.9.19 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a body heat flux,” Section 16.9.18 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a surface heat flux,” Section 16.9.17 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a fluid wall boundary condition,” Section 16.10.12 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a surface film condition interaction,” Section 15.13.22 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a concentrated film condition interaction,” Section 15.13.23 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a surface radiative interaction,” Section 15.13.24 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a concentrated radiative interaction,” Section 15.13.25 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Thermal loads can be applied in heat transfer analysis, in fully coupled temperature-displacement analysis, fully coupled thermal-electrical-structural analysis, and in coupled thermal-electrical analysis, as outlined in “Prescribed conditions: overview,” Section 33.1.1. The following types of thermal loads are available: • Concentrated heat flux prescribed at nodes. • Distributed heat flux prescribed on element faces or surfaces. • Body heat flux per unit volume. • Boundary convection defined at nodes, on element faces, or on surfaces. • Boundary radiation defined at nodes, on element faces, or on surfaces. See “Applying loads: overview,” Section 33.4.1, for general information that applies to all types of loading. Modeling thermal radiation The following types of radiation heat exchange can be modeled using Abaqus: • Exchange between a nonconcave surface and a nonreflecting environment. This type of radiation is modeled using boundary radiation loads defined at nodes, on element faces, or on surfaces, as described below. • Exchange between two surfaces within close proximity of each other in which temperature gradients along the surfaces are not large. This type of radiation is modeled using the gap radiation capability described in “Thermal contact properties,” Section 36.2.1. • Exchange between surfaces that constitute a cavity. This type of radiation is modeled using the cavity radiation capability available in Abaqus/Standard and described in “Cavity radiation,” Section 40.1.1, or through the average-temperature radiation condition described in “Specifying average-temperature radiation conditions,” below. Prescribing heat fluxes directly Concentrated heat fluxes can be prescribed at nodes (or node sets). Distributed heat fluxes can be defined on element faces or surfaces. Specifying concentrated heat fluxes By default, a concentrated heat flux is applied to degree of freedom 11. For shell heat transfer elements concentrated heat fluxes can be prescribed through the thickness of the shell by specifying degree of freedom 11, 12, 13, etc. Temperature variation through the thickness of shell elements is described in “Choosing a shell element,” Section 29.6.2. Input File Usage: *CFLUX node number or node set name, degree of freedom, heat flux magnitude Abaqus/CAE Usage: Load module: Create Load: choose Thermal for the Category and Concentrated heat flux for the Types for Selected Step: select region: Magnitude: heat flux magnitude Defining the values of concentrated nodal flux from a user-specified file You can define nodal flux using nodal flux output from a particular step and increment in the output database (.odb) file of a previous Abaqus analysis. The part (.prt) file from the original analysis is also required when reading data from the output database file. In this case both the previous model and the current model must be defined consistently, including node numbering, which must be the same in both models. If the models are defined in terms of an assembly of part instances, part instance naming must be the same. Input File Usage: Abaqus/CAE Usage: *CFLUX, FILE=file, STEP=step, INC=inc Defining the values of concentrated nodal flux from a user-specified file is not supported in Abaqus/CAE. Specifying element-based distributed heat fluxes You can specify element-based distributed surface fluxes (on element faces) or body fluxes (flux per unit volume). For surface fluxes you must identify the face of the element upon which the flux is prescribed in the flux label (for example, Sn or SnNU for continuum elements). The distributed flux types available depend on the element type. Part VI, “Elements,” lists the distributed fluxes that are available for particular elements. Input File Usage: *DFLUX element number or element set name, load type label, flux magnitude Abaqus/CAE Usage: Use the following input to define a distributed surface flux: where load type label is Sn, SPOS, SNEG, S1, S2, or BF Load module: Create Load: choose Thermal for the Category and Surface heat flux for the Types for Selected Step: select region: Distribution: select an analytical field, Magnitude: flux magnitude Use the following input to define a distributed body flux: Load module: Create Load: choose Thermal for the Category and Body heat flux for the Types for Selected Step: select region: Distribution: Uniform or select an analytical field, Magnitude: flux magnitude Specifying surface-based distributed heat fluxes When you specify distributed surface fluxes on a surface, the surface that contains the element and face information is defined as described in “Element-based surface definition,” Section 2.3.2. You must specify the surface name, the heat flux label, and the heat flux magnitude. Input File Usage: *DSFLUX surface name, S, flux magnitude Abaqus/CAE Usage: Use the following input to specify surface-based distributed heat fluxes: Load module: Create Load: choose Thermal for the Category and Surface heat flux for the Types for Selected Step: select region: Distribution: Uniform, Magnitude: flux magnitude Use the following input to specify surface-based distributed wall heat fluxes in Abaqus/CFD: Load module: Create Boundary Condition: Step: flow_step: choose Fluid for the Category and Fluid wall condition for the Types for Selected Step: select region: Thermal Energy: Specify: Heat flux, Magnitude: flux magnitude Modifying or removing heat fluxes Heat fluxes can be added, modified, or removed as described in “Applying loads: overview,” Section 33.4.1. Specifying time-dependent heat fluxes The magnitude of a concentrated or a distributed heat flux can be controlled by referring to an amplitude curve. If different magnitude variations are needed for different fluxes, the flux definitions can be repeated, with each referring to its own amplitude curve. See “Prescribed conditions: overview,” Section 33.1.1, and “Amplitude curves,” Section 33.1.2, for details. Defining nonuniform distributed heat flux in a user subroutine In Abaqus/Standard a nonuniform distributed flux (element-based or surface-based) can be defined in user subroutine DFLUX. The specified reference magnitude will be passed into user subroutine DFLUX as FLUX(1). If the magnitude is omitted, FLUX(1) will be passed in as zero. Input File Usage: Use the following option to define a nonuniform element-based heat flux: *DFLUX element number or element set name, load type label, flux magnitude where load type label is SnNU, SPOSNU, SNEGNU, S1NU, S2NU, or BFNU. Use the following option to define a nonuniform surface-based heat flux: *DSFLUX surface name, SNU, flux magnitude For example, for general heat transfer shell elements (“Three-dimensional conventional shell element library,” Section 29.6.7) a uniform surface flux of 10.0 per unit area on the top face (SPOS) of shell element 100 can be applied by *DFLUX 100, SPOS, 10.0 When the variation of the (nonuniform) flux magnitude is defined by means of user subroutine DFLUX, the distributed flux type label SPOSNU is used. *DFLUX 100, SPOSNU, magnitude Abaqus/CAE Usage: Use the following input to define a nonuniform element-based body flux: Load module: Create Load: choose Thermal for the Category and Body heat flux for the Types for Selected Step: select region: Distribution: User-defined, Magnitude: flux magnitude Use the following input to define a nonuniform surface-based heat flux: Load module: Create Load: choose Thermal for the Category and Surface heat flux for the Types for Selected Step: select region: Distribution: User-defined, Magnitude: flux magnitude Nonuniform element-based distributed surface fluxes are not supported in Abaqus/CAE. Prescribing boundary convection Heat flux on a surface due to convection is governed by where is the heat flux across the surface, is a reference film coefficient, is the temperature at this point on the surface, and is a reference sink temperature value. Heat flux due to convection can be defined on element faces, on surfaces, or at nodes. Specifying element-based film conditions You can define the sink temperature value, , and the film coefficient, h, on element faces. The convection is applied to element edges in two dimensions and to element faces in three dimensions. The edge or face of the element upon which the film is placed is identified by a film load type label and depends on the element type . You must specify the element number or element set name, the film load type label, a sink temperature, and a film coefficient. Input File Usage: *FILM element number or element set name, film load type label, , h Abaqus/CAE Usage: Element-based film conditions are supported in Abaqus/CAE only for the film coefficient. Interaction module: Create Interaction: Surface film condition: select region: Definition: select an analytical field: Film coefficient: h Specifying surface-based film conditions You can define the sink temperature value, , and the film coefficient, h, on a surface. The surface that contains the element and face information is defined as described in “Element-based surface definition,” Section 2.3.2. You must specify the surface name, the film load type, a sink temperature, and a film coefficient. Input File Usage: *SFILM surface name, F or FNU, , h Abaqus/CAE Usage: Interaction module: Create Interaction: Surface film condition: select region: Definition: Embedded Coefficient or User-defined: Film coefficient: h and Sink temperature: Specifying node-based film conditions A node-based film condition requires that you define the nodal area for a specified node number or node set; the sink temperature value, ; and the film coefficient, h. The associated degree of freedom is 11. For shell type elements where the film is associated with a degree of freedom other than 11, you can specify the concentrated film for a duplicate node that is constrained to the appropriate degree of freedom of the shell node by using an equation constraint . Input File Usage: *CFILM node number or node set name, nodal area, , h Abaqus/CAE Usage: Interaction module: Create Interaction: Concentrated film condition: select region: Definition: Embedded Coefficient, User-defined, or select an analytical field: Associated nodal area: nodal area, Film coefficient: h, Sink temperature: Specifying temperature- and field-variable-dependent film conditions If the film coefficient is a function of temperature, you can specify the film property data separately and specify the name of the property table instead of the film coefficient in the film condition definition. You can specify multiple film property tables to define different variations of the film coefficient, h, as a function of surface temperature and/or field variables. Each film property table must be named. This name is referred to by the film condition definitions. A new film property table can be defined in a restart step. If a film property table with an existing name is encountered, the second definition is ignored. Input File Usage: For element-based film conditions, use the following options: *FILM PROPERTY, NAME=film property table name *FILM element number or element set name, film load type label, , film property table name For surface-based film conditions, use the following options: *FILM PROPERTY, NAME=film property table name *SFILM surface name, F, , film property table name For node-based film conditions, use the following options: *FILM PROPERTY, NAME=film property table name *CFILM node number or node set name, nodal area, The *FILM PROPERTY option must appear in the model definition portion of the input file. , film property table name Interaction module: Create Interaction Property: Name: film property table name and Film condition Create Interaction: Surface film condition or Concentrated film condition: select region: Definition: Property Reference and Film interaction property: film property table name Abaqus/CAE Usage: Modifying or removing film conditions Film conditions can be added, modified, or removed as described in “Applying loads: overview,” Section 33.4.1. Specifying time-dependent film conditions For a uniform film both the sink temperature and the film coefficient can be varied with time by referring to amplitude definitions. One amplitude curve defines the variation of the sink temperature, , with time. Another amplitude curve defines the variation of the film coefficient, h, with time. See “Prescribed conditions: overview,” Section 33.1.1, and “Amplitude curves,” Section 33.1.2, for more information. Input File Usage: Abaqus/CAE Usage: Use the following options to define time-dependent film conditions: *AMPLITUDE, NAME=temp_amp *AMPLITUDE, NAME=h_amp *FILM, AMPLITUDE=temp_amp, FILM AMPLITUDE=h_amp *SFILM, AMPLITUDE=temp_amp, FILM AMPLITUDE=h_amp *CFILM, AMPLITUDE=temp_amp, FILM AMPLITUDE=h_amp Use the following input to define time-dependent film conditions. If you select an analytical field to define the interaction, the analytical field affects only the film coefficient. Interaction module: Create Amplitude: Name: h_amp Create Amplitude: Name: temp_amp Create Interaction: Surface film condition or Concentrated film condition: select region: Definition: Embedded Coefficient or select an analytical field: Film coefficient amplitude: h_amp and Sink amplitude: temp_amp Examples A uniform, time-dependent film condition can be defined for face 2 of element 3 by *AMPLITUDE, NAME=sink 0.0, 0.5, 1.0, 0.9 *AMPLITUDE, NAME=famp 0.0, 1.0, 1.0, 22.0 … *STEP ** For an Abaqus/Standard analysis: *HEAT TRANSFER ** For an Abaqus/Explicit analysis: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT … *FILM, AMPLITUDE=sink, FILM AMPLITUDE=famp 3, F2, 90.0, 2.0 A uniform, temperature-dependent film coefficient and a time-dependent sink temperature can be defined for face 2 of element 3 by *AMPLITUDE, NAME=sink 0.0, 0.5, 1.0, 0.9 *FILM PROPERTY, NAME=filmp 80.0 2.0, 2.3, 90.0 8.5, 180.0 … *STEP ** For an Abaqus/Standard analysis: *HEAT TRANSFER ** For an Abaqus/Explicit analysis: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT … *FILM, AMPLITUDE=sink 3, F2, 90.0, filmp A uniform, temperature-dependent film coefficient and a time-dependent sink temperature can be defined for node 2, where the nodal area is 50, by *AMPLITUDE, NAME=sink 0.0, 0.5, 1.0, 0.9 *FILM PROPERTY, NAME=filmp 2.0, 2.3, 80.0 90.0 8.5, 180.0 … *STEP ** For an Abaqus/Standard analysis: *HEAT TRANSFER ** For an Abaqus/Explicit analysis: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT … *CFILM, AMPLITUDE=sink, 2, 50, 90.0, filmp Defining nonuniform film conditions in a user subroutine In Abaqus/Standard a nonuniform film coefficient can be defined as a function of position, time, temperature, etc. in user subroutine FILM for element-based, surface-based, as well as node-based film conditions. Amplitude references are ignored if a nonuniform film is prescribed. Input File Usage: Use the following option to define a nonuniform film coefficient for an element- based film condition: *FILM element number or element set name, FnNU Use the following option to define a nonuniform film coefficient for a surface- based film condition: *SFILM surface name, FNU Use the following option to define a nonuniform film coefficient for a node- based film condition: *CFILM, USER node number or node set name, nodal area Element-based film conditions to define a nonuniform film coefficient are not supported in Abaqus/CAE. However, similar functionality is available using surface-based film conditions. Use the following option to define a nonuniform film coefficient for a surface-based film condition: Interaction module: Create Interaction: Surface film condition: select region: Definition: User-defined Use the following option to define a nonuniform film coefficient for a node- based film condition: Interaction module: Create Interaction: Concentrated film condition: select region: Definition: User-defined 33.4.4–9 Prescribing boundary radiation Heat flux on a surface due to radiation to the environment is governed by where is the heat flux across the surface, is the emissivity of the surface, is the Stefan-Boltzmann constant, is the temperature at this point on the surface, is an ambient temperature value, and is the value of absolute zero on the temperature scale being used. Heat flux due to radiation can be defined on element faces, on surfaces, or at nodes. Specifying element-based radiation To specify element-based radiation within a heat transfer or coupled temperature-displacement step definition, you must provide the ambient temperature value, . The radiation is applied to element edges in two dimensions and to element faces in three dimensions. The edge or face of the element upon which the radiation occurs is identified by a radiation type label depending on the element type . , and the emissivity of the surface, Input File Usage: *RADIATE element number or element set name, Rn, , Abaqus/CAE Usage: Interaction module: Create Interaction: Surface radiation: select region: Radiation type: To ambient, Emissivity distribution: select an analytical field, Emissivity: , and Ambient temperature: Specifying surface-based radiation to ambient You can apply the radiation to a surface rather than to individual element faces. The surface that contains the element and face information is defined as described in “Element-based surface definition,” Section 2.3.2. You must specify the surface name; the radiation load type label, R (or RPOS, RNEG in the case of shells); the ambient temperature value, ; and the emissivity of the surface, . Input File Usage: *SRADIATE surface name, R, , Abaqus/CAE Usage: Interaction module: Create Interaction: Surface radiation: select region: Radiation type: To ambient, Emissivity distribution: Uniform, Emissivity: , and Ambient temperature: Specifying node-based radiation to ambient To specify node-based radiation within a heat transfer or coupled temperature-displacement step definition, you must provide the nodal area for a specified node number or node set; the ambient temperature value, . The associated degree of freedom is 11. For shell elements where the concentrated radiation is associated with a degree of freedom other than 11, you can specify the required data for a duplicate node that is constrained to the appropriate degree of freedom of the shell node by using an equation constraint. ; and the emissivity of the surface, Input File Usage: *CRADIATE node number or node set name, nodal area, , Abaqus/CAE Usage: Interaction module: Create Interaction: Concentrated radiation to ambient: select region: Associated nodal area: Emissivity: and Ambient temperature: Specifying time-dependent radiation The user-specified value of the ambient temperature, , can be varied throughout the step by referring to an amplitude definition. See “Applying loads: overview,” Section 33.4.1, and “Amplitude curves,” Section 33.1.2, for details. Specifying average-temperature radiation conditions The average-temperature radiation condition is an approximation to the cavity radiation problem, where the radiative flux per unit area into a facet is with the average temperature for the surface being calculated as The average temperature in the cavity is computed at the beginning of each increment and held constant over the increment. Therefore, the average-temperature radiation condition has some dependency on the increment size, and you need to ensure that the increment size you use is appropriate for your model. If you see large changes in temperature over an increment, you may need to reduce the increment size. Input File Usage: Use the following option to define the average-temperature radiation condition on a surface: *SRADIATE surface name, AVG, , Abaqus/CAE Usage: Interaction module: Create Interaction: Surface radiation: select the surface region: Radiation type: Cavity approximation (3D only), Emissivity: Specifying the value of absolute zero You can specify the value of absolute zero, this value as model data. By default, the value of absolute zero is 0.0. , on the temperature scale being used; you must specify Input File Usage: Abaqus/CAE Usage: *PHYSICAL CONSTANTS, ABSOLUTE ZERO= Any module: Model→Edit Attributes→model_name: Absolute zero temperature: Specifying the value of the Stefan-Boltzmann constant If boundary radiation is prescribed, you must specify the Stefan-Boltzmann constant, be specified as model data. ; this value must Input File Usage: Abaqus/CAE Usage: *PHYSICAL CONSTANTS, STEFAN BOLTZMANN= Any module: Model→Edit Attributes→model_name: Stefan-Boltzmann constant: Modifying or removing boundary radiation Boundary radiation conditions can be added, modified, or removed as described in “Applying loads: overview,” Section 33.4.1. 33.4.5 ELECTROMAGNETIC LOADS Products: Abaqus/Standard Abaqus/CAE References • “Prescribed conditions: overview,” Section 33.1.1 • “Applying loads: overview,” Section 33.4.1 • *CECHARGE • *CECURRENT • *DECHARGE • *DECURRENT • *DSECHARGE • *DSECURRENT • “Defining a concentrated current,” Section 16.9.25 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a surface current,” Section 16.9.26 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a body current,” Section 16.9.27 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a surface current density,” Section 16.9.28 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a body current density,” Section 16.9.29 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a concentrated charge,” Section 16.9.30 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a surface charge,” Section 16.9.31 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a body charge,” Section 16.9.32 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview As outlined in “Prescribed conditions: overview,” Section 33.1.1, electromagnetic loads can be applied in “Piezoelectric analysis,” Section 6.7.2; “Coupled thermal-electrical analysis,” Section 6.7.3; “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4; “Eddy current analysis,” Section 6.7.5; and “Magnetostatic analysis,” Section 6.7.6. The types of electromagnetic loads available depend on the analysis being performed, as described in the sections below. See “Applying loads: overview,” Section 33.4.1, for general information that applies to all types of loading. Defining time-dependent electromagnetic loads The prescribed magnitude of a concentrated or a distributed electromagnetic load can vary with time during a step according to an amplitude definition, as described in “Prescribed conditions: overview,” Section 33.1.1. If different variations are needed for different loads, each load can refer to its own amplitude definition. In a time-harmonic eddy current analysis all loads are assumed to be time-harmonic. Modifying electromagnetic loads Concentrated or distributed electromagnetic loads can be added, modified, or removed as described in “Applying loads: overview,” Section 33.4.1. Prescribing electromagnetic loads for piezoelectric analyses In a piezoelectric analysis a concentrated electric charge can be prescribed at nodes, a distributed electric surface charge can be defined on element faces and surfaces, and a distributed electric body charge can be defined on elements. Specifying concentrated electric charge To specify a concentrated electric charge, specify the node or node set and the magnitude of the charge. Input File Usage: *CECHARGE node number or node set name, , charge magnitude Abaqus/CAE Usage: Load module: Create Load: choose Electrical/Magnetic for the Category and Concentrated charge for the Types for Selected Step; Magnitude: charge magnitude Specifying element-based distributed electric charge You can specify a distributed surface charge (on element faces) or a distributed body charge (charge per unit volume). For an element-based surface charge you must identify the face of the element upon which the charge is prescribed in the charge label. The distributed charge types available depend on the element type. Part VI, “Elements,” lists the distributed charges that are available for particular elements. Input File Usage: *DECHARGE element number or element set name, charge label, charge magnitude Abaqus/CAE Usage: Use the following input to define a distributed surface charge on element faces: where charge label is ESn or EBF Load module: Create Load: choose Electrical/Magnetic for the Category and Surface charge for the Types for Selected Step; Distribution: select an analytical field, Magnitude: charge magnitude Use the following input to define a body charge: Load module: Create Load: choose Electrical/Magnetic for the Category and Body charge for the Types for Selected Step Specifying surface-based distributed electric charge When you specify a distributed electric charge on a surface, the element-based surface contains the element and face information. You must specify the surface name, the electric charge label, and the electric charge magnitude. Input File Usage: *DSECHARGE surface name, ES, charge magnitude Abaqus/CAE Usage: Load module: Create Load: choose Electrical/Magnetic for the Category and Surface charge for the Types for Selected Step; Distribution: Uniform, Magnitude: charge magnitude Specifying electric charge in direct-solution steady-state dynamics analysis In the direct-solution steady-state dynamics procedure, electric charges are given in terms of their real and imaginary components. Input File Usage: Use the following options to define electric charges in direct-integration steady- state dynamics analysis: Abaqus/CAE Usage: *CECHARGE, REAL or IMAGINARY (real or imaginary component) *DECHARGE, REAL or IMAGINARY *DSECHARGE, REAL or IMAGINARY Load module: Create Load: choose Electrical/Magnetic for the Category and Concentrated charge, Surface charge, or Body charge for the Types for Selected Step; Magnitude: real component + imaginary component Loading in mode-based and subspace-based procedures Electrical charge loads should be used only in conjunction with residual modes in the eigenvalue extraction step, due to the “massless” mode effect. Since the electrical potential degrees of freedom do not have any associated mass, these degrees of freedom are essentially eliminated (similar to Guyan reduction or mass condensation) during the eigenvalue extraction. The residual modes represent the static response corresponding to the electrical charge loads, which will adequately represent the potential degree of freedom in the eigenspace. Prescribing electromagnetic loads for coupled thermal-electrical and fully coupled thermal-electrical-structural analyses In a coupled thermal-electrical analysis and fully coupled thermal-electrical-structural analysis a concentrated current can be prescribed at nodes, distributed current densities can be defined on element faces and surfaces, and distributed body currents can be defined on elements. Specifying concentrated current density To define concentrated currents, specify the node or node set and the magnitude of the current. Input File Usage: *CECURRENT node number or node set name, , current magnitude Abaqus/CAE Usage: Load module: Create Load: choose Electrical/Magnetic for the Category and Concentrated current for the Types for Selected Step; Magnitude: current magnitude Specifying element-based distributed current density You can specify distributed surface current densities (on element faces) or distributed body current densities (current per unit volume). For element-based surface current densities you must identify the face of the element upon which the current is prescribed in the current label. The distributed current types available depend on the element type. Part VI, “Elements,” lists the distributed current densities that are available for particular elements. *DECURRENT element number or element set name, current density label, current density magnitude Input File Usage: where current density label is CSn, CS1, CS2, or CBF Abaqus/CAE Usage: Use the following input to define a distributed surface current density on element faces: Load module: Create Load: choose Electrical/Magnetic for the Category and Surface current for the Types for Selected Step; Distribution: select an analytical field, Magnitude: current density magnitude Use the following input to define a body current density: Load module: Create Load: choose Electrical/Magnetic for the Category and Body current for the Types for Selected Step Specifying surface-based distributed current densities When you specify distributed current densities on a surface, the element-based surface contains the element and face information. You must specify the surface name, the current density label, and the current density magnitude. Input File Usage: *DSECURRENT surface name, CS, current density magnitude Abaqus/CAE Usage: Load module: Create Load: choose Electrical/Magnetic for the Category and Surface current for the Types for Selected Step: Distribution: Uniform, Magnitude: current density magnitude Prescribing electromagnetic loads for eddy current and/or magnetostatic analyses In an eddy current analysis a distributed surface current density vector can be defined on surfaces and a distributed volume current density vector can be defined on elements. Specifying element-based distributed current density vectors When you define a distributed volume current density vector, you must specify the element or element set, the current density vector label, the magnitude of the current density vector, the vector components of the current density, and an optional orientation name that defines the local coordinate system in which the vector components are specified. By default, the vector components of the current density are defined with respect to the global directions. The specified current density vector direction components are normalized by Abaqus and, thus, do not contribute to the magnitude of the load. Input File Usage: *DECURRENT element number or element set name, CJ, current density vector magnitude, current density vector direction components, orientation name Abaqus/CAE Usage: Load module: Create Load: choose Electrical/Magnetic for the Category and Body current density for the Types for Selected Step; Distribution: Uniform Specifying surface-based distributed current density vectors When you specify distributed current density vectors on a surface, the element-based surface contains the element and face information. You must specify the surface name, the current density vector label, and the magnitude of the current density vector, the vector components of the current density, and an optional orientation name that defines the local coordinate system in which the surface current density is specified. By default, the vector components of the current density are defined with respect to the global directions. The specified current density vector direction components are normalized by Abaqus and, thus, do Input File Usage: not contribute to the magnitude of the load. *DSECURRENT surface name, CK, current density vector magnitude, current density vector direction components, orientation name Abaqus/CAE Usage: Load module: Create Load: choose Electrical/Magnetic for the Category and Surface current density for the Types for Selected Step; Distribution: Uniform Defining nonuniform current density vectors in a user subroutine Nonuniform volume current density vectors can be defined with user subroutine UDECURRENT, and nonuniform surface current density vectors can be defined with user subroutine UDSECURRENT. If the magnitude and direction components are given, the values are passed into the user subroutine. Input File Usage: Use the following option to define nonuniform element-based current density vectors: *DECURRENT element number or element set name, CJNU, current density vector magnitude, current density vector direction components, orientation name Use the following option to define nonuniform surface-based current density vectors: *DSECURRENT surface name, CKNU, current density vector magnitude, current density vector direction components, orientation name Abaqus/CAE Usage: Use the following option to define nonuniform volume current density: Load module: Create Load: choose Electrical/Magnetic for the Category and Body current density for the Types for Selected Step; Distribution: User-defined Use the following option to define nonuniform surface current density: Load module: Create Load: choose Electrical/Magnetic for the Category and Surface current density for the Types for Selected Step; Distribution: User-defined Specifying real and imaginary components of current density vectors in a time-harmonic eddy current analysis In a time-harmonic eddy current analysis, current density vectors are given in terms of their real (in- phase) and imaginary (out-of-phase) components. Input File Usage: Use the following options to define current density vectors: Abaqus/CAE Usage: *DECURRENT, REAL or IMAGINARY *DSECURRENT, REAL or IMAGINARY Load module: Create Load: choose Electrical/Magnetic for the Category and Body current density or Surface current density for the Types for Selected Step; real components + imaginary components 33.4.6 ACOUSTIC AND SHOCK LOADS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Applying loads: overview,” Section 33.4.1 • “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1 • *AMPLITUDE • *BOUNDARY • *CLOAD • *CONWEP CHARGE PROPERTY • *IMPEDANCE • *IMPEDANCE PROPERTY • *INCIDENT WAVE • *INCIDENT WAVE FLUID PROPERTY • *INCIDENT WAVE INTERACTION • *INCIDENT WAVE INTERACTION PROPERTY • *INCIDENT WAVE PROPERTY • *INCIDENT WAVE REFLECTION • *SIMPEDANCE • *UNDEX CHARGE PROPERTY • “Defining acoustic impedance,” Section 15.13.17 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining incident waves,” Section 15.13.18 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining an acoustic impedance interaction property,” Section 15.14.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining an incident wave interaction property,” Section 15.14.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Acoustic loads can be applied only in transient or steady-state dynamic analysis procedures. The following types of acoustic loads are available: • Boundary impedance defined on element faces or on surfaces. • Nonreflecting radiation boundaries in exterior problems such as a structure vibrating in an acoustic medium of infinite extent. • Concentrated pressure-conjugate loads prescribed at acoustic element nodes. • Temporally and spatially varying pressure loading on acoustic and solid surfaces due to incident waves traveling through the acoustic medium. Specified boundary impedance A boundary impedance specifies the relationship between the pressure of an acoustic medium and the normal motion at the boundary. Such a condition is applied, for example, to include the effect of small- amplitude “sloshing” in a gravity field or the effect of a compressible, possibly dissipative, lining (such as a carpet) between an acoustic medium and a fixed, rigid wall or structure. The impedance boundary condition at any point along the acoustic medium surface is governed by where is the acoustic particle velocity in the outward normal direction of the acoustic medium surface, is the acoustic pressure, is the time rate of change of the acoustic pressure, is the proportionality coefficient between the pressure and the displacement normal to the surface, and is the proportionality coefficient between the pressure and the velocity normal to the surface. This model can be conceptualized as a spring and dashpot in series placed between the acoustic medium and a rigid wall. The spring and dashpot parameters are , respectively, defined per unit area of the interface surface. These reactive acoustic boundaries can have a significant effect on the pressure distribution in the acoustic medium, in particular if the coefficients are chosen such that the boundary is energy absorbing. If no impedance, loads, or fluid-solid coupling are specified on the surface of an acoustic mesh, the acceleration of that surface is assumed to be zero. This is equivalent to the presence of a rigid wall at that boundary. and and Use of the subspace-based steady-state dynamics procedure is not recommended if reactive acoustic boundaries with strong absorption characteristics are used. Since the effect of is not taken into account in an eigenfrequency extraction step, the eigenmodes may have shapes that are significantly different from the exact solution. Sloshing of a free surface To model small-amplitude “sloshing” of a free surface in a gravity field, set and , where is the density of the fluid and g is the gravitational acceleration (assumed to be directed normal to the surface). This relation holds for small volumetric drag. Acoustic-structural interface The impedance boundary condition can also be placed at an acoustic-structural interface. In this case the boundary condition can be conceptualized as a spring and dashpot in series placed between the acoustic medium and the structure. The expression for the outward velocity still holds, with now being the relative outward velocity of the acoustic medium and the structure: where is the velocity of the structure, is the outward normal to the acoustic medium. is the velocity of the acoustic medium at the boundary, and Steady-state dynamics In a steady-state dynamics analysis the expression for the outward velocity can be written in complex form as where is the circular frequency (radians/second) and we define The term is its complex impedance. Thus, a required complex impedance or admittance value can be entered for a given frequency by specifying the parameters is the complex admittance of the boundary, and and . Specifying impedance conditions You specify impedance coefficient data in an impedance property table. You can describe an impedance table in terms of the admittance parameters, , or in terms of the real and imaginary parts and of the impedance. In the latter case Abaqus converts the user-defined table of impedance data to the admittance parameter form for the analysis. The parameters in the table can be specified over a range of frequencies. The required values are interpolated from the table in steady-state harmonic response analysis only; for other analysis types, only the first table entry is used. The name of the impedance property table is referred to from a surface-based or element-based impedance definition. In Abaqus/CAE impedance conditions are always surface-based; surfaces can be defined as collections of geometric faces and edges or collections of element faces and edges. In a steady-state dynamics analysis you cannot specify impedance conditions on a surface on which incident wave loading is applied. Input File Usage: Use the following option to specify an impedance using a table of admittance parameters (default): *IMPEDANCE PROPERTY, NAME=impedance property table name, DATA=ADMITTANCE Use the following option to specify an impedance using a table of the real and imaginary parts of the impedance: *IMPEDANCE PROPERTY, NAME=impedance property table name, DATA=IMPEDANCE Abaqus/CAE Usage: Use the following input to specify an impedance using a table of admittance parameters: Interaction module: Create Interaction Property: Name: impedance property table name and Acoustic impedance: Data type: Admittance Use the following input to specify an impedance using a table of the real and imaginary parts of the impedance: Interaction module: Create Interaction Property: Name: impedance property table name and Acoustic impedance: Data type: Impedance Specifying surface-based impedance conditions You can define the impedance condition on a surface. The impedance is applied to element edges in two dimensions and to element faces in three dimensions. The element-based surface contains the element and face information. Input File Usage: Abaqus/CAE Usage: *SIMPEDANCE, PROPERTY=impedance property table name surface name Interaction module: Create Interaction: Acoustic impedance: select surface: Definition: Tabular, Acoustic impedance property: impedance property table name Specifying element-based impedance conditions Alternatively, you can define the impedance condition on element faces. The impedance is applied to element edges in two dimensions and to element faces in three dimensions. The edge or face of the element upon which the impedance is placed is identified by an impedance load type and depends on the element type . Input File Usage: *IMPEDANCE, PROPERTY=impedance property table name element number or set name, impedance load type label Abaqus/CAE Usage: Element-based impedance conditions are not supported in Abaqus/CAE. However, similar functionality is available using surface-based impedance conditions. Modifying or removing impedance conditions Impedance conditions can be added, modified, or removed as described in “Applying loads: overview,” Section 33.4.1. Radiation boundaries for exterior problems An exterior problem such as a structure vibrating in an acoustic medium of infinite extent is often of interest. Such a problem can be modeled by using acoustic elements to model the region between the structure and a simple geometric surface (located away from the structure) and applying a radiating (nonreflecting) boundary condition at that surface. The radiating boundary conditions are approximate, so the error in an exterior acoustic analysis is controlled not only by the usual finite element discretization error but also by the error in the approximate radiation condition. In Abaqus the radiation boundary conditions converge to the exact condition in the limit as they become infinitely distant from the radiating structure. In practice, these radiation conditions provide accurate results when the surface is at least one-half wavelength away from the structure at the lowest frequency of interest. Except in the case of a plane wave absorbing condition with zero volumetric drag, the impedance parameters in Abaqus/Standard are frequency dependent. The frequency-dependent parameters are used in the direct-solution and subspace-based steady-state dynamics procedures. In direct time integration procedures the zero-drag values for the constants are used. These values will give good results when the drag is small. (Small volumetric drag here means is the density where of the acoustic medium and is the circular excitation frequency or sound wave frequency.) and A direct-solution steady-state dynamics procedure (“Direct-solution steady-state dynamic analysis,” Section 6.3.4) must include both real and complex terms if nonreflecting (also called quiet) boundaries are present, because nonreflecting boundaries represent a form of damping in the system. Several radiating boundary conditions are implemented as special cases of the impedance boundary condition. The details of the formulation are given in “Coupled acoustic-structural medium analysis,” Section 2.9.1 of the Abaqus Theory Manual. Element-based impedance conditions are not supported in Abaqus/CAE. However, similar functionality is available using surface-based impedance conditions. Planar nonreflecting boundary condition The simplest nonreflecting boundary condition available in Abaqus assumes that the plane waves are normally incident on the exterior surface. This planar boundary condition ignores the curvature of the boundary and the possibility that waves in the simulation may impinge on the boundary at an arbitrary angle. The planar nonreflecting condition provides an approximation: acoustic waves are transmitted across such a boundary with little reflection of energy back into the acoustic medium. The amount of energy reflected is small if the boundary is far away from major acoustic disturbances and is reasonably orthogonal to the direction of dominant wave propagation. Thus, if an exterior (unbounded domain) problem is to be solved, the nonreflecting boundary should be placed far enough away from the sound source so that the assumption of normally impinging waves is sufficiently accurate. This condition would be used, for example, on the exhaust end of a muffler. Input File Usage: Use either of the following options (default): *SIMPEDANCE, NONREFLECTING=PLANAR *IMPEDANCE, NONREFLECTING=PLANAR Abaqus/CAE Usage: Use the following input boundary condition: to specify a surface-based planar nonreflecting Interaction module: Create Interaction: Acoustic impedance: select surface: Definition: Nonreflecting, Nonreflecting type: Planar Improved nonreflecting boundary condition for plane waves For the planar nonreflecting boundary condition to be accurate, the plane waves must be normally incident to a planar boundary. However, the angle of incidence is generally unknown in advance. A radiating boundary condition that is exact for plane waves with arbitrary angles of incidence is available in Abaqus. The radiating boundary can have any arbitrary shape. This boundary impedance is implemented only for transient dynamics. Input File Usage: Use either of the following options: Abaqus/CAE Usage: *SIMPEDANCE, NONREFLECTING=IMPROVED *IMPEDANCE, NONREFLECTING=IMPROVED Use the following input nonreflecting boundary condition: to specify a surface-based improved planar Interaction module: Create Interaction: Acoustic impedance: select surface: Definition: Nonreflecting, Nonreflecting type: Improved planar Geometry-based nonreflecting boundary conditions Four other types of absorbing boundary conditions that take the geometry of the radiating boundary into account are implemented in Abaqus: circular, spherical, elliptical, and prolate spheroidal. These boundary conditions offer improved performance over the planar nonreflecting condition if the nonreflecting surface has a simple, convex shape and is close to the acoustic sources. The various types of absorbing boundaries are selected by defining the required geometric parameters for the element-based or surface-based impedance definition. The geometric parameters affect the nonreflecting surface impedance. To specify a nonreflecting boundary that is circular in two dimensions or a right circular cylinder in three dimensions, you must specify the radius of the circle. To specify a nonreflecting spherical boundary condition, you must specify the radius of the sphere. To specify a nonreflecting boundary that is elliptical in two dimensions or a right elliptical cylinder in three dimensions or to specify a prolate spheroid boundary condition, you must specify the shape, location, and orientation of the radiating surface. The two parameters specifying the shape of the surface are the semimajor axis and the eccentricity. The semimajor axis, a, of an ellipse or prolate spheroid is analogous to the radius of a sphere: it is one-half the length of the longest line segment connecting two points on the surface. The semiminor axis, b, is one-half the length of the longest line segment that connects two points on the surface and is orthogonal to the semimajor axis line. The eccentricity, . , is defined as See “Acoustic radiation impedance of a sphere in breathing mode,” Section 1.11.3 of the Abaqus Benchmarks Manual, and “Acoustic-structural interaction in an infinite acoustic medium,” Section 1.11.4 of the Abaqus Benchmarks Manual, for benchmark problems showing the use of these conditions. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *SIMPEDANCE, NONREFLECTING=CIRCULAR *SIMPEDANCE, NONREFLECTING=SPHERICAL *SIMPEDANCE, NONREFLECTING=ELLIPTICAL *SIMPEDANCE, NONREFLECTING=PROLATE SPHEROIDAL In each case, the *IMPEDANCE element-based option can be used instead of *SIMPEDANCE. Use the following input to specify surface-based geometric nonreflecting boundary conditions: Interaction module: Create Interaction: Acoustic impedance: select surface: Definition: Nonreflecting, Nonreflecting type: Circular, Spherical, Elliptical, or Prolate spheroidal Combining different radiation conditions in the same problem Since the radiation boundary conditions for the different shapes are spatially local and do not involve discretization in the infinite exterior domain, an exterior boundary can consist of the combination of several shapes. The appropriate boundary condition can then be applied to each part of the boundary. For example, a circular cylinder can be terminated with hemispheres , or an elliptical cylinder can be terminated with prolate spheroidal halves. This modeling technique is most effective if the boundaries between surfaces are continuous in slope as well as displacement, although this is not essential. Concentrated pressure-conjugate load Distributed “loads” on acoustic elements can be interpreted as normal pressure gradients per unit density (dimensions of force per unit mass or acceleration). When used in Abaqus, the applied distributed loads must be integrated over a surface area, yielding a quantity with dimensions of force times area per unit mass (or volumetric acceleration). For analyses in the frequency domain and for transient dynamic analyses where the volumetric drag is zero, this acoustic load is equal to the volumetric acceleration of the fluid on the boundary. For example, a horizontal, flat rigid plate oscillating vertically imposes an acceleration on the acoustic fluid and an acoustic “load” equal to this acceleration times the surface area of the plate. For the transient dynamics formulation in the presence of volumetric drag, however, the specified “load” is slightly different. It is also a force times area per unit mass; but this force effect is partially lost to the volumetric drag, so the resulting volumetric acceleration of the fluid on the boundary is reduced. Noting this distinction for the special case of volumetric drag and transient dynamics, it is nevertheless convenient to refer to acoustic “loads” as volumetric accelerations in general. An inward volumetric acceleration can be applied by a positive concentrated load on degree of freedom 8 at a node of an acoustic element that is on the boundary of the acoustic medium. In Abaqus/Standard you can specify the in-phase (real) part of a load (default) and the out-of-phase (imaginary) part of a load. Inward particle accelerations (force per unit mass in transient dynamics) on the face of an acoustic element should be lumped to concentrated loads representing inward volumetric accelerations on the nodes of the face in the same way that pressure on a face is lumped to nodal forces on stress/displacement elements. Input File Usage: Use the following option to define the real part of the load: *CLOAD, REAL Use the following option to define the imaginary part of the load: *CLOAD, IMAGINARY Load module: Create Load: choose Acoustic for the Category and Inward volume acceleration for the Types for Selected Step Abaqus/CAE Usage: Incident wave loading due to external sources Abaqus provides a type of distributed load for loads due to external wave sources. Individual spherical monopole or individual or diffuse planar sources can be defined, subjecting the fluid and solid region of interest to an incident field of waves. Waves produced by an explosion or sound source propagate from the source, impinging on and passing over the structure, producing a temporally and spatially varying load on the structural surface. In the fluid the pressure field is affected by reflections and emissions from the structure as well as by the incident field from the source itself. The incident wave loads on acoustic and/or solid meshes depend on the location of the source node, the properties of the propagating fluid, and the reference time history or frequency dependence specified at the reference (“standoff”) node as indicated in Figure 33.4.6–1. Several distinct modeling methods can be used in Abaqus with incident wave loading, requiring different approaches to applying the incident wave loads. For problems involving solid and structural elements only (for example, where the incident wave field is due to waves in air) the wave loading is applied roughly like a distributed surface load. This might apply to an analysis of blast loads in air on a vehicle or building . In Abaqus/Explicit the CONWEP model can be used for air blast loading on solid and structural elements, without the need to model the fluid medium. “Deformation of a sandwich plate under CONWEP blast loading,” Section 9.1.8 of the Abaqus Example Problems Manual, is an example of a blast loading problem. Incident wave loads (with the exception of CONWEP loading) can be applied to beam structures as well; this is a common modeling method for ship whipping analysis and for steel frame buildings subject to blast loads. Incident wave loads can be applied to surfaces defined on two- or three-dimensional beam elements. However, incident wave loads can be applied only to three-dimensional beams for transient dynamic analysis where beam fluid inertia is defined. Incident wave loads cannot be defined on frame elements, line spring elements, three-dimensional open-section beam elements, or three-dimensional Euler-Bernoulli beams. In underwater explosion analyses (for example, a ship or submerged vehicle subjected to an underwater explosion loading as depicted in Figure 33.4.6–4 and Figure 33.4.6–5) the fluid is also discretized using a finite element model to capture the effects of the fluid stiffness and inertia. For these problems involving both solid and acoustic elements, two formulations of the acoustic pressure field Specify speed of sound and density for propagating wave acoustic mesh exterior surface structural mesh fluid surface solid surface reference or "standoff" node source node (where explosion charge occurs) Figure 33.4.6–1 Incident wave loading model. exist. First, the acoustic elements can be used to model the total pressure in the medium, including the effects of the incident field and the overall system’s response. Alternatively, the acoustic elements can be used to model only the response of the medium to the wave loads, not the wave pulse itself. The former case will be referred to as the “total wave” formulation, the latter as the “scattered wave” formulation. Incident wave interactions are also used to model sound fields impinging on structures or acoustic domains. The acoustic field scattered by a structure or the sound transmitted through the structure may be of interest. Usually, sound scattering and transmission problems are modeled using the scattered formulation with steady-state dynamic procedures. Transient procedures can also be used, in a manner analogous to underwater explosion analysis problems. Scattered and total wave formulations The distinction between the total wave formulation and the scattered wave formulation is relevant only when incident wave loads are applied. The total wave formulation is more closely analogous to structural loading than the scattered wave formulation: the boundary of the acoustic medium is specified as a loaded surface, and a time-varying load is applied there, which generates a response in the acoustic medium. This response is equal to the total acoustic pressure in the medium. The scattered wave formulation exploits the fact that when the acoustic medium is linear, the response in the medium can be decomposed into a sum of the incident wave and the scattered field. The total wave formulation must be used when the acoustic medium is nonlinear due to possible fluid cavitation . Table 33.4.6–1 describes the procedure types for which each formulation is supported. Table 33.4.6–1 Supported procedures for scattered and total wave formulations. Procedure Scattered Total Wave Steady-state dynamics Transient Yes Yes No Yes Scattered wave formulation When the mechanics of a fluid can be described as linear, the observed total acoustic pressure can be decomposed into two components: the known incident wave and the “scattered” wave that is produced by the interaction of the incident wave with structures and/or fluid boundaries. When this superposition is applicable, it is common practice to seek the “scattered” wave field solution directly. When using the scattered wave formulation, the pressures at the acoustic nodes are defined to be only the scattered part of the total pressure. Both acoustic and solid surfaces at the acoustic-structural interface should be loaded in this case. When using incident wave loads in steady-state dynamic procedures, the scattered wave formulation must be used. Input File Usage: Use the following option to specify the scattered wave formulation (default): Abaqus/CAE Usage: *ACOUSTIC WAVE FORMULATION, TYPE=SCATTERED WAVE Any module: Model→Edit Attributes→model_name. Toggle on Specify acoustic wave formulation: select Scattered wave Total wave formulation The total wave formulation is particularly applicable when the acoustic medium is capable of cavitation, rendering the fluid mechanical behavior nonlinear. It should also be used if the problem contains either a curved or a finite extent boundary where the pressure history is prescribed. Only the outer acoustic surfaces should be loaded with the incident wave in this case, and the incident wave source must be located exterior to the fluid model. Any impedance or nonreflecting condition that may exist on this outer acoustic boundary applies only on the part of the acoustic solution that does not include the prescribed incident wave field (that is, only the scattered field is subject to the nonreflecting condition). Thus, the applied incident wave loading will travel into the problem domain without being affected by the nonreflecting conditions on the outer acoustic surface. In the total wave formulation the acoustic pressure degree of freedom stands for the total dynamic acoustic pressure, including contributions from incident and scattered waves and, in Abaqus/Explicit, the dynamic effects of fluid cavitation. The pressure degree of freedom does not include the acoustic static pressure, which can be specified as an initial condition . This acoustic static pressure is used only in determining the cavitation status of the acoustic element nodes and does not apply any static loads to the acoustic or structural mesh at their common wetted interface. It does not apply to analyses using Abaqus/Standard. Input File Usage: Use the following option to specify the total wave formulation: Abaqus/CAE Usage: *ACOUSTIC WAVE FORMULATION, TYPE=TOTAL WAVE Any module: Model→Edit Attributes→model_name. Toggle on Specify acoustic wave formulation: select Total wave Initialization of acoustic fields For transient dynamics, when the total wave formulation is used with the incident wave standoff point located inside the acoustic finite element domain, the acoustic solution is initialized to the values of the incoming incident wave. This initialization is performed automatically, for pressure-based incident wave amplitude definitions only, at the beginning of the first direct-integration dynamic step in an analysis; in restarted analyses, steps are counted from the beginning of the initial analysis. This initialization not only saves computational time but also applies the incident wave loading without significant numerical dissipation or distortion. During the initialization phase all incident wave loading definitions in the first dynamic analysis step are considered, and all acoustic element nodes are initialized to the incident wave field at time zero. Incident wave loads specified with different source locations count as separate load definitions for the purpose of initialization of the acoustic nodes. Any reflections of the incident wave loads are also taken into account during the initialization phase. Describing incident wave loading To use incident wave loading, you must define the following: • information that establishes the direction and other properties of the incident wave, • the time history or frequency dependence of the source pulse at some reference (“standoff”) point, • the fluid and/or solid surfaces to be loaded, and • any reflection plane outside the problem domain, such as a seabed in an underwater explosion study, that would reflect the incident wave onto the problem domain. Two interfaces are available in Abaqus for applying incident wave loads: a preferred interface that is supported in Abaqus/CAE and an alternative interface that has been available in previous releases and is not supported in Abaqus/CAE. The preferred interface is conceptually the same as the alternative interface and uses essentially the same data. The preferred interface options include the term “interaction” to distinguish them from the incident wave and incident wave property options of the alternative interface. Unless otherwise specified, the discussion in this section applies to both of the interfaces. The usages for the preferred interface are included in the discussion; the usages for the alternative interface are described in “Alternative incident wave loading interface,” below. Refer to the example problems discussed at the end of this section to see how the incident wave loading is specified using the preferred interface. Prescribing geometric properties and the speed of the incident wave You must refer to a property definition for each prescribed incident wave. Incident wave loads in Abaqus may be either planar, spherical, or diffuse. You select a planar incident wave (default), spherical incident wave, or a diffuse field in the incident wave property definition. Planar incident waves maintain constant amplitude as they travel in space; consequently, the speed and direction of travel are the critical parameters to define. The speed is defined in the incident wave interaction property definition, and the direction is determined by the locations of the source and standoff points you define as part of the incident wave interaction. For spherical incident wave definitions, the wave reduces in amplitude as a function of space. By default, the amplitude of a spherical wave is inversely proportional to the distance from the source; this behavior is called “acoustic” propagation. For the preferred interface you can modify the default propagation behavior to define spatial decay of the incident wave field. The dimensionless constants , between the source point are used to define the spatial decay as a function of the distance , and and the loaded point and the distance between the source point and the standoff point: Refer to “Loading due to an incident dilatational wave field,” Section 6.3.1 of the Abaqus Theory Manual, for details of the generalized spatial decay formulation. In Abaqus incident wave interactions can be used to simulate diffuse incident fields. Diffuse fields are characteristic of reverberant spaces or other situations in which waves from many directions strike a surface. For example, reverberant chambers are constructed intentionally in acoustic test facilities for sound transmission loss measurements. The diffuse field model used in Abaqus, as shown in Figure 33.4.6–2, allows you to specify a seed number deterministic incident plane waves travel along vectors distributed over a hemisphere so that the incident power per solid angle approximates a diffuse incident field. ; The fluid and the solid surfaces where the incident loading acts are specified in the incident wave loading definition. The incoming wave load is further described by the locations of its source point and of a reference (“standoff”) point where the wave amplitude is specified. For information on how to specify these surfaces and the standoff point, see “Identifying the fluid and the solid surfaces for incident wave loading,” and “The standoff point” below. For a planar wave the specified locations of the source and the standoff points are used to define the direction of wave propagation. The speed of the incident wave is prescribed by giving the properties for the incident wave-bearing acoustic medium. These specified properties should be consistent with the properties specified for the fluid discretized using acoustic elements. For the preferred interface you must define nodes corresponding to the source and standoff points for the incident wave; the node numbers or set names must be specified for each incident wave definition. “Source” Unit hemisphere oriented along source-standoff vector Plane wave along one of N2 directions Plane normal to source-standoff vector N seed point columns “Standoff” N seed point rows FE surface to be loaded Figure 33.4.6–2 Diffuse loading model. The node set names, if used, must contain only a single node. Neither the source node nor the standoff node should be connected to any elements in the model. Input File Usage: *INCIDENT WAVE INTERACTION PROPERTY, NAME=wave property name, TYPE=PLANE or SPHERE speed of sound, fluid mass density, A, B, C *INCIDENT WAVE INTERACTION, PROPERTY=wave property name fluid surface name, source node, standoff node, reference magnitude The constants A, B, and C apply only for spherical incident waves with generalized spatial decay propagation. *INCIDENT WAVE INTERACTION PROPERTY, NAME=wave property name, TYPE=DIFFUSE speed of sound, fluid mass density *INCIDENT WAVE INTERACTION, PROPERTY=wave property name fluid surface name, source node, standoff node, reference magnitude, N Abaqus/CAE Usage: The seed number N generates planar incident waves with directions distributed on a hemisphere centered at the standoff point. Interaction module: Create Interaction Property: Name: wave property name and Incident wave, Speed of sound in fluid: speed of sound, Fluid density: fluid mass density Select one of the following definitions: Definition: Planar Definition: Spherical, Propagation model: Acoustic Definition: Spherical, Propagation model: Generalized decay, enter values for A, B, and C Definition: Diffuse, Seed number: N Create Interaction: Incident wave: select the source point, select the standoff point, select the region: Wave property: wave property name, Reference magnitude: reference magnitude Identifying the fluid and the solid surfaces for incident wave loading In the scattered wave formulation the incident wave loading must be specified on all fluid and solid surfaces that reflect the incident wave with two exceptions: • those fluid surfaces that have the pressure values directly prescribed using boundary conditions; and • those fluid surfaces that have symmetry conditions (the symmetry must hold for both the loading and the geometry). In problems with a fluid-solid interface both surfaces must be specified in the incident wave loading definition for the scattered formulation. See “Example: submarine close to the free surface,” shown in Figure 33.4.6–4. When the total pressure-based formulation is specified, the incident wave loading must be specified only on the fluid surfaces that border the infinite region that is excluded from the model. Typically, these surfaces have a nonreflecting radiation condition specified on them, and the implementation ensures that the radiation condition is enforced only on the scattered response of the modeled domain and not on the incident wave itself. See “Example: submarine close to the free surface,” and “Example: surface ship,” shown in Figure 33.4.6–4 and Figure 33.4.6–5, respectively. In certain problems, such as blast loads in air, you may decide that the blast wave loads on a structure need to be modeled, but the surrounding fluid medium itself does not. In these problems the incident wave loading is specified only on the solid surfaces since the fluid medium is not modeled. The distinction between the scattered wave formulation and the total wave formulation for handling the incident wave loading is not relevant in these problems since the wave propagation in the fluid medium is of no interest. The standoff point In transient analyses the standoff point is a reference point used to specify the pulse loading time history: it is the point at which the user-defined pulse history is assumed to apply with no time delay, phase shift, or spreading loss. In steady-state analyses using discrete planar or spherical sources, the standoff point is the point at which the incident field has zero phase. In transient analyses the standoff point should be defined so that it is closer to the source than any point on the surfaces in the model that would reflect the incident wave. Doing so ensures that all the points on these surfaces will be loaded with the specified time history of the source and that the analysis begins before the wave overtakes any portion of these surfaces. To save analysis time, the standoff point is typically on or near the solid surface where the incoming incident wave would be first deflected . However, the standoff point is a fixed point in the analysis: if the loaded surfaces move before the incident wave loading begins, due to previous analysis steps or geometric adjustments, the surfaces may envelop the specified standoff point. Care should be taken to define a standoff point such that it remains closer to the incident wave source point than any point on the loaded surfaces at the onset of the loading. When the total wave formulation is used and the incident wave loading is specified in the first step of the analysis in terms of pressure history, Abaqus automatically initializes the pressure and the pressure rate at the acoustic nodes to values based on the incident wave loading. This allows the acoustic analysis to start with the incident waves partially propagated into the problem domain at time zero and assumes that this propagation had taken place with negligible effect of any volumetric dissipative sources such as the fluid drag. When the incident wave loading is specified in terms of the pressure values, the recommendations given above for selecting a standoff point are valid with the total wave formulation as well. However, when the incident wave loading is specified in terms of acceleration values, the automatic initialization is not done and the standoff point should be located near the exterior fluid boundary of the model such that the standoff point is closer to the source than any point on the exterior boundary. See “Example: submarine close to the free surface,” and “Example: surface ship,” shown in Figure 33.4.6–4 and Figure 33.4.6–5, respectively. In steady-state analyses the role of the standoff point is somewhat different. When the incident wave interaction property is of planar or spherical type, you define the real and imaginary parts of the magnitude at the standoff point. Separately, the specified real and imaginary incident waves are taken to have zero phase at the standoff point (combined, these two waves could be equivalent to a single wave with nonzero phase at the standoff). Every location on the loaded surface has a phase shift in the applied pressure or acoustic traction, corresponding to the difference in propagation time between the loaded point and the standoff. This means that an incident wave defined, for example, with a pure real value at the standoff point generates both real and imaginary tractions at all the other points on the loaded surface. When the incident wave is of diffuse type, the role of the standoff and source points is primarily to orient the loaded surface with respect to the incoming reverberant field. The model used for diffuse incident wave loading applies a set of deterministically defined plane waves, whose directions are defined as vectors connecting the standoff point and an array of points on a hemisphere. This hemisphere is centered at the standoff point, and its apex is the source point. The array of points is set according to the specified seed, points on the hemisphere. The algorithm concentrates the points so that the incident waves in the diffuse field model are concentrated at normal incidence, with fewer waves at oblique angles. The specified amplitude value and reference magnitude are divided equally among the incident waves. The orientation of , and a deterministic algorithm that arranges the hemisphere containing the incident waves in the diffuse model is the same for all of the points on the loaded surface—it does not vary with the local normal vector on the surface. Defining the amplitude of the source pulse For transient analyses the time history to be specified by the user is that observed at the standoff point: histories at a point on the loaded surface are computed from the wave type and the location of that point relative to the standoff point. The time history of the acoustic source pulse can be defined either in terms of the fluid pressure values or the fluid particle acceleration values. Pressure time histories can be used for any type of element, such as acoustic, structural, or solid elements; acceleration time histories are applicable only for acoustic elements. In either case a reference magnitude is specified for any given incident-wave-loaded surface, and a reference to a time-history data table defined by an amplitude curve is specified. The reference magnitude varies with time according to the amplitude definition. For steady-state dynamic analyses the amplitude definition specified as part of the incident wave interaction definition is interpreted as the frequency dependence of the wave at the standoff point. Currently the source pulse description in terms of fluid particle acceleration history is limited to planar incident waves acting on fluid surfaces in transient analyses. Further, if an impedance condition is specified on the same fluid surface along with incident wave loading, the source pulse is restricted to the pressure history type even for planar incident waves. The source pulse in terms of pressure history can be used without these limitations; i.e., pressure-history-based incident wave loading can be used with fluid or solid surfaces, with or without impedance, and for both planar and spherical incident waves. When the source pulse is specified using pressure values and is applied on a fluid surface, the pressure gradient is computed and applied as a pressure-conjugate load on these surfaces. Hence, it is desirable to define the pulse amplitude to begin with a zero value, particularly when the cavitation in the fluid is a concern. If the structural response is of primary concern and the scattered formulation is being used, any initial jump in the pressure amplitude can be addressed by applying additional concentrated loads on the structural nodes that are tied to the acoustic mesh, corresponding to the initial jump in the incident wave pressure amplitude. Clearly, the additional load on any given structural node should be active from the instance the incident wave first arrives at that structural node. However, the scattered wave solution in the fluid still needs careful interpretation taking the initial jump into account. Input File Usage: Use the following option to define the time history in terms of fluid pressure values: *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=amplitude data table name solid or fluid surface name, source node, standoff node, reference magnitude Use the following option to define the time history in terms of fluid particle acceleration values: *INCIDENT WAVE INTERACTION, ACCELERATION AMPLITUDE=amplitude data table name fluid surface name, source node, standoff node, reference magnitude ACOUSTIC AND SHOCK LOADS Use the following option to define the real part of the loading (default): *INCIDENT WAVE INTERACTION, REAL Use the following option to define the imaginary part of the loading: *INCIDENT WAVE INTERACTION, IMAGINARY Interaction module: Create Interaction: Incident wave: select the source point, select the standoff point, select the region: Reference magnitude: reference magnitude Use the following options to define the time history in terms of fluid pressure values or fluid particle acceleration values: Definition: Pressure or Acceleration, Pressure amplitude or Acceleration amplitude: amplitude data table name Use the following options to define the real or imaginary part of the loading: Toggle on Real amplitude and/or Imaginary amplitude: amplitude data table name Defining bubble loading for spherical incident wave loading An underwater explosion forms a highly compressed gas bubble that interacts with the surrounding water, generating an outward-propagating shock wave. The gas bubble floats upward as it generates these waves changing the relative positions of the source and the loaded surfaces. The loading effects due to bubble formation can be defined for spherical incident wave loading by using a bubble definition in conjunction with the incident wave loading definition. The bubble dynamics can be described using a model internal to Abaqus or by using tabulated data. Abaqus has a built-in mechanical model of the bubble interacting with the surrounding fluid, which is simulated numerically to generate a set of data prior to running the finite element analysis. You can specify the explosive material parameters, ending time, and other parameters that affect the computation of the bubble amplitude curve used, as shown in Table 33.4.6–2. Table 33.4.6–2 Parameters that define the bubble behavior. Name Dimensions Description Default FL−2 (LM−1/3 )1+A Charge constant T/(M LB ) Charge constant Dimensionless Similitude spatial exponent Dimensionless Similitude temporal exponent F/L2 Charge constant Dimensionless Ratio of specific heats for explosion gas None None None None None None Name Dimensions Description Default None None None None None None None None 1.0 0.0 2.0 None 1500 M/L3 Dimensionless Dimensionless Dimensionless L/T2 F/L2 Charge material density Mass of charge Initial charge depth X-direction cosine of the free surface normal Y-direction cosine of the free surface normal Z-direction cosine of the free surface normal Acceleration due to gravity Atmospheric pressure at free surface Dimensionless Wave effect parameter Dimensionless Bubble drag coefficient Dimensionless Bubble drag exponent Dimensionless Dimensionless Dimensionless Dimensionless M/L3 L/T Maximum allowable time in bubble simulation Maximum allowable number of steps in bubble simulation Relative error tolerance parameter for bubble simulation Absolute error tolerance parameter for bubble simulation 1 × 10−11 1 × 10−11 Error control exponent for bubble simulation 0.2 Fluid mass density Fluid speed of sound None None All of the parameters specified affect only the bubble amplitude; other physical parameters in the problem are independent. You can suppress the effects of wave loss in the bubble dynamics and introduce empirical flow drag, if desired. Detailed information about the bubble mechanical model is given in “Loading due to an incident dilatational wave field,” Section 6.3.1 of the Abaqus Theory Manual. In an underwater explosion event a bubble migrates upward toward, and possibly reaches, the free water surface. If the bubble migration reaches the free water surface during the specified analysis time, Abaqus applies loads of zero magnitude after this point. Model data about the bubble simulation are written to the data (.dat) file. During an Abaqus/Standard analysis history data are written each increment to the output database (.odb) file. The history data include the radius of the bubble and the bubble depth below the free water surface. For reference, the pressure and acoustic load quantities at the standoff point are also written to the data file; these load terms include the direct plane-wave term and the spherical spreading (“afterflow”) effect . For the preferred interface the loading effects due to bubble formation can be defined for spherical incident wave loading using the UNDEX charge property definition. Because the bubble simulation uses spherical symmetry, the incident wave interaction property must define a spherical wave. You can also specify incident wave loading due to bubble dynamics using tabulated data for the pressure and source migration. For the preferred interface you specify independent amplitude curves for the pressure at the standoff point and any source node location time histories. The source location amplitude names are referred to from boundary condition definitions for the source node. Input File Usage: Use the following options to specify loading effects due to bubble formation using the UNDEX charge property definition: *INCIDENT WAVE INTERACTION PROPERTY, NAME=wave property name, TYPE=SPHERE *UNDEX CHARGE PROPERTY data defining the UNDEX charge *INCIDENT WAVE INTERACTION, PROPERTY=wave property name, UNDEX fluid surface name, source node, standoff node, reference magnitude Use the following options to specify pressure at the standoff point using tabulated data: *AMPLITUDE, DEFINITION=TABULAR, NAME=pressure *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=pressure solid or fluid surface name, source node, standoff node, reference magnitude Use the following options to specify source node location time histories using tabulated data: *AMPLITUDE, DEFINITION=TABULAR, NAME=name *BOUNDARY, TYPE=DISPLACEMENT or VELOCITY, AMPLITUDE=name source node, degrees of freedom Abaqus/CAE Usage: Use the following input to specify loading effects due to bubble formation using the UNDEX charge property definition: Interaction module: Create Interaction Property: Name: wave property name and Incident wave: Definition: Spherical, Propagation model: UNDEX charge, enter data defining the UNDEX charge Create Interaction: Incident wave: Definition: UNDEX, Wave property: wave property name, enter data defining the UNDEX charge Use the following input to specify pressure at the standoff point using tabulated data: Load or Interaction module: Create Amplitude: Name: pressure and select Tabular Interaction module: Create Interaction: Incident wave: select the standoff point: Definition: Pressure, Pressure amplitude: pressure Use the following input to specify source node location time histories using tabulated data: Load or Interaction module: Create Amplitude: Name: name and select Tabular Load module: Create Boundary Condition: select step: Displacement/Rotation or Velocity/Angular velocity: select the source node as the region and toggle on the degree or degrees of freedom, Amplitude: name Modeling incident wave loading on a moving structure To model the effect of relative motion between a structure (such as a ship) and the wave source during the analysis using the preferred interface, the source node may be assigned a velocity. It is assumed that the entire fluid-solid model is moving at a velocity with respect to the source node during the loading and that the speed of the model’s motion is low compared to the speed of propagation of the incident wave. That is, the effect of the speed of the source is neglected in the computation of the loads, but the change in position of the source is included. This is equivalent to assuming that the relative motion between the source and the model is at a low Mach number. Relative motion can be specified only for transient analyses. In addition to prescribing boundary conditions at the source node, a small mass element must be defined at the source node. Input File Usage: Use the following option to assign a velocity to the source node: *BOUNDARY, TYPE=DISPLACEMENT or VELOCITY, AMPLITUDE=name source node, degrees of freedom Abaqus/CAE Usage: Load module: Create Boundary Condition: select step: Velocity/Angular velocity or Displacement/Rotation: select regions and toggle on the degree or degrees of freedom, Amplitude: name Specifying the reflection effects The waves emanating from the source may reflect off plane surfaces, such as seabeds or sea surfaces, before reaching the specified standoff point. Thus, the incident wave loading consists of the waves arriving from a direct path from the source, as well as those arriving from reflections off the planes. In Abaqus an arbitrary number of these planes can be defined, each with its own location, orientation, and reflection coefficient. If no reflection coefficient is specified, the plane is assumed to be nonreflective; a zero reflected If a reflection coefficient is specified, the magnitude of the reflected waves are pressure is applied. modified by the reflection coefficient according to the formula: Only real values for are used. The reflection planes are allowed only for incident waves that are defined in terms of fluid pressure values. Only one reflection off each plane is considered. If the effect of many successive reflections is important, these surfaces should be part of the finite element model. Reflection planes should not be used at a boundary of the finite element model if the total wave formulation is used, since in that case the incident wave will be reflected automatically by that boundary. Input File Usage: Use the following option in conjunction with the *INCIDENT WAVE INTERACTION option to define an incident wave reflection plane: Abaqus/CAE Usage: *INCIDENT WAVE REFLECTION Incident wave reflections are not supported in Abaqus/CAE. Boundary with prescribed pressure The acoustic pressure degree of freedom at nodes of acoustic elements can be prescribed using a boundary condition. However, since you can use the nodal acoustic pressure in an Abaqus analysis to refer to the total pressure at that point or to only the scattered component, care must be exercised in some circumstances. When the total wave formulation is used, a boundary condition alone is sufficient to specify a prescribed total dynamic pressure on a boundary. In an analysis without incident wave loading, the nodal degree of freedom is generally equal to the total acoustic pressure at that point. Therefore, its value can be prescribed using a boundary condition in a manner consistent with other boundary conditions in Abaqus. For example, you may set the acoustic pressure at all of the nodes at a duct inlet to a prescribed amplitude to analyze the propagation of waves along the duct. The free surface of a body of water can be modeled by setting the acoustic pressure to zero at the surface. When incident wave loading is used, the scattered wave formulation defines the nodal acoustic degree of freedom to be equal to the scattered pressure. Consequently, a boundary condition definition for this degree of freedom affects the scattered pressure only. The total acoustic pressure at a node is not directly accessible in this formulation. Specification of the total pressure in a scattered formulation analysis is nevertheless required in some instances (for example, when modeling a free surface of a body of water). In this case, one of the following methods should be used. If the fluid surface with prescribed total pressure is planar, unbroken, and of infinite extent, an incident wave reflection plane and a boundary condition can be used together to model the fact that the total pressure is zero on the free surface. A “soft” incident wave reflection plane coincident with the free surface will make sure that the structure is subjected to the incident wave load reflected off the free surface. A boundary condition setting the acoustic pressure in the surface equal to zero will make sure that any scattered waves emitted by the structure are reflected properly. The scattered wave solution in the fluid must be interpreted taking into consideration the fact that the incident field now includes a reflection of the source as well. If the fluid surface with prescribed total pressure is planar but broken by an object, such as a floating ship, this modeling technique may still be applied. However, the reflected loads due to the incident wave are computed as if the reflection plane passes through the hull of the ship; this approximation neglects some diffraction effects and may or may not be applicable in all situations of interest. Alternatively, the free surface condition of the fluid can be eliminated by modeling the top layer of the fluid using structural elements, such as membrane elements, instead of acoustic elements. The “structural fluid” surface and the “acoustic fluid” surface are then coupled using either a surface-based mesh tie constraint (“Mesh tie constraints,” Section 34.3.1) or, in Abaqus/Standard, acoustic-structural interface elements; and the incident wave loading must be applied on both the “structural fluid” and the “acoustic fluid” surfaces. The material properties of the “structural fluid” elements should be similar to those of the adjacent acoustic fluid. In Abaqus/Explicit the thickness of the “structural fluid” elements must be such that the masses at nodes on either side of the coupling constraint are nearly equal. This modeling technique allows the geometry of the surface on which total pressure is to be prescribed to depart from an unbroken, infinite plane. As a secondary benefit of this technique, you can obtain the velocity profile on the free surface since the displacement degrees of freedom are now activated at the If a nonzero pressure boundary condition is desired, it can be applied as a “structural fluid” nodes. distributed loading on the other side of the “structural fluid” elements. Input File Usage: Use the following options for the first modeling technique with the default scattered wave formulation: *BOUNDARY *INCIDENT WAVE REFLECTION Use the following option for the second modeling technique with the default scattered wave formulation: *TIE *INCIDENT WAVE INTERACTION Use the following option with the total wave formulation: Abaqus/CAE Usage: *BOUNDARY Load module: Create BC: choose Other for the Category and Acoustic pressure for the Types for Selected Step Defining air blast loading for incident shock waves using the CONWEP model in Abaqus/Explicit An explosion in air forms a highly compressed gas mass that interacts with the surrounding air, generating an outward-propagating shock wave. The loading effects due to an explosion in air can be defined, for spherical incident waves (air blast) or hemispherical incident waves (surface blast), by empirical data provided by the CONWEP model in conjunction with the incident wave loading definition. Unlike an acoustic wave, a blast wave corresponds to a shock wave with discontinuities in pressure, density, etc. across the wave front. Figure 33.4.6–3 shows a typical pressure history of a blast wave. Pressure max Exponential decay Positive phase atm Time of detonation Time of arrival Negative phase Time Figure 33.4.6–3 Pressure history of a blast wave. The CONWEP model uses a scaled distance based on the distance of the loading surface from the source of the explosion and the amount of explosive detonated. For a given scaled distance, the model provides the following empirical data: the maximum overpressure (above atmospheric), the arrival time, the positive phase duration, and the exponential decay coefficient for both the incident pressure and the reflected pressure. Using these parameters, the entire time history of both the incident pressure and reflected pressure as shown in Figure 33.4.6–3 can be constructed. Use of a standoff point is not required. , on a surface due to the blast wave is a function of the incident pressure, , which is defined as the angle between the normal of the loading surface and the vector that points from the surface to the explosion source. The total pressure is defined as , and the angle of incidence, , the reflected pressure, The total pressure, The air blast loading due to the total pressure can be scaled using a magnitude scale factor. A detonation time can be specified if the explosion does not occur at the start of the analysis. The detonation time needs to be given in total time; see “Conventions,” Section 1.2.2, for a description of the time convention. The arrival time at a location is defined as the elapsed time for the wave to arrive at that location after detonation. The CONWEP empirical data are given in a specific set of units, which must be converted to the units used in the analysis. You will need to specify multiplying factors for conversion of these units to SI units. For the specification of the mass of the explosive in TNT equivalence, you can choose any convenient mass unit, which can be different from the mass unit used in the analysis. For computation of the pressure loading, you will need to specify multiplying factors for conversion of length, time, and pressure units used in the analysis to SI units. Some typical conversion multiplier values are given in Table 33.4.6–3. Table 33.4.6–3 Multipliers used in conjunction with the CONWEP model for conversion to SI units. Quantity Unit SI Unit Multiplier for conversion to SI Mass Mass Length Length Time Pressure Pressure Pressure ton lb mm ft msec MPa psi psf kg kg sec Pa Pa Pa 1000 0.45359 0.001 0.3048 0.001 10−6 6894.8 47.88 For any given amount of explosive, the CONWEP empirical data are valid only within a range of distances from the source. The minimum distance at which the data are valid corresponds to the charge radius. Thus, the analysis terminates if the distance of any part of the loading surface from the source is less than the charge radius. For distances that are larger than the maximum valid range, linear extrapolation is used up to an extended maximum range where the reflected pressure decreases to zero. No loading is applied beyond the extended maximum range. The CONWEP empirical data do not account for shadowing by intervening objects or for any effects due to confinement. In the definition of incident wave interaction using the CONWEP model, you cannot use incident wave reflection. The CONWEP pressure load can be requested as element face variable output to the output database file . Input File Usage: Use the following options to specify loading effects due to explosion in air using the CONWEP charge property definition: *INCIDENT WAVE INTERACTION PROPERTY, NAME=wave property name, TYPE=AIR BLAST or SURFACE BLAST *CONWEP CHARGE PROPERTY data defining the CONWEP charge *INCIDENT WAVE INTERACTION, PROPERTY=wave property name, CONWEP loading surface name, source node, detonation time, magnitude scale factor Abaqus/CAE Usage: Use the following options to specify loading effects due to explosion in air using the CONWEP charge property definition: Interaction module: Create Interaction Property: Name: wave property name and Incident wave: Definition: Air blast or Surface blast: enter data defining the CONWEP charge Interaction module: Create Interaction: Name: incident wave name and Incident wave: select the source point: CONWEP (Air/Surface blast): select the region: CONWEP Data: enter data defining the time of detonation and magnitude scale factor Modifying or removing incident wave loads Only the incident wave loads that are specified in a particular step are applied in that step; previous definitions are removed automatically. Consequently, incident wave loads that are active during two subsequent steps should be specified in each step. This is akin to the behavior that can be specified for other types of loads by releasing any load of that type in a step . Alternative incident wave loading interface In general, the concepts of the alternative incident wave loading interface are the same as the preferred interface; however, the syntax for specifying the incident wave loading is different. The preferred incident wave loading interface is supported in Abaqus/CAE. The alternative interface is not supported in Abaqus/CAE. For conceptual information, see “Incident wave loading due to external sources.” Prescribing the geometric properties and the speed of the incident wave (alternative interface) Conceptually, the alternative interface is the same as the preferred interface; however, the usages are different. For conceptual information, see “Prescribing geometric properties and the speed of the incident wave.” Input File Usage: Abaqus/CAE Usage: *INCIDENT WAVE PROPERTY, NAME=wave property name, TYPE=PLANE or SPHERE data lines to specify the location of the acoustic source and the standoff point *INCIDENT WAVE FLUID PROPERTY bulk modulus, mass density *INCIDENT WAVE, PROPERTY=wave property name The alternative incident wave loading interface is not Abaqus/CAE. supported in Defining the time history of the source pulse (alternative interface) Conceptually, the alternative interface is the same as the preferred interface; however, the usages are different. For conceptual information, see “Defining the amplitude of the source pulse.” Input File Usage: Use the following option to define the time history in terms of fluid pressure values: *INCIDENT WAVE, PRESSURE AMPLITUDE=amplitude data table name solid or fluid surface name, reference magnitude Use the following option to define the time history in terms of fluid particle acceleration values: *INCIDENT WAVE, ACCELERATION AMPLITUDE=amplitude data table name fluid surface name, reference magnitude Abaqus/CAE Usage: The alternative incident wave loading interface is not Abaqus/CAE. supported in Defining bubble loading for spherical incident wave loading (alternative interface) Conceptually, the alternative interface is the same as the preferred interface; however, the usages are different. For conceptual information, see “Defining bubble loading for spherical incident wave loading.” To define the bubble dynamics using a model internal to Abaqus, you can specify a bubble amplitude. Use of the bubble loading amplitude is generally similar to the use of any other amplitude in Abaqus. Input File Usage: Use the following options: *AMPLITUDE, DEFINITION=BUBBLE, NAME=name *INCIDENT WAVE PROPERTY, TYPE=SPHERE, NAME=wave property name *INCIDENT WAVE, PRESSURE AMPLITUDE=name solid or fluid surface name, reference magnitude Abaqus/CAE Usage: The alternative incident wave loading interface is not Abaqus/CAE. supported in To define the bubble dynamics using tabulated data for the pressure and source migration, you can specify independent amplitude curves for the pressure at the standoff point and any source location time histories. The source location amplitude names, or floating point data for source point coordinates that remain fixed, are referred to in the incident wave property definition. The amplitude name for the pressure amplitude is referred to in the incident wave loading definition in the usual manner. Input File Usage: Use the following options: *AMPLITUDE, DEFINITION=TABULAR, NAME=Pressure *AMPLITUDE, DEFINITION=TABULAR, NAME=X *AMPLITUDE, DEFINITION=TABULAR, NAME=Y *AMPLITUDE, DEFINITION=TABULAR, NAME=Z *INCIDENT WAVE PROPERTY, TYPE=SPHERE, NAME=wave property name {standoff point data} X, Y, Z *INCIDENT WAVE, PRESSURE AMPLITUDE=Pressure solid or fluid surface name, reference magnitude Abaqus/CAE Usage: The alternative incident wave loading interface is not Abaqus/CAE. supported in Specifying the reflection effects (alternative interface) Conceptually, the alternative interface is the same as the preferred interface; however, the usages are different. For conceptual information, see “Specifying the reflection effects.” Input File Usage: Use the following option in conjunction with the *INCIDENT WAVE option to define an incident wave reflection plane: Abaqus/CAE Usage: *INCIDENT WAVE REFLECTION The alternative incident wave loading interface is not Abaqus/CAE. supported in Modeling incident wave loading on a moving structure (alternative interface) To model the effect of rigid motion of a structure such as a ship during the incident wave loading history, the standoff point can have a specified velocity. It is assumed that the entire fluid-solid model is moving at this velocity with respect to the source point during the loading and that the speed of the model’s motion is low compared to the speed of propagation of the incident wave. Input File Usage: *INCIDENT WAVE PROPERTY, NAME=wave property name data line to specify the velocity of the standoff point Abaqus/CAE Usage: The alternative incident wave loading interface is not Abaqus/CAE. supported in Example: submarine close to the free surface The problem shown in Figure 33.4.6–4 has the following features: a free surface reflection plane, a wet solid surface the boundary of the underwater explosion loading is also shown. as a , and of the finite modeled domain separating the infinite acoustic medium. The source S , seabed that is tied to the solid surface , the fluid surface Free surface A 0 Acoustic medium Source Seabed A sb Solid surface Asw Fluid surface Afw inf model boundary Figure 33.4.6–4 Incident wave loading on a submarine lying near a free surface. Scattered wave solution Here the scattered wave response in the acoustic medium is of interest along with that of the structure to the incident wave loading. Cavitation in the fluid is not considered in a scattered wave formulation. Similarly, the initial hydrostatic pressure in the fluid is not modeled. The zero dynamic acoustic pressure boundary condition on the free surface requires both a “soft” and a zero scattered pressure boundary condition at , and on . The incident wave loading can be only of pressure amplitude type since the reflection plane coinciding with the free surface the nodes on this free surface. The incident wave loading is applied on the fluid surface, the wet solid surface, loading includes a solid surface. A good location for the standoff node is marked as A in Figure 33.4.6–4. This node is in the fluid, close to the structure, and closer to incident wave source S than any portion of the seabed or the free surface. The standoff node’s offset from the loaded surfaces is exaggerated for emphasis in the figure. The radiation condition is specified on the acoustic surface such that the scattered wave impinging on this boundary with the infinite medium does not reflect back into the computational domain. The seabed is modeled with an incident wave reflection plane on surface . The reflection loss at this seabed surface is modeled using an impedance property. If the response of the structure in the nonlinear regime is of interest, the initial stress state in the structure should be established using Abaqus/Standard in a static analysis. The stress state in the structure is then imported into Abaqus/Explicit, and the loading on the solid surfaces causing the initial stress state is respecified in the acoustic analysis. The following template schematically shows some of the Abaqus input file options that are used to solve this problem using the scattered wave formulation: *HEADING … *SURFACE, NAME= Data lines to define the acoustic surface that is wetting the solid *SURFACE, NAME= Data lines to define the solid surface that is wetted by the fluid *SURFACE, NAME= Data lines to define the acoustic surface separating the modeled region from the infinite medium *INCIDENT WAVE INTERACTION PROPERTY, NAME=IWPROP *AMPLITUDE, DEFINITION=TABULAR, NAME=PRESSUREVTIME *TIE, NAME=COUPLING , *STEP ** For an Abaqus/Standard analysis: *DYNAMIC ** For an Abaqus/Explicit analysis: *DYNAMIC, EXPLICIT ** Load the acoustic surface *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP , source node, standoff node, reference magnitude *INCIDENT WAVE REFLECTION Data lines for the reflection plane over the seabed *INCIDENT WAVE REFLECTION Data lines for a "soft" reflection plane over the free surface ** Load the solid surface *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP , seabed_Q . , source node, standoff node, reference magnitude *INCIDENT WAVE REFLECTION Data lines for the reflection plane over the seabed *INCIDENT WAVE REFLECTION , seabed_Q Data lines for a "soft" reflection plane over the free surface *BOUNDARY ** zero pressure boundary condition on the free surface Set of nodes on the free surface *SIMPEDANCE , 8, 8, 0.0 . , *END STEP Total wave solution Here the total wave response in the acoustic medium is of interest along with that of the structure to the incident wave loading. Cavitation in the fluid may be included. Similarly, a linearly varying initial hydrostatic pressure in the fluid can be specified. The zero dynamic acoustic pressure boundary condition on the free surfaces requires only a zero pressure boundary condition at the nodes on this free surface. A reflection plane should not be included along the free surface. The incident wave loading is applied only on the fluid surface, , that separates the modeled region from the surrounding infinite acoustic medium. No incident wave should be applied directly on the structure surfaces. If the incident wave is considered planar, an acceleration-type amplitude can be used with the incident wave loading. Otherwise, a pressure-type amplitude must be used with the incident wave loading. An ideal location for the standoff node depends on the type of amplitude used for the time history of the incident wave loading. The location A shown in Figure 33.4.6–4 can be used if the incident wave loading time history is of pressure amplitude type. Otherwise, the location B that is just on the boundary and closer to the source S than any part of either the seabed or the free surface can be used. The nonreflecting impedance condition is specified on the acoustic surface, , such that the scattered part of the total wave impinging on this boundary with the infinite medium does not reflect back into the computational domain. The seabed is modeled with an incident wave reflection plane on the surface . If the response of the structure in the nonlinear regime is of interest, the initial stress state in the structure should be established using Abaqus/Standard in a static analysis. The stress state in the structure is then imported into Abaqus/Explicit, and the loading on the solid surfaces causing the initial stress state is respecified in the acoustic analysis. The following template schematically shows some of the input file options that are used to solve this problem using the total wave formulation: *HEADING … *ACOUSTIC WAVE FORMULATION, TYPE=TOTAL WAVE *MATERIAL, NAME=CAVITATING_FLUID *ACOUSTIC MEDIUM, BULK MODULUS Data lines to define the fluid bulk modulus *ACOUSTIC MEDIUM, CAVITATION LIMIT Data lines to define the fluid cavitation limit … *SURFACE, NAME= Data lines to define the acoustic surface that is wetting the solid *SURFACE, NAME= Data lines to define the solid surface that is wetted by the fluid *SURFACE, NAME= Data lines to define the acoustic surface separating the modeled region from the infinite medium *INCIDENT WAVE INTERACTION PROPERTY, NAME=IWPROP *AMPLITUDE, DEFINITION=TABULAR, NAME=PRESSUREVTIME Data lines to define the pressure-time history at the standoff point *TIE, NAME=COUPLING , *INITIAL CONDITIONS, TYPE=ACOUSTIC STATIC PRESSURE Data lines to define the initial linear hydrostatic pressure in the fluid *STEP *DYNAMIC, EXPLICIT ** Load the acoustic surface *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP , source node, standoff node, reference magnitude *INCIDENT WAVE REFLECTION Data lines for the reflection plane over the seabed *BOUNDARY ** zero pressure boundary condition on the free surface Set of nodes on the free surface *SIMPEDANCE , seabed_Q , 8, 8, 0.0 , *END STEP Example: submarine in deep water This problem is similar to the previous example of a submarine close to the free surface except for the following differences. There is no free surface in this problem; and the fluid surface, , and the fluid medium completely enclose the structure. If the structure is sufficiently deep in the water, hydrostatic pressure may be considered uniform instead of varying linearly with depth. Under this assumption, the initial stress state in the structure can be established with a uniform pressure loading all around it, if desired. In addition, if the structure is sufficiently deep in the water, the hydrostatic pressure may be significant compared to the incident wave loading; hence, the cavitation in the fluid may not be of concern. Example: surface ship Here the effect of underwater explosion loading on a surface ship is of interest . This problem is similar to the previous example of a submarine close to the free surface except for the Free surface A 01 Free surface A 02 Wet solid surface Asw Fluid surface Afw Source Seabed A sb inf model boundary Figure 33.4.6–5 Modeling of incident wave loading on a surface ship. following differences. The free surface of fluid is not continuous, and a part of the structure is exposed to the atmosphere. A soft reflection plane coinciding with the free surface is not used in this problem as in the submarine problems under the scattered wave formulation. To be able to use the scattered wave formulation in this case, the modeling technique is used in which the free surface is replaced with “structural fluid” elements. A layer of fluid at the free surface is modeled using non-acoustic elements such as membrane elements. These elements are coupled to the underlying acoustic fluid using a mesh tie constraint. The non-acoustic elements have properties similar to the fluid itself since these elements are replacing the fluid medium near the free surface and should have a thickness similar to the height of the adjacent acoustic elements. Incident wave loading with the scattered wave formulation must now be applied on these newly created surfaces as well. This technique has the added advantage of providing the deformed shape of the free surface under the loading. The following template shows some of the Abaqus input file options used for this case: *HEADING … *SURFACE, NAME=A01_structuralfluid Data lines to define the "structural fluid" surface *SURFACE, NAME=A01_acousticfluid Data lines to define the adjacent acoustic fluid surface *SURFACE, NAME=A02_structuralfluid Data lines to define the "structural fluid" surface *SURFACE, NAME=A02_acousticfluid Data lines to define the adjacent acoustic fluid surface *SURFACE, NAME=Asw_solid Data lines to define the actual solid surface that is wetted by the fluid *SURFACE, NAME=Asw_fluid Data lines to define the actual acoustic surface that is adjacent to the structure *SURFACE, NAME= Data lines to define the acoustic surface separating the modeled region from the infinite medium *INCIDENT WAVE INTERACTION PROPERTY, NAME=IWPROP *AMPLITUDE, DEFINITION=TABULAR, NAME=PRESSUREVTIME Data lines to define the pressure-time history at the standoff point *TIE, NAME=COUPLING Asw_fluid, Asw_solid A01_acousticfluid, A01_structuralfluid A02_acousticfluid, A02_structuralfluid *STEP ** For an Abaqus/Standard analysis: *DYNAMIC ** For an Abaqus/Explicit analysis: *DYNAMIC, EXPLICIT ** Load the acoustic surfaces *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP A01_acousticfluid, source point, standoff point, reference magnitude *INCIDENT WAVE REFLECTION Data lines for the reflection plane over the seabed *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP A02_acousticfluid, source point, standoff point, reference magnitude *INCIDENT WAVE REFLECTION Data lines for the reflection plane over the seabed *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP Asw_fluid, source point, standoff point, reference magnitude *INCIDENT WAVE REFLECTION Data lines for the reflection plane over the seabed ** Load the solid surfaces *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP A01_structuralfluid, source point, standoff point, reference magnitude *INCIDENT WAVE REFLECTION Data lines for the reflection plane over the seabed *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=PRESSUREVTIME, , seabed_Q , seabed_Q , seabed_Q , seabed_Q PROPERTY=IWPROP A02_structuralfluid, source point, standoff point, reference magnitude *INCIDENT WAVE REFLECTION Data lines for the reflection plane over the seabed *INCIDENT WAVE INTERACTION, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP Asw_solid, source point, standoff point, reference magnitude *INCIDENT WAVE REFLECTION Data lines for the reflection plane over the seabed *SIMPEDANCE , seabed_Q , seabed_Q , *END STEP Compared to the total wave formulation analysis of a submarine close to the free surface, the following differences are noteworthy. As shown in Figure 33.4.6–5, the free surface with zero dynamic pressure boundary condition is now split into two parts: . The fluid surface wetting the ship ( ), which are tied together, do not encircle the whole structure. Besides these differences, the modeling considerations for the surface ship problem are similar to the total wave analysis of the submarine near the free surface. ) and the wetted ship surface ( and Example: airblast loading on a structure Here the effect of airblast (explosion in the air) loading on a structure is of interest . Since the stiffness and inertia of the air medium are negligible, the acoustic medium is not modeled. Rather the incident wave loading is applied directly on the structure itself. The solid surface where the incident wave loading is applied is shown in Figure 33.4.6–6. Since the acoustic medium is not modeled, the total wave and the scattered wave formulations are identical. Example: fluid cavitation without incident wave loading You may be interested in modeling acoustic problems in Abaqus/Explicit where the loading is applied through either prescribed pressure boundaries or specified pressure-conjugate concentrated loads. Choice of the scattered or the total wave formulation is not relevant in these problems even when the acoustic medium is capable of cavitation. Outer solid surface A sw Source Standoff point Figure 33.4.6–6 Modeling of airblast loading on a structure. 33.4.7 PORE FLUID FLOW Products: Abaqus/Standard Abaqus/CAE References • “Applying loads: overview,” Section 33.4.1 • *CFLOW • *DFLOW • *DSFLOW • *FLOW • *SFLOW • “Defining a surface pore fluid flow,” Section 16.9.22 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a concentrated pore fluid flow,” Section 16.9.21 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Pore fluid flow can be prescribed in coupled pore fluid diffusion/stress analysis and in the geostatic stress field procedure . Pore fluid flow can be prescribed by: • defining seepage coefficients and sink pore pressures on element faces or surfaces; • defining drainage-only seepage coefficients on element faces or surfaces that are applied only when surface pore pressures are positive; or • prescribing an outward normal flow velocity directly at nodes, on element faces, or on surfaces. Defining pore fluid flow as a function of the current pore pressure in consolidation analysis In consolidation analysis you can provide seepage coefficients and sink pore pressures on element faces or surfaces to control normal pore fluid flow from the interior of the region modeled to the exterior of the region. The surface condition assumes that the pore fluid flows in proportion to the difference between the current pore pressure on the surface, , and some reference value of pore pressure, : where is the component of the pore fluid velocity in the direction of the outward normal to the surface; is the seepage coefficient; is the current pore pressure at this point on the surface; and is a reference pore pressure value. Specifying element-based pore fluid flow To define element-based pore fluid flow, specify the element or element set name; the distributed load type; the reference pore pressure, . The face of the elements upon which the normal flow is enforced is identified by a seepage distributed load type. The seepage types available depend on the element type . ; and the reference seepage coefficient, Input File Usage: *FLOW element number or element set name, Qn, , Abaqus/CAE Usage: Pore fluid flow cannot be defined as a function of the current pore pressure in Abaqus/CAE. Specifying surface-based pore fluid flow To define surface-based pore fluid flow, specify a surface name, the seepage flow type, the reference pore pressure, and the reference seepage coefficient. The element-based surface contains the element and face information. Input File Usage: *SFLOW surface name, Q, , Abaqus/CAE Usage: Pore fluid flow cannot be defined as a function of the current pore pressure in Abaqus/CAE. Defining drainage-only flow Drainage-only flow types can be specified for element-based or surface-based pore fluid flow to indicate that normal pore fluid flow occurs only from the interior to the exterior region of the model. The drainage- only flow surface condition assumes that the pore fluid flows in proportion to the magnitude of the current pore pressure on the surface, , when that pressure is positive: where is the component of the pore fluid velocity in the direction of the outward normal to the surface; is the seepage coefficient; and is the current pore pressure at this point on the surface. Figure 33.4.7–1 illustrates this pore pressure–velocity relationship. This surface condition is designed for use with the total pore pressure formulation , mainly for cases where the phreatic surface intersects an exterior surface that is free to drain. See “Calculation of phreatic surface in an earth dam,” Section 10.1.2 of the Abaqus Example Problems Manual, for an example of this type of calculation. , ks pore pressure, uw Figure 33.4.7–1 Drainage-only pore pressure–velocity relationship. When surface pore pressures are negative, the constraint will properly enforce the condition that no fluid can enter the interior region. When surface pore pressures are positive, the constraint will permit fluid flow from the interior to the exterior region of the model. When the seepage coefficient value, , is large, this flow will approximately enforce the requirement that the pore pressure should be zero on a freely draining surface. To achieve this condition, it is necessary to choose the value of to be much larger than a characteristic seepage coefficient for the material in the underlying elements: where is the permeability of the underlying material; is the fluid specific weight; and is a characteristic length of the underlying elements. Values of could result in poor conditioning of the model. In all cases the freely draining flow type represents discontinuously nonlinear behavior, and its use may require appropriate solution controls . will be adequate for most analyses. Larger values of Input File Usage: Use the following option to define element-based drainage-only flow: *FLOW element number or element set name, QnD, Use the following option to define surface-based drainage-only flow: *SFLOW surface name, QD, Abaqus/CAE Usage: Pore fluid flow cannot be defined as a function of the current pore pressure in Abaqus/CAE. Modifying or removing seepage coefficients and reference pore pressures Seepage coefficients and reference pore pressures can be added, modified, or removed as described in “Applying loads: overview,” Section 33.4.1. Specifying a time-dependent reference pore pressure , can be controlled by referring to an amplitude curve. The magnitude of the reference pore pressure, If different variations are needed for different portions of the flow, repeat the flow definition with each referring to its own amplitude curve. See “Applying loads: overview,” Section 33.4.1, and “Amplitude curves,” Section 33.1.2, for details. Defining nonuniform flow in a user subroutine To define nonuniform flow, the variation of the reference pore pressure and the seepage coefficient as functions of position, time, pore pressure, etc. can be defined in user subroutine FLOW. Input File Usage: Use the following option to define a nonuniform element-based flow: *FLOW element number or element set name, QnNU Use the following option to define a nonuniform surface-based flow: Abaqus/CAE Usage: *SFLOW surface name, QNU User subroutine FLOW is not supported in Abaqus/CAE. Prescribing seepage flow velocity and seepage flow directly in consolidation analysis You can directly prescribe an outward normal flow velocity, flow at a node in consolidation analysis. , across a surface or an outward normal Prescribing element-based seepage flow velocity To prescribe an element-based seepage flow velocity, specify the element or element set name, the seepage type, and the outward normal flow velocity. The face of the element for which the seepage flow is being defined is identified by the seepage type. The seepage types available depend on the element type . Input File Usage: *DFLOW element number or element set name, Sn, Abaqus/CAE Usage: Load module: Create Load: choose Fluid for the Category and Surface pore fluid for the Types for Selected Step: select region: Distribution: select an analytical field, Magnitude: Prescribing surface-based seepage flow velocity To prescribe a surface-based seepage flow velocity, specify a surface name, the seepage flow type, and the pore fluid velocity. The element-based surface contains the element and face information. Input File Usage: *DSFLOW surface name, S, Abaqus/CAE Usage: Load module: Create Load: choose Fluid for the Category and Surface pore fluid for the Types for Selected Step: select region: Distribution: Uniform, Magnitude: Prescribing node-based seepage flow To prescribe node-based seepage flow, specify the node or node set name and the magnitude of the flow per unit time. Input File Usage: *CFLOW node number or node set name, , magnitude Abaqus/CAE Usage: Load module: Create Load: choose Fluid for the Category and Concentrated pore fluid for the Types for Selected Step: select region: Magnitude: magnitude Modifying or removing seepage flow velocities and seepage flow Seepage flow velocities can be added, modified, or removed as described in “Applying loads: overview,” Section 33.4.1. Specifying time-dependent flow velocity and flow The magnitude of the seepage velocity, , can be controlled by referring to an amplitude curve. To specify different variations for different flows, repeat the seepage flow velocity or seepage flow definition with each referring to its own amplitude curve. See “Applying loads: overview,” Section 33.4.1, and “Amplitude curves,” Section 33.1.2, for details. Defining nonuniform flow velocities in a user subroutine To define nonuniform element-based or surface-based flow, the variation of the seepage magnitude as a function of position, time, pore pressure, etc. can be defined in user subroutine DFLOW. If the optional , is specified directly, this value is passed into user subroutine DFLOW in the variable seepage velocity, used to define the seepage magnitude. Input File Usage: Use the following option to define nonuniform element-based flow: *DFLOW element number or element set name, SnNU, Use the following option to define nonuniform surface-based flow: *DSFLOW surface name, SNU, Abaqus/CAE Usage: Use the following input to define nonuniform surface-based flow: Load module: Create Load: choose Fluid for the Category and Surface pore fluid for the Types for Selected Step: select region: Distribution: User-defined, Magnitude: Nonuniform element-based flow is not supported in Abaqus/CAE. 33.5 Prescribed assembly loads • “Prescribed assembly loads,” Section 33.5.1 33.5.1 PRESCRIBED ASSEMBLY LOADS Products: Abaqus/Standard Abaqus/CAE References • “Prescribed conditions: overview,” Section 33.1.1 • *BOUNDARY • *CLOAD • *PRE-TENSION SECTION • *SURFACE • Chapter 22, “Bolt loads,” of the Abaqus/CAE User’s Manual Overview Assembly loads: • can be used to simulate the loading of fasteners in a structure; • are applied across user-defined pre-tension sections; • are applied to pre-tension nodes that are associated with the pre-tension sections; and • require the specification of pre-tension loads or tightening adjustments. Concept of an assembly load Figure 33.5.1–1 is a simple example that illustrates the concept of an assembly load. pre-tension section gasket (cid:0)(cid:0)(cid:0)(cid:0)(cid:0) (cid:0)(cid:0)(cid:0)(cid:0)(cid:0) bolt Figure 33.5.1–1 Example of assembly load. Container A is sealed by pre-tensioning the bolts that hold the lid, which places the gasket under pressure. This pre-tensioning is simulated in Abaqus/Standard by adding a “cutting surface,” or pre-tension section, in the bolt, as shown in Figure 33.5.1–1, and subjecting it to a tensile load. By modifying the elements on one side of the surface, Abaqus/Standard can automatically adjust the length of the bolt at the pre-tension section to achieve the prescribed amount of pre-tension. In later steps further length changes can be prevented so that the bolt acts as a standard, deformable component responding to other loadings on the assembly. Modeling an assembly load Abaqus/Standard allows you to prescribe assembly loads across fasteners that are modeled by continuum, truss, or beam elements. The steps needed to model an assembly load vary slightly depending on the type of elements used to model the fasteners. Modeling a fastener with continuum elements In continuum elements the pre-tension section is defined as a surface inside the fastener that “cuts” it into two parts . The pre-tension section can be a group of surfaces for cases where a fastener is composed of several segments. pre-tension section elements chosen by user to describe the pre-tension section Figure 33.5.1–2 Pre-tension section defined using continuum elements. The element-based surface contains the element and face information . You must convert the surface into a pre-tension section across which pre- tension loads can be applied and assign a controlling node to the pre-tension section. Input File Usage: Abaqus/CAE Usage: Use the following options to model an assembly load across a fastener that is modeled with continuum elements: *SURFACE, TYPE=ELEMENT, NAME=surface_name *PRE-TENSION SECTION, SURFACE=surface_name, NODE=n Load module: Create Load: choose Mechanical for the Category and Bolt load for the Types for Selected Step Assigning a controlling node to the pre-tension section The assembly load is transmitted across the pre-tension section by means of the pre-tension node. The pre-tension node should not be attached to any element in the model. It has only one degree of freedom (degree of freedom 1), which represents the relative displacement at the two sides of the cut in the direction of the normal . The coordinates of this node are not important. pre-tension section pre-tension node Figure 33.5.1–3 Normal to the pre-tension section; this normal should face away from the underlying elements. Defining the normal to the pre-tension section Abaqus/Standard computes an average normal to the section—in the positive surface direction, facing away from the continuum elements used to generate the surface—to determine the direction along which the pre-tension is applied. You may also specify the normal directly (when the desired direction of loading is different from the average normal to the pre-tension section). The normal is not updated when performing large-displacement analysis. Recognizing elements on either side of the pre-tension section For all the elements that are connected to the pre-tension section by at least one node, Abaqus/Standard must determine on which side of the pre-tension section each element is located. This process is crucial for the prescribed assembly load to work properly. The elements used to define the section are referred to as “base elements” in this discussion. All elements on the same side of the section as the base elements are referred to as the “underlying elements.” All elements connected to the section that share faces (or in two-dimensional problems, edges) with the base elements are added to the list of underlying elements. This is a repetitive process that enables Abaqus/Standard to find the underlying elements in almost all meshes—triangles; wedges; tetrahedra; and embedded beams, trusses, shells, and membranes—that were not used in the definition of the surface . embedded beam element pre-tension section region 1{ region 2 base elements underlying elements that share facets with the base elements Figure 33.5.1–4 The base elements are used to find the underlying elements. In most cases this process will group all of the elements that are connected to the section into two regions, as shown in the figure. In rare instances this process may group the elements in more than two regions, in particular if line elements cross over element boundaries. An example is shown in Figure 33.5.1–5; it has three regions, where region 1 is the underlying region. For each region other than region 1 an additional step is necessary to determine on which side of the section the region is located. Abaqus/Standard computes an average normal, , for all the nodes of the region that belong to the section; it also computes an average position ( ) of all these nodes. In addition, it computes an average position ( and ) of the remaining nodes of the region. If the dot product between the normal the vector is negative, the region is assumed to be an underlying region and is added to region 1. This additional step is illustrated in Figure 33.5.1–5 for regions 2 and 3. This additional step produces an incorrect separation for the beam element shown in Figure 33.5.1–6 since the beam is not found to be an underlying element. If the pre-tension section has an odd shape and one or more line elements that cross over element boundaries are connected to it, consult the list of the underlying elements given in the data (.dat) file to make sure that the underlying elements are listed correctly. pre-tension section region 1 region 2 beam element (region 3) position of A, B, and n for region 2 position of A, B, and n for region 3 Figure 33.5.1–5 An additional underlying element is found. pre-tension section beam element region 1 Figure 33.5.1–6 An additional underlying element is not found. Elements that are connected only to the nodes on the pre-tension section, including single-node elements (such as SPRING1, DASHPOT1, and MASS elements) are not included as underlying elements: they are considered to be attached to the other side of the section. Modeling a fastener with truss or beam elements When a pre-tensioned component is modeled with truss or beam elements, the pre-tension section is reduced to a point. The section is assumed to be located at the last node of the element as defined by the element connectivity , with its normal along the element directed from the first to the last node. As a result, the section is defined entirely by just specifying the element to which an assembly load must be prescribed and associating it with a pre-tension node. Input File Usage: Use the following option to model an assembly load across fasteners modeled with beam or truss elements: Abaqus/CAE Usage: *PRE-TENSION SECTION, ELEMENT=element_number, NODE=n Load module: Create Load: choose Mechanical for the Category and Bolt load for the Types for Selected Step As in the case of a surface-based pre-tension section, the node has only one degree of freedom (degree of freedom 1), which represents the relative displacement on the two sides of the cut in the direction of the normal . The coordinates of the node are not important. pre-tension node pre-tension section beam or truss element Figure 33.5.1–7 Pre-tension section defined using a truss or beam element. Defining the normal to the pre-tension section Abaqus/Standard computes the normal as the vector from the first to the last node in the connectivity of the underlying element. Alternatively, you can specify the normal to the section directly. This normal is not updated during large-displacement analysis. Defining multiple pre-tension sections You can define multiple pre-tension sections by repeating the pre-tension section definition input. Each pre-tension section should have its own pre-tension node. Use with nodal transformations A local coordinate system cannot be used at a pre-tension node. It can be used at nodes located on pre-tension sections. Applying the prescribed assembly load The pre-tension load is transmitted across the pre-tension section by means of the pre-tension node. Prescribing the pre-tension force You can apply a concentrated load to the pre-tension node. This load is the self-equilibrating force carried across the pre-tension section, acting in the direction of the normal on the part of the fastener underlying the pre-tension section (the part that contains the elements that were used in the definition of the pre- tension section; see Figure 33.5.1–8). Input File Usage: Abaqus/CAE Usage: *CLOAD Load module: Create Load: choose Mechanical for the Category and Bolt load for the Types for Selected Step: select surface and if, necessary, datum axis: Method: Apply force pre-tension node underlying part Figure 33.5.1–8 The prescribed assembly load is given at the pre-tension node and applied in direction . Prescribing a tightening adjustment You can prescribe a tightening adjustment of the pre-tension section by using a nonzero boundary condition at the pre-tension node (which corresponds to a prescribed change in the length of the component cut by the pre-tension section in the direction of the normal). Input File Usage: Abaqus/CAE Usage: *BOUNDARY Load module: Create Load: choose Mechanical for the Category and Bolt load for the Types for Selected Step: select surface and if, necessary, datum axis: Method: Adjust length Controlling the pre-tension node during the analysis You can maintain the initial adjustment of the pre-tension section by using a boundary condition fixing the degrees of freedom at their current values at the start of the step once an initial pre-tension is applied in the fastener; this technique enables the load across the pre-tension section to change according to the externally applied loads to maintain equilibrium. If the initial adjustment of a section is not maintained, the force in the fastener will remain constant. When a pre-tension node is not controlled by a boundary condition, make sure that the components of the structure are kinematically constrained; otherwise, the structure could fall apart due to the presence of rigid body modes. Abaqus/Standard will issue a warning message if it does not find any boundary condition or load on a pre-tension node during the first step of the analysis. Display of results Abaqus/Standard automatically adjusts the length of the component at the pre-tension section to achieve the prescribed amount of pre-tension. This adjustment is done by moving the nodes of the underlying elements that lie on the pre-tension section relative to the same nodes when they appear in the other elements connected to the pre-tension section. As a result, the underlying elements will appear shrunk, even though they carry tensile stresses when a pre-tension is applied. Limitations when using assembly loads Assembly loads are subject to the following limitations: • An assembly load cannot be specified within a substructure. • If a submodeling analysis is performed (“Submodeling: overview,” Section 10.2.1), any pre-tension section should not cross regions where driven nodes are specified. In other words, a pre-tension section should appear either entirely in the region of the global model that is not part of a submodel or entirely in the region of the global model that is part of a submodel. In the latter case, a pre-tension section must also appear in the submodel when the submodel analysis is performed. • Nodes of a pre-tension section should not be connected to other parts of the body through multi-point constraints (“General multi-point constraints,” Section 34.2.2). These nodes can be connected to other parts of the body through equations (“Linear constraint equations,” Section 34.2.1). However, an equation connecting a node on the pre-tension section to a node located on the underlying side of the section introduces a constraint that spans across the pre-tension cut and, therefore, interacts directly with the application of the pre-tension load. On the other hand, an equation connecting a node on the pre-tension section to a node on the other side of the section does not influence the application of the pre-tension load. Procedures Any of the Abaqus/Standard procedures that use element types with displacement degrees of freedom can be used. Static analysis is the most likely procedure type to be used when prescribing the initial pre-tension (“Static stress analysis,” Section 6.2.2). Other analysis types such as coupled temperature-displacement (“Sequentially coupled thermal-stress analysis,” Section 16.1.2) or coupled thermal-electrical-structural (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4) can also be used. Once the initial pre-tension is applied, a static or dynamic analysis (“Dynamic analysis procedures: overview,” Section 6.3.1) may, for instance, be used to apply additional loads while maintaining the tightening adjustment. Output The total force across the pre-tension section is the sum of the reaction force at the pre-tension node plus any concentrated load specified at that node. The total force across the pre-tension section is available as output using the output variable identifier TF . The forces are along the normal direction. The shear force across the pre-tension section is not available for output. The tightening adjustment of the pre-tension section is available as the displacement of the pre- tension node. The output of displacement is requested using output identifier U. Only the adjustment normal to the pre-tension section is output since there is no adjustment in any other direction. The stress distribution across the pre-tension section is not available directly; however, the stresses in the underlying elements can be displayed readily. Alternatively, a tied contact pair can be inserted at the location of the pre-tension section to enable stress distribution output by means of output identifiers CPRESS and CSHEAR. See “Defining tied contact in Abaqus/Standard,” Section 35.3.7, for details on defining tied contact. Input file template *HEADING Prescribed assembly load; example using continuum elements … *NODE Optionally define the pre-tension node *SURFACE, NAME=name Data lines that specify the elements and their associated faces to define the pre-tension section *PRE-TENSION SECTION, SURFACE=name, NODE=pre-tension_node ** *STEP ** Application of the pre-tension across the section *STATIC Data line to control time incrementation *CLOAD pre-tension_node, 1, pre-tension_value or *BOUNDARY,AMPLITUDE=amplitude pre-tension_node, 1, 1, tightening adjustment *END STEP *STEP ** maintain the tightening adjustment and apply new loads *STATIC or *DYNAMIC Data line to control time incrementation *BOUNDARY,FIXED pre-tension_node, 1, 1 *BOUNDARY Data lines to prescribe other boundary conditions *CLOAD or *DLOAD Data lines to prescribe other loading conditions … *END STEP 33.6 Predefined fields • “Predefined fields,” Section 33.6.1 33.6.1 PREDEFINED FIELDS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Prescribed conditions: overview,” Section 33.1.1 • *TEMPERATURE • *FIELD • *PRESSURE STRESS • *MASS FLOW RATE • “Defining a temperature field,” Section 16.11.9 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview This section describes how to specify the values of the following types of predefined fields during an analysis: • temperature, • field variables, • equivalent pressure stress, and • mass flow rate. The procedures in which these fields can be used are outlined in “Prescribed conditions: overview,” Section 33.1.1. Temperature, field variables, equivalent pressure stress, and mass flow rate are time-dependent, predefined (not solution-dependent) fields that exist over the spatial domain of the model. They can be defined: • by entering the data directly, • by reading an Abaqus results file generated during a previous analysis (usually an Abaqus/Standard heat transfer analysis), or • in an Abaqus/Standard user subroutine. Temperature can also be defined by reading an Abaqus output database file generated during a previous analysis. In Abaqus/Standard field variables can also be defined by reading an Abaqus output database file generated during a previous analysis. Field variables can also be made solution dependent, which allows you to introduce additional nonlinearities in the Abaqus material models. Predefined temperature In stress/displacement analysis the temperature difference between a predefined temperature field and any initial temperatures (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) will create thermal strains if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The predefined temperature field also affects temperature-dependent material properties, if any. In Abaqus/Explicit temperature-dependent material properties may cause longer run times than constant properties. You define the magnitude and time variation of temperature at the nodes, and Abaqus interpolates the temperatures to the material points. Input File Usage: Use the following option to specify a predefined temperature field: Abaqus/CAE Usage: *TEMPERATURE Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step Restrictions Do not specify predefined temperature fields in a pure heat transfer analysis, a coupled thermal-electrical analysis, a fully coupled temperature-displacement analysis, or a fully coupled thermal-electrical- structural analysis; instead, specify a boundary condition (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) to prescribe temperature degrees of freedom (11, 12, ...). Predefined temperature fields cannot be specified in an adiabatic analysis step or in any mode-based dynamic analysis step. To specify a predefined temperature field in a restart analysis, the corresponding predefined field must have been specified in the original analysis as either initial temperatures or a predefined temperature field. Predefined field variables The usage and treatment of predefined field variables is exactly analogous to that of temperature. You can prescribe the magnitude and time variation of the field at all of the nodes of the model, and Abaqus will interpolate the values to the material points. When prescribing field variable values, you must specify the field variable number being defined; the default is field variable number 1. Field variables must be numbered consecutively starting from one. Repeat the field variable definition to define more than one field variable. The field variable can be a real field (such as an electromagnetic field) generated by a previous simulation (Abaqus or another analysis code). It can also be an artificial field that you define to modify certain material properties during the course of an analysis. For example, suppose that you wish to vary Young’s modulus linearly between 30 × 106 and 35 × 106 during the response. The linear elastic material definition shown in Table 33.6.1–1 could be used. Table 33.6.1–1 Sample material definition. Number of field variable dependencies: 1 Young’s modulus 30.E6 35.E6 Poisson’s ratio Value of field variable 1 0.3 0.3 1.0 2.0 Define an initial condition to specify the initial value of field variable 1 as 1.0 for a node set. Then, define a predefined field variable in the analysis step to specify the value of field variable 1 as 2.0 for the node set. Young’s modulus will vary smoothly over the course of the step as the field variable’s value is ramped from 1.0 to 2.0 at all nodes in the node set. Field variables can also be used to vary real properties in space by making the properties depend on field variables, as above, and by assigning different field variable values to different nodes. Making properties depend on field variables will increase the computer time required, since Abaqus must perform the necessary table look-ups. In an Abaqus/Standard stress/displacement analysis the difference between a predefined field variable and its initial value (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) will create volumetric strains analogous to thermal strains if a field expansion coefficient (for the corresponding field variable) is given for the material (“Thermal expansion,” Section 26.1.2). Input File Usage: Use the following option to specify a predefined field variable: Abaqus/CAE Usage: *FIELD, VARIABLE=n Predefined field variables are not supported in Abaqus/CAE. Restrictions To specify a predefined field variable in a restart analysis, the corresponding predefined field must have been specified in the original analysis as either an initial field variable value or a predefined field variable. Predefined pressure stress You can apply equivalent pressure stress as a predefined field in a mass diffusion analysis. The usage and treatment of pressure stresses is analogous to that of temperatures and field variables. In Abaqus equivalent pressure stresses are positive when they are compressive. Input File Usage: Use the following option to specify a predefined equivalent pressure stress field: Abaqus/CAE Usage: *PRESSURE STRESS Predefined equivalent pressure stress is not supported in Abaqus/CAE. Restrictions Predefined equivalent pressure stress fields can be specified only in a mass diffusion procedure . To specify a predefined equivalent pressure stress field in a restart analysis, the corresponding predefined field must have been specified in the original analysis as either initial pressure stresses or a predefined equivalent pressure stress field. Predefined mass flow rate You can specify the mass flow rate per unit area (or through the entire section for one-dimensional elements) for forced convection/diffusion elements in a heat transfer analysis. The usage and treatment of mass flow rate is analogous to that of temperatures and field variables. Input File Usage: Abaqus/CAE Usage: Use the following option to specify a predefined mass flow rate field: *MASS FLOW RATE Predefined mass flow rate is not supported in Abaqus/CAE. Restrictions A predefined mass flow rate field can be specified only with forced convection/diffusion elements in a heat transfer procedure . To specify a predefined mass flow rate field in a restart analysis, the corresponding predefined field must have been specified in the original analysis by using either initial mass flow rates or a predefined mass flow rate field. Reading initial values of a field from a user-specified results file An Abaqus/Standard results file can be used to specify initial values of • temperature ; • field variables ; and • pressure stress . Field variable values must be read from the temperature record . The part (.prt) file from the original analysis is also required when reading data from the results file. If the zero increment results were requested as output to the Abaqus/Standard results file , you can define initial values of prescribed fields as those existing at the beginning of a step (the zero increment) in the previous heat transfer analysis (field variables and temperatures) or stress/displacement analysis (pressure stress). The .fil file extension is optional. Reading initial values of a temperature field from a user-specified output database file An Abaqus/Standard output database file can be used to specify initial values of temperature . The part (.prt) file from the original analysis is also required when reading data from the output database file. Temperature values can be read between dissimilar meshes, as described in “Interpolating initial temperatures for dissimilar meshes from a user-specified results or output database file” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. Initializing predefined field variables from a user-specified output database file in Abaqus/Standard In Abaqus/Standard nodal values of temperature (NT), normalized concentrations (NNC), and electric potential (EPOT) can be used to initialize predefined fields . The part (.prt) file from the original analysis is also required when reading data from the output database file. The scalar nodal values can be mapped between dissimilar meshes, as described in “Defining initial predefined field variables by interpolating scalar nodal output variables for dissimilar meshes from a user-specified output database file” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. Defining time-dependent fields The prescribed magnitude of a field can vary with time during a step according to an amplitude function. See “Prescribed conditions: overview,” Section 33.1.1, and “Amplitude curves,” Section 33.1.2, for details. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *TEMPERATURE, AMPLITUDE=amplitude_name *FIELD, AMPLITUDE=amplitude_name *PRESSURE STRESS, AMPLITUDE=amplitude_name *MASS FLOW RATE, AMPLITUDE=amplitude_name In Abaqus/CAE only predefined temperature fields are available. Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: Direct specification or select an analytical field or a discrete field, Amplitude: amplitude_name Field propagation By default, all fields defined in the previous general analysis step remain unchanged in the subsequent general step or in subsequent consecutive linear perturbation steps. Fields do not propagate between linear perturbation steps. You define the fields in effect for a given step relative to the preexisting fields. At each new step the existing fields can be modified and additional fields can be specified. If you specify additional values for a field, the definition of the field will be extended to those nodes where it was previously undefined. Alternatively, you can release all previously applied fields of a given type in a step and specify new ones. In this case any fields of that type that are to be retained must be respecified. Modifying fields By default, when you modify existing temperatures, field variables, pressure stresses, or mass flow rates, all existing values of the field remain. Input File Usage: Use one of the following options to modify an existing field or to specify an additional field: *TEMPERATURE, OP=MOD *FIELD, OP=MOD *PRESSURE STRESS, OP=MOD *MASS FLOW RATE, OP=MOD In Abaqus/CAE only predefined temperature fields are available. Load module: Create Predefined Field or Predefined Field Manager: Edit Abaqus/CAE Usage: Removing fields A field that is removed is reset to the value given as an initial condition or to zero if no initial condition was defined. When fields are reset to their initial conditions, the amplitude referred to in the field definition does not apply. In Abaqus/Standard the amplitude variation defined for the step governs the behavior; in most Abaqus/Standard procedures the default is to ramp the fields back to their initial conditions . In Abaqus/Explicit the values are always ramped linearly over the step back to their initial conditions. If the temperatures, field variables, pressure stresses, or mass flow rates are reset to a new value (not to their initial conditions), the amplitude referred to in the field definition applies. If you choose to remove any field in a step, no fields of that type will be propagated from the previous general step. All fields of the same type that are in effect during this step must be respecified. Input File Usage: Use one of the following options to release all previously applied fields of a particular type and to specify new fields: *TEMPERATURE, OP=NEW *FIELD, OP=NEW *PRESSURE STRESS, OP=NEW *MASS FLOW RATE, OP=NEW If the OP=NEW parameter is used on any field option in a step, it must be used on all field options of the same type within the step. Abaqus/CAE Usage: Use the following option to reset a temperature field to the value prescribed in the initial step (or to zero if no initial value was defined): Load module: temperature field editor: Reset to initial Reading the values of a field directly from an alternate input file The data for predefined temperature, field variables, pressure stress, or mass flow rate can be contained in a separate input file . Input File Usage: Use one of the following options: *TEMPERATURE, INPUT=file_name *FIELD, INPUT=file_name *PRESSURE STRESS, INPUT=file_name *MASS FLOW RATE, INPUT=file_name If the INPUT parameter is omitted, it is assumed that the data lines follow the keyword line. Abaqus/CAE Usage: You cannot read field data from a separate input file in Abaqus/CAE. Reading the values of a field from a user-specified file Nodal temperatures calculated during an Abaqus/Standard heat transfer or coupled thermal-electrical analysis can be used to define temperatures in a subsequent analysis. The temperatures must have been written to the results or output database file. If nodal temperatures are written to the results file during an Abaqus/Standard heat transfer or coupled thermal-electrical analysis, they can be used to define field variables in a subsequent analysis. In Abaqus/Standard if nodal values of temperature (NT), normalized concentrations (NNC), or electric potential (EPOT) are written to the output database file, they can be used to define field variables in a subsequent Abaqus/Standard analysis. In Abaqus/Standard equivalent pressure stresses calculated during a mechanical analysis can be used in a subsequent mass diffusion analysis if the element output variable SINV was written to the results file averaged at the nodes . Once the data are available in a results file or output database file, they can be read into a subsequent analysis as a predefined field. Data for field variables and pressure stress can be read from a previously generated results file. In Abaqus/Standard data can also be read from a previously generated output database file. Data for temperatures can be read from a previously generated results or output database file. Data for temperatures (and field variables in Abaqus/Standard) to be interpolated between dissimilar meshes can be read only from the output database file. The part (.prt) file from the original analysis is also required when reading data from the results or output database file. When the output file of an Abaqus analysis involving beam and/or shell elements is used to define temperatures, you must ensure that the number of temperature points through the section defined for corresponding elements is consistent between the two analyses. Inconsistent temperature point definition will result in an incorrect transfer of prescribed field quantities. Reading field values from a user-specified results file To read field values from a user-specified results file, the data must have been written to the results file as nodal output . Only nodal quantities can be read from the results file. Since field variables can be written to the results file only as element quantities (record key 9), they cannot be read directly into a subsequent analysis. In this case you must generate a results file with the field data in the temperature record, even if the field variable in the current analysis is the same as a field variable in the previous analysis. Multiple results files must be generated for multiple field variables. To generate the results file, you can write a program to create a results file (without running an Abaqus analysis) according to the format described in Chapter 5, “File Output Format.” Examples of such programs are shown in that chapter. If the values will be read in as temperatures or field variables, the data must be written as nodal quantities with record key 201. If the values will be read in as a pressure stress field, the data must be averaged at the nodes (as explained in “Output to the data and results files,” Section 4.1.2) and written as record key 12. Specifying the results file to be read You must specify the name of the results file from which the data are to be read for a temperature, field variable, or pressure stress. The .fil file extension is optional. If both .fil and .odb files exist for a temperature field and no extension is specified, the results file will be used. Input File Usage: Abaqus/CAE Usage: *TEMPERATURE, FILE=file *FIELD, FILE=file *PRESSURE STRESS, FILE=file In Abaqus/CAE only predefined temperature fields are available. Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file Creating a cyclic temperature history In a direct cyclic analysis in Abaqus/Standard the temperature values must be cyclic over the step: the start value must be equal to the end value. To create a cyclic temperature history from a prior heat transfer analysis that is not cyclic, you can set the starting time, f (measured relative to the total step time period, ), after which the temperatures read from the results file will be ramped back to their initial condition , the temperature value is equal to values. At any time point where obtained from the results file at time t, as illustrated in Figure 33.6.1–1. is the initial condition value, and , is the interpolated value Input File Usage: Use the following option to set the starting time for a cyclic temperature history: Abaqus/CAE Usage: *TEMPERATURE, FILE=file, BTRAMP=f Cyclic temperature histories are not supported in Abaqus/CAE. Temp ini Temp ft Figure 33.6.1–1 Ramp temperatures to their initial condition values after to create a cyclic temperature history. Reading temperature values from a user-specified output database file To read temperature values from a user-specified output database file, the temperatures must have been written to the output database file as nodal output . Specifying the output database file to be read for a temperature field You must specify the name of the output database file from which the data are to be read for a temperature field. The .odb extension must be included if both results and output database files exist. Only the data for the part instances that are common to both the analyses will be transferred. If the part instance names differ, you must activate the general interpolation capability. Input File Usage: Abaqus/CAE Usage: *TEMPERATURE, FILE=file Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file Defining fields using nodal scalar output values from a user-specified output database file In Abaqus/Standard if nodal values of temperature (NT), normalized concentrations (NNC), or electric potential (EPOT) are written to the output database file, they can be used to define field variables in a subsequent Abaqus/Standard analysis. To read these values from a user-specified output database file, they must have been written to the output database file as nodal output . Specifying the output database file to be read for a field variable You must specify the name of the output database file from which the data are to be read for a field variable. The .odb extension must be included if both results and output database files exist. Input File Usage: Abaqus/CAE Usage: *FIELD, FILE=file, OUTPUT VARIABLE=scalar nodal output variable, Predefined field variables are not supported in Abaqus/CAE. Interpolating data between meshes Data can be mapped between the same meshes, between meshes that differ only in the element order (first-order element in heat transfer analysis and second-order element in thermal-stress analysis), or between dissimilar meshes of matching element dimensionality (solid element to solid element or shell element to shell element). If data are mapped between the same meshes, no additional computations are required. To transfer data between meshes that differ only in the element order, you must activate the midside node capability. To map data between dissimilar meshes, you must activate the general interpolation capability. The midside node capability is available only for temperatures. The midside node capability and the general interpolation capability are mutually exclusive. Using second-order stress elements with first-order heat transfer elements (the midside node capability) In some cases it makes sense to perform an Abaqus/Standard heat transfer analysis using first-order elements followed by a thermal-stress analysis using second-order elements (and an otherwise similar mesh). For example, a heat transfer analysis including latent heat effects—for which first-order elements are best suited—can be followed by a stress analysis using second-order elements, which generally have superior deformation characteristics. In addition, the first-order temperature field calculated in the heat transfer analysis is consistent with the first-order thermal strain field provided by the second-order stress/displacement elements. For the instances in which there is a change in the order of interpolation of element temperature variables between the heat transfer analysis and the stress analysis, temperatures must be assigned to the midside nodes of the stress/displacement elements based on the temperatures of the corner nodes of the heat transfer elements. If you specify that the midside node temperatures are needed, Abaqus will interpolate the temperatures of the midside nodes of the second-order stress/displacement elements from the corner nodes using first-order interpolation. If the midside node capability is activated in cases where both the heat transfer analysis and the stress analysis are performed with second-order elements, it is ignored. One exception is that if variable-node second-order stress/displacement elements are used in the stress analysis, activating the midside node capability will cause Abaqus to interpolate the temperatures of the midface nodes in the variable node elements from the corner or midside nodes using first-order interpolation. Since it is assumed that the corner node temperatures have been generated in a previous heat transfer analysis, the midside node capability can be used only when the temperature field values are read from a user-specified results or output database file. You must ensure that the nodal temperatures calculated during the heat transfer analysis are written to the results or output database file. Once the temperatures of the corner nodes are read in the subsequent stress/displacement analysis, Abaqus interpolates the midside node temperatures so that all nodes have temperatures assigned to them. You must ensure that all temperatures of the corner nodes belonging to elements for which midside node temperatures are to be interpolated are read from the heat transfer analysis results or output database file. If the corner node temperatures are defined using a mixture of direct data input, reading from the results file or output database file, and user subroutine UTEMP, midside node temperatures that give unrealistic temperature fields may result. In practice, the capability for calculating midside node temperatures is most useful when temperatures generated by a heat transfer analysis are read from the results or output database file for the whole mesh during the stress analysis. Once the midside node capability is activated in a step, the capability will remain active throughout the remainder of the analysis. Values of temperature for nodes that existed in the original analysis but do not exist in the current analysis will be ignored. Similarly, if additional nodes (but not midside nodes) exist in the current analysis, the values of fields at these nodes cannot be prescribed by reading the output files. Input File Usage: Use the following option to interpolate temperatures between meshes that differ only in the element order: Abaqus/CAE Usage: *TEMPERATURE, FILE=file, MIDSIDE Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file, Mesh compatibility: Compatible, and toggle on Interpolate midside nodes Interpolating temperatures between dissimilar meshes (the general interpolation capability) In some cases the model for a heat transfer analysis and the model for a thermal-stress analysis may require different meshes; for example, you may want to model a smooth temperature distribution in the heat transfer analysis and stress concentration regions in the thermal-stress analysis. Both meshes have to be different and independent of each other in such cases. Abaqus offers a general interpolation capability that allows for the use of dissimilar meshes for heat transfer and thermal-stress analyses. The interpolation is always based on the initial (undeformed) configurations. If the mesh for which the temperature field is obtained is quite different from the initial (undeformed) configuration for the thermal-stress analysis, the interpolation may not work properly even when using the tolerance parameters discussed below. Temperatures can be interpolated between dissimilar meshes only when the temperatures are read from an output database file. If temperatures for nodes in the heat transfer analysis that are needed for interpolation are not written to the output database file, the values at those nodes are assumed to be zero, which may lead to incorrect results for the temperature values in the stress analysis. Similarly, if additional nodes exist in the mesh for the stress analysis, the values of temperatures at these nodes are assumed to be zero. Interpolation of temperatures can also be used for specifying temperature as a field variable in a submodel thermal-stress analysis where the temperature values are read directly from a global heat transfer analysis. You can specify an interpolation tolerance for use in locating the nodes in the heat transfer analysis. The tolerance can be specified as an absolute value or as a fraction of the average element size. In a multistep thermal-stress analysis in which several steps read the temperature values from the same file, Abaqus interpolates the temperature values only once. If different interpolation tolerance values are used for each step, the interpolation is based on the largest specified tolerance value. If a restart analysis is performed from a particular step in the thermal-stress analysis, the restart interpolation is based on the tolerance value specified for that step. Input File Usage: Abaqus/CAE Usage: Use the following option to interpolate temperatures between dissimilar meshes: *TEMPERATURE, FILE=file.odb, INTERPOLATE Use the following option to specify the interpolation tolerance as an absolute value: *TEMPERATURE, FILE=file.odb, INTERPOLATE, ABSOLUTE EXTERIOR TOLERANCE=tolerance Use the following option to specify the interpolation tolerance as a fraction of the average element size: *TEMPERATURE, FILE=file.odb, INTERPOLATE, EXTERIOR TOLERANCE=tolerance Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file.odb, Mesh compatibility: Incompatible, exterior tolerance: absolute or relative tolerance Interpolating temperatures between dissimilar meshes with user-specified regions When regions of elements in the heat transfer analysis are close or touching, the dissimilar mesh interpolation capability can result in an ambiguous temperature association. For example, consider a node in the current model that lies on or close to a boundary between two adjacent parts in the heat transfer model, and consider a case where temperatures in these parts are different. When interpolating, Abaqus will identify a corresponding parent element at the boundary for this node from the heat transfer analysis. This parent element identification is done using a tolerance-based search method. Hence, in this example the parent element might be found in either of the adjacent parts, resulting in an ambiguous temperature definition at the node. You can eliminate this ambiguity by specifying the source regions from which temperatures are to be interpolated. The source region refers to the heat transfer analysis and is specified by an element set. The target region refers to the current analysis and is specified by a node set. Input File Usage: Abaqus/CAE Usage: Use the following option to interpolate temperatures between dissimilar meshes with user-specified regions: *TEMPERATURE, FILE=file.odb, INTERPOLATE, DRIVING ELSETS You cannot specify the regions where temperatures are to be interpolated in Abaqus/CAE. Interpolating scalar nodal output variables between dissimilar meshes (the general interpolation capability) onto field variables in Abaqus/Standard Abaqus/Standard offers a general interpolation capability that allows for nodal values of temperature, normalized concentration, and electric potential from one analysis to be mapped onto field variables in a subsequent analysis in the cases where the meshes in the two analyses are dissimilar. The interpolation is always based on the initial (undeformed) configurations. If the mesh for which the field variable is obtained is quite different from the initial (undeformed) configuration for the original analysis, the interpolation may not work properly even when using the tolerance parameters discussed below. Temperatures, normalized concentrations, and electric potentials can be interpolated between dissimilar meshes onto field variables only when they are read from an output database file. If scalar values for nodes in the current analysis that are needed for interpolation are not written to the output database file, the values at those nodes are assumed to be zero, which may lead to incorrect results for the field variables. Similarly, if additional nodes exist in the mesh for the current analysis, the values of the field variables at these nodes are assumed to be zero. You can specify an interpolation tolerance for use in locating the nodes in the original analysis. The tolerance can be specified as an absolute value or as a fraction of the average element size. In a multistep analysis in which several steps read nodal output variables values from the same file, Abaqus interpolates the nodal values only once. If different interpolation tolerance values are used for each step, the interpolation is based on the largest specified tolerance value. If a restart analysis is performed from a particular step in the original analysis, the restart interpolation is based on the tolerance value specified for that step. Input File Usage: Use the following option to interpolate scalar nodal output variables between dissimilar meshes: *FIELD, FILE=file.odb, OUTPUT VARIABLE=scalar nodal output variable, INTERPOLATE Use the following option to specify the interpolation tolerance as an absolute value: *FIELD, FILE=file.odb, OUTPUT VARIABLE=scalar nodal output variable, INTERPOLATE, ABSOLUTE EXTERIOR TOLERANCE=tolerance Use the following option to specify the interpolation tolerance as a fraction of the average element size: *FIELD, FILE=file.odb, OUTPUT VARIABLE=scalar nodal output variable, INTERPOLATE, EXTERIOR TOLERANCE=tolerance Abaqus/CAE Usage: Predefined field variables are not supported in Abaqus/CAE. Specifying the step and increment to be read from the file You can specify the first and last step, respectively, from which results will be read. Similarly, you can specify the first and last increment, respectively, from which results will be read. You can specify any combination of these values. Any zero-increment file output that is present in the results file of an Abaqus/Standard analysis (written only if the zero increment results are requested; see “Obtaining results at the beginning of a step” in “Output,” Section 4.1.1) will be ignored. Results must have been written to the results or output database file at the specified step and increment. If you do not specify the first step from which to read, Abaqus will begin reading results from the first step available in the results or output database file. If you do not specify the first increment from which to read, Abaqus will begin reading results from the first increment available in the first step from which results will be read (the first increment following the zero increment if zero-increment file output is present in the results file). If you do not specify the last step from which to read, the first step from which results will be read will also be the last step. If you do not specify the last increment from which to read, Abaqus will read the results or output database file until it reaches the last available increment in the last step from which results will be read. Input File Usage: Use one of the following options: *TEMPERATURE, FILE=file, BSTEP=bstep, BINC=binc, ESTEP=estep, EINC=einc *FIELD, FILE=file, BSTEP=bstep, BINC=binc, ESTEP=estep, EINC=einc *PRESSURE STRESS, FILE=file, BSTEP=bstep, BINC=binc, ESTEP=estep, EINC=einc For example, the following input would read temperature data from output database file heat.odb beginning at Step 2, increment 2, and ending at Step 3, increment 5: *TEMPERATURE, FILE=heat.odb, BSTEP=2, BINC=2, ESTEP=3, EINC=5 Abaqus/CAE Usage: In Abaqus/CAE only predefined temperature fields are available. Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: From results or output database file, File name: file, Begin step: bstep, Begin increment: binc, End step: estep, and End increment: einc Interpolation in time When Abaqus reads temperature, field variable, or equivalent pressure stress data from a results file or temperatures from an output database file, it must obtain values of the field at the time points used by the analysis. Since data corresponding to these time points are usually not present in the results or output database files, Abaqus will interpolate linearly in time between the time points stored in the file to obtain values at the time points required by the analysis. Since the interpolation is linear, you must take care to provide sufficient data in the results or output database file to make this interpolation meaningful. For the purpose of such interpolation the time period of the results being read in is determined as follows: • The period starts at the time of the most recent increment written, of the relevant field, that precedes the beginning increment (either user-specified or default). For example if your results file contains temperature field data at increments 5, 10, and 15; and you specify a beginning increment number of 10 when reading these results; the results period starts with the time associated with increment 5 since that is the most recent increment that precedes the specified beginning increment of 10. You can ensure that the results starting time matches the beginning time of the beginning increment you specify by writing the results data with an increment frequency of 1. • The period ends at the completion of the ending increment (either user-specified or default). If the analysis requires data at a time point prior to the first increment for which data are available in the either of files, Abaqus will interpolate between the given initial condition data and the data of the first increment stored in the file. Reading results for multiple fields If data for multiple fields are being read in the same step and the time values corresponding to the starting step and increment or to the ending step and increment are different for different fields, Abaqus interpolates through the total time period from the earliest time point chosen in any file to the latest. For example, suppose the starting increment in the starting step in the temperature file begins at 3 sec and the ending increment in the ending step ends at 6 sec. During the same step we also read field variable data, for which the starting increment in the starting step begins at 2 sec and the ending increment in the ending step ends at 5 sec. In such a case the time period used for interpolation is from 2 sec to 6 sec. Automatic adjustment of the time scale It is convenient to set the period of the step equal to the time period of the files being read in. Otherwise, Abaqus will automatically scale the time period from the results or output database file to match the time period of the stress analysis. The scale factor is is the time period of the stress analysis and is the total time period obtained from all results or output database files, as described above. , where Obtaining results at a particular point in time In Abaqus/Standard it is sometimes desirable to carry out a calculation corresponding to the field values at a particular point in time. For example, suppose that temperature data are available in the output file for increment 10 at time and that you wish to carry out a static and increment 15 at time and to obtain the intermediate result at . In this case Abaqus must interpolate linearly between analysis based on temperature values at the results at . To accomplish this task, you should specify an initial time increment of 4.5 and a time period of 5. for the static analysis step and read the temperature values from the output file starting at Step 1, Increment 1 and ending at Step 1, Increment 15. Specifying a starting increment of 1 instead of 10 ensures that is the entire time period stored in the output file, not just the period between increments 10 and 15; hence, the scale factor between the output file data and the static analysis is unity, and the initial time of 4.5 has the desired meaning. Initial transients To track initial transients accurately, Abaqus/Standard may automatically reduce the initial time increment for the step. If the user-specified suggested initial time increment is greater than the scaled value of the first time increment read from the Abaqus/Standard results file, Abaqus/Standard will use that scaled value. Restrictions The following restrictions exist: • Temperatures and field variables cannot be read from a user-specified file in a modified Riks static analysis step (“Unstable collapse and postbuckling analysis,” Section 6.2.4). • Temperature cannot be interpolated from a coupled thermal-electrical analysis. • Equivalent pressure stress cannot be read from the results file if the model is defined in terms of an assembly of part instances. • In Abaqus/Explicit field variables cannot be read from the output database file. • Pressure stress cannot be read from the output database file. • Elements that do not support interpolation for temperature mapping include the complete libraries of convective heat transfer elements, axisymmetric elements with nonlinear axisymmetric deformation, axisymmetric surface elements, hydrostatic fluid elements, solid infinite stress elements, and coupled thermal/electrical elements. Other specific elements that are not supported include: GKPS6, GKPE6, GKAX6, GK3D18, GK3D12M, GK3D4L, GK3D6L, GKPS4N, GKAX6N, GK3D18N, GK3D12MN, GK3D4LN, and GK3D6LN. Defining the values of a predefined field in a user subroutine In Abaqus/Standard you can specify predefined temperatures, field variables, equivalent pressure stresses, or mass flow rates at the nodes in a user subroutine. Temperature values can be defined in user subroutine UTEMP; field variable values, in user subroutine UFIELD; equivalent pressure stress values, in user subroutine UPRESS; and mass flow rates, in user subroutine UMASFL. The user subroutine (UTEMP, UFIELD, UPRESS, or UMASFL) will be called for each specified node. Field values entered directly will be ignored. If a results or output database file has been specified in addition to the user subroutine, values read from the results or output database file will be passed into the user subroutine for possible modification. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *TEMPERATURE, USER *FIELD, USER *PRESSURE STRESS, USER *MASS FLOW RATE, USER In Abaqus/CAE only predefined temperature fields are available. Load module: Create Predefined Field: Step: analysis_step: choose Other for the Category and Temperature for the Types for Selected Step: select region: Distribution: User-defined or From results or output database file and user-defined Updating multiple predefined field variables If multiple field variables are predefined, only one field variable at a time can be redefined in user subroutine UFIELD. There are situations in which the analysis requires a number of field variables that are predefined with respect to the solution but depend on each other. You can specify the number of field variables to be updated simultaneously at a point, n. Abaqus/Standard passes information about n field variables at each specified node into UFIELD. You can update all or part of the field variables used in the analysis but must remember that the field variables are numbered consecutively from 1. If, for example, you have four field variables in the analysis and want to update the second and third variables simultaneously in subroutine UFIELD, you must specify n=3. In this case Abaqus/Standard passes information about the first three field variables into subroutine UFIELD, and you update only the second and third variables. Input File Usage: Abaqus/CAE Usage: *FIELD, USER, NUMBER=n Predefined field variables are not supported in Abaqus/CAE. Defining solution-dependent field variables In Abaqus/Standard solution-dependent field variables can be defined in user subroutine USDFLD. The values of predefined field variables or initial fields can be passed into user subroutine USDFLD and can be changed in that routine—see “Material data definition,” Section 21.1.2. Changes to the field variables in USDFLD are local to the material point and do not affect the nodal values. Data hierarchy If both results or output database file input and direct data input are used in the same step, the direct data input will take precedence if both define the field at the same node. If user subroutine input is specified, the values given directly are ignored and the user subroutine modifies the values read from the results or output database file. Element type considerations You can specify either one or several values of a predefined field at a node, depending on the element type that is used. You should note the following considerations when choosing the form of predefined field specification. Use in a mass diffusion analysis For solid elements only one value can be given at a node. Since only solid elements can be used in mass diffusion analysis, this is the only way to define equivalent pressure stresses at a node. Use with beam and shell elements The following possibilities exist for temperatures and field variable specification in beam and shell elements: • For shell and beam elements with general cross-section definitions, the temperature and field variable magnitude at points in the section is defined by the value at the reference surface. Any gradient of these variables specified across the section is ignored. • For shell and beam elements with cross-sections that require numerical integration, the temperature and field variable magnitudes at points in the section can be defined either from the value at the reference surface and the gradient or gradients across the section or by giving the values at a number of points across the section. The choice between these two methods is made in the section definition . See Part VI, “Elements,” for the details of use with each element type. The default, if only one value is given, is a constant magnitude across the section. Temperature and field variable compatibility across elements Abaqus assumes that the field definitions (including initial conditions) at all the nodes of any element are compatible with the field definition method chosen for the element. Cases may arise where the definition of a field changes from one element to the next (for example, when two adjacent shell elements have a different number of section points through the thickness or when the temperature and field variable magnitudes for one beam element are defined by giving the values at a number of points across the section while those for the abutting beam element are defined from the value at the reference surface and the gradient or gradients across the section). In these cases separate nodes should be used on the interface between such elements and multi-point constraints should be applied to make the displacements and rotations the same at corresponding nodes ; otherwise, the fields on the nodes at the interface will be used for each adjacent element with the field definition method chosen for the element. Constraints Overview Multi-point constraints Surface-based constraints Embedded elements Element end release Overconstraint checks CONSTRAINTS 34.1 34.2 34.3 34.4 34.5 34.1 Overview • “Kinematic constraints: overview,” Section 34.1.1 34.1.1 KINEMATIC CONSTRAINTS: OVERVIEW The following types of kinematic constraints can be defined: • Equations: Linear multi-point constraints can be given in the form of an equation . • Multi-point constraints: Multi-point constraints (MPCs) specify linear or nonlinear constraints between nodes. These relations between nodes can be the default types that are provided in Abaqus or, in Abaqus/Standard, can be coded in the form of a user subroutine. “General multi-point constraints,” Section 34.2.2, explains the use of MPCs and lists the available default constraints. • Kinematic coupling: In Abaqus/Standard a node or group of nodes can be constrained to a reference node. Similar to multi-point constraints, the kinematic coupling constraint allows general node-by-node specification of constrained degrees of freedom . • Surface-based tie constraints: Two surfaces can be tied together. Each node on the first surface (the slave surface) will have the same values for its degrees of freedom as the point on the second surface (the master surface) to which it is closest . In the case of surface elements tied to a beam surface, the offset distances between the surface elements and the beam are used in the definition of constraints, which include the rotational degrees of freedom of the beam. • Surface-based coupling constraints: A group of nodes located on a surface can be constrained to a reference node. This constraint may be kinematic, in which the group of coupling nodes can be constrained to the rigid body motion defined by the reference node, or distributing, in which the group of coupling nodes can be constrained to the rigid body motion defined by the reference node in an average sense . • Surface-based shell-to-solid coupling: An edge-based surface on a three-dimensional shell element mesh can be coupled to an element- or node-based surface on a three-dimensional solid mesh. The coupling is enforced by the creation of an internal set of distributing coupling constraints . • Mesh-independent spot welds: Two or more surfaces can be bonded together using fasteners such as spot welds . Distributed coupling constraints are created on each of the connected surfaces. The connection is modeled independent of the mesh. • Embedded elements: An element or a group of elements can be embedded in a group of host elements . Abaqus will search for the geometric relationships between nodes on the embedded elements and the host elements. If a node on an embedded element lies within a host element, the degrees of freedom at the node will be eliminated by constraining them to the interpolated values of the degrees of freedom of the host element. Host elements cannot be embedded themselves. • Release: In Abaqus/Standard a local rotational degree of freedom or a combination of local rotational degrees of freedom can be released at one or both ends of a beam element . Boundary conditions are also a type of kinematic constraint in stress analysis because they define the support of the structure or give fixed displacements at nodal points. Specification of boundary conditions is discussed in “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Connector elements can be used to impose element-based kinematic constraints for mechanism-type analysis. See “Connectors: overview,” Section 31.1.1. Contact interactions, described in Part IX, “Interactions,” can be used to enforce constraints between bodies that come into contact. Contact interactions can be used in mechanical as well as coupled thermal- mechanical, coupled thermal-electrical-structural, and coupled pore fluid-mechanical analysis. “Overconstraint checks,” Section 34.6.1, describes the overconstraint checks and the automatic resolution of some overconstraints performed in Abaqus/Standard. Multiple kinematic constraints at a node It is possible to use a single node in several multi-point constraints, kinematic coupling constraints, tie constraints, and constraint equations. However, the constraint dependencies are handled differently in Abaqus/Standard and Abaqus/Explicit. Multiple constraints in Abaqus/Standard In Abaqus/Standard kinematic constraints are usually imposed by eliminating degrees of freedom at the dependent nodes. Once a variable has been eliminated, it cannot be referenced in any boundary condition or in any subsequent multi-point constraint, kinematic coupling constraint, tie constraint, or constraint equation. If you intend to use a variable that is eliminated in one constraint equation as the retained variable in another constraint equation, you must order the input so that the constraint equation in which the variable is eliminated follows the other constraint equations. MPC types BEAM, CYCLSYM, LINK, PIN, REVOLUTE, TIE, and UNIVERSAL, as well as the kinematic coupling and tie constraints, are sorted internally by Abaqus/Standard to obtain a proper elimination order when possible. Excessive chaining of multi-point constraints, kinematic coupling constraints, and constraint equations is not recommended and may result in a degradation in performance during analysis preprocessing. Whenever possible, it is best to relate the behavior of several nodes (grouped into a node set) to a single node by using one multi-point constraint, kinematic coupling constraint, or constraint equation. Multiple constraints in Abaqus/Explicit Kinematic constraints in Abaqus/Explicit can be defined in any order without regard to constraint dependencies. With the exception of constraints arising from kinematic contact pairs, Abaqus/Explicit solves for all kinematic constraints simultaneously. Thus, nodes involved in a combination of multi-point constraints, constraint equations, connector element kinematic constraints, rigid body constraints, and constraints due to boundary conditions will simultaneously satisfy these constraints as long as they are not conflicting. Redundant and closed loop constraints are acceptable. Since the above constraints are enforced independent of contact constraints, the penalty contact algorithm should be used for nodes involved in both kinematic constraints and contact pair definitions. The penalty contact algorithm introduces numerical softening through the use of penalty springs and does not interfere with kinematic constraints. If a node that participates in a kinematic constraint is used in a kinematic contact pair, the contact constraint will most likely override the kinematic constraint. Except for rigid bodies, Abaqus/Explicit will not prevent you from defining these conditions, but the results cannot be guaranteed. If a kinematic constraint is defined for a node on a rigid body, the penalty contact algorithm must be used for all contact pairs involving the rigid body. To obtain accurate reaction force and moment output from Abaqus/Explicit at nodes that are constrained by boundary conditions in addition to one or more of the kinematic constraints described above, it may sometimes be necessary to run the analysis in double precision. In such a situation a double precision run will also yield a better estimate of the work done by the reaction forces and moments, thereby providing a more accurate value of the energy due to the external work reported by Abaqus/Explicit. Abaqus/Explicit uses a penalty method to solve for constraints in certain situations. The penalties are weighted based on the masses of nodes participating in the constraint and the stable time increment. The penalty formulation attempts to satisfy the constraint approximately (i.e., a very small lack of compliance exits after imposition of the constraint). One situation in which the penalty approach is used to solve the constraint is when slave nodes of a tie constraint participate in other constraints such as multi-point constraints, kinematic coupling constraints, constraint equations, connector elements, rigid body constraints, or constraints due to boundary conditions. In this case the lack of compliance in the tie constraint is not carried across step boundaries; therefore, noisy accelerations and energy imbalance may be observed at step boundaries for certain problems. An alternative modeling approach (such as simply reversing the master and slave surfaces in the tie constraint) may switch to a different solution approach and thus resolve the above mentioned inaccuracies. In Abaqus/Explicit when there are two or more overlapping distributed coupling constraints or overlapping distributed coupling and tie constraints, and the elements underlying the participating surfaces have very low densities, the lack of compliance may result in an inaccurate solution. Specifying reasonable density values for underlying elements may reduce the lack of compliance and improve solution accuracy. Abaqus/Explicit always uses a geometrically nonlinear formulation for the enforcement of kinematic constraints. This is the case even when you have designated a particular analysis step as being geometrically linear. Consequently, results in these geometrically linear analyses could be hard to interpret, particularly when the loading in the model is high (displacements are large) and a geometrically nonlinear formulation should have been used. Initial conditions at constrained nodes You should not think of initial conditions as boundary conditions at the beginning of the analysis. When you prescribe initial conditions at a set of nodes that are constrained kinematically, Abaqus processes the prescribed values to determine an initial value that is then redistributed to the nodes involved in the constraints in a kinematically consistent manner via a “mass” weighted averaging method: the initial value prescribed at each node involved in the constraint is weighted with the corresponding “mass” at the node. Consequently, the values of the initial conditions that you specified at the nodes are recomputed, and in many cases the output of the prescribed quantity at these nodes at the beginning of the analysis will be different from the values that you have specified. Correct modeling practices consist of specifying initial conditions at all nodes involved in the constraints in a manner consistent with constraint itself. This behavior is probably best understood via a simple example. Consider a model consisting of two nodes each with a mass of 1.0 constrained by boundary conditions in global directions 2 and 3 and allowed to move freely along the global 1-direction while their relative motions is also constrained via a rigid connection such as a BEAM connector. Assume that you have specified an initial translational velocity along the global 1-direction only at the first node of 10.0 units and you have not specified initial conditions at the second node. Consequently, Abaqus will consider that the initial velocity is 0.0 at the second node. This initial velocity field is inconsistent with the kinematic constraint enforced by the BEAM connector because the constraint would be violated if the initial conditions were to be enforced even for an infinitesimally short period of time. The outcome is that Abaqus will compute an initial velocity field that would redistribute the momentum of the first node in a manner consistent with the constraint. In this particular example, the net effect is that both nodes will end up with an initial velocity of 5.0 units along the global 1-direction. Most likely, this is not what you intended. Correct modeling practice in this case would be to specify an initial velocity of 10.0 units at both nodes involved in the constraint. In this case Abaqus will still recompute the initial values, but the outcome would be an initial velocity of 10.0 units at both nodes, as intended. The same principle applies in more complicated modeling situations. For example, if you prescribe initial translational velocities at the nodes of the kinematic constraint, an average translational velocity of the constrained nodes is computed by calculating a mass weighted average of the velocities at the individual nodes. Depending on the nature of the kinematic constraint, initial translational velocities at the nodes of a constraint may also give rise to an average rotational velocity about the center of mass of the constraint. The velocity of each individual node of the constraint is then recomputed from the average translational and rotational velocities at the center of mass of the constraint. The “mass”-type quantity used in the weighting varies depending on the nature of the prescribed quantity: if the initial condition is prescribed on the rotational velocities, the rotary inertia at the nodes is used in the weighting; if temperature initial conditions are prescribed, the thermal capacitance at the nodes is used in the weighting; and so on. In all cases, you should specify initial conditions at all nodes involved in the constraint that are consistent with the constraint. This is typically accomplished by specifying the same initial conditions at all nodes involved in the constraint. 34.2 Multi-point constraints • “Linear constraint equations,” Section 34.2.1 • “General multi-point constraints,” Section 34.2.2 • “Kinematic coupling constraints,” Section 34.2.3 34.2.1 LINEAR CONSTRAINT EQUATIONS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Kinematic constraints: overview,” Section 34.1.1 • *EQUATION • “Defining equation constraints,” Section 15.15.9 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A linear multi-point constraint requires that a linear combination of nodal variables is equal to zero; that is, is a nodal variable at node P, degree of freedom i; and the are coefficients that define the relative motion of the nodes. , where In Abaqus/Explicit linear constraint equations can be used only to constrain mechanical degrees of freedom. Defining a linear constraint equation A linear constraint equation is defined in Abaqus by specifying: • the number of terms in the equation, N; • the nodes, P, and the degrees of freedom, i, corresponding to the nodal variables • the coefficients, . ; and For example, to impose the equation you would first write the equation in the standard form, There are three terms in this equation (N=3). P=5, i=3, =1.0, Q=6, j=1, =−1.0, R=1000, k=3, and =1.0. Input File Usage: *EQUATION P, i, , Q, j, , etc. For example, the following input could be used to define the equation constraint above: *EQUATION 5, 3, 1.0, 6, 1, -1.0, 1000, 3, 1.0 Either node sets or individual nodes can be specified as input. If node sets are used, corresponding set entries will be matched to each other. If sorted node sets are given as input, you must ensure that the nodes are numbered such that they will match up with each other correctly once sorted. The nodes in an unsorted node set will be used in the order that they are given in defining the set . If the first entry is a single node, subsequent entries must be single nodes. If the first entry is a node set, subsequent entries can be either node sets or single nodes. The latter option is useful if a degree of freedom at each of a set of nodes depends on a degree of freedom of a single node, such as may occur in certain symmetry conditions or in the simulation of a rigid body. Abaqus/CAE Usage: Interaction module: Create Constraint: Equation The nodes must be specified as sets. The first set can contain one or more points. Subsequent sets must contain only a single point. In Abaqus/Standard the first nodal variable specified ( ) will be eliminated to impose the constraint (in the above equation constraint, degree of freedom 3 at node 5 will be eliminated); therefore, it should not be used to apply boundary conditions, nor should it be used in any subsequent multi-point constraint, kinematic coupling constraint, tie constraint, or equation constraint . In addition, the coefficient should not be set to zero. These restrictions do not apply in Abaqus/Explicit. corresponding to In Abaqus/Standard a linear multi-point constraint cannot be used to connect two rigid bodies at nodes other than the reference nodes, since multi-point constraints use degree-of-freedom elimination and the other nodes on a rigid body do not have independent degrees of freedom. In Abaqus/Explicit a rigid body reference node or any other node on a rigid body can be used in an equation constraint definition. Use with transformed coordinate systems If a local coordinate system (“Transformed coordinate systems,” Section 2.1.5) is defined for any node involved in the equation, the variables at that node appear in the equation in the local system. Use within a part If an equation constraint is defined at the part (or part instance) level, the nodal variables are transformed initially according to the positioning data given for each instance of the part . Note: Equation constraints cannot be defined at the part (or part instance) level in Abaqus/CAE. Prescribing a nonhomogeneous constraint It is sometimes necessary to impose a constraint in the form where as is a prescribed value that may vary with time, t. This is easily done by rewriting the equation to be and introducing a node, Z, that is not attached to any element in the model. Choosing some convenient degree of freedom m at node Z allows the prescribed value to be imposed through a boundary condition specification. If necessary, an amplitude reference can be provided to give the variation with time ; such an amplitude reference is required in Abaqus/Explicit for prescribed displacements. For example, assume that node 1000 in the example above is a “dummy” node that appears only in this equation and is not attached to any other part of the model. Defining a boundary condition to constrain degree of freedom 3 at node 1000 to −12.5 would impose the constraint Constraint forces and global equilibrium Linear constraint equations introduce constraint forces at all degrees of freedom appearing in the equations. These forces are considered external, but they are not included in reaction force output. Therefore, the totals provided at the end of the reaction force output tables may reflect an incomplete measure of global equilibrium. To illustrate this behavior, consider a spring-supported beam subjected to a concentrated load as shown in Figure 34.2.1–1. The static reaction forces are . In Figure 34.2.1–2 and , which constrains the same structure is subjected to the additional linear constraint equation , and the the beam to remain horizontal. This introduces constraint forces . These reaction forces produce a global force balance in the new reaction forces are Y-direction, but since the constraint forces are not included in reaction force output, the global moment balance about point A cannot be verified. and P = 9 y 2 1 R = –3 y R = – 6 y Figure 34.2.1–1 Beam with no linear constraints. F = 1.5 y R = – 4.5 y P = 9 y F = –1.5 y 2 1 R = – 4.5 y Figure 34.2.1–2 Beam with linear constraint . Constraint forces and are not included in reaction force output. The global force balance can also be incomplete. This is demonstrated in Figure 34.2.1–3, where a . , are not included in the reaction force output, producing pulley connection between nodes A and B is represented by the linear constraint equation The constraint forces at the pulley, incomplete global force balances in both the X- and Y-directions. and P = 9 y F = –9 F = –9 R = 9x Figure 34.2.1–3 Pulley connection represented by the linear constraint . Constraint forces and are not included in reaction force output. Obtaining the constraint force The linear constraint generates constraint forces at all the degrees of freedom involved in the equation. For a given constraint equation these forces are proportional to their respective coefficients. To find the constraint forces, introduce a node Z that is not attached to any element in the model; rewrite the constraint equation as and specify a zero displacement boundary condition at degree of freedom m of node Z. The reaction force obtained at node Z will be equal to the constraint force acting at node P in degree of freedom i. The constraint force in any term with coefficient in the constraint equation is obtained by multiplying the constraint force at node P in degree of freedom i with the ratio . For example, if the equation is and the forces in the constraint are needed, the equation can be rewritten as is the opposite of the coefficient , the constraint force at node 5 is the same as the reaction force at node 1000. Since the coefficient , the constraint force at node 6 is the opposite of the reaction where node 1000 is the fixed “dummy” node. Since the coefficient of of of force at node 1000. is the same as the coefficient of Defining a constraint in a deformed state Sometimes we may wish to impose an equation starting at a certain point in the analysis: where represents the change in displacement after time . The equation can be rewritten as (which is assumed to further changes are restrained in Abaqus/Standard by applying a boundary condition fixing the degree of freedom where, again, node Z is not attached to any element in the model. Prior to time be at the end of a step), degree of freedom m of node Z is left unrestrained. After time in at its current values at the start of the step. Reading the data from an alternate input file Input File Usage: The input for a linear constraint equation can be contained in a separate input file. *EQUATION, INPUT=file_name If the INPUT parameter is omitted, it is assumed that the data lines follow the keyword line. Abaqus/CAE Usage: Interaction module: Create Constraint: Equation: click mouse button 3 while holding the cursor over the data table, and select Read from File 34.2.2 GENERAL MULTI-POINT CONSTRAINTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Kinematic constraints: overview,” Section 34.1.1 • *MPC • “Defining MPC constraints,” Section 15.15.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • Chapter 24, “Connectors,” of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Multi-point constraints (MPCs): • allow constraints to be imposed between different degrees of freedom of the model; and • can be quite general (nonlinear and nonhomogeneous). The most commonly required constraints are available directly by choosing an MPC type and giving the associated data. The available MPC types are described below; MPCs that are available only in Abaqus/Standard are designated with an (S) . In Abaqus/Standard the constraints can also be given by user subroutine MPC. Linear constraints can be given directly by defining a linear constraint equation . In Abaqus/Explicit some multi-point constraints can be modeled more effectively using rigid bodies . Several MPC types are also available with connector elements (“Connector elements,” Section 31.1.2). Although the connector elements impose the same kinematic constraint, connectors do not eliminate degrees of freedom. MPC constraint forces are not available as output quantities. Therefore, to output the forces required to enforce the constraint specified in an MPC, you should use an equivalent connector element. Connector element force, moment, and kinematic output is readily available and is defined in “Connector element library,” Section 31.1.4. Identifying the nodes involved in the MPC For any MPC type, either node sets or individual nodes can be given as input. If the first entry is a node, subsequent entries must be nodes. If the first entry is a node set, subsequent entries can be either node sets or single nodes. The latter option is useful if a degree of freedom at each of a set of nodes depends on a degree of freedom of a single node, such as may occur in certain symmetry conditions or in the simulation of a rigid body. If node sets are used, corresponding set entries will be constrained to each other. If sorted node sets are given as input, you must ensure that the nodes are numbered such that they will match up correctly when sorted. The nodes in an unsorted node set will be used in the order that they are given in defining the set. In Abaqus/Standard multi-point constraints cannot be used to connect two rigid bodies at nodes other than the reference nodes, since multi-point constraints use degree-of-freedom elimination and the other nodes on a rigid body do not have independent degrees of freedom. In Abaqus/Explicit a rigid body reference node or any other node on a rigid body can be used in a multi-point constraint definition. Abaqus/CAE uses connectors to define multi-point constraints between two points and constraints to define multi-point constraints between a point and slave nodes in a region. Set-to-set multi-point constraints and unsorted node sets are not supported in Abaqus/CAE. Input File Usage: Abaqus/CAE Usage: *MPC Use the following options to define a multi-point constraint between two points: Interaction module: Connector→Geometry→Create Wire Feature Connector→Section→Create: Connection Category: MPC, MPC type: select type Connector→Assignment→Create: select wires: Section: select MPC connector section Use the following options to define a multi-point constraint between a point and slave nodes in a region: Interaction module: Constraint→Create: MPC Constraint: select control point and region; MPC type: select type Use with transformed coordinate systems Local coordinate systems can be defined for any nodes connected to MPCs. Some special considerations apply for user-defined MPCs, as described in “MPC,” Section 1.1.14 of the Abaqus User Subroutines Reference Manual. Defining multiple multi-point constraints at a point See “Kinematic constraints: overview,” Section 34.1.1, for details on how multiple kinematic constraints at a point are treated in Abaqus/Standard and Abaqus/Explicit. In Abaqus/Standard MPCs are usually imposed by eliminating the degree of freedom at the first node given (the dependent degree of freedom). MPC types BEAM, CYCLSYM, LINK, PIN, REVOLUTE, TIE, and UNIVERSAL are sorted internally by Abaqus/Standard so that the MPC in which a node is used as a dependent node is the last MPC that uses this node. Therefore, groups of these MPCs can be given in any order. However, even for these MPCs, a node can be used only once as a dependent node. In other cases dependent degrees of freedom should not be used subsequently to impose kinematic constraints; this generally precludes the use of the first node in an MPC definition as an independent node in any subsequent multi-point constraint, equation constraint, kinematic coupling constraint, or tie constraint definition. Using MPCs in implicit dynamic analysis In implicit dynamic analysis Abaqus/Standard enforces MPCs rigorously for the displacements. The velocities and accelerations are derived from the displacements with the relations defined by the dynamic integration operator . For linear MPCs (such as PIN, TIE, and mesh refinement MPCs) and geometrically linear analysis the velocities obtained in this way satisfy the constraint exactly. However, the accelerations satisfy the constraint only approximately. If nonlinear MPCs (such as BEAM, LINK, and SLIDER) are used in geometrically nonlinear analysis, both the velocities and accelerations satisfy the constraint only approximately. In most cases the approximation is quite accurate, but in some cases high frequency oscillations may occur in the accelerations of the nodes involved in the MPC. Using nonlinear MPCs in geometrically linear Abaqus/Standard analysis If a nonlinear MPC is used in a geometrically linear Abaqus/Standard analysis , the MPC is linearized. For example, if MPC LINK is used in a geometrically nonlinear Abaqus/Standard analysis, the distance between the two nodes of the link remains constant. If it is used in a geometrically linear Abaqus/Standard analysis, the distance between the two nodes is held constant after projection onto the direction of the line between the original positions of the nodes. The difference should be noticeable only if the magnitudes of the rotations and displacements are not small. Defining MPCs in a user subroutine In Abaqus/Standard you can define multi-point constraints in user subroutine MPC. Constraints defined in user subroutine MPC can only use degrees of freedom that also exist on an element somewhere in the same model. For example, if a model contains no elements with rotational degrees of freedom, user subroutine MPC cannot use degrees of freedom 4, 5, or 6. This limitation can be overcome by adding a suitable element somewhere in the model to introduce the required degrees of freedom. This element can be added so that it does not affect the response of the model. Constraints defined in the user subroutine are applied to the transformed degrees of freedom. A boundary nonlinearity occurs in Abaqus/Standard when MPCs are activated/deactivated in a user subroutine. Input File Usage: Abaqus/CAE Usage: *MPC, USER Use one of the following options: Interaction module: Create Connector Section: select MPC as the Connection Category and User-defined as the MPC Type Interaction module: Create Constraint: MPC Constraint; select User-defined as the MPC Type Specifying the version of user subroutine MPC You must specify whether the user subroutine will be coded in degree of freedom mode or in nodal mode. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *MPC, USER, MODE=DOF *MPC, USER, MODE=NODE Use one of the following options: Interaction module: Create Connector Section: select MPC as the Connection Category and User-defined as the MPC Type, choose DOF-by-DOF or Node-by-Node Interaction module: Create Constraint: MPC Constraint: select User-defined as the MPC Type, choose DOF-by-DOF or Node-by-Node Reading the data from an alternate input file The input for an MPC definition can be contained in a separate input file. Input File Usage: *MPC, INPUT=file_name If the INPUT parameter is omitted, it is assumed that the data lines follow the keyword line. Abaqus/CAE Usage: Reading data from an alternate input file is not supported in Abaqus/CAE. MPCs for mesh refinement LINEAR QUADRATIC(S) BILINEAR(S) C BIQUAD(S) This MPC is a standard method for mesh refinement of first-order elements. It applies to all active degrees of freedom at the involved nodes including temperature, pressure, and electrical potential. In Abaqus/Explicit it might be preferable to use a surface-based tie constraint for mesh refinement, particularly when one or more of the meshes to be constrained involve shell elements with thickness. This MPC is a standard method for mesh refinement of second-order elements. It applies to all active degrees of freedom at the involved nodes with the exception of temperature degrees of freedom in coupled temperature-displacement analysis and coupled thermal-electrical-structural analysis and to pressure degrees of freedom in coupled pore pressure analysis. For refinement using second-order pore pressure or coupled-temperature displacement elements, the P LINEAR or T LINEAR MPC must be used in conjunction with this MPC. This MPC is a standard method for mesh refinement of first-order solid elements in three dimensions. It applies to all active degrees of freedom at the involved nodes including temperature, pressure, and electrical potential. This MPC is a standard method for mesh refinement of second-order solid It applies to all active degrees of freedom at the elements in three dimensions. involved nodes with the exception of temperature degrees of freedom in coupled thermal-electrical-structural and temperature-displacement analysis and to pressure degrees of freedom in coupled pore pressure analysis. For refinement using pore pressure or coupled-temperature displacement elements in three dimensions, the P BILINEAR or T BILINEAR MPC must be used in conjunction with this MPC. analysis coupled P LINEAR(S) T LINEAR(S) P BILINEAR(S) T BILINEAR(S) This MPC can be used in conjunction with the QUADRATIC MPC for mesh refinement of second-order, fully coupled pore fluid flow-displacement elements. It applies to pressure degrees of freedom only. For acoustic analysis it applies the same constraint as the LINEAR MPC. This MPC can be used in conjunction with the QUADRATIC MPC for mesh refinement of second-order, fully coupled temperature-displacement and fully coupled thermal-electrical-structural elements. It applies to temperature degrees of freedom only. For heat transfer analysis it applies the same constraint as the LINEAR MPC. This MPC can be used in conjunction with the C BIQUAD MPC for mesh refinement of pore fluid flow-displacement elements in three dimensions. It applies to pressure degrees of freedom only. For acoustic analysis it applies the same constraint as the BILINEAR MPC. fully coupled temperature-displacement This MPC can be used in conjunction with the C BIQUAD MPC for mesh refinement of and fully coupled thermal-electrical-structural elements in three dimensions. It applies to temperature degrees of freedom only. For heat transfer analysis it applies the same constraint as the BILINEAR MPC. Using mesh refinement MPCs with shell or beam elements The Abaqus/Standard shell elements S4R5, S8R5, S9R5, and STRI65 use a penalty method to enforce transverse shear constraints on the edges of the element. The use of mesh refinement MPCs LINEAR and QUADRATIC may, therefore, lead to overconstraining or “shear locking” of the bending behavior. Graded meshes, using the triangular elements as necessary to create a transition zone, are recommended for mesh refinement with these elements. The shear flexible beam elements in Abaqus/Standard such as B31 or B32 will also “lock” if used as stiffeners along a mesh line where the mesh refinement MPCs are used. For shell elements in Abaqus/Explicit the rotational degrees of freedom are not constrained by the LINEAR MPC; therefore, a hinge is formed along the line defined by the constrained nodes. Using MPC type LINEAR MPC type LINEAR is a standard method for mesh refinement of first-order elements. However, in Abaqus/Explicit it might be preferable to use a surface-based tie constraint for mesh refinement, particularly when one or more of the meshes to be constrained involve shell elements with thickness. This MPC constrains each degree of freedom at node p to be interpolated linearly from the corresponding degrees of freedom at nodes a and b . Figure 34.2.2–1 LINEAR type MPC. Input data Give the nodes p, a, and b as shown in Figure 34.2.2–1. *MPC LINEAR, p, a, b Input File Usage: Abaqus/CAE Usage: Mesh refinement multi-point constraints are not supported in Abaqus/CAE. Using MPC type QUADRATIC MPC type QUADRATIC is a standard method for mesh refinement of second-order elements. This MPC type is available only in Abaqus/Standard. This MPC constrains each degree of freedom at node p (where p is either ) to be interpolated quadratically from the corresponding degrees of freedom at nodes a, b, and c (Figure 34.2.2–2). For coupled temperature-displacement, coupled thermal-electrical-structural, or pore pressure elements, only the displacement degrees of freedom are constrained. or p2 p1 p2 p1 Figure 34.2.2–2 QUADRATIC type MPC. Input data Give the nodes p, a, b, and c as shown in Figure 34.2.2–2, where p is either or . Input File Usage: *MPC QUADRATIC, p, a, b, c Abaqus/CAE Usage: Mesh refinement multi-point constraints are not supported in Abaqus/CAE. Using MPC type BILINEAR MPC type BILINEAR is a standard method for mesh refinement of first-order solid elements in three dimensions. This MPC type is available only in Abaqus/Standard. This MPC constrains each degree of freedom at node p to be interpolated bilinearly from the corresponding degrees of freedom at nodes a, b, c, and d (Figure 34.2.2–3). Figure 34.2.2–3 BILINEAR type MPC. Input data Give the nodes p, a, b, c, and d as shown in Figure 34.2.2–3. Input File Usage: *MPC BILINEAR, p, a, b, c, d Abaqus/CAE Usage: Mesh refinement multi-point constraints are not supported in Abaqus/CAE. Using MPC type C BIQUAD MPC type C BIQUAD is a standard method for mesh refinement of second-order solid elements in three dimensions. This MPC type is available only in Abaqus/Standard. This MPC constrains each degree of freedom at node p to be interpolated by a constrained biquadratic from the corresponding degrees of freedom at the eight nodes a, b, c, d, e, f, g, and h (Figure 34.2.2–4). For coupled temperature-displacement, coupled thermal-electrical-structural, or pore pressure elements, only the displacement degrees of freedom are constrained. Figure 34.2.2–4 C BIQUAD type MPC. Input data Give the nodes p, a, b, c, d, e, f, g, and h as shown in Figure 34.2.2–4. Input File Usage: *MPC C BIQUAD, p, a, b, c, d, e, f, g, h Abaqus/CAE Usage: Mesh refinement multi-point constraints are not supported in Abaqus/CAE. Using MPC types P LINEAR and T LINEAR The P LINEAR MPC can be used in conjunction with the QUADRATIC MPC for mesh refinement of second-order, fully coupled pore fluid flow-displacement elements. The T LINEAR MPC can be used in conjunction with the QUADRATIC MPC for mesh refinement of second-order, fully coupled temperature-displacement and fully coupled thermal-electrical-structural elements. These MPC types are available only in Abaqus/Standard. These MPCs constrain the pore pressure (P LINEAR) or temperature (T LINEAR) degree of freedom at node p to be interpolated linearly from the degrees of freedom at nodes a and b (Figure 34.2.2–5). Figure 34.2.2–5 P LINEAR and T LINEAR MPCs. Input data Give the nodes p, a, and b as shown in Figure 34.2.2–5. Input File Usage: Use the following option to define a P LINEAR MPC: *MPC P LINEAR, p, a, b Use the following option to define a T LINEAR MPC: *MPC T LINEAR, p, a, b Abaqus/CAE Usage: Mesh refinement multi-point constraints are not supported in Abaqus/CAE. Using MPC types P BILINEAR and T BILINEAR The P BILINEAR MPC can be used in conjunction with the C BIQUAD MPC for mesh refinement of pore fluid flow-displacement elements in three dimensions. The T BILINEAR MPC can be used in conjunction with the C BIQUAD MPC for mesh refinement of fully coupled temperature-displacement and fully coupled thermal-electrical-structural elements in three dimensions. These MPC types are available only in Abaqus/Standard. These MPCs constrain the pore pressure (P LINEAR) or temperature (T LINEAR) at node p to be interpolated bilinearly from the pore pressure or temperature at nodes a, b, c, and d (Figure 34.2.2–6). Figure 34.2.2–6 P BILINEAR and T BILINEAR MPCs. Input data Give the nodes p, a, b, c, and d as shown in Figure 34.2.2–6. Input File Usage: Use the following option to define a P BILINEAR MPC: *MPC P BILINEAR, p, a, b, c, d Use the following option to define a T BILINEAR MPC: *MPC T BILINEAR, p, a, b, c, d Abaqus/CAE Usage: Mesh refinement multi-point constraints are not supported in Abaqus/CAE. MPCs for connections and joints BEAM CYCLSYM(S) ELBOW(S) LINK PIN REVOLUTE(S) SLIDER TIE UNIVERSAL(S) V LOCAL(S) Provide a rigid beam between two nodes to constrain the displacement and rotation at the first node to the displacement and rotation at the second node, corresponding to the presence of a rigid beam between the two nodes. Constrain nodes to impose cyclic symmetry in a model. Constrain two nodes of ELBOW31 or ELBOW32 elements together, where the cross-sectional direction, , changes . Provide a pinned rigid link between two nodes to keep the distance between the two nodes constant. The displacements of the first node are modified to enforce this constraint. The rotations at the nodes, if they exist, are not involved in this constraint. Provide a pinned joint between two nodes. This MPC makes the displacements equal but leaves the rotations, if they exist, independent of each other. Provide a revolute joint. Keep a node on a straight line defined by two other nodes, but allow the possibility of moving along the line and allow the line to change length. Make all active degrees of freedom equal at two nodes. Provide a universal joint. Allow the velocity at the constrained node to be expressed in terms of velocity components at the third node defined in a local, body axis system. These local velocity components can be constrained, thus providing prescribed velocity boundary conditions in a rotating, body axis system. See “Connectors: overview,” Section 31.1.1, for element-based versions of several of these MPCs for connections and joints. Using MPC type BEAM MPC type BEAM provides a rigid beam between two nodes to constrain the displacement and rotation at the first node to the displacement and rotation at the second node, corresponding to the presence of a rigid beam between the two nodes. beam node shell node beam node shell node Figure 34.2.2–7 BEAM type MPC. Input data Give the nodes a and b as shown in Figure 34.2.2–7. Input File Usage: *MPC BEAM, a, b Abaqus/CAE Usage: Use one of the following options: Interaction module: Create Connector Section: select MPC as the Connection Category and Beam as the MPC Type Interaction module: Create Constraint: MPC Constraint; select Beam as the MPC Type Constraining a beam stiffener to a shell The general method of using a beam as a stiffener on a shell is to define the beam and shell elements with separate nodes. These nodes can then be constrained to each other using BEAM type MPCs. A more economical way, when applicable, is to use the same node for the beam node and the shell node and then define the offset of the center of the cross-section of the beam in the beam section data. Figure 34.2.2–8 shows a T-shaped stiffener attached to a shell, using the I-beam cross-section. This is done by setting l equal to the distance between the node and the underside of the lower flange and setting the thickness of the top flange to zero. This approach can be used with all beam elements that use TRAPEZOID, I, or ARBITRARY beam sections. node t1 b = 0. t = 0. b1 Figure 34.2.2–8 Stiffened shell. Using MPC type CYCLSYM MPC type CYCLSYM is used to enforce proper constraints on the radial faces bounding a segment of a cyclic symmetric structure . This MPC type is available only in Abaqus/Standard. MPC type CYCLSYM imposes the cyclic symmetry by equating radial, circumferential, and axial displacement components (and rotations, if active) at the two nodes (a and b). The symmetry axis can be defined by the original coordinates of two additional nodes (c and d) that do not need to be connected to any element in the structure. Scalar degrees of freedom (such as temperature) are made equal. original part intended to be analyzed possessing cyclic symmetry axis of cyclic symmetry section actually modeled Figure 34.2.2–9 MPC type CYCLSYM. Input data Give the nodes a, b, and (optionally) node c and/or d that define the axis of symmetry as shown in Figure 34.2.2–9. Node set names can be used instead of the nodes a and b. If neither c nor d is given, the global z-axis is taken to be the axis of cyclic symmetry. If only node c is given, the symmetry axis passes through c and is parallel to the global z-axis. Thus, node d is not needed in two-dimensional cases. Input File Usage: Abaqus/CAE Usage: *MPC CYCLSYM, a, b, c, d Cyclic symmetry multi-point constraints are not supported in Abaqus/CAE. Using MPC type ELBOW MPC type ELBOW constrains two nodes of ELBOW31 or ELBOW32 elements together, where the cross-sectional direction, , changes . This MPC type is available only in Abaqus/Standard. a2(0,1,0) a2(0,0,1) Figure 34.2.2–10 ELBOW type MPC. Input data Give the nodes a and b as shown in Figure 34.2.2–10. Input File Usage: Abaqus/CAE Usage: *MPC ELBOW, a, b Use one of the following options: Interaction module: Create Connector Section: select MPC as the Connection Category and Elbow as the MPC Type Interaction module: Create Constraint: MPC Constraint; select Elbow as the MPC Type Using MPC type LINK MPC type LINK provides a pinned rigid link between two nodes to keep the distance between the nodes constant, as shown in Figure 34.2.2–11. The displacements of the first node are modified to enforce this constraint. The rotations at the nodes, if they exist, are not involved in this constraint. Figure 34.2.2–11 MPC type LINK. Input data Give the nodes a and b as shown in Figure 34.2.2–11. Input File Usage: Abaqus/CAE Usage: *MPC LINK, a, b Use one of the following options: Interaction module: Create Connector Section: select MPC as the Connection Category and Link as the MPC Type Interaction module: Create Constraint: MPC Constraint; select Link as the MPC Type Using MPC type PIN MPC type PIN provides a pinned joint between two nodes. This MPC makes the global displacements equal but leaves the rotations, if they exist, independent of each other, as shown in Figure 34.2.2–12. u a = u b u a = u b u a = u b φ a ≠ φ b φ a ≠ φ b φ a ≠ φ b ub φb ub φb ua φa ua φa φb ub Figure 34.2.2–12 MPC type PIN. φa ua Input data Give the nodes a and b as shown in Figure 34.2.2–12. Input File Usage: Abaqus/CAE Usage: *MPC PIN, a, b Use one of the following options: Interaction module: Create Connector Section: select MPC as the Connection Category and Pin as the MPC Type Interaction module: Create Constraint: MPC Constraint; select Pin as the MPC Type Using MPC type REVOLUTE This MPC type is available only in Abaqus/Standard. A revolute joint is a joint in which relative rotation is allowed between two nodes about an axis that rotates during the motion . The axis of the joint is defined in the initial configuration as the line from node b to node c. If these nodes are coincident, the axis is assumed to be the global z-axis. The rotation of the joint axis is that of node b. The relative rotation in the joint is a single variable and is stored as degree of freedom 6 at node c. This degree of freedom can be used with other members in the model, but caution should be used because of the nonstandard use of degree of freedom 6. For example, a SPRING1 element (a spring to ground) might be attached to this degree of freedom. Since the degree of freedom measures a relative rotation, this spring would then be a torsional spring between nodes a and b. The displacements at node a are not constrained by the REVOLUTE MPC to be the same as the displacements at node b. Thus, the joint definition must usually be completed either by using a PIN type MPC between nodes a and b or by using suitable stiffness members between these two nodes. An example of a revolute joint and application of the REVOLUTE MPC is provided in “Revolute MPC verification: rotation of a crank,” Section 1.3.8 of the Abaqus Benchmarks Manual. See “Revolute joint,” Section 6.6.3 of the Abaqus Theory Manual, for more details on revolute joints. Figure 34.2.2–13 Revolute joint. Input data Give the nodes a, b, and c as shown in Figure 34.2.2–13. Degree of freedom 6 at node c defines the relative rotation between nodes a and b; therefore, this degree of freedom does not obey the standard convention for degrees of freedom in Abaqus. Input File Usage: Abaqus/CAE Usage: *MPC REVOLUTE, a, b, c Revolute joint multi-point constraints are not supported in Abaqus/CAE. Using MPC type SLIDER MPC type SLIDER keeps a node on a straight line defined by two other nodes but allows the possibility of moving along the line and allows the line to change length. When transitioning from multiple layers of solid elements to shells, it is often desirable to constrain the nodes on the free edge of the solid elements to remain in a straight line. (This constraint is consistent with shell theory.) The SLIDER MPC can perform this function without restraining the “thinning” behavior of the solid layers. The SS LINEAR MPC is then used to attach the shell element to this edge. In Abaqus/Standard when a SLIDER MPC is used with one of the shell-solid MPCs—SS LINEAR, SS BILINEAR, or SSF BILINEAR—it must be given following the shell-solid MPCs. Input data For each node p shown in Figure 34.2.2–14 and Figure 34.2.2–15, give the nodes p, a, and b for each line of nodes that should remain straight. For each node q shown in Figure 34.2.2–14, give the nodes q, c, and d, and so on for each line of nodes that should remain straight. Input File Usage: Abaqus/CAE Usage: *MPC SLIDER, p, a, b SLIDER, q, c, d Slider multi-point constraints are not supported in Abaqus/CAE. edge node line Solid elements (8-node) edge node line p5 p4 p3 p2 p1 q2 q1 Solid elements (20-node) midside node line Figure 34.2.2–14 SLIDER type MPC used at a shell-solid intersection. a, b are nodes on the outer pipe p1, p2 are nodes on the inner pipe p2 p1 Figure 34.2.2–15 SLIDER type MPC used to model a telescoping beam. Using MPC type TIE MPC type TIE makes the global displacements and rotations as well as all other active degrees of freedom equal at two nodes. If there are different degrees of freedom active at the two nodes, only those in common will be constrained. MPC type TIE is usually used to join two parts of a mesh when corresponding nodes on the two parts are to be fully connected (“zipping up” a mesh). For example, when a mesh is generated on a cylindrical body, the solution at the nodes at 0° and those at 360° must be the same. This can be done either by renumbering the nodes on one of the mesh extremes or by using this MPC for each pair of corresponding nodes, as shown in Figure 34.2.2–16. a1 b1 a2 b2 a3 b3 Figure 34.2.2–16 Example of use of TIE MPC. Input data Give the nodes a and b as shown in Figure 34.2.2–16. Input File Usage: Abaqus/CAE Usage: *MPC TIE, a, b Use one of the following options: Interaction module: Create Connector Section: select MPC as the Connection Category and Tie as the MPC Type Interaction module: Create Constraint: MPC Constraint; select Tie as the MPC Type Using MPC type UNIVERSAL This MPC type is available only in Abaqus/Standard. A universal joint is a joint in which relative rotation is allowed between two nodes, about two axes that are connected rigidly, and each of which rotates with the rotation of one end of the joint . Such a joint might be used to couple two shafts that have an angular misalignment. The first axis of the joint, which is attached to node b, is defined in the initial configuration as the line from node b to node c. If these nodes are coincident, the axis is assumed to be the global z-axis. The second axis of the joint is at right angles to the first axis and is in the plane defined by the first axis and node d. The relative rotations in the joint are stored as degree of freedom 6 at the nodes c and d. These degrees of freedom can be used with other members in the model, but caution should be used because of the nonstandard use of degree of freedom 6. For example, a SPRING1 element (a spring to ground) might be attached to one of these degrees of freedom. Since the degree of freedom measures a relative rotation, this spring would then be a torsional spring, restraining that component of relative rotation. The displacements at node a are not constrained by the UNIVERSAL MPC to be the same as the displacements at node b. Thus, the joint definition must usually be completed either by using a PIN type MPC between nodes a and b or by using suitable stiffness members between these two nodes. See “Universal joint,” Section 6.6.4 of the Abaqus Theory Manual, for more details on universal joints. Figure 34.2.2–17 Universal joint. Input data Give the nodes a, b, c, and d as shown in Figure 34.2.2–17. Degrees of freedom 6 at nodes c and d define the relative rotation in the joint; therefore, these degrees of freedom do not obey the standard convention for degrees of freedom in Abaqus. Input File Usage: Abaqus/CAE Usage: *MPC UNIVERSAL, a, b, c, d Universal joint multi-point constraints are not supported in Abaqus/CAE. Using MPC type V LOCAL This MPC type is available only in Abaqus/Standard. As shown in Figure 34.2.2–18, MPC type V LOCAL constrains the velocity components associated with degrees of freedom 1, 2, and 3 at a first node (a) to be equal to the velocity components at a third node (c) along local, rotating directions. These local directions rotate according to the rotation at a second node (b). In the initial configuration the first local direction is from the second to the third node of the MPC (from b to c, as indicated by the arrows in Figure 34.2.2–18), or it is the global z-axis if these nodes coincide. The other local directions are then defined by the standard Abaqus convention for such directions . In Figure 34.2.2–18 this MPC is applied to nodes d, e, and f in the same manner. MPC type V LOCAL can be useful for defining a complex motion within a model. For example, the MPC can be used to model the steering of an automobile in a dynamic analysis for which the resulting inertial effects are of interest. See “Local velocity constraint,” Section 6.6.5 of the Abaqus Theory Manual, for more details on the local velocity constraint. a,b d,e Figure 34.2.2–18 Local velocity constraint. Input data Give the node whose velocity components are constrained (node a or d in Figure 34.2.2–18), the node whose rotation defines the rotation of the local directions (node b or e in Figure 34.2.2–18), and the node whose velocity components are in these local directions (node c or f in Figure 34.2.2–18). Nodes a and b (or d and e) can be the same. *MPC V LOCAL, a, b, c V LOCAL, d, e, f Local velocity component multi-point constraints are not supported in Abaqus/CAE. Abaqus/CAE Usage: Input File Usage: MPCs for transitions SS LINEAR SS BILINEAR(S) SSF BILINEAR(S) Constrain a shell node to a solid node line for linear elements (S4, S4R, S4R5, C3D8, C3D8R, SAX1, CAX4, etc.). Constrain a shell node to a solid node line for edge lines on quadratic elements (S8R, S8R5, C3D20, C3D20R, SAX2, CAX8, etc.). Constrain a midside node of a quadratic shell element (S8R, S8R5) to midface lines on 20-node bricks (C3D20, C3D20R, etc.). Modeling a shell-to-solid element transition The SLIDER, SS LINEAR, SS BILINEAR, and SSF BILINEAR MPCs allow for a transition from shell element modeling to solid element modeling on a shell surface. This modeling technique can be used to obtain solutions at shell-solid intersections or other discontinuities, where the local modeling should use full three-dimensional theory but the other parts of the structure can be modeled as shells. The shell- to-solid submodeling capability (“Submodeling: overview,” Section 10.2.1) and the surface-based shell- to-solid coupling constraint (“Shell-to-solid coupling,” Section 34.3.3) can also be used to obtain more accurate solutions in such cases, with considerably less modeling effort. , , …, b in Figure 34.2.2–14 and lines In Abaqus/Standard the MPC usage assumes that the interface between the shell and solid elements is a surface containing the normals to the shell along the line of intersection of the meshes, so that the lines of nodes on the solid mesh side of the interface in the normal direction to the surface are straight lines. (Line a, in Figure 34.2.2–19 to Figure 34.2.2–20 , should be straight lines.) It also assumes that the nodes of the solid elements are spaced uniformly on the interface surface as indicated in Figure 34.2.2–14 and Figure 34.2.2–19 to Figure 34.2.2–20. For each shell node on the edge use MPC type SS LINEAR, SS BILINEAR, or SSF BILINEAR, as appropriate, to constrain the shell node to the corresponding line or face of solid element nodes through the thickness. Then, use a SLIDER MPC to constrain each interior node on the line through the thickness to remain on the straight line defined by the bottom and top nodes of that line. For an example, see “*MPC,” Section 5.1.17 of the Abaqus Verification Manual. , …, The SS BILINEAR and SSF BILINEAR MPCs are not intended for use with the variable node solid elements (C3D27, C3D27H, C3D27R, and C3D27RH). In Abaqus/Standard MPCs SS LINEAR, SS BILINEAR, and SSF BILINEAR eliminate all displacement components and two of the rotation components at the shell node, and the SLIDER MPC eliminates two displacement components at each interior solid element node in the interface. Therefore, any boundary conditions needed at the interface (such as those required when the shell/solid interface intersects a symmetry plane) should be applied only to the top and bottom nodes on the solid element side of the interface. Using MPC type SS LINEAR MPC type SS LINEAR constrains a shell corner node to a line of edge nodes on solid elements for linear elements (S4, S4R, or S4R5; C3D8, C3D8R; SAX1; CAX4; etc.). The constrained nodes need not lie exactly on these lines, but it is suggested that they be in close proximity to the lines for meaningful results. pn p2 p1 Figure 34.2.2–19 SS LINEAR type MPC. 4-node shells to 8-node bricks. Input data Give the shell node, S, then the list of nodes along the corresponding line through the thickness in the solid element mesh. In Abaqus/Explicit only two solid nodes can be given. Referring to Figure 34.2.2–19, in Abaqus/Standard give S, . The shell , …, node number must be different from the solid mesh node numbers. , and in Abaqus/Explicit give S, , where , , Input File Usage: In Abaqus/Standard use the following option: *MPC SS LINEAR, S, , , …, In Abaqus/Explicit use the following option: *MPC SS LINEAR, S, , Abaqus/CAE Usage: Multi-point constraints for transitions are not supported in Abaqus/CAE. Using MPC type SS BILINEAR MPC type SS BILINEAR constrains a corner node of a quadratic shell element (S8R, S8R5) to a line of edge nodes on 20-node bricks. This MPC type is available only in Abaqus/Standard. The constrained node need not lie exactly on the line, but it is suggested that it be in close proximity to the line for meaningful results. pn p4 p3 p2 p1 Figure 34.2.2–20 SS BILINEAR type MPC. Corner of 8-node shell to edge of 20-node bricks. Input data Give the shell node, S, then the list of nodes along the corresponding line through the thickness in the solid element mesh. Referring to Figure 34.2.2–20, give S, . The shell node number must be different from the solid mesh node numbers. ,…, , Input File Usage: *MPC SS BILINEAR, S, , , …, Abaqus/CAE Usage: Multi-point constraints for transitions are not supported in Abaqus/CAE. Using MPC type SSF BILINEAR MPC type SSF BILINEAR constrains a midside node on a quadratic shell element (S8R, S8R5) to a line of midface nodes on solid 20-node bricks. This MPC type is available only in Abaqus/Standard. The constrained node need not lie exactly on the line, but it is suggested that it be in close proximity to the line for meaningful results. pn-2 p6 p4 p1 pn-1 p7 p2 pn p8 p5 p3 Figure 34.2.2–21 SSF BILINEAR type MPC. Midside of 8-node shell to surface of 20-node bricks. Input data Give the shell node, S, then the list of nodes on the solid face, in the order Figure 34.2.2–21. , ,…, as shown in Input File Usage: *MPC SSF BILINEAR, S, , , …, Abaqus/CAE Usage: Multi-point constraints for transitions are not supported in Abaqus/CAE. 34.2.3 KINEMATIC COUPLING CONSTRAINTS Product: Abaqus/Standard References • “Kinematic constraints: overview,” Section 34.1.1 • *KINEMATIC COUPLING Overview Kinematic coupling constraints: • limit the motion of a group of nodes to the rigid body motion defined by a reference node; • can be applied only to specific user-specified degrees of freedom at the constrained nodes; • can be specified with respect to local coordinate systems at the constrained nodes; and • can be used in geometrically linear or nonlinear analysis. The preferred method of providing a kinematic constraint of this type is described in “Coupling constraints,” Section 34.3.2. Typical applications The kinematic coupling constraints are useful in cases where a large number of nodes (the “coupling” nodes) are constrained to the rigid body motion of a single node and the degrees of freedom that participate in the constraint are selected individually in a local coordinate system. In many such cases MPCs either are not available or would have to be prescribed individually for each constrained node. A typical example is shown in Figure 34.2.3–1, where a kinematic coupling constraint is used to prescribe a twisting motion to a model without constraining radial motions. In other applications the kinematic coupling constraint can be used to provide coupling between continuum and structural elements. Defining the constraint A kinematic coupling constraint requires the specification of a reference node, coupling nodes, and the constrained degrees of freedom at these nodes. The reference node has both translational and rotational degrees of freedom. Kinematic constraints are imposed by eliminating degrees of freedom at the coupling nodes. Once any combination of displacement degrees of freedom at a coupling node is constrained, additional displacement constraints—such as MPCs, boundary conditions, or other kinematic coupling definitions—cannot be applied to any coupling node involved in a kinematic coupling constraint. The same limitation applies for rotational degrees of freedom. Input File Usage: To constrain all available degrees of freedom: *KINEMATIC COUPLING, REF NODE=node coupling node number or node set reference node (node 500) constrained nodes that are free to translate radially (COUPLESET) axis of cylindrical coordinate system (COUPLEAXIS) Figure 34.2.3–1 A kinematic coupling constraint used to transmit rotation to a structure while permitting radial motion. To constrain a single degree of freedom: *KINEMATIC COUPLING, REF NODE=node coupling node number or node set, dof To constrain a range of degrees of freedom: *KINEMATIC COUPLING, REF NODE=node coupling node number or node set, first dof, last dof To specify non-contiguous lists of constrained degrees of freedom, repeat the node numbers or node sets on subsequent data lines. For example, the following input is used to constrain degrees of freedom 1, 2, 3, and 6 at node 10 to the motion of reference node 5: *KINEMATIC COUPLING, REF NODE=5 10, 1, 3 10, 6 Translational degrees of freedom Translational degrees of freedom are constrained by eliminating the specified degrees of freedom at the coupling nodes. When all translational degrees of freedom are specified, the coupling nodes follow the rigid body motion of the reference node. Rotational degrees of freedom All combinations of selected rotational degrees of freedom result in rotational behavior that is identical to existing MPC types. Specifically: • Selection of three rotational degrees of freedom along with three displacement degrees of freedom is equivalent to MPC type BEAM. • Selection of two rotational degrees of freedom is equivalent to MPC type REVOLUTE. • Selection of one rotational degree of freedom is equivalent to MPC type UNIVERSAL. Internal nodes are created by the kinematic coupling to enforce the constraints that are equivalent to MPC types REVOLUTE and UNIVERSAL. These nodes have the same degrees of freedom as the additional nodes used in these MPC types and are included in the residual check for nonlinear analysis. Specifying a local coordinate system The constrained degrees of freedom at the coupling nodes can be specified in a local coordinate system instead of the (default) global coordinate system . Figure 34.2.3–1 illustrates the use of a local coordinate system definition with a kinematic coupling constraint to constrain all but the radial translation of a group of nodes to a reference node. In this example a local cylindrical coordinate system is defined that has its axis coincident with the structure’s axis. The coupling node constraints are then specified in this local coordinate system. In this example the constrained nodes are attached to continuum elements; thus, only translational degrees of freedom need to be specified. *KINEMATIC COUPLING, REF NODE=node, ORIENTATION=name For example, the following input is used to specify the kinematic coupling constraint shown in Figure 34.2.3–1: Input File Usage: *ORIENTATION, SYSTEM=CYLINDRICAL, NAME=COUPLEAXIS 0.0, -1.0, 0.0, 0.0, 1.0, 0.0 *KINEMATIC COUPLING, REF NODE=500, ORIENTATION=COUPLEAXIS COUPLESET, 2, 3 Constraint directions and finite rotations In geometrically nonlinear analysis steps, the coordinate system in which the constrained degrees of freedom are specified will rotate with the reference node regardless of whether the constrained degrees of freedom are specified in the global coordinate system or in a local system. Thus, the constraint shown in Figure 34.2.3–1 will enable free radial motion throughout arbitrary rotations of the structure. Radial motion in this case is defined as motion normal to the structure’s axis (defined in the undeformed configuration by points a and b in the figure), with this axis rotating with the reference node. Therefore, the free radial expansion shown in Figure 34.2.3–1 will not refer to an axis parallel to the global y-axis for general rotations of the reference node but will refer to an axis that rotates with the structure. Rotation of the constraint directions is not affected by the selection of the constrained degrees of freedom. 34.3 Surface-based constraints • “Mesh tie constraints,” Section 34.3.1 • “Coupling constraints,” Section 34.3.2 • “Shell-to-solid coupling,” Section 34.3.3 • “Mesh-independent fasteners,” Section 34.3.4 34.3.1 MESH TIE CONSTRAINTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Surfaces: overview,” Section 2.3.1 • *TIE • “Defining tie constraints,” Section 15.15.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Using contact and constraint detection,” Section 15.16 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A surface-based tie constraint: • ties two surfaces together for the duration of a simulation; • can be used only with surface-based constraint definitions; • can be used in mechanical, coupled temperature-displacement, coupled thermal-electrical- pore pressure-displacement, coupled structural, pressure–displacement, coupled thermal-electrical, or heat transfer simulations; pressure, acoustic acoustic coupled • can also be used to create a constraint on a surface so that it follows the motion of a three-dimensional beam; • is useful for mesh refinement purposes, especially for three-dimensional problems; • allows for rapid transitions in mesh density within the model; • constrains each of the nodes on the slave surface to have the same motion and the same value of temperature, pore pressure, acoustic pressure, or electrical potential as the point on the master surface to which it is closest; • will take the initial thickness and offset of shell elements underlying the surface into account by default; and • eliminates the degrees of freedom of the slave surface nodes that are constrained, where possible. Defining a tie constraint for a pair of surfaces A surface-based tie constraint can be used to make the translational and rotational motion as well as all other active degrees of freedom equal for a pair of surfaces. By default, as discussed below, nodes are tied only where the surfaces are close to one another. One surface in the constraint is designated to be the slave surface; the other surface is the master surface. A name must be assigned to this constraint and may be used in postprocessing with Abaqus/CAE. Input File Usage: *TIE, NAME=name slave_surface_name, master_surface_name Abaqus/CAE Usage: Interaction module: Create Constraint: Tie Defining the surfaces to be constrained Either element-based or node-based surfaces can be used as the slave surface. Any surface type (element- based, node-based, or analytical) can be used as the master surface. You may need to take some surface restrictions into consideration depending on which tie formulation is used and whether the analysis is conducted in Abaqus/Standard or Abaqus/Explicit. Two tie formulations are available: the surface-to- surface formulation, which is used by default in Abaqus/Standard, and the more traditional node-to- surface formulation, which is used by default in Abaqus/Explicit; these formulations are discussed in more detail later in this section. Table 34.3.1–1 and Table 34.3.1–2 provide comparisons of surface restrictions for the different formulations and analysis codes. Table 34.3.1–1 Comparison of characteristics for surface-based tie formulations. Tie formulation Optimized stress accuracy Node-based surfaces allowed Surface-to-surface (Abaqus/Standard or Abaqus/Explicit) Node-to-surface in Abaqus/Standard Node-to-surface in Abaqus/Explicit Yes No No Reverts to node- to-surface formulation Yes Yes Mixture of rigid and deformable subregions allowed Treatment of nodes/facets shared between master and slave surfaces No No Yes Eliminated from slave Eliminated from slave Eliminated from master The surface-to-surface formulation generally avoids stress noise at tied interfaces. As indicated in Table 34.3.1–1 and Table 34.3.1–2, only a few surface restrictions apply to the surface-to-surface formulation: this formulation reverts to the node-to-surface formulation if a node-based or edge-based surface is used. The surface-to-surface formulation does not allow for a mixture of rigid and deformable portions of a surface, and the master surface must not contain T-intersections. Any nodes shared between the slave and master surfaces will not be tied with the surface-to-surface formulation. The same comments apply to both Abaqus/Standard and Abaqus/Explicit in these tables for the surface-to-surface formulation. With the more traditional node-to-surface formulation additional surface restrictions apply in Abaqus/Standard but fewer restrictions apply in Abaqus/Explicit in comparison to the surface-to-surface Table 34.3.1–2 Comparison of element-based surface characteristics allowed for surface-based tie formulations. Surface Characteristics (Yes=allowed, No=not allowed) Double-sided Discontinuous T-intersection Edge-based Tie formulation Surface-to-surface (Abaqus/Standard or Abaqus/Explicit) Master: Yes Slave: Yes Master: Yes Slave: Yes Master: No Slave: Yes Node-to-surface in Abaqus/Standard Node-to-surface in Abaqus/Explicit Master: Yes Slave: Yes Master: Yes Slave: Yes Master: Yes Slave: Yes Master: Yes Slave: Yes Master: No Slave: Yes Master: Yes Slave: Yes Reverts to node-to-surface formulation if either surface is edge-based Master: Yes Slave: Yes Master: Yes Slave: Yes formulation. Relatively stringent restrictions on master surface connectivity for the node-to-surface tie formulation in Abaqus/Standard are indicated in Table 34.3.1–2: the master surface must be simply connected and must not contain complex intersections such as T-intersections . Differences with the node-to-surface formulation in Abaqus/Explicit are apparent in Table 34.3.1–1: partially rigid surfaces can be used and the treatment of shared portions of slave and master surfaces is unique to this case. Nodes and faces that are shared between the master and slave surfaces are eliminated automatically from the master surface in this case if the paired surfaces are either both element-based or both node-based, enabling the possibility of tying multiple slave surfaces (defined over various regions of the model) to a common master surface defined over the entire model. This is a convenient way to define tie constraints in large models, as it eliminates the need for defining specialized master surfaces for each surface pairing; however, you must still take care that slave surfaces do not include portions of the opposing surface to which they should be tied (for example, no tie constraints will be generated if the master and slave surfaces are identical). In the node-to-surface formulation in Abaqus/Explicit all facets attached to nodes that are common between slave and master surfaces are excluded from being tied to slave nodes. Sometimes when meshes are transitioned from one type of element to another type or from one element size to another element size, common nodes may exist at the interface of the two regions. Typically, a tie constraint is defined at the interface of the two zones to stitch the two meshes together. In a situation like this common nodes may get tied to a neighboring facet on the interface and may cause undesirable mesh distortion due to the tie adjustment. One possible way to avoid the undesirable mesh distortion is to specify a very small position tolerance for the tie pair. Another situation that may arise when common nodes occur between the slave and master surfaces at the interface of mesh transition zones is that slave nodes in the vicinity of the common node may not get tied. This happens due to the exclusion of master facets attached to the common nodes. Therefore, care must be taken to ensure that elements in different mesh zones do not share common nodes at the interface. For all such common nodes, duplicate nodes occupying the same physical location should be defined. Input File Usage: Use the *SURFACE option to define the slave and master surfaces used in the constraint : Abaqus/CAE Usage: *SURFACE, NAME=slave_surface_name *SURFACE, NAME=master_surface_name In Abaqus/CAE you can select one or more faces directly in the viewport when you are prompted to select a surface. In addition, you can define surfaces as collections of faces and edges using the Surface toolset. Specifying the subset of slave nodes to be constrained By default, Abaqus uses a position tolerance criterion to determine the constrained nodes based on the distance between the slave nodes and the master surface. Alternatively, you can specify a node set containing the slave nodes to be constrained regardless of their distance to the master surface. Using the position tolerance criterion The default position tolerance criterion ensures that nodes are tied only where the slave and master surfaces are close to one another in the initial configuration. For example, consider the case shown in Figure 34.3.1–1. Surfaces Comp1_surf and Comp2_surf are defined to cover all exposed faces of Component 1 and Component 2, respectively. These two surfaces can be used as the slave and master surfaces in a tie constraint to tie the two components in the desired region, because only the nodes at the initial interface between the two surfaces are tied. desired tie region Component 1 Component 2 Figure 34.3.1–1 Example of two components to be tied together. The default value of the position tolerance, , typically results in desired tie constraints with little effort. Details regarding the calculation of distances between surfaces and default values of the position tolerances are provided below. You can modify the position tolerance if desired. Input File Usage: Abaqus/CAE Usage: Use the following option to use the default position tolerance: *TIE Use the following option to specify a position tolerance: *TIE, POSITION TOLERANCE=distance Interaction module: Create Constraint: Tie: Position Tolerance: Specify distance Calculating the distance between surfaces The following factors influence the calculation of the distance between surfaces for a particular slave node: • Shell thickness. By default, calculations of distances between surfaces account for shell thickness and offset effects for element-based slave or master surfaces: the distance is measured from the actual top or bottom side of the surface, whichever is closer to the other surface. Alternatively, you can specify that surface thicknesses and offsets should be ignored, which also has implications for nodal position adjustments for resolving initial gaps (discussed later). Input File Usage: Use the following option to ignore surface thicknesses and offsets in the distance calculations: Abaqus/CAE Usage: *TIE, NO THICKNESS Interaction module: Create Constraint: Tie: Exclude shell element thickness • Whether the surface-to-surface or node-to-surface constraint formulation (discussed below) is used. If a position tolerance is in effect, a constraint is generated at a slave node for either formulation if the distance between the surfaces, as calculated at the slave node, does not exceed . Additional slave nodes may be tied if the surface-to-surface constraint formulation is used along with an element- based slave surface and a master surface that is not node-based, because the following addendum to the position tolerance criterion applies in such cases: if the distance between the surfaces is within over a significant portion of a slave face (or segment in two dimensions) that forms an angle of less than 30° with the master surface, all slave nodes attached to such a face (or segment) are considered to satisfy the position tolerance. • The types of surfaces involved (element-based, node-based, or analytical). Position tolerance for an element-based master surface The default position tolerance for element-based master surfaces is 5% or 10% of the typical master facet diagonal length for the node-to-surface and surface-to-surface tie formulations, respectively. When using an element-based master surface, the distance between surfaces for a particular point on a slave surface is based on the closest point on the master surface (which may be on the edge of the master surface or within a facet). Figure 34.3.1–2 shows an example with no thickness: nodes 2–14 satisfy the position tolerance criterion for the node-to-surface and surface-to-surface constraint formulations. Significant portions of the end slave segments (that is, the segment connecting nodes 1 and 2 and the slave surface 15 14 13 10 11 12 element-based master surface position tolerance Figure 34.3.1–2 Tolerance region around an element-based master surface with no thickness. segment connecting nodes 14 and 15) are within the position tolerance shown, so nodes 1 and 15 would also satisfy the position tolerance criterion for the surface-to-surface constraint formulation except for the fact that the angle between the slave and master surfaces is slightly greater than 30° at those locations. Position tolerance for a node-based master surface The default position tolerance for a node-based master surface is based on the average distance between nodes in the master surface. The distance between the surfaces for a particular slave node is based on If this distance is less than the position tolerance, Abaqus will create a tie the closest master node. constraint between the slave node, the closest master node, and other master nodes in similar proximity to the slave node. For mismatched meshes across a tied interface, the distance between slave and master nodes can be much larger than the “normal” distance between the surfaces, which can lead to confusion when using a position tolerance criterion with a node-based master surface. Figure 34.3.1–3 shows how the tolerance region is defined around a node-based master surface. The surface-to-surface constraint formulation reverts to the node-to-surface constraint formulation for a node-based master surface. slave surface 10 11 12 position tolerance 15 14 13 node-based master surface Figure 34.3.1–3 Tolerance region around a node-based master surface with no thickness. Position tolerance for an analytical rigid master surface The default position tolerance for tie constraints between an element-based slave surface and an analytical rigid master surface is 5% or 10% of the typical slave facet diagonal length for the node-to-surface and surface-to-surface tied formulations, respectively. The default position tolerance for tie constraints between a node-based slave surface and an analytical rigid master surface is 5% of the typical distance between slave nodes. When using an analytical rigid master surface, the distance between surfaces for a particular point on the slave surface is based on the closest point on the master surface. Specifying the constrained nodes directly This method allows you direct control over which slave nodes are tied. Input File Usage: Abaqus/CAE Usage: *TIE, TIED NSET=node_set_label Specifying the constrained nodes directly is not supported in Abaqus/CAE. Unconstrained nodes in tie constraint pairs Abaqus does not constrain slave nodes to the master surface unless they are included in the tied node set or within the tolerance distance from the master surface at the start of the analysis, as discussed above. Any slave nodes not satisfying these criteria will remain unconstrained for the duration of the simulation; they will never interact with the master surface as part of the tie constraint. In mechanical simulations an unconstrained slave node can penetrate the master surface freely unless contact is defined between the slave node and master surface. The general contact algorithm in Abaqus/Explicit will generate contact exclusions automatically for slave node–master surface combinations corresponding to constrained nodes of tie constraint pairs, but no such contact exclusions are generated for nodes outside the position tolerance of the constraints. In a thermal, acoustic, electrical, or pore pressure simulation an unconstrained slave node will not exchange heat, fluid pressure, electrical current, or pore fluid pressure with the master surface. Determining which slave nodes have been tied and which slave nodes have not been tied For each tie constraint pair, Abaqus creates a node set comprising slave nodes that will be tied and a node set comprising slave nodes that will be left unconstrained. These node sets are available for display during postprocessing in Abaqus/CAE, where they are listed as internal node sets. In addition, Abaqus prints a table in the data (.dat) file listing each slave node and the master surface nodes to which it will be tied if model definition data are requested . If a constraint cannot be formed for a given slave node, Abaqus/Standard issues a warning message in the data file. In Abaqus/Explicit you can also request two nodal field output variables: TIEDSTATUS will help you identify the constrained and unconstrained slave nodes, and TIEADJUST will help you visualize the adjustment performed at the nodes . A tied node that participates in more than one tie definition as a slave as well as a master is shown as “tied” regardless of whether it got tied as a slave node or as a master node. When creating a model with surface-based tie constraints, it is important to use the information provided by Abaqus to identify any unconstrained nodes and to make any necessary modifications to the model to constrain them. Constraining the rotational degrees of freedom By default, Abaqus will constrain the rotational degrees of freedom when they exist on both slave and master surfaces . You can specify that the rotational degrees of freedom should not be tied. Input File Usage: Abaqus/CAE Usage: *TIE, NO ROTATION Interaction module: Create Constraint: Tie: toggle off Tie rotational DOFs if applicable Constraining the faces of a cyclic symmetric structure in Abaqus/Standard You can enforce proper constraints on the faces bounding a repetitive sector of a cyclic symmetric structure . This makes it possible to define a single sector of the cyclic symmetry model together with its axis of cyclic symmetry to define the behavior of the 360° model. Cyclic symmetry models can be used within the following procedures: static; quasi-static; eigenfrequency extraction, based on the Lanczos solver technique; steady-state dynamics, based on modal superposition; and heat transfer. If an eigenfrequency extraction is performed on a cyclic symmetric model, the nodes involved in the cyclic symmetry constraint cannot be used in any other constraint (e.g., multi-point constraints, equations, rigid bodies, couplings, or kinematic couplings). Input File Usage: *TIE, CYCLIC SYMMETRY This parameter can be used only with the *CYCLIC SYMMETRY MODEL option. Abaqus/CAE Usage: Interaction module: Interaction→Create: Cyclic symmetry The surface-based tie constraint formulation Abaqus uses the criteria discussed above to determine which slave nodes will be tied to the master surface. Abaqus then forms constraints between these slave nodes and the nodes on the master surface. A key aspect in forming the constraint for each slave node is determining the tie coefficients. These coefficients are used to interpolate quantities from the master nodes to the tie point. Abaqus can use one of two approaches to generate the coefficients: the “surface-to-surface” approach or the “node-to-surface” approach. If an analysis carried out with Abaqus/Standard is imported into Abaqus/Explicit or vice-versa, the tie constraints are not imported and must be redefined. If the imported analysis is essentially a continuation of the original analysis, it is important that the tie constraints are as similar as possible. Hence, you should make sure that the same constraint type is used. If the default approach was used in the original Abaqus/Standard analysis, the surface-to-surface approach should be specified in the Abaqus/Explicit analysis. Similarly, if the default approach was used in the original Abaqus/Explicit analysis, the node-to-surface approach should be specified in the Abaqus/Standard analysis. slave surface defined on shell structure master surface defined on shell structure slave surface defined on shell structure Displacement and rotation degrees of freedom are tied, unless you specify that the rotation degrees of freedom should not be tied. master surface defined on shell structure Displacement and rotation degrees of freedom are tied, unless you specify that the rotation degrees of freedom should not be tied. slave surface defined on shell structure master surface defined on solid structure Only displacement degrees of freedom are tied. Figure 34.3.1–4 Surface-based tie algorithm. The “surface-to-surface” approach The “surface-to-surface” approach minimizes numerical noise for tied interfaces involving mismatched meshes. The surface-to-surface approach enforces constraints in an average sense over a finite region, rather at discrete points as in the traditional node-to-surface approach. The surface-to-surface formulation for surface-based tie constraints is similar to the surface-to-surface contact formulation ; however, a fundamental difference is that each surface-based tie constraint involves only one slave node (and multiple master nodes), whereas each surface-to-surface contact constraint involves multiple slave nodes. The surface-to-surface approach is used by default in Abaqus/Standard with exceptions noted below, and it is optional in Abaqus/Explicit. For the case of infinite acoustic elements tied to shell elements in Abaqus/Standard the added cost of the surface-to-surface approach can be quite significant; therefore, the node-to-surface approach is used by default in this case. If the surface-to-surface approach is “on by default” or explicitly specified, Abaqus automatically reverts to the node-to-surface approach for individual tie constraints in the following circumstances: • if either of the surfaces being tied is node-based; • if the projection along the slave surface normal direction does not intersect the master surface; or • if single-sided slave and master surfaces have surface normals in approximately the same direction. Abaqus/Explicit may automatically add a small amount of artificial mass to the model to maintain numerical stability if the surface-to-surface approach is specified. The surface-to-surface approach generally involves more master nodes per constraint than the node- to-surface approach, which tends to increase the solver bandwidth in Abaqus/Standard and, therefore, can increase solution cost. In most applications the extra cost is fairly small, but the cost can become significant in some cases. The following factors (especially in combination) can lead to the surface-to- surface approach being quite costly: • A large fraction of tied nodes (degrees of freedom) in the model • The master surface being more refined than the slave surface • Multiple layers of tied shells, such that the master surface of one tie constraint acts as the slave surface of another tie constraint Input File Usage: Abaqus/CAE Usage: *TIE, TYPE=SURFACE TO SURFACE Interaction module: Create Constraint: Tie: Discretization method: Surface to surface The “node-to-surface” approach The traditional “node-to-surface” approach (which is used by default in Abaqus/Explicit and is optional in Abaqus/Standard) sets the coefficients equal to the interpolation functions at the point where the slave node projects onto the master surface. This approach is somewhat more efficient and robust for complex surfaces. For the node-to-surface method of establishing the tie coefficients with an element-based master surface, the point on the surface closest to each slave node is calculated and used to determine the master nodes that are going to form the constraint . For example, nodes 202, 203, 302, and 303 are used to constrain node a; nodes 204 and 304 are used to constrain node b; and node 402 is used to constrain node c. Input File Usage: Abaqus/CAE Usage: *TIE, TYPE=NODE TO SURFACE Interaction module: Create Constraint: Tie: Discretization method: Node to surface 103 104 203 102 202 302 101 201 301 slave surface nodes 204 303 304 403 404 503 504 502 402 401 501 Figure 34.3.1–5 Searching for the points on an element-based master surface that are closest to nodes a, b, and c. Choosing the slave and master surfaces of a surface-based tie constraint The choice of slave and master surfaces can have a significant effect on the accuracy of the solution, in particular if the “node-to-surface” approach is used. The effect is much less (and the accuracy generally better) for the “surface-to-surface” approach. In either case, if both surfaces in a constraint pair are deformable surfaces, the master surface should be chosen as the surface with the coarser mesh for best accuracy. In Abaqus/Standard a rigid surface cannot act as a slave surface in a tie constraint. To comply with this rule, the capability to automatically resolve overconstraints in Abaqus/Standard will modify tie constraint definitions in the following cases: • Tie constraints between two surfaces of the same rigid body are removed. • Tie constraints between two surfaces of two rigid bodies are replaced by a BEAM-type connector between the respective rigid body reference nodes. • Tie constraints specified with a purely rigid slave surface and a purely deformable master surface are modified to reverse the master and slave assignments unless this is not possible due to other modeling restrictions (in which case an error message is issued). These methods are not applied if the slave surface that you specified is partially rigid and partially deformable; Abaqus/Standard issues an error message in such cases. In acoustic, structural-acoustic, and elastic wave propagation problems care should be exercised when tying meshes of highly dissimilar refinement. If two media have different wave speeds, the optimal meshes for each of the media will have different characteristic element lengths: the faster medium will have larger elements. If surfaces of these meshes are used in a tie constraint, the surface of the finer mesh (of the slower medium) should be designated as the slave. Nevertheless, in the region near the tied surfaces, the physical wave phenomena in both fast and slow media will typically have length scales characteristic of the slower medium; that is, of the shortest length scale in the physical problem. Therefore, if these phenomena are important, the mesh of the faster medium should be refined to the scale of the slower medium in the vicinity of the contact region. Adjusting the surfaces and considering offsets By default, with the exceptions mentioned below, Abaqus will automatically reposition the slave nodes to be tied in the initial configuration without causing strain to resolve gaps such that the surfaces are just touching, accounting for any shell thickness (unless you have specified that thickness should not be accounted for, as discussed above in the context of the position tolerance criterion) but not accounting for beam or membrane thickness. One exception is that no adjustments are made where tied surfaces are closer together than the combined half-shell thickness. All adjustments are performed such that the slave and master surfaces are never pushed apart; that is, the reference surfaces will only become closer as a result of the adjustments. It is recommended that you allow the automatic adjustments to occur, especially if neither surface has rotations; in this case a constant offset vector is used, so incorrect behavior of the constraint under rigid body rotation can occur when slave nodes are not lying exactly on the master surface. Adjustments are not made if the slave surface belongs to a substructure or when either the slave or master surface is a beam element-based surface; in the latter cases you should locate the beam element nodes with the desired offset from the other surface. Input File Usage: Abaqus/CAE Usage: *TIE, ADJUST=YES or NO Interaction module: Create Constraint: Tie: toggle Adjust slave node initial position Criteria for adjustment A slave node is considered for adjustment if both of the following conditions are met: • The slave node satisfies whatever criterion is in effect for generating a constraint (either because it satisfies the position tolerance criterion or belongs to the specified node set of constrained slave nodes, as previously discussed). • The slave node is more than the combined thickness of the slave and master surfaces away from its projection point on the master reference surface, accounting for any offset of the element reference surfaces from the respective element midsurfaces. For an element-based master surface a slave node will be moved toward the closest point on the master surface; for a node-based master surface a slave node will be moved toward the closest master node. The corrected position of an adjusted slave node is determined from the combined effects of shell element thickness and any specified reference surface offset relative to the shell midsurface of either slave or master surfaces. Figure 34.3.1–6 shows the adjusted slave node position in an example with two shell element-based surfaces tied together (in this example one of the element reference surfaces is offset from the element midsurface). It is assumed that the surfaces were farther apart than shown in Figure 34.3.1–6 prior to the adjustment; otherwise, the slave nodes would not have been adjusted. slave reference surface slave shell midsurface master shell reference and midsurface shell (s) – shell (m) slave shell element has offset = 1/2 (SPOS) Figure 34.3.1–6 Adjusted slave node position for two shell element-based surfaces tied together. The slave shell element has an offset of 0.5. Adjustments are made only for slave nodes that are included in the user-specified tied node set or that meet the tolerance criteria described above. Adjustments for overlapping constraints Nodal adjustments for tie constraints are processed sequentially in the order of the constraint definitions at the start of an analysis. If different constraint or contact definitions involve the same nodes, some adjustments may cause lack of compliance for contact or constraint definitions that were previously processed. These conflicts are less likely to occur in Abaqus/Explicit because the adjustments in Abaqus/Explicit are automatically processed in the chaining order discussed in “Overlapping constraints.” These conflicts can be avoided in Abaqus/Standard in some cases by changing the processing order of constraint and contact definitions: nodes in common between different contact or constraint definitions should be processed first as slave nodes and later as master nodes. Input File Usage: Abaqus/CAE Usage: To change the processing order of constraint and contact definitions, change the order of the definitions in the input file. Constraint and contact definitions are processed in the order in which they appear. To change the processing order of constraint and contact definitions, change the names of the constraints and interactions in the model. Constraints and interactions are processed alphabetically according to their name. Accounting for an offset between tied surfaces Abaqus allows a gap to exist between tied surfaces. Such gaps may exist if you prevent nodal adjustments for tied surfaces. A gap between the reference surfaces may remain due to the presence of shell thickness even if nodal adjustments are performed. Figure 34.3.1–7 shows some cases where an offset between the reference surfaces may be desirable for tied surface pairs to account for shell or beam thickness. solid (s) – solid (m) shell (s) – solid (m) solid (s) – shell (m) shell (s) - shell (m) solid (s) – beam (m) shell (s) – beam (m) beam (s) – solid (m) beam (s) – shell (m) beam (s) – beam (m) Figure 34.3.1–7 Tie constraints being applied between surfaces based on various element types (h = offset between slave and master surfaces). Rigid body motion is properly accounted for when the nodes are separated by a finite distance when at least one of the surfaces is based on shell or beam elements; when the master surface is an analytical rigid surface; or, in the case of node-based surfaces, when the nodes on at least one surface have active rotational degrees of freedom. The nature of the constraint on translational motion between surfaces in Abaqus depends on whether there is an offset between the surfaces and on which surfaces have rotational degrees of freedom, as discussed below. Neither surface has rotational degrees of freedom If neither surface has rotational degrees of freedom, the global translational degrees of freedom of the slave node and the closest point on the master surface are constrained to be the same. When an offset exists, Abaqus will enforce the constraint through the fixed offset like a PIN-type MPC when the nodes in the MPC are not coincident. Because the fixed offset does not rotate, the surface-based constraint will not represent rigid body rotation correctly. The constraint will represent rigid body motion correctly when the offset is zero. This behavior can be ensured by specifying that all tied slave nodes should be moved onto the master surface. Only one surface has rotational degrees of freedom If the slave surface has rotational degrees of freedom and the master surface does not, the translational motion is constrained at the closest point on the master reference surface. When the reference surfaces are offset, a moment will be applied to each slave node based on the constraint force times the offset distance. Similarly, if the master surface has rotational degrees of freedom and the slave surface does not, the translational motion is constrained at each slave node and a moment will be applied to the relevant nodes on the master surface if an offset exists. In either case the surface-based constraint will behave correctly under rigid body rotation regardless of the amount of offset. Both surfaces have rotational degrees of freedom If both surfaces have rotational degrees of freedom, are not offset, and the rotations are tied, each slave node is constrained to the master surface like a TIE-type MPC. If an offset exists between the surfaces, the constraint acts like a BEAM-type MPC between the slave node and the closest point on the master reference surface. If the rotations are not tied, Abaqus allows you to choose the location of the translational constraint. It can be enforced at the master reference surface, the slave reference surface, or anywhere in between. The location of the translational constraint enforcement for surfaces where the rotations are not tied will affect the distribution of moment to each of the surfaces. The most physically reasonable choice is to locate the constraint at the point where the actual top or bottom sides of each surface meet. The constraint then models a perfect adhesive between the surfaces, which transfers shear stress to each surface. Abaqus will choose the location of the translational constraint as follows: • If the master surface is shell element-based, the translational constraint is enforced on the top or bottom side of the master surface. • If the slave surface is shell element-based and the master surface is not, the translational constraint is enforced at the top or bottom side of the slave surface. • Otherwise, the translational constraint is enforced at the master reference surface. To override these default locations, you can specify a constraint ratio for the tie constraint equal to the fractional distance between the master reference surface and the slave node at which the translational constraint should act. Figure 34.3.1–8 shows an example of the use of a constraint ratio to prescribe the location of the translational constraint between two shell surfaces that are tied together with no rotational constraints. The distance between the master reference surface and the slave reference surface is b. The slave reference surface pin rigid beams master reference surface constraint ratio, r = a/b Figure 34.3.1–8 Use of a constraint ratio to prescribe the location of the translational constraint. prescribed constraint ratio, r, is then used to locate the translational constraint at a distance a from the master reference surface. All distances are measured along the vector between the slave node and its projection point onto the master reference surface. The constraint behavior is then similar to that of two rigid beams pinned together, as shown. Input File Usage: Abaqus/CAE Usage: *TIE, CONSTRAINT RATIO=value Interaction module: Create Constraint: Tie: Constraint ratio Constraining a surface to a three-dimensional beam The master surface for a tie constraint can be based on three-dimensional beam elements. For this case each slave node is projected onto the line formed by the nodes of the beam elements in the undeformed configuration to find the projection point. During the subsequent analysis the motion of each slave node is rigidly constrained to the motion (translation and rotation) of its projection point; i.e., each slave node and its projection point are connected by a rigid beam. Constraining other elements to a beam element-based master surface allows modeling of interactions between the surface of a (complex) beam section and its surroundings, without having to model the beam with continuum and/or shell elements. This feature can be particularly useful for modeling acoustic-structural interactions. Note: Abaqus/CAE currently does not support master surfaces based on beam elements. Use of tie constraints in non-mechanical simulations The surface-based tie constraint capability can be used in models where the nodal degrees of freedom on both the slave and master surfaces include electrical potential, pore pressure, acoustic pressure, and/or temperature. Except for the type of nodal degree of freedom being constrained, Abaqus uses exactly the same formulation for the tie constraint in nonmechanical simulations as it does for mechanical simulations. In general, degrees of freedom common to both surfaces are tied, and any other degrees of freedom are unconstrained. The case of structural-acoustic constraints is the exception to this rule. Here, appropriate relations between the acoustic pressure on the fluid surface and displacements on the solid surface are formed internally . The displacements and/or pressure degrees of freedom on the surfaces are the only ones affected; rotations are ignored by the tie constraint in this case. The internally computed structural-acoustic coupling conditions use surface areas and normal directions associated with the slave surface elements. The slave surface for structural-acoustic tie constraints cannot be a node-based surface. In two-dimensional analyses the out-of-plane thickness of the slave elements is required. Generally, this thickness is the thickness specified on the section definition for the slave surface elements. However, when beam elements form the slave surface in a tie constraint pair with acoustic elements, a unit thickness in the out-of-plane direction is assumed for the beams. In Abaqus/Standard you can define coupling between solid medium and acoustic medium infinite elements along the surfaces that extend to infinity. These surfaces are defined using the edges of the acoustic elements and sides numbered “2” and higher of the solid medium infinite elements. The infinite surfaces of solid medium and acoustic infinite elements can be coupled only through the use of a surface- based tie constraint. As shown in Figure 34.3.1–9, the acoustic infinite elements must be the slave elements and the edges of the acoustic infinite elements should lie within the specified position tolerance to the solid medium infinite element base facets. position tolerance solid infinite element master surface slave surface acoustic infinite element Figure 34.3.1–9 Use of a surface-based tie constraint to prescribe the coupling between solid medium and acoustic medium infinite elements. If the base facets of acoustic infinite elements are to be coupled to solid medium finite elements, to solid medium infinite elements, or to structural elements, either a surface-based tie constraint or acoustic- structural interaction elements can be used. Surfaces defined on solid medium infinite elements cannot be used in a surface-based tie constraint in Abaqus/Explicit. Table 34.3.1–3 enumerates all possible cases. For other slave-master pairings not listed in this table, an error message will be issued. Table 34.3.1–3 Possible slave-master surface pairings. Slave Surface Master Surface Degrees of Freedom Tied Acoustic Acoustic Stress Stress Heat-Stress Stress Acoustic Acoustic pressure Stress Translations Acoustic Acoustic pressure Stress Stress Translations and/or rotations Translations and/or rotations Heat-Stress Translations and/or rotations Heat-Stress Heat-Stress Temperature, translations and/or rotations The following surface pairings are available only in Abaqus/Standard: Heat transfer Heat transfer Temperature Electrical-Heat Heat transfer Temperature Heat transfer Electrical-Heat Temperature Electrical-Heat Electrical-Heat Temperature and electric potential Pore-Stress Pore-Stress Stress Pore-Stress Pore pressure and translations Stress Translations Pore-Stress Translations Tie constraints versus tied contact in Abaqus/Standard There are the following advantages to using a surface-based tie constraint in Abaqus/Standard instead of defining tied contact as discussed in “Defining tied contact in Abaqus/Standard,” Section 35.3.7: • Degrees of freedom of the slave surface nodes will be eliminated. • The tie constraint is more efficient in terms of the size of the fronts of the operator matrix because fewer master surface nodes are associated with each slave node. • Rotational degrees of freedom as well as translational degrees of freedom can be tied. • Tie constraints are much more general since they allow the use of general surfaces. • Surface offsets and shell thickness are taken into account. Overlapping constraints In a model with multiple tie constraint definitions it is possible that the slave and master surfaces of different tie constraint definitions may intersect. If two tie constraint definitions have part or all of their master surfaces in common or if the surfaces tied are layered (i.e., the master surface of one tie constraint definition acts as the slave surface of a subsequent tie constraint definition), Abaqus will attempt to chain the constraint definitions together. This will reduce the number of degrees of freedom and lower the computational expense, resulting in faster run times. However, in a model with multiple tie constraint definitions if nodes on the slave surface of one tie constraint definition are part of the slave surface of other tie constraint definitions, an overconstraint occurs. In most cases the overconstraint is due to the existence of redundant constraints, and it is safe to eliminate this redundancy. However, the overconstraint may also be due to conflicting constraints, in which case the problem is due to a modeling error that you should correct. Simulation results will vary depending on which constraint is removed to avoid an overconstraint if the overlapping constraints are not identical. It is recommended that, wherever possible, you order the slave and master surfaces of the constraint definitions to avoid intersecting slave surfaces. See “Adjustments for overlapping constraints” for a discussion of initial strain-free adjustments for overlapping constraints. Overconstrained slave nodes in Abaqus/Standard If an overconstraint occurs, Abaqus/Standard issues an error message unless the constraints are redundant or nearly redundant, as discussed below. As discussed previously, each tie constraint involves a single slave node and a set of master nodes with nonzero tie coefficents. Abaqus/Standard considers tie constraints involving the same slave node to be nearly redundant if at least one node is common among the respective sets of master nodes with nonzero tie coefficients. In such cases, rather than issuing an error message, Abaqus/Standard issues a warning message and only enforces one of the constraints. The surface-based tie constraint is imposed in Abaqus/Standard by eliminating the degrees of therefore, nodes on the slave surface should not be used to apply freedom on the slave surface; boundary conditions, nor should they be used in any subsequent tie, multi-point, equation, or kinematic coupling constraint . Overconstrained slave nodes in Abaqus/Explicit In contrast, Abaqus/Explicit treats overconstraints with a penalty method, thus enforcing the constraints in an average sense; the computational cost of the analysis may increase in these cases. In addition, if the slave surface for a tie constraint definition in Abaqus/Explicit is part of a rigid body while the master surface comprises a deformable element- or node-based surface and the master surface acts as the slave surface in a subsequent tie constraint definition, the resolution of the resulting constraints can prove to be computationally intensive. It is recommended that, wherever possible, you order the slave and master surfaces of the constraint definitions to avoid such a situation. Nullifying the tie constraint on slave nodes due to element deletion in Abaqus/Explicit In Abaqus/Explicit tie constraints are nullified as underlying elements of tied surfaces are deleted due to material point failure. The tie constraint between a slave node and its corresponding master nodes is deleted when either all the elements attached to the slave node are deleted or the master element to which the slave node is tied is deleted. Limitations The following limitations exist for tie constraints: • Surface-based tie constraints cannot be used to connect gasket elements that model thickness- direction behavior only. • A rigid surface cannot act as a slave surface in a constraint pair in Abaqus/Standard. • A slave node of a tie constraint cannot act as a slave node of another constraint in Abaqus/Standard. • Tie constraints cannot be used to tie infinite elements to finite elements in Abaqus/Explicit. To couple infinite and finite elements in Abaqus/Explicit, the elements must share nodes. • The axisymmetric solid Fourier elements with nonlinear, asymmetric deformation cannot form element-based surfaces; therefore, such surfaces cannot be used in tie constraints. 34.3.2 COUPLING CONSTRAINTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Surfaces: overview,” Section 2.3.1 • *COUPLING • *KINEMATIC • *DISTRIBUTING • “Defining coupling constraints,” Section 15.15.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The surface-based coupling constraint: • couples the motion of a collection of nodes on a surface to the motion of a reference node; • is of type kinematic when the group of nodes is coupled to the rigid body motion defined by the reference node; • is of type distributing when the group of nodes can be constrained to the rigid body motion defined by a reference node in an average sense by allowing control over the transmission of forces through weight factors specified at the coupling nodes; • automatically selects the coupling nodes located on a surface lying within a region of influence; • can be used with two- or three-dimensional stress/displacement elements; and • can be used in geometrically linear and nonlinear analysis. Surface-based coupling definitions The surface-based coupling constraint in Abaqus provides coupling between a reference node and a group of nodes referred to as the “coupling nodes.” This option provides the same functionality as the kinematic coupling constraint and the distributing coupling elements (DCOUP2D, DCOUP3D) in Abaqus/Standard with a surface-based user interface. The coupling nodes are selected automatically by specifying a surface and an optional influence region. The procedure used to define the coupling nodes is discussed below. For a distributing coupling constraint, the distributing weight factors are calculated automatically if the surface is an element-based surface. In such a case the weight factors are based on the tributary area at each coupling node, except for a surface along a shell edge, where the weight factors are based on the tributary edge length. Furthermore, the distributing weight factors can be modified using one of several weighting methods, which allow the forces transferred to the coupling nodes to vary inversely with the radial distance from the reference node. Typical applications The coupling constraint is useful when a group of coupling nodes is constrained to the rigid body motion of a single node. The coupling constraint can be employed effectively in the following applications: • To apply loads or boundary conditions to a model. Figure 34.3.2–1 illustrates the use of a kinematic coupling constraint to prescribe a twisting motion to a model without constraining the radial motion. reference node axis of cylindrical coordinate system constrained nodes that are free to translate radially surface that defines the coupling nodes Figure 34.3.2–1 Kinematic coupling constraint. Figure 34.3.2–2 illustrates a distributing coupling constraint used to prescribe a displacement and rotation condition on a boundary where relative motion between the nodes on the boundary is required. In this example a twist is prescribed at the end of the structure that is expected to warp and/or deform within the end surface. • To distribute loads on a model, where the load distribution can be described with a moment-of-inertia expression. Examples of such cases include the classic bolt-pattern and weld-pattern distribution expressions. • To apply dimensionality transitions between continuum and structural elements. For example, a distributing coupling allows flexible coupling between structural and solid elements. • To model end conditions. For example, modeling a rigid end plate or modeling plane sections of a solid to remain planar can be done easily with a kinematic coupling definition. • To simplify modeling of complex constraints. In a kinematic coupling definition the degrees of freedom that participate in the constraint may be selected individually in a local coordinate system. • To model interactions with other constraints, such as connector elements. For example, a hinged part may be modeled more realistically by two distributing coupling definitions, whose reference nodes warping is permitted by the coupling element reference node prescribed rotation surface that defines the coupling nodes coupling nodes Figure 34.3.2–2 Distributing coupling constraint. are connected by a hinge connector element. The load transfer then occurs between two “clouds” of nodes, rather than between two single nodes. “Substructure analysis of a one-piston engine model,” Section 4.1.10 of the Abaqus Example Problems Manual, illustrates this use of connector elements in conjunction with coupling constraints to model a one-piston engine. Defining the coupling constraint Defining a coupling constraint requires the specification of the reference node (also called the constraint control point), the coupling nodes, and the constraint type. The coupling constraint associates the reference node with the coupling nodes. A name must be assigned to the constraint and may be used in postprocessing with Abaqus/CAE. A node number or node set name may be specified for the reference node. If a node set is specified, the node set must contain exactly one node. The reference node for a kinematic coupling constraint has both translational and rotational degrees of freedom. The surface on which the coupling nodes are located can be node-based; element-based; or, in Abaqus/Explicit, a combination of both surface types. You can specify an optional radius of influence that limits the coupling nodes to a specific region on the surface. Details on how coupling nodes are defined by specifying an influence region are discussed below. The constraint type can be either kinematic or distributing, as discussed below. Input File Usage: Abaqus/CAE Usage: Use the following options: *COUPLING, CONSTRAINT NAME=name, REF NODE=n, SURFACE=surface *KINEMATIC or *DISTRIBUTING Interaction module: Create Constraint: Coupling: Coupling type: Kinematic or Distributing Specifying a region of influence By default, coupling nodes belonging to the entire surface are selected for the coupling definition. You can limit the coupling nodes to lie within a spherical region centered about the reference node by defining a radius of influence. The procedure by which coupling nodes are selected for the constraint definition depends on the surface type: • For a node-based surface, all the nodes defined by the surface definition that fall within the influence region are selected for the coupling definitions. • For an element-based surface, the surface facets that are either fully or partially inscribed by the influence region are determined. All nodes belonging to these facets, whether or not these nodes fall within the influence region, are selected for the coupling nodes. When the influence radius is less than the distance to the closest coupling node, Abaqus selects all nodes belonging to the closest facet. If the projection of the reference node on the surface falls on an edge or a vertex of multiple facets, all nodes belonging to these facets adjoining the edge or vertex are included in the coupling definition. In the case where the influence radius is less than the distance to the closest coupling node, adjacent surface faces must have consistent normal directions; otherwise, Abaqus issues an error message. • A distributing coupling constraint must include at least two coupling nodes. If fewer than two coupling nodes are found, Abaqus issues an error message during input file preprocessing. Input File Usage: *COUPLING, CONSTRAINT NAME=name, REF NODE=n, SURFACE=surface, INFLUENCE RADIUS=r Abaqus/CAE Usage: Interaction module: Create Constraint: Coupling: Influence radius: Specify Kinematic coupling constraints Kinematic coupling constrains the motion of the coupling nodes to the rigid body motion of the reference node. The constraint can be applied to user-specified degrees of freedom at the coupling nodes with respect to the global or a local coordinate system. Kinematic constraints are imposed by eliminating degrees of freedom at the coupling nodes. In Abaqus/Standard once any combination of displacement degrees of freedom at a coupling node is constrained, additional displacement constraints—such as MPCs, boundary conditions, or other kinematic coupling definitions—cannot be applied to any coupling node involved in a kinematic coupling constraint. The same limitation applies for rotational degrees of freedom. This restriction does not apply in Abaqus/Explicit. See “Kinematic constraints: overview,” Section 34.1.1, for more information. Input File Usage: Use both of the following options to define a kinematic coupling constraint: *COUPLING *KINEMATIC first dof, last dof For example, the following coupling constraint is used to constrain degrees of freedom 1, 2, and 6 on surface surfA to reference node 1000: *COUPLING, CONSTRAINT NAME=C1, REF NODE=1000, SURFACE=surfA *KINEMATIC 1, 2 6, Abaqus/CAE Usage: Interaction module: Create Constraint: Coupling: Coupling type: Kinematic: toggle on the degrees of freedom Translational degrees of freedom Translational degrees of freedom are constrained by eliminating the specified degrees of freedom at the coupling nodes. When all translational degrees of freedom are specified, the coupling nodes follow the rigid body motion of the reference node. Rotational degrees of freedom Rotational degrees of freedom are constrained by eliminating the specified degrees of freedom at the coupling nodes. All combinations of selected rotational degrees of freedom result in rotational behavior identical to existing MPC types: • Selection of three rotational degrees of freedom along with three displacement degrees of freedom is equivalent to MPC type BEAM. • Selection of two rotational degrees of freedom is equivalent to MPC type REVOLUTE in Abaqus/Standard. • Selection of one rotational degree of freedom is equivalent to MPC type UNIVERSAL in Abaqus/Standard. In Abaqus/Standard internal nodes are created by the kinematic coupling to enforce the constraints that are equivalent to MPC types REVOLUTE and UNIVERSAL. These nodes have the same degrees of freedom as the additional nodes used in these MPC types and are included in the residual check for nonlinear analysis. Specifying a local coordinate system The kinematic coupling constraint can be specified with respect to a local coordinate system instead of the global coordinate system . Figure 34.3.2–1 illustrates the use of a local coordinate system to constrain all but the radial translation degrees of freedom of the coupling nodes to the reference node. In this example a local cylindrical coordinate system is defined that has its axis coincident with the structure’s axis. The coupling node constraints are then specified in this local coordinate system. Input File Usage: *COUPLING, ORIENTATION=local For example, the following input is used to specify the kinematic coupling constraint shown in Figure 34.3.2–1: *ORIENTATION, SYSTEM=CYLINDRICAL, NAME=COUPLEAXIS 0.0, -1.0, 0.0, 0.0, 1.0, 0.0 *COUPLING, REF NODE=500, SURFACE=Endcap, ORIENTATION=COUPLEAXIS *KINEMATIC 2, 3 Abaqus/CAE Usage: Interaction module: Create Constraint: Coupling: Edit: select local coordinate system Constraint direction and finite rotation In geometrically nonlinear analysis steps the coordinate system in which the constrained degrees of freedom are specified will rotate with the reference node regardless of whether the constrained degrees of freedom are specified in the global coordinate system or in a local coordinate system. Distributing coupling constraints Distributing coupling constrains the motion of the coupling nodes to the translation and rotation of the reference node. This constraint is enforced in an average sense in a way that enables control of the transmission of loads through weight factors at the coupling nodes. Forces and moments at the reference node are distributed either as a coupling node-force distribution only (default) or as a coupling node-force and moment distribution. The constraint distributes loads such that the resultants of the forces (and moments) at the coupling nodes are equivalent to the forces and moments at the reference node. For cases of more than a few coupling nodes, the distribution of forces/moments is not determined by equilibrium alone, and distributing weight factors are used to define the force distribution. The moment constraint between the rotation degrees of freedom at the reference node and the average rotation of the cloud nodes can be released in one direction in a two-dimensional analysis and one, two, or three directions in a three-dimensional analysis. In a three-dimensional analysis you can specify the moment constraint directions in the global coordinate system or in a local coordinate system. All available translational degrees of freedom at the reference node are always coupled to the average translation of the coupling nodes. In a three-dimensional Abaqus/Standard analysis if all three moment constraints are released by specifying only degrees of freedom 1 through 3, only translation degrees of freedom will be activated on the reference node. If only one or two rotation degrees of freedom have been released, all three rotation degrees of freedom are activated at the reference node. In this case you must ensure that proper constraints have been placed on the unconstrained rotation degrees of freedom to avoid numerical singularities. Most often this is accomplished by using boundary conditions or by attaching the reference node to an element such as a beam or shell that will provide rotational stiffness to the unconstrained rotation degrees of freedom. In Abaqus/Explicit releasing one or more of the moment constraints may lead to significant computational performance degradation. This is also the case when other constraints intersect the cloud of coupling nodes. In these cases, the degradation in performance is particularly noticeable when a large number of such distributed couplings are present in the model or when the size of the constrained “cloud” is large. For that matter, when the modeling conditions mentioned above are encountered, the size of the coupling nodes cloud is limited to 1000. To alleviate the released moment constraint issue, the following modeling technique can be used (also available in Abaqus/Standard): constrain all moments in the distributed coupling and use an appropriate connector element at the reference node (such as REVOLUTE, HINGE, CARDAN or BUSHING) to model released moments at the coupling’s reference node. This technique has also the advantage of being able to specify finite compliance such as elasticity, plasticity or damage in the “released” rotational component. Input File Usage: *DISTRIBUTING first dof, last dof If no degrees of freedom are specified, all available degrees of freedom are coupled. If you specify one or more rotation degrees of freedom but not all available translation degrees of freedom, Abaqus issues a warning message and adds all available translation degrees of freedom to the constraint. For example, the following coupling constraint is used to constrain degrees of freedom 1–5 on the reference node 1000 to the average translation and rotation of surface surfA: *COUPLING, CONSTRAINT NAME=C1, REF NODE=1000, SURFACE=surfA *DISTRIBUTING 1, 5 In this example the moment constraint between the reference node and the coupling nodes will be released in the 6-direction but will be enforced in the 4- and 5-directions. This provides a “revolute-like” rotation connection between the reference node and the coupling nodes . Interaction module: Create Constraint: Coupling: Coupling type: Distributing: toggle on the rotational degrees of freedom (Abaqus/CAE automatically constrains the translational degrees of freedom) Abaqus/CAE Usage: Node-based surface User-defined weight factors are used for node-based surfaces. The cross-sectional areas specified in the surface definition are used as the weight factors . Element-based surface For element-based surfaces the weight factors are calculated by Abaqus. The default weight distribution is based on the tributary surface area at each coupling node, except for a surface along a shell edge where the weight distribution is based on the tributary edge length. The procedure used to calculate the default weight factors is designed to ensure that if a radius of influence is prescribed, the default weight distribution varies smoothly with the influence radius. Calculating the default distributing weight factors The procedure to calculate the distributing weight factors depends on whether or not an influence radius is specified. • If no influence radius is specified, the entire surface is used in the coupling definition. In this case all nodes located on the surface are included in the coupling definition and the distributing weight factor at each coupling node is equal to the tributary surface area. • If an influence radius is specified, the default distributing weight factors at the coupling nodes are calculated as follows: 1. A “participation factor” is calculated for each surface facet. The participation factor is defined below. 2. The tributary nodal area (or tributary edge length along a shell edge) at each facet node is computed and is multiplied by the facet participation factor. 3. The coupling node distributing weight factor is computed as the sum of the corresponding facet nodal areas (calculated above) for all joining facets. Calculating the facet participation factor The participation factor defines the proportion of the facet’s area that contributes to the distributing weight factors when an influence radius is specified. The participation factor varies between zero and one. To define the participation factor, the distance of the facet node closest to the reference node, , and the distance of the facet node farthest from the reference node, , are calculated. • If , where and a participation factor of one is used. is the influence radius, all facet nodes lie within the influence region; • If is set to zero. , none of the facet nodes lie within the influence region; and the participation factor • If , the facet is partially inscribed in the influence region; and the facet is assigned a participation factor equal to . If all coupling nodes fall outside the influence radius (i.e., for all facets), Abaqus selects all nodes belonging to the closest facets (as outlined under “Specifying a region of influence”) and uses a participation factor equal to one. Weighting methods You can modify the default weight distribution defined above. Various weighting methods are provided that monotonically decrease with radial distance from the reference node. For each case the default weight distribution that is based on the tributary surface area (or tributary edge length along a shell edge) is scaled by the weight factor . If the weighting method is not specified, a uniform weighting method is used in which all weight factors are equal to 1.0. A linearly decreasing weighting scheme COUPLING CONSTRAINTS is the coupling node radial distance from the reference where node, and is the weight factor at coupling node i, is the distance to the furthest coupling node. Input File Usage: Abaqus/CAE Usage: *DISTRIBUTING, WEIGHTING METHOD=LINEAR Interaction module: Create Constraint: Coupling: Coupling type: Distributing: Weighting method: Linear Quadratic polynomial weight distribution A quadratic polynomial weight distribution defined by Input File Usage: Abaqus/CAE Usage: *DISTRIBUTING, WEIGHTING METHOD=QUADRATIC Interaction module: Create Constraint: Coupling: Coupling type: Distributing: Weighting method: Quadratic Monotonically decreasing weight distribution A monotonically decreasing weight distribution according to the cubic polynomial Input File Usage: Abaqus/CAE Usage: *DISTRIBUTING, WEIGHTING METHOD=CUBIC Interaction module: Create Constraint: Coupling: Coupling type: Distributing: Weighting method: Cubic Specifying a local coordinate system The distributing coupling constraint can be specified with respect to a local coordinate system instead of the global coordinate system . Figure 34.3.2–2 illustrates the use of a local coordinate system to release the moment constraints between the reference node and the coupling nodes in the local 4- and 6-directions, providing a “universal-like” rotation connection. In this example a local rectangular coordinate system is defined that has its local y-axis coincident with the global z-axis. The moment constraint is specified in this local coordinate system. Input File Usage: *COUPLING, ORIENTATION=local For example, the following input is used to specify the distributing coupling constraint shown in Figure 34.3.2–2: *ORIENTATION, SYSTEM=RECTANGULAR, NAME=COUPLEAXIS 0.0, 1.0, 0.0, 0.0, 0.0, 1.0 *COUPLING, REF NODE=500, SURFACE=Endcap, ORIENTATION=COUPLEAXIS *DISTRIBUTING 1, 3 5, 5 Abaqus/CAE Usage: Interaction module: Create Constraint: Coupling: Edit: select local coordinate system Defining the surface coupling method There are two methods available to couple the motion of the reference node to the average motion of the coupling nodes: the continuum coupling method and the structural coupling method. The continuum coupling method is used by default. Continuum coupling method The default continuum coupling method couples the translation and rotation of the reference node to the average translation of the coupling nodes. The constraint distributes the forces and moments at the reference node as a coupling nodes force distribution only. No moments are distributed at the coupling nodes. The force distribution is equivalent to the classic bolt pattern force distribution when the weight factors are interpreted as bolt cross-section areas. The constraint enforces a rigid beam connection between the attachment point and a point located at the weighted center of position of the coupling nodes. For further details, see “Distributing coupling elements,” Section 3.9.8 of the Abaqus Theory Manual. Input File Usage: Abaqus/CAE Usage: *DISTRIBUTING , COUPLING=CONTINUUM Coupling the motion of the reference node to the average motion of the coupling nodes is not supported in Abaqus/CAE. Structural coupling method The structural coupling method couples the translation and rotation of the reference node to the translation and the rotation motion of the coupling nodes. The method is particularly suited for bending-like applications of shells when the coupling constraint spans small patches of nodes and the reference node is chosen to be on or very close to the constrained surface. The constraint distributes forces and moments at the reference node as a coupling node-force and moment distribution. For this coupling method to be active, all rotation degrees of freedom at all coupling nodes must be active (as would be the case when the constraint is applied to a shell surface) and the constraints must be specified in all degrees of freedom (default). In addition, for the constraint to be meaningful, the local (or global) z-axis used in the constraint should be such that it is parallel to the average normal direction of the constrained surface. With respect to translations, the constraint enforces a rigid beam connection between the reference node and a moving point that remains at all times in the vicinity of the constrained surface. The location of this moving point is determined by the approximate current curvature of the surface, the current location of the weighted center of position of the coupling nodes , and the z-axis used in the constraint. This choice avoids unrealistic contact interactions if multiple pairs of distributed coupling constraints are used to fasten shell surfaces . With respect to rotations, the constraint is different along different local directions. Along the z-axis (twist direction), the constraint is identical to the one enforced via the continuum coupling method . By contrast, the rotational constraint in the plane perpendicular to the z-axis relates the in-plane reference node rotations to the in-plane rotations of the coupling nodes in the immediate vicinity of the reference node. This choice provides a more realistic (compliant) response when the constrained surface is small and deforms primarily in a bending mode. Input File Usage: Abaqus/CAE Usage: *DISTRIBUTING, COUPLING=STRUCTURAL Coupling the motion of the reference node to the average motion of the coupling nodes is not supported in Abaqus/CAE. Moment release and finite rotation In geometrically nonlinear analysis steps the coordinate system of the degrees of freedom that define the moment release rotates with the reference node regardless of whether the global coordinate system or a local coordinate system is used. Colinear coupling node arrangements The distributing coupling constraint transmits moments at the reference node as a force distribution among the coupling nodes, even if these nodes have rotational degrees of freedom. Thus, when the coupling node arrangement is colinear, the constraint is not capable of transmitting all components of a moment at the reference node. Specifically, the moment component that is parallel to the colinear coupling node arrangement will not be transmitted. When this case arises, a warning message is issued that identifies the axis about which the element will not transmit a moment. Limitations • A distributing coupling constraint cannot be used with axisymmetric elements with asymmetric deformation. This element type is not compatible with the distributing coupling constraint. • If a distributing coupling constraint is used with axisymmetric elements with twist, the constraint It will involve only the will not include the twist degree of freedom 5 in those elements. displacement degrees of freedom 1 and 2. • A distributing coupling definition with a large number of coupling nodes produces a large wavefront in Abaqus/Standard. This may result in significant memory usage and a long solution time to solve the finite element equilibrium equations. • A distributing coupling constraint cannot involve more than 46,000 degrees of freedom in Abaqus/Standard, which implies an upper limit of 23,000 nodes per constraint for two-dimensional and axisymmetric cases and an upper limit of 15,333 nodes per constraint for three-dimensional cases. 34.3.3 SHELL-TO-SOLID COUPLING Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Coupling constraints,” Section 34.3.2 • “Surfaces: overview,” Section 2.3.1 • *SHELL TO SOLID COUPLING • “Defining shell-to-solid coupling constraints,” Section 15.15.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Surface-based shell-to-solid coupling: • allows for a transition from shell element modeling to solid element modeling; • is most useful when local modeling should use a full three-dimensional analysis but other parts of the structure can be modeled as shells; • uses a set of internally defined distributing coupling constraints to couple the motion of a “line” of nodes along the edge of a shell model to the motion of a set of nodes on a solid surface; • automatically selects the coupling nodes located on a solid surface lying within a region of influence; • can be used with three-dimensional stress/displacement shell and solid (continuum) elements; • does not require any alignment between the solid and shell element meshes; and • can be used in geometrically linear and nonlinear analysis. Shell-to-solid coupling Shell-to-solid coupling in Abaqus is a surface-based technique for coupling shell elements to solid elements. Figure 34.3.3–1 illustrates two examples taken from “Shell-to-solid submodeling and shell-to-solid coupling of a pipe joint,” Section 1.1.10 of the Abaqus Example Problems Manual, and “The pinched cylinder problem,” Section 2.3.2 of the Abaqus Benchmarks Manual. Shell-to-solid coupling is intended to be used for mesh refinement studies where local modeling requires a relatively fine through-the-thickness solid mesh coupled to the edge of a shell mesh, as shown in Figure 34.3.3–2. In such a case Abaqus will assemble constraints that couple the displacement and rotation of each shell node to the average displacement and rotation of the solid surface in the vicinity of the shell node. As shown in Figure 34.3.3–2, the coupling occurs along a shell-to-solid interface defined by two user-specified surfaces: an edge-based shell surface and an element- or node-based solid surface . The shell surface (Figure 34.3.3–3) is referred to as the “shell shell elements solid elements solid elements shell elements Figure 34.3.3–1 Typical examples of shell-to-solid coupling. refined solid mesh shell-to-solid interface shell mesh Figure 34.3.3–2 Shell-to-solid interface. edge.” The shell element edges that define the edge-based shell surface are referred to as “edge facets.” The edge facets are either linear or parabolic segments depending if the underlying shell elements are linear or quadratic. solid solid surface shell shell edge Figure 34.3.3–3 Shell and solid surfaces. The shell-to-solid coupling is enforced by the automatic creation of an internal set of distributing coupling constraints between nodes on the shell edge and nodes on the solid surface. Abaqus uses default or user-defined distance and tolerance parameters (discussed below) to determine which nodes on the shell edge will be coupled to which nodes on the solid surface. For each shell node involved in the coupling, a distinct internal distributing coupling constraint is created with the shell node acting as the reference node and the associated solid nodes acting as the coupling nodes. Each internal constraint distributes the forces and moments acting at its shell node as forces acting on the related set of coupling surface nodes in a self-equilibrating manner. The resulting line of constraints enforces the shell-to-solid coupling. Defining shell-to-solid coupling Defining a shell-to-solid coupling constraint requires the specification of a constraint name, an edge- based shell surface, and an element- or node-based solid surface. Input File Usage: *SHELL TO SOLID COUPLING, CONSTRAINT NAME=name shell_surface, solid_surface Abaqus/CAE Usage: Interaction module: Create Constraint: Shell-to-solid coupling Abaqus automatically determines which nodes on the two surfaces participate in the coupling and creates appropriate internal distributed coupling constraints. You can also control which nodes on the two surfaces participate in the coupling by specifying a position tolerance and/or influence distance as described below. The resulting coupling constraint definitions are printed to the data file when model definition data are requested . Abaqus will also create an internal node set that contains all the solid nodes included in the coupling; the node set can be visualized using the Visualization module of Abaqus/CAE. The name of the internal node set is the name assigned to the coupling constraint. Controlling the shell nodes included in the coupling A position tolerance determines the absolute distance from the solid surface within which all shell nodes to be included in the coupling must lie. Shell nodes that lie outside this tolerance are not coupled to the solid surface. When using an element-based solid surface, the defined distance between a shell node and the solid surface is the projected distance measured along a line extending from the shell node to the closest point on the solid surface (which may be on the edge of the solid surface). The default position tolerance when using an element-based solid surface is 5% of the length of a typical facet on the shell edge. For a node-based solid surface the defined distance of a shell node to the surface is the distance to the closest node on the solid surface. The default position tolerance when using a node-based solid surface is based on the average distance between nodes on the solid surface. You can specify a nondefault position tolerance for element- or node-based solid surfaces.. Input File Usage: Abaqus/CAE Usage: *SHELL TO SOLID COUPLING, POSITION TOLERANCE=distance Interaction module: Create Constraint: Shell-to-solid coupling: select the surfaces: choose Specify distance for the Position Tolerance Controlling the solid nodes included in the coupling A geometric tolerance, which is referred to as the influence distance, is defined for each edge facet. For a given node or element facet on the solid surface to be included in the coupling constraint, its perpendicular distance from at least one edge facet must be less than or equal to the influence distance defined for that edge facet. The default influence distance for an edge facet is half the thickness of the underlying shell element. The default automatically accounts for any offset or nodal thickness included with the shell element’s cross-section definition. You can specify a nondefault influence distance. Input File Usage: Abaqus/CAE Usage: *SHELL TO SOLID COUPLING, INFLUENCE DISTANCE=distance Interaction module: Create Constraint: Shell-to-solid coupling: select the surfaces: choose Specify value for the Influence Distance A user-defined influence distance is optional in all cases except when an edge facet involved in the coupling is associated with a general arbitrary elastic shell section definition in which you specified the general stiffness. In this case since the shell thickness is not defined directly, you must supply an influence distance. Computation of the internal coupling constraints This section outlines the basic procedure used by Abaqus to compute the internal shell-to-solid coupling constraints. A single distinct internal distributing coupling constraint is created for each shell node that lies within the position tolerance from the solid surface. Internal coupling constraints are not created for shell nodes that lie outside this tolerance. The shell node acts as the reference node, and a set of nodes on the solid surface act as the coupling nodes. Abaqus finds the coupling nodes on the solid surface and computes the weight factors for the internal constraints by considering each shell edge facet separately. The following procedure is carried out for each edge facet: 1. Abaqus finds all nodes on the solid element surface that lie within the region of influence (discussed below) of the current edge facet. These nodes are included in the coupling constraint. 2. Abaqus then computes a set of weight factors for the solid nodes. A weight factor is a measure of both the tributary area of the solid node contained within the region of influence and the relative position of the solid node with respect to each shell node. The tributary areas for node-based surfaces are the cross-sectional areas that you specified when you defined the surface. For element-based surfaces the tributary areas are calculated by Abaqus. The sum of all the weight factors in each coupling constraint is a measure of the total tributary area of the solid surface that is contained within the region of influence. 3. The above procedure is carried out for all the shell edge facets contained within the shell surface. If a shell node belongs to more than one edge facet, all the coupling nodes and weight factors are combined into a single distributing constraint definition. The resulting line of constraints along the shell edge enforces the shell-to-solid coupling. There are two situations in which a shell node might satisfy the position tolerance but no coupling constraint is defined. If a shell node lies within the position tolerance but is not connected by an edge facet to at least one other shell node that also satisfies the tolerance, a coupling constraint is not created for this shell node. In this case it may be necessary to increase the position tolerance. Alternatively, if nonzero weight factors are not computed for at least two solid nodes associated with the shell node, a coupling constraint is not created for this shell node. The most likely cause for zero weight factors is that the influence distance is too small. In the case of a node-based surface, zero weights might also arise if the default cross-sectional area is used. For shell-to-solid coupling the default area is zero. The region of influence for an edge facet The region of influence of an edge facet is defined by a cylindrical volume whose centerline is the edge facet and whose radius is the edge facet’s influence distance. The ends of the cylindrical volume are defined by two bounding planes whose normals are the shell tangents at the two ends of the edge facet . In this example a region of influence is constructed for shell edge 2–3. For a node-based solid surface only the nodes that lie within or on the boundary of the region of influence are assigned to the current edge facet and included in the coupling definition. For an element-based solid surface each solid facet node is associated with part of the facet surface. If the part of the facet assigned to a given solid node falls within the region of influence, that node is included in the coupling definition. Using the normal on an element-based solid surface to restrict solid nodes that are used in the coupling In the case of an element-based solid surface Abaqus will compare the normal of each solid facet within the region of influence to the normal of the solid surface closest to the centerline of the cylindrical volume . In general, if the normal of a surface facet is not within 20° of the normal at the centerline, the nodes on the solid surface facet are not included in the coupling definition. For the case illustrated in Figure 34.3.3–4 this check would prevent nodes on the top and bottom surface of the solid solid shell region of influence for edge facet 2-3 shell node edge facet Figure 34.3.3–4 Regions of influence for an edge facet. mesh from being coupled to the shell nodes even if the influence distance was arbitrarily large and the solid surface definition included all sides of the solid geometry. This check is not used if the centerline is on or near a feature edge of the solid mesh where the normal is not well defined . Comments, restrictions, and modeling recommendations for shell-to-solid coupling • The shell-to-solid coupling formulation assumes that the interface surface between the shell and solid elements is normal to the shell. Therefore, while the solid surface can be curved in a direction tangent to the shell edge, it should be straight in the direction along the shell normals. This is an assumption on the geometry of the surfaces, not on the mesh. It is not necessary for the nodes on the solid surface to line up with each other or to line up with the shell nodes. • The shell-to-solid coupling capability is designed for analyses where the solid mesh is fine with respect to the shell thickness. It is recommended that at least two solid elements be included through the thickness at a shell-to-solid interface. Along the shell-to-solid interface the length of a shell edge facet should in general be of the same order as the characteristic surface dimension of a solid element facet. • An assumption used in the design of the shell-to-solid coupling algorithms is that the weight factors are based upon accurate nodal tributary areas, such as those automatically computed by Abaqus when an element-based surface is used. Therefore, it is generally recommended that an element- based solid surface be used instead of a node-based solid surface. However, in cases where the shell and solid meshes align with each other, it is sometimes advantageous to use a node-based solid surface especially when a homogenous solution is expected. • Figure 34.3.3–5 illustrates some recommended modeling practices for shell-to-solid coupling. If the shell reference surface is not offset, the shell edge should be centrally located with respect to the thickness direction of the solid (Figure 34.3.3–5(a)). The solid surface should include only the portion needed for the coupling (the shaded region shown in Figure 34.3.3–5(a)). solid shell edge centrally located with respect to the thickness direction of the solid solid surface only includes portion of solid where coupling is needed (a) shell mesh solid at least two shell elements between feature angles on the solid shell mesh (b) Figure 34.3.3–5 Modeling recommendations for the shell-to-solid interface. • The shell-to-solid interface can be defined around geometric feature angles (corners), (Figure 34.3.3–5(b)). However, it is recommended that the feature angles satisfy 60° < < 300°. In addition, as illustrated in Figure 34.3.3–5(b), at least two shell element edges should be included between each feature angle. • If an offset is defined for the shell section and the reference shell edge is placed at or near a feature edge on the solid surface (Figure 34.3.3–6), the solid surface should include only the side of the solid that you want to be included in the coupling definition. shell reference surface containing shell nodes solid offset shell midsurface In this example, it is recommended that the solid surface definition only include the shaded region. Figure 34.3.3–6 Modeling recommendations for the shell-to-solid interface with a shell offset. For example, if the top of the solid in Figure 34.3.3–6 is included in the surface definition, Abaqus includes nodes on the top of the surface in the coupling constraint, which is not what you intended. You intended only that the shell be coupled to the shaded region of the solid in Figure 34.3.3–6. Therefore, the solid surface definition should include only this region. • Care must be taken in interpreting the local stress and strain fields in the immediate vicinity of the shell-to-solid interface. This is especially true if the shell-to-solid interface includes corners or edges. The interface should be placed at least a distance more than the shell thickness away from the region in the solid mesh where the stress and strain fields are of interest. • The shell-to-solid interface should be located in a region of the model where shell theory is a valid modeling approximation. • Corners or kinks may exist in models made of shell elements. At such corners or kinks the shell elements only approximate the distribution of the material away from the midsurface of the shell. While the global moments and forces between the shell and solid models are transferred correctly, the local stress and displacement fields in the region of the shell-to-solid interface may be inaccurate. • Only displacement degrees of freedom in the solid elements and displacement and rotation degrees of freedom in the shell elements are coupled in shell-to-solid coupling. Shell-to-solid coupling does not couple other degrees of freedom such as temperature, pressure, etc. • Shell-to-solid coupling can be used to couple three-dimensional shells to all three-dimensional library,” solid element (“Cylindrical cylindrical elements except continuum elements Section 28.1.5). 34.3.4 MESH-INDEPENDENT FASTENERS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Surfaces: overview,” Section 2.3.1 • “Coupling constraints,” Section 34.3.2 • “Connector elements,” Section 31.1.2 • *FASTENER • *FASTENER PROPERTY • “About fasteners,” Section 29.1 of the Abaqus/CAE User’s Manual Overview The mesh-independent fastener capability: • is a convenient method to define a point-to-point connection between two or more surfaces such as a spot weld or rivet connection; • uses spatial coordinates of fastener locations to define point-to-point connections independent of underlying meshes; • combines either connector elements or BEAM MPCs with distributing coupling constraints to provide a connection that can be located anywhere between two or more surfaces regardless of the mesh refinement or location of nodes on each surface; • can be used to connect both deformable and rigid element-based surfaces; • can model either rigid, elastic, or inelastic connections with failure by using the generality of connector behavior definitions; and • is available only in three dimensions. Introduction Many applications require modeling of point-to-point connections between parts. These connections may be in the form of spot welds, rivets, screws, bolts, or other types of fastening mechanisms. There may be hundreds or even thousands of these connections in a large system model such as an automobile or airframe. The fastener can be located anywhere between the parts that are to be connected regardless of the mesh. In other words, the location of the fastener can be independent of the location of the nodes on the surfaces to be connected. Instead, the attachment to each of the parts being connected is distributed to several nodes in the surfaces to be connected in the neighborhood of the fastening points. Figure 34.3.4–1 shows a typical one-layer and two-layer fastener configuration. Each layer connects two fastening points using either a connector element or a BEAM MPC. Each fastening point is connected to the surface using Number of layers = 2 layer 1 Radius of influence layer 2 Fastening point Number of layers = 1 Fastening point Figure 34.3.4–1 Typical one-layer and two-layer fastener configuration. a distributing coupling constraint that couples the displacement and rotation of each fastening point to the average displacement and rotation of the nearby nodes. The mesh-independent fastener capability in Abaqus is designed to model these connections in a convenient manner. The fastener automatically: • determines the locations of nodes and orientations of connector elements or BEAM MPCs between two or more surfaces; • generates distributing coupling constraints to attach the connector elements or BEAM MPCs to each surface in a mesh-independent manner; and • calculates weights for the distributing coupling constraints that complete the mesh-independent connection. For an example of the use of mesh-independent fasteners, see “Buckling of a column with spot welds,” Section 1.2.3 of the Abaqus Example Problems Manual. Mesh-independent fasteners are referred to as point-based fasteners by Abaqus/CAE. For more information, see “About fasteners,” Section 29.1 of the Abaqus/CAE User’s Manual. It is also possible to assemble fasteners in Abaqus/CAE using connector elements, coupling constraints, etc. For further details, see “About assembled fasteners,” Section 29.1.3 of the Abaqus/CAE User’s Manual. Fastener interactions Fasteners are defined in groups called interactions, which are assigned names. Each interaction defines one or more fasteners. The number of individual fasteners is equal to the number of positioning points used to locate the fasteners. Fastening points on each surface are found by considering the position of the positioning point as discussed in subsequent sections. Fasteners can be defined using connector elements or BEAM MPCs. BEAM MPCs allow modeling of perfectly rigid connectors between components; while connector elements allow you to model much more complex behavior, such as deformable connectors that include the effects of elasticity, damage, plasticity, and friction. Input File Usage: Abaqus/CAE Usage: *FASTENER, INTERACTION NAME=name Interaction module: Special→Fasteners→Create: Name: name, Type: Point-based Defining fasteners using BEAM MPCs For modeling perfectly rigid connections you need not define fasteners using connector elements. Instead, Abaqus can internally generate BEAM MPCs connecting the fastening points of the fasteners. In this approach you assign a reference node set containing a list of user-defined nodes to the fastener interaction. The nodes in this reference node set will be used as positioning points to locate the fasteners. If single-layer fasteners are to be modeled, Abaqus generates single BEAM MPCs with each node in the reference node set becoming the first node of the BEAM MPC. The second node of each BEAM MPC will be generated internally by Abaqus. If multi-layer fasteners are to be defined, Abaqus generates linked sets of BEAM MPCs with each node in the reference node set becoming the first node of the first BEAM MPC in each linked set. The subsequent nodes in each linked set will be generated internally by Abaqus. For multi-layer fasteners each linked set contains as many BEAM MPCs as the number of layers in the fastener. Input File Usage: Abaqus/CAE Usage: Use the following options: *FASTENER, INTERACTION NAME=name, REFERENCE NODE SET=node set label *NSET, NSET=node set label Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Property: Section: Rigid MPC Defining fasteners using connector elements Using connector elements as the basis for a point-to-point connection allows for very complex behavior to be modeled with fasteners. Like other uses of connector elements, the connection can be fully rigid or may allow for unconstrained relative motion in local connector components. In addition, deformable behavior can be specified using a connector behavior definition that can include the effects of elasticity, damping, plasticity, damage, and friction. There are two methods to define fasteners that use connector elements to model the behavior between fastening points. For both methods the fastener interaction refers to an element set containing the connector elements. You must specify a connector section definition that refers to this element set. You should be careful when specifying the connector orientation (if needed) as discussed below in “Defining the fastener orientation.” Defining the connector elements directly The most controlled approach to specifying fasteners using connector elements is to define the connector elements explicitly and associate them with an element set. The fastener interaction refers to the element set. Each fastener in the fastener interaction corresponds to one or more connector elements depending on the number of layers of the fastener . A single connector element is associated with each layer, and the two nodes of the connector element correspond to the fastening points of the two adjacent surfaces. When specifying a multi-layer fastener, the connector elements for each layer should share nodes with the connector elements of adjacent layers. 200 100 single layer fastener modeled with connectors 200 100 201 101 nodes connector elements positioning point location specified by user multi-layer fastener modeled with connectors Figure 34.3.4–2 Single- and multi-layer fasteners modeled with connector elements. For a single-layer fastener the positioning point used to locate the fastener and its fastening points is taken as the nodal coordinates of the first node of the connector element. For a multi-layer fastener the positioning point is taken as the first node of the first connector in a linked set of connectors with as many members as layers. Examples of defining a single-layer and multi-layer fastener are included at the end of this section. Input File Usage: Abaqus/CAE Usage: Use the following options: *FASTENER, INTERACTION NAME=name, ELSET=element set label blank line *ELEMENT, TYPE=CONN3D2, ELSET=element set label *CONNECTOR SECTION, ELSET=element set label For point-based fasteners in Abaqus/CAE, you cannot define the connector elements directly; the connector elements are generated by Abaqus. Connector elements generated by Abaqus In this approach you do not need to explicitly define the connector elements that connect the fastening points of the fastener. The fastener interaction refers to an empty element set. You must specify a connector section definition that refers to this element set. In addition, you assign a reference node set containing a list of user-defined nodes to the fastener interaction. The nodes in this reference node set are used as positioning points to locate the fasteners. If single-layer fasteners are to be modeled, Abaqus generates single connector elements with each node in the reference node set becoming the first node of a connector element. The second node of each connector element will be generated internally by Abaqus. If multi-layer fasteners are to be defined, Abaqus generates linked sets of connector elements with each node in the reference node set becoming the first node of the first connector element in each linked set. The subsequent nodes in each linked set will be generated internally by Abaqus. For multi-layer fasteners each linked set contains as many connector elements as the number of layers in the fastener. The connector elements are given internally generated element numbers and assigned to the named user-specified element set. You can use this element set to request output for these connector elements. However, this element set should not be included in another element set definition. Input File Usage: Abaqus/CAE Usage: Use the following options: *FASTENER, INTERACTION NAME=name, ELSET=element set label, REFERENCE NODE SET=node set label blank line *NSET, NSET=node set label *CONNECTOR SECTION, ELSET=element set label Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Property: Section: Connector section: select connector section Example: using connector elements to define single-layer fasteners directly To define a single-layer fastener directly using connector elements: • Define two connector elements with user element numbers 100 and 200 and user-defined node numbers 1, 2 and 3, 4, respectively, and include them in an element set. Nodes 1 and 3 act as the positioning points for the two fasteners . • Refer to the element set in the fastener interaction and connector section definitions. • Assign section properties to the fasteners. Suppose in this example that relative displacements between the fastening points are to be allowed. Therefore, the fasteners must be assigned a section that has available components of motion; for example, a CARTESIAN section can be used. • The relative displacement between the fastening points gives rise to elastic deformations. Hence, the material between the fasteners is modeled as linear elastic with a spring stiffness of 10000 using connector elasticity. The following input can be used: *FASTENER, INTERACTION NAME=fastinter, ELSET=fastconn, PROPERTY=fastprop blank line surface1, surface2 *ELEMENT, TYPE=CONN3D2, ELSET=fastconn 100, 1, 2 200, 3, 4 *CONNECTOR SECTION, ELSET=fastconn, BEHAVIOR=behav CARTESIAN, *CONNECTOR BEHAVIOR, NAME=behav *CONNECTOR ELASTICITY, COMPONENT=1 10000, *CONNECTOR ELASTICITY, COMPONENT=2 10000, *CONNECTOR ELASTICITY, COMPONENT=3 10000, Example: using connector elements to define multi-layer fasteners directly To define a multi-layer fastener directly using connector elements: • Define two linked sets of connector elements with each linked set containing exactly two connectors. The first linked set comprises element numbers 100 and 101, with node numbers 1, 2 and 2, 3, respectively. The second linked set comprises element numbers 200 and 201, with node numbers 4, 5 and 5, 6, respectively. Include the connector elements in an element set. Nodes 1 and 4 act as the positioning points for the two fasteners . • Refer to the element set in the fastener interaction and connector section definitions • Assign section properties to the fasteners. Suppose in this example that rigid beam-type behavior between the fastening points is to be modeled; in that case the fasteners must be assigned a BEAM section. The following input can be used: *FASTENER, INTERACTION NAME=fastinter, ELSET=fastconn, PROPERTY=fastprop blank line surface1, surface2, surface3 *ELEMENT, TYPE=CONN3D2, ELSET=fastconn 100, 1, 2 101, 2, 3 200, 4, 5 201, 5, 6 *CONNECTOR SECTION, ELSET=fastconn BEAM, Specifying the positioning points, projection method, and fastening points Each interaction defines one or more fasteners. The number of individual fasteners is equal to the number of positioning points used to locate the fasteners. Positioning points are nodes defined at the fastener locations and assigned as a reference node set to the interaction. In general, a positioning point should be located as close to the surfaces being connected as possible. The reference node specifying the positioning point can be one of the nodes on the connected surfaces or can be defined separately. Abaqus determines the actual points where the fastener layers attach to the surfaces that are being connected by first projecting the positioning point onto the closest surface. Abaqus offers the following projection methods to find fastening points on the specified surfaces to form fasteners: • Face-to-face • Face-to-edge • Edge-to-face • Edge-to-edge The choice of method depends on how the surfaces are oriented relative to each other. Fastening surfaces that are nearly parallel to each other Most commonly the surfaces to be fastened together are nearly parallel to each other; in which case the fastening points are located on element facets away from the periphery of the surfaces. The face-to-face projection method is most appropriate for such situations. It is also the default projection method. In the face-to-face projection method, Abaqus projects each positioning point onto the closest surface along a directed line segment normal to the surface. Alternatively, you can specify the projection direction. Specifying the direction may be useful when two-dimensional drawings are used to identify the positioning point locations and those locations are known precisely in two dimensions but not in a third. For this case the direction specified is typically the normal to the plane of the drawing. Once the fastening point on the closest surface has been identified, Abaqus determines the points on the other surface or surfaces to be connected by projecting the first fastening point onto the other surfaces along the fastener normal direction, which is typically normal to the closest surface. Figure 34.3.4–3 shows the two ways of locating the projection points. When surfaces to be fastened are not exactly parallel, Abaqus sometimes sets attachment points to be at the closest facet edges or corner on the surface, rather than along the fastener normal direction. The location of the positioning point (a node in the reference node set) might not coincide with the locations of the fastening points found by Abaqus. Hence, the coordinates of the node at the positioning point may change from their user-prescribed values when the node is shifted to a fastening point. If the node at the positioning point is part of the connectivity of a user-defined element, this can cause the element whose connectivity includes that node to undergo unacceptable initial distortions. In such situations it is recommended that you define the node at the positioning point separately. In general, you should not specify this node to be one of the nodes of the connected surfaces. Input File Usage: Use the following option to allow Abaqus to define the projection direction: *FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=FACETOFACE (default) blank line Use the following option to define the projection direction directly: *FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=FACETOFACE (default) x-component, y-component, z-component Positioning point Projection direction specified by user Projection normal for surface Positioning point First fastening point Second fastening point Figure 34.3.4–3 Directed and normal projection to locate the fastening points for the face-to-face projection method. Abaqus/CAE Usage: Use the following input to allow Abaqus to define the projection direction: Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Domain tabbed page: Direction vector: Default, Criteria tabbed page: Attachment method: Face-to-Face Use the following input to define the projection direction directly: Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Domain tabbed page: Direction vector: Specify, Criteria tabbed page: Attachment method: Face-to-Face Fastening nearly perpendicular surfaces When you need to fasten surfaces that are perpendicular or nearly perpendicular to each other; i.e., forming a T-intersection, the face-to-edge or the edge-to-face projection methods are appropriate choices. Figure 34.3.4–4 shows attachments for the face-to-edge and edge-to-face projection methods. Creating the first fastening point on a face In the face-to-edge projection method Abaqus projects the positioning point onto the closest surface along a directed line segment normal to the surface. The subsequent fastening points are found by searching for the closest points on the remaining specified surfaces. The closest fastening point may fall on the edge or a corner of a surface. Input File Usage: *FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=FACETOEDGE blank line First fastening point Subsequent fastening point First fastening point Positioning point Subsequent fastening point Positioning point Figure 34.3.4–4 Face-to-edge and edge-to-face projection methods to locate fastening points for surfaces that form T-intersections. Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Criteria: Attachment method: Face-to-Edge Creating the first fastening point on an edge In the edge-to-face projection method, the first fastening point is found by searching for the closest point on the specified surface or surfaces. The closest point may be on the edge or corner of the surface. For subsequent fastening points Abaqus projects the previous fastening point along a directed line segment normal to the surface. Input File Usage: *FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=EDGETOFACE blank line Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Criteria: Attachment method: Edge-to-Face Fastening abutting surfaces When it is desired to form fasteners between surfaces that are butting against each other, the edge-to-edge projection method is appropriate. In this method the first as well as the subsequent fastening points are located by searching for the closest point on the specified surface or surfaces. The fastening points in this method may be located on the edge of a surface. Figure 34.3.4–5 shows attachments for the edge-to-edge projection method. Input File Usage: *FASTENER, REFERENCE NODE SET=node set label, ATTACHMENT METHOD=EDGETOEDGE blank line First fastening point Positioning point Subsequent fastening point Figure 34.3.4–5 Edge-to-edge projection method to locate fastening points for abutting surfaces. Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: select positioning points: Criteria: Attachment method: Edge-to-Edge Specifying the surfaces to be fastened Once the positioning points have been specified, the surfaces to be fastened can be specified using two different approaches. In the first approach you directly specify the surfaces that are to be connected with a fastener. In the second approach you specify a search zone, and Abaqus automatically identifies the surfaces that are to be connected. However, in the second approach Abaqus does not distinguish between coincident facets. Hence, if coincident facets are to be fastened, you should specify distinct surfaces containing each of the coincident facets and use the first approach. Only element-based surfaces defined on faces can be fastened together . Forming fasteners on user-specified surfaces If you specify multiple surfaces as part of the interaction definition, the surfaces to be fastened are restricted to these surfaces. In general, specifying multiple surfaces is the preferred way of defining fasteners; this method leads to a more precise fastener construct definition. The number of layers of each fastener is one less than the number of surfaces specified. One fastening point is found on each surface. Input File Usage: *FASTENER first data line surface1, surface2, surface3, etc. Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Domain: Approach: Fasten specified surfaces by proximity, select surfaces When you select multiple surfaces for a single surface region, Abaqus/CAE combines the multiple surfaces using the single-surface search method, as described in “Forming fasteners on surfaces inside a user-specified search zone” below. Controlling connectivity of fasteners on user-specified surfaces By default, the connectivity of the fastening points is determined by their relative position along the fastener projection direction. For example, the default connectivity for the two-layer example shown in Figure 34.3.4–1 connects fastening point A to point B (layer 1) and point B to point C (layer 2). You can control the connectivity of the fastening points when the fasteners are formed on user- specified surfaces. You can specify that the connectivity of the fastening points be defined by the order in which you specified their associated surfaces. Input File Usage: *FASTENER, UNSORTED first data line surface1, surface2, surface3, etc. If user-specified surfaces are not included on the data lines, the UNSORTED parameter is ignored. Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Domain: Approach: Fasten in specified order, select surfaces Forming fasteners on surfaces inside a user-specified search zone If you do not specify any surfaces as part of the interaction definition, Abaqus searches for fastening points on all element facets that fall within a sphere of user-specified radius R with its center at the positioning point. If you do not specify the search radius, Abaqus computes a default search radius based on five times the facet thickness (for shell element facets) or the characteristic element length (for other element types) in the vicinity of each positioning point. To refine the search, you can specify a single surface definition that will limit the facet search to element facets belonging to that surface. In this case you must define a collective surface that includes at least each connected surface. A combined surface can also be used . To refine the search further, you can specify a positive integer value, N, for the number of layers of each fastener. Abaqus searches for the fastening points closest to the positioning point. If BEAM MPCs are used to model the fastener, a warning message is issued if the requisite number of fastening points is not found. However, if connector elements are used to model the fastener and the requisite number of fastening points is not found, Abaqus issues an error message. Thus, when specifying the number of layers, you should ensure that the search radius has been specified such that fastening points can be found. If multiple surfaces are listed as part of the fastener definition, the number of layers for each fastener is ignored. If a user-specified search radius is used for the multiple surface case, Abaqus searches for fastening points on all facets belonging to each of the listed surfaces that fall within a sphere of user- specified radius R with its center at the positioning point. Facets of the listed multiple surfaces that lie outside this sphere are not included in the search. A maximum of 15 layers can be specified for a particular fastener definition. Input File Usage: *FASTENER, SEARCH RADIUS=R, NUMBER OF LAYERS=N first data line Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Criteria: Search radius: Specify: R, Maximum layers for projection: Specify: N Defining the radius of influence Each fastening point is associated with a group of nodes on the surface in the immediate neighborhood of the fastening point called a region of influence. The motion of the fastening point is then coupled in a weighted sense to the motion of the nodes in this region by a distributed coupling constraint. Several weighting options are available and are discussed in the next section. To define the region of influence, Abaqus computes an internal radius of influence based on the geometric properties of the fastener, the characteristic length of the connected facets, and the type of weighting function used. The default radius of influence is always chosen to be the largest of the internally computed radius of influence, the physical fastener radius, and the distance of the projection point to the closest node. You can also specify the desired radius of influence. However, Abaqus overrides a user-specified radius of influence that is smaller than the computed default radius of influence. In any case each region of influence will contain a minimum of three nodes. Input File Usage: *FASTENER, RADIUS OF INFLUENCE=distance blank line Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Adjust: Influence radius: Specify: distance Defining the weighting method The weighting methods available for the distributed coupling constraints created for a fastener interaction are the same as those available for the surface-based coupling constraints in Abaqus . Besides an area-based uniform weighting scheme, various weighting methods are provided that monotonically decrease with radial distance from the fastening point: linear, quadratic, and cubic polynomial weight distributions. By default, Abaqus uses the uniform weighting method. You can modify the default weighting distribution. The default radius of influence calculated by Abaqus is larger for higher-order weighting methods since the resulting weights for nodes away from the fastening point contribute comparatively little to the motion of the fastening point. Hence, to ensure that there is a sufficient “smearing” effect, it becomes necessary to increase the number of nodes in the region of influence by increasing the size of the default radius of influence. In comparison, for a uniform weighting scheme, surface nodes away from the fastening point contribute significantly to the motion of the fastening point. For this case the default radius of influence chosen can be comparatively small, since even with a small number of nodes in the region of influence, the smearing effect is sufficiently strong. If fewer than three cloud nodes are found, increasing the radius of influence may help in forming the fastener by including more nodes in the cloud of coupling nodes. Use the following option to specify a uniform weight distribution: MESH-INDEPENDENT FASTENERS *FASTENER, WEIGHTING METHOD=UNIFORM blank line Use the following option to specify a linear weight distribution: *FASTENER, WEIGHTING METHOD=LINEAR blank line Use the following option to specify a quadratic polynomial weight distribution: *FASTENER, WEIGHTING METHOD=QUADRATIC blank line Use the following option to specify a cubic polynomial weight distribution: *FASTENER, WEIGHTING METHOD=CUBIC blank line Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Formulation: Weighting method: Uniform, Linear, Quadratic, or Cubic Defining the fastener orientation Each fastener is formulated in a local coordinate system that rotates with the motion of the fastener. By default, Abaqus defines the local system by projecting the global coordinate system onto the surfaces that are being fastened according to the usual convention for surfaces in space . Local directions specified in this manner are such that the local z-axis for each fastener is normal to the surface that is closest to the reference node for the fastener. You can override the default local system by specifying a local coordinate system for the fastener interaction. Generally, the user-defined orientation should be such that the local z-axis of the orientation is approximately normal to the surfaces that are being connected and the local x- and y-axes are approximately tangent to the surfaces that are being connected. By default, Abaqus adjusts the user-defined orientation such that the local z-axis for each fastener is normal to the surface that is closest to the reference node for the fastener. In cases where you wish to define the local directions precisely, you can specify that Abaqus should not adjust them. Fasteners support only rectangular, cylindrical, and spherical orientation definitions. Additional rotations defined as part of the orientation definition are ignored. In geometrically nonlinear analysis steps the local directions rotate with the motion of the fastener reference node. Local coordinate system when connector elements are used If a connector element is used to model a fastener, the local coordinate system defined on the connector section, , to determine the final local coordinate system of the connector element, , operates on the local coordinate system for the fastener, . In other words, and In the above equations are assumed to be orthogonal rotation matrices with the local 1-, 2-, and 3-directions being the first, second, and third rows, respectively. The local coordinate system for a connector element modeling a fastener should be specified with respect to the local coordinate system of the fastener. The orientation displayed in the Visualization module of Abaqus/CAE (Abaqus/Viewer) is at all fastener locations unless you specify not to write the orientations to the database; in this case, only is displayed. If connector field output is requested, field output for additional nodal rotation at the connector nodes is generated automatically to ensure that the appropriate connector orientation directions are displayed as the analysis progresses. Otherwise, the orientation computed at the beginning of the analysis is displayed at all times with the updated orientations used for computation purposes. For example, suppose you use a HINGE connector and want the released rotational degree of freedom, which is in the connector’s local 1-direction, to be normal to the surfaces that are being fastenened. If the default local coordinate system is used for the fastener (local 3-direction normal to the surface), the local 1-direction for the connector should be set to (0., 0., 1.); i.e., the local 3-direction of the fastener. When compounded with the local coordinate system for the fastener, the local 1-direction for the connector will be normal to the surface. See “Mesh-independent spot welds,” Section 5.1.16 of the Abaqus Verification Manual, for an example of a compounded orientation. Input File Usage: *FASTENER, ORIENTATION=orientation name, ADJUST ORIENTATION=NO blank line Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Adjust: Fastener CSYS: Edit: select local coordinate system, toggle off Adjust CSYS to make local Z-axis normal to closest surface Clarifications regarding the computation of A few clarifications regarding the default definition of are necessary for a precise understanding of the behavior when connector elements are used to model fasteners. The positioning point is always projected on the closest surface to be fastened. Therefore, the choice of coordinates of the reference node relative to the stack of surfaces to be fastened determines which surface is used to compute the local directions. Typically this choice does not matter much in realistic applications because the surfaces to be fastened are more or less parallel to each other in the fastener area. The projection of the reference node on the closest surface generates a fastening point for the connector element. The local z-axis for each fastener ( ) is normal to the surface at this fastening point. The fastening point generated on the closest surface is by default the first fastening point and, therefore, the first connector node. The precise direction into which the local z-axis is pointing is chosen such that the dot product with the unit vector pointing from the first node of the connector to the second node of the connector is positive. As explained above, you can control the connectivity of the fastening points in the connectors by specifying unsorted surfaces. Therefore, you can control the precise direction the local z-axis is pointing along the surface normal by either selecting appropriate coordinates for the reference node and/or by using unsorted surfaces. The two tangential directions in are computed by default according to the usual convention for surfaces in space . The global X-axis is projected onto the closest surface at the location of the fastening point to determine the local x-axis in . If the global X-axis is within 0.1 degrees of being normal to the surface, the local x-axis in is the projection of the global Z-axis on the closest surface. The local y-axis in is then at right angles to the local x-axis and z-axis so that the three local axes form a right-handed set. In the rare cases when the default definition of does not suit your application, you can always specify the orientation directly. Common modeling practices In most applications the default choice for at both connector nodes would result in a combined with a choice of global system for that is most suitable. The connection type that you choose depends on several modeling considerations, but very often the BUSHING connection type offers the best choice. To simplify the discussion, consider that only two surfaces are being fastened, a very common situation as illustrated in the spot weld example in “Connector functions for coupled behavior,” Section 31.2.4. For this common choice, has the local z-axis normal to the closest surface and pointing from the first fastening point (first connector node) toward the second fastening point (second connector node). This choice ensures that for a fastener subjected to a tension load (fastened plates pulled apart) a positive force always develops in the connector along the local z-axis (CTF3) regardless of the choice of coordinates for the positioning point and/or use of unsorted surfaces. Conversely, if a compression load is applied (fastened plates pressed against each other), a negative force develops in the connector. In most cases, the behavior in the tangential plane defined by the local x- and local y-axes is isotropic; therefore, the precise orientation of these two axes is of less interest to you. The spot weld example in “Connector functions for coupled behavior,” Section 31.2.4, illustrates such a typical case where the (isotropic) magnitude of two in-plane forces ( ) are used in the kinetic behavior of the connector element. ) and of the two moments ( If you need to specify anisotropic behavior in the tangential plane, you need to understand precisely how the directions in are defined. As explained above, the choice of coordinates for the positioning point relative to the stack of surfaces to be fastened and/or use of unsorted surfaces determines the precise direction of the default local axes. In most cases you have two common modeling choices. In the first case you can specify the coordinates of the positioning points to be exactly on or very close to the surface onto which the first fastening points (connector nodes) are to be placed and use the default sorted surfaces. In this case you do not need to specify the surfaces to be fastened individually. However, in many practical situations imprecise geometry for the surfaces to be fastened and/or inexact coordinates of the fastener reference nodes make the consistent placement of the reference nodes in the vicinity of one particular surface very hard to accomplish. The second modeling technique consists of using sorted surfaces. The exact location of the reference node with respect to the surface stack to be fastened is not that important because the first fastening point is always on the first specified surface. In this case you do have to specify two or more individual surfaces to be fastened. In the rare cases when neither of these modeling techniques suits your application, you can specify the fastener orientation directly to match your needs exactly. Defining the surface coupling method There are two methods available to couple the motion of each fastening point to the motion of the associated coupling nodes on the fastened surfaces: the continuum coupling method and the structural coupling method. The continuum coupling method is used by default. In many cases when the pair of fastened surfaces are close to each other, unrealistic contact interactions may occur between the two surfaces if the continuum coupling method is used. This is particularly the case in shell bending applications. Moreover, in many situations the continuum coupling method can yield an overly stiff response if the two surfaces are pried apart, especially when the fastener radius is small. The structural coupling method can be used to alleviate these issues. Continuum coupling method The default continuum coupling method couples the translation and rotation of each fastening point to the average translation of the group of coupling nodes on each of the fastened surfaces. The constraint distributes the forces and moments at the fastening point as a coupling node-force distribution only. The force distribution is equivalent to the classic bolt pattern force distribution when the weight factors are interpreted as bolt cross-section areas. For each pair of fastening point and group of coupling nodes, the constraint enforces a rigid beam connection between the fastening point and a point located at the weighted center of position of the coupling nodes. The formulation is discussed in detail in “Distributing coupling elements,” Section 3.9.8 of the Abaqus Theory Manual. Input File Usage: *FASTENER, COUPLING=CONTINUUM Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Formulation: Coupling type: Continuum distributing Structural coupling method The structural coupling method couples the translation and rotation of each fastening point to the translation and the rotation motion of the group of coupling nodes on each of the fastened surfaces. The constraint distributes forces and moments at the fastening point as coupling nodes forces and moments. For this coupling method to be active, all rotation degrees of freedom at all coupling nodes must be active (as would be the case when shells are fastened together) and all degrees of freedom must be constrained (which is the default; see “Defining fastener properties” below). With respect to translations, for each pair of fastening point and group of coupling nodes, the constraint enforces a rigid beam connection between the fastening point and a moving point that remains at all times in the vicinity of the fastened surface. The location of this moving point is determined by the current curvature of the surface, the current location of the weighted center of position of the coupling nodes, and the fastener projection direction. This choice avoids unrealistic contact interactions between the fastened surfaces when the surfaces are close to each other (typically the case). With respect to rotations, for each pair of fastening point and group of coupling nodes, the constraint is different along different local directions. Along the projection direction (the twist direction), the constraint is identical to the one enforced via the continuum coupling method . By contrast, the rotational constraint in the plane perpendicular to the projection direction relates the in-plane fastening point rotations to the in-plane rotations of the coupling nodes in the immediate vicinity of the fastening point. This choice provides a more realistic response when the fastened surfaces are pried apart. Input File Usage: Abaqus/CAE Usage: *FASTENER, COUPLING=STRUCTURAL Interaction module: Special→Fasteners→Create: Point-based: Formulation: Coupling type: Structural distributing Defining fastener properties Each fastener interaction definition must refer to a property, which defines the geometric section properties of the fastener. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *FASTENER, PROPERTY=fastener property name *FASTENER PROPERTY, NAME=fastener property name Interaction module: Special→Fasteners→Create: Point-based: Property Geometric section quantities Fasteners are assumed to have a circular projection onto the connected surfaces. You are required to specify the radius of the fastener. Input File Usage: *FASTENER PROPERTY Abaqus/CAE Usage: Interaction module: Special→Fasteners→Create: Point-based: Property: Physical radius: r Mass In many cases fasteners may add mass to the assembly. To model the added mass, specify an additional mass that is assigned to each fastener and lumped to the fastening points. *FASTENER PROPERTY, MASS=mass value Interaction module: Special→Fasteners→Create: Point-based: Property: Additional mass: mass value Abaqus/CAE Usage: Input File Usage: Releasing degrees of freedom on fasteners using connector elements For fasteners modeled with connector elements, translational as well as rotational degrees of freedom can be released by prescribing connector section types that have unconstrained (available) degrees of freedom. For example, a HINGE connector can be used to release the rotational degree of freedom in the connector’s local 1-direction. Releasing degrees of freedom on fasteners using BEAM MPCs For fasteners modeled with BEAM MPCs, the moment constraint between the rotation degrees of freedom at the fastening points and the average rotation of the coupling nodes can be released in one, two, or three directions. You can specify the moment constraint directions in the default local coordinate system or a user-defined local coordinate system. The three translational degrees of freedom at the fastening points are always coupled to the average translation of the coupling nodes. You specify the degrees of freedom of the fastening point to be coupled to the average motion of the coupling nodes as part of the fastener property definition. If no degrees of freedom are specified as part of the fastener property definition, all six degrees of freedom are coupled. If you specify one or more degrees of freedom but not all available translation degrees of freedom, Abaqus issues a warning message and adds all the available translation degrees of freedom to the constraint. If a user-specified local orientation is specified for the fastener interaction, the local degrees of freedom are with respect to the user-defined coordinate system. *FASTENER PROPERTY section properties first dof, last dof Input File Usage: For example, if the default local coordinate system is used, the following property definition would release the relative rotation constraint of the connected parts about the surface normal: *FASTENER PROPERTY section properties 1, 5 The above property definition might be used to approximate a riveted connection. Abaqus/CAE always constrains all translational degrees of freedom in a fastener. Use the following input to remove constraints on the rotational degrees of freedom: Interaction module: Special→Fasteners→Create: Point-based: Formulation: toggle off UR1, UR2, or UR3 Abaqus/CAE Usage: Overconstraints in fasteners modeled with BEAM MPCs There are several instances in which a model with fasteners modeled with BEAM MPCs might be overconstrained. Described below are two potential overconstraints that Abaqus automatically attempts to detect and resolve during solver input file processing. Fasteners and rigid bodies Fasteners can be used to connect both deformable and rigid element-based surfaces. However, if the fasteners are modeled with BEAM MPCs, potential overconstraints may arise if more than one rigid surface is involved in a given fastener definition. Abaqus automatically attempts to remove these types of overconstraints by allowing at most one rigid surface in any individual fastener definition. A warning message is generated if an overconstraint of this type is detected. For example, suppose surfaces A and C in Figure 34.3.4–1 are part of the same rigid body, and surface B is deformable. Abaqus automatically removes either surface A or surface C from the fastener definition and only forms the fastener between the deformable surface and the remaining rigid surface. If surface A and surface C belong to two separate rigid bodies, their respective rigid body reference nodes will be joined by an internally generated BEAM MPC. In another example, suppose all three surfaces in Figure 34.3.4–1 are rigid. In this case no fastener will be formed, and the unique rigid body reference nodes for surfaces A, B, and C will be joined by beam MPCs. Unresolvable overconstraints may arise if inconsistent kinematic constraints (such as displacement boundary conditions) are placed on rigid body reference nodes that have been joined by BEAM MPCs. In this case you must modify the model to resolve the overconstraints. Possible courses of action include removing some of the rigid surfaces from the fastener definitions or removing inconsistent kinematic conditions on the rigid body reference nodes. The above-described procedure to resolve overconstraints with fasteners and rigid bodies will preserve the kinematics of the original model. In Abaqus/Standard you can bypass the overconstraint checks and prevent automatic model modifications in the model preprocessor . Overlapping fasteners Potential overconstraints exist with rigid fasteners if all the coupling nodes of any associated distributing coupling element are wholly contained within one or more other fastener definitions. This can happen if the spacing between positioning points is small compared to the typical element size in a mesh (which is often the case in automotive models). To avoid overconstraints in this situation, Abaqus uses a penalty formulation for all fastener distributing coupling elements that satisfy the above criteria. The penalty distributing coupling formulation relaxes, to a small degree, the constraint between the motion of the distributing coupling element reference node and its coupling nodes. Output If fasteners are modeled using connector elements, connector element output variables can be used to request output for fasteners . No fastener output is available if the fasteners are modeled using BEAM MPCs. 34.4 Embedded elements • “Embedded elements,” Section 34.4.1 34.4.1 EMBEDDED ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Kinematic constraints: overview,” Section 34.1.1 • *EMBEDDED ELEMENT • “Defining embedded region constraints,” Section 15.15.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The embedded element technique: • is used to specify an element or a group of elements that lie embedded in a group of host elements whose response will be used to constrain the translational degrees of freedom of the embedded nodes (i.e., nodes of embedded elements); • can be used in geometrically linear or nonlinear analysis; • is not available for host elements with rotational degrees of freedom; • can be used to model a set of rebar-reinforced membrane, shell, or surface elements that lie embedded in a set of three-dimensional solid (continuum) elements; a set of truss or beam elements that lie embedded in a set of solid elements; or a set of solid elements that lie embedded in another set of solid elements; • will not constrain rotational degrees of freedom of the embedded nodes when shell or beam elements are embedded in solid elements; and • can be imported from Abaqus/Standard into Abaqus/Explicit and vice versa. Introduction The embedded element technique is used to specify that an element or group of elements is embedded in “host” elements. The embedded element technique can be used to model rebar reinforcement. Abaqus searches for the geometric relationships between nodes of the embedded elements and the host elements. If a node of an embedded element lies within a host element, the translational degrees of freedom at the node are eliminated and the node becomes an “embedded node.” The translational degrees of freedom of the embedded node are constrained to the interpolated values of the corresponding degrees of freedom of the host element. Embedded elements are allowed to have rotational degrees of freedom, but these rotations are not constrained by the embedding. Multiple embedded element definitions are allowed. Available embedded element types Different element types can be used in the element set containing embedded elements and the element set containing the host elements. However, all the host elements can have only translational degrees of freedom, and the number of translational degrees of freedom at a node on the embedded element must be identical to the number of translational degrees of freedom at a node on the host element. The following general types of “embedded elements-in-host elements” are provided: • Two-dimensional models: – Beam-in-solid – Solid-in-solid – Truss-in-solid • Axisymmetric models: – Membrane-in-solid (Abaqus/Standard only) – Shell-in-solid – Solid-in-solid – Surface-in-solid (Abaqus/Standard only) • Three-dimensional models: – Beam-in-solid – Membrane-in-solid – Shell-in-solid – Solid-in-solid – Surface-in-solid – Truss-in-solid Specifying the host elements By default, the elements in the vicinity of the embedded elements are searched for elements that contain embedded nodes; the embedded nodes are then constrained by the response of these host elements. To preclude certain elements from constraining the embedded nodes, you can define a host element set; the search will be limited to this subset of the host elements in the model. This feature is strongly recommended if the embedded nodes are close to discontinuities in the model (cracks, contact pairs, etc.). Input File Usage: *EMBEDDED ELEMENT, HOST ELSET=name The *EMBEDDED ELEMENT option must be included in the model definition portion of the input file. Multiple *EMBEDDED ELEMENT options are allowed. Abaqus/CAE Usage: Interaction module: Create Constraint: Embedded region: choose Select Region from the prompt area when selecting the host region Specifying the embedded elements You must specify the embedded elements. Individual elements or element sets can be specified. An embedded element may share some nodes with host elements. These nodes, however, will not be considered to be embedded nodes. Input File Usage: *EMBEDDED ELEMENT embedded elements Abaqus/CAE Usage: Interaction module: Create Constraint: Embedded region: select the embedded region Defining geometric tolerances A geometric tolerance is used to define how far an embedded node can lie outside the regions of the host elements in the model. By default, embedded nodes must lie within a distance calculated by multiplying the average size of all non-embedded elements in the model by 0.05; however, you can change this tolerance. You can define the geometric tolerance as a fraction of the average size of all non-embedded elements in the model. Alternatively, you can define the geometric tolerance as an absolute distance in the length units chosen for the model. If you specify both exterior tolerances, Abaqus uses the tighter tolerance of the two. The average size of all the non-embedded elements is calculated and multiplied by the fractional exterior, which is then compared to the absolute exterior tolerance to determine the tighter tolerance of the two. The exterior tolerance for embedded elements in host elements is indicated by the shaded region in Figure 34.4.1–1. Nodes on the host elements Nodes on the embedded elements Edges of the host elements Edges of the embedded elements Figure 34.4.1–1 The exterior tolerance for embedded elements. If an embedded node is located inside the specified tolerance zone, the node is constrained to the host elements. The position of this node will be adjusted to move the node precisely onto the host elements. If an embedded node is located outside the specified tolerance zone, an error message will be issued. Input File Usage: Use the following option to define the tolerance as a fraction: *EMBEDDED ELEMENT, EXTERIOR TOLERANCE=tolerance Use the following option to define the tolerance as an absolute distance: *EMBEDDED ELEMENT, ABSOLUTE EXTERIOR TOLERANCE=tolerance Abaqus/CAE Usage: Interaction module: Create Constraint: Embedded region: Fractional exterior tolerance or Absolute exterior tolerance Adjusting the positions of embedded nodes If an embedded node lies close to an element edge or an element face within a host element, it is computationally efficient to make a small adjustment to the position of the embedded node so that the node will lie precisely on the edge or face of the host element. A small tolerance, below which the weight factors of the nodes on a host element associated with an embedded node will be zeroed out, is defined. The small weight factors will be redistributed to the other nodes on the host element in proportion to their initial weights, and the position of the embedded node will be adjusted based on the new weight factors. This adjustment is performed only at the start of the analysis and does not create any strain in the model. It is most useful for making small adjustments to make the embedded nodes lie on the edge or face of a host element. If a large nondefault value of the roundoff tolerance is used to make significant adjustments to the positions of the embedded nodes, you should carefully review the mesh obtained after adjusting. Input File Usage: Abaqus/CAE Usage: *EMBEDDED ELEMENT, ROUNDOFF TOLERANCE=tolerance Interaction module: Create Constraint: Embedded region: Weight factor roundoff tolerance Use with other multiple kinematic constraints If an embedded node is also tied by multi-point, equation, kinematic coupling, surface-based tie, or rigid body constraints, an overconstraint is introduced and an error message will be issued. If a boundary condition is applied to an embedded node, the embedded element definition always takes precedence. The boundary condition will be neglected, and a warning message will be issued. Defining surfaces on embedded elements Embedded elements have no exterior (free) surface due to the embedding. Consequently, their faces are not part of the all-inclusive surface defined automatically for interactions modeled with general contact. In addition, any surface definitions based on these elements must have the face identifier specified explicitly . Limitations The following limitations exist for the embedded element technique: • Elements with rotational degrees of freedom (except axisymmetric elements with twist) cannot be used as host elements. • Rotational, temperature, pore pressure, acoustic pressure, and electrical potential degrees of freedom at an embedded node are not constrained. • Host elements cannot be embedded themselves. • The material defined for the host element is not replaced by the material defined for the embedded element at the same location of the integration point. • Additional mass and stiffness due to the embedded elements are added to the model. • If modified tetrahedron elements are used as host elements, only the corner nodes are used to constrain the appropriate embedded nodes. Example Consider the example in Figure 34.4.1–2. 1 3 Nodes on the host elements Nodes on the embedded elements Edges of the host elements Edges of the embedded elements Figure 34.4.1–2 Elements lie embedded in host elements. Elements 3 (truss) and 4 (membrane) lie embedded in elements 1 and 2. Element 1 is formed by nodes a, b, c, d, e, f, g, and h; element 2 is formed by nodes e, f, g, h, i, j, k, and l; element 3 is formed by nodes A and B; and element 4 is formed by nodes C, D, E, and F. If the host element set includes elements 1 and 2 and the embedded element sets contain elements 3 and 4, respectively, Abaqus will attempt to find if there are any embedded nodes (A, B, C, D, E, and F) lying within host elements 1 or 2. If node A is found to be lying close to the a-b-f-e face of element 1, all the degrees of freedom at node A are constrained to nodes a, b, f, and e, with appropriate weight factors being determined based on the geometric location of node A in element 1. Similarly, if node B is found to be lying inside element 1 and node E is found to be lying close to the g–k edge of element 2, respectively, all the degrees of freedom at node B are constrained to nodes a, b, c, d, e, f, g, and h, and all the degrees of freedom at node E are constrained to nodes g and k, with appropriate weight factors being determined based on the geometric location of node B in element 1 and the geometric location of node E on the g–k edge of element 2, respectively. You should make sure that all the nodes on the embedded elements are properly constrained to nodes on the host elements. This can be verified by performing a data check analysis . For each embedded node a list of nodes that are used to constrain this node and the associated weight factors are output to the data file during the data check analysis. An error message is issued if an embedded node is not constrained. Template *HEADING … *NODE Data line to define the nodal coordinates *ELEMENT, TYPE=C3D8, ELSET=SOLID3D Data line to define the solid elements *ELEMENT, TYPE=T3D2, ELSET=TRUSS Data line to define the truss elements *ELEMENT, TYPE=M3D4, ELSET=MEMB Data line to define the membrane elements *EMBEDDED ELEMENT, EXTERIOR TOLERANCE=tolerance, HOST ELSET=SOLID3D TRUSS, MEMB *STEP *STATIC (or any other allowable procedure) Data line to define step time and control incrementation … *END STEP 34.5 Element end release • “Element end release,” Section 34.5.1 34.5.1 ELEMENT END RELEASE Product: Abaqus/Standard References • “Kinematic constraints: overview,” Section 34.1.1 • *RELEASE Overview Element end release: • allows a rotational degree of freedom or a combination of rotational degrees of freedom to be released at one or both ends of an element or element set; • can be used in geometrically linear or nonlinear analysis; and • is available only for beam and pipe elements in Abaqus/Standard. Introduction Element end release is used to model hinged connections (hinged in one, two, or three orthogonal directions) at one or both ends of the element. By releasing rotational degrees of freedom, an element end is allowed to rotate freely relative to the node about the chosen degrees of freedom. Any rotational degrees of freedom that are not released are shared with the node. You must be careful not to release a given degree of freedom at a node for all elements that share that node; otherwise, the node has no stiffness for that degree of freedom and Abaqus/Standard issues zero pivot warning messages. Element end release operates on the element local degrees of freedom. See “Beam element cross- , t) for beam-type elements. -axis, the -axis, and the rotation about the local t-axis for beams in space. For beams -axis is active (which coincides with rotations about the section orientation,” Section 29.3.4, for a definition of the local axes ( The rotational degrees of freedom affected by the release are the rotation about the local rotation about the local in a plane, only the rotation about the local negative global z-axis). , Equivalent MPCs If only one rotational degree of freedom is released, the kinematic constraint is equivalent to MPC type REVOLUTE plus MPC type PIN between two nodes. If two rotational degrees of freedom are released, the kinematic constraint is equivalent to MPC type UNIVERSAL plus MPC type PIN. If all rotational degrees of freedom are released, the kinematic constraint is equivalent to MPC type PIN. See “General multi-point constraints,” Section 34.2.2, for details. Identifying the element end involved in the release Either element sets or individual elements can be specified for a release definition. Degrees of freedom can be released at the first, second, or first and second ends of an element. The first end of the element, S1, is node 1 on the element as defined by the element connectivity; the second end, S2, is the last node (node 2 or 3, as appropriate) on the element. See “Beam element library,” Section 29.3.8, for a definition of the node ordering for beam elements. Identifying the local rotational degrees of freedom involved in the release Rotation combination codes rather than degrees of freedom are specified to identify the rotational degrees of freedom involved in the release. M1 M2 refers to the rotation about the refers to the rotation about the -axis, -axis, M1-M2 refers to a combination of rotational degrees of freedom about the -axis and the -axis, M1-T M2-T refers to the rotation about the t-axis, refers to a combination of rotational degrees of freedom about the refers to a combination of rotational degrees of freedom about the -axis and the t-axis, -axis and the t-axis, and ALLM represents a combination of all the rotational degrees of freedom (i.e., M1, M2, and T). Input File Usage: *RELEASE element number or element set, element end ID, release combination code -axis at the For example, to release the rotational degree of freedom about the first end of element 10 and all the rotational degrees of freedom at the second end of the element, use the following input: *RELEASE 10, S1, M1 10, S2, ALLM Use with transformed coordinate systems Transformations applied to released nodes (“Transformed coordinate systems,” Section 2.1.5) have no influence on the release. The release operates on the local degrees of freedom for the element. Reading the data from an alternate input file The data for a release definition can be contained in a separate input file. Input File Usage: *RELEASE, INPUT=file_name If the INPUT parameter is omitted, it is assumed that the data lines follow the keyword line. 34.6 Overconstraint checks • “Overconstraint checks,” Section 34.6.1 34.6.1 OVERCONSTRAINT CHECKS Product: Abaqus/Standard References • “Rigid body definition,” Section 2.4.1 • “Connectors: overview,” Section 31.1.1 • “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1 • “General multi-point constraints,” Section 34.2.2 • “Mesh tie constraints,” Section 34.3.1 • “Coupling constraints,” Section 34.3.2 • “Mesh-independent fasteners,” Section 34.3.4 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • *BASE MOTION • *CONSTRAINT CONTROLS Overview An overconstraint means applying multiple consistent or inconsistent kinematic constraints. Many models have nodal degrees of freedom that are overconstrained. Such overconstraints may lead to inaccurate solutions or nonconvergence. Common examples of situations that may lead to overconstraints include (but are not limited to): • contact slave nodes that are involved in boundary conditions or multi-point constraints; • edges of surfaces involved in a surface-based tie constraint that are included in contact slave surfaces or have symmetry boundary conditions; and • boundary conditions applied to nodes already involved in coupling or rigid body constraints. The overconstraint checks performed in Abaqus/Standard: • check for overconstraints caused by combinations of the following: base motions, boundary conditions, contact pairs, coupling constraints, linear constraint equations, mesh-independent spot welds, multi-point constraints, rigid body constraints, and surface-based tie constraints; • check for overconstraints resulting from kinematic constraints introduced through connector elements, coupling elements, special-purpose contact elements, and elements with incompressible material behavior; • identify through detailed messages the constraints that cause overconstraints; • automatically resolve a limited set of consistent overconstraints detected during model preprocessing and during an Abaqus/Standard analysis; • use the equation solver to detect overconstraints that cannot be resolved automatically; and • can have the default behavior modified. Overconstraints: general remarks In general, the term overconstraint refers to multiple constraints acting on the same degree of freedom. Overconstraints are then categorized as consistent (if all the constraints are compatible with each other) or inconsistent (if the constraints are incompatible with each other). Consistent overconstraints are also called redundant constraints, and inconsistent overconstraints are also called conflicting constraints. In Abaqus/Standard the following types of constraints, in combination, may lead to overconstraints: • boundary conditions or base motions, • contact pairs, • coupling constraints, • mesh-independent spot welds, • multi-point constraints or linear constraint equations, • surface-based tie constraints, and • rigid body constraints. In addition to these constraints the following elements impose kinematic constraints and, when used in combination with each other or with the above constraints, may lead to overconstraints: • connector elements, • special-purpose contact elements, and • hybrid elements for incompressible material response. An illustration of several consistent overconstraints is given in Figure 34.6.1–1. The upper block is built from three separately meshed regions, which are connected together using a surface-based tie constraint. This block is in contact with the lower rigid block, which is made rigid by specifying a rigid body constraint. The rigid block’s reference node is fixed. Symmetry boundary conditions are used at the left edge of the upper block, and rough friction is defined for the surface interaction between the upper and lower blocks. The following redundant constraints can be identified: • Intersecting tie constraints: At (A) three nodes share the same location, and their relative motions are constrained by two surface-based tie constraints (one vertical and one horizontal). Only two constraints (two dependent nodes and one independent node) are needed to fully constrain the motion of the three nodes, but three constraints are generated internally (one for the horizontal tie constraint and two for the vertical one). Therefore, one redundant constraint exists. • Tie constraint and symmetry boundary condition: At (B) nodes 141 and 151 have their motion constrained horizontally by the symmetry boundary condition, but their relative motion is also constrained by the surface-based tie constraint. Therefore, one redundant constraint exists. • Rough friction and symmetry boundary condition: At (C) node 101 is constrained horizontally by the symmetry boundary condition. The rough friction contact acts in the same direction as the boundary condition. Therefore, one redundant constraint exists. reference node + rigid punch tie constraints (A) symmetry boundary conditions (B) (C) 141 151 101 501 625 423 801 301 rigid body reference node for lower block + rough friction (D) symmetry line Figure 34.6.1–1 Model with redundant constraints. • Tie constraint and contact interactions: At (D) nodes 801 and 301 are involved in the surface-based tie constraint, but two contact constraints (one at each node) act in the vertical direction. Therefore, one redundant constraint exists. Even in this simple model the number of redundant constraints is surprisingly large. If not appropriately accounted for, the redundant constraints can lead to convergence difficulties, even nonconvergence. Moreover, in the cases when a solution is obtained (despite the convergence difficulties), the reported reaction forces and contact pressures may be inaccurate. Abaqus/Standard checks for the inappropriate use of combinations of constraints for the majority of constraint and element types listed in this section. Depending on the complexity of the constraints involved, Abaqus/Standard identifies three classes of consistent and inconsistent overconstraints. Overconstraints detected in the model preprocessor Many relatively simple overconstraints can be identified by inspecting the constraints defined If a consistent overconstraint is detected, the unnecessary constraints are eliminated at a node. automatically and a warning message is generated. If the overconstraints are inconsistent, the analysis is stopped and an error message is generated. Overconstraints detected and resolved in an Abaqus/Standard analysis Some overconstraints involving contact interactions may become overconstrained only during an analysis due to changes in contact status. Certain of these cases are detectable and eliminated automatically by Abaqus/Standard. Appropriate messages are issued. Overconstraints detected by the equation solver Many overconstraints involve complex interactions between various constraint definitions and element types. Automatic resolution of these situations may not be possible. In such cases the equation solver will detect the overconstraint, and a detailed message listing potential causes of the problem will be issued. Overconstraints detected in the model preprocessor In this section we consider overconstraints that involve two or more of the following: • surface-based tie constraints, • rigid body constraints, • boundary conditions, and • connector elements. While the number of cases handled automatically in the model preprocessor is limited, many often- encountered situations are corrected. The list of overconstraints to be resolved automatically in the preprocessor is organized based on the constraint types involved. Each case is illustrated by examples. Intersecting tie constraints Examples of intersecting tie constraint definitions are shown in Figure 34.6.1–2. In both cases there is at least one node that, if not properly treated, will be redundantly constrained. In the case on the left, the three edges belonging to the three surfaces overlap (shown here in an exploded view for clarity). Each of the three end nodes on either end occupy the same location. Therefore, one redundant tie constraint exists. In the case shown on the right, four adjacent meshes are “glued” together using four tie constraints. Only three constraints are needed to “glue” the center nodes together, but four are generated (one from each tie constraint). Therefore, one constraint is not needed and in both cases one constraint is removed. Tie constraint inside a rigid body constraint An example of a tie constraint inside a rigid body constraint is shown in Figure 34.6.1–3(a). Two surfaces are connected by a tie constraint, and the two element sets are included in the same rigid body. Since the motion of all the nodes is constrained to the motion of the rigid body’s reference node, the tie constraint is redundant. The tie constraint definition is removed from the model. tie constraint between faces AM–CD AB–HJ CE–FG HI–FN C J tie constraint between faces ABCD–IJKL EFGH–KLNM ABRS–EHPO nodes B, H, K are at the same location F N (a) nodes A, E, L are at the same location (b) Figure 34.6.1–2 Consistent overconstraints due to intersecting tie constraints. rigid body includes all elements tie constraint along this line tie constraint tie constraint deformable rigid element set 2 element set 1 rigid body 1 rigid body 2 reference node 1 reference node 2 + + internally generated connector element (a) (b) (c) Figure 34.6.1–3 Consistent overconstraints due to combinations of tie and rigid body constraints. Tie constraint between two rigid bodies An example of a tie constraint between two rigid bodies is shown in Figure 34.6.1–3(b). If the two surfaces are connected by a tie constraint at more than two or three points (in two- or three-dimensional analyses, respectively), the tie constraint definition is redundant. A connector type BEAM is placed between the two reference nodes, and the tie constraint is removed. Tie constraint between a deformable and a rigid body An example of connecting a deformable body to a rigid body with a surface-based tie constraint is shown in Figure 34.6.1–3(c). If the slave surface in the tie constraint definition belongs to the rigid body, the tie and the rigid body constraints are redundant for the slave nodes. If possible, Abaqus/Standard will switch the master and the slave surface in the tie constraint definition. If switching the master and the slave surfaces is not possible due to other modeling restrictions, an error message is issued and the analysis is stopped. Intersecting rigid bodies Figure 34.6.1–4(a) illustrates the case when two rigid bodies partially overlap and, thus, the union of the two bodies behaves as one rigid body. However, the motion of the nodes in this region is governed by the motion of the two rigid body reference nodes; hence, the model is overconstrained. In Figure 34.6.1–4(b) several rigid bodies are included in a larger rigid body definition. The nodes belonging to the included bodies will be overconstrained. reference node 1 + reference node 2 rigid body 1 + internally generated connector element (type BEAM) rigid body 2 overlapping region rigid body 1 rigid body 2 reference node 1 reference node 2 + + (a) (b) Figure 34.6.1–4 Rigid body including other rigid bodies. In both cases the rigid body constraint will be enforced only once for the nodes that belong to several rigid bodies. To enforce the rigid behavior of the ensemble, connector elements of type BEAM are generated between the rigid body reference nodes to ensure a rigid connection between the intersecting rigid body definitions. Tie constraints and boundary conditions There are numerous cases of overconstraints when a surface-based tie constraint and a boundary condition are used together, as illustrated in Figure 34.6.1–5. tie constraint between faces BJIE and AFHK symmetry boundary conditions along 1-direction on the faces CDEB and AFGM tie constraint node a node b boundary condition of 0.1 at node a, dof 1 boundary condition of 0.2 at node b, dof 1 (a) (b) Figure 34.6.1–5 Overconstraints involving tie constraints and boundary conditions. In the first case nodes A and B are constrained to move together by the tie constraint. The vertical symmetry boundary conditions will constrain the motion of both nodes in the horizontal direction, generating one redundant constraint. In the second case the two specified boundary conditions conflict, thus generating a conflicting constraint. For every tie-dependent node with a boundary condition, Abaqus/Standard first determines which independent nodes are involved in the tie constraint . If only one independent node is involved, Abaqus/Standard will transfer the boundary conditions from the dependent node to the independent node. If conflicting boundary conditions are detected at the independent node during the transferring process, the analysis is stopped and an error message is issued. If several independent nodes are involved, Abaqus/Standard checks if the specified boundary conditions at all the nodes involved in the constraint are identical. If no conflicts are identified, the boundary conditions at the independent node are redundant and, therefore, ignored. Otherwise, an error message is issued, and the analysis is stopped. Rigid body constraints and boundary conditions Combinations of rigid body constraints and boundary conditions can lead to overconstrained models when boundary conditions are specified at nodes other than the reference node (Figure 34.6.1–6). In Figure 34.6.1–6(a) boundary conditions are specified at several nodes belonging to the rigid body. In Figure 34.6.1–6(b) symmetry boundary conditions are specified on the flat surface of the rigid body, and the body is spun around an axis perpendicular to the symmetry plane at the reference node. boundary conditions specified at nodes a, b, and c symmetry boundary conditions rigid body + face normal + reference node reference node (a) rigid body (b) Figure 34.6.1–6 Overconstraints due to boundary conditions applied at rigid body nodes. In case (a) if the specified boundary conditions are not consistent with the rigid constraint, the model will be inconsistently overconstrained. In case (b) if the reference node has the symmetry boundary conditions, there is no need to have symmetry boundary conditions at the nodes of the flat surface. Abaqus/Standard will attempt to remove all boundary conditions specified at the dependent nodes and redefine them at the reference node. To do so, the consistency of the boundary conditions specified at the dependent nodes is checked. If the boundary conditions are not identical, an error message is issued and the analysis is stopped (since otherwise the solution of a nonlinear system of equations would be required in the general case to assess whether the boundary conditions are consistent or not). Otherwise, Abaqus/Standard will try to merge the boundary conditions at the dependent nodes with those at the reference node by: • checking the consistency of the overlapping boundary conditions; • moving to the reference node any boundary conditions specified at the dependent nodes but not specified at the reference node; and • applying additional zero rotational boundary conditions at the reference node to compensate for the removed displacement constraints from the dependent nodes. To illustrate, refer to Figure 34.6.1–6(b): as the symmetry boundary conditions specified at the dependent nodes are consistent with each other, they are removed from the dependent nodes and applied to the reference node (boundary condition in the 2-direction). In addition, the symmetry constraints preclude rotations about the 1- and 3-directions; therefore, zero rotational boundary conditions are applied to the reference node about these axes. Connector elements and rigid bodies In most cases detection and automatic resolution of redundant constraints involving connector elements cannot be done by simple inspection of the constraints involved. However, the examples shown in Figure 34.6.1–7 are simple enough to be resolved automatically. It is assumed that the connector elements are connected to nodes on the rigid body whose rotational degrees of freedom are dependent on the rotation of the reference node. In Figure 34.6.1–7(a) the connector elements are assumed to enforce some kinematic constraints. They are redundant since the rigid body definition constrains the motion of all nodes to the motion of the rigid body’s reference node. Abaqus/Standard automatically removes the connector elements from the model. reference node connector rigid body composed of both ELSET1 and ELSET2 + connector reference node 1 + ELSET 1 ELSET 2 rigid body 1 rigid body 2 + reference node 2 connector (a) BEAM connector (b) Figure 34.6.1–7 Redundant constraints involving rigid bodies and connector elements. When connector elements are placed between two rigid bodies (as in Figure 34.6.1–7(b)), the model may be redundantly constrained. As shown in Figure 34.6.1–7(b), if a connector element of type BEAM (or WELD) is placed between two rigid bodies, the connection is rigid and any additional connector elements between the two rigid bodies are redundant. Abaqus/Standard will automatically remove these redundant connector elements. When the ensemble of connector elements placed between two rigid bodies enforces more than the necessary translational and rotational constraints between the two rigid bodies, but none of the connectors is of type BEAM (or WELD), only warning messages are issued to signal the overconstraint In these cases none of the connector elements can be eliminated automatically since the situation. connection between the two rigid bodies may become underconstrained. To illustrate this situation, assume that in Figure 34.6.1–7(b) the two connectors were of type SLOT and TRANSLATOR. Thus, four translational constraints (in three dimensions) are enforced between the two rigid bodies, rendering the system overconstrained since only three translational constraints are needed to fully constrain the relative translation between the two bodies. However, if the SLOT were eliminated from the model, the model would become underconstrained and different from the original one. Only a warning message is issued in this case. Coupling constraints and rigid bodies When all or some of the nodes involved in a kinematic coupling constraint belong to the same rigid body, the coupling constraint becomes redundant. The situation is illustrated in Figure 34.6.1–8. Node 101 is the reference node for the coupling constraint involving nodes 1001–1005. At the same time nodes 1001–1003 are included in the rigid body definition with reference node 102. rigid body 102 rigid body reference node 1001 1002 1003 1004 101 x coupling reference node 1005 Figure 34.6.1–8 Redundant constraints involving coupling constraints and rigid bodies. If the coupling constraint was defined as kinematic, it will not be enforced at nodes 1001–1003 to avoid overconstraining the model. The removed overconstraint may be inconsistent such as when incompatible boundary conditions are prescribed at the two reference nodes. However, the constraint will be enforced at nodes 1004 and 1005 since these nodes do not belong to the rigid body. If a distributing coupling constraint was used instead, the model would not be overconstrained. However, if node 101 was added to the rigid body definition and nodes 1004 and 1005 were not included in the coupling constraint, the model would be overconstrained. Indeed, all nodes involved in the coupling constraint would be already constrained by the rigid body definition, making the coupling constraint redundant. To avoid the overconstraint, Abaqus/Standard will not enforce the coupling constraint in this case. Coupling constraints and boundary conditions When boundary conditions are specified at all nodes involved in a distributing coupling constraint, the model may become overconstrained. Abaqus/Standard will issue a warning message outlining the cause of the potential overconstraint. Spot welds and rigid bodies Potential overconstraints that may arise when a rigid body is involved in a mesh-independent spot weld definition are discussed in “Mesh-independent fasteners,” Section 34.3.4. Overconstraints detected and resolved during analysis There are numerous situations when contact interactions in combination with other constraint types may lead to overconstraints. Since contact status typically changes during the analysis, it is not possible to detect redundant constraints associated with contact in the model preprocessor. Instead, these checks are performed during the analysis. Due to the complexities associated with contact interactions, only a limited number of redundant constraint cases are resolved automatically. Contact interactions and tie constraints Redundant constraints are common in cases when slave nodes used in surface-based tie constraints (“Mesh tie constraints,” Section 34.3.1) are also slave nodes in contact, as illustrated in Figure 34.6.1–9. In Figure 34.6.1–9(a) nodes 5 and 9 are connected with a tie constraint, and both are in contact with a master surface. Since the two nodes are tied together, one of the contact constraints is redundant. A similar situation is presented in Figure 34.6.1–9(b): two mismatched solid meshes are connected with a tie constraint, and contact is defined with a flat rigid surface. Node S is a dependent node in the tie constraint, so its motion is determined by that of nodes B and C. Therefore, any contact constraint applied at node S is redundant. Moreover, the contact constraints at nodes G and H are redundant, since the motion of these nodes is determined by nodes B and C, respectively. To eliminate these redundancies when all nodes involved in the tie constraint are in contact, Abaqus/Standard will automatically apply a tie-type constraint between the Lagrange multipliers associated with the contact constraint. The redundant contact constraint is eliminated. The contact pressure and the friction forces at the slave node are recovered from the pressures and friction forces at the associated tie-independent nodes. Deleting contact elements to remove overconstraints Instead of letting Abaqus remove overconstraints by tying Lagrange multipliers, you can apply constraint controls that delete the contact elements associated with tied slave nodes. If you use this technique, contact-related output is not available for the tied slave nodes. Input File Usage: *CONSTRAINT CONTROLS, DELETE SLAVE distributed load on these faces 7 6 4 tie constraint between these surfaces 14 1 11 (a) D E A F C H B G (b) master surface completely fixed 13 12 tie constraint between faces ABCD and FGHE contact master surface Figure 34.6.1–9 Redundant constraints arising from contact interactions and tie constraints. Contact interactions and prescribed boundary conditions Contact interactions and prescribed boundary conditions may lead to redundant constraints if either normal contact with the default “hard contact” formulation (“Contact pressure-overclosure relationships,” Section 36.1.2) or frictional contact with the Lagrange multiplier formulation is invoked. Abaqus/Standard attempts to resolve these types of redundant constraints for contact pairs involving rigid surfaces. Checks related to normal contact interactions In Figure 34.6.1–10 the fixed analytical rigid master surface is in contact with a slave node that has a fixed boundary condition specified in the direction normal to the contact surface. If during a particular increment in the analysis the node is in contact, the contact constraint is redundant and will not be enforced during that increment. If the boundary condition at the slave node is in conflict with the boundary conditions at the rigid surface’s reference node, an error message is issued and the analysis is stopped. distributed load boundary condition in direction normal to the master surface + rigid master surface reference node completely fixed Figure 34.6.1–10 Overconstraints involving normal contact interactions and boundary conditions. The contact and boundary conditions related to overconstraints are removed automatically only if the master surface is defined as an analytical rigid surface. In all other cases, if an overconstraint occurs during the analysis, a zero pivot message is issued by the equation solver and the chains of constraints responsible for the overconstraint are clearly outlined. Checks related to Lagrange friction A common redundant constraint case is depicted in Figure 34.6.1–11. The symmetry boundary conditions combined with the Lagrange friction are redundant. The slave node is in contact and the tangent to the surface is in approximately the same direction as the specified boundary condition at the slave node. To avoid redundancy, at this node Abaqus/Standard will switch from the Lagrange friction formulation to the default penalty formulation (“Frictional behavior,” Section 36.1.5) if the motion of the master nodes is prescribed in the tangent direction. symmetry boundary conditions on faces BDEF and ACHJ nodes A, G, and C are overconstrained Lagrange friction Figure 34.6.1–11 Lagrange friction and boundary conditions. Overconstraints detected in the equation solver All overconstraints that cannot be identified and resolved during preprocessing or during the analysis need to be detected by the equation solver. Examples include models with contact interactions where slave nodes are driven by specified boundary conditions into partially fixed rigid surfaces; contact with multiple master surfaces; closed-loop and multiple-loop mechanisms in which rigid bodies are connected by connector elements; and many more. By default, equation solver overconstraint checks are performed continuously during the analysis. Abaqus/Standard will not resolve overconstraints detected by the equation solver. Instead, detailed messages with information regarding the kinematic constraints involved in the overconstraint will be issued. The message first identifies the nodes involved in either a consistent or an inconsistent overconstraint by using zero pivot information from the Gauss elimination in the solver (“Direct linear equation solver,” Section 6.1.5). A detailed message containing constraint information is then issued. The 4-bar mechanism shown in Figure 34.6.1–12 illustrates this strategy. Four three-dimensional rigid bodies are defined as follows: the rigid body with reference node 10001 includes nodes 2 and 101; the rigid body with reference node 10002 includes nodes 3 and 102; the rigid body with reference node 10003 includes nodes 4 and 103; and the rigid body with reference node 10004 includes nodes 1 and 104. The four rigid bodies are connected with four JOIN and REVOLUTE combination connector elements defined as follows: element 20001 between nodes 1 and 101; element 20002 between nodes 2 and 102; element 20003 between nodes 3 and 103; and element 20004 between nodes 4 and 104. Each connector element enforces three translation and two rotation constraints (“Connectors: overview,” Section 31.1.1), and all four revolute axis directions are parallel. The bottom rigid body (with reference node 10004) is fixed. The motion of the bottom left REVOLUTE connector (element 20001) is prescribed to rotate the mechanism. When Abaqus/Standard attempts to find a solution for this model, three zero pivots are identified in the first increment of the analysis suggesting that there are three constraints too many in the model. element 20002 102 10002 element 20003 10001 101 connector motion 103 10003 element 20001 104 10004 (fixed) element 20004 Figure 34.6.1–12 Hard-to-detect redundant constraints. Eventually, one would have to remove three constraints to render the model properly constrained. In this simple example a count of the degrees of freedom and constraints confirms the number of overconstraints, as follows. There are four rigid bodies in the model, with a total of 24 degrees of freedom. The reference node 10004 is completely fixed with a boundary condition, constraining six degrees of freedom; and the prescribed connector motion enforces one rotational constraint, constraining one degree of freedom. Hence, there are 17 degrees of freedom remaining. Each of the four connector elements enforces five constraints, for a total of 20 constraints. Thus, there are three constraints too many in the model, which matches the number of zero pivots identified by the equation solver. To help you identify the constraints that should be removed, the following message is produced in the message (.msg) file outlining the chains of constraints that generated the overconstraint: ***WARNING: SOLVER PROBLEM. ZERO PIVOT WHEN PROCESSING ELEMENT 20004 INTERNAL NODE 1 D.O.F. 4 An overconstraint was detected at one of the OVERCONSTRAINT CHECKS: Lagrange multipliers associated with element 20004. There are multiple constraints applied directly or chained constraints that are applied indirectly to this element. The following is a list of nodes and chained constraints between these nodes that most likely lead to the detected overconstraint. LAGRANGE MULTIPLIER: 4 <-> 104: connector element 20004 type JOIN REVOLUTE constraining 3 translations and 2 rotations ..4 -> 10003: *RIGID BODY (or *COUPLING-KINEMATIC) ....10003 -> 103: *RIGID BODY (or *COUPLING-KINEMATIC) ......103 -> 3: connector element 20003 type JOIN REVOLUTE constraining 3 translations 2 rotations and ........3 -> 10002: *RIGID BODY (or *COUPLING-KINEMATIC) ..........10002 -> 102: *RIGID BODY (or *COUPLING-KINEMATIC) ............102 -> 2: connector element 20002 type JOIN REVOLUTE constraining 3 translations and 2 rotations ..............2 -> 10001: *RIGID BODY (or *COUPLING-KINEMATIC) ................10001 -> 101: *RIGID BODY (or *COUPLING-KINEMATIC) ..................101 -> 1: connector element 20001 type JOIN REVOLUTE constraining translations ....................1 -> 10004: *RIGID BODY (or *COUPLING-KINEMATIC) ......................10004 -> *BOUNDARY in degrees of freedom and 2 rotations ......................10004 -> 104: *RIGID BODY ....................1 -> 101: connector element 20001 with *CONNECTOR MOTION in components (or *COUPLING-KINEMATIC) Please analyze these constraint loops and remove unnecessary constraints. First, the message identifies the user-defined or, in this case, the internally defined (Lagrange multiplier) node at which a zero pivot was identified. A typical line in this output issues information related to one constraint. For example, the first line in this output LAGRANGE MULTIPLIER: 4 <-> 104: connector element 20004 type JOIN REVOLUTE constraining 3 translations and 2 rotations informs you that the Lagrange multiplier on which the zero pivot occurs enforces one of the five constraints (JOIN and REVOLUTE) associated with connector element 20004 between user-defined nodes 4 and 104. Each of the subsequent lines conveys information related to one constraint in the chains of constraints originating at the zero pivot node or in chains adjacent to them. For example, the line ....10003 -> 103: *RIGID BODY (or *COUPLING - KINEMATIC) informs you that there is a rigid body constraint between nodes 10003 and 103, while the line .....................10004 -> *BOUNDARY in degrees of freedom states that there is a boundary condition constraint fixing degrees of freedom 1 through 6 at node 10004. Indentation levels (the dots in front of the node numbers) identify links in a chain of constraints. Each time a constraint is found to link another node in a particular chain, the indentation is increased by two dots and the constraint information is printed out. For example, starting from the top of the message, the Lagrange multiplier is connected to node 4, node 4 is connected to node 10003, node 10003 is connected to node 103, and so on. When the indentation on a certain line is less than or equal to the indentation on the previous line, a chain of constraints has ended on the previous line. For example, a chain has ended on the line .....................10004 -> *BOUNDARY in degrees of freedom since the next line has equal indentation. Three chains of constraints (in correspondence with the three zero pivots that were found) that most likely generated the overconstraint can be identified in the model above. Starting from the top, one can first identify a chain of constraints that terminates in a boundary condition (ground): Lagrange multiplier: 4 –> 10003 –> 103 –> 3 –> 10002 –> 2 –> 10001 –> 101 –> 1 –> 10004 –> *BOUNDARY Since the indentation of the two lines starting with node 10004 is the same, one should expect another chain of constraints to include the constraint output on the second of the two lines. Indeed, one can identify a closed loop of constraints: Lagrange multiplier : 4–> 10003 –> 103 –> 3 –> 10002 –> 2 –> 10001 –> 101 –> 1 –> 10004 –> 104 <-> 4 Finally, since the two lines starting with node 1 have the same indentation, one expects that a separate chain of constraints will include the last line in the output. A third (closed) loop 101 –> 1 –> 101 is identified. If the chains of constraints terminate in a free end (not ending in a constraint), the chain does not have any contribution in generating the overconstraint. There are no such chains in this example. Correcting an overconstrained model A node set containing all the nodes in the chains of constraints associated with a particular zero pivot is generated automatically and can be displayed in the Visualization module of Abaqus/CAE. There is no unique way to remove the overconstraints in this model. For example, if one JOIN and REVOLUTE (five constraints) combination is replaced with a SLOT connector element, which enforces only the two translation constraints in the plane of the mechanism, there are no redundancies. Alternatively, you could remove the REVOLUTE from one of the connector elements and also use a SLOT connection instead of a JOIN in one of the other connector elements. Another alternative is to relax some of the constraints. In the example outlined here, an elastic body could replace one or more of the rigid bodies. You could also relax the Lagrange multiplier-based constraints (e.g., JOIN or REVOLUTE) by using CARTESIAN and CARDAN connection types with appropriate elastic stiffnesses . After analyzing the chains of constraints, you have to decide which constraints have to be removed to render the model properly constrained and also best fit the modeling goals. For this example the three constraints cannot be removed randomly. Removing any three combinations of the six boundary conditions, for example, would make the problem worse: the model is still overconstrained, and three rigid body modes have been added to the model. Moreover, you should remove the constraints that do not affect the kinematics of the model. For example, you cannot completely remove a JOIN connection from any of the connector elements since the model would be different from that originally intended. Controlling the overconstraint checks By default, Abaqus/Standard will attempt to remove as many redundant constraints as possible, as discussed in the sections above. When it is not possible to remove a redundant constraint or an inconsistent overconstraint is detected, a detailed message is issued identifying the constraints contributing to the overconstraint. You can modify this default behavior by prescribing constraint controls for the model or the step. Overconstraints may produce damaging and unpredictable behavior. Therefore, it is strongly recommended that overconstraint checking be used in both the preprocessor and during the analysis at least during the first running of a model. Furthermore, it is recommended that the original model be changed to correct any overconstraints identified by Abaqus/Standard. Only after establishing confidence that the model is free of overconstraints should constraint checks be turned off. The only advantage of turning off the constraint checks is a minor speedup of the analysis. Bypassing the overconstraint checks The overconstraint checks performed during input file preprocessing and during the analysis can be bypassed. Bypassing these checks is not recommended, as it may allow a model with overconstraints to enter into the analysis code. Bypassing the overconstraint checks is not step dependent; i.e., the setting is defined as model data and affects the entire analysis. Input File Usage: *CONSTRAINT CONTROLS, NO CHECKS Preventing automatic redundant constraint resolution Automatic model modifications in the model preprocessor can be prevented. In this case Abaqus/Standard will still perform overconstraint checks, but no automatic redundant constraint resolution will be performed; only appropriate error messages will be issued. Preventing constraint resolution is not step dependent; i.e., the setting is defined as model data and affects the entire analysis. Input File Usage: *CONSTRAINT CONTROLS, NO CHANGES Changing the frequency of the overconstraint checks By default, the overconstraint checks are performed at every increment during the analysis. You can modify the frequency of these checks (in increments) for each step in the analysis. If the frequency is set equal to zero, no overconstraint checks are performed during that analysis step. The frequency specification is maintained in subsequent steps until the value is reset. Input File Usage: *CONSTRAINT CONTROLS, CHECK FREQUENCY=n Stopping the analysis when overconstraints are detected By default, the analysis continues even though an overconstraint is detected. This behavior can be changed on a step-dependent basis. The analysis can be stopped the first time an overconstraint is detected in a step, or it can be stopped only if a converged solution is obtained despite the fact that overconstraints exist. This setting is maintained in subsequent steps until it is reset. Input File Usage: Use one of the following options: *CONSTRAINT CONTROLS, TERMINATE ANALYSIS=FIRST OCCURRENCE *CONSTRAINT CONTROLS, TERMINATE ANALYSIS=CONVERGED • Chapter 35, “Defining Contact Interactions” • Chapter 36, “Contact Property Models” • Chapter 37, “Contact Formulations and Numerical Methods” • Chapter 38, “Contact Difficulties and Diagnostics” • Chapter 39, “Contact Elements in Abaqus/Standard” 35. Defining Contact Interactions Overview Defining general contact in Abaqus/Standard Defining contact pairs in Abaqus/Standard Defining general contact in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit 35.1 35.2 35.3 35.4 35.1 Overview • “Contact interaction analysis: overview,” Section 35.1.1 35.1.1 CONTACT INTERACTION ANALYSIS: OVERVIEW This section presents an overview of the contact analysis capabilities in Abaqus. Available contact algorithms in Abaqus Abaqus provides more than one approach for defining contact. Abaqus/Standard includes the following approaches for defining contact: • general contact; • contact pairs; and • contact elements. Abaqus/Explicit includes the following approaches for defining contact: • general contact; and • contact pairs. Each approach has somewhat unique advantages and limitations. The remainder of this section is organized as follows: • first, discuss common aspects of the surface-based contact-definition approaches (i.e., contact pairs and general contact); • next, provide an overview of the contact definition approaches in Abaqus/Standard and the contact definition approaches in Abaqus/Explicit; • finally, discuss compatibility between the contact algorithms Abaqus/Explicit. in Abaqus/Standard and Defining a surface-based contact simulation A contact simulation using contact pairs or general contact is defined by specifying: • surface definitions for the bodies that could potentially be in contact; • the surfaces that interact with one another (the contact interactions); • any nondefault surface properties to be considered in the contact interactions; • the mechanical and thermal contact property models, such as the pressure-overclosure relationship, the friction coefficient, or the contact conduction coefficient; • any nondefault aspects of the contact formulation; and • any algorithmic contact controls for the analysis. In many cases you do not need to explicitly specify many of the aspects listed above because the default settings are usually appropriate. Surfaces Surfaces can be defined at the beginning of a simulation or upon restart as part of the model definition . Abaqus has four classifications of contact surfaces: • element-based deformable and rigid surfaces (“Element-based surface definition,” Section 2.3.2); • node-based deformable and rigid surfaces (“Node-based surface definition,” Section 2.3.3); • analytical rigid surfaces (“Analytical rigid surface definition,” Section 2.3.4); and • Eulerian material surfaces for Abaqus/Explicit (“Eulerian surface definition,” Section 2.3.5). Surfaces of the same type can be combined to create new surfaces . However, with regard to contact a combined surface can be used only with general contact in Abaqus/Explicit. When the general contact algorithm is used, Abaqus also provides a default all-inclusive, automatically defined surface that includes all element-based surface facets (in Abaqus/Standard and in Abaqus/Explicit), all analytical rigid surfaces (in Abaqus/Explicit only), and all Eulerian materials (in Abaqus/Explicit only) in the model. Contact interactions Contact interactions for contact pairs and general contact are defined by specifying surface pairings and self-contact surfaces. General contact interactions typically are defined by specifying self-contact for the default surface, which allows an easy, yet powerful, definition of contact. (Self-contact for a surface that spans multiple bodies implies self-contact for each body as well as contact between the bodies.) At least one surface in an interaction must be a non-node-based surface, and at least one surface in an interaction must be a non-analytical rigid surface. Additional restrictions and guidelines for contact surfaces are discussed for each contact definition approach. The definition of contact pairs is discussed in detail in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1, and “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1. The definition of general contact interactions is discussed in detail in “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1, and “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1. Surface properties Nondefault surface properties (such as thickness and, in some cases, offset) can be defined for particular surfaces in a contact model. In addition, you can control which edges of a surface will be included in the general contact domain in Abaqus/Explicit. Surface properties for contact pairs are discussed in “Assigning surface properties for contact pairs in Abaqus/Standard,” Section 35.3.2, and “Assigning surface properties for contact pairs in Abaqus/Explicit,” Section 35.5.2. Surface properties for general contact are discussed in “Surface properties for general contact in Abaqus/Standard,” Section 35.2.2, and “Assigning surface properties for general contact in Abaqus/Explicit,” Section 35.4.2. Contact properties Contact interactions in a model can refer to a contact property definition, in much the same way that elements refer to an element property definition. By default, the surfaces interact (have constraints) only in the normal direction to resist penetration. The other mechanical contact interaction models available depend on the contact algorithm and whether Abaqus/Standard or Abaqus/Explicit is used . Some of the available models are: • softened contact (“Contact pressure-overclosure relationships,” Section 36.1.2, and “Frictional behavior,” Section 36.1.5); • contact damping (“Contact damping,” Section 36.1.3, and “Frictional behavior,” Section 36.1.5); • friction (“Frictional behavior,” Section 36.1.5); • a user-defined constitutive model for surface interactions (“User-defined interfacial constitutive behavior,” Section 36.1.6); and • spot welds bonding two surfaces together until the welds fail (“Breakable bonds,” Section 36.1.9). The thermal, thermal-electrical, and pore-fluid surface interaction models available in Abaqus are discussed in “Thermal contact properties,” Section 36.2.1; “Electrical contact properties,” Section 36.3.1; and “Pore fluid contact properties,” Section 36.4.1, respectively. Contact interaction models are defined as model data except for contact pairs in Abaqus/Explicit, in which case they are defined as history data. Information on assigning contact properties to contact pairs can be found in “Assigning contact properties for contact pairs in Abaqus/Standard,” Section 35.3.3, and “Assigning contact properties for contact pairs in Abaqus/Explicit,” Section 35.5.3. Information on assigning contact properties to general contact interactions can be found in “Contact properties for general contact in Abaqus/Standard,” Section 35.2.3, and “Assigning contact properties for general contact in Abaqus/Explicit,” Section 35.4.3. Numerical controls The default algorithmic controls for contact analyses are usually sufficient, but you can adjust numerical controls for some special cases. For example, depending on the contact algorithm used, the numerical controls for the contact formulation, the master and slave roles for the contact surfaces, and the sliding formulation are provided. Information on contact formulations and numerical methods used by the contact algorithms is provided in “Contact formulations in Abaqus/Standard,” Section 37.1.1, and “Contact formulations for contact pairs in Abaqus/Explicit,” Section 37.2.2. The available numerical controls for the various contact algorithms are discussed in “Numerical controls for general contact in Abaqus/Standard,” Section 35.2.6; “Adjusting contact controls in Abaqus/Standard,” Section 35.3.6; “Contact controls for general contact in Abaqus/Explicit,” Section 35.4.5; and “Contact controls for contact pairs in Abaqus/Explicit,” Section 35.5.5. Contact simulation capabilities in Abaqus/Standard Abaqus/Standard provides the following approaches for defining contact interactions: general contact, contact pairs, and contact elements. Contact pairs and general contact both use surfaces to define contact; comparisons of these approaches are provided later in this section. Contact elements are provided for certain interactions that cannot be modeled with either general contact or contact pairs; however, it is generally recommended to use general contact or contact pairs if possible. Capabilities of contact pairs and general contact in Abaqus/Standard Contact pairs and general contact combine to provide the following capabilities in Abaqus/Standard: • Contact between two deformable bodies. The structures can be either two- or three-dimensional, and they can undergo either small or finite sliding. Examples of such problems include the assembly of a cylinder head gasket and the slipping between the two components of a threaded connector. • Contact between a rigid surface and a deformable body. The structures can be either two- or three- dimensional, and they can undergo either small or finite sliding. Examples of such problems include metal forming simulations and analyses of rubber seals being compressed between two components. • Finite-sliding self-contact of a single deformable body. An example of such a problem is a complex rubber seal that folds over on itself. • Small-sliding or finite-sliding interaction between a set of points and a rigid surface. These models can be either two- or three-dimensional. An example of this type of problem is the pull-in of an underwater cable that is resting on the seabed, with the seabed modeled as a rigid surface. • Contact between a set of points and a deformable surface. These models can be either two- or three-dimensional. An example of this class of contact problem is the design of a bearing where one of the bearing surfaces is modeled with substructures. • Problems where two separate surfaces need to be “tied” together so that there is no relative motion between them. This modeling technique allows for joining dissimilar meshes. • Coupled thermal-mechanical interaction between deformable bodies with finite relative motion. The analysis of a disc brake is an example of such a problem. • Coupled thermal-electrical-structural interaction between deformable bodies with finite relative motion. An example of this type of problem is the analysis of resistance spot welding. • Coupled pore fluid-mechanical interaction between bodies. An example of this type of problem is the analysis of the interfaces between layered soil material at a waste disposal site. Coupled thermal-mechanical and coupled thermal-electrical-structural interactions can be included in any of the above examples as long as both of the surfaces are deformable. Choosing between general contact or contact pairs in Abaqus/Standard For most contact problems you have a choice of whether to define contact interactions using general contact or contact pairs. In Abaqus/Standard the distinction between general contact and contact pairs lies primarily in the user interface, the default numerical settings, and the available options. The general contact and contact pair implementations share many underlying algorithms. The contact interaction domain, contact properties, and surface attributes are specified independently for general contact, offering a more flexible way to add detail incrementally to a model. The simple interface for specifying general contact allows for a highly automated contact definition; however, it is also possible to define contact with the general contact interface to mimic traditional contact pairs. Conversely, specifying self-contact of a surface spanning multiple bodies with the contact pair user interface (if the surface-to-surface formulation is used) mimics the highly automated approach often used for general contact. In Abaqus/Standard, traditional pairwise specifications of contact interactions will often result in more efficient or robust analyses as compared to an all-inclusive self-contact approach to defining contact. Therefore, there is often a trade-off between ease of defining contact and analysis performance. Abaqus/CAE provides a contact detection tool that greatly simplifies the process of creating traditional contact pairs for Abaqus/Standard . Default settings for general contact and contact pairs Differences in default settings for general contact and contact pairs in Abaqus/Standard include the following: • Contact formulation: General contact uses the finite-sliding, surface-to-surface formulation supplemented by the finite-sliding, edge-to-surface formulation. Contact pairs use the finite-sliding, node-to-surface formulation by default except when the contact detection tool in Abaqus/CAE is used to create the contact pairs, in which case the finite-sliding, surface-to-surface formulation is used by default. See “Contact formulations in Abaqus/Standard,” Section 37.1.1, for a discussion of contact formulations. • Treatment of shell thickness and offset: General contact automatically accounts for thicknesses and offsets associated with shell-like surfaces. Contact pairs that use the finite-sliding, node-to-surface formulation do not account for shell thicknesses and offsets. See “Surface properties for general contact in Abaqus/Standard,” Section 35.2.2, and “Assigning surface properties for contact pairs in Abaqus/Standard,” Section 35.3.2, for discussions of surface properties for contact in Abaqus/Standard. • Contact constraint enforcement: General contact uses the penalty method to enforce the contact constraints by default. Contact pairs that use the finite-sliding, node-to-surface formulation use a Lagrange multiplier method to enforce contact constraints by default in most cases. See “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2, for a discussion of contact constraint enforcement methods. • Treatment of initial overclosures: General contact eliminates initial overclosures with strain-free adjustments by default. Contact pairs treat initial overclosures as interference fits to be resolved in the first increment of the analysis by default. See “Controlling initial contact status in Abaqus/Standard,” Section 35.2.4; “Modeling contact interference fits in Abaqus/Standard,” Section 35.3.4; and “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 35.3.5; for more information on contact initialization in Abaqus/Standard. • Master-slave assignments: General contact automatically assigns pure master and slave roles for most contact interactions and automatically assigns balanced master-slave roles to other contact interactions. The user must assign master and slave roles for most contact pairs. See “Numerical controls for general contact in Abaqus/Standard,” Section 35.2.6, and “Choosing the master and slave roles in a two-surface contact pair” in “Contact formulations in Abaqus/Standard,” Section 37.1.1, for discussions of master and slave roles for contacting surfaces. The first three differences listed above disappear if you specify the finite-sliding, surface-to-surface formulation for contact pairs. Additional contact pair capabilities The following capabilities are available only for contact pairs in Abaqus/Standard (they are not available for general contact in Abaqus/Standard): • Contact involving analytical rigid surfaces or rigid surfaces defined with user subroutine RSURFU (however, element-based rigid surfaces can be included in either general contact or contact pairs). • Contact involving node-based surfaces or surfaces on three-dimensional beam elements. • Small-sliding contact and tied contact. • The finite-sliding, node-to-surface contact formulation. • Debonding and cohesive contact behavior. • Surface interactions in analyses without displacement degrees of freedom, such as pure heat transfer. • Pressure-penetration loading. • Local definitions of some numerical contact controls. • Symmetric model generation. A single analysis can include general contact and contact pair definitions. For example, you may choose to model contact interactions involving analytical rigid surfaces with contact pairs and other contact interactions with general contact. General contact automatically avoids processing contact interactions that are treated by contact pairs. Contact simulations requiring contact elements Surface-based contact methods associated with general contact and contact pairs cannot be used for certain classes of problems. Abaqus/Standard provides a library of contact elements for these problems. Examples of such problems are: • Contact interaction between two pipelines or tubes modeled with pipe, beam, or truss elements where one pipe lies inside the other (such as a J-tube pull in offshore piping installation) or the pipes lie next to each other (available in both two and three dimensions; see “Tube-to-tube contact elements,” Section 39.3.1). • Contact between two nodes along a fixed direction in space. An example of such a problem is the interaction of a piping system with its supports . • Simulations using axisymmetric elements with asymmetric deformations, CAXAn and SAXAn elements. See “Contact modeling if asymmetric-axisymmetric elements are present,” Section 35.3.10, for details. • Heat transfer analyses where the heat flow is one-dimensional. An example of such a problem is the heat flow in a piping system that is discontinuous. The thermal interaction in this problem is one-dimensional, so no surfaces can be defined . Defining a contact simulation using contact elements The steps required for defining a contact simulation using contact elements are similar to those needed when defining a surface-based contact simulation: • create the contact elements or slide lines; • assign element section properties to the contact elements; • associate sets of contact elements with the slide lines if applicable; and • define the contact property models for the contact elements. The first three steps are discussed in Chapter 39, “Contact Elements in Abaqus/Standard,” in the sections for each type of contact element. The contact property models for contact elements are identical to those used for surface-based contact. Contact simulation capabilities in Abaqus/Explicit Abaqus/Explicit provides two algorithms for modeling contact interactions. The general (“automatic”) contact algorithm allows very simple definitions of contact with very few restrictions on the types of surfaces involved . The contact pair algorithm has more restrictions on the types of surfaces involved and often requires more careful definition of contact; however, it allows for some interaction behaviors that currently are not available with the general contact algorithm . The general contact and contact pairs algoirthms in Abaqus/Explicit differ by more than the user interface; in general they use completely separate implementations with many key differences in the designs of the numerical algorithms. The two contact algorithms combine to provide the following capabilities in Abaqus/Explicit: • Contact between rigid and/or deformable bodies. • Contact of a body with itself. • Finite-sliding or small-sliding contact. • Contact with eroding bodies (due to element failure). A node-based surface must be used to model the eroding body if contact pairs are used. General contact allows element-based surfaces to be defined on eroding bodies, so contact between any number of eroding bodies can be modeled. • General constitutive models for the contact behavior, including user-defined models through user subroutines, relating constraint pressure and shear traction to penetration distance and relative tangential motion. • Thermal interaction at the surface of a body; for example, conductive heat transfer. • Contact between Eulerian material and Lagrangian bodies. • A friction coefficient defined in terms of average surface temperature and/or field variables. Choosing between general contact or contact pairs in Abaqus/Explicit Contact definitions are not entirely automatic with the general contact algorithm but are greatly simplified. The generality of this algorithm is primarily in the relaxed restrictions on the surfaces that can be used in contact. The general contact algorithm in Abaqus/Explicit allows the following (none of which are allowed with the contact pair algorithm in Abaqus/Explicit): • A surface can span unattached bodies. • More than two surface facets can share a common edge (allowing “T-intersections” in shells, for example). • A surface can include deformable and rigid regions; furthermore, the rigid regions need not be from the same rigid body. • A surface can have mixed parent element types; for example, adjacent surface facets can be on shell and solid elements. • A surface can be based on combinations of surfaces of the same type. • An element-based surface can be defined on the interior of solid bodies for use in modeling erosion due to element failure. • A surface can be defined on the exterior of an Eulerian material instance . Other benefits of the general contact algorithm in Abaqus/Explicit include the following: • The general contact algorithm can enforce edge-to-edge contact for geometric feature edges, perimeter edges of structural elements, and edges defined by beam and truss elements, unlike the contact pair algorithm. • The general contact algorithm is the only option for enforcing contact between Eulerian materials and Lagrangian bodies . • The general contact algorithm eliminates problematic, nonphysical “bull-nose” extensions that may arise at shell surface perimeters in the contact pair algorithm. • With the general contact algorithm each slave node can see contact with multiple facets per increment; with the contact pair algorithm each slave node can see contact with only one facet per increment unless multiple surface pairings are specified. Likewise, each contact edge can see contact with multiple edges per increment when the general contact algorithm is used. • The general contact algorithm has some built-in smoothing for element-based surfaces that can be beneficial for modeling contact near corners. • The general contact algorithm, unlike the contact pair algorithm, removes contact faces and contact edges from the contact domain and, if an interior surface is defined, activates newly exposed surface faces as elements fail. Thus, element-based surfaces can be used to describe eroding solids. This allows contact between multiple eroding solids to be modeled since a node-based surface does not need to be defined on the eroding solid. • Contact state information (such as the proper contact normal orientation for double-sided surfaces) is transferred across step boundaries in the general contact algorithm even if the contact domain is modified; in the contact pair algorithm, contact state information is transferred across step boundaries only for contact pairs with no modifications. • The contact interaction domain, contact properties, and surface attributes are specified independently for the general contact algorithm, offering a more flexible way to add detail incrementally to a model. • The general contact algorithm does not place any restrictions on the domain decomposition for domain level parallelization . • The general contact algorithm in Abaqus/Explicit has been developed to minimize the need for algorithmic controls. See “Knee bolster impact with general contact,” Section 2.1.9 of the Abaqus Example Problems Manual; “Crimp forming with general contact,” Section 2.1.10 of the Abaqus Example Problems Manual; and “Collapse of a stack of blocks with general contact,” Section 2.1.11 of the Abaqus Example Problems Manual, for example analyses that use the general contact algorithm. Although the general contact algorithm is more powerful and allows for simpler contact definitions, the contact pair algorithm must be used in certain cases where more specialized contact features are desired. The following features are available in Abaqus/Explicit only when the contact pair algorithm is used: • Two-dimensional surfaces • Kinematically enforced contact • Small-sliding contact Section 37.2.2) In addition, the general contact algorithm in Abaqus/Explicit places more restrictions on adaptive meshing than the contact pair algorithm . the speedup factor if loop-level parallelization is used: the contact pair algorithm includes some loop-level parallelization, while the general contact algorithm has no loop-level parallelization. Contact output is more complete for a contact pair analysis. The choice of contact algorithm may affect The two contact algorithms can be used together in the same Abaqus/Explicit analysis. The general contact algorithm automatically avoids processing interactions that are treated by the contact pair algorithm. Compatibility between Abaqus/Standard and Abaqus/Explicit There are fundamental differences in the mechanical contact algorithms in Abaqus/Standard and Abaqus/Explicit even though the input syntax is similar. The main differences are the following: • Contact pair and general contact definitions in Abaqus/Standard are model definition data (although contact pairs can be removed for a portion of the analysis and added back to the model in a later step of the analysis, as discussed in “Removing and reactivating contact pairs” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1). In the contact pair algorithm in Abaqus/Explicit contact constraints are history definition data ; in the general contact algorithm in Abaqus/Explicit contact definitions can be either model or history data. • Abaqus/Standard typically uses a pure master-slave relationship for the contact constraints; whereas Abaqus/Explicit typically uses balanced master-slave contact by default. This difference is primarily due to overconstraint issues unique to Abaqus/Standard. • The contact formulations in Abaqus/Standard and Abaqus/Explicit differ in many respects due to different convergence, performance, and numerical requirements: – Abaqus/Standard provides surface-to-surface and edge-to-surface formulations, which Abaqus/Explicit does not; – Abaqus/Explicit provides an edge-to-edge formulation, which Abaqus/Standard does not; – Abaqus/Standard and Abaqus/Explicit both provide node-to-surface formulations, but some details associated with surface smoothing, etc. differ in the respective implementations. • The constraint enforcement methods in Abaqus/Standard and Abaqus/Explicit differ in some respects. For example, both analysis codes provide penalty constraint methods, but the default penalty stiffnesses differ (this is primarily due to the effect of the penalty stiffness on the stable time increment for Abaqus/Explicit). • The small-sliding contact capability in Abaqus/Standard transfers the load to the master nodes according to the current position of the slave node, but the small-sliding contact capability in Abaqus/Explicit always transfers the load through the anchor point due to a numerical limitation associated with the implementation. • Abaqus/Explicit can account for the thickness and midsurface offset of shells and membranes in the contact penetration calculations (although in some cases changes in the thickness upon deformation are not accounted for in the contact calculations). Abaqus/Standard cannot account for the thickness and offset of shells and membranes when using the finite-sliding, node-to-surface contact formulation (but can account for the original thickness and offset in all other contact formulations). As a result of these differences, contact definitions specified in an Abaqus/Standard analysis cannot be imported into an Abaqus/Explicit analysis and vice versa . However, in many cases you can successfully respecify a contact definition in an import analysis. 35.2 Defining general contact in Abaqus/Standard • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • “Surface properties for general contact in Abaqus/Standard,” Section 35.2.2 • “Contact properties for general contact in Abaqus/Standard,” Section 35.2.3 • “Controlling initial contact status in Abaqus/Standard,” Section 35.2.4 • “Stabilization for general contact in Abaqus/Standard,” Section 35.2.5 • “Numerical controls for general contact in Abaqus/Standard,” Section 35.2.6 35.2.1 DEFINING GENERAL CONTACT INTERACTIONS IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Contact interaction analysis: overview,” Section 35.1.1 • *CONTACT • *CONTACT INCLUSIONS • *CONTACT EXCLUSIONS • “Defining general contact,” Section 15.13.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Abaqus/Standard provides two algorithms for modeling contact and interaction problems: the general contact algorithm and the contact pair algorithm. See “Contact interaction analysis: overview,” Section 35.1.1, for a comparison of the two algorithms. This section describes how to include general contact in an Abaqus/Standard analysis, how to specify the regions of the model that may be involved in general contact interactions, and how to obtain output from a general contact analysis. The general contact algorithm in Abaqus/Standard: • is specified as part of the model definition; • allows very simple definitions of contact with very few restrictions on the types of surfaces involved; • uses sophisticated tracking algorithms to ensure that proper contact conditions are enforced efficiently; • can be used simultaneously with the contact pair algorithm (i.e., some interactions can be modeled with the general contact algorithm, while others are modeled with the contact pair algorithm); • can be used with two- or three-dimensional surfaces; and • uses the finite-sliding, surface-to-surface contact formulation. Defining a general contact interaction The definition of a general contact interaction consists of specifying: • the general contact algorithm and defining the contact domain (i.e., the surfaces that interact with one another), as described in this section; • the contact surface properties (“Surface properties for general contact in Abaqus/Standard,” Section 35.2.2); • the mechanical contact property models Abaqus/Standard,” Section 35.2.3); (“Contact properties for general contact in • the controls associated with the initial contact state (“Controlling initial contact status in Abaqus/Standard,” Section 35.2.4); and • the algorithmic contact controls (“Numerical controls for general contact in Abaqus/Standard,” Section 35.2.6). An example of an analysis that uses general contact to define contact between the various components of an assembly is described in “Impact analysis of a pawl-ratchet device,” Section 2.1.17 of the Abaqus Example Problems Manual. Surfaces used for general contact The general contact algorithm in Abaqus/Standard allows for quite general characteristics in the surfaces that it uses, as discussed in “Contact interaction analysis: overview,” Section 35.1.1. For detailed information on defining surfaces in Abaqus/Standard for use with the general contact algorithm, see “Element-based surface definition,” Section 2.3.2. A convenient method of specifying the contact domain is using cropped surfaces. Such surfaces can be used to perform “contact in a box” by using a contact domain that is enclosed in a specified rectangular box in the original configuration. For more information, see “Operating on surfaces,” Section 2.3.6. In addition, Abaqus/Standard automatically defines an all-inclusive surface that is convenient for prescribing the contact domain, as discussed later in this section. The all-inclusive automatically defined surface includes all element-based surface facets. The general contact algorithm in Abaqus/Standard uses the surface-to-surface contact formulation as the primary formulation and can use the edge-to-surface contact formulation as a supplementary formulation. The general contact algorithm does not consider contact involving analytical surfaces or node-based surfaces, although these surface types can be included in contact pairs in analyses that also use general contact. Considerations for edge-to-surface contact The general contact algorithm can consider three-dimensional edge-to-surface contact, which is more effective at resolving some interactions than the surface-to-surface contact formulation. The edge-to- surface contact formulation is primarily intended to avoid localized penetration of a feature’s edge of one surface into a relatively smooth portion of another surface when the normal directions of the respective surface facets in the active contact region form an oblique angle. The model shown in Figure 35.2.1–1 will benefit from supplementary edge-to-surface contact enforcement because the active contact zone corresponds to a feature edge during some periods of the insertion loading. Supplementary edge-to- surface contact enforcement is not necessary for the model shown in Figure 35.2.1–2 because the surface- to-surface contact formulation is able to adequately resist the penetrations. By default, when a surface is used in a general contact interaction, all applicable facets are included in the contact definition along with edges of solid and shell elements with feature angles of at least 45°. See “Feature edges” in “Surface properties for general contact in Abaqus/Standard,” Section 35.2.2 for a discussion of controls related to which feature edges are considered for edge-to-surface contact. Edge-to- surface contact constraints never participate in thermal, electrical, or pore pressure contact properties. For example, in a coupled temperature-displacement analysis, surface-to-surface constraints can influence Figure 35.2.1–1 Snap-fit example involving feature edge-to-surface contact with an oblique angle between surface normals in the contact region. Figure 35.2.1–2 Example with feature-edges at the perimeter of an active contact region that has opposing surface normals. mechanical and thermal interactions; but, if edge-to-surface constraints are included, they will only help resist penetrations. The contact area associated with a feature edge depends on the mesh size; therefore, contact pressures (in units of force per area) associated with edge-to-surface contact are mesh dependent. Both surface-to-surface and edge-to-surface contact constraints may be active at the same nodes. To help avoid numerical overconstraint issues, edge-to-surface contact constraints are always enforced with a penalty method. Including general contact in an analysis General contact in Abaqus/Standard is defined at the beginning of an analysis. Only one general contact definition can be specified, and this definition is in effect for every step of the analysis. Input File Usage: Use the following option to indicate the beginning of a general contact definition: Abaqus/CAE Usage: *CONTACT This option can appear only once in the model definition. Interaction module: Create Interaction: Step: Initial, General contact (Standard) Defining the general contact domain You specify the regions of the model that can potentially come into contact with each other by defining general contact inclusions and exclusions. Only one contact inclusions definition and one contact exclusions definition are allowed in the model definition. All contact inclusions in an analysis are applied first, then all contact exclusions are applied, regardless of the order in which they are specified. The contact exclusions take precedence over the contact inclusions. The general contact algorithm will consider only those interactions specified by the contact inclusions definition and not specified by the contact exclusions definition. General contact interactions typically are defined by specifying self-contact for the default automatically generated surface provided by Abaqus/Standard. All surfaces used in the general contact algorithm can span multiple unattached bodies, so self-contact in this algorithm is not limited to contact of a single body with itself. For example, self-contact of a surface that spans two bodies implies contact between the bodies as well as contact of each body with itself. Specifying contact inclusions Define contact inclusions to specify the regions of the model that should be considered for contact purposes. Specifying “automatic” contact for the entire model You can specify self-contact for a default unnamed, all-inclusive surface defined automatically by Abaqus/Standard. This default surface contains, with the exceptions noted below, all exterior element faces. This is the simplest way to define the contact domain. The default surface does not include faces that belong only to cohesive elements. In fact, the default surface is generated as if cohesive elements were not present. See “Modeling with cohesive elements,” Section 32.5.3, for further discussion of contact modeling issues related to cohesive elements. Input File Usage: Use both of the following options to specify “automatic” contact for the entire model: *CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR The *CONTACT INCLUSIONS option should have no data lines when the ALL EXTERIOR parameter is used. Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Standard): Included surface pairs: All* with self Specifying individual contact interactions Alternatively, you can define the general contact domain directly by specifying the individual contact surface pairings. Self-contact will be modeled only if the two surfaces specified in a pair overlap (or are identical) and will be modeled only in the overlapping region. In some cases computational performance and robustness can be improved by including only portions of surfaces in the general contact domain that will experience contact during an analysis. Multiple surface pairings can be included in the contact domain. All of the surfaces specified must be element-based surfaces. Input File Usage: Use both of the following options to specify individual contact interactions: *CONTACT *CONTACT INCLUSIONS surface_1, surface_2 At least one data line must be specified when the ALL EXTERIOR parameter is omitted. Either or both of the data line entries can be left blank, but each data line must contain at least a comma; an error message will be issued for empty data lines. If the first surface name is omitted, the default unnamed, all-inclusive, automatically generated surface is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is assumed. Leaving both data line entries blank is equivalent to using the ALL EXTERIOR parameter. Interaction module: Create Interaction: General contact (Standard): Included surface pairs: Selected surface pairs: Edit, select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of included pairs Abaqus/CAE Usage: Examples The following input specifies that contact should be enforced between the default all-inclusive, automatically generated surface and surface_2, including self-contact in any overlap regions: *CONTACT *CONTACT INCLUSIONS , surface_2 Either of the following methods can be used to define self-contact for surface_1: or *CONTACT *CONTACT INCLUSIONS surface_1, *CONTACT *CONTACT INCLUSIONS surface_1, surface_1 Specifying contact exclusions You can refine the contact domain definition by specifying the regions of the model to exclude from contact. Possible motivations for specifying contact exclusions include: • avoiding physically unreasonable contact interactions; • improving computational performance by excluding parts of the model that are not likely to interact. Contact will be ignored for all the surface pairings specified, even if these interactions are specified directly or indirectly in the contact inclusions definition. Multiple surface pairings can be excluded from the contact domain. All of the surfaces specified must be element-based surfaces. Keep in mind that surfaces can be defined to span multiple unattached bodies, so self-contact exclusions are not limited to exclusions of single-body contact. Input File Usage: Use both of the following options to specify contact exclusions: *CONTACT *CONTACT EXCLUSIONS surface_1, surface_2 Either or both of the data line entries can be left blank. If the first surface name is omitted, the default unnamed, all-inclusive, automatically generated surface is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is excluded from the contact domain. Interaction module: Create Interaction: General contact (Standard): Excluded surface pairs: Edit, select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of excluded pairs Abaqus/CAE Usage: Automatically generated contact exclusions Abaqus/Standard automatically generates contact exclusions for general contact in some situations. • Contact exclusions are generated automatically for interactions that are defined with the contact pair algorithm or surface-based tie constraints to avoid redundant (and possibly inconsistent) enforcement of these interaction constraints. if a contact pair is defined for surface_1 and surface_2 and “automatic” general contact is defined for the entire model, Abaqus/Standard generates a contact exclusion for general contact between surface_1 and For example, surface_2 so that interactions between these surfaces are modeled only with the contact pair algorithm. These automatically generated contact exclusions are in effect throughout the analysis. • Abaqus/Standard automatically generates contact exclusions for self-contact of each rigid body in the model, because it is not possible for a rigid body to contact itself. • When you specify pure master-slave contact surface weighting for a particular general contact surface pair, contact exclusions are generated automatically for the master-slave orientation opposite to that specified . • Abaqus/Standard assigns default pure master-slave roles for contact involving disconnected bodies within the general contact domain, and contact exclusions are generated by default for the opposite master-slave orientations. Options to override the default pure master-slave assignments with alternative pure master-slave assignments or balanced master-slave assignments are discussed in “Numerical controls for general contact in Abaqus/Standard,” Section 35.2.6. • Contact exclusions are generated automatically for portions of surfaces that are severely overclosed in the initial configuration of the model. See “Controlling initial contact status in Abaqus/Standard,” Section 35.2.4, for more information. Examples The following input specifies that the contact domain is based on self-contact of an all-inclusive, automatically generated surface but that contact (including self-contact in any overlap regions) should be ignored between the all-inclusive, automatically generated surface and surface_2: *CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR *CONTACT EXCLUSIONS , surface_2 Either of the following methods can be used to exclude self-contact for surface_1 from the contact domain: *CONTACT EXCLUSIONS surface_1, or Output *CONTACT EXCLUSIONS surface_1, surface_1 nodal variables (sometimes Output variables associated with contact fall called constraint variables) and whole surface variables. In addition, Abaqus outputs an array of diagnostic information associated with contact interactions, as discussed in “Contact diagnostics in an Abaqus/Standard analysis,” Section 38.1.1, and internal surfaces generated for general contact. into two categories: For more detailed discussions of variables associated with thermal, electrical, and pore fluid analyses, see the sections on the related contact properties in Chapter 36, “Contact Property Models.” General contact domain and component surfaces the following internal surfaces associated with general contact: Abaqus/Standard generates General_Contact_Faces, General_Contact_Edges, General_Contact_Faces_k, and General_Contact_Edges_k, where k corresponds to an automatically assigned “component number.” The two internal surfaces for general contact without a component number contain all surface faces and all feature edges, respectively, included in the general contact domain. Each feature edge component surface, General_Contact_Edges_k, has a subset of face edges (satisfying the feature edge criteria) of the corresponding face component surface, General_Contact_Faces_k. The face component surfaces have no nodes in common with each other. A lowered-numbered face-based component surface will act as a master surface to a higher-numbered face-based component surface for the surface-to-surface formulation by default. Component numbers do not is considered by the edge-to-surface formulation. Component surfaces are referred to in diagnostic messages for both formulation types. influence what Internal surfaces can be viewed using display groups in the Visualization module of Abaqus/CAE. Internal surface names generated by Abaqus/Standard should not be used in model definitions. Nodal contact variables Nodal contact variables can be contoured on contact surfaces in the Visualization module of Abaqus/CAE. Nodal contact variables include contact pressure and force, frictional shear stress and force, relative tangential motion (slip) of the surfaces during contact, clearance between surfaces, heat or fluid flux per unit area, and fluid pressure. Many of the nodal contact variables written to the output database (.odb) file are often available for all contact nodes, regardless of whether they act as slave or master nodes. In such cases the nodal values are generally affected by more than one contact constraint. Other nodal contact variables are available only at nodes acting as slave nodes. In these cases the value at each slave node reflects a value associated with a particular contact constraint. Most contact output to the data (.dat) and results (.fil) files is associated with individual constraints. Contact pressure The contact pressure distribution is of key interest in many Abaqus analyses. You can view the contact pressure on all contact surfaces except for analytical rigid surfaces and discrete rigid surfaces based on rigid-type elements (the latter restriction does not apply to general contact). You can view a contour plot of the contact pressure error indicator next to a contour plot of the contact pressure to gain perspective on local accuracy of the contact pressure solution in regions where the contact pressure solution is of interest . In some cases you may observe the contact pressure extending beyond the actual contact zone due to the following factors: • The contour plots are constructed by interpolating nodal values, which can cause nonzero values to appear within portions of facets outside of the contact region. For example, this effect is often noticeable at corners, such as when two same-sized, aligned blocks are in contact—if the contact surfaces wrap around the corners, the contact pressure contours will extend slightly around the corners. • To minimize contact stress noise within a region of active contact, Abaqus/Standard computes nodal contact stresses as weighted averages of values associated with active contact constraints in which a node participates. Some filtering is applied to reduce the contact stress values reported for nodes on the fringe of the active contact region (that only weakly participate in contact constraints), but this filtering is not “perfect,” which can result in the contact zone size appearing somewhat exaggerated. Similarly, contact status output will also be affected at nodes that lie on the fringe of the active contact region. In such cases the contact status may be reported as closed at nodes in the exaggerated region even though it is open. Due to these factors, trying to infer the contact force distribution from the contact stress distribution can be somewhat misleading. Instead, you can request nodal contact force output, which accurately represents the contact force distribution present in the analysis. Contact stresses due to edge-to-surface interactions Contact stresses (CSTRESS) reported byAbaqus/Standard to the output database (.odb) file contain contributions from both surface-to-surface and edge-to-surface constraints, if active. Contact stresses (in units of force per area) solely due to edge-to-surface constraints can be output as a separate field (CSTRESSETOS) for visualizing regions where the edge-to-surface contact constraints are active. The edge-to-surface formulation computes contact pressures in units of force per area, by dividing contact force per edge length by a representative surface facet length. Since the contact area depends on the mesh size, edge-to-surface contact stresses are mesh dependent. In addition, because edges represent a discontinuity in the surface smoothness, the true contact stress solution near an edge is commonly characterized by a strong gradient. Error indicators output for contact stresses (CSTRESSERI) are typically quite high for regions in which edge-to-surface constraints are significant. Whole surface variables Whole surface variables are only marginally supported for general contact in Abaqus/Standard because these variable are associated with the overall general contact domain by default rather than individual surfaces associated with general contact. The only way to limit whole surface variables to be affected by a portion of the general contact domain is to specify a node set in the output request. Whole surface variables are computed as sums over all nodes (or optionally limited to a particular node set) of general contact while acting as slave nodes. For example, CFN is the total force acting on slave nodes due to contact pressure. CFN and other whole surface variables for general contact are typically of little utility, because contributions to the variable from different interactions within general contact will often cancel one another and the net result will typically depend on internal assignments of master and slave roles. Requesting output Certain contact variables must be requested as a group. For example, to output the clearance between surfaces (COPEN), you must request the variable CDISP (contact displacements). CDISP outputs both COPEN and CSLIP (tangential motion of the surfaces during contact). A complete listing of available contact variables and identifiers is given in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Output requests can be limited by specifying a node set containing a subset of the nodes acting as slave nodes for some general contact interactions. Instructions on forming these output requests are available in the following sections: • To request output to the data (.dat) file, see “Surface output from Abaqus/Standard” in “Output to the data and results files,” Section 4.1.2. • To request output to the output database (.odb) file, see “Surface output in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3. Output of tangential results Abaqus reports the values of tangential variables (frictional shear stress, viscous shear stress, and relative tangential motion) with respect to the slip directions defined on the surfaces. The definition of slip directions is explained in “Local tangent directions on a surface” in “Contact formulations in Abaqus/Standard,” Section 37.1.1. These directions do not always correspond to the global coordinate system, and they rotate with the contact pair in a geometrically nonlinear analysis. Abaqus/Standard calculates tangential results at each constraint point by taking the scalar product , associated with the constraint point. The number of the variable’s vector and a slip direction, at the end of a variable’s name indicates whether the variable corresponds to the first or second slip direction. For example, CSHEAR1 is the frictional shear stress component in the first slip direction, while CSHEAR2 is the frictional shear stress component in the second slip direction. or Definition of accumulated incremental relative motion (slip) Abaqus/Standard defines the incremental relative motion (also known as slip) as the scalar product of the incremental relative nodal displacement vector and a slip direction. The incremental relative nodal displacement vector measures the motion of a slave node relative to the motion of the master surface. The incremental slip is accumulated only when the slave node is contacting the master surface. The sums of all such incremental slips during the analysis are reported as CSLIP1 and CSLIP2. Details about the calculation of this quantity can be found in “Small-sliding interaction between bodies,” Section 5.1.1 of the Abaqus Theory Manual; “Finite-sliding interaction between deformable bodies,” Section 5.1.2 of the Abaqus Theory Manual; and “Finite-sliding interaction between a deformable and a rigid body,” Section 5.1.3 of the Abaqus Theory Manual. Extending the range for which contact opening output is provided for gaps To reduce computational costs, detailed computations to monitor potential points of interaction are avoided by default where surfaces are separated by a distance greater than the minimum gap distance at which contact forces (or thermal fluxes, etc.) may be transmitted. Therefore, contact opening (COPEN) output is typically not provided where surfaces are opened by more than a small amount compared to surface facet dimensions. You can extend the range for which Abaqus/Standard provides contact opening output; COPEN will be provided up to gap distances equal to a specified “tracking thickness.” Using this control may increase computational cost due to extra contact tracking computations, especially if you specify a large tracking thickness value. Input File Usage: Abaqus/CAE Usage: *SURFACE INTERACTION, TRACKING THICKNESS=value You cannot adjust the default tracking thickness in Abaqus/CAE. 35.2.2 SURFACE PROPERTIES FOR GENERAL CONTACT IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • *CONTACT • *SURFACE PROPERTY ASSIGNMENT • “Specifying surface property assignments for general contact,” Section 15.13.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Surface property assignments: • can be used to specify geometric corrections for regions of a surface; • can be used to change the contact thickness used for regions of a surface based on structural elements or to add a contact thickness for regions of a surface based on solid elements; • can be used to specify surface offsets for regions of a surface based on shell, membrane, rigid, and surface elements; • can be applied selectively to particular regions within a general contact domain; and • cannot be applied to analytical rigid surfaces. Assigning surface properties You can assign nondefault surface properties to surfaces involved in general contact interactions. These properties are considered only when the surfaces are involved in general contact interactions; they are not considered when the surfaces are involved in other interactions such as contact pairs. The general contact algorithm does not consider surface properties specified as part of the surface definition. Surface properties for general contact in Abaqus/Standard are assigned at the beginning of an analysis and cannot be modified across steps. The surface names used to specify the regions with nondefault surface properties do not have to correspond to the surface names used to specify the general contact domain. In many cases the contact interaction will be defined for a large domain, while nondefault surface properties will be assigned to a subset of this domain. Any surface property assignments for regions that fall outside the general contact domain will be ignored. The last assignment will take precedence if the specified regions overlap. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY This option must be used in conjunction with the *CONTACT option and should appear at most once for each value of the PROPERTY parameter discussed below; the data line can be repeated as often as necessary to assign surface properties to different regions. Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Standard): Surface Properties Surface geometry correction By default, contact calculations are based on unsmoothed, faceted representations of the finite element surfaces in a general contact domain. An optional contact smoothing technique simulates a more realistic representation of curved surfaces in the contact calculations, resulting in improved contact stress and pressure accuracy. This contact smoothing technique is discussed in “Smoothing contact surfaces in Abaqus/Standard,” Section 37.1.3. Surface thickness The default surface thickness is equal to the original parent element thickness. Alternatively, you can specify a value for the surface thickness or a thickness scaling factor. A nonzero thickness can be assigned to solid element surfaces; for example, to model the effect of a finite thickness surface coating. Using the original parent element thickness The default surface thickness is equal to the original parent element thickness. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=THICKNESS surface, ORIGINAL (default) Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Standard): Surface Properties: Surface thickness assignments: Edit: Select surface, click the arrows to transfer surface to list of thickness assignments, and enter ORIGINAL in the Thickness column. Specifying a value for the surface thickness You can specify the surface thickness value directly. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=THICKNESS surface, value Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Standard): Surface Properties: Surface thickness assignments: Edit: Select surface, click the arrows to transfer surface to list of thickness assignments, and enter a value for the surface thickness magnitude in the Thickness column. Applying a scale factor to the surface thickness You can apply a scale factor to any value of the surface thickness. For example, if you specify that the original parent element thickness should be used for surf1 and apply a scale factor of 0.5, a value of one half the original parent element thickness will be used for surf1 when it is involved in a general contact interaction (all other surfaces included in the general contact domain will use the default original parent element thickness). Scaling the surface thickness in this way can be used to avoid initial overclosures in some situations. Abaqus/Standard will automatically adjust surface positions to resolve initial overclosures associated with general contact. However, if nodal position adjustments are undesirable (for example, if they would introduce an imperfection in an otherwise flat part, resulting in an unrealistic buckling mode), you may prefer to reduce the surface thickness and avoid the overclosures entirely. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=THICKNESS surface, value or label, scale_factor If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Standard): Surface Properties: Surface thickness assignments: Edit: Select surface, click the arrows to transfer surface to list of thickness assignments, and enter a Scale Factor. Abaqus/CAE Usage: Surface offset A surface offset is the distance between the midplane of a thin body and its reference plane (defined by the nodal coordinates and element connectivities). It is computed by multiplying the offset fraction (specified as a fraction of the surface thickness) by the surface thickness and the element facet normal. This defines the position of the midsurface and, thus, the position of the body with respect to the reference surface; the coordinates of the nodes on the reference surface are not modified. Surface offsets can be specified only for surfaces defined on shell and similar elements (i.e., membrane, rigid, and surface elements). Surface offsets specified for other elements (e.g., solid or beam elements) will be ignored. By default, surface offsets specified in element section definitions will be used in the general contact algorithm. You specify the surface offset as a fraction of the surface thickness. The surface offset fraction can be set equal to the offset fraction used for the surface’s parent elements or to a specified value. Surface offsets specified for general contact do not change the element integration. Input File Usage: Use the following option to use the surface offset fraction from the surface’s parent elements (default): *SURFACE PROPERTY ASSIGNMENT, PROPERTY=OFFSET FRACTION surface, ORIGINAL Abaqus/CAE Usage: Use the following option to specify a value for the surface offset fraction: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=OFFSET FRACTION surface, offset The offset can be specified as a value or a label (SPOS or SNEG). Specifying SPOS is equivalent to specifying a value of 0.5; specifying SNEG is equivalent to specifying a value of −0.5. Interaction module: Create Interaction: General contact (Standard): Surface Properties: Shell/Membrane offset assignments: Edit: Select surface, and click the arrows to transfer surface to list of offset assignments. In the Offset Fraction column, enter ORIGINAL to use the surface offset fraction from the surface's parent elements, enter SPOS to use a surface offset fraction of 0.5, enter SNEG to use a surface offset fraction of −0.5, or enter a value for the surface offset fraction. Feature edges General contact in Abaqus/Standard includes a supplementary edge-to-surface contact formulation for feature edges of solid and shell bodies, as discussed in “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1. By default, the edge-to-surface contact formulation considers perimeter edges and edges corresponding to initial geometric feature angles of 45° and higher. You can control the feature edge criterion globally or locally. Some aspects of the contact property assignment options apply only to the surface-to-surface formulation . The edge-to-surface formulation always uses the penalty enforcement method and only involves displacement degrees of freedom. For example, the edge-to-surface formulation does not contribute to thermal gap conductance across a contact interface. Specifying a cutoff feature angle The feature angle is the angle formed between normals of two facets connected to an edge. The angles between facets are based on the initial configuration. A negative angle results at concave meetings of facets; therefore, these edges are never included in the contact domain. Figure 35.4.2–4 shows some examples of how the feature angle is calculated for different edges.The feature angle for edge A is 90° (the angle between ). Edge C forms a T-intersection with three facets (shown in two dimensions in Figure 35.4.2–5); its feature angles are 0°, −90°, and −90°. Perimeter edges (for example, edge D in Figure 35.4.2–4) can be thought of as a special type of feature edge where the feature angle is 180°. ); the feature angle for edge B is −25° (the angle between and and If a feature angle criterion is in effect (by default or because you specified it), geometric edges of solid and shell bodies with feature angles greater than or equal to the specified angle are included in the general contact domain. The contact inclusion and exclusion options (discussed in “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1) apply to both the surface-to-surface contact n2 n1 n2 n2 n3 ( )_ 25o n3 n1 SURFACE PROPERTIES FOR Abaqus/Standard GENERAL CONTACT ( )_ n5 n4 n5 n4 n7 D (perimeter edge) n5 (+) 180 n7 n6 0o n II n Figure 35.2.2–1 Calculating the feature angle. _ 90o _ 90o arrows are perpendicular to surface facets Figure 35.2.2–2 Feature angles for a T-intersection (for example, edge C in Figure 35.4.2–4). formulation and the edge-to-surface contact formulation (and further control which portions of surfaces may interact with either formulation). The sign of the feature angle is considered when determining whether or not a geometric feature edge should be included in the general contact domain. For example, if a cutoff feature angle of 20° were specified, edge A would be activated as a feature edge in the contact model (because the feature angle of 90° is greater than the cutoff of 20°) but edges B and C would not be activated (because the feature angle at edge B is −25° and the maximum feature angle at edge C is 0°, which are both less than the cutoff of 20°). The cutoff feature angle cannot be set to less than 0° or more than 180°. Specifying a small cutoff feature angle (for example, less than 20°) may considerably increase run time without a major impact on the results compared to a larger cutoff angle (> 20°). The default feature angle cutoff is 45°. Figure 35.4.2–6 illustrates further how the feature angle is used to determine which geometric feature edges are activated in the general contact domain. The table to the right of the figure lists the feature angle values for various edges in the model. Edges connected to shell facets, but not on the shell perimeter, have more than one corresponding feature angle. The largest feature angle at an edge is compared to the default or specified cutoff feature angle. For example, if the default cutoff feature angle Thin solid lines indicate feature edges. Thick solid lines indicate shell perimeter edges. Edge Largest feature angle at edge Other feature angles at edge Shells Solid Dashed lines indicate element boundaries for which edge-to-edge contact is not modeled. approximately +105 o approximately 30 _ o o 0 +180 o o +90 o 0 none none _ 90 o none _ o 90 _ _ o o 90 , 90 Figure 35.2.2–3 Feature edges activated in the general contact domain for the default cutoff feature angle of 45°. of 45° is in effect, edges A, D, and E would be considered for edge-to-surface contact, while edges B, C, and F would be ignored for edge-to-surface contact. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, feature_angle_value Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Standard): Surface Properties: Feature edge criteria assignments: Edit: Select the surface, click the arrows to transfer the surface to the list of feature assignments, and enter a numerical value for the cutoff feature angle (in degrees) in the Feature Edge Criteria column. Specifying that only perimeter edges should be activated You can specify that only perimeter edges should be considered by the edge-to-surface formulation globally or in a local region. Perimeter edges occur on “physical” perimeters of shell elements and on “artificial” edges that occur when a subset of exposed facets on a body are included in the general contact domain. The classification of an edge as being on the perimeter of the contact domain (or as a geometric edge with a particular feature angle) is based on the contact inclusion and contact exclusion definitions and the mesh characteristics. When structural elements share nodes with continuum elements, the perimeter edges will not be activated on the structural elements because the criterion to designate them as such is no longer satisfied. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, PERIMETER EDGES Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Standard): Surface Properties: Feature edge criteria assignments: Edit: Select the surface, click the arrows to transfer the surface to the list of feature assignments, and enter PERIMETER in the Feature Edge Criteria column. Specifying that feature edges should not be included You can specify that no edges should be considered by the edge-to-surface formulation globally or in a local region. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, NO FEATURE EDGES Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Standard): Surface Properties: Feature edge criteria assignments: Edit: Select the surface, click the arrows to transfer the surface to the list of feature assignments, and enter NONE in the Feature Edge Criteria column. 35.2.3 CONTACT PROPERTIES FOR GENERAL CONTACT IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • “Mechanical contact properties: overview,” Section 36.1.1 • “Contact pressure-overclosure relationships,” Section 36.1.2 • “Contact damping,” Section 36.1.3 • “Frictional behavior,” Section 36.1.5 • *CONTACT • *CONTACT PROPERTY ASSIGNMENT • *SURFACE INTERACTION • “Specifying and modifying contact property assignments for general contact,” Section 15.13.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Contact properties: • define the surface interaction models that govern the behavior of surfaces when they are in contact; and • can be applied selectively to particular regions within a general contact domain. Assigning contact properties The default contact property model in Abaqus/Standard assumes “hard” contact in the normal direction, no friction, no thermal interactions, etc. You can assign a nondefault contact property definition (surface interaction) to specified regions of the general contact domain. Contact properties for general contact in Abaqus/Standard are assigned at the beginning of the analysis and cannot be modified across steps, with an exception for changes to the friction model, as discussed below. The surface names used to specify the regions where nondefault contact properties should be assigned do not have to correspond to the surface names used to specify the general contact domain. In many cases the contact interaction will be defined for a large domain, while nondefault contact properties will be assigned to a subset of this domain. Any contact property assignments for regions that fall outside of the general contact domain will be ignored. The last assignment will take precedence if the specified regions overlap. Input File Usage: *CONTACT PROPERTY ASSIGNMENT surface_1, surface_2, interaction_property_name Abaqus/CAE Usage: This option must be used in conjunction with the *CONTACT option and should appear at most once; the data line can be repeated as often as necessary to assign contact properties to different regions. If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is assumed. Surfaces can be defined to span multiple unattached bodies, so self-contact is not limited to contact of a single body with itself. If the interaction property name is omitted, the unnamed set of default contact If an interaction property name properties in Abaqus/Standard is assumed. is specified, it must also appear as the value of the NAME parameter on a *SURFACE INTERACTION option in the model portion of the input file. Use the following options to assign a global contact property to the entire general contact domain: Interaction module: Create Interaction: General contact (Standard): Contact Properties: Global property assignment: interaction_property_name Use the following options to assign contact properties to individual surface pairs: Interaction module: Create Interaction: General contact (Standard): Contact Properties: Individual property assignments: Edit: select the surfaces and the contact property in the columns on the left, and click the arrows in the middle to transfer them to the list of contact property assignments In Abaqus/CAE you must assign a global contact property; Abaqus/CAE does not assume a default contact interaction property. Contact properties assigned to individual surface pairs override the global assignment. Changing friction properties during an analysis The friction properties associated with a given named surface interaction definition can be modified in any particular step of an Abaqus/Standard analysis, as discussed in “Changing friction properties during an Abaqus/Standard analysis” in “Frictional behavior,” Section 36.1.5. Example The following contact property assignments are specified below as model data in a general contact analysis: • a global assignment of contProp1 to the entire general contact domain; • a local assignment of contProp2 to self-contact for surf1; • a local assignment of the default Abaqus contact property to contact between surf2 and surf3; and • a local assignment of contProp3 to contact between the entire contact domain and surf4. The friction coefficient for contProp3 is reset from the initial value of 0.20 to 0.05 in the second step. *SURFACE INTERACTION, NAME=contProp1 *FRICTION 0.1 *SURFACE INTERACTION, NAME=contProp2 *FRICTION 0.15 *SURFACE INTERACTION, NAME=contProp3 *FRICTION 0.20 *CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR *CONTACT PROPERTY ASSIGNMENT , , contProp1 surf1, surf1, contProp2 surf2, surf3, , surf4, contProp3 … *STEP Step1 *STATIC … *END STEP *STEP Step2 *STATIC … *CHANGE FRICTION, INTERACTION NAME=contProp3 *FRICTION 0.05 *END STEP 35.2.4 CONTROLLING INITIAL CONTACT STATUS IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • *CONTACT INITIALIZATION ASSIGNMENT • *CONTACT INITIALIZATION DATA • “Creating contact initializations,” Section 15.12.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Specifying and modifying contact initialization assignments for general contact,” Section 15.13.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Contact initialization controls for general contact in Abaqus/Standard: • can be used to specify whether initial overclosures should be resolved without generating stresses and strains or treated as interference fits that are gradually resolved over multiple increments; and • can be used to specify nondefault search zones that determine which nodes are affected in the case of strain-free adjustments or interference fits. Abaqus/Standard initializes the contact state based on the gap or penetration state observed in the initial geometry. Small initial contact overclosures are resolved by default using strain-free adjustments to the positions of surface nodes. You can define alternative contact initialization methods and then assign them to contact interactions. For example, you can choose to have initial overclosures for certain interactions treated as interference fits. Default contact initialization method By default, the general contact algorithm adjusts the initial positions of surface nodes during preprocessing to remove small initial surface overclosures without generating strains or stresses in the model, as shown in Figure 35.2.4–1. These adjustments are intended to correct only minor mismatches associated with mesh generation. General contact automatically assigns master and slave roles for contact interactions, as discussed in “Numerical controls for general contact in Abaqus/Standard,” Section 35.2.6. Abaqus/Standard calculates an overclosure tolerance based on the size of the underlying element facets on a slave surface. Slave surfaces in a particular interaction are repositioned onto the associated master surface (using strain-free adjustments) if the two surfaces are initially overclosed by a distance smaller than the calculated tolerance. Initial gaps between surfaces remain unchanged by default adjustments. If a portion of a slave surface is initially overclosed by a distance greater than the calculated tolerance, Abaqus/Standard automatically generates a contact exclusion for this surface portion and its associated Figure 35.2.4–1 Configuration of contact surfaces after strain-free adjustments to resolve overclosure. master surface. Therefore, general contact does not create interactions between surfaces (or portions of surfaces) that are severely overclosed in the initial configuration of the model, and these surfaces can freely penetrate each other throughout the analysis. General contact uses the finite-sliding, surface-to-surface contact formulation, so penetration/gap calculations are computed as averages over finite regions; therefore, it is possible for penetrations and gaps to be present at individual surface nodes after the adjustments. The default adjustments will not resolve initial crossings of two reference surfaces associated with shells or membranes, although techniques to resolve such cases are discussed in “Assigning contact initializations to shell surfaces.” Defining alternative contact initialization methods You can define alternative contact initialization methods if the default behavior is not desired. For example, you may want to increase the tolerance for deep penetrations or specify that certain openings should be adjusted to a “just touching” status. Furthermore, some analyses call for initial overclosures to be treated as interference fits rather than resolved with strain-free adjustments. To modify the contact initialization behavior, you must define one or more alternate contact initialization methods and then identify which surface pairings are to use which methods. You assign a name to each contact initialization method. This name is used in the assignment of a contact initialization method to specific surface pairings . Input File Usage: *CONTACT INITIALIZATION DATA, NAME=contact_initialization_method_name Abaqus/CAE Usage: Interaction module: Interaction→Contact Initialization→Create: Name: contact_initialization_method_name Increasing the search zones for strain-free adjustments As discussed above in “Default contact initialization method,” initial gaps and large initial overclosures between surfaces are not adjusted by the default contact initialization methods. You can optionally specify nondefault search distances both above and below the surfaces in an interaction; slave surfaces that lie within these search distances are repositioned directly onto their associated master surface using strain-free nodal adjustments. Abaqus/Standard takes shell thickness into account when calculating these search distances. Specifying a search distance above a surface is used to close small initial gaps between surfaces. Specifying a search distance below a surface is used to increase the default overclosure tolerance that Abaqus/Standard uses when performing strain-free adjustments; if you specify a search distance smaller than the default overclosure tolerance, Abaqus/Standard uses the default tolerance instead. As with the default initialization behavior, contact exclusions are created for initial overclosures that are larger than the specified search zone. Increasing the extent of the search zones for strain-free adjustments can potentially increase the computational cost of an analysis. It is not generally recommended that you specify a large search zone since this may cause mesh distortion when nodes are repositioned over large distances. Input File Usage: *CONTACT INITIALIZATION DATA, SEARCH ABOVE=a, SEARCH BELOW=b Abaqus/CAE Usage: Interaction module: Interaction→Contact Initialization→Create: Resolve with strain-free adjustments: Ignore overclosures greater than: b, Ignore initial openings greater than: a Specifying an initial clearance distance By default, the strain-free adjustments discussed above will adjust initial nodal positions such that surfaces are “just-touching” (with zero penetration/separation). Alternatively, Abaqus/Standard can make the adjustments to achieve an initial clearance distance that you specify. The adjustments will occur only for regions that satisfy the search zone tolerances, as discussed above. Mesh distortion can occur if large strain-free adjustments are necessary to achieve the specified initial clearance distance. Input File Usage: Abaqus/CAE Usage: *CONTACT INITIALIZATION DATA, INITIAL CLEARANCE=h Interaction module: Interaction→Contact Initialization→Create: Specify clearance distance: h Modeling interference fits the general contact algorithm in Abaqus/Standard can treat initial overclosures as Optionally, interference fits. The general contact algorithm uses a shrink-fit method to gradually resolve the interference distance over the first step of the analysis (if multiple load increments are used for the first step) as shown in Figure 35.2.4–2, such that the fraction of the interference resolved up to and including a particular increment approximately corresponds to the fraction of the step completed. Stresses and strains are generated as the interference is resolved. Gradually resolving interference over several increments improves robustness (compared to always resolving the full interference in the first increment, which is the default for contact pairs) for cases in which a nonlinear response occurs for “interference-fit loading.” It is generally recommended that you do not apply other loads while the interference fit is being resolved. Because contact conditions are enforced in an average sense in a region around each constraint location for the surface-to-surface contact formulation used by general contact in Abaqus/Standard, BEGINNING OF STEP MIDDLE OF STEP END OF STEP Figure 35.2.4–2 Gradual resolution of contact interference fit. penetrations or gaps may be observed at slave nodes when surface-to-surface constraints are in a zero-penetration state. Input File Usage: Abaqus/CAE Usage: *CONTACT INITIALIZATION DATA, INTERFERENCE FIT Interaction module: Interaction→Contact Initialization→Create: Treat as interference fits Increasing the tolerance for interference fits Abaqus/Standard calculates an overclosure tolerance based on the size of the underlying element facets on a slave surface . An interference fit between two surfaces affects only those slave surfaces that are overclosed by a distance smaller than the calculated tolerance; contact is ignored entirely for surfaces that are overclosed by a distance greater than the calculated tolerance. Optionally, you can redefine the overclosure tolerance to include larger overclosures in the If you specify a tolerance that is smaller than the default calculated tolerance, interference fit. Abaqus/Standard uses the default calculated tolerance instead. Input File Usage: *CONTACT INITIALIZATION DATA, INTERFERENCE FIT, SEARCH BELOW=b Abaqus/CAE Usage: Interaction module: Interaction→Contact Initialization→Create: Treat as interference fits: Ignore overclosures greater than: b Specifying the interference distance By default, the interference distance is implied by the initial overclosure of the mesh; alternatively, you can specify the interference distance. In this case Abaqus/Standard first makes strain-free adjustments of nodal positions such that the initial overclosure in the adjusted configuration corresponds to the specified interference distance and then invokes the shrink fit method discuss above, as depicted in Figure 35.2.4–3. Mesh distortion can occur if large strain-free adjustments are necessary to achieve the specified interference distance. The search region for the strain-free adjustments and subsequent shrink fit resolution is at least at large as the search region for the case discussed previously in which the interference distance is not specified. The search region will include overclosures at least as large as the specified interference fit and openings at least as large as the optionally specified search distance above a surface. Input File Usage: *CONTACT INITIALIZATION DATA, INTERFERENCE FIT=h, SEARCH ABOVE=a, SEARCH BELOW=b Abaqus/CAE Usage: Interaction module: Interaction→Contact Initialization→Create: Treat as interference fits: Specify interference distance: h: Ignore overclosures greater than: b, Ignore initial openings greater than: a Deactivating friction while resolving interference fits The presence of a friction model can degrade the robustness of resolving interference fits. It is generally recommended that you temporarily deactivate friction models while Abaqus/Standard resolves interference fits. You can deactivate the friction model in the first step while interference fits are resolved using the “change friction” method discussed in “Changing friction properties during an Abaqus/Standard analysis” in “Frictional behavior,” Section 36.1.5. Cases in which interference fit resolution with contact pairs is preferred Large interferences may be difficult to resolve with the finite-sliding, surface-to-surface formulation. Using this formulation, overclosures tend to be resolved along the slave facet normal directions; using the node-to-surface formulation, which is available only with the contact pair algorithm, overclosures tend to be resolved along the master surface normal directions. Figure 35.2.4–4 illustrates a case where differing normal directions lead to undesirable tangential motion during an interference fit. In some cases it may be preferable to resolve large initial overclosures with node-to-surface discretization using the contact pair algorithm . Original mesh geometry After strain-free adjustments Middle of step End of step Figure 35.2.4–3 Treatment of a specified interference distance that differs from the interference implied by the original mesh. surface-to-surface node-to-surface master surface overclosure resolution direction Figure 35.2.4–4 Comparison of contact formulations in an example with a large interference fit. Assigning contact initialization methods You can assign contact initialization methods to selected surface pairings. The surface names used in the assignment of contact initialization methods do not have to correspond to the surface names used to specify the general contact domain. In many cases nondefault contact initialization methods will be assigned to a subset of the overall general contact domain. Any contact initialization assignments for regions that fall outside of the general contact domain are ignored. The last assignment takes precedence if the specified interactions overlap. Input File Usage: Use the following option to assign contact inititialization methods: *CONTACT INITIALIZATION ASSIGNMENT surface_1, surface_2, contact_initialization_method_name This option must be used in conjunction with the *CONTACT option. The data line can be repeated as often as necessary to assign contact initialization methods to different regions. If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is assumed. Keep in mind that surfaces can be defined to span multiple unattached bodies, so self-contact is not limited to contact of a single body with itself. If the contact initialization method name is omitted, the default contact initialization method in Abaqus/Standard is assumed. If a contact initialization method name is specified, it must also appear as the value of the NAME Abaqus/CAE Usage: parameter on a *CONTACT INITIALIZATION DATA option in the model portion of the input file. Interaction module: Create Interaction: General contact (Standard): Contact Properties: Initialization assignments: Edit: select the surfaces and the initialization in the columns on the left, and click the arrows in the middle to transfer them to the list of contact initialization assignments Assigning contact initializations to shell surfaces The surfaces in a contact initialization assignment can be either single- or double-sided. Single-sided surfaces must have consistent surface normal orientations for adjacent faces. Strain-free adjustments will not move surface nodes past the reference surface of the opposing surface if the assignment of a contact initialization method is made with double-sided surfaces. Using single-sided surfaces in the assignment of a contact initialization method for shells or membranes provides enhanced control over contact initialization for cases in which shell or membrane reference surfaces are initially crossed or are initially on the wrong side of each other. Figure 35.2.4–5 shows examples of adjustments for nearby segments of shell surfaces. For the case shown on the left it is assumed that single-sided surfaces with normal directions pointing away from each another are used in the assignment of the contact initialization method. In this case nodes are moved across the opposing reference surface during the strain-free adjustments. For the case shown on the right in Figure 35.2.4–5 it is assumed that single-sided surfaces with normal directions pointing toward each other are used in the assignment of the contact initialization method. In this case an initial gap is observed between the single-sided surfaces (which is also the case if double-sided surfaces are used in the contact initialization assignment). No strain-free adjustments will be made by default for openings such as this; however, if a nondefault contact initialization method is specified with an initial opening search tolerance set to a value exceeding the initial separation distance, strain-free adjustments will close the gap as shown in the figure (without moving nodes past the opposing reference surface). Examples The following contact initialization assignments are specified below as model data in a general contact analysis: • a global assignment of shrink_fit to the entire general contact domain; • a local assignment of shrink_fit_local to contact between surfaces surface_A and surface_B—the search zone is specified explicitly to increase the default overclosure tolerance; • a local assignment of the default Abaqus contact surface_C and surface_D; and initialization method to contact between • a local assignment of sfa_pickside to contact between double-sided surfaces surface_1 each surface, surface_1_TOP and side of and surface_2 by specifying one surface_2_BOTTOM, in the data lines . Surface 1 top Overclosure Gap Surface 1 bottom Surface 2 top Surface 2 bottom Overclosure resolution Gap resolution Surface 2 Surface 1 Surface 1 Surface 2 Figure 35.2.4–5 Strain-free adjustments during contact initialization for single-sided shell surfaces. *CONTACT INITIALIZATION DATA, NAME=shrink_fit, INTERFERENCE FIT *CONTACT INITIALIZATION DATA, NAME=shrink_fit_local, INTERFERENCE FIT, SEARCH BELOW = 15.0 *CONTACT INITIALIZATION DATA, NAME=sfa_pickside, SEARCH BELOW = 10.0 … *CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR *CONTACT INITIALIZATION ASSIGNMENT , , shrink_fit surface_A, surface_B, shrink_fit_local surface_C, surface_D, surface_1_TOP, surface_2_BOTTOM, sfa_pickside 35.2.5 STABILIZATION FOR GENERAL CONTACT IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • *CONTACT • *CONTACT STABILIZATION • “Creating contact stabilization definitions,” Section 15.12.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Specifying and modifying contact stabilization assignments for general contact,” Section 15.13.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Contact stabilization for general contact in Abaqus/Standard: • is often helpful in stabilizing unconstrained rigid body modes in static analyses; • can be applied selectively to particular regions within a general contact domain; and • can vary over time. Stabilization based on viscous damping of relative motion between surfaces Contact stabilization is based on viscous damping opposing incremental relative motion between nearby surfaces, in the same manner as contact damping . The most common purpose of contact stabilization is to stabilize otherwise unconstrained “rigid body motion” before contact closure and friction restrain such motions. A goal of artificial stabilization, such as contact stabilization, is to provide enough stabilization to enable a robust, efficient simulation without degrading the accuracy of the results. In most cases contact stabilization is not activated by default (an exception is discussed in “Contact at a single point” in “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 38.1.2), so you will generally need to activate contact stabilization if convergence problems associated with unconstrained rigid body modes may be present in your analysis. Once activated, contact stabilization is highly automated. The following expressions for the normal pressure, , associated with contact stabilization involve many semi-automated factors to facilitate achieving the desired stabilization characteristics: , and shear stress, where and is a damping coefficient; are the relative normal and tangential velocities, respectively, between nearby points on opposing contact surfaces; is a constant scale factor; is a time-dependent scale factor; is a scale factor based on the increment number; is a scale factor based on the separation distance; and is a constant scale factor for tangential stabilization. The damping coefficient and relative velocities are computed by Abaqus/Standard. The damping coefficient is equal to a fixed, small fraction, , times a representative stiffness of elements underlying the contact surfaces, . Relative velocities in a static analysis are computed by dividing relative incremental displacements, , by the time increment size, , times the time period of the step, and . Therefore, the following contact stabilization expressions apply to statics: where the portions within brackets can be thought of as stabilization stiffnesses (representing resistance to relative motion between nearby surfaces). The stabilization stiffness is inversely proportional to the time increment size, which is a desirable characteristic. Stabilization stiffness increases if the time increment size is reduced, which happens automatically in Abaqus/Standard if convergence difficulties occur for a particular time increment size. Assigning stabilization to interactions Contact stabilization assignments for specific interactions within general contact can be made globally or locally and are specified as part of step definitions. In most cases you only need to specify which interactions are eligible for contact stabilization without adjusting the scale factors discussed previously. Input File Usage: Use the following option to specify which interactions should use contact stabilization: *CONTACT STABILIZATION surf_1, surf_2 If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted, contact between the first surface and itself is assumed. Abaqus/CAE Usage: Use the following options to assign contact stabilization definitions to individual surface pairs: Interaction module: Create Interaction: General contact (Standard): Contact Properties: Stabilization assignments: Edit: select the surfaces and the stabilization name in the columns on the left, and click the arrows in the middle to transfer them to the list of contact stabilization assignments Specifying stabilization scale factors In some cases you may want to adjust one or more scale factors associated with contact stabilization. You can use multiple instances of this option to achieve different scale factor settings for different general contact interactions. Constant scale factors The default setting of As shown in the expressions above for the stabilization pressure and shear stress, the scale factor applies to normal and tangential stabilization, whereas the scale factor stabilization. The default setting of the constant scale factor applies only to tangential is unity for the specified interactions. is zero such that no tangential stabilization stiffness exists by default for the specified interactions. Normal-direction-only contact stabilization is adequate in many cases. Other analyses can benefit from tangential stabilization stiffness; however, if you specify a nonzero setting of , keep in mind that tangential contact stabilization often absorbs significant energy if large relative tangential motion occurs between nearby surfaces. Large energy absorbed by stabilization is one indication that analysis results are likely to be significantly affected by the stabilization. Normal contact stabilization is much less likely to absorb significant energy and, thus, tends to have less influence on the results. Input File Usage: *CONTACT STABILIZATION, SCALE FACTOR= TANGENT FRACTION= , Abaqus/CAE Usage: Interaction module: Interaction→Contact Stabilization→Create: Scale factor: , Tangential factor: Time-dependent scale factors and control time-dependence of the contact stabilization. By default, is a per-increment reduction factor (equal to 0.1 by default) and The scale factors is equal to the fraction of the step remaining. The other factor varies according to , where is the increment number within a step. These defaults imply that the stabilization is reduced by more than an order of magnitude in successive increments of the same size and that no stabilization is applied in the final increment of a step. The defaults are appropriate for most cases in which contact stabilization is intended to provide stabilization in initial increments while contact is being established. amplitude curve that will govern Two options are provided for adjusting the time-dependent scale factors: you can refer to an (recall the expression given previously). For example, if unstable modes remain after contact is established, , and you can specify the value of you may want to remain equal to unity throughout a step for certain interactions, which can be accomplished by referring to an amplitude with a constant value of one and setting the per-increment reduction factor, , equal to one. and Input File Usage: *AMPLITUDE, NAME=name *CONTACT STABILIZATION, AMPLITUDE=name, REDUCTION PER INCREMENT= Abaqus/CAE Usage: Load or Interaction module: Create Amplitude: Name: name Interaction module: Interaction→Contact Stabilization→Create: Reduction factor: , Amplitude: name Resetting time-dependent scale factors in subsequent steps Contact stabilization definitions do not affect subsequent steps unless an amplitude reference is specified. If an amplitude based on the total time is specified, the same amplitude curve continues to govern the variation of in subsequent steps until a new contact stabilization definition is assigned If an amplitude based on the step time is specified, the amplitude curve governs to the interaction. remains constant (at the ending value) in subsequent steps until a new contact stabilization definition is assigned to the interaction. In both cases you can also reset the contact stabilization definition to remove stabilization from a step. Resetting ensures that contact stabilization options from prior steps do not affect the current step. for a single step and Input File Usage: Abaqus/CAE Usage: *CONTACT STABILIZATION, RESET Load or Interaction module: Create Amplitude: Name: name Interaction module: Interaction→Contact Stabilization→Create: Reset values from previous steps Gap-dependent scale factor The scale factor controls contact stabilization as a function of the local separation distance between surfaces. By default, this factor is unity for zero gap distance and is zero when the gap distance is greater than or equal to a characteristic surface dimension. You can control the gap distance at which becomes zero. Specifying a large value for this threshold distance is not recommended because of the tendency to increase solution cost per iteration (due to increased connectivity) as the threshold distance increases. Input File Usage: Abaqus/CAE Usage: *CONTACT STABILIZATION, RANGE=distance Interaction module: Interaction→Contact Stabilization→Create: Zero stabilization distance: Specify: distance Hierarchy of contact stabilization definitions The interface discussed above is the recommended method for specifying contact stabilization for general contact; however, contact stabilization can be introduced for general contact interactions in two other ways. The order of precedence in cases of overlap is as follows: • First priority is given to the contact stabilization assignment options discussed in this section. • Second priority is given to the contact stabilization assignment options discussed in “Automatic stabilization of rigid body motions in contact problems” in “Adjusting contact controls in Abaqus/Standard,” Section 35.3.6. • Third priority is given to the default contact stabilization discussed in “Contact at a single point” in “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 38.1.2. 35.2.6 NUMERICAL CONTROLS FOR GENERAL CONTACT IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • *CONTACT • *CONTACT FORMULATION • *CONTACT CONTROLS • “Specifying master-slave assignments for general contact,” Section 15.13.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Numerical controls associated with the general contact algorithm in Abaqus/Standard: • should not be modified from their default settings for the majority of problems; • can be used for problems where the default settings do not provide cost-effective solutions; • can be used to control the master-slave roles and the sliding formulation; and • in some cases can be applied selectively to particular regions within a general contact domain. Contact formulation The general contact algorithm uses the finite-sliding, surface-to-surface contact formulation, which is discussed in “Contact formulations in Abaqus/Standard,” Section 37.1.1. Other contact formulations are not available for general contact in Abaqus/Standard. Constraint enforcement method The general contact algorithm uses a penalty method to enforce active contact constraints by default. Other constraint enforcement methods can be specified as part of the surface interaction (i.e., contact property) definition, as discussed in “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2. Assignment of contact properties to general contact interactions is discussed in “Contact properties for general contact in Abaqus/Standard,” Section 35.2.3. Numerical controls for friction Numerical controls associated with friction are discussed in “Frictional behavior,” Section 36.1.5. Master and slave roles The surface-to-surface contact formulation used by general contact generates individual contact constraints using a master-slave approach, as discussed in “Contact formulations in Abaqus/Standard,” Section 37.1.1. Abaqus/Standard assigns default pure master-slave roles for contact involving disconnected bodies within the general contact domain. Internal surfaces are generated automatically using the naming convention General_Contact_Faces_k, where k corresponds to an automatically assigned component number. By default, the lowered-number component surfaces will act as master surfaces to the higher-numbered component surfaces. You can determine the default pure master-slave roles by viewing the automatically generated internal surfaces in the Visualization module of Abaqus/CAE . Self-contact within a body is treated with balanced master-slave contact by default, with each surface node acting as a master node in some constraints and as a slave node in other constraints. For example, if the general contact domain spans three disconnected bodies, the following three internal “component-surfaces” for general contact are created automatically: • General_Contact_Faces_1 • General_Contact_Faces_2 • General_Contact_Faces_3 By default, the first surface listed acts as a master to the other two, and General_Contact_Faces_2 acts as a master to General_Contact_Faces_3. Self-contact within each of these three surfaces is modeled with balanced master-slave contact by default. Specifying non-default master-slave roles You can override the default master-slave roles by specifying pure master-slave roles or by specifying that balanced master-slave contact should be used. The default master-slave treatment works well in most cases. Keep the following points in mind when modifying the master-slave assignments, in addition to other factors discussed in this section: • Do not use the internally generated component surfaces when assigning alternative master-slave roles (instead, use surface names that you define). • The master-slave role assignments are part of the model definition and cannot be modified from step to step. • The guidelines for assigning pure master-slave roles for contact pairs discussed in “Defining contact between two separate surfaces” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1, are also applicable for situations in which you reassign pure master-slave roles for general contact. • The limitations of balanced (symmetric) master-slave contact pairs discussed in “Using symmetric master-slave contact pairs to improve contact modeling” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1, are also applicable for situations in which you reassign balanced master-slave contact for general contact. Balanced master-slave contact can result in reduced robustness due to the increased number of constraints and the possibility of overconstraints. Input File Usage: Use the following option to indicate that the first surface should be considered the slave surface: *CONTACT FORMULATION, TYPE=MASTER SLAVE ROLES surf_1, surf_2, SLAVE Use the following option to indicate that the first surface should be considered the master surface: *CONTACT FORMULATION, TYPE=MASTER SLAVE ROLES surf_1, surf_2, MASTER If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. The second surface name must be specified. Use the following option to specify that balanced master-slave contact should be used between two surfaces: *CONTACT FORMULATION, TYPE=MASTER SLAVE ROLES surf_1, surf_2, BALANCED If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted, contact between the first surface and itself is assumed. Interaction module: Create Interaction: General contact (Standard): Contact Formulation: Master-slave assignments: Edit: select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of master-slave assignments. In the First Surface Type column, enter SLAVE to indicate that the first surface should be considered the slave surface, enter MASTER to indicate that the first surface should be considered the master surface, or enter BALANCED to specify that balanced master-slave contact should be used between the two surfaces. Abaqus/CAE Usage: Automatically generated contact exclusions Abaqus/Standard automatically generates contact exclusions for the master-slave roles opposite to specified pure master-slave roles; therefore, self-contact is excluded for any regions of the two surfaces that overlap. For example, specifying that the general contact interaction between surf_A and surf_B should use pure master-slave contact with surf_A considered to be the slave surface would result in exclusions being generated internally for master faces of surf_A contacting slave faces of surf_B; self-contact would be excluded for the region of overlap between surf_A and surf_B. An error message is issued if the second surface name is omitted or is the same as the first surface name since this input would result in the exclusion of self-contact for the surface. Smoothness of contact force redistribution upon sliding You can control the smoothness of nodal contact force redistribution upon sliding. The default setting, which is generally appropriate, results in the smoothness of the nodal force redistribution being of the same order as the elements underlying the slave surface; that is, linear redistribution smoothness for linear elements, and quadratic redistribution smoothness for second-order elements. Quadratic redistribution smoothness usually tends to improve convergence behavior and improve resolution of contact stresses within regions of rapidly varying contact stresses. However, quadratic redistribution smoothness tends to increase the number of nodes involved in each constraint, which can increase the computational cost of the equation solver. Linear redistribution smoothness tends to provide better resolution of contact stresses near edges of active contact regions and, therefore, occasionally results in better convergence behavior. Input File Usage: Use the following option to indicate that the smoothness of the contact force redistribution upon sliding should be of the same order as the elements underlying the slave surface: *CONTACT FORMULATION, TYPE=SLIDING TRANSITION surf_1, surf_2, ELEMENT ORDER SMOOTHING If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted, contact between the first surface and itself is assumed. Use the following option to indicate linear smoothness of the contact force redistribution upon sliding: *CONTACT FORMULATION, TYPE=SLIDING TRANSITION surf_1, surf_2, LINEAR SMOOTHING If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted, contact between the first surface and itself is assumed. Use the following option to indicate quadratic smoothness of the contact force redistribution upon sliding: *CONTACT FORMULATION, TYPE=SLIDING TRANSITION surf_1, surf_2, QUADRATIC SMOOTHING If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted, contact between the first surface and itself is assumed. Additional global numerical controls for general contact Some additional numerical contact controls can be modified globally from step-to-step for general contact; you cannot specify contact controls for individual surface pairings within the general contact domain. You can apply contact stabilization to address rigid body modes that occur prior to the establishment of contact in the model, and you can adjust the tolerances used by Abaqus/Standard to determine contact penetrations and separations; both techniques are discussed in “Adjusting contact controls in Abaqus/Standard,” Section 35.3.6. 35.3 Defining contact pairs in Abaqus/Standard • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • “Assigning surface properties for contact pairs in Abaqus/Standard,” Section 35.3.2 • “Assigning contact properties for contact pairs in Abaqus/Standard,” Section 35.3.3 • “Modeling contact interference fits in Abaqus/Standard,” Section 35.3.4 • “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 35.3.5 • “Adjusting contact controls in Abaqus/Standard,” Section 35.3.6 • “Defining tied contact in Abaqus/Standard,” Section 35.3.7 • “Extending master surfaces and slide lines,” Section 35.3.8 • “Contact modeling if substructures are present,” Section 35.3.9 • “Contact modeling if asymmetric-axisymmetric elements are present,” Section 35.3.10 35.3.1 DEFINING CONTACT PAIRS IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Element-based surface definition,” Section 2.3.2 • “Node-based surface definition,” Section 2.3.3 • “Analytical rigid surface definition,” Section 2.3.4 • “Contact interaction analysis: overview,” Section 35.1.1 • *CONTACT PAIR • *SURFACE • *MODEL CHANGE • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining self-contact,” Section 15.13.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Using contact and constraint detection,” Section 15.16 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Contact pairs in Abaqus/Standard: • can be used to define interactions between bodies in mechanical, coupled temperature- displacement, coupled thermal-electrical-structural, coupled pore pressure-displacement, coupled thermal-electrical, and heat transfer simulations; • are part of the model definition; • can be formed using a pair of rigid or deformable surfaces or a single deformable surface; • do not have to use surfaces with matching meshes; and • cannot be formed with one two-dimensional surface and one three-dimensional surface. You can define contact in Abaqus/Standard in terms of two surfaces that may interact with each other as a “contact pair” or in terms of a single surface that may interact with itself in “self-contact.” Abaqus/Standard enforces contact conditions by forming equations involving groups of nearby nodes from the respective surfaces or, in the case of self-contact, from separate regions of the same surface. This section describes various aspects of defining contact pairs and refers to other sections for additional details. Defining contact pairs To define a contact pair, you must indicate which pairs of surfaces may interact with one another or which surfaces may interact with themselves. Contact surfaces should extend far enough to include all regions that may come into contact during an analysis; however, including additional surface nodes and faces that never experience contact may result in significant extra computational cost (for example, extending a slave surface such that it includes many nodes that remain separated from the master surface throughout an analysis can significantly increase memory usage unless penalty contact enforcement is used). Every contact pair is assigned a contact formulation (either explicitly or by default) and must refer to an interaction property. Discussion of the various available contact formulations (based on whether the tracking approach assumes finite- or small-sliding—and whether the contact discretization is based on a node-to-surface or surface-to-surface approach) is provided in “Contact formulations in Abaqus/Standard,” Section 37.1.1. Interaction property definitions are discussed in “Assigning contact properties for contact pairs in Abaqus/Standard,” Section 35.3.3. Defining contact between two separate surfaces When a contact pair contains two surfaces, the two surfaces are not allowed to include any of the same nodes and you must choose which surface will be the slave and which will be the master. The selection of master and slave surfaces is discussed in detail in “Choosing the master and slave roles in a two-surface contact pair” in “Contact formulations in Abaqus/Standard,” Section 37.1.1. For simple contact pairs consisting of two deformable surfaces, the following basic guidelines can be used: • The larger of the two surfaces should act as the master surface. • If the surfaces are of comparable size, the surface on the stiffer body should act as the master surface. • If the surfaces are of comparable size and stiffness, the surface with the coarser mesh should act as the master surface. Defining contact pairs using the finite-sliding, node-to-surface formulation Abaqus/Standard uses a finite-sliding, node-to-surface formulation by default. Input File Usage: *CONTACT PAIR, INTERACTION=interaction_property_name slave_surface_name, master_surface_name Abaqus/CAE Usage: You can also specify the contact discretization directly: *CONTACT PAIR, INTERACTION=interaction_property_name, TYPE=NODE TO SURFACE slave_surface_name, master_surface_name Interaction module: Create Interaction: Surface-to-surface contact (Standard): select the master surface, click Surface or Node Region, select the slave surface, Interaction editor, Sliding formulation: Finite sliding, Discretization method: Node to surface, Contact interaction property: interaction_property_name Defining contact pairs using the finite-sliding, surface-to-surface formulation A node-based slave surface precludes the use of surface-to-surface discretization. Some contact capabilities are not available with the finite-sliding, surface-to-surface formulation, including crack propagation . Input File Usage: Use the following option to define contact constraints using the finite-sliding, surface-to-surface formulation: Abaqus/CAE Usage: *CONTACT PAIR, INTERACTION=interaction_property_name, TYPE=SURFACE TO SURFACE slave_surface_name, master_surface_name Interaction module: Create Interaction: Surface-to-surface contact (Standard): select the master surface, click Surface, select the slave surface, Interaction editor, Sliding formulation: Finite sliding, Discretization method: Surface to surface, Contact interaction property: interaction_property_name Defining contact pairs using the small-sliding, node-to-surface formulation The small-sliding tracking approach uses node-to-surface discretization by default. For an explanation of when the small-sliding tracking approach is appropriate in an analysis, see “Using the small-sliding tracking approach” in “Contact formulations in Abaqus/Standard,” Section 37.1.1. Input File Usage: Abaqus/CAE Usage: *CONTACT PAIR, INTERACTION=interaction_property_name, SMALL SLIDING slave_surface_name, master_surface_name You can also specify the contact discretization directly: *CONTACT PAIR, INTERACTION=interaction_property_name, SMALL SLIDING, TYPE=NODE TO SURFACE slave_surface_name, master_surface_name Interaction module: Create Interaction: Surface-to-surface contact (Standard): select the master surface, click Surface or Node Region, select the slave surface, Interaction editor, Sliding formulation: Small sliding, Discretization method: Node to surface, Contact interaction property: interaction_property_name Defining contact pairs using the small-sliding, surface-to-surface formulation A node-based slave surface precludes the use of surface-to-surface discretization. Input File Usage: *CONTACT PAIR, INTERACTION=interaction_property_name, SMALL SLIDING, TYPE=SURFACE TO SURFACE slave_surface_name, master_surface_name Abaqus/CAE Usage: Interaction module: Create Interaction: Surface-to-surface contact (Standard): select the master surface, click Surface, select the slave surface, Interaction editor, Sliding formulation: Small sliding, Discretization method: Surface to surface, Contact interaction property: interaction_property_name Using symmetric master-slave contact pairs to improve contact modeling For node-to-surface contact it is possible for master surface nodes to penetrate the slave surface without resistance with the strict master-slave algorithm used by Abaqus/Standard. This penetration tends to occur if the master surface is more refined than the slave surface or a large contact pressure develops between soft bodies. Refining the slave surface mesh often minimizes the penetration of the master surface nodes. If the refinement technique does not work or is not practical, a symmetric master-slave method can be used if both surfaces are element-based surfaces with deformable or deformable-made-rigid parent elements. To use this method, define two contact pairs using the same two surfaces, but switch the roles of master and slave surface for the two contact pairs. This method causes Abaqus/Standard to treat each surface as a master surface and, thus, involves additional computational expense because contact searches must be conducted twice for the same contact pair. The increased accuracy provided by this method must be compared to the additional computational cost. All of the contact formulations are available for symmetric master-slave contact pairs, and can be applied using the same options discussed above. Input File Usage: Abaqus/CAE Usage: *CONTACT PAIR, INTERACTION=interaction_property_name surface_1, surface_2 surface_2, surface_1 Interaction module: Create Interaction: Surface-to-surface contact (Standard): select the master surface, click Surface, select the slave surface Copy this interaction to a new interaction, and edit the new interaction. In the interaction editor, click Switch to reverse the master and slave surfaces. Limitations of symmetric master-slave contact pairs Using symmetric master-slave contact pairs can lead to overconstraint problems when very stiff or “hard” contact conditions are enforced. See “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2, for a discussion of overconstraints and alternate constraint enforcement methods. For softened contact conditions, use of symmetric master-slave contact pairs will cause deviations from the specified pressure-versus-overclosure behavior, because both contact pairs contribute to the overall interface stress without accounting for one another. For example, symmetric master-slave contact pairs effectively double the overall contact stiffness if a linear pressure-overclosure relationship is specified. Likewise, use of symmetric master-slave contact pairs will cause deviations from the friction model if an optional shear stress limit is specified , because the contact stresses observed by each contact pair will be approximately one-half of the total interface stress. Similarly, it can be difficult to interpret the results at the interface for symmetric master-slave contact pairs. In this case both surfaces at the interface act as slave surfaces, so each has contact constraint values associated with it. The constraint values that represent contact pressures are not independent of each other. Therefore, the constraint values reported in the data (.dat) and results (.fil) files represent only a part of the total interface pressure and have to be summed to obtain the total. In the output database, mechanical contact variables are reported at the nodes on both the master and slave surfaces per contact pair and not just the slave surface where constraints are formed. Consequently, two result sets are available per surface of a symmetric master-slave contact pair; once when a surface acts as a slave and once as a master. For nodal contact pressures the Visualization module of Abaqus/CAE only reports the maximum of the two pressure values associated with a node when the surface containing the node acts either as a master or as a slave surface. Even in this case, the contact pressures do not represent the true interface pressure. Apart from contact pressures, some contact output may be confusing with symmetric master-slave contact pairs. For example, Abaqus/Standard may report a positive opening distance on one side of a contact interface but zero opening distance (i.e., touching) on the opposite side of the interface. Typically this is caused by the shape or relative mesh refinement of the two surfaces. Defining self-contact Define contact between a single surface and itself by specifying only a single surface or by specifying the same surface twice. The small-sliding tracking approach cannot be used with self-contact. Defining self-contact using node-to-surface discretization Abaqus/Standard uses node-to-surface contact discretization by default for self-contact. Input File Usage: Use either of the following options: Abaqus/CAE Usage: *CONTACT PAIR, INTERACTION=interaction_property_name surface_1, *CONTACT PAIR, INTERACTION=interaction_property_name surface_1, surface_1 Interaction module: Create Interaction: Self-contact (Standard): select the surface Interaction editor, Discretization method: Node to surface, Contact interaction property: interaction_property_name or Interaction module: Create Interaction: Surface-to-surface contact (Standard): select the surface, click Surface, select the surface again Interaction editor, Sliding formulation: Finite sliding, Discretization method: Node to surface, Contact interaction property: interaction_property_name Defining self-contact using surface-to-surface discretization Surface-to-surface discretization often leads to more accurate modeling of self-contact simulations. However, because the self-contact surface is acting as both a master and a slave, surface-to-surface discretization can sometimes significantly increase the solution cost. Input File Usage: Use either of the following options: *CONTACT PAIR, INTERACTION=interaction_property_name, TYPE=SURFACE TO SURFACE surface_1, *CONTACT PAIR, INTERACTION=interaction_property_name, TYPE=SURFACE TO SURFACE surface_1, surface_1 Abaqus/CAE Usage: Interaction module: Create Interaction: Self-contact (Standard): select the surface Interaction editor, Discretization method: Surface to surface, Contact interaction property: interaction_property_name or Interaction module: Create Interaction: Surface-to-surface contact (Standard): select the surface, click Surface, select the surface again Interaction editor, Sliding formulation: Finite sliding, Discretization method: Surface to surface, Contact interaction property: interaction_property_name Limitations of self-contact Self-contact is valid only for mechanical surface interactions and is limited to finite sliding with element- based surfaces. A node of a self-contact surface can be both a slave node and a member of the master surface for two-dimensional self-contact using the surface-to-surface formulation and for all three-dimensional self-contact. In these cases the contact behavior is similar to symmetric master-slave contact pairs, and the issues discussed in “Using symmetric master-slave contact pairs to improve contact modeling apply. Abaqus/Standard automatically applies some numerical “softening” to contact conditions in these cases, as discussed in “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2. Direct enforcement of hard contact conditions is the default constraint enforcement method for two- dimensional self-contact using the node-to-surface formulation. In this case, each node adjacent to a vertex where a two-dimensional surface folds onto itself is automatically assigned a slave or master role during the analysis. Since contact constraints directly resist penetrations at nodes that act as slave nodes, there is some possibility of unresolved penetrations at nodes that only act as master nodes for two-dimensional self-contact using the node-to-surface formulation. Selecting surfaces used in contact pairs Methods for creating surfaces are discussed in “Element-based surface definition,” Section 2.3.2; “Node-based surface definition,” Section 2.3.3; and “Analytical rigid surface definition,” Section 2.3.4; those sections discuss general restrictions for the various surface types. Considerations related to surface characteristics for various contact formulations are discussed in “Contact formulations in Abaqus/Standard,” Section 37.1.1. Additional considerations for surfaces used in contact definitions are discussed below. Orientation considerations for shell-like surfaces Abaqus/Standard requires master contact surfaces to be single-sided for node-to-surface contact and for some surface-to-surface contact formulations . This requires that you consider the proper orientation for master surfaces defined on elements, such as shells and membranes, that have positive and negative directions. For node-to-surface contact the orientation of slave surface normals is irrelevant, but for surface-to-surface contact the orientation of single-sided slave surfaces is taken into consideration. Double-sided element-based surfaces are allowed for the default surface-to-surface contact formulations, although they are not always appropriate for cases with deep initial penetrations. If the master and slave surfaces are both double-sided, the positive or negative orientation of the contact normal direction will be chosen such as to minimize (or avoid) penetrations for each contact constraint. If either or both of the surfaces are single-sided, the positive or negative orientation of the contact normal direction will be determined from the single-sided surface normals rather than the relative positions of the surfaces. When the orientation of a contact surface is relevant to the contact formulation, you must consider the following aspects for surfaces on structural (beam and shell), membrane, truss, or rigid elements: • Adjacent surface faces must have consistent normal directions. Abaqus/Standard will issue an error message if adjacent surface faces have inconsistent normals on a single-sided surface whose orientation is relevant to the contact formulation. • Except for initial interference fit problems , the slave surface should be on the same side of the master surface as the outward normal. If, in the initial configuration, the slave surface is on the opposite side of the master surface as the outward normal, Abaqus/Standard will detect overclosure of the surfaces and may have difficulty finding an initial solution if the overclosure is severe. An improper specification of the outward normal will often cause an analysis to immediately fail to converge. Figure 35.3.1–1 illustrates the proper and improper specification of a master surface’s outward normal. • Contact will be ignored with surface-to-surface discretization if single-sided slave and master surfaces have normal directions that are in approximately the same direction (for example, contact will not be enforced if the dot product of the slave and master surface normals is positive). master surface outward normal slave surface Incorrect master surface orientation Correct master surface orientation Figure 35.3.1–1 Example of proper and improper master surface orientation. The following output from a data check analysis can be useful in identifying incorrectly oriented master surfaces: • Initial clearances can be displayed in Abaqus/CAE with a contour plot of the variable COPEN at increment 0 of the first step; initial overclosures correspond to negative clearances. • Abaqus/Standard provides a detailed printout of the model’s initial contact state. Surface connectivity restrictions Certain connectivity restrictions apply to contact surfaces depending on the type of contact formulation. Surface connectivity restrictions for the various contact formulations are summarized in Table 35.3.1–1. As indicated in this table, the connectivity restrictions are sometimes different for master and slave surfaces. Self-contact surfaces act as both master and slave surfaces; therefore, if a restriction applies to either a master or slave surface, it also applies to self-contact. The potential connectivity restrictions referred to in Table 35.3.1–1 are described below: • Discontinuous surfaces: Discontinuous contact surfaces are allowed in many cases, but the master surface for finite-sliding, node-to-surface contact cannot be made up of two or more disconnected regions (they must be continuous across element edges in three-dimensional models or across nodes in two-dimensional models). Figure 35.3.1–2 shows examples of continuous surfaces, whereas Figure 35.3.1–3 and Figure 35.3.1–4 show examples of discontinuous surfaces. Figure 35.3.1–5 shows an automatically generated free surface resulting from the specification of an element set consisting of two disjointed groups of elements. The resulting surface is not continuous since it is composed of two disjoint open curves, so this surface would be invalid as a master surface for finite-sliding, node-to-surface contact. Table 35.3.1–1 Summary of which connectivity characteristics of element-based surfaces are allowed for various contact formulations. Connectivity characteristics Contact formulation Discontinuous (or 3-D faces joined at only one node) T-intersection Finite-sliding, node-to-surface Master: Not allowed Slave: Allowed Master: Not allowed Slave: Allowed Small-sliding, node-to-surface Master: Allowed Slave: Allowed Master: Not allowed Slave: Allowed Finite-sliding, surface-to-surface Master: Allowed Slave: Allowed Master: Allowed Slave: Allowed Small-sliding, surface-to-surface Master: Allowed Slave: Allowed Master: Not allowed Slave: Allowed Closed 2-D surface Closed 3-D surface Open 2-D surface Open 3-D surface Figure 35.3.1–2 Examples of continuous surfaces. Figure 35.3.1–3 Example of a discontinuous 2-D surface. Figure 35.3.1–4 Example of a discontinuous 3-D surface. user-specified element set automatically generated free surface Figure 35.3.1–5 Example of a discontinuous surface resulting from automatic free surface generation with a disjoint element set. • Portions of three-dimensional surfaces joined at only one node: The finite-sliding, node-to-surface contact formulation also does not allow three-dimensional master surface faces to be joined at a single node (they must be joined across a common element edge). Figure 35.3.1–6 shows an example of a surface with two faces connected by a single node. Figure 35.3.1–6 Example of a 3-D surface with two faces sharing a single node. • Surfaces with T-intersections: In some cases a contact surface cannot have more than two surface faces sharing a common master node in two dimensions or a common master edge in three dimensions. For example, Figure 35.3.1–7 shows examples of surfaces with T-intersections, in which three faces share a common node in two dimensions or a common edge in three dimensions. While more than two surface faces can share a common slave node in two dimensions or a common edge in three dimensions for node-to-surface formulations, the slave faces must be single-sided, which precludes the most common T-intersection cases for node-to-surface formulations. T-intersection in 2-D T-intersection in 3-D Figure 35.3.1–7 Examples of surfaces with T-intersections. Analytical rigid surfaces Analytical rigid surfaces are often effective for efficiently modeling curved, rigid geometries, as discussed in “Analytical rigid surface definition,” Section 2.3.4. For rare cases in which a very large number (thousands) of segments would be necessary to define an analytical rigid surface, better performance can be achieved with an element-based rigid surface . Three-dimensional beam and truss surfaces Abaqus/Standard cannot use three-dimensional beams or trusses to form a master surface because the elements do not have enough information to create unique surface normals. However, these elements can be used to define a slave surface. Two-dimensional beams and trusses can be used to form both master and slave surfaces. Edge-based surfaces Edge-based surfaces (“Element-based surface definition,” Section 2.3.2) on three-dimensional shell elements cannot be used in a contact analysis in Abaqus/Standard. Limitations of node-based surfaces Use node-based surfaces with caution when the contact property definition includes user-defined softened contact properties or thermal or electrical interactions because the contact constitutive behavior (which relies on accurate calculation of contact pressure, heat flux, or electric current) will not be enforced correctly unless the precise surface area is associated with each node. For details, see “Contact pressure- overclosure relationships,” Section 36.1.2; “Thermal contact properties,” Section 36.2.1; or “Electrical contact properties,” Section 36.3.1. Removing and reactivating contact pairs You can temporarily remove contact pairs from a simulation, which may result in significant computational savings by eliminating unnecessary contact searches and updates of surface orientations during the simulation. Removal and reactivation of contact pairs is commonly used in complicated forming processes where multiple tools need to interact with the workpiece at different stages in the analysis. You cannot remove tied contact pairs from a simulation . Removing contact pairs Removal of contact pairs is a useful technique for uncoupling components of an assembly until they should be brought together (such as tooling in manufacturing process simulations). Significant computational expense may be saved by removing a contact pair and introducing it at the proper time, thus eliminating the need to monitor the contact conditions except when they are relevant. Input File Usage: *MODEL CHANGE, TYPE=CONTACT PAIR, REMOVE slave_surface, master_surface Abaqus/CAE Usage: Use one of the following options: Repeat the data line as needed. Interaction module: Create Interaction: surface-to-surface contact or self-contact interaction editor: toggle off Active in this step Interaction module: interaction manager: select interaction, Deactivate Removal of contact forces associated with closed contact pairs If the surfaces are in contact when a contact pair is removed, Abaqus/Standard stores the corresponding contact forces (or heat fluxes if thermal interactions are present, or electrical currents if it is a coupled-thermal electrical analysis) for every node on each surface. Abaqus/Standard automatically ramps these forces (or heat fluxes or electrical currents) linearly down to zero magnitude during the removal step. Abaqus/Standard always removes the contact constraints for mechanical surface interactions instantaneously. Care must be taken in removing contact pairs in transient procedures. In transient heat transfer, fully coupled temperature-displacement, or fully coupled thermal-electrical-structural analysis if the fluxes are high and the step is long, this ramping down may have the effect of cooling down or heating up the rest of the body. In dynamic analysis if the forces are high and the step is long, kinetic energy can be imparted to the remaining portion of the model. This problem can be avoided by removing the contact pairs in a very short transient step prior to the rest of the analysis. This step can be done in a single increment. Using an allowable contact interference to deactivate contact pairs A contact pair with mechanical contact interactions can be deactivated during an analysis by assigning a very large allowable contact interference to the contact pairs . This method has the disadvantage of not reducing the computational cost of the analysis because the contact algorithm will still calculate the contact conditions for the contact pair in each increment. Reactivating contact pairs All contact pairs that will be used in a simulation must be created at the start of the analysis; they cannot be created once the simulation has begun. However, contact pairs can be created, removed at the start of the analysis in the first step, and then reactivated at a later point during the simulation. In Abaqus/CAE you can create contact pairs in any step. If a contact pair is created in a step other than the initial step, Abaqus/CAE automatically deactivates the contact pair in the initial step and reactivates it in the step in which you created it. Input File Usage: *MODEL CHANGE, TYPE=CONTACT PAIR, ADD slave_surface, master_surface Repeat the data line as needed. Abaqus/CAE Usage: Interaction module: Create Interaction: surface-to-surface contact or self-contact interaction editor: toggle on Active in this step Reactivating overclosed contact pairs When a contact pair is reactivated, the contact constraint becomes active immediately. In mechanical simulations it is possible for the surfaces of a contact pair to move such that they become overclosed while the contact pair is inactive. If this overclosure is too severe when the contact pair is reactivated, Abaqus/Standard may encounter convergence problems as it tries to enforce the suddenly activated contact constraint. To avoid such problems, you can specify a permissible interference value, v, for the contact pair that is larger than the overclosure for the contact pair. Abaqus/Standard will ramp v down to zero during the step. For details on specifying allowable interferences, see “Modeling contact interference fits in Abaqus/Standard,” Section 35.3.4. Output Output variables associated with the interaction of contact pairs fall into two categories: nodal variables (sometimes called constraint variables) and whole surface variables. In addition, Abaqus outputs an array of diagnostic information associated with contact interactions, as discussed in “Contact diagnostics in an Abaqus/Standard analysis,” Section 38.1.1. For more detailed discussions of variables associated with thermal, electrical, and pore fluid analyses, see the sections on the related contact properties in Chapter 36, “Contact Property Models.” Nodal contact variables Nodal contact variables can be contoured on contact surfaces in the Visualization module of Abaqus/CAE. Nodal contact variables include contact pressure and force, frictional shear stress and force, relative tangential motion (slip) of the surfaces during contact, clearance between surfaces, heat or fluid flux per unit area, fluid pressure, and electrical current per unit area. Many of the nodal contact variables written to the output database (.odb) file are often available for all contact nodes, regardless of whether they act as slave or master nodes. In such cases the nodal values are generally affected by more than one contact constraint. Other nodal contact variables are available only at nodes acting as slave nodes. In these cases the value at each slave node reflects a value associated with a particular contact constraint. Most contact output to the data (.dat) and results (.fil) files is associated with individual constraints. The contact pressure distribution is of key interest in many Abaqus analyses. You can view the contact pressure on all contact surfaces except for analytical rigid surfaces and discrete rigid surfaces based on rigid-type elements (the latter restriction does not apply to general contact). You can view a contour plot of the contact pressure error indicator next to a contour plot of the contact pressure to gain perspective on local accuracy of the contact pressure solution in regions where the contact pressure solution is of interest . In some cases you may observe the contact pressure extending beyond the actual contact zone due to the following factors: • The contour plots are constructed by interpolating nodal values, which can cause nonzero values to appear within portions of facets outside of the contact region. For example, this effect is often noticeable at corners, such as when two same-sized, aligned blocks are in contact—if the contact surfaces wrap around the corners, the contact pressure contours will extend slightly around the corners. • To minimize contact stress noise within a region of active contact, Abaqus/Standard computes nodal contact stresses as weighted averages of values associated with active contact constraints in which a node participates. Some filtering is applied to reduce the contact stress values reported for nodes on the fringe of the active contact region (that only weakly participate in contact constraints), but this filtering is not “perfect,” which can result in the contact zone size appearing somewhat exaggerated. Similarly, contact status output will also be affected at nodes that lie on the fringe of the active contact region. In such cases, the contact status may be reported as closed at nodes in the exaggerated region even though it is open. Due to these factors, trying to infer the contact force distribution from the contact stress distribution can be somewhat misleading. Instead, you can request nodal contact force output, which accurately represents the contact force distribution present in the analysis. Whole surface variables Whole surface variables are attributes of an entire slave surface. Available as history output, these variables record the total force and moment due to contact pressure and frictional stress, the center of pressure and frictional stress (defined as the point closest to the centroid of the surface that lies on the line of action of the resultant force for which the resultant moment is minimal), and the total contact area (defined as the sum of all the facets where there is contact force). The last letter of each variable name (except the variable CAREA) denotes which contact force distribution on the surface is used to calculate the resultant: Normal contact forces are used to derive the resultant quantity. Shear contact forces are used to derive the resultant quantity. The sum of the normal and shear contact forces is used to derive the resultant quantity. For example, CFN is the total force due to contact pressure, CFS is the total force due to frictional stress, and CFT is the total force due to both contact pressure and frictional stress. Each total moment output variable will not necessarily equal the cross product of the respective center of force vector and resultant force vector. Forces acting on two different nodes of a surface may have components acting in opposite directions, such that these nodal force components generate a net moment but not a net force; therefore, the total moment may not arise entirely from the resultant force. The center of force output variables tend to be most meaningful when the surface nodal forces act in approximately the same direction. Requesting output Certain contact variables must be requested as a group. For example, to output the clearance between surfaces (COPEN), you must request the variable CDISP (contact displacements). CDISP outputs both COPEN and CSLIP (tangential motion of the surfaces during contact). A complete listing of available contact pair variables and identifiers is given in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Output requests can be limited to individual contact pairs or portions of a slave surface. You can: • request output associated with a given contact pair; • request output associated with a given slave surface, including contributions from all of the contact pairs to which the slave surface belongs; and • limit the output by specifying a node set containing a subset of the nodes on the slave surface. Instructions on forming these output requests are available in the following sections: • To request output to the data (.dat) file, see “Surface output from Abaqus/Standard” in “Output to the data and results files,” Section 4.1.2. • To request output to the output database (.odb) file, see “Surface output in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3. Differences for small-sliding and finite-sliding contact For small-sliding contact problems the contact area is calculated in the input file preprocessor from the undeformed shape of the model; thus, it does not change throughout the analysis, and contact pressures for small-sliding contact are calculated according to this invariant contact area. This behavior is different from that in finite-sliding contact problems, where the contact area and contact pressures are calculated according to the deformed shape of the model. Output of tangential results Abaqus reports the values of tangential variables (frictional shear stress, viscous shear stress, and relative tangential motion) with respect to the slip directions defined on the surfaces. The definition of slip directions is explained in “Local tangent directions on a surface” in “Contact formulations in Abaqus/Standard,” Section 37.1.1. These directions do not always correspond to the global coordinate system, and they rotate with the contact pair in a geometrically nonlinear analysis. Abaqus/Standard calculates tangential results at each constraint point by taking the scalar product of the variable’s vector and a slip direction, , associated with the constraint point. The number at the end of a variable’s name indicates whether the variable corresponds to the first or second slip direction. For example, CSHEAR1 is the frictional shear stress component in the first slip direction, while CSHEAR2 is the frictional shear stress component in the second slip direction. or Definition of accumulated incremental relative motion (slip) Abaqus/Standard defines the incremental relative motion (also known as slip) as the scalar product of the incremental relative nodal displacement vector and a slip direction. The incremental relative nodal displacement vector measures the motion of a slave node relative to the motion of the master surface. The incremental slip is accumulated only when the slave node is contacting the master surface. The sums of all such incremental slips during the analysis are reported as CSLIP1 and CSLIP2. Details about the calculation of this quantity can be found in “Small-sliding interaction between bodies,” Section 5.1.1 of the Abaqus Theory Manual; “Finite-sliding interaction between deformable bodies,” Section 5.1.2 of the Abaqus Theory Manual; and “Finite-sliding interaction between a deformable and a rigid body,” Section 5.1.3 of the Abaqus Theory Manual. Extending the range for which contact opening output is provided for gaps To reduce computational costs, detailed computations to monitor potential points of interaction are avoided by default where surfaces are separated by a distance greater than the minimum gap distance at which contact forces (or thermal fluxes, etc.) may be transmitted. Therefore, contact opening (COPEN) output is typically not provided for finite-sliding contact where surfaces are opened by more than a small amount compared to surface facet dimensions. You can extend the range in which Abaqus/Standard provides contact opening output; COPEN will be provided up to gap distances equal to a specified “tracking thickness.” Using this control may increase computational cost due to extra contact tracking computations, especially if you specify a large tracking thickness value. Input File Usage: Abaqus/CAE Usage: *SURFACE INTERACTION, TRACKING THICKNESS=value You cannot adjust the default tracking thickness in Abaqus/CAE. Output for axisymmetric models In an axisymmetric analysis the total forces and moments transmitted between the contacting bodies as a result of contact pressure and frictional stress are computed in the same manner as in a two-dimensional analysis. Therefore, the component of the total forces along the r-axis is nonzero, and the components of the total moments include contributions from the total forces along the r-axis. Obtaining the “maximum torque” that can be transmitted about the z-axis in an axisymmetric analysis When modeling surface-based contact with axisymmetric elements (element types CAX and CGAX), Abaqus/Standard can calculate the maximum torque (output variable CTRQ) that can be transmitted This capability is often of interest when modeling threaded connectors . The maximum torque, T, is defined as where p is the pressure transmitted across the interface, r is the radius to a point on the interface, and s is the current distance along the interface in the r–z plane. This definition of “torque” effectively assumes a friction coefficient of unity. 35.3.2 ASSIGNING SURFACE PROPERTIES FOR CONTACT PAIRS IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • *CONTACT PAIR • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining self-contact,” Section 15.13.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview This section describes how to modify the properties associated with surfaces in a contact pair definition. Accounting for shell and membrane thickness All of the contact formulations except the finite-sliding, node-to-surface formulation account for initial shell and membrane thicknesses for element-based surfaces by default. The finite-sliding, node-to-surface formulation will not account for surface thickness. Node-based surfaces have no thickness, regardless of which element types are connected to the surface nodes. Accounting for element thicknesses in contact calculations is generally desirable, but you can avoid having thickness considered if it is not desired. Input File Usage: Abaqus/CAE Usage: *CONTACT PAIR, NO THICKNESS Interaction module: interaction editor: Sliding formulation: Small sliding or Finite sliding, Discretization method: Surface to surface or Node to surface, toggle on Exclude shell/membrane element thickness Example Consider the case of a shell pinched between two rigid surfaces, as shown in Figure 35.3.2–1. In this example contact pairs using the small-sliding, node-to-surface formulation are defined between the top surface of the shell and the top rigid surface and between the bottom surface of the shell and the bottom rigid surface. Although the shell surfaces are defined at the shell reference location, the contact interactions account for the thickness of the shell and are offset from the reference surface. The penalty constraint enforcement method is used to avoid overconstraining slave nodes. The following input is used: *SURFACE, NAME=TOP_RIG_SURF TOP_RIG_ELS, *SURFACE, NAME=SHELL_TOP_SURF deformable shell rigid solids shell reference surface shell thickness contact interactions Figure 35.3.2–1 Shell pinched between two rigid bodies. SHELL_ELS,SPOS *SURFACE, NAME=SHELL_BOT_SURF SHELL_ELS,SNEG *SURFACE, NAME=BOT_RIG_SURF BOT_RIG_ELS, *CONTACT PAIR, INTERACTION=INTER_AL, SMALL SLIDING SHELL_TOP_SURF, TOP_RIG_SURF SHELL_BOT_SURF, BOT_RIG_SURF *SURFACE INTERACTION, NAME=INTER_AL *SURFACE BEHAVIOR, PENALTY Specifying surface geometry corrections With the finite element method, curved geometric surfaces are naturally approximated as a faceted group of connected element faces. The use of a faceted surface geometry rather than the true surface geometry can significantly contribute to contact stress inaccuracy in contact pairs, especially when the magnitude of the differences between the faceted and true surface is not small with respect to the deformation of the components in contact. Methods for overcoming convergence and accuracy difficulties associated with faceted surfaces in contact interactions are discussed in “Contact formulations in Abaqus/Standard,” Section 37.1.1, and “Smoothing contact surfaces in Abaqus/Standard,” Section 37.1.3. 35.3.3 ASSIGNING CONTACT PROPERTIES FOR CONTACT PAIRS IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Contact interaction analysis: overview,” Section 35.1.1 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • *CONTACT PAIR • *SURFACE INTERACTION • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining self-contact,” Section 15.13.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Using contact and constraint detection,” Section 15.16 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Contact properties: • define the mechanical and thermal surface interaction models that govern the behavior of surfaces when they are in contact; and • are assigned to individual contact pairs. Assigning a surface interaction definition to a contact pair A surface interaction definition specifies the constitutive contact properties and the constraint enforcement methods used by a contact pair. Every contact pair in a model must refer to a surface interaction definition, even if the contact pair uses the default contact property models. See “Mechanical contact properties: overview,” Section 36.1.1, for information on defining contact properties. A non-default constraint enforcement method can be specified as part of a surface interaction definition, as described in “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2. Multiple contact pairs can refer to the same surface interaction definition. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *CONTACT PAIR, INTERACTION=interaction_property_name *SURFACE INTERACTION, NAME=interaction_property_name Interaction module: Create Interaction Property: Name: interaction_property_name, Contact Interaction editor: Contact interaction property: interaction_property_name Example Figure 35.3.3–1 shows the mesh used in this example. For purposes of this example, the surface ASURF is the slave surface of the contact pair. The property definition for the contact pair (GRATING) uses the finite-sliding, node-to-surface formulation with a friction model with =0.4 and uses the default “hard” contact model for the behavior normal to the surfaces. ESETB ESETA 502 BSURF 201 501 202 101 102 103 ASURF Figure 35.3.3–1 Mechanical surface interaction with friction and finite sliding. *HEADING … *SURFACE, NAME=ASURF ESETA, *SURFACE, NAME=BSURF ESETB, *CONTACT PAIR, INTERACTION=GRATING ASURF, BSURF *SURFACE INTERACTION, NAME=GRATING *FRICTION 0.4 *NSET, NSET=SNODES 101, 102, 103 *STEP, NLGEOM … *END STEP 35.3.4 MODELING CONTACT INTERFERENCE FITS IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • *CONTACT INTERFERENCE • “Specifying interference fit options” in “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Interference fits in Abaqus/Standard: • occur by default when the contact formulation computes overclosures between surfaces in the initial configuration of a model; • are resolved in the first increment of a step by default; • can be gradually resolved over multiple increments; • result in stresses and strains in a model as overclosures are resolved; • can be specified for both surface-based contact pairs and contact elements; and • cannot be specified for self-contact. Abaqus/Standard offers alternative methods to resolve initial overclosures with strain-free adjustments and to model specific overclosures or clearances different from those calculated from the initial configuration. These methods are discussed in “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 35.3.5. Resolving excessive initial overclosures If there are large overclosures in the initial configuration of model, Abaqus/Standard may not be able to resolve the interference fit in a single increment. Abaqus/Standard provides alternative methods that allow overclosures to be resolved gradually over multiple increments. The default contact constraint imposed at each constraint location is that the current penetration is positive. To alter this constraint, you can specify an allowable is interference, , that will be ramped down over the course of a step. The specified allowable interference modifies the contact constraint as follows: . Penetration exists when Thus, specifying a positive value for causes Abaqus/Standard to ignore penetrations up to that magnitude. Figure 35.3.4–1 illustrates a typical interference fit problem. If the penetration in the model is or request an automatic shrink fit. In either case Abaqus/Standard will , you may declare BEGINNING OF STEP MIDDLE OF STEP END OF STEP Figure 35.3.4–1 Interference fit with contact surfaces. consider the two bodies to be just in contact at the start of the simulation. As the allowable interference, , is decreased during the step, Abaqus/Standard pushes the surfaces apart until there is no more allowable penetration. There are three different ways in which to specify the allowable interference, . By default, in all cases the value of the specified allowable interference is applied instantaneously at the start of the step and then ramped down to zero linearly over the step, unless you specify an amplitude reference that defines a particular allowable interference-time variation. It is recommended that you specify allowable interferences in a step separate from the rest of the analysis; additional loads may adversely affect the resolution of the interference fit and the response to loading with partially-resolved interferences may be non-physical. Once the overclosures are resolved, you can continue the analysis in a new step. When the contact interference is specified, output variable COPEN does not reflect the actual overclosure value during the step; it reflects the actual value only at the end of the step. You must specify the contact pairs or contact elements at which the allowable interference should apply. Input File Usage: Abaqus/CAE Usage: Use the following option to define an allowable interference for contact pairs: *CONTACT INTERFERENCE, TYPE=CONTACT PAIR slave surface, master surface, ... Use the following option to define an allowable interference for contact elements: *CONTACT INTERFERENCE, TYPE=ELEMENT contact element set, ... Interaction module: interaction editor: Interference Fit: Gradually remove slave node overclosure during the step, Uniform allowable interference, Magnitude at start of step: Element-based contact is not supported in Abaqus/CAE. Using a nondefault amplitude curve for the allowable interference You can define a time-varying allowable contact interference by creating an amplitude curve and then referring to this curve from the contact interference definition. The amplitude will be ignored, however, if the Riks method is used. Input File Usage: Abaqus/CAE Usage: *CONTACT INTERFERENCE, AMPLITUDE=amplitude_curve_name Interaction module: interaction editor: Interference Fit: Gradually remove slave node overclosure during the step, Uniform allowable interference, Amplitude: amplitude_curve_name Removing or modifying the allowable contact interferences By default, only the allowable contact interferences defined or redefined by a particular contact interference definition will be modified. Alternatively, you can specify that all previously defined allowable contact interferences should be removed from the model and only those defined with this definition will remain. Input File Usage: Use the following option to add or modify an allowable contact interference definition: *CONTACT INTERFERENCE, OP=MOD Use the following option to remove all previously defined allowable contact interferences: *CONTACT INTERFERENCE, OP=NEW Abaqus/CAE Usage: Contact interferences in Abaqus/CAE propagate along with the interaction for which they are defined. You cannot remove all previously defined contact interferences at once in Abaqus/CAE. Specifying the same allowable contact interference for an entire surface A single allowable interference can be specified for every node on the slave surface or every slave node in the specified set of contact elements. The concepts of slave nodes for the various families of contact elements are discussed in their respective sections. The specified allowable contact interferences are included in the current penetrations of the slave nodes reported in the message file when you request detailed contact printout. Thus, any slave node that penetrates the master surface by less than the allowable interference will be reported as being open. Using the automatic “shrink” fit method This method is applicable only during the first step of an analysis and requires no interference value. With this method Abaqus/Standard assigns a different to each slave node that is equal to that node’s initial penetration (or zero if the point is initially open) except for the finite-sliding, surface-to-surface formulation, in which case the same value of , corresponding to the maximum penetration of the contact pair, is assigned to all constraints that are initially closed. These automatically calculated allowable contact interferences are not included in the current penetrations reported in the message file when detailed contact printout is requested. When the automatic “shrink” fit method is used, only the default amplitude curve, a linear ramp to zero magnitude, can be used. Input File Usage: Abaqus/CAE Usage: *CONTACT INTERFERENCE, SHRINK Interaction module: interaction editor: Interference Fit: Gradually remove slave node overclosure during the step, Automatic shrink fit Applying an allowable contact interference with a shift vector In this method you specify a uniform allowable interference . The allowable interference value, is applied to the , defines the magnitude of a shift vector. A relative shift slave nodes before Abaqus/Standard determines the contact conditions. In certain applications, such as contact simulations of threaded connectors, shifting the surfaces in a specified direction is more effective than simply allowing an interference. and a direction Figure 35.3.4–2 illustrates the potential difference that can result when using an allowable contact interference with a shift vector rather than using a uniform allowable contact interference. In case (a) a shift direction is defined as well as an allowable interference , while in case (b) the standard approach is used, with an allowable interference . The magnitude of is the same in both cases, but it is less than the penetration in case (a) and more than the penetration in case (b). In case (a) contact is detected immediately for slave node A, and the penetration is resolved with that node sliding along segment because node A is shifted in the direction Abaqus/Standard determines that node A is closest to segment before Abaqus/Standard checks for contact. After the shift and moves the node onto that segment. S1 S2 a) b) Figure 35.3.4–2 Effect of direction definition on interference accommodation: a) with direction, b) without direction. In case (b) slave node A detects contact with segment remains in its initial position. Thus, node A will slide along segment because that is the closest segment when node A if no shift direction is provided. Input File Usage: Abaqus/CAE Usage: , Z-direction cosine of , X-direction cosine of *CONTACT INTERFERENCE slave surface, master surface, cosine of ... Interaction module: interaction editor: Interference Fit: Gradually remove slave node overclosure during the step, Uniform allowable interference, Magnitude at start of step: , Along direction: , Y-direction Interference fits for surface-to-surface discretization Because contact conditions are enforced in an average sense in a region around each constraint location for surface-to-surface contact, penetrations or gaps may be observed at slave nodes when surface-to- surface constraints are in a zero-penetration state. Large interferences may be difficult surface-to-surface formulation. Using this formulation, overclosures tend to be resolved along the slave facet normal to resolve with the finite-sliding, directions; using node-to-surface contact, overclosures tend to be resolved along the master surface Figure 35.3.4–3 illustrates a case where differing normal directions lead to normal directions. undesirable tangential motion during an interference fit. In some cases it may be preferable to resolve large initial overclosures with node-to-surface discretization. surface-to-surface node-to-surface master surface overclosure resolution direction Figure 35.3.4–3 Comparison of contact formulations in an example with a large interference fit. Friction and contact interferences Frequently, an actual assembly process is modeled as an interference fit problem. If frictional interface properties are desired, they should usually be introduced after the initial interference has been resolved. The initial interference problem should be modeled under frictionless conditions since the physical assembly process is not typically modeled exactly. Friction can be introduced in subsequent steps . 35.3.5 ADJUSTING INITIAL SURFACE POSITIONS AND SPECIFYING INITIAL CLEARANCES IN Abaqus/Standard CONTACT PAIRS Products: Abaqus/Standard Abaqus/CAE References • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • “Modeling contact interference fits in Abaqus/Standard,” Section 35.3.4 • “Defining tied contact in Abaqus/Standard,” Section 35.3.7 • “Contact formulations in Abaqus/Standard,” Section 37.1.1 • *CLEARANCE • *CONTACT PAIR • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Using contact and constraint detection,” Section 15.16 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Adjusting the position of surfaces in an Abaqus/Standard contact pair: • can be performed only at the start of a simulation; • causes Abaqus/Standard to move the nodes of the slave surface so that they precisely contact the master surface (with some exceptions for surface-to-surface discretization and overlapping interaction definitions); • does not create any strain in the model; • can eliminate small gaps or penetrations caused by numerical roundoff when a graphical preprocessor such as Abaqus/CAE is used and, thus, prevent possible convergence problems; • is required when two surfaces are tied together for the duration of the analysis; • should not be used to correct gross errors in the mesh design; • cannot be used with symmetric master-slave contact; and • will account for shell and membrane thicknesses and shell offsets (these factors are accounted for in the adjustment zone and in the adjustments) for contact formulations other than the default finite-sliding, node-to-surface contact formulation . In addition to adjusting two surfaces into precise contact, Abaqus/Standard offers various methods to define the initial clearances between two surfaces precisely in both magnitude and direction. Responses to negative clearances, or interference fits, are discussed in “Modeling contact interference fits in Abaqus/Standard,” Section 35.3.4. Adjusting the surfaces in a contact pair You can have Abaqus/Standard adjust the position of the slave surface of a contact pair by specifying either a floating point value a for the depth of an “adjustment zone” around the master surface or a node set label. Abaqus/Standard does not adjust the nodes on the slave surface by default for contact pairs; rather initial overclosures are treated as interference fits by default for contact pairs. Comments unique to surface-to-surface contact The following points apply to contact pairs with surface-to-surface discretization : for • Strain-free adjustments to slave node positions may not result in exactly zero gap with respect to the master surface as measured at a slave node. The adjustments are made to achieve zero gap between the surfaces in an average sense in a region near each slave node within the adjustment zone. • The magnitude of strain-free adjustments is limited to half the typical facet length. For instances of initial overclosures exceeding this limit, an allowable penetration equal to the initial overclosure is stored for the associated contact constraints such that penetrations deeper than the initial overclosure are resisted during the analysis, but penetrations less than the initial overclosure are not resisted. • Strain-free adjustments will occur for some slave nodes outside the adjustment zone if a significant portion of a slave face (or segment in two dimensions) to which it is attached is within the adjustment zone. The discussion in the remainder of this section applies directly to node-to-surface contact discretizations (for which contact is enforced at discrete points—slave nodes) but should be considered within the context of the above points for surface-to-surface contact discretizations. Using an “adjustment zone” when adjusting surfaces When you specify a, the depth of the “adjustment zone,” Abaqus/Standard forms an adjustment zone extending a distance a from the master surface. Abaqus/Standard measures the distance along the master surface normals that pass through the nodes of the slave surface. Any nodes on the slave surface that are within the “adjustment zone” in the initial geometry of the model are moved precisely onto the master surface. The motion of these slave nodes does not create any strain in the model; it is treated as a change in the model definition. An example of adjusting the surfaces of a contact pair is shown in Figure 35.3.5–1 and Figure 35.3.5–2. If you specify a negative value for a, Abaqus/Standard will issue an error message. Input File Usage: Abaqus/CAE Usage: *CONTACT PAIR, ADJUST=a slave_surface, master_surface ... Interaction module: contact interaction editor: Specify tolerance for adjustment zone: a adjust Figure 35.3.5–1 Initial configuration of the contact surfaces showing the “adjustment zone.” The slave surface is in bold. Figure 35.3.5–2 Configuration of the contact surfaces after the adjustment. Nodes within the adjustment zone and overclosed nodes have been moved. Adjusting overclosed slave nodes using an adjustment zone When you specify the depth of the adjustment zone, Abaqus/Standard moves any slave nodes penetrating the master surface in the initial configuration so that they just contact the master surface. Specifying a value of 0.0 for a causes Abaqus/Standard to adjust only those slave nodes that are penetrating the master surface. Figure 35.3.5–3 shows the effect of specifying a=0.0 in the example shown in Figure 35.3.5–1. If you do not have Abaqus/Standard adjust the position of the slave surface, slave nodes that are overclosed in the initial configuration will remain overclosed at the start of the simulation, which may cause convergence problems. Using a node set label when adjusting surfaces You can specify a node set label instead of an adjustment zone depth when only a subset of the slave nodes should be adjusted and specifying a may cause the inappropriate adjustment of other slave nodes. Abaqus/Standard adjusts only those nodes on the slave surface belonging to the node set. The node set can contain nodes that are not on the slave surface at all: Abaqus/Standard will ignore them and adjust only the nodes in the node set that are part of the slave surface. Figure 35.3.5–3 Adjusted configuration of contact surfaces when a=0. Abaqus/Standard moves any slave nodes in the specified node set regardless of how far they are from the master surface. The adjustments of the nodes from their initial configurations do not create strains in the elements forming the slave surface. If Abaqus/Standard adjusts slave nodes that are far from the master surface, the elements may become poorly shaped, which can cause convergence difficulties. *CONTACT PAIR, ADJUST=node_set_label slave_surface, master_surface ... Interaction module: contact interaction editor: Adjust slave nodes in set: node_set_label Abaqus/CAE Usage: Input File Usage: Adjusting overclosed slave nodes using a node set label Because Abaqus/Standard adjusts only the slave nodes in the specified node set, any overclosed slave nodes not in the specified node set remain overclosed at the start of the simulation. Using a node set label may, therefore, cause convergence problems if severely overclosed slave nodes, which need to be adjusted, are not included in the node set. This behavior is different from that seen if a is specified, in which case Abaqus/Standard adjusts all of the overclosed nodes on the slave surface. Adjustments for overlapping contact pairs Nodal adjustment definitions are processed sequentially at the start of an analysis. If different constraint or contact definitions involve the same nodes, some adjustments may cause lack of compliance for contact or constraint definitions that were previously processed. These conflicts can be avoided in some cases by changing the processing order of constraint and contact definitions: nodes in common between different contact or constraint definitions should be processed first as slave nodes and later as master nodes. Input File Usage: Abaqus/CAE Usage: To change the processing order of constraint and contact definitions, change the order of the definitions in the input file. Constraint and contact definitions are processed in the order in which they appear. To change the processing order of constraint and contact definitions, change the names of the constraints and interactions in the model. Constraints and interactions are processed alphabetically according to their name. When to adjust contact surface pairs There are several instances when adjusting the surfaces in a contact pair is required or strongly recommended: • When tying two surfaces together for the duration of the analysis . • When using small- or infinitesimal-sliding contact . • When specifying a precise initial clearance or initial overclosure for the contact surfaces by defining an allowable contact interference . Defining a precise initial clearance or overclosure for small-sliding contact You can define precise initial clearance or overclosure values and contact directions for the nodes on the slave surface when they would not be computed accurately enough from the nodal coordinates; for example, if the initial clearance is very small compared to the coordinate values. The initial clearance or overclosure value calculated at every slave node (based on the coordinates of the slave node and the master surface) is overwritten by the value that you specify. This procedure is performed internally, and it does not affect the coordinates of the slave nodes. If you define a clearance, Abaqus/Standard will treat the two surfaces as not being in contact, regardless of their nodal coordinates. If you define an overclosure, Abaqus/Standard will treat the two surfaces as an interference fit and attempt to resolve the overclosure in the first increment. If the defined overclosure is large, you may need to specify an allowable interference that is ramped off over several increments. See “Modeling contact interference fits in Abaqus/Standard,” Section 35.3.4, for further discussion of interference fits. You can define initial clearance or overclosure values only for small-sliding contact (“Contact formulations in Abaqus/Standard,” Section 37.1.1). For a technique that can be used to model clearances or overclosures between finite-sliding contact pairs, see “Alternative methods for specifying precise initial clearances or overclosures” below. Specifying a uniform clearance or overclosure for the surfaces You can specify a uniform clearance or overclosure for a contact pair by identifying the master and slave surfaces of the contact pair and the desired initial clearance, (positive for a clearance; negative for an overclosure). No other data are needed. Input File Usage: *CLEARANCE, SLAVE=surface_name, MASTER=surface_name, VALUE= Abaqus/CAE Usage: Interaction module: contact interaction editor: Clearance: Initial clearance: Uniform value across slave surface: Specifying spatially varying clearances or overclosures for the surfaces Alternatively, you can specify spatially varying clearances or overclosures for a contact pair by identifying the master and slave surfaces of the contact pair and providing a table of data specifying the clearance at a single node or a set of nodes belonging to the slave surface. Any slave surface node that is not identified will use the clearance that Abaqus/Standard calculates from the initial geometry of the surfaces. Input File Usage: *CLEARANCE, SLAVE=surface_name, MASTER=surface_name, TABULAR node number or node set label, clearance value Repeat the data line as often as necessary. Abaqus/CAE Usage: You cannot specify initial clearance or overclosure values using a table of data in Abaqus/CAE. Reading spatially varying clearances or overclosures from an external file Abaqus/Standard can read the spatially varying clearances or overclosures for a contact pair from an external file. Input File Usage: *CLEARANCE, SLAVE=surface_name, MASTER=surface_name, TABULAR, INPUT=file_name Abaqus/CAE Usage: You cannot specify initial clearance or overclosure values using an external input file in Abaqus/CAE. Specifying the surface normal for the contact calculations Normally Abaqus/Standard calculates the surface normal used for the contact calculations from the geometry of the discretized surfaces, using the algorithms described in “Contact formulations in Abaqus/Standard,” Section 37.1.1. When specifying spatially varying clearances or overclosures, you can redefine the contact direction that Abaqus/Standard uses with each slave node by specifying the components of this vector. The vector must be defined in the global Cartesian coordinate system, and it should define the master surface’s desired outward normal direction. Input File Usage: *CLEARANCE, SLAVE=surface_name, MASTER=surface_name, TABULAR node number or node set label, clearance value, first normal component, second normal component, third normal component Repeat the data line as often as necessary. Abaqus/CAE Usage: You cannot redefine contact directions in Abaqus/CAE, except for threaded bolt connections . Generating the contact normal directions for a threaded bolt connection automatically Alternatively, for a single-threaded bolt connection the contact normal directions for each slave node can be generated automatically by specifying the thread geometry data and two points used to define a vector on the axis of the bolt/bolt hole. Either the bolt or bolt hole can be a master or slave surface. However, the vector defining the axis of the bolt or bolt hole must be chosen appropriately. For example, when the bolt surface is chosen to be the master surface, the vector should be oriented to point from the tip of the bolt to the head of the bolt if the bolt is in tension and from the head to the tip if the bolt is in compression. If the bolt surface is chosen to be the slave surface and the bolt is in tension, the bolt axis should be flipped (i.e., from the head to the tip) and a negative half-thread angle should be specified. An incorrect bolt axis direction will not engage the contact interaction, and the surfaces will be unconstrained. You should check the stresses in the bolt to make sure that the contact is engaged. Input File Usage: Abaqus/CAE Usage: *CLEARANCE, SLAVE=surface_name, MASTER=surface_name, TABULAR, BOLT half-thread angle, pitch, major bolt diameter, mean bolt diameter node number or node set label, clearance value, coordinates of points a and b on the axis of the bolt/bolt hole Repeat the second data line as often as necessary. Interaction module: contact interaction editor: Clearance: Initial clearance: Computed for single-threaded bolt or Specify for single-threaded bolt: clearance value, Clearance region on slave surface: Edit Region: select region, Bolt direction vector: Edit: select axis, Half-thread angle: half-thread angle, Pitch: pitch, Bolt diameter: Major: major bolt diameter or Mean: mean bolt diameter Visualizing the precise initial clearances or overclosures Abaqus/Standard does not adjust the coordinates of the slave surface when precise initial clearances or overclosures are specified. Therefore, the specified clearances or overclosures cannot be seen in the model in Abaqus/CAE. Thus, depending on the initial geometry of the surfaces and the magnitude of the clearances or overclosures, the surfaces may appear open or closed in Abaqus/CAE when they are actually just in contact. However, the actual clearance can be displayed in Abaqus/CAE by plotting a contour plot of the variable COPEN. Alternative methods for specifying precise initial clearances or overclosures Abaqus/Standard offers an alternative method of defining precise initial clearances or overclosures that is applicable to both small-sliding and finite-sliding contact pairs. In this method you specify an adjustment zone depth for the contact pair (as described above in “Adjusting the surfaces in a contact pair”) to move the surfaces forming the contact pair exactly into contact at the start of the analysis. Then, in the first step of the simulation you specify an allowable contact interference, , for the contact pair . The contact interference definition must refer to an amplitude curve; the form of the amplitude curve depends on whether a clearance or an overclosure is being defined and is described below. The clearance or overclosure will be uniform across the surfaces. Input File Usage: Use all of the following options: *CONTACT PAIR, ADJUST=a slave_surface, master_surface *AMPLITUDE, NAME=amplitude_name *CONTACT INTERFERENCE, AMPLITUDE=amplitude_name slave_surface, master_surface, Abaqus/CAE Usage: Interaction module: contact interaction editor: Specify tolerance for adjustment zone: a, Interference Fit: toggle on Uniform allowable interference, Amplitude: amplitude_name, Magnitude at start of step: Specifying a precise clearance by defining an allowable contact interference To specify a precise clearance by defining an allowable contact interference, the amplitude curve should have a constant magnitude for the duration of the step. A positive value should be given as the allowable interference, . When viewed in Abaqus/CAE, these surfaces will appear to penetrate each other when they are in contact. The surfaces start the simulation with coordinates that have them exactly touching, but the specified interference makes them behave as if they have a clearance between them. Specifying a precise overclosure by defining an allowable contact interference To specify a precise overclosure by defining an allowable contact interference, the amplitude curve should ramp from zero to unity over the duration of the step to allow Abaqus/Standard to resolve the overclosure gradually. A negative value should be given as the allowable interference, . When viewed in Abaqus/CAE, the surfaces start the simulation with coordinates that have them exactly touching, but the specified interference makes them behave as if they are overclosed. As Abaqus/Standard resolves the overclosure, these surfaces will appear to separate from each other. When the gap between the two surfaces is equal to a distance of , the surfaces will behave as if they are precisely in contact. 35.3.6 ADJUSTING CONTACT CONTROLS IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • *CONTACT CONTROLS • *CONTACT PAIR • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining self-contact,” Section 15.13.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Specifying contact controls in an Abaqus/Standard analysis,” Section 15.13.9 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Contact controls in Abaqus/Standard: • should not be modified from the default settings for the majority of problems; • can be used for problems where the standard contact controls do not provide cost-effective solutions; • can be used for problems where the standard controls do not effectively establish the desired contact conditions; and • can be used in some situations to control whether supplementary contact constraints are created. Problems that benefit from adjustments to the contact controls in Abaqus/Standard are generally large models with complicated geometries and numerous contact interfaces. Applying contact controls You can apply contact controls on a step-by-step basis to all of the contact pairs and contact elements that are active in the step or to individual contact pairs. This makes it possible to apply contact controls to a specific contact pair to take the simulation through a difficult phase. Contact controls remain in effect until they are either changed or reset to their default values. If in any given step the contact controls are declared for both the entire model and for a specific contact pair, the controls for the specific contact pair will override those for the entire model for that contact pair. In addition, you can specify supplementary contact constraints on individual contact pairs as described below in “Supplementary contact constraints.” Input File Usage: To apply contact controls to all contact pairs and contact elements: *CONTACT CONTROLS contact control options To apply contact controls to a specific contact pair: *CONTACT CONTROLS, SLAVE=slave surface, MASTER=master surface contact control options Repeat this option to apply contact controls to several contact pairs. Abaqus/CAE Usage: Contact controls in Abaqus/CAE can be applied only to specific contact pairs: Interaction module: Interaction→Contact Controls→Create: Abaqus/Standard contact controls Contact interaction editor: Contact controls: contact controls name Resetting contact controls You can reset all contact controls to their default values, or you can reset the controls for a specific contact pair. Input File Usage: To reset all contact controls: *CONTACT CONTROLS, RESET To reset the controls for a specific contact pair: *CONTACT CONTROLS, SLAVE=slave surface, MASTER=master surface, RESET Abaqus/CAE Usage: Interaction module: contact interaction editor: Contact controls: (Default) You cannot reset all contact controls at once in Abaqus/CAE. Automatic stabilization of rigid body motions in contact problems Abaqus/Standard offers contact stabilization to help automatically control rigid body motion in static problems before contact closure and friction restrain such motion. It is recommended that you first try to stabilize rigid body motion through modeling techniques (modifying geometry, imposing boundary conditions, etc.). The automatic stabilization capability is meant to be used in cases in which it is clear that contact will be established, but the exact positioning of multiple bodies is difficult during modeling. It is not meant to simulate general rigid body dynamics; nor is it meant for contact chattering situations or to resolve initially tight clearances between mating surfaces. When automatic contact stabilization is used, Abaqus/Standard activates viscous damping for relative motions of the contact pair at all slave nodes, in the same manner as contact damping . Unlike most contact controls, which carry over to subsequent steps until they are modified or reset, automatic stabilization damping is applied only for the duration of the step in which it is specified. In subsequent steps the stabilization is removed, even if contact was not established or if rigid body motions appear later because of complete separation of the contact pair. If needed, you should specify stabilization for subsequent steps as well. By default, the damping coefficient: • is calculated automatically for each contact constraint based on the stiffness of the underlying elements and the step time, • is applied to all contact pairs equally in the normal and tangential directions, • is ramped down linearly over the step, • is active only when the distance between the contact surfaces is smaller than a characteristic surface dimension, and • is zero for contact modeled with contact elements (such as gap contact elements, tube-to-tube contact elements, etc.). Although the automatically calculated damping coefficient typically provides enough damping to eliminate the rigid body modes without having a major effect on the solution, there is no guarantee that the value is optimal or even suitable. This is particularly true for thin shell models, in which the damping may be too high. Hence, you may have to increase the damping if the convergence behavior is problematic or decrease the damping if it distorts the solution. The first case is obvious, but the latter case requires a post-analysis check. There are several ways to carry out such checks. The simplest method is to consider the ratio between the energy dissipated by viscous damping and a more general energy measure for the model, such as the elastic strain energy. These quantities can be obtained as output variables ALLSD and ALLSE, respectively. More detailed information can be obtained by comparing the contact damping stresses CDSTRESS (with the individual components CDPRESS, CDSHEAR1, and CDSHEAR2) to the true contact stresses CSTRESS (with the individual components CPRESS, CSHEAR1, and CSHEAR2). If the contact damping stresses are too high, you should decrease the damping. The comparison should be made after contact is firmly established; the contact damping stresses will always be relatively high when contact is not yet or only partially established. The easiest way to increase or decrease the amount of damping is to specify a factor by which the automatically calculated damping coefficient will be multiplied. Typically, you should initially consider changing the default damping by (at least) an order of magnitude; if that addresses the problem sufficiently, you can do some subsequent fine-tuning. In some cases a larger or smaller factor may be needed; this is not a problem as long as a converged solution is obtained and the dissipated energy and contact damping stresses are sufficiently small. It is also possible to specify the damping coefficient directly. Direct specification of the damping value is not easy and may require some trial and error. For efficiency reasons this may best be done on a similar model of reduced size. If the damping coefficient is specified directly, any multiplication factor specified for the default damping coefficient is ignored. Input File Usage: To use the default damping coefficient: *CONTACT CONTROLS, STABILIZE To specify a scale factor for the default damping coefficient: *CONTACT CONTROLS, STABILIZE=factor To specify the damping coefficient directly: *CONTACT CONTROLS, STABILIZE damping coefficient Abaqus/CAE Usage: Interaction module: Abaqus/Standard contact controls editor: Stabilization: Automatic stabilization, Factor: factor or Stabilization coefficient: damping coefficient Specifying the stabilization ramp-down factor You can specify the ramp-down factor at the end of the step. By default, this value is equal to zero, so that the damping vanishes completely at the end of the step. Entering a nonzero value for this factor can be useful in cases where the rigid body modes are not fully constrained at the end of the step; for example, if the problem is frictionless and sliding motions can occur but there is no net force in the sliding direction. In that case it is usually desirable to maintain the small damping in the next step by using the value used for the ramp-down as the multiplication factor for the damping coefficient. If needed, you can maintain this damping level by setting the ramp-down factor equal to one. *CONTACT CONTROLS, STABILIZE , ramp-down factor Input File Usage: Abaqus/CAE Usage: Interaction module: Abaqus/Standard contact controls editor: Stabilization: Automatic stabilization or Stabilization coefficient, Fraction of damping at end of step: ramp-down factor Specifying the damping range By default, the opening distance over which the damping is applied (the damping range) is equal to the characteristic slave surface facet dimension; if such a dimension is not available (for example, in the case of a node-based surface), a characteristic element length obtained for the whole model is used. The damping is 100% of the reference value for openings less than half the damping range and from there is ramped to zero for an opening equal to the damping range. Alternatively, you can specify the damping range directly, overriding the calculated value. This can be useful if the damping should work only for a narrow gap, or if the damping should be in effect regardless of the opening distance. In the latter case a large value should be entered. Input File Usage: *CONTACT CONTROLS, STABILIZE , , damping range Abaqus/CAE Usage: Interaction module: Abaqus/Standard contact controls editor: Stabilization: Automatic stabilization or Stabilization coefficient, Clearance at which damping becomes zero: Specify: damping range Specifying tangential damping By default, the damping in the tangential direction is the same as the damping in the normal direction. However, if a lower or higher value is desired, you can decrease or increase the tangential damping or set it to zero. Input File Usage: *CONTACT CONTROLS, STABILIZE, TANGENT FRACTION=value Abaqus/CAE Usage: Interaction module: Abaqus/Standard contact controls editor: Stabilization: Automatic stabilization or Stabilization coefficient, Tangent fraction: value Contact controls associated with normal contact constraints These controls allow you to specify that nodes on the contact interfaces can violate “hard” contact conditions. In addition, these controls can be used to modify the behavior of the “softened” pressure- overclosure relationships and the augmented Lagrangian or penalty contact constraint enforcement. The no separation pressure-overclosure relationships cannot be modified by the contact controls. A node can violate the contact condition in one of two ways. First, Abaqus/Standard may consider that there is no contact at that node, even though the node has penetrated the master surface by a small distance. Second, Abaqus/Standard may consider that there is contact at a node, even though the normal pressure transmitted between the contacting surfaces at the node is negative (that is, a tensile stress is being transmitted). Modifying the behavior of the augmented Lagrangian or penalty contact constraint enforcement For augmented Lagrangian contact you can specify the allowable penetration (either directly or as a fraction of a characteristic contact surface dimension) that is permitted to violate the impenetrability condition. In addition, for augmented Lagrangian or penalty contact you can scale the default penalty stiffness calculated by Abaqus/Standard. Controls for the augmented Lagrange and penalty constraint enforcement methods are discussed in “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2. Modifying the tangential penalty stiffness in linear perturbation steps The penalty stiffness used to enforce tangential constraints in linear perturbation steps generally In perturbation steps differs from the penalty stiffness used to enforce sticking in a general step. Abaqus/Standard activates the tangential contact constraints when the corresponding normal constraint is active in the base state and the contact property (surface interaction) definition includes a friction model. By default, the tangential penalty stiffness is equal to the default normal penalty stiffness. You can scale the tangential penalty stiffness to simulate sticking/slipping conditions on a step-by- step basis. This scaling only affects the perturbation step in which it is specified; it will not carry over to subsequent steps. If you want the same scale factor applied in a series of perturbation steps, you must specify the scale factor explicitly in each step. Some procedures that rely on a frequency analysis, such as complex frequency analysis and subspace-based steady-state dynamic analysis, are influenced by the scaling of the tangential stiffness that was in effect for the prior frequency analysis and the scaling of the tangential stiffness that is in effect for these steps. In such cases consistent scaling is recommended for these steps. For other mode-based procedures based on a frequency analysis, the scaling of the tangential stiffness is ignored and only the effect of the previous frequency analysis is considered. Input File Usage: To modify the tangential penalty stiffness for all contact pairs in a linear perturbation step: *CONTACT CONTROLS, PERTURBATION TANGENT SCALE FACTOR=factor To modify the tangential penalty stiffness for a specific contact pair in a linear perturbation step: *CONTACT CONTROLS, PERTURBATION TANGENT SCALE FACTOR=factor, SLAVE=slave surface, MASTER=master surface Abaqus/CAE Usage: Modifying the tangential penalty stiffness in linear perturbation steps is not supported in Abaqus/CAE. Contact controls associated with second-order faces Second-order elements not only provide higher accuracy but also capture stress concentrations more effectively and are better for modeling geometric features than first-order elements. Surfaces based on second-order element types work well with the surface-to-surface contact formulation but, in some cases, do not work well with the node-to-surface formulation . Some second-order element types are not well-suited for underlying the slave surface with the combination of a node-to-surface contact formulation and strict enforcement of “hard” contact conditions because of the distribution of equivalent nodal forces when a pressure acts on the face of the element. As shown in Figure 35.3.6–1, a constant pressure applied to the face of a second-order element without a midface node produces forces at the corner nodes acting in the opposite sense of the pressure. This ambiguous nature of the nodal forces in second-order elements can cause Abaqus/Standard to alter its internal contact logic inadequately. Slave surfaces based on second-order tetrahedral elements can also be problematic for the node-to-surface contact formulation because the distribution of equivalent nodal forces for a pressure acting on a face of these elements is such that the corner nodes have zero force. Options available in Abaqus/Standard to make it easier to use node-to-surface contact pairs involving second-order slave faces are discussed below. You can also avoid potential difficulties by using the surface-to-surface contact formulation, which is generally preferable. Manually or automatically adjusting element types Modified 10-node tetrahedral elements (C3D10M, etc.) do not cause fundamental difficulties for the node-to-surface contact formulation and often provide a viable option to 10-node second-order tetrahedral elements (C3D10, C3D10I, etc.) for models with node-to-surface contact pairs. Trade-offs in characteristics of modified 10-node tetrahedral elements versus second-order tetrahedral elements are discussed in “Modified triangular and tetrahedral elements” in “Solid (continuum) elements,” Section 28.1.1. If desired, you must make this adjustment to the element type as it does not occur automatically. Abaqus/Standard automatically adds midface nodes to underlying (serendipity) elements of most 8-node slave facets associated with node-to-surface contact pairs. For the three-dimensional 18-node gasket elements, the midface nodes are also generated automatically if they are not given in the element connectivity. The presence of the midface node results in a distribution of nodal forces that is not ambiguous for the contact algorithm. The element families C3D20(RH), C3D15(H), S8R5, q = pA r = pA 12 Figure 35.3.6–1 Equivalent nodal loads produced by a constant pressure on the second-order element face in “hard” contact simulations. and M3D8 are converted to the families C3D27(RH), C3D15V(H), S9R5, and M3D9, respectively. Since Abaqus/Standard does not convert second-order coupled temperature-displacement, coupled thermal-electrical-structural, and coupled pore pressure–displacement elements, you should use an alternative method to avoid problems with serendipity elements in the node-to-surface contact formulation in those cases. Abaqus/Standard will interpolate nodal quantities, such as temperature and field variables, at the automatically generated midface nodes when values are prescribed at any of the user-defined nodes. By default, Abaqus/Standard does not automatically add midface nodes to second-order serendipity elements that form a slave surface for surface-to-surface contact pairs; however, an option is available to enable the same algorithm for automatically adding midface nodes as used by node-to-surface contact pairs. Input File Usage: *CONTACT PAIR, TYPE=SURFACE TO SURFACE, MIDFACE NODES=YES Abaqus/CAE Usage: You cannot enable automatic conversion of serendipity elements underlying slave surfaces of surface-to-surface contact pairs in Abaqus/CAE. Supplementary contact constraints Another approach to avoiding difficulties that certain element types present to the node-to-surface contact formulation is to add supplementary contact constraints without changing the underlying element formulation. This approach is applicable only to cases in which node-to-surface contact pairs use penalty or augmented Lagrange constraint enforcement or a softened pressure-overclosure relationship, because it would result in overconstrained conditions if strictly enforced “hard” contact conditions are in effect. Supplementary contact constraints are sometimes helpful for improving convergence behavior or for improving the smoothness and accuracy of the contact pressure and underlying element stress; however, the extra constraints present some risk of degrading convergence behavior. Supplementary constraints are used selectively by default for node-to-surface contact pairs with 6-node slave faces of non-modified elements and 8-node slave faces unless strictly enforced “hard” contact conditions are in effect. You can deactivate supplementary constraints or add activate supplementary constraints for additional second-order element types underlying the slave surface. Input File Usage: *CONTACT PAIR, INTERACTION=interaction_property_name, SUPPLEMENTARY CONSTRAINTS=SELECTIVE slave_surface_name, master_surface_name Use the following option to add supplementary contact constraints for additional second-order element types: *CONTACT PAIR, INTERACTION=interaction_property_name, SUPPLEMENTARY CONSTRAINTS=YES slave_surface_name, master_surface_name Use the following option to forgo supplementary contact constraints: *CONTACT PAIR, INTERACTION=interaction_property_name, SUPPLEMENTARY CONSTRAINTS=NO slave_surface_name, master_surface_name Abaqus/CAE Usage: For a node-to-surface contact formulation: Interaction module: Create Interaction: Surface-to-surface contact (Standard): select the master surface; click Surface; select the slave surface; Interaction editor; Use supplementary contact points: Selectively, Always, or Never; Contact interaction property: interaction_property_name Smoothness of contact force redistribution upon sliding for surface-to-surface contact pairs You can control the smoothness of nodal contact force redistribution upon sliding for surface-to-surface contact pairs. The default setting, which is generally appropriate, results in the smoothness of the nodal force redistribution being of the same order as the elements underlying the slave surface; that is, linear redistribution smoothness for linear elements, and quadratic redistribution smoothness for second-order elements. Quadratic redistribution smoothness usually tends to improve convergence behavior and improve resolution of contact stresses within regions of rapidly varying contact stresses. However, quadratic redistribution smoothness tends to increase the number of nodes involved in each constraint, which can increase the computational cost of the equation solver. Linear redistribution smoothness tends to provide better resolution of contact stresses near edges of active contact regions and, therefore, occasionally results in better convergence behavior. Input File Usage: Use the following option to indicate that the smoothness of the contact force redistribution upon sliding should be of the same order as the elements underlying the slave surface for surface-to-surface contact pairs: *CONTACT PAIR, TYPE=SURFACE TO SURFACE, SLIDING TRANSITION=ELEMENT ORDER SMOOTHING slave_surface_name, master_surface_name Use the following option to indicate linear smoothness of the contact force redistribution upon sliding for surface-to-surface contact pairs: *CONTACT PAIR, TYPE=SURFACE TO SURFACE, SLIDING TRANSITION=LINEAR slave_surface_name, master_surface_name Use the following option to indicate quadratic smoothness of the contact force redistribution upon sliding for surface-to-surface contact pairs: *CONTACT PAIR, TYPE=SURFACE TO SURFACE, SLIDING TRANSITION=QUADRATIC slave_surface_name, master_surface_name Abaqus/CAE Usage: You cannot change the default contact force redistribution in Abaqus/CAE. 35.3.7 DEFINING TIED CONTACT IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 35.3.5 • *CONTACT PAIR • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Using contact and constraint detection,” Section 15.16 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Tied contact in Abaqus/Standard: • ties two surfaces forming a contact pair together for the duration of a simulation; • can be used in mechanical, coupled temperature-displacement, coupled thermal-electrical- transfer structural, coupled pore pressure-displacement, coupled thermal-electrical, or heat simulations; • constrains each of the nodes on the slave surface to have the same value of displacement, temperature, pore pressure, or electrical potential as the point on the master surface that it contacts; • allows for rapid transitions in mesh density within the model; • requires the adjustment of the contact pair surfaces; and • cannot be used with self-contact or symmetric master-slave contact. It is preferable to use the surface-based tie constraint capability instead of tied contact . Defining tied contact for a contact pair To “tie” the surfaces of a contact pair together for an analysis, you must also adjust the surfaces because, as described below, it is very important that the tied surfaces be precisely in contact at the start of the simulation. See “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 35.3.5, for details on adjusting surfaces. As always, you must associate the contact pair with a contact interaction property definition. Input File Usage: *CONTACT PAIR, TIED, ADJUST=a or node_set_label, INTERACTION=name Abaqus/CAE Usage: Interaction module: Interaction→Create: select a Slave Node/Surface Adjustment option: toggle on Tie adjusted surfaces The tied contact formulation When a contact pair uses the tied contact formulation, Abaqus/Standard uses the undeformed configuration of the model to determine which slave nodes are within the adjustment zone , accounting for any shell or membrane thickness by default. Abaqus/Standard then adjusts these slave nodes’ positions into a zero-penetration state and forms constraints between these slave nodes and the surrounding nodes on the master surface. The constraints are formed with either a “surface-to-surface” or a “node-to-surface” approach, similar to small-sliding contact. The traditional node-to-surface approach is used by default for tied contact. The user interface for selecting between the surface-to-surface and node-to-surface approaches and to avoid consideration of shell and membrane thickness for tied contact is the same as for small-sliding contact . Use of tied contact in mechanical simulations The tied contact formulation constrains only translational degrees of freedom in mechanical simulations. Abaqus/Standard places no constraints on the rotational degrees of freedom of structural elements involved in tied contact pairs. Self-contact is not supported with tied contact. Self-contact is designed for finite-sliding situations in which it is not obvious from the original geometry which parts of the surface will come into contact during the deformation. Mechanical constraints for tied contact are strictly enforced with a direct Lagrange multiplier method by default. Alternatively, you can specify that these constraints should be enforced with a penalty or augmented Lagrange constraint method . The constraint enforcement method specified will be applied to the tangential constraints in addition to the normal constraints. Softened contact pressure-overclosure linear—see “Contact pressure-overclosure relationships,” relationships (exponential, Section 36.1.2) are ignored for tied contact. tabular, or Use of tied contact in nonmechanical simulations The tied contact capability can be used in models where the nodal degrees of freedom include electrical potential and/or temperature. Except for the nodal degree of freedom being constrained, Abaqus/Standard uses exactly the same formulation for tied contact in nonmechanical simulations as it does for mechanical simulations. Unconstrained nodes in tied contact pairs Abaqus/Standard does not constrain slave nodes to the master surface unless they are precisely in contact with the master surface at the start of the analysis. Any slave nodes not precisely in contact at the start of the analysis—e.g., either open or overclosed—will remain unconstrained for the duration of the simulation; they will never interact with the master surface. In mechanical simulations an unconstrained slave node can penetrate the master surface freely. In a thermal, electrical, or pore pressure simulation an unconstrained slave node will not exchange heat, electrical current, or pore fluid with the master surface. To avoid such unconstrained nodes in tied contact pairs, use the capability for adjusting the surfaces of a contact pair described in “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 35.3.5. This capability moves slave nodes onto the master surface before Abaqus/Standard checks for the initial contact state. It is intended only for nodes that are close to the master surface and is not intended to correct large errors in the mesh geometry. Checking that slave nodes are constrained Abaqus/Standard prints a table in the data (.dat) file identifying the predominant slave node and other nodes involved in each constraint. If Abaqus/Standard cannot form a constraint for a given slave node acting as a predominant slave node, either because it is not in contact with the master surface or it cannot “see” the master surface, it will issue a warning message in the data file. For an explanation of when a slave node would not “see” a master surface and how to correct this problem, see “Contact formulations in Abaqus/Standard,” Section 37.1.1. When creating a model with tied contact, it is important to use this information provided by Abaqus/Standard to identify any unconstrained nodes and to make any necessary modifications to the model to constrain them. 35.3.8 EXTENDING MASTER SURFACES AND SLIDE LINES Product: Abaqus/Standard References • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 38.1.2 • *CONTACT PAIR • *SLIDE LINE Overview Extending the master surface or a slide line: • can prevent nodes from “falling off” or getting trapped behind the master surface (or slide line) in finite-sliding problems; • allows the slave node to find a master surface when the slave node has no intersection with the master surface at the start of the analysis in small- and infinitesimal-sliding problems; • can avoid numerical roundoff difficulties associated with contact modeling; • should not be used in lieu of proper contact modeling techniques; • should not be used to reduce the number of underlying elements of a contact surface; and • applies only to contact pairs that use a node-to-surface discretization. Extending the master surface for small-sliding, node-to-surface contact If a slave node cannot find an intersection with the master surface at the start of the analysis, it will be free to penetrate the master surface because no local tangent plane will be formed. This type of problem, which typically occurs for node-to-surface contact when the slave node is aligned with the edge of the master surface, is illustrated in Figure 35.3.8–1 and may be caused by numerical roundoff errors when a preprocessor is used to generate the nodal coordinates. Cases such as that shown in Figure 35.3.8–1 are not problematic for the small-sliding, surface-to-surface formulation because the constraint formulation considers the region of the slave surface near a slave node. Slave Node Slave Node Master Surface Master Surface No intersection (e = 0) Intersection found (e > 0) Figure 35.3.8–1 Slave node fails to find an intersection with the master surface for small-sliding, node-to-surface contact if e=0. For node-to-surface contact you can specify the size of the extension zone, e, as a fraction of the end segment or facet edge length . If e is set to zero, Abaqus will not extend the ends. The value given must lie between 0.0 and 0.2. The default value is 0.1 for node-to-surface contact; surface extensions are not available for surface-to-surface contact. Input File Usage: *CONTACT PAIR, SMALL SLIDING, EXTENSION ZONE=e Extending the master surface or slide line in finite-sliding, node-to-surface contact To prevent slave nodes from “falling off” or getting trapped behind the master surface, an open surface or slide line can be extended for finite-sliding, node-to-surface contact. You can specify the size of the extension zone, e, as a fraction of the end segment or facet edge length . The geometry in the extension zone is extrapolated from the end segment or facet edge. If e is set to zero, Abaqus/Standard will not extend the ends. The value given must lie between 0.0 and 0.2. The default value is 0.1 for node-to-surface contact. Surface extensions are not available for surface-to-surface contact; for finite-sliding, surface-to-surface contact, constraints are located within slave faces, and “falling off” will not occur until nearly the entire slave facet slides off the master surface. Extensions for finite-sliding, node-to-surface contact should be considered only if other modeling techniques to prevent “falling off” are not feasible and when the slave node is expected to travel in the extended zone for a short period of the solution phase or during nonconverged iterations. Input File Usage: Use either of the following options: *CONTACT PAIR, EXTENSION ZONE=e *SLIDE LINE, ELSET=element_set_name, EXTENSION ZONE=e Master Surface Extension Zone Extension Zone e × l1 l 2 e × l2 e × l2 l2 Master Surface l1 e × l1 Open 2-D Master Surface Open Axisymmetric Surface Extension Zone Slave Node 2-D Slide Line Slave Node e × l3 e × l1 2l Extension Zone e × l2 Open Slide Line e × l4 1l 4l e × l1 Master Surface 3l 2l e × l2 3-D Master Surface Figure 35.3.8–2 Definition of size of extension zone. CONTACT MODELING IF SUBSTRUCTURES ARE PRESENT CONTACT WITH SUBSTRUCTURES Product: Abaqus/Standard References • “Element-based surface definition,” Section 2.3.2 • “Node-based surface definition,” Section 2.3.3 • “Using substructures,” Section 10.1.1 • “Membrane elements,” Section 29.1.1 • “Surface elements,” Section 32.7.1 • “Contact interaction analysis: overview,” Section 35.1.1 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 Overview Contact in Abaqus/Standard involving substructures: • is not part of the substructure definition; • requires retaining nodes on the exterior of the substructure; • requires the definition of a contact surface on the retained nodes; and • can be between the exterior of one substructure and another surface, the exterior of one substructure and the exterior of another substructure, and the exterior of one substructure and itself. Defining the contact surface of a substructure Since a substructure consists only of a group of retained nodal degrees of freedom, it has no surface geometry upon which Abaqus/Standard can define a contact surface. One of the following methods must be used to define the surface geometry of the substructure: • mesh the exterior of the substructure with surface elements, • mesh the exterior of the substructure with structural elements, • use a node-based surface, or • use contact elements. Meshing the surface of the substructure with surface or structural elements provides the most flexibility in defining the contact conditions; the surface can be used as either a master or slave surface in the simulation. Using a node-based surface is probably the easiest method to use, but the limitations inherent to node-based surfaces (such as the inability to act as a master surface, the need to define nodal contact areas for exact contact stress recovery, and the lack of visualization of contact stresses) may limit the usefulness of this approach. Contact elements can be a useful method if the model uses matched meshes. Meshing the surface of the substructure with surface elements The surface geometry of the body being modeled with a substructure can be designated by defining elements on the retained surface nodes of the substructure. The elements can be used to create an element-based surface , which can then be used as part of a contact pair. Whenever possible, it is recommended that you use surface elements to mesh the exterior of a substructure. Surface elements will accurately define the surface geometry of the substructure without introducing any additional stiffness to the model; the stiffness of the underlying body is built into the substructure. See “Surface elements,” Section 32.7.1, for more information about surface elements. Figure 35.3.9–1 shows a simulation where both of the contacting bodies have been modeled with substructures. The nodes retained in the model are indicated in the figure. If this were a three-dimensional model, general surface elements would be used to reconstruct the appropriate surface geometries of the original mesh. ⇒ (a) critical model (b) nodes retained for contact resolution Figure 35.3.9–1 Substructuring in a contact simulation. Limitations of surface elements Surface elements cannot be used to overlay substructures in planar models. Surface elements also cannot be used to overlay a substructure that consists of second-order, three-dimensional elements with midface nodes (C3D27(R)(H) or C3D15V(H)). Surface elements with midface nodes are not currently available in Abaqus/Standard, and the 8-node surface element (SFM3D8) is not well suited for contact modeling. Meshing the surface of the substructure with structural elements Although surface elements are generally preferable for use in substructure contact situations, you can also use structural elements to define the surface geometry of a substructure. You can use membrane elements in three-dimensional models and axisymmetric models, and trusses in planar models. Define the elements to have very small thickness or area and define their material property to have a very small elastic modulus so that their contribution to the stiffness of the model is negligible. If the model in Figure 35.3.9–1 were a planar model, truss elements would be used to connect the nodes and define the surface geometry. The truss elements would have a very small cross-sectional area and refer to a material property with very low stiffness so that they do not add any significant stiffness to the underlying bodies. Limitations of structural elements Membrane elements cannot be used to overlay a substructure that consists of second-order, three-dimensional brick elements of type C3D20(R)(H) if the substructure will be used as a slave surface. Normally, Abaqus/Standard automatically converts C3D20(R)(H) brick elements to elements with midface nodes C3D27(R)(H) because this class of elements performs better in contact simulations. that does Abaqus/Standard also converts any second-order, not have a midface node when it is used in a slave surface . Therefore, if second-order membrane elements (type M3D8) are used to reconstruct the surface topology of a substructure consisting of C3D20 elements, Abaqus/Standard will convert them to M3D9 elements when the surface is used as a slave surface. The midface nodes that are generated automatically will not correspond to any retained nodes and, thus, will have zero stiffness. The lack of stiffness at these nodes will cause numerical problems during the analysis. Membrane elements can be used if elements of type C3D27(R)(H) have been used on the surface of the substructure. three-dimensional structural element Using a node-based surface to define the substructure’s surface If the retained nodes of the substructures are associated with the slave surface of a contact pair, the retained nodes can be included in a node-based surface . In this case it is not necessary to overlay the surface of the substructure with elements. Using contact elements to define the substructure’s surface GAP elements (“Gap contact elements,” Section 39.2.1) can be used to define the contact interactions in the model. These elements require that matching nodes be present on the opposite sides of the contact surfaces and allow only for small relative sliding between the surfaces. This latter assumption is usually consistent with the assumption of linear behavior that is built into a substructure. CONTACT MODELING IF ASYMMETRIC-AXISYMMETRIC ELEMENTS ARE PRESENT ASYMM.-AXISYMM. CONTACT Product: Abaqus/Standard References • “Slide line contact elements,” Section 39.4.1 • “Rigid surface contact elements,” Section 39.5.1 • *ASYMMETRIC-AXISYMMETRIC Overview Modeling contact in asymmetric-axisymmetric problems: • requires the use of contact elements (ISL or IRS); • requires independent contact elements on each circumferential plane; and • can be done only on certain circumferential planes. Modeling contact in asymmetric-axisymmetric problems asymmetric CAXA or SAXA elements are used to model problems where initially axisymmetric structures may undergo asymmetric deformations. These asymmetric deformations may include asymmetric contact conditions. The surface-based contact capability cannot be used to model such problems; contact elements (ISL or IRS) must be used. Independent sets of two-dimensional contact elements must be created for each circumferential plane in the CAXA or SAXA elements. You must specify the angle, , of the circumferential plane with which each set of contact elements is associated and the number of Fourier modes, n, used with the underlying CAXA or SAXA elements. Input File Usage: Use both of the following options: *INTERFACE, ELSET=element_set_name *ASYMMETRIC-AXISYMMETRIC, MODE=n, ANGLE= where the ELSET parameter refers to a set of ISL- or IRS-type contact elements. Limitations on contact in asymmetric-axisymmetric problems If the circumferential planes in an asymmetric-axisymmetric problem rotate more than a few degrees, Abaqus/Standard can model contact conditions correctly only on the =0 and 180 circumferential planes. The asymmetric-axisymmetric elements have internal degrees of freedom for the rotation and out-of- plane motion of the circumferential planes, but these degrees of freedom are not accounted for in the contact elements. Ignoring these degrees of freedom means that Abaqus/Standard keeps the contact directions fixed in initial circumferential planes and the position of the nodes is projected back onto these initial planes for contact calculations. If the rotation and motion of the nodes from these initial planes are small, the errors caused by this approach are minimal. If they are large, the errors will become very large, making the results unrealistic. 35.4 Defining general contact in Abaqus/Explicit • “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1 • “Assigning surface properties for general contact in Abaqus/Explicit,” Section 35.4.2 • “Assigning contact properties for general contact in Abaqus/Explicit,” Section 35.4.3 • “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 35.4.4 • “Contact controls for general contact in Abaqus/Explicit,” Section 35.4.5 35.4.1 DEFINING GENERAL CONTACT INTERACTIONS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Contact interaction analysis: overview,” Section 35.1.1 • *CONTACT • *CONTACT INCLUSIONS • *CONTACT EXCLUSIONS • “Defining general contact,” Section 15.13.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Abaqus/Explicit provides two algorithms for modeling contact and interaction problems: the general contact algorithm and the contact pair algorithm. See “Contact interaction analysis: overview,” Section 35.1.1, for a comparison of the two algorithms. This section describes how to include general contact in an Abaqus/Explicit analysis, how to specify the regions of the model that may be involved in general contact interactions, and how to obtain output from a general contact analysis. The general contact algorithm in Abaqus/Explicit: • is specified as part of the model or history definition of the model; • allows very simple definitions of contact with very few restrictions on the types of surfaces involved; • uses sophisticated tracking algorithms to ensure that proper contact conditions are enforced efficiently; • can be used simultaneously with the contact pair algorithm (i.e., some interactions can be modeled with the general contact algorithm, while others are modeled with the contact pair algorithm); • can be used only with three-dimensional surfaces; • can be used only in mechanical finite-sliding contact analyses; and • does not support kinematic constraint enforcement (contact constraints are enforced with the penalty method). Defining a general contact interaction The definition of a general contact interaction consists of specifying: • the general contact algorithm and defining the contact domain (i.e., the surfaces that interact with one another), as described in this section; • the contact surface properties Abaqus/Explicit,” Section 35.4.2); (“Assigning surface properties for general contact in • the mechanical contact property models (“Assigning contact properties for general contact in Abaqus/Explicit,” Section 35.4.3); • the contact Section 37.2.1); formulation (“Contact formulation for general contact in Abaqus/Explicit,” • the initial clearance between contact surfaces (“Controlling initial contact status for general contact in Abaqus/Explicit,” Section 35.4.4); and • the algorithmic contact controls (“Contact controls for general contact in Abaqus/Explicit,” Section 35.4.5). Surfaces used for general contact The general contact algorithm allows for very general characteristics in the surfaces that it uses, as discussed in “Contact interaction analysis: overview,” Section 35.1.1. For detailed information on defining surfaces in Abaqus/Explicit for use with the general contact algorithm, see “Element-based surface definition,” Section 2.3.2; “Node-based surface definition,” Section 2.3.3; “Analytical rigid surface definition,” Section 2.3.4; “Eulerian surface definition,” Section 2.3.5; and “Operating on surfaces,” Section 2.3.6. Two-dimensional surfaces cannot be used with the general contact algorithm. A convenient method of specifying the contact domain is using cropped surfaces. Such surfaces can be used to perform “contact in a box” by using a contact domain that is enclosed in a specified rectangular box in the original configuration. For more information, see “Operating on surfaces,” Section 2.3.6. In addition, Abaqus/Explicit automatically defines an all-inclusive surface that is convenient for prescribing the contact domain, as discussed later in this section. The all-inclusive automatically defined surface includes all element-based surface facets as well as all analytical rigid surfaces and surfaces on all Eulerian materials. The general contact algorithm generates contact forces to resist node-into-face, node-into-analytical rigid surface, and edge-into-edge contact penetrations. The primary mechanism for enforcing contact is node-to-face contact (the only mechanism used in the contact pair algorithm). If analytical rigid surfaces are present in the contact domain, the general contact algorithm also enforces node-to-analytical rigid surface contact. Considerations for edge-to-edge contact The general contact algorithm also considers edge-to-edge contact, which is very effective in enforcing contact that cannot be detected as penetrations of nodes into faces. For example, contact between beam segments and shell perimeter edges usually is detected only as edge-to-edge contact. The terminology “contact edges” refers to feature edges of surface facets (on both shells and solids) as well as to segments representing beam and truss elements. The contact edges representing beam and truss elements have a circular cross-section, regardless of the actual cross-section of the beam or truss element. The radius of a contact edge representing a truss element is derived from the cross-sectional area specified on the truss section definition (it is equal to the radius of a solid circular section with an equivalent cross-sectional area). For beams with circular cross-sections, the radius of the contact edge is equivalent to the section radius. For beams with non-circular cross-sections, the radius of the contact edge is equal to the radius of a circumscribed circle around the section. If geometric feature edges, which can optionally be included in the contact domain. Abaqus/Explicit GENERAL CONTACT Thick solid lines indicate shell perimeter edges and "contact edges" corresponding to beams. Beam Solid Shells Dashed lines indicate element boundaries for which edge-to-edge contact is not modeled. Figure 35.4.1–1 General contact domain, including edge-to-edge contact. connected edges have different radii, a nodal radius is first computed as the minimum radius of the adjacent contact edges, and the radius of the edge cross-section is interpolated linearly over the length of the contact edge from the nodal values. Shell element edges reflect the shell thickness in the normal direction and do not extend past the perimeter (similar to shell nodes and facets). Some numerical rounding of features occurs for both node-to-facet and edge-to-edge contact. To model contact between edges that are not cylindrical in shape, surface elements can be attached to the edge nodes using surface-based tie constraints and node-to-face contact can be defined between the surface elements . This technique is useful for modeling geometric details important to the contact definition that are not modeled with the underlying element geometry. Surface elements can also be defined around shell elements in which Abaqus has reduced the contact thickness (i.e., if the thickness exceeds the surface facet edge lengths or diagonal lengths) so that the true surface thickness can be modeled. However, using surface elements with general contact requires a physically reasonable mass to be associated with the surface element nodes, and care must be taken not to alter the bulk mass properties when transferring mass to the surface elements from the underlying elements. By default, when a surface is used in a general contact interaction, all applicable facets, analytical rigid surfaces, nodes, perimeter edges, and beam and truss segments are included in the contact definition. You can control which feature edges are considered for edge-to-edge contact, as discussed in “Assigning surface properties for general contact in Abaqus/Explicit,” Section 35.4.2. Geometric feature edges and perimeter edges do not have to be included explicitly in a surface definition (by using edge identifiers) for them to be considered for edge-to-edge contact. Eulerian-Lagrangian contact The general contact algorithm also enforces contact between Eulerian materials and Lagrangian surfaces. This algorithm automatically compensates for mesh size discrepancies to prevent penetration of Eulerian material through the Lagrangian surface. The all-inclusive surface that is defined by Abaqus/Explicit can be used to enforce contact between all Eulerian materials and all Lagrangian bodies in a model; you can also specify individual Eulerian surfaces in the contact domain . Eulerian-Lagrangian contact is enforced only for Lagrangian surfaces defined on solid and shell elements. Other surface types, such as beam edges and analytical rigid surfaces, are ignored. Contact interactions between Eulerian materials and interactions due to Eulerian material self-contact are handled naturally by the Eulerian formulation; these interactions do not require a general contact definition. See “Interactions” in “Eulerian analysis,” Section 14.1.1, for more information. Including general contact in an analysis If a general contact definition does not appear in a step, any general contact definition active in the previous step will be propagated to the current step. For convenience, general contact can be defined as model data. A general contact definition specified as model data is considered to be defined in the initial step, or “Step 0,” of the analysis; it can be modified or removed in Step 1 or later steps. Input File Usage: Use the following option to indicate the beginning of a general contact definition: *CONTACT This option can appear only once per step. Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Explicit) Removing general contact definitions You can remove the previously specified general contact definition and specify a new one. Input File Usage: Abaqus/CAE Usage: *CONTACT, OP=NEW Interaction module: interaction manager: select interaction, Deactivate Modifying general contact definitions Alternatively, you can make changes to an existing general contact definition. In this case the existing general contact definition remains active and any additional information specified is appended to the general contact definition. Contact state information (such as the proper contact normal orientation for double-sided surfaces) is transferred across step boundaries even if the contact domain is modified. *CONTACT, OP=MOD Input File Usage: Abaqus/CAE Usage: Interaction module: interaction manager: select interaction, Edit Example Each part of a general contact definition is considered independently when it is modified. For example, the following contact definition is specified in Step 1 (the individual options are discussed later in this section): *CONTACT *CONTACT INCLUSIONS surf_1, *CONTACT EXCLUSIONS surf_a, surf_b This contact definition is then modified in Step 2 with the following input: *CONTACT, OP=MOD *CONTACT INCLUSIONS surf_2, surf_3 *CONTACT EXCLUSIONS surf_a, surf_c An equivalent contact definition for Step 2 could be specified as follows: *CONTACT, OP=NEW *CONTACT INCLUSIONS surf_1, surf_2, surf_3 *CONTACT EXCLUSIONS surf_a, surf_b surf_a, surf_c Defining the general contact domain You specify the regions of the model that can potentially come into contact with each other by defining general contact inclusions and exclusions. Only one contact inclusions definition and one contact exclusions definition are allowed per step. All contact inclusions in an analysis are applied first, then all contact exclusions are applied, regardless of the order in which they are specified. The contact exclusions take precedence over the contact inclusions. The general contact algorithm will consider only those interactions specified by the contact inclusions definition and not specified by the contact exclusions definition. General contact interactions typically are defined by specifying self-contact for the default automatically generated surface provided by Abaqus/Explicit. All surfaces used in the general contact algorithm can span multiple unattached bodies, so self-contact in this algorithm is not limited to contact of a single body with itself. For example, self-contact of a surface that spans two bodies implies contact between the bodies as well as contact of each body with itself. Specifying contact inclusions Define contact inclusions to specify the regions of the model that should be considered for contact purposes. Specifying “automatic” contact for the entire model You can specify self-contact for a default unnamed, all-inclusive surface defined automatically by Abaqus/Explicit. This default surface contains, with the exceptions noted below, all exterior element faces, all analytical rigid surfaces and all edges based on beam and truss elements in the model, as well as the nodes attached to these faces and edges; in addition, feature edges are included according to the user-specified criteria . This is the simplest way to define the contact domain. With this approach contact is modeled for all node-to-facet, node-to-analytical rigid surface, and edge-to-edge interactions of the nodes, facets, analytical rigid surfaces, and contact edges of the default surface. This default surface does not include the following: • Nodes that cannot be part of an element-based surface; for example, nodes attached only to point masses or connectors. • Faces, edges, and nodes that belong only to cohesive elements. In fact, this default surface is generated as if cohesive elements were not present. See “Modeling with cohesive elements,” Section 32.5.3, for further discussion of contact modeling issues related to cohesive elements. Input File Usage: Use both of the following options to specify “automatic” contact for the entire model: *CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR The *CONTACT INCLUSIONS option should have no data lines when the ALL EXTERIOR parameter is used. Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: All* with self Specifying individual contact interactions Alternatively, you can define the general contact domain directly by specifying the individual contact surface pairings. Self-contact will be modeled only if the two surfaces specified in a pair overlap (or are identical) and will be modeled only in the overlapping region. Multiple surface pairings can be included in the contact domain. At least one surface in each pair must be either an element-based surface or an analytical rigid surface. Input File Usage: Use both of the following options to specify individual contact interactions: *CONTACT *CONTACT INCLUSIONS surface_1, surface_2 At least one data line must be specified when the ALL EXTERIOR parameter is omitted. Either or both of the data line entries can be left blank, but each data line must contain at least a comma; an error message will be issued for empty data lines. If the first surface name is omitted, the default unnamed, all-inclusive, automatically generated surface is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is assumed. Leaving both data line entries blank is equivalent to using the ALL EXTERIOR parameter. Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: Selected surface pairs: Edit, select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of included pairs Abaqus/CAE Usage: Examples The following input specifies that contact should be enforced between the default all-inclusive, automatically generated surface and surface_2, including self-contact in any overlap regions: *CONTACT *CONTACT INCLUSIONS , surface_2 Either of the following methods can be used to define self-contact for surface_1: or *CONTACT *CONTACT INCLUSIONS surface_1, *CONTACT *CONTACT INCLUSIONS surface_1, surface_1 The following input can be used to introduce a node-based surface containing point masses to the contact domain as well as specify self-contact for the default all-inclusive, automatically generated surface: *CONTACT *CONTACT INCLUSIONS , , node_based_surf Specifying contact exclusions You can refine the contact domain definition by specifying the regions of the model to exclude from contact. The primary motivation for specifying contact exclusions is to avoid physically unreasonable contact interactions. For example, a finite element model may contain multiple forming tools, but not all of the tools participate in the forming process simultaneously; you can specify contact exclusions to prevent certain tools from participating in the contact model in certain steps. You do not need to be concerned with specifying contact exclusions for parts of the model that are not likely to interact, since these exclusions typically will have minimal effect on computational performance. Contact will be ignored for all the surface pairings specified, even if these interactions are specified directly or indirectly in the contact inclusions definition. Multiple surface pairings can be excluded from the contact domain. At least one surface in each pair must be either an element-based surface or an analytical rigid surface. Keep in mind that surfaces can be defined to span multiple unattached bodies, so self-contact exclusions are not limited to exclusions of single-body contact. You cannot exclude only one side of shell-like surfaces. If a side label (SPOS or SNEG) is used in defining an element-based shell-like surface and that surface is excluded from contact, Abaqus/Explicit will exclude all faces associated with these elements. Input File Usage: Use both of the following options to specify contact exclusions: *CONTACT *CONTACT EXCLUSIONS surface_1, surface_2 Either or both of the data line entries can be left blank. If the first surface name is omitted, the default unnamed, all-inclusive, automatically generated surface is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is excluded from the contact domain. Interaction module: Create Interaction: General contact (Explicit): Excluded surface pairs: Edit, select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of excluded pairs Abaqus/CAE Usage: Automatically generated contact exclusions Abaqus/Explicit automatically generates contact exclusions for general contact in some situations. • Contact exclusions are generated automatically for interactions that are defined with the contact pair algorithm or surface-based tie constraints to avoid redundant (and possibly inconsistent) if a contact pair is defined for enforcement of these interaction constraints. surface_1 and surface_2 and “automatic” general contact is defined for the entire model, Abaqus/Explicit would generate a contact exclusion for general contact between surface_1 and surface_2, so that interactions between these surfaces would be modeled only with the contact pair algorithm. These automatically generated contact exclusions are in effect only during the steps in which the contact pair algorithm or surface-based tie constraint interactions are active. For example, • Abaqus/Explicit automatically generates contact exclusions for self-contact of each rigid body in the model, because it is not possible for a rigid body to contact itself. • When you specify pure master-slave contact surface weighting for a particular general contact surface pair, contact exclusions are generated automatically for the master-slave orientation opposite to that specified . • The general contact algorithm, unlike the contact pair algorithm, activates and deactivates contact faces and contact edges in the contact domain based on the failure status of the underlying elements. See “Modeling surface erosion” below for details. Examples The following input specifies that the contact domain is based on self-contact of an all-inclusive, automatically generated surface but that contact (including self-contact in any overlap regions) should be ignored between the all-inclusive, automatically generated surface and surface_2: *CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR *CONTACT EXCLUSIONS , surface_2 Either of the following methods can be used to exclude self-contact for surface_1 from the contact domain: *CONTACT EXCLUSIONS surface_1, or *CONTACT EXCLUSIONS surface_1, surface_1 Modeling surface erosion General contact allows the use of element-based surfaces to model surface erosion for analyses. If an appropriate “interior” surface is defined, the surface topology will evolve to match the exterior of elements that have not failed. Alternatively, if only one of the bodies can erode, a node-based surface can be used to model surface erosion; this approach can be used with either the general contact or contact pair algorithms. However, even if only one body can erode, it is recommended to define an element-based surface for the eroding body to avoid the usual limitations of node-based surfaces . The general contact algorithm modifies the list of contact faces and contact edges that are active in the contact domain based on the failure status of the underlying elements (element failure is discussed in “Dynamic failure models,” Section 23.2.8). General contact considers a face only if its underlying element has not failed and it is not coincident with a face from an adjacent element that has not failed; thus, exterior faces are initially active, and interior faces are initially inactive. Once an element fails, its faces are removed from the contact domain, and any interior faces that have been exposed are activated. A contact edge is removed when all the elements that contain the edge have failed. New contact edges are not created as elements erode. Based on this algorithm, the active contact domain evolves during the analysis as elements fail . newly exposed faces surface topology before the shaded elements have failed surface topology after failure Figure 35.4.1–2 Topology of an eroding contact surface. You can control whether contact nodes remain in the contact domain after all the surrounding elements have failed. By default, these nodes remain in the contact domain and act as free-floating point masses that can experience contact with faces that are still part of the contact domain. You can specify that nodes of element-based surfaces should erode (i.e., be removed from the contact domain) once all contact faces and contact edges to which they are attached have eroded. Further discussion of this technique, including reasons for and against nodal erosion, can be found in “Contact controls for general contact in Abaqus/Explicit,” Section 35.4.5. Erosion of surfaces specified on solid elements For a solid element mesh consisting of elements that may fail, every face that can potentially be involved in contact (both exterior and interior faces) should be included in the contact domain. The general contact algorithm will activate and deactivate faces as necessary when elements fail. For example, you define an element set ELERODE that contains all the solid elements in the model that refer to a material failure model. First, you must create a surface SURFERODE containing all of the interior and exterior faces of these elements. You could define this surface using the automatic free surface and interior surface generation methods in Abaqus/Explicit. Assuming all the elements in ELERODE are of type C3D8R, you could alternatively define the surface by specifying the faces S1 through S6 directly. See “Creating surfaces on solid, continuum shell, and cohesive elements” in “Element-based surface definition,” Section 2.3.2, for a discussion of these three methods. Next, you must construct the contact domain. Defining “automatic” general contact for the entire model is not sufficient because the contact domain created when this method is used does not include any interior faces. Therefore, you must define the pairwise interactions with the erodable surface explicitly in the contact inclusions definition, as outlined in Table 35.4.1–1. Alternatively, you could create a more concise definition of the same contact domain by first defining a surface named SURFALL that includes all exterior faces in the entire model and all interior faces of element set ELERODE. In this case, since all faces (exterior and interior) in the contact domain are Table 35.4.1–1 Contact inclusions definitions. Contact inclusions Input file syntax Abaqus/CAE syntax Self-contact for the default all-inclusive surface specifies contact between every exterior face in the model , Contact between the default all-inclusive surface and SURFERODE specifies contact between every exterior face and SURFERODE , SURFERODE First Surface: (All*) Second Surface: (Self) First Surface: (All*) Second Surface: SURFERODE Self-contact for SURFERODE specifies self-contact between the eroding bodies SURFERODE, First Surface: SURFERODE Second Surface: (Self) defined in one surface, there is no need to define contact explicitly between the exterior and interior faces. It would be adequate to specify only self-contact for SURFALL. Abaqus/Explicit automatically computes a nonzero contact thickness associated with interior faces based on element dimensions, and this default value cannot be changed via a surface property assignment. Erosion of surfaces specified on structural elements For structural elements, the general contact algorithm checks the underlying elements of the faces (or “contact edges” on beam and truss elements) for failure. Once the underlying element fails, the face is removed. As with solids, feature edges on structural elements are removed once all of the surrounding faces have failed. A perimeter edge (e.g., on the perimeter of a shell element mesh) is removed once the face it is connected to fails. New perimeter edges are not created to conform to the new perimeter created by the removal of a face. Memory use The amount of contact data used to describe the surface topology is proportional to the number of faces included in the contact domain. Including a large number of interior faces in the contact domain can potentially increase memory use significantly compared to analyses in which the contact domain is defined using only exterior faces. Consider creating a surface on a cubic mesh of C3D8R elements with n elements per side. A surface including the exterior faces of the mesh (suitable for modeling contact without element failure) would contain 6n2 element faces. A surface including both exterior and interior faces of the mesh (suitable for modeling contact with element failure for every element in the mesh) would contain 6n3 element faces. For large meshes the memory use can increase easily by an order of magnitude when interior element faces are included in the contact domain to model erosion. Therefore, it is recommended to include only those interior element faces in the contact domain that could possibly participate in contact. Output The surfaces that compose the general contact domain are available as output in addition to the contact analysis output variables. General contact domain surfaces defined: the following internal General_Contact_Edges_k, General_Contact_Faces_k, surfaces when a general contact domain Abaqus/Explicit generates is and General_Contact_Nodes_k, where k is the step number. General_Contact_Nodes_k contains only nodes in the general contact domain that are not included in the other two surfaces. For example, General_Contact_Faces_2 would contain all surface faces (interior and exterior) that were initially included in the general contact domain for Step 2. These surfaces contain the contact faces, edges, and nodes that were included in the contact domain at the beginning of the step and are not modified to reflect surface erosion. These internal surfaces can be viewed using display groups in the Visualization module of Abaqus/CAE . The internal surface names used by Abaqus/Explicit should not appear in the input file. General contact output variables You can write the contact surface variables associated with general contact interactions to the Abaqus output database (.odb) file . The available variables are contact pressure, normal contact force, frictional force, and whole surface resultant quantities (i.e., force, moment, center of pressure, and total area in contact). Field output The generic variables CSTRESS and CFORCE are valid field output requests for general contact in Abaqus/Explicit. If CSTRESS is requested for the general contact domain, the variable CPRESS (contact pressure) can be contoured in Abaqus/CAE. If CFORCE is requested for the general contact domain, the variables CNORMF (normal contact force) and CSHEARF (shear contact force) can be plotted as vectors in a symbol plot in Abaqus/CAE. For general contact CPRESS is calculated as the magnitude of the net contact normal force (the CNORMF vector) per unit area (it is an unsigned value). This convention for reporting contact pressure is different from the convention used for contact pairs. The direction of action of the net contact pressure for general contact can be determined by examining a plot of CNORMF. CNORMF and CSHEARF are resultant force quantities. If a double-sided surface is contacted on both sides, the resultant force is a vector sum of the force from each side of the surface (for example, the contact normal force will be zero for a double-sided surface that is pinched with equal and opposite forces on each side of the surface). History output Several whole surface contact force-derived variables are available as history output. You can specify the surface from which the contact force resultants will be calculated. Force distributions on the surface due to general contact are used to calculate the surface force resultants; forces due to contact pair interactions are not included and must be output separately. The contact state of a surface is output as a set of force (CFN, CFS, and CFT) and moment (CMN, CMS, and CMT) resultants with respect to the origin. Additional variables give the center of force (XN, XS, and XT) on the surface (defined as the point closest to the centroid of the surface that lies on the line of action of the resultant force for which the resultant moment is minimal). The last letter of each variable name denotes which contact force distribution on the surface is used to calculate the resultant: the letter N denotes that the normal contact forces are used to derive the resultant quantity; the letter S denotes that the shear contact forces are used to derive the resultant quantity; and the letter T denotes that the sum of the normal and shear contact forces are used to derive the resultant quantity. Each total moment output variable will not necessarily equal the cross product of the respective center of force vector and resultant force vector. Forces acting on two different nodes of a surface may have components acting in opposite directions, such that these nodal force components generate a net moment but not a net force; therefore, the total moment may not arise entirely from the resultant force. The center of force output variables tend to be most meaningful when the surface nodal forces act in approximately the same direction. The total area in contact at a given time can be requested using output variable CAREA, defined as the sum of all the facets where there is contact force. The contact area reported by CAREA is generally slightly larger than the true contact area for reasonably meshed contact surfaces; therefore, interpretation of CAREA should be done with care. The discrepancy between the CAREA output and the true contact area decreases as the mesh density increases. Using contact inclusions or exclusions to limit CAREA output to smaller contact surfaces may also reduce the discrepancy in some cases. Since the CAREA output is an approximation of the true contact area, deriving force or stress values using this output may not yield accurate values; requesting contact force and stress directly is the most appropriate way to obtain accurate results. Requesting element output when modeling surface erosion When modeling the erosion of surfaces, it is useful to request additional element field output of the element status (output variable STATUS). Failed elements (with an element status of zero) can then be excluded from the display group in the Visualization module of Abaqus/CAE so that the active contact surface can be identified and contact results on the active contact surface can be viewed. 35.4.2 ASSIGNING SURFACE PROPERTIES FOR GENERAL CONTACT IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1 • *CONTACT • *SURFACE PROPERTY ASSIGNMENT • “Specifying surface property assignments for general contact,” Section 15.13.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Surface property assignments: • can be used to change the contact thickness used for regions of a surface based on structural elements or to add a contact thickness for regions of a surface based on solid elements; • can be used to specify surface offsets for regions of a surface based on shell, membrane, rigid, and surface elements; • can be used to specify which edges of a model should be included in the general contact domain; • can be used to specify geometric corrections for regions of a surface; • can be applied selectively to particular regions within a general contact domain; and • cannot be applied to analytical rigid surfaces. Assigning surface properties You can assign nondefault surface properties to surfaces involved in general contact interactions. These properties are considered only when the surfaces are involved in general contact interactions; they are not considered when the surfaces are involved in other interactions such as contact pairs. The general contact algorithm does not consider surface properties specified as part of the surface definition. Surface property assignments propagate through all analysis steps in which the general contact interaction is active. The surface names used to specify the regions with nondefault surface properties do not have to correspond to the surface names used to specify the general contact domain. In many cases the contact interaction will be defined for a large domain, while nondefault surface properties will be assigned to a subset of this domain. Any surface property assignments for regions that fall outside the general contact domain will be ignored. The last assignment will take precedence if the specified regions overlap. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY This option must be used in conjunction with the *CONTACT option. It should appear at most once per step for each value of the PROPERTY parameter discussed below; the data line can be repeated as often as necessary to assign surface properties to different regions. Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Explicit): Surface Properties Surface thickness The default calculation of the nodal surface thickness (described in detail below) is appropriate for most analyses; one exception is sheet forming analysis, in which the thinning of a sheet significantly influences contact. This case can be modeled by specifying that the decreasing parent element thickness should be used. As a third alternative, you can specify a value for the surface thickness. A nonzero thickness can be assigned to solid element surfaces, for example, to model the effect of a finite-thickness surface coating. “Element-based surface definition,” Section 2.3.2, contains information on the spatial variation of the surface thickness. Specifying the original or decreasing thickness results in a zero thickness for node-based surfaces; you can specify a nonzero thickness for a node-based surface used with the general contact algorithm (the contact pair algorithm will not consider a nonzero thickness for such surfaces). The general contact algorithm requires that the contact thickness does not exceed a certain fraction of the surface facet edge lengths or diagonal lengths. This fraction generally varies from 20% to 60% based on the geometry of the element. The general contact algorithm will scale back the contact thickness automatically where necessary without affecting the thickness used in the element computations for the underlying elements. Diagnostic information is provided in the status (.sta) file if such scaling is performed. To bypass this limitation on thickness, the contact surface can be modeled with surface elements . The surface elements must be attached to the underlying elements using a surface-based tie constraint , and a physically reasonable mass must be associated with the surface elements. This requires a significant fraction of the mass to be transferred to the surface elements from the underlying elements without appreciably altering the bulk mass properties. Alternatively, contact controls settings can be used to limit the thickness reduction checks . The “bull-nose” effect that occurs at shell perimeters with the contact pair algorithm is avoided with the general contact algorithm by default. Shell element edges, nodes, and facets reflect the shell thickness in the normal direction only and do not extend past the perimeter. Contact controls settings can be used to turn off the bull-nose prevention checks . Using the original parent element thickness By default, the nodal thickness for surfaces based on shell, membrane, or rigid elements equals the minimum original thickness of the surrounding elements . specified element thickness (constant over element) interpolated surface thickness nodal surface thickness Figure 35.4.2–1 Continuous variation of surface thickness across facet boundaries. Table 35.4.2–1 Thicknesses corresponding to Figure 35.4.2–1. Node Element Specified element thickness Nodal surface thickness (minimum of adjacent element thicknesses) 0.5 0.5 0.9 0.9 0.5 0.5 0.5 0.9 0.9 The surface thickness within a facet is interpolated from the nodal values; the interpolated surface thickness never extends past the specified element or nodal thickness, which may be significant with respect to initial overclosures. The default nodal surface thickness is zero for regions of a surface based on solid elements. If a spatially varying nodal thickness is defined for the underlying elements , the nodal surface thickness may not correspond exactly to the specified nodal thickness . element thickness (constant over element) nodal surface thickness specified nodal thickness interpolated surface thickness Figure 35.4.2–2 Small discrepancy between the nodal surface thickness and the specified nodal thickness. Table 35.4.2–2 Thicknesses corresponding to Figure 35.4.2–2. Node Element Specified nodal thickness Element thickness (average of specified nodal thickness) Nodal surface thickness (minimum of adjacent element thicknesses) 0.5 0.5 0.5 0.9 0.9 0.9 0.5 0.5 0.7 0.9 0.9 35.4.2–4 0.5 0.5 0.5 0.7 0.9 The nodal surface thickness distribution will tend to be more diffuse than the specified nodal thickness distribution (because the specified nodal thicknesses are averaged to compute the element thicknesses, and the minimum of the surrounding element thicknesses is the nodal surface thickness). Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=THICKNESS surface, ORIGINAL (default) Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Shell/Membrane thickness assignments: Edit: Select surface, click the arrows to transfer surface to list of thickness assignments, and enter ORIGINAL in the Thickness column. Using the decreasing parent element thickness If you specify that the decreasing parent element thickness should be used, only decreases in the parent element thickness are reflected in the contact surface thickness; if the parent element thickness actually increases during the analysis, the contact thickness will remain constant. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=THICKNESS surface, THINNING Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Shell/Membrane thickness assignments: Edit: Select surface, click the arrows to transfer surface to list of thickness assignments, and enter THINNING in the Thickness column. Specifying a value for the surface thickness You can directly specify the surface thickness value. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=THICKNESS surface, value Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Shell/Membrane thickness assignments: Edit: Select surface, click the arrows to transfer surface to list of thickness assignments, and enter a value for the surface thickness magnitude in the Thickness column. Applying a scale factor to the surface thickness You can apply a scale factor to any value of the surface thickness. For example, if you specify that the decreasing parent element thickness should be used for surf1 and apply a scale factor of 0.5, a value of one half the decreasing parent element thickness will be used for surf1 when it is involved in a general contact interaction (all other surfaces included in the general contact domain will use the default original parent element thickness). Scaling the surface thickness in this way can be used to avoid initial overclosures in some situations. Abaqus/Explicit will automatically adjust surface positions to resolve initial overclosures . However, if nodal position adjustments are undesirable (for example, if they would introduce an imperfection in an otherwise flat part, resulting in an unrealistic buckling mode), you may prefer to reduce the surface thickness and avoid the overclosures entirely. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=THICKNESS surface, value or label, scale_factor If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Shell/Membrane thickness assignments: Edit: Select surface, click the arrows to transfer surface to list of thickness assignments, and enter a Scale Factor. Abaqus/CAE Usage: Surface offset A surface offset is the distance between the midplane of a thin body and its reference plane (defined by the nodal coordinates and element connectivities). It is computed by multiplying the offset fraction (specified as a fraction of the surface thickness) by the surface thickness and the element facet normal. This defines the position of the midsurface and, thus, the position of the body with respect to the reference surface; the coordinates of the nodes on the reference surface are not modified. Surface offsets can be specified only for surfaces defined on shell and similar elements (i.e., membrane, rigid, and surface elements). Surface offsets specified for other elements (e.g., solid or beam elements) will be ignored. By default, surface offsets specified in element section definitions will be used in the general contact algorithm. The surface offset at each node is the average of the maximum and minimum offsets among the faces connected to the node. The offset at a point within a facet is interpolated from the nodal values. At complex intersections (edges connected to more than two faces) the surface offset is set to zero. Figure 35.4.2–3 shows some examples of the positioning of the contact surface with respect to the reference surface for various combinations of surface offsets. Surface offsets used in the general contact algorithm are constrained to lie between −0.5 and 0.5 of the thickness. You specify the surface offset as a fraction of the surface thickness. The surface offset fraction can be set equal to the offset fraction used for the surface’s parent elements or to a specified value. Surface offsets specified for general contact do not change the element integration. midsurface = reference surface thickness offset fraction = 0.0 at the horizontal and tilted surfaces reference surface midsurface reference surface midsurface element normals offset fraction = 0.5 at the horizontal and tilted surfaces offset fraction = 0.5 at the horizontal surface offset fraction = 0.0 at the tilted surface (assumed that linear elements are used) Figure 35.4.2–3 Specifying surface offsets for general contact. Input File Usage: Use the following option to use the surface offset fraction from the surface’s parent elements (default): *SURFACE PROPERTY ASSIGNMENT, PROPERTY=OFFSET FRACTION surface, ORIGINAL Use the following option to specify a value for the surface offset fraction: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=OFFSET FRACTION surface, offset The offset can be specified as a value or a label (SPOS or SNEG). Specifying SPOS is equivalent to specifying a value of 0.5; specifying SNEG is equivalent to specifying a value of −0.5. Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Shell/Membrane offset assignments: Edit: Select surface, and click the arrows to transfer surface to list of offset assignments. In the Offset Fraction column, enter ORIGINAL to use the surface offset fraction from the surface's parent elements, enter SPOS to use a surface offset fraction of 0.5, enter SNEG to use a surface offset fraction of −0.5, or enter a value for the surface offset fraction. Feature edges Feature edges of a model are defined on beam and truss elements and edges of faces (perimeter and otherwise) of solid and structural elements. By default, edge-to-edge contact in the general contact algorithm in Abaqus/Explicit accounts for perimeter edges as well as “contact edges” of beam and truss elements. You can control which feature edges should be activated in the general contact domain by specifying feature edge criteria. By default, only perimeter edges are activated. Feature edge criteria have no effect on “edges” of beam and truss elements—they are activated by their inclusion in the contact domain. The feature angle The feature angle is the angle formed between the normals of the two facets connected to an edge. The angles between facets are based on the initial configuration. A negative angle will result at concave meetings of facets; therefore, these edges are never included in the contact domain. Figure 35.4.2–4 shows some examples of how the feature angle is calculated for different edges. (+) n2 n1 n2 n2 n3 ( )_ 25o n3 n1 ( )_ n5 n4 n5 n4 n7 D (perimeter edge) n5 (+) 180 n7 n6 0o n II n Figure 35.4.2–4 Calculating the feature angle. The feature angle for edge A is 90° (the angle between (the angle between in Figure 35.4.2–5); its feature angles are 0°, −90°, and −90°. ); the feature angle for edge B is −25° ). Edge C forms a T-intersection with three facets (shown in two dimensions and and _ 90o _ 90o arrows are perpendicular to surface facets Figure 35.4.2–5 Feature angles for a T-intersection (for example, edge C in Figure 35.4.2–4). Perimeter edges (for example, edge D in Figure 35.4.2–4) can be thought of as a special type of feature edge where the feature angle is 180°. The sign of the feature angle is considered when determining whether or not a geometric feature edge should be activated in the general contact domain. For example, if a cutoff feature angle of 20° were specified, edge A would be activated as a feature edge in the contact model (90° > 20°) but edges B and C would not be activated: −25° < 20° and 0° (the maximum feature angle for edge C) < 20°. Figure 35.4.2–6 illustrates further how the feature angle is used to determine which geometric feature edges should be activated in the general contact domain. Thin solid lines indicate feature edges. Thick solid lines indicate shell perimeter edges. Edge Largest feature angle at edge Other feature angles at edge Shells Solid Dashed lines indicate element boundaries for which edge-to-edge contact is not modeled. approximately +105 o approximately 30 _ o o 0 +180 o o +90 o 0 none none _ 90 o none _ o 90 _ _ o o 90 , 90 Figure 35.4.2–6 Feature edges activated in the general contact domain for a cutoff feature angle of 20°. The table to the right of the figure lists the feature angle values for various edges in the model. Edges connected to more than two facets, as well as edges connected to two shell facets, have more than one corresponding feature angle. The largest feature angle at an edge is compared to the specified cutoff feature angle. For example, if a cutoff feature angle of 20° were specified, edges A, D, and E would be considered feature edges, while edges B, C, and F would be ignored for edge-to-edge contact. Specifying that only perimeter edges should be activated By default, only perimeter edges are included in the general contact domain. Perimeter edges occur on “physical” perimeters of shell elements and on “artificial” edges that occur when a subset of exposed facets on a body are included in the general contact domain. When structural elements share nodes with continuum elements, the perimeter edges will not be activated on the structural elements because the criterion to designate them as such is no longer satisfied. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, PERIMETER EDGES (default) Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Feature edge criteria assignments: Edit: Select surface, click the arrows to transfer surface to list of feature assignments, and enter PERIMETER in the Feature Edge Criteria column. Specifying particular feature edges to be activated You can choose particular feature edges on surface, structural, and rigid elements to be activated in domain. A surface containing a list of element labels and edge identifiers is used to specify the edges to activate. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, PICKED EDGES Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Feature edge criteria assignments: Edit: Select the surface, click the arrows to transfer the surface to the list of feature assignments, and enter PICKED in the Feature Edge Criteria column. Specifying that all feature edges should be activated You can choose to activate all edges in a given surface in the general contact domain. This will activate all edges of every face specified in the given surface. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, ALL EDGES Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Feature edge criteria assignments: Edit: Select the surface, click the arrows to transfer the surface to the list of feature assignments, and enter ALL in the Feature Edge Criteria column. Specifying that all feature edges should be deactivated You can choose to deactivate all feature edges (including perimeter edges) in the general contact domain. This option does not deactivate “contact edges” associated with beam and truss elements. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, NO FEATURE EDGES Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Feature edge criteria assignments: Edit: Select the surface, click the arrows to transfer the surface to the list of feature assignments, and enter NONE in the Feature Edge Criteria column. Specifying a cutoff feature angle If you specify a cutoff feature angle as the feature edge criteria, perimeter edges and geometric edges with feature angles greater than or equal to the specified angle are activated in the general contact domain. As described previously, you can activate additional feature edges if needed. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, feature_angle_value Abaqus/CAE Usage: If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Feature edge criteria assignments: Edit: Select surface, click the arrows to transfer surface to list of feature assignments, and enter a value for the cutoff feature angle (in degrees) in the Feature Edge Criteria column. Example: assigning different feature edge criteria to different regions You can assign a different feature edge criteria to different regions of the general contact domain. For example, the input shown in the following table could be used to specify that none of the feature edges of surf1, only perimeter edges of surf2, and perimeter edges and feature edges of surf3 with a feature angle greater than 30° should be considered for edge-to-edge contact: Input File Syntax Abaqus/CAE Syntax surf1, NO FEATURE EDGES Surface: surf1, Feature Edge Criteria: NONE surf2, PERIMETER EDGES Surface: surf2, Feature Edge Criteria: PERIMETER surf3, 30 Surface: surf3, Feature Edge Criteria: 30 Primary and secondary feature edges To cut down on the computational cost in certain situations, it may be desirable to identify a limited number of feature edges on a surface (presumably at locations where there are sharp gradients in the surface normals) as “primary” feature edges. A more relaxed criterion can be used to denote certain other edges on the surface as “secondary” feature edges. If secondary feature edges are specified in addition to primary feature edges, Abaqus/Explicit enforces edge-to-edge contact between primary feature edges and between primary feature edges and secondary feature edges only. Edge-to-edge contact is not enforced between secondary feature edges. This ensures that interpenetrations are avoided at locations where there are “true” edges in the model, without the need to activate primary feature edges at locations where the gradients in the surface normals are only moderate. A judicious choice of criteria for selecting primary and secondary feature edges can lead to significant savings in computational costs. Secondary feature edges can be selected for a surface by specifying a secondary feature edge criterion in addition to the criterion used to select the primary feature edges for that surface. If the secondary feature edge criterion is omitted, only primary feature edges are activated for the surface. Allowable criteria for secondary feature edges are: • all edges that have not been selected as primary feature edges; • all picked edges that have not been selected as primary feature edges; • all perimeter edges that have not been selected as primary feature edges; and • all edges with a feature angle greater than a specified cutoff angle value that have not been selected as primary feature edges. The allowable values for the secondary feature edge criterion permit possible combinations of criteria for primary feature edges and secondary feature edges, shown in Table 35.4.2–3. Table 35.4.2–3 Valid combinations of primary feature edge and secondary feature edge criteria. Primary Feature Edge Criterion Secondary Feature Edge Criterion No feature edges All edges All remaining edges, picked edges, perimeter edges, cutoff angle Any criterion specified for secondary feature edges will be ignored Primary Feature Edge Criterion Secondary Feature Edge Criterion Picked edges Perimeter edges Cutoff angle All remaining edges, perimeter edges, cutoff angle All remaining edges, picked edges, cutoff angle All remaining edges, picked edges, perimeter edges, cutoff angle Specifying all remaining edges as secondary feature edges You can specify that all edges belonging to the surface that have not been selected as primary feature edges become secondary feature edges. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, primary feature edge criterion, ALL REMAINING EDGES If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Abaqus/CAE Usage: Secondary feature edges are not supported in Abaqus/CAE. Specifying picked edges as secondary feature edges You can specify that all picked edges of the surface that have not already been selected as primary feature edges become secondary feature edges. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, primary feature edge criterion, PICKED EDGES If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Abaqus/CAE Usage: Secondary feature edges are not supported in Abaqus/CAE. Specifying perimeter edges as secondary feature edges You can specify that all perimeter edges of the surface that have not already been selected as primary feature edges become secondary feature edges. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, primary feature edge criterion, PERIMETER EDGES If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Abaqus/CAE Usage: Secondary feature edges are not supported in Abaqus/CAE. Specifying a cutoff feature angle for secondary feature edges You can specify that edges on the surface with a feature angle greater than the specified value that have not been selected as primary feature edges become secondary feature edges. If an angle value has also been specified for primary feature edges, the angle value specified for secondary feature edges must be smaller than the value specified for primary edges. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, primary feature edge criterion, feature_angle_value If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Abaqus/CAE Usage: Secondary feature edges are not supported in Abaqus/CAE. Specifying that edges are activated only as secondary feature edges For a particular surface you may not want to activate any primary feature edges; instead, you might want to activate all or some edges on the surface as secondary feature edges (to enforce contact between these secondary feature edges and primary feature edges on another surface in the model). In that case you can specify that no feature edges should be activated as the primary feature edge criterion for the surface, while using any criterion of choice for the secondary feature edges. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=FEATURE EDGE CRITERIA surface, NO FEATURE EDGES, secondary feature edge criterion If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Abaqus/CAE Usage: Secondary feature edges are not supported in Abaqus/CAE. Surface geometry correction By default, contact calculations are based on unsmoothed, faceted representations of the finite element surfaces in a general contact domain. Discrepancies between the true surface geometry and the faceted surface geometry may result in significant noise in the solution. Optional contact smoothing techniques simulate a more realistic representation of curved surfaces in the contact calculations. These techniques allow a discretized surface with discontinuous surface normals to more closely approximate the behavior of a smooth surface during an analysis. Improvements to results with the surface correction include more accurate contact stresses and less solution noise upon relative sliding between contact surfaces. Contact smoothing can be specified for surfaces in a general contact domain using a surface property assignment. A single surface property assignment specifies all of the surfaces to be smoothed, as well as the appropriate geometry correction method for each surface. Three geometry correction methods can be employed: • The circumferential smoothing method is applicable to surfaces approximating a portion of a surface of revolution. • The spherical smoothing method is applicable to surfaces approximating a portion of a sphere. • The toroidal smoothing method is applicable to surfaces approximating a portion of a torus (i.e., a circular arc revolved about an axis). For each surface, you must specify the appropriate geometry correction method and either the approximate axis of revolution (for circumferential or toroidal smoothing) or the approximate spherical center (for spherical smoothing). For toroidal smoothing, you must also specify the distance of the center of the circular arc from the axis of revolution, and the line joining point (Xa , Ya , Za ) and the center of the circular arc should be perpendicular to the axis of revolution. Input File Usage: Use the following option to apply a geometric correction: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=GEOMETRIC CORRECTION data lines to define smoothing regions Use the following data line to apply circumferential smoothing to a surface with an axis of symmetry passing through points (Xa , Ya , Za ) and (Xb , Yb, Zb ): surface, CIRCUMFERENTIAL, Xa , Ya, Za , Xb , Yb , Zb Use the following data line to apply spherical smoothing to a surface with a spherical center at point (Xa , Ya , Za ): surface, SPHERICAL, Xa, Ya , Za Use the following data line to apply toroidal smoothing to a surface with an axis of symmetry passing through points (Xa , Ya , Za ) and (Xb , Yb, Zb ) with the center of the revolved circular arc at a distance R from the axis of symmetry: surface, TOROIDAL, Xa , Ya, Za , Xb , Yb , Zb, R Repeat the data lines as many times as necessary to define the appropriate geometry corrections for all surfaces in the contact domain. Contact surface smoothing can be applied only to native geometry models in Abaqus/CAE. Abaqus/CAE can automatically detect all circumferential and spherical surfaces in the general contact domain that can be smoothed and apply the appropriate smoothing. Use the following option to enable automatic surface smoothing of a model: Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Surface smoothing assignments: Edit: toggle on Automatically assign smoothing for geometric faces 35.4.2–15 Use the following option to manually apply smoothing to a surface: Interaction module: Create Interaction: General contact (Explicit): Surface Properties: Surface smoothing assignments: Edit: Select the surface, click the arrows to transfer the surface to the list of smoothing assignments. In the Smoothing Option column, select REVOLUTION to apply circumferential smoothing, select SPHERICAL to apply spherical smoothing, or select NONE to prevent smoothing of the surface. Toroidal surface smoothing cannot be defined in Abaqus/CAE. Considerations for geometric correction The contact smoothing technique assumes that the initial locations of the surface nodes lie on the true initial surface geometry, with the exception of midedge nodes of C3D10M elements. This smoothing technique remains effective even if the midedge nodes of C3D10M elements do not lie on the true initial geometry (models meshed using Abaqus/CAE always have midedge nodes placed on the true initial geometry, but this may not be the case with other meshing preprocessors). The effects of contact smoothing tend to be most significant for analyses involving small deformation, and the smoothing technique works well for cases involving large relative motion between the surfaces. For analyses with large deformation this smoothing technique typically has an insignificant effect on the solution. However, in some cases—especially where the underlying elements can fail—the smoothing can degrade the solution accuracy after large deformation. Effects of geometric correction The impact of contact surface smoothing can be demonstrated by a simple model of contact between concentric cylinders with a small clearance between them. With a matched mesh as shown in Figure 35.4.2–7 there are no initial overclosures; there are no initial strain-free initial displacement adjustments. However, if the inner cylinder is rotated, the cylinders develop stresses as contact is detected due to the linear faceted representation of the master surface. This behavior is improved when the circumferential smoothing technique is applied to the contacting surfaces of the two cylinders. therefore, Figure 35.4.2–7 Concentric cylinders with matched mesh. S, Mises (Avg: 75%) +8.165e+02 +7.487e+02 +6.809e+02 +6.131e+02 +5.453e+02 +4.775e+02 +4.097e+02 +3.419e+02 +2.741e+02 +2.063e+02 +1.385e+02 +7.071e+01 +2.905e+00 Figure 35.4.2–8 Stesses as cylinder rotates. 35.4.3 ASSIGNING CONTACT PROPERTIES FOR GENERAL CONTACT IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1 • “Mechanical contact properties: overview,” Section 36.1.1 • “Contact pressure-overclosure relationships,” Section 36.1.2 • “Contact damping,” Section 36.1.3 • “Frictional behavior,” Section 36.1.5 • *CONTACT • *CONTACT PROPERTY ASSIGNMENT • *SURFACE INTERACTION • “Specifying and modifying contact property assignments for general contact,” Section 15.13.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Contact properties: • define the mechanical surface interaction models that govern the behavior of surfaces when they are in contact; and • can be applied selectively to particular regions within a general contact domain. Assigning contact properties The default contact property model in Abaqus/Explicit assumes “hard” contact in the normal direction, no friction, no thermal interactions, etc. You can assign a nondefault contact property definition (surface interaction) to specified regions of the general contact domain. Contact property assignments propagate through all analysis steps in which the general contact interaction is active. The surface names used to specify the regions where nondefault contact properties should be assigned do not have to correspond to the surface names used to specify the general contact domain. In many cases the contact interaction will be defined for a large domain, while nondefault contact properties will be assigned to a subset of this domain. Any contact property assignments for regions that fall outside of the general contact domain will be ignored. The last assignment will take precedence if the specified regions overlap. Input File Usage: *CONTACT PROPERTY ASSIGNMENT surface_1, surface_2, interaction_property_name This option must be used in conjunction with the *CONTACT option. It should appear at most once per step; the data line can be repeated as often as necessary to assign contact properties to different regions. If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted or is the same as the first surface name, contact between the first surface and itself is assumed. Keep in mind that surfaces can be defined to span multiple unattached bodies, so self-contact is not limited to contact of a single body with itself. If the interaction property name is omitted, the unnamed set of default contact properties in Abaqus/Explicit is assumed. If an interaction property name is specified, it must also appear as the value of the NAME parameter on a *SURFACE INTERACTION option in the model portion of the input file. Interaction module: Create Interaction: General contact (Explicit): Contact Properties: Individual property assignments: Edit: select the surfaces and the contact property in the columns on the left, and click the arrows in the middle to transfer them to the list of contact property assignments or Global property assignment: interaction_property_name In Abaqus/CAE you must assign a contact property definition to every general contact interaction; Abaqus/CAE does not assume a default contact interaction property. Abaqus/CAE Usage: Example The following contact property assignments are specified below for the first step in a general contact analysis: • a global assignment of contProp1 to the entire general contact domain; • a local assignment of contProp2 to self-contact for surf1; • a local assignment of the default Abaqus contact property to contact between surf2 and surf3; and • a local assignment of contProp3 to contact between the entire contact domain and surf4. *SURFACE INTERACTION, NAME=contProp1 *FRICTION 0.1 *SURFACE INTERACTION, NAME=contProp2 *FRICTION 0.15 *SURFACE INTERACTION, NAME=contProp3 *FRICTION 0.20 *STEP Step1 *DYNAMIC, EXPLICIT … *CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR *CONTACT PROPERTY ASSIGNMENT , , contProp1 surf1, surf1, contProp2 surf2, surf3, , surf4, contProp3 Changing contact properties Contact property models for general contact interactions are independent of the steps in which they are used and cannot be modified from step to step. To change the contact properties used in a given step, you must specify a new contact property assignment that refers to a different contact property model. Example For example, the following input could be used to change the friction coefficient used for contact between the entire general contact domain and surf4 in the second step of the analysis started in the previous example: *STEP Step2 *DYNAMIC, EXPLICIT … *CONTACT *CONTACT PROPERTY ASSIGNMENT , surf4, contProp2 35.4.4 CONTROLLING INITIAL CONTACT STATUS FOR GENERAL CONTACT IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1 • *CONTACT • *CONTACT CLEARANCE • *CONTACT CLEARANCE ASSIGNMENT • “Producing a deformed shape plot,” Section 43.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Initial clearances for surface interactions included in the general contact domain: • are set to zero automatically for small initial overclosures (e.g., for small penetrations caused by numerical roundoff when a graphical preprocessor such as Abaqus/CAE is used); • can be specified to resolve large initial overclosures that are not resolved automatically; • can be specified to separate entangled double-sided surfaces; • can be specified to model an initial gap between surfaces; • are enforced without creating any strains or momentum in the model; • should not be specified to correct gross errors in the mesh design; and • can be used to identify an initially bonded node set in crack propagation analyses. Default adjustments for initial overclosures in the first step of the simulation Abaqus/Explicit automatically adjusts the positions of surfaces to remove small initial overclosures that exist in the general contact domain in the first step of a simulation. The adjustments are made with strain-free initial displacements. This automatic adjustment of surface position is intended to correct only minor mismatches associated with mesh generation and is done even when the interaction is defined through user subroutine VUINTERACTION. Conflicting adjustments from separate contacts, boundary conditions, tie constraints, coupling constraints, and rigid body constraints can cause incomplete resolution of initial overclosures. This can occur, for example, when a slave node is pinched between two master facets. Initial overclosures that are not resolved by repositioning nodes are stored as temporary contact offsets to avoid large contact forces at the beginning of an analysis. The penalty contact force is computed as ; where k is the penalty stiffness, is the current penetration distance. If is the initial unresolved penetration distance, and ever decreases below , is reset to . Because of the lack of a unique outward direction from double-sided facets, the resolution of large initial penetrations for double-sided surfaces can be difficult. Initial penetration will be detected only when a slave node lies within the thickness of the underlying element, and the initial penetration will be resolved by moving the slave node to the nearest free surface as shown in Figure 35.4.4–1. corrected position of slave node original position of slave node master surface thickness master node Figure 35.4.4–1 Correction of initial overclosure for contact involving two double-sided surfaces. Slave nodes that are trapped on opposite sides of a double-sided master surface will often lead to serious problems, which may not become apparent until later in the analysis. Surfaces that are initially crossed often indicate a modeling problem for single-sided surfaces as well, because the initial search for slave nodes in the interior of solids is limited to a distance of about 15% of the facet dimensions; slave nodes more deeply penetrated than this are ignored by the algorithm to adjust initial overclosures. Initial overclosure information—including node adjustment data, contact offsets, crossed surfaces, nodes that could not be corrected, and any warnings—is written to the status (.sta) file, the message (.msg) file, and the output database (.odb) file. The default tolerance used to report gross initial penetrations, which could indicate an error with your model definition, depends on the contact type. Node-to-surface contact uses the characteristic length of the contact facet, edge-to-edge contact uses the length of the tracked edge, and the typical element dimension is used for node-to-analytical rigid surface contact. For more information on the overclosure warnings, see “Contact diagnostics in an Abaqus/Explicit analysis,” Section 38.2.1, and Chapter 41, “Viewing diagnostic output,” of the Abaqus/CAE User’s Manual. Default adjustments of overclosed surfaces during subsequent steps in the simulation Initial penetrations are stored as temporary contact offsets that do not generate contact forces in the following cases: • If the general contact domain is created in steps other than the first step (i.e., the contact definition follows a step in which no contact was defined) or • if an Abaqus/Standard analysis is imported into Abaqus/Explicit and the contact interaction is not defined with user subroutine VUINTERACTION. However, deep penetrations may not be treated correctly; they may be ignored or, in the case of penetrations past the midsurface of shells, the wrong contact directions may be used. Initial overclosure and crossed surface diagnostics can be requested to diagnose these problems . If the general contact domain is extended after the first step, Abaqus/Explicit does not take any special actions to gradually resolve initial penetrations for the newly introduced interactions: penalty contact forces will be applied proportional to the penetration, or the penetration may be ignored. In addition, initial overclosure and crossed surface diagnostics are not available for these new interactions. Specifying initial clearances and controlling initial overclosure adjustments In some cases the default algorithm will not correctly resolve initial overclosures, or a precise initial gap (i.e., a positive clearance) between surfaces may need to be modeled. Specifically, deep penetrations may be ignored, tangled double-sided surfaces may not be separated correctly , and gaps between curved surfaces in the discretized model may be inconsistent with the non-discretized model. To resolve these issues, you can define contact clearances and assign them to contact interactions. Examples are given below. Defining contact clearances You must assign a name to each contact clearance definition that is used to associate the clearance definition with a contact interaction. Input File Usage: Abaqus/CAE Usage: *CONTACT CLEARANCE, NAME=clearance_name Contact clearances for general contact are not supported in Abaqus/CAE. Applying contact clearances by adjusting the nodal coordinates or by creating contact offsets Clearances are applied to the model by adjusting the nodal coordinates or by creating contact offsets. By default, contact clearances are resolved by adjusting the nodal coordinates without creating strain or momentum in the model (this method can be used only in the first step of an analysis). Alternatively, contact offsets can be created for clearance specifications. These offsets are permanent (as opposed to temporary offsets created during the default initial overclosure resolution procedure) and are not ramped to zero as the surfaces separate. Contact offsets will also be created for clearances specified via nodal adjustments if the clearance violations cannot be resolved due to conflicting adjustments from separate contacts, boundary conditions, tie constraints, coupling constraints or rigid body constraints. Clearances can be applied via contact offsets in steps in which the whole contact domain is newly defined (i.e., no contact was defined in the previous step) and in the first step of an import analysis. Input File Usage: Use the following option to apply contact clearances by adjusting the nodal coordinates (default): *CONTACT CLEARANCE, NAME=clearance_name, ADJUST=YES Abaqus/CAE Usage: Use the following option to apply contact clearances by creating contact offsets: *CONTACT CLEARANCE, NAME=clearance_name, ADJUST=NO Contact clearances for general contact are not supported in Abaqus/CAE. Setting the value of the initial clearance You can define the clearance as a single value for the whole interaction or as a nodal distribution to define a clearance per slave node . If a distribution is defined and the clearance is omitted for a slave node, the clearance value will be interpolated from the values at the master nodes. The slave node will be ignored if clearance values are specified for neither the slave node nor all of the nodes of the nearest master face. The clearance values must be non-negative for slave nodes on solid element surfaces. The default value is 0.0 if a value or distribution is not given. Input File Usage: *CONTACT CLEARANCE, NAME=clearance_name, CLEARANCE=value or distribution_name Abaqus/CAE Usage: Contact clearances for general contact are not supported in Abaqus/CAE. Defining search zones You can specify search distances to define “zones” above and below the surfaces. Slave nodes that lie within these zones will be given the specified clearance values with respect to their closest master faces by pulling them closer or pushing them farther away, regardless of their initial positions (overclosure or initial gap bigger than the clearance defined). Nodes whose closest point is a perimeter edge will be excluded from the clearance specification. The default value for each search distance for solid elements is approximately one-tenth of the element size of the elements attached to the slave node. The default value for each search distance for structural elements (e.g., shell elements) is the thickness associated with the slave node. Input File Usage: Abaqus/CAE Usage: Defining a search node set *CONTACT CLEARANCE, NAME=clearance_name, SEARCH ABOVE=value, SEARCH BELOW=value Contact clearances for general contact are not supported in Abaqus/CAE. As an alternative to specifying search distances, you can specify a search node set, containing the slave nodes for which clearance has been defined. Slave nodes that belong to this node set will be given the specified clearance values with respect to their closest master faces by pulling them closer or pushing them farther away, regardless of their initial positions (overclosure or initial gap bigger than the clearance defined). If a search node set has been specified, no clearance will be applied to slave nodes that do not belong to the specified search node set. When a search node set is specified, there is a default search distance value associated with the maximum element size for solid elements or the thickness for structural elements (e.g., shell elements) associated with the nodes. The position of any node beyond the search distance is not adjusted. Input File Usage: *CONTACT CLEARANCE, NAME=clearance_name, SEARCH NSET=node set name Abaqus/CAE Usage: Contact clearances for general contact are not supported in Abaqus/CAE. Assigning contact clearances to contact interactions You can assign initial clearance definitions to node-to-face interactions (except self-contact interactions) in the general contact domain. Initial clearance definitions cannot be assigned to node-to-analytical rigid surface interactions. For node-to-face interactions, the clearances defined between two surfaces apply to the interaction between the slave nodes in each surface and the whole of the other surface. When nodal adjustments are used to resolve clearance violations, the adjustments are made to satisfy the clearance specification with respect to each slave node’s nearest master face in the initial configuration. Contact offsets are set to the value of the clearance violation between each slave node and its nearest master face in the initial configuration, and the slave nodes are then offset by that value with respect to the whole of the other surface during the analysis. The surfaces specified must be single-sided and cannot contain complex intersections of faces (i.e., an edge cannot be connected to more than two faces) or discontinuous normals. Surfaces defined on solid elements will satisfy these requirements automatically. These restrictions arise from the definition of a clearance for surfaces on double-sided elements: a node has a positive (negative) clearance with respect to a surface if it is above (below) the surface as defined by the surface normal . A negative clearance of a node with respect to a surface on double-sided elements does not indicate a state of penetration, but rather that the node has a gap with the other side of the elements underlying the surface. topsurf negative clearance with respect to topsurf botsurf positive clearance with respect to botsurf Figure 35.4.4–2 Contact clearance sign convention for double-sided elements. By default, clearances are applied to all master-slave views of the surface pair that exist in the contact domain. In addition, if clearances between two element-based surfaces are specified to be resolved via nodal adjustments, the nodal adjustment procedure can be directed to perform the adjustments for one master-slave view of the surface pair (this applies only to the nodal adjustment procedure and does not apply to the contact formulation used between the surfaces during the analysis). Input File Usage: Use the following option to specify clearances for all master-slave views of the given surface pair (default): *CONTACT CLEARANCE ASSIGNMENT surface_1, surface_2, clearance_name Use the following option to specify clearances between the nodes of the second surface and the faces of the first surface (the first surface is treated as the master surface): *CONTACT CLEARANCE ASSIGNMENT surface_1, surface_2, clearance_name, MASTER Use the following option to specify clearances between the nodes of the first surface and the faces of the second surface (the first surface is treated as the slave surface): *CONTACT CLEARANCE ASSIGNMENT surface_1, surface_2, clearance_name, SLAVE Abaqus/CAE Usage: Contact clearances for general contact are not supported in Abaqus/CAE. Examples The default algorithm to resolve initial overclosures does not detect penetrations of solid element surfaces that are greater than approximately 15% of the dimension of facets attached to the slave node. Figure 35.4.4–3 shows two solid elements with large initial penetrations that will not be detected during the default initial overclosure resolution procedure. initial overclosures detected in this zone only surf1 surf2 0.2 Figure 35.4.4–3 Undetected large penetrations of solid elements. A zero clearance can be defined explicitly for the overclosed portions of this model to resolve the initial overclosures. Define the clearance definition as follows: *CONTACT CLEARANCE, NAME=c1, ADJUST=YES, SEARCH BELOW=0.2 SEARCH ABOVE=0.0 and assign it to the interaction between surf1 and surf2: *CONTACT *CONTACT CLEARANCE ASSIGNMENT surf1, surf2, c1 The resulting adjustment is shown in Figure 35.4.4–4. Adjusting the nodal coordinates may degrade the mesh geometry by creating imperfections that were not initially present, may reduce the element size and correspondingly the stable time increment size, or may cause elements to invert and prevent the analysis from continuing. In such cases it is preferable to bypass the nodal coordinate adjustments and specify the storage of a contact offset. initial position adjusted position Figure 35.4.4–4 Resolution of large penetrations of solid elements. The initial overclosure adjustment algorithm must also be directed to separate entangled double-sided surfaces. Figure 35.4.4–1 shows the default adjustments made for entangled shell surfaces assuming the nodes of surf3 have fixed boundary conditions. Figure 35.4.4–5 shows the adjustments made from the following clearance definition and assignment: *CONTACT CLEARANCE, NAME=c2, ADJUST=YES, SEARCH BELOW=1.5, SEARCH ABOVE=0.0 ... *CONTACT *CONTACT CLEARANCE ASSIGNMENT surf3, surf4, c2 If the nodes of surf3 are not fixed, the clearance interaction can be set to pure master-slave (with surf3 defined as the master) to prevent the geometry of surf3 from being modified. In cases where the geometry of the mesh is important or if nodal adjustments conflict, contact offsets should be created. Conflicting nodal adjustments are a common problem when specifying clearances via nodal adjustment for curved surfaces with a balanced master-slave interaction. Adjustments of nodes tend to change the curvature of curved surfaces because the clearance “constraint” can be satisfied only corrected position of surf4 single-sided surface surf3 (fixed) thickness =1.0 original position of surf4 Figure 35.4.4–5 Separation of tangled double-sided surfaces. if the surface meshes are coincident (and a zero clearance is specified) or if the surfaces are flat . Figure 35.4.4–6 Specifying a uniform initial gap between concentric circular surfaces. Identifying potentially partially bonded surfaces You can specify a search node set to identify which slave nodes will be tagged as initially bonded in a VCCT crack propagation analysis. See “Crack propagation analysis,” Section 11.4.3, for more details. Input File Usage: Use the following options: *CONTACT CLEARANCE, NAME=clearance_name, SEARCH NSET=node set name *CONTACT CLEARANCE ASSIGNMENT surface_1, surface_2, clearance_name 35.4.5 CONTACT CONTROLS FOR GENERAL CONTACT IN Abaqus/Explicit Product: Abaqus/Explicit References • “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1 • “Assigning surface properties for contact pairs in Abaqus/Explicit,” Section 35.5.2 • *CONTACT • *CONTACT CONTROLS ASSIGNMENT Overview Contact controls for the general contact algorithm: • can be used to selectively scale the default penalty stiffness for particular regions within a general contact domain; • can be used to control whether nodes are removed from the general contact domain once all of the faces and edges to which they are attached have eroded; • can be used to activate a nondefault tracking algorithm for node-to-face contact in particular regions within a general contact domain; • can be used to control whether checks need to be performed to prevent folds in general contact surfaces from inverting on themselves; • can be used to modify the default initial overclosure resolution method for one or more pairs of surfaces in the general contact domain; and • can be used to modify the default contact thickness reduction checks. Scaling default penalty stiffnesses The general contact algorithm uses a penalty method to enforce the contact constraints . The “spring” stiffness that relates the contact force to the penetration distance is chosen automatically by Abaqus/Explicit, such that the effect on the time increment is minimal yet the allowed penetration is not significant in most analyses. Significant penetrations may develop in an analysis if any of the following factors are present: • Displacement-controlled loading • Materials at the contact interface that are purely elastic or stiffen with deformation • Deformable elements (especially membrane and surface elements) that have relatively little mass of their own and are constrained via methods other than boundary conditions (for example, connectors) involved in contact • Rigid bodies that have relatively little mass or rotary inertia of their own and are constrained via methods other than boundary conditions (for example, connectors) involved in contact See “The Hertz contact problem,” Section 1.1.11 of the Abaqus Benchmarks Manual, for an example in which the first two of these factors combine such that the contact penetrations with the default penalty stiffness are significant. You can specify a scale factor by which to modify penalty stiffnesses for specified interactions within the general contact domain. This scaling may affect the automatic time incrementation. Use of a large scale factor is likely to increase the computational time required for an analysis because of the reduction in the time increment that is necessary to maintain numerical stability . The user-specified (variable) mass scaling does not take into account the effect of contact when it computes the necessary increase of mass. In general, this effect is not significant as the default penalty stiffness will decrease the stable time increment only by very small amounts. However, if high penalty scale factors are specified, the stable time increment could be reduced significantly despite the specified mass scaling. The surface names used to specify the regions where nondefault penalty stiffness should be assigned do not have to correspond to the surface names used to specify the general contact domain. In many cases the contact interaction will be defined for a large domain, while a nondefault penalty stiffness will be assigned to a subset of this domain. If the surfaces to which a nondefault penalty stiffness is assigned fall outside the general contact domain, the controls assignment will be ignored. The last assignment will take precedence if the specified regions overlap. Input File Usage: *CONTACT CONTROLS ASSIGNMENT, TYPE=SCALE PENALTY surface_1, surface_2, scale_factor This option must be used in conjunction with the *CONTACT option. It should appear at most once per step; the data line can be repeated as often as necessary to assign penalty stiffness scale factors to different regions. If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted or is the same as the first surface name, the specified contact controls are assigned to contact interactions between the first surface and itself. Keep in mind that surfaces can be defined to span multiple unattached bodies, so self-contact is not limited to contact of a single body with itself. Control of nodal erosion You can control whether contact nodes remain in the contact domain after all the surrounding faces and edges have eroded due to element failure. By default, these nodes remain in the contact domain and act as free-floating point masses that can experience contact with faces that are still part of the contact domain. You can specify that nodes of element-based surfaces should erode (i.e., be removed from the contact domain) once all contact faces and contact edges to which they are attached have eroded. Nodes that you include in the contact domain only with node-based surfaces are never removed from the contact domain. Computational cost can increase as a result of free-flying nodes if nodal erosion is not specified, particularly for analyses conducted in parallel. The increased computational cost is related to the likelihood of free-flying nodes moving far away from the elements that remain active, which stretches the volume of the contact domain and thereby tends to increase contact search costs as well as the cost of communication between processors in parallel analysis. However, contact involving free-flying nodes can contribute significant momentum transfer in some cases, which will not be accounted for if nodal erosion is specified. Input File Usage: *CONTACT CONTROLS ASSIGNMENT, NODAL EROSION=NO This option must be used in conjunction with the *CONTACT option. This parameter setting applies to the entire general contact domain. Activating the nondefault tracking algorithm for node-to-face contact A nondefault contact tracking algorithm is available that utilizes more local topological and geometric information in tracking contact between nodes and faces. This algorithm may lead to more robust contact tracking in certain modeling situations, for instance during the inflation event of a folded air-bag. The tracking algorithm is activated on a surface-by-surface basis. You must specify the surface name for which the tracking algorithm needs to be activated. All contact interactions in the contact domain in which nodes of the specified surface contact faces belonging to either the surface itself (self- contact) or faces belonging to any other surface (for which node-to-face contact has not been excluded) will be tracked using the nondefault node-to-face tracking scheme. The surface names used to specify the regions where the nondefault tracking algorithm should be used do not have to correspond to the surface names used to specify the general contact domain. In many cases the contact interaction will be defined for a large domain, while the nondefault tracking algorithm will be assigned to a subset of this domain. If the surfaces for which the nondefault tracking algorithm needs to be activated fall outside the general contact domain, the controls assignment is ignored. Input File Usage: *CONTACT CONTROLS ASSIGNMENT, TYPE=FOLD TRACKING surface_1 This option must be used in conjunction with the *CONTACT option. It should appear at most once per step; the data line can be repeated as often as necessary to activate the nondefault tracking algorithm in different regions of the contact domain. If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Activating the fold inversion check If a general contact surface contains sharp folds, significant loading events (for example, those encountered during the inflation of a folded airbag) may cause one or more of the folds to invert. Inversion is most likely to occur at a fold where edge-to-edge contact has not been activated on the edges of the faces forming the fold. The presence of edge-to-edge constraints usually prevents a fold from inverting. Inversion of a fold, in the absence of edge-to-edge contact constraints, may induce errors in the node-to-face contact tracking algorithm and may result in a node that was being tracked on a face that forms part of an inverted fold getting “snagged” on the wrong side of the tracked face. To avoid such situations, it may be desirable to activate the fold inversion check for models containing sharp folds. The fold inversion check detects situations where a fold is about to invert and applies a force field to the faces forming the fold to prevent the fold from inverting. The fold inversion check is activated on a surface-by-surface basis. You must specify the surface name for which the fold inversion check needs to be activated. If activated for a particular surface, the fold inversion check applies to all folds within that surface. The surface names used to specify the regions where the fold inversion check should be activated do not have to correspond to the surface names used to specify the general contact domain. In many cases the contact interaction will be defined for a large domain, while the fold inversion check will be activated in a subset of this domain. If the surfaces for which the fold inversion check needs to be activated fall outside the general contact domain, the controls assignment is ignored. *CONTACT CONTROLS ASSIGNMENT, TYPE=FOLD INVERSION CHECK surface_1 Input File Usage: This option must be used in conjunction with the *CONTACT option. It should appear at most once per step; the data line can be repeated as often as necessary to activate the fold inversion check in different regions of the contact domain. If the surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. Activating the default tracking algorithm for edge-to-edge contact The default contact tracking algorithm utilizes more local information than the alternative tracking algorithm in tracking contact between edges and typically reduces the extent of global tracking required. The use of this algorithm may lead to smaller computational times in analyses that have extensive edge-to-edge contact defined (for example, during the inflation simulation of a folded airbag, where it may be desirable to activate all feature edges on the airbag membrane surface to accurately enforce contact during the inflation event). The default tracking algorithm can be explicitly specified, though all edge-to-edge contact in the contact domain will be enforced using the default tracking algorithm if contact controls are not specified for the tracking algorithm. Input File Usage: *CONTACT CONTROLS ASSIGNMENT, TYPE=ENHANCED EDGE TRACKING (default) This option must be used in conjunction with the *CONTACT option. This parameter setting applies to the entire general contact domain. An alternative tracking algorithm for edge-to-edge contact An alternative contact tracking algorithm is available that utilizes less local information than the default tracking algorithm in tracking contact between edges. This algorithm typically increases the extent of global tracking required and, hence, in most analyses the computational time. When the alternative edge tracking algorithm is specified, all edge-to-edge contact in the contact domain is enforced using this algorithm. Input File Usage: *CONTACT CONTROLS ASSIGNMENT, TYPE=EDGE TRACKING If specified, this option must be used in conjunction with the *CONTACT option. This parameter setting applies to the entire general contact domain. Control of initial overclosure resolution By default, Abaqus/Explicit automatically adjusts the positions of surfaces to remove small initial overclosures that exist in the general contact domain in the first step of a simulation. Conflicting adjustments from separate contact definitions, boundary conditions, tie constraints, and rigid body constraints can cause incomplete resolution of initial overclosures. Initial overclosures that are not resolved by repositioning nodes are stored as initial contact offsets to avoid large contact forces at the beginning of an analysis. Alternatively, in certain situations it may be desirable to avoid nodal adjustments altogether between a pair of surfaces and to treat all initial overclosures between the surfaces as temporary contact offsets. You can then specify the surfaces for which the initial overclosures should not be resolved by nodal adjustments and which should instead be stored as offsets. Input File Usage: *CONTACT CONTROLS ASSIGNMENT, AUTOMATIC OVERCLOSURE RESOLUTION surface_1, surface_2, STORE OFFSETS This option must be used in conjunction with the *CONTACT option. It should appear at most once per step; the data line can be repeated as often as necessary to assign a nondefault overclosure resolution method to different regions. If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. If the second surface name is omitted or is the same as the first surface name, the specified contact controls are assigned to contact interactions between the first surface and itself. Control of contact thickness reduction checks By default, the general contact algorithm requires that the contact thickness does not exceed a certain fraction of the surface facet edge lengths or diagonal lengths. This fraction generally varies from 20% to 60% based on the geometry of the element and whether the element is near a shell perimeter. The general contact algorithm will scale back the contact thickness automatically where necessary without affecting the thickness used in the element computations for the underlying elements. To check whether the thickness needs to be reduced in any particular region in the model, the contact algorithm first assigns the full thickness to each contact node, represented by a sphere centered at the node with a diameter equal to the thickness. Next, the thickness is reduced so that the spheres do not overlap with any neighboring facets that are not attached directly to the node, preventing spurious self-contact from developing. Then, the nodes on the perimeter of shells are moved a maximum of 50% of the facet size in the plane of the facet away from the perimeter to eliminate the “bull-nose” effect that occurs with the contact pair algorithm . If the thickness of the shell perimeter nodes is greater than twice the maximum perimeter offset, a final thickness reduction is performed to eliminate the remainder of the “bull-nose.” If the default thickness reductions are unacceptable in particular regions of the model, you can exclude self-contact for those regions via contact exclusion definitions and activate a control for the contact thickness reduction checks. Input File Usage: Use the following option to eliminate thickness reductions in regions of the model that are excluded from self-contact, while still reducing thickness at shell perimeters where perimeter offsets are insufficient to avoid the “bull-nose” effect: *CONTACT CONTROLS ASSIGNMENT, CONTACT THICKNESS REDUCTION=SELF Use the following option to eliminate thickness reductions in regions of the model that are excluded from self-contact and at all shell perimeters (a “bull- nose” will form at shell perimeter nodes if the thickness is greater than twice the maximum perimeter offset): *CONTACT CONTROLS ASSIGNMENT, CONTACT THICKNESS REDUCTION=NOPERIMSELF 35.5 Defining contact pairs in Abaqus/Explicit • “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1 • “Assigning surface properties for contact pairs in Abaqus/Explicit,” Section 35.5.2 • “Assigning contact properties for contact pairs in Abaqus/Explicit,” Section 35.5.3 • “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 35.5.4 • “Contact controls for contact pairs in Abaqus/Explicit,” Section 35.5.5 35.5.1 DEFINING CONTACT PAIRS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Element-based surface definition,” Section 2.3.2 • “Node-based surface definition,” Section 2.3.3 • “Analytical rigid surface definition,” Section 2.3.4 • “Contact interaction analysis: overview,” Section 35.1.1 • *CONTACT CONTROLS • *CONTACT PAIR • *SURFACE • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining self-contact,” Section 15.13.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Abaqus/Explicit provides two algorithms for modeling contact and interaction problems: the general contact algorithm and the contact pair algorithm. See “Contact interaction analysis: overview,” Section 35.1.1, for a comparison of the two algorithms. This section describes how to define contact pairs with surfaces for contact simulations in Abaqus/Explicit. Contact pairs in Abaqus/Explicit: • are part of the history definition of the model and can be created, modified, and removed from step to step (unlike Abaqus/Standard, where contact pairs are model data); • use sophisticated tracking algorithms to ensure that proper contact conditions are enforced efficiently; • can be used simultaneously with the general contact algorithm (i.e., some interactions can be modeled with contact pairs, while others are modeled with the general contact algorithm); • can be formed using a pair of rigid or deformable surfaces or a single deformable surface; • do not have to use surfaces with matching meshes; • cannot be formed with one two-dimensional surface and one three-dimensional surface; and • cannot be used for self-contact where the surface is composed of both first-order elements and second-order elements. Defining a contact pair interaction The definition of a contact pair interaction in Abaqus/Explicit consists of specifying: • the contact pair algorithm and the surfaces that interact with one another, as described in this section; • the contact surface properties (“Assigning surface properties for contact pairs in Abaqus/Explicit,” Section 35.5.2); • the mechanical contact property models (“Assigning contact properties for contact pairs in Abaqus/Explicit,” Section 35.5.3); • the contact Section 37.2.2); formulation (“Contact formulations for contact pairs in Abaqus/Explicit,” • the contact constraint enforcement method (“Contact constraint enforcement methods in Abaqus/Explicit,” Section 37.2.3); and • the algorithmic contact controls (“Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit,” Section 38.2.2). Defining a contact pair containing two surfaces To define a contact pair, you must indicate which pairs of surfaces will interact with each other. The order in which the surfaces are specified is important only when a nondefault weighting factor is specified . See “Element-based surface definition,” Section 2.3.2; “Node-based surface definition,” Section 2.3.3; and “Analytical rigid surface definition,” Section 2.3.4, for information on defining surfaces for use in contact pairs. Input File Usage: *CONTACT PAIR surface_1_name, surface_2_name Abaqus/CAE Usage: Interaction module: Create Interaction: Surface-to-surface contact (Explicit): select the first surface, click Surface, select the second surface Defining self-contact Define contact between a single surface and itself by specifying only a single surface or by specifying the same surface twice. Input File Usage: Use either of the following options: *CONTACT PAIR surface_1, *CONTACT PAIR surface_1, surface_1 Abaqus/CAE Usage: Interaction module: Create Interaction: Self-contact (Explicit): select the surface or Surface-to-surface contact (Explicit): select the surface, click Surface, select the surface again Limitations with self-contact The following limitations are enforced for a contact pair with self-contact: • The balanced master-slave contact algorithm will always be used for the contact pair (a nondefault weighting factor cannot be specified for the contact pair). • A contact thickness must be considered for self-contact surfaces on shell or membrane elements ; i.e., a zero surface thickness causes Abaqus/Explicit to issue an error message. By default, the contact thickness is equal to the current thickness. • The contact thickness for self-contact should not exceed the edge lengths or diagonal lengths of the facets. You can reduce the contact thickness, if necessary; see “Controlling the effects of surface thickness and offset in contact calculations” in “Assigning surface properties for contact pairs in Abaqus/Explicit,” Section 35.5.2. • A specialized finite-sliding tracking algorithm must be used. The use of the small-sliding contact formulation is not supported and causes Abaqus/Explicit to issue an error message. • Contact will be recognized between any node on a self-contact surface and any other point on the same surface, including either side of shells or membranes (i.e., self-contact on shells and membranes is independent of the face identifier specified in the surface definition). Removing and adding contact pairs Removal and addition of contact pairs: • can be used to simulate complicated forming processes where multiple tools need to interact with the workpiece at different stages; • can be used to extend surfaces to prevent one surface from sliding off another; • can result in significant computational savings by eliminating unnecessary contact searches; and • can be used to change the definition of a contact pair. Adding contact pairs By default, the contact pairs specified are added to the list of active contact pairs in the model. Initial penetrations should be avoided for contact pairs introduced after the first step, as large nodal accelerations and severe element distortions can result . Redefining a contact pair by deleting it and adding it in the same step can also lead to problems, because the “state” information associated with the slave nodes in contact will be reinitialized. For example, a penalty contact slave node with a penetration past the midsurface of a double-sided master surface would be allowed to pass through the master surface if the contact state were reinitialized. *CONTACT PAIR, OP=ADD Interaction module: Create Interaction Abaqus/CAE Usage: Input File Usage: Removing contact pairs Removal of contact pairs is a useful technique for simulating complicated forming processes where multiple tools will contact the same workpiece. Removing a contact pair once it is no longer needed eliminates the need to monitor the contact conditions and reduces the cost of the simulation. Input File Usage: Abaqus/CAE Usage: *CONTACT PAIR, OP=DELETE Interaction module: interaction manager: Deactivate General restrictions on surfaces used in contact pairs The following general restrictions (in addition to those discussed in “Element-based surface definition,” Section 2.3.2) apply to all surfaces used in contact pairs: • The surface normals of a surface must point toward the other surface that it may contact except when the surface is double-sided, as discussed below. • Element-based surfaces should not be used in contact pairs if the underlying elements may fail . Use general contact (“Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1) or node-based surfaces (“Node- based surface definition,” Section 2.3.3) in such cases. • The surface must be continuous, as discussed below. • Continuum and structural elements cannot be mixed in the same surface definition. • Deformable elements cannot be combined with elements that are part of a rigid body to define a single surface. These restrictions do not apply to surfaces used with the general contact algorithm (“Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1). The following restrictions apply to the surfaces forming a kinematic contact pair: • Rigid surfaces must always be the master surface. • Slave surfaces must be part of a deformable body. • A node-based surface can be used only as a slave surface. The following restrictions apply to the surfaces forming a penalty contact pair: • Analytical rigid surfaces must always be the master surface. • A node-based surface can be used only as a slave surface. Orienting the surface’s normal The orientation of a surface’s normal can be critical for the proper detection of contact between two contacting surfaces. At the point of closest proximity the normals of a single-sided master surface forming the contact pair should always point toward the slave surface. If, in the initial configuration of the model, a single-sided master surface’s normal points away from its slave surface, Abaqus/Explicit will detect that the slave surface penetrates the master surface. Abaqus/Explicit will attempt to resolve this initial overclosure of the contact pair with strain-free displacements before the start of the simulation (see “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 35.5.4). Abaqus/Explicit may have difficulty with the simulation if the overclosure is too severe. In most of these cases the analysis will terminate immediately, and an error message about severely distorted elements will be issued. You must give particular attention to checking that analytical rigid surfaces or single-sided Surface surfaces created on shell, membrane, or rigid elements have the proper orientation. orientation errors can often be quickly and easily detected by running a data check analysis (“Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2) and inspecting the deformed configuration in Abaqus/CAE. If large displacements have occurred, they may be due to an incorrect surface orientation. The proper and improper orientation of a rigid and deformable surface is shown in Figure 35.5.1–1. rigid surface outward normal deformable surface Incorrect rigid surface orientation Correct rigid surface orientation Figure 35.5.1–1 Example of proper and improper surface orientation with a rigid surface. It is not necessary for the normals of all of the underlying shell or membrane elements to have if possible, Abaqus/Explicit will define a consistent positive orientation for a double-sided surface: the surface such that its facets have consistent normals, even if the underlying elements do not have consistent normals. The facet normals will be the same as the element normals if the element normals are all consistent; otherwise, an arbitrary positive orientation is chosen for the surface. For double-sided surfaces the positive orientation is significant only with respect to the sign of the contact pressure output variable, CPRESS, as discussed in “Element-based surface definition,” Section 2.3.2. Defining a continuous surface A contact pair surface cannot be made up of two or more disconnected regions. The definition of analytical rigid surfaces automatically ensures that these surfaces are continuous. However, care must be taken to define surfaces formed with elements so that they are continuous across element edges in three-dimensional models or through nodes in two-dimensional models. This continuity requirement has several implications for what constitutes a valid or invalid surface definition. In two dimensions the surface must be either a simple, nonintersecting curve with two terminal ends or a closed loop. Figure 35.5.1–2 shows examples of valid and invalid two-dimensional surfaces for use in contact pairs. Valid Closed Simply Connected 2D Surface Valid Open Simply Connected 2D Surface Invalid 2D Surface Figure 35.5.1–2 Valid and invalid 2-D surfaces. In three dimensions an edge of an element face belonging to a valid surface may be either on the perimeter of the surface or shared by one other face. Two element faces forming a contact pair surface cannot be joined just at a shared node; they must be joined across a common element edge. An element edge cannot be shared by more than two surface facets. Figure 35.5.1–3 illustrates valid and invalid three-dimensional surfaces for use in contact pairs. The continuity requirement applies to both automatically generated free surfaces and surfaces defined with element face identifiers . Figure 35.5.1–4 shows an automatically generated free surface resulting from the specification of an element set consisting of two disjointed groups of elements. The resulting surface is not continuous since it is composed of two disjoint open curves. Restrictions for two-dimensional contact simulations The following restrictions apply when defining a contact simulation for two-dimensional (planar) or axisymmetric problems: • A contact pair cannot involve a planar surface and an axisymmetric surface. This restriction applies only to deformable and element-based rigid surfaces. • Defining a contact pair that contains two surfaces formed by planar elements of different sizes in the out-of-plane direction (“depth”) is not recommended and will result in a warning message. In such a case frictional stresses are calculated based on a weighted average depth, with the weighting for the first surface equal to the user-specified contact surface weighting factor. The out-of-plane Valid Simply Connected Surface Invalid Surface Invalid Surface Figure 35.5.1–3 Valid and invalid 3-D surfaces. user-specified element set automatically generated free surface Figure 35.5.1–4 Automatic free surface generation. thickness for two-dimensional beam element-based surfaces is always assumed to be one. As a result, the contact pressure acting on such a surface can be considered as a line force as well. • When more than one contact pair involves contact between the same rigid surface formed by planar elements and different planar deforming surfaces, the deforming surfaces must all have the same depth; otherwise, a warning message will be issued. The depth value used for calculating contact stresses will then be taken from one of these deforming surfaces, but this choice cannot be predicted. Limitations in contact simulations with three-dimensional beam and truss elements Element-based surfaces cannot be formed on three-dimensional beam or truss elements, so node-based surfaces must be used to define a surface on these elements. Because a node-based surface must be used, a surface on three-dimensional beam or truss elements must always form the slave surface in a pure master-slave contact pair. Therefore, it is not possible to have two three-dimensional beam or truss structures contact each other. Output You can write the contact surface variables associated with the interaction of contact pairs to the Abaqus output database (.odb) file. The surface variables for a mechanical contact analysis include contact pressure and force, frictional shear stress and force, relative tangential motion (slip) of the surfaces during contact, whole surface resultant quantities (i.e., force, moment, center of pressure, and total area in contact), the status of bonded nodes, and the maximum torque transmitted about the z-axis of axisymmetric elements. Additional discussion on requesting contact surface output can be found in “Surface output in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3. Output from thermal interactions is discussed in “Thermal contact properties,” Section 36.2.1. Field output The generic variables CSTRESS, CFORCE, FSLIP, and FSLIPR are valid field output requests for Abaqus/Explicit. If CSTRESS is requested for a contact pair, the variables CPRESS (contact pressure), CSHEAR1 (contact traction in the local 1-direction), and, if the contact interaction is three-dimensional, CSHEAR2 (contact traction in the local 2-direction) can be contoured in Abaqus/CAE for each discrete (i.e., non-analytical) surface in a contact pair. Contours of contact pressure (CPRESS) on surfaces used with the contact pair algorithm will be displayed using the convention that a positive pressure represents compressive contact on the positive side of the surface. The positive side of the surface can be determined by drawing the surface normals in the Visualization module of Abaqus/CAE. Following this convention, the sign of CPRESS will be reversed for contact on the negative (back) side of a double-sided surface, so negative values of CPRESS may be seen if contact occurs on the back side of a double-sided surface. If contact from separate contact pairs occurs on both sides of the double-sided surface at the same point, the value of CPRESS is given for each contact pair separately. If CFORCE is requested for a contact pair, the variables CNORMF (normal contact force) and CSHEARF (shear contact force) can be plotted as vectors in a symbol plot in Abaqus/CAE for each discrete (i.e., non-analytical) surface in a contact pair. If FSLIPR is requested, FSLIPR (the magnitude of the slip rate for slave nodes in contact) can be contoured in Abaqus/CAE for each slave surface in a contact pair. In addition, for three-dimensional contact interactions involving an analytical rigid surface and for all two-dimensional contact interactions, components of net slip rate based on local tangent directions (FSLIPR1 and, in three dimensions, FSLIPR2) can also be contoured in Abaqus/CAE for each slave surface in a contact pair if FSLIPR is requested. All of the slip rate variables associated with FSLIPR are zero whenever a slave node is not in contact. If FSLIP is requested, FSLIPEQ (the length of the overall slip path for a slave node while it is in contact) can be contoured in Abaqus/CAE for each slave surface in a contact pair. In addition, for three-dimensional contact interactions involving an analytical rigid surface and for all two-dimensional contact interactions, components of net slip (FSLIP1 and, in three dimensions, FSLIP2) can also be contoured in Abaqus/CAE for each slave surface in a contact pair if FSLIP is requested. These slip variables are equivalent to the slip rate variables integrated over time: FSLIPEQ, FSLIP1, and FSLIP2 are equivalent to FSLIPR, FSLIPR1, and FSLIPR2 integrated over time, respectively. Therefore, these slip variables account only for relative motions that occur while slave nodes are in contact. History output Several whole surface contact variables are available as history output. These variables record the contact state of a surface as a set of force (CFN, CFS, and CFT) and moment (CMN, CMS, and CMT) resultants with respect to the origin. Additional variables give the center of pressure (XN, XS, and XT) on the surface (defined as the point closest to the centroid of the surface that lies on the line of action of the resultant force for which the resultant moment is minimal). The last letter of each variable name (except the variable CAREA) denotes which contact force distribution on the surface is used to calculate the resultant: the letter N denotes that the normal contact forces are used to derive the resultant quantity; the letter S denotes that the shear contact forces are used to derive the resultant quantity; and the letter T denotes that the sum of the normal and shear contact forces are used to derive the resultant quantity. These history output variables will be written twice to the output database once for each surface involved in the contact pair. Each total moment output variable will not necessarily equal the cross product of the respective center of force vector and resultant force vector. Forces acting on two different nodes of a surface may have components acting in opposite directions, such that these nodal force components generate a net moment but not a net force; therefore, the total moment may not arise entirely from the resultant force. The center of force output variables tend to be most meaningful when the surface nodal forces act in approximately the same direction. The total area in contact at a given time can be requested using output variable CAREA, defined as the sum of all the facets where there is contact force. The contact area reported by CAREA is generally slightly larger than the true contact area for reasonably meshed contact surfaces; therefore, interpretation of CAREA should be done with care. The discrepancy between the CAREA output and the true contact area decreases as the mesh density increases. Using contact inclusions or exclusions to limit CAREA output to smaller contact surfaces may also reduce the discrepancy in some cases. Since the CAREA output is an approximation of the true contact area, deriving force or stress values using this output may not yield accurate values; requesting contact force and stress directly is the most appropriate way to obtain accurate results. Detailed history output on the status of bonded surfaces is available from an Abaqus/Explicit simulation. Details can be found in “Breakable bonds,” Section 36.1.9. Obtaining the “maximum torque” that can be transmitted about the z-axis in an axisymmetric analysis When modeling surface-based contact with axisymmetric (CAX) elements, Abaqus/Explicit can calculate the maximum torque (output variable CTRQ) that can be transmitted about the z-axis. The maximum torque, T, is defined as where p is the pressure transmitted across the interface, r is the radius to a point on the interface, and s is the current distance along the interface in the r–z plane. This definition of “torque” effectively assumes a friction coefficient of unity. 35.5.2 ASSIGNING SURFACE PROPERTIES FOR CONTACT PAIRS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1 • *CONTACT PAIR • *SURFACE • “Specifying geometric properties for mechanical contact property options” in “Defining a contact interaction property,” Section 15.14.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview This section describes how to modify the surface properties for contact interactions in Abaqus/Explicit defined with the contact pair algorithm, including the surface thickness and offset. Shell, membrane, or rigid element thickness and shell or rigid element offset To define surfaces on shell, membrane, or rigid elements such that they are in contact at the start of the analysis, the element thicknesses must be considered when defining the nodal coordinates; otherwise, the surfaces in the contact pair will be overclosed. Surface thickness and surface offset are properties that are inherited from underlying shell and membrane elements by default. For a surface based on rigid elements, the default surface thickness and offset correspond to the thickness and offset defined for the rigid body to which the elements belong . The surface thickness and offset are zero for surfaces based on solid elements. By default, the nodal thickness for surfaces based on shell, membrane, or rigid elements equals the minimum thickness of the surrounding elements . The surface thickness within a facet is interpolated from the nodal values; the interpolated surface thickness never extends past the specified element or nodal thickness, which may be significant with respect to initial overclosures. If a spatially varying nodal thickness is defined for the underlying elements , the nodal surface thickness may not correspond exactly to the specified nodal thickness . The nodal surface thickness distribution will tend to be more diffuse than the specified nodal thickness distribution (because the specified nodal thicknesses are averaged to compute the element thicknesses, and the minimum of the surrounding element thicknesses is the nodal surface thickness). Effects of surface thickness and offsets, as well as methods for modifying the surface thickness and for avoiding surface offsets, are discussed below. specified element thickness (constant over element) interpolated surface thickness nodal surface thickness Figure 35.5.2–1 Continuous variation of surface thickness across facet boundaries. Table 35.5.2–1 Thicknesses corresponding to Figure 35.5.2–1. node element specified element thickness nodal surface thickness (minimum of adjacent element thicknesses) 0.5 0.5 0.5 0.9 0.9 0.5 0.5 0.9 0.9 element thickness (constant over element) nodal surface thickness specified nodal thickness interpolated surface thickness Figure 35.5.2–2 Small discrepancy between the nodal surface thickness and the specified nodal thickness. Table 35.5.2–2 Thicknesses corresponding to Figure 35.5.2–2. node element specified nodal thickness element thickness (average of specified nodal thickness) nodal surface thickness (minimum of adjacent element thicknesses) 0.5 0.5 0.5 0.9 0.9 0.9 0.5 0.5 0.7 0.9 0.9 35.5.2–3 0.5 0.5 0.5 0.7 0.9 Effects of surface thickness and offsets Accounting for thickness in the contact pair algorithm will cause the surface to extend past the parent element boundary in the plane of the element by an amount equal to one-half its thickness. For example, this surface extension, which is semi-circular in shape, will cause contact to be established between the edge of a shell and an opposing surface before the node on the shell boundary reaches the opposing surface. The extension is present for both single-sided and double-sided surfaces. Figure 35.5.2–3 demonstrates this concept. Such “bull-nose” extensions are avoided when the general contact algorithm (“Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1) is used. The effect of a shell or rigid offset on a surface is shown in Figure 35.5.2–4. Poorly defined surfaces can result near corners if large offsets are present, as shown in Figure 35.5.2–5. You should consider this when defining a model. A warning message will be issued if the offset magnitude is greater than one-half of any of the parent shell element edge lengths. However, at acute corners it is possible for an offset less than one-half of the parent element size to result in a poorly defined contact surface (and in this case no warning will be given). contacting surface surface extension shell nodes shell reference surface contact established Figure 35.5.2–3 Extension of contact surface for edge contact without zero surface thickness. midsurface t/2 t/2 offset contact surface, same as shell outer surface except at edges reference surface Figure 35.5.2–4 Extension of contact surface if a shell offset is present. nodal offset adjusted nodal position shell midsurface reference surface Figure 35.5.2–5 Example of a poorly defined surface near a corner when a large shell offset is present. Controlling the effects of surface thickness and offset in contact calculations You can control the thickness and offset used in the contact calculations only; they do not affect surface- based constraints. These settings are intended primarily for self-contact surfaces since you cannot force zero thickness for these surfaces, as described below. Self-contact surfaces should not contain facets that are thicker than their edge or diagonal lengths. Extremely large thicknesses will cause nodes to appear to be penetrating nearby facets in even a flat self-contact surface due to the algorithmic use of a semi-circular tube with a radius of half the contact thickness around the edge of each facet . outer boundary of node penetration outer boundary of overall surface outer boundary of facet reference surface Figure 35.5.2–6 Undesired penetration resulting from a large thickness in a self-contact surface. You can scale the effective thickness used for all of the facets on a surface by a single factor, f. Alternatively, you can adjust only the thicknesses for surface facets in which the thickness to minimum edge or diagonal length ratio exceeds a specified value, r; the amount by which a facet thickness is adjusted may vary during an analysis because of changes in the facet size. If the thickness to element size ratio exceeds 1.0 in the initial configuration for a self-contact surface, an error message recommending that you adjust the thickness will be issued. You should not specify extremely small values for f or r for double-sided surfaces or surfaces that will be involved in self-contact since these surfaces must have a contact thickness that is significant compared to the facet size. For surfaces involved only in two-surface contact it is acceptable to set f=0.0; however, it is computationally more efficient to use the method described below to force a zero surface thickness. It is also possible to enforce the offset but not the thickness in the surface model by setting the scale factor, f, equal to zero. Input File Usage: Abaqus/CAE Usage: Use the following option to scale the surface thickness by a single factor: *SURFACE, NAME=name, SCALE THICK=f Use the following option to adjust the thickness to element size ratios: *SURFACE, NAME=name, MAX RATIO=r You cannot scale the thickness of a contact surface in Abaqus/CAE. Forcing zero surface thickness and offset You can force the surface thickness and offset to be zero, rather than inherit the thickness and offset of underlying shell, membrane, or rigid elements. In this case the contact surface is taken as the reference surface . midsurface t/2 t/2 shell surfaces reference surface and contact surface Figure 35.5.2–7 Contact surface with zero thickness and offset. You cannot ignore the thickness for a surface that is used as a contact surface for single-surface (self) contact. If one of the surfaces in a contact pair is a double-sided surface, zero thickness can be forced on only one of the two surfaces: at least one surface in a contact pair involving double-sided surfaces must have a nonzero thickness. The ability to force zero surface thickness is useful for performing parameter studies on the thickness or offset of a model since you can change the thickness and offset without also having to move the mesh to control the initial separation between the surfaces. Input File Usage: Abaqus/CAE Usage: *SURFACE, NAME=name, NO THICK You cannot force a surface thickness to be zero in Abaqus/CAE. Example Contact calculations are generally most accurate with the default treatment of thickness and offset. However, when a shell offset of half the original shell thickness has been specified, forcing zero surface thickness will give an accurate representation of one side of the surface. This approach can be more accurate near a corner (especially on the exterior side of a corner) than if the offset and thickness are enforced for the surface, as shown in Figure 35.5.2–8. default surface desired midsurface reference surface Shell model with offset equal to half the thickness surface if zero thickness is forced adjusted nodal position midsurface contact surfaces contact surface Figure 35.5.2–8 Forcing zero surface thickness when the shell offset is half the original shell thickness. Forcing zero surface offset For situations in which it is desirable to ignore the effect of the offset but when it is still necessary to model the thickness in the contact calculations, you can force only the surface offset to be zero without affecting the surface thickness. In this case the contact surface is the outside surface of an imaginary shell, membrane, or rigid element whose midsurface is at the reference surface . This method could be used for a self-contact surface that would be poorly defined if the offset were enforced (thickness must be enforced for self-contact surfaces). Input File Usage: Abaqus/CAE Usage: *SURFACE, NAME=name, NO OFFSET You cannot force a surface offset to be zero in Abaqus/CAE. midsurface t/2 t/2 shell surfaces contact surface reference surface Figure 35.5.2–9 Contact surface with zero offset. Defining additional contact thicknesses for a contact pair interaction You can specify a contact offset for a contact pair interaction in addition to any element thicknesses or midsurface offsets already defined for the elements underlying the contact pair surfaces. For small sliding this includes contact offsets defined by initial clearances . The specified offset value will be applied as an additional thickness of a layer separating the two surfaces, not as an additional thickness for each surface in the contact pair. This value can be positive or negative. This technique is often used in conjunction with softened behavior to model the thickness of a thin layer between two contacting surfaces. Input File Usage: Abaqus/CAE Usage: *SURFACE INTERACTION, PAD THICKNESS=value Interaction module: contact property editor: Mechanical→Geometric Properties: toggle on Thickness of interfacial layer (Explicit): value 35.5.3 ASSIGNING CONTACT PROPERTIES FOR CONTACT PAIRS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Mechanical contact properties: overview,” Section 36.1.1 • “Contact pressure-overclosure relationships,” Section 36.1.2 • “Contact damping,” Section 36.1.3 • “Frictional behavior,” Section 36.1.5 • “User-defined interfacial constitutive behavior,” Section 36.1.6 • “Breakable bonds,” Section 36.1.9 • *CONTACT PAIR • *SURFACE INTERACTION • “Interaction property editors,” Section 15.9.3 of the Abaqus/CAE User’s Manual Overview Contact properties: • define the mechanical and thermal surface interaction models that govern the behavior of surfaces when they are in contact; and • are assigned to individual contact pairs. Assigning a contact property definition to a contact pair If nondefault contact properties are desired, you can refer to a contact property definition that governs the interaction of the two surfaces. Multiple contact pairs can refer to the same contact property definition. Input File Usage: Use both of the following options: *CONTACT PAIR, INTERACTION=interaction_property_name surface_1, surface_2 *SURFACE INTERACTION, NAME=interaction_property_name Interaction module: Abaqus/CAE Usage: Create Interaction Property: Name: interaction_property_name, Contact Interaction editor: Contact interaction property: interaction_property_name Example Figure 35.5.3–1 shows the mesh used in this example. For purposes of this example, a balanced master- slave contact pair is used. The property definition for the contact pair (GRATING) uses a friction model where =0.4. ESETB ESETA 502 BSURF 201 501 202 101 102 103 ASURF Figure 35.5.3–1 Surface interaction with friction. *HEADING … *SURFACE, NAME=ASURF ESETA, *SURFACE, NAME=BSURF ESETB, … *STEP Step1 *DYNAMIC, EXPLICIT … *CONTACT PAIR, INTERACTION=GRATING ASURF, BSURF *SURFACE INTERACTION, NAME=GRATING *FRICTION 0.4 Changing contact properties Contact property models are defined as model or history data for a contact pair analysis. You can modify the contact properties from step to step; however, the old contact pair should be deleted and redefined using the new interaction. Example For example, the following input could be used to change the friction coefficient used for contact between ASURF and BSURF in the second step of the analysis started in the previous example: *STEP Step2 *DYNAMIC, EXPLICIT … *CONTACT PAIR, INTERACTION=GRATING,OP=DELETE ASURF, BSURF *SURFACE INTERACTION, NAME=GRATING_NEW *FRICTION 0.5 *CONTACT PAIR, INTERACTION=GRATING_NEW ASURF, BSURF 35.5.4 ADJUSTING INITIAL SURFACE POSITIONS AND SPECIFYING INITIAL CLEARANCES FOR CONTACT PAIRS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1 • *CLEARANCE • *CONTACT PAIR • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Adjustments to the positions of the slave nodes in an Abaqus/Explicit contact pair: • are performed for all contact pairs that have slave nodes that are overclosed and that do not have specified initial clearances, except when nodes of a rigid body act as slave nodes; • can eliminate small gaps or penetrations caused by numerical roundoff when a graphical preprocessor such as Abaqus/CAE is used; • do not create any strains or momentum in the model during the first step of a simulation; • do create strains and momentum in subsequent steps of a simulation; • should not be used to correct gross errors in the mesh design; and • should not be used to resolve initial overclosures involving a slave node that is pinched between two master surfaces. If the small-sliding contact formulation is used, an alternative to adjusting the position of the surfaces is to define the initial clearances between the surfaces precisely in both magnitude and direction. Adjustments of overclosed surfaces in the first step of the simulation Abaqus/Explicit will automatically adjust the positions of surfaces to remove any initial overclosures that exist when a contact pair is defined in the first step of a simulation, except when nodes of a rigid body act as a slave nodes or user subroutine VUINTER is used. The adjustments are made with strain-free initial displacements to the slave nodes on the surfaces. Therefore, when a balanced master-slave contact pair is defined, nodes on both surfaces may be adjusted. This automatic adjustment of surface position is intended to correct only minor mismatches associated with mesh generation. You can review the surface adjustments in the status (.sta) file, the message (.msg) file, and the output database (.odb) file; see “Contact diagnostics in an Abaqus/Explicit analysis,” Section 38.2.1, for more information. Some softened contact models have nonzero contact pressure at zero overclosure . For these models some initial, nonequilibrated contact pressure may be present at the beginning of an analysis, as the adjustments are made to satisfy zero overclosure rather than zero contact pressure. Large initial contact pressures may cause excessive distortion of elements near the contact surfaces. Conflicting adjustments from separate contact pairs will cause incomplete resolution of initial overclosures and will lead to a noisy solution or severe distortion of elements. This can occur when a slave node is pinched between two master surfaces. Because of the lack of a unique outward direction from double-sided facets, the resolution of large initial penetrations for double-sided surfaces can be difficult. Initial penetration will be detected only when a slave node lies within the thickness of the underlying element, and the initial penetration will be resolved by moving the slave node to the nearest free surface as shown in Figure 35.5.4–1. corrected position of slave node original position of slave node master surface thickness master node Figure 35.5.4–1 Correction of initial overclosure for a contact pair involving two double-sided surfaces. A warning message will be issued to the status (.sta) file if two adjacent slave nodes (connected by a facet edge) are detected on opposite sides of a double-sided master surface involved in contact defined with the contact pair algorithm. No such warning will be issued for node-based surface nodes on opposite sides of a double-sided master surface, because adjacency cannot be determined among the node-based surface nodes. If the master surface is a single-sided surface, initial overclosures will be resolved using the surface normal of the master surface, as shown in Figure 35.5.4–2. Having slave nodes trapped on opposite sides of a double-sided master surface will often lead to serious problems, which may not became apparent until later in an analysis. Therefore, a data check analysis is recommended prior to running a large contact pair analysis so that you can check for warning messages side of surface (SPOS or SNEG) used in single-sided contact corrected position of slave node original position of slave node master surface thickness master node Figure 35.5.4–2 Correction of initial overclosure for a contact pair involving a single-sided and a double-sided surface. in the status file (.sta) and check for mislocated adjacent slave nodes on opposite sides of the master surface. The adjustments affect only the nodes on the surfaces. Excessive distortion of neighboring elements may result if this feature is used to correct for gross errors in the initial geometry, causing the analysis to end with an error message. Nodes on a rigid body can act as slave nodes only for penalty contact pairs. Initial penetrations of slave nodes that are part of a rigid body are not resolved with strain-free corrections; i.e., the slave nodes are not adjusted. These penetrations are likely to cause artificially large contact forces in the first increments of an analysis and should, therefore, be avoided in the mesh definition. Adjustments of overclosed surfaces during subsequent steps in the simulation If contact pairs are defined in later steps with initially overclosed surfaces, Abaqus/Explicit does not take any special actions to gradually resolve these initial penetrations: contact forces will be applied according to whatever contact constraint enforcement method is being used. These contact forces may be very large, causing large accelerations and velocities and possible distortion of elements. Initial penetrations have the potential to cause problems for contact pairs introduced in any step if a VUINTER user subroutine is used; but in that case you control the application of contact forces. Minimizing the noise associated with adjustments of initially overclosed surfaces When a balanced master-slave contact pair is used for situations where the initial overclosure adjustments are not very small, non-negligible errors may persist in the adjusted geometry and can lead to a noisy oscillation (or “ringing”) in the contact procedure. This problem can sometimes be mitigated by modifying the contact pair to be a pure master-slave relationship using a weighting factor; see “Contact surface weighting” in “Contact formulations for contact pairs in Abaqus/Explicit,” Section 37.2.2, for details. Specifying initial clearance values precisely You can define initial clearances and contact directions precisely for the nodes on the slave surface when they would not be computed accurately enough from the nodal coordinates; for example, if Initial clearances and contact the initial clearance is very small compared to the coordinate values. directions can be defined only in small-sliding contact analyses (“Contact formulations for contact pairs in Abaqus/Explicit,” Section 37.2.2). The initial clearance value calculated at every slave node based on the coordinates of the slave node and the master surface is overwritten by the value that you specify. This procedure does not alter the coordinates of the slave nodes. When the balanced-master slave contact algorithm is invoked for the contact pair, the initial clearance values can be defined on one or both of the surfaces. Initial clearances defined on contact surfaces that act only as master surfaces will be ignored. Specifying a uniform clearance for the surfaces You can specify a uniform clearance for a contact pair by identifying the contact pair and the desired initial clearance, Input File Usage: Abaqus/CAE Usage: (the value must be positive). No other data are needed. *CLEARANCE, CPSET=cpset_name, VALUE= Interaction module: contact interaction editor: Clearance: Initial clearance: Uniform value across slave surface: Specifying spatially varying clearances for the surfaces Alternatively, you can specify spatially varying clearances for a contact pair by identifying the contact pair and a table of data specifying the clearance at a single node or a set of nodes belonging to the slave surface. Any slave surface node that is not identified will use the clearance that Abaqus/Explicit calculates from the initial geometry of the surfaces. Input File Usage: Abaqus/CAE Usage: *CLEARANCE, CPSET=cpset_name, TABULAR You cannot specify initial clearance or overclosure values using a table of data in Abaqus/CAE. Reading spatially varying clearances from an external file Input File Usage: Abaqus/Explicit can read the spatially varying clearances for a contact pair from an external file. *CLEARANCE, CPSET=cpset_name, TABULAR, INPUT=file_name You cannot specify initial clearance or overclosure values using an external input file in Abaqus/CAE. Abaqus/CAE Usage: Specifying the surface normal for the contact calculations Normally Abaqus/Explicit calculates the surface normal used for the contact calculations from the geometry of the discretized surfaces, using the algorithms described in “Contact formulations for contact pairs in Abaqus/Explicit,” Section 37.2.2. When specifying spatially varying clearances, you can redefine the contact direction that Abaqus/Explicit uses with each slave node by specifying the components of this vector. The vector must define the global Cartesian components of the outward normal to the master surface. Input File Usage: *CLEARANCE, SLAVE=surface_name, MASTER=surface_name, TABULAR node number or node set label, clearance value, first normal component, second normal component, third normal component Repeat the data line as often as necessary. Abaqus/CAE Usage: You cannot redefine contact directions in Abaqus/CAE, except for thread bolt connections . Generating the contact normal directions for a thread bolt connection automatically Alternatively, for a single-threaded bolt connection the contact normal directions for each slave node can be generated automatically by specifying the thread geometry data and two points used to define a vector on the axis of the bolt/bolt hole. The axis vector should be oriented to point from the tip of the bolt to the head of the bolt when in tension and from the head to the tip when in compression. Input File Usage: Abaqus/CAE Usage: *CLEARANCE, CPSET=cpset_name, TABULAR, BOLT half-thread angle, pitch, major bolt diameter, mean bolt diameter node number or node set label, clearance value, coordinates of points a and b on the axis of the bolt/bolt hole Repeat the second data line as often as necessary. Interaction module: contact interaction editor: Clearance: Initial clearance: Computed for single-threaded bolt or Specify for single-threaded bolt: clearance value, Clearance region on slave surface: Edit Region: select region, Bolt direction vector: Edit: select axis, Half-thread angle: half-thread angle, Pitch: pitch, Bolt diameter: Major: major bolt diameter or Mean: mean bolt diameter 35.5.5 CONTACT CONTROLS FOR CONTACT PAIRS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1 • *CONTACT CONTROLS • “Specifying contact controls in an Abaqus/Explicit analysis,” Section 15.13.10 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Contact controls for Abaqus/Explicit contact pairs can be used • to scale the stiffness used by penalty contact constraints, and • to adjust the search algorithms that track the motions between two surfaces. Scaling default penalty stiffnesses If you use the penalty method to enforce contact constraints in a contact pair , Abaqus/Explicit resists penetrations between surfaces by applying a “spring” stiffness to penetrating nodes. The “spring” stiffness that relates the contact force to the penetration distance is chosen automatically by Abaqus/Explicit, such that the effect on the time increment is minimal yet the allowed penetration is not significant in most analyses. Significant penetrations may develop in an analysis if any of the following factors are present: • Displacement-controlled loading • Materials at the contact interface that are purely elastic or stiffen with deformation • Deformable elements (especially membrane and surface elements) that have relatively little mass of their own and are constrained via methods other than boundary conditions (for example, connectors) involved in contact • Rigid bodies that have relatively little mass or rotary inertia of their own and are constrained via methods other than boundary conditions (for example, connectors) involved in contact See “The Hertz contact problem,” Section 1.1.11 of the Abaqus Benchmarks Manual, for an example in which the first two of these factors combine such that the contact penetrations with the default penalty stiffness are significant. You can specify a scale factor by which to modify penalty stiffnesses for specified contact pairs. This scaling may affect the automatic time incrementation. Use of a large scale factor is likely to increase the computational time required for an analysis because of the reduction in the time increment that is necessary to maintain numerical stability . Input File Usage: Use both of the following options to scale the default penalty stiffnesses: Abaqus/CAE Usage: *CONTACT PAIR, MECHANICAL CONSTRAINT=PENALTY, CPSET=contact_pair_set_name surface_1, surface_2 *CONTACT CONTROLS, CPSET=contact_pair_set_name, SCALE PENALTY=factor Interaction module: Create Contact Controls: Name: contact_controls_name, Abaqus/Explicit contact controls: Penalty stiffness scaling factor: factor Interaction editor: Mechanical constraint formulation: Penalty contact method, Contact controls: contact_controls_name Adjusting the finite-sliding contact tracking algorithm In a finite-sliding contact pair, searches are conducted continually throughout an analysis to track the relative motion between the two contacting surfaces. The contact tracking algorithm consists of an expensive, periodic global search and a less expensive, regular local search; the search algorithms are discussed in detail in “Contact tracking algorithms” in “Contact formulations for contact pairs in Abaqus/Explicit,” Section 37.2.2. You can use contact controls to adjust the frequency and cost of these searches. Specifying more frequent global contact searches By default for two-surface contact pairs, Abaqus/Explicit performs a more thorough search of the master faces near each slave node every one hundred increments, which is sufficient for most analyses. However, there are some valid contact situations where a global search needs to be used more or less often during the step. Figure 35.5.5–1 illustrates a situation that might require more frequent global tracking. The master surface is a valid surface, but it contains a hole. The slave node shown identifies the shaded element facet as the closest master surface facet during an increment. The local contact search looks at this master surface facet and its neighbors. If the slave node displaces across the hole in relatively few increments, the potential contact between the slave node and the master surface facets across the hole will not be detected because the local contact search will still be checking the shaded facet. This same situation can occur when a slave node moves rapidly across a deep valley in the master surface. The solution to this problem is to conduct global contact searches more frequently. You can specify the number of increments between global searches, n, for a given contact pair, if a value other than the default of 100 is desired. Input File Usage: Use both of the following options: *CONTACT PAIR, CPSET=contact_pair_set_name *CONTACT CONTROLS, CPSET=contact_pair_set_name, GLOBTRKINC=n master surface slave node previous nearest master face trajectory of slave node Figure 35.5.5–1 Example where local search may fail. Abaqus/CAE Usage: Interaction module: Create Contact Controls: Name: contact_controls_name, Abaqus/Explicit contact controls: Specify max number of increments: n Interaction editor: Contact controls: contact_controls_name Using a more conservative local contact search The default local contact search used by Abaqus/Explicit uses techniques that allow it to use a minimum amount of computational time. If the local contact search has difficulty enforcing the appropriate contact conditions, a more conservative local contact search may resolve the problem. The contact search specified has no effect on contact pairs using self-contact. Input File Usage: Use both of the following options: *CONTACT PAIR, CPSET=contact_pair_set_name *CONTACT CONTROLS, CPSET=contact_pair_set_name, FASTLOCALTRK=NO Abaqus/CAE Usage: Interaction module: Create Contact Controls: Name: contact_controls_name, Abaqus/Explicit contact controls: toggle off Fast local tracking Interaction editor: Contact controls: contact_controls_name Tracking contact with highly warped surfaces Calculating the correct contact conditions along a surface that is highly warped is very difficult, especially when the relative velocity of the contacting surfaces is very large. By default, Abaqus/Explicit monitors the orientation of every deformable master surface formed by element faces every 20 increments to check that the surface is not highly warped; rigid faceted surfaces are checked for large warping only at the beginning of a step. If a surface becomes highly warped, a warning message is issued in the status (.sta) file , and a more accurate algorithm is used to calculate each slave node’s nearest point on the warped master surface. The alternate algorithm provides a more accurate solution but uses slightly more computational time. Redefining the criteria for a highly warped surface By default, Abaqus/Explicit considers a surface to be highly warped when the angle between surface normals at the nodes of a facet varies by more than 20°. The maximum variation of the surface normal over a facet is called the out-of-plane warping angle. You can change the default value of the out-of-plane warping angle cutoff from step to step for any contact pair in the model. Input File Usage: *CONTACT CONTROLS, CPSET=contact_pair_set_name, WARP CUT OFF=angle Abaqus/CAE Usage: Interaction module: Create Contact Controls: Name: contact_controls_name, Abaqus/Explicit contact controls: Angle criteria for highly warped facet (degrees): angle Interaction editor: Contact controls: contact_controls_name Modifying how frequently Abaqus/Explicit checks for warped surfaces You can specify the frequency, in increments, at which Abaqus/Explicit checks for warped surfaces for any contact pair in the model. The frequency can be changed from step to step. Checking for warped surfaces more frequently (the default is every 20 increments) will cause a slight increase in computational time for the analysis. Input File Usage: *CONTACT CONTROLS, CPSET=contact_pair_set_name, WARP CHECK PERIOD=n Abaqus/CAE Usage: Interaction module: Create Contact Controls: Name: contact_controls_name, Abaqus/Explicit contact controls: Warp check increment: n Interaction editor: Contact controls: contact_controls_name 36. Contact Property Models Mechanical contact properties Thermal contact properties Electrical contact properties Pore fluid contact properties 36.1 36.2 36.3 36.1 Mechanical contact properties • “Mechanical contact properties: overview,” Section 36.1.1 • “Contact pressure-overclosure relationships,” Section 36.1.2 • “Contact damping,” Section 36.1.3 • “Contact blockage,” Section 36.1.4 • “Frictional behavior,” Section 36.1.5 • “User-defined interfacial constitutive behavior,” Section 36.1.6 • “Pressure penetration loading,” Section 36.1.7 • “Interaction of debonded surfaces,” Section 36.1.8 • “Breakable bonds,” Section 36.1.9 • “Surface-based cohesive behavior,” Section 36.1.10 36.1.1 MECHANICAL CONTACT PROPERTIES: OVERVIEW References • “Contact interaction analysis: overview,” Section 35.1.1 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • “Assigning contact properties for general contact in Abaqus/Explicit,” Section 35.4.3 • “Assigning contact properties for contact pairs in Abaqus/Explicit,” Section 35.5.3 • “Contact pressure-overclosure relationships,” Section 36.1.2 • “Contact damping,” Section 36.1.3 • “Contact blockage,” Section 36.1.4 • “Frictional behavior,” Section 36.1.5 • “User-defined interfacial constitutive behavior,” Section 36.1.6 • “Pressure penetration loading,” Section 36.1.7 • “Interaction of debonded surfaces,” Section 36.1.8 • “Breakable bonds,” Section 36.1.9 • “Surface-based cohesive behavior,” Section 36.1.10 • *SURFACE INTERACTION • “Understanding interaction properties,” Section 15.4 of the Abaqus/CAE User’s Manual Overview In a mechanical contact simulation the interaction between contacting bodies is defined by assigning a contact property model to a contact interaction . Mechanical contact property models: • may include a constitutive model for the contact pressure-overclosure relationship that governs the motion of the surfaces; • may include a damping model that defines forces resisting the relative motions of the contacting surfaces; • may include a friction model that defines the force resisting the relative tangential motion of the surfaces; • may include a constitutive model in which you define the normal and tangential behavior in user subroutine UINTER in Abaqus/Standard; • may include a constitutive model in which you define the normal and tangential behavior in user subroutine VUINTER in Abaqus/Explicit when using the contact pair algorithm; • may include a constitutive model in which you define the normal and tangential behavior in user subroutine VUINTERACTION in Abaqus/Explicit when using the general contact algorithm; • in Abaqus/Standard may include a constitutive model for the penetration of fluid between two contacting surfaces; • in Abaqus/Standard may include a constitutive model for the interaction of debonded surfaces; • in Abaqus/Explicit may include a constitutive model that simulates the failure of bonds connecting the interacting bodies; and • may include surface-based cohesive behavior that allows modeling of delamination of bonds or “sticky” contact using progressive damage evolution models. This section provides a general outline of how to define the components of a mechanical contact property model. Specific details about the different components of the contact property models and the algorithms used for the contact calculations are found in other sections of this chapter. Defining the contact property model There are different methods for defining the components of a mechanical contact property model. Defining the contact pressure-overclosure relationship The default contact pressure-overclosure relationship used by Abaqus is referred to as the “hard” contact model. Hard contact implies that: • the surfaces transmit no contact pressure unless the nodes of the slave surface contact the master surface; • no penetration is allowed at each constraint location (depending on the constraint enforcement method used, this condition will either be strictly satisfied or approximated); • there is no limit to the magnitude of contact pressure that can be transmitted when the surfaces are in contact. You can define a nondefault pressure-overclosure relationship for a surface interaction. The various pressure-overclosure relationships available in Abaqus are discussed in “Contact pressure-overclosure relationships,” Section 36.1.2, and the constraint methods available to enforce these relationships are discussed in “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2. Defining a surface interaction model with damping between the surfaces You can define damping forces to oppose the relative motion between the interacting surfaces. In Abaqus/Standard the specified contact damping affects the motion in the normal direction only, whereas in Abaqus/Explicit contact damping can affect both the relative tangential motion and the motion normal to the surfaces. The details of the contact damping model are discussed in “Contact damping,” Section 36.1.3. Defining contact blockage in Abaqus/Explicit In Abaqus/Explicit you can control the combination of surfaces that can cause blockage of flow out of a surface-based fluid cavity. The details of contact blockage are discussed in “Contact blockage,” Section 36.1.4. Defining a friction model By default, Abaqus assumes that contact between surfaces is frictionless. You can include a friction model as part of a surface interaction definition. Details of the various friction models available in Abaqus are discussed in “Frictional behavior,” Section 36.1.5. User-defined interfacial constitutive behavior Instead of choosing one or some combination of the various interfacial behavior models that are available in Abaqus, you can define any special or proprietary interfacial constitutive behavior through a user subroutine. In Abaqus/Standard you can use the subroutine UINTER; whereas in Abaqus/Explicit you can use VUINTER if you are using the contact pair algorithm and VUINTERACTION if you are using the general contact algorithm. In Abaqus/Explicit a penalty enforcement of the contact constraint must be used for interacting surfaces whose interfacial behavior is governed by VUINTER or VUINTERACTION. Details of the definition of a user-defined interfacial constitutive behavior are discussed in “User- defined interfacial constitutive behavior,” Section 36.1.6. Defining a pressure penetration load in Abaqus/Standard You can define pressure penetration loads to simulate the penetration of fluid between two contacting surfaces in Abaqus/Standard. The details of the pressure penetration model are discussed in “Pressure penetration loading,” Section 36.1.7. Defining the interaction of debonded surfaces in Abaqus/Standard You can allow two initially bonded surfaces to debond in Abaqus/Standard, as discussed in “Crack propagation analysis,” Section 11.4.3. The details of the contact interaction model after debonding are discussed in “Interaction of debonded surfaces,” Section 36.1.8. Defining breakable bonds in Abaqus/Explicit In Abaqus/Explicit you can define breakable bonds that connect the interacting surfaces. The kinematic contact pair algorithm must be used when defining breakable bonds. The breakable bonds affect both the relative tangential motion and the motion normal to the surfaces. Breakable bonds cannot be used with analytical rigid surfaces. The details of the breakable bond model, known as the spot weld model, are discussed in “Breakable bonds,” Section 36.1.9. Defining surface-based cohesive behavior You can define surface-based cohesive behavior to model delamination of initially bonded surfaces or to model “sticky” contact between parts that are initially separated but bond on coming into contact, with the possibility that the bond may undergo progressive damage and fail. Surface-based cohesive behavior framework in Abaqus/Explicit and within the contact pair framework in Abaqus/Standard. The details of the surface-based cohesive behavior model are discussed in “Surface-based cohesive behavior,” Section 36.1.10. is modeled within the general contact CONTACT PRESSURE-OVERCLOSURE RELATIONSHIPS CONTACT PRESSURE-OVERCLOSURE Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Mechanical contact properties: overview,” Section 36.1.1 • *CONTACT CONTROLS • *SURFACE BEHAVIOR • “Creating interaction properties,” Section 15.12.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Customizing contact controls,” Section 15.12.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview In Abaqus the following contact pressure-overclosure relationships can be used to define the contact model: • the “hard” contact relationship minimizes the penetration of the slave surface into the master surface at the constraint locations and does not allow the transfer of tensile stress across the interface; • a “softened” contact relationship in which the contact pressure is a linear function of the clearance between the surfaces; • a “softened” contact relationship in which the contact pressure is an exponential function of the clearance between the surfaces (in Abaqus/Explicit this relationship is available only for the contact pair algorithm); • a “softened” contact relationship in which a tabular pressure-overclosure curve is constructed by progressively scaling the default penalty stiffness (available only for general contact in Abaqus/Explicit); • a “softened” contact relationship in which the contact pressure is a piecewise linear (tabular) function of the clearance between the surfaces; and • a relationship in which there is no separation of the surfaces once they contact. In addition, a viscous damping relationship can be defined that will affect the pressure-overclosure relationship; see “Contact damping,” Section 36.1.3, for more information. In Abaqus/Standard pressure penetration loads can be applied to model fluid penetrating into the surface between two contacting bodies; see “Pressure penetration loading,” Section 36.1.7. Including a contact pressure-overclosure relationship in a contact property definition By default, a “hard” contact pressure-overclosure relationship is used for both surface-based contact and element-based contact. You can include a nondefault contact pressure-overclosure relationship in a specific contact property definition. Input File Usage: Abaqus/CAE Usage: the Use both of the following options for surface-based contact: *SURFACE INTERACTION, NAME=interaction_property_name *SURFACE BEHAVIOR Use both of Abaqus/Standard: *INTERFACE or *GAP, ELSET=name *SURFACE BEHAVIOR Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Default following options for element-based contact in Element-based contact is not supported in Abaqus/CAE. Using the “hard” contact relationship The most common contact pressure-overclosure relationship is shown in Figure 36.1.2–1, although the zero-penetration condition may or may not be strictly enforced depending on the constraint enforcement method used (the constraint enforcement methods are discussed in “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2, and “Contact constraint enforcement methods in Abaqus/Explicit,” Section 37.2.3). When surfaces are in contact, any contact pressure can be transmitted between them. The surfaces separate if the contact pressure reduces to zero. Separated surfaces come into contact when the clearance between them reduces to zero. Input File Usage: *SURFACE BEHAVIOR (omit parameter to obtain the default “hard” pressure-overclosure relationship) the PRESSURE-OVERCLOSURE Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Default: Pressure-Overclosure: Hard Contact Using a “softened” contact relationship Three types of “softened” contact relationships are available in Abaqus. The pressure-overclosure relationship can be prescribed by using a linear law, a tabular piecewise-linear law, or an exponential law (in Abaqus/Explicit available only with the contact pair algorithm). For contact involving element-based surfaces and for element-based contact (available only in Abaqus/Standard), the “softened” contact relationships are specified in terms of overclosure (or clearance) versus contact pressure. For contact involving a node-based surface or nodal contact elements (such as GAP and ITT elements) for which an area or length dimension is not defined, softened contact is specified in terms of overclosure (or clearance) versus contact force. For slave surfaces on Contact pressure Any pressure possible when in contact No pressure when no contact Clearance Figure 36.1.2–1 Default pressure-overclosure relationship. beam-type elements in Abaqus/Standard and for the contact pair algorithm in Abaqus/Explicit, specify pressure as force per unit length. If the general contact algorithm in Abaqus/Explicit is being used for slave surfaces on beam-type elements, specify pressure as force per unit area. When using softened contact relationships that have nonzero pressure at zero overclosure (not allowed with the general contact algorithm) in Abaqus/Explicit, you should be aware that initial, nonequilibrated contact pressures may be present in the analysis . “Softened” contact versus “hard” contact The “softened” contact pressure-overclosure relationships might be used to model a soft, thin layer on one or both surfaces. In Abaqus/Standard they are also sometimes useful for numerical reasons because they can make it easier to resolve the contact condition. Using “softened” contact in implicit dynamic simulations Use the softened contact relationship with caution in implicit dynamic impact simulations. If this relationship is used in such a simulation, Abaqus/Standard will not use the impact algorithm, which destroys kinetic energy of the nodes on the surface when impact occurs, but will instead assume a perfectly elastic collision. The consequence of this change is that the slave nodes bounce back immediately after impact with the master surface; hence, extensive “chattering” may result, leading to convergence problems and small time increments. However, softened contact may work well in implicit dynamic calculations where impact effects are not important; for example, if contact changes are primarily due to sliding motion along a curved surface, such as may occur in low-speed metal forming applications. Using “softened” contact in explicit dynamic simulations In Abaqus/Explicit softened contact can be enforced with either the kinematic or the penalty constraint enforcement method . With penalty enforcement the contact collisions are elastic except for the influence of contact damping, whereas with softened kinematic contact some energy will be absorbed by the impact because of algorithmic characteristics: the energy absorbed tends to increase as the contact stiffness increases. Another consideration is the effect on the time increment: with kinematic enforcement the stable time increment is independent of the contact stiffness, but with penalty contact the time increment decreases as the contact stiffness increases. “Softened” contact defined as a linear function In a linear pressure-overclosure relationship the surfaces transmit contact pressure when the overclosure between them, measured in the contact (normal) direction, is greater than zero. The linear pressure- overclosure relationship is identical to a tabular relationship with two data points, where the first point is located at the origin. You specify the slope of the pressure-overclosure relationship, k. Input File Usage: Abaqus/CAE Usage: *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=LINEAR Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Default: Pressure-Overclosure: Linear, Contact stiffness: k “Softened” contact defined in tabular form form, as shown in To define a piecewise-linear pressure-overclosure relationship in tabular Figure 36.1.2–2, you specify data pairs ( ) of pressure versus overclosure (where overclosure corresponds to negative clearance). You must specify the data as an increasing function of pressure and overclosure. In this relationship the surfaces transmit contact pressure when the overclosure between them, measured in the contact (normal) direction, is greater than is the overclosure at zero pressure. For the general contact algorithm in Abaqus/Explicit must be zero. For overclosures greater than the pressure-overclosure relationship is extrapolated based on the last slope computed from the user-specified data . , where , Input File Usage: Abaqus/CAE Usage: *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=TABULAR Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Default: Pressure-Overclosure: Tabular “Softened” contact defined as a geometric scaling of the default contact stiffness An alternative piecewise linear tabular pressure-overclosure relationship can be constructed by geometrically scaling the default contact stiffness. This model provides a simple interface to increase the default contact stiffness when a critical penetration is exceeded. A penetration measure, , is Pressure p (pn,hn) (p3,h3) (p2,h2) (0,h1) Clearance c Overclosure h Figure 36.1.2–2 “Softened” pressure-overclosure relationship defined in tabular form. defined either directly or as a fraction, , in the contact region. Each time the current penetration exceeds a multiple of this penetration measure, the contact stiffness is scaled by a factor, . The initial stiffness is set equal to the default contact stiffness, , of the minimum element length, , multiplied by a factor, . Pressure dflt elem = segment number = default stiffness = element length = initial scale factor = geometric scale factor = overclosure factor = r L = overclosure measure elem segment i Ki = s0 k dflt si-1 1 0 (i -1) d i d Overclosure Figure 36.1.2–3 “Softened” scale factor pressure-overclosure relationship. This option is available only for the general contact algorithm in Abaqus/Explicit. Input File Usage: Abaqus/CAE Usage: *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=SCALE FACTOR Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Default: Pressure-Overclosure: Scale Factor (General Contact) “Softened” contact defined with an exponential law In an exponential (soft) contact pressure-overclosure relationship the surfaces begin to transmit contact pressure once the clearance between them, measured in the contact (normal) direction, reduces to . The contact pressure transmitted between the surfaces then increases exponentially as the clearance continues to diminish. Figure 36.1.2–4 illustrates this behavior in Abaqus/Standard. In Abaqus/Explicit this behavior is available only for the contact pair algorithm. Contact pressure Exponential pressure-overclosure relationship p 0 Clearance c 0 Figure 36.1.2–4 Exponential “softened” pressure-overclosure relationship in Abaqus/Standard. In Abaqus/Explicit you can specify an optional limit on the contact stiffness that the model can attain, ; this limit is useful for penalty contact to mitigate the effect that large will be set to infinity for stiffnesses have on reducing the stable time increment. By default, kinematic contact and to the default penalty stiffness for penalty contact. You specify ; the contact pressure at zero clearance, ; and, optionally in Abaqus/Explicit, . Input File Usage: *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=EXPONENTIAL , , Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Default: Pressure-Overclosure: Exponential, Pressure , Clearance , Specify: 36.1.2–6 Contact pressure Kmax Exponential pressure-overclosure relationship p0 Clearance c0 Overclosure Figure 36.1.2–5 Exponential “softened” pressure-overclosure relationship in Abaqus/Explicit. Using the no separation relationship You can indicate that Abaqus should use the contact pressure-overclosure relationship that prevents surfaces from separating once they have come into contact. In Abaqus/Explicit this relationship can be specified only for pure master-slave contact pairs and cannot be used with adaptive meshing or with the general contact algorithm. The no separation relationship is often used with the rough friction model to model nonintermittent, rough frictional contact. Using this combination of surface interaction models causes surfaces to remain fully bonded together (no separation and no tangential sliding) once they contact, even if the contact pressure between them is tensile. Input File Usage: Abaqus/CAE Usage: *SURFACE BEHAVIOR, NO SEPARATION Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Default: Pressure-Overclosure: Hard, toggle off Allow separation after contact “Softened” contact with the no separation relationship in Abaqus/Explicit In Abaqus/Explicit if a softened contact relationship is specified with the no separation relationship, the pressure-overclosure relationship will include tensile behavior. The exponential relationship cannot be used with no separation behavior. For the tabular relationship, a point must be specified on the zero pressure axis, and the slope will continue into the tensile regime following the same slope as the first two data points . The linear relationship will have a linear tensile pressure-overclosure relationship with the same slope that is used for the compressive behavior. pressure p (compressive) (pn,hn) clearance c (0,hi) overclosure h (p2,h2) (p1,h1) (tensile) Figure 36.1.2–6 Piecewise linear “softened” pressure-overclosure relationship with tensile behavior in Abaqus/Explicit. Surface interaction output variables related to the contact pressure-overclosure Abaqus/Standard provides both the clearance, COPEN, and the contact pressure, CPRESS, as output to the data, results, and output database files. Output to these files is requested as described in “Output to the data and results files,” Section 4.1.2, and “Output to the output database,” Section 4.1.3. Abaqus/Explicit provides the contact pressure, CPRESS, as output to the output database file . In the data, results, and output database files the output variable CPRESS gives the viscous damping pressures for an open slave node. This variable also gives the contact pressure for a closed slave node. In printed output a “VD” status indicates that the forces are for viscous damping. Contours of the contact pressure on the slave surface can be plotted in Abaqus/CAE. 36.1.3 CONTACT DAMPING Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Mechanical contact properties: overview,” Section 36.1.1 • *CONTACT DAMPING • “Creating interaction properties,” Section 15.12.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Contact damping: • can be defined to oppose the relative motion between the interacting surfaces (in addition to the contact pressure-overclosure relationships discussed in “Contact pressure-overclosure relationships,” Section 36.1.2, and the friction models discussed in “Frictional behavior,” Section 36.1.5); • can affect both the motion normal and tangential to the surfaces; • in the normal direction is proportional to the relative velocity between the surfaces; • in the tangential direction is proportional to the relative tangential velocity in Abaqus/Standard and to the “elastic slip rate” associated with friction in Abaqus/Explicit—hence, in Abaqus/Explicit it does not resist the bulk of tangential sliding; • is not applicable for linear perturbation procedures; • in Abaqus/Standard it contributes to the force and stiffness definition and should generally be used only when it is otherwise impossible to obtain a solution—the best method for allowing a viscous pressure and shear stress to be transmitted between the contact surfaces in Abaqus/Standard to reduce convergence difficulties due to the sudden violation of contact constraints (common in some snap-through and buckling problems involving contact) is to specify the damping on a step-by-step basis using contact controls, as discussed in “Automatic stabilization of rigid body motions in contact problems” in “Adjusting contact controls in Abaqus/Standard,” Section 35.3.6; and • can be useful in Abaqus/Explicit to reduce solution noise—a small amount of viscous contact damping is used by default for softened contact and penalty contact in Abaqus/Explicit, as discussed below. Defining viscous contact damping for relative motions of surfaces In Abaqus/Standard the damping coefficient, is a function of surface clearance, as shown in , Figure 36.1.3–1. The damping coefficient is defined as a proportionality constant with units of pressure divided by velocity. Damping coefficient Clearance co co Figure 36.1.3–1 Damping coefficient-clearance relationship for viscous damping in Abaqus/Standard. In Abaqus/Explicit the damping coefficient will remain at the specified constant value while the surfaces are in contact and at zero otherwise. The damping coefficient can be defined as a proportionality constant with units of pressure divided by velocity or as a unitless fraction of critical damping. To define viscous damping, you must include it in a contact property definition. Input File Usage: Use both of the following options for surface-based contact: *SURFACE INTERACTION, NAME=interaction_property_name *CONTACT DAMPING Use both of Abaqus/Standard: following options the for element-based contact in Abaqus/CAE Usage: *INTERFACE or *GAP, ELSET=name *CONTACT DAMPING Interaction module: contact property editor: Mechanical→Damping Element-based contact is not supported in Abaqus/CAE. Damping and pressure-overclosure relationships In Abaqus/Standard the viscous damping relationship can be used with any contact relationship . In Abaqus/Explicit contact damping is not available for hard kinematic contact. Softened kinematic contact and all penalty contact will have default damping in the form of a critical damping fraction with = 0.03. Specifying the damping coefficient such that the damping force is directly proportional to the rate of relative motion between the surfaces You can specify damping directly in terms of the damping coefficient with units of pressure per velocity such that the damping forces will be calculated with is the rate of relative motion between the two surfaces. , where A is the nodal area and For contact involving element-based surfaces and for element-based contact (available only in Abaqus/Standard), the damping coefficient is specified in terms of contact pressure. For contact involving a node-based surface or nodal contact elements (such as GAP elements and ITT elements) for which an area or length dimension has not been defined, must be specified as force per velocity. For slave surfaces on beam-type elements, specify as force per unit length per velocity. Input File Usage: Use the following syntax in Abaqus/Standard: *CONTACT DAMPING, DEFINITION=DAMPING COEFFICIENT , , Use the following syntax in Abaqus/Explicit: *CONTACT DAMPING, DEFINITION=DAMPING COEFFICIENT Abaqus/CAE Usage: Use the following syntax in Abaqus/Standard: Interaction module: contact property editor: Mechanical→Damping: Definition: Damping coefficient, Linear or Bilinear, Damping Coeff. , Clearance c and ( =0 for Linear and for Bilinear) Use the following syntax in Abaqus/Explicit: Interaction module: contact property editor: Mechanical→Damping: Definition: Damping coefficient, Step, Damping Coeff. Specifying the damping coefficient as a fraction of critical damping in Abaqus/Explicit In Abaqus/Explicit you can specify a unitless damping coefficient in terms of the fraction of critical damping associated with the contact stiffness; this method is not available in Abaqus/Standard. The damping forces will be calculated with is the nodal contact stiffness (in units of is the rate of relative motion between the two surfaces. , where m is the nodal mass, ), and Input File Usage: *CONTACT DAMPING, DEFINITION=CRITICAL DAMPING FRACTION critical damping fraction Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Damping: Definition: Critical damping fraction, Crit. Damping Fraction critical damping fraction Specifying the tangential damping coefficient You can specify the ratio of the tangential damping coefficient to the normal damping coefficient, also called the tangent fraction. The tangential damping uses the same form of damping as the normal damping. Tangential If tangential damping is damping can be specified only in conjunction with normal damping. activated in Abaqus/Standard, the damping stress is proportional to the relative tangential velocity. In Abaqus/Explicit tangential damping will be ignored if hard kinematic contact is used in the tangential direction or if friction is not defined. As stated previously, damping in the tangential direction in Abaqus/Explicit is proportional to the elastic slip rate rather than the total rate of relative sliding. For Abaqus/Standard the default value for the tangent fraction is 0.0; therefore, by default, the damping coefficient for the tangential direction is zero. For Abaqus/Explicit the default value for the tangent fraction is 1.0; therefore, by default, the damping coefficient for the tangential direction is equal to the damping coefficient for the normal direction. Furthermore, in Abaqus/Explicit softened contact and hard penalty contact have a default critical damping fraction of 0.03. Input File Usage: Abaqus/CAE Usage: *CONTACT DAMPING, TANGENT FRACTION=value Interaction module: contact property editor: Mechanical→Damping: Tangent fraction: Specify value: value Choosing the appropriate coefficients for viscous damping in Abaqus/Standard In Abaqus/Standard the appropriate magnitude for the local contact damping factor, , is problem- dependent. In some cases a simple calculation can be used to determine the magnitude; in other cases a reasonable value for must be determined by trial and error. A reasonable value is one that has minimal impact on the solution prior to the unstable behavior in the model. A preliminary value can be found by looking at the contact pressures and velocities in the model before damping is added, as described below. It may be difficult to determine the nodal velocities prior to the unstable behavior if output was not requested frequently. In such a situation the information in the message (.msg) file can be used to estimate the peak nodal velocity. By default, Abaqus/Standard provides the peak nodal displacement increment at every converged increment in this file. This displacement increment can be used along with the time increment to calculate a peak nodal velocity for the model. Although this velocity may not be very close to the actual relative velocity of the surfaces, it should be within an order of magnitude and is a reasonable value to use in calculating an initial viscous damping coefficient. The maximum contact pressure between the surfaces also needs to be estimated. The viscous damping coefficient should then be set to a value that is a few orders of magnitude less than the ratio of the estimated maximum contact pressure over the calculated nodal velocity. If it is not feasible to obtain the pressure and velocities as discussed above, a high damping value should be used initially and repeated analyses should be performed with smaller and smaller values. An appropriate value for is one that is large enough to enable the analysis to get past any unstable response but not so large that the results at earlier or later times are affected significantly. “Snap-through buckling analysis of circular arches,” Section 1.2.1 of the Abaqus Example Problems Manual, demonstrates how the magnitude of the damping coefficient can be determined using the methods explained above. The following example outlines how the value might be chosen for a typical case. Consider a simple modification to the two-dimensional Euler column buckling problem: add rigid surfaces parallel and on either side of the column so that the beam will contact the surfaces when it buckles. As the axial load is of contact will lift off the surface and the beam will buckle into a higher mode. Figure 36.1.3–2 shows this shape. CONTACT DAMPING Figure 36.1.3–2 Constrained Euler buckling example for viscous damping. When the column first buckles, the contact force, F, that the column exerts on one of the rigid surfaces can be approximated as where h is the separation distance between the rigid surfaces, l is the beam length, P is the applied load, and is the buckling load. The approximation of the contact force entails the assumption that a single point comes into contact and that the shape of the buckled column does not change. The units of are contact force per velocity, assuming that a node-based surface is used in this model. The velocity of the column, v, at the point of contact can be approximated as where value for the damping coefficient: is the time increment. These estimates for the contact force and the column velocity give a This value can be used as a starting value, but different values should be tested. 36.1.4 CONTACT BLOCKAGE Product: Abaqus/Explicit References • “Mechanical contact properties: overview,” Section 36.1.1 • “Surface-based fluid cavities: overview,” Section 11.5.1 • “Fluid exchange definition,” Section 11.5.3 • *BLOCKAGE • *FLUID EXCHANGE ACTIVATION • *SURFACE INTERACTION Overview The blockage of flow out of a cavity due to an obstruction caused by contacting surfaces: • can be defined selectively for particular surfaces that may fully or partially cause the blockage; and • can be accounted for only when the surfaces are used with the general contact algorithm. Surfaces used to account for contact blockage To consider an obstruction by contacting surfaces as discussed in “Accounting for blockage due to contacting boundary surfaces” in “Fluid exchange definition,” Section 11.5.3, you must define a surface to represent the leakage area on the boundary of the fluid cavity. In addition, you must specify that the contacting surfaces can potentially cause blockage. All the surfaces (the surface on the boundary of the fluid cavity and the contacting surfaces) must be included in a general contact domain. To account for contact blockage, the nodes on the surfaces must be in node-to-face contact. When the nodes on the surface on the boundary of the fluid cavity come into contact with the contacting surfaces, the slave nodes are marked as active nodes for contact blockage. The contact blockage is also considered in the edge-to-edge contact . Input File Usage: Use the following options to specify that two contacting surfaces can cause blockage: *CONTACT PROPERTY ASSIGNMENT surface_1, surface_2, property_name *SURFACE INTERACTION, NAME=property_name *BLOCKAGE Determining the obstruction area Abaqus/Explicit determines the obstruction area by calculating the area fraction of the surface on the boundary of the fluid cavity that is not blocked by contacting surfaces. For each element face of this surface representing the leakage area, the blocked area is calculated based on the active nodes for contact blockage. The element blocked area is determined by is the element area, is the element blocked area, is the total number of element nodes, where and is the total number of active nodes for contact blockage in the element. The element is fully blocked by the contacting surfaces when all element nodes are active for contact blockage. The total obstruction area is the sum of all the element blocked areas. The leakage area used in the fluid exchange calculation is obtained by subtracting the total obstruction area from the total area of the surface if the effective area is not specified for the fluid exchange. If both the effective area and a surface are specified , the leakage area used in the fluid exchange calculation is obtained by using the ratio of the total obstruction area to the total area of the surface multiplied by the effective area. In this case a node-based surface can be used, and the leakage area is obtained by using the ratio of the total active contact blockage nodes to the total number of nodes defined in the surface. 36.1.5 FRICTIONAL BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Mechanical contact properties: overview,” Section 36.1.1 • “FRIC,” Section 1.1.8 of the Abaqus User Subroutines Reference Manual • “FRIC_COEF,” Section 1.1.9 of the Abaqus User Subroutines Reference Manual • “VFRIC,” Section 1.2.4 of the Abaqus User Subroutines Reference Manual • “VFRIC_COEF,” Section 1.2.5 of the Abaqus User Subroutines Reference Manual • “VFRICTION,” Section 1.2.6 of the Abaqus User Subroutines Reference Manual • *FRICTION • *CHANGE FRICTION • “Creating interaction properties,” Section 15.12.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview When surfaces are in contact they usually transmit shear as well as normal forces across their interface. There is generally a relationship between these two force components. The relationship, known as the friction between the contacting bodies, is usually expressed in terms of the stresses at the interface of the bodies. The friction models available in Abaqus: • include the classical isotropic Coulomb friction model , which in Abaqus: – in its general form allows the friction coefficient to be defined in terms of slip rate, contact pressure, average surface temperature at the contact point, and field variables; and – provides the option for you to define a static and a kinetic friction coefficient with a smooth transition zone defined by an exponential curve; • allow the introduction of a shear stress limit, , which is the maximum value of shear stress that can be carried by the interface before the surfaces begin to slide; • include an anisotropic extension of the basic Coulomb friction model in Abaqus/Standard; • include a model that eliminates frictional slip when surfaces are in contact; • include a “softened” interface model for sticking friction in Abaqus/Explicit in which the shear stress is a function of elastic slip; • can be implemented with a stiffness (penalty) method, a kinematic method (in Abaqus/Explicit), or a Lagrange multiplier method (in Abaqus/Standard), depending on the contact algorithm used; and • can be defined in user subroutines FRIC or FRIC_COEF (in Abaqus/Standard) or VFRIC, VFRICTION, or VFRIC_COEF (in Abaqus/Explicit). In Abaqus/Standard tangential damping forces can be introduced proportional to the relative tangential velocity, while in Abaqus/Explicit tangential damping forces can be introduced proportional to the rate of relative elastic slip between the contacting surfaces . Including friction properties in a contact property definition Abaqus assumes by default that the interaction between contacting bodies is frictionless. You can include a friction model in a contact property definition for both surface-based contact and element-based contact. Input File Usage: Abaqus/CAE Usage: the Use both of the following options for surface-based contact: *SURFACE INTERACTION, NAME=interaction_property_name *FRICTION Use both of Abaqus/Standard: *INTERFACE or *GAP, ELSET=name *FRICTION Interaction module: contact property editor: Mechanical→Tangential Behavior following options for element-based contact in Changing friction properties during an analysis Element-based contact is not supported in Abaqus/CAE. The methods used to change friction properties during an analysis differ between Abaqus/Standard and Abaqus/Explicit. Changing friction properties during an Abaqus/Standard analysis It is possible to remove, to modify, or to add a friction model that does not involve a user subroutine to a contact property definition in any particular step of an Abaqus/Standard simulation. In some models, such as shrink-fit contact interference problems, friction should not be added until after the first steps have been completed. In other models friction might be removed or lowered to represent the introduction of a lubricant between the bodies. You must identify which contact property definition or contact element set is being changed. Input File Usage: Abaqus/CAE Usage: Use both of the following options for surface-based contact: *CHANGE FRICTION, INTERACTION=name *FRICTION Use both of the following options for element-based contact: *CHANGE FRICTION, ELSET=name *FRICTION Define a contact property with a new friction definition. Then change the contact property assigned to an interaction in a particular step. Interaction module: Contact property editor: Mechanical→Tangential Behavior Interaction editor: Contact interaction property: new_interaction_property_name Element-based contact is not supported in Abaqus/CAE. Specifying the time variation of the change in friction properties You can specify an amplitude curve to define the time variation of changes in friction coefficients and, if applicable, allowable elastic slip throughout the step. If you do not specify an amplitude curve, changes in these friction properties are either applied immediately at the beginning of the step or ramped up linearly over the step, depending on the default amplitude variation assigned to the step , with some exceptions as described below. For many step types the default transition type is a linear ramping from old to new values, which helps avoid convergence problems that can occur upon sudden changes in friction properties. Amplitude curves used to control variations in friction properties are subjected to the following restrictions: • a tabular or smooth step amplitude definition must be used, • only amplitudes with monotonically increasing values between 0.0 and 1.0 are accepted, and • the amplitude must be defined in terms of step time and using relative magnitudes. The value of a friction coefficient or allowable elastic slip in effect at a given time is typically equal to the value of the property at the start of the step plus the current amplitude value times the anticipated change in property value over the step. Variations in friction properties must consider the following: • Changes in the type of frictional constraint enforcement method (penalty or Lagrange multiplier methods), changes between a “rough” friction model and a finite friction coefficient, and changes to friction properties other than the friction coefficient or allowable elastic slip always occur at the beginning of a step. • If a friction coefficient is dependent on slip rate, contact pressure, average surface temperature at the contact point, or field variables, the estimate of the final value of the friction coefficient for the step (which is used in calculating the anticipated change in the friction coefficient over the step) assumes that the current slip rate, contact pressure, etc. will remain in effect at the end of the step. • If a friction coefficient is changed during the first step of an analysis, its value at the start of the step is equal to zero for this calculation, regardless of the original friction definition in the model. • Changes in allowable elastic slip always occur at the beginning of a step when an exponential-decay friction model is used or when frictional properties are changed during the first general step or during a steady-state transport step that is preceded by a step type other than steady-state transport. Input File Usage: Abaqus/CAE Usage: *CHANGE FRICTION, AMPLITUDE=name Time-dependent changes Abaqus/CAE. in friction properties are not supported in Resetting the frictional properties to their default values You can reset the frictional properties of the specified contact property definition or element set to their original values. Input File Usage: Abaqus/CAE Usage: Use either of the following options: *CHANGE FRICTION, RESET, INTERACTION=name *CHANGE FRICTION, RESET, ELSET=name In this case the *FRICTION option is not needed. Interaction module: Contact property editor: Mechanical→Tangential Behavior: Friction formulation: Frictionless Interaction editor: Contact interaction property: default_interaction_property_name Changing friction properties during an Abaqus/Explicit analysis In Abaqus/Explicit the friction definition is specified as part of the model definition for a general contact analysis and as part of the history definition for a contact pair analysis. See “Assigning contact properties for general contact in Abaqus/Explicit,” Section 35.4.3, and “Assigning contact properties for contact pairs in Abaqus/Explicit,” Section 35.5.3, for information on changing aspects of any contact property definition during an Abaqus/Explicit analysis. Using the basic Coulomb friction model The basic concept of the Coulomb friction model is to relate the maximum allowable frictional (shear) stress across an interface to the contact pressure between the contacting bodies. In the basic form of the Coulomb friction model, two contacting surfaces can carry shear stresses up to a certain magnitude across their interface before they start sliding relative to one another; this state is known as sticking. The Coulomb friction model defines this critical shear stress, , at which sliding of the surfaces starts as a fraction of the contact pressure, p, between the surfaces ( ). The stick/slip calculations determine when a point transitions from sticking to slipping or from slipping to sticking. The fraction, , is known as the coefficient of friction. For the case when the slave surface consists of a node-based surface, the contact pressure is equal to the normal contact force divided by the cross-sectional area at the contact node. In Abaqus/Standard the default cross-sectional area is 1.0; you can specify a cross-sectional area associated with every node in the node-based surface when the surface is defined or, alternatively, assign the same area to every node through the contact property definition. In Abaqus/Explicit the cross-sectional area is always 1.0, and you cannot change it. The basic friction model assumes that is the same in all directions (isotropic friction). For a three-dimensional simulation there are two orthogonal components of shear stress, , along the interface between the two bodies. These components act in the slip directions for the contact surfaces or contact elements. The slip directions for contact surfaces are defined in “Contact formulations in and Abaqus/Standard,” Section 37.1.1, and those for contact elements are defined in the sections describing contact modeling with those elements. Abaqus combines the two shear stress components into an “equivalent shear stress,” . , for the stick/slip calculations, where In addition, Abaqus combines the two slip velocity components into an equivalent slip rate, . The stick/slip calculations define a surface in the contact pressure–shear stress space along which a point transitions from sticking to slipping. equivalent shear stress critical shear stress in default model stick region μ (constant friction coefficient) contact pressure Figure 36.1.5–1 Slip regions for the basic Coulomb friction model. There are two ways to define the basic Coulomb friction model in Abaqus. In the default model the friction coefficient is defined as a function of the equivalent slip rate and contact pressure. Alternatively, you can specify the static and kinetic friction coefficients directly. Using the default model In the default model you define the coefficient of friction directly as , , , and is the equivalent slip rate, p is the contact pressure, where at the contact point, and is the average temperature at the contact point. is the average predefined field variable are the temperature and predefined field variables at points A and B on the surfaces. Point A is a node on the slave surface, and point B corresponds to the nearest point on the opposing master surface. The temperature and field variables are interpolated along the surface at location B. If the master surface consists of a rigid body, the temperature and field variable at the reference node are used. Dependence on is not available with the general contact algorithm in Abaqus/Explicit. and The friction coefficient can depend on slip rate, contact pressure, temperature, and field variables. By default, it is assumed that the friction coefficients do not depend on field variables. The coefficient of friction can be set to any nonnegative value. A zero friction coefficient means that no shear forces will develop and the contact surfaces are free to slide. You do not need to define a friction model for such a case. Input File Usage: *FRICTION, DEPENDENCIES=n , , p, , Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: Penalty: Friction If necessary, toggle on Use slip-rate-dependent data, Use contact- pressure-dependent data, and/or Use temperature-dependent data; and/or specify the Number of field variable dependencies in addition to slip rate, contact pressure, and temperature. Specifying static and kinetic friction coefficients Experimental data show that the friction coefficient that opposes the initiation of slipping from a sticking condition is different from the friction coefficient that opposes established slipping. The former is typically referred to as the “static” friction coefficient, and the latter is referred to as the “kinetic” friction coefficient. Typically, the static friction coefficient is higher than the kinetic friction coefficient. In the default model the static friction coefficient corresponds to the value given at zero slip rate, and the kinetic friction coefficient corresponds to the value given at the highest slip rate. The transition between static and kinetic friction is defined by the values given at intermediate slip rates. In this model the static and kinetic friction coefficients can be functions of contact pressure, temperature, and field variables. Abaqus also provides a model to specify a static and a kinetic friction coefficient directly. In this model it is assumed that the friction coefficient decays exponentially from the static value to the kinetic value according to the formula: is the kinetic friction coefficient, where is a user-defined decay is the static friction coefficient, coefficient, and is the slip rate . This model can be used only with isotropic friction and does not allow dependence on contact pressure, temperature, or field variables. There are two ways of defining this model. Providing the static, kinetic, and decay coefficients directly You can provide the static friction coefficient, the kinetic friction coefficient, and the decay coefficient directly . μ = μ k + (μ s − μ k) e−dc eq eq Figure 36.1.5–2 Exponential decay friction model. Input File Usage: *FRICTION, EXPONENTIAL DECAY , , Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: Static-Kinetic Exponential Decay: Friction, Definition: Coefficients Using test data to fit the exponential model , Alternatively, you can provide test data points to fit the exponential model. At least two data points must be provided. The first point represents the static coefficient of friction specified at , and the second point, ( ) (shown in Figure 36.1.5–3), corresponds to an experimental measurement taken at a reference slip rate . An additional data point can be specified to characterize the exponential decay. If this additional data point is omitted, Abaqus will automatically provide a third data point, ( ), to model the assumed asymptotic value of the friction coefficient at infinite velocity. In such a case is chosen such that , . *FRICTION, EXPONENTIAL DECAY, TEST DATA Input File Usage: , Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: Static-Kinetic Exponential Decay: Friction, Definition: Test data (γ = 0, μ 1 = μ s) 1 (γ 2, μ 2) ∞ (γ 3 = γ ∞, μ 3 = μ = ∞ k) 1 = 0.0 eq Figure 36.1.5–3 Exponential decay friction model specified with test data points. Using the optional shear stress limit , so that, regardless of the magnitude of You can specify an optional equivalent shear stress limit, the contact pressure stress, sliding will occur if the magnitude of the equivalent shear stress reaches this value . A value of zero is not allowed. equivalent shear stress max critical shear stress in model with τ max limit μ (constant friction coefficient) stick region contact pressure Figure 36.1.5–4 Slip regions for the friction model with a limit on the critical shear stress. This shear stress limit is typically introduced in cases when the contact pressure stress may become very large (as can happen in some manufacturing processes), causing the Coulomb theory to provide a critical shear stress at the interface that exceeds the yield stress in the material beneath the contact surface. A reasonable upper bound estimate for is the Mises yield stress of the material adjacent to the surface; however, empirical data are the best source for . , where is Input File Usage: Abaqus/CAE Usage: *FRICTION, TAUMAX= Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: Penalty or Lagrange Multiplier: Shear Stress, Shear stress limit: Specify: Limitations with the shear stress limit In Abaqus/Explicit a shear stress limit cannot be used when a contact pair uses a node-based surface as one of the surfaces. Using the anisotropic friction model in Abaqus/Standard The anisotropic friction model available in Abaqus/Standard allows for different friction coefficients in the two orthogonal directions on the contact surface. These orthogonal directions coincide with the slip directions defined in “Contact formulations in Abaqus/Standard,” Section 37.1.1; and those for contact elements are described in the sections defining contact modeling with those elements. The orientation of the slip directions cannot be changed. If you indicate that the anisotropic friction model should be used, you must specify two friction is the coefficient of is the coefficient of friction in the first slip direction and coefficients, where friction in the second slip direction. The critical shear stress surface is an ellipse in extreme points being in contact pressure between the surfaces. The direction of slip, stress surface. and space with the two . The size of this ellipse will change with the change , is orthogonal to the critical shear – The friction coefficients can depend on slip rate, contact pressure, temperature, and field variables. By default, it is assumed that the friction coefficients do not depend on field variables. Input File Usage: *FRICTION, ANISOTROPIC, DEPENDENCIES=n , , , p, , Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: Penalty: Friction, Directionality: Anisotropic toggle on Use slip-rate-dependent data, Use contact- If necessary, pressure-dependent data, and/or Use temperature-dependent data; and/or specify the Number of field variable dependencies in addition to slip rate, contact pressure, and temperature. crit 2 = μ 2 P stick region crit 1 = μ 1 P direction of slip dγ Figure 36.1.5–5 Critical shear stress surface for the anisotropic friction model. Preventing slipping regardless of contact pressure Abaqus offers the option of specifying an infinite coefficient of friction ( ). This type of surface interaction is called “rough” friction, and with it all relative sliding motion between two contacting surfaces is prevented (except for the possibility of “elastic slip” associated with penalty enforcement) as long as the corresponding normal-direction contact constraints are active. In most cases Abaqus/Standard uses a penalty method to enforce these tangential constraints; however, a Lagrange multiplier method is used during general (non-perturbation) analysis steps if the corresponding normal-direction constraints have directly enforced “hard contact” or exponential pressure-overclosure behavior. Abaqus/Explicit uses either a kinematic or penalty method, depending on the contact formulation chosen. Rough friction is intended for nonintermittent contact; once surfaces close and undergo rough friction, they should remain closed. Convergence difficulties may arise in Abaqus/Standard if a closed contact interface with rough friction opens, especially if large shear stresses have developed. The rough friction model is typically used in conjunction with the no separation contact pressure-overclosure relationship for motions normal to the surfaces , which prohibits separation of the surfaces once they are closed. When rough friction is used with the no separation relationship for hard contact in Abaqus/Explicit specified with the kinematic contact method, no relative motions of the surfaces will occur. For hard contact in Abaqus/Explicit specified with the penalty contact method, relative motions will be limited to the elastic slip and penetration corresponding to the inexact satisfaction of the contact constraints by the applied penalty forces. When softened tangential behavior is specified in Abaqus/Explicit , the relative surface motions will be governed by the specified softening behavior. Input File Usage: Abaqus/CAE Usage: *FRICTION, ROUGH Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: Rough Shear stress versus elastic slip while sticking In some cases some incremental slip may occur even though the friction model determines that the current frictional state is “sticking.” In other words, the slope of the shear (frictional) stress versus total slip relationship may be finite while in the “sticking” state, as shown in Figure 36.1.5–6. shear stress sticking friction slipping friction crit total slip Figure 36.1.5–6 Elastic slip versus shear traction relationship for sticking and slipping friction. corresponds to Young’s modulus, and The relationship shown in this figure is analogous to elastic-plastic material behavior without hardening: corresponds to yield stress; sticking friction corresponds to the elastic regime, and slipping friction corresponds to the plastic regime. A finite value of the sticking stiffness may reflect a user-specified physical behavior or may be characteristic of the constraint enforcement method. Frictional constraints are enforced with a stiffness (penalty method) by default in Abaqus/Standard and for the general contact algorithm in Abaqus/Explicit; in this case the sticking stiffness will have a finite value. An infinite sticking stiffness, in which case the elastic slip is always zero, can be achieved with the optional Lagrange multiplier method for imposing frictional constraints in Abaqus/Standard In or with the kinematic constraint method (available only for contact pairs) in Abaqus/Explicit. Abaqus/Explicit some tangential contact damping acts on the elastic slip rate by default, as discussed in “Contact damping,” Section 36.1.3. Tangential softening to reflect a physical behavior is available only in Abaqus/Explicit. Defining tangential softening in Abaqus/Explicit To activate softened tangential behavior in Abaqus/Explicit, specify the slope of the shear stress versus in Figure 36.1.5–6). User subroutine VFRIC cannot be used in conjunction elastic slip relationship ( with softened tangential behavior. Input File Usage: Abaqus/CAE Usage: *FRICTION, SHEAR TRACTION SLOPE= Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: Penalty or Static-Kinetic Exponential Decay: Elastic Slip, Specify: Stiffness method for imposing frictional constraints in Abaqus/Standard The stiffness method used for friction in Abaqus/Standard is a penalty method that permits some relative motion of the surfaces (an “elastic slip”) when they should be sticking (similar to the allowable elastic slip defined with softened tangential behavior in Abaqus/Explicit). While the surfaces are sticking (i.e., ), the magnitude of sliding is limited to this elastic slip. Abaqus continually adjusts the magnitude of the penalty constraint to enforce this condition. The stiffness method in Abaqus/Standard requires the selection of an allowable elastic slip, . Using a large in the simulation makes convergence of the solution more rapid at the expense of solution accuracy (there is greater relative motion of the surfaces when they should be sticking). Behavior in which no slip is permitted in the sticking state is approximated more accurately by allowing only a small is chosen very small, convergence problems may occur; in that case, it may be better to use the Lagrange multiplier method to apply the sticking constraint . . If The default value of allowable elastic slip used by Abaqus/Standard generally works very well, providing a conservative balance between efficiency and accuracy. Abaqus/Standard calculates as a small fraction of the “characteristic contact surface length,” , and scans all of the facets of all the slave surfaces when calculating . Abaqus/Standard reports the value of used for each contact pair in the data (.dat) file if you request detailed printout of contact constraint information . The allowable elastic slip is given as , where is 0.005. is the slip tolerance; the default value of This method of calculating the allowable elastic slip is used for all analysis procedures (“Steady-state transport analysis,” . The steady-state transport analysis in Abaqus/Standard except Section 6.4.1), in which the penalty constraint is based on a maximum allowable slip rate, maximum slip rate is calculated as where is the angular spinning rate and R is the radius of the rolling structure. Cases in which the default elastic slip value may not be suitable In certain situations the default value for the allowable elastic slip may not be suitable. For example, slave surfaces defined by node-based surfaces or some contact element types, such as GAPUNI elements, have no physical dimensions and Abaqus/Standard cannot estimate a value of . For models containing only node-based surfaces or these types of contact elements, Abaqus/Standard first tries to use the “characteristic contact surface length” of the other contact pairs in the model. If there are none, it calculates using all of the elements in the model and issues a warning message. If a model contains no elements for which a characteristic length can be determined (for example, if it contains only substructures), Abaqus/Standard has no information with which to calculate . As a result, it uses a value of 1.0 and issues a warning message. If the contact surface face dimensions vary greatly, the average value of may be unreasonable for some contact surfaces. The elastic slip should then be specified directly for the surfaces with a much smaller “characteristic face dimension.” There are two methods for modifying the allowable elastic slip. One method is to specify the other is to specify the slip tolerance, steps . . Some analyses call for nondefault or directly; only in specific Specifying the allowable elastic slip directly You can provide the absolute magnitude of directly. Specify a reasonable value for the relative displacement that may occur before surfaces actually begin to slip. Typically, the allowable elastic slip is set to a small fraction (10−2 –10−4 ) of a “characteristic contact surface face dimension.” In a steady-state transport analysis you can define the maximum allowable viscous slip rate, . The specified allowable elastic slip will be used only for the contact pairs referencing the contact property definition that contains the friction definition. For example, three surfaces ASURF, BSURF, and CSURF form two contact pairs that each refer to their own contact property definition, as shown below. Contact Pair Contact Property ASURF, BSURF DEFAULT CSURF, BSURF NONDEF 0.1 In the DEFAULT contact property definition no value for for the friction interaction between ASURF and BSURF would be the default value contact property definition a value of 0.1 is specified for for the friction interaction between CSURF and BSURF. *FRICTION, ELASTIC SLIP= Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: Penalty or Static-Kinetic Exponential Decay: Elastic Slip, Absolute distance: is specified, so the allowable elastic slip used . In the NONDEF , which will be the allowable elastic slip used Abaqus/CAE Usage: Input File Usage: Changing the default slip tolerance You can alter the default value of the slip tolerance, . This method of altering the default elastic slip is convenient if the goal is to increase computational efficiency, in which case a value larger than the default of 0.005 would be given, or if the goal is to increase accuracy, in which case a value smaller than the default would be given. Input File Usage: Abaqus/CAE Usage: *FRICTION, SLIP TOLERANCE= Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: Penalty or Static-Kinetic Exponential Decay: Elastic Slip, Fraction of characteristic surface dimension: Stiffness method for imposing frictional constraints in Abaqus/Explicit The stiffness method used for friction with the general contact algorithm in Abaqus/Explicit and, optionally, with the contact pair method in Abaqus/Explicit is a penalty method that permits some relative motion of the surfaces (an “elastic slip”) when they should be sticking (similar to the allowable elastic slip defined with softened tangential behavior in Abaqus/Explicit). While the surfaces are sticking (i.e., ), the magnitude of sliding is limited to this elastic slip. Abaqus continually adjusts the magnitude of the penalty constraint to enforce this condition. In Abaqus/Explicit you can choose to have contact constraints for the contact pair algorithm enforced with the penalty method; the general contact algorithm always uses a penalty method . The default penalty stiffness for frictional constraints is chosen automatically by Abaqus/Explicit and is the same as would be used for normal hard contact constraints. Softening in the normal direction does not affect the penalty stiffness used to enforce stick conditions. If tangential softening is specified , the penalty stiffness will be equal to the value specified for the slope of the shear stress versus elastic slip relationship. You can specify a scale factor to adjust the penalty stiffness, as discussed in “Contact controls for general contact in Abaqus/Explicit,” Section 35.4.5, and “Contact controls for contact pairs in Abaqus/Explicit,” Section 35.5.5. Lagrange multiplier method for imposing frictional constraints in Abaqus/Standard In Abaqus/Standard the sticking constraints at an interface between two surfaces can be enforced exactly by using the Lagrange multiplier implementation. With this method there is no relative motion between two closed surfaces until . However, the Lagrange multipliers increase the computational cost of the analysis by adding more degrees of freedom to the model and often by increasing the number of iterations required to obtain a converged solution. The Lagrange multiplier formulation may even prevent convergence of the solution, especially if many points are iterating between sticking and slipping conditions. This effect can occur particularly if locally there is a strong interaction between slipping/sticking conditions and contact stresses. Because of the added cost of using the Lagrange friction formulation, it should be used only in problems where the resolution of the stick/slip behavior is of utmost importance, such as modeling fretting between two bodies. In typical metal forming applications or for contact of rubber components, accurate resolution of the stick/slip behavior is not important enough to justify the added costs of the Lagrange multiplier formulation. Input File Usage: Abaqus/CAE Usage: *FRICTION, LAGRANGE Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: Lagrange Multiplier Kinematic method for imposing frictional constraints in Abaqus/Explicit By default, the contact pair algorithm in Abaqus/Explicit uses a kinematic method for imposing frictional constraints . The kinematic method applies sticking constraints in a way similar to the optional Lagrange multiplier method in Abaqus/Standard; however, the algorithm is quite different. The value of the force required to enforce sticking at a node is first calculated using the mass associated with the node; the distance the node has slipped; the time increment; and additionally for softened contact, the current value of the elastic slip and the elastic slip versus shear stress slope. For hard contact this sticking force is that which is required to maintain the node’s position on the opposite surface in the predicted configuration. For softened contact this force is consistent with the user-specified value for the slope of the shear stress versus elastic slip relationship. The sticking force for each node is calculated using the mass associated with the node, the distance the node has slipped, the shear traction-elastic slip slope (if softened contact is specified in the tangential direction), and the time increment. If the shear stress at the node calculated using this force is less than , the node is considered to be sticking and this force is applied to each surface in opposing directions. If the shear stress exceeds is applied. In either case the forces result in acceleration corrections tangential to the surface at the slave node and either the nodes of the master surface facet or the points on the analytical rigid surface that it contacts. , the surfaces are slipping and the force corresponding to User-defined friction model You can define the shear stress between contacting surfaces through a user subroutine when the friction behavior provided by Abaqus is not sufficient. The shear stress can be defined as a function of a number of variables such as slip, slip rate, temperature, and field variables. You can also introduce a number of solution-dependent state variables that you can update and use within the friction user subroutines. You can declare a number of properties or constants associated with your friction model and use these values in the user subroutine. In addition to the friction user subroutines, subroutines are available for defining the complete mechanical interaction between surfaces, including the interaction in the normal direction as well as the frictional behavior in the tangential direction; see “User-defined interfacial constitutive behavior,” Section 36.1.6, for more information. Defining generic frictional behavior You can define a generic frictional behavior between contacting surfaces using user subroutine FRIC in Abaqus/Standard. In Abaqus/Explicit the generic frictional behavior for contact pairs is defined in user subroutine VFRIC, while the generic frictional behavior for general contact is defined in user subroutine VFRICTION. Input File Usage: Use the following option to define a frictional behavior with user subroutine FRIC or VFRIC: Abaqus/CAE Usage: *FRICTION, USER, DEPVAR=n, PROPERTIES=p Use the following option to define a frictional behavior with user subroutine VFRICTION: *FRICTION, USER=FRICTION, DEPVAR=n, PROPERTIES=p Use the following options to define a frictional behavior with user subroutine FRIC or VFRIC: Interaction module: contact property editor: Mechanical→Tangential Behavior: Friction formulation: User-defined, Number of state-dependent variables: n, Friction Properties User subroutine VFRICTION is not supported in Abaqus/CAE. Defining complex isotropic friction Abaqus provides a simple way to specify complex isotropic frictional behavior when the expression for the friction coefficient can be defined explicitly. You need only to specify the friction coefficient, and Abaqus will compute the resulting frictional forces. Abaqus/Standard provides user subroutine FRIC_COEF and Abaqus/Explicit provides user subroutine VFRIC_COEF for this purpose. VFRIC_COEF can be used only with general contact. Input File Usage: Abaqus/CAE Usage: *FRICTION, USER=COEFFICIENT, PROPERTIES=p User subroutines FRIC_COEF and VFRIC_COEF are not supported in Abaqus/CAE. Improving Abaqus/Standard simulations that include friction in the surface interactions Several features of the frictional interaction of surfaces can have a strong influence on the rate of convergence in an Abaqus/Standard simulation. Unsymmetric terms in the system of equations Friction constraints produce unsymmetric terms when the surfaces are sliding relative to each other. These terms have a strong effect on the convergence rate if frictional stresses have a substantial influence on the overall displacement field and the magnitude of the frictional stresses is highly solution dependent. Abaqus/Standard will automatically use the unsymmetric solution scheme if is pressure- or if dependent. solution scheme in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2. If desired, you can turn off the unsymmetric solution scheme; see “Matrix storage and No slip occurs with rough friction; the contribution to the stiffness will be fully symmetric, and Abaqus/Standard will use the symmetric solution scheme by default. Heat generated by frictional interaction of surfaces In fully coupled temperature-displacement analysis and fully coupled thermal-electrical-structural analysis, all dissipated mechanical (frictional) energy is converted to heat and distributed equally between the two surfaces by default. This behavior can be modified; for details about this and other thermal surface interactions, see “Thermal contact properties,” Section 36.2.1. Temperature and field-variable dependence of friction properties for structural elements Temperature and field-variable distributions in beam and shell elements can generally include gradients through the cross-section of the element. Contact between these elements occurs at the reference surface; therefore, temperature and field-variable gradients in the element are not considered when determining friction properties that depend on these variables. Surface interaction variables related to friction Abaqus provides output of the shear stresses at points on the slave surface that use a surface interaction model containing frictional properties. The shear stresses, CSHEAR1 and CSHEAR2, are given in the two orthogonal slip directions, which are constructed on the master surface . There is only one slip direction in two-dimensional problems. Details about how to request contact surface variable output are given in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1, and “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1. Contour plots of these variables can also be plotted in Abaqus/CAE. Additional reference • Oden, J. T., and J. A. C. Martins, “Models and Computational Methods for Dynamic Friction Phenomena,” Computer Methods in Applied Mechanics and Engineering, vol. 52, pp. 527–634, 1985. 36.1.6 USER-DEFINED INTERFACIAL CONSTITUTIVE BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit References • “UINTER,” Section 1.1.38 of the Abaqus User Subroutines Reference Manual • “VUINTER,” Section 1.2.15 of the Abaqus User Subroutines Reference Manual • “VUINTERACTION,” Section 1.2.16 of the Abaqus User Subroutines Reference Manual • *SURFACE INTERACTION Overview User-defined interfacial constitutive behavior: • is provided so that any constitutive behavior across an interface can be added to the library of existing models such as softened contact and Coulomb friction; • requires that a constitutive model (or a library of models) for the interface be programmed in user subroutine UINTER in Abaqus/Standard; • requires that a constitutive model (or a library of models) for the interface be programmed in user subroutine VUINTER in Abaqus/Explicit when using the contact pair algorithm; • requires that a constitutive model (or a library of models) for the interface be programmed in user subroutine VUINTERACTION in Abaqus/Explicit when using the general contact algorithm; • is available only for surface-based contact definition involved in stress/displacement, coupled temperature-displacement, coupled thermal-electrical-structural, or heat transfer analysis; and • requires considerable effort and expertise: the feature is very general and powerful, but it is intended for advanced users. Purpose of user subroutines UINTER, VUINTER, and VUINTERACTION User subroutines UINTER, VUINTER, and VUINTERACTION provide a very general interface for you to define the constitutive behavior across the interface between two surfaces. These subroutines replace all built-in interfacial constitutive behavior models; hence, no other contact property definitions (e.g., friction, thermal conductance, etc.) can be specified in conjunction with them. In a stress/displacement analysis you must define the stresses, both normal and tangential, at the slave node (or points on the slave surface) at the current point in time. In a coupled temperature-displacement analysis and a coupled thermal-electrical-structural analysis you must also define the heat flux across the interface. The constitutive calculation thus involves computing the stresses and heat fluxes based on the increments in relative position of the slave node with respect to the master surface (which act as strains in this context), temperature at the surface, and predefined field variables. The calculations would typically involve solution-dependent state variables, which can be updated inside these routines. If contact damping is to be included in the interfacial constitutive model, you must include the damping contribution in the stress definition. When a user subroutine is used to define the interfacial constitutive behavior, all decisions regarding the contact status of a slave node must be made inside the subroutine based on the information provided. You can make such decisions based on the values of the relative position of the point on the slave surface with respect to the master surface and appropriately defined solution-dependent state variables. Thus, usage of this feature involves not only developing a constitutive behavior of the interface but also developing conditions under which contact is active at a given point on the slave surface. The interface is always assumed to be massless. User subroutine UINTER will be called for each contact constraint location of affected contact pairs in each iteration of an Abaqus/Standard analysis. The input to this user subroutine includes the current relative position of a particular constraint point on the slave surface with respect to the corresponding closest point on the master surface, as well as the incremental relative motion between these two points. Values of temperature and field variables at the constraint point on the slave surface and the corresponding closest point on the master surface and several other variables are also provided as input. In addition to defining the contact stress or heat flux, appropriate Jacobian terms must also be defined to ensure proper convergence characteristics in Abaqus/Standard. User subroutine VUINTER will be called multiple times for the affected contact pairs in each time increment of an Abaqus/Explicit analysis. All slave nodes are processed in each call to VUINTER, whereas only a single constraint is processed in each call to UINTER. Similar input is provided to VUINTER as UINTER. User subroutine VUINTERACTION will be called multiple times for each interacting surface in each time increment of an Abaqus/Explicit analysis. Points of potential contact for a given interaction are processed in blocks in calls to VUINTERACTION. Similar input is provided to VUINTERACTION as VUINTER. Interfacial constants You must specify the number of interfacial constants that are needed in user subroutine UINTER, VUINTER, or VUINTERACTION; and you must provide values for all these constants. All surface constitutive behavior calculations and all decisions regarding the contact status at a slave node (or a point on the slave surface in question) must be programmed in the user subroutine. Any other contact property definitions included in the analysis are reported as an error. Input File Usage: For contact interactions defined through user subroutine UINTER or VUINTER: *SURFACE INTERACTION, USER, PROPERTIES=number_of_material_constants For contact interactions defined through user subroutine VUINTERACTION: *SURFACE INTERACTION, USER=INTERACTION, PROPERTIES=number_of_material_constants Tracking thickness when VUINTERACTION is used A surface interaction is considered active if the interacting surfaces are within a separation distance called the tracking thickness. Abaqus/Explicit uses an internal default value for the tracking thickness. Alternatively, you can specify the tracking thickness in conjunction with a user-defined surface In this case contacting surfaces whose proximity is within this thickness are interaction model. available for user-defined interactions. Use of a user-specified tracking thickness is supported only with node-to-surface contact and not with edge-to-edge contact. Input File Usage: *SURFACE INTERACTION, USER=INTERACTION, TRACKING THICKNESS=tracking_thickness Interfacial state Constitutive models used to define the interfacial behavior may require the storage of solution-dependent state variables. You must allocate storage space for these variables by indicating the number of variables. There is no restriction on the number of state variables associated with a user-defined constitutive behavior for the interface. User subroutine UINTER is called for points on the slave surface at each iteration of every increment. User subroutine VUINTER is called in every time increment for each master-slave view of each contact pair it affects, as discussed earlier. User subroutine VUINTERACTION is called in every time increment for each pair of surfaces actively interacting, as discussed earlier. Each subroutine is provided with the state of the slave node or potential contact point at the start of the increment (the state includes stress, flux, solution-dependent state variables, temperature, and any predefined field variables) and with the increments in temperature, predefined state variables, relative position, and time. Input File Usage: Use the following option to allocate storage space for solution-dependent state variables: *SURFACE INTERACTION, DEPVAR=number_of_state_variables Use with the unsymmetric equation solver in Abaqus/Standard If the constitutive Jacobian matrix, equation solution capability in Abaqus/Standard . , is not symmetric, you should invoke the unsymmetric Input File Usage: *SURFACE INTERACTION, USER, UNSYMM Defining the contact status in Abaqus/Standard In addition to defining the constitutive behavior, in Abaqus/Standard you may also update the flags LOPENCLOSE, LSTATE, and LSDI. The flag LOPENCLOSE is useful when UINTER is used to model standard contact between two surfaces (similar to the default hard contact in Abaqus). It should be set to 0 to indicate an open status and to 1 to indicate a closed status. At the beginning of the analysis it is set to −1 before UINTER is called. A change in this flag from one iteration to the next will have two consequences. It will result in output related to the change in contact status if detailed contact output has been requested to the message file , and it will also trigger a severe discontinuity iteration. The flag LSTATE can be used to store the current contact status of the points on the slave surface in non-standard situations where a simple open/close status is not appropriate. An example of such a situation is debonding, where three different states can be defined—fully bonded, partially bonded or debonding, and fully debonded. You can assign an integer to each of these states and set LSTATE accordingly. At the beginning of the analysis LSTATE is set to −1 before UINTER is called. When this flag is used and it changes from one iteration to the next, you can output messages to the message file (unit 7) related to such a change in state directly from user subroutine UINTER. The flag LPRINT is provided to allow you to output messages related to change in contact status only when you request detailed contact output to the message file. In such a situation the LSDI flag may be set to 1 to trigger a severe discontinuity iteration (this issue is discussed in detail later). An example of a situation where both the flags LOPENCLOSE and LSTATE can be used arises in the modeling of debonding between two surfaces. When the surface is in a state of transition from bonded to debonded, the flag LSTATE may be used, while the flag LOPENCLOSE may be left to its original value of −1. However, once complete debonding has taken place, the contact between the two surfaces may be modeled using standard hard contact. In that situation the LSTATE flag may be set to −1, and the LOPENCLOSE flag used. Any time one of these two flags is set to −1, Abaqus/Standard assumes that it is not being used. A change of these flags from some other value to −1 does not result in contact-status related output or severe discontinuity iterations. Similarly, a change of these flags from −1 to some other value will not result in contact-status related output or severe discontinuity iterations. If these flags are not used, there will be no output related to change in contact status unless you decide to output messages that are not based on these flags directly from UINTER. Severe discontinuity iterations in Abaqus/Standard Abaqus/Standard classifies iterations in which the contact state at the end of the iteration is different from the state assumed for that iteration as severe discontinuity iterations. The treatment of severe discontinuity iterations by Abaqus/Standard is discussed in “Severe discontinuities in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2. When you define the interfacial constitutive behavior through user subroutine UINTER and do not use the LOPENCLOSE flag, it is your responsibility to provide Abaqus/Standard with input on how an iteration should be treated. The flag LSDI is provided in user subroutine UINTER for this purpose. It is set to 0 before each call to UINTER; you should set it to 1 to treat the current iteration as a severe discontinuity iteration. If the LOPENCLOSE flag is used, the value of this flag alone determines whether a severe discontinuity iteration is necessary or not, and the LSDI flag is ignored. Use with contact in Abaqus/Explicit The penalty contact algorithm must be used with user subroutines VUINTER and VUINTERACTION; see “Penalty contact algorithm” in “Contact constraint enforcement methods in Abaqus/Explicit,” Section 37.2.3. When VUINTER is used and balanced master-slave contact is specified (i.e., the contact pair weighting factor is not equal to 0.0 or 1.0), VUINTER will be called for each surface in the contact pair that can act as a slave surface. The forces and fluxes defined in VUINTER will be multiplied by the weight value for the master-slave view before they are applied. Effects on solution time in Abaqus/Explicit Abaqus/Explicit accounts for the contact stiffness and conductance in the stable time increment calculation. Specifying stresses and fluxes in the user subroutine that correspond to large contact stiffness (e.g., large slope of contact pressure versus penetration) and large contact conductance will cause a significant drop in the stable time increment and, therefore, an increase in the solution time. Tangent stiffnesses and conductances are determined by Abaqus/Explicit using a finite difference method. User subroutine VUINTER is called three times per increment for each master-slave view of each two-dimensional contact pair that references it and four times per increment for each three-dimensional contact pair that references it. User subroutine VUINTERACTION is called four times per increment for each active surface interaction that references it. The user subroutines are called once with the actual configuration and subsequently with perturbed configurations based on displacement perturbations in the normal direction, the tangential direction, and, in three-dimensional cases, the tangential direction, respectively . For example, each component of contact stiffness is computed as a difference in contact stress divided by a difference in relative position. You do not have access to the computed values of contact stiffness and conductance, but you can control the constitutive behavior of the model. Estimated default penalty stiffness (and conductance) values are provided to the user subroutines for comparison purposes. Contact stiffnesses or conductances that exceed the default penalty values can significantly reduce the time increment size. The default penalty stiffnesses and conductances are based on an assumption that all slave nodes are in contact. In the case of VUINTER, if only a fraction of the slave nodes are in contact, higher penalties than are reported in VUINTER would be assigned in some cases with the default penalty algorithm. Any changes to state variables are ignored for the perturbation calls. In the case of VUINTER there can be significant additional CPU expense associated with contact tracking. Since the contact state is unknown on entry to VUINTER, all nodes on the slave surface must be tracked in every increment. This can increase the cost of an analysis significantly compared to the contact models in Abaqus/Explicit if a large proportion of the slave nodes are not involved in contact. In the case of VUINTERACTION there can be significant additional CPU expense associated with contact tracking only if the tracking thickness is large compared to the element facet size on contacting surfaces. Use with other subroutines Any other user subroutine that does not deal with constitutive behavior across an interface can be used in conjunction with UINTER, VUINTER, or VUINTERACTION. For example, user subroutines UMAT and UMATHT can be used in conjunction with UINTER to define the constitutive mechanical and thermal behaviors of the material underlying the contact surfaces. User subroutine VUMAT can be used in conjunction with VUINTER to define the mechanical constitutive behavior of the material underlying the contact surfaces. However, user subroutines FRIC, GAPCON, and GAPELECTR—available in Abaqus/Standard for defining mechanical, thermal, and electrical interactions between surfaces—can be used in conjunction with UINTER only if they are referenced on separate surface interactions. The same restriction applies to user subroutine VFRIC used in conjunction with VUINTER and to user subroutines VFRICTION or VFRIC_COEF used in conjunction with VUINTERACTION. Use with contact controls In Abaqus/Standard contact controls will not have any effect when used at an interface whose constitutive behavior is defined through user subroutine UINTER. In Abaqus/Explicit contact controls can be specified for a contact pair referencing a user-defined In the case of user subroutine VUINTERACTION the default penalty stiffness surface interaction. argument includes any scale factor specified; whereas with user subroutine VUINTER the scale factor is ignored. Output Most of the standard output variables that are normally available in an analysis involving contact are available with this capability. Output for UINTER The variables COPEN and CSLIP represent the relative positions normal and tangential to the interface, respectively. The surface-based thermal interaction variable, SFDR, contains the heat flux due to the total energy dissipated due to friction, and not some fraction of it. This is unlike using the built-in capability in Abaqus/Standard, where SFDR may contain the heat flux due to only a fraction of the total frictional dissipation, depending on the specified fraction of the dissipated energy that is converted into heat. In addition, the surface-based thermal interaction variable WEIGHT, which represents the weighting factor for heat flux (generated by frictional sliding) distribution between the surfaces, is not available with this capability. Additional user-defined output variables can be defined for UINTER by using the solution- dependent state variables (SDV). Output for VUINTER and VUINTERACTION All contact output variables in Abaqus/Explicit will be available except output for spot welds (BONDSTAT and BONDLOAD). The following user subroutine variables will contribute to the associated total energy variables: the variable sed will contribute to the energy output variable ALLSE; sfd will contribute to ALLFD; scd will contribute to ALLCD; spd will contribute to ALLPD; and svd will contribute to ALLVD. If SFDR is requested, sfd, scd, spd, and svd will also be used to calculate the heat generated at the interface (for output purposes only; the generated heat will not be applied to the model). The default values of the fraction of mechanical energy converted into heat and the weighting factor for the distribution of heat between the two surfaces (1.0 and 0.5, respectively) are used. User-defined, solution-dependent state variables associated with the user subroutine cannot be output to the output database (.odb) file or results (.fil) file. 36.1.7 PRESSURE PENETRATION LOADING Products: Abaqus/Standard Abaqus/CAE References • *PRESSURE PENETRATION • *SURFACE • *CONTACT PAIR • “Defining pressure penetration,” Section 15.13.16 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Pressure penetration loads simulated with contact pairs: • model the penetration of fluid between two contacting structures; and • allow the fluid to penetrate from multiple locations on the surface. Defining pressure penetration loads between contacting bodies Distributed pressure penetration loads allow for the simulation of fluid penetrating into the surface to the surfaces. between two contacting bodies and application of the fluid pressure normal Element-based contact surfaces are used to model the interactions between the bodies . The surfaces are modeled as slave and master contact surfaces . Any contact formulation can be used. The bodies forming the joint may both be deformable, as would be the case with threaded connectors; or one may be rigid, as would occur when a soft gasket is used as a seal between stiffer structures. You specify the nodes exposed to the fluid pressure, the magnitude of the fluid pressure, and the critical contact pressure below which fluid penetration starts to occur. See “Pressure penetration loading with surface-based contact,” Section 6.4.1 of the Abaqus Theory Manual, for more details. Input File Usage: *PRESSURE PENETRATION, SLAVE=slave1, MASTER=master1 slave surface node or node set, master surface node or node set, magnitude, critical contact pressure Abaqus/CAE Usage: If a node set is specified, it can contain only one node in two dimensions; in three dimensions it can contain any number of nodes. Interaction module: Create Interaction: Surface-to-surface contact (Standard), Name: contact_interaction_name; select master and slave surfaces Create Interaction: Pressure penetration; Contact interaction: contact_interaction_name, Region on Master: select face, edge, or point, Region on Slave: select face, edge, or point, Critical Contact Pressure: critical contact pressure, Fluid Pressure: magnitude Specifying a pressure penetration criterion A single slave-node-based penetration criterion is used. Fluid will penetrate into the surface between the contacting bodies from one or multiple locations, which are exposed to the fluid, until a point is reached where the contact pressure is greater than the specified critical value, cutting off further penetration of the fluid. Specifying a penetration time for the fluid pressure When the fluid pressure penetration criterion is satisfied, the fluid pressure is applied normal to the surfaces. If the full current fluid pressure is applied immediately, the resulting large changes in the strains near the contact surfaces can cause convergence difficulties. For large-strain problems severe mesh distortion can also occur. To ensure a smooth solution, the fluid pressure is ramped up linearly over a time period from zero pressure penetration load to the full current magnitude. You can specify the time period taken for the fluid pressure penetration load to reach the full current magnitude on newly penetrated surface segments. If the accumulated increment size, measured immediately after the penetration, is greater than the penetration time, the full current fluid pressure penetration load will be applied; otherwise, the fluid pressure on the newly penetrated surface segments is ramped up linearly to the current magnitude over the penetration time period, possibly over a number of increments. When the penetration time is equal to 0, the current fluid pressure is applied immediately once the fluid pressure penetration criterion is satisfied. The default penetration time is chosen to be 0.001 of the total step time. The penetration time is ignored in a linear perturbation analysis. Input File Usage: Abaqus/CAE Usage: *PRESSURE PENETRATION, PENETRATION TIME=n Interaction module: Create Interaction: Pressure penetration; Penetration time: n Specifying the nodes exposed to the fluid pressure The fluid can penetrate from either one or multiple locations of the surface. You must identify a node or node set on the slave surface of the contacting bodies that defines where the surface is exposed to the fluid pressure. In two dimensions if the master surface is not an analytical rigid surface , you must also identify a node or node set on the master surface that defines where the surface is exposed to the fluid pressure. You can specify multiple nodes or node sets if multiple locations of the surface are exposed to the fluid. These nodes or node sets are always subjected to the pressure penetration load if they are on the slave surface, regardless of their contact status. The fluid then starts to penetrate into the surface between the two contacting bodies from these nodes or node sets. Specifying the applied fluid pressure You must define the reference magnitude of the fluid pressure. You can define the variation of the fluid pressure during a step by referring to an amplitude curve. By default, the reference magnitude is applied immediately at the beginning of the step or ramped up linearly over the step, depending on the amplitude variation assigned to the step . The fluid pressure penetration load will be applied to the element surface based on the pressure penetration criterion at the beginning of an increment and will remain constant over that increment even if the fluid penetrates further during that increment. A nodal integration scheme is used to integrate the distributed fluid pressure penetration load over an element in two dimensions, while in three dimensions Gauss integration scheme is used; the variation of the distributed fluid pressure over an element will be determined by the load magnitudes at the element’s nodes. Input File Usage: Use the following option to define the variation of the fluid pressure during a step: Abaqus/CAE Usage: *PRESSURE PENETRATION, AMPLITUDE=name Interaction module: Create Interaction: Pressure penetration; Amplitude: name Removing or modifying the pressure penetration loads After pressure penetration loads are applied to the element surfaces, they will not be removed automatically even when contact between the surfaces is reestablished. At each new step the fluid pressure penetration loading, however, can be modified or completely redefined in a manner similar to the way that distributed loads can be defined . Input File Usage: Use the following option to modify the fluid pressure penetration loads that were applied in previous steps: *PRESSURE PENETRATION, OP=MOD (default) In this case the slave nodes exposed to the fluid pressure must be specified on the data lines. If the master surface is not an analytical rigid surface, the master nodes exposed to the fluid pressure must also be specified on the data lines for planar or axisymmetric models. Use the following option to remove all fluid pressure penetration loads and, optionally, to specify new fluid pressure penetration loads: *PRESSURE PENETRATION, OP=NEW When OP=NEW is used to remove all fluid pressure penetration loads, no data line is needed. However, when OP=NEW is used to specify new fluid pressure penetration loads, the nodes exposed to the fluid pressure must be specified on the data lines. OP=NEW must be used when defining new exposed nodes. In addition, when OP=NEW is used to re-specify a previously defined pressure penetration load, the fluid pressure loading will revert to its last known configuration first, even if the contact status has subsequently changed. Abaqus/CAE Usage: Use the following option to modify a fluid pressure penetration that was applied in a previous step: Interaction module: Interaction Manager: select interaction, Edit Use the following option to remove a fluid pressure penetration that was applied in a previous step: Interaction module: Interaction Manager: select interaction, Deactivate Specifying a critical mechanical contact pressure To account for the asperities on the contacting surfaces, a critical contact pressure, below which fluid penetration starts to occur, is introduced. The higher this value, the easier the fluid penetrates. The default value of the critical contact pressure is zero, in which case fluid penetration occurs only if contact is lost. Use in linear perturbation analysis Linear perturbation analyses can be performed from time to time during a fully nonlinear analysis by including linear perturbation steps between the general analysis steps. Because contact conditions cannot change during a linear perturbation analysis, the fluid will not penetrate further into the surface and it remains as it was defined in the base state. The fluid pressure magnitude applied in the previous general analysis step, however, can be modified during a linear perturbation analysis step. In matrix generation and steady-state dynamic analyses (direct or modal—see “Direct-solution steady-state dynamic analysis,” Section 6.3.4, and “Mode-based steady-state dynamic analysis,” Section 6.3.8) you can specify both the real (in-phase) and imaginary (out-of-phase) parts of the loading. Input File Usage: Use the following option to define the real (in-phase) part of the loading: *PRESSURE PENETRATION, REAL (default) Use the following option to define the imaginary (out-of-phase) part of the loading: *PRESSURE PENETRATION, IMAGINARY The REAL or IMAGINARY parameters are ignored in all procedures other than steady-state dynamics. Abaqus/CAE Usage: Use the following option to define the real (in-phase) part of the loading: Interaction module: Create Interaction: Pressure penetration; Fluid Pressure (Real) Use the following option to define the imaginary (out-of-phase) part of the loading: Interaction module: Create Interaction: Pressure penetration; Fluid Pressure (Imaginary) Limitations with pressure penetration loads Each slave surface subjected to pressure penetration loading must be continuous and cannot be a closed loop. Pressure penetration loading cannot be used with a node-based slave surface. The pressure penetration load applied at any increment is based on the contact status at the beginning of that increment. You should, therefore, be careful in interpreting the results at the end of an increment during which the contact status has changed. Small time increments are recommended to obtain accurate results. When pressure penetrates into contacting bodies between an analytical rigid surface and a deformable surface, no pressure penetration load will be applied to the analytical rigid surface. The reference node on the analytical rigid surface should, therefore, be constrained in all directions. To account for the effect of fluid pressure penetration loads on the rigid surface, the analytical rigid surface should be replaced with an element-based rigid surface. When fluid with different pressure loads penetrates into an element simultaneously from multiple locations on a surface, the maximum value of the fluid pressure loads is applied to the element. In large-displacement analyses pressure penetration loads introduce unsymmetric load stiffness matrix terms. Using the unsymmetric matrix storage and solution scheme for the analysis step may improve the convergence rate of the equilibrium iterations. See “Defining an analysis,” Section 6.1.2, for more information on the unsymmetric matrix storage and solution scheme. Only solid, shell, cylindrical, and rigid elements are supported for three-dimensional pressure penetration. Output You can request the fluid pressure load, PPRESS, at the nodes on the slave surface as surface output to the data, results, and output database files . 36.1.8 INTERACTION OF DEBONDED SURFACES Product: Abaqus/Standard References • “Contact pressure-overclosure relationships,” Section 36.1.2 • “Frictional behavior,” Section 36.1.5 • “Thermal contact properties,” Section 36.2.1 • “Pore fluid contact properties,” Section 36.4.1 • *DEBOND • *FRACTURE CRITERION Overview This section outlines briefly how initially bonded surfaces may interact once they have started to debond. Details on defining a crack propagation analysis can be found in “Crack propagation analysis,” Section 11.4.3. When two initially bonded surfaces start to debond: • the debonded slave surface nodes are released and can move freely; • the tractions acting on the slave surface nodes at the instant of debonding are ramped down to zero using a user-supplied amplitude curve; and • the contact property models assigned to the contact pair formed by the two surfaces start to govern the interaction of the surfaces. Frictional interactions of debonding surfaces Once the surfaces start to debond, the friction model assigned to the surfaces will govern the tangential motion of the debonded slave nodes. Friction generates forces tangential to the interface when the surfaces are closed. The frictional forces are independent of the debonding tractions that Abaqus/Standard applies and ramp off once a slave node debonds; the debonding tractions have no influence on the frictional behavior of a surface. Interaction models for behavior normal to the debonding surfaces The crack propagation capability in Abaqus/Standard was designed for use in classical fracture It is intended that the capability be used with the default “hard” contact mechanics problems. pressure-clearance model. the nondefault pressure-clearance models when the surfaces can debond. Abaqus/Standard will prevent the use of one of Thermal interaction of bonded and debonding surfaces Crack propagation simulations can be performed as coupled temperature-displacement analyses in Abaqus/Standard. While bonded, the surfaces are treated as having complete continuity of the temperature field across the interface. Once the surfaces start to debond, the thermal contact property models assigned to the surfaces will govern the thermal interactions across the debonded portion of the interface. Pore fluid interaction of bonded and debonding surfaces Crack propagation simulations can be performed in coupled pore pressure-displacement analyses. Whether the surfaces are bonded or are debonding, they are treated as having complete continuity of the pore pressure field across the interface. 36.1.9 BREAKABLE BONDS Product: Abaqus/Explicit References • “Contact formulations for contact pairs in Abaqus/Explicit,” Section 37.2.2 • *BOND • *SURFACE INTERACTION • *CONTACT PAIR Overview Breakable bonds, such as spot welds, between surfaces: • can be defined only at the nodes of the slave surface of a pure master-slave contact pair; • can be defined only in the first step of a simulation; • constrain the slave node to the master surface until the failure criterion of the bond is met; • are designed to provide a simple simulation of spot weld failure under relatively monotonic straining, such as occurs during an impact of a vehicle structure; • do not constrain the rotational degrees of freedom at the node; • use either a time to failure or a damaged failure model to simulate the postfailure response of the bonds; • use the default contact property model (“Mechanical contact properties: overview,” Section 36.1.1) once the bonds have been broken; and • can be used only between two deformable surfaces with the kinematic contact pair algorithm. Specifying spot welds for a contact pair A contact pair that contains spot welds must be a pure master-slave contact pair; therefore, spot welds If the contact pair consists of two deformable surfaces, cannot be used with single-surface contact. Abaqus/Explicit would normally use a balanced master-slave contact pair. In such situations you must specify a weighting factor to define a pure master-slave contact pair. Contact pairs containing spot welds must be defined in the first step of a simulation. The spot welds are located at the nodes of the slave surface of the contact pair. Spot welds can also be modeled more accurately using fasteners instead of breakable bonds. Fasteners have the advantage of being mesh independent in their definition and are convenient for defining point-to-point connections between two or more surfaces with the capability to model plasticity, damage, and failure behavior. However, fasteners are intended to be used in three dimensions; therefore, the fastener method cannot be used to specify spot welds for contact pairs in a two-dimensional case. If non-breakable bonds (rigid spot welds) are to be modeled, it is recommended that you use the mesh-independent spot weld feature (“Mesh-independent fasteners,” Section 34.3.4). All of the slave nodes which are bonded to a master surface can be grouped together into a node set. Input File Usage: Use all of the following options: *CONTACT PAIR, MECHANICAL CONSTRAINT=KINEMATIC, INTERACTION=interaction_property_name *SURFACE INTERACTION, NAME=interaction_property_name *BOND node_set_name, … Adjustments to the initial positions of the bonded nodes Nodes that are bonded to a master surface with spot welds should be defined so that they contact If the bonded nodes are not in contact initially, the surface in the model’s initial configuration. Abaqus/Explicit will enforce the bonded constraint by prescribing strain-free displacements to those nodes. The nodes will begin the simulation exactly in contact with the master surface. If the spot welds are defined incorrectly, this automatic adjustment of the nodes may cause the analysis to end immediately as a result of excessive initial distortion of elements that are connected to the bonded nodes. Forces carried by a spot weld Abaqus assumes that a spot weld carries a force normal to the surface onto which the node is welded, . The magnitude of the resultant , and two orthogonal shear forces tangent to the surface, , shear force, , is defined as . The normal force is positive in tension. A spot weld is assumed to be so small that it carries no moments or torque. As a result, spot welds do not impose any constraints on rotational degrees of freedom. Defining the failure criterion for the spot welds The failure criterion for a spot weld is defined as where and is the force required to cause failure in tension (Mode I loading), is the force required to cause failure in pure shear (Mode II loading), and are defined above. A typical yield surface for spot welds is shown in Figure 36.1.9–1. By specifying a very large value for either , the yield criteria of the spot welds can be made independent of either shear forces or normal forces, as shown in Figure 36.1.9–2. or sF F f yield surface F f F n Figure 36.1.9–1 Typical yield surface for spot welds. F = ∞ sF F f yield surface sF F = ∞ yield surface nF nF F f shear failure only tensile failure only Figure 36.1.9–2 Degenerate yield surfaces for spot welds. Input File Usage: *BOND node_set_name, , Spot weld forces sometimes exhibit significant noise, which can cause the spot weld to reach its failure criterion when a filtered solution of the spot weld forces would still be well within the strength limits of the spot weld. This is characterized by a noisy time history of the BONDSTAT variable and can correspond to an unrealistically early onset of failure of a spot weld. Two models for deterioration of a spot weld after the onset of failure are discussed below: a time to failure model and a postfailure damage model. With the time to failure model a single, spurious spike in the constraint force history that just exceeds the spot weld strength will lead to complete failure of the spot weld. The postfailure damage model may mitigate the effects of noise in the spot weld force. Defining the postfailure behavior of the spot welds Once the constraint forces on a spot weld exceed the failure criterion, the spot weld fails and deteriorates until the weld is broken completely. The behavior of the spot weld during this deterioration process can be simulated using either a damaged failure model or by linearly reducing the constraint forces to zero over a specified time period. With either model, the applied constraint forces from a spot weld are limited by the size of the yield surface as defined by the failure criterion. Deterioration of the spot weld is modeled by shrinking the yield surface to zero while retaining its original shape. If the predicted constraint forces exceed the yield surface, the applied forces are calculated using a radial flow rule to return to the yield surface. After complete failure, the node behaves like the rest of the slave nodes in the contact pair. The node may recontact the master surface, but the weld plays no further role. Defining the time to failure model You specify the time to failure, , which is the time required for the spot weld to fail completely after the initial failure criterion has been exceeded. Once failure is detected, the weld constraint is relaxed linearly over the time . Abaqus/Explicit shrinks the yield surface to zero over the time period : where t is the time since Abaqus/Explicit detected initial failure of the weld. Input File Usage: *BOND node_set_name, , , , Defining the postfailure damage model As stated above, if the predicted constraint forces exceed the failure criterion, the forces carried by the spot weld are calculated using a radial flow rule to return to the yield surface. Since the forces in the weld in this case are less than the constraint forces required to constrain the welded node on the master surface, the welded node will move relative to the master surface. The work expended during this relative motion is used to determine how the yield surface degrades. During failure the behavior of the weld is assumed to be such that any stretching of the weld in the normal direction, or any shearing of the weld, dissipates energy. Abaqus/Explicit assumes a linear force- displacement relationship after failure, thus resulting in the behaviors sketched in Figure 36.1.9–3 when the weld is subjected to pure Mode I or pure Mode II loading. More general loadings create combinations of these responses. You define the amount of energy that the weld can dissipate in Mode I and Mode II by specifying the breakage displacements in the normal and shear directions under pure Mode I and Mode II loading, and . nF F f sF F f nu u f u f su Figure 36.1.9–3 Typical postfailure behavior in pure tension/compression (Mode I) and in pure shear (Mode II). Using these linear force-displacement relationships, the failure criterion for the damaged failure model is where is the energy expended in Mode I; is the energy expended in Mode II; is the breakage energy in Mode I, which is calculated as is the breakage energy in Mode II, which is calculated as ; and . Input File Usage: *BOND node_set_name, , , , , , Post-yield surface interactions in spot welds Any friction, contact damping, or softening defined at the spot weld will not affect the analysis until the weld is broken completely; i.e., until the failure surface has shrunk to zero. Bead size of the spot weld The initial bead size of the spot weld, , is taken into account by offsetting the slave surface node associated with the spot weld from the master surface by an amount equal to the bead size during the penetration calculations. A master or slave surface defined on shell or membrane elements is itself offset from the midplane of the element by the half-thickness of the shell or membrane. If the damaged failure model is chosen to characterize the postfailure behavior, the size of the spot weld bead may grow due to tensile yielding of the spot weld. The size of the spot weld is equal to the sum of accumulated after the failure of the spot weld. After the weld has broken, the and the size of the bead at breakage is taken into account for subsequent contact between the weld node and the master surface. Available output for spot welds You can examine the forces carried by spot welds in Abaqus/CAE by generating a vector plot of the reaction forces on the surface (output variable CFORCE). Two output variables specifically related to spot welds, the bond status and bond load, are available for use in Abaqus/CAE. These variables can be written as history output to the output database (.odb) file. They can be used in X–Y plots in Abaqus/CAE. Definition of bond status The bond status (output variable BONDSTAT) is a measure of how close a spot weld is to complete failure. The bond status varies between 0.0 and 1.0 and is defined to be if the time to failure postfailure model is chosen or if the damaged failure model is chosen. With either model, the bond status is equal to 1.0 before the spot weld fails. Definition of bond load The bond load (output variable BONDLOAD) is a measure of how close the current constraint forces at a spot weld are to its failure surface. The value of the bond load also varies between 0.0 and 1.0 and is defined to be if the damaged failure model is chosen. For the time to failure model, the bond load is defined to be prior to failure. Then, the bond load is 1.0 from the moment of first yield until total failure, at which point the bond load becomes 0.0. Example: Spot welds and output requests The spot-welded nodes in node set WELDS are a subset of the nodes on surface A, which is the slave surface of the pure master-slave contact pair. *NSET, NSET=WELDS node set definition *CONTACT PAIR, MECHANICAL CONSTRAINT=KINEMATIC, INTERACTION=A TO B, WEIGHT=0. slave surface A, master surface B *SURFACE INTERACTION, NAME=A TO B *BOND WELDS, *OUTPUT, HISTORY, TIME INTERVAL=0.001 *CONTACT OUTPUT, NSET=WELDS BONDSTAT, BONDLOAD , , , , , Here damaged failure model is chosen. must be specified if the time to failure model is used, or and must be specified if the 36.1.10 SURFACE-BASED COHESIVE BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Progressive damage and failure,” Section 24.1.1 • “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1 • “Mechanical contact properties: overview,” Section 36.1.1 • “Crack propagation analysis,” Section 11.4.3 • *COHESIVE BEHAVIOR • *SURFACE INTERACTION • *DAMAGE INITIATION • *DAMAGE EVOLUTION • *DAMAGE STABILIZATION • *FRACTURE CRITERION • “Specifying cohesive behavior properties for mechanical contact property options” in “Defining a contact interaction property,” Section 15.14.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Specifying cohesive damage properties for mechanical contact property options” in “Defining a contact interaction property,” Section 15.14.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The features described in this section allow the specification of generalized traction-separation behavior for surfaces. This behavior offers capabilities that are very similar to cohesive elements that are defined using a traction-separation law . However, surface-based cohesive behavior is typically easier to define and allows simulation of a wider range of cohesive interactions, such as two “sticky” surfaces coming into contact during an analysis. Surface-based cohesive behavior is primarily intended for situations in which the interface thickness is negligibly small. If the interface adhesive layer has a finite thickness and macroscopic properties (such as stiffness and strength) of the adhesive material are available, it may be more appropriate to model the response using conventional cohesive elements . In Abaqus/Explicit the surface-based cohesive behavior framework can also be used to model crack propagation in initially partially bonded surfaces via linear elastic fracture mechanics principles (LEFM) as implemented using the Virtual Crack Closure Technique (VCCT). Surface-based cohesive behavior: • is defined as a surface interaction property; • can be used to model the delamination at interfaces directly in terms of traction versus separation; • can be used to model “sticky” contact (i.e., surfaces or parts of surfaces that are not initially in contact may bond on coming into contact; subsequently the bond may damage and fail); • can be restricted to surface regions that are initially in contact and, in Abaqus/Standard, to portions of surface regions that are initially in contact; • allows specification of cohesive data such as the fracture energy as a function of the ratio of normal to shear displacements (mode mix) at the interface; • assumes a linear elastic traction-separation law prior to damage; • assumes that failure of the cohesive bond is characterized by progressive degradation of the cohesive stiffness, which is driven by a damage process (in Abaqus/Explicit brittle fracture can also be modeled using a VCCT fracture crierion); • allows specification of post-failure cohesive behavior if failed nodes re-enter contact; • is implemented within the general contact algorithmic framework in Abaqus/Explicit and within the contact pair framework in Abaqus/Standard; • can be used to enforce “rough friction” surface interactions, the “no separation” contact relationship, or a combined “no separation and rough friction” behavior within the general contact framework in Abaqus/Explicit; • is enforced only for node-to-face contact interactions in Abaqus/Explicit and is not available for edge-to-edge and node-to-analytical rigid surface contact interactions; • cannot be used in a coupled Eulerian-Lagrangian analysis in Abaqus/Explicit; and • can be used for all Abaqus/Standard contact formulations except the finite sliding, surface-to-surface formulation. Defining cohesive behavior in Abaqus/Explicit Cohesive behavior in Abaqus/Explicit is defined as part of the surface interaction properties that are assigned to the applicable surfaces. General contact must be defined for the model. Input File Usage: Use the following options to define cohesive behavior between two surfaces in a general contact definition: *SURFACE INTERACTION, NAME=name *COHESIVE BEHAVIOR *CONTACT *CONTACT PROPERTY ASSIGNMENT surface1, surface2, name Abaqus/CAE Usage: Use the following option to define cohesive behavior between two surfaces: Interaction module: contact property editor: Mechanical→Cohesive Behavior Use the following option to define contact between two surfaces: Interaction module: interaction editor: General contact (Explicit): specify Contact interaction property Contact formulation for cohesive behavior in Abaqus/Explicit In Abaqus/Explicit overconstraints can arise in certain situations if the balanced master-slave formulation is enforced in addition to the cohesive constraint. To prevent this from occurring, a pure master-slave formulation is enforced for surfaces with cohesive behavior in Abaqus/Explicit. If cohesive behavior is defined between two surfaces, the first surface defined in the contact property assignment is treated as a slave surface and the second surface as its corresponding master surface. For contact interactions between the cohesive surfaces and other parts of the general contact domain, the default contact formulation (balanced master-slave) is applicable, unless a nondefault general contact formulation has been defined . The surface-based cohesive behavior is available only for node-to-face contact interactions; it is not available for edge- to-edge interactions. Hence, it is not possible to define surface-based cohesion between edges of beam and truss elements. In addition, contact definitions related to thermal interactions are ignored when surface-based cohesive behavior is defined. Care should be exercised when cohesive behavior is used in conjunction with stacked conventional shell elements. Depending on the load case, the specialized contact formulation may lead to approximate normal contact forces, which in turn may induce approximate transverse shear behavior in the stacked shells that affect the bending behavior of the stack. Continuum shells should be used instead of conventional shells in such modeling scenarios. Resolving initial overclosures and gaps in Abaqus/Explicit In many debonding applications using cohesive surfaces, it may be desirable to begin the analysis with the surfaces just touching each other. This requires the resolution of initial overclosures and gaps between the surfaces at the start of the analysis to ensure that the slave nodes are precisely in contact with the master surface. In Abaqus/Explicit small initial overclosures are set to zero by default. To resolve large initial overclosures or to close initial gaps between the surfaces, an appropriate contact clearance specification may be defined, as explained in “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 35.4.4. Since a pure-master slave formulation is enforced for cohesive surfaces, only nodes of the slave surface will undergo strain-free corrections to resolve any initial overclosures or gaps with their master facets; the nodes of the master facets will not be moved. Defining cohesive behavior in Abaqus/Standard Cohesive behavior in Abaqus/Standard is defined as part of the surface interaction properties that are assigned to a contact pair. Cohesive behavior cannot be assigned to contact pairs using the finite sliding, surface-to-surface formulation . Input File Usage: Use the following options to define cohesive behavior between the surfaces in a contact pair: *SURFACE INTERACTION, NAME=name *COHESIVE BEHAVIOR *CONTACT PAIR, INTERACTION=name surface1, surface2 Abaqus/CAE Usage: Use the following option to define cohesive behavior between two surfaces: Interaction module: contact property editor: Mechanical→Cohesive Behavior Use the following option to define surface-to-surface contact between two surfaces: Interaction module: interaction editor: Surface-to-surface contact (Standard): Bonding tabbed page: specify Contact interaction property Resolving initial overclosures and gaps in Abaqus/Standard As discussed above, it is often desirable in debonding applications for the cohesive surfaces to begin the analysis just touching each other. Abaqus/Standard offers some tools for adjusting slave nodes in a contact pair so that they precisely contact the master surface, thereby eliminating initial overclosures and gaps. If nodes are not adjusted, even an extremely small initial gap will cause the contact constraints to be initialized to inactive and, thus, not cohered. These tools are described in “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 35.3.5. Controlling the set of cohered nodes By default, cohesive constraint forces can potentially act on all nodes of the surfaces for which cohesive behavior is defined. Slave nodes that are initially contacting the master surface can experience cohesive forces at the start of the analysis, and slave nodes that are not initially contacting the master surface can experience cohesive forces if they contact the master surface during the analysis. There may, however, be situations where it is desirable to enforce cohesive behavior only for portions of surfaces that are contacting at the start of the analysis. Restricting cohesive behavior to initially contacting nodes As part of the cohesive behavior definition, you can indicate that only those nodes that are in contact with the master surface at the start of the step should experience cohesive forces. Any new contacts that occur during the step will not experience cohesive constraint forces; they will be modeled only as compressive contact. Input File Usage: *COHESIVE BEHAVIOR, ELIGIBILITY=ORIGINAL CONTACTS Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Cohesive Behavior: Only slave nodes initially in contact Restricting cohesive behavior to specified nodes In Abaqus/Standard you can specify a subset of initially slave nodes that should experience cohesive forces. Strain-free adjustments will be made for those nodes initially not in contact but specified in the node set. All slave nodes outside of this set (including those that are initially contacting the master surface) will experience only compressive contact forces over the course of the analysis. This method is particularly useful for modeling crack propagation along an existing fault line. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=CONTACT *COHESIVE BEHAVIOR, ELIGIBILITY=SPECIFIED CONTACTS Interaction module: contact property editor: Mechanical→Cohesive Behavior: Specify the bonding node set in the surface- to-surface (Standard) interaction Interaction module: interaction editor: Bonding tabbed page: Limit bonding to slave nodes in sub-set Interaction of traction-separation behavior with compressive and friction behavior In the contact normal direction, the pressure overclosure relationship governing the compressive behavior between the surfaces does not interact with the cohesive behavior, since they each describe the interaction between the surfaces in a different contact regime. The pressure overclosure relationship governs the behavior only when a slave node is “closed” (i.e., it is in contact with the master surface); the cohesive behavior contributes to the contact normal stress only when a slave node is “open” (i.e., not in contact). In the case of “sticky” cohesive behavior—where the two surfaces are not initially in contact—cohesive effects are activated in the increment after the slave node status changes from open to closed. In the shear direction, if the cohesive stiffness is undamaged, it is assumed that the cohesive model is active and the friction model is dormant. Any tangential slip is assumed to be purely elastic in nature and is resisted by the cohesive strength of the bond, resulting in shear forces. If damage has been defined, the cohesive contribution to the shear stresses starts degrading with damage evolution. Once the cohesive stiffness starts degrading, the friction model activates and begins contributing to the shear stresses. The elastic stick stiffness of the friction model is ramped up in proportion to the degradation of the elastic cohesive stiffness. Prior to the ultimate failure of the cohesive bond, and following the initiation of the degradation of the cohesive bond, the shear stress is a combination of the cohesive contribution and the contribution from the friction model. Once maximum degradation has been reached, the cohesive contribution to the shear stresses is zero, and the only contribution to the shear stresses is from the friction model. Applying cohesive material concepts to surface-based cohesive behavior The formulae and laws that govern cohesive surface behavior are very similar to those used for cohesive elements with traction-separation constitutive behavior (“Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6). The similarities extend to the linear elastic traction-separation model, damage initiation criteria, and damage evolution laws. However, it is important to recognize that damage in surface-based cohesive behavior is an interaction property, not a material property. Concepts of strain and displacement (used in behavior model formulae for cohesive elements) are reinterpreted as contact separations; contact separations are the relative displacements between the nodes on the slave surface and their corresponding projection points on the master surface along the contact normal and shear directions. Stresses are defined for surface-based cohesive behavior as the cohesive forces acting along the contact normal and shear directions divided by the current area at each contact point. The specifics of the surface-based cohesive behavior model are discussed in the sections that follow. Linear elastic traction-separation behavior The available traction-separation model in Abaqus assumes initially linear elastic behavior followed by the initiation and evolution of damage. The elastic behavior is written in terms of an elastic constitutive matrix that relates the normal and shear stresses to the normal and shear separations across the interface. traction stress vector, , , consists of three components (two components in two-dimensional problems): , which represent the normal (along the local 3-direction in three dimensions and along the local 2-direction in two dimensions) and the two shear tractions (along the local 1- and 2-directions in three dimensions and along the local 1-direction in two dimensions), respectively. The corresponding separations are denoted by , and , and (in three-dimensional problems) The nominal , . The elastic behavior can then be written as Uncoupled traction-separation behavior The simplest specification of cohesive behavior generates contact penalties that enforce the cohesive constraint in both normal and tangential directions. By default, the normal and tangential stiffness components will not be coupled: pure normal separation by itself does not give rise to cohesive forces in the shear directions, and pure shear slip with zero normal separation does not give rise to any cohesive forces in the normal direction. For uncoupled traction-separation behavior, the terms must be defined, as well as any dependencies on temperature or field variables. If these terms are not defined, Abaqus uses default contact penalties to model the traction-separation behavior. , and , Input File Usage: Abaqus/CAE Usage: *COHESIVE BEHAVIOR, TYPE=UNCOUPLED (default) Interaction module: contact property editor: Mechanical→Cohesive Behavior: Specify stiffness coefficients: Uncoupled Coupled traction-separation behavior In its full generality, the elasticity matrix provides fully coupled behavior between all components of the traction vector and separation vector and can depend on temperature and/or field variables. All terms in the matrix must be defined for coupled traction-separation behavior. Input File Usage: Abaqus/CAE Usage: *COHESIVE BEHAVIOR, TYPE=COUPLED Interaction module: contact property editor: Mechanical→Cohesive Behavior: Specify stiffness coefficients: Coupled Cohesive behavior in the normal or shear direction only To restrict the cohesive constraint to act along the contact normal direction only, define uncoupled cohesive behavior and specify zero values for the shear stiffness components, . and Alternatively, if only tangential cohesive constraints are to be enforced, the normal stiffness term, , can be set to zero, in which case the normal “separations” will not be constrained. Normal compressive forces are resisted as per the usual contact behavior. Damage modeling Damage modeling allows you to simulate the degradation and eventual failure of the bond between two cohesive surfaces. The failure mechanism consists of two ingredients: a damage initiation criterion and a damage evolution law. The initial response is assumed to be linear as discussed above. However, once a damage initiation criterion is met, damage can occur according to a user-defined damage evolution law. Figure 36.1.10–1 shows a typical traction-separation response with a failure mechanism. If the damage initiation criterion is specified without a corresponding damage evolution model, Abaqus evaluates the damage initiation criterion for output purposes only; there is no effect on the response of the cohesive surfaces (i.e., no damage will occur). Cohesive surfaces do not undergo damage under pure compression. Damage of the traction-separation response for cohesive surfaces is defined within the same general framework used for conventional materials , except the damage behavior is specified as part of the interaction properties for the surfaces. Multiple damage response mechanisms are not available for cohesive surfaces: cohesive surfaces can have only one damage initiation criterion and only one damage evolution law. Input File Usage: Use the following options to define damage initiation and damage evolution for cohesive surfaces: *SURFACE INTERACTION, NAME=name *COHESIVE BEHAVIOR *DAMAGE INITIATION *DAMAGE EVOLUTION Interaction module: contact property editor: Mechanical→Damage: Damage Initiation and Damage Evolution tabbed pages Abaqus/CAE Usage: traction t (t , t ) n s t δ (δ ,δ ) δ (δ ,δ ) separation Figure 36.1.10–1 Typical traction-separation response. Damage initiation Damage initiation refers to the beginning of degradation of the cohesive response at a contact point. The process of degradation begins when the contact stresses and/or contact separations satisfy certain damage initiation criteria that you specify. Several damage initiation criteria are available and are discussed below. Each damage initiation criterion also has an output variable associated with it to indicate whether the criterion is met. A value of 1 or higher indicates that the initiation criterion has been met. Damage initiation criteria that do not have an associated evolution law affect only output. Thus, you can use these criteria to evaluate the propensity of the material to undergo damage without actually modeling the damage process (i.e., without actually specifying damage evolution). , , and In the discussion below, represent the peak values of the contact stress when the separation is either purely normal to the interface or purely in the first or the second shear direction, respectively. Likewise, represent the peak values of the contact separation, when the separation is either purely along the contact normal or purely in the first or the second shear direction, respectively. The symbol used in the discussion below represents the Macaulay bracket with the usual interpretation. The Macaulay brackets are used to signify that a purely compressive displacement (i.e., a contact penetration) or a purely compressive stress state does not initiate damage. , and , Maximum stress criterion Damage is assumed to initiate when the maximum contact stress ratio (as defined in the expression below) reaches a value of one. This criterion can be represented as Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=MAXS Interaction module: contact property editor: Mechanical→Damage: Initiation tabbed page: Criterion: Maximum nominal stress Maximum separation criterion Damage is assumed to initiate when the maximum separation ratio (as defined in the expression below) reaches a value of one. This criterion can be represented as Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=MAXU Interaction module: contact property editor: Mechanical→Damage: Initiation tabbed page: Criterion: Maximum separation Quadratic stress criterion Damage is assumed to initiate when a quadratic interaction function involving the contact stress ratios (as defined in the expression below) reaches a value of one. This criterion can be represented as Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=QUADS Interaction module: contact property editor: Mechanical→Damage: Initiation tabbed page: Criterion: Quadratic traction Quadratic separation criterion Damage is assumed to initiate when a quadratic interaction function involving the separation ratios (as defined in the expression below) reaches a value of one. This criterion can be represented as Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=QUADU Interaction module: contact property editor: Mechanical→Damage: Initiation tabbed page: Criterion: Quadratic separation Damage evolution The damage evolution law describes the rate at which the cohesive stiffness is degraded once the corresponding initiation criterion is reached. The general framework for describing the evolution of damage in bulk materials (as opposed to interfaces modeled using cohesive surfaces) is described in “Damage evolution and element removal for ductile metals,” Section 24.2.3. Conceptually, similar ideas apply for describing damage evolution in cohesive surfaces. A scalar damage variable, D, represents the overall damage at the contact point. It initially has a value of 0. If damage evolution is modeled, D monotonically evolves from 0 to 1 upon further loading after the initiation of damage. The contact stress components are affected by the damage according to otherwise (no damage to compressive stiffness); , where for the current separations without damage. , and are the contact stress components predicted by the elastic traction-separation behavior To describe the evolution of damage under a combination of normal and shear separations across the interface, it is useful to introduce an effective separation (Camanho and Davila, 2002) defined as it can be While this formula was originally applied to damage evolution in cohesive elements, reinterpreted in terms of contact separations for cohesive surface behavior, as discussed above . Mixed-mode definition The relative proportions of normal and shear separations at a contact point define the mode mix at the point. Abaqus uses two measures of mode mix, one based on energies and the other based on tractions. You can choose one of these measures when you specify the mode dependence of the damage evolution process. Denoting by the work done by the tractions and their conjugate separations in the normal, first, and second shear directions, respectively, and defining , the mode-mix definitions based on energies are as follows: , and , Clearly, only two of the three quantities defined above are independent. It is also useful to define the quantity to denote the portion of the total work done by the shear traction and the corresponding separation components. As discussed later, Abaqus requires that you specify material properties related to damage evolution as functions of ) and (or, equivalently, . The corresponding definitions of the mode mix based on traction components are given by where definition (before they are normalized by the factor is a measure of the effective shear traction. The angular measures used in the above ) are illustrated in Figure 36.1.10–2. t~ normal t n t t Shear 2 t s Shear 1 Figure 36.1.10–2 Mode-mix measures based on traction. The mode-mix ratios defined in terms of energies and tractions can be quite different in general. The following example illustrates this point. In terms of energies a separation in the purely normal direction is one for which , irrespective of the values of the normal and the shear tractions. In particular, for coupled traction-separation behavior both the normal and shear tractions may be nonzero for a purely normal separation. For this case the definition of mode mix based on energies would indicate a purely normal separation, while the definition based on tractions would suggest a mix of both normal and shear separation. and There are two components to the definition of damage evolution. The first component involves specifying either the effective separation at complete failure, , relative to the effective separation at the initiation of damage, . The second component to the definition of damage evolution is the specification of the nature of the evolution of the damage variable, D, between initiation of damage and final failure. This can be done by either defining linear or exponential softening laws or specifying D directly as a tabular function of the effective separation relative to the effective separation at damage initiation. The data described above will in general be functions of the mode mix, temperature, and/or field variables. ; or the energy dissipated due to failure, traction δ o δ f separation Figure 36.1.10–3 Linear damage evolution. Figure 36.1.10–4 is a schematic representation of the dependence of damage initiation and evolution on the mode mix for a traction-separation response with isotropic shear behavior. The figure shows the traction on the vertical axis and the magnitudes of the normal and the shear separations along the two horizontal axes. The unshaded triangles in the two vertical coordinate planes represent the response under pure normal and pure shear separation, respectively. All intermediate vertical planes (that contain the vertical axis) represent the damage response under mixed-mode conditions with different mode mixes. The dependence of the damage evolution data on the mode mix can be defined either in tabular form or, in the case of an energy-based definition, analytically. The manner in which the damage evolution data are specified as a function of the mode mix is discussed later in this section. Figure 36.1.10–4 Illustration of mixed-mode response in cohesive interactions. Unloading subsequent to damage initiation is always assumed to occur linearly toward the origin of the traction-separation plane, as shown in Figure 36.1.10–3. Reloading subsequent to unloading also occurs along the same linear path until the softening envelope (line AB) is reached. Once the softening envelope is reached, further reloading follows this envelope as indicated by the arrow in Figure 36.1.10–3. Input File Usage: Abaqus/CAE Usage: Use the following option to use the mode-mix definition based on energies: *DAMAGE EVOLUTION, MODE MIX RATIO=ENERGY Use the following option to use the mode-mix definition based on tractions: *DAMAGE EVOLUTION, MODE MIX RATIO=TRACTION Interaction module: contact property editor: Mechanical→Damage: Evolution tabbed page: toggle on Specify mixed-mode behavior: Mode mix ratio: Energy or Traction Evolution based on effective separation You specify the quantity the effective separation at damage initiation, (i.e., the effective separation at complete failure, , relative to , as shown in Figure 36.1.10–3) as a tabular function of the mode mix, temperature, and/or field variables. In addition, you also choose either a linear or an exponential softening law that defines the detailed evolution (between initiation and complete failure) of the damage variable, D, as a function of the effective separation beyond damage initiation. Alternatively, instead of using linear or exponential softening, you can specify the damage variable, D, directly as a tabular function of the effective separation after the initiation of damage, ; mode mix; temperature; and/or field variables. Linear damage evolution For linear softening Abaqus uses an evolution of the damage variable, D, that reduces (in the case of damage evolution under a constant mode mix, temperature, and field variables) to the following expression: In the preceding expression and in all later references, refers to the maximum value of the effective separation attained during the loading history. The assumption of a constant mode mix at a contact point between initiation of damage and final failure is customary for problems involving monotonic damage (or monotonic fracture). Input File Usage: Use the following option to specify linear damage evolution: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=LINEAR Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Damage: Evolution tabbed page: Type: Displacement: Softening: Linear Exponential damage evolution For exponential softening Abaqus uses an evolution of the damage variable, D, that reduces (in the case of damage evolution under a constant mode mix, temperature, and field variables) to In the expression above is a non-dimensional parameter that defines the rate of damage evolution and is the exponential function. Input File Usage: Use the following option to specify exponential softening: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=EXPONENTIAL Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Damage: Evolution tabbed page: Type: Displacement: Softening: Exponential traction δ o δ f separation Figure 36.1.10–5 Exponential damage evolution. Tabular damage evolution For tabular softening you define the evolution of D directly in tabular form. D must be specified as a function of the effective separation relative to the effective separation at initiation, mode mix, temperature, and/or field variables. Input File Usage: Use the following option to define the damage variable directly in tabular form: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=TABULAR Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Damage: Evolution tabbed page: Type: Displacement: Softening: Tabular Evolution based on energy Damage evolution can be defined based on the energy that is dissipated as a result of the damage process, also called the fracture energy. The fracture energy is equal to the area under the traction-separation curve . You specify the fracture energy as a property of the cohesive interaction and choose either a linear or an exponential softening behavior. Abaqus ensures that the area under the linear or the exponential damaged response is equal to the fracture energy. The dependence of the fracture energy on the mode mix can be specified either directly in tabular form or by using analytical forms as described below. When the analytical forms are used, the mode-mix ratio is assumed to be defined in terms of energies. Tabular form The simplest way to define the dependence of the fracture energy is to specify it directly as a function of the mode mix in tabular form. Input File Usage: Use the following option to specify fracture energy as a function of the mode mix in tabular form: *DAMAGE EVOLUTION, TYPE=ENERGY, MIXED MODE BEHAVIOR=TABULAR Abaqus/CAE Usage: Interaction module: contact property editor: Contact: Mechanical→Damage: Evolution tabbed page: Type: Energy: toggle on Specify mixed mode behavior: Tabular Power law form The dependence of the fracture energy on the mode mix can be defined based on a power law fracture criterion. The power law criterion states that failure under mixed-mode conditions is governed by a power law interaction of the energies required to cause failure in the individual (normal and two shear) modes. It is given by The mixed-mode fracture energy when the above condition is satisfied. In other words, You specify the quantities failure in the normal, the first, and the second shear directions, respectively. , and , , which refer to the critical fracture energies required to cause Input File Usage: Use the following option to define the fracture energy as a function of the mode mix using the analytical power law fracture criterion: Abaqus/CAE Usage: *DAMAGE EVOLUTION, TYPE=ENERGY, MIXED MODE BEHAVIOR=POWER LAW, POWER= Interaction module: contact property editor: Mechanical→Damage: Evolution tabbed page: Type: Energy: toggle on Specify mixed mode behavior: Power law: Benzeggagh-Kenane (BK) form The Benzeggagh-Kenane fracture criterion (Benzeggagh and Kenane, 1996) is particularly useful when the critical fracture energies during separation purely along the first and the second shear directions are the same; i.e., . It is given by where and . Input File Usage: , , and is a cohesive property parameter. You specify , , Use the following option to define the fracture energy as a function of the mode mix using the analytical BK fracture criterion: *DAMAGE EVOLUTION, TYPE=ENERGY, MIXED MODE BEHAVIOR=BK, POWER= Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Damage: Evolution tabbed page: Type: Energy: toggle on Specify mixed mode behavior: Benzeggagh-Kenane: Linear damage evolution For linear softening Abaqus uses an evolution of the damage variable, D, that reduces to where maximum value of the effective separation attained during the loading history. as the effective traction at damage initiation. with refers to the Input File Usage: Use the following option to specify linear damage evolution: Abaqus/CAE Usage: *DAMAGE EVOLUTION, TYPE=ENERGY, SOFTENING=LINEAR Interaction module: contact property editor: Mechanical→Damage: Evolution tabbed page: Type: Energy: Softening: Linear Exponential damage evolution For exponential softening Abaqus uses an evolution of the damage variable, D, that reduces to In the expression above is the elastic energy at damage initiation. In this case the traction might not drop immediately after damage initiation, which is different from what is seen in Figure 36.1.10–5. and are the effective traction and separation, respectively. Input File Usage: Use the following option to specify exponential softening: *DAMAGE EVOLUTION, TYPE=ENERGY, SOFTENING=EXPONENTIAL Abaqus/CAE Usage: Interaction module: contact property editor: Mechanical→Damage: Evolution tabbed page: Type: Energy: Softening: Exponential Defining damage evolution data as a tabular function of mode mix As discussed earlier, the data defining the evolution of damage at the cohesive interface can be tabular functions of the mode mix. The manner in which this dependence must be defined in Abaqus is outlined below for mode-mix definitions based on energy and traction, respectively. In the following discussion it is assumed that the evolution is defined in terms of energy. Similar observations can also be made for evolution definitions based on effective separation. Mode mix based on energy and . The quantity For an energy-based definition of mode mix, in the most general case of a three-dimensional state of separation with anisotropic shear behavior the fracture energy, , must be defined as a function of is a measure of the fraction of the total separation that is shear, while is a measure of the fraction of the total shear separation that is in the second shear direction. Figure 36.1.10–6 shows a schematic of the fracture energy versus mode-mix behavior. The limiting cases of pure normal and pure shear separations in the first and second shear directions are denoted in Figure 36.1.10–6 by , respectively. The lines labeled “Modes n-s,” “Modes n-t,” and “Modes s-t” show the transition in behavior between the pure normal and the pure shear in the first direction, pure normal and pure shear in the second direction, and pure shears in the first and second directions, respectively. In general, must be specified as a function of . In the discussion that follows we at various fixed values of refer to a data set of as a “data block.” versus The following guidelines are useful in defining the fracture energy as a function of the mode mix: corresponding to a fixed , and , • For a two-dimensional problem only. The data column corresponding to only one “data block” is needed. needs to be defined as a function of in this case) must be left blank. Hence, essentially ( • For a three-dimensional problem with isotropic shear response, the shear behavior is defined by the . Therefore, in this case a single ) also suffices to define the fracture energy and not by the individual values of and sum “data block” (the “data block” for as a function of the mode mix. at a fixed value of “data blocks” would be needed. As discussed earlier, each “data block” would contain • In the most general case of three-dimensional problems with anisotropic shear behavior, several versus can vary between 0 and 1.0. The case (the first data point in any “data block”), which corresponds to a purely normal mode, can never be achieved when (i.e., the only valid point on line OB in Figure 36.1.10–6 is the point O, which corresponds to a purely normal separation). However, in the tabular definition of the fracture energy as a function of mode mix, this point simply serves to set a limit that ensures a continuous change in fracture energy as a purely normal state is approached from various combinations of normal and shear separations. Hence, the fracture energy . In each “data block” Modes n-s Modes s-t Modes n-t m + m = ( 2 3 G s G T ( 1.0 1.0 Figure 36.1.10–6 Fracture energy as a function of mode mix. m 3 m + m = ( 2 3 ( G t GS of the first data point in each “data block” must always be set equal to the fracture energy in a purely normal separation ( ). As an example of the anisotropic shear case, consider that you want to input three “data blocks” corresponding to fixed values of 0., 0.2, and 1.0, respectively. For each of the three “data blocks,” the first data point must be for the reasons discussed above. The rest of the data points in each “data block” define the variation of the fracture energy with increasing proportions of shear separation. Mode mix based on traction at various fixed values of needs to The fracture energy needs to be specified in tabular form of be specified as a function of . A “data block” in this case corresponds to a set of data for may vary from 0 (purely versus normal separation) to 1 (purely shear separation). An important restriction is that each data block must specify the same value of the fracture energy for . This restriction ensures that the energy required for fracture as the traction vector approaches the normal direction does not depend on the orientation of the projection of the traction vector on the shear plane . . In each “data block” , at a fixed value of . Thus, versus and Viscous regularization in Abaqus/Standard Models exhibiting various forms of softening behavior and stiffness degradation often lead to severe convergence difficulties in Abaqus/Standard. Viscous regularization of the constitutive equations defining surface-based cohesive behavior can be used to overcome some of these convergence difficulties. This technique is also applicable to cohesive elements, fastener damage, and the concrete material model in Abaqus/Standard. Viscous regularization damping causes the tangent stiffness matrix that defines the contact stresses to be positive for sufficiently small time increments. The approximate amount of energy associated with viscous regularization over the whole model is available using output variable ALLVD. Input File Usage: Abaqus/CAE Usage: *DAMAGE STABILIZATION Interaction module: Stabilization tabbed page: Viscosity coefficient contact property editor: Mechanical→Damage: Post-failure behavior Two types of post-failure behavior can be specified to define the cohesive behavior at a node on the slave surface after the maximum degradation value, , has been reached at the node. By default, once fully degraded, normal contact behavior is enforced at the node and no further cohesive constraints are enforced. If the slave node re-enters contact, penetrations will give rise to compressive contact stresses, and frictional stresses will be applied in the shear directions according to the prescribed friction model, if any. Separations can occur without giving rise to any cohesive stresses. In some situations it may be desirable to enforce cohesive behavior again if a slave node re-enters contact, even after maximum degradation has been reached. For cohesive behavior allowing repeated contacts, the overall damage variable will be re-initialized to zero when a failed slave node re-enters contact. Subsequently, normal separations may give rise to tensile cohesive stresses, and shear separations may give rise to tangential cohesive stresses in accordance with the type of cohesive behavior defined. Further loading can again cause the cohesive stresses to undergo progressive damage, degrade, and fail. Input File Usage: Abaqus/CAE Usage: Use the following option to enforce cohesive behavior subsequent to maximum degradation: *COHESIVE BEHAVIOR, REPEATED CONTACTS Interaction module: contact property editor: Mechanical→Cohesive Behavior: Allow cohesive behavior during repeated post-failure contacts Virtual Crack Closure Technique in Abaqus/Explicit In Abaqus/Explicit, the surface-based cohesive behavior framework can be used to model brittle crack propagation problems based on linear elastic fracture mechanics principles. The Virtual Crack Closure Technique (VCCT) fracture criterion can be used to model crack propagation in initially partially bonded surfaces. A detailed discussion of this topic can be found in “Crack propagation analysis,” Section 11.4.3. The VCCT fracture criterion cannot be combined with a damage-based surface behavior of the traction-separation response. However, you can use a surface-based VCCT fracture criterion in conjunction with cohesive elements. VCCT could model brittle failure/crack propagation while the cohesive elements could model other aspects of the bonded interface such as stitches. Input File Usage: Use the following options to enforce cohesive behavior subsequent maximum degradation: *COHESIVE BEHAVIOR *FRACTURE CRITERION, TYPE= VCCT to Cohesive surfaces versus cohesive elements As described above, the formulation used for surface-based cohesive behavior is very similar to that for cohesive elements with traction-separation response. However, certain differences exist. Interface thickness effects are never considered for cohesive surfaces; in cohesive elements with traction-separation response, thickness effects can be incorporated by either specifying a nonzero thickness for the interface or by requiring the initial constitutive thickness to be determined from the nodal coordinates of the cohesive elements. Since thickness effects are not considered for cohesive surfaces, material properties used to describe the constitutive response for traction-separation cohesive elements with thickness effects may not be directly reusable for cohesive surfaces. For cohesive surfaces the cohesive constraint is enforced at each slave node; in cohesive elements the cohesive constraints are calculated at the material points (for the locations of material points in cohesive elements, see “Two-dimensional cohesive element library,” Section 32.5.8, and “Three-dimensional cohesive element library,” Section 32.5.9). Hence for cohesive surfaces, refining the slave surface as compared to the master surface will likely lead to improved constraint satisfaction and more accurate results. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for cohesive surfaces with traction-separation behavior: CSDMG CSMAXSCRT CSMAXUCRT Overall value of the scalar damage variable, D. This variable indicates whether the maximum contact stress damage initiation criterion has been satisfied at a contact point. It is evaluated as . This variable indicates whether the maximum separation damage initiation criterion has been satisfied at a contact point. It is evaluated as . CSQUADSCRT This variable indicates whether the quadratic contact stress damage initiation criterion has been satisfied at a contact point. It is evaluated as . CSQUADUCRT This variable indicates whether the quadratic separation damage initiation criterion has been satisfied at a contact point. It is evaluated as . For the variables above that indicate whether a certain damage initiation criterion has been satisfied or not, a value that is less than 1.0 indicates that the criterion has not been satisfied, while a value of 1.0 indicates that the criterion has been satisfied. If damage evolution is specified for this criterion, the maximum value of this variable does not exceed 1.0. Additional references • Benzeggagh, M. L., and M. Kenane, “Measurement of Mixed-Mode Delamination Fracture Toughness of Unidirectional Glass/Epoxy Composites with Mixed-Mode Bending Apparatus,” Composites Science and Technology, vol. 56, pp. 439–449, 1996. • Camanho, P. P., and C. G. Davila, “Mixed-Mode Decohesion Finite Elements for the Simulation of Delamination in Composite Materials,” NASA/TM-2002–211737, pp. 1–37, 2002. 36.2 Thermal contact properties • “Thermal contact properties,” Section 36.2.1 36.2.1 THERMAL CONTACT PROPERTIES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Contact interaction analysis: overview,” Section 35.1.1 • “User-defined interfacial constitutive behavior,” Section 36.1.6 • “GAPCON,” Section 1.1.10 of the Abaqus User Subroutines Reference Manual • *GAP • *GAP CONDUCTANCE • *GAP HEAT GENERATION • *GAP RADIATION • *INTERFACE • *SURFACE INTERACTION • “Creating interaction properties,” Section 15.12.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Thermal interaction at the surface of a body: • can be included in heat transfer problems (“Uncoupled heat transfer analysis,” Section 6.5.2; “Fully coupled thermal-stress analysis,” Section 6.5.3; “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4; and “Coupled thermal-electrical analysis,” Section 6.7.3); • can involve conductive heat transfer between surfaces; • can involve radiative heat transfer between surfaces when the surfaces are separated by a narrow gap; • in Abaqus/Standard can involve convective heat flow across the boundary layer between a solid surface and a moving fluid; • can involve heat generated by frictional work in fully coupled thermal-mechanical or fully coupled thermal-electrical-structural simulations; and • in Abaqus/Standard can involve heat generated by an electrical current (Joule heating) in fully coupled thermal-electrical and fully coupled thermal-electrical-structural analyses. General radiative heat transfer between surfaces is not discussed in this section. For information on modeling these types of problems in Abaqus/Standard, see “Cavity radiation,” Section 40.1.1. The thermal contact property models described here are for bodies in close proximity or in contact. For these problems gap radiation may be more efficient and robust than cavity radiation. Including thermal properties in a contact property definition All of the thermal properties discussed in this section—gap conductance, gap radiation, and gap heat generation—can be included in a contact property definition for both surface-based contact and element-based contact. All three types of thermal properties can be included in the same contact property definition. The thermal contact property model between two surfaces can also be completely defined through user subroutine UINTER, VUINTER, or VUINTERACTION . Input File Usage: Use the following options for surface-based contact: *SURFACE INTERACTION, NAME=name *GAP CONDUCTANCE *GAP RADIATION *GAP HEAT GENERATION Use the following options for element-based contact in Abaqus/Standard: *INTERFACE or *GAP, ELSET=name *GAP CONDUCTANCE *GAP RADIATION *GAP HEAT GENERATION Use the following option for user-defined, surface-based contact: *SURFACE INTERACTION, USER Interaction module: contact property editor: Thermal→Thermal Conductance, Heat Generation, and/or Radiation Element-based contact and user-defined surface-based contact are not supported in Abaqus/CAE. Abaqus/CAE Usage: Thermal contact considerations in Abaqus/Explicit Gap conductance and gap radiation are enforced in Abaqus/Explicit with an explicit algorithm analogous to the penalty method for mechanical contact interaction. Therefore, gap conductance and gap radiation can influence the stability condition; although in a fully coupled temperature-displacement analysis the mechanical portion of the system usually governs the overall stability condition . Extremely large values of gap conductance or gap radiation can result in a decrease in the stable time increment, which will be accounted for by the automatic time incrementation algorithm in Abaqus/Explicit. Gap heat generation is applied within whichever algorithm (kinematic or penalty) is used to enforce the mechanical contact constraints. Gap heat generation has no effect on the stable time increment. Thermal contact fluxes may be inaccurate during increments in which mesh adaptivity occurs if the mechanical contact constraints are enforced kinematically, because mesh adjustments occur in Abaqus/Explicit between the determination of the mechanical contact state for kinematic contact and the calculation of thermal contact fluxes. For example, mesh adjustments for adaptivity may cause for pressure-dependent gap conductance, the gap conduction discontinuity in the contact pressure: coefficient will be set based on the pressure determined by the kinematic contact algorithm prior to the mesh adjustment, even though the thermal contact flux is applied after the mesh adjustment. The significance of this inaccuracy on the solution will depend on the size and frequency of the mesh adjustments and the degree of variation in the conduction coefficient. This inaccuracy can be avoided by enforcing the mechanical contact constraints with the penalty method. Thermal contact for general contact works analogously to thermal contact for contact pairs. Gap conductance, gap radiation, and gap heat generation can all be specified and incorporated in general contact definitions through contact property assignments. As discussed above, large values of gap conductance or gap radiation can result in performance degradation, particularly since more surfaces are typically involved in general contact than in contact pairs. Thermal contact properties cannot be specified for general contact involving edge-to-edge contact or Eulerian elements. Thermal contact properties are ignored when shell elements are used to define surfaces involved in a contact pair definition. In these cases general contact should be used. Modeling conductance between surfaces The conductive heat transfer between the contact surfaces is assumed to be defined by and where q is the heat flux per unit area crossing the interface from point A on one surface to point B on the other, are the temperatures of the points on the surfaces, and k is the gap conductance. Point A is a node on the slave surface; and point B is the location on the master surface contacting the slave node or, if the surfaces are not in contact, the location on the master surface with a surface normal that intersects the slave node. You can define k directly or, in Abaqus/Standard, in user subroutine GAPCON. Defining the gap conductance directly When defining k directly, define it as where Abaqus Version 6.12 ID: Printed on: is the clearance between A and B, is the contact pressure transmitted across the interface between A and B, is the average of the surface temperatures at A and B, is the average of the magnitudes of the mass flow rates per unit is the average of any predefined field variables at A and B, and Defining gap conductance as a function of clearance You can create a table of data defining the dependence of k on the variables listed above. The default in Abaqus is to make k a function of the clearance d. When k is a function of gap clearance, d, the tabular data must start at zero clearance (closed gap) and define k as d increases. At least two pairs of points must be given to define k as a function of the clearance. The value of k drops to zero immediately after the last data point, so there is no heat conductance when the clearance is greater than the value corresponding to the last data point. If gap conductance is not also defined as a function of contact pressure, k will remain constant at the zero clearance value for all pressures, as shown in Figure 36.2.1–1(a). Input File Usage: *GAP CONDUCTANCE , d, Abaqus/CAE Usage: Interaction module: contact property editor: Thermal→Thermal Conductance: Definition: Tabular, Use only clearance- dependency data (a) (b) Figure 36.2.1–1 Examples of input data to define the gap conductance as a function of clearance or contact pressure. Defining gap conductance as a function of contact pressure You can define k as a function of the contact pressure, p. When k is a function of contact pressure at the interface, the tabular data must start at zero contact pressure (or, in the case of contact that can support a tensile force, the data point with the most negative pressure) and define k as p increases. The value of k remains constant for contact pressures outside of the interval defined by the data points. If gap conductance is not also defined as a function of clearance, k is zero for all positive values of clearance and discontinuous at zero clearance, as shown in Figure 36.2.1–1(b). Input File Usage: *GAP CONDUCTANCE, PRESSURE , p, Abaqus/CAE Usage: Interaction module: contact property editor: Thermal→Thermal Conductance: Definition: Tabular, Use only pressure-dependency data Gap conductance as a function of both clearance and contact pressure k can depend on both clearance and pressure. A discontinuity in k is allowed at . At the state of zero clearance and zero pressure the value of k corresponding to the zero pressure data point is used, as shown in Figure 36.2.1–2(a). and dependence on pressure for negative contact pressure dclearance (a) pcontact dclearance pcontact (b) dependence on clearance prior to contact Figure 36.2.1–2 Examples of input data to define the gap conductance as a function of both clearance and contact pressure. In the case of no-separation contact, once contact occurs the conductance is always evaluated based on the portion of the curve that defines the pressure dependence. The gap conductance, k, remains constant for contact pressures outside of the interval defined by the data points, as shown in Figure 36.2.1–2(b). The pressure dependence of k is extended into the negative pressure region even if no data points with negative pressure are included. *GAP CONDUCTANCE Input File Usage: for the zero clearance data , d, *GAP CONDUCTANCE, PRESSURE , p, for the zero pressure data point: For example, the following input defines point and *SURFACE INTERACTION, NAME=name *GAP CONDUCTANCE 20.0, 0.0 10.0, 0.1 … *GAP CONDUCTANCE, PRESSURE 50.0, 0.0 65.0, 100.0 70.0, 250.0 … Abaqus/CAE Usage: Interaction module: contact property editor: Thermal→Thermal Conductance: Definition: Tabular, Use both clearance- and pressure-dependency data Using gap conductance to model convective heat transfer from a surface in Abaqus/Standard Generally, mass flow rates are defined in Abaqus/Standard only for nodes associated with forced convection elements. However, they can be defined for any node in a model. By using the dependence of k on the average mass flow rate at the interface (in addition to other dependencies), it is possible for the contact property definition to simulate convective heat transfer to the boundary layer between a solid and a moving fluid. If mass flow rates are given only for nodes on one side of the interface, which is typically the case when simulating convective heat transfer, the average mass flow rate used to define k will be half the magnitude specified. Input File Usage: Abaqus/CAE Usage: , *GAP CONDUCTANCE k, d, Interaction module: contact property editor: Thermal→Thermal Conductance: Definition: Tabular, Clearance Dependency and/or Pressure Dependency, toggle on Use mass flow rate-dependent data (Standard only) Defining gap conductance to be a function of predefined field variables In addition to the dependencies mentioned previously, the gap conductance can be dependent on any number of predefined field variables, . To make the gap conductance depend on field variables, at least two data points are required for each field variable value. Input File Usage: Abaqus/CAE Usage: , , *GAP CONDUCTANCE, DEPENDENCIES=n k, d, Interaction module: contact property editor: Thermal→Thermal Conductance: Definition: Tabular, Clearance Dependency and/or Pressure Dependency, Number of field variables: n Defining the gap conductance using user subroutine GAPCON In Abaqus/Standard k can be defined in user subroutine GAPCON. In this case there is greater flexibility in specifying the dependencies of k. It is no longer necessary to define k as a function of the average of the two surface’s temperatures, mass flow rates, or field variables. Input File Usage: Abaqus/CAE Usage: *GAP CONDUCTANCE, USER Interaction module: contact property editor: Thermal→Thermal Conductance: Definition: User-defined Defining the gap conductance to be strongly dependent on temperature If k depends strongly on temperature, the unsymmetric terms in the calculations start to become increasingly important in Abaqus/Standard. Using the unsymmetric matrix storage and solution scheme for the step may improve the convergence rate in the analysis . Temperature and field-variable dependence of gap conductance for structural elements Temperature and field-variable distributions in beam and shell elements can generally include gradients through the cross-section of the element. Contact between these elements occurs at the reference surface; therefore, temperature and field-variable gradients in the element are not considered when determining gap conductance, even in cases where the properties are also clearance dependent. Modeling radiation between surfaces when the gap is small transfer between closely spaced contact surfaces occurs in Abaqus assumes that radiative heat the direction of the normal between the surfaces. this normal corresponds to the master surface normal . connectivity defines the normal direction. In models using surface-based contact The gap radiation functionality in Abaqus is intended for modeling radiation between surfaces across a narrow gap. A more general capability for modeling radiation is available in Abaqus/Standard . Radiative heat transfer is defined as a function of clearance between the surfaces through the effective viewfactor. Abaqus maintains the radiative heat flux even when the surfaces are in contact. This causes only a minor inaccuracy since normally the heat flux from conduction is much larger than the radiative heat flux. Abaqus defines the heat flow per unit surface area between corresponding points as where q is the heat flux per unit surface area crossing the gap at this point from surface A to surface B, and used, and the coefficient C is given by are the temperatures of the two surfaces, is the absolute zero on the temperature scale being is the Stefan-Boltzmann constant, where viewfactor, which corresponds to viewing the master surface from the slave surface. are the surface emissivities, and F is the effective and The viewfactor F must be defined as a function of the clearance, d, and should have a value between 0.0 and 1.0. At least two pairs of points are required to define the viewfactor, and the tabular data must start at zero clearance (closed gap) and define the viewfactor as the clearance increases. The value of F drops to zero immediately after the last data point, so there is no radiative heat transfer when the clearance is greater than the value corresponding to the last data point . 1.0 0.0 Figure 36.2.1–3 Example of input data to define the viewfactor as a function of clearance. Input File Usage: *GAP RADIATION , , , Abaqus/CAE Usage: … Interaction module: contact property editor: Thermal→Radiation: Emissivity of master surface: , Viewfactor and Clearance , Emissivity of slave surface: Specifying the value of absolute zero You must specify the value of . Input File Usage: Abaqus/CAE Usage: *PHYSICAL CONSTANTS, ABSOLUTE ZERO= Any module: Model→Edit Attributes→model_name: Absolute zero temperature: Specifying the Stefan-Boltzmann constant You must specify the Stefan-Boltzmann constant, . Input File Usage: Abaqus/CAE Usage: *PHYSICAL CONSTANTS, STEFAN BOLTZMANN= Any module: Model→Edit Attributes→model_name: Stefan-Boltzmann constant: Improving convergence in Abaqus/Standard Since the heat flux due to radiation is a strongly nonlinear function of the temperature, the radiation equations are strongly nonsymmetric and using the unsymmetric matrix storage and solution scheme for the step may improve the convergence rate in Abaqus/Standard . Modeling heat generated by nonthermal surface interactions In fully coupled temperature-displacement, fully coupled thermal-electrical-structural, or coupled thermal-electrical simulations, Abaqus allows for heat generation due to the dissipation of energy created by the mechanical or electrical interaction of contacting surfaces. The source of the heat in a fully coupled temperature-displacement analysis and a fully coupled thermal-electrical-structural analysis is frictional sliding; the source in a coupled thermal-electrical and a fully coupled thermal-electrical-structural analysis simulation is the flow of electrical current across the interface surfaces. By default, Abaqus releases all of the dissipated energy as heat between the surfaces and distributes it equally between the two interacting surfaces. You can specify the fraction of dissipated energy converted into heat, weighting factor, f (default is 0.5), for distribution of the heat between the interacting surfaces. includes a factor to convert mechanical energy into thermal energy. (default is 1.0), and the often f = 1.0 indicates that all of the generated heat flows into the first (slave) surface of the contact pair. f = 0.0 indicates that all of the generated heat flows into the opposite (master) surface. Unless valid experimental data suggest otherwise, it is best to assume the default value of f = 0.5 because this value evenly distributes the generated heat between the surfaces. If user subroutine UINTER, VUINTER, or VUINTERACTION is used to define the interfacial constitutive behavior, all gap heat generation effects will be turned off; you must supply an additional heat flux in the user subroutine to model these effects. *GAP HEAT GENERATION , f Input File Usage: Abaqus/CAE Usage: Interaction module: contact property editor: Thermal→Heat Generation: Specify: and f Heat generated due to frictional sliding In coupled thermal-mechanical and coupled thermal-electrical-structural surface interactions, the rate of frictional energy dissipation is given by is the frictional stress and where surface is assumed to be is the slip rate. The amount of this energy released as heat on each and and f are defined above. The heat flux into the slave surface is , and the heat into the master where surface is . Heat generated due to flow of electrical current in Abaqus/Standard In a coupled thermal-electrical analysis and a fully coupled thermal-electrical-structural analysis , the rate of electrical energy dissipated by electric current flowing across the interface is where J is the electrical current density and The amount of this energy released as heat on each of the interface surfaces is assumed to be are the electrical potentials on the two surfaces. and and where surface is and f are defined in the same way as for frictional dissipation. Again, the heat flux into the slave . , and the heat into the master surface is Surface-based interaction variables for thermal contact property models Abaqus provides many output variables related to the thermal interaction of surfaces. In Abaqus/Standard the values of these variables are always given at the nodes of the slave surface. In Abaqus/Explicit these variables can be output for master and slave surfaces, although they are not available for analytical surfaces. The variables are available only for simulations that use surface-based contact definitions. They can be requested as surface output to the data, results, or output database files . Surface-based interaction variables for heat fluxes The following variables are available for any simulation in which heat transfer can occur (fully coupled temperature-displacement, fully coupled thermal-electrical-structural, coupled thermal-electrical, or pure heat transfer analyses): HFL HFLA HTL HTLA Heat flux per unit area leaving the surface. HFL multiplied by the nodal area. Time integrated HFL. Time integrated HFLA. Abaqus/Standard provides all of these variables by default whenever surface output is requested to the data or results file and thermal surface interactions are present. These variables can also be displayed in contour plots in the Visualization module of Abaqus/CAE (Abaqus/Viewer). Surface-based interaction variables for heat generated by frictional sliding The following variables are available for fully coupled temperature-displacement simulations in which there is frictional interaction between contacting surfaces or user subroutine UINTER, VUINTER, or VUINTERACTION is used: SFDR SFDRA SFDRT SFDRTA WEIGHT Heat flux per unit area entering the surface due to frictional dissipation (includes ). When user subroutine UINTER, heat flux to both surfaces, and VUINTER, or VUINTERACTION is used to define the interfacial thermal constitutive behavior, this quantity represents the heat flux resulting from the total energy dissipation due to friction and other dissipative effects. The effects of gap heat generation are turned off. SFDR multiplied by the nodal area. Time integrated SFDR. Time integrated SFDRA. Weighting factor, f, for heat flux distribution between the surfaces (available only in Abaqus/Standard; not available when the constitutive behavior of the interface is defined using user subroutine UINTER). Abaqus/Standard does not provide these variables by default when surface output is requested to the data or results file; you must specify the variable identifiers. Contour plots of these variables can also be created in the Visualization module of Abaqus/CAE (Abaqus/Viewer). Surface-based interaction variables for heat generated by electrical currents The following variables are available for any coupled thermal-electrical and any fully coupled thermal- electrical-structural simulation: SJD SJDA SJDT SJDTA Heat flux per unit area generated by the electrical current, includes heat flux to both surfaces ( and ). SJD multiplied by area. Time integrated SJD. Time integrated SJDA. WEIGHT Weighting factor, f, for heat flux distribution between the surfaces. Abaqus/Standard does not provide these variables by default when surface output is requested to the data or results file; you must specify the variable identifiers. Contour plots of these variables can also be plotted in the Visualization module of Abaqus/CAE (Abaqus/Viewer). Thermal interaction variables for thermal gap elements Abaqus/Standard provides the heat flux per unit area across the thermal gap elements as output. Request element output of the variable identifier HFL to the data, results, or output database file . The only nonzero component will be HFL1: there is no heat flux tangential to the interface defined by the gap element. A positive value of HFL1 indicates heat flowing in the direction of the normal to the master surface side of the element . Contours of the heat flux across the thermal contact elements can be plotted using Abaqus/CAE. Thermal interactions involving rigid bodies Various factors to consider when modeling thermal interactions involving rigid bodies are discussed in “Rigid body definition,” Section 2.4.1. For example, Abaqus/Standard does not allow modeling of thermal interactions with analytical rigid surfaces. Modeling thermal interactions with node-based surfaces The following limitations apply to fully coupled thermal-electrical-structural and fully coupled thermal- stress analyses in Abaqus/Standard: • No heat flow will occur across a contact pair involving a node-based surface. • No heat generation will occur for a contact pair involving a node-based surface. These limitations do not apply to Abaqus/Explicit and do not apply to other analysis types involving thermal overview,” Section 6.5.1). interactions in Abaqus/Standard . Thermal interactions between surfaces with nodes containing multiple temperature degrees of freedom When the surfaces involved in a thermal interaction are defined on shell elements that have multiple temperature degrees of freedom at each node, the choice of the temperature degree of freedom at a given node for the thermal interaction depends on how the surface is defined. For an element-based surface the temperature degree of freedom closest to the surface is chosen; i.e., the first temperature degree of freedom at the node for the bottom surface and the last temperature degree of freedom at the node for the top surface. For a node-based surface the first temperature degree of freedom at the node is always chosen for a thermal interaction. 36.3 Electrical contact properties • “Electrical contact properties,” Section 36.3.1 36.3.1 ELECTRICAL CONTACT PROPERTIES Products: Abaqus/Standard Abaqus/CAE References • “Contact interaction analysis: overview,” Section 35.1.1 • “Thermal contact properties,” Section 36.2.1 • “GAPELECTR,” Section 1.1.11 of the Abaqus User Subroutines Reference Manual • *GAP ELECTRICAL CONDUCTANCE • *SURFACE INTERACTION • “Specifying gap conductance for electrical contact property options” in “Defining a contact interaction property,” Section 15.14.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Electrical conduction between two bodies: • is proportional to the difference in electric potentials across the interface; • is a function of the clearance between the surfaces; • can be a function of contact pressure; • can be a function of surface temperatures and/or predefined field variables on the surfaces; and • can generate heat at the interface. See “Coupled thermal-electrical analysis,” Section 6.7.3, and “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4, for details on coupled thermal-electrical and coupled thermal-electrical- structural analyses. Including gap electrical conductance properties in a contact property definition You can include electrical conductance properties in a contact property definition for surface-based contact. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *SURFACE INTERACTION, NAME=name *GAP ELECTRICAL CONDUCTANCE Interaction module: contact property editor: Electrical→Electrical Conductance Modeling electrical conductance between surfaces Abaqus/Standard models the electrical current flowing between two surfaces as where J is the electrical current density flowing across the interface from point A on one surface to point B on the other, is the gap electrical conductance. Point A corresponds to a node on the slave surface of the contact pair. Point B is the point of the master surface in contact with point A. are the electrical potentials on opposite points on the surfaces, and and You can provide the electrical conductance directly or in user subroutine GAPELECTR. Defining σg directly When the gap electrical conductance is defined directly, Abaqus/Standard assumes that where is the average of the surface temperatures at A and B, is the clearance between A and B, is the contact pressure transmitted across the interface between A and B, and is the average of any predefined field variables at A and B. Defining gap electrical conductance as a function of clearance a function of the clearance, d. When You can create a table of data defining the dependence of in Abaqus is to make tabular data must start at zero clearance (closed gap) and define value of electrical conductance is not also defined as a function of contact pressure, the zero clearance value for all pressures, as shown in Figure 36.3.1–1(a). on the variables listed above. The default is a function of gap clearance, d, the as a function of the clearance. The remains constant for clearances outside of the interval defined by the data points. If gap will remain constant at Σg Σg (a) (b) Figure 36.3.1–1 Examples of defining the gap electrical conductance as a function of clearance (a) or contact pressure (b). Input File Usage: *GAP ELECTRICAL CONDUCTANCE , , Abaqus/CAE Usage: Interaction module: contact property editor: Electrical→Electrical Conductance; Definition: Tabular; Use only clearance- dependency data Defining gap electrical conductance as a function of contact pressure as a function of the contact pressure, p. When is a function of contact pressure You can define at the interface, the tabular data must start at zero contact pressure (or, in the case of contact that can support a tensile force, the data point with the most negative pressure) and define as p increases. The value of remains constant for contact pressures outside of the interval defined by the data points. If gap electrical conductance is not also defined as a function of clearance, is zero for all positive values of clearance and discontinuous at zero clearance, as shown in Figure 36.3.1–1(b). *GAP ELECTRICAL CONDUCTANCE, PRESSURE Input File Usage: , , Abaqus/CAE Usage: Interaction module: contact property editor: Electrical→Electrical Conductance; Definition: Tabular; Use only pressure-dependency data Gap electrical conductance as a function of both clearance and contact pressure to depend on both clearance and pressure. A discontinuity in You can define and that defines the pressure dependence. The gap electrical conductance, pressures outside of the interval defined by the data points. The pressure dependence of into the negative pressure region even if no data points with negative pressure are included. . Once contact occurs, the conductance is always evaluated based on the portion of the curve , remains constant for contact is extended is allowed at Input File Usage: Use both of the following options: *GAP ELECTRICAL CONDUCTANCE , , *GAP ELECTRICAL CONDUCTANCE, PRESSURE , , Abaqus/CAE Usage: Interaction module: contact property editor: Electrical→Electrical Conductance; Definition: Tabular; Use both clearance- and pressure-dependency data Defining gap electrical conductance to be a function of predefined field variables . By The gap electrical conductance can be dependent on any number of predefined field variables, default, it is assumed that the electrical conductivity depends only on the surface separation and, possibly, on the average interface temperature. Input File Usage: *GAP ELECTRICAL CONDUCTANCE, DEPENDENCIES=n Abaqus/CAE Usage: Interaction module: contact property editor: Electrical→Electrical Conductance; Definition: Tabular, Clearance Dependency and/or Pressure Dependency, Number of field variables: n Defining σg using user subroutine GAPELECTR When dependencies of define is defined in user subroutine GAPELECTR, there is greater flexibility in specifying the than there is using direct tabular input. For example, it is no longer necessary to as a function of the average of the two surfaces’ temperatures or field variables: Input File Usage: Abaqus/CAE Usage: *GAP ELECTRICAL CONDUCTANCE, USER Interaction module: contact property editor: Electrical→Electrical Conductance; Definition: User-defined Modeling heat generated by electrical conduction between surfaces Abaqus/Standard can include the effect of heat generated by electrical conduction between surfaces in a coupled thermal-electrical and a fully coupled thermal-electrical-structural analysis. By default, all dissipated electrical energy is converted to heat and distributed equally between the two surfaces. You can modify the fraction of electrical energy that is released as heat and the distribution between the two surfaces; see “Modeling heat generated by nonthermal surface interactions” in “Thermal contact properties,” Section 36.2.1, for details. Surface-based output variables for electrical contact property models Abaqus/Standard provides the following output variables related to the electrical interaction of surfaces: ECD ECDA ECDT ECDTA Electric current per unit area leaving slave surface. ECD multiplied by the area associated with the slave node. Time integrated ECD. Time integrated ECDA. The values of these variables are always given at the nodes of the slave surface. They can be requested as surface output to the data, results, or output database files . Contour plots of these variables can also be displayed in the Visualization module of Abaqus/CAE (Abaqus/Viewer). 36.4 Pore fluid contact properties • “Pore fluid contact properties,” Section 36.4.1 36.4.1 PORE FLUID CONTACT PROPERTIES Product: Abaqus/Standard References • “Contact interaction analysis: overview,” Section 35.1.1 • *CONTACT PERMEABILITY • *SURFACE • *SURFACE INTERACTION • *CONTACT PAIR Overview The pore fluid contact property models: • are often used in geotechnical applications, where pore pressure continuity between material on opposite sides of an interface must be maintained; • govern pore fluid flow across a contact interface and into a gap region for nearby contact surfaces; • are applicable when pore pressure degrees of freedom are present on both sides of a contact interface (if pore pressure degrees of freedom are present on only one side of a contact interface, the surfaces are treated as impermeable); • affect the pore fluid flow normal to the contact surfaces; • can apply to small- and finite-sliding contact formulations; and • assume that there is no fluid flowing tangentially to the surface. Contact in coupled pore fluid diffusion/stress analysis involves displacement constraints to resist penetrations and pore fluid contact properties that influence the fluid flow. See “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1, for details on coupled pore fluid diffusion/stress analyses. See “Defining the constitutive response of fluid within the cohesive element gap,” Section 32.5.7, for details on the use of pore pressure cohesive elements as an alternative to using contact models and pore fluid contact properties. Contact pressure in pore fluid interactions The pore fluid contact properties discussed in this section apply when pore pressure degrees of freedom exist on both sides of a contact interface. In such cases the calculated contact pressure is effective; it does not include the pore fluid pressure contribution. If only one side of a contact interface includes pore pressure degrees of freedom, no fluid flow into or across the contact interface occurs. In this case the reported contact pressure represents the total pressure, including the effective structural and pore fluid pressure contributions; but only the effective contact pressure is used for the computation of friction. Including pore fluid properties in a contact property definition Abaqus/Standard assumes that pore fluid flows in the normal direction at a contact interface and does not flow tangentially along the interface. Two contributions to the fluid flow into each surface at a contact interface are generally present, as shown in Figure 36.4.1–1. The fluid flow into the master and slave surface at corresponding points on the interface are , respectively. and • One contribution ( ) is associated with flow across the interface. A positive value of corresponds to flow out from the master surface and into the slave surface. • The other contribution ( for the slave surface and for the master surface) is associated with removing or adding fluid from the region between the surfaces while the gap distance is changing. The sign convention is such that are positive when these contributions flow into the respective surfaces (while the gap width decreases). The sum of (which is the same as the sum of ) is equal to negative one times the rate of change of and the gap width up to the threshold distance discussed in “Controlling the distance within which pore fluid contact properties are active.” and and In steady-state analyses the rate of separation of the surfaces is zero, so the fluid flow contributions and are zero; all fluid flowing out of one surface flows into the other in steady-state analyses. Slave surface d1 qS1= qgap S1 + qacross1 qM1= qgap M1 – qacross1 d2 Master surface Figure 36.4.1–1 Flow patterns in the interface contact element. Pore fluid flow at a contact interface typically occurs even if contact permeability characteristics are not explicitly specified in the contact property definition. Alternatively, you can directly specify contact permeability characteristics for enhanced control over the flow of fluid across a contact interface. Input File Usage: *SURFACE INTERACTION, NAME=interaction_name *CONTACT PERMEABILITY Controlling the distance within which pore fluid contact properties are active The models governing fluid flow across a contact interface are most appropriate for two surfaces in contact or separated by a relatively small gap distance. By default, Abaqus assumes no fluid flow occurs once the surfaces have separated by a distance larger than the characteristic element length of the underlying surfaces. Alternatively, you can directly specify a cutoff gap distance beyond which no fluid flow occurs. Separate controls are provided for the contribution of fluid flow across the interface ( ) and the contribution of fluid flow into the interface ( ). Input File Usage: ) for the Use the following option to specify a cutoff distance ( contribution of fluid flow across the contact interface ( *CONTACT PERMEABILITY, CUTOFF FLOW ACROSS= Use the following option to specify a cutoff distance ( of fluid flow into the contact interface ( *CONTACT PERMEABILITY, CUTOFF GAP FILL= ): ): ) for the contribution Controlling contact permeability associated with fluid flow across a contact interface If you do not specify contact permeability characteristics, the default model ensures continuity of the pore pressures on opposite sides of a contact interface while the contact separation is less than the threshold distance discussed in “Controlling the distance within which pore fluid contact properties are active”: where that contact permeability across the interface is infinite. and are pore pressures at points on opposite sides of the interface. This relationship implies Alternatively, you can specify a contact permeability, k, such that fluid flow across a contact , discussed above in “Including pore fluid properties in a contact property definition”) interface ( is proportional to the difference in pore pressure magnitudes across the interface: When defining k directly, define it as where is the contact pressure transmitted across the interface between A and B, is the average of the pore pressures at A and B, is the average of the surface temperatures at A and B, and is the average of any predefined field variables at A and B. Figure 36.4.1–2 shows an example of k depending on the contact pressure. Use tabular data to specify the value of k at one or more contact pressures as p increases. The value of k remains constant for contact pressures outside of the interval defined by the data points. Once the surfaces have separated, k remains at a constant value until the separation between the surfaces exceeds the specified flow cutoff distance , at which point k drops to zero. specified data points dclearance dacross_cutoff pcontact Figure 36.4.1–2 Contact-pressure-dependent contact permeability. Input File Usage: *CONTACT PERMEABILITY , , , Defining gap permeability to be a function of predefined field variables In addition to the dependencies mentioned previously, the gap permeability can be dependent on any number of predefined field variables, . To make the gap permeability depend on field variables, at least two data points are required for each field variable value. Input File Usage: *CONTACT PERMEABILITY, DEPENDENCIES=n , , , , Coupled heat transfer–pore fluid contact properties Heat transfer can be considered simultaneously with pore fluid flow, in which case heat flow across the contact interface can occur in conjunction with fluid flow. These various contact property aspects are defined with separate options as part of a single contact property definition that you assign to the contact interaction; see “Thermal contact properties,” Section 36.2.1, for details on defining heat transfer properties. Output You can write the contact surface variables associated with the interaction of contact pairs to the Abaqus/Standard data (.dat), results (.fil), and output database (.odb) files. In addition to the surface variables associated with the mechanical contact analysis (shear stresses, contact pressures, etc.) several pore fluid-related variables (such as pore fluid volume flux per unit area) on the contact interface can be reported. A detailed discussion of these output requests can be found in “Surface output from Abaqus/Standard” in “Output to the data and results files,” Section 4.1.2, and “Surface output in Abaqus/Standard and Abaqus/Explicit” in “Output to the output database,” Section 4.1.3. Abaqus/Standard provides the following output variables related to the pore fluid interaction of surfaces: PFL PFLA PTL PTLA TPFL TPTL Pore volume flux per unit area leaving the slave surface. PFL multiplied by the area associated with the slave node. Time integrated PFL. Time integrated PFLA. Total pore volume flux leaving the slave surface. Time integrated TPFL. 37. Contact Formulations and Numerical Methods Contact formulations and numerical methods in Abaqus/Standard Contact formulations and numerical methods in Abaqus/Explicit 37.1 37.1 Contact formulations and numerical methods in Abaqus/Standard • “Contact formulations in Abaqus/Standard,” Section 37.1.1 • “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2 • “Smoothing contact surfaces in Abaqus/Standard,” Section 37.1.3 37.1.1 CONTACT FORMULATIONS IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Surfaces: overview,” Section 2.3.1 • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • *CONTACT • *CONTACT PAIR • “Defining general contact,” Section 15.13.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining self-contact,” Section 15.13.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Using contact and constraint detection,” Section 15.16 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Abaqus/Standard provides several contact fomulations. Each formulation is based on a choice of a contact discretization, a tracking approach, and assignment of “master” and “slave” roles to the contact surfaces. For general contact interactions, the discretization, tracking approach, and surface role assignments are selected automatically by Abaqus/Standard; for contact pairs, you can specify these aspects of the contact formulation using the interface described in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1. The default contact formulation is applicable in most situations, but you may find it desirable to choose another formulation in some cases. This section discusses in detail the formulations that Abaqus/Standard uses in contact simulations. Your choice of a tracking approach will have a considerable impact on how contact surfaces interact. In Abaqus/Standard there are two tracking approaches to account for the relative motion of two interacting surfaces in mechanical contact simulations: • finite sliding, which is the most general and allows any arbitrary motion of the surfaces ; and • small sliding, which assumes that although two bodies may undergo large motions, there will be relatively little sliding of one surface along the other . You can choose between node-to-surface contact discretization and true surface-to-surface contact discretization for each of the above tracking approaches. Formulations for general contact in Abaqus/Standard always uses the finite-sliding, surface-to-surface contact General contact formulation. This formulation can also be used for contact pairs, but it is not the default. The discussions in this section of finite-sliding, surface-to-surface contact apply equally to general contact and to contact pairs. In a general contact domain the master and slave roles are assigned to surfaces automatically, although it is possible to override these default assignments. The behavior of master surfaces and slave surfaces is consistent across general contact and contact pair interactions. The specification of master and slave surfaces in a general contact domain is covered in detail in “Numerical controls for general contact in Abaqus/Standard,” Section 35.2.6. Discretization of contact pair surfaces Abaqus/Standard applies conditional constraints at various locations on interacting surfaces to simulate contact conditions. The locations and conditions of these constraints depend on the contact discretization used in the overall contact formulation. Abaqus/Standard offers two contact discretization options: a traditional “node-to-surface” discretization and a true “surface-to-surface” discretization. Node-to-surface contact discretization With traditional node-to-surface discretization the contact conditions are established such that each “slave” node on one side of a contact interface effectively interacts with a point of projection on the “master” surface on the opposite side of the contact interface . Thus, each contact condition involves a single slave node and a group of nearby master nodes from which values are interpolated to the projection point. Traditional node-to-surface discretization has the following characteristics: • The slave nodes are constrained not to penetrate into the master surface; however, the nodes of the master surface can, in principle, penetrate into the slave surface (for example, see the case on the upper-right of Figure 37.1.1–2). • The contact direction is based on the normal of the master surface. • The only information needed for the slave surface is the location and surface area associated with each node; the direction of the slave surface normal and slave surface curvature are not relevant. Thus, the slave surface can be defined as a group of nodes—a node-based surface. • Node-to-surface discretization is available even if a node-based surface is not used in a contact pair definition. Surface-to-surface contact discretization Surface-to-surface discretization considers the shape of both the slave and master surfaces in the region of contact constraints. Surface-to-surface discretization has the following key characteristics: master surface slave surface closest point to A closest point to B Figure 37.1.1–1 Node-to-surface contact discretization. Node-to-Surface Contact Node-to-Surface Contact slave master master slave Surface-to-Surface Contact Surface-to-Surface Contact slave master master slave Figure 37.1.1–2 Comparison of contact enforcement for different master-slave assignments with node-to-surface and surface-to-surface contact discretizations. • The surface-to-surface formulation enforces contact conditions in an average sense over regions nearby slave nodes rather than only at individual slave nodes. The averaging regions are approximately centered on slave nodes, so each contact constraint will predominantly consider one slave node but will also consider adjacent slave nodes. Some penetration may be observed at individual nodes; however, large, undetected penetrations of master nodes into the slave surface do not occur with this discretization. Figure 37.1.1–2 compares contact enforcement for node-to-surface and surface-to-surface contact for an example with dissimilar mesh refinement on the contacting bodies. • The contact direction is based on an average normal of the slave surface in the region surrounding a slave node. • Surface-to-surface discretization is not applicable if a node-based surface is used in the contact pair definition. Choosing a contact discretization In general, surface-to-surface discretization provides more accurate stress and pressure results than node- to-surface discretization if the surface geometry is reasonably well represented by the contact surfaces. Figure 37.1.1–3 shows an example of improved contact pressure accuracy with surface-to-surface contact compared to node-to-surface contact. Figure 37.1.1–3 Comparison of contact pressure accuracy for node-to-surface and surface-to-surface contact discretizations. Since node-to-surface discretization simply resists penetrations of slave nodes into the master surface, forces tend to concentrate at these slave nodes. This concentration leads to spikes and valleys in the distribution of pressure across the surface. Surface-to-surface discretization resists penetrations in an average sense over finite regions of the slave surface, which has a smoothing effect. As the mesh is refined, the discrepancies between the discretizations lessen, but for a given mesh refinement the surface- to-surface approach tends to provide more accurate stresses. Contact using surface-to-surface discretization is also less sensitive to master and slave surface designations than node-to-surface contact . Figure 37.1.1–4 shows a simple model involving two blocks with dissimilar mesh densities. uniform pressure Figure 37.1.1–4 Test model for comparison of different master and slave surface designations. The bottom block is fixed to the ground, and a uniform pressure of 100 Pa is applied to the top face of the top block. Analytically, the top block should exert a uniform pressure of 100 Pa on the bottom block across the entire contact interface. Table 37.1.1–1 compares the Abaqus analysis results for different contact discretizations and slave surface designations. Table 37.1.1–1 Error (from analytical results) for various discretization/slave surface combinations. Contact discretization Slave Surface Maximum error in CPRESS Node-to-surface Surface-to-surface Top block Bottom block Top block Bottom block 13% 31% ~1% ~1% If the surface geometry is not well-represented due to the use of a coarse mesh, significant inaccuracies can exist regardless of whether surface-to-surface contact or node-to-surface contact In some cases surface smoothing techniques available for surface-to-surface contact can is used. significantly improve solutions obtained with a coarse mesh. See “Smoothing contact surfaces in Abaqus/Standard,” Section 37.1.3, for a discussion of surface smoothing options for surface-to-surface contact. Surface-to-surface discretization generally involves more nodes per constraint and can, therefore, increase solution cost. In most applications the extra cost is fairly small, but the cost can become significant in some cases. The following factors (especially in combination) can lead to surface-to-surface contact being costly: • A large fraction of the model is involved in contact. • The master surface is more refined than the slave surface. • Multiple layers of shells are involved in contact, such that the master surface of one contact pair acts as the slave surface of another contact pair. The surface-to-surface formulation is primarily intended for common situations in which normal directions of contacting surfaces are approximately opposite. The node-to-surface contact formulation is often preferable for treating contact involving feature edges or corners if the respective slave and master facet normal directions are not approximately opposite in the active contact region. Contact tracking approaches In Abaqus/Standard there are two tracking approaches to account for the relative motion of two interacting surfaces in mechanical contact simulations. The finite-sliding tracking approach Finite-sliding contact is the most general tracking approach and allows for arbitrary relative separation, sliding, and rotation of the contacting surfaces. For finite-sliding contact the connectivity of the currently active contact constraints changes upon relative tangential motion of the contacting surfaces. For a detailed description of how Abaqus/Standard calculates finite-sliding contact, see “Using the finite-sliding tracking approach” later in this section. The small-sliding tracking approach Small-sliding contact assumes that there will be relatively little sliding of one surface along the other and is based on linearized approximations of the master surface per constraint. The groups of nodes involved with individual contact constraints are fixed throughout the analysis for small-sliding contact, although the active/inactive status of these constraints typically can change during the analysis. You should consider using small-sliding contact when the approximations are reasonable, due to computational savings and added robustness. For a detailed description of how Abaqus/Standard calculates small-sliding contact, see “Using the small-sliding tracking approach” later in this section. Choosing the master and slave roles in a two-surface contact pair Abaqus/Standard enforces the following rules related to the assignment of the master and slave roles for contact surfaces: • Analytical rigid surfaces and rigid-element-based surfaces must always be the master surface. • A node-based surface can act only as a slave surface and always uses node-to-surface contact. • Slave surfaces must always be attached to deformable bodies or deformable bodies defined as rigid. • Both surfaces in a contact pair cannot be rigid surfaces with the exception of deformable surfaces defined as rigid . When both surfaces in a contact pair are element-based and attached to either deformable bodies or deformable bodies defined as rigid, you have to choose which surface will be the slave surface and which will be the master surface. This choice is particularly important for node-to-surface contact. Generally, if a smaller surface contacts a larger surface, it is best to choose the smaller surface as the slave surface. If that distinction cannot be made, the master surface should be chosen as the surface of the stiffer body or as the surface with the coarser mesh if the two surfaces are on structures with comparable stiffnesses. The stiffness of the structure and not just the material should be considered when choosing the master and slave surface. For example, a thin sheet of metal may be less stiff than a larger block of rubber even though the steel has a larger modulus than the rubber material. If the stiffness and mesh density are the same on both surfaces, the preferred choice is not always obvious. The choice of master and slave roles typically has much less effect on the results with a surface-to- surface contact formulation than with a node-to-surface contact formulation. However, the assignment of master and slave roles can have a significant effect on performance with surface-to-surface contact if the two surfaces have dissimilar mesh refinement; the solution can become quite expensive if the slave surface is much coarser than the master surface. Fundamental choices affecting the contact formulation Your choice of contact discretization and tracking approach have considerable impact on an analysis. In addition to the qualities already discussed, certain combinations of discretizations and tracking approaches have their own characteristics and limitations associated with them. These characteristics are summarized in Table 37.1.1–2. You should also consider the solution costs associated with the various contact formulations. Accounting for shell thickness Most contact formulations will account for the surface thickness of a shell when calculating contact constraints. However, the finite-sliding, node-to-surface formulation will not account for shell thicknesses. These calculations are discussed in more detail in “Accounting for shell and membrane thickness” in “Assigning surface properties for contact pairs in Abaqus/Standard,” Section 35.3.2. Allowing for self-contact Self-contact is typically the result of large deformation in a model. It is often difficult to predict which regions will be involved in the contact or how they will move relative to each other. Therefore, self- contact cannot use the small-sliding tracking approach. Table 37.1.1–2 Comparison of contact formulation characteristics. Contact formulation Characteristic Node-to-surface Surface-to-surface Finite-sliding Small-sliding Finite-sliding Small-sliding Account for shell thickness by default Allow self-contact Allow double-sided surfaces No Yes Yes No Slave surface only Slave surface only Surface smoothing by default Some smoothing of master surface Yes for anchor points; each constraint uses flat approximation of master surface Yes Yes Yes1 No Yes No Yes No for anchor points; each constraint uses flat approximation of master surface Augmented Lagrange method for 3-D self-contact; otherwise, direct method Direct method Penalty method Direct method No No Yes Yes Default constraint enforcement method Ensure moment equilibrium for offset reference surfaces with friction 1 Double-sided master surfaces are allowed with the finite-sliding, surface-to-surface formulation only if the path-based tracking algorithm is used . Double-sided slave surfaces are allowed with both tracking algorithms if the master surface is not user defined. Allowing double-sided surfaces Doubled-sided contact surfaces based on shell-like elements are allowed to act as slave and/or master surfaces for the surface-to-surface contact formulation by default and are allowed to act as the slave surface for the node-to-surface contact formulation. For a shell-like surface to act as the master surface for the surface-to-surface formulation with the optional state-based tracking algorithm or for the node-to-surface contact formulation, the surface must be defined as single-sided (see “Defining single-sided surfaces” in “Element-based surface definition,” Section 2.3.2, and “Orientation considerations for shell-like surfaces” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1, for more information). Surface smoothing When using node-to-surface discretization, corners or small protrusions of a jagged master surface are allowed to penetrate the spaces between nodes in the node-based surface. It is sometimes possible for a slave node sliding along the master surface to snag on these corners. Therefore, Abaqus/Standard automatically smooths the master surface for contact calculations utilizing node-to-surface discretization to minimize this phenomenon. The details are discussed further in “Smoothing master surfaces for the finite-sliding, node-to-surface formulation” later in this section. No surface smoothing occurs by default when using surface-to-surface discretization. Surface-to-surface discretization considers contact conditions in an average sense over a finite region, which tends to alleviate problems associated with small protrusions of the master surface penetrating the slave surface and introduces some inherent smoothing characteristics at the constraint level. However, this inherent smoothing typically does not significantly mitigate errors associated with poor geometric representations of curved surfaces when a relatively coarse mesh is used. In some cases nondefault circumferential or spherical surface smoothing methods available for surface-to-surface contact can significantly improve solutions obtained with a coarse mesh . Constraint enforcement methods In many cases Abaqus/Standard strictly enforces the contact constraints discussed previously by default. However, strict enforcement of contact constraints can sometimes lead to overconstraint issues (for example, see “Overconstraint checks,” Section 34.6.1) or convergence difficulty. To address these issues and allow for decreased solution cost with typically minimal sacrifice to solution accuracy, Abaqus/Standard also provides penalty-based constraint enforcement methods. The numerical constraint enforcement methods (and defaults) are discussed in detail in “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2. Moment equilibrium Based on Newton’s third law of motion, contact forces should be self-equilibrating; that is, the net contact forces acting on the respective surfaces for each active contact constraint should be equal and opposite and effectively act through a common point. Contact constraints based on surface-to-surface contact discretization always exhibit this characteristic. Contact constraints based on node-to-surface discretization always generate zero net force, but under certain circumstances can generate a net moment in the numerical solution. Frictional forces associated with node-to-surface contact constraints will generate net moment if an offset exists between the respective reference surfaces. The following factors can contribute to a normal-direction offset between nodes of respective contact surfaces while contact constraints are active: • The presence of a softened pressure-versus-overclosure behavior (due to a user-specified, softened pressure-overclosure model or use of a constraint enforcement method, such as the penalty method, that exhibits numerical softening. • Contact calculations accounting for shell or membrane thicknesses (which is not allowed with the finite-sliding, node-to-surface formulation). • User-specified initial contact clearances . • Various usages of special-purpose contact elements, such as tube-to-tube contact elements , result in some normal distance between nodes that interact with each other. While undesirable, the net moment that sometimes occurs with node-to-surface contact constraints is typically not significantly detrimental to the analysis results. Effect of the contact discretization method on solution cost There is no easy way to predict which contact discretization method will result in lower overall solution cost. Basic trends include: • Node-to-surface contact discretization tends to be less costly per iteration than surface-to-surface contact discretization (because surface-to-surface contact discretization generally involves more nodes per constraint). • Contact conditions with finite-sliding contact tend to converge in fewer iterations with surface-to- surface contact discretization than with node-to-surface contact discretization (because surface-to- surface contact discretization has more continuous behavior upon sliding). Using the finite-sliding tracking approach The finite-sliding tracking approach allows for arbitrary separation, sliding, and rotation of the surfaces. Abaqus/Standard contact pairs use a finite-sliding, node-to-surface contact formulation by default. General contact in Abaqus/Standard always uses a finite-sliding, surface-to-surface contact formulation. Example Consider the case shown in Figure 37.1.1–5, with surface ASURF acting as the slave surface to surface BSURF in a finite-sliding, node-to-surface contact pair. In this example slave node 101 may come into contact anywhere along the master surface BSURF. While in contact, it is constrained to slide along BSURF, irrespective of the orientation and deformation of this surface. This behavior is possible because Abaqus/Standard tracks the position of node 101 relative to the master surface BSURF as the bodies deform. Figure 37.1.1–6 shows the possible evolution of the contact between node 101 and its master surface BSURF. Node 101 is in contact with the element face with end nodes 201 and 202 at time . The load transfer at this time occurs between node 101 and nodes 201 and 202 only. Later on, at time , node 101 may find itself in contact with the element face with end nodes 501 and 502. Then the load transfer will occur between node 101 and nodes 501 and 502. ESETB ESETA 502 BSURF 201 501 202 101 102 103 ASURF Figure 37.1.1–5 Contacting bodies. BSURF 201 t = t 1 202 501 502 t = t 2 101 t = 0 Figure 37.1.1–6 Trajectory of node 101 in finite-sliding contact. Path-based versus state-based tracking algorithms Brief descriptions of the tracking algorithms available in Abaqus/Standard are provided below so that you can be aware of their characteristics and available options. Path-based tracking algorithm The “path-based” tracking algorithm carefully considers the relative paths of points on the slave surface with respect to the master surface within each increment and allows for double-sided shell and membrane master surfaces. The path-based tracking algorithm is available only for finite-sliding, surface-to-surface contact interactions involving element-based master surfaces and is the default for those interactions. The path-based algorithm is sometimes more effective than the state-based algorithm for analyses involving self-contact or large incremental relative motion. Input File Usage: Use the following option to specify use of the path-based tracking algorithm: Abaqus/CAE Usage: *CONTACT PAIR, INTERACTION=interaction_property_name, TYPE=SURFACE TO SURFACE, TRACKING=PATH Interaction module: surface-to-surface contact or self-contact interaction editor: Discretization method: Surface to surface, Contact tracking: Two configurations (path) State-based tracking algorithm The “state-based” tracking algorithm updates the tracking state based on the tracking state associated with the beginning of the increment together with geometric information associated with the predicted configuration. This algorithm is well-suited for most finite-sliding analyses but requires the use of single- sided surfaces and occasionally has difficulty tracking large incremental motion. State-based tracking may miss detecting contact if the incremental relative motion exceeds the dimensions of the master surface or if the incremental motion cuts across corners of the master surface; specifying an upper bound for the increment size helps avoid these problems. The state-based tracking algorithm is: • the only tracking algorithm available for finite-sliding, node-to-surface contact pairs; • the only tracking algorithm available for finite-sliding contact interactions involving an analytical rigid master surface; • a non-default option for finite-sliding, surface-to-surface contact pairs involving an element-based master surface. Input File Usage: Use the following option to specify use of the state-based tracking algorithm: Abaqus/CAE Usage: *CONTACT PAIR, INTERACTION=interaction_property_name, TYPE=SURFACE TO SURFACE, TRACKING=STATE Interaction module: surface-to-surface contact or self-contact interaction editor: Discretization method: Surface to surface, Contact tracking: Single configuration (state) Smoothing master surfaces for the finite-sliding, node-to-surface formulation The finite-sliding, node-to-surface contact formulation requires that master surfaces have continuous surface normals at all points. Convergence problems can result if master surfaces that do not have continuous surface normals are used in finite-sliding, node-to-surface contact analyses; slave nodes tend to get “stuck” at points where the master surface normals are discontinuous. Abaqus/Standard automatically smooths the surface normals of element-based master surfaces used in finite-sliding, node-to-surface contact simulations, including those modeled with slide lines. You are expected to create smooth analytical rigid surfaces . No such smoothing of master surface normals is needed with the finite-sliding, surface-to-surface formulation. Smoothing deformable master surfaces and rigid surfaces defined with rigid elements For finite-sliding, node-to-surface contact simulations with planar or axisymmetric deformable master surfaces, Abaqus/Standard will smooth any discontinuous transitions between two first-order element faces with parabolic curves. Discontinuous transitions between two second-order element faces are smoothed with cubic curves connecting two points located on the element’s faces. This smoothing is shown in Figure 37.1.1–7 for first-order elements (linear segments) and in Figure 37.1.1–8 for second-order elements (parabolic segments). For finite-sliding, node-to-surface simulations with three-dimensional deformable master surfaces and rigid master surfaces using rigid elements, Abaqus/Standard will smooth any discontinuous surface normal transitions between the master surface facets. master surface linear segments smooth transition l 1 l 2 a 1 a 2 Figure 37.1.1–7 Smoothing between linear segments. master surface quadratic segments smooth transition l 1 l 2 a 1 a 2 Figure 37.1.1–8 Smoothing between quadratic segments. You can control the degree of smoothing of the master surface in node-to-surface contact simulations or in analyses using slide lines and contact elements by specifying a fraction f. The default value of f is 0.2. are For planar or axisymmetric deformable master surfaces, the lengths of the element facets that join at the surface node and . Abaqus/Standard will construct either a parabolic or a cubic segment between two points at distances from the node at which the discontinuity exists; this smoothed segment will be used in the contact calculations. Thus, the contact surface will differ from the faceted element geometry. Smoothing affects only segments where the normal to the deformable master surface is discontinuous at the node joining two elements: it does not affect the two segments adjacent to the midside nodes on second-order element faces. , where and and For three-dimensional, element-based master surfaces, f is defined as a fraction of the dimension of a facet as shown in Figure 37.1.1–9. The normal vector of a point within the region bounded by the dashed lines is computed to be normal to the facet. Outside this region the normal is smoothed with respect to the adjacent facets, using a generalization of the two-dimensional approach shown in Figure 37.1.1–7 and Figure 37.1.1–8. The physical geometry of a three-dimensional facet is not smoothed; only the surface normal definitions associated with the facet are affected by the smoothing operation. The implementation of the normal-direction smoothing algorithm is slightly different for surfaces based on rigid type elements than other element types. This difference typically has minimal effect on the convergence behavior or solution results; however, for example, different solution behavior may occasionally be observed between otherwise identical analyses in which a rigid body is modeled with R3D4 elements in one case and S4R elements assigned to a rigid body in another case. fl2 fl2 l2 l3 fl3 fl3 fl2 l2 fl2 fl1 fl1 fl1 fl1 l1 l1 Figure 37.1.1–9 Smoothing of a three-dimensional master surface. Input File Usage: Use the following option for node-to-surface contact simulations: *CONTACT PAIR, INTERACTION=interaction_property_name, SMOOTH=f Use the following option when using slide lines and contact elements: *SLIDE LINE, ELSET=name, SMOOTH=f Abaqus/CAE Usage: Interaction module: Interaction→Create: Surface-to-surface contact (Standard) or Self-contact (Standard): Degree of smoothing for master surface: f Smoothing a deformable master surface along symmetry edges When a two-dimensional or axisymmetric deformable master surface ends at a symmetry plane and node-to-surface discretization is used, Abaqus/Standard will smooth and calculate the proper surface normals and tangent planes of the end segment if the boundary condition at the symmetry end is specified with the symmetry “type” boundary XSYMM or YSYMM. This smoothing procedure is accomplished by reflecting the end segment about the symmetry plane and constructing either a parabolic or a cubic segment between the end segment and the reflected segment. Thus, the contact surface may differ from the faceted element geometry near the end. Abaqus/Standard will automatically adjust the surface normal and tangent planes at of an axisymmetric master surface regardless of whether a symmetry boundary condition is defined. The finite-sliding, surface-to-surface formulation has no special treatment for surfaces ending at a symmetry plane. See “Modifying the master surface normals” in “Contact formulations in Abaqus/Standard,” Section 37.1.1, for a discussion of how the small-sliding, node-to- surface formulation treats master surfaces ending at a symmetry plane. See “Small-sliding, surface-to- surface contact” in “Contact formulations in Abaqus/Standard,” Section 37.1.1, for a discussion of how the small-sliding, node-to-surface formulation treats slave surfaces ending at a symmetry plane. Overriding the default smoothing behavior for finite-sliding, node-to-surface contact To model a master surface with corners in two dimensions (fold lines in three dimensions), break the surface into multiple surfaces. This technique prevents Abaqus/Standard from smoothing out the corners or fold lines and allows Abaqus/Standard to introduce constraints associated with each surface if a slave node is in contact with an interior corner or fold in the master surface. To accurately model the master surface with a corner shown in Figure 37.1.1–10, you must define two contact pairs: the first contact pair has ASURF as the slave surface and BSURFA as the master surface; the second contact pair has ASURF as the slave surface and BSURFB as the master surface. Finite sliding in a geometrically linear analysis Finite-sliding simulations usually include nonlinear geometric effects because such simulations generally involve large deformations and large rotations. However, it is also possible to use the finite-sliding tracking approach in a geometrically linear analysis . The load transfer paths between the surfaces and the contact direction are updated in finite-sliding, geometrically linear analyses. This capability is useful for analyzing finite sliding between two stiff bodies that do not undergo large rotations. Unsymmetric terms in finite-sliding contact simulations Normal contact constraints due to node-to-surface discretization produce unsymmetric terms in the system of equations when three-dimensional faceted surfaces come in contact. These terms have a BSURFA ASURF BSURFB corner Figure 37.1.1–10 Master surface with a corner. strong effect on the convergence rate in regions on the master surfaces with large differences in surface normals between facets. Normal contact constraints due to surface-to-surface discretization produce unsymmetric terms in both two- and three-dimensional cases. These terms have a strong effect on the convergence rate in regions where the master and slave surfaces are not parallel to each other. In both cases you should use the unsymmetric solution scheme for the step to improve the convergence rate of the simulation . Contact simulations that involve strong frictional effects can also produce unsymmetric terms. See “Unsymmetric terms in the system of equations” in “Frictional behavior,” Section 36.1.5, for details. Using the small-sliding tracking approach For a large class of contact problems the general tracking of the finite-sliding approach is unnecessary, even though geometric nonlinearity may need to be considered. Abaqus/Standard provides a small- sliding tracking approach for such problems. For geometrically nonlinear analyses this formulation assumes that the surfaces may undergo arbitrarily large rotations but that a slave node will interact with the same local area of the master surface throughout the analysis. For geometrically linear analyses the small-sliding approach reduces to an infinitesimal-sliding and rotation approach, in which it is assumed that both the relative motion of the surfaces and the absolute motion of the contacting bodies are small. Abaqus/Standard attempts to associate a planar approximation of the master surface with each slave node of a small-sliding contact pair. Contact interactions are considered between a given slave node (or region nearby a given slave node for the surface-to-surface formulation) and the associated local tangent plane. An example for the small-sliding, node-to-surface formulation is shown in Figure 37.1.1–11 (for example, the slave node is typically constrained not to penetrate this local tangent plane). Each local tangent plane, which is a line in two dimensions, is defined by an anchor point, , on the master surface and an orientation vector at the anchor point . 103 slave surface 102 N(X0) 104 N3 X0 N2 local tangent plane master surface N4 Figure 37.1.1–11 Definition of the anchor point and local tangent plane used by the small-sliding, node-to-surface formulation for node 103. The algorithm used to define anchor points is described below. If an anchor point cannot be determined for a particular slave node, no contact constraint will be enforced for that slave node. Having a local tangent plane for each slave node means that for the small-sliding tracking approach Abaqus/Standard does not have to monitor slave nodes for possible contact along the entire master surface. Therefore, small-sliding contact is generally less expensive computationally than finite-sliding contact. The cost savings are often most dramatic in three-dimensional contact problems. Small-sliding, node-to-surface contact For node-to-surface contact Abaqus/Standard chooses the anchor point of a slave node’s local tangent plane such that the vector from the anchor point to the slave node coincides with a smoothly varying normal vector on the master surface. The anchor point is chosen before the analysis starts using the initial configuration of the model. Smoothly varying master surface normals is The algorithm requires that the master surface have a smoothly varying normal vector any point on the master surface. The first step in defining is to construct the unit normal vectors at each node of the master surface. Abaqus/Standard forms these nodal normals by averaging the normals of the element faces making up the master surface; only the element faces in the surface definition will contribute to the nodal normals and, thus, to . Abaqus/Standard uses the initial nodal coordinates to compute these normals. , where Figure 37.1.1–11 shows the nodal unit normals for a master surface, the anchor point local tangent plane associated with slave node 103. Abaqus/Standard uses the nodal unit normals , along with the shape functions of the element containing the two nodes, to construct , and the and on the 2–3 element face. Abaqus/Standard chooses the anchor point of the local tangent plane for node 103 so that is the contact direction for slave node 103 and defines the orientation of the local tangent plane. In this example, as in many cases, the local tangent plane is only an approximation of the actual mesh geometry. passes through node 103. Modifying the master surface normals Defining user-specified nodal normals on the master surface will improve the local tangent planes calculated for the small-sliding, node-to-surface formulation in some cases. For example, a default nodal normal corresponding to an average normal among adjacent facets can cause significant deviation from the true surface normal direction at perimeter nodes, as shown in Figure 37.1.1–12. The nodal normal does not point along the symmetry plane, which means that slave node 100 will never intersect the master surface. In a small-sliding problem if a slave node fails to intersect the master surface at the start of the analysis, it will be free to penetrate the master surface because no local tangent plane will be formed. master surface CSURF slave surface DSURF N1 100 symmetry plane Figure 37.1.1–12 Master surface normal at node 1 in a small-sliding model of concentric cylinders. With the default slave node 100 will never contact CSURF. Defining a user-specified normal (1.00E+00, 0.00E+00, 0.00E+00) at node 1 on the master surface CSURF will correct the problem, as shown in Figure 37.1.1–13. This method allows slave node 100 to see the master surface, and the correct contact normal direction will be used. Master surface normals at perimeter nodes are adjusted automatically to lie along the symmetry plane if boundary conditions are specified at these nodes in symmetry “type” format (XSYMM, YSYMM, or ZSYMM—see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). master surface CSURF slave surface DSURF 100 N1 tangent plane Figure 37.1.1–13 The modified master surface normal at node 1 of CSURF now allows slave node 100 to contact CSURF. Small-sliding, surface-to-surface contact A key difference with the surface-to-surface approach is that more than one slave node is involved in each contact constraint (except when the slave surface is based on gasket elements, as discussed below). This is related to the fact that the surface-to-surface formulation enforces contact conditions in an average sense over regions nearby slave nodes rather than only at individual slave nodes . The small-sliding, surface-to-surface contact formulation is a limit case of the finite-sliding, surface-to-surface formulation, using a planar approximation of the master surface per averaging region of the slave surface. The constraint participation factors for the slave nodes remain constant for small-sliding contact. The effective center-of-action on the slave surface per contact constraint may differ slightly from the location of the predominant slave node associated with the constraint. A special version of the small-sliding, surface-to-surface formulation is used if the slave surface is based on gasket elements to avoid a tendency to trigger unstable deformation modes in the gasket elements. This special formulation has only one slave node per contact constraint and preserves the accuracy advantages of the surface-to-surface formulation, but it is not well-suited for extension to finite-sliding and is otherwise not as generally applicable as the regular small-sliding, surface-to-surface formulation. (The finite-sliding, surface-to-surface formulation always uses multiple slave nodes per constraint and is not recommended for contact involving gasket elements.) The small-sliding, surface-to-surface contact formulation determines master anchor points and normal directions in a manner similar to that used by the small-sliding, node-to-surface contact formulation; however, there are some differences. For the surface-to-surface approach the anchor point approximately corresponds to the center of the zone on the master surface where the averaging region of the slave projects onto the master surface. This projection occurs along the slave surface normal direction. This method does not make use of smoothed master surface nodal normals. The anchor point location typically does not depend significantly on whether node-to-surface or surface-to-surface discretization is used, unless the surfaces are significantly separated and non-parallel in the initial configuration (in which case small-sliding contact may not be appropriate). Abaqus/Standard automatically reverts to the node-to-surface approach for individual small-sliding contact constraints in the following circumstances, even if you have specified use of the surface-to- surface approach: • if the slave surface is a node-based surface; • if the projection along the slave surface normal direction does not intersect the master surface (but an anchor point can be found using the interpolated master surface normal direction algorithm discussed above for the small-sliding, node-to-surface formulation); or • if single-sided slave and master surfaces have surface normals in approximately the same direction. For constraints based on surface-to-surface discretization it is not necessary that the constraint associated with a node on a symmetry plane is parallel to the symmetry plane. Hence, there is usually no need to specify specific normal directions. As in the case of node-to-surface contact, the contact direction points from the anchor point to the slave node, and the tangent plane is normal to this direction. The contact normal for the small-sliding, surface-to-surface formulation is adjusted automatically to lie along the symmetry plane for each slave node that has a boundary condition specified in symmetry “type” format (XSYMM, YSYMM, or ZSYMM—see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). Orientation of local tangent planes The local tangent plane is by definition orthogonal to the contact direction. You can override the default contact direction to specify a direction with a spatially varying clearance or overclosure definition . Once the contact direction is defined, the orientation of the local tangent plane with respect to the master surface facet remains fixed. Because small-sliding contact considers nonlinear geometric effects, Abaqus/Standard continuously updates the orientation of the local tangent plane to account for the rotation and, assuming that the master surface is deformable, the deformation of the master surface. The position of the anchor point relative to the surrounding nodes on the master surface facet does not change as the master surface deforms. Load transfer In a small-sliding analysis each constraint can transfer load only to a limited number of nodes on the master surface. These nodes on the master surface are chosen based on their initial proximity to the anchor point. The magnitude of load transferred to each master surface node is based on proximity in the current, deformed configuration to the center-of-action on the slave surface (which corresponds to a slave node for the node-to-surface formulation). For example, in Figure 37.1.1–11 node 103 transmits load to both nodes 2 and 3 on the master surface if node-to-surface discretization is used (if surface-to-surface discretization is used, load may be transmitted to additional nearby master nodes). Thus, if node 103 contacts the local tangent plane, a larger share of the force would be transmitted to the master surface node, 2 or 3, closer to the slave node. When the anchor point corresponds to a node on the master surface, as is the case with slave node 104 and master surface node 3 in Figure 37.1.1–11, the transmitted load for node-to-surface contact is shared by the node at and all of the master surface nodes that share an adjacent surface facet with that node (additional master nodes may take part in the load transfer for surface-to-surface contact). In Figure 37.1.1–11 the three master surface nodes sharing the force transmitted by slave node 104 are nodes 2, 3, and 4. As the center-of-action on the slave surface for a constraint slides along its local tangent plane, Abaqus/Standard updates the distribution among the master surface nodes. However, no additional master surface nodes are ever added to the original list of nodes associated with a given small-sliding constraint. The constraint will continue to transmit load to the original list of master surface nodes, regardless of the sliding distance. Figure 37.1.1–14 shows the potential problem that arises if small sliding is used but the relative tangential motion of the surfaces is not “small.” It shows the possible evolution of contact between slave node 101 in Figure 37.1.1–5 and its master surface BSURF. Using the unit normal vectors is found for slave node 101; for the purposes of this example, assume that it lies at the midpoint of the 201–202 face. With this location of the local tangent plane for node 101 is parallel with the 201–202 face. The load transfer always occurs between node 101 and nodes 201 and 202, no matter how far node 101 slides along the local tangent plane. Therefore, if node 101 moves as shown in Figure 37.1.1–14, it will continue to transmit load to nodes 201 and 202 when, in fact, it really slid off the mesh forming the master surface BSURF. , the anchor point and 201 X0 202 BSURF N201 101 t = 0 N202 101 t > 0 Figure 37.1.1–14 Excessive sliding in a small-sliding contact analysis. What can be considered small sliding A contact pair in a small-sliding contact simulation should not grossly violate any of the assumptions or limitations outlined above. Adhere to the following guidelines: • Slave nodes should slide less than an element length from their corresponding anchor point and still be contacting their local tangent plane. If the master surface is highly curved, the slave nodes should slide only a fraction of an element length. The accumulated slip at a slave node (CSLIP) can provide a good estimate of how far a slave node has moved. • The local tangent planes formed by Abaqus/Standard should be a good approximation of the if necessary, define a user-specified normal (“Normal definitions at nodes,” mesh geometry; Section 2.1.4) to improve the smoothly varying master surface normal, . • The rotation and deformation of the master surface should not cause the local tangent planes to become a poor representation of the master surface during the course of the analysis. Choosing the master and slave surfaces in small-sliding problems The basic guidelines given in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1, should still be followed in a small-sliding simulation—the slave surface should be the more refined surface or the surface on the more deformable body. However, in a small-sliding simulation more thought must be given when defining the master surface. With small-sliding contact each slave node views the master surface as a flat surface, which can be significantly different than the true shape of the surface, even in the local region near the anchor point. In some cases the local tangent planes provide a good local approximation to the master surface in the initial configuration, but deformation and rotation of the master surface can reorient the local tangent planes such that they become a poor representation of the master surface. Figure 37.1.1–15 shows an example where distortion of the master surface results in such a situation. This problem can be minimized to some extent by using a more refined mesh on the master surface, thus providing more element faces to control the motion of the tangent planes. Excessive mesh refinement should not be necessary since only small sliding should occur. Infinitesimal sliding As was mentioned before, the small-sliding tracking approach reduces to an infinitesimal-sliding tracking approach for geometrically linear analyses. Infinitesimal sliding assumes that both the relative motions of the surfaces and the absolute motions of the model remain small. The orientations of the local tangent planes are not updated, and the load transfer paths and the weightings assigned to each master surface node remain constant during an infinitesimal-sliding simulation. As in the case of small sliding, you can choose between node-to-surface and surface-to-surface discretizations with the infinitesimal-sliding tracking approach. The same user interface applies, and the default is node-to-surface discretization. Local tangent directions on a surface Local tangent directions on a contact surface (sometimes called “slip directions”) are a reference orientation by which Abaqus calculates tangential behavior in a contact interaction. Abaqus/Standard calculates the initial orientation of the two local tangent directions by default. The local tangent directions rotate with the contact surface in a geometrically nonlinear analysis. initial configuration local tangent plane master surface slave surface large deformation Figure 37.1.1–15 Master surface deformation in a small-sliding contact analysis can cause problems with the local tangent planes. Calculating the initial local tangent directions for a two-dimensional surface Two-dimensional and standard axisymmetric models have only one local . Abaqus/Standard defines the orientation of this direction by the cross product of the vector into the plane of the model (0., 0., 1.0) and the contact normal vector. tangent direction, Models consisting of generalized axisymmetric bodies have a second local tangent direction, , to account for the component of slip associated with relative differences in circumferential twist between contacting bodies. The first local tangent direction at any point on the surface is always tangent to the master surface in the local r–z plane. The second local tangent direction is orthogonal to this plane in the local circumferential direction. For more information about generalized axisymmetric models, see “Generalized axisymmetric stress/displacement elements with twist” in “Choosing the element’s dimensionality,” Section 27.1.2. Calculating the initial local tangent directions for a three-dimensional surface By default, Abaqus/Standard determines the initial orientation of the two local tangent directions, and , using the following conventions: • Finite-sliding, surface-to-surface formulation: The default initial orientations of the two local tangent directions are based on the slave surface normal, using the standard convention for calculating surface tangents with the assumption that the contact normal corresponds to the negative normal to the slave surface. • Finite-sliding, node-to-surface formulation: For contact involving a slave surface based on three-dimensional beam-type elements, the first and second local tangent directions are defined along the length of the beam and transverse to the beam, respectively. For contact involving an analytical rigid surface and a slave surface that is not based on three-dimensional beam-type elements, the first local tangent direction is tangential to the cross-section used to generate the analytical rigid surface, and the second local tangent direction is orthogonal to the plane of the cross-section in which the contact occurs. In other cases, default initial orientations of the two local tangent directions are calculated by first computing tentative directions. For element-based slave surfaces the tentative directions are based on the slave surface using the standard convention for calculating surface tangents. For node-based slave surfaces the tentative directions are set at each node to coincide with the global x- and y-axes, respectively. Abaqus constructs an orthogonal triad of , becomes aligned with the master ), then rotates this triad such that (where , and and and surface normal at the tracked point on the master surface. • Small-sliding, surface-to-surface formulation: The default initial orientations of the two local tangent directions are based on the slave surface normal, using the standard convention for calculating surface tangents, except for contact involving analytical rigid surfaces, in which case the local tangent directions are based on the master surface normal. • Small-sliding, node-to-surface formulation: The default initial orientations of the two local tangent directions are calculated at each point on the master surface based on the master surface normal, using the standard convention for calculating surface tangents. Defining alternative initial local tangent directions for contact pair surfaces If the default local tangent directions are not convenient to prescribe an anisotropic friction model or to view contact output, you can define the local tangent directions for three-dimensional contact pair surfaces. You cannot redefine the local tangent directions for the following types of surfaces: • Surfaces in a general contact domain • Analytical rigid surfaces • Two-dimensional surfaces You define the local tangent directions by associating an orientation definition with a contact pair surface. You can assign an orientation only to one surface of a contact pair. The surface on which an orientation can be defined is the same surface on which the default orientation would be calculated . For example, an orientation can be defined only on the slave surface in deformable versus deformable finite-sliding contact. If a second orientation is also given, an error message is issued. Therefore, it is not possible to redefine the local tangent directions for finite-sliding contact between a deformable slave surface and an analytical rigid surface. An orientation that is defined on a slave surface of a contact pair that is generated from three- dimensional truss-type elements or from a list of nodes without rotational degree of freedoms will not be rotated if the slave surface undergoes finite motion. In this case a warning message is issued during input processing. Input File Usage: *CONTACT PAIR, INTERACTION=interaction_property_name slave surface name, master surface name, orientation for slave surface slave surface name, master surface name, , orientation for master surface Abaqus/CAE Usage: You cannot define alternative local tangent directions for contact pairs in Abaqus/CAE. Evolution of the local tangent directions For geometrically nonlinear analyses the local tangent directions rotate with the surface on which these directions were initially calculated or redefined using an orientation definition as described above with the exception that the local tangent direction rotates with the master surface for the small-sliding, surface- to-surface formulation. These rotated local tangent directions are further rotated to ensure that the normal vector, computed using the cross product of the rotated local tangent directions, corresponds to the normal vector on the master surface when the slave node comes into contact. 37.1.2 CONTACT CONSTRAINT ENFORCEMENT METHODS IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • “Mechanical contact properties: overview,” Section 36.1.1 • “Contact pressure-overclosure relationships,” Section 36.1.2 • *SURFACE BEHAVIOR • *CONTACT CONTROLS • “Defining general contact,” Section 15.13.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a contact interaction property,” Section 15.14.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Contact constraint enforcement methods in Abaqus/Standard: • are specified as part of the surface interaction definition; • determine how contact constraints imposed by a physical pressure-overclosure relationship are resolved numerically in an analysis; • can either strictly enforce or approximate the physical pressure-overclosure relationships; • can be modified to resolve convergence difficulties due to overconstraints; and • sometimes utilize Lagrange multiplier degrees of freedom. The available constraint enforcement methods for normal contact in Abaqus/Standard are discussed in detail in this section. The frictional constraint enforcement methods in Abaqus/Standard are assigned independently of those for the normal contact constraints and are discussed in “Frictional behavior,” Section 36.1.5. The use of Lagrange multipliers in contact calculations is also covered in this section. Available constraint enforcement methods in Abaqus/Standard There are three contact constraint enforcement methods available in Abaqus/Standard: • The direct method attempts to strictly enforce a given pressure-overclosure behavior per constraint, without approximation or use of augmentation iterations. • The penalty method is a stiff approximation of hard contact. • The augmented Lagrange method uses the same kind of stiff approximation as the penalty method, but also uses augmentation iterations to improve the accuracy of the approximation. The default constraint enforcement method depends on interaction characteristics, as follows: • The penalty method is used by default for finite-sliding, surface-to-surface contact (including general contact) if a “hard” pressure-overclosure relationship is in effect. • The augmented Lagrange method is used by default for three-dimensional self-contact with node- to-surface discretization if a “hard” pressure-overclosure relationship is in effect. • The direct method is the default in all other cases. You should consider the following factors when choosing the contact enforcement method: • The direct method must be used for contact pairs with a “softened” pressure-overclosure relationship . • The direct method strictly enforces the specified pressure-overclosure behavior consistent with the constraint formulation • The penalty or augmented Lagrange constraint enforcement methods sometimes provide more efficient solutions (generally due to reduced calculation costs per iteration and a lower number of overall iterations per analysis) at some (typically small) sacrifice in solution accuracy. See the discussions of the penalty and augmented Lagrange methods below. • Overconstraints due to overlapping contact definitions or the combination of contact and other constraint types should be avoided for directly enforced hard contact. Direct method The direct method strictly enforces a given pressure-overclosure behavior for each constraint, without approximation or use of augmentation iterations. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *SURFACE INTERACTION, NAME=interaction_property_name *SURFACE BEHAVIOR, DIRECT Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Direct (Standard) Direct method for hard pressure-overclosure behavior The direct method can be used to strictly enforce a “hard” pressure-overclosure relationship. Lagrange multipliers are always used in this case. Direct method for softened pressure-overclosure relationships The direct method is the only method that can be used to enforce “softened” pressure-overclosure relationships. The direct method can be used to model softened contact behavior regardless of the type of contact formulation; however, modeling stiff interface behavior with a contact formulation that is prone to overconstraints can be difficult. Lagrange multipliers are used if the slope of the pressure-overclosure curve exceeds 1000 times the underlying element stiffness (as computed by Abaqus/Standard); otherwise, the constraints are enforced without Lagrange multipliers. The usage of Lagrange multipliers, thus, depends on the contact pressure. Softened pressure-overclosure relationships are discussed in more detail in “Contact pressure-overclosure relationships,” Section 36.1.2. Limitations of the direct method Because of its strict interpretation of contact constraints, hard contact simulations utilizing the direct enforcement method are susceptible to overconstraint issues. As a result, directly enforced hard contact is not available for contact pairs defined using three-dimensional self-contact with node-to-surface discretization. In this instance you can use an alternate enforcement method or the direct method with a softened pressure-overclosure relationship. You may experience similar overconstraint problems with symmetric master-slave contact pairs . Although directly enforced hard contact is the default for these contact pairs, it is recommended that you use an alternate enforcement method or a softened contact relationship. Certain second-order element faces do not perform well in directly enforced hard contact relationships. See “Three-dimensional surfaces with second-order faces and a node-to-surface formulation” in “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 38.1.2, for details on this issue. Penalty method The penalty method approximates hard pressure-overclosure behavior. With this method the contact force is proportional to the penetration distance, so some degree of penetration will occur. Advantages of the penalty method include: • Numerical softening associated with the penalty method can mitigate overconstraint issues and reduce the number of iterations required in an analysis. • The penalty method can be implemented such that no Lagrange multipliers are used, which allows for improved solver efficiency. Choosing a penalty method Abaqus/Standard offers linear and nonlinear variations of the penalty method. With the linear penalty method the so-called penalty stiffness is constant, so the pressure-overclosure relationship is linear. With the nonlinear penalty method the penalty stiffness increases linearly between regions of constant low initial stiffness and constant high final stiffness, resulting in a nonlinear pressure-overclosure relationship. The default penalty method is linear. A comparison of the linear and nonlinear pressure-overclosure relationships with the default settings is shown in Figure 37.1.2–1. Contact pressure K i=0.1K lin C0=0 K f=10K lin Nonlinear Linear Klin Overclosure Figure 37.1.2–1 Comparison of linear and nonlinear pressure-overclosure relationships with default settings. Linear penalty method When the linear penalty method is used, Abaqus/Standard will, by default, set the penalty stiffness to 10 times a representative underlying element stiffness. You can scale or reassign the penalty stiffness, as discussed in “Modifying a linear penalty stiffness” below. Contact penetrations resulting from the default penalty stiffness will not significantly affect the results in most cases; however, these penetrations can sometimes contribute to some degree of stress inaccuracy (for example, with displacement-controlled loading and a coarse mesh). The linear penalty method is used by default for the finite-sliding, surface- to-surface contact formulation. Input File Usage: Abaqus/CAE Usage: Nonlinear penalty method Use both of the following options to specify the linear penalty method: *SURFACE INTERACTION, NAME=interaction_property_name *SURFACE BEHAVIOR, PENALTY=LINEAR Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Penalty (Standard), Behavior: Linear With the nonlinear penalty method, the pressure-overclosure curve has four distinct regions shown in Figure 37.1.2–2. • Inactive contact regime: The contact pressure remains zero for clearances greater than default setting of is zero. . The • Constant initial penalty stiffness regime: The contact pressure varies linearly, with a slope equal to . The default initial penalty stiffness, is 1% of a , is equal to the representative underlying element stiffness. The default value of for penetrations (overclosures) in the range to characteristic length computed by Abaqus/Standard to represent a typical facet size. Contact pressure Final stiffness Kf Initial stiffness Ki Clearance C 0 Overclosure Penalty stiffness Kf Ki Overclosure Clearance C0 Figure 37.1.2–2 Nonlinear penalty pressure-overclosure relationship. • Stiffening regime: The contact pressure varies quadratically for penetrations in the range while the penalty stiffness increases linearly from to to , . The default final penalty stiffness, is , is equal to 100 times the representative underlying element stiffness. The default value of 3% of the same characteristic length used to compute (discussed above). • Constant final penalty stiffness regime: The contact pressure varies linearly, with a slope equal to for penetrations greater than . The low initial penalty stiffness typically results in better convergence of the Newton iterations and better robustness, while the higher final stiffness keeps the overclosure at an acceptable level as the contact pressure builds up. Input File Usage: Abaqus/CAE Usage: Use both of the following options to specify the nonlinear penalty method: *SURFACE INTERACTION, NAME=interaction_property_name *SURFACE BEHAVIOR, PENALTY=NONLINEAR Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Penalty (Standard), Behavior: Nonlinear Modifying the penalty stiffness If you are interested in investigating the effects of modifying the penalty stiffness, it is generally recommended that you consider order-of-magnitude changes. Increasing the penalty stiffness above the threshold value discussed above will, by default, introduce Lagrange multipliers. Modifying a linear penalty stiffness As part of the surface behavior definition, you can specify the linear penalty stiffness, shift the pressure- overclosure relationship by specifying the clearance at which the contact pressure is zero, or scale the default or specified penalty stiffness by a factor. Input File Usage: To modify the linear penalty behavior in the surface behavior definition: *SURFACE BEHAVIOR, PENALTY=LINEAR penalty stiffness, clearance at zero pressure, factor Abaqus/CAE Usage: To modify the linear penalty behavior in the surface behavior definition: Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Penalty (Standard), Behavior: Linear, Stiffness value: Specify: penalty stiffness, Stiffness scale factor: factor, Clearance at which contact pressure is zero: clearance at zero pressure Modifying a nonlinear penalty stiffness As part of the surface behavior definition, you can specify the final nonlinear penalty stiffness, shift the pressure-overclosure relationship by specifying the clearance at which the contact pressure is zero, or scale the default or specified penalty stiffness by a factor. In addition, you can control directly the ratio of the initial to the final penalty stiffness, the scale factor, and the ratio that determines and . Input File Usage: To modify the nonlinear penalty behavior in the surface behavior definition: *SURFACE BEHAVIOR, PENALTY=NONLINEAR final penalty stiffness, clearance at zero pressure, factor, upper quadratic limit scale factor, ratio of initial penalty stiffness over final penalty stiffness, lower quadratic limit ratio Abaqus/CAE Usage: To modify the nonlinear penalty behavior in the surface behavior definition: Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Penalty (Standard), Behavior: Nonlinear, Maximum stiffness value: Specify: final penalty stiffness, Stiffness scale factor: factor, Initial/Final stiffness ratio: ratio of initial penalty stiffness over final penalty stiffness, Upper quadratic limit scale factor: upper quadratic limit scale factor, Lower quadratic limit ratio: lower quadratic limit ratio, Clearance at which contact pressure is zero: clearance at zero pressure Scaling the penalty stiffness on a step-by-step basis You can also scale the penalty stiffness on a step-by-step basis, which will act as an additional multiplier on any scale factor specified as part of the surface behavior definition. Input File Usage: Abaqus/CAE Usage: To scale the penalty stiffness on a step-by-step basis: *CONTACT CONTROLS, STIFFNESS SCALE FACTOR=factor To scale the penalty stiffness on a step-by-step basis: Interaction module: Abaqus/Standard contact controls editor: Augmented Lagrange: Stiffness scale factor: factor Limitations of the penalty method The penalty method cannot be used for debonded surfaces. If the penalty method is specified, Lagrange multipliers are always used during analysis steps with the following procedures: • Design sensitivity analysis • Direct steady-state dynamic analysis • Quasi-Newton method If surface elements have been used to define a contact surface on the exterior of a substructure , Abaqus/Standard interprets the underlying element stiffness to be zero. This can lead to difficulty in determining the default penalty stiffness and may cause numerical problems during the analysis. Augmented Lagrange method The linear penalty method can be used within an augmentation iteration scheme that drives down the penetration distance. This so-called augmented Lagrange method applies only to hard pressure-overclosure relationships. The following describes the sequence that occurs in each increment with this approach: 1. Abaqus/Standard finds a converged solution with the penalty method. 2. If a slave node penetrates the master surface by more than a specified penetration tolerance, the contact pressure is “augmented” and another series of iterations is executed until convergence is once again achieved. 3. Abaqus/Standard continues to augment the contact pressure and find the corresponding converged solution until the actual penetration is less than the penetration tolerance. The augmented Lagrange method may require additional iterations in some cases; however, this approach can make the resolution of contact conditions easier and avoid problems with overconstraints, while keeping penetrations small. The augmented Lagrange method is used by default for three-dimensional self-contact using node-to-surface discretization. The default penetration tolerance is one-tenth of a percent of the characteristic interface length except in the following cases: • if you specify a penalty stiffness scaling factor, , of less than 1.0 (using the interface discussed below), Abaqus/Standard will automatically scale the default penetration tolerance by a factor of (which will be greater than or equal to 1.0); • the default penetration tolerance for finite-sliding, surface-to-surface contact is five percent of the characteristic interface length, subject to the scaling discussed in the previous bullet point. The default penalty stiffness for the augmented Lagrange method is 1000 times the representative underlying element stiffness. Lagrange multipliers are used for the augmented Lagrange method if the penalty stiffness exceeds 1000 times the representative underlying element stiffness computed by Abaqus/Standard; otherwise, no Lagrange multipliers are used. Therefore, Lagrange multipliers are not used for the augmented Lagrange method with the default penalty stiffness. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *SURFACE INTERACTION, NAME=interaction_property_name *SURFACE BEHAVIOR, AUGMENTED LAGRANGE Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Augmented Lagrange (Standard) Modifying the penetration tolerance for the augmented Lagrange method You can modify the penetration tolerance for the augmented Lagrange method on a step-by-step basis by specifying an absolute or relative penetration tolerance. The relative penetration tolerance is specified with respect to a characteristic length computed by Abaqus/Standard. The default penetration tolerance was discussed above. The default penetration tolerance is increased automatically if you set the penalty stiffness scale factor to a value less than 1.0 (also discussed above); however, Abaqus/Standard will not adjust any directly specified penetration tolerance. Choosing a very small penetration tolerance may result in an excessive number of augmentation iterations. Input File Usage: Abaqus/CAE Usage: To specify an absolute penetration tolerance: *CONTACT CONTROLS, ABSOLUTE PENETRATION TOLERANCE=tolerance To specify a relative penetration tolerance: *CONTACT CONTROLS, RELATIVE PENETRATION TOLERANCE=tolerance Interaction module: Abaqus/Standard contact controls editor: Augmented Lagrange: Penetration tolerance: Absolute: tolerance or Relative: tolerance Modifying the penalty stiffness for the augmented Lagrange method As with the penalty method, you can specify the penalty stiffness, shift the pressure-overclosure relationship by specifying the clearance at which the contact pressure is zero, or scale the default or specified penalty stiffness by a factor as part of the surface behavior definition. You can also scale the penalty stiffness on a step-by-step basis, which will act as an additional multiplier on any scale factor specified as part of the surface behavior definition. Choosing a very low penalty stiffness may result in an excessive number of augmentation iterations. Input File Usage: To modify the penalty behavior in the surface behavior definition: *SURFACE BEHAVIOR, AUGMENTED LAGRANGE penalty stiffness, clearance at zero pressure, factor To scale the penalty stiffness on a step-by-step basis: Abaqus/CAE Usage: *CONTACT CONTROLS, STIFFNESS SCALE FACTOR=factor To modify the penalty behavior in the surface behavior definition: Interaction module: contact property editor: Mechanical→Normal Behavior: Constraint enforcement method: Augmented Lagrange (Standard), Stiffness value: Specify: penalty stiffness, Stiffness scale factor: factor, Clearance at which contact pressure is zero: clearance at zero pressure To scale the penalty stiffness on a step-by-step basis: Interaction module: Abaqus/Standard contact controls editor: Augmented Lagrange: Stiffness scale factor: factor Modifying the number of allowed augmentations for the augmented Lagrange method You can define the number of allowed augmentations for the augmented Lagrange method. Input File Usage: *CONTROLS, PARAMETERS=TIME INCREMENTATION , , , , , , , , , , , , Abaqus/CAE Usage: Defining the number of allowed augmentations for the augmented Lagrange method is not supported in Abaqus/CAE. Limitations of the augmented Lagrange method The augmented Lagrange method cannot be used for debonded surfaces. If the augmented Lagrange method is specified, Lagrange multipliers are always used during analysis steps with the following procedures: • Design sensitivity analysis • Direct steady-state dynamic analysis • Quasi-Newton method If surface elements have been used to define a contact surface on the exterior of a substructure , Abaqus/Standard interprets the underlying element stiffness to be zero. This can lead to difficulty in determining the default penalty stiffness and may cause numerical problems during the analysis. Use of Lagrange multiplier degrees of freedom by the various methods Using Lagrange multipliers to enforce contact constraints can add significantly to the solution cost, but they also protect against numerical errors related to ill-conditioning that can occur if a high contact stiffness is in effect. Abaqus/Standard automatically chooses whether the constraint method makes use of Lagrange multipliers, based on a comparison of the contact stiffness to the underlying element stiffness. Table 37.1.2–1 summarizes the use of Lagrange multipliers. Lagrange multipliers are not used for the default contact stiffnesses associated with the penalty and augmented Lagrange approximations of hard contact. Any Lagrange multipliers associated with contact are present only for active contact constraints, so the number of equations may change as the contact status changes. Table 37.1.2–1 Use of Lagrange multipliers in constraint enforcement methods. Constraint Method Direct, hard contact Direct, exponential softened contact Direct, linear softened contact Direct, tabular softened contact Penalty, hard contact Augmented Lagrange, hard contact If If If If If Use Lagrange Multipliers Yes Always No1 Never If If If If If = slope of pressure-overclosure relationship = penalty stiffness = underlying element stiffness 1Lagrange multipliers are always used, regardless of the constraint enforcement method or stiffness, in the following cases: design sensitivity analyses, direct steady-state dynamics analyses, analyses using the quasi-Newton method. 37.1.3 SMOOTHING CONTACT SURFACES IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • *CONTACT • *CONTACT PAIR • *SURFACE PROPERTY ASSIGNMENT • *SURFACE SMOOTHING Overview With the finite element method, curved geometric surfaces are naturally approximated as a faceted group of connected element faces. The use of a faceted surface geometry rather than the true surface geometry can significantly contribute to contact stress inaccuracy in contact interactions, especially when the magnitude of the differences between the faceted and true surface is not small with respect to the deformation of the components in contact. Contact stress output is of primary importance in many Abaqus/Standard applications; for example, the distribution of contact pressures can be used to identify wear patterns and peak pressure values to determine relative lives of machine parts. Furthermore, discontinuities in the surface normal direction at surface facet boundaries can contribute to convergence difficulties. Abaqus/Standard offers techniques for overcoming the accuracy and convergence difficulties associated with faceted surfaces in contact interactions. These techniques allow a discretized surface with discontinuous surface normals to more closely approximate the behavior of a smooth surface with continuous normals during an analysis. The smoothing technique used in node-to-surface contact is different from the smoothing technique used in surface-to-surface and general contact: • Node-to-surface contact smoothing is applied by default and affects the entire master surface. • Surface-to-surface contact smoothing is not applied by default, but it can be applied to any surface regions whose geometry is roughly axisymmetric. Surface-to-surface contact typically gives the most accurate results. Smoothing master surfaces for node-to-surface contact pairs Surface smoothing in node-to-surface contact pairs improves numerical stability and sometimes improves solution accuracy. Slave nodes traveling along a master surface tend to “snag” on sharp corners, resulting in convergence difficulties. Because of this behavior, Abaqus/Standard automatically smooths the master surface in node-to-surface contact pairs. This smoothing technique recalculates the master surface normals along facet edges and, depending on the type of surface, may affect the surface geometry. The details of smoothing for node-to-surface contact formulations are discussed in “Smoothing master surfaces for the finite-sliding, node-to-surface formulation” in “Contact formulations in Abaqus/Standard,” Section 37.1.1, and “Using the small-sliding tracking approach” in “Contact formulations in Abaqus/Standard,” Section 37.1.1. Smoothing contact surfaces for surface-to-surface contact Smooth surfaces are not usually necessary in surface-to-surface contact to ensure analysis convergence; therefore, no smoothing is applied to these surfaces by default. However, an optional smoothing technique is available for improving the contact stress and pressure accuracy for axisymmetric (or nearly axisymmetric) surfaces in surface-to-surface contact interactions. Surface-to-surface contact smoothing can be applied to specific surface regions. These regions must be roughly axisymmetric (all points on the surface are nearly equidistant from a single axis) or roughly spherical (all points on the surface are nearly equidistant from a single point). The pin insertion model in Figure 37.1.3–1 could benefit from surface-to-surface contact smoothing: the body of the pin and the hole are axisymmetric surfaces, and the head of the pin is a spherical surface. Surface-to-surface contact smoothing would also be effective if the surfaces were not perfectly axisymmetric or spherical; for example, if the pin body were slightly elliptical. Figure 37.1.3–1 Surface-to-surface contact model with surface smoothing. Applying contact smoothing to surface-to-surface contact pairs Surface-to-surface contact smoothing for contact pairs is enabled by creating a surface smoothing definition. A contact pair definition references this smoothing definition to apply geometric corrections in the contact formulation (the physical geometry of the model is not altered). The surface smoothing definition lists all of the faceted regions in the contact pair surfaces that must be smoothed, as well as the geometry correction method that should be applied to each region. Three geometry correction methods can be employed: • The circumferential smoothing method is applicable to surfaces approximating a portion of a circle in two dimensions or a portion of a surface of revolution in three dimensions. • The spherical smoothing method is applicable to surfaces approximating a portion of a sphere in three dimensions. • The toroidal smoothing method is applicable to surfaces approximating a portion of a torus in three dimensions (i.e., a circular arc revolved about an axis). Each surface-to-surface contact pair refers to a single smoothing definition; therefore, a smoothing definition must list all of the smoothed regions and applicable geometry correction methods for the contact pair. Geometry corrections can be applied to master surfaces and to slave surfaces; you can also apply corrections to selected regions of each surface. A surface smoothing definition can include multiple regions and different geometric correction methods for each region. For each region, you must specify the appropriate geometry correction method and either the approximate axis of revolution (for circumferential or toroidal smoothing) or the approximate spherical center (for spherical smoothing). For toroidal smoothing, you must also specify the distance of the center of the circular arc from the axis of revolution, and the line joining point (Xa , Ya , Za ) and the center of the circular arc should be perpendicular to the axis of revolution. Input File Usage: Use both of smoothing: the following options to apply surface-to-surface contact *CONTACT PAIR, GEOMETRIC CORRECTION=smoothing_name *SURFACE SMOOTHING, NAME=smoothing_name data lines to define smoothing regions Use the following data line to apply circumferential smoothing to surface regions with an axis of symmetry passing through points (Xa , Ya , Za ) and (Xb , Yb, Zb): slave_region, master_region, CIRCUMFERENTIAL, Xa , Ya, Za , Xb , Yb, Zb Use the following data line to apply spherical smoothing to surface regions with a spherical center at point (Xa , Ya , Za ): slave_region, master_region, SPHERICAL, Xa, Ya , Za Use the following data line to apply toroidal smoothing to surface regions with an axis of symmetry passing through points (Xa , Ya , Za ) and (Xb , Yb, Zb) with the center of the revolved circular arc at a distance R from the axis of symmetry: slave_region, master_region, TOROIDAL, Xa , Ya, Za , Xb , Yb, Zb , R Repeat the data lines as many times as necessary to define the appropriate geometry corrections for all surfaces in the contact pair. Abaqus/CAE Usage: Abaqus/CAE can automatically identify any circumferential or spherical surfaces in a contact interaction that will benefit from contact smoothing and apply the necessary geometry correction methods. Interaction module: contact interaction editor: Surface Smoothing: Automatically smooth geometry surfaces Surface-to-surface contact smoothing cannot be applied to surfaces on orphan mesh models. Toroidal surface smoothing cannot be defined in Abaqus/CAE. Example To improve contact pressure accuracy for the model in Figure 37.1.3–1, contact smoothing can be applied to both the master and slave surfaces. Two different geometric correction methods are required for the pin (the slave surface), so additional surfaces are defined corresponding to regions of the slave surface. Spherical smoothing is defined for the tip of the pin. Since the body of the pin and the hole share an axis of revolution, a single circumferential smoothing technique is applied to both of these surfaces. This surface smoothing definition applies even if the cross-sectional shapes of the pin and hole deviate from perfect circles. *CONTACT PAIR, TYPE=SURFACE TO SURFACE, INTERACTION=FRICTION1, GEOMETRIC CORRECTION=SMOOTH1 PIN, HOLE *SURFACE INTERACTION, NAME=FRICTION1 *SURFACE SMOOTHING, NAME=SMOOTH1 PIN_TIP, , SPHERICAL, Xb , Yb , Zb PIN_BODY, HOLE, CIRCUMFERENTIAL, Xa , Ya , Za , Xb, Yb , Zb Applying contact smoothing to general contact surfaces Contact smoothing can be specified for surfaces in a general contact domain using a surface property assignment. A single surface property assignment specifies all of the surfaces to be smoothed, as well as the appropriate geometry correction method for each surface. General contact uses the same geometry correction methods as contact pairs: • The circumferential smoothing method is applicable to surfaces approximating a portion of a circle in two dimensions or a portion of a surface of revolution in three dimensions. • The spherical smoothing method is applicable to surfaces approximating a portion of a sphere in three dimensions. • The toroidal smoothing method is applicable to surfaces approximating a portion of a torus in three dimensions (i.e., a circular arc revolved about an axis). For each surface, you must specify the appropriate geometry correction method and either the approximate axis of revolution (for circumferential or toroidal smoothing) or the approximate spherical center (for spherical smoothing). For toroidal smoothing, you must also specify the distance of the center of the circular arc from the axis of revolution, and the line joining point (Xa , Ya , Za ) and the center of the circular arc should be perpendicular to the axis of revolution. Input File Usage: *SURFACE PROPERTY ASSIGNMENT, PROPERTY=GEOMETRIC CORRECTION data lines to define smoothing regions Use the following data line to apply circumferential smoothing to a surface with an axis of symmetry passing through points (Xa , Ya , Za ) and (Xb , Yb, Zb ): surface, CIRCUMFERENTIAL, Xa , Ya, Za , Xb , Yb , Zb Use the following data line to apply spherical smoothing to a surface with a spherical center at point (Xa , Ya , Za ): surface, SPHERICAL, Xa, Ya , Za Use the following data line to apply toroidal smoothing to a surface with an axis of symmetry passing through points (Xa , Ya , Za ) and (Xb , Yb, Zb ) with the center of the revolved circular arc at a distance R from the axis of symmetry: surface, TOROIDAL, Xa , Ya, Za , Xb , Yb , Zb, R Repeat the data lines as many times as necessary to define the appropriate geometry corrections for all surfaces in the contact domain. Contact surface smoothing can be applied only to native geometry models in Abaqus/CAE. By default, Abaqus/CAE automatically detects all circumferential and spherical surfaces in the general contact domain that can be smoothed and applies the appropriate smoothing. Use the following option to prevent automatic surface smoothing of a model: Interaction module: Create Interaction: General contact (Standard): Surface Properties: Surface smoothing assignments: Edit: toggle off Automatically assign smoothing for geometric faces Use the following option to manually apply smoothing to a surface: Interaction module: Create Interaction: General contact (Standard): Surface Properties: Surface smoothing assignments: Edit: Select surface, click the arrows to transfer surface to list of smoothing assignments. In the Smoothing Option column, select REVOLUTION to apply circumferential smoothing, select SPHERICAL to apply spherical smoothing, or select NONE to prevent smoothing of the surface. Toroidal surface smoothing cannot be defined in Abaqus/CAE. 37.1.3–5 Considerations for using surface-to-surface contact smoothing The surface-to-surface contact smoothing technique assumes that the initial locations of surface nodes lie on the true initial surface geometry, with the exception of midside nodes of higher-order elements. This smoothing technique remains effective even if the midside nodes of higher-order elements do not lie on the true initial geometry (models meshed using Abaqus/CAE always have midside nodes placed on the true initial geometry, but this may not be the case with other meshing preprocessors). The effects of surface-to-surface contact smoothing tend to be most significant for analyses involving small deformation and coarse mesh discretization with first-order elements in the contact region; however, significant improvements to contact stress solutions are common even when the mesh is quite refined or higher-order elements are used. For analyses with large deformation this smoothing technique typically has an insignificant effect on solutions. However, in some cases the smoothing can degrade the solution accuracy after large deformation; therefore, it is not recommended to use surface-to-surface contact smoothing for large-deformation analyses. The effectiveness of surface-to-surface contact smoothing does not degrade upon relative motion between contact surfaces; for example, the smoothing technique works well for cases involving large sliding but small deformation. Effects of contact surface smoothing The impact of contact surface smoothing can be demonstrated by a simple model of an interference fit between concentric cylinders modeled with first-order elements of different sizes, as shown in Figure 37.1.3–2. Discrepancies between the true surface geometry and the faceted surface geometry result in noise in the contact pressure solution. If the interference distance and resulting deformation distance is small with respect to the geometry discrepancy, this noise can have a significant effect on the accuracy of the solution. Although surface-to-surface contact typically handles these discrepancies better than node-to-surface contact, it is not unusual for the maximum deviation from the analytical pressure solution to be upward of 100%. The effects of the noise become less apparent for larger deformations, but they are never completely eliminated. Figure 37.1.3–2 Initial mesh geometry for interference fit model. Modeling the interference fit with a surface-to-surface contact pair and using circumferential contact smoothing consistently yields low-noise pressure results that are within 3% of the analytical solution, regardless of the size of the interference distance. The effect is drastically noticeable for small-deformation analyses, but improvements can be observed even for larger deformations. For a node-to-surface contact pair, increasing the smoothing fraction to the maximum value of 0.5 marginally reduces the noise in the pressure solution in a two-dimensional model. Increasing the smoothing factor in a three-dimensional model has little effect on accuracy, since physical surfaces are not smoothed for three-dimensional node-to-surface smoothing; see “Smoothing master surfaces for the finite-sliding, node-to-surface formulation” in “Contact formulations in Abaqus/Standard,” Section 37.1.1, for more information. 37.2 Contact formulations and numerical methods in Abaqus/Explicit • “Contact formulation for general contact in Abaqus/Explicit,” Section 37.2.1 • “Contact formulations for contact pairs in Abaqus/Explicit,” Section 37.2.2 • “Contact constraint enforcement methods in Abaqus/Explicit,” Section 37.2.3 37.2.1 CONTACT FORMULATION FOR GENERAL CONTACT IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1 • *CONTACT • *CONTACT FORMULATION • “Specifying master-slave assignments for general contact,” Section 15.13.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The contact formulation used with the general contact algorithm in Abaqus/Explicit: • includes the contact surface weighting, surface polarity, and the sliding formulation; and • can be applied selectively to particular regions within a general contact domain. The general contact formulation uses a penalty method to enforce contact constraints between surfaces; the constraint enforcement method is discussed in “Contact constraint enforcement methods in Abaqus/Explicit,” Section 37.2.3. Specifying the contact formulation Currently you can specify only the contact surface weighting and polarity for the general contact algorithm. The contact formulation propagates through all analysis steps in which the general contact interaction is active. The surface names used to specify the regions where a nondefault contact formulation should be assigned do not have to correspond to the surface names used to specify the general contact domain. In many cases the contact interaction will be defined for a large domain, while a nondefault contact formulation will be assigned to a subset of this domain. Any contact formulation assignments for regions that fall outside the general contact domain will be ignored. The last assignment will take precedence if the specified regions overlap. Input File Usage: *CONTACT FORMULATION This option must be used in conjunction with the *CONTACT option. It should appear at most once per step for each value of the TYPE parameter; the data line can be repeated as often as necessary to assign contact formulations to different regions. Abaqus/CAE Usage: Interaction module: Create Interaction: General contact (Explicit): Contact Formulation Contact surface weighting Generally, contact constraints in a finite element model are applied in a discrete manner, meaning that for hard contact a node on one surface is constrained to not penetrate the other surface. In pure master-slave contact the node with the constraint is part of the slave surface and the surface with which it interacts is called the master surface. For balanced master-slave contact Abaqus/Explicit calculates the contact constraints twice for each set of surfaces in contact, in the form of penalty forces: once with the first surface acting as the master surface and once with the second surface acting as the master surface. The weighted average of the two corrections (or forces) is applied to the contact interaction. Balanced master-slave contact minimizes the penetration of the contacting bodies and, thus, provides better enforcement of contact constraints and more accurate results in most cases. In pure master-slave contact the nodes on the master surface can, in principle, penetrate the slave surface unhindered . slave nodes cannot penetrate master segments master surface (segments) penetration slave surface (nodes) gap master node can penetrate slave segment Figure 37.2.1–1 Master surface penetrations into the slave surface in pure master-slave contact due to coarse discretization. The general contact algorithm in Abaqus/Explicit uses balanced master-slave weighting whenever possible; pure master-slave weighting is used for contact interactions involving node-based surfaces, which can act only as pure slave surfaces and for contact interactions involving analytical rigid surfaces, which can act only as pure master surfaces. Surface-based cohesive behavior also always uses a pure master-slave algorithm. However, you can choose to specify a pure master-slave weighting for other interactions as well. There is no master-slave relationship for edge-to-edge contact; both contacting edges are given equal weighting. Specifying pure master-slave weighting for node-to-face contact You can specify that a general contact interaction should use pure master-slave weighting for node-to- face contact. This specification has no effect on edge-to-edge contact and cannot be used to make a node-based surface act as a master surface. When two originally flat surfaces contact one another, a more uniform penetration distance distribution (and consequently pressure distribution) may result with pure master-slave weighting where the more refined surface acts as the slave surface as compared to balanced master-slave weighting. This can be particularly evident if the mesh densities of the contacting surfaces differ significantly—with balanced weighting the contact penetrations will be smaller near the nodes of the coarsely meshed surface. Abaqus/Explicit will automatically generate contact exclusions for the master-slave orientation opposite to that specified; therefore, node-to-face self-contact will be excluded for any regions of the two surfaces that overlap. For example, specifying that the general contact interaction between surf_A and surf_B should use pure master-slave weighting with surf_A considered to be the slave surface would result in exclusions being generated internally for faces of surf_A contacting nodes of surf_B; node-to-face self-contact would be excluded for the region of overlap between surf_A and surf_B. A warning message will be issued if the second surface name is omitted or is the same as the first surface name since this input would result in the exclusion of node–face self-contact for the surface. Input File Usage: Use the following option to indicate that the first surface should be considered the slave surface (default): *CONTACT FORMULATION, TYPE=PURE MASTER-SLAVE surf_1, surf_2, SLAVE Use the following option to indicate that the first surface should be considered the master surface: *CONTACT FORMULATION, TYPE=PURE MASTER-SLAVE surf_1, surf_2, MASTER If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. The second surface name must be specified. Interaction module: Create Interaction: General contact (Explicit): Contact Formulation: Pure master-slave assignments: Edit: select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of master-slave assignments. In the First Surface Type column, enter SLAVE to indicate that the first surface should be considered the slave surface, and enter MASTER to indicate that the first surface should be considered the master surface. Abaqus/CAE Usage: Contact surface polarity By default, general contact considers both sides of all double-sided elements in surfaces specified to be included for contact purposes (side labels of double-sided elements are ignored). This default can be overridden for node-to-face and Eulerian-Lagrangian contact and in some cases results in more accurate enforcement of contact. Surface polarity is not considered for edge-to-edge contact, including edges activated on faces of solid elements. Specifying surface polarity for node-to-face and Eulerian-Lagrangian contact Changing the polarity of double-sided elements forces the contact algorithm to treat them as if they were solid elements. More accuracy may be gained by converting double-sided elements to single-sided if there is a chance that slave nodes may be “caught” behind the surface in node-to-face contact or if material contained on one side of a double-sided surface leaks to the other side in Eulerian-Lagrangian contact. Improvements in performance and memory use may also be observed with Eulerian-Lagrangian contact if double-sided Lagrangian surfaces are converted to single-sided for contact with all Eulerian material surfaces. Input File Usage: Use the following option to indicate that the sides of the (double-sided) elements specified in the second surface’s definition should be considered for contact with the first surface: *CONTACT FORMULATION, TYPE=POLARITY surf_1, surf_2 Use the following option to indicate that the SPOS side of the (double-sided) elements in the second surface should be considered for contact with the first surface: *CONTACT FORMULATION, TYPE=POLARITY surf_1, surf_2, SPOS Use the following option to indicate that the SNEG side of the (double-sided) elements in the second surface should be considered for contact with the first surface: *CONTACT FORMULATION, TYPE=POLARITY surf_1, surf_2, SNEG Use the following option to indicate that both sides of the (double-sided) elements in the second surface should be considered for contact with the first surface: *CONTACT FORMULATION, TYPE=POLARITY surf_1, surf_2, TWO SIDED If the first surface name is omitted, a default surface that encompasses the entire general contact domain is assumed. The second surface name must be specified. Sliding formulation Currently only the finite-sliding formulation is available for general contact in Abaqus/Explicit. This formulation allows for arbitrary separation, sliding, and rotation of the surfaces in contact. For cases in which small-sliding or infinitesimal-sliding assumptions would be preferred, the contact pair algorithm should be used . Abaqus/Explicit is designed to simulate highly nonlinear events or processes. Because it is possible for a node on one surface to contact any of the facets on the opposite surface, Abaqus/Explicit must use sophisticated search algorithms for tracking the motions of the surfaces. The finite-sliding contact search algorithm is designed to be robust, yet computationally efficient. This algorithm assumes that the incremental relative tangential motion between surfaces does not significantly exceed the dimensions of the master surface facets, but there is no limit to the overall relative motion between surfaces. It is rare for the incremental motion to exceed the facet size because of the small time increment used in explicit dynamic analyses. In cases involving relative surface velocities that exceed material wave speeds it may be necessary to reduce the time increment. The contact search algorithm uses a global search when a contact interaction is first introduced, and a hierarchical global/local search algorithm is used thereafter. No user control of the search algorithm is needed. 37.2.2 CONTACT FORMULATIONS FOR CONTACT PAIRS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Surfaces: overview,” Section 2.3.1 • “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1 • *CONTACT PAIR • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The contact formulation for the contact pair algorithm in Abaqus/Explicit includes: • the contact surface weighting (balanced or pure master-slave); and • the sliding formulation (finite, small, or infinitesimal). You can also specify the method that is used to enforce contact constraints in the contact pair; these methods are discussed in “Contact constraint enforcement methods in Abaqus/Explicit,” Section 37.2.3. Contact surface weighting Both the pure master-slave and the balanced master-slave contact algorithms are available in Abaqus/Explicit. By default, Abaqus/Explicit will decide which algorithm to use for any given contact pair based on the nature of the two surfaces forming the contact pair and whether kinematic or penalty enforcement of contact constraints is used. You can override the defaults in some cases. Default choices for the contact pair weighting Abaqus/Explicit uses the pure master-slave, kinematic contact algorithm, by default, in the following situations (the first surface in each situation listed is designated the master surface): • when a rigid surface contacts a deformable surface; • when an element-based surface contacts a node-based surface; or • when a surface based on continuum elements contacts a surface based on shell or membrane elements. By default, Abaqus/Explicit uses the balanced master-slave, kinematic contact algorithm in the following situations: • when a single surface contacts itself (referred to as self-contact or single-surface contact); or • when two deformable surfaces that are meshed with similar elements (i.e., either both surfaces have shells or membranes or both have continuum elements) contact each other. If the penalty contact algorithm is specified, Abaqus/Explicit uses pure master-slave weighting, by default, in the following situations (the first surface in each situation listed is designated the master surface): • when an analytical rigid surface contacts a deformable surface; or • when an analytical rigid surface or an element-based surface contacts a node-based surface. If the penalty contact algorithm is specified, Abaqus/Explicit chooses balanced master-slave weighting, by default, in the following situations: • when a single surface contacts itself (referred to as self-contact or single-surface contact); or • when two element-based surfaces contact each other. Balanced master-slave weighting means that the corrections produced by both sets of contact calculations are weighted equally. Modifying the default choices for the contact pair weighting When the kinematic contact method is chosen, you can override the default contact pair weighting only when two separate deformable element-based surfaces are contacting each other, which corresponds to the last situation in each list for kinematic contact given in the previous section. The following aspects should be considered when deciding whether or not to override the default choice. First, the balanced master-slave contact algorithm requires more computational time, but it is typically more accurate. Second, when the densities differ by orders of magnitude, the less dense body should be a pure slave surface. Contact-induced noise can occur if a surface on a much denser body is at all weighted as a slave surface. Finally, to avoid significant penetration for hard contact, the surface with the finer mesh should not be the master surface in the pure master-slave contact pair. When the penalty contact method is chosen, you can choose to specify a pure master-slave weighting to reduce computational time. When two originally flat surfaces contact one another, a more uniform penetration distance distribution (and consequently pressure distribution) may result with pure master- slave weighting as compared to balanced master-slave weighting. This can be particularly evident if the mesh densities of the contacting surfaces differ significantly—with balanced weighting the contact penetrations will be smaller near the nodes of the coarsely meshed surface. However, balanced master- slave weighting provides better enforcement of contact constraints in most cases. You define a weighting factor, f, to specify the master-slave weighting. Set f=1.0 to designate the first surface in the contact pair as the master surface and the second surface as the slave surface. Set f=0.0 to designate the first surface in the contact pair as the slave surface and the second surface as the master surface. Specifying any value of f between 0 and 1.0 invokes the balanced master-slave contact algorithm. When f=0.5, which is the default for balanced master-slave contact pairs, Abaqus/Explicit weights each set of corrections equally. In contrast, Abaqus/Standard uses a pure master-slave contact algorithm; the slave surface must always be given first, as in the f=0.0 case above. *CONTACT PAIR, WEIGHT=f Interaction module: interaction editor: Weighting factor Specify f Abaqus/CAE Usage: Input File Usage: Sliding formulation In Abaqus/Explicit there are three approaches to account for the relative motion of the two surfaces forming a contact pair: • finite sliding, which is the most general and allows any arbitrary motion of the surfaces; • small sliding, which assumes that although two bodies may undergo large motions, there will be relatively little sliding of one surface along the other; or • infinitesimal sliding and rotation, which assumes that both the relative motion of the surfaces and the absolute motion of the contacting bodies are small. The small-sliding and infinitesimal-sliding formulations cannot be used for contact pairs using the penalty contact algorithm or involving self-contact or analytical rigid surfaces. Using the finite-sliding formulation The finite-sliding formulation allows for arbitrary separation, sliding, and rotation of the surfaces. Abaqus/Explicit uses this formulation by default. Only the finite-sliding approach is available for self-contact or contact involving analytical rigid surfaces. Input File Usage: Abaqus/CAE Usage: *CONTACT PAIR Interaction module: interaction editor: Sliding formulation: Finite sliding Example The following input defines finite-sliding contact between the surfaces ASURF and BSURF, shown in Figure 37.2.2–1, with ASURF acting as the slave surface: *SURFACE,NAME=ASURF ESETA, *SURFACE,NAME=BSURF ESETB, *CONTACT PAIR,INTERACTION=PAIR1, WEIGHT=0.0 ASURF, BSURF *SURFACE INTERACTION,NAME=PAIR1 In the example shown in Figure 37.2.2–1 slave node 101 may come into contact anywhere along the master surface BSURF. While in contact, it is constrained to slide along BSURF, irrespective of the orientation and deformation of this surface. This behavior is possible because Abaqus/Explicit tracks the position of node 101 relative to the master surface BSURF as the bodies deform. Figure 37.2.2–2 shows the possible evolution of the contact between node 101 and its master surface BSURF. Node 101 is in contact with the element face with end nodes 201 and 202 at time . The load transfer at this time occurs between node 101 and nodes 201 and 202 only. Later on, at time , node 101 may find itself in contact with the element face with end nodes 501 and 502. Then the load transfer will occur between node 101 and nodes 501 and 502. ESETB ESETA 502 BSURF 201 501 202 101 102 103 ASURF Figure 37.2.2–1 Contacting bodies. BSURF 201 t = t 1 202 501 502 t = t 2 101 t = 0 Figure 37.2.2–2 Trajectory of node 101 in finite-sliding contact. Finite sliding in a geometrically linear analysis Finite-sliding simulations usually include nonlinear geometric effects because such simulations generally involve large deformations and large rotations. However, it is also possible to use the finite-sliding formulation in a geometrically linear analysis . The load transfer paths between the surfaces and the contact direction are updated in finite-sliding, geometrically linear analysis. This capability is useful for analyzing finite sliding between two stiff bodies that do not undergo large rotations. Using the small-sliding formulation For a large class of contact problems the general tracking of the finite-sliding formulation is unnecessary, even though geometric nonlinearity must be considered. Abaqus/Explicit provides a small-sliding contact formulation for such problems. This formulation assumes that the surfaces may undergo arbitrarily large rotations but that a slave node will interact with the same local area of the master surface throughout the analysis. Contact pairs that use the small-sliding formulation must be defined in the first step of the simulation, although they may remain active after the first step. A large-displacement formulation (the default) should be used for the step in which the small-sliding contact formulation should be used. In a small-sliding analysis every slave node interacts with its own local tangent plane on the master surface . The slave node is constrained not to penetrate this local tangent plane. Each local tangent plane, which is a line in two dimensions, is defined by an anchor point, , on the master surface and an orientation vector at the anchor point . 104 N(X0) N3 X0 103 slave surface 102 N2 local tangent plane master surface N4 Figure 37.2.2–3 Definition of the anchor point and local tangent plane for node 103. Having a local tangent plane for each slave node means that for the small-sliding formulation Abaqus/Explicit does not have to monitor slave nodes for possible contact along the entire master surface. Therefore, small-sliding contact is less expensive computationally than finite-sliding contact. The cost savings are most dramatic in three-dimensional contact problems. When the balanced master-slave contact algorithm is invoked with the small-sliding formulation, anchor points and tangent planes will be computed for both surfaces. Input File Usage: Use both of the following options: *STEP, NLGEOM=YES … *CONTACT PAIR, SMALL SLIDING For example, the following options define small-sliding contact between the two bodies shown in Figure 37.2.2–1: *STEP, NLGEOM=YES … *SURFACE, NAME=ASURF ESETA, *SURFACE, NAME=BSURF ESETB, *CONTACT PAIR, SMALL SLIDING, WEIGHT=0.0 ASURF, BSURF Abaqus/CAE Usage: Interaction module: interaction editor: Sliding formulation: Small sliding Step module: step editor: Nlgeom: On Anchor point and tangent plane definition The anchor point and the tangent plane orientation are chosen before the analysis starts using the initial configuration of the model. The anchor point and the tangent plane orientation remain fixed with respect to the master surface facet for all steps in which the contact pair is active. No contact constraints are enforced for slave nodes whose nearest point lies on the free perimeter of the master surface in the original configuration and that do not project onto any master surface facet. Abaqus/Explicit chooses the anchor point as the nearest point on the master surface. The orientation of the tangent plane is calculated by default from the normals at the master surface nodes, or you can specify it directly. • Master surface normals: The first step in defining the tangent plane orientation is to construct the unit normal vectors at each node of the master surface. Abaqus/Explicit forms these nodal normals by averaging the normals of the element faces making up the master surface; only the element faces in the surface definition will contribute to the nodal normals. The tangent plane orientation is then calculated from the master surface nodal normals and the element shape functions at the anchor point. Figure 37.2.2–3 shows the nodal unit normals for a master surface, the anchor point , and the local tangent plane associated with slave node 103. Abaqus/Explicit uses the closest point on the master surface as the anchor point. is the contact direction for slave node 103 and defines the orientation of the local tangent plane. In this example, as in many cases, the local tangent plane is only an approximation of the actual mesh geometry. • Master surface normals at symmetry planes: Sometimes the master surface normal and the local tangent plane that Abaqus/Explicit calculates are not suitable for the desired analysis. The most common situation where unsuitable surface normals are calculated occurs when a curved master surface ends at a symmetry plane and the boundary conditions have been specified in direct format rather than in symmetry “type” format (XSYMM, YSYMM, or ZSYMM—see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). In this case the correct normals should be in the symmetry plane; however, because the surface facets that abut the symmetry plane usually form an angle with the plane, the normal will project away from the symmetry plane. The effect of this behavior can be that a slave node does not project onto any master surface facet (the slave node is said not to “intersect” the master surface). No contact constraints will be enforced for such slave nodes. However, if symmetry “type” format boundary conditions are specified, contact constraints will be enforced as described below. The finite-sliding formulations use no special treatment for master surfaces ending at a symmetry plane. Figure 37.2.2–4 shows two concentric cylinders that contact each other; the inner cylinder is chosen as the master surface CSURF, and a half-symmetry model is used. Since Abaqus/Explicit calculates the nodal normals from the approximate, finite element model, the nodal normal does not point along the symmetry plane, which means that slave node 100 has no anchor point within the perimeter of the master surface. Whether or not contact is enforced for node 100 depends on how the symmetry boundary condition is specified. If the individual components are specified rather than a symmetry “type” boundary condition, slave node 100 will be free to penetrate the master surface. If the symmetry “type” format is used, the master normal at the node on the symmetry plane will be corrected to lie along the symmetry plane and contact will be enforced on the tangent plane as shown in Figure 37.2.2–5. Defining a YSYMM “type” boundary condition at node 1 to specify the symmetry plane will allow slave node 100 to see the master surface CSURF. master surface CSURF slave surface DSURF N1 100 symmetry plane Figure 37.2.2–4 Master surface normal at node 1 in a small-sliding model of concentric cylinders. With the default slave node 100 will never contact CSURF. • Modifying the local tangent plane orientation: In some cases the contact direction, , defined from the master surface averaged normals will not define the contact surface accurately. The most common example of this is a circular surface meshed with nonuniform length facets. Figure 37.2.2–6 shows how the averaged master normals will not be oriented correctly in the radial direction. In this case you should specify the contact direction directly for each slave node by defining spatially varying initial clearances . The location of the anchor point is not affected by reorienting the tangent plane using an initial clearance definition. master surface CSURF slave surface DSURF 100 N1 tangent plane Figure 37.2.2–5 The modified master surface normal at node 1 of CSURF now allows slave node 100 to contact CSURF. averaged master normal actual surface master surface Figure 37.2.2–6 Poorly oriented averaged master surface normals for an irregularly meshed circular surface. Local tangent plane rotation The local tangent plane is always orthogonal to the contact direction. The contact direction is taken as the interpolated normal of the master surface at the anchor point, , or as the direction specified with a spatially varying clearance definition . Once the contact direction has been defined, the orientation of the local tangent plane with respect to the master surface facet remains fixed. Because the small-sliding formulation considers nonlinear geometric effects, Abaqus/Explicit continuously updates the orientation of the local tangent plane to account for the rotation of the master surface facet. The position of the anchor point relative to the surrounding nodes on the master surface facet does not change as the master surface deforms. Load transfer In a small-sliding analysis the slave node will transfer load to the nodes of the master surface facet containing the anchor point, with the magnitude of the load transferred to each node weighted by its proximity to the anchor point. For example, in Figure 37.2.2–3 node 103 transmits load to both nodes 2 and 3 on the master surface. Thus, if node 103 impacts the local tangent plane, a larger share of the force would be transmitted to node 3 because it is closer to the anchor point . As a slave node slides along its local tangent plane, Abaqus/Explicit does not update the distribution of load transferred by a given slave node to its associated master surface nodes; the distribution is based solely on the position of the anchor point. This is unlike the small-sliding formulation in Abaqus/Standard, which does update the load distribution to the master surface nodes as sliding occurs, so that no net moment is associated with the contact forces acting on slave and master nodes per active contact constraint, regardless of the amount of sliding. Some net moment will be associated with the contact forces after sliding has occurred with the small-sliding formulation in Abaqus/Explicit. This net moment will not be significant if the sliding is truly small compared to element dimensions, but otherwise it can result in non-physical behavior and poor accounting of energy. , the anchor point Figure 37.2.2–7 shows the potential problem that arises if small sliding is used but the relative tangential motion of the surfaces is not “small.” It shows the possible evolution of contact between slave node 101 in Figure 37.2.2–1 and its master surface BSURF. Using the unit normal vectors and was found for slave node 101; for the purposes of this example, assume that it lies at the midpoint of the 201–202 face. With this location of the local tangent plane for node 101 is parallel with the 201–202 face. The load transfer always occurs at the original anchor point between nodes 201 and 202, no matter how far node 101 has slid along the local tangent plane. Therefore, if node 101 moves as shown in Figure 37.2.2–7, it will continue to transmit load equally to nodes 201 and 202 when, in fact, it really slid off the mesh forming the master surface BSURF. What can be considered small sliding A contact pair in a small-sliding contact simulation should not grossly violate any of the assumptions or limitations outlined above. Adhere to the following guidelines: • Slave nodes should slide less than an element length from their corresponding anchor point and still be contacting their local tangent plane. If the master surface is highly curved, the slave nodes should slide only a fraction of an element length. • The local tangent planes formed by Abaqus/Explicit should be a good approximation of the mesh geometry; if necessary, use an initial clearance definition (“Specifying initial clearance values precisely” in “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 35.5.4) to improve the tangent plane orientation. 201 X0 202 BSURF N201 101 t = 0 N202 101 t > 0 Figure 37.2.2–7 Excessive sliding in a small-sliding contact analysis. • The rotation and deformation of the master surface should not cause the local tangent planes to become a poor representation of the master surface during the course of the analysis. Master surface refinement in small-sliding problems The basic guidelines for pure master-slave contact given previously in this section should still be followed in a small-sliding simulation. However, in a small-sliding simulation more thought must be given to the degree of refinement for the master surface. The smoothly varying master surface normal and the local tangent planes that are formed with it are crucial to the success of a small-sliding analysis. As has been mentioned previously, there are several methods that can be used to modify ; however, they only control the initial configuration of the local tangent planes. The deformation and rotation of the master surface can reorient the local tangent planes such that they become a poor representation of the master surface. Figure 37.2.2–8 shows an example where distortion of the master surface results in such a situation. This problem can be minimized to some extent by using a more refined mesh on the master surface, thus providing more element faces to control the motion of the tangent planes. Excessive mesh refinement should not be necessary since only small sliding should occur. Using the infinitesimal-sliding formulation The difference between the infinitesimal-sliding and small-sliding formulations is that the infinitesimal- sliding formulation ignores nonlinear geometric effects. To specify the infinitesimal-sliding formulation, you choose the small-sliding contact formulation and a small-displacement formulation for the analysis step. Infinitesimal sliding assumes that both the relative motions of the surfaces and the absolute motions of the model remain small. The orientations of the local tangent planes are not updated, and the load transfer paths and the weightings assigned to each master surface node remain constant during an infinitesimal-sliding simulation. initial configuration local tangent plane master surface slave surface large deformation Figure 37.2.2–8 Master surface deformation in a small-sliding contact analysis can cause problems with the local tangent planes. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *STEP, NLGEOM=NO … *CONTACT PAIR, SMALL SLIDING Interaction module: interaction editor: Sliding formulation: Small sliding Step module: step editor: Nlgeom: Off Contact tracking algorithms A large portion of the computational cost associated with Abaqus/Explicit contact pairs derives from the algorithms used to track the relative motion between two contacting surfaces. There are two tracking approaches for the contact pair algorithm in Abaqus/Explicit, depending on the sliding formulation that is used: finite sliding and small/infinitesimal sliding. Finite-sliding tracking Abaqus/Explicit is designed to simulate highly nonlinear events or processes. Because it is possible for a node on one surface to contact any of the facets on the opposite surface, Abaqus/Explicit must use sophisticated search algorithms for tracking the motions of the surfaces. The contact search algorithm is designed to be robust, yet computationally efficient. This algorithm assumes that the incremental relative tangential motion between surfaces does not significantly exceed the dimensions of the master surface facets, but there is no limit to the overall relative motion between surfaces. It is rare for the incremental motion to exceed the facet size because of the small time increment used in explicit dynamic analyses. In cases involving relative surface velocities that exceed material wave speeds, it may be necessary to reduce the time increment. The contact search algorithm uses a global search at the beginning of each step, and a hierarchical global/local search algorithm is used for the other increments. The default contact search algorithm can handle the majority of typical contact situations. However, there are some situations that require special attention. We will consider a pure master-slave contact pair for discussion purposes. For a balanced master-slave contact pair, the contact search computations are performed twice for each contact pair. Global contact searches A global search determines the globally nearest master surface facet for each slave node in a given contact pair. A bucket sorting algorithm is used to minimize the computational expense of these searches. A two-dimensional example, without consideration of “buckets,” is shown in Figure 37.2.2–9. master surface 100 10 101 11 102 12 13 48 49 50 51 slave surface 52 53 location of tracked master node searched master faces Figure 37.2.2–9 Global search in two dimensions. The global search computes the distance from node 50 to all of the master surface facets in the same bucket as node 50. It determines that the nearest facet on the master surface to node 50 is the facet of element 10. Node 100 is the node on this facet that is nearest to node 50, and it is designated the tracked master surface node. This search is conducted for each slave node, comparing each node against all of the facets on the master surface that are in the same bucket. By default, Abaqus/Explicit performs a global search every one hundred increments for two-surface contact pairs. The frequency of the global search can be manually adjusted, as discussed in “Contact controls for contact pairs in Abaqus/Explicit,” Section 35.5.5. Despite the bucket sorting algorithm, global searches are computationally expensive: performing a global contact search in every increment will more than double the run time of many Abaqus/Explicit contact analyses. Local contact searches Abaqus/Explicit uses a local contact search to track the motion of the surfaces during most increments of an analysis. In this approach a given slave node searches only the facets that are attached to the previously tracked master surface node. Abaqus/Explicit determines which adjacent facet is the nearest to the slave node. It then determines which node on that facet is the closest master surface node to the slave node and updates the tracked master surface node. If the closest master surface node is not the same as the previously tracked master surface node, Abaqus/Explicit performs another iteration of the local search. In the example shown in Figure 37.2.2–10, node 50 moves as shown during an increment. In the first iteration of the search Abaqus/Explicit finds that the master surface facet on element 10 is still the closest facet of those attached to node 100 but that node 101 is now the tracked master surface node. Because the previously tracked node was node 100, Abaqus/Explicit performs another iteration. In this second iteration a new element, element 11, is found to be the closest facet and the closest master surface node is 102. Another iteration is performed because the identity of the tracked master surface node changed. In the third iteration the identity of the tracked node does not change, so Abaqus/Explicit designates node 102 as the tracked master surface node for slave node 50. A local search is substantially less expensive computationally than a global search. A slightly more expensive local search algorithm can be employed in situations where contact is not being properly enforced; this alternate algorithm is discussed in “Contact controls for contact pairs in Abaqus/Explicit,” Section 35.5.5. Tracking approach for self-contact pairs Abaqus/Explicit uses similar contact searching methods for simulations with self-contact as for two- surface contact; however, more frequent global searches are often necessary for self-contact problems. By default, contact pairs with self-contact use a global contact search every four increments, compared to every 100 increments for two-surface contact pairs; the frequency of the global searches can be manually adjusted . If several facets that are unconnected to each other are found to be near a slave node during global tracking, global tracking automatically will be performed more frequently than the specified number of increments. Despite this precaution, the self-contact algorithm will be less robust if you specify a search frequency that is significantly lower than the default. master surface 100 101 10 11 102 12 13 48 49 50 slave surface 51 52 ⇒ motion of slave surface location of previously tracked master node location of currently tracked master node Figure 37.2.2–10 Local search in two dimensions. Small-sliding (or infinitesimal-sliding) tracking approach When the small-sliding or infinitesimal-sliding contact approach is invoked , Abaqus/Explicit performs a single global search at the beginning of the first step to determine the globally nearest master surface facet for each slave node in the given contact pair. Once the nearest facet has been determined, the nearest point on that facet defines the anchor point. Contact constraints will not be applied to slave nodes that do not project onto any master surface facet. No further tracking is performed during the step or for subsequent steps in which the contact pair remains active. This makes the small-sliding/infinitesimal-sliding contact approach less expensive computationally than the finite-sliding contact approach. The cost savings are most significant for three-dimensional contact problems. 37.2.3 CONTACT CONSTRAINT ENFORCEMENT METHODS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Defining general contact interactions in Abaqus/Explicit,” Section 35.4.1 • “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1 • *CONTACT • *CONTACT PAIR • “Specifying master-slave assignments for general contact,” Section 15.13.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Abaqus/Explicit uses two different methods to enforce contact constraints: • The kinematic contact algorithm uses a kinematic predictor/corrector contact algorithm to strictly enforce contact constraints (for example, no penetrations are allowed). • The penalty contact algorithm has a weaker enforcement of contact constraints but allows for treatment of more general types of contact. Contact pairs in Abaqus/Explicit use kinematic enforcement by default, but penalty enforcement can be specified for individual contact pairs. General contact always uses penalty enforcement. Both methods conserve momentum between the contacting bodies. Kinematic contact algorithm A summary of the default kinematic algorithm that Abaqus/Explicit uses to enforce contact with the contact pair algorithm is presented below. It is a predictor/corrector algorithm and, therefore, has no influence on the stable time increment. It is easier to describe the algorithm by first considering a pure master-slave contact pair. Kinematic enforcement of contact conditions in a pure master-slave contact pair In this case in each increment of the analysis Abaqus/Explicit first advances the kinematic state of the model into a predicted configuration without considering the contact conditions. Abaqus/Explicit then determines which slave nodes in the predicted configuration penetrate the master surfaces. The depth of each slave node’s penetration, the mass associated with it, and the time increment are used to calculate the resisting force required to oppose penetration. For hard contact, this is the force which, had it been applied during the increment, would have caused the slave node to exactly contact the master surface. The next step depends on the type of master surface used. • When the master surface is formed by element faces, the resisting forces of all the slave nodes are distributed to the nodes on the master surface. The mass of each contacting slave node is also distributed to the master surface nodes and added to their mass to determine the total inertial mass of the contacting interfaces. Abaqus/Explicit uses these distributed forces and masses to calculate an acceleration correction for the master surface nodes. Acceleration corrections for the slave nodes are then determined using the predicted penetration for each node, the time increment, and the acceleration corrections for the master surface nodes. Abaqus/Explicit uses these acceleration corrections to obtain a corrected configuration in which the contact constraints are enforced. • In the case of an analytical rigid master surface, the resisting forces of all slave nodes are applied as generalized forces on the associated rigid body. The mass of each contacting slave node is added to the rigid body to determine the total inertial mass of the contacting interfaces. The generalized forces and added masses are used to calculate an acceleration correction for the analytical rigid master surface. Acceleration corrections for the slave nodes are then determined by the corrected motion of the master surface. When using hard kinematic contact, it is still possible with the pure master-slave algorithm for the master surface to penetrate the slave surface in the corrected configuration . slave nodes cannot penetrate master segments master surface (segments) penetration slave surface (nodes) gap master node can penetrate slave segment Figure 37.2.3–1 Master surface penetrations into the slave surface of a pure master-slave contact pair due to coarse discretization. Using a sufficiently refined mesh on the slave surface will minimize such penetrations. Softened kinematic contact will allow penetrations since corrections are made to satisfy the pressure-overclosure relationship at the slave-nodes, not the condition of zero penetration. Kinematic enforcement of contact conditions in a balanced master-slave contact pair The kinematic contact algorithm for a balanced master-slave contact pair applies acceleration corrections that are linear combinations of pure master-slave corrections calculated in exactly the same manner as outlined above. One set of corrections is calculated considering one surface as the master surface, and the other corrections are calculated considering that same surface as the slave surface. Abaqus/Explicit then applies a weighted average of the two values. The exact weighting for each correction depends on the weighting factor specified for the contact pair . The default for balanced master-slave contact is to weight each correction equally. Hard kinematic contact will minimize the penetration of the surfaces. However, after the initial weighted correction is applied, it is possible to still have some penetration of the surfaces. Therefore, Abaqus/Explicit uses a second contact correction to resolve any remaining overclosure in a balanced master-slave contact pair that uses hard kinematic contact. Both master-slave assignment combinations are again considered, but weighting factors are not used when combining the contributions to form the second applied acceleration correction. It is possible that small gaps between the contacting surfaces will be created during the second correction if there was some residual penetration after the first correction: the magnitude of the gaps after the second correction will generally be much smaller than the penetration after the first correction. The effect of the second correction is illustrated in Figure 37.2.3–2 to Figure 37.2.3–5. The second contact correction described above is not conducted in the case when a softened kinematic contact formulation is used. This may lead to penetration values that may not be exactly synchronized with the pressure-overclosure curve. Moreover, the frictional shear forces (if any) may not reflect the specified coefficient of friction exactly when non-sticking sliding occurs. Use a pure master-slave kinematic formulation to avoid these inaccuracies. Figure 37.2.3–2 Effect of second contact corrections; initial configuration. balanced slave-master contact pair Figure 37.2.3–3 Final configuration when the second contact correction is used. balanced slave-master contact pair Figure 37.2.3–4 Final configuration if the second contact correction were to be omitted. Energy considerations for hard kinematic contact The kinematic contact algorithm strictly enforces contact constraints and conserves momentum. To achieve these qualities with a discretized model, some energy is absorbed upon impact. For example, consider a linear elastic beam modeled with several elements that impacts a rigid wall as shown in Figure 37.2.3–6. The kinetic energy of the leading node is absorbed by the contact algorithm upon impact. A stress wave passes through the truss, and the truss eventually rebounds from the wall. The kinetic energy after the rebound is smaller than before the impact because of the contact node’s energy loss upon impact. As the mesh is refined, this energy loss is reduced because the mass and kinetic energy of the leading node of the truss become less significant. Contact forces can also exert negative external work upon impact since contact forces act over the entire increment in which impact occurs, including the fraction of the increment prior to impact. The opposing contact forces, which are equal in magnitude, act over different distances, thereby exerting a pure slave-master contact pair master node can penetrate slave surface Figure 37.2.3–5 Final configuration when a pure master-slave contact pair is used. The master surface is defined on the bottom elements. v0 Figure 37.2.3–6 Beam impacting a fixed rigid wall. nonzero net work. The net external work of these forces is negative, and the absolute value of the net external work does not exceed the contact node’s kinetic energy loss upon impact. These energies are insignificant in most models but can be significant in high-speed impacts, where high mesh refinement near the contact interface is recommended. Penalty contact algorithm The penalty contact algorithm results in less stringent enforcement of contact constraints than the kinematic contact algorithm, but the penalty algorithm allows for treatment of more general types of contact (for example, contact between two rigid bodies). The penalty contact method is well suited for very general contact modeling, including the following situations: • multiple contacts per node, • contact between rigid bodies, and • contact of surfaces also involved in other types of constraints (such as MPCs). Since the penalty algorithm introduces additional stiffness behavior into a model, this stiffness can influence the stable time increment. Abaqus/Explicit automatically accounts for the effect of the penalty stiffnesses in the automatic time incrementation, although this effect is usually small, as discussed below. The penalty enforcement method is always used by the general contact algorithm. For contact pairs, you can specify the penalty method as an alternative to the default kinematic enforcement method. When the penalty method is chosen for enforcing contact constraints in the normal direction, it is also used to enforce sticking friction . Input File Usage: Use the following option to select the penalty contact algorithm for a contact pair: *CONTACT PAIR, MECHANICAL CONSTRAINT=PENALTY surface_1, surface_2 Abaqus/CAE Usage: Interaction module: interaction editor: Mechanical constraint formulation: Penalty contact method Penalty enforcement of contact conditions for pure master-slave surface weighting The penalty contact algorithm searches for slave node penetrations in the current configuration, including node-into-face, node-into-analytical rigid surface, and edge-into-edge penetrations. For node-to-face contact, forces that are a function of the penetration distance are applied to the slave nodes to oppose the penetration, while equal and opposite forces act on the master surface at the penetration point. The master surface contact forces are distributed to the nodes of the master faces being penetrated. For node- to-analytical rigid surface contact, forces that are a function of the penetration distance are applied to the slave nodes to oppose the penetration, while equal and opposite forces act on the analytical rigid surface at the penetration point. The contact forces acting at the penetration point of the analytical rigid surface result in equivalent forces and moments at the reference node of the rigid body corresponding to the analytical rigid surface. For edge-to-edge contact, the opposing contact forces are distributed to the nodes of the two contacting edges. As with the pure master-slave kinematic contact algorithm, there is no resistance to master surface nodes penetrating slave surface faces with the pure master-slave penalty contact algorithm. Using a sufficiently refined mesh on the slave surface will help correct this problem. Penalty enforcement of contact conditions for balanced master-slave surface weighting The penalty contact algorithm for balanced master-slave contact surfaces computes contact forces that are linear combinations of pure master-slave forces calculated in the manner outlined above. One set of forces is calculated considering one surface as the master surface, and the other forces are calculated considering that same surface as the slave surface. Abaqus/Explicit then applies a weighted average of the two values. The weighting used with each set of forces depends on the weighting factor specified for the surfaces . The default for balanced master-slave contact pairs and general contact is to weight each of the two sets of forces equally. Scaling the penalty stiffness The “spring” stiffness that relates the contact force to the penetration distance is chosen automatically by Abaqus/Explicit for hard penalty contact, such that the effect on the time increment is minimal yet the allowed penetration is not significant in most analyses. The default penalty stiffness is based on a representative stiffness of the underlying elements. A scale factor is applied to this representative stiffness to set the default penalty. Consequently, the penetration distance will typically be greater than the parent elements’ elastic deformation normal to the contact interface. In purely elastic problems this penetration can affect the stress solution significantly, as demonstrated in “The Hertz contact problem,” Section 1.1.11 of the Abaqus Benchmarks Manual. When element or node-based rigid bodies are involved in contact interactions, for numerical stability reasons Abaqus/Explicit will compute penalties at each contacting node on the rigid body by considering the overall inertia properties of the body. Consequently, the contact penalties will be different from the case when these elements were not converted to rigid and thus the penetrations in the two cases may be different. You can specify a factor by which to scale the default penalty stiffnesses, as described in “Contact controls for general contact in Abaqus/Explicit,” Section 35.4.5, and “Contact controls for contact pairs in Abaqus/Explicit,” Section 35.5.5. This scaling may affect the automatic time incrementation. Use of a large scale factor is likely to increase the computational time required for an analysis because of the reduction in the time increment that is necessary to maintain numerical stability. Choosing between the kinematic and penalty contact algorithms The penalty contact algorithm can model some types of contact that the kinematic contact algorithm cannot. Element-based rigid surfaces are not restricted to acting only as master surfaces within the penalty algorithm as they are within the kinematic algorithm. Thus, the penalty method allows modeling of contact between rigid surfaces, except when both surfaces are analytical rigid surfaces or when both surfaces are node-based. The penalty contact algorithm must be used for all contact pairs involving a rigid body if a linear constraint equation, multi-point constraint, surface-based tie constraint, or connector element is defined for a node on the rigid body. For all other cases, Abaqus/Explicit enforces equations, multi-point constraints, tie constraints, embedded element constraints, and kinematic constraints (defined using connector elements) independently of contact constraints; therefore, if a degree of freedom participates in a linear constraint equation, multi-point constraint, tie constraint, embedded element constraint, or kinematic constraint in addition to a contact constraint, the contact constraint will usually override these constraints . Hence, the penalty contact algorithm is recommended if these constraints need to be strictly enforced. Impact is plastic when the default hard, kinematic contact algorithm is used; and the kinetic energy of the contacting nodes is lost. This loss in energy is insignificant for a refined mesh but can be significant with a coarse mesh. Penalty contact and softened kinematic contact introduce numerical softening to the contact enforcement analogous to adding elastic springs to the contact interface, which means that these algorithms do not dissipate energy upon impact (the energy stored in the springs is recoverable). This distinction between the algorithms is particularly apparent if a point mass with no force acting upon it impacts a fixed rigid wall: with penalty contact and softened kinematic contact the point mass will bounce away, but with hard kinematic contact the point mass will stick to the wall. A further difference between kinematic and penalty contact is that the critical time increment is unaffected by kinematic contact but can be affected by penalty contact. For hard penalty contact, default penalty stiffnesses are chosen such that the stable time increments of the deformable parent elements of contact surface facets are effectively reduced by approximately 4% for increments in which contact forces are being transmitted; default penalty stiffnesses of node-based surface nodes require a 1% decrease in the element-by-element time increment to ensure numerical stability. Penalty stiffnesses between rigid bodies are chosen by default to have no effect on the stable time increment. If the default penalty stiffnesses are overridden by a penalty scale factor or softened contact behavior , the time increment is modified based on the maximum stiffness active in the contact interface. Increasing the penalty stiffnesses may decrease the stable time increment significantly . If the overall stable time increment is not controlled by elements on the contact interface, the penalty contact algorithm usually will not affect the time increment. Penalty contact and softened kinematic contact cannot be used with the breakable bond model; hard kinematic contact must be used for this model. Table 37.2.3–1 Effect of scale factor on time increment. Penalty scale factor Lower bound to ratio of the time increment with contact divided by the time increment without contact 1.0 10.0 100.0 1000.0 10000.0 0.96 0.34 0.13 0.04 0.013 38. Contact Difficulties and Diagnostics Resolving contact difficulties in Abaqus/Standard Resolving contact difficulties in Abaqus/Explicit 38.1 38.1 Resolving contact difficulties in Abaqus/Standard • “Contact diagnostics in an Abaqus/Standard analysis,” Section 38.1.1 • “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 38.1.2 38.1.1 CONTACT DIAGNOSTICS IN AN Abaqus/Standard ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Output to the data and results files,” Section 4.1.2 • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • “Contact formulations in Abaqus/Standard,” Section 37.1.1 • *CONTACT PRINT • *PREPRINT • *PRINT • Chapter 41, “Viewing diagnostic output,” of the Abaqus/CAE User’s Manual Overview Diagnostics of an Abaqus/Standard analysis can be used to: • check the initial contact conditions in a model; and • track contact statuses over the course of the analysis. Diagnostic information is available in several locations: • The output database • The job diagnostics tool in the Visualization module of Abaqus/CAE • The data (.dat) file • The message (.msg) file Reviewing the adjustments of initially overclosed surfaces strain-free adjustments of nodal positions are performed by Abaqus/Standard under Initial various circumstances to remove contact overclosures or to remove overclosures or gaps between surfaces of surface-based tie constraints . The initial configuration of the model is determined after these strain-free adjustments are applied. There are two sources of information on the adjustments of overclosed surfaces: the data (.dat) file and the output database (.odb) file. Output of information on strain-free adjustments to the data file By default, information about a limited number of strain-free nodal adjustments is provided in the data (.dat) file. Requesting more detailed output concerning contact constraints provides information for all strain-free adjustments, regardless of the number of nodes adjusted. Input File Usage: Abaqus/CAE Usage: *PREPRINT, CONTACT=YES Job module: job editor: General: Preprocessor Printout: Print contact constraint data Visualizing strain-free adjustments Output variable STRAINFREE contains nodal vectors representing initial strain-free adjustments. By default, this output variable is written to the output database (.odb) file for the original field output frame at zero time if any strain-free adjustments are made by Abaqus/Standard. A symbol plot of this variable in the Visualization module of Abaqus/CAE shows vectors that represent how individual nodes have been adjusted, and a contour plot of this variable shows the distribution of the adjustment magnitude (you must select the original output frame at zero time in the Visualization module of Abaqus/CAE before choosing the STRAINFREE output variable). Initial nodal positions written to the output database file by Abaqus/Standard include the effects of strain-free adjustments, so plots of the initial configuration show the adjusted nodal positions. Reviewing initial contact conditions Before conducting an analysis, perform a data check on the model to review the initial contact conditions . The data check creates an output database and calculates the variable COPEN (contact opening) on each slave surface based on the initial configuration of the model. You can create a contour plot of COPEN in the Visualization module of Abaqus/CAE to check for overclosed surfaces in the model assembly (an overclosure corresponds to a negative value of COPEN). In addition, you can instruct Abaqus to print detailed information about the initial contact conditions to the data file during the data check (this information is not printed by default). The data file lists the status (open or closed) and clearance distance for each constraint point on a slave surface, the internally generated contact element number associated with each slave node or facet, and a summary of contact interaction properties. Internally generated contact elements are not user-defined and do not appear in the input file, so they can be difficult to locate if an error or warning message refers to them. The information in the data file can be used to locate these contact elements in the model. The data file also lists the key parameters for every contact interaction in the model. These parameters include: • slave and master surface names; • interaction property; • value of ; • degree of smoothing on the master surface ; • characteristic length used in penetration tolerance calculations ; • extension ratio applied to master surface edges ; and • contact formulation. Parameters are listed only for the interactions to which they are applicable. For example, , surface smoothing, and the extension ratio are not used for surface-to-surface contact calculations (including general contact), so Abaqus does not report values for these parameters in surface-to-surface interactions. Input File Usage: Abaqus/CAE Usage: Use the following option to print information about initial contact conditions to the data file: *PREPRINT, CONTACT=YES Job module: job editor: General: Preprocessor Printout: Print contact constraint data Output of master surface nodes associated with slave nodes for small-sliding contact When you print initial contact conditions to the data file for contact pairs using the small-sliding tracking approach, Abaqus creates an output table showing the master nodes associated with each slave node. Each row of the table lists a slave node and the master nodes to which the slave node transfers load when in contact with the master surface. The number of nodes in the table indicates whether or not the anchor point for a slave node lies on an element face or at a node. For details on the small-sliding tracking approach and load transfer, see “Using the small-sliding tracking approach” in “Contact formulations in Abaqus/Standard,” Section 37.1.1. In the output shown below for a two-dimensional model, slave node 2 has an anchor point at master surface node 101 because it interacts with three master surface nodes. Slave node 1 has an anchor point between nodes 100 and 101. This table also provides a list of slave nodes that did not find an intersection with the master surface. This is important because these nodes have no local tangent plane and, hence, can penetrate the master surface. SMALL SLIDING NON-RIGID AX ELEMENT(S) INTERNALLY GENERATED FOR SLAVE BLANK AND MASTER SPHERE WITH SURFACE INTERACTION INF1 ELEMENT NUMBER SLAVE NODE(S) NODE(S) MASTER 46 101 100 47 50 102 101 100 NO INTERSECTION ***WARNING: 1 SLAVE NODES FOUND NO INTERSECTION WITH A MASTER SURFACE Tracking contact status during a simulation Abaqus provides two methods for tracking the status of contact interactions over the course of an analysis: the diagnostics tool available in the Visualization module of Abaqus/CAE and contact output to the data (.dat) file.You can write contact output to the data (.dat) file for tracking the status of contact interactions over the course of an analysis. Tracking contact status helps you ensure contact surfaces are defined appropriately, troubleshoot a terminated contact analysis, and verify that contact interactions behave realistically. The diagnostics tool in Abaqus/CAE provides a good overview of how contact conditions evolve throughout a simulation. It is useful for reviewing terminated analyses because it reports contact change calculations in every iteration. The data file offers a more detailed summary of the overall contact conditions and the forces driving these conditions. However, it only provides output for successfully completed increments. Contact diagnostics in the Visualization module of Abaqus/CAE The diagnostics tool in the Visualization module of Abaqus/CAE can be used with the following procedure types: • static stress/displacement; • coupled thermal/stress; and • coupled pore fluid flow/stress. The diagnostics tool tracks all changes in contact during an analysis. Each time a constraint point’s contact status changes from closed to open, it is recorded as an “opening.” Each time the status changes from open to closed, it is recorded as an “overclosure.” If the contact interaction involves frictional effects, the diagnostics note when a constraint point begins sliding along the master surface (“slipping”) and when a constraint point in motion stops on the master surface (“sticking”). The diagnostics tool lists the constraint point involved in the status change and allows you to highlight the location of the constraint point in the model. The calculated clearance or overclosure distance is also shown, and the maximum penetration is reported when the penetration tolerance for augmented Lagrange contact is exceeded . For the default contact convergence criteria, the diagnostics tool shows the maximum penetration error and the maximum estimated contact force error; these determine whether the contact conditions have converged (for details, see “Severe discontinuities in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2). If you choose to use the traditional contact convergence criteria, these error measures are not reported. For analyses involving Lagrange friction, the diagnostics show the maximum slip error for points that should be sticking . For detailed instructions on using the diagnostics tool, see Chapter 41, “Viewing diagnostic output,” of the Abaqus/CAE User’s Manual. The contact diagnostic information available in Abaqus/CAE can also be printed to the Abaqus message file. For details, see “The Abaqus/Standard message file” in “Output,” Section 4.1.1. Contact output in the data file When you request contact output to the data file , Abaqus lists the contact status for every constraint point at each increment of the analysis. The values of CPRESS, CSHEAR, COPEN, and CSLIP at each constraint point are also reported by default. Example: Forming a channel Contact diagnostics are often helpful in confirming that the interactions in a model are behaving realistically and as intended. The diagnostics also provide a means of tracing the evolution of contact statuses on a node-by-node basis. In this example the diagnostics are based on a channel forming model. The channel is formed from a steel plate (or blank) with appreciable thickness. The blank is modeled with two-dimensional, plane strain elements; the forming tools (die, holder, and punch) are modeled as analytical rigid surfaces. The initial and final configurations of the model are displayed in Figure 38.1.1–1. Undeformed shape Deformed shape Figure 38.1.1–1 Model for channel-forming example. extruded for visualization purposes.) (The blank has been If you include a step or prescribed condition in your model intended to establish contact between two surfaces, the diagnostics tool in Abaqus/CAE can confirm the success of this modeling technique. In this example contact must be firmly established between the blank, the die, and the holder before the forming process begins. Small but consistent overclosures in the nodes along the surface of the blank indicate that the contact conditions are appropriate to begin forming the channel . You can also use the contact conditions to review changes in contact status throughout the forming process. Figure 38.1.1–3 depicts the onset of slipping for two nodes on the blank. This information might be used to confirm frictional or material effects. For example, you can draw the following conclusions about these diagnostics in the channel forming analysis: • If the slipping does not occur until well into the forming process, frictional forces were probably holding the blank in place between the die and holder. Overclosures Figure 38.1.1–2 Diagnostics confirming contact conditions between the blank, die, and holder. • Since all the nodes on the blank do not slip simultaneously, there is most likely some mild stretching and nonuniform deformation occurring in the blank. For more insight on the slipping nodes, refer to the data file. The following excerpt lists a portion of the blank-die interaction in the same increment depicted in Figure 38.1.1–3: NODE FOOT- NOTE CPRESS CSHEAR1 COPEN CSLIP1 290 295 300 305 OP SL ST ST 0.000 0.000 4.4632E+06 -4.4632E+05 9.5643E+06 -9.3177E+05 2.9421E+06 -2.7867E+05 4.1155E-07 -2.8783E-07 -5.1137E-06 -4.8711E-06 -4.7359E-06 0.000 0.000 0.000 The contact status is indicated in the “footnote” column: open (OP), closed and sticking tangentially (ST), or closed and sliding tangentially (SL). In the absence of frictional properties the two contact statuses are open (OP) and closed (CL). In the output above node 290 is open; consequently, the contact pressure variable CPRESS is zero. The COPEN variable reports that this node is 4.1155 × 10−7 length units away from the master surface. The SL footnote for node 295 indicates that it is in contact with the master surface (the die) and is “slipping.” The critical shear stress, , where p is the value of contact pressure shown under CPRESS and is the coefficient of friction for the contact = 0.1; the critical shear stress (4.4632 × 106 × 0.1 = 4.4632 × 105 ) is equal interaction. In this model to the frictional shear stress CSHEAR1, so the node is slipping. In the case of node 300 the critical shear stress (9.5643 × 106 × 0.1 = 9.5643 × 105 ) is greater than the frictional shear stress, so the node is sticking. Likewise for node 305. , can be determined by the equation The CSLIP1 variable is the total accumulated (integrated) slip at the slave node. Accumulated slip and slip directions are discussed in more detail in “Output of tangential results” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1. Diagnosing a terminated contact analysis Contact diagnostics provide invaluable information when trying to resolve errors in a terminated analysis. The diagnostics let you review trends in the model’s contact status, visually identify regions of the model involved in contact difficulties, and numerically quantify the severity of an error. For a more general discussion of common errors associated with using contact in Abaqus/Standard analyses, refer to “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 38.1.2. Excessive severe discontinuity iterations Establishing contact conditions is a common source of difficulty in an implicit static contact analysis. If an analysis terminates because it exceeds the maximum number of severe discontinuity iterations , the contact diagnostics give insight into how to resolve the problem. You can plot the number of contact status changes over the course of an attempt, as shown in Figure 38.1.1–4. If the changes are tending toward zero, increasing the allowed number of severe discontinuity iterations or adjusting the SDI conversion settings may allow Abaqus to resolve the contact conditions. If the changes are not tending toward zero, you will need to revise your model or investigate other options. Using the visualization tools, you can see which areas of the model are involved in contact changes. If a particular contact pair or surface region is causing a majority of the status fluctuations, you may need to modify the characteristics of the associated interaction. For example, it is typically easier to resolve contact conditions for contact pairs using the small-sliding tracking approach (if it is applicable) than for those using the finite-sliding tracking approach. Chattering The contact diagnostics tool makes it very easy to detect chattering in a model. In this situation the same node or constraint appears in the diagnostics summary for every iteration, alternating as an overclosure or an opening. The classic chattering scenario produces diagnostics plots that tend toward zero but level off at a low number due to the oscillating contact status . Techniques Points now slipping Figure 38.1.1–3 Diagnostics for the onset of slipping. Iteration Iteration Figure 38.1.1–4 Changes in contact status during an attempt. for resolving contact chattering problems are discussed in “Excessive iterations in contact simulations” in “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 38.1.2. Unrealistic and severe overclosures When reviewing diagnostics, you may notice overclosures during unconverged iterations for nodes or constraint points that are located outside of the regions that are contacting in a converged state. The reported overclosure value for these nodes will be significantly greater than the overclosures for nodes within the contacting regions, as seen in the highlighted constraint point in Figure 38.1.1–5. This is an indication of physical or numerical instabilities in the model. You should take steps to more firmly establish contact before proceeding with the simulation or add some form of stabilization to the model . Using smaller increments can sometimes enable a solution to be obtained in these cases. Nonconverging force equations Contact diagnostics do not always involve severe discontinuity iterations. Poorly defined contact can lead to nonconvergence of the force equations in an analysis . If the same node appears repeatedly as the location of maximum residuals and corrections, investigate the contact conditions around that node. Consider the example in Figure 38.1.1–7. The diagnostics highlight the “problem node” on the perimeter of the slave surface. A closer look in the vicinity of this node reveals that the slave surface mesh is too coarse. Slave nodes along the perimeter of the surface are touching the master surface, but the next row of nodes is “hanging over” the rim of the master surface. If this contact pair uses node-to-surface contact discretization, the master surface can penetrate the slave surface with little resistance between the nodes. Such penetrations can cause the nonconverging force equations seen in the diagnostics. Any situation in which the master surface is free to penetrate the slave surface can prevent an analysis from converging. Potential solutions include: • switching the master and slave assignments; • using surface-to-surface discretization (however, using surface-to-surface discretization without refining a coarse slave mesh may lead to inaccurate stress results, even if the analysis does converge); or • refining the mesh on the slave surface. Figure 38.1.1–5 The overclosure at one constraint point is significantly higher than the overclosures at other constraint points. Figure 38.1.1–6 The diagnostics tool reports equilibrium difficulties. Figure 38.1.1–7 Two surfaces in a region of nonconverging force equations. 38.1.2 COMMON DIFFICULTIES ASSOCIATED WITH CONTACT MODELING IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining general contact interactions in Abaqus/Standard,” Section 35.2.1 • “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • *CONTACT • *CONTACT PAIR • *CONTACT INITIALIZATION DATA • “Defining general contact,” Section 15.13.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining surface-to-surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Using contact and constraint detection,” Section 15.16 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview This section highlights the difficulties that are most commonly encountered when modeling contact interactions with Abaqus/Standard. Recommendations on how to circumvent these problems are presented. Difficulties resolving initial contact conditions It is important to understand how Abaqus/Standard interprets and resolves contact conditions at the start If necessary, you can check initial contact conditions in the message file . Unintentional contact openings or overclosures can lead to poor interpretations of surface geometry, unintentional motion in a model, and failure of an analysis to converge. Removing initial contact openings and overclosures When modeling the contact between two faceted surfaces, it is often possible for small gaps or penetrations to occur at individual nodes. This problem is particularly common when the two surfaces have dissimilar meshes. Abaqus/Standard uses two default methods for dealing with initial penetrations: • In general contact small initial overclosures are automatically adjusted to remove the penetrations. • In contact pairs initial overclosures are interpreted as interference fits and resolved accordingly . You can improve the accuracy of a contact simulation by having Abaqus/Standard adjust the position of the slave surface to ensure that all slave nodes that should initially be in contact with the master surface start out in contact without any penetration . When an intended initial clearance or overclosure is small compared to typical dimensions of the bodies in contact and a small-sliding contact pair is used, you can specify the clearance or overclosure precisely . The small-sliding contact tracking approach is more sensitive than the finite-sliding tracking approach to initial local gaps at the contact interface. In small-sliding contact each slave node interacts with a contact plane defined from the finite element approximation of the master surface, as discussed in “Contact formulations in Abaqus/Standard,” Section 37.1.1. Abaqus/Standard can define these planes only when each slave node can be projected onto the master surface. Having these slave nodes start the simulation contacting the master surface allows Abaqus/Standard to form the most accurate contact planes for the slave nodes. Large unintended initial overclosures The contact initialization algorithm may occasionally infer large initial overclosures where you do not intend initial overclosures to exist. For example, specifying incorrect surface normals can cause the contact initialization algorithm to interpret a physical gap as a penetration, as discussed in “Orientation considerations for shell-like surfaces” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1. Minor changes to the surface or contact definition will typically avoid undesired overclosures, but these situations typically call for some diagnosis to determine how to avoid the problem. Identifying the location of unintended overclosures The first step in resolving a large initial overclosure is to identify the location of the problem: • If initial overclosures are treated as interference fits to be resolved in the first increment (which is the default behavior for contact pairs; see “Modeling contact interference fits in Abaqus/Standard,” Section 35.3.4), a contour plot of the contact opening distance output variable (COPEN) for the initial output frame will show which regions have initial overclosures (penetrations correspond to negative values of COPEN). • If initial overclosures are resolved with strain-free adjustments, a contour plot of the output variable STRAINFREE for the initial output frame will show where adjustments occurred . However, large strain-free adjustments may cause the mesh to become highly distorted, making it difficult to fully diagnose the problem; in such cases, perform a datacheck analysis with initial overclosures instead treated as interference fits to be resolved in the first increment to facilitate diagnosis (as discussed above). Once you identify the location of an unintended initial overclosure, limiting the display in the Visualization module of Abaqus/CAE to the master and slave surfaces of the interaction involved in the initial overclosure is helpful for identifying the cause of an unintended initial overclosure . Viewing the surface normals may help determine whether unintended overclosures are due to incorrect surface normals. Overclosures on discontinuous surfaces In this case a Figure 38.1.2–1 shows an example with a large, unintended initial overclosure. single contact pair with discontinuous surfaces is meant to enforce contact in two distinct regions (Table 35.3.1–1 “Orientation considerations for shell-like surfaces” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1, shows which contact formulations allow discontinuous surfaces). The arrows in Figure 38.1.2–1 show the positive normal direction for each surface region. The surface-to-surface contact formulation searches along the slave-surface normal direction (in the positive and negative directions) for potential interaction points on the master surface. The search emanating from point A identifies point B as the only potential interaction point for point A in this example. The contact pair interprets this as a valid penetration because no better candidate interaction location is found and surface normals are opposed at points A and B. Methods to avoid this unintended overclosure include: • defining separate contact pairs with continuous surfaces for each of the two distinct contact regions; and • specifying general contact, which filters out nearly all unintended initial overclosures. Interpreted as a penetration for a single contact pair with discontinuous surfaces B A Slave Master Slave Master Figure 38.1.2–1 Example of an unintended initial overclosure due to a modeling error involving discontinuous surfaces. Overclosures on three-dimensional surfaces The cause of unintended initial overclosures may be less obvious for three-dimensional models with complex surfaces. The most important step in overcoming this problem is identifying which regions of respective surfaces are involved in an unintended initial overclosure. For a surface-to-surface contact pair without strain-free adjustments, a portion of the master surface should be apparent behind the slave surface (opposite the slave surface normal direction) at a distance consistent with the reported (negative) COPEN value. For a node-to-surface contact pair, the direction to the interaction point on the master surface typically corresponds to a local minimum distance between the slave and master surfaces. Resolving large interference fits As previously discussed, Abaqus/Standard optionally interprets initial overclosures as interference fits. You should use one of the methods discussed above to remove any initial overclosures that are an unintended result of mesh discretization or errors in defining contact surfaces. In some cases the interference fit may be intended but may be too large to be resolved robustly with the method that is used by default for contact pairs in Abaqus/Standard (which is to resolve overclosures in a single increment). In this situation you should modify the contact model to allow resolution of overclosures over multiple increments . If you choose to have initial overclosures treated as interference fits for general contact, they are automatically resolved over multiple increments . Preventing rigid body motion in contact simulations Rigid body motion is generally not a problem in dynamic analysis. In static problems rigid body motion occurs when a body is not sufficiently restrained. “Numerical singularity” warning messages and very large displacements indicate unconstrained motion in a static analysis. Therefore, if contact is used to constrain rigid body motion in static problems, ensure that the appropriate surface pairs are initially in contact . If necessary, define the model geometry to give a small initial overclosure to the contact pair, or use boundary conditions to move the structures into contact in the first step. The boundary conditions, which are unnecessary in subsequent steps, can be removed after the body is adequately constrained through contact with other components. Similarly, if a rigid body is meant to translate only, constrain its rotational degrees of freedom. Frictional sticking can constrain rigid body motion. However, contact pressure must develop before friction can be generated. Therefore, friction is not effective in constraining rigid body motion when surfaces first come into contact. You must temporarily eliminate rigid body motion by defining a boundary condition or by grounding the body with soft springs or dashpots. If you are unable to prevent rigid body motion through modeling techniques, Abaqus/Standard offers some tools to automatically stabilize rigid bodies in contact simulations. These tools are discussed in “Automatic stabilization of rigid body motions in contact problems” in “Adjusting contact controls in Abaqus/Standard,” Section 35.3.6. Poorly defined surfaces Over the course of an analysis, you may notice undesirable behavior between contact surfaces (excessive penetration, unexpected openings, inaccurate application of forces, etc.). This behavior often results in nonconvergence and termination of an analysis. These problems can arise from a number of causes related to mesh, element selection, and surface geometry. Defining duplicate nodes on the master surface When defining three-dimensional surfaces for use in finite-sliding applications, avoid defining two surface nodes with the same coordinates. Such a definition can give rise to a seam, or crack, in the surface as shown in Figure 38.1.2–2. Both vertices have the same coordinates. They are separated to show the crack in the surface. Figure 38.1.2–2 Example of doubly defined surface node. If viewed with the default plotting options in Abaqus/CAE, this surface will appear to be a valid, continuous surface; however, if this surface is used as the master surface for finite-sliding, node-to-surface contact, a slave node sliding along the surface may fall through this crack and get “stuck” behind the master surface. Similar problems can occur for finite-sliding, surface-to-surface contact. Typically, convergence problems will result that may cause Abaqus/Standard to terminate the analysis. Use the edge display options in the Visualization module of Abaqus/CAE to identify any unwanted cracks in the surfaces used in the model. The cracks will appear as extra perimeter lines in the interior of the surface. Duplicate nodes can be avoided easily by equivalencing nodes when creating the model in a preprocessor. Avoiding problems with contact along the perimeters of surfaces When modeling finite-sliding contact, ensure that the master surface definition extends far enough to account for all expected motions of the contacting parts. Contact along the perimeter of master surfaces should be avoided with the node-to-surface contact formulation.. Abaqus/Standard assumes that the mating slave surface nodes can fall off the free edge of the master surface, which can cause problems if a slave node wraps around and approaches its mating master surface from behind. Figure 38.1.2–3 illustrates appropriate and inappropriate master surface definitions. trimmed master surface slave surface untrimmed master surface Inappropriate master surface definition Appropriate master surface definition Figure 38.1.2–3 Example of master surface extension. A slave node that falls off a master surface in one iteration may find itself contacting the surface in the very next iteration; this phenomenon is known as chattering. If chattering continues, Abaqus/Standard may not be able to find a solution. This problem is less likely with the surface-to-surface formulation approach, because each contact constraint is based on a region of the slave surface rather than individual slave nodes. Request detailed contact printout to the message (.msg) file to monitor the history of a slave node that might slide off the master surface . The message file output will show the cyclic opening and closing of contact at a slave node, which will indicate where the master surface needs to be modified. For node-to-surface contact you can extend the master surface beyond the perimeter of the physical body that it approximates to avoid chattering problems. Chattering can also occur with some contact elements, such as slide line and rigid surface contact elements. Slide line contact elements can also be extended. See “Extending master surfaces and slide lines,” Section 35.3.8, for details. Falling off small-sliding master surfaces Falling off the edge of a master surface in small-sliding contact problems is not an issue since slave nodes do not slide on the actual surface of the model. Instead, each slave node interacts with a flat, infinite contact plane. This plane is associated with the set of master surface nodes that are closest to the slave node in the undeformed configuration. For details about small-sliding contact, see “Contact formulations in Abaqus/Standard,” Section 37.1.1. Falling off surfaces modeled with interface elements Falling off the edge of a surface modeled with interface elements is not an issue since the slave nodes slide on a flat, infinite contact plane. Using poorly meshed surfaces Several problems are caused by surfaces created on very coarse meshes. Some of these problems depend on your choice of contact discretization, as discussed later in “Discrepancies between contact formulations.” Penetrations with coarsely meshed slave surfaces When a coarsely meshed surface is used as a slave surface for node-to-surface contact, the master surface nodes can grossly penetrate the slave surface without resistance . This situation is common when nonmatching meshes come into contact. Refining the slave surface tends to alleviate this problem. slave nodes cannot penetrate master segments master surface (segments) penetration slave surface (nodes) gap master node can penetrate slave segment Figure 38.1.2–4 Master surface penetrations into the slave surface due to a coarse mesh of the slave surface for node-to-surface contact. Surface-to-surface contact will generally resist penetrations of master nodes into a coarse slave surface; however, this formulation can add significant computational expense if the slave mesh is significantly coarser than the master mesh . Contact occurring at a single element If the mesh on a surface is too coarse, it is possible for a contact interaction to occur entirely within the bounds of a single element. This typically happens when the two contacting surfaces have dissimilar curvature, as depicted in Figure 38.1.2–5. Master surface Slave surface Figure 38.1.2–5 The master surface contacts the slave surface at a single element face. The results from such an interaction are unreliable and generally unrealistic. If the model in Figure 38.1.2–5 uses node-to-surface contact, the master surface penetrates the slave surface without resistance until it encounters a slave node, as discussed above. If the master and slave designations are reversed, the contact constraint is applied at a single slave node; this concentration creates inaccurately high calculations of the contact pressure. If the model uses surface-to-surface contact, excessive penetration is not likely to occur. However, with only a small number of constraint points involved in the interaction, the averaging algorithm used to enforce surface-to-surface contact performs poorly. Inaccurate contact stress and pressure calculations result. If contact is occurring at a single element, refine the mesh to spread the interaction across multiple element faces. Coarsely meshed master surfaces and small-sliding contact Coarsely meshed, curved master surfaces in small-sliding simulations can lead to unacceptable solution accuracy due to the approximate nature of the “master planes.” Using a more refined mesh to define the master surface will improve the overall accuracy of the solution in small-sliding problems. However, unless perfectly matching meshes are used, local oscillations in the contact stress may still be observed, even in refined models. Nonmatched surface meshes with second-order heat transfer elements Inaccurate local results may occur if second-order heat transfer elements are used to model a thermal interface and the meshes do not match across the surfaces. The worst results will be obtained when the midside node of an element on one surface is closest to the corner node of an element on the other surface. If a nonmatching mesh must be used in the model, use first-order elements or use a more refined mesh. Three-dimensional surfaces with second-order faces and a node-to-surface formulation Second-order elements not only provide higher accuracy but also capture stress concentrations more effectively and are better for modeling geometric features than first-order elements. Surfaces based on second-order element types work well with the surface-to-surface contact formulation but, in some cases, do not work well with the node-to-surface formulation . Some second-order element types are not well-suited for underlying the slave surface with the combination of a node-to-surface contact formulation and strict enforcement of “hard” contact conditions, because of the distribution of equivalent nodal forces when a pressure acts on the face of the element. As shown in Figure 38.1.2–6, a constant pressure applied to the face of a second-order element without a midface node produces forces at the corner nodes acting in the opposite sense of the pressure. q = pA r = pA 12 Figure 38.1.2–6 Equivalent nodal loads produced by a constant pressure on the second-order element face in “hard” contact simulations. Abaqus/Standard bases important decisions for the node-to-surface contact formulation on contact forces acting on individual slave nodes; the ambiguous nature of the nodal forces in second-order elements can cause Abaqus/Standard to make a wrong decision. To circumvent this problem, Abaqus/Standard automatically converts most three-dimensional second-order elements with no midface node (serendipity elements) that form a slave surface into elements with a midface node. For the three-dimensional 18- node gasket elements, the midface nodes are also generated automatically if they are not given in the element connectivity. The presence of the midface node results in a distribution of nodal forces that is not ambiguous for the contact algorithm. The element families C3D20(RH), C3D15(H), S8R5, and M3D8 are converted to the families C3D27(RH), C3D15V(H), S9R5, and M3D9, respectively. Since Abaqus/Standard does not convert second-order coupled temperature-displacement, coupled thermal-electrical-structural, and coupled pore pressure–displacement elements, you should specify a penalty or augmented Lagrange constraint enforcement method to approximate hard pressure-overclosure behavior . Abaqus/Standard will interpolate nodal quantities, such as temperature and field variables, at the automatically generated midface nodes when values are prescribed at any of the user-defined nodes. Second-order tetrahedral elements (C3D10 and C3D10I) have zero contact force at their corner nodes. This combination of second-order triangular slave facets, a node-to-surface contact formulation, and strict enforcement of “hard” contact conditions is disallowed to avoid a high likelihood of convergence problems and poor predictions of contact pressures that would occur with this combination. To avoid this combination, use at least one of the following alternatives: • Use the surface-to-surface contact formulation (generally recommended) instead of the node-to- surface contact formulation; • Use the penalty constraint enforcement method (generally recommended) or augmented Lagrange constraint enforcement method instead of strict enforcement of “hard” contact conditions; or • Use modified 10-node tetrahedral elements (C3D10M) instead of second-order tetrahedral elements. Excessive iterations in contact simulations Abaqus/Standard offers a number of methods to adjust the solver iteration scheme, sometimes resulting in a more efficient analysis with a minimal effect on accuracy. Converting severe discontinuity iterations in weakly determined contact conditions By default, Abaqus/Standard continues to iterate until the severe discontinuities associated with changes in contact status are sufficiently small (or no severe discontinuities occur) and the equilibrium (flux) tolerances are satisfied. Alternatively, you can choose a different approach in which Abaqus/Standard continues to iterate until no severe discontinuities occur. These two approaches are discussed in more detail in “Severe discontinuities in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2. The default treatment of severe discontinuity iterations reduces the likelihood of excessive iterations associated with chattering between contact states when the contact conditions are weakly determined. An example of a region with weakly determined contact conditions is near the center of a flat punch that contacts a thin plate supported at its edges. Controlling the increment size based on penetration distance in unconverged iterations For most types of contact, if during an iteration the penetration calculated for any contact pair exceeds a specific distance ( ), Abaqus/Standard abandons the increment and tries again with a smaller increment size. There is no critical penetration distance for finite-sliding, surface-to-surface contact (including general contact) and for small-sliding contact in geometrically linear analyses. The default value of is the radius of a sphere that circumscribes a characteristic surface element face. When calculating the default value, Abaqus/Standard uses only the slave surface of the contact pair. for each contact pair in the model is printed in the data (.dat) file. While the default The value of value of should prove to be sufficient for the majority of contact simulations, in some cases it may be necessary to change the default value for a given contact pair. These cases include: • Models in which the master surface is highly curved. The default value of may sometimes lead to situations as shown in Figure 38.1.2–7. During the iterative solution process a slave node initially at point a may move to point b, penetrating the master surface with overclosure h less than . Abaqus/Standard may attempt to move the slave node to point c on the master surface. To avoid this situation, specify a smaller value for to force Abaqus/Standard to abandon the increment and to try a smaller increment size. crit S Slave node M Master surface a-b-c Trajectory of slave node Figure 38.1.2–7 Effect of the critical penetration distance on a highly curved master surface. • Models in which Abaqus/Standard cannot calculate a reasonable because a node-based surface is used. If there are other contact pairs in the model with surfaces, Abaqus/Standard uses the average dimension of all of the slave surface element faces. If there are no other contact pairs, Abaqus/Standard uses a characteristic element dimension of the entire model. • Models in which the contact face dimensions in a slave surface vary greatly. • Models in which the slave surface mesh is very refined compared with the typical surface dimensions so that overclosures much larger than the default can be resolved easily. • Models in which contact pairs with softened contact allow significant penetration . Input File Usage: Abaqus/CAE Usage: *CONTACT PAIR, HCRIT= You cannot adjust the default value of in Abaqus/CAE. Difficulties interpreting the results of contact simulations Although an analysis involving contact runs to completion, the results may seem unrealistic. This is sometimes due to modeling errors and sometimes due to the specialized output format of certain contact formulations. In addition to degrading contact output, the factors discussed below also tend to degrade convergence behavior, so avoiding these factors may improve convergence behavior. Oscillating contact pressures when using second-order elements in “hard” contact simulations Nonuniform contact pressure distributions are likely to occur when very different mesh densities are used on the two deformable surfaces making up a contact interaction. The nonuniformity can be particularly pronounced when “hard” contact is modeled and both surfaces are modeled with second-order elements, including modified, second-order tetrahedral elements. In such cases oscillations and “spikes” in the contact pressure may occur. Smoother contact pressures may be obtained for surfaces modeled with second-order elements by using penalty-type contact constraint enforcement . Inaccurate contact stresses when using second-order axisymmetric elements at the symmetry axis For second-order axisymmetric elements the contact area is zero at a node lying on the symmetry axis . To avoid numerical singularity problems caused by a zero contact area, Abaqus/Standard calculates the contact area as if the node were a small distance from the symmetry axis. This may result in inaccurate local contact stresses calculated for nodes located on the symmetry axis. Self-contact Contact of a surface with itself (self-contact) is provided for cases in which the original geometry is very different from the (deformed) geometry at which contact takes place. It would then be difficult for you to predict which parts of the surface will come into contact with each other. Where possible, it is always computationally more economical to declare parts of the surface as master and parts as slave. The same unpredictability makes it impossible to determine a priori which side will be the master and which side the slave. Therefore, Abaqus/Standard uses a symmetric contact model: every single node of the surface can be a slave node and can simultaneously belong to master segments with respect to all other nodes. Because each surface is acting as both a slave and a master, the results of symmetric contact analyses can be confusing and inconsistent. These difficulties are discussed more fully in “Using symmetric master-slave contact pairs to improve contact modeling” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1. Overconstraining the model The term overconstraint refers to a situation in which multiple kinematic constraints outnumber the degrees of freedom on which they act. Overconstraints often lead to inaccurate solutions or failure to obtain a converged solution. Contact conditions strictly enforced with the direct constraint enforcement method (using Lagrange multipliers) are sometimes involved in overconstraints. See “Overconstraint checks,” Section 34.6.1, for a detailed discussion and examples of overconstraints and how Abaqus/Standard will treat overconstraints based on the following classifications: • Overconstraints detected in the model preprocessor • Overconstraints detected and resolved during analysis • Overconstraints detected in the equation solver Abaqus/Standard will automatically resolve many types of overconstraints; however, many overconstraints involving contact cannot be resolved and will be exposed to the equation solver. The equation solver will often issue “zero pivot” or “numerical singularity” warning messages as a result of overconstraints; when this occurs, Abaqus/Standard will provide a warning message with information that is helpful for determining what contributed to the overconstraint so that you can resolve it. Occasionally overconstraints do not create warning messages; this does not necessarily mean that the overconstraints have not adversely affected the analysis. Overconstraints involving softened contact Contact conditions with a softened behavior or enforced with the penalty or augmented Lagrange method will not combine with other constraints to cause “strict overconstraints”; however, “softened overconstraints” can: • cause zero pivots or ill-conditioning in the equation solver if the stiffness contributions associated with contact are many orders of magnitude higher than the stiffness contributions from typical elements; • prevent a tight penetration tolerance from being achieved with the augmented Lagrange method; and • cause oscillations in contact stress solutions, particularly if the contact stiffness is high. Some types of contact use the penalty or augmented Lagrange method by default to approximate hard pressure-overclosure behavior due to the prevalence of redundant or “competing” contact conditions. For a discussion of available constraint enforcement methods and default behavior, see “Contact constraint enforcement methods in Abaqus/Standard,” Section 37.1.2. Inaccurate contact forces due to overconstraints If nodes in a contact pair are overconstrained but the equation solver does find a solution, the contact forces become indeterminate and may become excessively high, particularly in tied contact pairs. Check the time average force (or moment, or flux) reported in the message file, or use Abaqus/CAE to view the diagnostic information interactively (for more information, see Chapter 41, “Viewing diagnostic output,” of the Abaqus/CAE User’s Manual). If it is many orders of magnitude larger than the residual forces (or moments, or fluxes), an overconstraint may have occurred, and there is no guarantee that Abaqus/Standard has found the correct solution. Another sign that the model is overconstrained is that the analysis begins to converge in a single iteration in every increment when the nonlinearities should require at least several iterations. Overconstraints should be avoided only by changing the contact definition or other constraint type involved. Overconstraints due to multiple surface interaction definitions at a single node Automatic resolution of contact overconstraints sometimes depends on whether two contact pairs refer to the same surface interaction definition. For example, consider a case in which two contact pairs have a common master surface and share some slave nodes (perhaps along a common edge of two slave surfaces). Overconstraints will occur at the common slave nodes if the two contact pairs refer to different surface interaction definitions (even if the surface interactions are equivalent); however, Abaqus/Standard automatically avoids these overconstraints if the two contact pairs refer to the same surface interaction definition. Discrepancies between contact formulations The different contact formulations available in Abaqus/Standard allow for a great deal of flexibility when modeling contact simulations. However, two nearly identical simulations that differ only in the contact formulation being used will sometimes generate varying results. This is primarily because of the different ways that contact formulations interpret contact conditions. Certain formulations are better suited to particular situations. Differences in penetrations The most observable difference between node-to-surface and surface-to-surface discretization is the amount of penetration that occurs between surfaces. This is because node-to-surface discretization computes penetrations only at slave nodes, while surface-to-surface discretization computes penetrations in an average sense over a finite region. For example, when a slave surface slides across a convex portion of a master surface, the slave surface will tend to ride a bit higher with surface-to-surface discretization than with node-to-surface discretization, as shown in Figure 38.1.2–8 (the opposite is true at a concave portion of a master surface). Figure 38.1.2–9 shows another case in which the two contact discretizations behave fundamentally differently due to the different approaches to computing penetrations. Both discretizations converge to the same behavior as the mesh is refined. The differences in computed penetrations can sometimes fundamentally affect the results of an analysis. Be aware of this possibility when converting models from one contact formulation to another. Various aspects of preexisting models, such as the friction coefficient or the pressure-overclosure relationship, may have been inadvertently “tuned” to the behavior that occurs with a particular contact formulation. Contact at a single point Figure 38.1.2–10 shows an example in which a circular rigid body is pushed into a deformable body. In the initial configuration shown, the two bodies touch at a single point, which corresponds to a slave node location. The following scenarios are likely for respective analyses of this model with node-to-surface and surface-to-surface discretization: Figure 38.1.2–8 Comparison of contact discretizations in an example with convex curvature in the master surface (forming application). master surface Constraints based on "averaged" penetration master surface Constraints based on slave nodes penetration slave surface Figure 38.1.2–9 Comparison of contact discretizations in an example with a relatively flexible slave surface wrapping around a corner of a master surface. • With node-to-surface discretization, the first iteration is performed with one active contact constraint. A converged solution is obtained with a reasonable number of iterations and increments. Figure 38.1.2–10 Example with two bodies initially touching at a single point. • With surface-to-surface discretization, penetrations are computed in an average sense over finite regions of the surface, so a positive gap distance is computed for all potential contact constraints even though the surfaces touch at one of the slave nodes. However, the finite-sliding, surface-to-surface contact formulation detects that the surfaces are initially touching and by default automatically activates localized contact damping in the neighborhood where the gap distance is zero. Without such damping, Abaqus/Standard may not obtain a converged solution due to an unconstrained rigid body mode. This contact damping typically has an insignificant effect on the converged solution, and the damping is completely removed by the end of the step. If you deactivate the automatic localized damping for surface-to-surface formulation—or if you are using the small-sliding, surface-to-surface formulation—you should use one of the techniques discussed above in “Difficulties resolving initial contact conditions” to remove the perceived initial gap between surfaces and prevent rigid body modes in the analysis. the finite-sliding, Input File Usage: Abaqus/CAE Usage: Use the following option to deactivate automatic localized contact damping at artificial surface gaps for contact pair definitions: *CONTACT PAIR, MINIMUM DISTANCE=NO Use the following option to deactivate automatic localized contact damping at artificial surface gaps for general contact definitions: *CONTACT INITIALIZATION DATA, MINIMUM DISTANCE=NO You cannot deactivate automatic localized contact damping at artificial surface gaps in Abaqus/CAE. Differences in contact normal direction Node-to-surface discretization uses a contact normal direction based on the master surface normal, whereas surface-to-surface discretization uses a contact normal direction based on the slave surface normal (averaged over a region nearby the slave node). For most active contact definitions the slave and master surfaces are nearly parallel, so the master and slave normals are approximately aligned; in which case this distinction in how the contact normal is determined is not significant. However, in some cases the differences in the contact normal can be significant. • When modeling large interference fits, surface-to-surface discretization can sometimes cause tangential motion of the slave surface as the overclosures are resolved. This tangential motion may have undesirable effects on an analysis. See “Controlling initial contact status in Abaqus/Standard,” Section 35.2.4, and “Modeling contact interference fits in Abaqus/Standard,” Section 35.3.4, for more details. • Contact constraints involving geometric edges of surfaces sometimes use a significantly different contact normal depending on which contact discretization approach is used, because the normals for the slave and master surfaces may not directly oppose each other. • The contact opening distance output variable (COPEN) can vary considerably depending on what type of contact formulation is used if the contact surfaces are not parallel. For node-to-surface discretization, the opening distance that is reported approximates the closest distance to the master surface; for surface-to-surface discretization, the opening distance that is reported corresponds to the distance from the slave surface to the master surface along the slave normal direction. The opening distance for surface-to-surface discretization is undefined if a line emanating from the slave surface in the slave normal direction does not intersect the master surface (as discussed in “Using the small-sliding tracking approach” in “Contact formulations in Abaqus/Standard,” Section 37.1.1, if a small-sliding constraint cannot be formed in such a case for the small-sliding, surface-to-surface formulation, Abaqus/Standard automatically reverts to the node-to-surface approach for individual constraints). Contact at corners The finite-sliding, surface-to-surface formulation is often better-suited than other contact formulations for modeling contact near corners. In the example shown in Figure 38.1.2–11, the slave surface is on the “outer” body (i.e., the body with a reentrant corner). With node-to-surface discretization a single constraint acts at the corner slave node in the “average” normal direction of the master surface, which often leads to poor resolution of contact, non-physical response, and even early termination of an analysis. However, surface-to-surface discretization generates two constraints near the corner for the respective faces, as shown in Figure 38.1.2–11, resulting in more stable contact behavior. Figure 38.1.2–11 Comparison of contact formulations in an example with abutting surfaces having respective interior and exterior corners. 38.2 Resolving contact difficulties in Abaqus/Explicit • “Contact diagnostics in an Abaqus/Explicit analysis,” Section 38.2.1 • “Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit,” Section 38.2.2 38.2.1 CONTACT DIAGNOSTICS IN AN Abaqus/Explicit ANALYSIS Products: Abaqus/Explicit Abaqus/CAE References • “Output to the data and results files,” Section 4.1.2 • “Contact interaction analysis: overview,” Section 35.1.1 • *DIAGNOSTICS • Chapter 41, “Viewing diagnostic output,” of the Abaqus/CAE User’s Manual Overview Contact diagnostics in Abaqus/Explicit allow you to get detailed information about the surfaces and progress of contact interactions. Diagnostics are available: • to review automatic adjustments between two surfaces, • to reveal potentially problematic initial surface configurations in a model, • to track excessive penetrations between two contacting surfaces, and • to review warnings associated with contact between warped surfaces. Reviewing the adjustments of initially overclosed surfaces Contacting surfaces that are overclosed in the initial configuration of the model are adjusted automatically by Abaqus/Explicit to remove the overclosures . There are three sources of information on the adjustments of overclosed surfaces: the status (.sta) file, the message (.msg) file, and the output database (.odb) file. Obtaining the adjustments of overclosed surfaces in the status and message files By default, Abaqus/Explicit writes all nodal adjustments and—for general contact surfaces—contact offsets to the message (.msg) file along with a summary listing of the maximum initial overclosure and the maximum nodal adjustment to the status (.sta) file for the contact pairs defined in the first step of a simulation. You can choose to suppress the information written to the message file and write only the summary information to the status file. The information written to the message and status files is also written to the output database (.odb) for use in Abaqus/CAE. Input File Usage: Use the following option to obtain both detailed diagnostic output to the message file and summary diagnostic output to the status file: *DIAGNOSTICS, CONTACT INITIAL OVERCLOSURE=DETAIL (default) Abaqus/CAE Usage: Use the following option to obtain only summary diagnostic output to the status file (no contact diagnostics will be written to the message file): *DIAGNOSTICS, CONTACT INITIAL OVERCLOSURE=SUMMARY You cannot control the diagnostic information for contact initial overclosures from within Abaqus/CAE. Use the following option to view the saved diagnostic information: Visualization module: Tools→Job Diagnostics Viewing the adjustments of surfaces In the first step the adjustments of initially overclosed surfaces can be viewed in Abaqus/CAE. Displaced shape plots that show the adjustments to the contact pairs defined in the first step can be plotted for the original field output frame at zero time. In the case of overclosures in steps other than the first, vector plots of nodal displacements and accelerations can be particularly helpful in visualizing the adjustments. Such plots can be viewed in Abaqus/CAE after a data check analysis . Visualizing the precise initial clearances for small-sliding contact pairs Abaqus/Explicit does not adjust the coordinates of the slave surface when precise initial clearances are specified for small-sliding contact pairs . Therefore, the specified clearances cannot be seen in a postprocessor such as the Visualization module of Abaqus/CAE. Thus, depending on the initial geometry of the surfaces and the magnitude of the clearances or overclosures, the surfaces may appear open or closed in the postprocessor when they are actually just in contact in the simulation. Detecting crossed surfaces in a general contact domain If a slave surface initially penetrates a double-sided master surface by a distance greater than the master surface’s thickness, the severely overclosed slave nodes will see the back side of the master surface as the appropriate contact force direction. These slave nodes in these crossed surfaces effectively become trapped behind the master surface. This issue is discussed in more detail in “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 35.4.4, and “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 35.5.4. For general contact definitions, diagnostic testing that identifies regions in which surfaces are crossed in the initial configuration is activated by default. When the diagnostic tests are activated, a warning message is issued to the message (.msg) file if two adjacent slave nodes (connected by a facet edge) are detected on opposite sides of a master surface. No such warning is issued for node-based surface nodes on opposite sides of a master surface, because adjacency cannot be determined among the node-based surface nodes. In some cases involving corners of master surfaces this warning message may be issued even though adjacent slave nodes are really on the same side of a master surface. The CPU cost of performing diagnostic testing on large models is potentially significant. You can choose to deactivate the diagnostic testing and avoid the extra CPU cost in such cases. Input File Usage: Use the following option to deactivate diagnostic testing for initially crossed surfaces: Abaqus/CAE Usage: *DIAGNOSTICS, DETECT CROSSED SURFACES=OFF You cannot exclude diagnostic testing for initially crossed surfaces from within Abaqus/CAE. Use the following option to view the saved diagnostic information: Visualization module: Tools→Job Diagnostics Excessive penetrations between general contact surfaces As described in “Contact constraint enforcement methods in Abaqus/Explicit,” Section 37.2.3, the penalty constraint enforcement method used by the general contact algorithm in Abaqus/Explicit allows slight penetrations of one surface into another surface. A “spring” stiffness is applied automatically to the surfaces to resist these penetrations. If the nodes involved in general contact do not have adequate mass, the default “spring” stiffness chosen automatically by Abaqus/Explicit may not be sufficient to prevent large penetrations. Such a situation can arise, for example, when a cloud of massless nodes, fully constrained by a kinematic coupling definition, contacts a fully constrained rigid face with no mass. By default, if during node-to-face contact, the penetration of a node into its tracked face exceeds 50% of the typical face dimension in the general contact domain, the penetration is regarded as excessive and Abaqus/Explicit issues a diagnostic message to the status (.sta) file. A node set containing deeply penetrated nodes is also written to the output database (.odb) file for use in Abaqus/CAE. You can control the fraction of the typical face dimension used to trigger the diagnostic message. Input File Usage: Use the following option to control the fraction of the typical element face dimension used to trigger the diagnostic message for deep penetrations: Abaqus/CAE Usage: *DIAGNOSTICS, DEEP PENETRATION FACTOR=value You cannot control the diagnostic information for deep penetrations from within Abaqus/CAE. Use the following option to view the saved diagnostic information: Visualization module: Tools→Job Diagnostics Warning messages for highly warped surfaces Calculating the correct contact conditions along a surface that is highly warped is very difficult, and Abaqus/Explicit employs a specialized algorithm to enforce contact between warped surfaces; this specialized algorithm is more expensive than the default contact algorithm . By default, Abaqus/Explicit checks for highly warped surfaces every 20 increments. Abaqus/Explicit writes a warning message in the status (.sta) file the first time that it detects that a surface is highly warped. The message is brief; it states only which surface has a highly warped facet. If additional facets on this surface become highly warped later in the analysis, no additional warning messages are issued. You can request more detailed diagnostic warning messages, if desired. In this case the message file will contain a warning every time a warped facet is found on a particular surface. The warnings will give the parent element associated with the warped facet (the parent element is the element whose face forms the facet) and the warping angle of the facet. The computation time and the size of the message file can increase significantly if detailed warnings are requested. You can switch back to the summary warnings in subsequent steps or suppress the warped surface warnings entirely. If the analysis terminates with a fatal error, the preselected output variables will be added automatically to the output database as field data for the last increment. Input File Usage: Use the following option to request detailed diagnostic warning output for warped surfaces: *DIAGNOSTICS, WARPED SURFACE=DETAIL Use the following option to request the default summary diagnostic output for warped surfaces: *DIAGNOSTICS, WARPED SURFACE=SUMMARY Use the following option to suppress diagnostic warning output for warped surfaces entirely: *DIAGNOSTICS, WARPED SURFACE=OFF Diagnostic output Abaqus/CAE. requests for warped surfaces are not supported in Abaqus/CAE Usage: 38.2.2 COMMON DIFFICULTIES ASSOCIATED WITH CONTACT MODELING USING CONTACT PAIRS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Defining contact pairs in Abaqus/Explicit,” Section 35.5.1 • *CONSTRAINT CONTROLS • *CONTACT PAIR Overview This section highlights the difficulties that are most commonly encountered when modeling contact interactions with contact pairs in Abaqus/Explicit. Most of these issues are not relevant when the general contact algorithm is used; refer to “Defining general contact interactions in Abaqus/Explicit,” interactions. Section 35.4.1, Recommendations on how to circumvent these problems are presented. for more information on the issues involved with general contact Defining duplicate nodes on the master surface When defining three-dimensional surfaces formed by element faces, avoid defining two surface nodes with the same coordinates. Such a definition can give rise to a seam, or crack, in the surface as shown in Figure 38.2.2–1. Both vertices have the same coordinates. They are separated to show the crack in the surface. Figure 38.2.2–1 Example of doubly defined surface node. If viewed with the default plotting options in Abaqus/CAE, this surface will appear to be a valid, continuous surface; however, a node sliding along this surface can fall through this crack and violate the contact conditions. If this were to happen, Abaqus/Explicit would enforce the contact conditions by applying a large acceleration to the node once overclosure is detected. The large resulting acceleration may create a noisy solution or cause the elements to distort badly. Use the edge display options in the Visualization module of Abaqus/CAE to identify any unwanted cracks in the surfaces used in the model. The cracks will appear as extra perimeter lines in the interior of the surface. Duplicate nodes can be avoided easily by equivalencing nodes when creating the model in a preprocessor. Using an inadequate surface definition for the desired contact conditions Occasionally, surface definitions may not be suitable for modeling the desired contact conditions in a problem. Figure 38.2.2–2 shows a two-dimensional model of a simple connection between two parts. surface 1 surface 2 surface 3 contact pair 1 = surface 1, surface 3 contact pair 2 = surface 2, surface 3 Analysis will stop after 1st increment with message that elements are badly distorted Figure 38.2.2–2 Surface definitions that are inadequate for the desired contact conditions. The surfaces shown in the figure are inadequate for the desired contact conditions that are also shown. At the start of the simulation, Abaqus/Explicit will detect that some of the nodes on surface 3 are behind surfaces 1 and 2. When the contact conditions are enforced, the motions of the surfaces will likely cause badly distorted elements. One solution to this problem is shown in Figure 38.2.2–3. surface 4 surface 5 contact pair = surface 4, surface 5 Figure 38.2.2–3 Surface definitions that are adequate for the desired contact conditions. The surfaces shown in that figure are suitable for the desired contact definition. Other solutions, such as using a pure master-slave contact pair, exist for this problem and may be more suitable, depending on the details of the intended simulation. Using poorly discretized surfaces Several problems are caused by surfaces created on very coarse meshes. Penetrations with coarsely discretized surfaces when using hard surface behavior When a coarsely discretized surface is used as the slave surface in a pure master-slave contact pair with hard surface behavior, an inaccurate solution may be produced as a result of the gross penetration of the master surface into the slave surface. This situation is shown in Figure 38.2.2–4. This problem can be minimized if the contact pair can be switched to a balanced master-slave contact pair. However, some contact pairs in Abaqus/Explicit must always use a pure master-slave formulation. In these cases the only solution to gross penetration is to refine the slave surface. Problems with coarsely discretized rigid surfaces For rigid surfaces formed by element faces, inaccurate results may be obtained if too few elements are used to represent a curved geometry. When a very coarse mesh is used on a curved geometry, it is possible for slave nodes to get “snagged” on the sharp vertices. In general, using a reasonable number of element faces to represent a curved surface will not increase the computational time of the simulations. However, a large number of element faces can significantly increase the memory that Abaqus/Explicit will need for the simulation. When a specific slave nodes cannot penetrate master segments master surface (segments) penetration slave surface (nodes) gap master node can penetrate slave segment Figure 38.2.2–4 Master surface penetrations into the slave surface due to coarse discretization. curved surface geometry can be modeled, using an analytical rigid surface may provide a more accurate geometric description while minimizing computational expense; see “Analytical rigid surface definition,” Section 2.3.4. Penalty contact behavior sensitivity in rigid-to-rigid interactions The contact penalties are, in general, determined from stable time increment considerations and masses of the nodes involved in contact. To compute a reliable contact penalty when rigid bodies are contacting each other, Abaqus/Explicit accounts in a comprehensive fashion for the inertial properties of the rigid bodies by distributing the mass of the rigid bodies at all nodes that might be involved in contact. Hence, the final contact penalty will depend on the size of the actual rigid surfaces that are included in the contact definitions. Consequently, the contact response (forces, penetrations) will depend somewhat on your choice in defining the contacting surfaces on the rigid bodies. If large penetrations occur, specifying realistic inertial properties for the rigid bodies will help in general to resolve the issue. Alternatively, you can use a scaling factor for the penalties to enforce contact in a more accurate fashion. Conflicts with boundary conditions If boundary constraints are applied to contact nodes on both surfaces of a contact pair in the direction that the contact constraints are active, the boundary constraints may override the contact constraints. For kinematic contact, contact force related quantities will be output as the force necessary to resolve the contact constraint in a single increment, causing misleading results for these output quantities if the boundary constraints violate the contact constraints. Contact force output for penalty contact does not show this behavior since the contact force is proportional only to the current penetration and does not depend on the time increment. Boundary constraints are not affected by contact constraints. Conflicts with multi-point constraints Using a multi-point constraint (MPC) with a node on a surface that is part of an active kinematic contact pair can generate conflicting kinematic constraints in the model. Abaqus/Explicit will not prevent you from using multi-point constraints on the nodes forming a surface. If the contact constraints and the constraints formed by the MPC are orthogonal, there will be no problems with the simulations. If they are not orthogonal, the solution may be noisy as Abaqus/Explicit tries to satisfy the conflicting constraints. Since within each increment kinematic contact constraints are applied after MPCs are applied, the MPCs on kinematic contact surfaces may be slightly out of compliance. In the case of an interaction between an MPC and penalty contact, the MPC is strictly enforced and any noncompliance in the contact pair will be resisted by penalty forces. Conflicting contact constraints on shell nodes with hard contact When a shell or membrane is pinched between two master surfaces using two kinematic contact pairs with hard contact behavior, one of the contact constraints will not be enforced exactly. In a quasi-static analysis it may be observed that the pinched slave node will oscillate about an “equilibrium” penetration depth with a decay rate that depends on the time increment and the ratio of the mass of the pinched node and the mass of the master surfaces. Decreasing the time increment size will increase the decay rate (quasi-static equilibrium will be reached more quickly). Reducing the mass of the nodes on the master surfaces (or increasing the mass of the pinched nodes) will also increase the decay rate, although a high ratio of slave mass to master mass can also lead to numerical difficulties for kinematic contact, as discussed below in “Large mass mismatch between contact surfaces.” Applying the loads to the model gradually will reduce the amplitude of the oscillation. In most analyses it is not desirable to alter the time increment or nodal masses arbitrarily, so the decay rate of the oscillation will be fixed. Either the loading rate can be modified or a softened contact model with contact damping can be used to control this oscillatory behavior. The quasi-static equilibrium penetration magnitude, , is approximately given by where f is the normal contact force, is the increment size, and m is the mass of the pinched node. The quasi-static equilibrium penetration will be minimal if it is small compared to the shell or membrane thickness. A change in the time increment size or loading on the pinched surfaces during the analysis causes the quasi-static equilibrium penetration to change, which can be responsible for large accelerations of surface nodes and can contribute to solution noise (typically, this behavior manifests as a jump in contact results such as CPRESS). Similar noisy behavior for pinched surfaces can occur across a step boundary, even if the time increment size is uniform across the step boundary. If one kinematic contact pair and one penalty contact pair are used to model the same type of pinching problem, the kinematic constraint is enforced exactly and the static value of the penetration in the penalty contact pair is somewhat larger than that which occurs when kinematic contact is used for both contact pairs (assuming that the penalty stiffness is set such that the analysis is numerically stable for the time increment being used). Multiple kinematic contact constraints on solid nodes If a node that is not attached to shell or membrane elements acts as a slave node in two or more simultaneous, kinematic contact constraints, the resulting contact corrections may be erroneous, possibly causing the analysis to abort with excessive element distortion. By “not attached to shell or membrane elements” we are referring to nodes attached to solid elements or point masses, for example. The majority of solid nodes typically are not involved in simultaneous contacts, but there are common exceptions where three or more bodies meet at corners. This limitation can be avoided by using penalty contact. For example, if a solid surface acts as a slave in two contact pairs and there is a possibility of simultaneous contacts for individual slave nodes, penalty enforcement of contact should be specified for one or both of the contact pairs. Redundant and degenerate contact constraints Redundant contact constraints are caused by overlapping or adjoining surfaces. For example, if contact is specified between a single surface and multiple overlapping surfaces, the contact constraints associated with the common nodes of the overlapping surfaces are redundant. Degenerate contact constraints occur if the slave surface and master surface of the same contact pair contain common nodes (a contact constraint cannot be formed between a node and itself). If redundant kinematic contact constraints are specified, Abaqus/Explicit will consolidate the constraints if both contact pairs use pure master-slave contact, the slave surfaces do not share facets, and the surface interaction and contact pair set names are identical. If the contact pair definitions differ, the analysis will terminate with an error, and one of the redundant constraints must be removed from the model definition to continue the analysis. Redundant penalty contact constraints may cause excessive initial overclosure adjustments, creating gaps in the place of initial overclosures. To correct this behavior, one of the constraints must be removed from the model definition. Redundant contact constraints involving both a penalty contact pair and a kinematic contact pair cause inefficiencies in the analysis. The kinematic contact constraints will override the penalty contact constraints, but the penalty contact constraints will still be considered in the automatic time increment estimate. If the surfaces in a two-surface contact pair contain common nodes, the contact constraint for each shared node cannot be generated. This is the equivalent of defining self-contact between the shared nodes and each surface. However, the two-surface contact logic (unlike the specialized self-contact logic) would erroneously detect contact between each shared node and itself. When this condition occurs, Abaqus/Explicit redefines the slave surfaces so that the shared nodes will not act as slave nodes in the contact pair. However, the shared nodes will still be used in the definition of a master surface in the contact pair. Large mass mismatch between contact surfaces Often very little mass is assigned to rigid bodies in quasi-static simulations because the mass has little influence on the physical problem. However, specifying a small rigid body mass can adversely affect the kinematic contact enforcement method. A force applied to a rigid body with very little mass can cause a large predicted displacement of the rigid body within an increment prior to the enforcement of contact constraints, so significant penetration may be present in the “predicted” configuration for kinematic contact, as shown in Figure 38.2.2–5. dpred tensile contact forces stretched (cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0) (cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0) (cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0)(cid:0) original configuration predicted configuration corrected configuration Figure 38.2.2–5 Undesirable numerical behavior of contact algorithm resulting from small rigid body mass. With hard kinematic contact each slave node that is penetrating its master surface in the predicted configuration will be brought to the position of its tracked point on the master surface in the corrected configuration, which, in this example, generates tensile contact forces at the outer slave nodes of the contact region. This undesirable effect can be avoided by increasing the mass of the rigid body, which will reduce the predicted displacement increment. A small rigid body mass can also adversely affect penalty enforcement of contact because small penalty stiffnesses will be assigned. Similar undesirable numerical behavior can occur for deformable-to-deformable contact if the nodal masses of the master nodes are orders of magnitude less than those of the slave nodes. This problem can often be avoided in such cases by using the pure master-slave algorithm with the master surface containing the more massive nodes. Contact noise associated with limited computer precision for hard contact is made for an initial overclosure, a penetration of up to Some contact noise may occur with hard contact models because of limited computer precision. This noise is rarely significant in an analysis, but it may be noticeable at the beginning of an analysis if initial displacements are used to make the mesh comply with contact constraints. For example, if an adjustment of may still exist in the first increment, where is the “machine epsilon” of the computer. The machine epsilon of a given computer is defined as the smallest positive number that can be added to 1 with the computed result being greater than 1; on most systems is approximately 6E−8 for single precision and 1E−16 for double precision. With the kinematic contact algorithm you can attribute initial accelerations of up to to limited machine precision, where =1E−6 sec, initial accelerations of up to 6E4 sec−2 can be attributed to limited machine precision. These accelerations is the time increment. For a single precision analysis in which are typically insignificant. They can be reduced by conducting the analysis with double precision or by specifying the nodal coordinates to be more compliant with contact constraints. Finite-sliding contact near a symmetry plane When a pure master-slave contact constraint with finite sliding is defined near a symmetry plane in the master surface, the corner slave node (node A in Figure 38.2.2–6) can, under some circumstances, slide freely along the symmetry plane without experiencing contact. If the master surface wraps around the corner (node 1), the slave node A may “track” on the master segment (1–6) on the symmetry plane, rather than on master segment (1–2). The result may be an inaccurate representation of the contact constraint as shown by the shaded area. symmetry plane 10 A0 B0 master surface slave surface Figure 38.2.2–6 Contact near a symmetry plane. The master surface is wrapped around the corner. If the master surface does not wrap around the corner (node 1 in Figure 38.2.2–7), the contact logic may give different results depending on how the symmetry boundary conditions have been defined for the master node 1 on the symmetry plane. If the symmetry boundary conditions on the master node are specified using boundary “type” format (i.e., XSYMM, YSYMM, or ZSYMM—see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1), the master surface is effectively extended beyond the symmetry plane (Figure 38.2.2–7); thus, the slave node A will be detected as a “penetrated” node (penetrated by distance a). Therefore, a correcting force would be applied on slave node A to push it below the master surface. symmetry plane XSYMM boundary condition A0 B0 master surface (extended) slave surface Figure 38.2.2–7 The master surface is extended across the symmetry plane because the symmetry boundary condition at node 1 is specified using boundary type XSYMM. If the symmetry boundary conditions on the master node 1 are specified using “direct” format (i.e., specifying the components of translations and rotations that are fixed), the master surface is not extended beyond the symmetry plane (Figure 38.2.2–8) and it is possible that contact will not be enforced correctly. To ensure proper enforcement of finite-sliding contact near symmetry planes, use balanced master- slave contact or use pure master-slave contact without extending the surface onto the symmetry plane and use symmetry “type” boundary conditions on the perimeter of the master surface nodes as discussed above. Special consideration of small-sliding contact near a symmetry plane is discussed in “Contact formulations for contact pairs in Abaqus/Explicit,” Section 37.2.2. Specifying initial clearance values precisely You can define initial clearances and contact directions precisely for the nodes on the slave surface . The initial clearance or overclosure value calculated at every slave node based on the coordinates of the slave node and the master surface is overwritten by the value that you specify; the coordinates of the slave nodes are not altered. This technique permits exact specification of initial clearances (and, possibly, contact directions) when they would not be computed accurately enough from the nodal coordinates; for example, if the symmetry plane Boundary conditions constraining degrees of freedom 1, 5, and 6 to 0.0 A0 master surface slave surface Figure 38.2.2–8 The master surface is not extended across the symmetry plane because the symmetry boundary conditions at node 1 are specified using direct format. initial clearance is very small compared to the coordinate values. It can be used only in small-sliding contact analyses (“Contact formulations for contact pairs in Abaqus/Explicit,” Section 37.2.2). When the balanced-master slave contact algorithm is invoked for the contact pair, the initial clearance values can be defined on one or both of the surfaces. Initial clearances defined on contact surfaces that act only as master surfaces will be ignored. Visualizing the precise initial clearances for small-sliding contact pairs Abaqus/Explicit does not adjust the coordinates of the slave surface when precise initial clearances are specified for small-sliding contact pairs . Therefore, the specified clearances cannot be seen in a postprocessor such as the Visualization module of Abaqus/CAE. Thus, depending on the initial geometry of the surfaces and the magnitude of the clearances or overclosures, the surfaces may appear open or closed in the postprocessor when they are actually just in contact. 39. Contact Elements in Abaqus/Standard Contact modeling with elements Gap contact elements Tube-to-tube contact elements Slide line contact elements Rigid surface contact elements 39.1 39.2 39.3 39.4 39.1 Contact modeling with elements • “Contact modeling with elements,” Section 39.1.1 39.1.1 CONTACT MODELING WITH ELEMENTS Abaqus/Standard offers a variety of contact elements that can be used when contact between two bodies cannot be simulated with the surface-based contact approach (Chapter 35, “Defining Contact Interactions”). These elements include the following: • Gap contact elements: Mechanical and thermal contact between two nodes is modeled with gap elements (“Gap contact elements,” Section 39.2.1). For example, these elements can be used to model the contact between a piping system and its supports. They can also be used to model an inextensible cable that supports only tensile loads. • Tube-to-tube contact elements: Contact between two pipes or tubes is modeled using tube-to-tube contact elements (“Tube-to-tube contact elements,” Section 39.3.1) in conjunction with slide lines. These elements can, for example, be used to simulate the process of running tubular components into an oil well (drill rod or J-tube analysis). They might also be used to simulate a catheter being inserted into a blood vessel. • Slide line contact elements: Finite-sliding contact between two axisymmetric structures that may undergo asymmetric deformations can be modeled using slide line contact elements (“Slide line contact elements,” Section 39.4.1) in conjunction with user-defined slide lines. Slide line elements can, for example, be used to model threaded connectors. • Rigid surface contact elements: Contact between an analytical rigid surface and an axisymmetric deformable body that may undergo asymmetric deformations can be modeled with rigid surface contact elements (“Rigid surface contact elements,” Section 39.5.1). For example, rigid surface contact elements might be used to model the contact between a rubber seal and a much stiffer structure. 39.2 Gap contact elements • “Gap contact elements,” Section 39.2.1 • “Gap element library,” Section 39.2.2 39.2.1 GAP CONTACT ELEMENTS Product: Abaqus/Standard References • “Gap element library,” Section 39.2.2 • *GAP Overview Gap elements: • allow for contact between two nodes; • allow for the nodes to be in contact (gap closed) or separated (gap open) with respect to particular directions and separation conditions; • are always defined in three dimensions but can also be used in two-dimensional and axisymmetric models; • allow contact to be defined on any type of element, including substructures and user-defined elements; • can be used to model contact in fixed or rotating directions; • can be used to model node-to-node contact and thermal interactions in a fixed direction in space in coupled temperature-displacement simulations; and • can be used to model node-to-node thermal interactions in heat transfer analyses. A general discussion of contact modeling in Abaqus/Standard can be found in Chapter 35, “Defining Contact Interactions.” Choosing and defining a gap element GAPUNI elements model contact between two nodes when the contact direction is fixed in space. GAPCYL elements model contact between two nodes when the contact direction is orthogonal to an axis. GAPSPHER elements model contact between two nodes when the contact direction is arbitrary in space. GAPUNIT elements model contact and thermal interactions between two nodes when the contact direction is fixed in space. DGAP elements model thermal interactions between two nodes in heat transfer analysis. Gap elements are defined by specifying the two nodes forming the gap and providing geometric data defining the initial state and, if necessary, the direction of the gap. Defining the gap element’s properties You must associate the gap behavior with a set of gap elements. Input File Usage: *GAP, ELSET=element_set_name GAPUNI and GAPUNIT elements The contact behavior of the interface being modeled with GAPUNI and GAPUNIT elements is defined by the initial separation distance (clearance), d, of the gap and the contact direction, . In addition, GAPUNIT elements have temperature degrees of freedom that allow modeling of thermal interactions in coupled temperature-displacement analyses. Clearance between GAPUNI nodes Abaqus/Standard defines the current clearance between two nodes of the gap, h, as and where are the total displacements at the first and the second node forming the GAPUNI element. Figure 39.2.1–1 shows the configuration of the GAPUNI element. When h becomes negative, the gap contact element is closed and the constraint is imposed. h = d + n · (u2 - u1) ≥ 0 Figure 39.2.1–1 GAPUNI and GAPUNIT contact elements. You specify a value for d. If you provide a positive value, the gap is open initially. If d=0, the gap is initially closed. If d is negative, the gap is considered overclosed at the start of the analysis and an initial interference fit problem is defined. Details about modeling interference fit problems with gap elements are discussed below. Input File Usage: *GAP Specifying the contact direction You can specify the contact direction. Otherwise, Abaqus/Standard will calculate the gap direction, by using the initial positions of the two nodes forming the element, and : , An error message is issued if In this situation you must define . The normal second, unless the gap is overclosed at the start of the analysis. In that case specify contact direction is used for the gap element. (if the two gap element nodes have the same initial coordinates). usually points from the first node of the element to the so that the correct If you specify the gap direction rather than allowing Abaqus/Standard to calculate it, the contact calculations consider only , the displacements of the gap element’s nodes, and the ordering of the nodes in the element definition: the initial coordinates of the nodes play no role in the calculations. The orientation of Input File Usage: does not change during the analysis. *GAP , X-direction cosine, Y-direction cosine, Z-direction cosine Local basis system for GAPUNI element output Abaqus/Standard reports the pressure transmitted across the gap and the shear stresses that are orthogonal to the contact direction as element output for GAPUNI elements. You must supply the contact area associated with these elements for Abaqus/Standard to compute the pressure and the shear stress values. It also reports the current clearance in the gap, h, and the relative motions of the GAPUNI nodes orthogonal to the contact direction. The relative motions and the shear stresses are reported in local surface directions that are formed using the standard Abaqus convention for defining directions on surfaces in space . The contact direction defines a surface in space on which the local axes are formed. Input File Usage: *GAP , , , , cross-sectional area GAPCYL elements GAPCYL elements can be used to model two very different contact situations: contact between two rigid tubes, where the smaller one is inside the larger tube, and contact between two rigid tubes along their external surfaces. Both cases are shown in Figure 39.2.1–2. The behavior of a GAPCYL element is defined by the initial separation distance between the nodes, d; the current positions of the element’s node; and the axis of the GAPCYL element. The axis of the GAPCYL element defines the plane in which the contact direction, , lies. You specify d and the direction cosines of the GAPCYL element axis. The value is not allowed: it would enforce the distance between the nodes to be exactly zero at all times, which does not correspond to a contact problem. Input File Usage: *GAP d, X-direction cosine, Y-direction cosine, Z-direction cosine Defining the gap clearance for Case 1 (when d is positive) If d is positive, the GAPCYL element models contact between two rigid tubes of different diameter, where the smaller tube is located inside the larger tube . In this case d is the maximum allowable separation. Each tube is represented by a node on its axis, with the axes connected by the GAPCYL element; and d corresponds to the difference between the radii of the tubes. Case 1 _ - x h = d - | x d = r2 - r1 _ | ≥ 0 Case 2 _ - x h = | x ) d = - (r1 + r2 _ | - | d | ≥ 0 Figure 39.2.1–2 Gap clearance for GAPCYL/GAPSPHER contact elements. The gap between the tubes closes when the two nodes become separated by more than d in any direction in the plane defined by the axis of the GAPCYL element. Abaqus/Standard defines the current gap opening, h, in GAPCYL elements for Case 1 as where GAPCYL element. is the current position of node N, d is the specified initial separation, and a is the axis of the If the initial position of the tube axes is such that the distance between them is less than d, the GAPCYL element is open initially. If the distance is equal to d, the element is closed initially; and if the distance is greater than d, an initial overclosure (interference) is defined. Details about modeling interference fit problems with gap elements are discussed below. Defining the gap clearance for Case 2 (when d is negative) If d is negative, the GAPCYL element models external contact between two parallel rigid cylinders . In this case is the minimum allowable separation of the nodes. Each cylinder is represented by a node on its axis connected by the GAPCYL element, and corresponds to the sum of the radii of the cylinders. The gap closes when the two nodes approach each other to within in any direction in the plane defined by the axis of the GAPCYL element. Abaqus/Standard defines the current gap opening, h, in GAPCYL elements for Case 2 as If the initial position of the cylinder axes is such that the distance between them is greater than , , the element is closed initially; and , an initial overclosure (interference) is defined. Details about modeling the GAPCYL element is open initially. If the distance is equal to if the distance is less than interference fit problems with gap elements are discussed below. Local basis system for GAPCYL element output Abaqus/Standard reports the pressure transmitted across the gap and the shear stresses that are orthogonal to the contact direction as element output for GAPCYL elements. You must supply the contact area associated with these elements for Abaqus/Standard to compute the pressure and the shear stress values. It also reports the current clearance in the gap, h, and the relative motions of the element’s nodes that are orthogonal to the contact direction. The relative motions and the shear stresses are reported in local surface directions that are formed using the standard Abaqus convention for defining directions on surfaces in space . The contact direction defines a surface in space on which the local axes are formed, and the slip is calculated from the relative motions in the surface directions. Abaqus/Standard updates the contact direction for GAPCYL elements based on the motion of the nodes forming the elements. However, the orientation of *GAP , , , , cross-sectional area Input File Usage: is not updated during the analysis. GAPSPHER elements GAPSPHER elements can be used to model two very different contact situations: contact between two rigid spheres where the smaller sphere is inside the larger, hollow sphere, and contact between two rigid spheres along their external surfaces. Both cases are shown in Figure 39.2.1–2. The behavior of a GAPSPHER element is defined by the minimum or maximum separation distance between the nodes, d, and the current positions of the element’s nodes. You specify the minimum or maximum separation distance, d. The contact direction is defined by the current position of the nodes. The value is not allowed: it would enforce the distance between the nodes to be exactly zero at all times, which does not correspond to a contact problem. Input File Usage: *GAP Defining the gap clearance for Case 1 (when d is positive) If d is positive, the GAPSPHER element models contact between a rigid sphere inside another (larger) hollow rigid sphere . In this case d is the maximum allowable separation of the nodes forming the gap. Each sphere is represented by a node at its center, with the centers connected by the GAPSPHER element; and d corresponds to the difference between the radii of the spheres. The gap closes when the two nodes become separated by more than d. Abaqus/Standard defines the current gap opening, h, for Case 1 as with the current position of node N and d the specified separation. If the initial position of the tube axes is such that the distance between them is less than d, the GAPSPHER element is open initially. If the distance is equal to d, the element is closed initially; and if the distance is greater than d, an initial overclosure (interference) is defined. Details about modeling interference fit problems with gap elements are discussed below. Defining the gap clearance for Case 2 (when d is negative) If d is negative, the GAPSPHER element models external contact between two rigid spheres . is the minimum allowable separation of the nodes forming the gap. Each sphere is represented by a node at its center connected by the GAPSPHER element; and corresponds to the sum of the radii of the spheres. The gap closes when the two nodes approach each In this case other to within . Abaqus/Standard defines the current gap opening, h, for Case 2 as If the initial position of the cylinder axes is such that the distance between them is greater than , , the element is closed initially; , an initial overclosure (interference) is defined. Details about modeling the GAPSPHER element is open initially. If the distance is equal to and if the distance is less than interference fit problems with gap elements are discussed below. Local basis system for GAPSPHER element output Abaqus/Standard reports the pressure transmitted across the gap and the shear stresses that are orthogonal to the contact direction as element output for GAPSPHER elements. You must supply the contact area associated with these elements for Abaqus/Standard to compute the pressure and the shear stress values. It also reports the current clearance in the gap, h, and the relative motions of the element’s node that are orthogonal to the contact direction. The relative motions and the shear stresses are reported in local surface directions that are formed using the standard Abaqus convention for defining directions on surfaces in space; see “Conventions,” Section 1.2.2. The contact direction defines a surface in space on which the local axes are formed, and the slip is calculated from the relative motions in the surface directions. Abaqus/Standard updates the contact direction for GAPSPHER elements based on the motion of the nodes forming the elements. *GAP , , , , cross-sectional area Input File Usage: DGAP elements DGAP elements are used to model thermal interactions between two nodes in heat transfer analyses. The behavior of the interaction being modeled is defined by the initial separation distance (clearance), d, of the gap. Clearance between DGAP nodes Abaqus/Standard defines the clearance between two nodes of the gap, h, as Since there are no displacements in a heat transfer analysis, the clearance remains unchanged. The clearance is used only for clearance-dependent thermal interactions. You specify a value for d. If you provide a positive value, the gap is open initially. If d=0, the gap is closed initially. If d is negative, the gap is considered overclosed but no interference fit is performed. The contact direction does not need to be specified: any contact direction specified is ignored in the analysis. You must supply the contact area associated with these elements for Abaqus/Standard to compute the heat flux value per unit area. Input File Usage: *GAP d, , , , cross-sectional area Defining nondefault mechanical interactions with gap elements The default mechanical interaction model for problems modeled with gap elements is “hard,” frictionless contact. You can assign optional mechanical interaction models. The following mechanical interaction models are available: • Friction. See “Frictional behavior,” Section 36.1.5, for details. • Modified “hard” contact, softened contact, and viscous damping. See “Contact pressure-overclosure relationships,” Section 36.1.2, and “Contact damping,” Section 36.1.3, for details. Defining thermal surface interactions with GAPUNIT and DGAP elements You can assign thermal interaction models to these elements. The following thermal interaction models are available: • Gap conduction. • Gap radiation. • Gap heat generation. These thermal interaction models are discussed in “Thermal contact properties,” Section 36.2.1. Modeling large initial interference with gap elements Specifying a large negative initial overclosure (interference) may lead to convergence problems as Abaqus/Standard tries to resolve the overclosure in a single increment. You can prescribe an allowable interference to allow Abaqus/Standard to resolve the overclosure gradually. See “Modeling contact interference fits in Abaqus/Standard,” Section 35.3.4, for more details on modeling interference fit problems. Input File Usage: *CONTACT INTERFERENCE, TYPE=ELEMENT 39.2.2 GAP ELEMENT LIBRARY Product: Abaqus/Standard References • “Gap contact elements,” Section 39.2.1 • *GAP Overview This section provides a reference to the gap elements available in Abaqus/Standard. Element types Stress/displacement elements GAPUNI Unidirectional gap between two nodes GAPCYL Cylindrical gap between two nodes GAPSPHER Spherical gap between two nodes Active degrees of freedom 1, 2, 3 Additional solution variables Three additional variables relating to the contact and friction forces. Coupled temperature-displacement element GAPUNIT Unidirectional gap and thermal interactions between two nodes Active degrees of freedom 1, 2, 3, 11 Additional solution variables Three additional variables relating to the contact and friction forces. Heat transfer element DGAP Thermal interactions between two nodes Active degree of freedom 11 Additional solution variables None. Nodal coordinates required For DGAP elements, and for GAPUNI and GAPUNIT if you specify the contact direction , the nodal coordinates are not used in the contact calculations; however, it is useful to define the coordinates of the two nodes for plotting purposes. GAPCYL and GAPSPHER: X, Y, Z Element property definition You can specify the initial clearance, the contact direction (normal to the interface), and the contact area. For GAPUNI, GAPUNIT, and DGAP elements, a negative clearance indicates an initial overclosure. For GAPCYL and GAPSPHER elements, specify the maximum separation as a positive number or the minimum separation as a negative number. Input File Usage: *GAP Element-based loading None. Element output S11 S12 S13 E11 E12 E13 Pressure transmitted between the surfaces. The pressure is defined as the force divided by the user-specified area. First frictional shear stress normal to the gap direction. Second frictional shear stress normal to the gap direction. Current opening h of the gap element. Relative displacement (“slip”) in the first direction orthogonal to the contact direction. Relative displacement (“slip”) in the second direction orthogonal to the contact direction. Available for elements with temperature degrees of freedom. HFL1 Heat flux across the interface in the contact direction. The increments of shear slip are the relative displacement increments projected onto the two local directions that are orthogonal to the contact direction. In two-dimensional or axisymmetric models when the contact direction is along the first axis (X or r), the active slip direction is E13 and the active shear stress is S13. In any other two-dimensional or axisymmetric case, the active slip direction is E12 and the active shear stress is S12. Two nodes: the ends of the gap. GAP LIBRARY 39.3 Tube-to-tube contact elements • “Tube-to-tube contact elements,” Section 39.3.1 • “Tube-to-tube contact element library,” Section 39.3.2 39.3.1 TUBE-TO-TUBE CONTACT ELEMENTS Product: Abaqus/Standard References • “Tube-to-tube contact element library,” Section 39.3.2 • *INTERFACE • *SLIDE LINE Overview Tube-to-tube elements: • model the finite-sliding interaction between two pipelines or tubes where one tube lies inside the other or between two tubes or rods that lie next to each other; • are slide line contact elements, in the sense that they assume that the relative motion of the two tubes or pipes is predominantly along the line defined by the axis of one of the tubes (the relative rotations of the tube or pipe axis are assumed to be small); • can be used with pipe, beam, or truss elements; and • do not consider deformations of the tube or pipe cross-section. Chapter 35, “Defining Contact Interactions,” contains a general discussion of contact modeling. Typical applications The tube-to-tube contact elements can be used to model two specific classes of tube-to-tube contact problems: internal (tube within a tube) contact and external contact, where the two tubes are roughly parallel and contact each other along their outer surfaces. It is not possible to use the surface-based contact approach for problems where two three-dimensional tubes contact each other. Choosing an appropriate element Use ITT21 elements with two-dimensional beam, pipe, or truss elements. Use ITT31 elements with three-dimensional beam, pipe, or truss elements. Each of these elements is defined by a single node. Associating the tube-to-tube contact elements with a slide line You must indicate which set of tube-to-tube contact elements will interact with a particular slide line. Details on defining slide lines are discussed below. Input File Usage: *SLIDE LINE, ELSET=element_set_name Defining the element’s section properties You must associate the geometric section properties with a set of tube-to-tube contact elements. *INTERFACE, ELSET=element_set_name Input File Usage: Defining the radial clearance when modeling contact between a pipe within another pipe You define the radial clearance between the pipes. Give a positive value to model contact between two pipes when one pipe (the one with the tube-to-tube contact elements) lies inside of the other pipe. The value given is the difference between the inner radius of the outer pipe and the outer radius of the inner pipe. Input File Usage: *INTERFACE radial clearance Defining the radial clearance when modeling contact between the outer surfaces of two pipes You can model external tube-to-tube contact by specifying a negative value for the radial clearance. The magnitude of the value must be the sum of the outer radii of the two pipes or rods. Local basis for contact output variables The element output variables for ITT elements are given in a local basis system associated with the slide line. The first tangent vector, , is defined by the sequence of the nodes forming the slide line. The direction of contact, , is the normal to the slide line that points toward the nodes of the ITT elements. For ITT31 elements Abaqus/Standard forms a second tangent vector, and . As the elements move, the local basis system will rotate with the axis of the slide line. , that is orthogonal to both Choosing which pipe (beam or truss) will have the slide line In the case of internal tube-to-tube contact, the slide line can be placed on the inner tube or the outer tube. Generally the slide line should be associated with the outer tube ; however, if the inner tube is stiffer than the outer tube, the slide line should be attached to the inner tube. If contact occurs between the exterior surface of the tubes, the slide line should be associated with the stiffer tube if the materials or tube radii are different or with the tube with the coarser mesh if they are the same. Defining the slide line You can specify the nodes that make up the slide line, or they can be generated as described below. If you choose to specify the nodes directly, you must specify them in a sequence that defines a continuous slide line. The nodal sequence defines a tangent vector for the slide line. The slide line must be made up of linear segments. Input File Usage: *SLIDE LINE, ELSET=element_set_name, TYPE=LINEAR first node number, second node number, etc. M L Nodes i, j, k, l, m, and n are specified in that order, thereby identifying a slide line progressing from i to node n. These nodes must lie on the outer tube. ITT-type elements are defined on nodes I, J, K, ... and interact with the slide line. Figure 39.3.1–1 Internal tube-to-tube contact example. Generating the slide line nodes Alternatively, you can indicate that the slide line nodes should be generated and specify only a first node number, a last node number, and an increment between node numbers. Input File Usage: *SLIDE LINE, GENERATE first node number, last node number, increment between node numbers Smoothing the slide line Convergence is often improved by smoothing the discontinuities in surface tangents between slide line segments, thereby providing a smoothly varying tangent along the slide line. For details about smoothing slide lines, see “Contact formulations in Abaqus/Standard,” Section 37.1.1. Defining nondefault mechanical surface interactions with tube-to-tube contact elements By default, Abaqus/Standard uses “hard,” frictionless contact with tube-to-tube contact elements. You can assign optional mechanical surface interaction models. The following mechanical surface interaction models are available: • Friction. See “Frictional behavior,” Section 36.1.5, for details. • Modified “hard” contact, softened contact, and viscous damping. See “Contact pressure-overclosure relationships,” Section 36.1.2, and “Contact damping,” Section 36.1.3, for details. 39.3.2 TUBE-TO-TUBE CONTACT ELEMENT LIBRARY Product: Abaqus/Standard References • “Tube-to-tube contact elements,” Section 39.3.1 • *INTERFACE • *SLIDE LINE Overview This section provides a reference to the tube-to-tube contact elements available in Abaqus/Standard. Element types ITT21 ITT31 Tube-to-tube element for use with two-dimensional beam and pipe elements Tube-to-tube element for use with three-dimensional beam and pipe elements Active degrees of freedom ITT21: 1, 2 ITT31: 1, 2, 3 Additional solution variables ITT21: Two additional variables relating to the contact forces. ITT31: Three additional variables relating to the contact forces. Nodal coordinates required ITT21: X, Y ITT31: X, Y, Z Element property definition Input File Usage: Use the following option to identify the second (outer) pipe with which the specified ITT contact elements on the first (inner) pipe can interact: *SLIDE LINE Use the following option to give the radial clearance between the pipes as a positive number when modeling a tube sliding within another tube: *INTERFACE pipes, the sum of the external radii of the pipes is given as a negative number. ITT ELEMENT LIBRARY Element-based loading None. Element output Stress components S11 S12 S13 Normal component of the force between the two pipes. Shear force between the two pipes, parallel to the axis of the second (outer) pipe. Shear force between the two pipes, normal to the contact direction and to the axis of the second (outer) pipe (for ITT31 only). Strain components E11 E12 E13 Overclosure of the surfaces in the direction normal to the tangent to the centerline of the second (outer) pipe. Accumulated relative tangential motion between the two pipes, parallel to the axis of the second (outer) pipe. Accumulated relative tangential motion between the two pipes, normal to the contact direction and to the axis of the second (outer) pipe (for ITT31 only). Outer pipeline nodes (Slide line) Node ordering and integration point numbering 2-D internal tube contact Inner pipeline nodes and integration points (ITT21 element) 2-D external tube contact First pipeline nodes and integration points (ITT21 element) Second pipeline nodes (Slide line) 3-D internal tube contact Inner pipeline nodes and integration points (ITT31 element) 3-D external tube contact First pipeline nodes and integration points (ITT31 element) 39.3.2–4 Abaqus Version 6.12 ID: Printed on: Outer pipeline nodes 39.4 Slide line contact elements • “Slide line contact elements,” Section 39.4.1 • “Axisymmetric slide line element library,” Section 39.4.2 39.4.1 SLIDE LINE CONTACT ELEMENTS Product: Abaqus/Standard References • “Axisymmetric slide line element library,” Section 39.4.2 • *INTERFACE • *SLIDE LINE Overview Slide line elements: • can model the finite-sliding interaction between two deforming bodies when the sliding occurs along a line (“slide line”) that lies in a specific plane; • assume that tangential motions orthogonal to a slide line are zero or small (Abaqus/Standard treats such motions as being infinitesimal); • can be used with axisymmetric stress/displacement elements; • are recommended for specific applications, such as when a contact surface is the surface of a substructure or when CAXA or SAXA elements are involved in contact; • are available for first- and second-order elements; and • use the same “master-slave” concepts for enforcing contact constraints seen in surface-based contact. For a general discussion of contact modeling, see Chapter 35, “Defining Contact Interactions.” Modeling contact between deformable bodies with slide lines Determining the location of the areas of contact and the surface tractions between contacting structures are common goals of Abaqus simulations . Slide lines and slide line contact elements can provide this information for simulations where both structures are deformable and the finite sliding of the structures occurs along well-defined lines. Local basis system for contact stresses and relative motions of the bodies Abaqus/Standard reports the contact stresses between the bodies and the relative motions of the bodies in a local basis system that is attached to the slide line surface. The local basis system is defined by the normal to the slide line, , and two orthogonal slip directions, . and Contact stress (including friction) Deformable structure Contact area Figure 39.4.1–1 Interaction between deformable structures. t2 T - stress transmitted between the surfaces S11 S12 S13 t1 Figure 39.4.1–2 Local system for interface contact normal and shear traction. Defining the local basis system The sequence of the nodes forming the slide line defines the tangent, normal, , where , and is called the contact plane. Abaqus/Standard defines the slide line normal as is the vector that is orthogonal to the contact plane. . The plane formed by the slide line As shown in Figure 39.4.1–3, a slide line is created using nodes i, j, k, …, p, which are specified in that order, thereby identifying the slide line tangent. Nodes I, J, K, …, N are the nodes of the slide line elements that are associated with this slide line. The slide line normal is defined by specifying , the normal to the contact plane. contact plane ISL element I slide line Figure 39.4.1–3 Defining the local basis for a slide line. The tangent to the slide line coincides with the first slip direction, , of the local basis system. The second slip direction, , is in the opposite direction of . The master-slave concept for slide lines and slide line elements When creating a model that contains slide line elements, it is useful to remember that Abaqus/Standard uses a strict “master-slave” concept to enforce the contact constraints. The slide line contact elements form the “slave” surface. The nodes that you specify to define the slide line define the “master” surface. The nodes of the slide line contact elements are constrained not to penetrate the master surface. The considerations for choosing the master and slave surfaces are the same regardless of whether surfaces or elements are used to define contact. The master surface should be chosen as the surface of the stiffer body if the materials are different or as the surface with the coarser mesh. If the materials and mesh density are the same on both surfaces, the choice is arbitrary. Defining the slide line (master surface) You can specify the nodes that make up the slide line, or they can be generated as described below. If you choose to specify the nodes directly, you must specify them in a sequence that defines a continuous slide line. The nodal sequence defines a tangent vector, , for the slide line. The slide line can be made up of linear or parabolic segments, depending on whether the model is made up of first-order or second-order elements. In either case convergence may be improved by smoothing the slide line. Defining a linear slide line When the surfaces of the bodies are meshed with first-order elements, define a slide line made up of linear element segments. As shown in Figure 39.4.1–4), nodes i, j, k, …, p are specified in that order, thereby identifying a slide line progressing from i through p. Nodes I, J, K, …, N are the nodes of the ISL-type elements that are associated with this slide line. Input File Usage: *SLIDE LINE, ELSET=element_set_name, TYPE=LINEAR first node number, second node number, etc. I Figure 39.4.1–4 First-order (linear) slide line example. Defining a parabolic slide line When the surfaces of the bodies are meshed with second-order elements, define a slide line made up of second-order element segments. In this case the slide line should consist of an odd number of nodes. As shown in Figure 39.4.1–5, nodes i, j, k, …, u are specified in that order, thereby identifying a slide line progressing from i through u. Nodes I, J, K, …, O are the nodes of the ISL-type elements that are associated with this slide line. Input File Usage: *SLIDE LINE, ELSET=element_set_name, TYPE=PARABOLIC first node number, second node number, etc. I Figure 39.4.1–5 Second-order (parabolic) slide line example. Generating the slide line nodes Alternatively, you can indicate that the slide line nodes should be generated and specify only a first node number, a last node number, and an increment between node numbers. Input File Usage: *SLIDE LINE, ELSET=element_set_name, GENERATE first node number, last node number, increment between node numbers Smoothing the slide line Convergence is often improved by smoothing the discontinuities in surface tangents between slide line segments, thereby providing a smoothly varying tangent along the slide line. For details about smoothing slide lines, see “Contact formulations in Abaqus/Standard,” Section 37.1.1. Defining slide line elements (slave surface) Many finite-sliding contact simulations can use the surface-based contact approach, described in Chapter 35, “Defining Contact Interactions,” to define the model. Axisymmetric stress/displacement and coupled temperature-displacement slide line elements are recommended only for specific applications, such as when a contact surface is the surface of a substructure or when CAXA or SAXA elements are involved in contact . The slide line contact elements define the slave surface. The contact area associated with each node on the slave surface is calculated using the current length of the slide line contact element and the constant “width” assigned to the element, which depends on the underlying finite elements. Associating the slide line elements with a slide line You must associate the slide line with a set of slide line contact elements. Details on defining slide lines are discussed below. Input File Usage: *SLIDE LINE, ELSET=element_set_name Defining the slide line element’s section properties You must associate the section properties with a set of slide line elements. There are no section data for axisymmetric slide line elements. *INTERFACE, ELSET=element_set_name Input File Usage: Defining nondefault mechanical surface interactions with slide line elements By default, Abaqus/Standard uses “hard,” frictionless contact with slide line elements. You can assign optional mechanical surface interaction models. The following mechanical surface interaction models are available: • Friction. See “Frictional behavior,” Section 36.1.5, for details. • Modified “hard” contact, softened contact, and viscous damping. See “Contact pressure-overclosure relationships,” Section 36.1.2, and “Contact damping,” Section 36.1.3, for details. Obtaining the “maximum torque” that can be transmitted across axisymmetric slide lines When modeling contact with slide lines with axisymmetric elements (type CAX and CGAX elements), Abaqus/Standard can calculate the maximum torque that can be transmitted across the axisymmetric slide lines. This capability is often of interest when modeling threaded connectors. The maximum torque, T, is defined as where p is the pressure transmitted across the interface, r is the radius to a point on the interface, and s is the current distance along the interface in the r–z plane. This definition of “torque” effectively assumes a friction coefficient of unity. You can request that this torque output be written to the data (.dat) file. The data are provided for every slide line in the model. You can specify the output frequency to limit how often Abaqus/Standard writes this output to the data file. The default output frequency is 1. For surface-based contact with axisymmetric elements, output variable CTRQ provides functionality similar to this torque output request . Input File Usage: *TORQUE PRINT, FREQUENCY=n 39.4.2 AXISYMMETRIC SLIDE LINE ELEMENT LIBRARY Product: Abaqus/Standard References • “Slide line contact elements,” Section 39.4.1 • *INTERFACE • *SLIDE LINE Overview This section provides a reference to the axisymmetric slide line elements available in Abaqus/Standard. Element types ISL21A ISL22A 2-node element for use with first-order axisymmetric elements 3-node element for use with second-order axisymmetric elements Active degrees of freedom 1, 2 at the nodes Additional solution variables Two additional variables at each node relating to the contact stresses. Nodal coordinates required r, z Element property definition Input File Usage: Use the following option to identify the slide line (master surface) with which the slide line elements interact: *SLIDE LINE Use the following option to define the slide line element’s section properties: *INTERFACE Element-based loading None. Element output Stress components S11 S12 Pressure between the node on the body and the slide line with which it interacts. Shear stress between the node on the body and the slide line with which it interacts. Strain components E11 E12 Separation between the node on the body and the slide line. Accumulated relative tangential displacement between the node on the body and the slide line. Node ordering and integration point numbering 2 - node element linear element master surface (defined as a slide line) integration points quadratic element 3 - node element integration points master surface (defined as a slide line) 39.5 Rigid surface contact elements • “Rigid surface contact elements,” Section 39.5.1 • “Axisymmetric rigid surface contact element library,” Section 39.5.2 39.5.1 RIGID SURFACE CONTACT ELEMENTS Product: Abaqus/Standard References • “Axisymmetric rigid surface contact element library,” Section 39.5.2 • “Analytical rigid surface definition,” Section 2.3.4 • *INTERFACE • *RIGID SURFACE Overview Rigid surface contact elements: • can be used to model contact between a rigid surface and a deformable body; • are needed only for several special-purpose applications, such as when a substructure contacts a rigid surface or when CAXA or SAXA element types are involved in contact; • can be used in both geometrically linear and nonlinear simulations; and • use the same “master-slave” concepts for enforcing contact constraints that are used in the surface- based contact capability in Abaqus/Standard. For most problems the surface-based contact capability described in Chapter 35, “Defining Contact Interactions,” provides a more direct and general method for modeling contact between a rigid surface and a deformable body. Modeling contact between rigid surfaces and rigid surface contact elements Determining the location of the areas of contact and the surface tractions between contacting structures are common goals of Abaqus simulations. Rigid surface contact elements can be used to model contact when one of the structures is assumed to be rigid. These elements need to be used only for specific applications, outlined below, because the surface-based contact definitions in Abaqus can be used for most simulations. Modeling contact with axisymmetric rigid surface contact elements Axisymmetric rigid surface contact elements should be used only in the following specific applications: • when the deformable surface is on a substructure , or • when CAXA or SAXA elements are involved in contact . Other planar, axisymmetric, or three-dimensional problems should use the surface-based contact capability. Local basis system for contact stress and relative motions of the surfaces Abaqus/Standard reports the contact stresses between the bodies and the relative motions of the bodies in a local basis system that is attached to the rigid surface. The normal to the rigid surface, which is also the contact direction, is defined when the rigid surface is created. For details, see “Analytical rigid In axisymmetric problems Abaqus/Standard defines the first local surface definition,” Section 2.3.4. tangent to lie in the plane of the model and the second orthogonal to this plane. The master-slave concept for rigid surface contact elements Rigid surface contact elements use a “master-slave” concept to enforce the contact constraints. The rigid surface contact elements form the “slave” surface, and the nodes of these elements are constrained not to penetrate into the rigid (“master”) surface. Defining the rigid surface You define the analytical rigid surface using the methods described in “Defining analytical rigid surfaces when drag chain or rigid surface elements are used” in “Analytical rigid surface definition,” Section 2.3.4. Assigning a rigid body reference node to the rigid surface The motion of a rigid surface is controlled by the motion of a single node, referred to as the rigid body reference node, that is associated with the rigid surface. When rigid surface contact elements are used in a model, the rigid body reference node is identified when defining the IRS elements . Defining the rigid surface contact elements The rigid surface contact elements define the slave surface. They also define the rigid body reference node for the rigid surface with which they interact. All IRS elements identify the rigid body reference node by including its node number as the last node in their connectivity. The nodes on the deformable body that form the IRS elements are always given first. In a model defined in terms of an assembly of part instances, the rigid surface definition and the reference node must appear inside the same part definition as the rigid surface contact elements. Example For example, the following input would be used to define IRS elements 1 and 2 that consist of two nodes on the deformable body and assign node 1000 as the rigid body reference node: *ELEMENT, TYPE=[IRS21A], ELSET=element_set_name 1, 10, 11, 1000 2, 11, 12, 1000 *RIGID SURFACE, ELSET=element_set_name A similar input structure is used for IRS22A elements. Associating an analytical rigid surface with a set of rigid surface contact elements You must identify the set of rigid surface contact elements that interact with a particular rigid surface. *RIGID SURFACE, ELSET=element_set_name Input File Usage: Defining the rigid surface element’s section properties You must associate the section properties with a set of rigid surface contact elements. There are no section data for axisymmetric rigid surface contact elements. Input File Usage: *INTERFACE, ELSET=element_set_name Defining nondefault mechanical surface interactions with rigid surface contact elements By default, Abaqus/Standard uses a “hard,” frictionless mechanical surface interaction model with rigid surface contact elements. You can assign optional mechanical surface interaction models. The following mechanical surface interaction models are available: • Friction. See “Frictional behavior,” Section 36.1.5, for details. • Modified “hard” contact, softened contact, and viscous damping. See “Contact pressure-overclosure relationships,” Section 36.1.2, and “Contact damping,” Section 36.1.3, for details. 39.5.2 AXISYMMETRIC RIGID SURFACE CONTACT ELEMENT LIBRARY Product: Abaqus/Standard References • “Analytical rigid surface definition,” Section 2.3.4 • “Rigid surface contact elements,” Section 39.5.1 • *RIGID SURFACE • *INTERFACE Overview This section provides a reference to the axisymmetric rigid surface contact elements available in Abaqus/Standard. Element types IRS21A IRS22A Axisymmetric rigid surface contact element for use with first-order axisymmetric elements Axisymmetric rigid surface contact element for use with second-order axisymmetric elements Active degrees of freedom 1, 2 at each node except the last node 1, 2, 6, the motion of the rigid body reference node, at the last node Additional solution variables Two additional variables at each node relating to the contact stresses. Nodal coordinates required r, z Element property definition Input File Usage: Use the following option to define the surface with which the elements interact: *RIGID SURFACE Use the following option to define the rigid surface element’s section properties: *INTERFACE Element-based loading None. Element output S11 S12 E11 E12 Pressure between the element and the rigid surface in the direction of the normal to the rigid surface. Shear component of the stress between the element and the rigid surface in the direction of the tangent to the rigid surface. Separation of the surfaces in the direction of the normal to the rigid surface at the closest point of the surface to the integration point on the element. Accumulated relative tangential displacement of the surfaces. Node ordering on elements The first two nodes in IRS21A and the first three nodes in IRS22A are on the deforming mesh. The last node is the rigid body reference node that defines the motion of the rigid body. Numbering of integration points for output The integration points are located at the nodes that lie on the surface of the deforming model and are numbered correspondingly. 40. Defining Cavity Radiation in Abaqus/Standard Defining cavity radiation 40.1 Defining cavity radiation • “Cavity radiation,” Section 40.1.1 40.1.1 CAVITY RADIATION Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Heat transfer analysis procedures: overview,” Section 6.5.1 • *CAVITY DEFINITION • *COUPLED THERMAL-ELECTRICAL • *CYCLIC • *EMISSIVITY • *HEAT TRANSFER • *MOTION • *PERIODIC • *PHYSICAL CONSTANTS • *RADIATION FILE • *RADIATION PRINT • *RADIATION OUTPUT • *RADIATION SYMMETRY • *RADIATION VIEWFACTOR • *REFLECTION • *SURFACE • *SURFACE PROPERTY • *VIEWFACTOR OUTPUT • “Cavity radiation,” Section 2.11.4 of the Abaqus Theory Manual • “Defining a cavity radiation interaction,” Section 15.13.21 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a cavity radiation interaction property,” Section 15.14.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Abaqus/Standard provides a cavity radiation capability for modeling heat transfer effects due to radiation in enclosures. This cavity radiation functionality: • can be included in heat transfer analysis problems without deformation (“Uncoupled heat transfer analysis,” Section 6.5.2, and “Coupled thermal-electrical analysis,” Section 6.7.3); • is provided for two-dimensional, three-dimensional, and axisymmetric cases; • accounts for symmetries, surface blocking, and surface motion within cavities; and • can include closed cavities or open cavities (implying that some radiation takes place to an exterior medium). Cavity radiation equations are not symmetric; therefore, the nonsymmetric matrix storage and solution scheme is invoked automatically in models that include cavity radiation . Each cavity defines a viewfactor matrix involving the geometric relations between the surfaces in the enclosure. These matrices may be updated a number of times during the analysis (due to moving surfaces in the cavity). Therefore, large cavity radiation problems may be computationally expensive. Instead, you should consider using: • gap radiation for modeling radiation between closely spaced surfaces; • average-temperature radiation conditions for modeling enclosures that are approximately isothermal, with constant emissivity, and do not require blocking or reflection considerations ; or • parallel cavity decomposition for parallel calculation of viewfactors and solution of the radiative heat transfer equations . Defining a cavity radiation problem Since cavity radiation effects are calculated only in heat transfer and coupled thermal-electrical procedures, the only kind of thermal-stress analysis that can include these effects is sequentially coupled thermal-stress analysis . Moreover, unless you allow cavity parallel decomposition , there is a software limit of 16,000 nodes and facets in Abaqus/Standard. Model definition When you define the model for a cavity radiation problem, you must: 1. define all of the surfaces in the cavity ; 2. define the radiation properties of each surface (i.e., the emissivity) and the physical constants ; and 3. construct cavities from the surfaces . History definition In the first step of a cavity radiation analysis you must associate with each cavity a radiation viewfactor definition, which controls the calculation of viewfactors for the cavity. You then may: 1. define cavity symmetries, if any ; 2. prescribe the motion of surfaces ; 3. define boundary conditions such as temperature and forced convection ; 4. control the cavity radiation and viewfactor calculations in each step (the specifications from the previous step are used if they are not redefined in a step; see “Controlling viewfactor calculation during the analysis”); 5. request output of heat transfer variables to the data and results files ; and 6. request output of the radiation viewfactor matrices . If any of the above are included in your analysis, they must be defined within a heat transfer or coupled thermal-electrical step definition. Defining surfaces Cavities are defined in Abaqus/Standard as collections of surfaces, which are composed of facets. In axisymmetric and two-dimensional cases a facet is a side of an element; in three-dimensional cases a facet is a face of a solid element or a surface of a shell element. Rigid surfaces cannot be used in cavity radiation problems. Surfaces are defined as described in “Element-based surface definition,” Section 2.3.2. You may associate each surface with a surface property definition as part of the surface option, or you may associate surfaces with surface properties as part of the cavity definition option. The surface properties are defined as described below. Input File Usage: Use the following option to define a surface with a surface property for use in a cavity radiation analysis: *SURFACE, TYPE=ELEMENT, NAME=surface_name, PROPERTY=property_name Use the following option to define a surface for use in a cavity radiation analysis in which surface properties are defined as part of the cavity definition: Abaqus/CAE Usage: *SURFACE, TYPE=ELEMENT, NAME=surface_name Interaction module: Create Interaction: Cavity radiation: select the initial surface region Restrictions Surfaces that are associated with cavity radiation are subject to the following restrictions in addition to the general surface definition restrictions outlined in “Element-based surface definition,” Section 2.3.2: • Surfaces cannot overlap because of the ambiguity that would result in the associated property definitions and in the blocking specification. • A surface can be used only in one cavity definition (the same surface cannot appear in two different cavities). In addition, the three-dimensional quadrilateral facets should be as close to planar as possible; otherwise, the quality of the viewfactor calculations will be compromised. Controlling spurious spatial oscillations The radiation flux for each facet is calculated based on the average of the nodal temperatures on that facet . This value of radiation flux is then distributed to each node in proportion to its area. Consequently, the mesh must be sufficiently fine that temperature differences across elements are small. Otherwise, computed fluxes at nodes with temperatures above the facet average will be excessively low, and the fluxes at nodes with below-average temperatures will be too high. This tends to induce a spatially oscillatory solution. This effect can be eliminated by reducing the element size in the vicinity of high temperature gradients. Defining surface radiation properties Cavity radiation problems are intrinsically nonlinear, due to the dependence of the radiative flux on the fourth power of the facet temperature. Further, nonlinearity can be introduced by describing the emissivity, , as a function of temperature. Defining the emissivity Emissivity is a dimensionless quantity with a value that is greater than or equal to zero and less than or equal to one. A value of corresponds to all radiation being reflected by the surface. A value of corresponds to black body radiation, where all radiation is absorbed by the surface. You can define , of a surface as a function of temperature and other predefined field variables. the emissivity, You must assign a name to the surface property that defines the emissivity. Input File Usage: Use both of the following options to define the emissivity of a surface: *SURFACE PROPERTY, NAME=property_name *EMISSIVITY The *EMISSIVITY option must appear directly after PROPERTY option in the model definition section of the input file. the *SURFACE If black body radiation is being defined ( used in the step definition to improve efficiency: ), the following option can be Abaqus/CAE Usage: *RADIATION VIEWFACTOR, REFLECTION=NO Use the following input to define gray body radiation: Interaction module: Create Interaction Property: Cavity radiation: enter the emissivity ( ) You can define the emissivity as a function of temperature and/or field variables. Use the following input to define black body radiation: Interaction module: Create Interaction: Cavity radiation: Use heat reflection: No Controlling the accuracy of temperature-dependent emissivity changes Abaqus/Standard evaluates the emissivity, , based on the temperature at the start of each increment and uses that emissivity value throughout the increment. When emissivity is a function of temperature or field variables, you can control the time incrementation for the heat transfer or coupled thermal-electrical step by specifying the maximum allowable emissivity change during an increment, . If this tolerance is exceeded, Abaqus/Standard will cut back the increment size until the maximum change in emissivity is less than the specified value. If you do not specify a value for , a default value of 0.1 is used. Input File Usage: Use either of the following options: Abaqus/CAE Usage: *HEAT TRANSFER, MXDEM= *COUPLED THERMAL-ELECTRICAL, MXDEM= Step module: Create Step: Heat transfer or Coupled thermal-electric: Incrementation: Automatic: Max. allowable emissivity change per increment: Defining the Stefan-Boltzmann constant and value of absolute zero You must define the Stefan-Boltzmann constant, default values for these constants. , and the value of absolute zero, ; there are no Input File Usage: *PHYSICAL CONSTANTS, STEFAN BOLTZMANN= , ABSOLUTE ZERO= This option can appear anywhere in the model definition portion of the input file. Abaqus/CAE Usage: Any module: Model→Edit Attributes→model_name. Enter values for Absolute zero temperature and Stefan-Boltzmann constant Constructing a cavity You construct cavities as collections of the surfaces defined as described above. Each surface can be used only in one cavity definition. Each cavity must have a unique name; this name is used to specify viewfactor calculations. The cavity name can also be used to request output. Setting surface properties By default, a cavity is assumed to consist of surfaces for which surface properties have already been defined. Instead, you may define surface properties as part of the cavity definition. Input File Usage: Use the following option to construct a cavity: *CAVITY DEFINITION, NAME=cavity_name, SET PROPERTY surface name, surface property name By using the SET PROPERTY parameter, you define the surface properties used in the cavity, overriding any property defined as part of the surface option. Abaqus/CAE Usage: Interaction module: Create Interaction: Cavity radiation: select the surface region. Use the Properties table to add or edit surfaces and cavity radiation interaction properties (emissivity). Creating a closed cavity By default, a cavity is assumed to be closed. Input File Usage: Abaqus/CAE Usage: Use the following option to construct a closed cavity: *CAVITY DEFINITION, NAME=cavity_name Interaction module: Create Interaction: Cavity radiation: Definition: Closed Creating an open cavity You can specify an open cavity by defining the reference temperature of the external medium. This ambient temperature value is converted to an absolute temperature scale based on the definition of absolute zero. You can verify the degree of opening in the cavity by specifying a tolerance for the accuracy of the viewfactor calculations; radiation to the external medium will take place only if the deviation of the sum of the viewfactors from unity is more than this tolerance. See “Controlling the accuracy of viewfactor calculations” below for details. Input File Usage: Abaqus/CAE Usage: Use the following option to create an open cavity: *CAVITY DEFINITION, NAME=cavity_name, AMBIENT TEMP= Interaction module: Create Interaction: Cavity radiation: Definition: Open, Ambient temperature: Creating a cavity with multiple openings or complex ambient conditions The open cavity definition allows for a cavity with a single opening into an ambient environment with a single, constant temperature value. If the cavity has multiple openings or the ambient temperature is not constant, you should model the surroundings differently. You should close any cavity openings with elements, and prescribe the temperatures of the external media on these elements. Since the cavity is now closed, you should not specify an ambient temperature with the cavity definition. The temperature definition that you use for the closing elements provides the ambient temperature, and it allows you to specify different temperatures, including variable temperatures, at the cavity openings. The elements modeling the external media should not share nodes with the cavity elements (so that conduction will not take place between them). The surfaces defined by the external media elements should have an emissivity of 1. Decomposing large cavities in parallel By default, Abaqus/Standard uses a single working thread for the calculation of the viewfactor matrix and solution of the radiative heat transfer equations . This method is robust and works well for small cavities composed of hundreds of facets, but it becomes inefficient and computationally expensive for large cavities composed of thousand of facets. Moreover, the memory requirements for these cavities may be prohibitively large for a single computational node (the viewfactor matrix is the size of the number of facets squared). In these cases you should consider allowing Abaqus/Standard to decompose the cavity among all CPUs during viewfactor calculations and solution of the radiative heat transfer equations. Input File Usage: Use the following option to activate cavity parallel decomposition: *CAVITY DEFINITION, NAME=cavity_name, PARALLEL DECOMPOSITION=ON Abaqus/CAE Usage: Cavity parallel decomposition is not supported in Abaqus/CAE. Solving radiative heat transfer equations in parallel Abaqus/Standard uses an iterative solution technique for obtaining the radiative heat fluxes when cavity parallel decomposition is enabled. This technique is based on Krylov methods, employs a preconditioner, and uses only MPI-based parallelization . This iterative technique is used only to solve the cavity radiation equations and does not require user intervention. You may still opt to use the either the iterative or direct sparse solvers for the solution of the heat transfer finite element equations. Convergence of models with decomposed cavities The exact cavity radiation equations are solved whether parallel decomposition is allowed or not; however, when parallel decomposition is active, Abaqus/Standard may require more iterations to obtain a solution. This slower rate of convergence comes from an approximation to the Jacobian (the linearization of the radiation fluxes) that is based on small changes of the irradiation (any part not due to emission from the surface). Models involving surfaces with low emissivities and steady-state analyses might be especially affected. If you encounter convergence problems with parallel decomposed cavities, you may consider • changing the analysis from steady-state to transient Section 6.5.2); or (“Uncoupled heat transfer analysis,” • allowing more solver iterations per time increment (“Convergence criteria for nonlinear problems,” Section 7.2.3). Kinematic constraints on models with decomposed cavities Kinematic constraints (for example, coupling constraints, linear constraint equations, multi-point constraints, or surface-based tie constraints) can be applied to any node or surface belonging to a cavity where parallel decomposition is allowed. However, the nodes or surfaces must be the independent (master) nodes or surfaces in the constraint definition. Defining cavity symmetries Taking advantage of geometric symmetry can reduce computational model size and simulation time. Instead of modeling all of the parts or components in a symmetric assembly, you can model a smaller repeated component and take symmetry into account in the definition of the cavity radiation interaction. In Abaqus/Standard cavity definitions with defined symmetries take into account the radiation interactions between each cavity facet and between all of the facets in the cavity and all of its symmetric images. Abaqus/Standard does not check that the model created using cavity symmetries is physically realistic. You must check the input and results carefully to ensure that a valid model is created. You must assign a name to each radiation symmetry definition for reference by a radiation viewfactor definition. The radiation viewfactor definition and corresponding radiation symmetry definition must appear in the same step. Cyclic, periodic, and/or reflection symmetries can be defined as described below. Input File Usage: Use all of the following options to define symmetry in a cavity radiation problem: *RADIATION VIEWFACTOR, SYMMETRY=symmetry_name *RADIATION SYMMETRY, NAME=symmetry_name *REFLECTION and/or *PERIODIC and/or *CYCLIC Interaction module: Create Interaction: Cavity radiation: Symmetry: Reflection, Periodic, and/or Cyclic Abaqus/CAE Usage: Reflection symmetry You define reflection symmetry to create a cavity that is composed of the user-defined cavity surface plus its reflected image through a line or plane. You must identify the dimensionality of the cavity when you define reflection symmetry. Reflection of two-dimensional cavities You can define the cavity symmetry by reflecting the cavity surface through a line, as shown in Figure 40.1.1–1. This type of reflection can be used only with two-dimensional cavities. Input File Usage: Abaqus/CAE Usage: *REFLECTION, TYPE=LINE Interaction module: Create Interaction: Cavity radiation: Symmetry: Reflection: select the symmetry line Reflection of three-dimensional cavities You can define the cavity symmetry by reflecting the cavity surface through a plane, as shown in Figure 40.1.1–2. This type of reflection can be used only with three-dimensional cavities. Input File Usage: Abaqus/CAE Usage: *REFLECTION, TYPE=PLANE Interaction module: Create Interaction: Cavity radiation: Symmetry: Reflection: select the symmetry plane Reflection of axisymmetric cavities You can define the cavity symmetry by reflecting the cavity surface through a line of constant z-coordinate, as shown in Figure 40.1.1–3. This type of reflection can be used only with axisymmetric cavities. Figure 40.1.1–1 Reflection symmetry through a line. Figure 40.1.1–2 Reflection symmetry through a plane. Input File Usage: Abaqus/CAE Usage: *REFLECTION, TYPE=ZCONST Interaction module: Create Interaction: Cavity radiation: Symmetry: Reflection: enter the z-axis symmetry value for the line of symmetry z = const symmetry line Figure 40.1.1–3 Reflection symmetry through a line of constant z-coordinate. Periodic symmetry You can define cavity symmetry by periodic repetition in a given direction. Physically, periodic symmetry is understood as an infinite number of repetitions of the same image at a periodic interval. Numerically, periodic symmetry has to be represented by a finite number of repetitions of the periodic image. You can define the number of repetitions used in the numerical calculation, n. The periodic symmetry will result in a cavity composed of the user-defined cavity plus twice n similar images, since the periodic symmetry is assumed to apply in both the positive and negative directions. By default, n=2. Although symmetries do not increase the size of the viewfactor matrix, they do make its calculation more expensive. Therefore, the number of repetitions should be minimized, but the value of n should be large enough that the viewfactor matrix is calculated accurately. Output variable VFTOT can be used to check the amount of closure implied by the symmetry. Periodic symmetry for defining the cavity radiation viewfactor matrix does not impose symmetry conditions automatically in the heat transfer analysis. It may be necessary to impose appropriate constraints on the temperature and loading conditions at the nodes on the periodic symmetry planes to obtain a meaningful solution from the underlying heat transfer analysis. You must identify the dimensionality of the cavity when you define periodic symmetry. Periodic symmetry of two-dimensional cavities You can create a cavity that is composed of a series of similar images generated by repetition along a two-dimensional distance vector, as shown in Figure 40.1.1–4. -2d -d 2d n = 2 Figure 40.1.1–4 Two-dimensional periodic symmetry. The repeated images are bounded by lines parallel to line ab. The distance vector must be defined so that it points away from line ab and into the domain of the model. This type of periodic symmetry can be used only with two-dimensional cavities. Input File Usage: Abaqus/CAE Usage: *PERIODIC, TYPE=2D, NR=n Interaction module: Create Interaction: Cavity radiation: Symmetry: Periodic: Number of periodic symmetries: n Periodic symmetry of three-dimensional cavities You can create a cavity that is composed of a series of similar images generated by repetition along a three-dimensional distance vector, as shown in Figure 40.1.1–5. The repeated images are bounded by planes that are parallel to plane abc. The distance vector must be defined so that it points away from plane abc and into the domain of the model. This type of periodic symmetry can be used only with three-dimensional cavities. 2d n = 2 -d -2d Figure 40.1.1–5 Three-dimensional periodic symmetry. Input File Usage: Abaqus/CAE Usage: *PERIODIC, TYPE=3D, NR=n Interaction module: Create Interaction: Cavity radiation: Symmetry: Periodic: Number of periodic symmetries: n Periodic symmetry of axisymmetric cavities You can create a cavity that is composed of a series of similar images generated by repetition in the z-direction, as shown in Figure 40.1.1–6. The repeated images are bounded by lines of constant z- coordinate. The z-distance vector must be defined so that it points away from the z-constant periodic symmetry reference line and into the domain of the model. This type of periodic symmetry can be used only with axisymmetric cavities. Input File Usage: Abaqus/CAE Usage: *PERIODIC, TYPE=ZDIR, NR=n Interaction module: Create Interaction: Cavity radiation: Symmetry: Periodic: Number of periodic symmetries: n Cyclic symmetry You can define cavity symmetry by cyclic repetition of the user-defined cavity surface about a point or an axis. The cavity defined by cyclic repetition must cover 360°. You must define the number of cyclically similar images that compose the cavity, n. The angle of rotation about a point or axis used to create cyclically similar images is equal to 360°/n. You must identify the dimensionality of the cavity when you define cyclic symmetry. Cyclic symmetry of two-dimensional cavities You can define the cavity symmetry by rotating the cavity about a point, l, as shown in Figure 40.1.1–7. The cavity surface defined in the model must be bounded by the line lk and a line passing through l at an 2d -d -2d n = 2 z = const periodic symm reference line Figure 40.1.1–6 Axisymmetric periodic symmetry. n = 4 Figure 40.1.1–7 Cyclic symmetry about a point. angle, measured counterclockwise when looking into the plane of the model, of 360°/n to lk. This type of cyclic symmetry can be used only for two-dimensional cavities. Input File Usage: Abaqus/CAE Usage: *CYCLIC, TYPE=POINT, NC=n Interaction module: Create Interaction: Cavity radiation: Symmetry: Cyclic: toggle on Use cyclic symmetric, Total number of sectors: n Cyclic symmetry of three-dimensional cavities You can define the cavity symmetry by rotating the cavity about an axis, lm, as shown in Figure 40.1.1–8. The cavity surface defined in the model must be bounded by the plane lmk and a plane passing through the line lm at an angle, measured clockwise when looking from l to m, of 360°/n to lmk. Line lk must be normal to line lm. This type of cyclic symmetry can be used only for three-dimensional cavities. n = 8 Figure 40.1.1–8 Cyclic symmetry about an axis. Input File Usage: Abaqus/CAE Usage: *CYCLIC, TYPE=AXIS, NC=n Interaction module: Create Interaction: Cavity radiation: Symmetry: Cyclic: toggle on Use cyclic symmetric, Total number of sectors: n Combining symmetries Reflection, periodic, and cyclic symmetries can be combined as shown in Table 40.1.1–1. Figure 40.1.1–9 through Figure 40.1.1–12 illustrate some possible symmetry combinations. Table 40.1.1–1 Permissible number of symmetry definitions used in combination. Reflection Periodic Cyclic 2-D 3-D Axi Restrictions • • • • • • • • • • • • • • • • • • • • , , , , , are normals to lines or planes of reflection symmetry. are distance vectors used to define periodic symmetry. is the direction of the axis of cyclic symmetry in three-dimensional cases. a 2 n1 b1 n2 b2 a 1 Figure 40.1.1–9 Combination of two reflection symmetries in two dimensions. a1 1d (n=3) b2 a2 2d (n=2) b1 Figure 40.1.1–10 Combination of two periodic symmetries in two dimensions. d (n=2) b1 a1 a2 b2 Figure 40.1.1–11 Combination of one reflection symmetry and one periodic symmetry in two dimensions. 10 d -10 d n = 4 (cyclic) n = 10 (periodic) Figure 40.1.1–12 Combination of one cyclic symmetry and one periodic symmetry in three dimensions. Prescribing motion during a cavity radiation analysis In many cavity radiation problems such as simulations of manufacturing sequences, radiation viewfactors change because surfaces are moved during the analysis. You can specify surface motions during heat transfer or coupled thermal-electrical analysis. The prescribed motions affect only the calculation of viewfactors (and, therefore, radiation fluxes) in heat transfer due to cavity radiation. They do not affect heat conduction, storage, or distributed flux contributions. You can define both the translational and rotational components of the motion within a step independently. For example, you can prescribe the translational motion of a node set according to a certain amplitude function and then prescribe the rotational motion of the node set according to a different amplitude function. In each step, each component of motion can be specified only once for any particular node. Motions can also be prescribed during steps in which the cavity radiation is turned off, as described below. Translational motion Translations, , are specified in terms of global x-, y-, and z-components unless a local coordinate system is defined at the nodes for which motion is specified; then translations are specified in terms of local x-, y-, and z-components . Translational displacements are always specified as total values of translational motion. This treatment of translations is consistent with that used for displacement boundary conditions (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) in stress/displacement analyses. The default is to apply translational motion. Translational velocities can also be specified. Translational velocities always refer to the current step; therefore, the rate of translational motion specified as a velocity is in effect only during the step for which it is defined. This behavior is different from velocity boundary conditions, where velocities stay in effect in subsequent steps if they are not redefined. Input File Usage: Use either of the following options to prescribe translational motion: *MOTION, TRANSLATION, TYPE=DISPLACEMENT *MOTION, TRANSLATION, TYPE=VELOCITY Surface motion is not supported with cavity radiation in Abaqus/CAE. Abaqus/CAE Usage: Rotational motion , can be defined by specifying the magnitude of the rotation Displacements due to a rigid body rotation, and the rotation axis. In three dimensions the rotation axis is defined by specifying two points, and , on the axis of rotation. In two dimensions the rotation axis is assumed to be normal to the plane of the model and is defined by specifying one point, . The coordinates of the points defining the axis of rotation must be defined in the configuration at the beginning of the step for which rigid body rotation is being defined. Motion due to rigid body rotation during a step is specified as the amount of rotation that takes place during that step only. Therefore, the rigid body rotation specified during a step is local to that step; if no rigid body rotation is specified in the following step, no further rotation occurs. The treatment of rigid body rotations is different from that of translations: rigid body rotations are specified incrementally from step to step while translations are specified as total values. Input File Usage: Use either of the following options to prescribe rotational motion: Abaqus/CAE Usage: *MOTION, ROTATION, TYPE=DISPLACEMENT *MOTION, ROTATION, TYPE=VELOCITY Surface motion is not supported with cavity radiation in Abaqus/CAE. Prescribing large rotational motions radians or complex sequences of rotations about Prescribed rotational motions of more than different directions in three-dimensional models are most simply defined by specifying rotational velocities, which allows the definition to be given in terms of the angular velocity instead of the total rotation. Abaqus/Standard calculates the increment of rotation as the average of the angular velocities at the beginning and end of each increment multiplied by the time increment. Section 1.2.2.) , 18.84955592, 0., 0., 0., 0., 0., 1. The angular velocity will be constant since the default variation for motions prescribed using a predefined velocity field in a heat transfer or coupled thermal-electrical step (both steady-state and transient) is a step function . An amplitude reference could be used to specify other variations of the angular velocity. If, in the next step, the same node (or node set) should have an additional rotation of radians about the global x-axis, assuming again a step time of 1.0, prescribe a constant angular velocity as follows: *MOTION, TYPE=VELOCITY, ROTATION node (node set), 1.570796327, 0., 0., 0., 1., 0., 0. Prescribing simultaneous rigid body rotations Motions involving two or more simultaneous rigid body rotations about different axes cannot be specified directly. An example of simultaneous rigid body rotations is a satellite rotating about its own axis while orbiting the earth. Such complex motions can be defined with user subroutine UMOTION. This subroutine allows specification of the time variation of the magnitude of the translational components of the motion (degrees of freedom 1–3) at each node. If you specify the magnitude of the translation as part of the prescribed motion definition, it will be modified by the amplitude curve (if any) and passed into subroutine UMOTION, where it can be redefined. When user subroutine UMOTION is used to define the motion of a certain node set in a step, only one prescribed motion can be defined in that step for that node set. The complete motion of all nodes in the node set during the step must be defined in the user subroutine. Input File Usage: Abaqus/CAE Usage: *MOTION, USER Surface motion is not supported with cavity radiation in Abaqus/CAE. Simultaneous translational and rotational motion Whenever simultaneous translational and rotational motion is specified, the total motion of a node during step k is defined as where of the node, and is the current location of the node due to the specified motion history, is the original location is the displacement of the node due to the translational motion specified in the step, is the displacement of the node due to rigid body rotation during step i. In these cases the translation is applied first and the rotation is then assumed to be about the translated due to rigid body rotation during step i is computed (material) axis. In other words, the displacement as the rotation about an axis defined by points and where In the preceding equations the prescribed rotational motion (they refer to the configuration at the beginning of step i) and the displacement due to translational motion during the step ( is the time at the end of step are the locations of the points used to define the axis of rotation for is , where and ). Example As an example, consider a three-dimensional problem with x–y planar motion as shown in Figure 40.1.1–13. 53.13 o Figure 40.1.1–13 Planar motion example. The centroid of the object of interest is initially located at . In the first step the object is translated 4 length units in the x-direction while at the same time it rotates clockwise 180° ( radians) about the z-axis at constant angular velocity. This motion moves the object from position A to position C in Figure 40.1.1–13. Halfway through this motion, at position B, the displacements due to the rigid body rotation are calculated by applying the translation to the z-axis (the axis of rotation) and then applying a 90° rotation about this translated axis. In the second step the object is translated −3 length units in the y-direction only. This motion places the object at position D with no additional rotation. Finally, in the third step the object is simultaneously translated 5 length units at an angle of 53.13° to the y-direction and rotated clockwise, again at constant angular velocity, through 180° about the z-axis. This motion returns the object to its original position. Assuming that each step time is 1.0, the input required for the above motion sequence is as follows: First step: *MOTION node set, 1, 1, 4. *MOTION, ROTATION, TYPE=VELOCITY node set, 3.14159265, 0., 3., 0., 0., 3., -1. Second step: *MOTION node set, 2, 2, -3. Third step: *MOTION node set, 1, 2, 0. *MOTION, ROTATION, TYPE=VELOCITY node set, 3.14159265, 4., 0., 0., 4., 0., -1. Controlling the time variation of the motion For any prescribed motion you can refer to an amplitude curve that gives the time variation of the motion throughout a step . Input File Usage: Use both of the following options: Abaqus/CAE Usage: *AMPLITUDE, NAME=amplitude *MOTION, AMPLITUDE=amplitude Surface motion is not supported with cavity radiation in Abaqus/CAE. Controlling the frequency of viewfactor recalculation due to motion You can control how viewfactors are recalculated during a step as a result of prescribed motion by specifying a value for the maximum allowable motion, max, for a particular node set. Viewfactor recalculation is triggered if a displacement component at any node in the specified node set exceeds the specified value for max. You must respecify the value of max and the node set in every step where recalculation is required; the values do not remain in effect for subsequent steps. Viewfactor recalculation can be expensive; use discretion when choosing a value for max. Input File Usage: *RADIATION VIEWFACTOR, MDISP=max, NSET=nset The max and nset values must always be specified together. Abaqus/CAE Usage: Viewfactor recalculation due to motion is not supported with cavity radiation in Abaqus/CAE. Controlling viewfactor calculation during the analysis The cavity radiation capability can be used in applications such as the simulation of manufacturing sequences where radiation viewfactors change during the simulation. Therefore, radiation viewfactor definitions provide significant flexibility for the control of viewfactor calculations during a step. Multiple radiation viewfactor definitions can be specified within a step definition if different types of radiation and viewfactor calculations are required for different cavities. Different types of viewfactor calculations can be specified for the same cavity in different steps of the analysis. By default, viewfactors are calculated at the beginning of the first step that includes a radiation viewfactor definition. Viewfactors are recalculated at the beginning of a subsequent step only if the viewfactor definition changes in that step; for example, if different surface blocking checks are specified for the same cavity. In a restart analysis Abaqus/Standard reads the radiation viewfactors from the user- specified restart step and increment and recalculates the viewfactors only if the viewfactor definitions have changed. You can specify the name of the cavity for which radiation viewfactor control is being specified. If you do not specify a cavity name, the radiation viewfactor definition applies to all cavities in the model. Input File Usage: Abaqus/CAE Usage: *RADIATION VIEWFACTOR, CAVITY=cavity_name Radiation viewfactors are defined separately for each cavity radiation interaction and apply to all steps in which that interaction is active. Activating and deactivating cavity radiation There are practical situations in which it may be useful to switch cavity radiation effects on and off during the analysis. For example, radiation may be taking place in a cavity that is then filled with a fluid so that radiation is no longer significant; later in the analysis, radiation may resume when the fluid is drained from the cavity. In such cases you can use a radiation viewfactor definition to switch the radiation on and off in any particular cavity during one or more steps of the analysis. When cavity radiation is switched back on after having been switched off, Abaqus/Standard will use the last viewfactors calculated in the last step in which cavity radiation was active. However, if motion is prescribed during the time that the cavity radiation is switched off and one of the displacement components of a node in the specified node set exceeds the value for the maximum allowable motion, max, specified in the step during which cavity radiation is switched off, the viewfactors will be recalculated at the beginning of the step in which the cavity radiation is switched back on. Input File Usage: Use the following option to turn viewfactor calculation off for a step: *RADIATION VIEWFACTOR, OFF Use one of the following options to turn viewfactor calculation back on in a subsequent step: *RADIATION VIEWFACTOR *RADIATION VIEWFACTOR, MDISP=max, NSET=nset Abaqus/CAE Usage: Radiation viewfactors cannot be turned off or on for a selected step. You can use the following options to turn a cavity radiation interaction off or on: Interaction module: Interaction Manager: select a step and a cavity radiation interaction, Activate or Deactivate Controlling the accuracy of viewfactor calculations Abaqus/Standard uses a progressive integration scheme for viewfactor calculation. When facets are sufficiently far from each other, a lumped area approximation is used. If the facets are close to each other but one of the facets is much larger than the other, an infinitesimal-to-finite approximation is used. For all other cases a contour integral is numerically calculated to compute the viewfactor. See “Viewfactor calculation,” Section 2.11.5 of the Abaqus Theory Manual, for details. Two nondimensional parameters are calculated for each facet pair to determine which integration scheme is used: and is the area of the smaller facet, is the area of the larger facet, and d is the distance where between their centroids. The lumped area approximation is used whenever the nondimensional distance square parameter , an infinitesimal-to-finite area has a default value of 5.0. If approximation is used if the facet area ratio has a default value of 64.0. Otherwise, a more precise calculation is performed, involving the numerical integration of a contour integral. , where , where and You can customize the accuracy and speed of the viewfactor calculation by specifying the and the number of integration points per edge. For example, Abaqus/Standard is set to zero. Likewise, the are parameters will used lumped area approximations throughout the whole model if more precise, albeit more expensive, numerical integration method will always be used if set to very large numbers. and Input File Usage: *RADIATION VIEWFACTOR, LUMPED AREA=P1, INFINITESIMAL=P2, INTEGRATION=integration points per edge Abaqus/CAE Usage: Interaction module: Create Interaction: Cavity radiation: Viewfactors: enter new values or accept the defaults for Infinitesimal facet area ratio, Gauss integration points per edge, and Lumped area distance-square value Viewfactor calculation checks for closed cavities You can provide a tolerance on the accuracy of the viewfactor calculation. In a closed cavity the sum of the viewfactors for each cavity facet should be one. Abaqus/Standard compares the value of the specified tolerance to the largest viewfactor matrix row sum deviation from unity; that is, . If the tolerance is violated for a closed cavity, the analysis is terminated. The default viewfactor tolerance is 0.05. Failure to meet this criterion may indicate a need for mesh refinement. Input File Usage: *RADIATION VIEWFACTOR, VTOL=tolerance Abaqus/CAE Usage: Interaction module: Create interaction: Cavity radiation: Viewfactors: Accuracy tolerance: tolerance Viewfactor calculations in cavities with symmetries The viewfactor calculations account for the closure of a cavity implied by any cavity symmetries. For cavities without periodic or cyclic symmetries the viewfactors are calculated exactly for two-dimensional geometries, but approximations are made for axisymmetric and three-dimensional geometries. These approximations become less accurate as the distance between surfaces decreases. Define heat radiation to model closely spaced surfaces . Viewfactor calculations in open cavities If the sum of the viewfactors for facets in an open cavity (defined by specifying a value for the ambient temperature) deviates from unity by more than the specified viewfactor tolerance, radiation to the ambience will take place. In nearly closed cavities this deviation may be small. If the tolerance is not violated, radiation to the external medium is not included even though the cavity is defined to be open; a warning message is issued to this effect. You can loosen the viewfactor tolerance to include such radiation. Controlling checks for surface blocking is transferred between surfaces that have unobstructed direct views of each other ; “blocking” may occur in geometrically complex cavities. Surface blocking checks may be computationally expensive in cavities with many surfaces; therefore, significant computational time may be saved by specifying which surfaces are potential blocking surfaces, as described below. Viewfactor calculations with blocking surfaces are especially sensitive to mesh refinement. If a mesh is too coarse, the viewfactors may not add up to one (in a closed cavity). To obtain accurate results, the mesh should be refined until the viewfactors can be summed accurately. Full blocking checks Input File Usage: By default, Abaqus/Standard will check for blocking of every surface with itself and all other surfaces. *RADIATION VIEWFACTOR, BLOCKING=ALL Interaction module: Create interaction: Cavity radiation: Properties: Blocking surface checks: All Abaqus/CAE Usage: Partial blocking checks You can specify a list of the potential blocking surfaces in the cavity. Input File Usage: Abaqus/CAE Usage: *RADIATION VIEWFACTOR, BLOCKING=PARTIAL Interaction module: Create interaction: Cavity radiation: Properties: Blocking surface checks: Partial Cavity with no blocking Example of partial blocking Another example of partial blocking Figure 40.1.1–14 Illustrations of blocking. No blocking checks You can indicate that there are no blocking surfaces in the cavity; in this case Abaqus omits all checks for blocking. Input File Usage: Abaqus/CAE Usage: *RADIATION VIEWFACTOR, BLOCKING=NO Interaction module: Create interaction: Cavity radiation: Properties: Blocking surface checks: None Reducing computations for surfaces that are far apart In cases where there are many surfaces in the cavity, surfaces separated by more than a certain distance may not be able to “see” each other for the purposes of radiation because of blocking by other surfaces. You can specify the distance beyond which viewfactors need not be calculated, which reduces the computational effort required for the viewfactor calculations. Input File Usage: Abaqus/CAE Usage: *RADIATION VIEWFACTOR, RANGE=distance Interaction module: Create interaction: Cavity radiation: Viewfactors: toggle on Specify blocking range: distance Memory usage in cavity radiation analyses The cavity radiation heat transfer between facets of a surface in Abaqus is modeled using a full, unsymmetric matrix defining interactions between each node and all others in the cavity. For surfaces with large numbers of nodes this matrix may be large, resulting in memory requirements that are significantly larger than those for the finite element portion of the analysis without the cavity radiation interaction. To minimize memory requirements and computational cost for cavity radiation heat transfer analysis, the cavity can be defined using a coarser mesh of heat transfer shell elements having a single degree of freedom per node. The overlaid element should have minimal heat capacity and conduction, and it should be used for the definition of the cavity in place of the physical, multiple-degree-of-freedom shell. The overlaid element should be used to define the master surface in a tied coupling constraint (“Mesh tie constraints,” Section 34.3.1); the multiple-degree-of-freedom, physical, heat transfer shell element forms the slave surface. Initial conditions By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures in a cavity radiation analysis; see “Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. In a heat transfer analysis involving forced convection through the mesh, you can define nonzero initial mass flow rates at the nodes of the forced convection/diffusion heat transfer elements in the model . Boundary conditions You can specify boundary conditions to prescribe temperatures (degree of freedom 11) at the nodes . Shell elements have additional temperature degrees of freedom 12, 13, etc. through the thickness . Boundary conditions can be specified as functions of time by referring to amplitude curves (“Amplitude curves,” Section 33.1.2). For purely diffusive elements, a boundary without any prescribed boundary conditions (natural boundary condition) corresponds to an insulated surface. For forced convection/diffusion elements, only the flux associated with conduction is zero; energy is free to convect across an unloaded surface. This natural boundary condition correctly models areas where fluid is crossing a surface (as, for example, at the upstream and downstream boundaries of the mesh) and prevents spurious reflections of energy back into the mesh. Loads The following types of loading can be prescribed in addition to the cavity radiation, as described in “Thermal loads,” Section 33.4.4: • Concentrated heat fluxes • Body fluxes and distributed surface fluxes • Convective film conditions and radiation conditions Predefined fields You cannot specify temperatures as field variables in heat transfer or coupled thermal-electrical analyses. Boundary conditions should be used instead, as described above. You can specify values of other user-defined field variables during the analysis. These values will affect field-variable-dependent material properties, if any. See “Predefined fields,” Section 33.6.1. Material options You must define the radiation properties of the surfaces as described above in “Defining surface radiation properties.” Other thermal properties such as conductivity, density, specific heat, and latent heat are defined as in uncoupled heat transfer analysis—see “Uncoupled heat transfer analysis,” Section 6.5.2, and “Thermal properties: overview,” Section 26.2.1. You can specify internal heat generation—see “Internal heat generation” in “Uncoupled heat transfer analysis,” Section 6.5.2. Thermal expansion coefficients are not meaningful in cavity radiation heat transfer analysis since deformation of the structure is not considered. Elements Any of the heat transfer or coupled thermal-electrical elements in Abaqus/Standard can be used in a cavity radiation analysis, transfer elements . Coupled temperature-displacement and coupled thermal-electrical-structural elements cannot be used in a cavity radiation analysis. including forced convection/diffusion heat In addition to the elements that you define, Abaqus/Standard uses internal elements that are generated automatically from your definition of radiation cavities. Output The following output variables are available for cavity radiation: Surface variables RADFL RADFLA RADTL RADTLA VFTOT FTEMP Radiation flux per unit area. This variable does include heat flux to ambient in an open cavity. Radiation flux over a facet. Time integrated radiation per unit area. Time integrated radiation over a facet. Total viewfactor for a facet (sum of the viewfactor values in the row of the viewfactor matrix corresponding to the facet). Facet temperature. All of the output variables are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Abaqus/CAE supports motion display and can display surface- and element-based results. Writing the viewfactor matrices to the results file You can write the viewfactor matrices for cavity radiation interactions in heat transfer or coupled thermal- electrical analyses to the results (.fil) file if parallel decomposition for the cavity is not enabled.. The entire radiation viewfactor matrix is written for each cavity radiation element in the specified cavity. You can control the frequency of viewfactor matrix output by specifying the required output frequency in increments. The default output frequency is 1. Specify an output frequency of 0 to suppress output. The output will always be written at the last increment of each step unless you specify an output frequency of 0. The record formats for the results file are described in “Results file output format,” Section 5.1.2. The file can be written in binary or ASCII format . Input File Usage: Abaqus/CAE Usage: *VIEWFACTOR OUTPUT, CAVITY=cavity_name, FREQUENCY=n Viewfactor output is not supported in Abaqus/CAE. Requesting surface variable output For the cavity radiation interaction, you can request cavity-, element-, or surface-based radiation output such as radiation fluxes, viewfactor totals for a facet, and facet temperatures to the data, results, and/or output database files. The output requests can be repeated as often as necessary to request output for different variables, different cavities, different surfaces, different element sets, etc. The surface variables that can be requested are listed above. You can specify the particular cavity, element set, or surface for which output is being requested. If you do not specify a cavity, element set, or surface, output will be provided for all cavities in the model. The same cavity, element set, or surface can appear in several radiation output requests. By default, no cavity radiation data output will be provided. If you define a radiation output request without specifying the desired output variables, all six cavity radiation surface variables will be output. You can control the frequency of radiation output by specifying the required output frequency in increments. The default output frequency is 1. Specify an output frequency of 0 to suppress output. The output will always be written at the last increment of each step unless you specify an output frequency of 0. Input File Usage: Use one of the following options to obtain output in the data file: *RADIATION PRINT, CAVITY=cavity_name, FREQUENCY=n *RADIATION PRINT, ELSET=element_set, FREQUENCY=n *RADIATION PRINT, SURFACE=surface_name, FREQUENCY=n Use one of the following options to obtain output in the results file: *RADIATION FILE, CAVITY=cavity_name, FREQUENCY=n *RADIATION FILE, ELSET=element_set, FREQUENCY=n *RADIATION FILE, SURFACE=surface_name, FREQUENCY=n Use the first option and one of the subsequent options to obtain output in the output database: *OUTPUT, FREQUENCY=n *RADIATION OUTPUT, CAVITY=cavity_name *RADIATION OUTPUT, ELSET=element_set *RADIATION OUTPUT, SURFACE=surface_name Cavity radiation output to the data file and the results file are not supported in Abaqus/CAE. Use the following options to obtain output in the output database: Step module: history output request editor: Thermal: select the output variables Abaqus/CAE Usage: Printed output The output tables generated by a radiation output request to the data file are organized on a surface-by- surface basis. The rows that will appear in a particular table are defined by choosing a cavity, surface, or element set: each row of a table corresponds to an individual element face that is part of the cavity, surface, or element set chosen. If all of the variables in a row of a table are zero, the row is not printed. The first column of each table is the element number, and the second column is the element face identifier. You choose the variables to appear in the remaining columns. There is no limit to the number of tables that can be defined. As an example, consider a heat transfer model containing a cavity named CAV1, which, in turn, is composed of surfaces SURF1 and SURF2. If you request output of radiation flux (RADFL) and facet temperature (FTEMP) to the data file for this model, two tables will appear in the data file. One table will contain RADFL and FTEMP output for all element faces composing surface SURF1, and the other table will contain the same output variables for all element faces making up surface SURF2. By default, Abaqus/Standard writes a summary of the maximum and minimum values in each column of the table. You can choose to suppress this summary. In addition, you can choose to print the total of each column in the table, which is useful, for example, to sum radiation fluxes over all facets composing a radiation surface. By default, these totals are not printed. Input File Usage: Use the following option to control output of the summary information to the data file: *RADIATION PRINT, SUMMARY=YES or NO Use the following option to control output of the totals to the data file: Abaqus/CAE Usage: *RADIATION PRINT, TOTALS=YES or NO Cavity radiation output to the data file is not supported in Abaqus/CAE. Input file template The following template shows the options required for a transient, cavity radiation analysis of a closed two-dimensional symmetric cavity. All surfaces within the cavity topcav have the same emissivity. The surface surf2 moves (translation only) during the analysis. In the second step surface surf2 stops moving, cavity radiation is turned off, all thermal loads except the surface convection are removed, and a steady-state heat transfer analysis is conducted to determine the final temperature of the system. *HEADING … *PHYSICAL CONSTANTS, ABSOLUTE ZERO= , STEFAN BOLTZMANN= *SURFACE, NAME=surf1, PROPERTY=surfp elset1, S1 elset2, S2 *SURFACE, NAME=surf2, PROPERTY=surfp elset3, *SURFACE PROPERTY, NAME=surfp *EMISSIVITY Data lines to define the emissivity of the surfaces in the model *CAVITY DEFINITION, NAME=topcav surf1, surf2 *INITIAL CONDITIONS, TYPE=TEMPERATURE Data lines to prescribe initial temperatures at the nodes *AMPLITUDE, NAME=motion Data lines to define amplitude curve to be used for motion of surface surf2 *AMPLITUDE, NAME=film Data lines to define amplitude curve to be used for the convection film coefficient, h ************* ** Step 1 ************* *STEP *HEAT TRANSFER, MXDEM= Data line to define incrementation *RADIATION VIEWFACTOR, CAVITY=topcav, VTOL=tol, SYMMETRY=outer, , DELTMX= NSET=nset, MDISP=max *RADIATION SYMMETRY, NAME=outer *REFLECTION, TYPE=LINE Data line to define line of symmetry *MOTION, TRANSLATION, TYPE=DISPLACEMENT, AMPLITUDE=motion Data line to define motion of nodes on surface surf2 *CFLUX and/or *DFLUX Data lines to define concentrated and/or distributed fluxes *BOUNDARY Data lines to prescribe temperatures at selected nodes *FILM, FILM AMPLITUDE=film Data lines to define surface convection ** *RADIATION PRINT, CAVITY=topcav, SUMMARY=YES, TOTALS=YES Data lines requesting cavity radiation surface variable output *RADIATION FILE, CAVITY=topcav, FREQUENCY=4 Data lines requesting cavity radiation surface variable output *NODE PRINT Data lines requesting nodal output such as temperatures *EL PRINT Data lines requesting element output such as heat flux *END STEP ************* ** Step 2 ************* *STEP *HEAT TRANSFER, STEADY STATE Data line to define incrementation *RADIATION VIEWFACTOR, OFF *CFLUX, OP=NEW *DFLUX, OP=NEW *END STEP SIMULIA is the Dassault Systèmes brand that delivers a scalable portfolio of Realistic Simulation solutions including the Abaqus product suite for Unified Finite Element Analysis; multiphysics solutions for insight into challenging engineering problems; and lifecycle management solutions for managing simulation data, processes, and intellectual property. By building on established technology, respected quality, and superior customer service, SIMULIA makes realistic simulation an integral business practice that improves product performance, reduces physical prototypes, and drives innovation. Headquartered in Providence, RI, USA, with R&D centers in Providence and in Vélizy, France, SIMULIA provides sales, services, and support through a global network of regional offices and distributors. For more information, visit www.simulia.com. About Dassault Systèmes As a world leader in 3D and Product Lifecycle Management (PLM) solutions, Dassault Systèmes brings value to more than 100,000 customers in 80 countries. A pioneer in the 3D software market since 1981, Dassault Systèmes develops and markets PLM application software and services that support industrial processes and provide a 3D vision of the entire lifecycle of products from conception to maintenance to recycling. The Dassault Systèmes portfolio consists of CATIA for designing the virtual product, SolidWorks for 3D mechanical design, DELMIA for virtual production, SIMULIA for virtual testing, ENOVIA for global collaborative lifecycle management, and 3DVIA for online 3D lifelike experiences. Dassault Systèmes’ shares are listed on Euronext Paris (#13065, DSY.PA), and Dassault Systèmes’ ADRs may be traded on the US Over-The-Counter (OTC) market (DASTY). For more information, visit www.3ds.com. fi , , , , , , , , . . , © . , , . / User’s Manual CAUTION: This documentation is intended for qualified users who will exercise sound engineering judgment and expertise in the use of the Abaqus Software. The Abaqus Software is inherently complex, and the examples and procedures in this documentation are not intended to be exhaustive or to apply to any particular situation. Users are cautioned to satisfy themselves as to the accuracy and results of their analyses. Dassault Systèmes and its subsidiaries, including Dassault Systèmes Simulia Corp., shall not be responsible for the accuracy or usefulness of any analysis performed using the Abaqus Software or the procedures, examples, or explanations in this documentation. Dassault Systèmes and its subsidiaries shall not be responsible for the consequences of any errors or omissions that may appear in this documentation. The Abaqus Software is available only under license from Dassault Systèmes or its subsidiary and may be used or reproduced only in accordance with the terms of such license. This documentation is subject to the terms and conditions of either the software license agreement signed by the parties, or, absent such an agreement, the then current software license agreement to which the documentation relates. This documentation and the software described in this documentation are subject to change without prior notice. No part of this documentation may be reproduced or distributed in any form without prior written permission of Dassault Systèmes or its subsidiary. The Abaqus Software is a product of Dassault Systèmes Simulia Corp., Providence, RI, USA. © Dassault Systèmes, 2012 Abaqus, the 3DS logo, SIMULIA, CATIA, and Unified FEA are trademarks or registered trademarks of Dassault Systèmes or its subsidiaries in the United States and/or other countries. Other company, product, and service names may be trademarks or service marks of their respective owners. For additional information concerning SIMULIA European Headquarters Fax: +1 401 276 4408, simulia.support@3ds.com, http://www.simulia.com Stationsplein 8-K, 6221 BT Maastricht, The Netherlands, Tel: +31 43 7999 084, Fax: +31 43 7999 306, simulia.europe.info@3ds.com Locations United States Australia Austria Benelux Canada China Finland France Germany India Italy Japan Korea Latin America Scandinavia United Kingdom Argentina Brazil Czech & Slovak Republics Greece Israel Malaysia Mexico New Zealand Poland Russia, Belarus & Ukraine Singapore South Africa Spain & Portugal Dassault Systèmes’ Centers of Simulation Excellence Fremont, CA, Tel: +1 510 794 5891, simulia.west.support@3ds.com West Lafayette, IN, Tel: +1 765 497 1373, simulia.central.support@3ds.com Northville, MI, Tel: +1 248 349 4669, simulia.greatlakes.info@3ds.com Woodbury, MN, Tel: +1 612 424 9044, simulia.central.support@3ds.com Mayfield Heights, OH, Tel: +1 216 378 1070, simulia.erie.info@3ds.com Mason, OH, Tel: +1 513 275 1430, simulia.central.support@3ds.com Warwick, RI, Tel: +1 401 739 3637, simulia.east.support@3ds.com Lewisville, TX, Tel: +1 972 221 6500, simulia.south.info@3ds.com Richmond VIC, Tel: +61 3 9421 2900, simulia.au.support@3ds.com Vienna, Tel: +43 1 22 707 200, simulia.at.info@3ds.com Maarssen, The Netherlands, Tel: +31 346 585 710, simulia.benelux.support@3ds.com Toronto, ON, Tel: +1 416 402 2219, simulia.greatlakes.info@3ds.com Beijing, P. R. China, Tel: +8610 6536 2288, simulia.cn.support@3ds.com Shanghai, P. R. China, Tel: +8621 3856 8000, simulia.cn.support@3ds.com Espoo, Tel: +358 40 902 2973, simulia.nordic.info@3ds.com Velizy Villacoublay Cedex, Tel: +33 1 61 62 72 72, simulia.fr.support@3ds.com Aachen, Tel: +49 241 474 01 0, simulia.de.info@3ds.com Munich, Tel: +49 89 543 48 77 0, simulia.de.info@3ds.com Chennai, Tamil Nadu, Tel: +91 44 43443000, simulia.in.info@3ds.com Lainate MI, Tel: +39 02 3343061, simulia.ity.info@3ds.com Tokyo, Tel: +81 3 5442 6302, simulia.jp.support@3ds.com Osaka, Tel: +81 6 7730 2703, simulia.jp.support@3ds.com Mapo-Gu, Seoul, Tel: +82 2 785 6707/8, simulia.kr.info@3ds.com Puerto Madero, Buenos Aires, Tel: +54 11 4312 8700, Horacio.Burbridge@3ds.com Stockholm, Sweden, Tel: +46 8 68430450, simulia.nordic.info@3ds.com Warrington, Tel: +44 1925 830900, simulia.uk.info@3ds.com Authorized Support Centers SMARTtech Sudamerica SRL, Buenos Aires, Tel: +54 11 4717 2717 KB Engineering, Buenos Aires, Tel: +54 11 4326 7542 Solaer Ingeniería, Buenos Aires, Tel: +54 221 489 1738 SMARTtech Mecânica, Sao Paulo-SP, Tel: +55 11 3168 3388 Synerma s. r. o., Psáry, Prague-West, Tel: +420 603 145 769, abaqus@synerma.cz 3 Dimensional Data Systems, Crete, Tel: +30 2821040012, support@3dds.gr ADCOM, Givataim, Tel: +972 3 7325311, shmulik.keidar@adcomsim.co.il WorleyParsons Services Sdn. Bhd., Kuala Lumpur, Tel: +603 2039 9000, abaqus.my@worleyparsons.com Kimeca.NET SA de CV, Mexico, Tel: +52 55 2459 2635 Matrix Applied Computing Ltd., Auckland, Tel: +64 9 623 1223, abaqus-tech@matrix.co.nz BudSoft Sp. z o.o., Poznań, Tel: +48 61 8508 466, info@budsoft.com.pl TESIS Ltd., Moscow, Tel: +7 495 612 44 22, info@tesis.com.ru WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com Finite Element Analysis Services (Pty) Ltd., Parklands, Tel: +27 21 556 6462, feas@feas.co.za Thailand Turkey Simutech Solution Corporation, Taipei, R.O.C., Tel: +886 2 2507 9550, camilla@simutech.com.tw WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com A-Ztech Ltd., Istanbul, Tel: +90 216 361 8850, info@a-ztech.com.tr Preface Support Both technical engineering support (for problems with creating a model or performing an analysis) and systems support (for installation, licensing, and hardware-related problems) for Abaqus are offered through a network of local support offices. Regional contact information is listed in the front of each Abaqus manual and is accessible from the Locations page at www.simulia.com. Support for SIMULIA products SIMULIA provides a knowledge database of answers and solutions to questions that we have answered, as well as guidelines on how to use Abaqus, SIMULIA Scenario Definition, Isight, and other SIMULIA products. You can also submit new requests for support. All support incidents are tracked. If you contact us by means outside the system to discuss an existing support problem and you know the incident or support request number, please mention it so that we can query the database to see what the latest action has been. Many questions about Abaqus can also be answered by visiting the Products page and the Support page at www.simulia.com. Anonymous ftp site To facilitate data transfer with SIMULIA, an anonymous ftp account is available at ftp.simulia.com. Login as user anonymous, and type your e-mail address as your password. Contact support before placing files on the site. Training All offices and representatives offer regularly scheduled public training classes. The courses are offered in a traditional classroom form and via the Web. We also provide training seminars at customer sites. All training classes and seminars include workshops to provide as much practical experience with Abaqus as possible. For a schedule and descriptions of available classes, see www.simulia.com or call your local office or representative. Feedback We welcome any suggestions for improvements to Abaqus software, the support program, or documentation. We will ensure that any enhancement requests you make are considered for future releases. If you wish to make a suggestion about the service or products, refer to www.simulia.com. Complaints should be made by contacting your local office or through www.simulia.com by visiting the Quality Assurance section of the 1.1.1 1.2.1 1.2.2 1.3.1 1.4.1 2.1.1 2.1.2 2.1.3 2.1.4 2.1.5 2.1.6 2.2.1 2.2.2 2.2.3 2.2.4 2.2.5 2.3.1 2.3.2 2.3.3 2.3.4 Contents Volume I PART I INTRODUCTION, SPATIAL MODELING, AND EXECUTION 1. Introduction Introduction: general Abaqus syntax and conventions Input syntax rules Conventions Abaqus model definition Defining a model in Abaqus Parametric modeling Parametric input 2. Spatial Modeling Node definition Node definition Parametric shape variation Nodal thicknesses Normal definitions at nodes Transformed coordinate systems Adjusting nodal coordinates Element definition Element definition Element foundations Defining reinforcement Defining rebar as an element property Orientations Surface definition Surfaces: overview Element-based surface definition Node-based surface definition Analytical rigid surface definition Eulerian surface definition Operating on surfaces Rigid body definition Rigid body definition Integrated output section definition Integrated output section definition Mass adjustment Adjust and/or redistribute mass of an element set Nonstructural mass definition Nonstructural mass definition Distribution definition Distribution definition Display body definition Display body definition Assembly definition Defining an assembly Matrix definition Defining matrices 3. Job Execution Execution procedures: overview Execution procedure for Abaqus: overview Execution procedures Obtaining information Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution SIMULIA Co-Simulation Engine controller execution Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution Abaqus/CAE execution Abaqus/Viewer execution Python execution Parametric studies Abaqus documentation Licensing utilities ASCII translation of results (.fil) files Joining results (.fil) files Querying the keyword/problem database ii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 2.3.5 2.3.6 2.4.1 2.5.1 2.6.1 2.7.1 2.8.1 2.9.1 2.10.1 2.11.1 3.1.1 3.2.1 3.2.2 3.2.3 3.2.4 3.2.5 3.2.6 3.2.7 3.2.8 3.2.9 3.2.10 Making user-defined executables and subroutines Input file and output database upgrade utility Generating output database reports Joining output database (.odb) files from restarted analyses Combining output from substructures Combining data from multiple output databases Network output database file connector Mapping thermal and magnetic loads Fixed format conversion utility Translating Nastran bulk data files to Abaqus input files Translating Abaqus files to Nastran bulk data files Translating ANSYS input files to Abaqus input files Translating PAM-CRASH input files to partial Abaqus input files Translating RADIOSS input files to partial Abaqus input files Translating Abaqus output database files to Nastran Output2 results files Translating LS-DYNA data files to Abaqus input files Exchanging Abaqus data with ZAERO Encrypting and decrypting Abaqus input data Job execution control Environment file settings Using the Abaqus environment settings Managing memory and disk resources Managing memory and disk use in Abaqus Parallel execution Parallel execution: overview Parallel execution in Abaqus/Standard Parallel execution in Abaqus/Explicit Parallel execution in Abaqus/CFD File extension definitions File extensions used by Abaqus FORTRAN unit numbers FORTRAN unit numbers used by Abaqus CONTENTS 3.2.14 3.2.15 3.2.16 3.2.17 3.2.18 3.2.19 3.2.20 3.2.21 3.2.22 3.2.23 3.2.24 3.2.25 3.2.26 3.2.27 3.2.28 3.2.29 3.2.30 3.2.31 3.2.32 3.2.33 3.3.1 3.4.1 3.5.1 3.5.2 3.5.3 3.5.4 3.6.1 3.7.1 4.1.2 4.1.3 4.1.4 4.2.1 4.2.2 4.2.3 4.3.1 5.1.1 5.1.2 5.1.3 5.1.4 CONTENTS 4. Output PART II OUTPUT Output Output to the data and results files Output to the output database Error indicator output Output variables Abaqus/Standard output variable identifiers Abaqus/Explicit output variable identifiers Abaqus/CFD output variable identifiers The postprocessing calculator The postprocessing calculator 5. File Output Format Accessing the results file Accessing the results file: overview Results file output format Accessing the results file information Utility routines for accessing the results file OI.1 Abaqus/Standard Output Variable Index OI.2 Abaqus/Explicit Output Variable Index OI.3 Abaqus/CFD Output Variable Index 6.1.1 6.1.2 6.1.3 6.1.4 6.1.5 6.1.6 6.2.1 6.2.2 6.2.3 6.2.4 6.2.5 6.2.6 6.2.7 6.3.1 6.3.2 6.3.3 6.3.4 6.3.5 6.3.6 6.3.7 6.3.8 6.3.9 6.3.10 6.3.11 6.4.1 6.5.1 6.5.2 Volume II PART III ANALYSIS PROCEDURES, SOLUTION, AND CONTROL 6. Analysis Procedures Introduction Solving analysis problems: overview Defining an analysis General and linear perturbation procedures Multiple load case analysis Direct linear equation solver Iterative linear equation solver Static stress/displacement analysis Static stress analysis procedures: overview Static stress analysis Eigenvalue buckling prediction Unstable collapse and postbuckling analysis Quasi-static analysis Direct cyclic analysis Low-cycle fatigue analysis using the direct cyclic approach Dynamic stress/displacement analysis Dynamic analysis procedures: overview Implicit dynamic analysis using direct integration Explicit dynamic analysis Direct-solution steady-state dynamic analysis Natural frequency extraction Complex eigenvalue extraction Transient modal dynamic analysis Mode-based steady-state dynamic analysis Subspace-based steady-state dynamic analysis Response spectrum analysis Random response analysis Steady-state transport analysis Steady-state transport analysis Heat transfer and thermal-stress analysis Heat transfer analysis procedures: overview Uncoupled heat transfer analysis 6.5.4 6.6.1 6.6.2 6.7.1 6.7.2 6.7.3 6.7.4 6.7.5 6.7.6 6.8.1 6.8.2 6.9.1 6.10.1 6.11.1 6.12.1 7.1.1 7.2.1 7.2.2 7.2.3 7.2.4 CONTENTS Fully coupled thermal-stress analysis Adiabatic analysis Fluid dynamic analysis Fluid dynamic analysis procedures: overview Incompressible fluid dynamic analysis Electromagnetic analysis Electromagnetic analysis procedures Piezoelectric analysis Coupled thermal-electrical analysis Fully coupled thermal-electrical-structural analysis Eddy current analysis Magnetostatic analysis Coupled pore fluid flow and stress analysis Coupled pore fluid diffusion and stress analysis Geostatic stress state Mass diffusion analysis Mass diffusion analysis Acoustic and shock analysis Acoustic, shock, and coupled acoustic-structural analysis Abaqus/Aqua analysis Abaqus/Aqua analysis Annealing Annealing procedure 7. Analysis Solution and Control Solving nonlinear problems Solving nonlinear problems Analysis convergence controls Convergence and time integration criteria: overview Commonly used control parameters Convergence criteria for nonlinear problems Time integration accuracy in transient problems ANALYSIS TECHNIQUES 8. Analysis Techniques: Introduction Analysis techniques: overview 9. Analysis Continuation Techniques Restarting an analysis Restarting an analysis Importing and transferring results Transferring results between Abaqus analyses: overview Transferring results between Abaqus/Explicit and Abaqus/Standard Transferring results from one Abaqus/Standard analysis to another Transferring results from one Abaqus/Explicit analysis to another 10. Modeling Abstractions Substructuring Using substructures Defining substructures Submodeling Submodeling: overview Node-based submodeling Surface-based submodeling Generating global matrices Generating matrices CONTENTS 8.1.1 9.1.1 9.2.1 9.2.2 9.2.3 9.2.4 10.1.1 10.1.2 10.2.1 10.2.2 10.2.3 10.3.1 Symmetric model generation, results transfer, and analysis of cyclic symmetry models Symmetric model generation Transferring results from a symmetric mesh or a partial three-dimensional mesh to a full three-dimensional mesh Analysis of models that exhibit cyclic symmetry Periodic media analysis Periodic media analysis Meshed beam cross-sections Meshed beam cross-sections vii 10.4.1 10.4.2 10.4.3 10.5.1 Modeling discontinuities as an enriched feature using the extended finite element method Modeling discontinuities as an enriched feature using the extended finite element 10.7.1 11.1.1 11.2.1 11.3.1 11.4.1 11.4.2 11.4.3 11.5.1 11.5.2 11.5.3 11.5.4 11.6.1 11.7.1 11.8.1 12.1.1 12.2.1 12.2.2 12.2.3 12.2.4 method 11. Special-Purpose Techniques Inertia relief Inertia relief Mesh modification or replacement Element and contact pair removal and reactivation Geometric imperfections Introducing a geometric imperfection into a model Fracture mechanics Fracture mechanics: overview Contour integral evaluation Crack propagation analysis Surface-based fluid modeling Surface-based fluid cavities: overview Fluid cavity definition Fluid exchange definition Inflator definition Mass scaling Mass scaling Selective subcycling Selective subcycling Steady-state detection Steady-state detection 12. Adaptivity Techniques Adaptivity techniques: overview Adaptivity techniques ALE adaptive meshing ALE adaptive meshing: overview Defining ALE adaptive mesh domains in Abaqus/Explicit ALE adaptive meshing and remapping in Abaqus/Explicit Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit 12.2.5 12.2.6 12.2.7 12.3.1 12.3.2 12.3.3 12.4.1 13.1.1 13.2.1 13.2.2 13.2.3 14.1.1 14.1.2 14.1.3 14.1.4 15.1.1 15.1.2 16.1.1 16.1.2 16.1.3 17.1.1 17.2.1 Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit Defining ALE adaptive mesh domains in Abaqus/Standard ALE adaptive meshing and remapping in Abaqus/Standard Adaptive remeshing Adaptive remeshing: overview Selection of error indicators influencing adaptive remeshing Solution-based mesh sizing Analysis continuation after mesh replacement Mesh-to-mesh solution mapping 13. Optimization Techniques Structural optimization: overview Structural optimization: overview Optimization models Design responses Objectives and constraints Creating Abaqus optimization models 14. Eulerian Analysis Eulerian analysis Defining Eulerian boundaries Eulerian mesh motion Defining adaptive mesh refinement in the Eulerian domain 15. Particle Methods Smoothed particle hydrodynamic analyses Smoothed particle hydrodynamic analysis Finite element conversion to SPH particles 16. Sequentially Coupled Multiphysics Analyses Predefined fields for sequential coupling Sequentially coupled thermal-stress analysis Predefined loads for sequential coupling 17. Co-simulation Co-simulation: overview Preparing an Abaqus analysis for co-simulation Preparing an Abaqus analysis for co-simulation Co-simulation between Abaqus solvers Abaqus/Standard to Abaqus/Explicit co-simulation Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation 18. Extending Abaqus Analysis Functionality User subroutines and utilities User subroutines: overview Available user subroutines Available utility routines 19. Design Sensitivity Analysis Design sensitivity analysis 20. Parametric Studies Scripting parametric studies Scripting parametric studies Parametric studies: commands aStudy.combine(): Combine parameter samples for parametric studies. aStudy.constrain(): Constrain parameter value combinations in parametric studies. aStudy.define(): Define parameters for parametric studies. aStudy.execute(): Execute the analysis of parametric study designs. aStudy.gather(): Gather the results of a parametric study. aStudy.generate(): Generate the analysis job data for a parametric study. aStudy.output(): Specify the source of parametric study results. aStudy=ParStudy(): Create a parametric study. aStudy.report(): Report parametric study results. aStudy.sample(): Sample parameters for parametric studies. 17.3.1 17.3.2 18.1.1 18.1.2 18.1.3 19.1.1 20.1.1 20.2.1 20.2.2 20.2.3 20.2.4 20.2.5 20.2.6 20.2.7 20.2.8 20.2.9 20.2.10 21.1.1 21.1.2 21.1.3 21.2.1 22.1.1 22.2.1 22.2.2 22.2.3 22.3.1 22.4.1 22.5.1 22.5.2 22.5.3 22.6.1 22.6.2 22.7.1 22.7.2 Volume III PART V MATERIALS 21. Materials: Introduction Introduction Material library: overview Material data definition Combining material behaviors General properties Density 22. Elastic Mechanical Properties Overview Elastic behavior: overview Linear elasticity Linear elastic behavior No compression or no tension Plane stress orthotropic failure measures Porous elasticity Elastic behavior of porous materials Hypoelasticity Hypoelastic behavior Hyperelasticity Hyperelastic behavior of rubberlike materials Hyperelastic behavior in elastomeric foams Anisotropic hyperelastic behavior Stress softening in elastomers Mullins effect Energy dissipation in elastomeric foams Viscoelasticity Time domain viscoelasticity Frequency domain viscoelasticity Nonlinear viscoelasticity Hysteresis in elastomers Parallel network viscoelastic model Rate sensitive elastomeric foams Low-density foams 23. Inelastic Mechanical Properties Overview Inelastic behavior Metal plasticity Classical metal plasticity Models for metals subjected to cyclic loading Rate-dependent yield Rate-dependent plasticity: creep and swelling Annealing or melting Anisotropic yield/creep Johnson-Cook plasticity Dynamic failure models Porous metal plasticity Cast iron plasticity Two-layer viscoplasticity ORNL – Oak Ridge National Laboratory constitutive model Deformation plasticity Other plasticity models Extended Drucker-Prager models Modified Drucker-Prager/Cap model Mohr-Coulomb plasticity Critical state (clay) plasticity model Crushable foam plasticity models Fabric materials Fabric material behavior Jointed materials Jointed material model Concrete Concrete smeared cracking Cracking model for concrete Concrete damaged plasticity xii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 22.8.1 22.8.2 22.9.1 23.1.1 23.2.1 23.2.2 23.2.3 23.2.4 23.2.5 23.2.6 23.2.7 23.2.8 23.2.9 23.2.10 23.2.11 23.2.12 23.2.13 23.3.1 23.3.2 23.3.3 23.3.4 23.3.5 23.4.1 23.5.1 23.7.1 24.1.1 24.2.1 24.2.2 24.2.3 24.3.1 24.3.2 24.3.3 24.4.1 24.4.2 24.4.3 25.1.1 25.2.1 26.1.1 26.1.2 26.1.3 26.1.4 26.2.1 26.2.2 26.2.3 26.2.4 Permanent set in rubberlike materials Permanent set in rubberlike materials 24. Progressive Damage and Failure Progressive damage and failure: overview Progressive damage and failure Damage and failure for ductile metals Damage and failure for ductile metals: overview Damage initiation for ductile metals Damage evolution and element removal for ductile metals Damage and failure for fiber-reinforced composites Damage and failure for fiber-reinforced composites: overview Damage initiation for fiber-reinforced composites Damage evolution and element removal for fiber-reinforced composites Damage and failure for ductile materials in low-cycle fatigue analysis Damage and failure for ductile materials in low-cycle fatigue analysis: overview Damage initiation for ductile materials in low-cycle fatigue Damage evolution for ductile materials in low-cycle fatigue 25. Hydrodynamic Properties Overview Hydrodynamic behavior: overview Equations of state Equation of state 26. Other Material Properties Mechanical properties Material damping Thermal expansion Field expansion Viscosity Heat transfer properties Thermal properties: overview Conductivity Specific heat Latent heat Acoustic properties Acoustic medium Mass diffusion properties Diffusivity Solubility Electromagnetic properties Electrical conductivity Piezoelectric behavior Magnetic permeability Pore fluid flow properties Pore fluid flow properties Permeability Porous bulk moduli Sorption Swelling gel Moisture swelling User materials User-defined mechanical material behavior User-defined thermal material behavior 26.3.1 26.4.1 26.4.2 26.5.1 26.5.2 26.5.3 26.6.1 26.6.2 26.6.3 26.6.4 26.6.5 26.6.6 26.7.1 26.7.2 27.1.1 27.1.2 27.1.3 27.1.4 28.1.1 28.1.2 28.1.3 28.1.4 28.1.5 28.1.6 28.1.7 28.2.1 28.2.2 28.3.1 28.3.2 28.4.1 28.4.2 28.5.1 28.5.2 29.1.1 29.1.2 29.1.3 Volume IV PART VI ELEMENTS 27. Elements: Introduction Element library: overview Choosing the element’s dimensionality Choosing the appropriate element for an analysis type Section controls 28. Continuum Elements General-purpose continuum elements Solid (continuum) elements One-dimensional solid (link) element library Two-dimensional solid element library Three-dimensional solid element library Cylindrical solid element library Axisymmetric solid element library Axisymmetric solid elements with nonlinear, asymmetric deformation Fluid continuum elements Fluid (continuum) elements Fluid element library Infinite elements Infinite elements Infinite element library Warping elements Warping elements Warping element library Particle elements Particle elements Particle element library 29. Structural Elements Membrane elements Membrane elements General membrane element library Cylindrical membrane element library Axisymmetric membrane element library Truss elements Truss elements Truss element library Beam elements Beam modeling: overview Choosing a beam cross-section Choosing a beam element Beam element cross-section orientation Beam section behavior Using a beam section integrated during the analysis to define the section behavior Using a general beam section to define the section behavior Beam element library Beam cross-section library Frame elements Frame elements Frame section behavior Frame element library Elbow elements Pipes and pipebends with deforming cross-sections: elbow elements Elbow element library Shell elements Shell elements: overview Choosing a shell element Defining the initial geometry of conventional shell elements Shell section behavior Using a shell section integrated during the analysis to define the section behavior Using a general shell section to define the section behavior Three-dimensional conventional shell element library Continuum shell element library Axisymmetric shell element library Axisymmetric shell elements with nonlinear, asymmetric deformation 29.1.4 29.2.1 29.2.2 29.3.1 29.3.2 29.3.3 29.3.4 29.3.5 29.3.6 29.3.7 29.3.8 29.3.9 29.4.1 29.4.2 29.4.3 29.5.1 29.5.2 29.6.1 29.6.2 29.6.3 29.6.4 29.6.5 29.6.6 29.6.7 29.6.8 29.6.9 29.6.10 30.1.1 30.1.2 30.2.1 30.2.2 30.3.1 30.3.2 30.4.1 30.4.2 31.1.1 31.1.2 31.1.3 31.1.4 31.1.5 31.2.1 31.2.2 31.2.3 31.2.4 31.2.5 31.2.6 31.2.7 31.2.8 31.2.9 31.2.10 32.1.1 32.1.2 30. Inertial, Rigid, and Capacitance Elements Point mass elements Point masses Mass element library Rotary inertia elements Rotary inertia Rotary inertia element library Rigid elements Rigid elements Rigid element library Capacitance elements Point capacitance Capacitance element library 31. Connector Elements Connector elements Connectors: overview Connector elements Connector actuation Connector element library Connection-type library Connector element behavior Connector behavior Connector elastic behavior Connector damping behavior Connector functions for coupled behavior Connector friction behavior Connector plastic behavior Connector damage behavior Connector stops and locks Connector failure behavior Connector uniaxial behavior 32. Special-Purpose Elements Spring elements Springs Spring element library Dashpot elements Dashpots Dashpot element library Flexible joint elements Flexible joint element Flexible joint element library Distributing coupling elements Distributing coupling elements Distributing coupling element library Cohesive elements Cohesive elements: overview Choosing a cohesive element Modeling with cohesive elements Defining the cohesive element’s initial geometry Defining the constitutive response of cohesive elements using a continuum approach Defining the constitutive response of cohesive elements using a traction-separation description Defining the constitutive response of fluid within the cohesive element gap Two-dimensional cohesive element library Three-dimensional cohesive element library Axisymmetric cohesive element library Gasket elements Gasket elements: overview Choosing a gasket element Including gasket elements in a model Defining the gasket element’s initial geometry Defining the gasket behavior using a material model Defining the gasket behavior directly using a gasket behavior model Two-dimensional gasket element library Three-dimensional gasket element library Axisymmetric gasket element library Surface elements Surface elements General surface element library Cylindrical surface element library Axisymmetric surface element library 32.2.1 32.2.2 32.3.1 32.3.2 32.4.1 32.4.2 32.5.1 32.5.2 32.5.3 32.5.4 32.5.5 32.5.6 32.5.7 32.5.8 32.5.9 32.5.10 32.6.1 32.6.2 32.6.3 32.6.4 32.6.5 32.6.6 32.6.7 32.6.8 32.6.9 32.7.1 32.7.2 32.7.3 32.7.4 32.8.1 32.8.2 32.9.1 32.9.2 32.10.1 32.10.2 32.11.1 32.11.2 32.12.1 32.12.2 32.13.1 32.13.2 32.14.1 32.14.2 32.15.1 32.15.2 Tube support elements Tube support elements Tube support element library Line spring elements Line spring elements for modeling part-through cracks in shells Line spring element library Elastic-plastic joints Elastic-plastic joints Elastic-plastic joint element library Drag chain elements Drag chains Drag chain element library Pipe-soil elements Pipe-soil interaction elements Pipe-soil interaction element library Acoustic interface elements Acoustic interface elements Acoustic interface element library Eulerian elements Eulerian elements Eulerian element library User-defined elements User-defined elements User-defined element library EI.1 Abaqus/Standard Element Index EI.2 Abaqus/Explicit Element Index EI.3 Abaqus/CFD Element Index Volume V PART VII PRESCRIBED CONDITIONS 33. Prescribed Conditions Overview Prescribed conditions: overview Amplitude curves Initial conditions Initial conditions in Abaqus/Standard and Abaqus/Explicit Initial conditions in Abaqus/CFD Boundary conditions Boundary conditions in Abaqus/Standard and Abaqus/Explicit Boundary conditions in Abaqus/CFD Loads Applying loads: overview Concentrated loads Distributed loads Thermal loads Electromagnetic loads Acoustic and shock loads Pore fluid flow Prescribed assembly loads Prescribed assembly loads Predefined fields Predefined fields PART VIII CONSTRAINTS 34. Constraints Overview Kinematic constraints: overview Multi-point constraints Linear constraint equations xx Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 33.1.1 33.1.2 33.2.1 33.2.2 33.3.1 33.3.2 33.4.1 33.4.2 33.4.3 33.4.4 33.4.5 33.4.6 33.4.7 33.5.1 34.2.2 34.2.3 34.3.1 34.3.2 34.3.3 34.3.4 34.4.1 34.5.1 34.6.1 35.1.1 35.2.1 35.2.2 35.2.3 35.2.4 35.2.5 35.2.6 35.3.1 35.3.2 35.3.3 35.3.4 35.3.5 35.3.6 35.3.7 35.3.8 General multi-point constraints Kinematic coupling constraints Surface-based constraints Mesh tie constraints Coupling constraints Shell-to-solid coupling Mesh-independent fasteners Embedded elements Embedded elements Element end release Element end release Overconstraint checks Overconstraint checks PART IX INTERACTIONS 35. Defining Contact Interactions Overview Contact interaction analysis: overview Defining general contact in Abaqus/Standard Defining general contact interactions in Abaqus/Standard Surface properties for general contact in Abaqus/Standard Contact properties for general contact in Abaqus/Standard Controlling initial contact status in Abaqus/Standard Stabilization for general contact in Abaqus/Standard Numerical controls for general contact in Abaqus/Standard Defining contact pairs in Abaqus/Standard Defining contact pairs in Abaqus/Standard Assigning surface properties for contact pairs in Abaqus/Standard Assigning contact properties for contact pairs in Abaqus/Standard Modeling contact interference fits in Abaqus/Standard Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs Adjusting contact controls in Abaqus/Standard Defining tied contact in Abaqus/Standard Extending master surfaces and slide lines Contact modeling if substructures are present Contact modeling if asymmetric-axisymmetric elements are present Defining general contact in Abaqus/Explicit Defining general contact interactions in Abaqus/Explicit Assigning surface properties for general contact in Abaqus/Explicit Assigning contact properties for general contact in Abaqus/Explicit Controlling initial contact status for general contact in Abaqus/Explicit Contact controls for general contact in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit Assigning surface properties for contact pairs in Abaqus/Explicit Assigning contact properties for contact pairs in Abaqus/Explicit Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit Contact controls for contact pairs in Abaqus/Explicit 36. Contact Property Models Mechanical contact properties Mechanical contact properties: overview Contact pressure-overclosure relationships Contact damping Contact blockage Frictional behavior User-defined interfacial constitutive behavior Pressure penetration loading Interaction of debonded surfaces Breakable bonds Surface-based cohesive behavior Thermal contact properties Thermal contact properties Electrical contact properties Electrical contact properties Pore fluid contact properties Pore fluid contact properties 37. Contact Formulations and Numerical Methods Contact formulations and numerical methods in Abaqus/Standard Contact formulations in Abaqus/Standard xxii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 35.3.9 35.3.10 35.4.1 35.4.2 35.4.3 35.4.4 35.4.5 35.5.1 35.5.2 35.5.3 35.5.4 35.5.5 36.1.1 36.1.2 36.1.3 36.1.4 36.1.5 36.1.6 36.1.7 36.1.8 36.1.9 36.1.10 36.2.1 37.1.2 37.1.3 37.2.1 37.2.2 37.2.3 38.1.1 38.1.2 38.2.1 38.2.2 39.1.1 39.2.1 39.2.2 39.3.1 39.3.2 39.4.1 39.4.2 39.5.1 39.5.2 40.1.1 Contact constraint enforcement methods in Abaqus/Standard Smoothing contact surfaces in Abaqus/Standard Contact formulations and numerical methods in Abaqus/Explicit Contact formulation for general contact in Abaqus/Explicit Contact formulations for contact pairs in Abaqus/Explicit Contact constraint enforcement methods in Abaqus/Explicit 38. Contact Difficulties and Diagnostics Resolving contact difficulties in Abaqus/Standard Contact diagnostics in an Abaqus/Standard analysis Common difficulties associated with contact modeling in Abaqus/Standard Resolving contact difficulties in Abaqus/Explicit Contact diagnostics in an Abaqus/Explicit analysis Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit 39. Contact Elements in Abaqus/Standard Contact modeling with elements Contact modeling with elements Gap contact elements Gap contact elements Gap element library Tube-to-tube contact elements Tube-to-tube contact elements Tube-to-tube contact element library Slide line contact elements Slide line contact elements Axisymmetric slide line element library Rigid surface contact elements Rigid surface contact elements Axisymmetric rigid surface contact element library 40. Defining Cavity Radiation in Abaqus/Standard Cavity radiation Printed on: • Chapter 21, “Materials: Introduction” • Chapter 22, “Elastic Mechanical Properties” • Chapter 23, “Inelastic Mechanical Properties” • Chapter 24, “Progressive Damage and Failure” • Chapter 25, “Hydrodynamic Properties” 21. Materials: Introduction Introduction General properties 21.1 21.1 Introduction • “Material library: overview,” Section 21.1.1 • “Material data definition,” Section 21.1.2 • “Combining material behaviors,” Section 21.1.3 21.1.1 MATERIAL LIBRARY: OVERVIEW This chapter describes how to define materials in Abaqus and contains brief descriptions of each of the material behaviors provided. Further details of the more advanced behaviors are provided in the Abaqus Theory Manual. Defining materials Materials are defined by: • selecting material behaviors and defining them (“Material data definition,” Section 21.1.2); and • combining complementary material behaviors such as elasticity and plasticity (“Combining material behaviors,” Section 21.1.3). A local coordinate system can be used for material calculations (“Orientations,” Section 2.2.5). Any anisotropic properties must be given in this local system. Available material behaviors The material library in Abaqus is intended to provide comprehensive coverage of both linear and nonlinear, isotropic and anisotropic material behaviors. The use of numerical integration in the elements, including numerical integration across the cross-sections of shells and beams, provides the flexibility to analyze the most complex composite structures. Material behaviors fall into the following general categories: • general properties (material damping, density, thermal expansion); • elastic mechanical properties; • inelastic mechanical properties; • thermal properties; • acoustic properties; • hydrostatic fluid properties; • equations of state; • mass diffusion properties; • electrical properties; and • pore fluid flow properties. Some of the mechanical behaviors offered are mutually exclusive: such behaviors cannot appear together in a single material definition. Some behaviors require the presence of other behaviors; for example, plasticity requires linear elasticity. Such requirements are discussed at the end of each material behavior description, as well as in “Combining material behaviors,” Section 21.1.3. Using material behaviors with various element types There are no general restrictions on the use of particular material behaviors with solid, shell, beam, and pipe elements. Any combination that makes sense is acceptable. The few restrictions that do exist are mentioned when that particular behavior is described in the pages that follow. A section on the elements available for use with a material behavior appears at the end of each material behavior description. Using complete material definitions A material definition can include behaviors that are not meaningful for the elements or analysis in which the material is being used. Such behaviors will be ignored. For example, a material definition can include heat transfer properties (conductivity, specific heat) as well as stress-strain properties (elastic moduli, yield stress, etc). When this material definition is used with uncoupled stress/displacement elements, the heat transfer properties are ignored by Abaqus; when it is used with heat transfer elements, the mechanical strength properties are ignored. This capability allows you to develop complete material definitions and use them in any analysis. Defining spatially varying material behavior for homogenous solid continuum elements using distributions in Abaqus/Standard In Abaqus/Standard spatially varying mass density (“Density,” Section 21.2.1), linear elastic behavior (“Linear elastic behavior,” Section 22.2.1), and thermal expansion (“Thermal expansion,” Section 26.1.2) can be defined for homogeneous solid continuum elements using distributions (“Distribution definition,” Section 2.8.1). Using distributions in a model with significant variation in material behavior can greatly simplify pre- and postprocessing and improve performance during the analysis by allowing a single material definition to define the spatially varying material behavior. Without distributions such a model may require many material definitions and associated section assignments. 21.1.2 MATERIAL DATA DEFINITION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Combining material behaviors,” Section 21.1.3 • *MATERIAL • “Creating materials,” Section 12.4.1 of the Abaqus/CAE User’s Manual Overview A material definition in Abaqus: • specifies the behavior of a material and supplies all the relevant property data; • can contain multiple material behaviors; • is assigned a name, which is used to refer to those parts of the model that are made of that material; • can have temperature and/or field variable dependence; • can have solution variable dependence in Abaqus/Standard; and • can be specified in a local coordinate system (“Orientations,” Section 2.2.5), which is required if the material is not isotropic. Material definitions Any number of materials can be defined in an analysis. Each material definition can contain any number of material behaviors, as required, to specify the complete material behavior. For example, in a linear static stress analysis only elastic material behavior may be needed, while in a more complicated analysis several material behaviors may be required. A name must be assigned to each material definition. This name allows the material to be referenced Input File Usage: from the section definitions used to assign this material to regions in the model. *MATERIAL, NAME=name Each material definition is specified in a data block, which is initiated by a *MATERIAL option. The material definition continues until an option that does not define a material behavior (such as another *MATERIAL option) is introduced, at which point the material definition is assumed to be complete. The order of the material behavior options is not important. All material behavior options within the data block are assumed to define the same material. Abaqus/CAE Usage: Property module: material editor: Name Use the menu bar under the Material Options list to add behaviors to a material. Large-strain considerations When giving material properties for finite-strain calculations, “stress” means “true” (Cauchy) stress (force per current area) and “strain” means logarithmic strain. For example, unless otherwise indicated, for uniaxial behavior Specifying material data as functions of temperature and independent field variables Material data are often specified as functions of independent variables such as temperature. Material properties are made temperature dependent by specifying them at several different temperatures. In some cases a material property can be defined as a function of variables calculated by Abaqus; for example, to define a work-hardening curve, stress must be given as a function of equivalent plastic strain. Material properties can also be dependent on “field variables” (user-defined variables that can represent any independent quantity and are defined at the nodes, as functions of time). For example, material moduli can be functions of weave density in a composite or of phase fraction in an alloy. See “Specifying field variable dependence” for details. The initial values of field variables are given as initial conditions and can be modified as functions of time during an analysis . This capability is useful if, for example, material properties change with time because of irradiation or some other precalculated environmental effect. Any material behaviors defined using a distribution in Abaqus/Standard (mass density, linear elastic behavior, and/or thermal expansion) cannot be defined with temperature and/or field dependence. However, material behaviors defined with distributions can be included in a material definition with other material behaviors that have temperature and/or field dependence. See “Density,” Section 21.2.1; “Linear elastic behavior,” Section 22.2.1; and “Thermal expansion,” Section 26.1.2. Interpolation of material data In the simplest case of a constant property, only the constant value is entered. When the material data are functions of only one variable, the data must be given in order of increasing values of the independent variable. Abaqus then interpolates linearly for values between those given. The property is assumed to be constant outside the range of independent variables given (except for fabric materials, where it is extrapolated linearly outside the specified range using the slope at the last specified data point). Thus, you can give as many or as few input values as are necessary for the material model. If the material data depend on the independent variable in a strongly nonlinear manner, you must specify enough data points so that a linear interpolation captures the nonlinear behavior accurately. When material properties depend on several variables, the variation of the properties with respect to the first variable must be given at fixed values of the other variables, in ascending values of the second variable, then of the third variable, and so on. The data must always be ordered so that the independent variables are given increasing values. This process ensures that the value of the material property is completely and uniquely defined at any values of the independent variables upon which the property depends. See “Input syntax rules,” Section 1.2.1, for further explanation and an example. Example: Temperature-dependent linear isotropic elasticity Figure 21.1.2–1 shows a simple, isotropic, linear elastic material, giving the Young’s modulus and the Poisson’s ratio as functions of temperature. Young s modulus, E Poisson s ratio, ν Temperature, θ Figure 21.1.2–1 Example of material definition. In this case six sets of values are used to specify the material description, as shown in the following table: Elastic Modulus Poisson’s Ratio Temperature , Abaqus assumes constant values for For temperatures that are outside the range defined by E and . The dotted lines on the graph represent the straight-line approximations that will be used for this model. In this example only one value of the thermal expansion coefficient is given, , and it is independent of temperature. and Example: Elastic-plastic material Figure 21.1.2–2 shows an elastic-plastic material for which the yield stress is dependent on the equivalent plastic strain and temperature. Elastic data: E1, ν (ε 11, σ 11 ) (ε 12 , σ 12 ) (ε 01 , σ 01 ) (ε 02 , σ 02 ) (ε 21, σ 21 ) (ε 31 , σ 31 ) (ε 22 , σ 22 ) (ε 32 , σ 32 ) θ = θ θ = θ2 εpl Figure 21.1.2–2 Example of material definition with two independent variables. In this case the second independent variable (temperature) must be held constant, while the yield stress is described as a function of the first independent variable (equivalent plastic strain). Then, a higher value of temperature is chosen and the dependence on equivalent plastic strain is given at this temperature. This process, as shown in the following table, is repeated as often as necessary to describe the property variations in as much detail as required: Yield Stress Equivalent Plastic Strain Temperature Specifying field variable dependence You can specify the number of user-defined field variable dependencies required for many material behaviors . If you do not specify a number of field variable dependencies for a material behavior with which field variable dependence is available, the material data are assumed not to depend on field variables. Input File Usage: *MATERIAL BEHAVIOR OPTION, DEPENDENCIES=n *MATERIAL BEHAVIOR OPTION refers to any material behavior option for which field dependence can be specified. Each data line can hold up to eight data items. If more field variable dependencies are required than fit on a single data line, more data lines can be added. For example, a linear, isotropic elastic material can be defined as a function of temperature and seven field variables ( *ELASTIC, TYPE=ISOTROPIC, DEPENDENCIES=7 ) as follows: E, , , , , , , , This pair of data lines would be repeated as often as necessary to define the material as a function of the temperature and field variables. Abaqus/CAE Usage: Property module: material editor: material behavior: Number of field variables: n material behavior refers to any material behavior for which field dependence can be specified. Specifying material data as functions of solution-dependent variables In Abaqus you can introduce dependence on solution variables with a user subroutine. User subroutines USDFLD in Abaqus/Standard and VUSDFLD in Abaqus/Explicit allow you to define field variables at a material point as functions of time, of material directions, and of any of the available material point quantities: those listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, for the case of USDFLD, and those listed in “Available output variable keys” in “Obtaining material point information in an Abaqus/Explicit analysis,” Section 2.1.7 of the Abaqus User Subroutines Reference Manual, for the case of VUSDFLD. Material properties defined as functions of these field variables may, thus, be dependent on the solution. User subroutines USDFLD and VUSDFLD are called at each material point for which the material definition includes a reference to the user subroutine. For general analysis steps the values of variables provided in user subroutines USDFLD and VUSDFLD are those corresponding to the start of the increment. Hence, the solution dependence introduced in this way is explicit: the material properties for a given increment are not influenced by the results obtained during the increment. Consequently, the accuracy of the results will generally depend on the time increment size. This is usually not a concern in Abaqus/Explicit because the stable time increment is usually sufficiently small to ensure good accuracy. In Abaqus/Standard you can control the time increment from inside subroutine USDFLD. For linear perturbation steps the solution variables in the base state are available. *USER DEFINED FIELD User subroutines USDFLD and VUSDFLD are not supported in Abaqus/CAE. Abaqus/CAE Usage: Input File Usage: Regularizing user-defined data in Abaqus/Explicit and Abaqus/CFD Interpolating material data as functions of independent variables requires table lookups of the material data values during the analysis. The table lookups occur frequently in Abaqus/Explicit and Abaqus/CFD, and are most economical if the interpolation is from regular intervals of the independent variables. For example, the data shown in Figure 21.1.2–1 are not regular because the intervals in temperature (the independent variable) between adjacent data points vary. You are not required to specify regular material data. Abaqus/Explicit and Abaqus/CFD will automatically regularize user-defined data. For example, the temperature values in Figure 21.1.2–1 may be defined at 10°, 20°, 25°, 28°, 30°, and 35° C. In this case Abaqus/Explicit and Abaqus/CFD can regularize the data by defining the data over 25 increments of 1° C and your piecewise linear data will be reproduced exactly. This regularization requires the expansion of your data from values at 6 temperature points to values at 26 temperature points. This example is a case where a simple regularization can reproduce your data exactly. If there are multiple independent variables, the concept of regular data also requires that the minimum and maximum values (the range) be constant for each independent variable while specifying the other independent variables. The material definition in Figure 21.1.2–2 illustrates a case where the material data are not regular since . Abaqus/Explicit will also regularize data involving multiple independent variables, although the data provided must satisfy the rules specified in “Input syntax rules,” Section 1.2.1. , and , Error tolerance used in regularizing user-defined data It is not always desirable to regularize the input data so that they are reproduced exactly in a piecewise linear manner. Suppose the yield stress is defined as a function of plastic strain in Abaqus/Explicit as follows: Yield Stress Plastic Strain 50000 75000 80000 85000 86000 .0 .001 .003 .010 1.0 It is possible to regularize the data exactly but it is not very economical, since it requires the subdivision of the data into 1000 regular intervals. Regularization is more difficult if the smallest interval you defined is small compared to the range of the independent variable. Abaqus/Explicit and Abaqus/CFD use an error tolerance to regularize the input data. The number of intervals in the range of each independent variable is chosen such that the error between the piecewise linear regularized data and each of your defined points is less than the tolerance times the range of the dependent variable. In some cases the number of intervals becomes excessive and Abaqus/Explicit or Abaqus/CFD cannot regularize the data using a reasonable number of intervals. The number of intervals considered reasonable depends on the number of intervals you define. If you defined 50 or less intervals, the maximum number of intervals used by Abaqus/Explicit and Abaqus/CFD for regularization is equal to 100 times the number of user-defined intervals. If you defined more than 50 intervals, the maximum number of intervals used for regularization is equal to 5000 plus 10 times the number of user-defined intervals above 50. If the number of intervals becomes excessive, the program stops during the data checking phase and issues an error message. You can either redefine the material data or change the tolerance value. The default tolerance is 0.03. The yield stress data in the example above are a typical case where such an error message may be issued. In this case you can simply remove the last data point since it produces only a small difference in the ultimate yield value. Input File Usage: Abaqus/CAE Usage: *MATERIAL, RTOL=tolerance Property module: material editor: General→Regularization: Rtol: tolerance Regularization of strain-rate-dependent data in Abaqus/Explicit Since strain rate dependence of data is usually measured at logarithmic intervals, Abaqus/Explicit regularizes strain rate data using logarithmic intervals rather than uniformly spaced intervals by default. This will generally provide a better match to typical strain-rate-dependent curves. You can specify linear strain rate regularization to use uniform intervals for regularization of strain rate data. The use of linear strain rate regularization affects only the regularization of strain rate as an independent variable and is relevant only if one of the following behaviors is used to define the material data: • low-density foams (“Low-density foams,” Section 22.9.1) • rate-dependent metal plasticity (“Classical metal plasticity,” Section 23.2.1) • rate-dependent viscoplasticity defined by yield stress ratios (“Rate-dependent yield,” Section 23.2.3) • shear failure defined using direct tabular data (“Dynamic failure models,” Section 23.2.8) • rate-dependent Drucker-Prager hardening (“Extended Drucker-Prager models,” Section 23.3.1) • rate-dependent concrete damaged plasticity (“Concrete damaged plasticity,” Section 23.6.3) • rate-dependent damage initiation criterion (“Damage initiation for ductile metals,” Section 24.2.2) Input File Usage: Use the following option to specify logarithmic regularization (default): *MATERIAL, STRAIN RATE REGULARIZATION=LOGARITHMIC Use the following option to specify linear regularization: Abaqus/CAE Usage: *MATERIAL, STRAIN RATE REGULARIZATION=LINEAR Property module: material editor: General→Regularization: Strain rate regularization: Logarithmic or Linear Evaluation of strain-rate-dependent data in Abaqus/Explicit Rate-sensitive material constitutive behavior may introduce nonphysical high-frequency oscillations in an explicit dynamic analysis. To overcome this problem, Abaqus/Explicit computes the equivalent plastic strain rate used for the evaluation of strain-rate-dependent data as Here and ( is the incremental change in equivalent plastic strain during the time increment , and are the strain rates at the beginning and end of the increment, respectively. The factor ) facilitates filtering high-frequency oscillations associated with strain-rate-dependent , directly. The default value is material behavior. You can specify the value of the strain rate factor, 0.9. A value of does not provide the desired filtering effect and should be avoided. Input File Usage: Abaqus/CAE Usage: *MATERIAL, SRATE FACTOR= You cannot specify the value of the strain rate factor in Abaqus/CAE. 21.1.3 COMBINING MATERIAL BEHAVIORS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Material data definition,” Section 21.1.2 • “Creating materials,” Section 12.4.1 of the Abaqus/CAE User’s Manual Overview Abaqus provides a broad range of possible material behaviors. A material is defined by choosing the appropriate behaviors for the purpose of an analysis. This section describes the general rules for combining material behaviors. Specific information for each material behavior is also summarized at the end of each material behavior description section in this chapter. Some of the material behaviors in Abaqus are completely unrestricted: they can be used alone or together with other behaviors. For example, thermal properties such as conductivity can be used in any material definition. They will be used in an analysis if the material is associated with elements that can solve heat transfer problems and if the analysis procedure allows for the thermal equilibrium equation to be solved. Some material behaviors in Abaqus require the presence of other material behaviors, and some exclude the use of other material behaviors. For example, metal plasticity requires the definition of elastic material behavior or an equation of state and excludes all other rate-independent plasticity behaviors. Complete material definitions Abaqus requires that the material be sufficiently defined to provide suitable properties for those elements with which the material is associated and for all of the analysis procedures through which the model will be run. Thus, a material associated with displacement or structural elements must include either a “Complete mechanical” category behavior or an “Elasticity” category behavior, as discussed below. In Abaqus/Explicit density (“Density,” Section 21.2.1) is required for all materials except hydrostatic fluids. It is not possible to modify or add to material definitions once an analysis is started. However, material definitions can be modified in an import analysis. For example, a static analysis can be run in Abaqus/Standard using a material definition that does not include a density specification. Density can be added to the material definition when the analysis is imported into Abaqus/Explicit. All aspects of a material’s behavior need not be fully defined; any behavior that is omitted is assumed not to exist in that part of the model. For example, if elastic material behavior is defined for a metal but metal plasticity is not defined, the material is assumed not to have a yield stress. You must ensure that the material is adequately defined for the purpose of the analysis. The material can include behaviors that are not relevant for the analysis, as described in “Material library: overview,” Section 21.1.1. Thus, you can include general material behavior libraries, without having to delete those behaviors that are not needed for a particular application. This generality offers great flexibility in material modeling. In Abaqus/Standard any material behaviors defined using a distribution (“Distribution definition,” Section 2.8.1) can be combined with almost all material behaviors in a manner identical to how they are combined when no distributions are used. For example, if the linear elastic material behavior is defined using a distribution, it can be combined with metal plasticity or any other material behavior that can normally be combined with linear elastic behavior. In addition, more than one material behavior defined with a distribution (linear elastic behavior and thermal expansion, for example) can be included in the same material definition. The only exception is that a material defined with concrete damaged plasticity (“Concrete damaged plasticity,” Section 23.6.3) cannot have any material behaviors defined with a distribution. Material behavior combination tables The material behavior combination tables that follow explain which behaviors must be used together. The tables also show the material behaviors that cannot be combined. Behaviors designated with an (S) are available only in Abaqus/Standard; behaviors designated with an (E) are available only in Abaqus/Explicit. The behaviors are assigned to categories because exclusions are best described in terms of those categories. Some of the categories require explanation: • “Complete mechanical behaviors” are those behaviors in Abaqus that, individually, completely define a material’s mechanical (stress-strain) behavior. A behavior in this category, therefore, excludes any other such behavior and also excludes any behavior that defines part of a material’s mechanical behavior: those behaviors that belong to the elasticity and plasticity categories. • “Elasticity, fabric, and equation of state behaviors” contains all of the basic elasticity behaviors in Abaqus. If a behavior from the “Complete mechanical behaviors” category is not used and mechanical behavior is required, a behavior must be selected from this category. This selection then excludes any other elasticity behavior. • “Enhancements for elasticity behaviors” contains behaviors that extend the modeling provided by the elasticity behaviors in Abaqus. • “Rate-independent plasticity behaviors” contains all of the basic plasticity behaviors in Abaqus except deformation plasticity, which is in the “Complete mechanical behaviors” category because it completely defines the material’s mechanical behavior. • “Rate-dependent plasticity behaviors” contains behaviors that extend the modeling provided by the rate-independent plasticity behaviors and by the linear elastic material behavior. If elastic-plastic behavior must be modeled, you should select an appropriate plasticity behavior from one of the plasticity behaviors categories and an elasticity behavior from one of the elasticity behaviors categories. General behaviors: These behaviors are unrestricted. Behavior Keyword Requires Elasticity, fabric, hyperelasticity, hyperfoam, low-density foam, or anisotropic hyperelasticity (except when used with beam or shell general sections or substructures) Required in Abaqus/Explicit, except for hydrostatic fluid elements Material damping *DAMPING Density *DENSITY Solution-dependent state variables *DEPVAR Thermal expansion *EXPANSION Complete mechanical behaviors: These behaviors are mutually exclusive and exclude all behaviors listed for elasticity, plasticity, and hydrostatic fluid behaviors, including all related enhancements. Behavior Keyword Acoustic medium Deformation plasticity(S) Mechanical user material *ACOUSTIC MEDIUM *DEFORMATION PLASTICITY *USER MATERIAL (, TYPE=MECHANICAL in Abaqus/Standard) Requires Density Elasticity, fabric, and equation of state behaviors: These behaviors are mutually exclusive. Behavior Elasticity Equation of state(E) Fabric(E) Hyperelasticity Hyperfoam Anisotropic hyperelasticity Hypoelasticity(S) Keyword Requires *ELASTIC *EOS *FABRIC *HYPERELASTIC *HYPERFOAM *ANISOTROPIC HYPERELASTIC *HYPOELASTIC Behavior Keyword Requires Porous elasticity (S) Low-density foam (E) *POROUS ELASTIC *LOW DENSITY FOAM Enhancements for elasticity behaviors: Behavior Keyword Requires *ELASTIC, TYPE=SHEAR Equation of state Elastic shear behavior for an equation of state(E) Strain-based failure measures Stress-based failure measures Hysteresis(S) *FAIL STRAIN *FAIL STRESS *HYSTERESIS Mullins effect *MULLINS EFFECT *NO COMPRESSION Elasticity Compressive failure theory(S) Tension failure theory(S) Viscoelasticity *NO TENSION *VISCOELASTIC Elasticity Elasticity Hyperelasticity (excludes all plasticity behaviors and Mullins effect) Hyperelasticity (excludes hysteresis), hyperfoam or anisotropic hyperelasticity Elasticity Elasticity, hyperelasticity, or hyperfoam (excludes all plasticity behaviors and all associated plasticity enhancements); or anisotropic hyperelasticity Equation of state Shear viscosity for an equation of state(E) *VISCOSITY Rate-independent plasticity behaviors: These behaviors are mutually exclusive. Behavior Keyword Requires Brittle cracking(E) Modified Drucker- Prager/Cap plasticity Cast iron plasticity *BRITTLE CRACKING *CAP PLASTICITY Isotropic elasticity and brittle shear Drucker-Prager/Cap plasticity hardening and isotropic elasticity or porous elasticity *CAST IRON PLASTICITY Cast iron compression hardening, cast iron tension hardening, and isotropic elasticity Keyword Requires MATERIAL BEHAVIORS Cam-clay plasticity *CLAY PLASTICITY Concrete(S) Concrete damaged plasticity Crushable foam plasticity Drucker-Prager plasticity *CONCRETE *CONCRETE DAMAGED PLASTICITY *CRUSHABLE FOAM *DRUCKER PRAGER Elasticity or porous elasticity (in Abaqus/Standard) Isotropic elasticity (in Abaqus/Explicit) Isotropic elasticity Concrete compression hardening, concrete tension stiffening, and isotropic elasticity Crushable foam hardening and isotropic elasticity Drucker-Prager hardening and isotropic elasticity or porous elasticity (in Abaqus/Standard) Drucker-Prager hardening and isotropic elasticity or the combination of an equation of state and isotropic linear elastic shear behavior for an equation of state (in Abaqus/Explicit) Plastic compaction behavior for an equation of state(E) Jointed material(S) Mohr-Coulomb plasticity Metal plasticity *EOS COMPACTION Linear equation of state *JOINTED MATERIAL *MOHR COULOMB *PLASTIC Isotropic elasticity and a local orientation Mohr-Coulomb hardening and isotropic elasticity Elasticity or hyperelasticity (in Abaqus/Standard) Isotropic elasticity, orthotropic elasticity (requires anisotropic yield), hyperelasticity, or the combination of an equation of state and isotropic linear elastic shear behavior for an equation of state (in Abaqus/Explicit) Rate-dependent plasticity behaviors: These behaviors are mutually exclusive, except metal creep and time-dependent volumetric swelling. Behavior Cap creep(S) Keyword *CAP CREEP Metal creep(S) *CREEP Requires Elasticity, modified Drucker-Prager/Cap plasticity, and Drucker-Prager/Cap plasticity hardening Elasticity (except when used to define rate-dependent gasket behavior; excludes all rate-independent plasticity behaviors except metal plasticity) Drucker-Prager creep(S) *DRUCKER PRAGER CREEP Elasticity, Drucker-Prager plasticity, and Drucker-Prager hardening Metal plasticity *PLASTIC, RATE Nonlinear viscoelasticity(S) Rate-dependent viscoplasticity *VISCOELASTIC, NONLINEAR *RATE DEPENDENT Time-dependent volumetric swelling(S) *SWELLING Elasticity or hyperelasticity (in Abaqus/Standard) Isotropic elasticity, orthotropic elasticity (requires anisotropic yield), hyperelasticity, or the combination of an equation of state and isotropic linear elastic shear behavior for an equation of state (in Abaqus/Explicit) Hyperelasticity Drucker-Prager plasticity, crushable foam plasticity, or metal plasticity Elasticity (excludes all rate-independent plasticity behaviors except metal plasticity) Two-layer viscoplasticity(S) *VISCOUS Elasticity and metal plasticity Enhancements for plasticity behaviors: Behavior Keyword Annealing temperature Brittle failure(E) *ANNEAL TEMPERATURE *BRITTLE FAILURE Requires Metal plasticity Brittle cracking and brittle shear Behavior Keyword Requires Cyclic hardening *CYCLIC HARDENING Inelastic heat fraction *INELASTIC HEAT FRACTION Oak Ridge National Laboratory constitutive model(S) *ORNL Porous material failure criteria(E) *POROUS FAILURE CRITERIA Porous metal plasticity *POROUS METAL PLASTICITY Anisotropic yield/creep *POTENTIAL Shear failure(E) Tension cutoff *SHEAR FAILURE *TENSION CUTOFF Metal plasticity with nonlinear isotropic/kinematic hardening Metal plasticity and specific heat Metal plasticity, cycled yield stress data, and, usually, metal creep Porous metal plasticity Metal plasticity Metal plasticity, metal creep, or two-layer viscoplasticity Metal plasticity Mohr-Coulomb plasticity Enhancement for elasticity or plasticity behaviors: Behavior Tensile failure(E) Keyword Requires *TENSILE FAILURE Damage initiation *DAMAGE INITIATION Metal plasticity or equation of state For elasticity behaviors: elasticity based on a traction-separation description for cohesive elements or elasticity model for fiber-reinforced composites For plasticity behaviors: elasticity and metal plasticity or Drucker-Prager plasticity Damage evolution Damage stabilization *DAMAGE EVOLUTION *DAMAGE STABILIZATION Damage initiation Damage evolution Thermal behaviors: These behaviors are unrestricted but exclude thermal user materials. Behavior Keyword Requires Thermal conductivity Volumetric heat generation(S) Latent heat Specific heat *CONDUCTIVITY *HEAT GENERATION *LATENT HEAT *SPECIFIC HEAT Density Density Complete thermal behavior: This behavior is unrestricted but excludes the thermal behaviors in the previous table. Behavior Keyword Requires Thermal user material(S) *USER MATERIAL, TYPE=THERMAL Density Pore fluid flow behaviors: These behaviors are unrestricted. Behavior Swelling gel(S) Keyword *GEL Moisture-driven swelling(S) *MOISTURE SWELLING Requires Permeability, porous bulk moduli, and absorption/exsorption behavior Permeability and absorption/exsorption behavior Permeability(S) Porous bulk moduli(S) *PERMEABILITY *POROUS BULK MODULI Permeability and either elasticity Absorption/exsorption behavior(S) *SORPTION or porous elasticity Permeability Electrical behaviors: These behaviors are unrestricted. Behavior Dielectricity(S) Electrical conductivity(S) Fraction of electric energy released as heat(S) Piezoelectricity(S) Keyword Requires *DIELECTRIC *ELECTRICAL CONDUCTIVITY *JOULE HEAT FRACTION *PIEZOELECTRIC Mass diffusion behaviors: These behaviors exclude all other behaviors. Behavior Keyword Mass diffusivity(S) Solubility(S) *DIFFUSIVITY *SOLUBILITY Requires Solubility Mass diffusivity Hydrostatic fluid behaviors: Behavior Keyword Requires Fluid bulk modulus(S) Hydrostatic fluid density Fluid thermal expansion coefficient(S) *FLUID BULK MODULUS Hydraulic fluid *FLUID DENSITY *FLUID EXPANSION Hydraulic fluid 21.2 General properties • “Density,” Section 21.2.1 21.2.1 DENSITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • *DENSITY • “Specifying material mass density,” Section 12.8.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A material’s mass density: • must be defined in Abaqus/Standard for eigenfrequency and transient dynamic analysis, transient heat transfer analysis, adiabatic stress analysis, and acoustic analysis; • must be defined in Abaqus/Standard for gravity, centrifugal, and rotary acceleration loading; • must be defined in Abaqus/Explicit for all materials except hydrostatic fluids; • must be defined in Abaqus/CFD for all fluids; • can be specified as a function of temperature and predefined variables; • can be distributed from nonstructural features (such as paint on sheet metal panels in a car) to the underlying elements using a nonstructural mass definition; and • can be defined with a distribution for solid continuum elements in Abaqus/Standard. Defining density Density can be defined as a function of temperature and field variables. However, for all elements in Abaqus/Standard with the exception of acoustic, heat transfer, coupled temperature-displacement, and coupled thermal-electrical elements , the density is a function of the initial values of temperature and field variables and changes in volume only. It will not be updated if temperatures and field variables change during the analysis. For Abaqus/Explicit the exception includes acoustic elements only. For Abaqus/CFD the density is considered constant for incompressible flows. For acoustic, heat transfer, coupled temperature-displacement, and coupled thermal-electrical elements in Abaqus/Standard and acoustic elements in Abaqus/Explicit, the density will be continually updated to the value corresponding to the current temperature and field variables. In an Abaqus/Standard analysis a spatially varying mass density can be defined for homogeneous solid continuum elements by using a distribution (“Distribution definition,” Section 2.8.1). The distribution must include a default value for the density. If a distribution is used, no dependencies on temperature and/or field variables for the density can be defined. Input File Usage: Use either of the following options: Abaqus/CAE Usage: *DENSITY *DENSITY, DEPENDENCIES=n Property module: material editor: General→Density You can toggle on Use temperature-dependent data to define the density as a function of temperature and/or select the Number of field variables to define the density as a function of field variables. Units Since Abaqus has no built-in dimensions, you must ensure that the density is given in consistent units. The use of consistent units, and density in particular, is discussed in “Conventions,” Section 1.2.2. If American or English units are used, you must be particularly careful that the density used is in units of ML , where mass is defined in units of FT L . Elements The density behavior described in this section is used to specify mass density for all elements, except rigid elements. Mass density for rigid elements is specified as part of the rigid body definition . In Abaqus/Explicit a nonzero mass density must be defined for all elements that are not part of a rigid body. In Abaqus/Standard density must be defined for heat transfer elements and acoustic elements; mass density can be defined for stress/displacement elements, coupled temperature-displacement elements, and elements including pore pressure. For elements that include pore pressure as a degree of freedom, the density of the dry material should be given for the porous medium in a coupled pore fluid flow/stress analysis. If you have a complex density for an acoustic medium, you should enter its real part here and convert the imaginary part into a volumetric drag, as discussed in “Acoustic medium,” Section 26.3.1. The mass contribution from features that have negligible structural stiffness can be added to the model by smearing the mass over an element set that is typically adjacent to the nonstructural feature. The nonstructural mass can be specified in the form of a total mass value, a mass per unit volume, a mass per unit area, or a mass per unit length . A nonstructural mass definition contributes additional mass to the specified element set and does not alter the underlying material density. 22. Elastic Mechanical Properties Overview Linear elasticity Porous elasticity Hypoelasticity Hyperelasticity Stress softening in elastomers Viscoelasticity Nonlinear Viscoelasticity Rate sensitive elastomeric foams 22.1 22.2 22.3 22.4 22.5 22.6 22.7 22.8 22.1 Overview • “Elastic behavior: overview,” Section 22.1.1 22.1.1 ELASTIC BEHAVIOR: OVERVIEW The material library in Abaqus includes several models of elastic behavior: • Linear elasticity: Linear elasticity (“Linear elastic behavior,” Section 22.2.1) is the simplest form of elasticity available in Abaqus. The linear elastic model can define isotropic, orthotropic, or anisotropic material behavior and is valid for small elastic strains. • Plane stress orthotropic failure: Failure theories are provided (“Plane stress orthotropic failure measures,” Section 22.2.3) for use with linear elasticity. They can be used to obtain postprocessed output requests. • Porous elasticity: The porous elastic model in Abaqus/Standard (“Elastic behavior of porous materials,” Section 22.3.1) is used for porous materials in which the volumetric part of the elastic strain varies with the logarithm of the equivalent pressure stress. This form of nonlinear elasticity is valid for small elastic strains. • Hypoelasticity: The hypoelastic model in Abaqus/Standard (“Hypoelastic behavior,” Section 22.4.1) is used for materials in which the rate of change of stress is defined by an elasticity matrix multiplying the rate of change of elastic strain, where the elasticity matrix is a function of the total elastic strain. This general, nonlinear elasticity is valid for small elastic strains. • Rubberlike hyperelasticity: For rubberlike material at finite strain the hyperelastic model (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1) provides a general strain energy potential to describe the material behavior for nearly incompressible elastomers. This nonlinear elasticity model is valid for large elastic strains. • Foam hyperelasticity: The hyperfoam model (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2) provides a general capability for elastomeric compressible foams at finite strains. This nonlinear elasticity model is valid for large strains (especially large volumetric changes). The low-density foam model in Abaqus/Explicit (“Low-density foams,” Section 22.9.1) is a nonlinear viscoelastic model suitable for specifying strain-rate sensitive behavior of low-density elastomeric foams such as used in crash and impact applications. The foam plasticity model (“Crushable foam plasticity models,” Section 23.3.5) should be used for foam materials that undergo permanent deformation. • Anisotropic hyperelasticity: The anisotropic hyperelastic model (“Anisotropic hyperelastic behavior,” Section 22.5.3) provides a general capability for modeling materials that exhibit highly anisotropic and nonlinear elastic behavior (such as biomedical soft tissues, fiber-reinforced elastomers, etc.). The model is valid for large elastic strains and captures the changes in the preferred material directions (or fiber directions) with deformation. • Fabric materials: The fabric model in Abaqus/Explicit (“Fabric material behavior,” Section 23.4.1) for woven fabrics captures the directional nature of the stiffness along the fill and the warp yarn directions. It also captures the shear response as the yarn directions rotate relative to each other. The model takes into account finite strains including large shear rotations. It captures the highly nonlinear elastic response of fabrics through the use of test data or a user subroutine, VFABRIC for the material characterization. The test data based fabric behavior can include nonlinear elasticity, permanent deformation, rate-dependent response, and damage accumulation. • Viscoelasticity: The viscoelastic model is used to specify time-dependent material behavior (“Time domain viscoelasticity,” Section 22.7.1). In Abaqus/Standard it is also used to specify frequency-dependent material behavior (“Frequency domain viscoelasticity,” Section 22.7.2). It must be combined with linear elasticity, rubberlike hyperelasticity, or foam hyperelasticity. • Parallel network viscoelastic model: The parallel network viscoelastic model in Abaqus/Standard (“Parallel network viscoelastic model,” Section 22.8.2) is intended for modeling nonlinear viscous behavior for materials subjected to large strains, such as polymers. The model consists of multiple parallel elastic and viscoelastic networks. The elastic response is defined using the hyperelastic material model, and the viscous response is specified using the flow rule derived from a creep potential. • Hysteresis: The hysteresis model in Abaqus/Standard (“Hysteresis in elastomers,” Section 22.8.1) is used to specify rate-dependent behavior of elastomers. It is used in conjunction with hyperelasticity. • Mullins effect: The Mullins effect model (“Mullins effect,” Section 22.6.1) is used to specify stress softening of filled rubber elastomers due to damage, a phenomenon referred to as Mullins effect. The model can also be used to include permanent energy dissipation and stress softening effects in elastomeric foams (“Energy dissipation in elastomeric foams,” Section 22.6.2). It is used in conjunction with rubberlike hyperelasticity or foam hyperelasticity. • No compression or no tension elasticity: The no compression or no tension models in Abaqus/Standard (“No compression or no tension,” Section 22.2.2) can be used when compressive or tensile principal stresses should not be generated. These options can be used only with linear elasticity. Thermal strain Thermal expansion can be introduced for any of the elasticity or fabric models (“Thermal expansion,” Section 26.1.2). Elastic strain magnitude Except in the hyperelasticity and fabric material models, the stresses are always assumed to be small compared to the tangent modulus of the elasticity relationship; that is, the elastic strain must be small (less than 5%). The total strain can be arbitrarily large if inelastic response such as metal plasticity is included in the material definition. For finite-strain calculations where the large strains are purely elastic, the fabric model (for woven fabrics), the hyperelastic model (for rubberlike behavior), or the foam hyperelasticity model (for elastomeric foams) should be used. The hyperelasticity and fabric models are the only models that give realistic predictions of actual material behavior at large elastic strains. The linear or, in Abaqus/Standard, porous elasticity models are appropriate in other cases where the large strains are inelastic. In Abaqus/Standard the linear elastic, porous elastic, and hypoelastic models will exhibit poor convergence characteristics if the stresses reach levels of 50% or more of the elastic moduli; this large strains. ELASTIC BEHAVIOR 22.2 Linear elasticity • “Linear elastic behavior,” Section 22.2.1 • “No compression or no tension,” Section 22.2.2 • “Plane stress orthotropic failure measures,” Section 22.2.3 22.2.1 LINEAR ELASTIC BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • *ELASTIC • “Creating a linear elastic material model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A linear elastic material model: • is valid for small elastic strains (normally less than 5%); • can be isotropic, orthotropic, or fully anisotropic; • can have properties that depend on temperature and/or other field variables; and • can be defined with a distribution for solid continuum elements in Abaqus/Standard. Defining linear elastic material behavior The total stress is defined from the total elastic strain as is the total stress (“true,” or Cauchy stress in finite-strain problems), is the fourth-order where elasticity tensor, and is the total elastic strain (log strain in finite-strain problems). Do not use the linear elastic material definition when the elastic strains may become large; use a hyperelastic model instead. Even in finite-strain problems the elastic strains should still be small (less than 5%). Defining linear elastic response for viscoelastic materials The elastic response of a viscoelastic material (“Time domain viscoelasticity,” Section 22.7.1) can be specified by defining either the instantaneous response or the long-term response of the material. To define the instantaneous response, experiments to determine the elastic constants have to be performed within time spans much shorter than the characteristic relaxation time of the material. Input File Usage: Abaqus/CAE Usage: *ELASTIC, MODULI=INSTANTANEOUS Property module: material editor: Mechanical→Elasticity→Elastic: Moduli time scale (for viscoelasticity): Instantaneous If, on the other hand, the long-term elastic response is used, data from experiments have to be collected after time spans much longer than the characteristic relaxation time of the viscoelastic material. Long-term elastic response is the default elastic material behavior. Input File Usage: Abaqus/CAE Usage: *ELASTIC, MODULI=LONG TERM Property module: material editor: Mechanical→Elasticity→Elastic: Moduli time scale (for viscoelasticity): Long-term Directional dependence of linear elasticity Depending on the number of symmetry planes for the elastic properties, a material can be classified as either isotropic (an infinite number of symmetry planes passing through every point) or anisotropic (no symmetry planes). Some materials have a restricted number of symmetry planes passing through every point; for example, orthotropic materials have two orthogonal symmetry planes for the elastic properties. The number of independent components of the elasticity tensor depends on such symmetry properties. You define the level of anisotropy and method of defining the elastic properties, as described below. If the material is anisotropic, a local orientation (“Orientations,” Section 2.2.5) must be used to define the direction of anisotropy. Stability of a linear elastic material Linear elastic materials must satisfy the conditions of material or Drucker stability . Stability requires that the tensor be positive definite, which leads to certain restrictions on the values of the elastic constants. The stress-strain relations for several different classes of material symmetries are given below. The appropriate restrictions on the elastic constants stemming from the stability criterion are also given. Defining isotropic elasticity The simplest form of linear elasticity is the isotropic case, and the stress-strain relationship is given by The elastic properties are completely defined by giving the Young’s modulus, E, and the Poisson’s . These ratio, parameters can be given as functions of temperature and of other predefined fields, if necessary. . The shear modulus, G, can be expressed in terms of E and as In Abaqus/Standard spatially varying isotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (“Distribution definition,” Section 2.8.1). The distribution must include default values for E and . If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined. Input File Usage: Abaqus/CAE Usage: *ELASTIC, TYPE=ISOTROPIC Property module: material editor: Mechanical→Elasticity→Elastic: Type: Isotropic Stability The stability criterion requires that . Values of Poisson’s ratio approaching 0.5 result in nearly incompressible behavior. With the exception of plane stress cases (including membranes and shells) or beams and trusses, such values generally require the use of “hybrid” elements in Abaqus/Standard and generate high frequency noise and result in excessively small stable time increments in Abaqus/Explicit. , and , Defining orthotropic elasticity by specifying the engineering constants Linear elasticity in an orthotropic material is most easily defined by giving the “engineering constants”: the three moduli , associated with the material’s principal directions. These moduli define the elastic compliance according to ; and the shear moduli ; Poisson’s ratios , and , , , , The quantity strain in the j-direction, when the material is stressed in the i-direction. In general, has the physical interpretation of the Poisson’s ratio that characterizes the transverse is not equal to . The engineering constants can also be given as functions of : they are related by = temperature and other predefined fields, if necessary. In Abaqus/Standard spatially varying orthotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (“Distribution definition,” Section 2.8.1). The distribution must include default values for the elastic moduli and Poisson’s ratios. If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined. Input File Usage: Abaqus/CAE Usage: *ELASTIC, TYPE=ENGINEERING CONSTANTS Property module: material editor: Mechanical→Elasticity→Elastic: Type: Engineering Constants Stability Material stability requires When the left-hand side of the inequality approaches zero, the material exhibits incompressible , the second, third, and fourth restrictions in the above set = behavior. Using the relations can also be expressed as Defining transversely isotropic elasticity A special subclass of orthotropy is transverse isotropy, which is characterized by a plane of isotropy at every point in the material. Assuming the 1–2 plane to be the plane of isotropy at every point, transverse isotropy requires that , where p and t stand = for “in-plane” and “transverse,” respectively. Thus, while has the physical interpretation of the Poisson’s ratio that characterizes the strain in the plane of isotropy resulting from stress normal to it, characterizes the transverse strain in the direction normal to the plane of isotropy resulting from are not equal and are related by stress in the plane of isotropy. In general, the quantities , and and = = = = = = = , , = . The stress-strain laws reduce to = where and the total number of independent constants is only five. In Abaqus/Standard spatially varying transverse isotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (“Distribution definition,” Section 2.8.1). The distribution must include default values for the elastic moduli and Poisson’s ratio. If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined. *ELASTIC, TYPE=ENGINEERING CONSTANTS Property module: material editor: Mechanical→Elasticity→Elastic: Type: Engineering Constants Abaqus/CAE Usage: Input File Usage: Stability In the transversely isotropic case the stability relations for orthotropic elasticity simplify to Defining orthotropic elasticity in plane stress Under plane stress conditions, such as in a shell element, only the values of , , , , , and are required to define an orthotropic material. (In all of the plane stress elements in Abaqus the and surface is the surface of plane stress, so that the plane stress condition is .) The shear moduli are included because they may be required for modeling transverse shear deformation in . In this case the stress-strain a shell. The Poisson’s ratio relations for the in-plane components of the stress and strain are of the form is implicitly given as In Abaqus/Standard spatially varying plane stress orthotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (“Distribution definition,” Section 2.8.1). The distribution must include default values for the elastic moduli and Poisson’s ratio. If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined. Input File Usage: Abaqus/CAE Usage: *ELASTIC, TYPE=LAMINA Property module: material editor: Mechanical→Elasticity→Elastic: Type: Lamina Stability Material stability for plane stress requires Defining orthotropic elasticity by specifying the terms in the elastic stiffness matrix Linear elasticity in an orthotropic material can also be defined by giving the nine independent elastic stiffness parameters, as functions of temperature and other predefined fields, if necessary. In this case the stress-strain relations are of the form For an orthotropic material the engineering constants define the matrix as where When the material stiffness parameters (the ) are given directly, Abaqus imposes the constraint for the plane stress case to reduce the material’s stiffness matrix as required. In Abaqus/Standard spatially varying orthotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (“Distribution definition,” Section 2.8.1). The distribution must include default values for the elastic moduli. If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined. Input File Usage: Abaqus/CAE Usage: *ELASTIC, TYPE=ORTHOTROPIC Property module: material editor: Mechanical→Elasticity→Elastic: Type: Orthotropic Stability The restrictions on the elastic constants due to material stability are The last relation leads to These restrictions in terms of the elastic stiffness parameters are equivalent to the restrictions in terms of the “engineering constants.” Incompressible behavior results when the left-hand side of the inequality approaches zero. Defining fully anisotropic elasticity For fully anisotropic elasticity 21 independent elastic stiffness parameters are needed. The stress-strain relations are as follows: When the material stiffness parameters (the ) are given directly, Abaqus imposes the constraint for the plane stress case to reduce the material’s stiffness matrix as required. In Abaqus/Standard spatially varying anisotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (“Distribution definition,” Section 2.8.1). The distribution must include default values for the elastic moduli. If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined. Input File Usage: Abaqus/CAE Usage: *ELASTIC, TYPE=ANISOTROPIC Property module: material editor: Mechanical→Elasticity→Elastic: Type: Anisotropic Stability The restrictions imposed upon the elastic constants by stability requirements are too complex to express in terms of simple equations. However, the requirement that is positive definite requires that all of the eigenvalues of the elasticity matrix be positive. Defining orthotropic elasticity for warping elements For two-dimensional meshed models of solid cross-section Timoshenko beam elements modeled with warping elements , Abaqus offers a linear elastic material definition that can have two different shear moduli in the user-specified material directions. In the user-specified directions the stress-strain relations are as follows: A local orientation is used to define the angle material directions. In the cross-section directions the stress-strain relations are as follows: between the global directions and the user-specified where represents the beam’s axial stress and and represent two shear stresses. Input File Usage: Abaqus/CAE Usage: *ELASTIC, TYPE=TRACTION Property module: material editor: Mechanical→Elasticity→Elastic: Type: Traction Stability The stability criterion requires that , , and . Defining elasticity in terms of tractions and separations for cohesive elements For cohesive elements used to model bonded interfaces Abaqus offers an elasticity definition that can be written directly in terms of the nominal tractions and the nominal strains. Both uncoupled and coupled behaviors are supported. For uncoupled behavior each traction component depends only on its conjugate nominal strain, while for coupled behavior the response is more general (as shown below). In the local element directions the stress-strain relations for uncoupled behavior are as follows: , The quantities directions, respectively; while the quantities For coupled traction separation behavior the stress-strain relations are as follows: represent the nominal tractions in the normal and the two local shear represent the corresponding nominal strains. , and , and , Input File Usage: Abaqus/CAE Usage: Use the following option to define uncoupled elastic behavior for cohesive elements: *ELASTIC, TYPE=TRACTION Use the following option to define coupled elastic behavior for cohesive elements: *ELASTIC, TYPE=COUPLED TRACTION Use the following option to define uncoupled elastic behavior for cohesive elements: Property module: material editor: Mechanical→Elasticity→Elastic: Type: Traction Use the following option to define coupled elastic behavior for cohesive elements: Property module: material editor: Mechanical→Elasticity→Elastic: Type: Coupled Traction Stability The stability criterion for uncoupled behavior requires that coupled behavior the stability criterion requires that: , , and . For Defining isotropic shear elasticity for equations of state in Abaqus/Explicit Abaqus/Explicit allows you to define isotropic shear elasticity to describe the deviatoric response of materials whose volumetric response is governed by an equation of state (“Elastic shear behavior” in “Equation of state,” Section 25.2.1). In this case the deviatoric stress-strain relationship is given by is the deviatoric stress and is the deviatoric elastic strain. You must provide the elastic shear where modulus, , when you define the elastic deviatoric behavior. Input File Usage: Abaqus/CAE Usage: *ELASTIC, TYPE=SHEAR Property module: material editor: Mechanical→Elasticity→Elastic: Type: Shear Elements Linear elasticity can be used with any stress/displacement element or coupled temperature-displacement element in Abaqus. The exceptions are traction elasticity, which can be used only with warping elements and cohesive elements; coupled traction elasticity, which can be used only with cohesive elements; shear elasticity, which can be used only with solid (continuum) elements except plane stress elements; and, in Abaqus/Explicit, anisotropic elasticity, which is not supported for truss, rebar, pipe, and beam elements. for isotropic elasticity), hybrid elements should be used in Abaqus/Standard. Compressible anisotropic elasticity should not be used with second-order hybrid continuum elements: inaccurate results and/or convergence problems may occur. If the material is (almost) incompressible (Poisson’s ratio 22.2.2 NO COMPRESSION OR NO TENSION Products: Abaqus/Standard Abaqus/CAE WARNING: Except when used with truss or beam elements, Abaqus/Standard does not form an exact material stiffness for this option. Therefore, the convergence can sometimes be slow. References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • “Linear elastic behavior,” Section 22.2.1 • *NO COMPRESSION • *NO TENSION • “Specifying elastic material properties” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The no compression and no tension elasticity models: • are used to modify the linear elasticity of the material so that compressive stress or tensile stress cannot be generated; and • can be used only in conjunction with an elasticity definition. Defining the modified elastic behavior The modified elastic behavior is obtained by first solving for the principal stresses assuming linear elasticity and then setting the appropriate principal stress values to zero. The associated stiffness matrix components will also be set to zero. These models are not history dependent: the directions in which the principal stresses are set to zero are recalculated at every iteration. The no compression effect for a one-dimensional stress case such as a truss or a layer of a beam in a plane is illustrated in Figure 22.2.2–1. No compression and no tension definitions modify only the elastic response of the material. Strain Stress A B C Time A B C Time Stress Strain Figure 22.2.2–1 A no compression elastic case with an imposed strain cycle. Input File Usage: Use one of the following options: *NO COMPRESSION *NO TENSION Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Elastic: No compression or No tension Stability Using no compression or no tension elasticity can make a model unstable: convergence difficulties may occur. Sometimes these difficulties can be overcome by overlaying each element that uses the no compression (or no tension) model with another element that uses a small value of Young’s modulus (small in comparison with the Young’s modulus of the element using modified elasticity). This technique creates a small “artificial” stiffness, which can stabilize the model. Use with other material models No compression and no tension definitions can be used only in conjunction with an elasticity definition. These definitions cannot be used with any other material option. Elements The no compression and no tension elasticity models can be used with any stress/displacement element in Abaqus/Standard. However, they cannot be used with shell elements or beam elements if section properties are pre-integrated using a general section definition. 22.2.3 PLANE STRESS ORTHOTROPIC FAILURE MEASURES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • “Linear elastic behavior,” Section 22.2.1 • *FAIL STRAIN • *FAIL STRESS • *ELASTIC • “Defining stress-based failure measures for an elastic model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining strain-based failure measures for an elastic model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The orthotropic plane stress failure measures: • are indications of material failure (normally used for fiber-reinforced composite materials; for alternative damage and failure models for fiber-reinforced composite materials, see “Damage and failure for fiber-reinforced composites: overview,” Section 24.3.1); • can be used only in conjunction with a linear elastic material model (with or without local material orientations); • can be used for any element that uses a plane stress formulation; that is, for plane stress continuum elements, shell elements, and membrane elements; • are postprocessed output requests and do not cause any material degradation; and • take values that are greater than or equal to 0.0, with values that are greater than or equal to 1.0 implying failure. Failure theories Five different failure theories are provided: four stress-based theories and one strain-based theory. We denote orthotropic material directions by 1 and 2, with the 1-material direction aligned with the fibers and the 2-material direction transverse to the fibers. For the failure theories to work correctly, the 1- and 2-directions of the user-defined elastic material constants must align with the fiber and the transverse- to-fiber directions, respectively. For applications other than fiber-reinforced composites, the 1- and 2- material directions should represent the strong and weak orthotropic-material directions, respectively. In all cases tensile values must be positive and compressive values must be negative. Stress-based failure theories The input data for the stress-based failure theories are tensile and compressive stress limits, in the 1-direction; tensile and compressive stress limits, (maximum shear stress), S, in the X–Y plane. , , in the 2-direction; and shear strength and and All four stress-based theories are defined and available with a single definition in Abaqus; the desired output is chosen by the output variables described at the end of this section. Input File Usage: Abaqus/CAE Usage: *FAIL STRESS Property module: material editor: Mechanical→Elasticity→Elastic: Suboptions→Fail Stress Maximum stress theory If stress failure criterion requires that ; otherwise, , . If , ; otherwise, . The maximum max Tsai-Hill theory If , criterion requires that ; otherwise, . If , ; otherwise, . The Tsai-Hill failure Tsai-Wu theory The Tsai-Wu failure criterion requires that The Tsai-Wu coefficients are defined as follows: is the equibiaxial stress at failure. If it is known, then otherwise, where . The default value of is zero. For the Tsai-Wu failure criterion either or must be given as input data. The coefficient is ignored if is given. Azzi-Tsai-Hill theory The Azzi-Tsai-Hill failure theory is the same as the Tsai-Hill theory, except that the absolute value of the cross product term is taken: This difference between the two failure criteria shows up only when and have opposite signs. Stress-based failure measures—failure envelopes ) in ( To illustrate the four stress-based failure measures, Figure 22.2.3–1, Figure 22.2.3–2, and Figure 22.2.3–3 show each failure envelope (i.e., ) stress space compared to the Tsai-Hill envelope – for a given value of in-plane shear stress. In each case the Tsai-Hill surface is the piecewise continuous elliptical surface with each quadrant of the surface defined by an ellipse centered at the origin. The parallelogram in Figure 22.2.3–1 defines the maximum stress surface. In Figure 22.2.3–2 the Tsai-Wu surface appears as the ellipse. In Figure 22.2.3–3 the Azzi-Tsai-Hill surface differs from the Tsai-Hill surface only in the second and fourth quadrants, where it is the outside bounding surface (i.e., further from the origin). Since all of the failure theories are calibrated by tensile and compressive failure under uniaxial stress, they all give the same values on the stress axes. 22 11 Figure 22.2.3–1 Tsai-Hill versus maximum stress failure envelope ( ). 22 11 Tsai-Hill Tsai-Wu Figure 22.2.3–2 Tsai-Hill versus Tsai-Wu failure envelope ( , ). 22 11 Tsai-Hill Azzi-Tsai-Hill Figure 22.2.3–3 Tsai-Hill versus Azzi-Tsai-Hill failure envelope ( ). Strain-based failure theory The input data for the strain-based theory are tensile and compressive strain limits, 1-direction; tensile and compressive strain limits, , in the , in the 2-direction; and shear strain limit, and and , in the X–Y plane. Input File Usage: Abaqus/CAE Usage: Maximum strain theory *FAIL STRAIN Property module: material editor: Mechanical→Elasticity→Elastic: Suboptions→Fail Strain If strain failure criterion requires that ; otherwise, , . If , ; otherwise, . The maximum max Elements The plane stress orthotropic failure measures can be used with any plane stress, shell, or membrane element in Abaqus. Output Abaqus provides output of the failure index, R, if failure measures are defined with the material description. The definition of the failure index and the different output variables are described below. Output failure indices Each of the stress-based failure theories defines a failure surface surrounding the origin in the three- dimensional space . Failure occurs any time a state of stress is either on or outside this surface. The failure index, R, is used to measure the proximity to the failure surface. R is defined as the scaling factor such that, for the given stress state , that is, simultaneously to lie on the failure surface. Values failure surface, while values is the scaling factor with which we need to multiply all of the stress components indicate that the state of stress is within the indicate failure. For the maximum stress theory . The failure index R is defined similarly for the maximum strain failure theory. R is the scaling factor such that, for the given strain state , For the maximum strain theory . Output variables Output variable CFAILURE will provide output for all of the stress- and strain-based failure theories . In Abaqus/Standard history output can also be requested for the individual stress theories with output variables MSTRS, TSAIH, TSAIW, and AZZIT and for the strain theory with output variable MSTRN. Output variables for the stress- and strain-based failure theories are always calculated at the material points of the element. In Abaqus/Standard element output can be requested at a location other than the material points ; in this case the output variables are first calculated at the material points, then interpolated to the element centroid or extrapolated to the nodes. 22.3 Porous elasticity • “Elastic behavior of porous materials,” Section 22.3.1 22.3.1 ELASTIC BEHAVIOR OF POROUS MATERIALS Products: Abaqus/Standard Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • *POROUS ELASTIC • *INITIAL CONDITIONS • “Creating a porous elastic material model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A porous elastic material model: • is valid for small elastic strains (normally less than 5%); • is a nonlinear, isotropic elasticity model in which the pressure stress varies as an exponential function of volumetric strain; • allows a zero or nonzero elastic tensile stress limit; and • can have properties that depend on temperature and other field variables. Defining the volumetric behavior Often, the elastic part of the volumetric behavior of porous materials is modeled accurately by assuming that the elastic part of the change in volume of the material is proportional to the logarithm of the pressure stress (Figure 22.3.1–1): is the “logarithmic bulk modulus”; where defined by is the initial void ratio; p is the equivalent pressure stress, is the initial value of the equivalent pressure stress; the current and reference configurations; and sense that as ). is the elastic part of the volume ratio between is the “elastic tensile strength” of the material (in the Input File Usage: Use all three of the following options to define a porous elastic material: *POROUS ELASTIC, SHEAR=G or POISSON to define and ol el -p p0 p0 el p Figure 22.3.1–1 Porous elastic volumetric behavior. Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=STRESS to define *INITIAL CONDITIONS, TYPE=RATIO to define Use all three of the following options to define a porous elastic material: Property module: material editor: Mechanical→Elasticity→Porous Elastic Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step Defining the shear behavior The deviatoric elastic behavior of a porous material can be defined in either of two ways. By defining the shear modulus Give the shear modulus, G. The deviatoric stress, elastic strain, , by , is then related to the deviatoric part of the total In this case the shear behavior is not affected by compaction of the material. Input File Usage: *POROUS ELASTIC, SHEAR=G Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Porous Elastic: Shear: G By defining Poisson’s ratio Define Poisson’s ratio, modulus and Poisson’s ratio as . The instantaneous shear modulus is then defined from the instantaneous bulk where is the logarithmic measure of the elastic volume change. In this case Thus, the elastic shear stiffness increases as the material is compacted. This equation is integrated to give the total stress–total elastic strain relationship. Input File Usage: Abaqus/CAE Usage: *POROUS ELASTIC, SHEAR=POISSON Property module: material editor: Mechanical→Elasticity→Porous Elastic: Shear: Poisson Use with other material models The porous elasticity model can be used by itself, or it can be combined with: • the “Extended Drucker-Prager models,” Section 23.3.1; • the “Modified Drucker-Prager/Cap model,” Section 23.3.2; • the “Critical state (clay) plasticity model,” Section 23.3.4; or • isotropic expansion to introduce thermal volume changes (“Thermal expansion,” Section 26.1.2). It is not possible to use porous elasticity with rate-dependent plasticity or viscoelasticity. Porous elasticity cannot be used with the porous metal plasticity model (“Porous metal plasticity,” Section 23.2.9). See “Combining material behaviors,” Section 21.1.3, for more details. Elements Porous elasticity cannot be used with hybrid elements or plane stress elements (including shells and membranes), but it can be used with any other pure stress/displacement element in Abaqus/Standard. If used with reduced-integration elements with total-stiffness hourglass control, Abaqus/Standard cannot calculate a default value for the hourglass stiffness of the element if the shear behavior is defined through Poisson’s ratio. Hence, you must specify the hourglass stiffness. See “Section controls,” Section 27.1.4, for details. If fluid pore pressure is important (such as in undrained soils), stress/displacement elements that include pore pressure can be used. 22.4 Hypoelasticity • “Hypoelastic behavior,” Section 22.4.1 22.4.1 HYPOELASTIC BEHAVIOR Products: Abaqus/Standard Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • *HYPOELASTIC • “Creating a hypoelastic material model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The hypoelastic material model: • is valid for small elastic strains—the stresses should not be large compared to the elastic modulus of the material; • is used when the load path is monotonic; and • must be defined by user subroutine UHYPEL if temperature dependence is to be included. Defining hypoelastic material behavior In a hypoelastic material the rate of change of stress is defined as a tangent modulus matrix multiplying the rate of change of the elastic strain: where tangent elasticity matrix, and problems). is the rate of change of the stress (the “true,” Cauchy, stress in finite-strain problems), is the is the rate of change of the elastic strain (the log strain in finite-strain Determining the hypoelastic material parameters The entries in strain invariants. The strain invariants are defined for this purpose as are provided by giving Young’s modulus, E, and Poisson’s ratio, , as functions of You can define the material parameters directly or by using a user subroutine. Direct specification You can define the variation of Young’s modulus and Poisson’s ratio directly by specifying E, and . , , , Input File Usage: Abaqus/CAE Usage: *HYPOELASTIC Property module: material editor: Mechanical→Elasticity→Hypoelastic User subroutine If specifying E and you can define the hypoelastic material by user subroutine UHYPEL. as functions of the strain invariants directly does not allow sufficient flexibility, Input File Usage: Abaqus/CAE Usage: *HYPOELASTIC, USER Property module: material editor: Mechanical→Elasticity→Hypoelastic: Use user subroutine UHYPEL Plane or uniaxial stress For plane stress and uniaxial stress states Abaqus/Standard does not compute the out-of-plane strain components. For the purpose of defining the above invariants, it is assumed that ; that is, the material is assumed to be incompressible. For example, in a uniaxial stress case (such as a truss element) this assumption implies that Large-displacement analysis For large-displacement analysis the strain measure in Abaqus is the integration of the rate of deformation. This strain measure corresponds to log strain if the principal directions do not rotate relative to the material. The strain invariant definitions should be interpreted in this way. Use with other material models The hypoelastic material model can be used only by itself in the material definition. It cannot be combined with viscoelasticity or with any inelastic response model. See “Combining material behaviors,” Section 21.1.3, for more details. Elements The hypoelastic material model can be used with any of the stress/displacement elements in Abaqus/Standard. 22.5 Hyperelasticity • “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 • “Hyperelastic behavior in elastomeric foams,” Section 22.5.2 • “Anisotropic hyperelastic behavior,” Section 22.5.3 22.5.1 HYPERELASTIC BEHAVIOR OF RUBBERLIKE MATERIALS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • “Mullins effect,” Section 22.6.1 • “Permanent set in rubberlike materials,” Section 23.7.1 • *HYPERELASTIC • *UNIAXIAL TEST DATA • *BIAXIAL TEST DATA • *PLANAR TEST DATA • *VOLUMETRIC TEST DATA • *MULLINS EFFECT • “Creating an isotropic hyperelastic material model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The hyperelastic material model: • is isotropic and nonlinear; • is valid for materials that exhibit instantaneous elastic response up to large strains (such as rubber, solid propellant, or other elastomeric materials); and • requires that geometric nonlinearity be accounted for during the analysis step (“General and linear perturbation procedures,” Section 6.1.3), since it is intended for finite-strain applications. Compressibility Most elastomers (solid, rubberlike materials) have very little compressibility compared to their shear flexibility. This behavior does not warrant special attention for plane stress, shell, membrane, beam, truss, or rebar elements, but the numerical solution can be quite sensitive to the degree of compressibility for three-dimensional solid, plane strain, and axisymmetric analysis elements. In cases where the material is highly confined (such as an O-ring used as a seal), the compressibility must be modeled correctly to obtain accurate results. In applications where the material is not highly confined, the degree of compressibility is typically not crucial; for example, it would be quite satisfactory in Abaqus/Standard to assume that the material is fully incompressible: the volume of the material cannot change except for thermal expansion. Another class of rubberlike materials is elastomeric foam, which is elastic but very compressible. Elastomeric foams are discussed in “Hyperelastic behavior in elastomeric foams,” Section 22.5.2. We can assess the relative compressibility of a material by the ratio of its initial bulk modulus, , since . This ratio can also be expressed in terms of Poisson’s ratio, to its initial shear modulus, , The table below provides some representative values. 10 20 50 100 1000 10,000 Poisson’s ratio 0.452 0.475 0.490 0.495 0.4995 0.49995 Compressibility in Abaqus/Standard In Abaqus/Standard the use of “hybrid” (mixed formulation) elements is recommended in both incompressible and almost incompressible cases. In plane stress, shell, and membrane elements the material is free to deform in the thickness direction. Similarly, in one-dimensional elements (such as beams, trusses, and rebars) the material is free to deform in the lateral directions. In these cases special treatment of the volumetric behavior is not necessary; the use of regular stress/displacement elements is satisfactory. Compressibility in Abaqus/Explicit Except for plane stress and uniaxial cases, it is not possible to assume that the material is fully incompressible in Abaqus/Explicit because the program has no mechanism for imposing such a Instead, we must provide some compressibility. The constraint at each material calculation point. difficulty is that, in many cases, the actual material behavior provides too little compressibility for the algorithms to work efficiently. Thus, except for plane stress and uniaxial cases, you must provide enough compressibility for the code to work, knowing that this makes the bulk behavior of the model softer than that of the actual material. Some judgment is, therefore, required to decide whether or not the solution is sufficiently accurate, or whether the problem can be modeled at all with Abaqus/Explicit because of this numerical limitation. If no value is given for the material compressibility in the hyperelastic model, by default Abaqus/Explicit assumes 20, corresponding to Poisson’s ratio of 0.475. Since typical unfilled elastomers have 0.49995) and filled elastomers have 0.497), this default provides much more compressibility than is available in most elastomers. However, if the elastomer is relatively unconfined, this softer modeling of the material’s bulk behavior usually provides quite accurate results. ratios in the range of 1,000 to 10,000 ( ratios in the range of 50 to 200 ( 0.4995 to 0.490 to Unfortunately, in cases where the material is highly confined—such as when it is in contact with stiff, metal parts and has a very small amount of free surface, especially when the loading is highly compressive—it may not be feasible to obtain accurate results with Abaqus/Explicit. If you are defining the compressibility rather than accepting the default value, an upper limit of . Larger ratios introduce high frequency noise into the dynamic 100 is suggested for the ratio of solution and require the use of excessively small time increments. Isotropy assumption In Abaqus all hyperelastic models are based on the assumption of isotropic behavior throughout the deformation history. Hence, the strain energy potential can be formulated as a function of the strain invariants. Strain energy potentials the Marlow form, Hyperelastic materials are described in terms of a “strain energy potential,” , which defines the strain energy stored in the material per unit of reference volume (volume in the initial configuration) as a function of the strain at that point in the material. There are several forms of strain energy potentials the Arruda-Boyce available in Abaqus to model approximately incompressible isotropic elastomers: form, the polynomial form, the reduced polynomial form, the Yeoh form, and the Van der Waals form. As will be pointed out below, the reduced polynomial and Mooney-Rivlin models can be viewed as particular cases of the polynomial model; the Yeoh and neo-Hookean potentials, in turn, can be viewed as special cases of the reduced polynomial model. Thus, we will occasionally refer collectively to these models as “polynomial models.” the Mooney-Rivlin form, the neo-Hookean form, the Ogden form, Generally, when data from multiple experimental tests are available (typically, this requires at least uniaxial and equibiaxial test data), the Ogden and Van der Waals forms are more accurate in fitting experimental results. If limited test data are available for calibration, the Arruda-Boyce, Van der Waals, Yeoh, or reduced polynomial forms provide reasonable behavior. When only one set of test data (uniaxial, equibiaxial, or planar test data) is available, the Marlow form is recommended. In this case a strain energy potential is constructed that will reproduce the test data exactly and that will have reasonable behavior in other deformation modes. Evaluating hyperelastic materials Abaqus/CAE allows you to evaluate hyperelastic material behavior by automatically creating response curves using selected strain energy potentials. In addition, you can provide experimental test data for a material without specifying a particular strain energy potential and have Abaqus/CAE evaluate the material to determine the optimal strain energy potential. See “Evaluating hyperelastic and viscoelastic material behavior,” Section 12.4.7 of the Abaqus/CAE User’s Manual, for details. Alternatively, you can use single-element test cases to evaluate the strain energy potential. You can use single-element test cases to evaluate the strain energy potential. Arruda-Boyce form The form of the Arruda-Boyce strain energy potential is where U is the strain energy per unit of reference volume; material parameters; is the first deviatoric strain invariant defined as , , and D are temperature-dependent where the deviatoric stretches as defined below in “Thermal expansion”; and ; J is the total volume ratio; is the elastic volume ratio are the principal stretches. The initial shear modulus, , is related to with the expression A typical value of , and the parameter are printed in the data (.dat) file if you request a printout of the model data from the analysis input . Both the initial shear modulus, is 7, for which file processor. The initial bulk modulus is related to D with the expression Marlow form The form of the Marlow strain energy potential is where U is the strain energy per unit of reference volume, with volumetric part; is the first deviatoric strain invariant defined as as its deviatoric part and as its where the deviatoric stretches is the elastic volume ratio as defined below in “Thermal expansion”; and are the principal stretches. The deviatoric part of the potential is defined by providing either uniaxial, equibiaxial, or planar test data; while the volumetric part is defined by providing the volumetric test data, defining the Poisson’s ratio, or specifying the lateral strains together with the uniaxial, equibiaxial, or planar test data. ; J is the total volume ratio; Mooney-Rivlin form The form of the Mooney-Rivlin strain energy potential is where U is the strain energy per unit of reference volume; material parameters; , are the first and second deviatoric strain invariants defined as , and and are temperature-dependent where the deviatoric stretches defined below in “Thermal expansion”; and bulk modulus are given by ; J is the total volume ratio; is the elastic volume ratio as are the principal stretches. The initial shear modulus and Neo-Hookean form The form of the neo-Hookean strain energy potential is where U is the strain energy per unit of reference volume; parameters; is the first deviatoric strain invariant defined as and are temperature-dependent material where the deviatoric stretches defined below in “Thermal expansion”; and bulk modulus are given by ; J is the total volume ratio; is the elastic volume ratio as are the principal stretches. The initial shear modulus and Ogden form The form of the Ogden strain energy potential is are the deviatoric principal stretches where parameter; and and bulk modulus for the Ogden form are given by , and , are the principal stretches; N is a material are temperature-dependent material parameters. The initial shear modulus ; The particular material models described above—the Mooney-Rivlin and neo-Hookean forms—can also be obtained from the general Ogden strain energy potential for special choices of and . Polynomial form The form of the polynomial strain energy potential is where U is the strain energy per unit of reference volume; N is a material parameter; temperature-dependent material parameters; defined as are are the first and second deviatoric strain invariants and and where the deviatoric stretches defined below in “Thermal expansion”; and bulk modulus are given by ; J is the total volume ratio; is the elastic volume ratio as are the principal stretches. The initial shear modulus and For cases where the nominal strains are small or only moderately large (< 100%), the first terms in the polynomial series usually provide a sufficiently accurate model. Some particular material models—the Mooney-Rivlin, neo-Hookean, and Yeoh forms—are obtained for special choices of . Reduced polynomial form The form of the reduced polynomial strain energy potential is where U is the strain energy per unit of reference volume; N is a material parameter; temperature-dependent material parameters; and is the first deviatoric strain invariant defined as are where the deviatoric stretches defined below in “Thermal expansion”; and bulk modulus are given by ; J is the total volume ratio; is the elastic volume ratio as are the principal stretches. The initial shear modulus and Van der Waals form The form of the Van der Waals strain energy potential is where and Here, U is the strain energy per unit of reference volume; stretch; a is the global interaction parameter; compressibility. These parameters can be temperature-dependent. deviatoric strain invariants defined as is the initial shear modulus; is the locking is an invariant mixture parameter; and D governs the are the first and second and where the deviatoric stretches defined below in “Thermal expansion”; and bulk modulus are given by ; J is the total volume ratio; is the elastic volume ratio as are the principal stretches. The initial shear modulus and Yeoh form The form of the Yeoh strain energy potential is where U is the strain energy per unit of reference volume; parameters; is the first deviatoric strain invariant defined as and are temperature-dependent material where the deviatoric stretches defined below in “Thermal expansion”; and bulk modulus are given by ; J is the total volume ratio; is the elastic volume ratio as are the principal stretches. The initial shear modulus and Thermal expansion Only isotropic thermal expansion is permitted with the hyperelastic material model. The elastic volume ratio, , relates the total volume ratio, J, and the thermal volume ratio, : is given by where thermal expansion coefficient (“Thermal expansion,” Section 26.1.2). is the linear thermal expansion strain that is obtained from the temperature and the isotropic Defining the hyperelastic material response The mechanical response of a material is defined by choosing a strain energy potential to fit the particular material. The strain energy potential forms in Abaqus are written as separable functions of a deviatoric component and a volumetric component; i.e., . Alternatively, in Abaqus/Standard you can define the strain energy potential with user subroutine UHYPER, in which case the strain energy potential need not be separable. Generally for the hyperelastic material models available in Abaqus, you can either directly specify material coefficients or provide experimental test data and have Abaqus automatically determine appropriate values of the coefficients. An exception is the Marlow form: in this case the deviatoric part of the strain energy potential must be defined with test data. The different methods for defining the strain energy potential are described in detail below. The properties of rubberlike materials can vary significantly from one batch to another; therefore, if data are used from several experiments, all of the experiments should be performed on specimens taken from the same batch of material, regardless of whether you or Abaqus compute the coefficients. Viscoelastic and hysteretic materials The elastic response of viscoelastic materials (“Time domain viscoelasticity,” Section 22.7.1, and “Parallel network viscoelastic model,” Section 22.8.2) and hysteretic materials (“Hysteresis in elastomers,” Section 22.8.1) can be specified by defining either the instantaneous response or the long-term response of such materials. To define the instantaneous response, the experiments outlined in the “Experimental tests” section that follows have to be performed within time spans much shorter than the characteristic relaxation times of these materials. Input File Usage: Abaqus/CAE Usage: *HYPERELASTIC, MODULI=INSTANTANEOUS Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; any Strain energy potential except Unknown: Moduli time scale (for viscoelasticity): Instantaneous If, on the other hand, the long-term elastic response is used, data from experiments have to be collected after time spans much longer than the characteristic relaxation times of these materials. Long- term elastic response is the default elastic material behavior. Input File Usage: Abaqus/CAE Usage: *HYPERELASTIC, MODULI=LONG TERM Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; any Strain energy potential except Unknown: Moduli time scale (for viscoelasticity): Long-term Accounting for compressibility Compressibility can be defined by specifying nonzero values for (except for the Marlow model), by setting the Poisson’s ratio to a value less than 0.5, or by providing test data that characterize the compressibility. The test data method is described later in this section. If you specify the Poisson’s ratio for hyperelasticity other than the Marlow model, Abaqus computes the initial bulk modulus from the initial shear modulus For the Marlow model the specified Poisson’s ratio represents a constant value, which determines the volumetric response throughout the deformation process. If must be equal to zero. In such a case the material is assumed to be fully incompressible in Abaqus/Standard, while Abaqus/Explicit will assume compressible behavior with (Poisson’s ratio of 0.475). is equal to zero, all of the Input File Usage: Abaqus/CAE Usage: *HYPERELASTIC, POISSON= Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; any Strain energy potential except Unknown or User-defined: Input source: Test data: Poisson's ratio: Specifying material coefficients directly The parameters of the hyperelastic strain energy potentials can be given directly as functions of temperature for all forms of the strain energy potential except the Marlow form. Input File Usage: Use one of the following options: *HYPERELASTIC, ARRUDA-BOYCE *HYPERELASTIC, MOONEY-RIVLIN *HYPERELASTIC, NEO HOOKE Abaqus/CAE Usage: ) ) *HYPERELASTIC, OGDEN, N=n ( *HYPERELASTIC, POLYNOMIAL, N=n ( *HYPERELASTIC, REDUCED POLYNOMIAL, N=n ( *HYPERELASTIC, VAN DER WAALS *HYPERELASTIC, YEOH Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; Input source: Coefficients and Strain energy potential: Arruda-Boyce, Mooney-Rivlin, Neo Hooke, Ogden, Polynomial, Reduced Polynomial, Van der Waals, or Yeoh ) Using test data to calibrate material coefficients The material coefficients of the hyperelastic models can be calibrated by Abaqus from experimental stress-strain data. In the case of the Marlow model, the test data directly characterize the strain energy potential (there are no material coefficients for this model); the Marlow model is described in detail below. The value of N and experimental stress-strain data can be specified for up to four simple tests: uniaxial, equibiaxial, planar, and, if the material is compressible, a volumetric compression test. Abaqus will then compute the material parameters. The material constants are determined through a least-squares-fit procedure, which minimizes the relative error in stress. For the n nominal-stress–nominal-strain data pairs, the relative error measure E is minimized, where is a stress value from the test data, and comes from one of the nominal stress expressions derived below . Abaqus minimizes the relative error rather than an absolute error measure since this provides a better fit at lower strains. This method is available for all strain energy potentials and any order of N except for the polynomial form, where a maximum of is allowed. The polynomial models are linear in terms of the constants ; therefore, a linear least- squares procedure can be used. The Arruda-Boyce, Ogden, and Van der Waals potentials are nonlinear in some of their coefficients, thus necessitating the use of a nonlinear least-squares procedure. “Fitting of hyperelastic and hyperfoam constants,” Section 4.6.2 of the Abaqus Theory Manual, contains a detailed derivation of the related equations. It is generally best to obtain data from several experiments involving different kinds of deformation over the range of strains of interest in the actual application and to use all of these data to determine the parameters. This is particularly true for the phenomenological models; i.e., the Ogden and the polynomial models. It has been observed that to achieve good accuracy and stability, it is necessary to fit these models using test data from more than one deformation state. In some cases, especially at large strains, removing the dependence on the second invariant may alleviate this limitation. The Arruda-Boyce, neo-Hookean, and Van der Waals models with = 0 offer a physical interpretation and provide a better prediction of general deformation modes when the parameters are based on only one test. An extensive discussion of this topic can be found in “Hyperelastic material behavior,” Section 4.6.1 of the Abaqus Theory Manual. This method does not allow the hyperelastic properties to be temperature dependent. However, if temperature-dependent test data are available, several curve fits can be conducted by performing a data check analysis on a simple input file. The temperature-dependent coefficients determined by Abaqus can then be entered directly in the actual analysis run. Optionally, the parameter in the Van der Waals model can be set to a fixed value while the other parameters are found using a least-squares curve fit. As many data points as required can be entered from each test. It is recommended that data from all four tests (on samples taken from the same piece of material) be included and that the data points cover the range of nominal strains expected to arise in the actual loading. For the (general) polynomial and Ogden models and for the coefficient in the Van der Waals model, the planar test data must be accompanied by the uniaxial test data, the biaxial test data, or both of these types of test data; otherwise, the solution to the least-squares fit will not be unique. The strain data should be given as nominal strain values (change in length per unit of original length). For the uniaxial, equibiaxial, and planar tests stress data are given as nominal stress values (force per unit of original cross-sectional area). These tests allow for entering both compression and tension data. Compressive stresses and strains are entered as negative values. If compressibility is to be specified, the or D can be computed from volumetric compression test data. Alternatively, compressibility can be defined by specifying a Poisson’s ratio, in which case Abaqus computes the bulk modulus from the initial shear modulus. If no such data are given, Abaqus/Standard assumes that D or all of the are zero, whereas Abaqus/Explicit assumes compressibility corresponding to a Poisson’s ratio of 0.475 . For these compression tests the stress data are given as pressure values. Input File Usage: Use one of the following options to select the strain energy potential: *HYPERELASTIC, TEST DATA INPUT, ARRUDA-BOYCE *HYPERELASTIC, TEST DATA INPUT, MOONEY-RIVLIN *HYPERELASTIC, TEST DATA INPUT, NEO HOOKE *HYPERELASTIC, TEST DATA INPUT, OGDEN, N=n ( ) *HYPERELASTIC, TEST DATA INPUT, POLYNOMIAL, N=n ( *HYPERELASTIC, TEST DATA INPUT, REDUCED POLYNOMIAL, N=n ( *HYPERELASTIC, TEST DATA INPUT, VAN DER WAALS *HYPERELASTIC, TEST DATA INPUT, VAN DER WAALS, BETA= ( *HYPERELASTIC, TEST DATA INPUT, YEOH In addition, use at least one and up to four of the following options to give the test data : ) ) ) *UNIAXIAL TEST DATA *BIAXIAL TEST DATA *PLANAR TEST DATA *VOLUMETRIC TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperelastic: Abaqus/CAE Usage: Material type: Isotropic; Input source: Test data and Strain energy potential: Arruda-Boyce, Mooney-Rivlin, Neo Hooke, Ogden, Polynomial, Reduced Polynomial, Van der Waals (Beta: Fitted value or Specify), or Yeoh In addition, use at least one and up to four of the following options to give the test data : Test Data→Uniaxial Test Data Test Data→Biaxial Test Data Test Data→Planar Test Data Test Data→Volumetric Test Data Alternatively, you can select Strain energy potential: Unknown to define the material temporarily without specifying a particular strain energy potential. Then select Material→Evaluate to have Abaqus/CAE evaluate the material to determine the optimal strain energy potential. Specifying the Marlow model The Marlow model assumes that the strain energy potential is independent of the second deviatoric invariant . This model is defined by providing test data that define the deviatoric behavior, and, optionally, the volumetric behavior if compressibility must be taken into account. Abaqus will construct a strain energy potential that reproduces the test data exactly, as shown in Figure 22.5.1–1. MARLOW TEST DATA Figure 22.5.1–1 The results of the Marlow model with test data. The interpolation and extrapolation of stress-strain data with the Marlow model is approximately linear for small and large strains. For intermediate strains in the range 0.1 to 1.0 a noticeable degree of nonlinearity may be observed in the interpolation/extrapolation with the Marlow model; for example, some nonlinearity is apparent between the 4th and 5th data points in Figure 22.5.1–1. To minimize undesirable nonlinearity, make sure that enough data points are specified in the intermediate strain range. The deviatoric behavior is defined by specifying uniaxial, biaxial, or planar test data. Generally, you can specify either the data from tension tests or the data from compression tests because the tests are equivalent . However, for beams, trusses, and rebars, the data from tension and compression tests can be specified together. Volumetric behavior is defined by using one of the following three methods: • Specify nominal lateral strains, in addition to nominal stresses and nominal strains, as part of the uniaxial, biaxial, or planar test data. • Specify Poisson’s ratio for the hyperelastic material. • Specify volumetric test data directly. Both hydrostatic tension and hydrostatic compression data can be specified. If only hydrostatic compression data are available, as is usually the case, Abaqus will assume that the hydrostatic pressure is an antisymmetric function of the nominal volumetric strain, . If you do not define volumetric behavior, Abaqus/Standard assumes fully incompressible behavior, while Abaqus/Explicit assumes compressibility corresponding to a Poisson’s ratio of 0.475. Material test data in which the stress does not vary smoothly with increasing strain may lead to convergence difficulty during the simulation. It is highly recommended that smooth test data be used to define the Marlow form. Abaqus provides a smoothing algorithm, which is described in detail later in this section. The test data for the Marlow model can also be given as a function of temperature and field variables. You must specify the number of user-defined field variable dependencies required. Uniaxial, biaxial, and planar test data must be given in ascending order of the nominal strains; volumetric test data must be given in descending order of the volume ratio. Input File Usage: To define the Marlow test data as a function of temperature and/or field variables, use the following option: Abaqus/CAE Usage: *HYPERELASTIC, MARLOW with one of the following first three options and, optionally, the fourth option: *UNIAXIAL TEST DATA, DEPENDENCIES=n *BIAXIAL TEST DATA, DEPENDENCIES=n *PLANAR TEST DATA, DEPENDENCIES=n *VOLUMETRIC TEST DATA, DEPENDENCIES=n Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; Input source: Test data and Strain energy potential: Marlow In addition, select one of the following first three options and, optionally, the fourth option to give the test data : Test Data→Uniaxial Test Data Test Data→Biaxial Test Data Test Data→Planar Test Data Test Data→Volumetric Test Data In each of the Test Data Editor dialog boxes, you can toggle on Use temperature-dependent data to define the test data as a function of temperature and/or select the Number of field variables to define the test data as a function of field variables. Alternatively, you can select Material→Evaluate to have Abaqus/CAE evaluate the material. If you included temperature dependencies, field variable dependencies, or lateral nominal strain in the test data—which can only be defined in the Marlow hyperelastic definition—Marlow will be the only strain energy potential available for evaluation. User subroutine specification in Abaqus/Standard An alternative method provided in Abaqus/Standard for defining the hyperelastic material parameters allows the strain energy potential to be defined in user subroutine UHYPER. Either compressible or incompressible behavior can be specified. Optionally, you can specify the number of property values needed as data in the user subroutine. The derivatives of the strain energy potential with respect to the strain invariants must be provided directly through user subroutine UHYPER. If needed, you can specify the number of solution-dependent variables . Input File Usage: Use one of the following two options: Abaqus/CAE Usage: *HYPERELASTIC, USER, TYPE=COMPRESSIBLE, PROPERTIES=n *HYPERELASTIC, USER, TYPE=INCOMPRESSIBLE, PROPERTIES=n Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; Input source: Coefficients and Strain energy potential: User-defined: optionally, toggle on Include compressibility and/or specify the Number of property values Experimental tests For a homogeneous material, homogeneous deformation modes suffice to characterize the material constants. Abaqus accepts test data from the following deformation modes: • Uniaxial tension and compression • Equibiaxial tension and compression • Planar tension and compression (also known as pure shear) • Volumetric tension and compression These modes are illustrated schematically in Figure 22.5.1–2 and are described below. The most commonly performed experiments are uniaxial tension, uniaxial compression, and planar tension. TENSION COMPRESSION UNIAXIAL TEST DATA TU, ∋ BIAXIAL TEST DATA TB, ∋ PLANAR TEST DATA TS, ∋ VOLUMETRIC TEST DATA p, 1=λ U= 1 + U , λ ∋ 2=λ 3= 1/ λ ÷ 1=λ 2=λ B= 1 + B , λ ∋ 3= 1/ λ 1=λ S= 1+ ∋ S , λ 2= 1, λ 3= 1/ λ 1=λ 2=λ 3= λ v , = λ Figure 22.5.1–2 Schematic illustrations of deformation modes. Combine data from these three test types to get a good characterization of the hyperelastic material behavior. For the incompressible version of the material model, the stress-strain relationships for the different tests are developed using derivatives of the strain energy function with respect to the strain invariants. We define these relations in terms of the nominal stress (the force divided by the original, undeformed area) and the nominal, or engineering, strain defined below. The deformation gradient, expressed in the principal directions of stretch, is , , and where configuration in the principal directions of a material fiber. The principal stretches, principal nominal strains, are the principal stretches: the ratios of current length to length in the original , are related to the , by Because we assume incompressibility and isothermal response, The deviatoric strain invariants in terms of the principal stretches are then and, hence, = 1. and Uniaxial tests The uniaxial deformation mode is characterized in terms of the principal stretches, , as where is the stretch in the loading direction. The nominal strain is defined by To derive the uniaxial nominal stress , we invoke the principle of virtual work: so that The uniaxial tension test is the most common of all the tests and is usually performed by pulling a “dog-bone” specimen. The uniaxial compression test is performed by loading a compression button between lubricated surfaces. The loading surfaces are lubricated to minimize any barreling effect in the button that would cause deviations from a homogeneous uniaxial compression stress-strain state. Input File Usage: Abaqus/CAE Usage: *UNIAXIAL TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; Input source: Test data and Test Data→Uniaxial Test Data Equibiaxial tests The equibiaxial deformation mode is characterized in terms of the principal stretches, , as where is the stretch in the two perpendicular loading directions. The nominal strain is defined by To develop the expression for the equibiaxial nominal stress, , we again use the principle of virtual work (assuming that the stress perpendicular to the loading direction is zero), so that In practice, the equibiaxial compression test is rarely performed because of experimental setup In addition, this deformation mode is equivalent to a uniaxial tension test, which is difficulties. straightforward to conduct. A more common test is the equibiaxial tension test, in which a stress state with two equal tensile stresses and zero shear stress is created. This state is usually achieved by stretching a square sheet in a biaxial testing machine. It can also be obtained by inflating a circular membrane into a spheroidal shape (like blowing up a balloon). The stress field in the middle of the membrane then closely approximates equibiaxial tension, provided that the thickness of the membrane is very much smaller than the radius of curvature at this point. However, the strain distribution will not be quite uniform, and local strain measurements will be required. Once the strain and radius of curvature are known, the nominal stress can be derived from the inflation pressure. Input File Usage: Abaqus/CAE Usage: *BIAXIAL TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; Input source: Test data and Test Data→Biaxial Test Data Planar tests The planar deformation mode is characterized in terms of the principal stretches, , as where is the stretch in the loading direction. Then, the nominal strain in the loading direction is This test is also called a “pure shear” test since, in terms of logarithmic strains, which corresponds to a state of pure shear at an angle of 45° to the loading direction. The principle of virtual work gives where is the nominal planar stress, so that For the (general) polynomial and Ogden models and for the coefficient in the Van der Waals model this equation alone will not determine the constants uniquely. The planar test data must be augmented by uniaxial test data and/or biaxial test data to determine the material parameters. Planar tests are usually done with a thin, short, and wide rectangular strip of material fixed on its wide edges to rigid loading clamps that are moved apart. If the separation direction is the 1-direction and the thickness direction is the 3-direction, the comparatively long size of the specimen in the 2-direction and the rigid clamps allow us to use the approximation ; that is, there is no deformation in the wide direction of the specimen. This deformation mode could also be called planar compression if the 3-direction is considered to be the primary direction. All forms of incompressible plane strain behavior are characterized by this deformation mode. Consequently, if plane strain analysis is performed, planar test data represent the relevant form of straining of the material. Input File Usage: Abaqus/CAE Usage: *PLANAR TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; Input source: Test data and Test Data→Planar Test Data Volumetric tests values (or D, for the Arruda-Boyce and The following discussion describes procedures for obtaining Van der Waals models) corresponding to the actual material behavior. With these values you can compare the material’s initial bulk modulus, for the polynomial model, values that will for Ogden’s model) and then judge whether , to its initial shear modulus ( provide results are sufficiently realistic. For Abaqus/Explicit caution should be used; should be less than 100. Otherwise, noisy solutions will be obtained and time increments will be excessively small . The and D can be calculated from data obtained in pure volumetric compression of a specimen (volumetric tension tests are much more difficult to perform). In a pure volumetric test (the volume ratio). Using the polynomial form of the strain energy potential, the total pressure stress on the specimen is obtained as ; therefore, and This equation can be used to determine the have curve are required to give two equations for the . If we are using a second-order polynomial series for U, we are needed. Therefore, a minimum of two points on the pressure-volume ratio . For the Ogden and reduced polynomial potentials . A linear least-squares fit is performed when more than N data can be determined for up to , and so two points are provided. An approximate way of conducting a volumetric test consists of using a cylindrical rubber specimen that fits snugly inside a rigid container and whose top surface is compressed by a rigid piston. Although both volumetric and deviatoric deformation are present, the deviatoric stresses will be several orders of magnitude smaller than the hydrostatic stresses (because the bulk modulus is much higher than the shear modulus) and can be neglected. The compressive stress imposed by the rigid piston is effectively the pressure, and the volumetric strain in the rubber cylinder is computed from the piston displacement. Nonzero values of affect the uniaxial, equibiaxial, and planar stress results. However, since the material is assumed to be only slightly compressible, the techniques described for obtaining the deviatoric coefficients should give sufficiently accurate values even though they assume that the material is fully incompressible. Input File Usage: Abaqus/CAE Usage: *VOLUMETRIC TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; Input source: Test data and Test Data→Volumetric Test Data Equivalent experimental tests The superposition of a tensile or compressive hydrostatic stress on a loaded, fully incompressible elastic body results in different stresses but does not change the deformation. Thus, Figure 22.5.1–3 shows that some apparently different loading conditions are actually equivalent in their deformations and, therefore, are equivalent tests: • Uniaxial tension • Uniaxial compression • Planar tension Equibiaxial compression Equibiaxial tension Planar compression On the other hand, the tensile and compressive cases of the uniaxial and equibiaxial modes are independent from each other: uniaxial tension and uniaxial compression provide independent data. p = -σ B = -σ + = Uniaxial tension Hydrostatic compression Equibiaxial compression p = -σ B = -σ + = Uniaxial compression Hydrostatic tension Equibiaxial tension The stresses, σi, shown here are true (Cauchy) stresses and not nominal stresses. Figure 22.5.1–3 Equivalent deformation modes through superposition of hydrostatic stress. Smoothing the test data Experimental test data often contain noise in the sense that the test variable is both slowly varying and also corrupted by random noise. This noise can affect the quality of the strain energy potential that Abaqus derives. This noise is particularly a problem with the Marlow form, where a strain energy potential that exactly describes the test data that are used to calibrate the model is computed. It is less of a concern with the other forms, since smooth functions are fitted through the test data. Abaqus provides a smoothing technique to remove the noise from the test data based on the Savitzky-Golay method. The idea is to replace each data point by a local average of its surrounding data points, so that the level of noise can be reduced without biasing the dominant trend of the test data. In the implementation a cubic polynomial is fitted through each data point i and n data points to the immediate left and right of that point. A least-squares method is used to fit the polynomial through these points. The value of data point i is then replaced by the value of the polynomial at the same position. Each polynomial is used to adjust one data point except near the ends of the curve, where a polynomial is used to adjust multiple points, because the first and last few points cannot be the center of the fitting set of data points. This process is applied repeatedly to all data points until two consecutive passes through the data produce nearly the same results. By default, the test data are not smoothed. If smoothing is specified, the default value is n=3. Alternatively, you can specify the number of data points to the left and right of a data point in the moving window within which a least-squares polynomial is fit. Input File Usage: For the Marlow form, use one of the first three options and, optionally, the fourth option; for the other potential forms, use one and up to four of the following options: Abaqus/CAE Usage: ) *UNIAXIAL TEST DATA, SMOOTH=n ( *BIAXIAL TEST DATA, SMOOTH=n ( ) *PLANAR TEST DATA, SMOOTH=n ( ) *VOLUMETRIC TEST DATA, SMOOTH=n ( Property module: material editor: Mechanical→Elasticity→Hyperelastic: Material type: Isotropic; Input source: Test data and Test Data→Uniaxial Test Data, Biaxial Test Data, Planar Test Data, or Volumetric Test Data ) In each of the Test Data Editor dialog boxes, toggle on Apply smoothing, and select a value for n ( ). Model prediction of material behavior versus experimental data Once the strain energy potential is determined, the behavior of the hyperelastic model in Abaqus is established. However, the quality of this behavior must be assessed: the prediction of material behavior under different deformation modes must be compared against the experimental data. You must judge whether the strain energy potentials determined by Abaqus are acceptable, based on the correlation between the Abaqus predictions and the experimental data. You can evaluate the hyperelastic behavior automatically in Abaqus/CAE. Alternatively, single-element test cases can be used to derive the nominal stress–nominal strain response of the material model.Single-element test cases can be used to derive the nominal stress–nominal strain response of the material model. See “Fitting of rubber test data,” Section 3.1.4 of the Abaqus Benchmarks Manual, which illustrates the entire process of fitting hyperelastic constants to a set of test data. Hyperelastic material stability An important consideration in judging the quality of the fit to experimental data is the concept of material or Drucker stability. Abaqus checks the Drucker stability of the material for the first three deformation modes described above. The Drucker stability condition for an incompressible material requires that the change in the stress, , following from any infinitesimal change in the logarithmic strain, , satisfies the inequality Using , where is the tangent material stiffness, the inequality becomes thus requiring the tangential material stiffness to be positive-definite. For an isotropic elastic formulation the inequality can be represented in terms of the principal stresses and strains, As before, since the material is assumed to be incompressible, we can choose any value for the hydrostatic pressure without affecting the strains. A convenient choice for the stability calculation is , which allows us to ignore the third term in the above equation. The relation between the changes in stress and in strain can then be obtained in the form of the matrix where that . For material stability must be positive-definite; thus, it is necessary This stability check is performed for the polynomial models, the Ogden potential, the Van der Waals ); form, and the Marlow form. The Arruda-Boyce form is always stable for positive values of ( , hence, it suffices to check the material coefficients to ensure stability. You should be careful when defining the or for the polynomial models or the Ogden form: especially when or some of the coefficients are strongly negative, instability at higher strain levels is likely to occur. , and unstable material behavior may result if these values are not defined correctly. When , the behavior at higher strains is strongly sensitive to the values of the Abaqus performs a check on the stability of the material for six different forms of loading—uniaxial tension and compression, equibiaxial tension and compression, and planar tension and compression—for . If an instability is found, Abaqus issues a warning message and prints the lowest absolute value of for which the instability is observed. Ideally, no instability occurs. If instabilities are observed at strain levels that are likely to occur in the analysis, it is strongly recommended that you either change the material model or (nominal strain range of ) at intervals carefully examine and revise the material input data. If user subroutine UHYPER is used to define the hyperelastic material, you are responsible for ensuring stability. Improving the accuracy and stability of the test data fit Unfortunately, the initial fit of the models to experimental data may not come out as well as expected. This is particularly true for the most general models, such as the (general) polynomial model and the Ogden model. For some of the simpler models, stability is assured by following some simple rules. • For positive values of the initial shear modulus, form is always stable. , and the locking stretch, , the Arruda-Boyce • For positive values of the coefficient • Given positive values of the initial shear modulus, the neo-Hookean form is always stable. , and the locking stretch, , the stability of the Van der Waals model depends on the global interaction parameter, a. • For the Yeoh model stability is assured if all will be negative, since this helps capture the S-shape feature of the stress-strain curve. Thus, reducing the absolute value of will help make the Yeoh model more stable. or magnifying the absolute value of . Typically, however, In all cases the following suggestions may improve the quality of the fit: • Both tension and compression data are allowed; compressive stresses and strains are entered as negative values. Use compression or tension data depending on the application: it is difficult to fit a single material model accurately to both tensile and compressive data. • Always use many more experimental data points than unknown coefficients. • If is used, experimental data should be available to at least 100% tensile strain or 50% compressive strain. • Perform different types of tests (e.g., compression and simple shear tests). Proper material behavior for a deformation mode requires test data to characterize that mode. • Check for warning messages about material instability or error messages about lack of convergence in fitting the test data. This check is especially important with new test data; a simple finite element model with the new test data can be run through the analysis input file processor to check the material stability. • Use the material evaluation capability in Abaqus/CAE to compare the response curves for different strain energy potentials to the experimental data. Alternatively, you can perform one-element simulations for simple deformation modes and compare the Abaqus results against the experimental data. The X–Y plotting options in the Visualization module of Abaqus/CAE can be used for this comparison. You can perform one-element simulations for simple deformation modes and compare the Abaqus results against the experimental data. • Delete some data points at very low strains if large strains are anticipated. A disproportionate number of low strain points may unnecessarily bias the accuracy of the fit toward the low strain range and cause greater errors in the large strain range. • Delete some data points at the highest strains if small to moderate strains are expected. The high strain points may force the fitting to lose accuracy and/or stability in the low strain range. • Pick data points at evenly spaced strain intervals over the expected range of strains, which will result in similar accuracy throughout the entire strain range. • The higher the order of N, the more oscillations are likely to occur, leading to instabilities in the stress-strain curves. If the (general) polynomial model is used, lower the order of N from 2 to 1 (3 to 2 for Ogden), especially if the maximum strain level is low (say, less than 100% strain). • If multiple types of test data are used and the fit still comes out poorly, some of the test data probably contain experimental errors. New tests may be needed. One way of determining which test data are erroneous is to first calibrate the initial shear modulus of the material. Then fit each type of test data separately in Abaqus and compute the shear modulus, , from the material constants using the relations Alternatively, the initial Young’s modulus, , can be calibrated and compared with The values of data. Elements or that are most different from or indicate the erroneous test The hyperelastic material model can be used with solid (continuum) elements, finite-strain shells (except S4), continuum shells, membranes, and one-dimensional elements (trusses and rebars). In Abaqus/Standard the hyperelastic material model can be also used with Timoshenko beams (B21, B22, B31, B31OS, B32, B32OS, PIPE21, PIPE22, PIPE31, PIPE32, and their “hybrid” equivalents). It cannot be used with Euler-Bernoulli beams (B23, B23H, B33, and B33H) and small-strain shells (STRI3, STRI65, S4R5, S8R, S8R5, S9R5). Pure displacement formulation versus hybrid formulation in Abaqus/Standard For continuum elements in Abaqus/Standard hyperelasticity can be used with the pure displacement formulation elements or with the “hybrid” (mixed formulation) elements. Because elastomeric materials are usually almost incompressible, fully integrated pure displacement method elements are not recommended for use with this material, except for plane stress cases. If fully or selectively reduced-integration displacement method elements are used with the almost incompressible form of this material model, a penalty method is used to impose the incompressibility constraint in anything except plane stress analysis. The penalty method can sometimes lead to numerical difficulties; therefore, the fully or selectively reduced-integrated “hybrid” formulation elements are recommended for use with hyperelastic materials. In general, an analysis using a single hybrid element will be only slightly more computationally expensive than an analysis using a regular displacement-based element. However, when the wavefront is optimized, the Lagrange multipliers may not be ordered independently of the regular degrees of freedom associated with the element. Thus, the wavefront of a very large mesh of second-order hybrid tetrahedra may be noticeably larger than that of an equivalent mesh using regular second-order tetrahedra. This may lead to significantly higher CPU costs, disk space, and memory requirements. Incompatible mode elements in Abaqus/Standard Incompatible mode elements should be used with caution in applications involving large strains. Convergence may be slow, and in hyperelastic applications inaccuracies may accumulate. Erroneous stresses may sometimes appear in incompatible mode hyperelastic elements that are unloaded after having been subjected to a complex deformation history. Procedures Hyperelasticity must always be used with geometrically nonlinear analyses (“General and linear perturbation procedures,” Section 6.1.3). 22.5.2 HYPERELASTIC BEHAVIOR IN ELASTOMERIC FOAMS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • “Energy dissipation in elastomeric foams,” Section 22.6.2 • *HYPERFOAM • *UNIAXIAL TEST DATA • *BIAXIAL TEST DATA • *PLANAR TEST DATA • *VOLUMETRIC TEST DATA • *SIMPLE SHEAR TEST DATA • *MULLINS EFFECT • “Creating a hyperfoam material model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The elastomeric foam material model: • is isotropic and nonlinear; • is valid for cellular solids whose porosity permits very large volumetric changes; • optionally allows the specification of energy dissipation and stress softening effects ; • can deform elastically to large strains, up to 90% strain in compression; and • requires that geometric nonlinearity be accounted for during the analysis step , since it is intended for finite-strain applications. Abaqus/Explicit also provides a separate foam material model intended to capture the strain-rate sensitive behavior of low-density elastomeric foams such as used in crash and impact applications . Mechanical behavior of elastomeric foams Cellular solids are made up of interconnected networks of solid struts or plates that form the edges and faces of cells. Foams are made up of polyhedral cells that pack in three dimensions. The foam cells can be either open (e.g., sponge) or closed (e.g., flotation foam). Common examples of elastomeric foam materials are cellular polymers such as cushions, padding, and packaging materials that utilize the excellent energy absorption properties of foams: the energy absorbed by foams is substantially greater than that absorbed by ordinary stiff elastic materials for a certain stress level. Another class of foam materials is crushable foams, which undergo permanent (plastic) deformation. Crushable foams are discussed in “Crushable foam plasticity models,” Section 23.3.5. Foams are commonly loaded in compression. Figure 22.5.2–1 shows a typical compressive stress- strain curve. Densification Plateau: Elastic buckling of cell walls Cell wall bending STRAIN Figure 22.5.2–1 Typical compressive stress-strain curve. Three stages can be distinguished during compression: 5%) the foam deforms in a linear elastic manner due to cell wall bending. 1. At small strains ( 2. The next stage is a plateau of deformation at almost constant stress, caused by the elastic buckling of the columns or plates that make up the cell edges or walls. In closed cells the enclosed gas pressure and membrane stretching increase the level and slope of the plateau. 3. Finally, a region of densification occurs, where the cell walls crush together, resulting in a rapid increase of compressive stress. Ultimate compressive nominal strains of 0.7 to 0.9 are typical. The tensile deformation mechanisms for small strains are similar to the compression mechanisms, but they differ for large strains. Figure 22.5.2–2 shows a typical tensile stress-strain curve. There are two stages during tension: 1. At small strains the foam deforms in a linear, elastic manner as a result of cell wall bending, similar to that in compression. 2. The cell walls rotate and align, resulting in rising stiffness. The walls are substantially aligned at a tensile strain of about . Further stretching results in increased axial strains in the walls. Cell wall alignment Cell wall bending STRAIN Figure 22.5.2–2 Typical tensile stress-strain curve. At small strains for both compression and tension, the average experimentally observed Poisson’s ratio, , of foams is 1/3. At larger strains it is commonly observed that Poisson’s ratio is effectively zero during compression: the buckling of the cell walls does not result in any significant lateral deformation. However, is nonzero during tension, which is a result of the alignment and stretching of the cell walls. The manufacture of foams often results in cells with different principal dimensions. This shape anisotropy results in different loading responses in different directions. However, the hyperfoam model does not take this kind of initial anisotropy into account. Strain energy potential In the elastomeric foam material model the elastic behavior of the foams is based on the strain energy function where N is a material parameter; , , and are temperature-dependent material parameters; and are the principal stretches. The elastic and thermal volume ratios, , by are related to the initial shear modulus, The coefficients and , are defined below. while the initial bulk modulus, , follows from For each term in the energy function, the coefficient determines the degree of compressibility. is related to the Poisson’s ratio, , by the expressions Thus, if ratio is valid for finite values of the logarithmic principal strains is the same for all terms, we have a single effective Poisson’s ratio, ; in uniaxial tension . This effective Poisson’s . Thermal expansion Only isotropic thermal expansion is permitted with the hyperfoam material model. The elastic volume ratio, and the thermal volume ratio, , relates the total volume ratio (current volume/reference volume), J, : is given by where thermal expansion coefficient (“Thermal expansion,” Section 26.1.2). is the linear thermal expansion strain that is obtained from the temperature and the isotropic Determining the hyperfoam material parameters The response of the material is defined by the parameters in the strain energy function, U; these parameters must be determined to use the hyperfoam model. Two methods are provided for defining the material parameters: you can specify the hyperfoam material parameters directly or specify test data and allow Abaqus to calculate the material parameters. The elastic response of a viscoelastic material (“Time domain viscoelasticity,” Section 22.7.1) can be specified by defining either the instantaneous response or the long-term response of such a material. To define the instantaneous response, the experiments outlined in the “Experimental tests” section that follows have to be performed within time spans much shorter than the characteristic relaxation time of the material. Input File Usage: Abaqus/CAE Usage: *HYPERFOAM, MODULI=INSTANTANEOUS Property module: material editor: Mechanical→Elasticity→Hyperfoam: Moduli time scale (for viscoelasticity): Instantaneous If, on the other hand, the long-term elastic response is used, data from experiments have to be collected after time spans much longer than the characteristic relaxation time of the viscoelastic material. Long-term elastic response is the default elastic material behavior. Input File Usage: Abaqus/CAE Usage: *HYPERFOAM, MODULI=LONG TERM Property module: material editor: Mechanical→Elasticity→Hyperfoam: Moduli time scale (for viscoelasticity): Long-term Direct specification , The default value of When the parameters N, , and is zero, which corresponds to an effective Poisson’s ratio of zero. The incompressible limit corresponds to all . However, this material model should not be used for approximately incompressible materials: use of the hyperelastic model (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1) is recommended if the effective Poisson’s ratio are specified directly, they can be functions of temperature. . Input File Usage: Abaqus/CAE Usage: Test data specification *HYPERFOAM, N=n ( Property module: material editor: Mechanical→Elasticity→Hyperfoam: Strain energy potential order: n ( on Use temperature-dependent data ); optionally, toggle ) The value of N and the experimental stress-strain data can be specified for up to five simple tests: uniaxial, equibiaxial, simple shear, planar, and volumetric. Abaqus contains a capability for obtaining the , and for the hyperfoam model with up to six terms (N=6) directly from test data. Poisson effects can be included either by means of a constant Poisson’s ratio or through specification of volumetric test data and/or lateral strains in the other test data. , It is important to recognize that the properties of foam materials can vary significantly from one batch to another. Therefore, all of the experiments should be performed on specimens taken from the same batch of material. This method does not allow the properties to be temperature dependent. As many data points as required can be entered from each test. Abaqus will then compute , . The technique uses a least squares fit to the experimental data so that the relative , and, if necessary, error in the nominal stress is minimized. It is recommended that data from the uniaxial, biaxial, and simple shear tests (on samples taken from the same piece of material) be included and that the data points cover the range of nominal strains expected to arise in the actual loading. The planar and volumetric tests are optional. For all tests the strain data, including the lateral strain data, should be given as nominal strain values (change in length per unit of original length). For the uniaxial, equibiaxial, simple shear, and planar tests, stress data are given as nominal stress values (force per unit of original cross-sectional area). The tests allow for both compression and tension data; compressive stresses and strains should be entered as negative values. For the volumetric tests the stress data are given as pressure values. Input File Usage: for all i), or Use the first option to define an effective Poisson’s ratio ( use the second option to define the lateral strains as part of the test data input: *HYPERFOAM, N=n, POISSON= , TEST DATA INPUT ( *HYPERFOAM, N=n, TEST DATA INPUT ( In addition, use at least one and up to five of these additional options to give the experimental stress-strain data : ). ) Abaqus/CAE Usage: *UNIAXIAL TEST DATA *BIAXIAL TEST DATA *PLANAR TEST DATA *SIMPLE SHEAR TEST DATA *VOLUMETRIC TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperfoam: toggle on Use test data; Strain energy potential order: n ( ); optionally, toggle on Use constant Poisson's ratio: and enter a value for the effective Poisson's ratio ( for all i) In addition, use at least one and up to five of the suboptions to give the experimental stress-strain data : Suboptions→Uniaxial Test Data Suboptions→Biaxial Test Data Suboptions→Planar Test Data Suboptions→Simple Shear Test Data Suboptions→Volumetric Test Data Experimental tests For a homogeneous material, homogeneous deformation modes suffice to characterize the material parameters. Abaqus accepts test data from the following deformation modes: • Uniaxial tension and compression • Equibiaxial tension and compression • Planar tension and compression (pure shear) • Simple shear • Volumetric tension and compression The stress-strain relations are defined in terms of the nominal stress (the force divided by the original, undeformed area) and the nominal, or engineering, strains, , are related to the principal nominal strains, . The principal stretches, , by Uniaxial, equibiaxial, and planar tests The deformation gradient, expressed in the principal directions of stretch, is , , and where are the principal stretches: the ratios of current length to length in the original configuration in the principal directions of a material fiber. The deformation modes are characterized in terms of the principal stretches, . The elastomeric foams are not incompressible, so that , are independently specified in the test data either as individual values from the measured lateral deformations or through the definition of an effective Poisson’s ratio. . The transverse stretches, , and the volume ratio, and/or The three deformation modes use a single form of the nominal stress-stretch relation, is the nominal stress and is the stretch in the loading direction. Because of the compressible where behavior, the planar mode does not result in a state of pure shear. In fact, if the effective Poisson’s ratio is zero, planar deformation is identical to uniaxial deformation. Uniaxial mode In uniaxial mode Input File Usage: Abaqus/CAE Usage: Equibiaxial mode . , , and *UNIAXIAL TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperfoam: toggle on Use test data, Suboptions→Uniaxial Test Data In equibiaxial mode Input File Usage: Abaqus/CAE Usage: . and *BIAXIAL TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperfoam: toggle on Use test data, Suboptions→Biaxial Test Data Planar mode In planar mode or biaxial test data. Input File Usage: Abaqus/CAE Usage: Simple shear tests , , and . Planar test data must be augmented by either uniaxial *PLANAR TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperfoam: toggle on Use test data, Suboptions→Planar Test Data Simple shear is described by the deformation gradient is the shear strain. For this deformation where shear deformation is shown in Figure 22.5.2–3. . A schematic illustration of simple shear strain γ = Δx fixed distance h Δx 22=TT τ =TS 11 Figure 22.5.2–3 Simple shear test. The nominal shear stress, , is where are the principal stretches in the plane of shearing, related to the shear strain by The stretch in the direction perpendicular to the shear plane is The transverse (tensile) stress, , developed during simple shear deformation due to the Poynting effect, is Input File Usage: Abaqus/CAE Usage: *SIMPLE SHEAR TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperfoam: toggle on Use test data, Suboptions→Simple Shear Test Data Volumetric tests The deformation gradient, deformation mode consists of all principal stretches being equal; , is the same for volumetric tests as for uniaxial tests. The volumetric The pressure-volumetric ratio relation is A volumetric compression test is illustrated in Figure 22.5.2–4. The pressure exerted on the foam specimen is the hydrostatic pressure of the fluid, and the decrease in the specimen volume is equal to the additional fluid entering the pressure chamber. The specimen is sealed against fluid penetration. Input File Usage: Abaqus/CAE Usage: *VOLUMETRIC TEST DATA Property module: material editor: Mechanical→Elasticity→Hyperfoam: toggle on Use test data, Suboptions→Volumetric Test Data Difference between compression and tension deformation 5%) foams behave similarly for both compression and tension. However, at For small strains ( large strains the deformation mechanisms differ for compression (buckling and crushing) and tension (alignment and stretching). Therefore, accurate hyperfoam modeling requires that the experimental data used to define the material parameters correspond to the dominant deformation modes of the problem being analyzed. If compression dominates, the pertinent tests are: • Uniaxial compression • Simple shear • Planar compression (if Poisson’s ratio ) volumetric gauge pressure gauge pump valve fluid foam rigid pressure chamber Figure 22.5.2–4 Volumetric compression test. • Volumetric compression (if Poisson’s ratio ) If tension dominates, the pertinent tests are: • Uniaxial tension • Simple shear • Biaxial tension (if Poisson’s ratio • Planar tension (if Poisson’s ratio ) ) Lateral strain data can also be used to define the compressibility of the foam. Measurement of the lateral strains may make other tests redundant; for example, providing lateral strains for a uniaxial test eliminates the need for a volumetric test. However, if volumetric test data are provided in addition to the lateral strain data for other tests, both the volumetric test data and the lateral strain data will be used in determining the compressibility of the foam. The hyperfoam model may not accurately fit Poisson’s ratio if it varies significantly between compression and tension. Model prediction of material behavior versus experimental data Once the elastomeric foam constants are determined, the behavior of the hyperfoam model in Abaqus is established. However, the quality of this behavior must be assessed: the prediction of material behavior under different deformation modes must be compared against the experimental data. You must judge whether the elastomeric foam constants determined by Abaqus are acceptable, based on the correlation between the Abaqus predictions and the experimental data. Single-element test cases can be used to calculate the nominal stress–nominal strain response of the material model. See “Fitting of elastomeric foam test data,” Section 3.1.5 of the Abaqus Benchmarks Manual, which illustrates the entire process of fitting elastomeric foam constants to a set of test data. Elastomeric foam material stability As with incompressible hyperelasticity, Abaqus checks the Drucker stability of the material for the deformation modes described above. The Drucker stability condition for a compressible material requires that the change in the Kirchhoff stress, , following from an infinitesimal change in the logarithmic strain, , satisfies the inequality where the Kirchhoff stress . Using , the inequality becomes This restriction requires that the tangential material stiffness be positive definite. For an isotropic elastic formulation the inequality can be represented in terms of the principal stresses and strains Thus, the relation between changes in the stress and changes in the strain can be obtained in the form of the matrix equation where Since must be positive definite, it is necessary that , , and : especially when You should be careful about defining the parameters , the behavior at higher strains is strongly sensitive to the values of these parameters, and unstable material behavior may result if these values are not defined correctly. When some of the coefficients are strongly negative, instability at higher strain levels is likely to occur. Abaqus performs a check on the stability of the material for nine different forms of loading—uniaxial tension and compression, equibiaxial tension and compression, simple shear, planar tension and compression, and volumetric tension and compression—for ), at intervals . If an instability is found, Abaqus issues a warning message and prints the lowest absolute value of for which the instability is observed. Ideally, no instability occurs. If instabilities are observed at strain levels that are likely to occur in the analysis, it is strongly recommended that you carefully examine and revise the material input data. (nominal strain range of Improving the accuracy and stability of the test data fit “Hyperelastic behavior of rubberlike materials,” Section 22.5.1, contains suggestions for improving the accuracy and stability of elastomeric modeling. “Fitting of elastomeric foam test data,” Section 3.1.5 of the Abaqus Benchmarks Manual, illustrates the process of fitting elastomeric foam test data. Elements The hyperfoam model can be used with solid (continuum) elements, finite-strain shells (except S4), and membranes. However, it cannot be used with one-dimensional solid elements (trusses and beams), small-strain shells (STRI3, STRI65, S4R5, S8R, S8R5, S9R5), or the Eulerian elements (EC3D8R and EC3D8RT). For continuum elements elastomeric foam hyperelasticity can be used with pure displacement formulation elements or, in Abaqus/Standard, with the “hybrid” (mixed formulation) elements. Since elastomeric foams are assumed to be very compressible, the use of hybrid elements will generally not yield any advantage over the use of purely displacement-based elements. Procedures The hyperfoam model must always be used with geometrically nonlinear analyses (“General and linear perturbation procedures,” Section 6.1.3). 22.5.3 ANISOTROPIC HYPERELASTIC BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • “Mullins effect,” Section 22.6.1 • *ANISOTROPIC HYPERELASTIC • *VISCOELASTIC • *MULLINS EFFECT • “Creating an anisotropic hyperelastic material model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The anisotropic hyperelastic material model: • provides a general capability for modeling materials that exhibit highly anisotropic and nonlinear elastic behavior (such as biomedical soft tissues, fiber-reinforced elastomers, etc.); • can be used in combination with large-strain time-domain viscoelasticity (“Time domain viscoelasticity,” Section 22.7.1); however, viscoelasticity is isotropic; • optionally allows the specification of energy dissipation and stress softening effects ; and • requires that geometric nonlinearity be accounted for during the analysis step (“General and linear perturbation procedures,” Section 6.1.3) since it is intended for finite-strain applications. Anisotropic hyperelasticity formulations Many materials of industrial and technological interest exhibit anisotropic elastic behavior due to the presence of preferred directions in their microstructure. Examples of such materials include common engineering materials (such as fiber-reinforced composites, reinforced rubber, wood, etc.) as well as soft biological tissues (arterial walls, heart tissue, etc.). When these materials are subjected to small deformations (less than 2–5%), their mechanical behavior can generally be modeled adequately using conventional anisotropic linear elasticity ( see “Defining fully anisotropic elasticity” in “Linear elastic behavior,” Section 22.2.1). Under large deformations, however, these materials exhibit highly anisotropic and nonlinear elastic behavior due to rearrangements in the microstructure, such as reorientation of the fiber directions with deformation. The simulation of these nonlinear large-strain effects calls for more advanced constitutive models formulated within the framework of anisotropic hyperelasticity. Hyperelastic materials are described in terms of a “strain energy potential,” , which defines the strain energy stored in the material per unit of reference volume (volume in the initial configuration) as a function of the deformation at that point in the material. Two distinct formulations are used for the representation of the strain energy potential of anisotropic hyperelastic materials: strain-based and invariant-based. Strain-based formulation In this case the strain energy function is expressed directly in terms of the components of a suitable strain tensor, such as the Green strain tensor : where is the deformation gradient; and is the identity matrix. Without loss of generality, the strain energy function can be written in the form is the right Cauchy-Green strain tensor; is Green’s strain; where right Cauchy-Green strain; as defined below in “Thermal expansion.” is the modified Green strain tensor; is the total volume change; and is the distortional part of the is the elastic volume ratio The underlying assumption in models based on the strain-based formulation is that the preferred material directions are initially aligned with an orthogonal coordinate system in the reference (stress-free) configuration. These directions may become non-orthogonal only after deformation. Examples of this form of strain energy function include the generalized Fung-type form described below. Invariant-based formulation Using the continuum theory of fiber-reinforced composites (Spencer, 1984) the strain energy function can be expressed directly in terms of the invariants of the deformation tensor and fiber directions. For example, consider a composite material that consists of an isotropic hyperelastic matrix reinforced with families of fibers. The directions of the fibers in the reference configuration are characterized by a set ). Assuming that the strain energy depends not only on deformation, of unit vectors but also on the fiber directions, the following form is postulated , ( The strain energy of the material must remain unchanged if both matrix and fibers in the reference configuration undergo a rigid body rotation. Then, following Spencer (1984), the strain energy can be expressed in terms of an irreducible set of scalar invariants that form the integrity basis of the tensor and the vectors : where and third strain invariant); are the first and second deviatoric strain invariants; are the pseudo-invariants of and is the elastic volume ratio (or , ; and , defined as: The terms between the directions of any two families of fibers in the reference configuration: are geometrical constants (independent of deformation) equal to the cosine of the angle Unlike for the case of the strain-based formulation, in the invariant-based formulation the fiber directions need not be orthogonal in the initial configuration. An example of an invariant-based energy function is the form proposed by Holzapfel, Gasser, and Ogden (2000) for arterial walls . Anisotropic strain energy potentials There are two forms of strain energy potentials available in Abaqus to model approximately incompressible anisotropic materials: the generalized Fung form (including fully anisotropic and orthotropic cases) and the form proposed by Holzapfel, Gasser, and Ogden for arterial walls. Both forms are adequate for modeling soft biological tissue. However, whereas Fung’s form is purely phenomenological, the Holzapfel-Gasser-Ogden form is micromechanically based. In addition, Abaqus provides a general capability to support user-defined forms of the strain energy potential via two sets of user subroutines: one for strain-based and one for invariant-based formulations. Generalized Fung form The generalized Fung strain energy potential has the following form: where U is the strain energy per unit of reference volume; parameters; is the elastic volume ratio as defined below in “Thermal expansion”; and and D are temperature-dependent material is defined as where be temperature dependent and is a dimensionless symmetric fourth-order tensor of anisotropic material constants that can are the components of the modified Green strain tensor. The initial deviatoric elasticity tensor, , and bulk modulus, , are given by Abaqus supports two forms of the generalized Fung model: fully anisotropic and orthotropic. The that must be specified depends on the level of anisotropy of the number of independent components material: 21 for the fully anisotropic case and 9 for the orthotropic case. Input File Usage: Use one of the following options: *ANISOTROPIC HYPERELASTIC, FUNG-ANISOTROPIC *ANISOTROPIC HYPERELASTIC, FUNG-ORTHOTROPIC Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Hyperelastic; Material type: Anisotropic; Strain energy potential: Fung- Anisotropic or Fung-Orthotropic Holzapfel-Gasser-Ogden form The form of the strain energy potential is based on that proposed by Holzapfel, Gasser, and Ogden (2000) and Gasser, Ogden, and Holzapfel (2006) for modeling arterial layers with distributed collagen fiber orientations: with where U is the strain energy per unit of reference volume; dependent material parameters; strain invariant; pseudo-invariants of , D, is the number of families of fibers ( and . is the elastic volume ratio as defined below in “Thermal expansion” and , , and ); are temperature- is the first deviatoric are The model assumes that the directions of the collagen fibers within each family are dispersed (with ) describes the is the orientation density function that characterizes rotational symmetry) about a mean preferred direction. The parameter level of dispersion in the fiber directions. If the distribution (it represents the normalized number of fibers with orientations in the range with respect to the mean direction), the parameter is defined as ( It is also assumed that all families of fibers have the same mechanical properties and the same dispersion. When the fibers are randomly distributed and the material becomes isotropic; this corresponds to a spherical orientation density function. the fibers are perfectly aligned (no dispersion). When The strain-like quantity characterizes the deformation of the family of fibers with mean direction . For perfectly aligned fibers ( ), . ), ; and for randomly distributed fibers ( The first two terms in the expression of the strain energy function represent the distortional and volumetric contributions of the non-collagenous isotropic ground material, and the third term represents the contributions from the different families of collagen fibers, taking into account the effects of dispersion. A basic assumption of the model is that collagen fibers can support tension only, because they would buckle under compressive loading. Thus, the anisotropic contribution in the strain energy function appears only when the strain of the fibers is positive or, equivalently, when . This condition is enforced by the term stands for the Macauley bracket and is defined as , where the operator . See “Anisotropic hyperelastic modeling of arterial layers,” Section 3.1.7 of the Abaqus Benchmarks Manual, for an example of an application of the Holzapfel-Gasser-Ogden energy potential to model arterial layers with distributed collagen fiber orientation. The initial deviatoric elasticity tensor, , and bulk modulus, , are given by where is the fourth-order unit tensor, and is the Heaviside unit step function. Input File Usage: *ANISOTROPIC HYPERELASTIC, HOLZAPFEL, LOCAL DIRECTIONS=N Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Hyperelastic; Material type: Anisotropic; Strain energy potential: Holzapfel, Number of local directions: N User-defined form: strain-based Alternatively, you can define the form of a strain-based strain energy potential directly with user subroutine UANISOHYPER_STRAIN in Abaqus/Standard or VUANISOHYPER_STRAIN in Abaqus/Explicit. The derivatives of the strain energy potential with respect to the components of the modified Green strain and the elastic volume ratio, , must be provided directly through these user subroutines. Either compressible or incompressible behavior can be specified in Abaqus/Standard; only nearly incompressible behavior is allowed in Abaqus/Explicit. Optionally, you can specify the number of property values needed as data in the user subroutine as well as the number of solution-dependent variables . Input File Usage: In Abaqus/Standard use the following option to define compressible behavior: *ANISOTROPIC HYPERELASTIC, USER, FORMULATION=STRAIN, TYPE=COMPRESSIBLE, PROPERTIES=n In Abaqus/Standard use the following option to define incompressible behavior: *ANISOTROPIC HYPERELASTIC, USER, FORMULATION=STRAIN, TYPE=INCOMPRESSIBLE, PROPERTIES=n In Abaqus/Explicit use the following option to define nearly incompressible behavior: *ANISOTROPIC HYPERELASTIC, USER, FORMULATION=STRAIN, PROPERTIES=n Property module: material editor: Mechanical→Elasticity→Hyperelastic; Material type: Anisotropic, Strain energy potential: User, Formulation: Strain, Type: Incompressible or Compressible, Number of property values: n Abaqus/CAE Usage: User-defined form: invariant-based Alternatively, you can define the form of an invariant-based strain energy potential directly with user subroutine UANISOHYPER_INV in Abaqus/Standard or VUANISOHYPER_INV in Abaqus/Explicit. Either compressible or incompressible behavior can be specified in Abaqus/Standard; only nearly incompressible behavior is allowed in Abaqus/Explicit. Optionally, you can specify the number of property values needed as data in the user subroutine and the number of solution-dependent variables . The derivatives of the strain energy potential with respect to the strain invariants must be provided directly through user subroutine UANISOHYPER_INV in Abaqus/Standard and VUANISOHYPER_INV in Abaqus/Explicit. Input File Usage: In Abaqus/Standard use the following option to define compressible behavior: *ANISOTROPIC HYPERELASTIC, USER, FORMULATION=INVARIANT, LOCAL DIRECTIONS=N, TYPE=COMPRESSIBLE, PROPERTIES=n In Abaqus/Standard use the following option to define incompressible behavior: *ANISOTROPIC HYPERELASTIC, USER, FORMULATION=INVARIANT, LOCAL DIRECTIONS=N, TYPE=INCOMPRESSIBLE, PROPERTIES=n In Abaqus/Explicit use the following option to define nearly incompressible behavior: *ANISOTROPIC HYPERELASTIC, USER, FORMULATION=INVARIANT, PROPERTIES=n Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Hyperelastic; Material type: Anisotropic, Strain energy potential: User, Formulation: Invariant, Type: Incompressible or Compressible, Number of local directions: N, Number of property values: n Definition of preferred material directions You must define the preferred material directions (or fiber directions) of the anisotropic hyperelastic material. For strain-based forms (such as the Fung form and user-defined forms using user subroutines UANISOHYPER_STRAIN or VUANISOHYPER_STRAIN), you must specify a local orientation system (“Orientations,” Section 2.2.5) to define the directions of anisotropy. Components of the modified Green strain tensor are calculated with respect to this system. For invariant-based forms of the strain energy function (such as the Holzapfel form and user-defined forms using user subroutines UANISOHYPER_INV or VUANISOHYPER_INV), you must specify the local direction vectors, , that characterize each family of fibers. These vectors need not be orthogonal in the initial configuration. Up to three local directions can be specified as part of the definition of a local orientation system (“Defining a local coordinate system directly” in “Orientations,” Section 2.2.5); the local directions are referred to this system. In Abaqus/CAE, the local direction vectors of the material are orthogonal and align with the axes of the assigned material orientation. The best practice is to assign the orientation using discrete orientations in Abaqus/CAE. Material directions can be output to the output database as described in “Output,” below. Compressibility Most soft tissues and fiber-reinforced elastomers have very little compressibility compared to their shear flexibility. This behavior does not warrant special attention for plane stress, shell, or membrane elements, but the numerical solution can be quite sensitive to the degree of compressibility for three-dimensional solid, plane strain, and axisymmetric elements. In cases where the material is highly confined (such as an O-ring used as a seal), the compressibility must be modeled correctly to obtain accurate results. In applications where the material is not highly confined, the degree of compressibility is typically not crucial; for example, it would be quite satisfactory in Abaqus/Standard to assume that the material is fully incompressible: the volume of the material cannot change except for thermal expansion. Compressibility in Abaqus/Standard In Abaqus/Standard the use of “hybrid” (mixed formulation) elements is required for incompressible materials. In plane stress, shell, and membrane elements the material is free to deform in the thickness direction. In this case special treatment of the volumetric behavior is not necessary; the use of regular stress/displacement elements is satisfactory. Compressibility in Abaqus/Explicit With the exception of the plane stress case, it is not possible to assume that the material is fully incompressible in Abaqus/Explicit because the program has no mechanism for imposing such a constraint at each material calculation point. Instead, some compressibility must be modeled. The difficulty is that, in many cases, the actual material behavior provides too little compressibility for the algorithms to work efficiently. Thus, except for the plane stress case, you must provide enough compressibility for the code to work, knowing that this makes the bulk behavior of the model softer than that of the actual material. Failing to provide enough compressibility may introduce high frequency noise into the dynamic solution and require the use of excessively small time increments. Some judgment is, therefore, required to decide whether or not the solution is sufficiently accurate or whether the problem can be modeled at all with Abaqus/Explicit because of this numerical limitation. If no value is given for the material compressibility of the anisotropic hyperelastic model, by default Abaqus/Explicit assumes the value is the largest value of the initial shear , where modulus (among the different material directions). The exception is for the case of user-defined forms, where some compressibility must be defined directly within user subroutine UANISOHYPER_INV or VUANISOHYPER_INV. Thermal expansion Both isotropic and orthotropic thermal expansion is permitted with the anisotropic hyperelastic material model. The elastic volume ratio, , relates the total volume ratio, J, and the thermal volume ratio, : is given by where thermal expansion coefficients (“Thermal expansion,” Section 26.1.2). are the principal thermal expansion strains that are obtained from the temperature and the Viscoelasticity Anisotropic hyperelastic models can be used in combination with isotropic viscoelasticity to model rate- dependent material behavior (“Time domain viscoelasticity,” Section 22.7.1). Because of the isotropy of viscoelasticity, the relaxation function is independent of the loading direction. This assumption may not be acceptable for modeling materials that exhibit strong anisotropy in their rate-dependent behavior; therefore, this option should be used with caution. The anisotropic hyperelastic response of rate-dependent materials (“Time domain viscoelasticity,” Section 22.7.1) can be specified by defining either the instantaneous response or the long-term response of such materials. Input File Usage: Use either of the following options: Abaqus/CAE Usage: *ANISOTROPIC HYPERELASTIC, MODULI=INSTANTANEOUS *ANISOTROPIC HYPERELASTIC, MODULI=LONG TERM Property module: material editor: Mechanical→Elasticity→Hyperelastic; Material type: Anisotropic; Moduli: Long term or Instantaneous Stress softening The response of typical anisotropic hyperelastic materials, such as reinforced rubbers and biological tissues, under cyclic loading and unloading usually displays stress softening effects during the first few cycles. After a few cycles the response of the material tends to stabilize and the material is said to be pre- conditioned. Stress softening effects, often referred to in the elastomers literature as Mullins effect, can be accounted for by using the anisotropic hyperelastic model in combination with the pseudo-elasticity model for Mullins effect in Abaqus . The stress softening effects provided by this model are isotropic. Elements The anisotropic hyperelastic material model can be used with solid (continuum) elements, finite-strain shells (except S4), continuum shells, and membranes. When used in combination with elements with plane stress formulations, Abaqus assumes fully incompressible behavior and ignores any amount of compressibility specified for the material. Pure displacement formulation versus hybrid formulation in Abaqus/Standard For continuum elements in Abaqus/Standard anisotropic hyperelasticity can be used with the pure displacement formulation elements or with the “hybrid” (mixed formulation) elements. Pure displacement formulation elements must be used with compressible materials, and “hybrid” (mixed formulation) elements must be used with incompressible materials. In general, an analysis using a single hybrid element will be only slightly more computationally expensive than an analysis using a regular displacement-based element. However, when the wavefront is optimized, the Lagrange multipliers may not be ordered independently of the regular degrees of freedom associated with the element. Thus, the wavefront of a very large mesh of second-order hybrid tetrahedra may be noticeably larger than that of an equivalent mesh using regular second-order tetrahedra. This may lead to significantly higher CPU costs, disk space, and memory requirements. Incompatible mode elements in Abaqus/Standard Incompatible mode elements should be used with caution in applications involving large strains. Convergence may be slow, and in hyperelastic applications inaccuracies may accumulate. Erroneous stresses may sometimes appear in incompatible mode anisotropic hyperelastic elements that are unloaded after having been subjected to a complex deformation history. Procedures Anisotropic hyperelasticity must always be used with geometrically nonlinear analyses (“General and linear perturbation procedures,” Section 6.1.3). Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), local material directions will be output whenever element field output is requested to the output database. The local directions are output as field variables (LOCALDIR1, LOCALDIR2, LOCALDIR3) representing the direction cosines; these variables can be visualized as vector plots in the Visualization module of Abaqus/CAE (Abaqus/Viewer). Output of local material directions is suppressed if no element field output is requested or if you specify not to have element material directions written to the output database . Additional references • Gasser, T. C., R. W. Ogden, and G. A. Holzapfel, “Hyperelastic Modelling of Arterial Layers with Distributed Collagen Fibre Orientations,” Journal of the Royal Society Interface, vol. 3, pp. 15–35, 2006. • Holzapfel, G. A., T. C. Gasser, and R. W. Ogden, “A New Constitutive Framework for Arterial Wall Mechanics and a Comparative Study of Material Models,” Journal of Elasticity, vol. 61, pp. 1–48, 2000. • Spencer, A. J. M., “Constitutive Theory for Strongly Anisotropic Solids,” A. J. M. Spencer (ed.), Continuum Theory of the Mechanics of Fibre-Reinforced Composites, CISM Courses and Lectures No. 282, International Centre for Mechanical Sciences, Springer-Verlag, Wien, pp. 1–32, 1984. 22.6 Stress softening in elastomers • “Mullins effect,” Section 22.6.1 • “Energy dissipation in elastomeric foams,” Section 22.6.2 22.6.1 MULLINS EFFECT Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Combining material behaviors,” Section 21.1.3 • “Elastic behavior: overview,” Section 22.1.1 • “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 • “Anisotropic hyperelastic behavior,” Section 22.5.3 • “Permanent set in rubberlike materials,” Section 23.7.1 • “Energy dissipation in elastomeric foams,” Section 22.6.2 • *HYPERELASTIC • *MULLINS EFFECT • *PLASTIC • *UNIAXIAL TEST DATA • *BIAXIAL TEST DATA • *PLANAR TEST DATA • “Mullins effect” in “Defining damage,” Section 12.9.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The Mullins effect model: • is intended for modeling stress softening of filled rubber elastomers under quasi-static cyclic loading, a phenomenon referred to in the literature as Mullins effect; • provides an extension to the well-known isotropic hyperelastic models; • is based on the theory of incompressible isotropic elasticity modified by the addition of a single variable, referred to as the damage variable; • assumes that only the deviatoric part of the material response is associated with damage; • is intended for modeling material response in situations where different parts of the model undergo different levels of damage resulting in a different material response; • is applied to the long-term modulus when combined with viscoelasticity; and • cannot be used with hysteresis. Abaqus provides a similar capability that can be applied to elastomeric foams . Material behavior The real behavior of filled rubber elastomers under cyclic loading conditions is quite complex. Certain idealizations have been made for modeling purposes. In essence, these idealizations result in two main components to the material behavior: the first component describes the response of a material point (from an undeformed state) under monotonic straining, and the second component is associated with damage and describes the unloading-reloading behavior. The idealized response and the two components are described in the following sections. Idealized material behavior When an elastomeric test specimen is subjected to simple tension from its virgin state, unloaded, and then reloaded, the stress required on reloading is less than that on the initial loading for stretches up to the maximum stretch achieved during the initial loading. This stress softening phenomenon is known as the Mullins effect and reflects damage incurred during previous loading. This type of material response is depicted qualitatively in Figure 22.6.1–1. c' b' stretch Figure 22.6.1–1 Idealized response of the Mullins effect model. This figure and the accompanying description is based on work by Ogden and Roxburgh (1999), which forms the basis of the model implemented in Abaqus. Consider the primary loading path of a previously unstressed material, with loading to an arbitrary point . On unloading from , the path . If further is a continuation of the primary loading path (which is the path that would be followed if there was no unloading). If loading is now stopped on reloading. If no further is followed. When the material is loaded again, the softened path is retraced as is followed, where is followed on unloading and then retraced back to loading is then applied, the path , the path at is applied, the curve loading beyond elastic. For loading beyond represents the subsequent material response, which is then , the primary path is again followed and the pattern described is repeated. This is an ideal representation of Mullins effect since in practice there is some permanent set upon unloading and/or viscoelastic effects such as hysteresis. Points such as and may not exist in reality in the sense that unloading from the primary curve followed by reloading to the maximum strain level attained earlier usually results in a stress that is somewhat lower than the stress corresponding to the primary curve. In addition, the cyclic response for some filled elastomers shows evidence of progressive damage during unloading from and subsequent reloading to a certain maximum strain level. Such progressive damage usually occurs during the first few cycles, and the material behavior soon stabilizes to a loading/unloading cycle that is followed beyond the first few cycles. More details regarding the actual behavior and how test data that display such behavior can be used to calibrate the Abaqus model for Mullins effect are discussed later and in “Analysis of a solid disc with Mullins effect and permanent set,” Section 3.1.7 of the Abaqus Example Problems Manual. The loading path will henceforth be referred to as the “primary hyperelastic behavior.” The primary hyperelastic behavior is defined by using a hyperelastic material model. Stress softening is interpreted as being due to damage at the microscopic level. As the material is loaded, the damage occurs by the severing of bonds between filler particles and the rubber molecular chains. Different chain links break at different deformation levels, thereby leading to continuous damage with macroscopic deformation. An equivalent interpretation is that the energy required to cause the damage is not recoverable. Primary hyperelastic behavior Hyperelastic materials are described in terms of a “strain energy potential” function that defines the strain energy stored in the material per unit reference volume (volume in the initial configuration). The quantity is the deformation gradient tensor. To account for Mullins effect, Ogden and Roxburgh propose a material description that is based on an energy function of the form , where the additional scalar variable, , represents damage in the material. The damage variable controls the material properties in the sense that it enables the material response to be governed by an energy function on unloading and subsequent submaximal reloading different from that on the primary (initial) loading path from a virgin state. Because of the above interpretation of , it is no longer appropriate to think of U as the stored elastic energy potential. Part of the energy is stored as strain energy, while the rest is dissipated due to damage. The shaded area in Figure 22.6.1–1 represents the energy dissipated by damage as a result of deformation until the point , while the unshaded part represents the recoverable strain energy. The following paragraphs provide a summary of the Mullins effect model in Abaqus. For further details, see “Mullins effect,” Section 4.7.1 of the Abaqus Theory Manual. In preparation for writing the constitutive equations for Mullins effect, it is useful to separate the deviatoric and the volumetric parts of the total strain energy density as In the above equation U, are the total, deviatoric, and volumetric parts of the strain energy density, respectively. All the hyperelasticity models in Abaqus use strain energy potential functions that are already separated into deviatoric and volumetric parts. For example, the polynomial models use a strain energy potential of the form , and where the symbols have the usual interpretations. The first term on the right represents the deviatoric part of the elastic strain energy density function, and the second term represents the volumetric part. Modified strain energy density function The Mullins effect is accounted for by using an augmented energy function of the form is a continuous function of the damage variable is the deviatoric part of the strain energy density of the primary hyperelastic behavior, where defined, for example, by the first term on the right-hand-side of the polynomial strain energy function given above; is the volumetric part of the strain energy density, defined, for example, by the second term on the right-hand-side of the polynomial strain energy function given above; represent the deviatoric principal stretches; and represents the elastic volume ratio. The function and is referred to as the “damage function.” When the deformation state of the material is on a point on the curve that represents the primary hyperelastic behavior, , and the augmented energy function reduces to the strain energy density function of the primary hyperelastic behavior. The damage variable varies continuously during the course of the deformation and always satisfies . The above form of the energy function is an extension of the form proposed by Ogden and Roxburgh to account for material compressibility. , , Stress computation With the above modification to the energy function, the stresses are given by and is the deviatoric stress corresponding to the primary hyperelastic behavior at the current where deviatoric deformation level is the hydrostatic pressure of the primary hyperelastic behavior at the current volumetric deformation level . Thus, the deviatoric stress as a result of Mullins effect is obtained by simply scaling the deviatoric stress of the primary hyperelastic behavior with the damage variable . The pressure stress is the same as that of the primary behavior. The model predicts loading/unloading along a single curve (that is different, in general, from the primary hyperelastic behavior) from any given strain level that passes through the origin of the stress-strain plot. It cannot capture permanent strains upon removal of load. The model also predicts that a purely volumetric deformation will not have any damage or Mullins effect associated with it. Damage variable The damage variable, , varies with the deformation according to where m are material parameters; and is the maximum value of at a material point during its deformation history; r, , and is the error function defined as When its minimum value, , given by , corresponding to a point on the primary curve, . On the other hand, attains and . While the parameters r and . For all intermediate values of varies upon removal of deformation, when monotonically between are dimensionless, the parameter m has the dimensions of energy. The equation for reduces to that proposed by Ogden and Roxburgh when . The material parameters may be specified directly or may be computed by Abaqus based on curve-fitting of unloading-reloading test data. These parameters are subject to the restrictions and m cannot both be zero). Alternatively, the damage can be defined through user subroutine UMULLINS in Abaqus/Standard and VUMULLINS in (the parameters , and , , variable Abaqus/Explicit. If the parameter and the parameter m has a value that is small compared to , the slope of the stress-strain curve at the initiation of unloading from relatively large strain levels may become very high. As a result, the response may become discontinuous, as illustrated in Figure 22.6.1–2. This kind of behavior may lead to convergence problems in Abaqus/Standard. In Abaqus/Explicit the high stiffness will lead to very small stable time increments, thereby leading to a degradation in performance. This problem can be avoided by choosing a small value for can be used to define the original Ogden-Roxburgh model. In Abaqus/Standard the default value of is 0. In Abaqus/Explicit, however, the default value of , it is assumed to be 0 in Abaqus/Standard and 0.1 in Abaqus/Explicit. is 0.1. Thus, if you do not specify a value for . The choice The parameters r, , and m do not have direct physical interpretations in general. The parameter m controls whether damage occurs at low strain levels. If , there is a significant amount of damage at low strain levels. On the other hand, a nonzero m leads to little or no damage at low strain levels. For further discussion regarding the implications of this model to the energy dissipation, see “Mullins ' ' stretch Figure 22.6.1–2 Overly stiff response at the initiation of unloading. effect,” Section 4.7.1 of the Abaqus Theory Manual. The qualitative effects of varying the parameters r and individually, while holding the other parameters fixed, are shown in Figure 22.6.1–3. σ~ η (β ) m 2 η (β ) m 1 σ~ σ~ increasing r increasing β stretch stretch Figure 22.6.1–3 Qualitative dependence of damage on material properties. The left figure shows the unloading-reloading curve from a certain maximum strain level for increasing values of r. It suggests that the parameter r controls the amount of damage, with decreasing damage for increasing r. This behavior follows from the fact that the larger the value of r, the less the damage variable can deviate from unity. The figure on the right shows the unloading-reloading curve from a certain maximum strain level for increasing values of also leads to lower amounts of damage. It also shows that the unloading-reloading response approaches the asymptotic response given by . . The figure suggests that increasing , faster for lower values of is the minimum value of , where values of r and m, . In particular, if is a function of , MULLINS EFFECT ( and ). For fixed The above relation is approximately true if is much greater than m. Specifying the Mullins effect material model in Abaqus The primary hyperelastic behavior is defined by using the hyperelastic material model . The Mullins effect model can be defined by specifying the Mullins effect parameters directly or by using test data to calibrate the parameters. Alternatively, you can define the Mullins effect model with user subroutine UMULLINS in Abaqus/Standard and VUMULLINS in Abaqus/Explicit. Specifying the parameters directly The parameters r, m, and field variables. Input File Usage: Abaqus/CAE Usage: of the Mullins effect can be given directly as functions of temperature and/or *MULLINS EFFECT Property module: material editor: Mechanical→Damage for Elastomers→Mullins Effect: Definition: Constants Using test data to calibrate the parameters Experimental unloading-reloading data from different strain levels can be specified for up to three simple tests: uniaxial, biaxial, and planar. Abaqus will then compute the material parameters using a nonlinear least-squares curve fitting algorithm. It is generally best to obtain data from several experiments involving different kinds of deformation over the range of strains of interest in the actual application and to use all these data to determine the parameters. It is also important to obtain a good curve-fit for the primary hyperelastic behavior if the primary behavior is defined using test data. . In this case the parameters m and By default, Abaqus attempts to fit all three parameters to the given data. This is possible in general, except in the situation when the test data correspond to unloading-reloading from only a single value of cannot be determined independently; one of them must be specified. If you specify neither m nor , Abaqus needs to assume a default value for one of these parameters. In light of the potential problems discussed earlier with in the above situation. The curve-fitting may also be carried out by specifying any one or two of the material parameters to be fixed, predetermined values. , Abaqus assumes that As many data points as required can be entered from each test. It is recommended that data from all three tests (on samples taken from the same piece of material) be included and that the data points cover unloading/reloading from/to the range of nominal strain expected to arise in the actual loading. The strain data should be given as nominal strain values (change in length per unit of original length). The stress data should be given as nominal stress values (force per unit of original cross-sectional area). These tests allow for entering both compression and tension data. Compressive stresses and strains are entered as negative values. For each set of test input, the data point with the maximum nominal strain identifies the point of unloading. This point is used by the curve-fitting algorithm to compute for that curve. Figure 22.6.1–4 shows some typical unloading-reloading data from three different strain levels. Nominal Strain Figure 22.6.1–4 Typical available test data for Mullins effect. The data include multiple loading and unloading cycles from each strain level. As Figure 22.6.1–4 indicates, the loading/unloading cycles from any given strain level do not occur along a single curve, and there is some amount of hysteresis. There is also some amount of permanent set upon removal of the applied load. The data also show evidence of progressive damage with repeated cycling at any given maximum strain level. The response appears to stabilize after a number of cycles. When such data are used to calibrate the Mullins effect model, the resulting response will capture the overall stiffness characteristics, while ignoring effects such as hysteresis, permanent set, or progressive damage. The above data can be provided to Abaqus in the following manner: • The primary curve can be made up of the data points indicated by the dashed curve in Figure 22.6.1–4. Essentially, this consists of an envelope of the first loading curves to the different strain levels. • The unloading-reloading curves from the three different strain levels can be specified by providing the data points as is; i.e., as the repeated unloading-reloading cycles shown in Figure 22.6.1–4. As discussed earlier, the data from the different strain levels need to be distinguished by providing them as different tables. For example, assuming that the test data correspond to the uniaxial tension state, three tables of uniaxial test data would have to be defined for the three different strain levels shown in Figure 22.6.1–4. In this case Abaqus will provide a best fit using all the data points (from all strain levels). The resulting fit would result in a response that is an average of all the test data at any given strain level. While permanent set may be modeled , hysteresis will be lost in the process. • Alternatively, you may provide any one unloading-reloading cycle from each different strain level. If the component is expected to undergo repeated cyclic loading, the latter may be, for example, the stabilized cycle at each strain level. On the other hand, if the component is expected to undergo predominantly monotonic loading with perhaps small amounts of unloading, the very first unloading curve at each strain level may be the appropriate input data for calibrating the Mullins coefficients. Once the Mullins effect constants are determined, the behavior of the Mullins effect model in the prediction of Abaqus is established. However, the quality of this behavior must be assessed: material behavior under different deformation modes must be compared against the experimental data. You must judge whether the Mullins effect constants determined by Abaqus are acceptable, based on the correlation between the Abaqus predictions and the experimental data. Single-element test cases can be used to derive the nominal stress–nominal strain response of the material model. The steps that can be taken for improving the quality of the fit for the Mullins effect parameters are similar in essence to the guidelines provided for curve fitting the primary hyperelastic behavior . In addition, the quality of the fit for the Mullins effect parameters depends on a good fit for the primary hyperelastic behavior, if the primary behavior is defined using test data. The quality of the fit can be evaluated by carrying out a numerical experiment with a single element that is loaded in the same mode for which test data has been provided. Alternatively, the numerical response for both the primary and the softening behavior can be obtained by requesting model definition data output and carrying out a data check analysis. The response computed by Abaqus is printed in the data (.dat) file along with the experimental data. This tabular data can be plotted in Abaqus/CAE for comparison and evaluation purposes. The primary hyperelastic behavior can also be evaluated with the automated material evaluation tools in Abaqus/CAE. Input File Usage: *MULLINS EFFECT, TEST DATA INPUT, BETA and/or M and/or R In addition, use at least one and up to three of the following options to give the unloading-reloading test data : *UNIAXIAL TEST DATA *BIAXIAL TEST DATA *PLANAR TEST DATA Abaqus/CAE Usage: Multiple unloading-reloading curves from different strain levels for any given test type can be entered by repeated specification of the appropriate test data option. Property module: material editor: Mechanical→Damage for Elastomers→Mullins Effect: Definition: Test Data Input: enter the values for up to two of the values r, m, and beta. In addition, select and enter data for at least one of the following: Add Test→Biaxial Test, Planar Test, or Uniaxial Test User subroutine specification An alternative method for defining the Mullins effect involves defining the damage variable in user subroutine UMULLINS in Abaqus/Standard and VUMULLINS in Abaqus/Explicit. Optionally, you can specify the number of property values needed as data in the user subroutine. You must provide the damage variable, . The latter contributes to the Jacobian of the overall system of equations and is necessary to ensure good convergence characteristics in Abaqus/Standard. If needed, you can specify the number of solution-dependent variables (“User subroutines: overview,” Section 18.1.1). These solution-dependent variables can be updated in the user subroutine. The damage dissipation energy and the recoverable part of the energy may also be defined for output purposes. , and its derivative, User subroutines UMULLINS and VUMULLINS can be used in combination with all hyperelastic potentials in Abaqus, including user-defined potentials (via user subroutines UHYPER, UANISOHYPER_INV, and UANISOHYPER_STRAIN Abaqus/Standard, and VUANISOHYPER_INV and VUANISOHYPER_STRAIN in Abaqus/Explicit). Input File Usage: Abaqus/CAE Usage: *MULLINS EFFECT, USER, PROPERTIES=constants Property module: material editor: Mechanical→Damage for Elastomers→Mullins Effect: Definition: User Defined Viscoelasticity When viscoelasticity is used in combination with Mullins effect, stress softening is applied to the long- term behavior. In this case specification of the parameter (which has units of energy) should be done carefully. If the underlying hyperelastic behavior is defined with an instantaneous modulus, will be interpreted to be instantaneous. Otherwise, is considered to be long term. Elements The Mullins effect material model can be used with all element types that support the use of the hyperelastic material model. Procedures The Mullins effect material model can be used in all procedure types that support the use of the hyperelastic material model. In linear perturbation steps in Abaqus/Standard the current material tangent stiffness is used to determine the response. Specifically, when a linear perturbation is carried out about a base state that is on the primary curve, the unloading tangent stiffness will be used. In Abaqus/Explicit the unloading tangent stiffness is always used to compute the stable time increment. As a result, the inclusion of Mullins effect leads to more increments in the analysis, even when no unloading actually takes place. The Mullins effect material model can also be used in a steady-state transport analysis in Abaqus/Standard to obtain steady-state rolling solutions. Issues related to the use of the Mullins effect in a steady-state transport analysis can be found in “Steady-state transport analysis,” Section 6.4.1, and “Analysis of a solid disc with Mullins effect and permanent set,” Section 3.1.7 of the Abaqus Example Problems Manual. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for the Mullins effect material model: DMENER ELDMD ALLDMD Energy dissipated per unit volume by damage. Total energy dissipated in element by damage. Energy dissipated in whole (or partial) model by damage. The contribution from ALLDMD is included in the total strain energy ALLIE. EDMDDEN Energy dissipated per unit volume in the element by damage. SENER ELSE ALLSE The recoverable part of the energy per unit volume. The recoverable part of the energy in the element. The recoverable part of the energy in the whole (partial) model. ESEDEN The recoverable part of the energy per unit volume in the element. The damage energy dissipation, represented by the shaded area in Figure 22.6.1–1 for deformation , is computed as follows. When the damaged material is in a fully unloaded state, the augmented until energy function has the residual value . The residual value of the energy function upon complete unloading represents the energy dissipated due to damage in the material. The recoverable part of the energy is obtained by subtracting the dissipated energy from the augmented energy as . The damage energy accumulates with progressive deformation along the primary curve and remains constant during unloading. During unloading, the recoverable part of the strain energy is released. The latter becomes zero when the material point is completely unloaded. Upon further reloading from a completely unloaded state, the recoverable part of the strain energy increases from zero. When the maximum strain that was attained earlier is exceeded upon reloading, further accumulation of damage energy occurs. Additional reference • Ogden, R. W., and D. G. Roxburgh, “A Pseudo-Elastic Model for the Mullins Effect in Filled Rubber,” Proceedings of the Royal Society of London, Series A, vol. 455, p. 2861–2877, 1999. 22.6.2 ENERGY DISSIPATION IN ELASTOMERIC FOAMS Products: Abaqus/Standard Abaqus/Explicit References • “Material library: overview,” Section 21.1.1 • “Combining material behaviors,” Section 21.1.3 • “Elastic behavior: overview,” Section 22.1.1 • “Hyperelastic behavior in elastomeric foams,” Section 22.5.2 • “Mullins effect,” Section 22.6.1 • *HYPERFOAM • *MULLINS EFFECT • *UNIAXIAL TEST DATA • *BIAXIAL TEST DATA • *PLANAR TEST DATA Overview Energy dissipation in elastomeric foams in Abaqus: • allows the modeling of permanent energy dissipation and stress softening effects in elastomeric foams; • uses an approach based on the Mullins effect for elastomeric rubbers (“Mullins effect,” Section 22.6.1); • provides an extension to the isotropic elastomeric foam model (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2); • is intended for modeling energy absorption in foam components subjected to dynamic loading under deformation rates that are high compared to the characteristic relaxation time of the foam; and • cannot be used with viscoelasticity. Energy dissipation in elastomeric foams Abaqus provides a mechanism to include permanent energy dissipation and stress softening effects in elastomeric foams. The approach is similar to that used to model the Mullins effect in elastomeric rubbers, described in “Mullins effect,” Section 22.6.1. The functionality is primarily intended for modeling energy absorption in foam components subjected to dynamic loading under deformation rates that are high compared to the characteristic relaxation time of the foam; in such cases it is acceptable to assume that the foam material is damaged permanently. The material response is depicted qualitatively in Figure 22.6.2–1. c' b' stretch Figure 22.6.2–1 Typical stress-stretch response of an elastomeric foam material with energy dissipation. . On unloading from , the path . If further loading is then applied, the path of a previously unstressed foam, with loading to an arbitrary is followed. When the material is loaded again, the Consider the primary loading path point softened path is retraced as (which is the path that would be followed if there is a continuation of the primary loading path were no unloading). If loading is now stopped at is followed on unloading and then retraced back to represents the subsequent material response, which is then elastic. For loading beyond , the primary path is again followed and the pattern described is repeated. The shaded area in Figure 22.6.2–1 represents the energy dissipated by damage in the material for deformation until , the path on reloading. If no further loading beyond is applied, the curve is followed, where . Modified strain energy density function Energy dissipation effects are accounted for by introducing an augmented strain energy density function of the form where is the strain energy potential for the primary foam behavior described in “Hyperelastic behavior in elastomeric foams,” Section 22.5.2, defined by the polynomial strain energy function represent the principal mechanical stretches and is a continuous function of the damage variable, The function , and is referred to as the “damage function.” The damage variable varies continuously during the course of the deformation and always satisfies satisfies the condition ; thus, when the deformation state of the material is on a point on the curve that and the augmented energy function reduces to represents the primary foam behavior, the strain energy potential for the primary foam behavior. on the points of the primary curve. The damage function , with The above expression of the augmented strain energy density function is similar to the form proposed by Ogden and Roxburgh to model the Mullins effect in filled rubber elastomers , with the difference that in the case of elastomeric foams an augmentation of the total strain energy (including the volumetric part) is considered. This modification is required for the model to predict energy absorption under pure hydrostatic loading of the foam. Stress computation With the above modification to the energy function, the stresses are given by is the stress corresponding to the primary foam behavior at the current deformation level where . Thus, the stress is obtained by simply scaling the stress of the primary foam behavior by the damage variable, . From any given strain level the model predicts unloading/reloading along a single curve (that is different, in general, from the primary foam behavior) that passes through the origin of the stress-strain plot. The model also predicts energy dissipation under purely volumetric deformation. Damage variable The damage variable, , varies with the deformation according to where are material parameters; and the primary curve, variable, is the maximum value of at a material point during its deformation history; r, is the error function. When . On the other hand, upon removal of deformation, when , and m , corresponding to a point on , the damage , attains its minimum value, , given by For all intermediate values of and . While the parameters r are dimensionless, the parameter m has the dimensions of energy. The material parameters can varies monotonically between and , be specified directly or can be computed by Abaqus based on curve fitting of unloading-reloading test data. These parameters are subject to the restrictions and , m cannot both be zero). Alternatively, the damage variable can be defined through user subroutine UMULLINS in Abaqus/Standard and VUMULLINS in Abaqus/Explicit. (the parameters , and If the parameter and the parameter m has a value that is small compared to , the slope of the stress-strain curve at the initiation of unloading from relatively large strain levels may become very high. As a result, the response may become discontinuous. This kind of behavior may lead to convergence problems in Abaqus/Standard. In Abaqus/Explicit the high stiffness will lead to very small stable time increments, thereby leading to a degradation in performance. This problem can be avoided by choosing a small value for is 0. In Abaqus/Explicit, however, the default value of , it is assumed to be 0 in Abaqus/Standard and 0.1 in Abaqus/Explicit. . In Abaqus/Standard the default value of is 0.1. Thus, if you do not specify a value for The parameters r, , and m do not have direct physical interpretations in general. The parameter m controls whether damage occurs at low strain levels. If , there is a significant amount of damage at low strain levels. On the other hand, a nonzero m leads to little or no damage at low strain levels. For further discussion regarding the implications of this model on the energy dissipation, see “Mullins effect,” Section 4.7.1 of the Abaqus Theory Manual. Specifying properties for energy dissipation in elastomeric foams The primary elastomeric foam behavior is defined by using the hyperfoam material model. Energy dissipation can be defined by specifying the parameters in the expression of the damage variable directly or by using test data to calibrate the parameters. Alternatively, you can define the Mullins effect model with user subroutine UMULLINS in Abaqus/Standard and VUMULLINS in Abaqus/Explicit. Specifying the parameters directly The parameters r, m, and of temperature and/or field variables. in the expression of the damage variable can be given directly as functions Input File Usage: Abaqus/CAE Usage: *MULLINS EFFECT Property module: material editor: Mechanical→Damage for Elastomers→Mullins Effect: Definition: Constants Using test data to calibrate the parameters Experimental unloading-reloading data from different strain levels can be specified for up to three simple tests: uniaxial, biaxial, and planar. Abaqus will then compute the material parameters using a nonlinear least-squares curve fitting algorithm. See “Mullins effect,” Section 22.6.1, for a detailed discussion of this approach. Input File Usage: *MULLINS EFFECT, TEST DATA INPUT, BETA and/or M and/or R In addition, use at least one and up to three of the following options to give the unloading-reloading test data: *UNIAXIAL TEST DATA *BIAXIAL TEST DATA *PLANAR TEST DATA Multiple unloading-reloading curves from different strain levels for any given test type can be entered by repeated specification of the appropriate test data option. Property module: material editor: Mechanical→Damage for Elastomers→Mullins Effect: Definition: Test Data Input: enter the values for up to two of the values r, m, and beta. In addition, enter data for at least one of the following Suboptions→Biaxial Test, Planar Test, or Uniaxial Test Abaqus/CAE Usage: User subroutine specification An alternative method for specifying energy dissipation involves defining the damage variable in user subroutine UMULLINS in Abaqus/Standard and VUMULLINS in Abaqus/Explicit. Optionally, you can specify the number of property values needed as data in the user subroutine. You must provide the damage variable, . The latter contributes to the Jacobian of the overall system of equations and is necessary to ensure good convergence characteristics in Abaqus/Standard. If needed, you can specify the number of solution-dependent variables (“User subroutines: overview,” Section 18.1.1). These solution-dependent variables can be updated in the user subroutine. The damage dissipation energy and the recoverable part of the energy can also be defined for output purposes. , and its derivative, Input File Usage: Abaqus/CAE Usage: *MULLINS EFFECT, USER, PROPERTIES=constants Property module: material editor: Mechanical→Damage for Elastomers→Mullins Effect: Definition: User Defined Elements The model can be used with all element types that support the use of the elastomeric foam material model. Procedures The model can be used in all procedure types that support the use of the elastomeric foam material model. In linear perturbation steps in Abaqus/Standard the current material tangent stiffness is used to determine the response. Specifically, when a linear perturbation is carried out about a base state that is on the primary curve, the unloading tangent stiffness will be used. In Abaqus/Explicit the unloading tangent stiffness is always used to compute the stable time increment. As a result, the inclusion of stress-softening effects may lead to more increments in the analysis, even when no unloading actually takes place. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning when energy dissipation is present in the model: DMENER ELDMD ALLDMD Energy dissipated per unit volume by damage. Total energy dissipated in element by damage. Energy dissipated in whole (or partial) model by damage. The contribution from ALLDMD is included in the total strain energy ALLIE. EDMDDEN Energy dissipated per unit volume in the element by damage. SENER ELSE ALLSE The recoverable part of the energy per unit volume. The recoverable part of the energy in the element. The recoverable part of the energy in the whole (partial) model. ESEDEN The recoverable part of the energy per unit volume in the element. The damage energy dissipation, represented by the shaded area in Figure 22.6.2–1 for deformation until , is computed as follows. When the damaged material is in a fully unloaded state, the augmented energy function has the residual value . The residual value of the energy function upon complete unloading represents the energy dissipated due to damage in the material. The recoverable part of the energy is obtained by subtracting the dissipated energy from the augmented energy as . The damage energy accumulates with progressive deformation along the primary curve and remains constant during unloading. During unloading, the recoverable part of the strain energy is released. The latter becomes zero when the material point is unloaded completely. Upon further reloading from a completely unloaded state, the recoverable part of the strain energy increases from zero. When the maximum strain that was attained earlier is exceeded upon reloading, further accumulation of damage energy occurs. 22.7 Viscoelasticity • “Time domain viscoelasticity,” Section 22.7.1 • “Frequency domain viscoelasticity,” Section 22.7.2 22.7.1 TIME DOMAIN VISCOELASTICITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • “Frequency domain viscoelasticity,” Section 22.7.2 • *VISCOELASTIC • *SHEAR TEST DATA • *VOLUMETRIC TEST DATA • *COMBINED TEST DATA • *TRS • “Defining time domain viscoelasticity” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The time domain viscoelastic material model: • describes isotropic rate-dependent material behavior for materials in which dissipative losses primarily caused by “viscous” (internal damping) effects must be modeled in the time domain; • assumes that the shear (deviatoric) and volumetric behaviors are independent in multiaxial stress states (except when used for an elastomeric foam); • can be used only in conjunction with “Linear elastic behavior,” Section 22.2.1; “Hyperelastic behavior of rubberlike materials,” Section 22.5.1; or “Hyperelastic behavior in elastomeric foams,” Section 22.5.2, to define the continuum elastic material properties; • can be used in Abaqus/Explicit with “Linear elastic traction-separation behavior” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6; • is active only during a transient static analysis (“Quasi-static analysis,” Section 6.2.5), a integration,” transient implicit dynamic analysis (“Implicit dynamic analysis using direct Section 6.3.2), an explicit dynamic analysis (“Explicit dynamic analysis,” Section 6.3.3), a steady-state transport analysis (“Steady-state transport analysis,” Section 6.4.1), a fully coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.3), a fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4), or a transient (consolidation) coupled pore fluid diffusion and stress analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1); • can be used in large-strain problems; • can be calibrated using time-dependent creep test data, time-dependent relaxation test data, or frequency-dependent cyclic test data; and • can be used to couple viscous dissipation with the temperature field in a fully coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.3) or a fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4). Defining the shear behavior Time domain viscoelasticity is available in Abaqus for small-strain applications where the rate-independent elastic response can be defined with a linear elastic material model and for large-strain applications where the rate-independent elastic response must be defined with a hyperelastic or hyperfoam material model. Small strain Consider a shear test at small strain in which a time varying shear strain, The response is the shear stress . The viscoelastic material model defines as , is applied to the material. where is the time-dependent “shear relaxation modulus” that characterizes the material’s response. This constitutive behavior can be illustrated by considering a relaxation test in which a strain is suddenly applied to a specimen and then held constant for a long time. The beginning of the experiment, when the strain is suddenly applied, is taken as zero time, so that (since for ), where is the fixed strain. The viscoelastic material model is “long-term elastic” in the sense that, after having been subjected to a constant strain for a very long time, the response settles down to a constant stress; i.e., as . The shear relaxation modulus can be written in dimensionless form: where form is the instantaneous shear modulus, so that the expression for the stress takes the The dimensionless relaxation function has the limiting values and . Anisotropic elasticity in Abaqus/Explicit The equation for the shear stress can be transformed by using integration by parts: It is convenient to write this equation in the form where is the instantaneous shear stress at time t. This can be generalized to multi-dimensions as is the deviatoric part of the stress tensor and where stress tensor. Here the viscoelasticity is assumed to be isotropic; independent of the loading direction. is the deviatoric part of the instantaneous i.e., the relaxation function is This form allows a straightforward generalization to anisotropic elastic deformations, where is the the deviatoric part of instantaneous stress tensor is computed as instantaneous deviatoric elasticity tensor, and is the deviatoric part of the strain tensor. . Here Large strain The above form also allows a straightforward generalization to nonlinear elastic deformations, where the deviatoric part of the instantaneous stress is computed using a hyperelastic strain enery potential. This generalization yields a linear viscoelasticity model, in the sense that the dimensionless stress relaxation function is independent of the magnitude of the deformation. In the above equation the instantaneous stress, , at time t. Therefore, to create a proper finite-strain formulation, it is necessary to map the stress that existed in the configuration at time into the configuration at time t. In Abaqus this is done by means of the “standard-push-forward” transformation with the relative deformation gradient influences the stress, , applied at time : which results in the following hereditary integral: where is the deviatoric part of the Kirchhoff stress. The finite-strain theory is described in more detail in “Finite-strain viscoelasticity,” Section 4.8.2 of the Abaqus Theory Manual. Defining the volumetric behavior The volumetric behavior can be written in a form that is similar to the shear behavior: where p is the hydrostatic pressure, dimensionless bulk relaxation modulus, and is the instantaneous elastic bulk modulus, is the is the volume strain. The above expansion applies to small as well as finite strain since the volume strains are generally small and there is no need to map the pressure from time to time t. Defining viscoelastic behavior for traction-separation elasticity in Abaqus/Explicit Time domain viscoelasticity can be used in Abaqus/Explicit to model rate-dependent behavior of cohesive elements with traction-separation elasticity (“Defining elasticity in terms of tractions and separations for cohesive elements” in “Linear elastic behavior,” Section 22.2.1). In this case the evolution equation for the normal and two shear nominal tractions take the form: , , and are the instantaneous nominal tractions at time t in the normal and the two where local shear directions, respectively. The functions now represent the dimensionless shear and normal relaxation moduli, respectively. Note the close similarity between the viscoelastic formulation for the continuum elastic response discussed in the previous sections and the formulation for cohesive behavior with traction-separation elasticity after reinterpreting shear and bulk relaxation as shear and normal relaxation. and For the case of uncoupled traction elasticity, the viscoelastic normal and shear behaviors are assumed to be independent. The normal relaxation modulus is defined as where and, therefore, independent of the local shear directions: is the instantaneous normal moduli. The shear relaxation modulus is assumed to be isotropic where and are the instantaneous shear moduli. For the case of coupled traction-separation elasticity the normal and shear relaxation moduli must be the same, , and you must use the same relaxation data for both behaviors. Temperature effects The effect of temperature, instantaneous stress, linear-elastic shear stress is rewritten as , on the material behavior is introduced through the dependence of the , on temperature and through a reduced time concept. The expression for the where the instantaneous shear modulus by is temperature dependent and is the reduced time, defined where is a shift function at time t. This reduced time concept for temperature dependence is usually referred to as thermo-rheologically simple (TRS) temperature dependence. Often the shift function is approximated by the Williams-Landel-Ferry (WLF) form. See “Thermo-rheologically simple temperature effects” below, for a description of the WLF and other forms of the shift function available in Abaqus. The reduced time concept is also used for the volumetric behavior, the large-strain formulation, and the traction-separation formulation. Numerical implementation Abaqus assumes that the viscoelastic material is defined by a Prony series expansion of the dimensionless relaxation modulus: where N, in the small-strain expression for the shear stress yields , and , , are material constants. For linear isotropic elasticity, substitution where The are interpreted as state variables that control the stress relaxation, and is the “creep” strain: the difference between the total mechanical strain and the instantaneous elastic strain (the stress divided by the instantaneous elastic modulus). In Abaqus/Standard is available as the creep strain output variable CE (“Abaqus/Standard output variable identifiers,” Section 4.2.1). A similar Prony series expansion is used for the volumetric response, which is valid for both small- and finite-strain applications: where Abaqus assumes that . For linear anisotropic elasticity, the Prony series expansion, in combination with the generalized small-strain expression for the deviatoric stress, yields where The are interpreted as state variables that control the stress relaxation. For finite strains, the Prony series expansion, in combination with the finite-strain expression for the shear stress, produces the following expression for the deviatoric stress: where The are interpreted as state variables that control the stress relaxation. For traction-separation elasticity, the Prony series expansion yields where The are interpreted as state variables that control the relaxation of the traction stresses. If the instantaneous material behavior is defined by linear elasticity or hyperelasticity, the bulk and shear behavior can be defined independently. However, if the instantaneous behavior is defined by the hyperfoam model, the deviatoric and volumetric constitutive behavior are coupled and it is mandatory to use the same relaxation data for both behaviors. For linear anisotropic elasticity, the same relaxation data should be used for both behaviors when the elasticity definition is such that the deviatoric and volumetric response is coupled. Similarly, for coupled traction-separation elasticity you must use the same relaxation data for the normal and shear behaviors. In all of the above expressions temperature dependence is readily introduced by replacing by and by . Determination of viscoelastic material parameters The above equations are used to model the time-dependent shear and volumetric behavior of a viscoelastic material. The relaxation parameters can be defined in one of four ways: direct specification of the Prony series parameters, inclusion of creep test data, inclusion of relaxation test data, or inclusion of frequency-dependent data obtained from sinusoidal oscillation experiments. Temperature effects are included in the same manner regardless of the method used to define the viscoelastic material. Abaqus/CAE allows you to evaluate the behavior of viscoelastic materials by automatically creating response curves based on experimental test data or coefficients. A viscoelastic material can be evaluated only if it is defined in the time domain and includes hyperelastic and/or elastic material data. See “Evaluating hyperelastic and viscoelastic material behavior,” Section 12.4.7 of the Abaqus/CAE User’s Manual. Direct specification , , and The Prony series parameters can be defined directly for each term in the Prony series. There is no restriction on the number of terms that can be used. If a relaxation time is associated with only one of the two moduli, leave the other one blank or enter a zero. The data should be given in ascending order of the relaxation time. The number of lines of data given defines the number of terms in the Prony series, N. If this model is used in conjunction with the hyperfoam material model, the two modulus ratios have to be the same ( ). Input File Usage: *VISCOELASTIC, TIME=PRONY The data line is repeated as often as needed to define the first, second, third, etc. terms in the Prony series. Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Time and Time: Prony Enter as many rows of data in the table as needed to define the first, second, third, etc. terms in the Prony series. Creep test data If creep test data are specified, Abaqus will calculate the terms in the Prony series automatically. The normalized shear and bulk compliances are defined as where shear stress in a shear creep test; volumetric strain, and . is the shear compliance, is the total shear strain, and is the volumetric compliance, is the constant pressure in a volumetric creep test. At time is the constant is the total , The creep data are converted to relaxation data through the convolution integrals Abaqus then uses the normalized shear modulus least-squares fit to determine the Prony series parameters. and normalized bulk modulus in a nonlinear Using the shear and volumetric test data consecutively The shear test data and volumetric test data can be used consecutively to define the normalized shear and bulk compliances as functions of time. A separate least-squares fit is performed on each data set; and the two derived sets of Prony series parameters, , are merged into one set of parameters, and . Input File Usage: Use the following three options. The first option is required. Only one of the second and third options is required. Abaqus/CAE Usage: *VISCOELASTIC, TIME=CREEP TEST DATA *SHEAR TEST DATA *VOLUMETRIC TEST DATA Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Time and Time: Creep test data In addition, select one or both of the following: Test Data→Shear Test Data Test Data→Volumetric Test Data Using the combined test data Alternatively, the combined test data can be used to specify the normalized shear and bulk compliances simultaneously as functions of time. A single least-squares fit is performed on the combined set of test data to determine one set of Prony series parameters, . Input File Usage: Use both of the following options: *VISCOELASTIC, TIME=CREEP TEST DATA *COMBINED TEST DATA Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Time, Time: Creep test data, and Test Data→Combined Test Data Abaqus/CAE Usage: Relaxation test data As with creep test data, Abaqus will calculate the Prony series parameters automatically from relaxation test data. Using the shear and volumetric test data consecutively Again, the shear test data and volumetric test data can be used consecutively to define the relaxation moduli as functions of time. A separate nonlinear least-squares fit is performed on each data set; and the two derived sets of Prony series parameters, , are merged into one set of parameters, . and Input File Usage: Use the following three options. The first option is required. Only one of the second and third options is required. Abaqus/CAE Usage: *VISCOELASTIC, TIME=RELAXATION TEST DATA *SHEAR TEST DATA *VOLUMETRIC TEST DATA Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Time and Time: Relaxation test data In addition, select one or both of the following: Test Data→Shear Test Data Test Data→Volumetric Test Data Using the combined test data Alternatively, the combined test data can be used to specify the relaxation moduli simultaneously as functions of time. A single least-squares fit is performed on the combined set of test data to determine one set of Prony series parameters, . Input File Usage: Abaqus/CAE Usage: Use both of the following options: *VISCOELASTIC, TIME=RELAXATION TEST DATA *COMBINED TEST DATA Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Time, Time: Relaxation test data, and Test Data→Combined Test Data Frequency-dependent test data The Prony series terms can also be calibrated using frequency-dependent test data. In this case Abaqus uses analytical expressions that relate the Prony series relaxation functions to the storage and loss moduli. The expressions for the shear moduli, obtained by converting the Prony series terms from the time domain to the frequency domain by making use of Fourier transforms, can be written as follows: is the storage modulus, where is the angular frequency, and N is the number of terms in the Prony series. These expressions are used in a nonlinear least-squares fit to determine the Prony series parameters from the storage and loss moduli cyclic test data obtained at M frequencies by minimizing the error function is the loss modulus, : where shear moduli. The expressions for the bulk moduli, are the test data and and and , respectively, are the instantaneous and long-term and , are written analogously. The frequency domain data are defined in tabular form by giving the real and imaginary parts of and —where is the circular frequency—as functions of frequency in cycles per time. is the Fourier transform of the nondimensional shear relaxation function frequency-dependent storage and loss moduli , and parts of are then given as and , , . Given the , the real and imaginary where properties. and are the long-term shear and bulk moduli determined from the elastic or hyperelastic Input File Usage: Abaqus/CAE Usage: *VISCOELASTIC, TIME=FREQUENCY DATA Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Time and Time: Frequency data Calibrating the Prony series parameters the error tolerance and You can specify two optional parameters related to the calibration of Prony series parameters for viscoelastic materials: . The error tolerance is the allowable average root-mean-square error of data points in the least-squares fit, and its default value is 0.01. is the maximum number of terms N in the Prony series, and its default (and maximum) value is 13. Abaqus will perform the least-squares fit from until convergence is achieved for the lowest N with respect to the error tolerance. to The following are some guidelines for determining the number of terms in the Prony series from test data. Based on these guidelines, you can choose . • There should be enough data pairs for determining all the parameters in the Prony series terms. Thus, assuming that N is the number of Prony series terms, there should be a total of at least data points in shear test data, test data, and data points in the frequency domain. data points in volumetric test data, data points in combined • The number of terms in the Prony series should be typically not more than the number of logarithmic “decades” spanned by the test data. The number of logarithmic “decades” is defined as are the maximum and minimum time in the test data, respectively. , where and Input File Usage: Abaqus/CAE Usage: *VISCOELASTIC, ERRTOL=error_tolerance, NMAX= Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Time; Time: Creep test data, Relaxation test data, or Frequency data; Maximum number of terms in the Prony series: ; and Allowable average root-mean-square error: error_tolerance Thermo-rheologically simple temperature effects Regardless of the method used to define the viscoelastic behavior, thermo-rheologically simple temperature effects can be included by specifying the method used to define the shift function. Abaqus supports the following forms of the shift function: the Arrhenius form, and user-defined forms. the Williams-Landel-Ferry (WLF) form, Thermo-rheologically simple temperature effects can also be included in the definition of equation of state models with viscous shear behavior . Williams-Landel-Ferry (WLF) form The shift function can be defined by the Williams-Landel-Ferry (WLF) approximation, which takes the form: is the reference temperature at which the relaxation data are given; where interest; and changes will be elastic, based on the instantaneous moduli. are calibration constants obtained at this temperature. If , is the temperature of , deformation For additional information on the WLF equation, see “Viscoelasticity,” Section 4.8.1 of the Abaqus Theory Manual. Input File Usage: Abaqus/CAE Usage: Arrhenius form *TRS, DEFINITION=WLF Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Time, Time: any method, and Suboptions→Trs: Shift function: WLF The Arrhenius shift function is commonly used for semi-crystalline polymers. It takes the form is the activation energy, where temperature scale being used, and is the temperature of interest. is the universal gas constant, is the absolute zero in the is the reference temperature at which the relaxation data are given, Input File Usage: Use the following option to define the Arrhenius shift function: *TRS, DEFINITION=ARRHENIUS In addition, use the *PHYSICAL CONSTANTS option to specify the universal gas constant and absolute zero. Abaqus/CAE Usage: The Arrhenius shift function is not supported in Abaqus/CAE. User-defined form The shift function can be specified alternatively in user subroutines UTRS in Abaqus/Standard and VUTRS in Abaqus/Explicit. Input File Usage: Abaqus/CAE Usage: *TRS, DEFINITION=USER Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Time, Time: any method, and Suboptions→Trs: Shift function: User subroutine UTRS Defining the rate-independent part of the material response In all cases elastic moduli must be specified to define the rate-independent part of the material behavior. Small-strain linear elastic behavior is defined by an elastic material model (“Linear elastic behavior,” Section 22.2.1), and large-deformation behavior is defined by a hyperelastic (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1) or hyperfoam (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2) material model. The rate-independent elasticity for any of these models can be defined in terms of either instantaneous elastic moduli or long-term elastic moduli. The choice of defining the elasticity in terms of instantaneous or long-term moduli is a matter of convenience only; it does not have an effect on the solution. The effective relaxation moduli are obtained by multiplying the instantaneous elastic moduli with the dimensionless relaxation functions as described below. Linear elastic isotropic materials For linear elastic isotropic material behavior and where defined instantaneous elastic moduli and : If long-term elastic moduli are defined, the instantaneous moduli are determined from and and . are the instantaneous shear and bulk moduli determined from the values of the user- Linear elastic anisotropic materials For linear elastic anisotropic material behavior the relaxation coefficients are applied to the elastic moduli as and and where values of the user-defined instantaneous elastic moduli are specified and they are unequal, Abaqus issues an error message if the elastic moduli the deviatoric and volumetric response is coupled. are the instantaneous deviatoric elasticity tensor and bulk moduli determined from the . If both shear and bulk relaxation coefficients is such that If long-term elastic moduli are defined, the instantaneous moduli are determined from Hyperelastic materials For hyperelastic material behavior the relaxation coefficients are applied either to the constants that define the energy function or directly to the energy function. For the polynomial function and its particular cases (reduced polynomial, Mooney-Rivlin, neo-Hookean, and Yeoh) for the Ogden function for the Arruda-Boyce and Van der Waals functions and for the Marlow function For the coefficients governing the compressible behavior of the polynomial models and the Ogden model for the Arruda-Boyce and Van der Waals functions and for the Marlow function If long-term elastic moduli are defined, the instantaneous moduli are determined from while the instantaneous bulk compliance moduli are obtained from for the Marlow functions we have Mullins effect If long-term moduli are defined for the underlying hyperelastic behavior, the instantaneous value of the parameter in Mullins effect is determined from Elastomeric foams For elastomeric foam material behavior the instantaneous shear and bulk relaxation coefficients are assumed to be equal and are applied to the material constants in the energy function: If only the shear relaxation coefficients are specified, the bulk relaxation coefficients are set equal to the shear relaxation coefficients and vice versa. If both shear and bulk relaxation coefficients are specified and they are unequal, Abaqus issues an error message. If long-term elastic moduli are defined, the instantaneous moduli are determined from Traction-separation elasticity For cohesive elements with uncoupled traction-separation elastic behavior: and where If long-term elastic moduli are defined, the instantaneous moduli are determined from is the instantaneous normal modulus and and are the instantaneous shear moduli. For cohesive elements with coupled traction-separation elastic behavior the shear and bulk relaxation coefficients must be equal: where instantaneous moduli are determined from is the user-defined instantaneous elasticity matrix. If long-term elastic moduli are defined, the Material response in different analysis procedures The time-domain viscoelastic material model is active during the following procedures: • transient static analysis (“Quasi-static analysis,” Section 6.2.5), • transient implicit dynamic analysis (“Implicit dynamic analysis using direct Section 6.3.2), integration,” • explicit dynamic analysis (“Explicit dynamic analysis,” Section 6.3.3), • steady-state transport analysis (“Steady-state transport analysis,” Section 6.4.1), • fully coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.3), • fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4), and • transient (consolidation) coupled pore fluid diffusion and stress analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). Viscoelastic material response is always ignored in a static analysis. It can also be ignored in a coupled temperature-displacement analysis, a coupled thermal-electrical-structural analysis, or a soils consolidation analysis by specifying that no creep or viscoelastic response is occurring during the step even if creep or viscoelastic material properties are defined . In these cases it is assumed that the loading is applied instantaneously, so that the resulting response corresponds to an elastic solution based on instantaneous elastic moduli. Abaqus/Standard also provides the option to obtain the fully relaxed long-term elastic solution directly in a static or steady-state transport analysis without having to perform a transient analysis. The long-term value is used for this purpose. The viscous damping stresses (the internal stresses associated with each of the Prony-series terms) are increased gradually from their values at the beginning of the step to their long-term values at the end of the step if the long-term value is specified. Use with other material models The viscoelastic material model must be combined with an elastic material model. It is used with the isotropic linear elasticity model (“Linear elastic behavior,” Section 22.2.1) to define classical, linear, small-strain, viscoelastic behavior or with the hyperelastic (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1) or hyperfoam (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2) models to define large-deformation, nonlinear, viscoelastic behavior. It can also be used with anisotropic linear elasticity and with traction-separation elastic behavior in Abaqus/Explicit. The elastic properties defined for these models can be temperature dependent. Viscoelasticity cannot be combined with any of the plasticity models. See “Combining material behaviors,” Section 21.1.3, for more details. Elements The time domain viscoelastic material model can be used with any stress/displacement, coupled temperature-displacement, or thermal-electrical-structural element in Abaqus. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning in Abaqus/Standard if viscoelasticity is defined: EE CE Elastic strain corresponding to the stress state at time t and the instantaneous elastic material properties. Equivalent creep strain defined as the difference between the total strain and the elastic strain. Considerations for steady-state transport analysis When a steady-state transport analysis (“Steady-state transport analysis,” Section 6.4.1) is combined with large-strain viscoelasticity, the viscous dissipation, CENER, is computed as the energy dissipated per revolution as a material point is transported around its streamline; that is, Consequently, all the material points in a given streamline report the same value for CENER, and other derived quantities such as ELCD and ALLCD also have the meaning of dissipation per revolution. The recoverable elastic strain energy density, SENER, is approximated as is the incremental energy input and is the time at the beginning of the current increment. where Since two different units are used in the quantities appearing in the above equation, a proper meaning cannot be assigned to quantities such as SENER, ELSE, ALLSE, and ALLIE. Considerations for large-strain viscoelasticity in Abaqus/Explicit For the case of large-strain viscoelasticity, Abaqus/Explicit does not compute the viscous dissipation for performance reasons. Instead, the contribution of viscous dissipation is included in the strain energy output, SENER; and CENER is output as zero. Consequently, special care must be exercised when interpreting strain energy results of large-strain viscoelastic materials in Abaqus/Explicit since they include viscous dissipation effects. 22.7.2 FREQUENCY DOMAIN VISCOELASTICITY Products: Abaqus/Standard Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • “Time domain viscoelasticity,” Section 22.7.1 • *VISCOELASTIC • “Defining frequency domain viscoelasticity” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The frequency domain viscoelastic material model: • describes frequency-dependent material behavior in small steady-state harmonic oscillations for those materials in which dissipative losses caused by “viscous” (internal damping) effects must be modeled in the frequency domain; • assumes that the shear (deviatoric) and volumetric behaviors are independent in multiaxial stress states; • can be used in large-strain problems; • can be used only in conjunction with “Linear elastic behavior,” Section 22.2.1; “Hyperelastic behavior of rubberlike materials,” Section 22.5.1; and “Hyperelastic behavior in elastomeric foams,” Section 22.5.2, to define the long-term elastic material properties; • can be used in conjunction with the elastic-damage gasket behavior (“Defining a nonlinear elastic model with damage” in “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6 ) to define the effective thickness-direction storage and loss moduli for gasket elements; and • is active only during the direct-solution steady-state dynamic (“Direct-solution steady-state dynamic analysis,” Section 6.3.4), the subspace-based steady-state dynamic (“Subspace-based the natural frequency extraction (“Natural steady-state dynamic analysis,” Section 6.3.9), frequency extraction,” Section 6.3.5), and the complex eigenvalue extraction (“Complex eigenvalue extraction,” Section 6.3.6) procedures. Defining the shear behavior Consider a shear test at small strain, in which a harmonically varying shear strain is applied: is the amplitude, where is the circular frequency, and t is time. We assume that the specimen has been oscillating for a very long time so that a steady-state solution is obtained. The solution for the shear stress then has the form , where (complex) Fourier transform are the shear storage and loss moduli. These moduli can be expressed in terms of the : of the nondimensional shear relaxation function and is the time-dependent shear relaxation modulus, where imaginary parts of viscoelasticity,” Section 4.8.3 of the Abaqus Theory Manual, for details. is the long-term shear modulus. , and and are the real and See “Frequency domain The above equation states that the material responds to steady-state harmonic strain with a stress of that lags the excitation that is in phase with the strain and a stress of magnitude magnitude by . Hence, we can regard the factor as the complex, frequency-dependent shear modulus of the steadily vibrating material. The absolute magnitude of the stress response is and the phase lag of the stress response is Measurements of and, thus, and as functions of frequency in an experiment can, thus, be used to define and as functions of frequency. Unless stated otherwise explicitly, all modulus measurements are assumed to be “true” quantities. and Defining the volumetric behavior In multiaxial stress states Abaqus/Standard assumes that the frequency dependence of the shear (deviatoric) and volumetric behaviors are independent. The volumetric behavior is defined by the bulk storage and loss moduli . Similar to the shear moduli, these moduli can also be expressed in terms of the (complex) Fourier transform of the nondimensional bulk relaxation function and : where is the long-term elastic bulk modulus. Large-strain viscoelasticity The linearized vibrations can also be associated with an elastomeric material whose long-term (elastic) response is nonlinear and involves finite strains (a hyperelastic material). We can retain the simplicity of the steady-state small-amplitude vibration response analysis in this case by assuming that the linear expression for the shear stress still governs the system, except that now the long-term shear modulus can vary with the amount of static prestrain : The essential simplification implied by this assumption is that the frequency-dependent part of the material’s response, defined by the Fourier transform of the relaxation function, is not affected by the magnitude of the prestrain. Thus, strain and frequency effects are separated, which is a reasonable approximation for many materials. Another implication of the above assumption is that the anisotropy of the viscoelastic moduli has the same strain dependence as the anisotropy of the long-term elastic moduli. Hence, the viscoelastic behavior in all deformed states can be characterized by measuring the (isotropic) viscoelastic moduli in the undeformed state. In situations where the above assumptions are not reasonable, the data can be specified based on measurements at the prestrain level about which the steady-state dynamic response is desired. In this case you must measure ) at the prestrain level of interest. Alternatively, the viscoelastic data can be given directly in terms of uniaxial and volumetric storage and loss moduli that may be specified as functions of frequency and prestrain (likewise , and , and , , The generalization of these concepts to arbitrary three-dimensional deformations is provided in Abaqus/Standard by assuming that the frequency-dependent material behavior has two independent components: one associated with shear (deviatoric) straining and the other associated with volumetric straining. therefore, defined for In the general case of a compressible material, kinematically small perturbations about a predeformed state as the model is, ; is the deviatoric stress, is the equivalent pressure stress, is the part of the stress increment caused by incremental straining (as distinct from the part of the stress increment caused by incremental rotation of the preexisting stress with respect to the coordinate system); ; 22.7.2–3 and where ; ; is the ratio of current to original volume; is the (small) incremental deviatoric strain, is the deviatoric strain rate, is the (small) incremental volumetric strain, is the rate of volumetric strain, is the deviatoric tangent elasticity matrix of the material in its predeformed state (for example, is the volumetric strain-rate/deviatoric stress-rate tangent elasticity matrix of the material in its predeformed state; and is the tangent bulk modulus of the predeformed material. is the tangent shear modulus of the prestrained material); ; ; For a fully incompressible material only the deviatoric terms in the first constitutive equation above remain and the viscoelastic behavior is completely defined by . Determination of viscoelastic material parameters The dissipative part of the material behavior is defined by giving the real and imaginary parts of and (for compressible materials) as functions of frequency. The moduli can be defined as functions of the frequency in one of three ways: by a power law, by tabular input, or by a Prony series expression for the shear and bulk relaxation moduli. Power law frequency dependence The frequency dependence can be defined by the power law formulæ and where a and b are real constants, cycles per time. and are complex constants, and is the frequency in Input File Usage: Abaqus/CAE Usage: *VISCOELASTIC, FREQUENCY=FORMULA Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Frequency and Frequency: Formula Tabular frequency dependence The frequency domain response can alternatively be defined in tabular form by giving the real and imaginary parts of is the circular frequency—as functions of frequency in cycles per time. Given the frequency-dependent storage and loss moduli , the real and imaginary parts of are then given as and —where , and and , , where properties. and are the long-term shear and bulk moduli determined from the elastic or hyperelastic Input File Usage: Abaqus/CAE Usage: *VISCOELASTIC, FREQUENCY=TABULAR Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Frequency and Frequency: Tabular Abaqus provides an alternative approach for specifying the viscoelastic properties of hyperelastic and hyperfoam materials. This approach involves the direct (tabular) specification of storage and loss moduli from uniaxial and volumetric tests, as functions of excitation frequency and a measure of the level of pre-strain. The level of pre-strain refers to the level of elastic deformation at the base state about which the steady-state harmonic response is desired. This approach is discussed in “Direct specification of storage and loss moduli for large-strain viscoelasticity” below. Prony series parameters The frequency dependence can also be obtained from a time domain Prony series description of the dimensionless shear and bulk relaxation moduli: where N, expression for the time-dependent shear modulus can be written in the frequency domain as follows: , are material constants. Using Fourier transforms, the , and , , is the loss modulus, is the storage modulus, is the angular frequency, and N is the where number of terms in the Prony series. The expressions for the bulk moduli, , are written analogously. Abaqus/Standard will automatically perform the conversion from the time domain to the frequency domain. The Prony series parameters can be defined in one of three ways: direct specification of the Prony series parameters, inclusion of creep test data, or inclusion of relaxation test data. If creep test data or relaxation test data are specified, Abaqus/Standard will determine the Prony series parameters in a nonlinear least-squares fit. A detailed description of the calibration of Prony series terms is provided in “Time domain viscoelasticity,” Section 22.7.1. and For the test data you can specify the normalized shear and bulk data separately as functions of time or specify the normalized shear and bulk data simultaneously. A nonlinear least-squares fit is performed to determine the Prony series parameters, . Input File Usage: Abaqus/CAE Usage: Use one of the following options to specify Prony data, creep test data, or relaxation test data: *VISCOELASTIC, FREQUENCY=PRONY *VISCOELASTIC, FREQUENCY=CREEP TEST DATA *VISCOELASTIC, FREQUENCY=RELAXATION TEST DATA Use one or both of the following options to specify the normalized shear and bulk data separately as functions of time: *SHEAR TEST DATA *VOLUMETRIC TEST DATA Use the following option to specify the normalized shear and bulk data simultaneously: *COMBINED TEST DATA Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Frequency and Frequency: Prony, Creep test data, or Relaxation test data Use one or both of the following options to specify the normalized shear and bulk data separately as functions of time: Test Data→Shear Test Data Test Data→Volumetric Test Data Use the following option to specify the normalized shear and bulk data simultaneously: Test Data→Combined Test Data Conversion of frequency-dependent elastic moduli For some cases of small straining of isotropic viscoelastic materials, the material data are provided as frequency-dependent uniaxial storage and loss moduli, and . In that case the data must be converted to obtain the frequency-dependent shear storage and loss , and bulk moduli, and moduli and . The complex shear modulus is obtained as a function of the complex uniaxial and bulk moduli with the expression Replacing the complex moduli by the appropriate storage and loss moduli, this expression transforms into After some algebra one obtains Shear strain only In many cases the viscous behavior is associated only with deviatoric straining, so that the bulk modulus is real and constant: . For this case the expressions for the shear moduli simplify to and Incompressible materials If the bulk modulus is very large compared to the shear modulus, the material can be considered to be incompressible and the expressions simplify further to Direct specification of storage and loss moduli for large-strain viscoelasticity For large-strain viscoelasticity Abaqus allows direct specification of storage and loss moduli from uniaxial and volumetric tests. This approach can be used when the assumption of the independence of viscoelastic properties on the pre-strain level is too restrictive. You specify the storage and loss moduli directly as tabular functions of frequency, and you specify the level of pre-strain at the base state about which the steady-state dynamic response is desired. For uniaxial test data the measure of pre-strain is the uniaxial nominal strain; for volumetric test data the measure of pre-strain is the volume ratio. Abaqus internally converts the data that you specify to ratios of shear/bulk storage and loss moduli to the corresponding long-term elastic moduli. Subsequently, the basic formulation described in “Large-strain viscoelasticity” above is used. For a general three-dimensional stress state it is assumed that the deviatoric part of the viscoelastic response depends on the level of pre-strain through the first invariant of the deviatoric left Cauchy-Green strain tensor , while the volumetric part depends on the pre-strain through the volume ratio. A consequence of these assumptions is that for the uniaxial case, data can be specified from a uniaxial-tension preload state or from a uniaxial-compression preload state but not both. The storage and loss moduli that you specify are assumed to be nominal quantities. Input File Usage: Use the following option to specify only the uniaxial storage and loss moduli: *VISCOELASTIC, PRELOAD=UNIAXIAL You can also use the following option to specify the volumetric (bulk) storage and loss moduli: *VISCOELASTIC, PRELOAD=VOLUMETRIC Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Frequency and Frequency: Tabular Use the following option to specify only the uniaxial storage and loss moduli: Type: Isotropic or Traction: Preload: Uniaxial Use the following option to specify only the volumetric storage and loss moduli: Type: Isotropic: Preload: Volumetric Use the following option to specify both uniaxial and volumetric moduli: Type: Isotropic: Preload: Uniaxial and Volumetric Defining the rate-independent part of the material behavior In all cases elastic moduli must be specified to define the rate-independent part of the material behavior. The elastic behavior is defined by an elastic, hyperelastic, or hyperfoam material model. Since the frequency domain viscoelastic material model is developed around the long-term elastic moduli, the rate-independent elasticity must be defined in terms of long-term elastic moduli. This implies that the response in any analysis procedure other than a direct-solution steady-state dynamic analysis (such as a static preloading analysis) corresponds to the fully relaxed long-term elastic solution. Use with other material models The viscoelastic material model must be combined with the isotropic linear elasticity model to define classical, linear, small-strain, viscoelastic behavior. It is combined with the hyperelastic or hyperfoam model to define large-deformation, nonlinear, viscoelastic behavior. The long-term elastic properties defined for these models can be temperature dependent. Viscoelasticity cannot be combined with any of the plasticity models. See “Combining material behaviors,” Section 21.1.3, for more details. Elements The frequency domain viscoelastic material model can be used with any stress/displacement element in Abaqus/Standard. 22.8 Nonlinear viscoelasticity • “Hysteresis in elastomers,” Section 22.8.1 • “Parallel network viscoelastic model,” Section 22.8.2 22.8.1 HYSTERESIS IN ELASTOMERS Products: Abaqus/Standard Abaqus/CAE References • “Elastic behavior: overview,” Section 22.1.1 • *HYSTERESIS • “Defining hysteretic behavior for an isotropic hyperelastic material model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The hysteresis material model: • defines strain-rate-dependent, hysteretic behavior of materials that undergo comparable elastic and inelastic strains; • provides inelastic response only for shear distortional behavior—the response to volumetric deformations is purely elastic; • can be used only in conjunction with “Hyperelastic behavior of rubberlike materials,” Section 22.5.1, to define the elastic response of the material—the elasticity can be defined either in terms of the instantaneous moduli or the long-term moduli; • is active during a static analysis (“Static stress analysis,” Section 6.2.2), a quasi-static analysis (“Quasi-static analysis,” Section 6.2.5), or a transient dynamic analysis using direct integration (“Implicit dynamic analysis using direct integration,” Section 6.3.2)—it cannot be used in fully coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.3), fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4), or steady-state transport analysis (“Steady-state transport analysis,” Section 6.4.1); • cannot be used to model temperature-dependent creep material properties—however, the elastic material properties can be temperature dependent; and • uses unsymmetric matrix storage and solution by default. Strain-rate-dependent material behavior for elastomers Nonlinear strain-rate dependence of elastomers is modeled by decomposing the mechanical response into that of an equilibrium network (A) corresponding to the state that is approached in long-time stress relaxation tests and that of a time-dependent network (B) that captures the nonlinear rate-dependent deviation from the equilibrium state. The total stress is assumed to be the sum of the stresses in the two networks. The deformation gradient, , is assumed to act on both networks and is decomposed into elastic and inelastic parts in network B according to the multiplicative decomposition The nonlinear rate-dependent material model is capable of reproducing the hysteretic behavior of elastomers subjected to repeated cyclic loading. It does not model “Mullins effect”—the initial softening of an elastomer when it is first subjected to a load. The material model is defined completely by: • a hyperelastic material model that characterizes the elastic response of the model; • a stress scaling factor, S, that defines the ratio of the stress carried by network B to the stress carried by network A under instantaneous loading; i.e., identical elastic stretching in both networks; • a positive exponent, m, generally greater than 1, characterizing the effective stress dependence of the effective creep strain rate in network B; • an exponent, C, restricted to lie in creep strain rate in network B; , characterizing the creep strain dependence of the effective • a nonnegative constant, A, in the expression for the effective creep strain rate—this constant also maintains dimensional consistency in the equation; and • a constant, E, in the expression for the effective creep strain rate—this constant regularizes the creep strain rate near the undeformed state. The effective creep strain rate in network B is given by the expression where B, and is the effective creep strain rate in network B, is the effective stress in network B. The chain stretch in network B, is the nominal creep strain in network , is defined as where is the deviatoric Cauchy stress tensor. . The effective stress in network B is defined as , where Defining strain-rate-dependent material behavior for elastomers The elasticity of the model is defined by a hyperelastic material model. You input the stress scaling factor and the creep parameters for network B directly when you define the hysteresis material model. Typical (sec)−1(MPa)−m , values of the material parameters for a common elastomer are , , , and (Bergstrom and Boyce, 1998; 2001). Input File Usage: Use both of the following options within the same material data block: Abaqus/CAE Usage: *HYSTERESIS *HYPERELASTIC Property module: material editor: Mechanical→Elasticity→Hyperelastic: Suboptions→Hysteresis The input of the parameter is not supported in Abaqus/CAE. Elements The use of the hysteresis material model is restricted to elements that can be used with hyperelastic materials (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1). this model cannot be used with elements based on the plane stress assumption (shell, membrane, and continuum plane stress elements). Hybrid elements can be used with this model only when the accompanying hyperelasticity definition is completely incompressible. When this model is used with reduced-integration elements, the instantaneous elastic moduli are used to calculate the default hourglass stiffness. In addition, Output In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables have special meaning if hysteretic behavior is defined: EE CE Elastic strain corresponding to the stress state at time t and the instantaneous elastic material properties. Equivalent creep strain defined as the difference between the total strain and the elastic strain. These strain measures are used to approximate the strain energy, SENER, and the viscous dissipation, CENER. These approximations may lead to underestimation of the strain energy and overestimation of the viscous dissipation since the effects of internal stresses on these energy quantities are neglected. This inaccuracies may be particularly noticeable in the case of nonmonotonic loading. Additional references • Bergstrom, J. S., and M. C. Boyce, “Constitutive Modeling of the Large Strain Time-Dependent Behavior of Elastomers,” Journal of the Mechanics and Physics of Solids, vol. 46, no. 5, pp. 931–954, May 1998. • Bergstrom, J. S., and M. C. Boyce, “Constitutive Modeling of the Time-Dependent and Cyclic Loading of Elastomers and Application to Soft Biological Tissues,” Mechanics of Materials, vol. 33, no. 9, pp. 523–530, 2001. 22.8.2 PARALLEL NETWORK VISCOELASTIC MODEL Product: Abaqus/Standard References • “Material library: overview,” Section 21.1.1 • “Combining material behaviors,” Section 21.1.3 • “Inelastic behavior,” Section 23.1.1 • *HYPERELASTIC • *VISCOELASTIC Overview The parallel network nonlinear viscoelastic model: • is intended for modeling materials that exhibit nonlinear viscous behavior and undergo large deformations; • consists of multiple elastic and viscoelastic networks in parallel; • uses a hyperelastic material model to specify the elastic response; and • uses multiplicative split of the deformation gradient and a flow rule derived from a creep potential to specify the viscous behavior. Material behavior The parallel network nonlinear viscoelastic model consists of multiple elastic and viscoelastic networks connected in parallel, as shown in Figure 22.8.2–1. The number of viscoelastic networks, N, can be arbitrary; however, at most one purely elastic equilibrium network (network 0 in Figure 22.8.2–1) is allowed in the model. If the elastic network is not defined, the stress in the material will relax completely over time. The model can be used to predict complex behavior of viscous materials subjected to finite strains, which cannot be modeled accurately using the linear viscoelastic model available in Abaqus . An example of such complex behavior is depicted in Figure 22.8.2–2, which shows normalized stress relaxation curves for three different strain levels. This behavior can be modeled accurately using the nonlinear viscoelastic model, but it cannot be captured with the linear model. In the latter case, the three curves would coincide. Elastic behavior The elastic part of the response for all the networks is specified using the hyperelastic material model. Any of the hyperelastic models available in Abaqus can be used . The same hyperelastic material definition is used for all the networks, scaled . . . . . . 0 . . . . . . Figure 22.8.2–1 Nonlinear viscoelastic model with multiple parallel networks. 1.00 0.95 0.90 0.85 sigma1 sigma2 sigma3 0.80 1.0 1.5 2.0 2.5 Time 3.0 3.5 4.0 Figure 22.8.2–2 Normalized stress relaxation curves for three different strain levels. by a stiffness ratio specific to each network. Consequently, only one hyperelastic material definition is required by the model along with the stiffness ratio for each network. The elastic response can be specified by defining either the instantaneous response or the long-term response. Viscous behavior Viscous behavior must be defined for each viscoelastic network. multiplicative split of the deformation gradient and the existence of the creep potential, which the flow rule is derived. In the multiplicative split the deformation gradient is expressed as It is modeled by assuming the , from is the elastic part of the deformation gradient (representing the hyperelastic behavior) and where is the creep part of the deformation gradient (representing the stress-free intermediate configuration). The creep potential is assumed to have the general form where is the Cauchy stress. If the potential is specified, the flow rule can be obtained from where is the symmetric part of the velocity gradient, , expressed in the current configuration and is the proportionality factor. In this model the creep potential is given by and the proportionality factor is taken as , where is the equivalent deviatoric Cauchy stress and is the equivalent creep stain rate. In this case the flow rule has the form or, equivalently is the Kirchhoff stress, where the deviatoric Kirchhoff stress, and be provided. In this model hyperborlic-sine model. is the determinant of is must can be determined from either a power-law strain hardening model or a . To complete the derivation, the evolution law for is the deviatoric Cauchy stress, , Power-law strain hardening model The power-law strain hardening model is available in the form is the equivalent creep strain rate, is the equivalent creep strain, is the equivalent deviatoric Kirchhoff stress, and are material parameters. A, m, and n Hyperbolic-sine law model The hyperbolic-sine law is available in the form where and are defined above, and A, B, and n are material parameters. Thermal expansion Only the isotropic thermal expansion is permitted with the nonlinear viscoelastic material (“Thermal expansion,” Section 26.1.2). Defining viscoelastic response The nonlinear viscoelastic response is defined by specifying the identifier, stiffness ratio, and creep law for each viscoelastic network. Specifying network identifier Each viscoelastic network in the material model must be assigned a unique network identifier or network id. The network identifiers must be consecutive integers starting with 1. The order in which they are specified is not important. Input File Usage: Use the following option to specify the network identifier: *VISCOELASTIC, NONLINEAR, NETWORKID=networkId Defining the stiffness ratio The contribution of each network to the overall response of the material is determined by the value of the stiffness ratio, , which is used to scale the elastic response of the network material. The sum of the stiffness ratios of the viscoelastic networks must be smaller than or equal to 1. If the sum of the ratios is equal to 1, the purely elastic equilibrium network is not created. If the sum of the ratios is smaller than 1, the equilibrium network is created with a stiffness ratio, , equal to where denotes the number of viscoelastic networks and is the stiffness ratio of network . Input File Usage: Use the following option to specify the network’s stiffness ratio: *VISCOELASTIC, NONLINEAR, SRATIO=ratio Specifying the creep law The definition of creep behavior in Abaqus/Standard is completed by specifying the creep law. Strain hardening power law creep model The strain hardening law is defined by specifying three material parameters: A, n, and m. For physically reasonable behavior A and n must be positive and −1 < m ≤ 0. Input File Usage: *VISCOELASTIC, NONLINEAR, LAW=STRAIN Hyperbolic sine creep model The hyperbolic sine creep law is specified by providing three nonnegative parameters: A, B, and n. Input File Usage: *VISCOELASTIC, NONLINEAR, LAW=HYPERB Material response in different analysis steps The material is active during all stress/displacement procedure types. However, the creep effects are taken into account only in a quasi-static analysis . In other stress/displacement procedures the evolution of the state variables is suppressed and the creep strain remains unchanged. Elements The nonlinear viscoelastic model is available with continuum elements that include mechanical behavior (elements that have displacement degrees of freedom), except for one-dimensional and plane stress elements. Output In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables have special meaning for the nonlinear viscoelastic material model: CEEQ CE CENER SENER The overall equivalent creep strain, defined as . The overall creep strain, defined as . The overall viscous dissipated energy per unit volume, defined as . The overall elastic strain energy density per unit volume, defined as . In the above definitions networks, the subscript or superscript to be the purely elastic network. denotes the stiffness ratio for network , denotes the number of viscoelastic is used to denote network quantities, and the network is assumed 22.9 Rate sensitive elastomeric foams • “Low-density foams,” Section 22.9.1 22.9.1 LOW-DENSITY FOAMS Products: Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • *LOW DENSITY FOAM • *UNIAXIAL TEST DATA • “Creating a low-density foam material model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The low-density foam material model: • is intended for low-density, highly compressible elastomeric foams with significant rate sensitive behavior (such as polyurethane foam); • requires the direct specification of uniaxial stress-strain curves at different strain rates for both tension and compression; • optionally allows the specification of lateral strain data to include Poisson effects; • allows for the specification of optional unloading stress-strain curves for better representation of the hysteretic behavior and energy absorption during cyclic loading; and • requires that geometric nonlinearity be accounted for during the analysis step , since it is intended for finite-strain applications. Mechanical response Low-density, highly compressible elastomeric foams are widely used in the automotive industry as energy absorbing materials. Foam padding is used in many passive safety systems, such as behind headliners for head impact protection, in door trims for pelvis and thorax protection, etc. Energy absorbing foams are also commonly used in packaging of hand-held and other electronic devices. The low-density foam material model in Abaqus/Explicit is intended to capture the highly strain-rate sensitive behavior of these materials. The model uses a pseudo visco-hyperelastic formulation whereby the strain energy potential is constructed numerically as a function of principal stretches and a set of internal variables associated with strain rate. By default the Poisson’s ratio of the material is assumed to be zero. With this assumption, the evaluation of the stress-strain response becomes uncoupled along the principal deformation directions. Optionally, nonzero Poisson effects can be specified to include coupling along the principal directions. The model requires as input the stress-strain response of the material for both uniaxial tension and uniaxial compression tests. Poisson effects can be included by also specifying lateral strain data for each of these tests. The tests can be performed at different strain rates. For each test the strain data should be given in nominal strain values (change in length per unit of original length), and the stress data should be given in nominal stress values (force per unit of original cross-sectional area). Uniaxial tension and compression curves are specified separately. The uniaxial stress and strain data are given in absolute values (positive in both tension and compression). On the other hand, when specified, the lateral strain data must be negative in tension and positive in compression, corresponding to a positive Poisson’s effect. The model does not support negative Poisson’s effect. Rate-dependent behavior is specified by providing the uniaxial stress-strain curves for different values of nominal strain rates. Both loading and unloading rate-dependent curves can be specified to better characterize the hysteretic behavior and energy absorption properties of the material during cyclic loading. Use positive values of nominal strain rates for loading curves and negative values for the unloading curves. Currently this option is available only with linear strain rate regularization . When the unloading behavior is not specified directly, the model assumes that unloading occurs along the loading curve associated with the smallest deformation rate. A representative schematic of typical rate-dependent uniaxial compression data is shown in Figure 22.9.1–1 with both loading and unloading curves. It is important that the specified rate-dependent stress-strain curves do not intersect. Otherwise, the material is unstable, and Abaqus issues an error message if an intersection between curves is found.  Figure 22.9.1–1 Rate-dependent loading/unloading stress-strain curves. During the analysis, the stress along each principal deformation direction is evaluated by interpolating the specified loading/unloading stress-strain curves using the corresponding values of principal nominal strain and strain rate. The stress is then corrected by a coupling term if non-zero Poisson effects are included. The representative response of the model for a uniaxial compression cycle is shown in Figure 22.9.1–1. Input File Usage: Use the following options to specify a low-density foam material: *LOW DENSITY FOAM *UNIAXIAL TEST DATA, DIRECTION=TENSION *UNIAXIAL TEST DATA, DIRECTION=COMPRESSION Use the first option to specify a low-density foam material with zero Poisson’s ratio (default), or use the second option to include Poisson effects by defining lateral strains as part of the test data input: *LOW DENSITY FOAM,LATERAL STRAIN DATA=NO (default) *LOW DENSITY FOAM, LATERAL STRAIN DATA=YES In addition, use these two options to give the experimental stress-strain data *UNIAXIAL TEST DATA, DIRECTION=TENSION *UNIAXIAL TEST DATA, DIRECTION=COMPRESSION Property module: material editor: Mechanical→Elasticity→Low Density Foam: Uniaxial Test Data→Uniaxial Tension Test Data, Uniaxial Test Data→Uniaxial Compression Test Data Input File Usage: Abaqus/CAE Usage: Relaxation coefficients , Unphysical jumps in stress due to sudden changes in the deformation rate are prevented using a technique based on viscous regularization. This technique also models stress relaxation effects in a very simplistic manner. In the case of a uniaxial test, for example, the relaxation time is given as , where is a linear viscosity parameter that , and controls the relaxation time when , and typically small values of this parameter should be used. is a nonlinear viscosity parameter that controls the relaxation time at higher values of deformation. controls the sensitivity of the relaxation speed (time The smaller this value, the shorter the relaxation time. to the stretch. The default values of these parameters are units), and are material parameters and is the stretch. (time units), . Input File Usage: Use the following option to specify relaxation coefficients: *LOW DENSITY FOAM , , Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Low Density Foam: Relaxation coefficients: mu0, mu1, alpha Strain rate When Poisson’s ratio is zero, three different strain rate measures can be used for the evaluation of the stress-strain response along each principal deformation direction for general three-dimensional the nominal volumetric strain rate, the nominal strain rate along each principal deformation states: deformation direction, or the maximum of the nominal strain rates along the principal deformation directions. By default, the nominal volumetric strain rate is used; this approach does not produce rate-sensitive behavior under volume-preserving deformation modes (e.g., simple shear). Alternatively, each principal stress can be evaluated based either on the nominal strain rate along the corresponding principal direction or the maximum of the nominal strain rates; both these approaches can provide rate-sensitive behavior for volume-preserving deformation modes. All three strain rate measures produce identical rate-dependent behavior for uniaxial loading conditions when the Poisson’s ratio is zero. When non-zero Poisson effects are defined, the model uses the maximum nominal strain rate along the principal deformation directions for the evaluation of the stress-strain response. This is the default and only strain rate measure available for this case. Input File Usage: Use the following option to use the volumetric strain rate (default when Poisson’s ratio is zero): *LOW DENSITY FOAM, STRAIN RATE=VOLUMETRIC Use the following option to use the nominal strain rate evaluated along each principal direction: *LOW DENSITY FOAM, STRAIN RATE=PRINCIPAL Use the following option to use the maximum of the nominal strain rates along the principal directions (default and only option available when Poisson’s ratio is not zero): Abaqus/CAE Usage: *LOW DENSITY FOAM, STRAIN RATE=MAX PRINCIPAL Use the following option to use the volumetric strain rate (default): Property module: material editor: Mechanical→Elasticity→Low Density Foam: Strain rate measure: Volumetric Use the following option to use the strain rate evaluated along each principal direction: Property module: material editor: Mechanical→Elasticity→Low Density Foam: Strain rate measure: Principal Extrapolation of stress-strain curves By default, for this material model and for strain values beyond the range of specified strains, Abaqus/Explicit extrapolates the stress-strain curves using the slope at the last data point. When the strain rate value exceeds the maximum specified strain rate, Abaqus/Explicit uses the stress-strain curve corresponding to the maximum specified strain rate by default. You can override this default and activate strain rate extrapolation based on the slope (with respect to strain rate). Input File Usage: Use the following option to activate strain rate extrapolation of loading curves: *LOW DENSITY FOAM, RATE EXTRAPOLATION=YES Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Low Density Foam: toggle on Extrapolate stress-strain curve beyond maximum strain rate Tension cutoff and failure Low-density foams have limited strength in tension and can easily rupture under excessive tensile loading. The model in Abaqus/Explicit provides the option to specify a cutoff value for the maximum principal tensile stress that the material can sustain. The maximum principal stresses computed by the program will stay at or below this value. You can also activate deletion (removal) of the element from the simulation when the tension cutoff value is reached, which provides a simple method for modeling rupture. Input File Usage: Use the following option to define a tension cutoff value without element deletion: *LOW DENSITY FOAM, TENSION CUTOFF=value Use the following option to allow element deletion when the tension cutoff value is met: Abaqus/CAE Usage: *LOW DENSITY FOAM, TENSION CUTOFF=value, FAIL=YES Use the following option to define a tension cutoff value: Property module: material editor: Mechanical→Elasticity→Low Density Foam: toggle on Maximum allowable principal tensile stress: value Use the following option to allow element deletion when the tension cutoff value is met: Property module: material editor: Mechanical→Elasticity→Low Density Foam: toggle on Remove elements exceeding maximum Thermal expansion Only isotropic thermal expansion is permitted with the low-density foam material model. The elastic volume ratio, and the thermal volume ratio, , relates the total volume ratio (current volume/reference volume), J, , via the simple relationship: is given by where thermal expansion coefficient (“Thermal expansion,” Section 26.1.2). is the linear thermal expansion strain that is obtained from the temperature and the isotropic Material stability The Drucker stability condition for a compressible material requires that the change in the Kirchhoff stress, , following from an infinitesimal change in the logarithmic strain, , satisfies the inequality where the Kirchhoff stress . Using , the inequality becomes This restriction requires that the tangential material stiffness be positive definite. For an isotropic elastic formulation the inequality can be represented in terms of the principal stresses and strains Thus, the relation between changes in the stress and changes in the strain can be obtained in the form of the matrix equation where . Since must be positive definite, it is necessary that When Poisson’s ratio is zero, the off diagonal terms of conditions for a positive definite matrix reduce to stress-strain curves in the space of Kirchhoff stress versus logarithmic strain must be positive. become zero. In that case the necessary ; that is, the slope of the specified uniaxial You should be careful defining the input data for the low-density foam model to ensure stable If an instability is found, Abaqus issues a warning message material response for all strain rates. and prints the lowest value of strain for which the instability is observed. Ideally, no instability should occur. If instabilities are observed at strain levels that are likely to occur in the analysis, it is strongly recommended that you carefully examine and revise the material input data. When nonzero Poisson effects are defined, it is highly recommended that you provide uniaxial test data in tension and compression for the same range of strain rates. Elements The low-density foam model can be used with solid (continuum) elements and generalized plane strain elements. One-dimensional solid elements (truss and rebar) are also available for the case when no lateral strains are specified (Poisson’s ratio is zero). The model cannot be used with shells, membranes, or the Eulerian elements (EC3D8R and EC3D8RT). Procedures The low-density foam model must always be used with geometrically nonlinear analyses (“General and linear perturbation procedures,” Section 6.1.3). 23. Inelastic Mechanical Properties Overview Metal plasticity Other plasticity models Fabric materials Jointed materials Concrete Permanent set in rubberlike materials 23.1 23.2 23.3 23.4 23.5 23.6 23.1 Overview • “Inelastic behavior,” Section 23.1.1 23.1.1 INELASTIC BEHAVIOR The material library in Abaqus includes several models of inelastic behavior: • Classical metal plasticity: The yield and inelastic flow of a metal at relatively low temperatures, where loading is relatively monotonic and creep effects are not important, can typically be described with the classical metal plasticity models (“Classical metal plasticity,” Section 23.2.1). In Abaqus these models use standard Mises or Hill yield surfaces with associated plastic flow. Perfect plasticity and isotropic hardening definitions are both available in the classical metal plasticity models. Common applications include crash analyses, metal forming, and general collapse studies; the models are simple and adequate for such cases. • Models for metals subjected to cyclic loading: A linear kinematic hardening model or a nonlinear isotropic/kinematic hardening model (“Models for metals subjected to cyclic loading,” Section 23.2.2) can be used in Abaqus to simulate the behavior of materials that are subjected to cyclic loading. The evolution law in these models consists of a kinematic hardening component (which describes the translation of the yield surface in stress space) and, for the nonlinear isotropic/kinematic hardening model, of an isotropic component (which describes the change of the elastic range). The Bauschinger effect and plastic shakedown can be modeled with both models, but the nonlinear isotropic/kinematic hardening model provides more accurate predictions. Ratchetting and relaxation of the mean stress are accounted for only by the nonlinear isotropic/kinematic model. In addition to these two models, the ORNL model in Abaqus/Standard can be used when simple life estimation is desired for the design of stainless steels subjected to low-cycle fatigue and creep fatigue . • Rate-dependent yield: As strain rates increase, many materials show an increase in their yield strength. Rate dependence (“Rate-dependent yield,” Section 23.2.3) can be defined in Abaqus for a number of plasticity models. Rate dependence can be used in both static and dynamic procedures. Applicable models include classical metal plasticity, extended Drucker-Prager plasticity, and crushable foam plasticity. • Creep and swelling: Abaqus/Standard provides a material model for classical metal creep behavior and time-dependent volumetric swelling behavior (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4). This model is intended for relatively slow (quasi-static) inelastic deformation of a model such as the high-temperature creeping flow of a metal or a piece of glass. The creep strain rate is assumed to be purely deviatoric, meaning that there is no volume change associated with this part of the inelastic straining. Creep can be used with the classical metal plasticity model, with the ORNL model, and to define rate-dependent gasket behavior (“Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6). Swelling can be used with the classical metal plasticity model. (Usage with the Drucker-Prager models is explained below.) • Annealing or melting: Abaqus provides a modeling capability for situations in which a loss of memory related to hardening occurs above a certain user-defined temperature, known as the annealing temperature (“Annealing or melting,” Section 23.2.5). It is intended for use with metals subjected to high-temperature deformation processes, in which the material may undergo melting and possibly In Abaqus annealing or melting can be modeled resolidification or some other form of annealing. with classical metal plasticity (Mises and Hill); in Abaqus/Explicit annealing or melting can also be modeled with Johnson-Cook plasticity. The annealing temperature is assumed to be a material property. See “Annealing procedure,” Section 6.12.1, for information on an alternative method for simulating annealing in Abaqus/Explicit. • Anisotropic yield and creep: Abaqus provides an anisotropic yield model (“Anisotropic yield/creep,” Section 23.2.6), which is available for use with materials modeled with classical metal plasticity (“Classical metal plasticity,” Section 23.2.1), kinematic hardening (“Models for metals subjected to cyclic loading,” Section 23.2.2), and/or creep (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) that exhibit different yield stresses in different directions. The Abaqus/Standard model includes creep; creep behavior is not available in Abaqus/Explicit. The model allows for the specification of different stress ratios for each stress component to define the initial anisotropy. The model is not adequate for cases in which the anisotropy changes significantly as the material deforms as a result of loading. • Johnson-Cook plasticity: The Johnson-Cook plasticity model in Abaqus/Explicit (“Johnson-Cook plasticity,” Section 23.2.7) is particularly suited to model high-strain-rate deformation of metals. This model is a particular type of Mises plasticity that includes analytical forms of the hardening law and rate dependence. It is generally used in adiabatic transient dynamic analysis. • Dynamic failure models: Two types of dynamic failure models are offered in Abaqus/Explicit for the Mises and Johnson-Cook plasticity models (“Dynamic failure models,” Section 23.2.8). One is the shear failure model, where the failure criterion is based on the accumulated equivalent plastic strain. Another is the tensile failure model, which uses the hydrostatic pressure stress as a failure measure to model dynamic spall or a pressure cutoff. Both models offer a number of failure choices including element removal and are applicable mainly in truly dynamic situations. In contrast, the progressive failure and damage models (Chapter 24, “Progressive Damage and Failure”) are suitable for both quasi-static and dynamic situations and have other significant advantages. • Porous metal plasticity: The porous metal plasticity model (“Porous metal plasticity,” Section 23.2.9) is used to model materials that exhibit damage in the form of void initiation and growth, and it can also be used for some powder metal process simulations at high relative densities (relative density is defined as the ratio of the volume of solid material to the total volume of the material). The model is based on Gurson’s porous metal plasticity theory with void nucleation and is intended for use with materials that have a relative density that is greater than 0.9. The model is adequate for relatively monotonic loading. • Cast iron plasticity: The cast iron plasticity model (“Cast iron plasticity,” Section 23.2.10) is used to model gray cast iron, which exhibits markedly different inelastic behavior in tension and compression. The microstructure of gray cast iron consists of a distribution of graphite flakes in a steel matrix. In tension the graphite flakes act as stress concentrators, while in compression the flakes serve to transmit stresses. The resulting material is brittle in tension, but in compression it is similar in behavior to steel. The differences in tensile and compressive plastic response include: (i) a yield stress in tension that is three to five times lower than the yield stress in compression; (ii) permanent volume increase in tension, but negligible inelastic volume change in compression; (iii) different hardening behavior in tension and compression. The model is adequate for relatively monotonic loading. • Two-layer viscoplasticity: The two-layer viscoplasticity model in Abaqus/Standard (“Two-layer viscoplasticity,” Section 23.2.11) is useful for modeling materials in which significant time-dependent behavior as well as plasticity is observed. For metals this typically occurs at elevated temperatures. The model has been shown to provide good results for thermomechanical loading. • ORNL constitutive model: The ORNL plasticity model in Abaqus/Standard (“ORNL – Oak Ridge National Laboratory constitutive model,” Section 23.2.12) is intended for cyclic loading and high-temperature creep of type 304 and 316 stainless steel. Plasticity and creep calculations are provided according to the specification in Nuclear Standard NEF 9-5T, “Guidelines and Procedures for Design of Class I Elevated Temperature Nuclear System Components.” This model is an extension of the linear kinematic hardening model (discussed above), which attempts to provide for simple life estimation for design purposes when low-cycle fatigue and creep fatigue are critical issues. • Deformation plasticity: Abaqus/Standard provides a deformation theory Ramberg-Osgood plasticity model (“Deformation plasticity,” Section 23.2.13) for use in developing fully plastic solutions for fracture mechanics applications in ductile metals. The model is most commonly applied in static loading with small-displacement analysis for which the fully plastic solution must be developed in a part of the model. • Extended Drucker-Prager plasticity and creep: The extended Drucker-Prager family of plasticity models (“Extended Drucker-Prager models,” Section 23.3.1) describes the behavior of granular materials or polymers in which the yield behavior depends on the equivalent pressure stress. The inelastic deformation may sometimes be associated with frictional mechanisms such as sliding of particles across each other. This class of models provides a choice of three different yield criteria. The differences in criteria are based on the shape of the yield surface in the meridional plane, which can be a linear form, a hyperbolic form, or a general exponent form. Inelastic time-dependent (creep) behavior coupled with the plastic behavior is also available in Abaqus/Standard for the linear form of the model. Creep behavior is not available in Abaqus/Explicit. • Modified Drucker-Prager/Cap plasticity and creep: The modified Drucker-Prager/Cap plasticity model (“Modified Drucker-Prager/Cap model,” Section 23.3.2) can be used to simulate geological materials that exhibit pressure-dependent yield. The addition of a cap yield surface helps control volume dilatancy when the material yields in shear and provides an inelastic hardening mechanism to represent In Abaqus/Standard inelastic time-dependent (creep) behavior coupled with the plastic compaction. plastic behavior is also available for this model; two creep mechanisms are possible: a cohesion, Drucker-Prager-like mechanism and a consolidation, cap-like mechanism. • Mohr-Coulomb plasticity: The Mohr-Coulomb plasticity model (“Mohr-Coulomb plasticity,” Section 23.3.3) can be used for design applications in the geotechnical engineering area. The model uses the classical Mohr-Coloumb yield criterion: a straight line in the meridional plane and an irregular hexagonal section in the deviatoric plane. However, the Abaqus Mohr-Coulomb model has a completely smooth flow potential instead of the classical hexagonal pyramid: the flow potential is a hyperbola in the meridional plane, and it uses the smooth deviatoric section proposed by Menétrey and Willam. • Critical state (clay) plasticity: The clay plasticity model (“Critical state (clay) plasticity model,” Section 23.3.4) describes the inelastic response of cohesionless soils. The model provides a reasonable match to the experimentally observed behavior of saturated clays. This model defines the inelastic behavior of a material by a yield function that depends on the three stress invariants, an associated flow assumption to define the plastic strain rate, and a strain hardening theory that changes the size of the yield surface according to the inelastic volumetric strain. • Crushable foam plasticity: The foam plasticity model (“Crushable foam plasticity models,” Section 23.3.5) is intended for modeling crushable foams that are typically used as energy absorption structures; however, other crushable materials such as balsa wood can also be simulated with this model. This model is most appropriate for relatively monotonic loading. The crushable foam model with isotropic hardening is applicable to polymeric foams as well as metallic foams. • Jointed material: The jointed material model in Abaqus/Standard (“Jointed material model,” Section 23.5.1) is intended to provide a simple, continuum model for a material that contains a high density of parallel joint surfaces in different orientations, such as sedimentary rock. This model is intended for applications where stresses are mainly compressive, and it provides a joint opening capability when the stress normal to the joint tries to become tensile. • Concrete: Three different constitutive models are offered in Abaqus for the analysis of concrete at low confining pressures: the smeared crack concrete model in Abaqus/Standard (“Concrete smeared cracking,” Section 23.6.1); the brittle cracking model in Abaqus/Explicit (“Cracking model for concrete,” Section 23.6.2); and the concrete damaged plasticity model in both Abaqus/Standard and Abaqus/Explicit (“Concrete damaged plasticity,” Section 23.6.3). Each model is designed to provide a general capability for modeling plain and reinforced concrete (as well as other similar quasi-brittle materials) in all types of structures: beams, trusses, shells, and solids. The smeared crack concrete model in Abaqus/Standard is intended for applications in which the concrete is subjected to essentially monotonic straining and a material point exhibits either tensile cracking or compressive crushing. Plastic straining in compression is controlled by a “compression” yield surface. Cracking is assumed to be the most important aspect of the behavior, and the representation of cracking and postcracking anisotropic behavior dominates the modeling. The brittle cracking model in Abaqus/Explicit is intended for applications in which the concrete behavior is dominated by tensile cracking and compressive failure is not important. The model includes consideration of the anisotropy induced by cracking. In compression, the model assumes elastic behavior. A simple brittle failure criterion is available to allow the removal of elements from a mesh. The concrete damaged plasticity model in Abaqus/Standard and Abaqus/Explicit is based on the assumption of scalar (isotropic) damage and is designed for applications in which the concrete is subjected to arbitrary loading conditions, including cyclic loading. The model takes into consideration the degradation of the elastic stiffness induced by plastic straining both in tension and compression. It also accounts for stiffness recovery effects under cyclic loading. • Progressive damage and failure: Abaqus/Explicit offers a general capability for modeling progressive damage and failure in ductile metals and fiber-reinforced composites (Chapter 24, “Progressive Damage and Failure”). Plasticity theories Most materials of engineering interest initially respond elastically. Elastic behavior means that the deformation is fully recoverable: when the load is removed, the specimen returns to its original shape. If the load exceeds some limit (the “yield load”), the deformation is no longer fully recoverable. Some part of the deformation will remain when the load is removed, as, for example, when a paperclip is bent too much or when a billet of metal is rolled or forged in a manufacturing process. Plasticity theories model the material’s mechanical response as it undergoes such nonrecoverable deformation in a ductile fashion. The theories have been developed most intensively for metals, but they are also applied to soils, concrete, rock, ice, crushable foam, and so on. These materials behave in very different ways. For example, large values of pure hydrostatic pressure cause very little inelastic deformation in metals, but quite small hydrostatic pressure values may cause a significant, nonrecoverable volume change in a soil sample. Nonetheless, the fundamental concepts of plasticity theories are sufficiently general that models based on these concepts have been developed successfully for a wide range of materials. Most of the plasticity models in Abaqus are “incremental” theories in which the mechanical strain rate is decomposed into an elastic part and a plastic (inelastic) part. Incremental plasticity models are usually formulated in terms of • a yield surface, which generalizes the concept of “yield load” into a test function that can be used to determine if the material responds purely elastically at a particular state of stress, temperature, etc; • a flow rule, which defines the inelastic deformation that occurs if the material point is no longer responding purely elastically; and • evolution laws that define the hardening—the way in which the yield and/or flow definitions change as inelastic deformation occurs. Abaqus/Standard also has a “deformation” plasticity model, in which the stress is defined from the total mechanical strain. This is a Ramberg-Osgood model (“Deformation plasticity,” Section 23.2.13) and is intended primarily for ductile fracture mechanics applications, where fully plastic solutions are often required. Elastic response The Abaqus plasticity models also need an elasticity definition to deal with the recoverable part of the strain. In Abaqus the elasticity is defined by including linear elastic behavior or, if relevant for some plasticity models, porous elastic behavior in the same material definition . In the case of the Mises and Johnson-Cook plasticity models in Abaqus/Explicit the elasticity can alternatively be defined using an equation of state with associated deviatoric behavior . When performing an elastic-plastic analysis at finite strains, Abaqus assumes that the plastic strains dominate the deformation and that the elastic strains are small. This restriction is imposed by the elasticity models that Abaqus uses. It is justified because most materials have a well-defined yield point that is a very small percentage of their Young’s modulus; for example, the yield stress of metals is typically less than 1% of the Young’s modulus of the material. Therefore, the elastic strains will also be less than this percentage, and the elastic response of the material can be modeled quite accurately as being linear. In Abaqus/Explicit the elastic strain energy reported is updated incrementally. The incremental is the incremental ) is computed as , where change in elastic strain energy ( change in total strain energy and is much smaller than and is the incremental change in plastic energy dissipation. for increments in which the deformation is almost all plastic. and and result in deviations from the true solutions that are Approximations in the calculations of insignificant compared to . Typically, the elastic strain energy solution is quite accurate, but in some rare cases the approximations in the calculations of can lead to a negative value reported for the elastic strain energy. These negative values are most likely to occur in an analysis that uses rate-dependent plasticity. As long as the absolute value of the elastic strain energy is very small compared to the total strain energy, a negative value for the elastic strain energy should not be considered an indication of a serious solution problem. but can be significant relative to and Stress and strain measures Most materials that exhibit ductile behavior (large inelastic strains) yield at stress levels that are orders of magnitude less than the elastic modulus of the material, which implies that the relevant stress and strain measures are “true” stress (Cauchy stress) and logarithmic strain. Material data for all of these models should, therefore, be given in these measures. If you have nominal stress-strain data for a uniaxial test and the material is isotropic, a simple conversion to true stress and logarithmic plastic strain is where E is the Young’s modulus. Example of stress-strain data input The example below illustrates the input of material data for the classical metal plasticity model with isotropic hardening (“Classical metal plasticity,” Section 23.2.1). Stress-strain data representing the material hardening behavior are necessary to define the model. An experimental hardening curve might appear as that shown in Figure 23.1.1–1. First yield occurs at 200 MPa (29000 lb/in2). The material then hardens to 300 MPa (43511 lb/in2 ) at one percent strain, after which it is perfectly plastic. Assuming that the Young’s modulus is 200000 MPa (29 × 106 lb/in2 ), the plastic strain at the one percent strain point is .01 − 300/200000=.0085. When the units are newtons and millimeters, the input is Yield Stress Plastic Strain 200. 300. 0. .0085 Plastic strain values, not total strain values, are used in defining the hardening behavior. Furthermore, the first data pair must correspond with the onset of plasticity (the plastic strain value must be zero in the first pair). These concepts are applicable when hardening data are defined in a tabular form for any of the following plasticity models: True stress, MPa 300 200 True stress, lb/in2 40000 30000 0.85 1.0 Log strain, percent Figure 23.1.1–1 Experimental hardening curve. • “Classical metal plasticity,” Section 23.2.1 • “Models for metals subjected to cyclic loading,” Section 23.2.2 • “Porous metal plasticity,” Section 23.2.9 (isotropic hardening classical metal plasticity must be defined for use with this model) • “Cast iron plasticity,” Section 23.2.10 • “ORNL – Oak Ridge National Laboratory constitutive model,” Section 23.2.12 • “Extended Drucker-Prager models,” Section 23.3.1 • “Modified Drucker-Prager/Cap model,” Section 23.3.2 • “Mohr-Coulomb plasticity,” Section 23.3.3 • “Critical state (clay) plasticity model,” Section 23.3.4 • “Crushable foam plasticity models,” Section 23.3.5 • “Concrete smeared cracking,” Section 23.6.1 The input required to define hardening is discussed in the referenced sections. Specifying initial equivalent plastic strains Initial values of equivalent plastic strain can be specified in Abaqus for elements that use classical metal plasticity (“Classical metal plasticity,” Section 23.2.1) or Drucker-Prager plasticity (“Extended Drucker-Prager models,” Section 23.3.1) by defining initial hardening conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). The equivalent plastic strain (output variable PEEQ) then contains the initial value of equivalent plastic strain plus any additional equivalent plastic strain due to plastic straining during the analysis. However, the plastic strain tensor (output variable PE) contains only the amount of straining due to deformation during the analysis. The simple one-dimensional example shown in Figure 23.1.1–2 illustrates the concept. The material . It is then hardened by loading it along . A new analysis that employs the same hardening curve is in an annealed configuration at point A; its yield stress is the path ; the new yield stress is εpl 21 C, E εpl ε Figure 23.1.1–2 Initial equivalent plastic strain example. . Plastic strain , starting from point D, by specifying a as the first analysis takes this material along the path total strain, will result and can be output (for instance) using output variable PE11. To obtain the correct yield stress, , should be provided as an initial condition. Likewise, the correct yield stress at point F is obtained from an equivalent plastic strain PEEQ , the equivalent plastic strain at point E, . 23.2 Metal plasticity • “Classical metal plasticity,” Section 23.2.1 • “Models for metals subjected to cyclic loading,” Section 23.2.2 • “Rate-dependent yield,” Section 23.2.3 • “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 • “Annealing or melting,” Section 23.2.5 • “Anisotropic yield/creep,” Section 23.2.6 • “Johnson-Cook plasticity,” Section 23.2.7 • “Dynamic failure models,” Section 23.2.8 • “Porous metal plasticity,” Section 23.2.9 • “Cast iron plasticity,” Section 23.2.10 • “Two-layer viscoplasticity,” Section 23.2.11 • “ORNL – Oak Ridge National Laboratory constitutive model,” Section 23.2.12 • “Deformation plasticity,” Section 23.2.13 23.2.1 CLASSICAL METAL PLASTICITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Rate-dependent yield,” Section 23.2.3 • “Anisotropic yield/creep,” Section 23.2.6 • “Johnson-Cook plasticity,” Section 23.2.7 • Chapter 24, “Progressive Damage and Failure” • “Dynamic failure models,” Section 23.2.8 • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • “UHARD,” Section 1.1.35 of the Abaqus User Subroutines Reference Manual • *PLASTIC • *RATE DEPENDENT • *POTENTIAL • “Defining classical metal plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The classical metal plasticity models: • use Mises or Hill yield surfaces with associated plastic flow, which allow for isotropic and anisotropic yield, respectively; • use perfect plasticity or isotropic hardening behavior; • can be used when rate-dependent effects are important; • are intended for applications such as crash analyses, metal forming, and general collapse studies (Plasticity models that include kinematic hardening and are, therefore, more suitable for cases involving cyclic loading are also available in Abaqus: see “Models for metals subjected to cyclic loading,” Section 23.2.2.); • can be used in any procedure that uses elements with displacement degrees of freedom; • can be used in a fully coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.3), a fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4), or an adiabatic thermal-stress analysis (“Adiabatic analysis,” Section 6.5.4) such that plastic dissipation results in the heating of a material; • can be used in conjunction with the models of progressive damage and failure in Abaqus (“Damage and failure for ductile metals: overview,” Section 24.2.1) to specify different damage initiation criteria and damage evolution laws that allow for the progressive degradation of the material stiffness and the removal of elements from the mesh; • can be used in conjunction with the shear failure model in Abaqus/Explicit to provide a simple ductile dynamic failure criterion that allows for the removal of elements from the mesh, although the progressive damage and failure methods discussed above are generally recommended instead; • can be used in conjunction with the tensile failure model in Abaqus/Explicit to provide a tensile spall criterion offering a number of failure choices and removal of elements from the mesh; and • must be used in conjunction with either the linear elastic material model (“Linear elastic behavior,” Section 22.2.1) or the equation of state material model (“Equation of state,” Section 25.2.1). Yield surfaces The Mises and Hill yield surfaces assume that yielding of the metal is independent of the equivalent pressure stress: this observation is confirmed experimentally for most metals (except voided metals) under positive pressure stress but may be inaccurate for metals under conditions of high triaxial tension when voids may nucleate and grow in the material. Such conditions can arise in stress fields near crack tips and in some extreme thermal loading cases such as those that might occur during welding processes. A porous metal plasticity model is provided in Abaqus for such situations. This model is described in “Porous metal plasticity,” Section 23.2.9. Mises yield surface The Mises yield surface is used to define isotropic yielding. It is defined by giving the value of the uniaxial yield stress as a function of uniaxial equivalent plastic strain, temperature, and/or field variables. In Abaqus/Standard the yield stress can alternatively be defined in user subroutine UHARD. Input File Usage: Abaqus/CAE Usage: *PLASTIC Property module: material editor: Mechanical→Plasticity→Plastic Hill yield surface , for the metal plasticity model and define a set of yield ratios, The Hill yield surface allows anisotropic yielding to be modeled. You must specify a reference yield stress, , separately. These data define the yield stress corresponding to each stress component as . Hill’s potential function is discussed in detail in “Anisotropic yield/creep,” Section 23.2.6. Yield ratios can be used to define three common forms of anisotropy associated with sheet metal forming: transverse anisotropy, planar anisotropy, and general anisotropy. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *PLASTIC (to specify the reference yield stress *POTENTIAL (to specify the yield ratios ) Property module: material editor: Mechanical→Plasticity→Plastic: Suboptions→Potential ) Hardening In Abaqus a perfectly plastic material (with no hardening) can be defined, or work hardening can be specified. Isotropic hardening, including Johnson-Cook hardening, is available in both Abaqus/Standard and Abaqus/Explicit. In addition, Abaqus provides kinematic hardening for materials subjected to cyclic loading. Perfect plasticity Perfect plasticity means that the yield stress does not change with plastic strain. It can be defined in tabular form for a range of temperatures and/or field variables; a single yield stress value per temperature and/or field variable specifies the onset of yield. Input File Usage: Abaqus/CAE Usage: *PLASTIC Property module: material editor: Mechanical→Plasticity→Plastic Isotropic hardening Isotropic hardening means that the yield surface changes size uniformly in all directions such that the yield stress increases (or decreases) in all stress directions as plastic straining occurs. Abaqus provides an isotropic hardening model, which is useful for cases involving gross plastic straining or in cases where the straining at each point is essentially in the same direction in strain space throughout the analysis. Although the model is referred to as a “hardening” model, strain softening or hardening followed by softening can be defined. Isotropic hardening plasticity is discussed in more detail in “Isotropic elasto- plasticity,” Section 4.3.2 of the Abaqus Theory Manual. If isotropic hardening is defined, the yield stress, , can be given as a tabular function of plastic strain and, if required, of temperature and/or other predefined field variables. The yield stress at a given state is simply interpolated from this table of data, and it remains constant for plastic strains exceeding the last value given as tabular data. Abaqus/Explicit will regularize the data into tables that are defined in terms of even intervals of the independent variables. In some cases where the yield stress is defined at uneven intervals of the independent variable (plastic strain) and the range of the independent variable is large compared to the smallest interval, Abaqus/Explicit may fail to obtain an accurate regularization of your data in a reasonable number of intervals. In this case the program will stop after all data are processed with an error message that you must redefine the material data. See “Material data definition,” Section 21.1.2, for a more detailed discussion of data regularization. Input File Usage: Abaqus/CAE Usage: *PLASTIC, HARDENING=ISOTROPIC (default if parameter is omitted) Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Isotropic Johnson-Cook isotropic hardening Johnson-Cook hardening is a particular type of isotropic hardening where the yield stress is given as an analytical function of equivalent plastic strain, strain rate, and temperature. This hardening law is suited for modeling high-rate deformation of many materials including most metals. Hill’s potential function cannot be used with Johnson-Cook hardening. For more details, see “Johnson-Cook plasticity,” Section 23.2.7. Input File Usage: Abaqus/CAE Usage: *PLASTIC, HARDENING=JOHNSON COOK Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Johnson-Cook User subroutine In Abaqus/Standard the yield stress for isotropic hardening, user subroutine UHARD. , can alternatively be described through Input File Usage: Abaqus/CAE Usage: *PLASTIC, HARDENING=USER Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: User Kinematic hardening Two kinematic hardening models are provided in Abaqus to model the cyclic loading of metals. The linear kinematic model approximates the hardening behavior with a constant rate of hardening. The more general nonlinear isotropic/kinematic model will give better predictions but requires more detailed calibration. For more details, see “Models for metals subjected to cyclic loading,” Section 23.2.2. Input File Usage: Use the following option to specify the linear kinematic model: *PLASTIC, HARDENING=KINEMATIC Use the following option to specify the nonlinear combined isotropic/kinematic model: Abaqus/CAE Usage: *PLASTIC, HARDENING=COMBINED Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Kinematic or Combined Flow rule Abaqus uses associated plastic flow. Therefore, as the material yields, the inelastic deformation rate is in the direction of the normal to the yield surface (the plastic deformation is volume invariant). This assumption is generally acceptable for most calculations with metals; the most obvious case where it is not appropriate is the detailed study of the localization of plastic flow in sheets of metal as the sheet develops texture and eventually tears apart. So long as the details of such effects are not of interest (or can be inferred from less detailed criteria, such as reaching a forming limit that is defined in terms of strain), the associated flow models in Abaqus used with the smooth Mises or Hill yield surfaces generally predict the behavior accurately. Rate dependence As strain rates increase, many materials show an increase in their yield strength. This effect becomes important in many metals when the strain rates range between 0.1 and 1 per second; and it can be very important for strain rates ranging between 10 and 100 per second, which are characteristic of high-energy dynamic events or manufacturing processes. There are multiple ways to introduce a strain-rate-dependent yield stress. Direct tabular data Test data can be provided as tables of yield stress values versus equivalent plastic strain at different ); one table per strain rate. Direct tabular data cannot be used equivalent plastic strain rates ( with Johnson-Cook hardening. The guidelines that govern the entry of this data are provided in “Rate-dependent yield,” Section 23.2.3. Input File Usage: Abaqus/CAE Usage: *PLASTIC, RATE= Property module: material editor: Mechanical→Plasticity→Plastic: Use strain-rate-dependent data Yield stress ratios Alternatively, you can specify the strain rate dependence by means of a scaling function. In this case you enter only one hardening curve, the static hardening curve, and then express the rate-dependent hardening curves in terms of the static relation; that is, we assume that where is the static yield stress, rate, and R is a ratio, defined as dependent yield,” Section 23.2.3. is the equivalent plastic strain, is the equivalent plastic strain . This method is described further in “Rate- at Input File Usage: Abaqus/CAE Usage: User subroutine Use both of the following options: *PLASTIC (to specify the static yield stress *RATE DEPENDENT (to specify the ratio Property module: material editor: Mechanical→Plasticity→Plastic: Suboptions→Rate Dependent ) ) In Abaqus/Standard user subroutine UHARD can be used to define a rate-dependent yield stress. You are provided the current equivalent plastic strain and equivalent plastic strain rate and are responsible for returning the yield stress and derivatives. Input File Usage: Abaqus/CAE Usage: *PLASTIC, HARDENING=USER Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: User Progressive damage and failure In Abaqus the metal plasticity material models can be used in conjunction with the progressive damage and failure models discussed in “Damage and failure for ductile metals: overview,” Section 24.2.1. The capability allows for the specification of one or more damage initiation criteria, including ductile, shear, forming limit diagram (FLD), forming limit stress diagram (FLSD), Müschenborn-Sonne forming limit diagram (MSFLD), and, in Abaqus/Explicit, Marciniak-Kuczynski (M-K) criteria. After damage initiation, the material stiffness is degraded progressively according to the specified damage evolution response. The model offers two failure choices, including the removal of elements from the mesh as a result of tearing or ripping of the structure. The progressive damage models allow for a smooth degradation of the material stiffness, making them suitable for both quasi-static and dynamic situations. This is a great advantage over the dynamic failure models discussed next. Input File Usage: Use the following options: Abaqus/CAE Usage: *PLASTIC *DAMAGE INITIATION *DAMAGE EVOLUTION Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution Shear and tensile dynamic failure in Abaqus/Explicit In Abaqus/Explicit the metal plasticity material models can be used in conjunction with the shear and tensile failure models (“Dynamic failure models,” Section 23.2.8) that are applicable in truly dynamic situations; however, the progressive damage and failure models discussed above are generally preferred. Shear failure The shear failure model provides a simple failure criterion that is suitable for high-strain-rate deformation of many materials including most metals. It offers two failure choices, including the removal of elements from the mesh as a result of tearing or ripping of the structure. The shear failure criterion is based on the value of the equivalent plastic strain and is applicable mainly to high-strain-rate, truly dynamic problems. For more details, see “Dynamic failure models,” Section 23.2.8. Input File Usage: Use both of the following options: *PLASTIC *SHEAR FAILURE The shear failure model is not supported in Abaqus/CAE. Abaqus/CAE Usage: Tensile failure The tensile failure model uses the hydrostatic pressure stress as a failure measure to model dynamic spall or a pressure cutoff. It offers a number of failure choices including element removal. Similarly to the shear failure model, the tensile failure model is suitable for high-strain-rate deformation of metals and is applicable to truly dynamic problems. For more details, see “Dynamic failure models,” Section 23.2.8. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *PLASTIC *TENSILE FAILURE The tensile failure model is not supported in Abaqus/CAE. Heat generation by plastic work Abaqus optionally allows for plastic dissipation to result in the heating of a material. Heat generation is typically used in the simulation of bulk metal forming or high-speed manufacturing processes involving large amounts of inelastic strain where the heating of the material caused by its deformation is an important effect because of temperature dependence of the material properties. It is applicable only to adiabatic thermal-stress analysis (“Adiabatic analysis,” Section 6.5.4), fully coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.3), or fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4). This effect is introduced by defining the fraction of the rate of inelastic dissipation that appears as a heat flux per volume. Input File Usage: Use all of the following options in the same material data block: *PLASTIC *SPECIFIC HEAT *DENSITY *INELASTIC HEAT FRACTION Use all of the following options for the same material: Property module: material editor: Mechanical→Plasticity→Plastic Thermal→Specific Heat General→Density Thermal→Inelastic Heat Fraction Abaqus/CAE Usage: Initial conditions When we need to study the behavior of a material that has already been subjected to some work hardening, initial equivalent plastic strain values can be provided to specify the yield stress corresponding to the work hardened state . *INITIAL CONDITIONS, TYPE=HARDENING Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step Abaqus/CAE Usage: Input File Usage: User subroutine specification in Abaqus/Standard For more complicated cases, initial conditions can be defined in Abaqus/Standard through user subroutine HARDINI. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING, USER Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined Elements Classical metal plasticity can be used with any elements that include mechanical behavior (elements that have displacement degrees of freedom). Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable the identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), following variable has special meaning for the classical metal plasticity models: PEEQ Equivalent plastic strain, equivalent plastic strain (zero or user-specified; see “Initial conditions”). where is the initial 23.2.2 MODELS FOR METALS SUBJECTED TO CYCLIC LOADING Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • “Anisotropic yield/creep,” Section 23.2.6 • “UHARD,” Section 1.1.35 of the Abaqus User Subroutines Reference Manual • *CYCLIC HARDENING • *PLASTIC • *POTENTIAL • “Defining classical metal plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The kinematic hardening models: • are used to simulate the inelastic behavior of materials that are subjected to cyclic loading; • include a linear kinematic hardening model and a nonlinear isotropic/kinematic hardening model; • include a nonlinear isotropic/kinematic hardening model with multiple backstresses; • can be used in any procedure that uses elements with displacement degrees of freedom; • in Abaqus/Standard cannot be used in adiabatic analyses, and the nonlinear isotropic/kinematic hardening model cannot be used in coupled temperature-displacement analyses; • can be used to model rate-dependent yield; • can be used with creep and swelling in Abaqus/Standard; and • require the use of the linear elasticity material model to define the elastic part of the response. Yield surfaces The kinematic hardening models used to model the behavior of metals subjected to cyclic loading are pressure-independent plasticity models; in other words, yielding of the metals is independent of the equivalent pressure stress. These models are suited for most metals subjected to cyclic loading conditions, except voided metals. The linear kinematic hardening model can be used with the Mises or Hill yield surface. The nonlinear isotropic/kinematic model can be used only with the Mises yield surface in Abaqus/Standard and with the Mises or Hill yield surface in Abaqus/Explicit. The pressure-independent yield surface is defined by the function where to the backstress is the yield stress and . For example, the equivalent Mises stress is defined as is the equivalent Mises stress or Hill’s potential with respect is the deviatoric stress tensor (defined as where equivalent pressure stress, and tensor. is the identity tensor) and , where is the stress tensor, p is the is the deviatoric part of the backstress Flow rule The kinematic hardening models assume associated plastic flow: where equivalent plastic strain is obtained from the following equivalent plastic work expression: is the equivalent plastic strain rate. The evolution of the is the rate of plastic flow and for isotropic Mises plasticity. The assumption of associated plastic flow which yields is acceptable for metals subjected to cyclic loading as long as microscopic details, such as localization of plastic flow occurring as a metal component ruptures due to cyclic fatigue loads, are not of interest. Hardening The linear kinematic hardening model has a constant hardening modulus, and the nonlinear isotropic/kinematic hardening model has both nonlinear kinematic and nonlinear isotropic hardening components. Linear kinematic hardening model The evolution law of this model consists of a linear kinematic hardening component that describes the translation of the yield surface in stress space through the backstress, . When temperature dependence is omitted, this evolution law is the linear Ziegler hardening law where the equivalent stress defining the size of the yield surface, , remains constant, the equivalent stress defining the size of the yield surface at zero plastic strain. is the equivalent plastic strain rate and C is the kinematic hardening modulus. In this model is , where Nonlinear isotropic/kinematic hardening model The evolution law of this model consists of two components: a nonlinear kinematic hardening component, which describes the translation of the yield surface in stress space through the backstress, ; and an isotropic hardening component, which describes the change of the equivalent stress defining the size of the yield surface, , as a function of plastic deformation. The kinematic hardening component is defined to be an additive combination of a purely kinematic term (linear Ziegler hardening law) and a relaxation term (the recall term), which introduces the nonlinearity. In addition, several kinematic hardening components (backstresses) can be superposed, which may considerably improve results in some cases. When temperature and field variable dependencies are omitted, the hardening laws for each backstress are and the overall backstress is computed from the relation and is the number of backstresses, and are material parameters that must be calibrated where from cyclic test data. determine the rate at are the initial kinematic hardening moduli, and which the kinematic hardening moduli decrease with increasing plastic deformation. The kinematic hardening law can be separated into a deviatoric part and a hydrostatic part; only the deviatoric part has an effect on the material behavior. When are zero, the model reduces to an isotropic hardening model. When all equal zero, the linear Ziegler hardening law is recovered. Calibration of the material parameters is discussed in “Usage and calibration of the kinematic hardening models,” below. Figure 23.2.2–1 shows an example of nonlinear kinematic hardening with three backstresses. Each of the backstresses covers a different range of strains, and the linear hardening law is retained for large strains. and The isotropic hardening behavior of the model defines the evolution of the yield surface size, . This evolution can be introduced by specifying , as a directly in user subroutine UHARD (in Abaqus/Standard function of the equivalent plastic strain, as a function of only), or by using the simple exponential law in tabular form, by specifying where is the maximum change in the size of the yield surface, and b defines the rate at which the size of the yield is the yield stress at zero plastic strain and and b are material parameters. [x1.E3] 70. ] [ 60. 50. 40. 30. 20. 10. = + + ) ) 4 0 10 1 0( × . . pl 20 2 0 10 1 0( × . . 500 pl × 4 0 10 . pl 0. 0.00 0.05 0.10 0.15 equivalent plastic strain 0.20 0.25 0.30 Figure 23.2.2–1 Kinematic hardening model with three backstresses. surface changes as plastic straining develops. When the equivalent stress defining the size of the yield surface remains constant ( ), the model reduces to a nonlinear kinematic hardening model. The evolution of the kinematic and the isotropic hardening components is illustrated in Figure 23.2.2–2 for unidirectional loading and in Figure 23.2.2–3 for multiaxial loading. The evolution law for the kinematic hardening component implies that the backstress is contained within a cylinder of radius at saturation (large plastic strains). It also implies that any stress point must lie within a cylinder of radius (using the notation of Figure 23.2.2–2) since the yield surface remains bounded. At large plastic strain any stress point is contained within a cylinder of radius is the equivalent stress defining the size of the yield surface at large plastic strain. If tabular data are provided for the isotropic is the last value given to define the size of the yield surface. If user subroutine UHARD component, is used, this value will depend on your implementation; otherwise, is the magnitude of , where , where . Predicted material behavior In the kinematic hardening models the center of the yield surface moves in stress space due to the kinematic hardening component. In addition, when the nonlinear isotropic/kinematic hardening model is used, the yield surface range may expand or contract due to the isotropic component. These features allow modeling of inelastic deformation in metals that are subjected to cycles of load or temperature, resulting in significant inelastic deformation and, possibly, low-cycle fatigue failure. These models account for the following phenomena:  max  0 0  0  =  0  N C   =1 s +  0 pl Figure 23.2.2–2 One-dimensional representation of the hardening in the nonlinear isotropic/kinematic model. s3 limit surface Ck ∑ γ= 3 1 ∂F s1 s2 yield surface Figure 23.2.2–3 Three-dimensional representation of the hardening in the nonlinear isotropic/kinematic model. • Bauschinger effect: This effect is characterized by a reduced yield stress upon load reversal after plastic deformation has occurred during the initial loading. This phenomenon decreases with continued cycling. The linear kinematic hardening component takes this effect into consideration, but a nonlinear component improves the shape of the cycles. Further improvement of the shape of the cycle can be obtained by using a nonlinear model with multiple backstresses. • Cyclic hardening with plastic shakedown: This phenomenon is characteristic of symmetric stress- or strain-controlled experiments. Soft or annealed metals tend to harden toward a stable limit, and initially hardened metals tend to soften. Figure 23.2.2–4 illustrates the behavior of a metal that hardens under prescribed symmetric strain cycles. Δε = constant time stabilized plastic shakedown Δε = constant Figure 23.2.2–4 Plastic shakedown. The kinematic hardening component of the models used alone predicts plastic shakedown after one stress cycle. The combination of the isotropic component together with the nonlinear kinematic component predicts shakedown after several cycles. • Ratchetting: Unsymmetric cycles of stress between prescribed limits will cause progressive “creep” or “ratchetting” in the direction of the mean stress (Figure 23.2.2–5). Typically, transient ratchetting is followed by stabilization (zero ratchet strain) for low mean stresses, while a constant increase in the accumulated ratchet strain is observed at high mean stresses. The nonlinear kinematic hardening component, used without the isotropic hardening component, predicts constant ratchet strain. The prediction of ratchetting is improved by adding isotropic hardening, in which case the ratchet strain may decrease until it becomes constant. However, in general the nonlinear hardening model with a single backstress predicts a too significant ratchetting effect. A considerable improvement in modeling ratchetting can be achieved by superposing several kinematic hardening models (backstresses) and choosing one of the models to be linear or nearly linear ( ), which results in a less pronounced ratchetting effect. 1 2 δε mean stress 1 2 δε ratchet strain Figure 23.2.2–5 Ratchetting. • Relaxation of the mean stress: This phenomenon is characteristic of an unsymmetric strain experiment, as shown in Figure 23.2.2–6. Figure 23.2.2–6 Relaxation of the mean stress. As the number of cycles increases, the mean stress tends to zero. The nonlinear kinematic hardening component of the nonlinear isotropic/kinematic hardening model accounts for this behavior. Limitations The linear kinematic model is a simple model that gives only a first approximation of the behavior of metals subjected to cyclic loading, as explained above. The nonlinear isotropic/kinematic hardening model can provide more accurate results in many cases involving cyclic loading, but it still has the following limitations: • The isotropic hardening is the same at all strain ranges. Physical observations, however, indicate that the amount of isotropic hardening depends on the magnitude of the strain range. Furthermore, if the specimen is cycled at two different strain ranges, one followed by the other, the deformation in the first cycle affects the isotropic hardening in the second cycle. Thus, the model is only a coarse approximation of actual cyclic behavior. It should be calibrated to the expected size of the strain cycles of importance in the application. • The same cyclic hardening behavior is predicted for proportional and nonproportional load cycles. Physical observations indicate that the cyclic hardening behavior of materials subjected to nonproportional loading may be very different from uniaxial behavior at a similar strain amplitude. The example problems “Simple proportional and nonproportional cyclic tests,” Section 3.2.8 of the Abaqus Benchmarks Manual, “Notched beam under cyclic loading,” Section 1.1.7 of the Abaqus Example Problems Manual and “Uniaxial ratchetting under tension and compression,” Section 1.1.8 of the Abaqus Example Problems Manual, illustrate the phenomena of cyclic hardening with plastic shakedown, ratchetting, and relaxation of the mean stress for the nonlinear isotropic/kinematic hardening model, as well as its limitations. Usage and calibration of the kinematic hardening models The linear kinematic model approximates the hardening behavior with a constant rate of hardening. This hardening rate should be matched to the average hardening rate measured in stabilized cycles over a strain range corresponding to that expected in the application. A stabilized cycle is obtained by cycling over a fixed strain range until a steady-state condition is reached; that is, until the stress-strain curve no longer changes shape from one cycle to the next. The more general nonlinear model will give better predictions but requires more detailed calibration. Linear kinematic hardening model The test data obtained from a half cycle of a unidirectional tension or compression experiment must be linearized, since this simple model can predict only linear hardening. The data are usually based on measurements of the stabilized behavior in strain cycles covering a strain range corresponding to the strain range that is anticipated to occur in the application. Abaqus expects you to provide only two data pairs to define this linear behavior: the yield stress, , at a finite plastic strain value, . The linear kinematic hardening modulus, C, is determined from the relation , at zero plastic strain and a yield stress, You can provide several sets of two data pairs as a function of temperature to define the variation of the linear kinematic hardening modulus with respect to temperature. If the Hill yield surface is desired for this model, you must specify a set of yield ratios, , independently . This model gives physically reasonable results for only relatively small strains (less than 5%). Input File Usage: Abaqus/CAE Usage: *PLASTIC, HARDENING=KINEMATIC Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Kinematic Nonlinear isotropic/kinematic hardening model , as a function of the The evolution of the equivalent stress defining the size of the yield surface, equivalent plastic strain, , defines the isotropic hardening component of the model. You can define this isotropic hardening component through an exponential law or directly in tabular form. It need not be defined if the yield surface remains fixed throughout the loading. In Abaqus/Explicit if the Hill yield surface is desired for this model, you must specify a set of yield ratios, , independently . The Hill yield surface cannot be used with this model in Abaqus/Standard. and The material parameters determine the kinematic hardening component of the model. Abaqus offers three different ways of providing data for the kinematic hardening component of the model: the parameters can be specified directly, half-cycle test data can be given, or test data obtained from a stabilized cycle can be given. The experiments required to calibrate the model are described below. and Defining the isotropic hardening component by the exponential law Specify the material parameters of the exponential law , and b directly if they are already calibrated from test data. These parameters can be specified as functions of temperature and/or field variables. , Input File Usage: Abaqus/CAE Usage: *CYCLIC HARDENING, PARAMETERS Property module: material editor: Mechanical→Plasticity→Plastic: Suboptions→Cyclic Hardening: toggle on Use parameters. Defining the isotropic hardening component by tabular data , as a tabular function of the equivalent plastic strain, Isotropic hardening can be introduced by specifying the equivalent stress defining the size of the yield surface, . The simplest way to obtain these data is to conduct a symmetric strain-controlled cyclic experiment with strain range . Since the material’s elastic modulus is large compared to its hardening modulus, this experiment can be interpreted approximately as repeated cycles over the same plastic strain range (using the notation of Figure 23.2.2–7, where E is the Young’s modulus of the material). The equivalent stress defining the size of the yield surface is at zero equivalent plastic strain; for the peak tensile stress points it is obtained by isolating the kinematic component from the yield stress as for each cycle i, where value in each cycle at a particular strain level, corresponding to is . Since the model predicts approximately the same backstress . The equivalent plastic strain εpl εpl Δεpl = εpl εpl − εpl Figure 23.2.2–7 Symmetric strain cycle experiment. , Data pairs ( ), including the value at zero equivalent plastic strain, are specified in tabulated form. The tabulated values defining the size of the yield surface should be provided for the entire equivalent plastic strain range to which the material may be subjected. The data can be provided as functions of temperature and/or field variables. To obtain accurate cyclic hardening data, such as would be needed for low-cycle fatigue calculations, the calibration experiment should be performed at a strain range, , that corresponds to the strain range anticipated in the analysis because the material model does not predict different isotropic hardening behavior at different strain ranges. This limitation also implies that, even though a component is made from the same material, it may have to be divided into several regions with different hardening properties corresponding to different anticipated strain ranges. Field variables and field variable dependence of these properties can also be used for this purpose. Abaqus allows the specification of strain rate effects in the isotropic component of the nonlinear isotropic/kinematic hardening model. The rate-dependent isotropic hardening data can be defined by , as a tabular function of the specifying the equivalent stress defining the size of the yield surface, equivalent plastic strain, , at different values of the equivalent plastic strain rate, . Input File Usage: Abaqus/CAE Usage: Use the following option to define isotropic hardening with tabular data: *CYCLIC HARDENING Use the following option to define rate-dependent isotropic hardening with tabular data: *CYCLIC HARDENING, RATE= Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Combined: Suboptions→Cyclic Hardening Defining the isotropic hardening component in a user subroutine in Abaqus/Standard directly in user subroutine UHARD. Specify may be dependent on equivalent plastic strain and temperature. This method cannot be used if the kinematic hardening component is specified by using half-cycle test data. Input File Usage: Abaqus/CAE Usage: *CYCLIC HARDENING, USER You cannot define the isotropic hardening component in user subroutine UHARD in Abaqus/CAE. Defining the kinematic hardening component by specifying the material parameters directly and can be specified directly as a function of temperature and/or field variables The parameters if they are already calibrated from test data. When depend on temperature and/or field variables, the response of the model under thermomechanical loading will generally depend on the history of temperature and/or field variables experienced at a material point. This dependency on temperature- history is small and fades away with increasing plastic deformation. However, if this effect is not desired, constant values for should be specified to make the material response completely independent of the history of temperature and field variables. The algorithm currently used to integrate the nonlinear isotropic/kinematic hardening model provides accurate solutions if the values of change moderately in an increment due to temperature and/or field variable dependence; however, this algorithm may not yield a solution with sufficient accuracy if the values of change abruptly in an increment. Input File Usage: Abaqus/CAE Usage: *PLASTIC, HARDENING=COMBINED, DATA TYPE=PARAMETERS, NUMBER BACKSTRESSES=n Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Combined, Data type: Parameters, Number of backstresses: n Defining the kinematic hardening component by specifying half-cycle test data can be based on the stress-strain data obtained from the first If limited test data are available, half cycle of a unidirectional tension or compression experiment. An example of such test data is shown in Figure 23.2.2–8. This approach is usually adequate when the simulation will involve only a few cycles of loading. and For each data point ( ) a value of ( is the overall backstress obtained by summing all the backstresses at this data point) is obtained from the test data as where hardening component or the initial yield stress if the isotropic hardening component is not defined. is the user-defined size of the yield surface at the corresponding plastic strain for the isotropic Integration of the backstress evolution laws over a half cycle yields the expressions 3, εpl 1, εpl 2, εpl σ εpl Figure 23.2.2–8 Half cycle of stress-strain data. which are used for calibrating and . , ,..., When test data are given as functions of temperature and/or field variables, Abaqus determines several sets of material parameters ( ), each corresponding to a given combination of , temperature and/or field variables. Generally, this results in temperature-history (and/or field variable- history) dependent material behavior because the values of vary with changes in temperature and/or field variables. This dependency on temperature-history is small and fades away with increasing plastic deformation. However, you can make the response of the material completely independent of the history of temperature and field variables by using constant values for the parameters . This can be achieved by running a data check analysis first; an appropriate constant values of can be determined from the information provided in the data file during the data check. The values for the parameters and the constant parameters can then be entered directly as described above. If the model with multiple backstresses is used, Abaqus obtains hardening parameters for different values of initial guesses and chooses the ones that give the best correlation with the experimental data provided. However, you should carefully examine the obtained parameters. In some cases it might be advantageous to obtain hardening parameters for different numbers of backstresses before choosing the set of parameters. Input File Usage: *PLASTIC, HARDENING=COMBINED, DATA TYPE=HALF CYCLE, NUMBER BACKSTRESSES=n Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Combined, Data type: Half Cycle, Number of backstresses: n Defining the kinematic hardening component by specifying test data from a stabilized cycle Stress-strain data can be obtained from the stabilized cycle of a specimen that is subjected to symmetric strain cycles. A stabilized cycle is obtained by cycling the specimen over a fixed strain range until a steady-state condition is reached; that is, until the stress-strain curve no longer changes shape from one cycle to the next. Such a stabilized cycle is shown in Figure 23.2.2–9. Each data pair ( ) must be specified with the strain axis shifted to , so that and, thus, . Δε pl = ε i − σi − Figure 23.2.2–9 Stress-strain data for a stabilized cycle. For each pair ( ) values of backstresses at this data point) are obtained from the test data as ( is the overall backstress obtained by summing all the where is the stabilized size of the yield surface. Integration of the backstress evolution laws over this uniaxial strain cycle, with an exact match for the first data pair ( ), provides the expressions where above equations enable calibration of the parameters denotes the and . backstress at the first data point (initial value of the backstress). The If the shapes of the stress-strain curves are significantly different for different strain ranges, you may want to obtain several calibrated values of . The tabular data of the stress-strain curves obtained at different strain ranges can be entered directly in Abaqus. Calibrated values corresponding to each strain range are reported in the data file, together with an averaged set of parameters, if model definition data are requested (see “Controlling the amount of analysis input file processor information written to the and , ,..., data file” in “Output,” Section 4.1.1). Abaqus will use the averaged set in the analysis. These parameters may have to be adjusted to improve the match to the test data at the strain range anticipated in the analysis. When test data are given as functions of temperature and/or field variables, Abaqus determines several sets of material parameters ( ), each corresponding to a given combination of , temperature and/or field variables. Generally, this results in temperature-history (and/or field variable- history) dependent material behavior because the values of vary with changes in temperature and/or field variables. This dependency on temperature-history is small and fades away with increasing plastic deformation. However, you can make the response of the material completely independent of the history of temperature and field variables by using constant values for the parameters . This can be achieved by running a data check analysis first; an appropriate constant values of can be determined from the information provided in the data file during the data check. The values for the parameters and the constant parameters can then be entered directly as described above. If the model with multiple backstresses is used, Abaqus obtains hardening parameters for different values of initial guesses and chooses the ones that give the best correlation with the experimental data provided. However, you should carefully examine the obtained parameters. In some cases it might be advantageous to obtain hardening parameters for different numbers of backstresses before choosing the set of parameters. The isotropic hardening component should be defined by specifying the equivalent stress defining the size of the yield surface at zero plastic strain, as well as the evolution of the equivalent stress as a function of equivalent plastic strain. If this component is not defined, Abaqus will assume that no cyclic hardening occurs so that the equivalent stress defining the size of the yield surface is constant and equal to (or the average of these quantities over several strain ranges when more than one strain range is provided). Since this size corresponds to the size of a saturated cycle, this is unlikely to provide accurate predictions of actual behavior, particularly in the initial cycles. Input File Usage: *PLASTIC, HARDENING=COMBINED, DATA TYPE=STABILIZED, NUMBER BACKSTRESSES=n Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Combined, Data type: Stabilized, Number of backstresses: n Initial conditions When we need to study the behavior of a material that has already been subjected to some hardening, Abaqus allows you to prescribe initial conditions for the equivalent plastic strain, , and for the backstresses, . When the nonlinear isotropic/kinematic hardening model is used, the initial conditions for each backstress, , must satisfy the condition for the model to produce a kinematic hardening response. Abaqus allows the specification of initial backstresses that violate these conditions. However, in this case the response corresponding to the backstress for which the condition is violated produces kinematic softening response: the magnitude of the backstress decreases with plastic straining from its initial value to the saturation value. If the condition is violated for any of the backstresses, the overall response of the material is not guaranteed to produce kinematic hardening response. The initial condition for the backstress has no limitations when the linear kinematic hardening model is used. You can specify the initial values of directly as initial conditions . Input File Usage: *INITIAL CONDITIONS, TYPE=HARDENING, NUMBER BACKSTRESSES=n Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Number of backstresses: n User subroutine specification in Abaqus/Standard For more complicated cases in Abaqus/Standard initial conditions can be defined through user subroutine HARDINI. Input File Usage: *INITIAL CONDITIONS, TYPE=HARDENING, USER, NUMBER BACKSTRESSES=n Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined, Number of backstresses: n Elements These models can be used with elements in Abaqus/Standard that include mechanical behavior (elements that have displacement degrees of freedom), except some beam elements in space. Beam elements in space that include shear stress caused by torsion (i.e., not thin-walled, open sections) and do not include hoop stress (i.e., not PIPE elements) cannot be used. In Abaqus/Explicit the kinematic hardening models can be used with any elements that include mechanical behavior, with the exception of one-dimensional elements (beams, pipes, and trusses) when the models are used with the Hill yield surface. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for the kinematic hardening models: Total kinematic hardening shift tensor components, kinematic hardening shift tensor components ( . ). All tensor components of all the kinematic hardening shift tensors, except the total shift tensor. Equivalent plastic strain, equivalent plastic strain (zero or user-specified; see “Initial conditions”). is the initial where 23.2.2–15 ALPHA ALPHAk ALPHAN PENER Plastic work, defined as: . This quantity is not guaranteed to be monotonically increasing for kinematic hardening models. To get a quantity that is monotonically increasing, the plastic dissipation needs to be computed as: . In Abaqus/Standard this quantity can be computed as a user-defined output variable in user subroutine UVARM. 23.2.3 RATE-DEPENDENT YIELD Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Classical metal plasticity,” Section 23.2.1 • “Models for metals subjected to cyclic loading,” Section 23.2.2 • “Johnson-Cook plasticity,” Section 23.2.7 • “Extended Drucker-Prager models,” Section 23.3.1 • “Crushable foam plasticity models,” Section 23.3.5 • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *RATE DEPENDENT • “Defining rate-dependent yield with yield stress ratios” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Rate-dependent yield: • is needed to define a material’s yield behavior accurately when the yield strength depends on the rate of straining and the anticipated strain rates are significant; • is available only for the isotropic hardening metal plasticity models (Mises and Johnson-Cook), the isotropic component of the nonlinear isotropic/kinematic plasticity models, the extended Drucker- Prager plasticity model, and the crushable foam plasticity model; • can be conveniently defined on the basis of work hardening parameters and field variables by providing tabular data for the isotropic hardening metal plasticity models, the isotropic component of the nonlinear isotropic/kinematic plasticity models, and the extended Drucker-Prager plasticity model; • can be defined through specification of user-defined overstress power law parameters, yield stress ratios, or Johnson-Cook rate dependence parameters (this last option is not available for the crushable foam plasticity model and is the only option available for the Johnson-Cook plasticity model); • cannot be used with any of the Abaqus/Standard creep models (metal creep, time-dependent volumetric swelling, Drucker-Prager creep, or cap creep) since creep behavior is already a rate-dependent mechanism; and • in dynamic analysis should be specified such that the yield stress increases with increasing strain rate. Work hardening dependencies Generally, a material’s yield stress, for the crushable foam model), is dependent on work hardening, which for isotropic hardening models is usually represented by a suitable measure of equivalent plastic strain, ; and predefined field variables, ; the inelastic strain rate, ; temperature, (or : Many materials show an increase in their yield strength as strain rates increase; this effect becomes important in many metals and polymers when the strain rates range between 0.1 and 1 per second, and it can be very important for strain rates ranging between 10 and 100 per second, which are characteristic of high-energy dynamic events or manufacturing processes. Defining hardening dependencies for various material models Strain rate dependence can be defined by entering hardening curves at different strain rates directly or by defining yield stress ratios to specify the rate dependence independently. Direct entry of test data Work hardening dependencies can be given quite generally as tabular data for the isotropic hardening Mises plasticity model, the isotropic component of the nonlinear isotropic/kinematic hardening model, and the extended Drucker-Prager plasticity model. The test data are entered as tables of yield stress values versus equivalent plastic strain at different equivalent plastic strain rates. The yield stress must be given as a function of the equivalent plastic strain and, if required, of temperature and of other predefined field variables. In defining this dependence at finite strains, “true” (Cauchy) stress and log strain values should be used. The hardening curve at each temperature must always start at zero plastic strain. For perfect plasticity only one yield stress, with zero plastic strain, should be defined at each temperature. It is possible to define the material to be strain softening as well as strain hardening. The work hardening data are repeated as often as needed to define stress-strain curves at different strain rates. The yield stress at a given strain and strain rate is interpolated directly from these tables. Input File Usage: Use one of the following options: *PLASTIC, HARDENING=ISOTROPIC, RATE= *CYCLIC HARDENING, RATE= *DRUCKER PRAGER HARDENING, RATE= Use one of the following models: Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Isotropic, Use strain-rate-dependent data Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker Prager Hardening: Use strain-rate-dependent data Cyclic hardening is not supported in Abaqus/CAE. Using yield stress ratios Alternatively, and as the only means of defining rate-dependent yield stress for the Johnson-Cook and the crushable foam plasticity models, the strain rate behavior can be assumed to be separable, so that the stress-strain dependence is similar at all strain rate levels: where (or in the foam model) is the static stress-strain behavior and is the ratio of the yield stress at nonzero strain rate to the static yield stress (so that ). Three methods are offered to define R in Abaqus: specifying an overstress power law, defining R directly as a tabular function, or specifying an analytical Johnson-Cook form to define R. Overstress power law The Cowper-Symonds overstress power law has the form where and of other predefined field variables. are material parameters that can be functions of temperature and, possibly, Input File Usage: Abaqus/CAE Usage: *RATE DEPENDENT, TYPE=POWER LAW Property module: material editor: Suboptions→Rate Dependent: Hardening: Power Law (available for valid plasticity models) Tabular function Alternatively, R can be entered directly as a tabular function of the equivalent plastic strain rate (or the axial plastic strain rate in a uniaxial compression test for the crushable foam model), ; temperature, ; and field variables, . Input File Usage: Abaqus/CAE Usage: *RATE DEPENDENT, TYPE=YIELD RATIO Property module: material editor: Suboptions→Rate Dependent: Hardening: Yield Ratio (available for valid plasticity models) Johnson-Cook rate dependence Johnson-Cook rate dependence has the form where and C are material constants that do not depend on temperature and are assumed not to depend on predefined field variables. Johnson-Cook rate dependence can be used in conjunction with the Johnson-Cook plasticity model, the isotropic hardening metal plasticity models, and the extended Drucker-Prager plasticity model (it cannot be used in conjunction with the crushable foam plasticity model). This is the only form of rate dependence available for the Johnson-Cook plasticity model. For more details, see “Johnson-Cook plasticity,” Section 23.2.7. Input File Usage: Abaqus/CAE Usage: *RATE DEPENDENT, TYPE=JOHNSON COOK Property module: material editor: Suboptions→Rate Dependent: Hardening: Johnson-Cook (available for valid plasticity models) Elements Rate-dependent yield can be used with all elements that include mechanical behavior (elements that have displacement degrees of freedom). 23.2.4 RATE-DEPENDENT PLASTICITY: CREEP AND SWELLING Products: Abaqus/Standard Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6 • *CREEP • *CREEP STRAIN RATE CONTROL • *POTENTIAL • *SWELLING • *RATIOS • “Defining a creep law” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining swelling” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The classical deviatoric metal creep behavior in Abaqus/Standard: • can be defined using user subroutine CREEP or by providing parameters as input for some simple creep laws; • can model either isotropic creep (using Mises stress potential) or anisotropic creep (using Hill’s anisotropic stress potential); • is active only during steps using the coupled temperature-displacement procedure, the transient soils consolidation procedure, and the quasi-static procedure; • requires that the material’s elasticity be defined as linear elastic behavior; • can be modified to implement the auxiliary creep hardening rules specified in Nuclear Standard NEF 9-5T, “Guidelines and Procedures for Design of Class 1 Elevated Temperature Nuclear System Components”; these rules are exercised by means of a constitutive model developed by Oak Ridge National Laboratory (“ORNL – Oak Ridge National Laboratory constitutive model,” Section 23.2.12); • can be used in combination with creep strain rate control in analyses in which the creep strain rate must be kept within a certain range; and • can potentially result in errors in calculated creep strains if anisotropic creep and plasticity occur simultaneously (discussed below). Rate-dependent gasket behavior in Abaqus/Standard: • uses unidirectional creep as part of the model of the gasket’s thickness-direction behavior; • can be defined using user subroutine CREEP or by providing parameters as input for some simple creep laws; • is active only during steps using the quasi-static procedure; and • requires that an elastic-plastic model be used to define the rate-independent part of the thickness- direction behavior of the gasket. Volumetric swelling behavior in Abaqus/Standard: • can be defined using user subroutine CREEP or by providing tabular input; • can be either isotropic or anisotropic; • is active only during steps using the coupled temperature-displacement procedure, the transient soils consolidation procedure, and the quasi-static procedure; and • requires that the material’s elasticity be defined as linear elastic behavior. Creep behavior Creep behavior is specified by the equivalent uniaxial behavior—the creep “law.” In practical cases creep laws are typically of very complex form to fit experimental data; therefore, the laws are defined with user subroutine CREEP, as discussed below. Alternatively, two common creep laws are provided in Abaqus/Standard: the power law and the hyperbolic-sine law models. These standard creep laws are used for modeling secondary or steady-state creep. Creep is defined by including creep behavior in the material model definition (“Material data definition,” Section 21.1.2). Alternatively, creep can be defined in conjunction with gasket behavior to define the rate-dependent behavior of a gasket. Input File Usage: Use the following options to include creep behavior in the material model definition: *MATERIAL *CREEP Use the following options to define creep in conjunction with gasket behavior: *GASKET BEHAVIOR *CREEP Property module: material editor: Mechanical→Plasticity→Creep Abaqus/CAE Usage: Choosing a creep model The power-law creep model is attractive for its simplicity. However, it is limited in its range of application. The time-hardening version of the power-law creep model is typically recommended only in cases when the stress state remains essentially constant. The strain-hardening version of power-law creep should be used when the stress state varies during an analysis. In the case where the stress is constant and there are no temperature and/or field dependencies, the time-hardening and the stresses should be relatively low. CREEP AND SWELLING In regions of high stress, such as around a crack tip, the creep strain rates frequently show an exponential dependence of stress. The hyperbolic-sine creep law shows exponential dependence on the stress, is the yield stress) and reduces to the power-law at low stress levels (with no explicit time dependence). , at high stress levels ( , where None of the above models is suitable for modeling creep under cyclic loading. The ORNL model (“ORNL – Oak Ridge National Laboratory constitutive model,” Section 23.2.12) is an empirical model for stainless steel that gives approximate results for cyclic loading without having to perform the cyclic loading numerically. Generally, creep models for cyclic loading are complicated and must be added to a model with user subroutine CREEP or with user subroutine UMAT. Modeling simultaneous creep and plasticity If creep and plasticity occur simultaneously and implicit creep integration is in effect, both behaviors may interact and a coupled system of constitutive equations needs to be solved. If creep and plasticity are isotropic, Abaqus/Standard properly takes into account such coupled behavior, even if the elasticity is anisotropic. However, if creep and plasticity are anisotropic, Abaqus/Standard integrates the creep equations without taking plasticity into account, which may lead to substantial errors in the creep strains. This situation develops only if plasticity and creep are active at the same time, such as would occur during a long-term load increase; one would not expect to have a problem if there is a short-term preloading phase in which plasticity dominates, followed by a creeping phase in which no further yielding occurs. Integration of the creep laws and rate-dependent plasticity are discussed in “Rate-dependent metal plasticity (creep),” Section 4.3.4 of the Abaqus Theory Manual. Power-law model The power-law model can be used in its “time hardening” form or in the corresponding “strain hardening” form. Time hardening form The “time hardening” form is the simpler of the two forms of the power-law model: where A, n, and m is the uniaxial equivalent creep strain rate, is the uniaxial equivalent deviatoric stress, is the total time, and are defined by you as functions of temperature. is Mises equivalent stress or Hill’s anisotropic equivalent deviatoric stress according to whether isotropic or anisotropic creep behavior is defined (discussed below). For physically reasonable behavior A and n must be positive and . Since total time is used in the expression, such reasonable behavior also typically requires that small step times compared to the creep time be used for any steps for which creep is not active in an analysis; this is necessary to avoid changes in hardening behavior in subsequent steps. Input File Usage: Abaqus/CAE Usage: *CREEP, LAW=TIME Property module: material editor: Mechanical→Plasticity→Creep: Law: Time-Hardening Strain hardening form The “strain hardening” form of the power law is where and are defined above and is the equivalent creep strain. Input File Usage: Abaqus/CAE Usage: *CREEP, LAW=STRAIN Property module: material editor: Mechanical→Plasticity→Creep: Law: Strain-Hardening Numerical difficulties Depending on the choice of units for either form of the power law, the value of A may be very small for typical creep strain rates. If A is less than 10−27 , numerical difficulties can cause errors in the material calculations; therefore, use another system of units to avoid such difficulties in the calculation of creep strain increments. Hyperbolic-sine law model The hyperbolic-sine law is available in the form where and A, B, and n are defined above, is the temperature, is the user-defined value of absolute zero on the temperature scale used, is the activation energy, is the universal gas constant, and are other material parameters. This model includes temperature dependence, which is apparent in the above expression; however, the parameters A, B, n, , and R cannot be defined as functions of temperature. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *CREEP, LAW=HYPERB *PHYSICAL CONSTANTS, ABSOLUTE ZERO= Define both of the following: Property module: material editor: Mechanical→Plasticity→Creep: Law: Hyperbolic-Sine Any module: Model→Edit Attributes→model_name: Absolute zero temperature Numerical difficulties As with the power law, A may be very small for typical creep strain rates. If A is very small (such as less than 10−27), use another system of units to avoid numerical difficulties in the calculation of creep strain increments. Anisotropic creep Anisotropic creep can be defined to specify the stress ratios that appear in Hill’s function. You must define the ratios in each direction that will be used to scale the stress value when the creep strain rate is calculated. The ratios can be defined as constant or dependent on temperature and other predefined field variables. The ratios are defined with respect to the user-defined local material directions or the default directions . Further details are provided in “Anisotropic yield/creep,” Section 23.2.6. Anisotropic creep is not available when creep is used to define a rate-dependent gasket behavior since only the gasket thickness-direction behavior can have rate-dependent behavior. Input File Usage: Abaqus/CAE Usage: *POTENTIAL Property module: material editor: Mechanical→Plasticity→Creep: Suboptions→Potential Volumetric swelling behavior As with the creep laws, volumetric swelling laws are usually complex and are most conveniently specified in user subroutine CREEP as discussed below. However, a means of tabular input is also provided for the form where are predefined fields such as irradiation fluxes in cases involving nuclear radiation effects. Up to six predefined fields can be specified. is the volumetric strain rate caused by swelling and , , Volumetric swelling cannot be used to define a rate-dependent gasket behavior. Input File Usage: Abaqus/CAE Usage: *SWELLING Property module: material editor: Mechanical→Plasticity→Swelling Anisotropic swelling Anisotropy can easily be included in the swelling behavior. If anisotropic swelling behavior is defined, the anisotropic swelling strain rate is expressed as is the volumetric swelling strain rate that you define either directly (discussed above) or in user where subroutine CREEP. The ratios are also user-defined. The directions of the components of the swelling strain rate are defined by the local material directions, which can be either user-defined or the default directions . , and , Input File Usage: Use both of the following options: *SWELLING *RATIOS Property module: material editor: Mechanical→Plasticity→Swelling: Suboptions→Ratios Abaqus/CAE Usage: User subroutine CREEP User subroutine CREEP provides a very general capability for implementing viscoplastic models such as creep and swelling models in which the strain rate potential can be written as a function of equivalent pressure stress, p; the Mises or Hill’s equivalent deviatoric stress, ; and any number of solution-dependent state variables. Solution-dependent state variables are used in conjunction with the constitutive definition; their values evolve with the solution and can be defined in this subroutine. Examples are hardening variables associated with the model. The user subroutine can also be used to define very general rate- and time-dependent thickness- direction gasket behavior. When an even more general form is required for the strain rate potential, user subroutine UMAT (“User-defined mechanical material behavior,” Section 26.7.1) can be used. Input File Usage: Use one or both of the following options. Only the first option can be used to define gasket behavior. Abaqus/CAE Usage: *CREEP, LAW=USER *SWELLING, LAW=USER Use one or both of the following models. Only the first model can be used to define gasket behavior. Property module: material editor: Mechanical→Plasticity→Creep: Law: User defined Mechanical→Plasticity→Swelling: Law: User subroutine CREEP Removing creep effects in an analysis step You can specify that no creep (or viscoelastic) response can occur during certain analysis steps, even if creep (or viscoelastic) material properties have been defined. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *COUPLED TEMPERATURE-DISPLACEMENT, CREEP=NONE *SOILS, CONSOLIDATION, CREEP=NONE Use one of the following options: Step module: Create Step: Coupled temp-displacement: toggle off Include creep/swelling/ viscoelastic behavior Soils: Pore fluid response: Transient consolidation: toggle off Include creep/swelling/viscoelastic behavior Integration Explicit integration, implicit integration, or both integration schemes can be used in a creep analysis, depending on the procedure used, the parameters specified for the procedure, the presence of plasticity, and whether or not geometric nonlinearity is requested. Application of explicit and implicit schemes Nonlinear creep problems are often solved efficiently by forward-difference integration of the inelastic strains (the “initial strain” method). This explicit method is computationally efficient because, unlike implicit methods, iteration is not required. Although this method is only conditionally stable, the numerical stability limit of the explicit operator is usually sufficiently large to allow the solution to be developed in a small number of time increments. Abaqus/Standard uses either an explicit or an implicit integration scheme or switches from explicit to implicit in the same step. These schemes are outlined first, followed by a description of which procedures use these integration schemes. 1. Integration scheme 1: Starts with explicit integration and switches to implicit integration based on either stability or if plasticity is active. The stability limit used in explicit integration is discussed in the next section. 2. Integration scheme 2: Starts with explicit integration and switches to implicit integration when plasticity is active. The stability criterion does not play a role here. 3. Integration scheme 3: Always uses implicit integration. The use of the above integration schemes is determined by the procedure type, your choice of the integration type to be used, as well as whether or not geometric nonlinearity is requested. For quasi-static and coupled temperature-displacement procedures, if you do not choose an integration type, integration scheme 1 is used for a geometrically linear analysis and integration scheme 3 is used for a geometrically nonlinear analysis. You can force Abaqus/Standard to use explicit integration for creep and swelling effects in coupled temperature-displacement or quasi-static procedures, when plasticity is not active throughout the step (integration scheme 2). Explicit integration can be used regardless of whether or not geometric nonlinearity has been requested . For a transient soils consolidation procedure, the implicit integration scheme (integration scheme 3) is always used, irrespective of whether a geometrically linear or nonlinear analysis is performed. Input File Usage: Abaqus/CAE Usage: Use one of the following options to restrict Abaqus/Standard to using explicit integration: *VISCO, CREEP=EXPLICIT *COUPLED TEMPERATURE-DISPLACEMENT, CREEP=EXPLICIT Use one of the following options to restrict Abaqus/Standard to using explicit integration: Step module: Create Step: Visco: Incrementation: Creep/swelling/viscoelastic integration: Explicit Coupled temp-displacement: toggle on Include creep/swelling/ viscoelastic behavior: Incrementation: Creep/swelling/viscoelastic integration: Explicit Automatic monitoring of stability limit during explicit integration Abaqus/Standard monitors the stability limit automatically during explicit integration. If, at any point in the model, the creep strain increment is larger than the total elastic strain, the problem will become unstable. Therefore, a stable time step, , is calculated every increment by where equivalent creep strain rate at time t. Furthermore, is the equivalent total elastic strain at time t, the beginning of the increment, and is the where is the Mises stress at time t, and where is the gradient of the deviatoric stress potential, is the elasticity matrix, and is an effective elastic modulus—for isotropic elasticity by Young’s modulus. can be approximated , is compared to the critical time increment, , which is calculated as follows: CREEP AND SWELLING The quantity errtol is an error tolerance that you define as discussed below. If is used as the time increment, which would mean that the stability criterion was limiting the size of the time step further than required by accuracy considerations. Abaqus/Standard will automatically switch to the backward difference operator (the implicit method, which is unconditionally stable) if is less than for nine consecutive increments, you have not restricted Abaqus/Standard to explicit integration as ). The stiffness matrix discussed above, and there is sufficient time left in the analysis (time left will be reformed at every iteration if the implicit algorithm is used. is less than , Specifying the tolerance for automatic incrementation The integration tolerance must be chosen so that increments in stress, Consider a one-dimensional example. The stress increment, , is , are calculated accurately. where E is the elastic modulus. For , and are the uniaxial elastic, total, and creep strain increments, respectively, and to be calculated accurately, the error in the creep strain increment, , , must be small compared to ; that is, Measuring the error in as leads to You define errtol for the applicable procedure by choosing an acceptable stress error tolerance and dividing this by a typical elastic modulus; therefore, it should be a small fraction of the ratio of the typical stress and the effective elastic modulus in a problem. It is important to recognize that this approach for selecting a value for errtol is often very conservative, and acceptable solutions can usually be obtained with higher values. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *VISCO, CETOL=errtol *COUPLED TEMPERATURE-DISPLACEMENT, CETOL=errtol *SOILS, CONSOLIDATION, CETOL=errtol Use one of the following options: Step module: Create Step: Visco: Incrementation: toggle on Creep/swelling/viscoelastic strain error tolerance, and enter a value Coupled temp-displacement: toggle on Include creep/swelling/ viscoelastic behavior: Incrementation: toggle on Creep/swelling/ viscoelastic strain error tolerance, and enter a value Soils: Pore fluid response: Transient consolidation: toggle on Include creep/swelling/viscoelastic behavior: Incrementation: toggle on Creep/swelling/viscoelastic strain error tolerance, and enter a value Loading control using creep strain rate In superplastic forming a controllable pressure is applied to deform a body. Superplastic materials can deform to very large strains, provided that the strain rates of the deformation are maintained within very tight tolerances. The objective of the superplastic analysis is to predict how the pressure must be controlled to form the component as fast as possible without exceeding a superplastic strain rate anywhere in the material. To achieve this using Abaqus/Standard, the controlling algorithm is as follows. During an increment Abaqus/Standard calculates , the maximum value of the ratio of the equivalent creep strain rate to the target creep strain rate for any integration point in a specified element set. If is less than 0.2 or greater than 3.0 in a given increment, the increment is abandoned and restarted with the following load modifications: or where p is the new load magnitude and , the increment is accepted; and at the beginning of the following time increment, the load magnitudes are modified as follows: is the old load magnitude. If When you activate the above algorithm, the loading in a creep and/or swelling problem can be controlled on the basis of the maximum equivalent creep strain rate found in a defined element set. As or a minimum requirement, this method is used to define a target equivalent creep strain rate; however, if required, it can also be used to define the target creep strain rate as a function of equivalent creep strain (measured as log strain), temperature, and other predefined field variables. The creep strain dependency curve at each temperature must always start at zero equivalent creep strain. A solution-dependent amplitude is used to define the minimum and maximum limits of the loading . Any number or combination of loads can be used. The current value of is available for output as discussed below. Input File Usage: Use all of the following options: *AMPLITUDE, NAME=name, DEFINITION=SOLUTION DEPENDENT *CLOAD, *DLOAD, *DSLOAD, and/or *BOUNDARY with AMPLITUDE=name *CREEP STRAIN RATE CONTROL, AMPLITUDE=name, ELSET=elset The *AMPLITUDE option must appear in the model definition portion of an input file, while the loading options (*CLOAD, *DLOAD, *DSLOAD, and *BOUNDARY) and the *CREEP STRAIN RATE CONTROL option should appear in each relevant step definition. Abaqus/CAE Usage: Creep strain rate control is not supported in Abaqus/CAE. Elements Rate-dependent plasticity (creep and swelling behavior) can be used with any continuum, shell, membrane, gasket, and beam element in Abaqus/Standard that has displacement degrees of freedom. Creep (but not swelling) can also be defined in the thickness direction of any gasket element in conjunction with the gasket behavior definition. Output In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables relate directly to creep and swelling models: CEEQ CESW Equivalent creep strain, . Magnitude of swelling strain. The following output, which is relevant only for an analysis with creep strain rate loading control as discussed above, is printed at the beginning of an increment and is written automatically to the results file and output database file when any output to these files is requested: RATIO Maximum value of the ratio of the equivalent creep strain rate to the target creep strain rate, . AMPCU Current value of the solution-dependent amplitude. 23.2.5 ANNEALING OR MELTING Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • *ANNEAL TEMPERATURE • “Specifying the annealing temperature of an elastic-plastic material” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview This capability: • is intended to model the effects of melting and resolidification in metals subjected to high-temperature processes or the effects of annealing at a material point when its temperature rises above a certain level; • is available for only the Mises, Johnson-Cook, and Hill plasticity models; • is intended to be used in conjunction with appropriate temperature-dependent material properties (in particular, the model assumes perfectly plastic behavior at or above the annealing or melting temperature); and • can be modeled simply by defining an annealing or melting temperature. Effects of annealing or melting When the temperature of a material point exceeds a user-specified value called the annealing temperature, Abaqus assumes that the material point loses its hardening memory. The effect of prior work hardening is removed by setting the equivalent plastic strain to zero. For kinematic and combined hardening models the backstress tensor is also reset to zero. If the temperature of the material point falls below the annealing temperature at a subsequent point in time, the material point can work harden again. Depending on the temperature history a material point may lose and accumulate memory several times, which in the context of modeling melting would correspond to repeated melting and resolidification. Any accumulated material damage is not healed when the annealing temperature is reached. Damage will continue to accumulate after annealing according to any damage model in effect . In Abaqus/Explicit an annealing step can be defined to simulate the annealing process for the entire model, independent of temperature; see “Annealing procedure,” Section 6.12.1, for details. Material properties The annealing temperature is a material property that can optionally be defined as a function of field variables. This material property must be used in conjunction with an appropriate definition of material properties as functions of temperature for the Mises plasticity model. In particular, the hardening behavior must be defined as a function of temperature and zero hardening must be specified at or above the annealing temperature. In general, hardening receives contributions from two sources. The first source of hardening can be classified broadly as static, and its effect is measured by the rate of change of the yield stress with respect to the plastic strain at a fixed strain rate. The second source of hardening can be classified broadly as rate dependent, and its effect is measured by the rate of change of the yield stress with respect to the strain rate at a fixed plastic strain. For the Mises plasticity model, if the material data that describe hardening (both static and rate- dependent contributions) are completely specified through tabular input of yield stress versus plastic strain at different values of the strain rate , the (temperature- dependent) static part of the hardening at each strain rate is specified by defining several yield stress versus plastic strain curves (each at a different temperature). For metals the yield stress at a fixed strain rate typically decreases with increasing temperature. Abaqus expects the hardening at each strain rate to vanish at or above the annealing temperature and issues an error message if you specify otherwise in the material definition. Zero (static) hardening can be specified by simply specifying a single data point (at zero plastic strain) in the yield stress versus plastic strain curve at or above the annealing temperature. In addition, you must also ensure that at or above the annealing temperature, the yield stress does not vary with the strain rate. This can be accomplished by specifying the same value of yield stress at all values of strain rate in the single data point approach discussed above. Alternatively, the static part of the hardening can be defined at zero strain rate, and the rate-dependent part can be defined utilizing the overstress power law . In that case, zero static hardening at or above the annealing temperature can be specified by specifying a single data point (at zero plastic strain) in the yield stress versus plastic strain curve at or above the annealing temperature. The overstress power law parameters can also be appropriately selected to ensure that at or above the annealing temperature the yield stress does not vary with strain rate. This can be accomplished by selecting a large value for the parameter (relative to the static yield stress) and setting the parameter . For hardening defined in Abaqus/Standard with user subroutine UHARD, Abaqus/Standard checks the hardening slope at or above the annealing temperature during the actual computations and issues an error message if appropriate. The Johnson-Cook plasticity model in Abaqus/Explicit requires a separate melting temperature to define the hardening behavior. If the annealing temperature is defined to be less than the melting temperature specified for the metal plasticity model, the hardening memory is removed at the annealing temperature and the melting temperature is used strictly to define the hardening function. Otherwise, the hardening memory is removed automatically at the melting temperature. Input File Usage: Abaqus/CAE Usage: *ANNEAL TEMPERATURE Property module: material editor: Mechanical→Plasticity→Plastic: Suboptions→Anneal Temperature Example: Annealing or melting The following input is an example of a typical usage of the annealing or melting capability. It is assumed that you have defined the static stress versus plastic strain behavior for the isotropic that the plastic behavior is rate independent. ANNEALING OR MELTING               pl 2 pl 1 pl  Figure 23.2.5–1 Stress versus plastic strain behavior. The plastic response corresponds to linear hardening below the annealing temperature and perfect plasticity at the annealing temperature. The elastic properties, which may also be temperature dependent, are not shown. Plasticity Data, Isotropic Hardening: Yield Stress Plastic Strain Temperature Anneal Temperature: Elements This capability can be used with all elements that include mechanical behavior (elements that have displacement degrees of freedom). Output Only the equivalent plastic strain (output variable PEEQ) and the backstress (output variable ALPHA) are reset to zero at the melting temperature. The plastic strain tensor (output variable PE) is not reset to zero and provides a measure of the total plastic deformation during the analysis. In Abaqus/Standard the plastic strain tensor also provides a measure of the plastic strain magnitude (output variable PEMAG). 23.2.6 ANISOTROPIC YIELD/CREEP Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • “Classical metal plasticity,” Section 23.2.1 • “Models for metals subjected to cyclic loading,” Section 23.2.2 • “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 • *POTENTIAL • “Defining anisotropic yield and creep” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Anisotropic yield and/or creep: • can be used for materials that exhibit different yield and/or creep behavior in different directions; • is introduced through user-defined stress ratios that are applied in Hill’s potential function; • can be used only in conjunction with the metal plasticity and, in Abaqus/Standard, the metal creep material models; • is available for the nonlinear isotropic/kinematic hardening model in Abaqus/Explicit (“Models for metals subjected to cyclic loading,” Section 23.2.2); and • can be used in conjunction with the models of progressive damage and failure in Abaqus/Explicit (“Damage and failure for ductile metals: overview,” Section 24.2.1) to specify different damage initiation criteria and damage evolution laws that allow for the progressive degradation of the material stiffness and the removal of elements from the mesh. Yield and creep stress ratios Anisotropic yield or creep behavior is modeled through the use of yield or creep stress ratios, case of anisotropic yield the yield ratios are defined with respect to a reference yield stress, the metal plasticity definition), such that if yield stress is . In the (given for is applied as the only nonzero stress, the corresponding . The plastic flow rule is defined below. In the case of anisotropic creep the creep strain rate is calculated. Thus, if user-defined creep law is . are creep ratios used to scale the stress value when the , used in the is the only nonzero stress, the equivalent stress, Yield and creep stress ratios can be defined as constants or as tabular functions of temperature and predefined field variables. A local orientation must be used to define the direction of anisotropy . Input File Usage: Use the following option to define the yield or creep stress ratios: *POTENTIAL This option must appear immediately after the *PLASTIC or the *CREEP material option data to which it applies. Thus, if anisotropic metal plasticity and anisotropic creep behavior are both required, the *POTENTIAL option must appear twice in the material definition, once after the metal plasticity data and again after the creep data. Abaqus/CAE Usage: Use one of the following models: Property module: material editor: Mechanical→Plasticity→Plastic: Suboptions→Potential Mechanical→Plasticity→Creep: Suboptions→Potential Anisotropic yield Hill’s potential function is a simple extension of the Mises function, which can be expressed in terms of rectangular Cartesian stress components as where are defined as and N are constants obtained by tests of the material in different orientations. They where each component; , , , is the measured yield stress value when is applied as the only nonzero stress is the user-defined reference yield stress specified for the metal plasticity definition; . The six yield are anisotropic yield stress ratios; and , and , stress ratios are, therefore, defined as follows (in the order in which you must provide them): Because of the form of the yield function, all of these ratios must be positive. If the constants F, G, and H are positive, the yield function is always well-defined. However, if one or more of these constants is negative, the yield function may be undefined for some stress states because the quantity under the square root is negative. The flow rule is where, from the definition of f above, Input File Usage: Abaqus/CAE Usage: Use both of the following options: *PLASTIC *POTENTIAL Property module: material editor: Mechanical→Plasticity→Plastic: Suboptions→Potential Anisotropic creep For anisotropic creep in Abaqus/Standard Hill’s function can be expressed as is the equivalent stress and F, G, H, L, M, and N are constants obtained by tests of the where material in different orientations. The constants are defined with the same general relations as those used for anisotropic yield (above); however, the reference yield stress, , is replaced by the uniaxial equivalent deviatoric stress, are referred (found in the creep law), and , and , , , , to as “anisotropic creep stress ratios.” The six creep stress ratios are, therefore, defined as follows (in the order in which they must be provided): You must define the ratios strain rate is calculated. If all six in each direction that will be used to scale the stress value when the creep values are set to unity, isotropic creep is obtained. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *CREEP *POTENTIAL Property module: material editor: Mechanical→Plasticity→Creep: Suboptions→Potential Defining anisotropic yield behavior on the basis of strain ratios (Lankford’s r-values) As discussed above, Hill’s anisotropic plasticity potential is defined in Abaqus from user input consisting of ratios of yield stress in different directions with respect to a reference stress. However, in some cases, such as sheet metal forming applications, it is common to find the anisotropic material data given in terms of ratios of width strain to thickness strain. Mathematical relationships are then necessary to convert the strain ratios to stress ratios that can be input into Abaqus. In sheet metal forming applications we are generally concerned with plane stress conditions. Consider to be the “rolling” and “cross” directions in the plane of the sheet; z is the thickness direction. From a design viewpoint, the type of anisotropy usually desired is that in which the sheet is isotropic in the plane and has an increased strength in the thickness direction, which is normally referred to as transverse anisotropy. Another type of anisotropy is characterized by different strengths in different directions in the plane of the sheet, which is called planar anisotropy. In a simple tension test performed in the x-direction in the plane of the sheet, the flow rule for this potential (given above) defines the incremental strain ratios (assuming small elastic strains) as Therefore, the ratio of width to thickness strain, often referred to as Lankford’s r-value, is Similarly, for a simple tension test performed in the y-direction in the plane of the sheet, the incremental strain ratios are and Transverse anisotropy A transversely anisotropic material is one where to be equal to , . If we define in the metal plasticity model and, using the relationships above, If (isotropic material), and the Mises isotropic plasticity model is recovered. Planar anisotropy In the case of planar anisotropy define in the metal plasticity model to be equal to , and are different and will all be different. If we and, using the relationships above, we obtain Again, if , and the Mises isotropic plasticity model is recovered. General anisotropy Thus far, we have only considered loading applied along the axes of anisotropy. To derive a more general anisotropic model in plane stress, the sheet must be loaded in one other direction in its plane. Suppose we perform a simple tension test at an angle to the x-direction; then, from equilibrium considerations we can write the nonzero stress components as is the applied tensile stress. Substituting these values in the flow equations and assuming small where elastic strains yields and Assuming small geometrical changes, the width strain increment (the increment of strain at right angles to the direction of loading, ) is written as and Lankford’s r-value for loading at an angle is One of the more commonly performed tests is that in which the loading direction is at 45°. In this case If . transverse or planar anisotropy and, using the relationships above, in the metal plasticity model, is equal to are as defined before for Progressive damage and failure In Abaqus/Explicit anisotropic yield can be used in conjunction with the models of progressive damage and failure discussed in “Damage and failure for ductile metals: overview,” Section 24.2.1. The capability allows for the specification of one or more damage initiation criteria, including ductile, shear, forming limit diagram (FLD), forming limit stress diagram (FLSD), and Müschenborn-Sonne forming limit diagram (MSFLD) criteria. After damage initiation, the material stiffness is degraded progressively according to the specified damage evolution response. The model offers two failure choices, including the removal of elements from the mesh as a result of tearing or ripping of the structure. The progressive damage models allow for a smooth degradation of the material stiffness, making them suitable for both quasi-static and dynamic situations. Input File Usage: Use the following options: *PLASTIC *DAMAGE INITIATION *DAMAGE EVOLUTION Property module: material editor: Mechanical→Damage for Ductile Metals→damage initiation type: specify the damage initiation criterion: Suboptions→Damage Evolution: specify the damage evolution parameters Abaqus/CAE Usage: Initial conditions When we need to study the behavior of a material that has already been subjected to some work hardening, Abaqus allows you to prescribe initial conditions for the equivalent plastic strain, , by specifying the conditions directly (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step User subroutine specification in Abaqus/Standard For more complicated cases, initial conditions can be defined in Abaqus/Standard through user subroutine HARDINI. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING, USER Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined Elements Anisotropic yield can be defined for any element that can be used with the classical metal plasticity models in Abaqus (“Classical metal plasticity,” Section 23.2.1) except one-dimensional elements in Abaqus/Explicit (beams and trusses). In Abaqus/Standard it can also be defined for any element that can be used with the linear kinematic hardening plasticity model (“Models for metals subjected to cyclic loading,” Section 23.2.2) but not with the nonlinear isotropic/kinematic hardening model. Likewise, anisotropic creep can be defined for any element that can be used with the classical metal creep model in Abaqus/Standard (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4). Output The standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2) and all output variables associated with the creep model (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4), classical metal plasticity models (“Classical metal plasticity,” Section 23.2.1), and the linear kinematic hardening plasticity model (“Models for metals subjected to cyclic loading,” Section 23.2.2) are available when anisotropic yield and creep are defined. The following variables have special meaning if anisotropic yield and creep are defined: PEEQ CEEQ is Equivalent plastic strain, the initial equivalent plastic strain (zero or user-specified; see “Initial conditions”). where Equivalent creep strain, 23.2.7 JOHNSON-COOK PLASTICITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Classical metal plasticity,” Section 23.2.1 • “Rate-dependent yield,” Section 23.2.3 • “Equation of state,” Section 25.2.1 • Chapter 24, “Progressive Damage and Failure” • “Dynamic failure models,” Section 23.2.8 • “Annealing or melting,” Section 23.2.5 • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *ANNEAL TEMPERATURE • *PLASTIC • *RATE DEPENDENT • *SHEAR FAILURE • *TENSILE FAILURE • *DAMAGE INITIATION • *DAMAGE EVOLUTION • “Using the Johnson-Cook hardening model to define classical metal plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The Johnson-Cook plasticity model: • is a particular type of Mises plasticity model with analytical forms of the hardening law and rate dependence; • is suitable for high-strain-rate deformation of many materials, including most metals; • is typically used in adiabatic transient dynamic simulations; • can be used in conjunction with the Johnson-Cook dynamic failure model in Abaqus/Explicit; • can be used in conjunction with the tensile failure model to model tensile spall or a pressure cutoff in Abaqus/Explicit; • can be used in conjunction with the progressive damage and failure models (Chapter 24, “Progressive Damage and Failure”) to specify different damage initiation criteria and damage evolution laws that allow for the progressive degradation of the material stiffness and the removal of elements from the mesh; and • must be used in conjunction with either the linear elastic material model (“Linear elastic behavior,” Section 22.2.1) or the equation of state material model (“Equation of state,” Section 25.2.1). Yield surface and flow rule A Mises yield surface with associated flow is used in the Johnson-Cook plasticity model. Johnson-Cook hardening Johnson-Cook hardening is a particular type of isotropic hardening where the static yield stress, assumed to be of the form , is where the transition temperature, is the equivalent plastic strain and A, B, n and m are material parameters measured at or below . is the nondimensional temperature defined as is the current temperature, where is the transition temperature defined as the one at or below which there is no temperature dependence on the expression of the yield stress. The material parameters must be measured at or below the transition temperature. is the melting temperature, and When resistance since to zero. If backstresses are specified for the model, these will also be set to zero. , the material will be melted and will behave like a fluid; there will be no shear . The hardening memory will be removed by setting the equivalent plastic strain If you include annealing behavior in the material definition and the annealing temperature is defined to be less than the melting temperature specified for the metal plasticity model, the hardening memory will be removed at the annealing temperature and the melting temperature will be used strictly to define the hardening function. Otherwise, the hardening memory will be removed automatically at the melting temperature. If the temperature of the material point falls below the annealing temperature at a subsequent point in time, the material point can work harden again. For more details, see “Annealing or melting,” Section 23.2.5. You provide the values of A, B, n, m, , and as part of the metal plasticity material definition. Input File Usage: Abaqus/CAE Usage: *PLASTIC, HARDENING=JOHNSON COOK Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Johnson-Cook Johnson-Cook strain rate dependence Johnson-Cook strain rate dependence assumes that and where is the yield stress at nonzero strain rate; and C is the equivalent plastic strain rate; are material parameters measured at or below the transition temperature, ; is the static yield stress; and is the ratio of the yield stress at nonzero strain rate to the static yield stress (so that ). The yield stress is, therefore, expressed as You provide the values of C and The use of Johnson-Cook hardening does not necessarily require the use of Johnson-Cook strain when you define Johnson-Cook rate dependence. rate dependence. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *PLASTIC, HARDENING=JOHNSON COOK *RATE DEPENDENT, TYPE=JOHNSON COOK Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Johnson-Cook: Suboptions→Rate Dependent: Hardening: Johnson-Cook Johnson-Cook dynamic failure Abaqus/Explicit provides a dynamic failure model specifically for the Johnson-Cook plasticity model, which is suitable only for high-strain-rate deformation of metals. This model is referred to as the “Johnson-Cook dynamic failure model.” Abaqus/Explicit also offers a more general implementation of the Johnson-Cook failure model as part of the family of damage initiation criteria, which is the recommended technique for modeling progressive damage and failure of materials (see “Damage and failure for ductile metals: overview,” Section 24.2.1). The Johnson-Cook dynamic failure model is based on the value of the equivalent plastic strain at element integration points; failure is assumed to occur when the damage parameter exceeds 1. The damage parameter, , is defined as is the strain at failure, and the summation where is an increment of the equivalent plastic strain, , is assumed to be dependent on is performed over all increments in the analysis. The strain at failure, (where a nondimensional plastic strain rate, , defined earlier p is the pressure stress and q is the Mises stress); and the nondimensional temperature, in the Johnson-Cook hardening model. The dependencies are assumed to be separable and are of the form ; a dimensionless pressure-deviatoric stress ratio, – are failure parameters measured at or below the transition temperature, where the reference strain rate. You provide the values of failure model. This expression for (1985) in the sign of the parameter experience an increase in expression will usually take positive values. is – when you define the Johnson-Cook dynamic differs from the original formula published by Johnson and Cook . This difference is motivated by the fact that most materials in the above with increasing pressure-deviatoric stress ratio; therefore, , and When this failure criterion is met, the deviatoric stress components are set to zero and remain zero for the rest of the analysis. Depending on your choice, the pressure stress may also be set to zero for the rest of calculation (if this is the case, you must specify element deletion and the element will be deleted) or it may be required to remain compressive for the rest of the calculation (if this is the case, you must choose not to use element deletion). By default, the elements that meet the failure criterion are deleted. The Johnson-Cook dynamic failure model is suitable for high-strain-rate deformation of metals; therefore, it is most applicable to truly dynamic situations. For quasi-static problems that require element removal, the progressive damage and failure models (Chapter 24, “Progressive Damage and Failure”) or the Gurson metal plasticity model (“Porous metal plasticity,” Section 23.2.9) are recommended. The use of the Johnson-Cook dynamic failure model requires the use of Johnson-Cook hardening but does not necessarily require the use of Johnson-Cook strain rate dependence. However, the rate- dependent term in the Johnson-Cook dynamic failure criterion will be included only if Johnson-Cook strain rate dependence is defined. The Johnson-Cook damage initiation criterion described in “Damage initiation for ductile metals,” Section 24.2.2, does not have these limitations. Input File Usage: Use both of the following options: *PLASTIC, HARDENING=JOHNSON COOK *SHEAR FAILURE, TYPE=JOHNSON COOK, ELEMENT DELETION=YES or NO Abaqus/CAE Usage: Johnson-Cook dynamic failure is not supported in Abaqus/CAE. Progressive damage and failure The Johnson-Cook plasticity model can be used in conjunction with the progressive damage and failure models discussed in “Damage and failure for ductile metals: overview,” Section 24.2.1. The capability allows for the specification of one or more damage initiation criteria, including ductile, shear, forming limit diagram (FLD), forming limit stress diagram (FLSD), Müschenborn-Sonne forming limit diagram (MSFLD), and, in Abaqus/Explicit, Marciniak-Kuczynski (M-K) criteria. After damage initiation, the material stiffness is degraded progressively according to the specified damage evolution response. The models offer two failure choices, including the removal of elements from the mesh as a result of tearing or ripping of the structure. The progressive damage models allow for a smooth degradation of the material stiffness, making them suitable for both quasi-static and dynamic situations. This is a great advantage over the dynamic failure models discussed above. Input File Usage: Abaqus/CAE Usage: Use the following options: *PLASTIC, HARDENING=JOHNSON COOK *DAMAGE INITIATION *DAMAGE EVOLUTION Property module: material editor: Mechanical→Damage for Ductile Metals→damage initiation type: specify the damage initiation criterion: Suboptions→Damage Evolution: specify the damage evolution parameters Tensile failure In Abaqus/Explicit the tensile failure model can be used in conjunction with the Johnson-Cook plasticity model to define tensile failure of the material. The tensile failure model uses the hydrostatic pressure stress as a failure measure to model dynamic spall or a pressure cutoff and offers a number of failure choices including element removal. Similar to the Johnson-Cook dynamic failure model, the Abaqus/Explicit tensile failure model is suitable for high-strain-rate deformation of metals and is most applicable to truly dynamic problems. For more details, see “Dynamic failure models,” Section 23.2.8. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *PLASTIC, HARDENING=JOHNSON COOK *TENSILE FAILURE The tensile failure model is not supported in Abaqus/CAE. Heat generation by plastic work Abaqus allows for an adiabatic thermal-stress analysis (“Adiabatic analysis,” Section 6.5.4), a fully coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.3), or a fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4) to be performed in which heat generated by plastic straining of a material is calculated. This method is typically used in the simulation of bulk metal forming or high-speed manufacturing processes involving large amounts of inelastic strain, where the heating of the material caused by its deformation is an important effect because of temperature dependence of the material properties. Since the Johnson-Cook plasticity model is motivated by high-strain-rate transient dynamic applications, temperature change in this model is generally computed by assuming adiabatic conditions (no heat transfer between elements). Heat is generated in an element by plastic work, and the resulting temperature rise is computed using the specific heat of the material. This effect is introduced by defining the fraction of the rate of inelastic dissipation that appears as a heat flux per volume. Input File Usage: Use all of the following options in the same material data block: *PLASTIC, HARDENING=JOHNSON COOK *SPECIFIC HEAT *DENSITY *INELASTIC HEAT FRACTION Abaqus/CAE Usage: Use all of the following options in the same material definition: Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Johnson-Cook Thermal→Specific Heat General→Density Thermal→Inelastic Heat Fraction Initial conditions When we need to study the behavior of a material that has already been subjected to some work hardening, initial equivalent plastic strain values can be provided to specify the yield stress corresponding to the work hardened state . An initial backstress, represents a constant kinematic shift of the yield surface, which can be useful for modeling the effects of residual stresses without considering them in the equilibrium solution. , can also be specified. The backstress Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step Elements The Johnson-Cook plasticity model can be used with any elements in Abaqus that include mechanical behavior (elements that have displacement degrees of freedom). Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for the Johnson-Cook plasticity model: PEEQ STATUS Additional reference Equivalent plastic strain, equivalent plastic strain (zero or user-specified; see “Initial conditions”). where is the initial Status of element. The status of an element is 1.0 if the element is active and 0.0 if the element is not. • Johnson, G. R., and W. H. Cook, “Fracture Characteristics of Three Metals Subjected to Various Strains, Strain rates, Temperatures and Pressures,” Engineering Fracture Mechanics, vol. 21, no. 1, pp. 31–48, 1985. 23.2.8 DYNAMIC FAILURE MODELS Product: Abaqus/Explicit References • “Equation of state,” Section 25.2.1 • “Classical metal plasticity,” Section 23.2.1 • “Rate-dependent yield,” Section 23.2.3 • “Johnson-Cook plasticity,” Section 23.2.7 • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *SHEAR FAILURE • *TENSILE FAILURE Overview The progressive damage and failure models described in “Damage and failure for ductile metals: overview,” Section 24.2.1, are the recommended method for modeling material damage and failure in Abaqus; these models are suitable for both quasi-static and dynamic situations. Abaqus/Explicit offers two additional element failure models suitable only for high-strain-rate dynamic problems. The shear failure model is driven by plastic yielding. The tensile failure model is driven by tensile loading. These failure models can be used to limit subsequent load-carrying capacity of an element (up to the point of removing the element) once a stress limit is reached. Both models can be used for the same material. The shear failure model: • is designed for high-strain-rate deformation of many materials, including most metals; • uses the equivalent plastic strain as a failure measure; • offers two choices for what occurs upon failure, including the removal of elements from the mesh; • can be used in conjunction with either the Mises or the Johnson-Cook plasticity models; and • can be used in conjunction with the tensile failure model. The tensile failure model: • is designed for high-strain-rate deformation of many materials, including most metals; • uses the hydrostatic pressure stress as a failure measure to model dynamic spall or a pressure cutoff; • offers a number of choices for what occurs upon failure, including the removal of elements from the mesh; • can be used in conjunction with either the Mises or the Johnson-Cook plasticity models or the equation of state material model; and • can be used in conjunction with the shear failure model. Shear failure model The shear failure model can be used in conjunction with the Mises or the Johnson-Cook plasticity models in Abaqus/Explicit to define shear failure of the material. Shear failure criterion The shear failure model is based on the value of the equivalent plastic strain at element integration points; failure is assumed to occur when the damage parameter exceeds 1. The damage parameter, , is defined as where strain, is an increment of the equivalent plastic is any initial value of the equivalent plastic strain, is the strain at failure, and the summation is performed over all increments in the analysis. , is assumed to depend on the plastic strain rate, The strain at failure, ; a dimensionless pressure-deviatoric stress ratio, (where p is the pressure stress and q is the Mises stress); temperature; and predefined field variables. There are two ways to define the strain at failure, . One is to use direct tabular data, where the dependencies are given in a tabular form. Alternatively, the analytical form proposed by Johnson and Cook can be invoked . When direct tabular data are used to define the shear failure model, the strain at failure, , must be given as a tabular function of the equivalent plastic strain rate, the pressure-deviatoric stress ratio, temperature, and predefined field variables. This method requires the use of the Mises plasticity model. . The shear failure data must be calibrated at or below the transition temperature, , defined in “Johnson-Cook plasticity,” Section 23.2.7. This method requires the use of the Johnson-Cook plasticity model. For the Johnson-Cook shear failure model, you must specify the failure parameters, – Input File Usage: Use both of the following options for the Mises plasticity model: *PLASTIC, HARDENING=ISOTROPIC *SHEAR FAILURE, TYPE=TABULAR Use both of the following options for the Johnson-Cook plasticity model: *PLASTIC, HARDENING=JOHNSON COOK *SHEAR FAILURE, TYPE=JOHNSON COOK Element removal When the shear failure criterion is met at an integration point, all the stress components will be set to zero and that material point fails. By default, if all of the material points at any one section of an element fail, the element is removed from the mesh; it is not necessary for all material points in the element to fail. For example, in a first-order reduced-integration solid element removal of the element takes place as soon as its only integration point fails. However, in a shell element all through-the-thickness integration points must fail before the element is removed from the mesh. In the case of second-order reduced-integration beam elements, failure of all integration points through the section at either of the two element integration locations along the beam axis leads, by default, to element removal. Similarly, in the modified triangular and tetrahedral solid elements failure at any one integration point leads, by default, to element removal. Element deletion is the default failure choice. An alternative failure choice, where the element is not deleted, is to specify that when the shear failure criterion is met at a material point, the deviatoric stress components will be set to zero for that point and will remain zero for the rest of the calculation. The pressure stress is then required to remain compressive; that is, if a negative pressure stress is computed in a failed material point in an increment, it is reset to zero. This failure choice is not allowed when using plane stress, shell, membrane, beam, pipe, and truss elements because the structural constraints may be violated. Input File Usage: Use the following option to allow element deletion when the failure criterion is met (the default): *SHEAR FAILURE, ELEMENT DELETION=YES Use the following option to allow the element to take hydrostatic compressive stress only when the failure criterion is met: *SHEAR FAILURE, ELEMENT DELETION=NO Determining when to use the shear failure model The shear failure model in Abaqus/Explicit is suitable for high-strain-rate dynamic problems where inertia is important. Improper use of the shear failure model may result in an incorrect simulation. For quasi-static problems that may require element removal, the progressive damage and failure models (Chapter 24, “Progressive Damage and Failure”) or the Gurson porous metal plasticity model (“Porous metal plasticity,” Section 23.2.9) are recommended. Tensile failure model The tensile failure model can be used in conjunction with either the Mises or the Johnson-Cook plasticity models or the equation of state material model in Abaqus/Explicit to define tensile failure of the material. Tensile failure criterion The Abaqus/Explicit tensile failure model uses the hydrostatic pressure stress as a failure measure to model dynamic spall or a pressure cutoff. The tensile failure criterion assumes that failure occurs when the pressure stress, p, becomes more tensile than the user-specified hydrostatic cutoff stress, . The hydrostatic cutoff stress may be a function of temperature and predefined field variables. There is no default value for this stress. The tensile failure model can be used with either the Mises or the Johnson-Cook plasticity models or the equation of state material model. Input File Usage: Use both of the following options for the Mises or Johnson-Cook plasticity models: *PLASTIC *TENSILE FAILURE Use both of the following options for the equation of state material model: *EOS *TENSILE FAILURE Failure choices When the tensile failure criterion is met at an element integration point, the material point fails. Five failure choices are offered for the failed material points: the default choice, which includes element removal, and four different spall models. These failure choices are described below. Element removal When the tensile failure criterion is met at an integration point, all the stress components will be set to zero and that material point fails. By default, if all of the material points at any one section of an element fail, the element is removed from the mesh; it is not necessary for all material points in the element to fail. For example, in a first-order reduced-integration solid element removal of the element takes place as soon as its only integration point fails. However, in a shell element all through-the-thickness integration points must fail before the element is removed from the mesh. In the case of second-order reduced-integration beam elements, failure of all integration points through the section at either of the two element integration locations along the beam axis leads, by default, to element removal. Similarly, in the modified triangular and tetrahedral solid elements failure at any one integration point leads, by default, to element removal. Input File Usage: *TENSILE FAILURE, ELEMENT DELETION=YES (default) Spall models An alternative failure choice that is based on spall (the crumbling of a material), rather than element removal, is also available. Four failure combinations are available in this category. When the tensile failure criterion is met at a material point, the deviatoric stress components may be unaffected or may be required to be zero, and the pressure stress may be limited by the hydrostatic cutoff stress or may be required to be compressive. Therefore, there are four possible failure combinations . These failure combinations are as follows: • Ductile shear and ductile pressure: this choice corresponds to point 1 in Figure 23.2.8–1 and models the case in which the deviatoric stress components are unaffected and the pressure stress is limited by the hydrostatic cutoff stress; i.e., . Input File Usage: *TENSILE FAILURE, ELEMENT DELETION=NO, SHEAR=DUCTILE, PRESSURE=DUCTILE • Brittle shear and ductile pressure: this choice corresponds to point 2 in Figure 23.2.8–1 and models the case in which the deviatoric stress components are set to zero and remain zero for −σ cutoff Figure 23.2.8–1 Tensile failure choices. the rest of the calculation, and the pressure stress is limited by the hydrostatic cutoff stress; i.e., . Input File Usage: *TENSILE FAILURE, ELEMENT DELETION=NO, SHEAR=BRITTLE, PRESSURE=DUCTILE • Brittle shear and brittle pressure: this choice corresponds to point 3 in Figure 23.2.8–1 and models the case in which the deviatoric stress components are set to zero and remain zero for the rest of the calculation, and the pressure stress is required to be compressive; i.e., . Input File Usage: *TENSILE FAILURE, ELEMENT DELETION=NO, SHEAR=BRITTLE, PRESSURE=BRITTLE • Ductile shear and brittle pressure: this choice corresponds to point 4 in Figure 23.2.8–1 and models the case in which the deviatoric stress components are unaffected and the pressure stress is required to be compressive; i.e., . Input File Usage: *TENSILE FAILURE, ELEMENT DELETION=NO, SHEAR=DUCTILE, PRESSURE=BRITTLE There is no default failure combination for the spall models. If you choose not to use the element deletion model, you must specify the failure combination explicitly. If the material’s deviatoric behavior is not defined (for example, the equation of state model without deviatoric behavior is used), the deviatoric part of the combination is meaningless and will be ignored. The spall models are not allowed when using plane stress, shell, membrane, beam, pipe, and truss elements. Determining when to use the tensile failure model The tensile failure model in Abaqus/Explicit is suitable for high-strain-rate dynamic problems in which inertia effects are important. Improper use of the tensile failure model may result in an incorrect simulation. Using the failure models with rebar It is possible to use the shear failure and/or the tensile failure models in elements for which rebars are also defined. When such elements fail according to the failure criterion, the base material contribution to the element stress-carrying capacity is removed or adjusted depending on the type of failure chosen, but the rebar contribution to the element stress-carrying capacity is not removed. However, if you also include failure in the rebar material definition, the rebar contribution to the element stress-carrying capacity will also be removed or adjusted if the failure criterion specified for the rebar is met. Elements The shear and tensile failure models with element deletion can be used with any elements in Abaqus/Explicit include mechanical behavior (elements that have displacement degrees of freedom). The shear and tensile failure models without element deletion can be used only with plane strain, axisymmetric, and three-dimensional solid (continuum) elements in Abaqus/Explicit. that Output In addition to the standard output identifiers available in Abaqus/Explicit (“Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variable has special meaning for the shear and tensile failure models: STATUS Status of element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). 23.2.9 POROUS METAL PLASTICITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *POROUS METAL PLASTICITY • *POROUS FAILURE CRITERIA • *VOID NUCLEATION • “Defining porous metal plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The porous metal plasticity model: • is used to model materials with a dilute concentration of voids in which the relative density is greater than 0.9; • is based on Gurson’s porous metal plasticity theory (Gurson, 1977) with void nucleation and, in Abaqus/Explicit, a failure definition; and • defines the inelastic flow of the porous metal on the basis of a potential function that characterizes the porosity in terms of a single state variable, the relative density. Elastic and plastic behavior You specify the elastic part of the response separately; only linear isotropic elasticity can be specified . You specify the hardening behavior of the fully dense matrix material by defining a metal plasticity model . Only isotropic hardening can be specified. The hardening curve must describe the yield stress of the matrix material as a function of plastic strain in the matrix material. In defining this dependence at finite strains, “true” (Cauchy) stress and log strain values should be given. Rate dependency effects for the matrix material can be modeled . Yield condition The relative density of a material, r, is defined as the ratio of the volume of solid material to the total volume of the material. The relationships defining the model are expressed in terms of the void volume fraction, f, which is defined as the ratio of the volume of voids to the total volume of the material. It follows that For a metal containing a dilute concentration of voids, Gurson (1977) proposed a yield condition as a function of the void volume fraction. This yield condition was later modified by Tvergaard (1981) to the form where is the deviatoric part of the Cauchy stress tensor ; is the effective Mises stress; is the hydrostatic pressure; is the yield stress of the fully dense matrix material as a function of equivalent plastic strain in the matrix; and are material parameters. , the , , The Cauchy stress is defined as the force per “current unit area,” comprised of voids and the solid (matrix) material. f = 0 (r = 1) implies that the material is fully dense, and the Gurson yield condition reduces to the Mises yield condition. f = 1 (r = 0) implies that the material is completely voided and has no stress carrying capacity. The model generally gives physically reasonable results only for 0.1 ( 0.9). The model is described in detail in “Porous metal plasticity,” Section 4.3.6 of the Abaqus Theory Manual, along with a discussion of its numerical implementation. If the porous metal plasticity model is used during a pore pressure analysis , the relative density, r, is tracked independently of the void ratio. Specifying q1 , q2 , and q3 , , and You specify the parameters metals the ranges of the parameters reported in the literature are = 1.0 to 2.25 . The original Gurson model is recovered when = 1.0. You can define these parameters as = tabular functions of temperature and/or field variables. directly for the porous metal plasticity model. For typical = 1.0 to 1.5, = 1.0, and = = Input File Usage: Abaqus/CAE Usage: *POROUS METAL PLASTICITY Property module: material editor: Mechanical→Plasticity→Porous Metal Plasticity Failure criteria in Abaqus/Explicit The porous metal plasticity model in Abaqus/Explicit allows for failure. In this case the yield condition is written as coalescence. This function is defined in terms of the void volume fraction: models the rapid loss of stress carrying capacity that accompanies void POROUS METAL PLASTICITY where is a critical value of the void volume fraction, and In the above relationship is the value of void volume fraction at which there is a complete loss of stress carrying capacity in the material. The user- specified parameters , due to mechanisms such as micro fracture and void coalescence. When , total failure at the material point occurs. In Abaqus/Explicit an element is removed once all of its material points have failed. model the material failure when and Input File Usage: Abaqus/CAE Usage: Use the following option in conjunction with the *POROUS METAL PLASTICITY option: *POROUS FAILURE CRITERIA Property module: material editor: Mechanical→Plasticity→Porous Metal Plasticity: Suboptions→Porous Failure Criteria Specifying the initial relative density You can specify the initial relative density of the porous material, you do not specify the initial relative density, Abaqus will assign it a value of 1.0. , at material points or at nodes. If At material points You can specify the initial relative density as part of the porous metal plasticity material definition. Input File Usage: Abaqus/CAE Usage: *POROUS METAL PLASTICITY, RELATIVE DENSITY= Property module: material editor: Mechanical→Plasticity→Porous Metal Plasticity: Relative density: At nodes Alternatively, you can specify the initial relative density at nodes as initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1); these values are interpolated to the material points. The initial conditions are applied only if the relative density is not specified as part of the porous metal plasticity material definition. When a discontinuity of the initial relative density field occurs at the element boundaries, separate nodes must be used to define the elements at these boundaries, with multi-point constraints applied to make the nodal displacements and rotations equivalent. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=RELATIVE DENSITY Initial relative density is not supported in Abaqus/CAE. Flow rule and hardening The presence of pressure in the yield condition results in nondeviatoric plastic strains. Plastic flow is assumed to be normal to the yield surface: The hardening of the fully dense matrix material is described through . The evolution of the equivalent plastic strain in the matrix material is obtained from the following equivalent plastic work expression: The model is illustrated in Figure 23.2.9–1, where the yield surfaces for different levels of void volume fraction are shown in the p–q plane. f = 0 (Mises) f = 0.01 f = 0.2 f = 0.4 | p | Figure 23.2.9–1 Schematic of the yield surface in the p–q plane. Figure 23.2.9–2 compares the behavior of a porous material (whose initial yield stress is ) in tension and compression against the behavior of the perfectly plastic matrix material. In compression the porous material “hardens” due to closing of the voids, and in tension it “softens” due to growth and nucleation of the voids. Void growth and nucleation The total change in void volume fraction is given as f = 0 (Mises) σ tension (f )0 compression (f )0 −σ Figure 23.2.9–2 Schematic of uniaxial behavior of a porous metal (perfectly plastic matrix material with initial volume fraction of voids = ). is change due to growth of existing voids and where is change due to nucleation of new voids. Growth of the existing voids is based on the law of conservation of mass and is expressed in terms of the void volume fraction: The nucleation of voids is given by a strain-controlled relationship: where The normal distribution of the nucleation strain has a mean value the volume fraction of the nucleated voids, and voids are nucleated only in tension. and standard deviation . is The nucleation function is assumed to have a normal distribution, as shown in Figure 23.2.9–3 for different values of the standard deviation . fN √2π √2π sN s < sN Material 1 Material 2 Figure 23.2.9–3 Nucleation function ε pl . Figure 23.2.9–4 shows the extent of softening in a uniaxial tension test of a porous material for different values of . f N f N f < f ε = ε s = s f = f 0 2 Figure 23.2.9–4 Softening (in uniaxial tension) as a function of . The following ranges of values are reported in the literature for typical metals: = 0.1 to 0.3, 0.05 to 0.1, and = 0.04 . You specify these parameters, which can be defined as tabular functions of temperature and predefined field variables. Abaqus will include void nucleation in a tensile field only when you include it in the material definition. In Abaqus/Standard the accuracy of the implicit integration of the void nucleation and growth equation is controlled by prescribing the maximum allowable time increment in the automatic time incrementation scheme. Input File Usage: Abaqus/CAE Usage: *VOID NUCLEATION Property module: material editor: Mechanical→Plasticity→Porous Metal Plasticity: Suboptions→Void Nucleation Initial conditions When we need to study the behavior of a material that has already been subjected to some work hardening, Abaqus allows you to prescribe initial conditions directly for the equivalent plastic strain, (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step Defining initial hardening conditions in a user subroutine For more complicated cases, initial conditions can be defined in Abaqus/Standard through user subroutine HARDINI. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING, USER Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined Elements The porous metal plasticity model can be used with any stress/displacement elements other than one- dimensional elements (beam, pipe, and truss elements) or elements for which the assumed stress state is plane stress (plane stress, shell, and membrane elements). Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning in the porous metal plasticity model: Equivalent plastic strain, equivalent plastic strain (zero or user-specified; see “Initial conditions”). where is the initial Void volume fraction. 23.2.9–7 PEEQ VVFG VVFN Void volume fraction due to void growth. Void volume fraction due to void nucleation. Additional references • Gurson, A. L., “Continuum Theory of Ductile Rupture by Void Nucleation and Growth: Part I—Yield Criteria and Flow Rules for Porous Ductile Materials,” Journal of Engineering Materials and Technology, vol. 99, pp. 2–15, 1977. • Tvergaard, V., “Influence of Voids on Shear Band Instabilities under Plane Strain Condition,” International Journal of Fracture Mechanics, vol. 17, pp. 389–407, 1981. 23.2.10 CAST IRON PLASTICITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Combining material behaviors,” Section 21.1.3 • “Inelastic behavior,” Section 23.1.1 • *CAST IRON COMPRESSION HARDENING • *CAST IRON PLASTICITY • *CAST IRON TENSION HARDENING • “Defining cast iron plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The cast iron plasticity model: • is intended for the constitutive modeling of gray cast iron; • provides elastic-plastic behavior with different yield strengths, flow, and hardening in tension and compression; • is based on a yield function that depends on the maximum principal stress under tensile loading conditions and pressure-independent (von Mises type) behavior under compressive loading conditions; • allows for simultaneous inelastic dilatation and inelastic shearing under tensile loading conditions; • allows only inelastic shearing under compressive loading conditions; • is intended for the simulation of material response only under essentially monotonic loading conditions; and • cannot be used to model rate dependence. Elastic and plastic behavior The cast iron plasticity model describes the mechanical behavior of gray cast iron, a material with a microstructure consisting of a distribution of graphite flakes in a steel matrix. In tension the graphite flakes act as stress concentrators, resulting in yielding as a function of the maximum principal stress, followed by brittle behavior. In compression the graphite flakes do not have an appreciable effect on the macroscopic response, resulting in a ductile behavior similar to that of many steels. You specify the elastic part of the response separately; only linear isotropic elasticity can be used . The elastic stiffness is assumed to be the same under tension and compression. The cast iron plasticity model is used to provide the value of the plastic “Poisson’s ratio,” which is the absolute value of the ratio of the transverse to the longitudinal plastic strain under uniaxial tension. The plastic Poisson’s ratio can vary with the plastic deformation. However, the model in Abaqus assumes that it is constant with respect to plastic deformation. It can depend on temperature and field variables. If no value is specified for the plastic Poisson’s ratio, a default value of 0.04 is assumed. This default value is based on experimental results for permanent volumetric strain under uniaxial tension . Independent hardening of the material under tension and compression can be specified as described below. The tension hardening data provide the uniaxial tension yield stress as a function of plastic strain, temperature, and field variables under uniaxial tension. The compression hardening data provide the uniaxial compression yield stress as a function of plastic strain, temperature, and field variables under uniaxial compression. compression tension Figure 23.2.10–1 Typical stress-strain response of gray cast iron under uniaxial tension and uniaxial compression. Input File Usage: Abaqus/CAE Usage: *CAST IRON PLASTICITY Property module: material editor: Mechanical→Plasticity→Cast Iron Plasticity Yield condition Abaqus makes use of a composite yield surface to describe the different behavior in tension and compression. In tension yielding is assumed to be governed by the maximum principal stress, while in compression yielding is assumed to be pressure independent and governed by the deviatoric stresses alone (Mises yield condition). The model is described in detail in “Cast iron plasticity,” Section 4.3.7 of the Abaqus Theory Manual. Flow rule For the purposes of discussing the flow and hardening behavior, it is useful to divide the meridional plane into the two regions shown in Figure 23.2.10–2. Mises stress, q Gt tensile region UC Gc compressive region equivalent pressure stress, p Figure 23.2.10–2 Schematic of the flow potentials in the p–q plane. The region to the left of the uniaxial compression line (labeled UC) is referred to as the “tensile region,” while the region to the right of the uniaxial compression line is referred to as the “compressive region.” The flow potential consists of the Mises cylinder in the compressive region and an ellipsoidal “cap” in the tensile region. The transition between the two surfaces is smooth. The projection of the flow potential on the meridional plane consists of a straight line in the compressive region and an ellipse in the tensile region. The corresponding projection on the deviatoric plane is a circle. A consequence of the above choice is that plastic flow results in inelastic volume expansion in the tensile region and no inelastic volume change in the compressive region . Nonassociated flow Since the flow potential is different from the yield surface (“nonassociated” flow), the material Jacobian matrix is unsymmetric. Hence, to improve convergence, use the unsymmetric matrix storage and solution scheme . Hardening Since the hardening of gray cast iron is different in uniaxial tension and uniaxial compression, you need to provide two sets of hardening data in tabular form: one based on a uniaxial tension experiment that defines . Here, compression, respectively. and the other based on a uniaxial compression experiment that defines are the equivalent plastic strains in uniaxial tension and uniaxial and Input File Usage: Abaqus/CAE Usage: Use both of the following options in conjunction with the *CAST IRON PLASTICITY option: *CAST IRON COMPRESSION HARDENING *CAST IRON TENSION HARDENING Property module: material editor: Mechanical→Plasticity→Cast Iron Plasticity: Compression Hardening and Tension Hardening Restrictions on material data The plastic Poisson’s ratio, , is expected to be less than 0.5 since experimental results suggest that there is a permanent increase in the volume of gray cast iron when it is loaded in uniaxial tension beyond yield. For the potential to be well-defined, must be greater than −1.0. Thus, the plastic Poisson’s ratio must satisfy −1.0 0.5. The cast iron plasticity material model is intended for modeling cast iron and other materials like cast iron for which the behavior in uniaxial tension and uniaxial compression matches the behavior shown in Figure 23.2.10–1. In particular, the model expects the initial yield stress in uniaxial tension to be less than the initial yield stress in uniaxial compression. Even if the overall stress-strain response and hardening behavior in uniaxial stress states of some material other than cast iron is consistent with that of cast iron, you must also ensure that the flow potential (which has been constructed specifically for modeling cast iron) for the model is meaningful for other materials. Abaqus issues a warning message only if the initial yield stress in uniaxial tension is equal to or greater than that in uniaxial compression. No other checks are carried out in this regard. If the yield stress in uniaxial tension is higher than that in uniaxial compression, a material point in uniaxial tension may actually yield at the initial yield stress specified for uniaxial compression. This apparent anomalous behavior is due to the fact that (as a result of unrealistic user-specified material properties) a uniaxial tension stressing path in stress space meets the compressive (Mises) part of the yield surface first. Elements The cast iron plasticity model can be used with any stress/displacement element in Abaqus other than elements for which the assumed stress state is plane stress (plane stress continuum, shell, and membrane elements). It can be used with one-dimensional elements (trusses and beams in a plane) and, in Abaqus/Standard, with beams in space. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable the identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), following variables have special meaning for the cast iron plasticity material model: PEEQ PEEQT Equivalent plastic strain in uniaxial compression, Equivalent plastic strain in uniaxial tension, . . 23.2.11 TWO-LAYER VISCOPLASTICITY Products: Abaqus/Standard Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Combining material behaviors,” Section 21.1.3 • “Inelastic behavior,” Section 23.1.1 • *ELASTIC • *PLASTIC • *VISCOUS • “Defining the viscous component of a two-layer viscoplasticity model” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The two-layer viscoplastic model: • is intended for modeling materials in which significant time-dependent behavior as well as plasticity is observed, which for metals typically occurs at elevated temperatures; • consists of an elastic-plastic network that is in parallel with an elastic-viscous network (in contrast to the coupled creep and plasticity capabilities in which the plastic and the viscous networks are in series); • is based on a Mises or Hill yield condition in the elastic-plastic network and any of the available creep models in Abaqus/Standard (except the hyperbolic creep law) in the elastic-viscous network; • assumes a deviatoric inelastic response (hence, the pressure-dependent plasticity or creep models cannot be used to define the behavior of the two networks); • is intended for modeling material response under fluctuating loads over a wide range of temperatures; and • has been shown to provide good results for thermomechanical loading. Material behavior The material behavior is broken down into three parts: elastic, plastic, and viscous. Figure 23.2.11–1 shows a one-dimensional idealization of this material model, with the elastic-plastic and the elastic- viscous networks in parallel. The following subsections describe the elastic and the inelastic (plastic and viscous) behavior in detail. K p H’ σ K η, m Figure 23.2.11–1 One-dimensional idealization of the two-layer viscoplasticity model. Elastic behavior The elastic part of the response for both networks is specified using a linear isotropic elasticity definition. Any one of the available elasticity models in Abaqus/Standard can be used to define the elastic behavior of the networks. Referring to the one-dimensional idealization (Figure 23.2.11–1), the ratio of the elastic modulus of the elastic-viscous network ( ) is given by ) to the total (instantaneous) modulus ( The user-specified ratio f, given as part of the viscous behavior definition as discussed later, apportions the total moduli specified for the elastic behavior among the elastic-viscous and the elastic-plastic networks. As a result, if isotropic elastic properties are defined, the Poisson’s ratios are the same in both networks. On the other hand, if anisotropic elasticity is defined, the same type of anisotropy holds for both networks. The properties specified for the elastic behavior are assumed to be the instantaneous properties ( ). Input File Usage: Abaqus/CAE Usage: *ELASTIC Property module: material editor: Mechanical→Elasticity→Elastic Plastic behavior A plasticity definition can be used to provide the static hardening data for the material model. All available metal plasticity models, including Hill’s plasticity model to define anisotropic yield (“Anisotropic yield/creep,” Section 23.2.6), can be used. The elastic-plastic network does not take into account rate-dependent yield. Hence, any specification of strain rate dependence for the plasticity model is not allowed. Input File Usage: Use the following options: *PLASTIC *POTENTIAL Property module: material editor: Mechanical→Plasticity→Plastic: Suboptions→Potential Abaqus/CAE Usage: Viscous behavior creep and swelling,” Section 23.2.4), except The viscous behavior of the material can be governed by any of the available creep laws in the Abaqus/Standard (“Rate-dependent plasticity: hyperbolic creep law. When you define the viscous behavior, you specify the viscosity parameters and choose the specific type of viscous behavior. If you choose to input the creep law through user subroutine CREEP, only deviatoric creep should be defined—more specifically, volumetric swelling behavior should not be defined within user subroutine CREEP. In addition, you also specify the fraction, f, that defines the ratio of the elastic modulus of the elastic-viscous network to the total (instantaneous) modulus. Viscous stress ratios can be specified under the viscous behavior definition to define anisotropic viscosity . All material properties can be specified as functions of temperature and predefined field variables. Input File Usage: Use the following options: *VISCOUS, LAW=TIME or STRAIN or USER *POTENTIAL Property module: material editor: Mechanical→Plasticity→Viscous: Suboptions→Potential Abaqus/CAE Usage: Thermal expansion Thermal expansion can be modeled by providing the thermal expansion coefficient of the material (“Thermal expansion,” Section 26.1.2). Anisotropic expansion can be defined in the usual manner. In the one-dimensional idealization the expansion element is assumed to be in series with the rest of the network. Calibration of material parameters The calibration procedure is best explained in the context of the one-dimensional idealization of the In the following discussion the viscous behavior is assumed to be governed by the material model. Norton-Hoff rate law, which is given by In the expression above the subscript V denotes quantities in the elastic-viscous network alone. This form of the rate law may be chosen, for example, by choosing a time-hardening power law for the viscous behavior and setting . For this basic case there are six material parameters that need to be calibrated (Figure 23.2.11–1). These are the elastic properties of the two networks, initial yield stress ; and the Norton-Hoff rate parameters, A and n. ; the hardening and ; the ; and the hardening, The experiment that needs to be performed is uniaxial tension under different constant strain rates. A static (effectively zero strain rate) uniaxial tension test determines the long-term modulus, ; the initial yield stress, . The hardening is assumed to be linear for illustration purposes. The material model is not limited to linear hardening, and any general hardening behavior can be defined for the plasticity model. The instantaneous elastic modulus, , can be measured by measuring the initial elastic response of the material under nonzero, relatively high, strain rates. Several such measurements at different applied strain rates can be compared until the instantaneous moduli does not change with a change in the applied strain rate. The difference between K and determines . To calibrate the parameters A and n, it is useful to recognize that the long-term (steady-state) , is a constant stress of . Under the assumption that the hardening modulus is negligible compared to ), the steady-state response of the overall material is given by behavior of the elastic-viscous network under a constant applied strain rate, magnitude the elastic modulus ( where one can plot the quantity constant value of applied strain rate is the total stress for a given total strain . To determine whether steady state has been reached, and note when it becomes a constant. The . By performing several tests at different values of the constant as a function of is equal to , it is possible to determine the constants A and n. Material response in different analysis steps The material is active during all stress/displacement procedure types. In a static analysis step where the long-term response is requested , only the elastic-plastic network will be active; the elastic-viscous network will not contribute in any manner. In particular, the stress in the viscous network will be zero during a long-term static response. If the creep effects are removed in a coupled temperature-displacement procedure or a soils consolidation procedure, the response of the elastic-viscous network will be assumed to be elastic only. During a linear perturbation step, only the elastic response of the networks is considered. Some stress/displacement procedure types (coupled temperature-displacement, soils consolidation, and quasi-static) allow user control of the time integration accuracy of the viscous constitutive equations through a user-specified error tolerance. In other procedure types where no such direct control is currently available (static, dynamic), you must choose appropriate time increments. These time increments must be small compared to the typical relaxation time of the material. Elements The two-layer viscoplastic model is not available for one-dimensional elements (beams and trusses). It can be used with any other element in Abaqus/Standard that includes mechanical behavior (elements that have displacement degrees of freedom). Output In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables have special meaning for the two-layer viscoplastic material model: EE PE VE PS VS PEEQ VEEQ SENER PENER VENER The elastic strain is defined as: . Plastic strain, , in the elastic-plastic network. Viscous strain, , in the elastic-viscous network. Stress, Stress, , in the elastic-plastic network. , in the elastic-viscous network. The equivalent plastic strain, defined as The equivalent viscous strain, defined as . . The elastic strain energy density per unit volume, defined as . The plastic dissipated energy per unit volume, defined as The viscous dissipated energy per unit volume, defined as . . The above definitions of the strain tensors imply that the total strain is related to the elastic, plastic, and viscous strains through the following relation: . The above definitions of the where according to the definitions given above output variables apply to all procedure types. In particular, when the long-term response is requested for a static procedure, the elastic-viscous network does not carry any stress and the definition of the elastic strain reduces to , which implies that the total stress is related to the elastic strain through the instantaneous elastic moduli. and Additional reference • Kichenin, J., “Comportement Thermomécanique du Polyéthylène—Application aux Structures Gazières,” Thèse de Doctorat de l’Ecole Polytechnique, Spécialité: Mécanique et Matériaux, 1992. 23.2.12 ORNL – OAK RIDGE NATIONAL LABORATORY CONSTITUTIVE MODEL Products: Abaqus/Standard Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • “Classical metal plasticity,” Section 23.2.1 • “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 • *ORNL • *PLASTIC • *CREEP • “Using the Oak Ridge National Laboratory (ORNL) constitutive model in plasticity and creep calculations” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Specifying cycled yield stress data for the ORNL model” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The Oak Ridge National Laboratory (ORNL) constitutive model: • allows for use of the rules defined in the Nuclear Standard NEF 9–5T, “Guidelines and Procedures for Design of Class 1 Elevated Temperature Nuclear System Components,” in plasticity and creep calculations; • is intended for use in modeling types 304 and 316 stainless steel at relatively high temperatures; • can be used only with the metal plasticity models (linear kinematic hardening only) and/or the strain hardening form of the metal creep law; and • is described in detail in “ORNL constitutive theory,” Section 4.3.8 of the Abaqus Theory Manual. Usage with plasticity The ORNL constitutive model in Abaqus/Standard is based on the March 1981 issue of the Nuclear Standard NEF 9–5T and on the October 1986 issue, which revises the constitutive model extensively. This model adds isotropic hardening of the plastic yield surface from a virgin material state to a Initially the material is assumed to harden kinematically according to a bilinear fully cycled state. If a strain reversal takes place or if the creep strain representation of the virgin stress-strain curve. reaches 0.2%, the yield surface expands isotropically to the user-defined tenth-cycle stress-strain curve. Further hardening occurs kinematically according to a bilinear representation of the tenth-cycle stress-strain curve. You must specify the virgin yield stress and the hardening through a plasticity model definition and the elastic part of the response through a linear elasticity model definition. You specify the tenth-cycle yield stress and hardening values separately. The yield stress at each temperature should be defined by giving its value at zero plastic strain and at one additional nonzero plastic strain point, thus giving a constant hardening rate (linear work hardening). Input File Usage: Use all of the following options in the same material data block: Abaqus/CAE Usage: *PLASTIC *ORNL *CYCLED PLASTIC Property module: material editor: Mechanical→Plasticity→Plastic: Suboptions→Ornl and Suboptions→Cycled Plastic Abaqus/Standard also allows you to invoke the optional kinematic shift ( ) reset procedure that is reset procedure explicitly, described in Section 4.3.5 of the Nuclear Standard. If you do not specify the it is not used. Input File Usage: Abaqus/CAE Usage: *ORNL, RESET Property module: material editor: Suboptions→Ornl: Invoke reset procedure Usage with creep The ORNL constitutive model assumes that creep uses the strain hardening formulation. It introduces auxiliary hardening rules when strain reversals occur. An algorithm providing details is presented in “ORNL constitutive theory,” Section 4.3.8 of the Abaqus Theory Manual. It can be used only when the creep behavior is defined by a strain-hardening power law. Input File Usage: Use both of the following options in the same material data block: Abaqus/CAE Usage: *CREEP, LAW=STRAIN *ORNL Property module: material editor: Mechanical→Plasticity→Creep: Law: Strain-Hardening: Suboptions→Ornl Translation of the yield surface during creep The ORNL formulation can also cause the center of the yield surface to translate during creep for use in subsequent plastic increments; this behavior is defined through two optional user-defined parameters. Specifying saturation rates for kinematic shift You can specify A, the saturation rates for kinematic shift caused by creep strain as defined by Equation (15) of Section 4.3.3–3 of the Nuclear Standard. The default value is 0.3. Set A=0.0 to use the 1986 revision of the standard. Input File Usage: *ORNL, A=A Abaqus/CAE Usage: Property module: material editor: Suboptions→Ornl: Saturation rates for kinematic shift: A Specifying the rate of kinematic shift You can specify H, the rate of kinematic shift with respect to creep strain (Equation (7) of Section 4.3.2–1 of the Nuclear Standard). Set H=0.0 to use the 1986 revision of the standard. If you do not specify a value for H, it is determined according to Section 4.3.3–3 of the 1981 revision of the standard. Input File Usage: Abaqus/CAE Usage: *ORNL, H=H Property module: material editor: Suboptions→Ornl: Rate of kinematic shift wrt creep strain: H Initial conditions When we need to study the behavior of a material that has already been subjected to some work hardening, initial equivalent plastic strain values can be provided to specify the yield stress corresponding to the work hardened state. See “Inelastic behavior,” Section 23.1.1, for additional details. Initial values can also be provided for the backstress tensor, , to include strain-induced anisotropy. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, for more information. For more complicated cases initial conditions can be defined through user subroutine HARDINI. Input File Usage: Use the following option to specify the initial equivalent plastic strain directly: *INITIAL CONDITIONS, TYPE=HARDENING Use the following option in Abaqus/Standard to specify the initial equivalent plastic strain in user subroutine HARDINI: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING, USER Use the following options to specify the initial equivalent plastic strain directly: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step Use the following options in Abaqus/Standard to specify the initial equivalent plastic strain in user subroutine HARDINI: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined Elements The ORNL constitutive model can be used with any elements in Abaqus/Standard that include mechanical behavior (elements that have displacement degrees of freedom). Output In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), variables associated with creep (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) and the kinematic hardening plasticity models (“Models for metals subjected to cyclic loading,” Section 23.2.2) are available for the ORNL constitutive model. 23.2.13 DEFORMATION PLASTICITY Products: Abaqus/Standard Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *DEFORMATION PLASTICITY • “Defining deformation plasticity” in “Defining other mechanical models,” Section 12.9.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The deformation theory Ramberg-Osgood plasticity model: • is primarily intended for use in developing fully plastic solutions for fracture mechanics applications in ductile metals; and • cannot appear with any other mechanical response material models since it completely describes the mechanical response of the material. One-dimensional model In one dimension the model is where is the stress; is the strain; is Young’s modulus (defined as the slope of the stress-strain curve at zero stress); is the “yield” offset; is the yield stress, in the sense that, when , ; and is the hardening exponent for the “plastic” (nonlinear) term: . The material behavior described by this model is nonlinear at all stress levels, but for commonly or more) the nonlinearity becomes significant only at used values of the hardening exponent ( stress magnitudes approaching or exceeding . Generalization to multiaxial stress states The one-dimensional model is generalized to multiaxial stress states using Hooke’s law for the linear term and the Mises stress potential and associated flow law for the nonlinear term: where is the strain tensor, is the stress tensor, is the equivalent hydrostatic stress, is the Mises equivalent stress, is the stress deviator, and is the Poisson’s ratio. The linear part of the behavior can be compressible or incompressible, depending on the value of the Poisson’s ratio, but the nonlinear part of the behavior is incompressible (because the flow is normal to the Mises stress potential). The model is described in detail in “Deformation plasticity,” Section 4.3.9 of the Abaqus Theory Manual. You specify the parameters E, , , n, and directly. They can be defined as a tabular function of temperature. Input File Usage: Abaqus/CAE Usage: Typical applications *DEFORMATION PLASTICITY Property module: material editor: Mechanical→Deformation Plasticity The deformation plasticity model is most commonly applied in static loading with small-displacement analysis, where the fully plastic solution must be developed in a part of the model. Generally, the load is ramped on until all points in the region being monitored satisfy the condition that the “plastic strain” dominates and, hence, exhibit fully plastic behavior, which is defined as or You can specify the name of a particular element set to be monitored in a static analysis step for fully plastic behavior. The step will end when the solutions at all constitutive calculation points in the element set are fully plastic, when the maximum number of increments specified for the step is reached, or when the time period specified for the static step is exceeded, whichever comes first. Input File Usage: Abaqus/CAE Usage: *STATIC, FULLY PLASTIC=ElsetName Step module: Create Step: General: Static, General: Other: Stop when region region is fully plastic. Elements Deformation plasticity can be used with any stress/displacement element in Abaqus/Standard. Since it will generally be used for cases when the deformation is dominated by plastic flow, the use of “hybrid” (mixed formulation) or reduced-integration elements is recommended with this material model. 23.3 Other plasticity models • “Extended Drucker-Prager models,” Section 23.3.1 • “Modified Drucker-Prager/Cap model,” Section 23.3.2 • “Mohr-Coulomb plasticity,” Section 23.3.3 • “Critical state (clay) plasticity model,” Section 23.3.4 • “Crushable foam plasticity models,” Section 23.3.5 23.3.1 EXTENDED DRUCKER-PRAGER MODELS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • “Rate-dependent yield,” Section 23.2.3 • “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 • Chapter 24, “Progressive Damage and Failure” • *DRUCKER PRAGER • *DRUCKER PRAGER HARDENING • *RATE DEPENDENT • *DRUCKER PRAGER CREEP • *TRIAXIAL TEST DATA • “Defining Drucker-Prager plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The extended Drucker-Prager models: • are used to model frictional materials, which are typically granular-like soils and rock, and exhibit pressure-dependent yield (the material becomes stronger as the pressure increases); • are used to model materials in which the compressive yield strength is greater than the tensile yield strength, such as those commonly found in composite and polymeric materials; • allow a material to harden and/or soften isotropically; • generally allow for volume change with inelastic behavior: the flow rule, defining the inelastic straining, allows simultaneous inelastic dilation (volume increase) and inelastic shearing; • can include creep in Abaqus/Standard if the material exhibits long-term inelastic deformations; • can be defined to be sensitive to the rate of straining, as is often the case in polymeric materials; • can be used in conjunction with either the elastic material model (“Linear elastic behavior,” Section 22.2.1) or, in Abaqus/Standard if creep is not defined, the porous elastic material model (“Elastic behavior of porous materials,” Section 22.3.1); • can be used in conjunction with an equation of state model (“Equation of state,” Section 25.2.1) to describe the hydrodynamic response of the material in Abaqus/Explicit; • can be used in conjunction with the models of progressive damage and failure (“Damage and failure for ductile metals: overview,” Section 24.2.1) to specify different damage initiation criteria and damage evolution laws that allow for the progressive degradation of the material stiffness and the removal of elements from the mesh; and • are intended to simulate material response under essentially monotonic loading. Yield criteria The yield criteria for this class of models are based on the shape of the yield surface in the meridional plane. The yield surface can have a linear form, a hyperbolic form, or a general exponent form. These surfaces are illustrated in Figure 23.3.1–1. The stress invariants and other terms in each of the three related yield criteria are defined later in this section. The linear model (Figure 23.3.1–1a) provides for a possibly noncircular yield surface in the deviatoric plane ( -plane) to match different yield values in triaxial tension and compression, associated inelastic flow in the deviatoric plane, and separate dilation and friction angles. Input data parameters define the shape of the yield and flow surfaces in the meridional and deviatoric planes as well as other characteristics of inelastic behavior such that a range of simple theories is provided—the original Drucker-Prager model is available within this model. However, this model cannot provide a close match to Mohr-Coulomb behavior, as described later in this section. The hyperbolic and general exponent models use a von Mises (circular) section in the deviatoric In the meridional plane a hyperbolic flow potential is used for both models, which, in stress plane. general, means nonassociated flow. The choice of model to be used depends largely on the analysis type, the kind of material, the experimental data available for calibration of the model parameters, and the range of pressure stress values that the material is likely to experience. It is common to have either triaxial test data at different levels of confining pressure or test data that are already calibrated in terms of a cohesion and a friction angle and, sometimes, a triaxial tensile strength value. If triaxial test data are available, the material parameters must be calibrated first. The accuracy with which the linear model can match these test data is limited by the fact that it assumes linear dependence of deviatoric stress on pressure stress. Although the hyperbolic model makes a similar assumption at high confining pressures, it provides a nonlinear relationship between deviatoric and pressure stress at low confining pressures, which may provide a better match of the triaxial experimental data. The hyperbolic model is useful for brittle materials for which both triaxial compression and triaxial tension data are available, which is a common situation for materials such as rocks. The most general of the three yield criteria is the exponent form. This criterion provides the most flexibility in matching triaxial test data. Abaqus determines the material parameters required for this model directly from the triaxial test data. A least-squares fit that minimizes the relative error in stress is used for this purpose. For cases where the experimental data are already calibrated in terms of a cohesion and a friction angle, the linear model can be used. If these parameters are provided for a Mohr-Coulomb model, it is necessary to convert them to Drucker-Prager parameters. The linear model is intended primarily for If tensile stresses are significant, applications where the stresses are for the most part compressive. hydrostatic tension data should be available (along with the cohesion and friction angle) and the hyperbolic model should be used. Calibration of these models is discussed later in this section. a) Linear Drucker-Prager: F = t − p tan β − d = 0 −d /tanβ −p b) Hyperbolic: F = √(d − p tan β) + q |0 |0 − p tan β − d = 0 −p c) Exponent form: F = aq − p − p = 0 Figure 23.3.1–1 Yield surfaces in the meridional plane. Hardening and rate dependence For granular materials these models are often used as a failure surface, in the sense that the material can exhibit unlimited flow when the stress reaches yield. This behavior is called perfect plasticity. The models are also provided with isotropic hardening. In this case plastic flow causes the yield surface to change size uniformly with respect to all stress directions. This hardening model is useful for cases involving gross plastic straining or in which the straining at each point is essentially in the same direction in strain space throughout the analysis. Although the model is referred to as an isotropic “hardening” model, strain softening, or hardening followed by softening, can be defined. As strain rates increase, many materials show an increase in their yield strength. This effect becomes important in many polymers when the strain rates range between 0.1 and 1 per second; it can be very important for strain rates ranging between 10 and 100 per second, which are characteristic of high-energy dynamic events or manufacturing processes. The effect is generally not as important in granular materials. The evolution of the yield surface with plastic deformation is described in terms of the equivalent stress , which can be chosen as either the uniaxial compression yield stress, the uniaxial tension yield stress, or the shear (cohesion) yield stress: where is the equivalent plastic strain rate, defined for the linear Drucker-Prager model as if hardening is defined in uniaxial = compression; = = if hardening is defined in uniaxial tension; if hardening is defined in pure shear, and defined for the hyperbolic and exponential Drucker-Prager models as is the equivalent plastic strain; is temperature; and are other predefined field variables. The functional dependence includes hardening as well as rate-dependent effects. The material data can be input either directly in a tabular format or by correlating it to static relations based on yield stress ratios. Rate dependence as described here is most suitable for moderate- to high-speed events in Abaqus/Standard. Time-dependent inelastic deformation at low deformation rates can be better represented by creep models. Such inelastic deformation, which can coexist with rate-independent plastic deformation, the existence of creep in an is described later in this section. However, Abaqus/Standard material definition precludes the use of rate dependence as described here. When using the Drucker-Prager material model, Abaqus allows you to prescribe initial hardening by defining initial equivalent plastic strain values, as discussed below along with other details regarding the use of initial conditions. Direct tabular data Test data are entered as tables of yield stress values versus equivalent plastic strain at different equivalent plastic strain rates; one table per strain rate. Compression data are more commonly available for geological materials, whereas tension data are usually available for polymeric materials. The guidelines on how to enter these data are provided in “Rate-dependent yield,” Section 23.2.3. Input File Usage: Abaqus/CAE Usage: *DRUCKER PRAGER HARDENING, RATE= Property module: material editor: Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker Prager Hardening: toggle on Use strain-rate-dependent data Yield stress ratios Alternatively, the strain rate behavior can be assumed to be separable, so that the stress-strain dependence is similar at all strain rates: where nonzero strain rate to the static yield stress (so that is the static stress-strain behavior and ). is the ratio of the yield stress at Two methods are offered to define R in Abaqus: specifying an overstress power law or defining the variable R directly as a tabular function of . Overstress power law The Cowper-Symonds overstress power law has the form and where of other predefined field variables. are material parameters that can be functions of temperature and, possibly, Input File Usage: Use both of the following options: Abaqus/CAE Usage: *DRUCKER PRAGER HARDENING *RATE DEPENDENT, TYPE=POWER LAW Property module: material editor: Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker Prager Hardening; Suboptions→Rate Dependent: Hardening: Power Law Tabular function When R is entered directly, it is entered as a tabular function of the equivalent plastic strain rate, temperature, . ; and predefined field variables, ; Input File Usage: Use both of the following options: Abaqus/CAE Usage: *DRUCKER PRAGER HARDENING *RATE DEPENDENT, TYPE=YIELD RATIO Property module: material editor: Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker Prager Hardening; Suboptions→Rate Dependent: Hardening: Yield Ratio Johnson-Cook rate dependence Johnson-Cook rate dependence has the form where on predefined field variables. and C are material constants that do not depend on temperature and are assumed not to depend Input File Usage: Abaqus/CAE Usage: *DRUCKER PRAGER HARDENING *RATE DEPENDENT, TYPE=JOHNSON COOK Property module: material editor: Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker Prager Hardening; Suboptions→Rate Dependent: Hardening: Johnson-Cook Stress invariants The yield stress surface makes use of two invariants, defined as the equivalent pressure stress, and the Mises equivalent stress, where is the stress deviator, defined as In addition, the linear model also uses the third invariant of deviatoric stress, Linear Drucker-Prager model The linear model is written in terms of all three stress invariants. It provides for a possibly noncircular yield surface in the deviatoric plane to match different yield values in triaxial tension and compression, associated inelastic flow in the deviatoric plane, and separate dilation and friction angles. Yield criterion The linear Drucker-Prager criterion is written as where is the slope of the linear yield surface in the p–t stress plane and is commonly referred to as the friction angle of the material; is the cohesion of the material; and is the ratio of the yield stress in triaxial tension to the yield stress in triaxial compression and, thus, controls the dependence of the yield surface on the value of the intermediate principal stress . In the case of hardening defined in uniaxial compression, the linear yield criterion precludes friction angles When 71.5° ( , 3), which is unlikely to be a limitation for real materials. , which implies that the yield surface is the von Mises circle in the deviatoric -plane), in which case the yield stresses in triaxial tension and compression principal stress plane (the are the same. To ensure that the yield surface remains convex requires The cohesion, d, of the material is related to the input data as . Plastic flow G is the flow potential, chosen in this model as S3 t = q 1+ 1_ ) - 1- 1_ K 3 )r )) _ 1_ Curve 1.0 0.8 S2 S1 Figure 23.3.1–2 Typical yield/flow surfaces of the linear model in the deviatoric plane. is the dilation angle in the p–t plane. A geometric interpretation of is shown in the where p–t diagram of Figure 23.3.1–3. In the case of hardening defined in uniaxial compression, this flow rule definition precludes dilation angles 3). This restriction is not seen as a limitation since it is unlikely this will be the case for real materials. 71.5° ( dεpl hardening Figure 23.3.1–3 Linear Drucker-Prager model: yield surface and flow direction in the p–t plane. For granular materials the linear model is normally used with nonassociated flow in the p–t plane, in the sense that the flow is assumed to be normal to the yield surface in the -plane but at an angle to the t-axis in the p–t plane, where usually results from setting and Nonassociated flow is also generally assumed when the model is used for polymeric materials. If the inelastic deformation is incompressible; if dilation angle. , as illustrated in Figure 23.3.1–3. Associated flow . , is referred to as the . The original Drucker-Prager model is available by setting , the material dilates. Hence, The relationship between the flow potential and the incremental plastic strain for the linear model is discussed in detail in “Models for granular or polymer behavior,” Section 4.4.2 of the Abaqus Theory Manual. Input File Usage: Abaqus/CAE Usage: *DRUCKER PRAGER, SHEAR CRITERION=LINEAR Property module: material editor: Mechanical→Plasticity→Drucker Prager: Shear criterion: Linear Nonassociated flow the material stiffness matrix is not symmetric; Nonassociated flow implies that the unsymmetric matrix storage and solution scheme should be used in Abaqus/Standard . If the difference between is not large and the region of the model in which inelastic deformation is occurring is confined, it is possible that a symmetric approximation to the material stiffness matrix will give an acceptable rate of convergence and the unsymmetric matrix scheme may not be needed. therefore, and Hyperbolic and general exponent models The hyperbolic and general exponent models available are written in terms of the first two stress invariants only. Hyperbolic yield criterion The hyperbolic yield criterion is a continuous combination of the maximum tensile stress condition of Rankine (tensile cutoff) and the linear Drucker-Prager condition at high confining stress. It is written as where and is the initial hydrostatic tension strength of the material; is the hardening parameter; is the initial value of ; and is the friction angle measured at high confining pressure, as shown in Figure 23.3.1–1(b). The hardening parameter, , can be obtained from test data as follows: The isotropic hardening assumed in this model treats Figure 23.3.1–4. as constant with respect to stress as depicted in hardening l0/tanβ l0/tanβ l0/tanβ Figure 23.3.1–4 Hyperbolic model: yield surface and hardening in the p–q plane. Input File Usage: Abaqus/CAE Usage: *DRUCKER PRAGER, SHEAR CRITERION=HYPERBOLIC Property module: material editor: Mechanical→Plasticity→Drucker Prager: Shear criterion: Hyperbolic General exponent yield criterion The general exponent form provides the most general yield criterion available in this class of models. The yield function is written as where and are material parameters that are independent of plastic deformation; and is the hardening parameter that represents the hydrostatic tension strength of the material as shown in Figure 23.3.1–1(c). is related to the input test data as The isotropic hardening assumed in this model treats a and b as constant with respect to stress, as depicted in Figure 23.3.1–5. 1/b t( )a hardening Figure 23.3.1–5 General exponent model: yield surface and hardening in the p–q plane. The material parameters a and b can be given directly. Alternatively, if triaxial test data at different levels of confining pressure are available, Abaqus will determine the material parameters from the triaxial test data, as discussed below. Input File Usage: Abaqus/CAE Usage: *DRUCKER PRAGER, SHEAR CRITERION=EXPONENT FORM Property module: material editor: Mechanical→Plasticity→Drucker Prager: Shear criterion: Exponent Form Plastic flow G is the flow potential, chosen in these models as a hyperbolic function: where is the dilation angle measured in the p–q plane at high confining pressure; is the initial yield stress, taken from the user-specified Drucker- Prager hardening data; and is a parameter, referred to as the eccentricity, that defines the rate at which the function approaches the asymptote (the flow potential tends to a straight line as the eccentricity tends to zero). Suitable default values are provided for stress used. , as described below. The value of will depend on the yield This flow potential, which is continuous and smooth, ensures that the flow direction is always uniquely defined. The function approaches the linear Drucker-Prager flow potential asymptotically at high confining pressure stress and intersects the hydrostatic pressure axis at 90°. A family of hyperbolic potentials in the meridional stress plane is shown in Figure 23.3.1–6. The flow potential is the von Mises circle in the deviatoric stress plane (the -plane). dεpl σ|0 ∋ Figure 23.3.1–6 Family of hyperbolic flow potentials in the p–q plane. , and the material For the hyperbolic model flow is nonassociated in the p–q plane if the dilation angle, friction angle, , are different. The hyperbolic model provides associated flow in the p–q plane only when ) is assumed if the flow potential is used with the hyperbolic model, so that associated flow is recovered when . A default value of and . For the general exponent model flow is always nonassociated in the p–q plane. The default flow potential eccentricity is , which implies that the material has almost the same dilation angle over a wide range of confining pressure stress values. Increasing the value of provides more curvature to the flow potential, implying that the dilation angle increases more rapidly as the confining pressure decreases. Values of that are significantly less than the default value may lead to convergence problems if the material is subjected to low confining pressures because of the very tight curvature of the flow potential locally where it intersects the p-axis. The relationship between the flow potential and the incremental plastic strain for the hyperbolic and general exponent models is discussed in detail in “Models for granular or polymer behavior,” Section 4.4.2 of the Abaqus Theory Manual. DRUCKER-PRAGER the material stiffness matrix is not symmetric; Nonassociated flow implies that the unsymmetric matrix storage and solution scheme should be used in Abaqus/Standard . If the difference between in the hyperbolic model is not large and if the region of the model in which inelastic deformation is occurring is confined, it is possible that a symmetric approximation to the material stiffness matrix will give an acceptable rate of convergence. In such cases the unsymmetric matrix scheme may not be needed. therefore, and Progressive damage and failure In Abaqus/Explicit the extended Drucker-Prager models can be used in conjunction with the models of progressive damage and failure discussed in “Damage and failure for ductile metals: overview,” Section 24.2.1. The capability allows for the specification of one or more damage initiation criteria, including ductile, shear, forming limit diagram (FLD), forming limit stress diagram (FLSD), and Müschenborn-Sonne forming limit diagram (MSFLD) criteria. After damage initiation, the material stiffness is degraded progressively according to the specified damage evolution response. The model offers two failure choices, including the removal of elements from the mesh as a result of tearing or ripping of the structure. The progressive damage models allow for a smooth degradation of the material stiffness, making them suitable for both quasi-static and dynamic situations. Input File Usage: Use the following options: Abaqus/CAE Usage: *DAMAGE INITIATION *DAMAGE EVOLUTION Property module: material editor: Mechanical→Damage for Ductile Metals→damage initiation type: specify the damage initiation criterion: Suboptions→Damage Evolution: specify the damage evolution parameters Matching experimental triaxial test data In such a test the Data for geological materials are most commonly available from triaxial testing. specimen is confined by a pressure stress that is held constant during the test. The loading is an additional tension or compression stress applied in one direction. Typical results include stress-strain curves at different levels of confinement, as shown in Figure 23.3.1–7. To calibrate the yield parameters for this class of models, you need to decide which point on each stress-strain curve will be used for calibration. For example, if you wish to calibrate the initial yield surface, the point in each stress-strain curve corresponding to initial deviation from elastic behavior should be used. Alternatively, if you wish to calibrate the ultimate yield surface, the point in each stress-strain curve corresponding to the peak stress should be used. One stress data point from each stress-strain curve at a different level of confinement is plotted in the meridional stress plane (p–t plane if the linear model is to be used, or p–q plane if the hyperbolic or general exponent model will be used). This technique calibrates the shape and position of the yield surface, as shown in Figure 23.3.1–8, and is adequate to define a model if it is to be used as a failure surface (perfect points chosen to define shape and position of yield surface -σ -σ -σ2 increasing confinement Figure 23.3.1–7 Triaxial tests with stress-strain curves for typical geological materials at different levels of confinement. Figure 23.3.1–8 Yield surface in meridional plane. plasticity). The models are also available with isotropic hardening, in which case hardening data are required to complete the calibration. In an isotropic hardening model plastic flow causes the yield surface to change size uniformly; in other words, only one of the stress-strain curves depicted in Figure 23.3.1–7 can be used to represent hardening. The curve that represents hardening most accurately over the range of loading conditions anticipated should be selected (usually the curve for the average anticipated value of pressure stress). As stated earlier, two types of triaxial test data are commonly available for geological materials. In a triaxial compression test the specimen is confined by pressure and an additional compression stress is superposed in one direction. Thus, the principal stresses are all negative, with (Figure 23.3.1–9a). minimum principal stresses, respectively. are the maximum, intermediate, and In the preceding inequality , and , -σ 1= σ ≥ 2 σ -σ -σ -σ DRUCKER-PRAGER ≥ 1 2 = σ -σ Figure 23.3.1–9 a) Triaxial compression and b) tension. The values of the stress invariants are and so that The triaxial compression results can, thus, be plotted in the meridional plane shown in Figure 23.3.1–8. Linear Drucker-Prager model Fitting the best straight line through the triaxial compression results provides Drucker-Prager model. and d for the linear Triaxial tension data are also needed to define K in the linear Drucker-Prager model. Under triaxial tension the specimen is again confined by pressure, after which the pressure in one direction is reduced. In this case the principal stresses are (Figure 23.3.1–9b). The stress invariants are now and so that Thus, K can be found by plotting these test results as q versus p and again fitting the best straight line. The triaxial compression and tension lines must intercept the p-axis at the same point, and the ratio of values of q for triaxial tension and compression at the same value of p then gives K (Figure 23.3.1–10). Best fit to triaxial compression data Best fit to triaxial tension data qc qt qt = K qc Figure 23.3.1–10 Linear model: fitting triaxial compression and tension data. Hyperbolic model and for the hyperbolic model. This fit is performed in the same manner as that used to obtain Fitting the best straight line through the triaxial compression results at high confining pressures provides and d for the linear Drucker-Prager model. In addition, hydrostatic tension data are required to complete the calibration of the hyperbolic model so that the initial hydrostatic tension strength, , can be defined. DRUCKER-PRAGER Given triaxial data in the meridional plane, Abaqus provides a capability to determine the material parameters a, b, and required for the exponent model. The parameters are determined on the basis of a “best fit” of the triaxial test data at different levels of confining stress. A least-squares fit which minimizes the relative error in stress is used to obtain the “best fit” values for a, b, and . The capability allows all three parameters to be calibrated or, if some of the parameters are known, only the remaining parameters to be calibrated. This ability is useful if only a few data points are available, in which case you may wish to fit the best straight line ( ) through the data points (effectively reducing the model to a linear Drucker-Prager model). Partial calibration can also be useful in a case when triaxial test data at low confinement are unreliable or unavailable, as is often the case for cohesionless materials. In this case a better fit may be obtained if the value of The data must be provided in terms of the principal stresses is the confining stress and is the stress in the loading direction. The Abaqus sign convention must be followed such that tensile stresses are positive and compressive stresses are negative. One pair of stresses must be entered from each triaxial test. As many data points as desired can be entered from triaxial tests at different levels of confining stress. and is specified and only a and b are calibrated. , where If the exponent model is used as a failure surface (perfect plasticity), the Drucker-Prager hardening behavior does not have to be specified. The hydrostatic tension strength, , obtained from the calibration will then be used as the failure stress. However, if the Drucker-Prager hardening behavior is specified together with the triaxial test data, the value of obtained from the calibration will be ignored. In this case Abaqus will interpolate directly from the hardening data. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *DRUCKER PRAGER, SHEAR CRITERION=EXPONENT FORM, TEST DATA *TRIAXIAL TEST DATA Property module: material editor: Mechanical→Plasticity→Drucker Prager: Shear criterion: Exponent Form, toggle on Use Suboption Triaxial Test Data, and select Suboptions→Triaxial Test Data Matching Mohr-Coulomb parameters to the Drucker-Prager model Sometimes experimental data are not directly available. Instead, you are provided with the friction angle and cohesion values for the Mohr-Coulomb model. In that case the simplest way to proceed is to use the Mohr-Coulomb model . In some situations it may be necessary to use the Drucker-Prager model instead of the Mohr-Coulomb model (such as when rate effects need to be considered), in which case we need to calculate values for the parameters of a Drucker- Prager model to provide a reasonable match to the Mohr-Coulomb parameters. The Mohr-Coulomb failure model is based on plotting Mohr’s circle for states of stress at failure in the plane of the maximum and minimum principal stresses. The failure line is the best straight line that touches these Mohr’s circles (Figure 23.3.1–11). σ s = 1 σ - m= 1+σ 2 σ (compressive stress) Figure 23.3.1–11 Mohr-Coulomb failure model. Therefore, the Mohr-Coulomb model is defined by where is negative in compression. From Mohr’s circle, Substituting for and , multiplying both sides by , and reducing, the Mohr-Coulomb model can be written as where is half of the difference between the maximum principal stress, (and is, therefore, the maximum shear stress), , and the minimum principal stress, is the average of the maximum and minimum principal stresses, and is the friction angle. Thus, the model assumes a linear relationship between deviatoric and pressure stress and, so, can be matched by the linear or hyperbolic Drucker-Prager models provided in Abaqus. The Mohr-Coulomb model assumes that failure is independent of the value of the intermediate principal stress, but the Drucker-Prager model does not. The failure of typical geotechnical materials generally includes some small dependence on the intermediate principal stress, but the Mohr-Coulomb model is generally considered to be sufficiently accurate for most applications. This model has vertices in the deviatoric plane . S3 Mohr-Coulomb S1 S2 Drucker-Prager Figure 23.3.1–12 Mohr-Coulomb model in the deviatoric plane. The implication is that, whenever the stress state has two equal principal stress values, the flow direction can change significantly with little or no change in stress. None of the models currently available in Abaqus can provide such behavior; even in the Mohr-Coulomb model the flow potential is smooth. This limitation is generally not a key concern in many design calculations involving Coulomb-like materials, but it can limit the accuracy of the calculations, especially in cases where flow localization is important. Matching plane strain response Plane strain problems are often encountered in geotechnical analysis; for example, long tunnels, footings, and embankments. Therefore, the constitutive model parameters are often matched to provide the same flow and failure response in plane strain. The matching procedure described below is carried out in terms of the linear Drucker-Prager model but is also applicable to the hyperbolic model at high levels of confining stress. The linear Drucker-Prager flow potential defines the plastic strain increment as where plane, we can take is the equivalent plastic strain increment. Since we wish to match the behavior in only one . Thus, , which implies that Writing this expression in terms of principal stresses provides with similar expressions for have , which provides the constraint and . Assume plane strain in the 1-direction. At limit load we must Using this constraint we can rewrite q and p in terms of the principal stresses in the plane of deformation, and , as and With these expressions the Drucker-Prager yield surface can be written in terms of and as The Mohr-Coulomb yield surface in the plane is By comparison, These relationships provide a match between the Mohr-Coulomb material parameters and linear Drucker-Prager material parameters in plane strain. Consider the two extreme cases of flow definition: associated flow, , and nondilatant flow, when . For associated flow and for nondilatant flow In either case is immediately available as and and The difference between these two approaches increases with the friction angle; however, the results are not very different for typical friction angles, as illustrated in Table 23.3.1–1. Table 23.3.1–1 Plane strain matching of Drucker-Prager and Mohr-Coulomb models. Mohr-Coulomb friction angle, Associated flow Nondilatant flow Drucker-Prager friction angle, Drucker-Prager friction angle, 10° 20° 30° 40° 50° 16.7° 30.2° 39.8° 46.2° 50.5° 1.70 1.60 1.44 1.24 1.02 16.7° 30.6° 40.9° 48.1° 53.0° 1.70 1.63 1.50 1.33 1.11 “Limit load calculations with granular materials,” Section 1.15.4 of the Abaqus Benchmarks Manual, and “Finite deformation of an elastic-plastic granular material,” Section 1.15.5 of the Abaqus Benchmarks Manual, show a comparison of the response of a simple loading of a granular material using the Drucker-Prager and Mohr-Coulomb models, using the plane strain approach to match the parameters of the two models. Matching triaxial test response Another approach to matching Mohr-Coulomb and Drucker-Prager model parameters for materials with low friction angles is to make the two models provide the same failure definition in triaxial compression and tension. The following matching procedure is applicable only to the linear Drucker-Prager model since this is the only model in this class that allows for different yield values in triaxial compression and tension. We can rewrite the Mohr-Coulomb model in terms of principal stresses: Using the results above for the stress invariants p, q, and r in triaxial compression and tension allows the linear Drucker-Prager model to be written for triaxial compression as and for triaxial tension as We wish to make these expressions identical to the Mohr-Coulomb model for all values of . This is possible by setting By comparing the Mohr-Coulomb model with the linear Drucker-Prager model, and, hence, from the previous result These results for and provide linear Drucker-Prager parameters that match the Mohr- Coulomb model in triaxial compression and tension. The value of K in the linear Drucker-Prager model is restricted to to remain convex. The result for K shows that this implies Mohr-Coulomb friction angle than this value. One approach in such circumstances is to choose for the yield surface . Many real materials have a larger and then to use the remaining equations to define . This approach matches the models for triaxial compression only, while providing the closest approximation that the model can provide to failure being independent of the intermediate principal stress. If is significantly larger than 22°, this approach may provide a poor Drucker-Prager match of the Mohr-Coulomb parameters. Therefore, this matching procedure is not generally recommended; use the Mohr-Coulomb model instead. and While using one-element tests to verify the calibration of the model, it should be noted that , the Abaqus output variables SP1, SP2, and SP3 correspond to the principal stresses respectively. , and , Creep models for the linear Drucker-Prager model Classical “creep” behavior of materials that exhibit plasticity according to the extended Drucker-Prager models can be defined in Abaqus/Standard. The creep behavior in such materials is intimately tied to the plasticity behavior (through the definitions of creep flow potentials and definitions of test data), so Drucker-Prager plasticity and Drucker-Prager hardening must be included in the material definition. Creep and plasticity can be active simultaneously, in which case the resulting equations are solved in a coupled manner. To model creep only (without rate-independent plastic deformation), large values for the yield stress should be provided in the Drucker-Prager hardening definition: the result is that the material follows the Drucker-Prager model while it creeps, without ever yielding. When using this technique, a value must also be defined for the eccentricity, since, as described below, both the initial yield stress and eccentricity affect the creep potentials. This capability is limited to the linear model with a von Mises (circular) section in the deviatoric stress plane ( ; i.e., no third stress invariant effects are taken into account) and can be combined only with linear elasticity. Creep behavior defined by the extended Drucker-Prager model is active only during soils consolidation, coupled temperature-displacement, and transient quasi-static procedures. Creep formulation The creep potential is hyperbolic, similar to the plastic flow potentials used in the hyperbolic and general exponent plasticity models. If creep properties are defined in Abaqus/Standard, the linear Drucker-Prager plasticity model also uses a hyperbolic plastic flow potential. As a consequence, if two analyses are run, one in which creep is not activated and another in which creep properties are specified but produce virtually no creep flow, the plasticity solutions will not be exactly the same: the solution with creep not activated uses a linear plastic potential, whereas the solution with creep activated uses a hyperbolic plastic potential. Equivalent creep surface and equivalent creep stress We adopt the notion of the existence of creep isosurfaces of stress points that share the same creep “intensity,” as measured by an equivalent creep stress. When the material plastifies, it is desirable to have the equivalent creep surface coincide with the yield surface; therefore, we define the equivalent creep surfaces by homogeneously scaling down the yield surface. In the p–q plane that translates into parallels to the yield surface, as depicted in Figure 23.3.1–13. Abaqus/Standard requires that creep properties be described in terms of the same type of data used to define work hardening properties. The equivalent creep stress, , is then determined as follows: material point yield surface equivalent creep surface σ−cr no creep Figure 23.3.1–13 Equivalent creep stress defined as the shear stress. Figure 23.3.1–13 shows how the equivalent point is determined when the material properties are in shear, with stress d. A consequence of these concepts is that there is a cone in p–q space inside which creep is not active since any point inside this cone would have a negative equivalent creep stress. Creep flow The creep strain rate in Abaqus/Standard is assumed to follow from the same hyperbolic potential as the plastic strain rate : where is the dilation angle measured in the p–q plane at high confining pressure; is the initial yield stress taken from the user-specified Drucker- Prager hardening data; and is a parameter, referred to as the eccentricity, that defines the rate at which the function approaches the asymptote (the creep potential tends to a straight line as the eccentricity tends to zero). Suitable default values are provided for , as described below. This creep potential, which is continuous and smooth, ensures that the creep flow direction is always uniquely defined. The function approaches the linear Drucker-Prager flow potential asymptotically at high confining pressure stress and intersects the hydrostatic pressure axis at 90°. A family of hyperbolic potentials in the meridional stress plane was shown in Figure 23.3.1–6. The creep potential is the von Mises circle in the deviatoric stress plane (the -plane). The default creep potential eccentricity is , which implies that the material has almost the same dilation angle over a wide range of confining pressure stress values. Increasing the value of provides more curvature to the creep potential, implying that the dilation angle increases as the confining pressure decreases. Values of that are significantly less than the default value may lead to convergence problems if the material is subjected to low confining pressures, because of the very tight curvature of the creep potential locally where it intersects the p-axis. For details on the behavior of these models refer to “Verification of creep integration,” Section 3.2.6 of the Abaqus Benchmarks Manual. If the creep material properties are defined by a compression test, numerical problems may arise for very low stress values. Abaqus/Standard protects for such a case, as described in “Models for granular or polymer behavior,” Section 4.4.2 of the Abaqus Theory Manual. Nonassociated flow The use of a creep potential different from the equivalent creep surface implies that the material stiffness matrix is not symmetric; therefore, the unsymmetric matrix storage and solution scheme should be used . If the difference between is not large and the region of the model in which inelastic deformation is occurring is confined, it is possible that a symmetric approximation to the material stiffness matrix will give an acceptable rate of convergence and the unsymmetric matrix scheme may not be needed. and Specifying a creep law The definition of creep behavior in Abaqus/Standard is completed by specifying the equivalent “uniaxial behavior”—the creep “law.” In many practical cases the creep “law” is defined through user subroutine CREEP because creep laws are usually of very complex form to fit experimental data. Data input methods are provided for some simple cases, including two forms of a power law model and a variation of the Singh-Mitchell law. User subroutine CREEP User subroutine CREEP provides a very general capability for implementing viscoplastic models in Abaqus/Standard in which the strain rate potential can be written as a function of the equivalent stress and any number of “solution-dependent state variables.” When used in conjunction with these material models, the equivalent creep stress, , is made available in the routine. Solution-dependent state variables are any variables that are used in conjunction with the constitutive definition and whose values evolve with the solution. Examples are hardening variables associated with the model. When a more general form is required for the stress potential, user subroutine UMAT can be used. Input File Usage: *DRUCKER PRAGER CREEP, LAW=USER Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker Prager Creep: Law: User “Time hardening” form of the power law model The “time hardening” form of the power law model is where A, n, and m if defined in pure shear, where is the equivalent creep strain rate, defined so that creep stress is defined in uniaxial compression, tension, and shear creep strain; is the equivalent creep stress; is the total time; and are user-defined creep material parameters specified as functions of temperature and field variables. if the equivalent if defined in uniaxial is the engineering Input File Usage: Abaqus/CAE Usage: *DRUCKER PRAGER CREEP, LAW=TIME Property module: material editor: Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker Prager Creep: Law: Time “Strain hardening” form of the power law model As an alternative to the “time hardening” form of the power law, as defined above, the corresponding “strain hardening” form can be used: For physically reasonable behavior A and n must be positive and . Input File Usage: Abaqus/CAE Usage: *DRUCKER PRAGER CREEP, LAW=STRAIN Property module: material editor: Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker Prager Creep: Law: Strain Singh-Mitchell law A second creep law available as data input is a variation of the Singh-Mitchell law: , t, and where , specified as functions of temperature and field variables. For physically reasonable behavior A and must be positive, , and m are user-defined creep material parameters should be small compared to the total time. are defined above and A, , and Input File Usage: Abaqus/CAE Usage: *DRUCKER PRAGER CREEP, LAW=SINGHM Property module: material editor: Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker Prager Creep: Law: SinghM Numerical difficulties Depending on the choice of units for the creep laws described above, the value of A may be very small for typical creep strain rates. If A is less than , numerical difficulties can cause errors in the material calculations; therefore, use another system of units to avoid such difficulties in the calculation of creep strain increments. Creep integration Abaqus/Standard provides both explicit and implicit time integration of creep and swelling behavior. The choice of the time integration scheme depends on the procedure type, the parameters specified for the procedure, the presence of plasticity, and whether or not a geometric linear or nonlinear analysis is requested, as discussed in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4. Initial conditions When we need to study the behavior of a material that has already been subjected to some work hardening, Abaqus allows you to prescribe initial conditions for the equivalent plastic strain, , by specifying the conditions directly . For more complicated cases initial conditions can be defined in Abaqus/Standard through user subroutine HARDINI. Input File Usage: Abaqus/CAE Usage: Use the following option to specify the initial equivalent plastic strain directly: *INITIAL CONDITIONS, TYPE=HARDENING Use the following option in Abaqus/Standard to specify the initial equivalent plastic strain in user subroutine HARDINI: *INITIAL CONDITIONS, TYPE=HARDENING, USER Use the following options to specify the initial equivalent plastic strain directly: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step Use the following options in Abaqus/Standard to specify the initial equivalent plastic strain in user subroutine HARDINI: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined Elements The Drucker-Prager models can be used with the following element types: plane strain, generalized plane strain, axisymmetric, and three-dimensional solid (continuum) elements. All Drucker-Prager models are also available in plane stress (plane stress, shell, and membrane elements), except for the linear Drucker- Prager model with creep. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for the Drucker-Prager plasticity/creep model: PEEQ Equivalent plastic strain. For the linear Drucker-Prager plasticity model PEEQ is defined as ; where is the initial equivalent plastic strain (zero or user-specified; see “Initial conditions”) and is the equivalent plastic strain rate. For the hyperbolic and exponential Drucker-Prager plasticity models PEEQ is the initial equivalent plastic strain and , where is defined as CEEQ Equivalent creep strain, . is the yield stress. 23.3.2 MODIFIED DRUCKER-PRAGER/CAP MODEL Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Inelastic behavior,” Section 23.1.1 • “Material library: overview,” Section 21.1.1 • “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 • “CREEP,” Section 1.1.1 of the Abaqus User Subroutines Reference Manual • *CAP PLASTICITY • *CAP HARDENING • *CAP CREEP • “Defining cap plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The modified Drucker-Prager/Cap plasticity/creep model: • is intended to model cohesive geological materials that exhibit pressure-dependent yield, such as soils and rocks; • is based on the addition of a cap yield surface to the Drucker-Prager plasticity model (“Extended Drucker-Prager models,” Section 23.3.1), which provides an inelastic hardening mechanism to account for plastic compaction and helps to control volume dilatancy when the material yields in shear; • can be used in Abaqus/Standard to simulate creep in materials exhibiting long-term inelastic deformation through a cohesion creep mechanism in the shear failure region and a consolidation creep mechanism in the cap region; • can be used in conjunction with either the elastic material model (“Linear elastic behavior,” Section 22.2.1) or, in Abaqus/Standard if creep is not defined, the porous elastic material model (“Elastic behavior of porous materials,” Section 22.3.1); and • provides a reasonable response to large stress reversals in the cap region; however, in the failure surface region the response is reasonable only for essentially monotonic loading. Yield surface The addition of the cap yield surface to the Drucker-Prager model serves two main purposes: it bounds the yield surface in hydrostatic compression, thus providing an inelastic hardening mechanism to represent plastic compaction; and it helps to control volume dilatancy when the material yields in shear by providing softening as a function of the inelastic volume increase created as the material yields on the Drucker-Prager shear failure surface. The yield surface has two principal segments: a pressure-dependent Drucker-Prager shear failure segment and a compression cap segment, as shown in Figure 23.3.2–1. The Drucker-Prager failure segment is a perfectly plastic yield surface (no hardening). Plastic flow on this segment produces inelastic volume increase (dilation) that causes the cap to soften. On the cap surface plastic flow causes the material to compact. The model is described in detail in “Drucker-Prager/Cap model for geological materials,” Section 4.4.4 of the Abaqus Theory Manual. Transition surface, Ft Shear failure, FS α(d+patanβ) Cap, Fc d+patanβ pa R(d+patanβ) pb Figure 23.3.2–1 Modified Drucker-Prager/Cap model: yield surfaces in the p–t plane. Failure surface The Drucker-Prager failure surface is written as where and and can depend on temperature, measure t is defined as represent the angle of friction of the material and its cohesion, respectively, . The deviatoric stress , and other predefined fields and is the equivalent pressure stress, is the Mises equivalent stress, is the third stress invariant, and is the deviatoric stress. is a material parameter that controls the dependence of the yield surface on the value of the intermediate principal stress, as shown in Figure 23.3.2–2. S3 t = q 1+ 1_ ) - 1- 1_ K 3 )r )) _ 1_ Curve 1.0 0.8 S2 S1 Figure 23.3.2–2 Typical yield/flow surfaces in the deviatoric plane. The yield surface is defined so that K is the ratio of the yield stress in triaxial tension to the yield stress in triaxial compression. implies that the yield surface is the von Mises circle in the deviatoric principal stress plane (the -plane), so that the yield stresses in triaxial tension and compression are the same; this is the default behavior in Abaqus/Standard and the only behavior available in Abaqus/Explicit. To ensure that the yield surface remains convex requires . Cap yield surface The cap yield surface has an elliptical shape with constant eccentricity in the meridional (p–t) plane (Figure 23.3.2–1) and also includes dependence on the third stress invariant in the deviatoric plane (Figure 23.3.2–2). The cap surface hardens or softens as a function of the volumetric inelastic strain: volumetric plastic and/or creep compaction (when yielding on the cap and/or creeping according to the consolidation mechanism, as described later in this section) causes hardening, while volumetric plastic and/or creep dilation (when yielding on the shear failure surface and/or creeping according to the cohesion mechanism, as described later in this section) causes softening. The cap yield surface is is a material parameter that controls the shape of the cap, is a small number where that we discuss later, and is an evolution parameter that represents the volumetric inelastic strain driven hardening/softening. The hardening/softening law is a user-defined piecewise linear function relating the hydrostatic compression yield stress, , and volumetric inelastic strain (Figure 23.3.2–3): pb -(ε in vol + ε + ε ) cr vol pl vol Figure 23.3.2–3 Typical Cap hardening. The volumetric inelastic strain axis in Figure 23.3.2–3 has an arbitrary origin: is the position on this axis corresponding to the initial state of the material when the analysis begins, thus defining the position of the cap ( ) in Figure 23.3.2–1 at the start of the analysis. The evolution parameter is given as The parameter is a small number (typically 0.01 to 0.05) used to define a transition yield surface, so that the model provides a smooth intersection between the cap and failure surfaces. Defining yield surface variables In You provide the variables d, Abaqus/Standard ). If desired, combinations of these variables can also be defined as a tabular function of temperature and other predefined field variables. , and K to define the shape of the yield surface. , while in Abaqus/Explicit K = 1 ( , R, , Input File Usage: Abaqus/CAE Usage: *CAP PLASTICITY Property module: material editor: Mechanical→Plasticity→Cap Plasticity Defining hardening parameters The hardening curve specified for this model interprets yielding in the hydrostatic pressure sense: the hydrostatic pressure yield stress is defined as a tabular function of the volumetric inelastic strain, and, if desired, a function of temperature and other predefined field variables. The range of values for which is defined should be sufficient to include all values of effective pressure stress that the material will be subjected to during the analysis. Input File Usage: Abaqus/CAE Usage: *CAP HARDENING Property module: material editor: Mechanical→Plasticity→Cap Plasticity: Suboptions→Cap Hardening Plastic flow Plastic flow is defined by a flow potential that is associated in the deviatoric plane, associated in the cap region in the meridional plane, and nonassociated in the failure surface and transition regions in the meridional plane. The flow potential surface that we use in the meridional plane is shown in Figure 23.3.2–4: it is made up of an elliptical portion in the cap region that is identical to the cap yield surface, and another elliptical portion in the failure and transition regions that provides the nonassociated flow component in the model, The two elliptical portions form a continuous and smooth potential surface. Similar ellipses Gs (Shear failure) Gc (cap) d+patanβ (1+α-α secβ)(d+patanβ) pa R(d+patanβ) Figure 23.3.2–4 Modified Drucker-Prager/Cap model: flow potential in the p–t plane. Nonassociated flow Nonassociated flow implies that the material stiffness matrix is not symmetric and the unsymmetric matrix storage and solution scheme should be used in Abaqus/Standard . If the region of the model in which nonassociated inelastic deformation is occurring is confined, it is possible that a symmetric approximation to the material stiffness matrix will give an acceptable rate of convergence; in such cases the unsymmetric matrix scheme may not be needed. Calibration At least three experiments are required to calibrate the simplest version of the Cap model: a hydrostatic compression test (an oedometer test is also acceptable) and either two triaxial compression tests or one triaxial compression test and one uniaxial compression test (more than two tests are recommended for a more accurate calibration). The hydrostatic compression test is performed by pressurizing the sample equally in all directions. The applied pressure and the volume change are recorded. The uniaxial compression test involves compressing the sample between two rigid platens. The load and displacement in the direction of loading are recorded. The lateral displacements should also be recorded so that the correct volume changes can be calibrated. Triaxial compression experiments are performed using a standard triaxial machine where a fixed confining pressure is maintained while the differential stress is applied. Several tests covering the range of confining pressures of interest are usually performed. Again, the stress and strain in the direction of loading are recorded, together with the lateral strain so that the correct volume changes can be calibrated. The friction angle, Unloading measurements in these tests are useful to calibrate the elasticity, particularly in cases where the initial elastic region is not well defined. The hydrostatic compression test stress-strain curve gives the evolution of the hydrostatic CAP MODEL , required for the cap hardening curve definition. , and cohesion, d, which define the shear failure dependence on hydrostatic pressure, are calculated by plotting the failure stresses of the two triaxial compression tests (or the triaxial compression test and the uniaxial compression test) in the pressure stress (p) versus shear stress (q) space: the slope of the straight line passing through the two points gives the angle and the intersection with the q-axis gives d. For more details on the calibration of and d, see the discussion on calibration in “Extended Drucker-Prager models,” Section 23.3.1. R represents the curvature of the cap part of the yield surface and can be calibrated from a number of triaxial tests at high confining pressures (in the cap region). R must be between 0.0001 and 1000.0. Abaqus/Standard creep model Classical “creep” behavior of materials that exhibit plasticity according to the capped Drucker-Prager plasticity model can be defined in Abaqus/Standard. The creep behavior in such materials is intimately tied to the plasticity behavior (through the definitions of creep flow potentials and definitions of test data), so cap plasticity and cap hardening must be included in the material definition. If no rate-independent plastic behavior is desired in the model, large values for the cohesion, d, as well as large values for the compression yield stress, , should be provided in the plasticity definition: as a result the material follows the capped Drucker-Prager model while it creeps, without ever yielding. This capability is limited to cases in which there is no third stress invariant dependence of the yield surface ( ) and cases in which the yield surface has no transition region ( ). The elastic behavior must be defined using linear isotropic elasticity . Creep behavior defined for the modified Drucker-Prager/Cap model is active only during soils consolidation, coupled temperature-displacement, and transient quasi-static procedures. Creep formulation This model has two possible creep mechanisms that are active in different loading regions: one is a cohesion mechanism, which follows the type of plasticity active in the shear-failure plasticity region, and the other is a consolidation mechanism, which follows the type of plasticity active in the cap plasticity region. Figure 23.3.2–5 shows the regions of applicability of the creep mechanisms in p–q space. Equivalent creep surface and equivalent creep stress for the cohesion creep mechanism Consider the cohesion creep mechanism first. We adopt the notion of the existence of creep isosurfaces of stress points that share the same creep “intensity,” as measured by an equivalent creep stress. Since it is desirable to have the equivalent creep surface coincide with the yield surface, we define the equivalent creep surfaces by homogeneously scaling down the yield surface. In the p–q plane the equivalent creep surfaces translate into surfaces that are parallel to the yield surface, as depicted in Figure 23.3.2–6. cohesion and consolidation creep n c r e si o (d+patanβ) no creep consolidation creep pa R(d+patanβ) Figure 23.3.2–5 Regions of activity of creep mechanisms. Abaqus/Standard requires that cohesion creep properties be measured in a uniaxial compression test. The equivalent creep stress, , is determined as follows: Abaqus/Standard also requires that be positive. Figure 23.3.2–6 shows such an equivalent creep stress. A consequence of these concepts is that there is a cone in p–q space inside which creep is not active. Any point inside this cone would have a negative equivalent creep stress. Equivalent creep surface and equivalent creep stress for the consolidation creep mechanism Next, consider the consolidation creep mechanism. In this case we wish to make creep dependent on the hydrostatic pressure above a threshold value of , with a smooth transition to the areas in which the mechanism is not active ( ). Therefore, we define equivalent creep surfaces as constant hydrostatic pressure surfaces (vertical lines in the p–q plane). Abaqus/Standard requires that consolidation creep properties be measured in a hydrostatic compression test. The effective creep pressure, , is then the point on the p-axis with a relative pressure of . This value is used in the uniaxial creep law. The equivalent volumetric creep strain rate produced by this type of law is defined as positive for a positive equivalent pressure. The internal tensor calculations in Abaqus/Standard account for the fact that a positive pressure will produce negative (that is, compressive) volumetric creep components. yield surface material point equivalent creep surface σ−cr no creep Figure 23.3.2–6 Equivalent creep stress for cohesion creep. Creep flow The creep strain rate produced by the cohesion mechanism is assumed to follow a potential that is similar to that of the creep strain rate in the Drucker-Prager creep model (“Extended Drucker-Prager models,” Section 23.3.1); that is, a hyperbolic function: This creep flow potential, which is continuous and smooth, ensures that the flow direction is always uniquely defined. The function approaches a parallel to the shear-failure yield surface asymptotically at high confining pressure stress and intersects the hydrostatic pressure axis at a right angle. A family of hyperbolic potentials in the meridional stress plane is shown in Figure 23.3.2–7. The cohesion creep potential is the von Mises circle in the deviatoric stress plane (the -plane). Abaqus/Standard protects for numerical problems that may arise for very low stress values. See “Drucker-Prager/Cap model for geological materials,” Section 4.4.4 of the Abaqus Theory Manual, for details. The creep strain rate produced by the consolidation mechanism is assumed to follow a potential that is similar to that of the plastic strain rate in the cap yield surface (Figure 23.3.2–8): The consolidation creep potential is the von Mises circle in the deviatoric stress plane (the -plane). The volumetric components of creep strain from both mechanisms contribute to the hardening/softening of the cap, as described previously. For details on the behavior of these models refer to “Verification of creep integration,” Section 3.2.6 of the Abaqus Benchmarks Manual. Δε cr Δε cr similar hyperboles material point Figure 23.3.2–7 Cohesion creep potentials in the p–q plane. pa material point Δε cr similar ellipses pa Δε cr Figure 23.3.2–8 Consolidation creep potentials in the p–q plane. Nonassociated flow The use of a creep potential for the cohesion mechanism different from the equivalent creep surface implies that the material stiffness matrix is not symmetric, and the unsymmetric matrix storage and If the region of the solution scheme should be used . model in which cohesive inelastic deformation is occurring is confined, it is possible that a symmetric approximation to the material stiffness matrix will give an acceptable rate of convergence; in such cases the unsymmetric matrix scheme may not be needed. Specifying creep laws The definition of the creep behavior is completed by specifying the equivalent “uniaxial behavior”—the creep “laws.” In many practical cases the creep laws are defined through user subroutine CREEP because creep laws are usually of complex form to fit experimental data. Data input methods are provided for some simple cases. User subroutine CREEP User subroutine CREEP provides a general capability for implementing viscoplastic models in which the strain rate potential can be written as a function of the equivalent stress and any number of “solution- dependent state variables.” When used in conjunction with these materials, the equivalent cohesion creep stress, , are made available in the routine. Solution-dependent state variables are any variables that are used in conjunction with the constitutive definition and whose values evolve with the solution. Examples are hardening variables associated with the model. When a more general form is required for the stress potential, user subroutine UMAT can be used. , and the effective creep pressure, Input File Usage: Abaqus/CAE Usage: Use either or both of the following options: *CAP CREEP, MECHANISM=COHESION, LAW=USER *CAP CREEP, MECHANISM=CONSOLIDATION, LAW=USER Define one or both of the following: Property module: material editor: Mechanical→Plasticity→Cap Plasticity: Suboptions→Cap Creep Cohesion: Law: User Suboptions→Cap Creep Consolidation: Law: User “Time hardening” form of the power law model With respect to the cohesion mechanism, the power law is available where A, n, and m is the equivalent creep strain rate; is the equivalent cohesion creep stress; is the total time; and are user-defined creep material parameters specified as functions of temperature and field variables. In using this form of the power law model with the consolidation mechanism, can be replaced by , the effective creep pressure, in the above relation. Input File Usage: Use either or both of the following options: *CAP CREEP, MECHANISM=COHESION, LAW=TIME *CAP CREEP, MECHANISM=CONSOLIDATION, LAW=TIME Abaqus/CAE Usage: Define one or both of the following: Property module: material editor: Mechanical→Plasticity→Cap Plasticity: Suboptions→Cap Creep Cohesion: Law: Time Suboptions→Cap Creep Consolidation: Law: Time “Strain hardening” form of the power law model As an alternative to the “time hardening” form of the power law, as defined above, the corresponding “strain hardening” form can be used. For the cohesion mechanism this law has the form In using this form of the power law model with the consolidation mechanism, can be replaced by , the effective creep pressure, in the above relation. Input File Usage: For physically reasonable behavior A and n must be positive and Use either or both of the following options: *CAP CREEP, MECHANISM=COHESION, LAW=STRAIN *CAP CREEP, MECHANISM=CONSOLIDATION, LAW=STRAIN Define one or both of the following: . Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Cap Plasticity: Suboptions→Cap Creep Cohesion: Law: Strain Suboptions→Cap Creep Consolidation: Law: Strain Singh-Mitchell law A second cohesion creep law available as data input is a variation of the Singh-Mitchell law: , t, and , where specified as functions of temperature and field variables. For physically reasonable behavior A and must be positive, , and m are user-defined creep material parameters should be small compared to the total time. are defined above and A, , and In using this variation of the Singh-Mitchell law with the consolidation mechanism, can be replaced by , the effective creep pressure, in the above relation. Input File Usage: Abaqus/CAE Usage: Use either or both of the following options: *CAP CREEP, MECHANISM=COHESION, LAW=SINGHM *CAP CREEP, MECHANISM=CONSOLIDATION, LAW=SINGHM Define one or both of the following: Property module: material editor: Mechanical→Plasticity→Cap Plasticity: Suboptions→Cap Creep Cohesion: Law: SinghM Suboptions→Cap Creep Consolidation: Law: SinghM Numerical difficulties Depending on the choice of units for the creep laws described above, the value of A may be very small for typical creep strain rates. If A is less than 10−27, numerical difficulties can cause errors in the material calculations; therefore, use another system of units to avoid such difficulties in the calculation of creep strain increments. Creep integration Abaqus/Standard provides both explicit and implicit time integration of creep and swelling behavior. The choice of the time integration scheme depends on the procedure type, the parameters specified for the procedure, the presence of plasticity, and whether or not a geometric linear or nonlinear analysis is requested, as discussed in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4. Initial conditions The initial stress at a point can be defined . If such a stress point lies outside the initially defined cap or transition yield surfaces and under the projection of the shear failure surface in the p–t plane (illustrated in Figure 23.3.2–1), Abaqus will try to adjust the initial position of the cap to make the stress point lie on the yield surface and a warning message will be issued. If the stress point lies outside the Drucker-Prager failure surface (or above its projection), an error message will be issued and execution will be terminated. Elements The modified Drucker-Prager/Cap material behavior can be used with plane strain, generalized plane strain, axisymmetric, and three-dimensional solid (continuum) elements. This model cannot be used with elements for which the assumed stress state is plane stress (plane stress, shell, and membrane elements). Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning in the cap plasticity/creep model: PEEQ PEQC , the cap position. Equivalent plastic strains for all three possible yield/failure surfaces (Drucker- Prager failure surface - PEQC1, cap surface - PEQC2, and transition surface - PEQC3) and the total volumetric inelastic strain (PEQC4). For each yield/failure is the surface, the equivalent plastic strain is corresponding rate of plastic flow. The total volumetric inelastic strain is defined as where CEEQ CESW Equivalent creep strain produced by the cohesion creep mechanism, defined as where is the equivalent creep stress. Equivalent creep strain produced by the consolidation creep mechanism, defined as is the equivalent creep pressure. , where 23.3.3 MOHR-COULOMB PLASTICITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *MOHR COULOMB • *MOHR COULOMB HARDENING • *TENSION CUTOFF • “Defining Mohr-Coulomb plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The Mohr-Coulomb plasticity model: • is used to model materials with the classical Mohr-Coloumb yield criterion; • allows the material to harden and/or soften isotropically; • uses a smooth flow potential that has a hyperbolic shape in the meridional stress plane and a piecewise elliptic shape in the deviatoric stress plane; • is used with the linear elastic material model (“Linear elastic behavior,” Section 22.2.1); • can be used with the Rankine surface (tension cutoff) to limit load carrying capacity near the tensile region; and • can be used for design applications in the geotechnical engineering area to simulate material response under essentially monotonic loading. Elastic behavior The elastic part of the response is specified as described in “Linear elastic behavior,” Section 22.2.1. Linear isotropic elasticity is assumed. Plastic behavior: yield criteria The yield surface is a composite of two different criteria: a shear criterion, known as the Mohr-Coulomb surface, and an optional tension cutoff criterion, modeled using the Rankine surface. Mohr-Coulomb surface The Mohr-Coulomb criterion assumes that yield occurs when the shear stress on any point in a material reaches a value that depends linearly on the normal stress in the same plane. The Mohr-Coulomb model is based on plotting Mohr’s circle for states of stress at yield in the plane of the maximum and minimum principal stresses. The yield line is the best straight line that touches these Mohr’s circles (Figure 23.3.3–1). s = σ 1 σ - m= 1+σ 2 σ (compressive stress) Figure 23.3.3–1 Mohr-Coulomb yield model. Therefore, the Mohr-Coulomb model is defined by where is negative in compression. From Mohr’s circle, Substituting for and , multiplying both sides by , and reducing, the Mohr-Coulomb model can be written as where is half of the difference between the maximum principal stress, (and is, therefore, the maximum shear stress), , and the minimum principal stress, is the average of the maximum and minimum principal stresses, and is the friction angle. For general states of stress the model is more conveniently written in terms of three stress invariants as where and is the slope of the Mohr-Coulomb yield surface in the p– stress plane , which is commonly referred to as the friction angle of the material and can depend on temperature and predefined field variables; is the cohesion of the material; and is the deviatoric polar angle defined as is the equivalent pressure stress, is the Mises equivalent stress, is the third invariant of deviatoric stress, and is the deviatoric stress. The friction angle, , controls the shape of the yield surface in the deviatoric plane as shown in Figure 23.3.3–2. The tension cutoff surface is shown for a meridional angle of . The friction angle range is the Mohr-Coulomb model reduces to the pressure- independent Tresca model with a perfectly hexagonal deviatoric section. In the case of the Mohr-Coulomb model reduces to the “tension cutoff” Rankine model with a triangular deviatoric section and (this limiting case is not permitted within the Mohr-Coulomb model described here). . In the case of When using one-element tests to verify the calibration of the model, the output variables SP1, SP2, , and and SP3 correspond to the principal stresses , respectively. , Tension cutoff Mohr-Coulomb Rmcq Meridional plane Θ = 0 Mohr-Coulomb (φ = 20°) Tresca (φ = 0°) Rankine (φ = 90°) Θ = 4π/3 Drucker-Prager (Mises) Θ = π/3 Θ = 2π/3 Deviatoric plane Figure 23.3.3–2 Mohr-Coulomb and tension cutoff surfaces in meridional and deviatoric planes. Isotropic cohesion hardening is assumed for the hardening behavior of the Mohr-Coulomb yield surface. The hardening curve must describe the cohesion yield stress as a function of plastic strain and, possibly, temperature and predefined field variables. In defining this dependence at finite strains, “true” (Cauchy) stress and logarithmic strain values should be given. An optional tension cutoff hardening (or softening) curve can be specified Rate dependency effects are not accounted for in this plasticity model. Input File Usage: Use the following options to specify the Mohr-Coulomb yield surface and cohesion hardening: Abaqus/CAE Usage: *MOHR COULOMB *MOHR COULOMB HARDENING Use the following options to specify the Mohr-Coulomb yield surface and cohesion hardening: Property module: material editor: Mechanical→Plasticity→Mohr Coulomb Plasticity Property module: material editor: Mechanical→Plasticity→Mohr Coulomb Plasticity: Cohesion Rankine surface In Abaqus tension cutoff is modeled using the Rankine surface, which is written as where the Rankine surface, as a function of tensile equivalent plastic strain, , and is the tension cutoff value representing softening (or hardening) of . Input File Usage: Use the following option to specify hardening or softening for the Rankine surface: Abaqus/CAE Usage: *TENSION CUTOFF Use the following option to specify hardening or softening for the Rankine surface: Property module: material editor: Mechanical→Plasticity→Mohr Coulomb Plasticity: toggle on Specify tension cutoff; Tension Cutoff Plastic behavior: flow potentials The flow potentials used for the Mohr-Coulomb yield surface and the tension cutoff surface are described below. Plastic flow on the Mohr-Coulomb yield surface The flow potential, G, for the Mohr-Coulomb yield surface is chosen as a hyperbolic function in the meridional stress plane and the smooth elliptic function proposed by Menétrey and Willam (1995) in the deviatoric stress plane: where and is the dilation angle measured in the p– depend on temperature and predefined field variables; plane at high confining pressure and can is the initial cohesion yield stress, ; is the deviatoric polar angle defined previously; is a parameter, referred to as the meridional eccentricity, that defines the rate at which the hyperbolic function approaches the asymptote (the flow potential tends to a straight line in the meridional stress plane as the meridional eccentricity tends to zero); and is a parameter, referred to as the deviatoric eccentricity, that describes the “out-of- roundedness” of the deviatoric section in terms of the ratio between the shear stress along the extension meridian ( ) and the shear stress along the compression meridian ( ). A default value of is provided for the meridional eccentricity, . By default, the deviatoric eccentricity, e, is calculated as is the Mohr-Coulomb friction angle; this calculation corresponds to matching the flow potential where to the yield surface in both triaxial tension and compression in the deviatoric plane. Alternatively, Abaqus allows you to consider this deviatoric eccentricity as an independent material parameter; in this case you provide its value directly. Convexity and smoothness of the elliptic function requires that . The upper limit, 0° when you do not specify the value of e), leads to (or 90° when you do not specify the value of e), leads to , which describes the Mises circle in the deviatoric plane. The lower limit, (or and would describe the Rankine triangle in the deviatoric plane (this limiting case is not permitted within the Mohr-Coulomb model described here). This flow potential, which is continuous and smooth, ensures that the flow direction is always uniquely defined. A family of hyperbolic potentials in the meridional stress plane is shown in Figure 23.3.3–3, and the flow potential in the deviatoric stress plane is shown in Figure 23.3.3–4. dεpl Rmwq εc |0 Figure 23.3.3–3 Family of hyperbolic flow potentials in the meridional stress plane. Θ = 0 Rankine (e = 1/2) Θ = π/3 Θ = 2π/3 Menetrey-Willam (1/2 < e ≤ 1) Θ = 4π/3 Mises (e = 1) Figure 23.3.3–4 Menétrey-Willam flow potential in the deviatoric stress plane. Flow in the meridional stress plane can be close to associated when the angle of friction, the angle of dilation, plane is, in general, nonassociated. Flow in the deviatoric stress plane is always nonassociated. , are equal and the meridional eccentricity, , and , is very small; however, flow in this Input File Usage: Use the following option to allow Abaqus to calculate the value of e (default): *MOHR COULOMB Use the following option to specify the value of e directly: *MOHR COULOMB, DEVIATORIC ECCENTRICITY=e Abaqus/CAE Usage: Use the following option to allow Abaqus to calculate the value of e (default): Property module: material editor: Mechanical→Plasticity→Mohr Coulomb Plasticity: Plasticity: Deviatoric eccentricity: Calculated default Use the following option to specify the value of e directly: Property module: material editor: Mechanical→Plasticity→Mohr Coulomb Plasticity: Plasticity: Deviatoric eccentricity: Specify: e Plastic flow on the Rankine surface A flow potential that results in a nearly associative flow is chosen for the Rankine surface and is constructed by modifying the Menétrey-Willam potential described earlier: where is the initial value of tension cutoff; is the meridional eccentricity, similar to defined earlier; and is the deviatoric eccentricity, similar to defined earlier. Abaqus uses values of and , for and , respectively. Nonassociated flow Since the plastic flow is nonassociated in general, the use of this Mohr-Coulomb model generally requires the unsymmetric matrix storage and solution scheme in Abaqus/Standard . Elements The Mohr-Coulomb plasticity model can be used with any stress/displacement elements other than one- dimensional elements (beam, pipe, and truss elements) or elements for which the assumed stress state is plane stress (plane stress, shell, and membrane elements). Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable the identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), following variables are available for the Mohr-Coulomb plasticity model: PEEQ PEEQT Equivalent plastic strain, Tensile equivalent plastic strain, , where c is the cohesion yield stress. , on the tension cutoff yield surface. Additional reference • Menétrey, Ph., and K. J. Willam, “Triaxial Failure Criterion for Concrete and its Generalization,” ACI Structural Journal, vol. 92, pp. 311–318, May/June 1995. 23.3.4 CRITICAL STATE (CLAY) PLASTICITY MODEL Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *CLAY PLASTICITY • *CLAY HARDENING • “Defining clay plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Critical state models,” Section 4.4.3 of the Abaqus Theory Manual Overview The clay plasticity model provided in Abaqus: • describes the inelastic behavior of the material by a yield function that depends on the three stress invariants, an associated flow assumption to define the plastic strain rate, and a strain hardening theory that changes the size of the yield surface according to the inelastic volumetric strain; • requires that the elastic part of the deformation be defined by using the linear elastic material model (“Linear elastic behavior,” Section 22.2.1) or, in Abaqus/Standard, the porous elastic material model (“Elastic behavior of porous materials,” Section 22.3.1) within the same material definition; and • allows for the hardening law to be defined by a piecewise linear form or, in Abaqus/Standard, by an exponential form. Yield surface The model is based on the yield surface is the equivalent pressure stress; is a deviatoric stress measure; is the Mises equivalent stress; is the third stress invariant; is a constant that defines the slope of the critical state line; 23.3.4–1 where is a constant that is equal to 1.0 on the “dry” side of the critical state line ( ) but may be different from 1.0 on the “wet” side of the critical state line ( introduces a different ellipse on the wet side of the critical state line; i.e., a tighter “cap” is obtained if as shown in Figure 23.3.4–1); is the size of the yield surface (Figure 23.3.4–1); and is the ratio of the flow stress in triaxial tension to the flow stress in triaxial compression and determines the shape of the yield surface in the plane of principal deviatoric stresses (the “ -plane”: see Figure 23.3.4–2); Abaqus requires that to ensure that the yield surface remains convex. The user-defined parameters M, variables, Theory Manual. as well as other predefined field . The model is described in detail in “Critical state models,” Section 4.4.3 of the Abaqus , and K can depend on temperature Input File Usage: Abaqus/CAE Usage: *CLAY PLASTICITY Property module: material editor: Mechanical→Plasticity→Clay Plasticity critical state line K = 1.0 β = 0.5 β = 1.0 Figure 23.3.4–1 Clay yield surfaces in the p–t plane. S3 t = 1_ q 1+ 1_ - 1- 1_ ) K 3 )r )) _ Curve 1.0 0.8 S2 Figure 23.3.4–2 Clay yield surface sections in the -plane. S1 Hardening law The hardening law can have an exponential form (Abaqus/Standard only), or a piecewise linear form. Exponential form in Abaqus/Standard The exponential form of the hardening law is written in terms of some of the porous elasticity parameters and, therefore, can be used only in conjunction with the Abaqus/Standard porous elastic material model. The size of the yield surface at any time is determined by the initial value of the hardening parameter, , and the amount of inelastic volume change that occurs according to the equation where is the inelastic volume change (that part of J, the ratio of current volume to initial volume, attributable to inelastic deformation); is the logarithmic bulk modulus of the material defined for the porous elastic material behavior; is the logarithmic hardening constant defined for the clay plasticity material behavior; and is the user-defined initial void ratio (“Defining initial void ratios in a porous medium” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Specifying the initial size of the yield surface directly The initial size of the yield surface is defined for clay plasticity by specifying the hardening parameter, , as a tabular function or by defining it analytically. can be defined along with , M, , and K, as a tabular function of temperature and other is a function only of the initial conditions; it will not change if predefined field variables. However, temperatures and field variables change during the analysis. Input File Usage: Use all of the following options: *INITIAL CONDITIONS, TYPE=RATIO *POROUS ELASTIC *CLAY PLASTICITY, HARDENING=EXPONENTIAL Use all of the following options: Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Porous Elastic Mechanical→Plasticity→Clay Plasticity: Hardening: Exponential Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step Specifying the initial size of the yield surface indirectly , which is the intercept of the The hardening parameter virgin consolidation line with the void ratio axis in the plot of void ratio, e, versus the logarithm of the effective pressure stress, (Figure 23.3.4–3). If this method is used, can be defined indirectly by specifying is defined by where is the user-defined initial value of the equivalent hydrostatic pressure stress . You define can be dependent on temperature and other predefined field variables. However, is a function only of the initial conditions; it will not change if temperatures and field variables change during the analysis. , and K; all the parameters except , M, , Input File Usage: Use all of the following options: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=RATIO *INITIAL CONDITIONS, TYPE=STRESS *POROUS ELASTIC *CLAY PLASTICITY, HARDENING=EXPONENTIAL, INTERCEPT= Use all of the following options: Property module: material editor: Mechanical→Elasticity→Porous Elastic e1 - locates initial consolidation state, by the intercept of the plastic line with In p = 0. , elastic slope de d( In p) = -κ plastic slope de d( In p) = -λ In p (p = effective pressure stress) Figure 23.3.4–3 Pure compression behavior for clay model. Mechanical→Plasticity→Clay Plasticity: Hardening: Exponential, Intercept: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Stress for the Types for Selected Step Piecewise linear form If the piecewise linear form of the hardening rule is used, the user-defined relationship relates the yield stress in hydrostatic compression, (Figure 23.3.4–4): to the corresponding volumetric plastic strain, , The evolution parameter, a, is then given by 0C -ε pl vol -(ε pl vol + ε ) pl vol Figure 23.3.4–4 Typical piecewise linear clay hardening/softening curve. The volumetric plastic strain axis has an arbitrary origin: to the initial state of the material, thus defining the initial hydrostatic pressure, yield surface size, values for which which the material will be subjected during the analysis. is the position on this axis corresponding , and, hence, the initial . This relationship is defined in tabular form as clay hardening data. The range of is defined should be sufficient to include all values of equivalent pressure stress to This form of the hardening law can be used in conjunction with either the linear elastic or, in Abaqus/Standard, the porous elastic material models. This is the only form of the hardening law supported in Abaqus/Explicit Input File Usage: Abaqus/CAE Usage: Use both of the following options: *CLAY PLASTICITY, HARDENING=TABULAR *CLAY HARDENING Property module: material editor: Mechanical→Plasticity→Clay Plasticity: Hardening: Tabular, Suboptions→Clay Hardening Calibration At least two experiments are required to calibrate the simplest version of the Cam-clay model: a hydrostatic compression test (an oedometer test is also acceptable) and a triaxial compression test (more than one triaxial test is useful for a more accurate calibration). Hydrostatic compression tests The hydrostatic compression test is performed by pressurizing the sample equally in all directions. The applied pressure and the volume change are recorded. The onset of yielding in the hydrostatic compression test immediately provides the initial position of the yield surface, and , are determined from the hydrostatic compression experimental data by plotting the logarithm of pressure versus void ratio. The void ratio, e, is related to the measured volume change as . The logarithmic bulk moduli, The slope of the line obtained for the elastic regime is a valid model . , and the slope in the inelastic range is . For Triaxial tests Triaxial compression experiments are performed using a standard triaxial machine where a fixed confining pressure is maintained while the differential stress is applied. Several tests covering the range of confining pressures of interest are usually performed. Again, the stress and strain in the direction of loading are recorded, together with the lateral strain so that the correct volume changes can be calibrated. The triaxial compression tests allow the calibration of the yield parameters M and . M is the ratio of the shear stress, q, to the pressure stress, p, at critical state and can be obtained from the stress values when the material has become perfectly plastic (critical state). represents the curvature of the cap part of the yield surface and can be calibrated from a number of triaxial tests at high confining pressures (on the “wet” side of critical state). must be between 0.0 and 1.0. To calibrate the parameter K, which controls the yield dependence on the third stress invariant, experimental results obtained from a true triaxial (cubical) test are necessary. These results are generally not available, and you may have to guess (the value of K is generally between 0.8 and 1.0) or ignore this effect. Unloading measurements Unloading measurements in hydrostatic and triaxial compression tests are useful to calibrate the elasticity, particularly in cases where the initial elastic region is not well defined. From these we can identify whether a constant shear modulus or a constant Poisson’s ratio should be used and what their values are. Initial conditions If an initial stress at a point is given such that the stress point lies outside the initially defined yield surface, Abaqus will try to adjust the initial position of the surface to make the stress point lie on it and issue a warning. However, if the stress point is such that the equivalent pressure stress, p, is negative, an error message will be issued and execution will be terminated. Elements The clay plasticity model can be used with plane strain, generalized plane strain, axisymmetric, and three-dimensional solid (continuum) elements in Abaqus. This model cannot be used with elements for which the assumed stress state is plane stress (plane stress, shell, and membrane elements). Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variable has special meaning for material points in the clay plasticity model: PEEQ Center of the yield surface, a. 23.3.5 CRUSHABLE FOAM PLASTICITY MODELS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • “Rate-dependent yield,” Section 23.2.3 • *CRUSHABLE FOAM • *CRUSHABLE FOAM HARDENING • *RATE DEPENDENT • “Defining crushable foam plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The crushable foam plasticity models: • are intended for the analysis of crushable foams that are typically used as energy absorption structures; • can be used to model crushable materials other than foams (such as balsa wood); • are used to model the enhanced ability of a foam material to deform in compression due to cell wall buckling processes (it is assumed that the resulting deformation is not recoverable instantaneously and can, thus, be idealized as being plastic for short duration events); • can be used to model the difference between a foam material’s compressive strength and its much smaller tensile bearing capacity resulting from cell wall breakage in tension; • must be used in conjunction with the linear elastic material model (“Linear elastic behavior,” Section 22.2.1); • can be used when rate-dependent effects are important; and • are intended to simulate material response under essentially monotonic loading. Elastic and plastic behavior The elastic part of the response is specified as described in “Linear elastic behavior,” Section 22.2.1. Only linear isotropic elasticity can be used. For the plastic part of the behavior, the yield surface is a Mises circle in the deviatoric stress plane and an ellipse in the meridional (p–q) stress plane. Two hardening models are available: the volumetric hardening model, where the point on the yield ellipse in the meridional plane that represents hydrostatic tension loading is fixed and the evolution of the yield surface is driven by the volumetric compacting plastic strain, and the isotropic hardening model, where the yield ellipse is centered at the origin in the p–q stress plane and evolves in a geometrically self-similar manner. This phenomenological isotropic model was originally developed for metallic foams by Deshpande and Fleck (2000). The hardening curve must describe the uniaxial compression yield stress as a function of the corresponding plastic strain. In defining this dependence at finite strains, “true” (Cauchy) stress and logarithmic strain values should be given. Both models predict similar behavior for compression-dominated loading. However, for hydrostatic tension loading the volumetric hardening model assumes a perfectly plastic behavior, while the isotropic hardening model predicts the same behavior in both hydrostatic tension and hydrostatic compression. Crushable foam model with volumetric hardening The crushable foam model with volumetric hardening uses a yield surface with an elliptical dependence of deviatoric stress on pressure stress. It assumes that the evolution of the yield surface is controlled by the volumetric compacting plastic strain experienced by the material. Yield surface The yield surface for the volumetric hardening model is defined as where is the pressure stress, is the Mises stress, is the deviatoric stress, is the size of the (horizontal) p-axis of the yield ellipse, is the size of the (vertical) q-axis of the yield ellipse, is the shape factor of the yield ellipse that defines the relative magnitude of the axes, is the center of the yield ellipse on the p-axis, is the strength of the material in hydrostatic tension, and is the yield stress in hydrostatic compression ( positive). is always The yield surface represents the Mises circle in the deviatoric stress plane and is an ellipse on the meridional stress plane, as depicted in Figure 23.3.5–1. uniaxial compression σ flow potential original surface yield surface -pt σ 0 -pt pc pc pc Figure 23.3.5–1 Crushable foam model with volumetric hardening: yield surface and flow potential in the p–q stress plane. The yield surface evolves in a self-similar fashion (constant computed using the initial yield stress in uniaxial compression, compression, (the initial value of ), and the yield strength in hydrostatic tension, : ); and the shape factor can be , the initial yield stress in hydrostatic with and For a valid yield surface the choice of strength ratios must be such that not the case, Abaqus will issue an error message and terminate execution. To define the shape of the yield surface, you provide the values of k and and . If this is . If desired, these variables can be defined as a tabular function of temperature and other predefined field variables. Input File Usage: Abaqus/CAE Usage: *CRUSHABLE FOAM, HARDENING=VOLUMETRIC Property module: material editor: Mechanical→Plasticity→Crushable Foam: Hardening: Volumetric Calibration ; the initial To use this model, one needs to know the initial yield stress in uniaxial compression, yield stress in hydrostatic compression, . Since foam ; and the yield strength in hydrostatic tension, materials are rarely tested in tension, it is usually necessary to guess the magnitude of the strength of the foam in hydrostatic tension, . The choice of tensile strength should not have a strong effect on the numerical results unless the foam is stressed in hydrostatic tension. A common approximation is to set equal to 5% to 10% of the initial yield stress in hydrostatic compression ; thus, = 0.05 to 0.10. Flow potential The plastic strain rate for the volumetric hardening model is assumed to be where G is the flow potential, chosen in this model as and is the equivalent plastic strain rate defined as The equivalent plastic strain rate is related to the rate of axial plastic strain, by , in uniaxial compression A geometrical representation of the flow potential in the p–q stress plane is shown in Figure 23.3.5–1. This potential gives a direction of flow that is identical to the stress direction for radial paths. This is motivated by simple laboratory experiments that suggest that loading in any principal direction causes insignificant deformation in the other directions. As a result, the plastic flow is nonassociative for the volumetric hardening model. For more details regarding plastic flow, see “Plasticity models: general discussion,” Section 4.2.1 of the Abaqus Theory Manual. Nonassociated flow The nonassociated plastic flow rule makes the material stiffness matrix unsymmetric; therefore, the unsymmetric matrix storage and solution scheme should be used in Abaqus/Standard . Usage of this scheme is especially important when large regions of the model are expected to flow plastically. Hardening remains fixed throughout any The yield surface intersects the p-axis at plastic deformation process. By contrast, the compressive strength, , evolves as a result of compaction (increase in density) or dilation (reduction in density) of the material. The evolution of the yield surface can be expressed through the evolution of the yield surface size on the hydrostatic stress axis, , as a function of the value of volumetric compacting plastic strain, constant, this relation can be obtained from user-provided uniaxial compression test data using . We assume that . With and along with the fact that in uniaxial compression for the volumetric hardening model. Thus, you provide input to the hardening law by specifying, in the usual tabular form, only the value of the yield stress in uniaxial compression as a function of the absolute value of the axial plastic strain. The table must start with a zero plastic strain (corresponding to the virgin state of the material), and the tabular entries must be given in ascending magnitude of . If desired, the yield stress can also be a function of temperature and other predefined field variables. Input File Usage: Abaqus/CAE Usage: *CRUSHABLE FOAM HARDENING Property module: material editor: Mechanical→Plasticity→Crushable Foam: Suboptions→Foam Hardening Rate dependence As strain rates increase, many materials show an increase in the yield stress. For many crushable foam materials this increase in yield stress becomes important when the strain rates are in the range of 0.1–1 per second and can be very important if the strain rates are in the range of 10–100 per second, as commonly occurs in high-energy dynamic events. Two methods for specifying strain-rate-dependent material behavior are available in Abaqus as discussed below. Both methods assume that the shapes of the hardening curves at different strain rates are similar, and either can be used in static or dynamic procedures. When rate dependence is included, the static stress-strain hardening behavior must be specified for the crushable foam as described above. Overstress power law You can specify a Cowper-Symonds overstress power law that defines strain rate dependence. This law has the form with where B is the size of the static yield surface and rate. The ratio R can be written as is the size of the yield surface at a nonzero strain where r is the uniaxial compression yield stress ratio defined by , specified as part of the crushable foam hardening definition, is the uniaxial compression yield stress at a given value of for the experiment with the lowest strain rate and can depend on temperature and predefined field variables; D and n are material parameters that can be functions of temperature and, possibly, of other predefined field variables. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *CRUSHABLE FOAM HARDENING *RATE DEPENDENT, TYPE=POWER LAW Property module: material editor: Mechanical→Plasticity→Crushable Foam: Suboptions→Foam Hardening; Suboptions→Rate Dependent: Hardening: Power Law The power-law rate dependency can be rewritten in the following form The procedure outlined below can be followed to obtain the material parameters D and n based on the uniaxial compression test data. 1. Compute R using the uniaxial compression yield stress ratio, r. 2. Convert the rate of the axial plastic strain, , to the corresponding equivalent plastic strain rate, . 3. Plot versus shown in Figure 23.3.5–2, the overstress power law is suitable. The slope of the line is the intercept of the . If the curve can be approximated by a straight line such as that , and axis is . ln p - p p + p t ln (D) ε pl ( ) ln Figure 23.3.5–2 Calibration of overstress power law data. Tabular input of yield ratio as a Rate-dependent behavior can alternatively be specified by giving a table of the ratio function of the absolute value of the rate of the axial plastic strain and, optionally, temperature and predefined field variables. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *CRUSHABLE FOAM HARDENING *RATE DEPENDENT, TYPE=YIELD RATIO Property module: material editor: Mechanical→Plasticity→Crushable Foam: Suboptions→Foam Hardening; Suboptions→Rate Dependent: Hardening: Yield Ratio Initial conditions When we need to study the behavior of a material that has already been subjected to some hardening, Abaqus allows you to prescribe initial conditions for the volumetric compacting plastic strain, . Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step Crushable foam model with isotropic hardening The isotropic hardening model uses a yield surface that is an ellipse centered at the origin in the p–q stress plane. The yield surface evolves in a self-similar manner, and the evolution is governed by the equivalent plastic strain (to be defined later). Yield surface The yield surface for the isotropic hardening model is defined as where is the pressure stress, is the Mises stress, is the deviatoric stress, is the size of the (vertical) q-axis of the yield ellipse, is the shape factor of the yield ellipse that defines the relative magnitude of the axes, is the yield stress in hydrostatic compression, and is the absolute value of the yield stress in uniaxial compression. The yield surface represents the Mises circle in the deviatoric stress plane. The shape of the yield surface , can be computed using in the meridional stress plane is depicted in Figure 23.3.5–3. The shape factor, the initial yield stress in uniaxial compression, , and the initial yield stress in hydrostatic compression, ), using the relation: (the initial value of with and . The particular case of To define the shape of the yield ellipse, you provide the value of k. For a valid yield surface the strength ratio must be such that corresponds to the Mises plasticity. In general, the initial yield strengths in uniaxial compression and in hydrostatic compression, , can be used to calculate the value of k. However, in many practical cases the stress versus strain response curves of crushable foam materials do not show clear yielding points, and the initial yield stress values cannot be determined exactly. Many of these response curves have a horizontal plateau—the yield stress is nearly a constant for a significantly large range of plastic strain values. If you have data from both uniaxial compression and hydrostatic compression, the plateau values of the two experimental curves can be used to calculate the ratio of k. Input File Usage: Abaqus/CAE Usage: *CRUSHABLE FOAM, HARDENING=ISOTROPIC Property module: material editor: Mechanical→Plasticity→Crushable Foam: Hardening: Isotropic Flow potential The flow potential for the isotropic hardening model is chosen as flow potential uniaxial compression CRUSHABLE FOAM yield surface original surface -pc -p c σ pc pc Figure 23.3.5–3 Crushable foam model with isotropic hardening: yield surface and flow potential in the p–q stress plane. where plastic Poisson’s ratio, , via represents the shape of the flow potential ellipse on the p–q stress plane. It is related to the The plastic Poisson’s ratio, which is the ratio of the transverse to the longitudinal plastic strain under uniaxial compression, must be in the range of −1 and 0.5; and the upper limit ( ) corresponds to the case of incompressible plastic flow ( ). For many low-density foams the plastic Poisson’s ratio is nearly zero, which corresponds to a value of . The plastic flow is associated when the value of . By default, the plastic flow is nonassociated to allow for the independent calibrations of the shape of the yield surface and the plastic Poisson’s ratio. If you have information only about the plastic Poisson’s ratio and choose to use associated plastic flow, the yield stress ratio k can be calculated from is the same as that of Alternatively, if only the shape of the yield surface is known and you choose to use associated plastic flow, the plastic Poisson’s ratio can be obtained from You provide the value of . Input File Usage: Abaqus/CAE Usage: *CRUSHABLE FOAM, HARDENING=ISOTROPIC Property module: material editor: Mechanical→Plasticity→Crushable Foam: Hardening: Isotropic Hardening A simple uniaxial compression test is sufficient to define the evolution of the yield surface. The hardening law defines the value of the yield stress in uniaxial compression as a function of the absolute value of the axial plastic strain. The piecewise linear relationship is entered in tabular form. The table must start with a zero plastic strain (corresponding to the virgin state of the materials), and the tabular entries must be given in ascending magnitude of . For values of plastic strain greater than the last user-specified value, the stress-strain relationship is extrapolated based on the last slope computed from the data. If desired, the yield stress can also be a function of temperature and other predefined field variables. Input File Usage: Abaqus/CAE Usage: *CRUSHABLE FOAM HARDENING Property module: material editor: Mechanical→Plasticity→Crushable Foam: Suboptions→Foam Hardening Rate dependence As strain rates increase, many materials show an increase in the yield stress. For many crushable foam materials this increase in yield stress becomes important when the strain rates are in the range of 0.1–1 per second and can be very important if the strain rates are in the range of 10–100 per second, as commonly occurs in high-energy dynamic events. Two methods for specifying strain-rate-dependent material behavior are available in Abaqus as discussed below. Both methods assume that the shapes of the hardening curves at different strain rates are similar, and either can be used in static or dynamic procedures. When rate dependence is included, the static stress-strain hardening behavior must be specified for the crushable foam as described above. Overstress power law You can specify a Cowper-Symonds overstress power law that defines strain rate dependence. This law has the form with where yield stress at a given value of , specified as part of the crushable foam hardening definition, is the static uniaxial compression is the yield for the experiment with the lowest strain rate, and axial plastic strain in uniaxial compression for the isotropic hardening model. is the equivalent plastic strain rate, which is equal to the rate of the The power-law rate dependency can be rewritten in the following form CRUSHABLE FOAM versus Plot in Figure 23.3.5–2, the overstress power law is suitable. The slope of the line is of the and, possibly, of other predefined field variables. . If the curve can be approximated by a straight line such as that shown , and the intercept . The material parameters D and n can be functions of temperature axis is Input File Usage: Use both of the following options: *CRUSHABLE FOAM HARDENING *RATE DEPENDENT, TYPE=POWER LAW Property module: material editor: Mechanical→Plasticity→Crushable Foam: Suboptions→Foam Hardening; Suboptions→Rate Dependent: Hardening: Power Law Abaqus/CAE Usage: Tabular input of yield ratio Rate-dependent behavior can alternatively be specified by giving a table of the ratio R as a function of the absolute value of the rate of the axial plastic strain and, optionally, temperature and predefined field variables. Input File Usage: Use both of the following options: *CRUSHABLE FOAM HARDENING *RATE DEPENDENT, TYPE=YIELD RATIO Property module: material editor: Mechanical→Plasticity→Crushable Foam: Suboptions→Foam Hardening; Suboptions→Rate Dependent: Hardening: Yield Ratio Abaqus/CAE Usage: Elements The crushable foam plasticity model can be used with plane strain, generalized plane strain, axisymmetric, and three-dimensional solid (continuum) elements. This model cannot be used with elements for which the stress state is assumed to be planar (plane stress, shell, and membrane elements) or with beam, pipe, or truss elements. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variable has special meaning for the crushable foam plasticity model: PEEQ For the volumetric hardening model, PEEQ is the volumetric compacting plastic strain defined as . For the isotropic hardening model, PEEQ is the equivalent is the uniaxial compression yield plastic strain defined as stress. , where The volumetric plastic strain, sum of direct plastic strain components. , is the trace of the plastic strain tensor; you can also calculate it as the For the volumetric hardening model, the initial values of the volumetric compacting plastic strain can be specified for elements that use the crushable foam material model, as described above. The volumetric compacting plastic strain (output variable PEEQ) provided by Abaqus then contains the initial value of the volumetric compacting plastic strain plus any additional volumetric compacting plastic strain due to plastic straining during the analysis. However, the plastic strain tensor (output variable PE) contains only the amount of straining due to deformation during the analysis. Additional reference • Deshpande, V. S., and N. A. Fleck, “Isotropic Constitutive Model for Metallic Foams,” Journal of the Mechanics and Physics of Solids, vol. 48, pp. 1253–1276, 2000. 23.4 Fabric materials • “Fabric material behavior,” Section 23.4.1 23.4.1 FABRIC MATERIAL BEHAVIOR Product: Abaqus/Explicit References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • “VFABRIC,” Section 1.2.3 of the Abaqus User Subroutines Reference Manual • *FABRIC • *UNIAXIAL • *LOADING DATA • *UNLOADING DATA • *EXPANSION • *DENSITY • *INITIAL CONDITIONS Overview The fabric material model: • is anisotropic and nonlinear; • is a phenomenological model that captures the mechanical response of a woven fabric made of yarns in the fill and the warp directions; • is valid for materials that exhibit two “structural” directions that may not be orthogonal to each other with deformation; • defines the local fabric stresses as a function of change in angle between the fibers (shear strain) and the nominal strains along the yarn directions; • allows for the computation of local fabric stresses based on test data or through user subroutine VFABRIC, which can be used to define a complex constitutive model; and • requires that geometric nonlinearity be accounted for during the analysis step (“General and linear perturbation procedures,” Section 6.1.3), since it is intended for finite-strain applications. The fabric material model defined based on test data: • assumes that the responses along the fill and the warp directions are independent of each other and that the shear response is independent of the direct response along the yarns; • can include separate loading and unloading responses; • can exhibit nonlinear elastic behavior, damaged elastic behavior, or elastic-plastic type behavior with permanent deformation upon complete unloading; • can deform elastically to large tensile and shear strains; and • can have properties that depend on temperature and/or other field variables. Fabric material behavior Woven fabrics are used in a number of engineering applications across various industries, including such products as automobile airbags; flexible structures like boat sails and parachutes; reinforcement in composites; architectural expressions in building roof structures; protective vests for military, police, and other security circles; and protective layers around the fuselage in planes. Woven fabrics consist of yarns woven in the fill and the warp directions. The yarn is crimped, or curved, as it is woven up and down over the cross yarns. The nonlinear mechanical behavior of the fabric arises from different sources: the nonlinear response of the individual yarns, the exchange of crimp between the fill and the warp yarns as they are stretched, and the contact and friction between the yarns in cross directions and between the yarns in the same direction. In general, the fabric exhibits a significant stiffness only along the yarn directions under tension. The tensile response in the fill and warp directions may be coupled due to the crimp exchange mentioned above. Under in-plane shear deformation, the fill and warp direction yarns rotate with respect to each other. The resistance increases with shear deformation as lateral contact is formed between the yarns in each direction. The fabrics typically have negligible stiffness in bending and in-plane compression. The behavior of woven fabrics is modeled phenomenologically in Abaqus/Explicit to capture the nonlinear anisotropic behavior of the fabric. The planar kinematic state of a given fabric is described in terms of the nominal direct strains in the fabric plane along the fill and the warp directions and the angle between the two yarn directions. The material orthogonal basis and the yarn local directions are illustrated in Figure 23.4.1–1 showing the reference and the deformed configurations. E2 N2 12 N1 E1 e2 n2 12 12 12 n1 e1 (a) Reference configuration (b) Deformed configuration Figure 23.4.1–1 Fabric kinematics The engineering nominal shear strain, , between the two yarn directions going from the reference to the deformed configuration. The nominal strains along the yarn directions in the deformed configuration are computed from the respective yarn stretch values, are defined as the and work conjugate of the above nominal strains. The fabric nominal stress, , is converted by Abaqus to the Cauchy stress, ; and the subsequent internal forces arising from the fabric deformation are computed. and . The corresponding nominal stress components , is defined as the change in angle, , and You can obtain output of the fabric nominal strains, the fabric nominal stresses, and the regular Cauchy stresses. The relationship between the Cauchy stress, , and the nominal stress, , is where is the volumetric Jacobian. Either experimental data or a user subroutine, VFABRIC, can be used to characterize the Abaqus/Explicit fabric material model, providing the nominal fabric stress as a function of the nominal fabric strains. The user subroutine allows for building a complex material model taking into account both the fabric structural parameters such as yarn spacing, yarn cross-section shape, etc. and the yarn material properties. The test data–based fabric model makes some simplifying assumptions but allows for nonlinear response including energy loss. The two models are presented below in detail. Both models capture the wrinkling of fabric under compression only in a smeared fashion. The application of fabric material in a crash simulation is illustrated in “Side curtain airbag impactor test,” Section 3.3.2 of the Abaqus Example Problems Manual. Test data–based fabric materials The fabric material model based on test data assumes that the responses along the fill and the warp directions are independent of each other and that the shear response is independent of the direct response along the yarn. Hence, each component-wise fabric stress response depends only on the fabric strain in that component. Thus, the overall behavior of the fabric consists of three independent component-wise responses: namely, the direct response along the fill yarn to the nominal strain in the fill yarn, the direct response along the warp yarn to the nominal strain in the warp yarn, and the shear response to the change in angle between the two yarns. Within each component you must provide test data defining the response of the fabric. To fully define the fabric response, the test data must cover all of the following attributes: • Within a component, separate test data can be defined for the fabric response in the tensile direction and in the compressive direction. • Within a deformation direction (tension or compression), both loading and unloading test data can be provided. • The loading and unloading test data can be classified according to three available behavior types: nonlinear elastic behavior, damaged elastic behavior, or elastic-plastic type behavior with permanent deformation. The behavior type determines how the fabric transitions from its loading response to its unloading response. When elastic, the test data in a particular component can also be rate dependent. When separate loading and unloading paths are required, the test data for the two deformation directions (tension and compression) must be given separately. Otherwise, the data for both tension and compression may be given in a single table. Input File Usage: Use the following options to define a fabric material using test data: *FABRIC *UNIAXIAL, COMPONENT=component *LOADING DATA, DIRECTION=deformation direction, TYPE=behavior type data lines to define loading data *UNLOADING DATA data lines to define unloading data Repeat all of the options underneath *FABRIC as often as necessary to account for each component and deformation direction. Specifying uniaxial behavior in a component direction Independent loading and unloading test data can be provided in each of the three component directions. The components correspond to the response along the fill yarn, the response along the warp yarn, and the shear response. Input File Usage: Use the following option to define the response along the fill yarn direction: *UNIAXIAL, COMPONENT=1 Use the following option to define the response along the warp yarn direction: *UNIAXIAL, COMPONENT=2 Use the following option to define the shear response: *UNIAXIAL, COMPONENT=SHEAR Defining the deformation direction The test data can be defined separately for tension and compression by specifying the deformation direction. If the deformation direction is defined (tension or compression), the tabular values defining tensile or compressive behavior should be specified with positive values of the stress and strain in the specified component and the loading data must start at the origin. If the behavior is not defined in a loading direction, the stress response will be zero in that direction (the fabric has no resistance in that direction). If the deformation direction is not defined, the data apply to both tension and compression. However, the behavior is then considered to be nonlinear elastic and no unloading response can be specified. The test data will be considered to be symmetric about the origin if either tensile or compressive data are omitted. Input File Usage: Use the following option to define tensile behavior: *LOADING DATA, DIRECTION=TENSION Use the following option to define compressive behavior: *LOADING DATA, DIRECTION=COMPRESSION Use the following option to define both tensile and compressive behavior in a single table: *LOADING DATA Compressive behavior In general, a fabric material does not have significant stiffness under compression. To prevent the collapse of wrinkled elements under compressive loading, the specified stress-strain curve should reinstate the compressive stiffness after a range of zero or very small resistance. Defining loading/unloading component-wise response for a fabric material To define the loading response, you specify the fabric stress as nonlinear functions of the fabric strain. This function can also depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and field variables. The unloading response can be defined in the following different ways: • You can specify several unloading curves that express the fabric stress as nonlinear functions of the fabric strain; Abaqus interpolates these curves to create an unloading curve that passes through the point of unloading in an analysis. • You can specify an energy dissipation factor (and a permanent deformation factor for models with permanent deformation), from which Abaqus calculates a quadratic unloading function. • You can specify an energy dissipation factor (and a permanent deformation factor for models with permanent deformation), from which Abaqus calculates an exponential unloading function. • You can specify the fabric stress as a nonlinear function of the fabric strain, as well as a transition slope; the fabric unloads along the specified transition slope until it intersects the specified unloading function, at which point it unloads according to the function. (This unloading definition is referred to as combined unloading.) • You can specify the fabric stress as a nonlinear function of the fabric strain; Abaqus shifts the specified unloading function along the strain axis so that it passes through the point of unloading in an analysis. The behavior type that is specified for the fabric dictates the type of unloading you can define, as summarized in Table 23.4.1–1. The different behavior types, as well as the associated loading and unloading curves, are discussed in more detail in the sections that follow. Defining nonlinear elastic behavior The elastic behavior can be nonlinear and, optionally, rate dependent. When the loading response is rate dependent, a separate unloading curve must also be specified. However, the unloading response need not be rate dependent. Defining rate-independent elasticity When the loading response is rate independent, the unloading response is also rate independent and occurs along the same user-specified loading curve as illustrated in Figure 23.4.1–2. An unloading curve does not need to be specified. Input File Usage: *LOADING DATA, TYPE=ELASTIC Table 23.4.1–1 Available unloading definitions for the fabric behavior types. Unloading definition Interpolated Quadratic Exponential Combined Shifted Material behavior type Nonlinear elastic (rate-dependent only) Damaged elastic Permanent deformation  loading curve  Figure 23.4.1–2 Nonlinear elastic rate-independent loading. Defining rate-dependent elasticity When the elastic response is rate dependent, both the loading and the unloading curves need to be specified. If the unloading data are not specified, the unloading occurs along the loading curve specified with the smallest rate of deformation. Unphysical jumps in the stress due to sudden changes in the rate of deformation are prevented using a technique based on viscoplastic regularization. This technique also helps model relaxation effects in a very simplistic manner, with the relaxation time given as are material parameters and is a linear viscosity parameter that controls the relaxation time when is a nonlinear viscosity parameter that controls the relaxation time at higher values of . Small values of this parameter should be used; a suggested value is 0.0001s. . The smaller is the stretch. , where , and , this value, the shorter the relaxation time. The suggested value for this parameter is 0.005s. controls the sensitivity of the relaxation speed to the fabric strain component. Figure 23.4.1–3 illustrates the loading/unloading behavior as the component is loaded at a rate and then unloaded at a rate .  Figure 23.4.1–3 Rate-dependent loading/unloading. The unloading path is determined by interpolating the specified unloading curves. The unloading need not be rate dependent, even though the loading response is rate dependent. When the unloading is rate dependent, the unloading path at any given component strain and strain rate is determined by interpolating the specified unloading curves. Input File Usage: Use the following options when the unloading is also rate dependent: *LOADING DATA, TYPE=ELASTIC, RATE DEPENDENT, DIRECTION *UNLOADING DATA, DEFINITION=INTERPOLATED CURVE, RATE DEPENDENT Use the following options when the unloading is rate independent: *LOADING DATA, TYPE=ELASTIC, RATE DEPENDENT, DIRECTION *UNLOADING DATA, DEFINITION=INTERPOLATED CURVE Defining models with damage The damage models dissipate energy upon unloading, and there is no permanent deformation upon complete unloading. You can specify the onset of damage by defining the strain above which the material response in unloading does not retrace the loading curve. The unloading behavior controls the amount of energy dissipated by damage mechanisms and can be specified in one of the following ways: • an analytical unloading curve (exponential/quadratic); • an unloading curve interpolated from multiple user-specified unloading curves; or • unloading along a transition unloading curve (constant slope specified by user) to the user-specified unloading curve (combined unloading). Input File Usage: Use the following options to define damage with quadratic unloading behavior: *LOADING DATA, TYPE=DAMAGE, DIRECTION *UNLOADING DATA, DEFINITION=QUADRATIC Use the following options to define damage with exponential unloading behavior: *LOADING DATA, TYPE=DAMAGE, DIRECTION *UNLOADING DATA, DEFINITION=EXPONENTIAL Use the following options to define damage with an interpolated unloading curve: *LOADING DATA, TYPE=DAMAGE, DIRECTION *UNLOADING DATA, DEFINITION=INTERPOLATED CURVE Use the following options to specify damage with combined unloading behavior: *LOADING DATA, TYPE=DAMAGE, DIRECTION *UNLOADING DATA, DEFINITION=COMBINED Defining onset of damage You can specify the onset of damage by defining the strain above which the material response in unloading does not retrace the loading curve. Input File Usage: *LOADING DATA, TYPE=DAMAGE, DAMAGE ONSET=value Specifying exponential/quadratic unloading The damage model in Figure 23.4.1–4 is based on an analytical unloading curve that is derived from an energy dissipation factor, (fraction of energy that is dissipated at any strain level). As the fabric component is loaded, the stress follows the path given by the loading curve. If the fabric component is unloaded (for example, at point B), the stress follows the unloading curve . Reloading after unloading follows the unloading curve until the loading is such that the strain becomes greater than , after which the loading path follows the loading curve. The arrows shown in Figure 23.4.1–4 illustrate the loading/unloading paths of this model.  primary loading curve exponential/quadratic unloading max  Figure 23.4.1–4 Exponential/quadratic unloading. The unloading response follows the loading curve when the calculated unloading curve lies above the loading curve to prevent energy generation and follows a zero stress response when the unloading curve yields a negative response. In such cases the dissipated energy will be less than the value specified by the energy dissipation factor. Specifying interpolated curve unloading The damage model in Figure 23.4.1–5 illustrates an interpolated unloading response based on multiple unloading curves that intersect the primary loading curve at increasing values of stress/strains. You can specify as many unloading curves as are necessary to define the unloading response. Each unloading curve always starts at point O, the point of zero stress and zero strains, since the damage models do not allow any permanent deformation. The unloading curves are stored in normalized form so that they intersect the loading curve at a unit stress for a unit strain, and the interpolation occurs between these normalized curves. If unloading occurs from a maximum strain for which an unloading curve is not specified, the unloading is interpolated from neighboring unloading curves. As the fabric component is loaded, the stress follows the path given by the loading curve. If the fabric is unloaded (for example, at point B), the stress follows the unloading curve . Reloading after unloading follows the unloading path , after which the loading path follows the loading curve. until the loading is such that the strain becomes greater than The unloading curve also has the same temperature and field variable dependencies as the loading curve. Specifying combined unloading As illustrated in Figure 23.4.1–6, you can specify an unloading curve curve in addition to the loading as well as a constant transition slope that connects the loading curve to the unloading  max primary loading curve unloading curves  Figure 23.4.1–5 Interpolated curve unloading. curve. As the fabric is loaded, the stress follows the path given by the loading curve. If the fabric is unloaded (for example at point B) the stress follows the unloading curve is defined by the constant transition slope, and lies on the specified unloading curve. Reloading after unloading follows the unloading path , after which the loading path follows the loading curve. until the loading is such that the strain becomes greater than . The path primary loading curve transition curve unloading curve max The unloading curve also has the same temperature and field variable dependencies as the loading Figure 23.4.1–6 Combined unloading. curve. Defining models with permanent deformation These models dissipate energy upon unloading and exhibit permanent deformation upon complete unloading. You can specify the onset of permanent deformation by defining the strain below which unloading occurs along the loading curve. The unloading behavior controls the amount of energy dissipated as well as the amount of permanent deformation. The unloading behavior can be specified in one of the following ways: Input File Usage: • an analytical unloading curve (exponential/quadratic); • an unloading curve interpolated from multiple user-specified unloading curves; or • an unloading curve obtained by shifting the user-specified unloading curve to the point of unloading. Use the following options to define permanent deformation with quadratic unloading behavior: *LOADING DATA, TYPE=PERMANENT DEFORMATION, DIRECTION *UNLOADING DATA, DEFINITION=QUADRATIC Use the following options to define permanent damage with exponential unloading behavior: *LOADING DATA, TYPE=PERMANENT DEFORMATION, DIRECTION *UNLOADING DATA, DEFINITION=EXPONENTIAL Use the following options to define permanent damage with an interpolated unloading curve: *LOADING DATA, TYPE=PERMANENT DEFORMATION, DIRECTION *UNLOADING DATA, DEFINITION=INTERPOLATED CURVE Use the following options to specify permanent damage with a shifted unloading curve: *LOADING DATA, TYPE=PERMANENT DEFORMATION, DIRECTION *UNLOADING DATA, DEFINITION=SHIFTED CURVE Defining the onset of permanent deformation By default, the onset of yield will be obtained as soon as the slope of the loading curve decreases by 10% from the maximum slope recorded up to that point while traversing along the loading curve. To override the default method of determining the onset of yield, you can specify either a value for the decrease in slope of the loading curve other than the default value of 10% (slope drop = 0.1) or by defining the strain below which unloading occurs along the loading curve. If a slope drop is specified, the onset of yield will be obtained as soon as the slope of the loading curve decreases by the specified factor from the maximum slope recorded up to that point. Input File Usage: Use the following options to specify the onset of yield by defining the strain below which unloading occurs along the loading curve: *LOADING DATA, TYPE=PERMANENT DEFORMATION, YIELD ONSET=value Use the following options to specify the onset of yield by defining a slope drop for the loading curve: *LOADING DATA, TYPE=PERMANENT DEFORMATION, SLOPE DROP=value Specifying exponential/quadratic unloading The model in Figure 23.4.1–7 illustrates an analytical unloading curve that is derived from an energy dissipation factor, (fraction of energy that is dissipated at any strain level), and a permanent deformation factor, . As the fabric component is loaded, the fabric stress follows the path given by the loading curve. If the component is unloaded (for example, at point B), the stress follows the unloading curve . Reloading . The point D corresponds to the permanent deformation, after unloading follows the unloading curve until the loading is such that the strain becomes greater than , after which the loading path follows the loading curve. The arrows shown in Figure 23.4.1–7 illustrate the loading/unloading paths of this model. primary loading curve max Dp max exponential/quadratic unloading Figure 23.4.1–7 Exponential/quadratic unloading. The unloading response follows the loading curve when the calculated unloading curve lies above the loading curve to prevent energy generation and follows a zero stress response when the unloading curve yields a negative response. In such cases the dissipated energy will be less than the value specified by the energy dissipation factor. Specifying interpolated curve unloading The model in Figure 23.4.1–8 illustrates an interpolated unloading response based on multiple unloading curves that intersect the primary loading curve at increasing values of stresses/strains.  primary loading curve unloading curves max  Figure 23.4.1–8 Interpolated curve unloading. You can specify as many unloading curves as are necessary to define the unloading response. The first point of each unloading curve defines the permanent deformation if the fabric component is completely unloaded. The unloading curves are stored in normalized form so that they intersect the loading curve at a unit stress for a unit strain, and the interpolation occurs between these normalized curves. If unloading occurs from a maximum strain for which an unloading curve is not specified, the unloading is interpolated from neighboring unloading curves. As the fabric is loaded, the stress follows the path given by the loading curve. If the fabric is unloaded (for example, at point B), the stress follows the unloading curve until the loading is such that the . Reloading after unloading follows the unloading path strain becomes greater than , after which the loading path follows the loading curve. The unloading curve also has the same temperature and field variable dependencies as the loading curve. Specifying shifted curve unloading You can specify an unloading curve passing through the origin in addition to the loading curve. The actual unloading curve is obtained by horizontally shifting the user-specified unloading curve to pass through the point of unloading as shown in Figure 23.4.1–9. The permanent deformation upon complete unloading is the horizontal shift applied to the unloading curve. The unloading curve also has the same temperature and field variable dependencies as the loading curve. unloading curve  primary loading curve shifted unloading curve max  Figure 23.4.1–9 Shifted curve unloading. Using different uniaxial models in tension and compression When appropriate, different uniaxial behavior models can be used in tension and compression. For example, response under tension can be plastic with exponential unloading, while the response in compression can be nonlinear elastic . User-defined fabric materials The mechanical response of a fabric material depends on a number of micro and meso-scale parameters covering the fabric construction and that of the individual yarns as a bundle of fibers. Often a multi-scale model becomes necessary to track the state of the fabric and its response to loading. Abaqus provides a specialized user subroutine, VFABRIC, to capture the complex fabric response given the deformed yarn directions and the strains along these directions. The density (“Density,” Section 21.2.1) is required when using a fabric material. Input File Usage: Use the following options to define a fabric material through user subroutine VFABRIC: *MATERIAL, NAME=name *FABRIC, USER *DENSITY Properties for a user-defined fabric material Any material constants that are needed in user subroutine VFABRIC must be specified as part of a user-defined fabric material definition. Abaqus can be used to compute the isotropic thermal expansion response under thermal loading, even as the remaining mechanical response is defined by the user primary loading curve unloading nonlinear elastic Figure 23.4.1–10 Different uniaxial models in tension and compression. subroutine. Alternatively, you can include the thermal expansion within the definition of the mechanical response in user subroutine VFABRIC. Input File Usage: Use the following option to define properties for a user-defined fabric material behavior: *FABRIC, USER, PROPERTIES=number_of_constants Material state Many mechanical constitutive models require the storage of solution-dependent state variables (plastic strains, “back stress,” saturation values, etc. in rate constitutive forms or historical data for theories written in integral form). You should allocate storage for these variables in the associated material definition . There is no restriction on the number of state variables associated with a user-defined fabric material. State variables associated with VFABRIC can be output to the output database (.odb) file and results (.fil) file using output identifiers SDV and SDVn . User subroutine VFABRIC is called for blocks of material points at each increment. When the subroutine is called, it is provided with the state at the start of the increment (fabric stress in the local system, solution-dependent state variables). It is also provided with the nominal fabric strains at the end of the increment and the incremental nominal fabric strains over the increment, both in the local system. The VFABRIC user material interface passes a block of material points to the subroutine on each call, which allows vectorization of the material subroutine. The temperature is provided to user subroutine VFABRIC at the start and the end of the increment. The temperature is passed in as information only and cannot be modified, even in a fully coupled thermal- stress analysis. However, if the inelastic heat fraction is defined in conjunction with the specific heat and conductivity in a fully coupled thermal-stress analysis, the heat flux due to inelastic energy dissipation is calculated automatically. If user subroutine VFABRIC is used to define an adiabatic material behavior (conversion of plastic work to heat) in an explicit dynamic procedure, the temperatures must be stored and integrated as user-defined state variables. Most often the temperatures are provided by specifying initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) and are constant throughout the analysis. Deleting elements from an Abaqus/Explicit mesh using state variables Element deletion in a mesh can be controlled during the course of an Abaqus/Explicit analysis through user subroutine VFABRIC. Deleted elements have no ability to carry stresses and, therefore, have no contribution to the stiffness of the model. You specify the state variable number controlling the element deletion flag. For example, specifying a state variable number of 4 indicates that the fourth state variable is the deletion flag in VFABRIC. The deletion state variable should be set to a value of one or zero in VFABRIC. A value of one indicates that the material point is active, while a value of zero indicates that Abaqus/Explicit should delete the material point from the model by setting the stresses to zero. The structure of the block of material points passed to user subroutine VFABRIC remains unchanged during the analysis; deleted material points are not removed from the block. Abaqus/Explicit will pass zero stresses and strain increments for all deleted material points. Once a material point has been flagged as deleted, it cannot be reactivated. An element will be deleted from the mesh only after all of the material points in the element are deleted. The status of an element can be determined by requesting output of the variable STATUS. This variable is equal to 1 if the element is active and equal to 0 if the element is deleted. Input File Usage: *DEPVAR, DELETE=variable number Thermal expansion You can define isotropic thermal expansion to specify the same coefficient of thermal expansion for the membrane and thickness-direction behaviors. The membrane thermal strains, , are obtained as explained in “Thermal expansion,” Section 26.1.2. The elastic stretch in a given direction, , relates the total stretch, , and the thermal stretch, : is given by where is the linear thermal expansion strain in that direction. Fabric thickness The thickness of a fabric is difficult to measure experimentally. Fortunately, an accurate value for thickness is not always required due to the fact that a nominal stress measure, defined as force per unit area in the reference configuration, is used to characterize the in-plane response. An initial thickness can be specified on the section definition. Accurate tracking of the thickness with deformation is necessary only if the material is used with shell elements and the bending response needs to be captured accurately. You can compute the thickness direction strain increment when the fabric is defined through user subroutine VFABRIC. For test data–based fabric materials the thickness is assumed to remain constant with deformation. For a test data–based fabric definition, you must use the thickness value specified on the section definition for converting the experimental load data (which are typically available as force applied per unit width of the fabric) to stress quantities. Defining a reference mesh (initial metric) Abaqus/Explicit allows the specification of a reference mesh (initial metric) for fabrics modeled with membrane elements. For example, this is useful in airbag simulations to model wrinkles and changes in yarn orientations that arise from the airbag folding process. A flat mesh may be suitable for the unstressed reference configuration, but the initial state may require a corresponding folded mesh defining the folded state. The angular orientation of the yarn in the reference configuration is updated to obtain the new orientation in the initial configuration. Input File Usage: Use the following option to define the reference configuration giving the element number and its nodal coordinates in the reference configuration: *INITIAL CONDITIONS, TYPE=REF COORDINATE Use the following option to define the reference configuration giving the node number and its coordinates in the reference configuration: *INITIAL CONDITIONS, TYPE=NODE REF COORDINATE Yarn behavior under initial compressive strains Defining a reference configuration that is different from the initial configuration generally results in nonzero stresses and strains in the initial configuration based on the material definition. By default, compressive initial strains in the yarn directions generate zero stresses. The stress remains zero as the strain is continuously recovered from the initial compressive values toward the strain-free state. Once the initial slack is recovered, any subsequent compressive/tensile strains generate stresses as per the material definition. Input File Usage: initial compressive strains are Use the following option to specify that recovered stress free (default): *FABRIC, STRESS FREE INITIAL SLACK=YES Use the following option to specify that initial compressive strains generate nonzero initial stresses: *FABRIC, STRESS FREE INITIAL SLACK=NO Defining yarn directions in the reference configuration In general, the yarn directions may not be orthogonal to each other in the reference configuration. You can specify these local directions with respect to the in-plane axes of an orthogonal orientation system at a material point. Both the local directions and the orthogonal system are defined together as a single orientation definition. See “Orientations,” Section 2.2.5, for more information. If the local directions are not specified, these directions are assumed to match the in-plane axes of the orthogonal system defined. The local direction may not remain orthogonal with deformation. Abaqus updates the local directions with deformation and computes the nominal strains along these directions and the angle between them (fabric shear strain). The constitutive behavior for the fabric defines the nominal stresses in the local system in terms of the fabric strain. Local yarn directions can be output to the output database as described in “Output,” below. Picture-frame shear fabric test The shear response of the fabric is typically studied using a picture-frame shear test. The reference and the deformed configuration for a picture-frame shear test under force is illustrated in Figure 23.4.1–11, where is the initial angle between the yarn directions. The four sides of the specimen are constrained not to change in their length even as the frame elongates and the angle between the yarn directions decreases with deformation.The relationship between the nominal shear stress, is the size of the picture-frame, and , and the applied force, , is where change in the angle between the yarn directions as is the initial volume of the specimen. The fabric engineering shear strain, , is related to the Use with other material models The fabric material model can be used by itself, or it can be combined with isotropic thermal expansion to introduce thermal volume changes (“Thermal expansion,” Section 26.1.2). See “Combining material behaviors,” Section 21.1.3, for more details. Thermal expansion can alternatively be an integral part of the constitutive model implemented in VFABRIC for user-defined fabric materials. For a test-data based fabric material, both the mass proportional and the stiffness proportional damping can be specified . If stiffness proportional damping is specified, Abaqus calculates the damping stress based on the current elastic stiffness of the material and the resulting damping stress is included in the reported stress output at the integration points. For a fabric material defined by user subroutine VFABRIC, mass proportional damping can be specified, but stiffness proportional damping must be defined within the user subroutine. L0 L0 L0 L0 12 N2 N1 12 n1 n2 (a) Reference configuration (b) Deformed configuration Figure 23.4.1–11 Picture-frame shear test on a fabric. Elements The fabric material model can be used with plane stress elements (plane stress solid elements, finite-strain shells, and membranes). It is recommended that the fabric material model be used with fully integrated or triangular membrane elements. When the fabric material model is used with shell elements, Abaqus does not compute a default transverse shear stiffness and you must specify it directly (see“Defining the transverse shear stiffness” in “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5). Procedures Fabric materials must always be used with geometrically nonlinear analyses (“General and linear perturbation procedures,” Section 6.1.3). Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for the fabric material models: EFABRIC SFABRIC Nominal fabric strain with components similar to that of LE, but with the direct components measuring the nominal strain along the yarn directions and the engineering shear component measuring the change in angle between the two yarn directions. Nominal fabric stress with components similar to that of the regular Cauchy stress, S, but with the direct components measuring the nominal stress along the yarn directions and the shear component measuring response to the change in angle between the two yarn directions. By default Abaqus outputs local material directions whenever element field output is requested to the output database for fabric models. The local directions are output as field variables (LOCALDIR1, LOCALDIR2, LOCALDIR3) representing the yarn direction cosines; these variables can be visualized as vector plots in the Visualization module of Abaqus/CAE (Abaqus/Viewer). Output of local material directions is suppressed if no element field output is requested or if you specify not to have element material directions written to the output database . 23.5 Jointed materials • “Jointed material model,” Section 23.5.1 23.5.1 JOINTED MATERIAL MODEL Product: Abaqus/Standard References • “Orientations,” Section 2.2.5 • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *JOINTED MATERIAL Overview The jointed material model: • is intended to provide a simple continuum model for a material containing a high density of parallel joint surfaces where each system of parallel joints is associated with a particular orientation, such as sedimentary rock; • assumes that the spacing of the joints of a particular orientation is sufficiently close compared to characteristic dimensions in the domain of the model such that the joints can be smeared into a continuum of slip systems; • provides for opening or frictional sliding of the joints in each of these systems (a “system” in this context is a joint orientation in a particular direction at a material calculation point); and • assumes that the elastic behavior of the material is isotropic and linear when all joints at a point are closed (isotropic linear elastic behavior must be included in the material definition; see “Defining isotropic elasticity” in “Linear elastic behavior,” Section 22.2.1). Joint opening/closing The jointed material model is intended primarily for applications where the stresses are mainly compressive. The model provides a joint opening capability when the stress normal to the joint tries to become tensile. In this case the stiffness of the material normal to the joint plane becomes zero instantaneously. Abaqus/Standard uses a stress-based joint opening criterion, whereas joint closing is monitored based on strain. Joint system a opens when the estimated pressure stress across the joint (normal to the joint surface) is no longer positive: In this case the material is assumed to have no elastic stiffness with respect to direct strain across the joint system. Open joints thus create anisotropic elastic response at a point. The joint system remains open so long as where elastic strain across the joint calculated in plane stress as is the component of direct elastic strain across the joint and is the component of direct where E is the Young’s modulus of the material, stresses in the plane of the joint. is the Poisson’s ratio, and , are the direct The shear response of open joints is governed by the shear retention parameter, , which represents the fraction of the elastic shear modulus retained when the joints are open ( =0 means no shear stiffness associated with open joints, while =1 corresponds to elastic shear stiffness in open joints; any value between these two extremes can be used). When a joint opens, the shear behavior may be brittle, depending on the shear retention factor used for open joints. In addition, the stiffness of the material normal to the joint plane suddenly goes to zero. For these reasons, in situations where the confining stresses are low or significant regions experience tensile behavior, the joint systems may experience a sequence of alternate opening and closing states from iteration to iteration. Typically such behavior manifests itself as oscillating global residual forces. The convergence rate associated with such discontinuous behavior may be very slow and, thus, prohibit obtaining a solution. This type of failure is more probable in cases where more than one joint system is modeled. Improving convergence when joints open and close repeatedly When the repeated opening and closing of joints makes convergence difficult, you can improve convergence by preventing a joint from opening. In this case an elastic stiffness is always associated with the joint. It is most useful when the opening and closing of joints is limited to small regions of the model. You can prevent a joint from opening only when the joint direction is specified, as described below. Input File Usage: *JOINTED MATERIAL, NO SEPARATION, JOINT DIRECTION Specifying nonzero shear retention in open joints You must specify nonzero shear retention in open joints directly. The parameter tabular function of temperature and predefined field variables. can be defined as a Input File Usage: *JOINTED MATERIAL, SHEAR RETENTION Compressive joint sliding The failure surface for sliding on joint system a is defined by where stress acting across the joint, is the magnitude of the shear stress resolved onto the joint surface, is the normal pressure is the cohesion for system a. So is the friction angle for system a, and strain on the system is given by , joint system a does not slip. When , joint system a slips. The inelastic (“plastic”) JOINTED MATERIAL where on the joint surface ( are orthogonal is the rate of inelastic shear strain in direction directions on the joint surface), is the magnitude of the inelastic strain rate, is a component of the shear stress on the joint surface, is the dilation angle for this joint system (choosing joint, while is the inelastic strain normal to the joint surface. causes dilation of the joint as it slips), and provides pure shear flow on the The sliding of the different joint systems at a point is independent, in the sense that sliding on one system does not change the failure criterion or the dilation angle for any other joint system at the same point. Up to three joint directions can be included in the material description. The orientations of the joint directions are given by referring to the names of user-defined local orientations (“Orientations,” Section 2.2.5) that define the joint orientations in the original configuration. Output of stress and strain components is in the global directions unless a local orientation is also used in the material’s section definition. The parameters , , and can be specified as tabular functions of temperature and/or predefined field variables for each joint direction. Input File Usage: Use both of the following options: *ORIENTATION, NAME=name *JOINTED MATERIAL, JOINT DIRECTION=name Repeat the *JOINTED MATERIAL option for each direction to be specified, up to three times. Joint directions and finite rotations In geometrically nonlinear analysis steps the joint directions always remain fixed in space. Bulk failure In addition to the joint systems, the jointed material model includes a bulk material failure mechanism, which is based on the Drucker-Prager failure criterion: where is the Mises equivalent deviatoric stress, is the deviatoric stress, is the equivalent pressure stress, is the friction angle for the bulk material, and is the cohesion for the bulk material. If this failure criterion is reached, the bulk inelastic flow is defined by where is the magnitude of the inelastic flow rate (chosen so that is the flow potential. Here in uniaxial compression in the 1-direction), and is the dilation angle for the bulk material. This bulk failure model is a simplified version of the extended Drucker-Prager model (“Extended Drucker-Prager models,” Section 23.3.1). This bulk failure system is independent of the joint systems in that bulk inelastic flow does not change the behavior of any joint system. If bulk material failure is to be modeled, a jointed material behavior must be specified to define the parameters associated with bulk material failure behavior. Thus, up to five jointed material behaviors can appear in the same material definition: three joint directions, shear retention in open joints, and bulk material failure. The parameters , , and can be specified as a tabular function of temperature and/or predefined field variables. Input File Usage: *JOINTED MATERIAL (the JOINT DIRECTION parameter must be omitted) Nonassociated flow in any joint system, whether it be associated with the joint surfaces or the bulk material, the flow If in that system is “nonassociated.” The implication is that the material stiffness matrix is not symmetric. Therefore, the unsymmetric matrix solution scheme should be used for the analysis step (“Defining an analysis,” Section 6.1.2), especially when large regions of the model are expected to flow plastically and when the difference between is not large, a symmetric approximation to the matrix can provide an acceptable rate of convergence of the equilibrium equations and, hence, a lower overall solution cost. Therefore, the unsymmetric matrix solution scheme is not invoked automatically when jointed material behavior is defined. is large. If the difference between and and Elements The jointed material model can be used with plane strain, generalized plane strain, axisymmetric, and three-dimensional solid (continuum) elements in Abaqus/Standard. This model cannot be used with elements for which the assumed stress state is plane stress (plane stress, shell, and membrane elements). 23.6 Concrete • “Concrete smeared cracking,” Section 23.6.1 • “Cracking model for concrete,” Section 23.6.2 • “Concrete damaged plasticity,” Section 23.6.3 23.6.1 CONCRETE SMEARED CRACKING Products: Abaqus/Standard Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *CONCRETE • *TENSION STIFFENING • *SHEAR RETENTION • *FAILURE RATIOS • “Defining concrete smeared cracking” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The smeared crack concrete model in Abaqus/Standard: • provides a general capability for modeling concrete in all types of structures, including beams, trusses, shells, and solids; • can be used for plain concrete, even though it is intended primarily for the analysis of reinforced concrete structures; • can be used with rebar to model concrete reinforcement; • is designed for applications in which the concrete is subjected to essentially monotonic straining at low confining pressures; • consists of an isotropically hardening yield surface that is active when the stress is dominantly compressive and an independent “crack detection surface” that determines if a point fails by cracking; • uses oriented damaged elasticity concepts (smeared cracking) to describe the reversible part of the material’s response after cracking failure; • requires that the linear elastic material model be used to define elastic properties; and • cannot be used with local orientations . See “Inelastic behavior,” Section 23.1.1, for a discussion of the concrete models available in Abaqus. Reinforcement Reinforcement in concrete structures is typically provided by means of rebars, which are one-dimensional strain theory elements (rods) that can be defined singly or embedded in oriented surfaces. Rebars are typically used with metal plasticity models to describe the behavior of the rebar material and are superposed on a mesh of standard element types used to model the concrete. With this modeling approach, the concrete behavior is considered independently of the rebar. Effects associated with the rebar/concrete interface, such as bond slip and dowel action, are modeled approximately by introducing some “tension stiffening” into the concrete modeling to simulate load transfer across cracks through the rebar. Details regarding tension stiffening are provided below. Defining the rebar can be tedious in complex problems, but it is important that this be done accurately since it may cause an analysis to fail due to lack of reinforcement in key regions of a model. See “Defining reinforcement,” Section 2.2.3, for more information regarding rebars. Cracking The model is intended as a model of concrete behavior for relatively monotonic loadings under fairly low confining pressures (less than four to five times the magnitude of the largest stress that can be carried by the concrete in uniaxial compression). Crack detection Cracking is assumed to be the most important aspect of the behavior, and representation of cracking and of postcracking behavior dominates the modeling. Cracking is assumed to occur when the stress reaches a failure surface that is called the “crack detection surface.” This failure surface is a linear relationship between the equivalent pressure stress, p, and the Mises equivalent deviatoric stress, q, and is illustrated in Figure 23.6.1–5. When a crack has been detected, its orientation is stored for subsequent calculations. Subsequent cracking at the same point is restricted to being orthogonal to this direction since stress components associated with an open crack are not included in the definition of the failure surface used for detecting the additional cracks. Cracks are irrecoverable: they remain for the rest of the calculation (but may open and close). No more than three cracks can occur at any point (two in a plane stress case, one in a uniaxial stress case). Following crack detection, the crack affects the calculations because a damaged elasticity model is used. Oriented, damaged elasticity is discussed in more detail in “An inelastic constitutive model for concrete,” Section 4.5.1 of the Abaqus Theory Manual. Smeared cracking The concrete model is a smeared crack model in the sense that it does not track individual “macro” cracks. Constitutive calculations are performed independently at each integration point of the finite element model. The presence of cracks enters into these calculations by the way in which the cracks affect the stress and material stiffness associated with the integration point. Tension stiffening The postfailure behavior for direct straining across cracks is modeled with tension stiffening, which allows you to define the strain-softening behavior for cracked concrete. This behavior also allows for the effects of the reinforcement interaction with concrete to be simulated in a simple manner. Tension stiffening is required in the concrete smeared cracking model. You can specify tension stiffening by means of a postfailure stress-strain relation or by applying a fracture energy cracking criterion. Postfailure stress-strain relation Specification of strain softening behavior in reinforced concrete generally means specifying the postfailure stress as a function of strain across the crack. In cases with little or no reinforcement this specification often introduces mesh sensitivity in the analysis results in the sense that the finite element predictions do not converge to a unique solution as the mesh is refined because mesh refinement leads to narrower crack bands. This problem typically occurs if only a few discrete cracks form in the structure, and mesh refinement does not result in formation of additional cracks. If cracks are evenly distributed (either due to the effect of rebar or due to the presence of stabilizing elastic material, as in the case of plate bending), mesh sensitivity is less of a concern. In practical calculations for reinforced concrete, the mesh is usually such that each element contains rebars. The interaction between the rebars and the concrete tends to reduce the mesh sensitivity, provided that a reasonable amount of tension stiffening is introduced in the concrete model to simulate this interaction (Figure 23.6.1–1). Stress, σ σ u Abaqus Version 6.6 ID: Printed on: Failure point "tension stiffening" curve t = σ u Strain, it depends on such factors as the density of The tension stiffening effect must be estimated; reinforcement, the quality of the bond between the rebar and the concrete, the relative size of the concrete aggregate compared to the rebar diameter, and the mesh. A reasonable starting point for relatively heavily reinforced concrete modeled with a fairly detailed mesh is to assume that the strain softening after failure reduces the stress linearly to zero at a total strain of about 10 times the strain at failure. The strain at failure in standard concretes is typically 10−4, which suggests that tension stiffening that reduces the stress to zero at a total strain of about 10−3 is reasonable. This parameter should be calibrated to a particular case. The choice of tension stiffening parameters is important in Abaqus/Standard since, generally, more tension stiffening makes it easier to obtain numerical solutions. Too little tension stiffening will cause the local cracking failure in the concrete to introduce temporarily unstable behavior in the overall response of the model. Few practical designs exhibit such behavior, so that the presence of this type of response in the analysis model usually indicates that the tension stiffening is unreasonably low. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *CONCRETE *TENSION STIFFENING, TYPE=STRAIN (default) Property module: material editor: Mechanical→Plasticity→Concrete Smeared Cracking: Suboptions→Tension Stiffening: Type: Strain Fracture energy cracking criterion As discussed earlier, when there is no reinforcement in significant regions of a concrete model, the strain softening approach for defining tension stiffening may introduce unreasonable mesh sensitivity into the results. Crisfield (1986) discusses this issue and concludes that Hillerborg’s (1976) proposal is adequate to allay the concern for many practical purposes. Hillerborg defines the energy required to open a unit area of crack as a material parameter, using brittle fracture concepts. With this approach the concrete’s brittle behavior is characterized by a stress-displacement response rather than a stress-strain response. Under tension a concrete specimen will crack across some section. After it has been pulled apart sufficiently for most of the stress to be removed (so that the elastic strain is small), its length will be determined primarily by the opening at the crack. The opening does not depend on the specimen’s length (Figure 23.6.1–2). Implementation The implementation of this stress-displacement concept in a finite element model requires the definition of a characteristic length associated with an integration point. The characteristic crack length is based on the element geometry and formulation: it is a typical length of a line across an element for a first-order element; it is half of the same typical length for a second-order element. For beams and trusses it is a characteristic length along the element axis. For membranes and shells it is a characteristic length in the reference surface. For axisymmetric elements it is a characteristic length in the r–z plane only. For cohesive elements it is equal to the constitutive thickness. This definition of the characteristic crack length is used because the direction in which cracks will occur is not known in advance. Therefore, elements with large aspect ratios will have rather different behavior depending on the direction in which Stress, σ σ u Figure 23.6.1–2 Fracture energy cracking model. u 0 u, displacement they crack: some mesh sensitivity remains because of this effect, and elements that are as close to square as possible are recommended. This approach to modeling the concrete’s brittle response requires the specification of the at which a linear approximation to the postfailure strain softening gives zero stress , occurs at a failure strain (defined by the failure stress divided by the Young’s modulus); however, the stress goes to zero at an ultimate displacement, , that is independent of the specimen length. The implication is that a displacement-loaded specimen can remain in static equilibrium after failure only if the specimen is short enough so that the strain at failure, , is less than the strain at this value of the displacement: displacement . The failure stress, where L is the length of the specimen. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *CONCRETE *TENSION STIFFENING, TYPE=DISPLACEMENT Property module: material editor: Mechanical→Plasticity→Concrete Smeared Cracking: Suboptions→Tension Stiffening: Type: Displacement Obtaining the ultimate displacement , where The ultimate displacement, , as is the maximum tensile stress that the concrete can carry. Typical values for , can be estimated from the fracture energy per unit area, are 0.05 mm (2 × 10−3 in) for a normal concrete to 0.08 mm (3 × 10−3 in) for a high strength concrete. A typical value for is about 10−4, so that the requirement is that mm (20 in). Critical length If the specimen is longer than the critical length, L, more strain energy is stored in the specimen than can be dissipated by the cracking process when it cracks under fixed displacement. Some of the strain energy must, therefore, be converted into kinetic energy, and the failure event must be dynamic even under prescribed displacement loading. This implies that, when this approach is used in finite elements, characteristic element dimensions must be less than this critical length, or additional (dynamic) considerations must be included. The analysis input file processor checks the characteristic length of each element using this concrete model and will not allow any element to have a characteristic length that exceeds . You must remesh with smaller elements where necessary or use the stress-strain definition of tension stiffening. Since the fracture energy approach is generally used only for plain concrete, this rarely places any limit on the meshing. Cracked shear retention As the concrete cracks, its shear stiffness is diminished. This effect is defined by specifying the reduction in the shear modulus as a function of the opening strain across the crack. You can also specify a reduced shear modulus for closed cracks. This reduced shear modulus will also have an effect when the normal stress across a crack becomes compressive. The new shear stiffness will have been degraded by the presence of the crack. The modulus for shearing of cracks is defined as , where G is the elastic shear modulus of the is a multiplying factor. The shear retention model assumes that the shear uncracked concrete and stiffness of open cracks reduces linearly to zero as the crack opening increases: for for is the direct strain across the crack and where that cracks that subsequently close have a reduced shear modulus: is a user-specified value. The model also assumes for where you specify . and can be defined with an optional dependency on temperature and/or predefined field variables. If shear retention is not included in the material definition for the concrete smeared cracking model, Abaqus/Standard will automatically invoke the default behavior for shear retention such that the shear response is unaffected by cracking (full shear retention). This assumption is often reasonable: in many cases, the overall response is not strongly dependent on the amount of shear retention. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *CONCRETE *SHEAR RETENTION Property module: material editor: Mechanical→Plasticity→Concrete Smeared Cracking: Suboptions→Shear Retention Compressive behavior When the principal stress components are dominantly compressive, the response of the concrete is modeled by an elastic-plastic theory using a simple form of yield surface written in terms of the equivalent pressure stress, p, and the Mises equivalent deviatoric stress, q; this surface is illustrated in Figure 23.6.1–5. Associated flow and isotropic hardening are used. This model significantly simplifies the actual behavior. The associated flow assumption generally over-predicts the inelastic volume strain. The yield surface cannot be matched accurately to data in triaxial tension and triaxial compression tests because of the omission of third stress invariant dependence. When the concrete is strained beyond the ultimate stress point, the assumption that the elastic response is not affected by the inelastic deformation is not realistic. In addition, when concrete is subjected to very high pressure stress, it exhibits inelastic response: no attempt has been made to build this behavior into the model. The simplifications associated with compressive behavior are introduced for the sake of In particular, while the assumption of associated flow is not justified by computational efficiency. experimental data, it can provide results that are acceptably close to measurements, provided that the range of pressure stress in the problem is not large. From a computational viewpoint, the associated flow assumption leads to enough symmetry in the Jacobian matrix of the integrated constitutive model (the “material stiffness matrix”) such that the overall equilibrium equation solution usually does not require unsymmetric equation solution. All of these limitations could be removed at some sacrifice in computational cost. You can define the stress-strain behavior of plain concrete in uniaxial compression outside the elastic range. Compressive stress data are provided as a tabular function of plastic strain and, if desired, temperature and field variables. Positive (absolute) values should be given for the compressive stress and strain. The stress-strain curve can be defined beyond the ultimate stress, into the strain-softening regime. Input File Usage: Abaqus/CAE Usage: *CONCRETE Property module: material editor: Mechanical→Plasticity→Concrete Smeared Cracking Uniaxial and multiaxial behavior The cracking and compressive responses of concrete that are incorporated in the concrete model are illustrated by the uniaxial response of a specimen shown in Figure 23.6.1–3. When concrete is loaded in compression, it initially exhibits elastic response. As the stress is increased, some nonrecoverable (inelastic) straining occurs and the response of the material softens. An ultimate stress is reached, after which the material loses strength until it can no longer carry any stress. If the load is removed at some point after inelastic straining has occurred, the unloading response is softer than the initial elastic response: the elasticity has been damaged. This effect is ignored in the model, since we assume that the applications involve primarily monotonic straining, with only occasional, minor unloadings. When a uniaxial concrete specimen is loaded in tension, it responds elastically until, at a stress that is typically 7%–10% of the ultimate compressive stress, cracks form. Cracks form so quickly that, even in the stiffest testing machines available, it is very difficult to observe the actual behavior. The Stress Failure point in compression (peak stress) Start of inelastic behavior Unload/reload response Idealized (elastic) unload/reload response Strain Softening Cracking failure Figure 23.6.1–3 Uniaxial behavior of plain concrete. model assumes that cracking causes damage, in the sense that open cracks can be represented by a loss of elastic stiffness. It is also assumed that there is no permanent strain associated with cracking. This will allow cracks to close completely if the stress across them becomes compressive. In multiaxial stress states these observations are generalized through the concept of surfaces of failure and flow in stress space. These surfaces are fitted to experimental data. The surfaces used are shown in Figure 23.6.1–4 and Figure 23.6.1–5. Failure surface You can specify failure ratios to define the shape of the failure surface (possibly as a function of temperature and predefined field variables). Four failure ratios can be specified: • The ratio of the ultimate biaxial compressive stress to the ultimate uniaxial compressive stress. • The absolute value of the ratio of the uniaxial tensile stress at failure to the ultimate uniaxial compressive stress. • The ratio of the magnitude of a principal component of plastic strain at ultimate stress in biaxial compression to the plastic strain at ultimate stress in uniaxial compression. "crack detection" surface uniaxial tension biaxial tension uniaxial compression "compression" surface biaxial compression Figure 23.6.1–4 Yield and failure surfaces in plane stress. • The ratio of the tensile principal stress at cracking, in plane stress, when the other principal stress is at the ultimate compressive value, to the tensile cracking stress under uniaxial tension. Input File Usage: Default values of the above ratios are used if you do not specify them. *FAILURE RATIOS Property module: material editor: Mechanical→Plasticity→Concrete Smeared Cracking: Suboptions→Failure Ratios Abaqus/CAE Usage: Response to strain reversals Because the model is intended for application to problems involving relatively monotonic straining, no attempt is made to include prediction of cyclic response or of the reduction in the elastic stiffness caused σ u "crack detection" surface "compression" surface σ u Figure 23.6.1–5 Yield and failure surfaces in the (p–q) plane. by inelastic straining under predominantly compressive stress. Nevertheless, it is likely that, even in those applications for which the model is designed, the strain trajectories will not be entirely radial, so that the model should predict the response to occasional strain reversals and strain trajectory direction changes in a reasonable way. Isotropic hardening of the “compressive” yield surface forms the basis of this aspect of the model’s inelastic response prediction when the principal stresses are dominantly compressive. Calibration A minimum of two experiments, uniaxial compression and uniaxial tension, is required to calibrate the simplest version of the concrete model (using all possible defaults and assuming temperature and field variable independence). Other experiments may be required to gain accuracy in postfailure behavior. Uniaxial compression and tension tests The uniaxial compression test involves compressing the sample between two rigid platens. The load and displacement in the direction of loading are recorded. From this, you can extract the stress-strain curve required for the concrete model directly. The uniaxial tension test is much more difficult to perform in the sense that it is necessary to have a stiff testing machine to be able to record the postfailure response. Quite often this test is not available, and you make an assumption about the tensile failure strength of the concrete (usually about 7%–10% of the compressive strength). The choice of tensile cracking stress is important; numerical problems may arise if very low cracking stresses are used (less than 1/100 or 1/1000 of the compressive strength). Postcracking tensile behavior The calibration of the postfailure response depends on the reinforcement present in the concrete. For plain concrete simulations the stress-displacement tension stiffening model should be used. Typical are 0.05 mm (2 × 10−3 in) for a normal concrete to 0.08 mm (3 × 10−3 in) for a high-strength values for concrete. For reinforced concrete simulations the stress-strain tension stiffening model should be used. A reasonable starting point for relatively heavily reinforced concrete modeled with a fairly detailed mesh is to assume that the strain softening after failure reduces the stress linearly to zero at a total strain of about 10 times the strain at failure. Since the strain at failure in standard concretes is typically 10−4 , this suggests that tension stiffening that reduces the stress to zero at a total strain of about 10−3 is reasonable. This parameter should be calibrated to a particular case. Postcracking shear behavior Combined tension and shear experiments are used to calibrate the postcracking shear behavior in Abaqus/Standard. These experiments are quite difficult to perform. If the test data are not available, a reasonable starting point is to assume that the shear retention factor, , goes linearly to zero at the same crack opening strain used for the tension stiffening model. Biaxial yield and flow parameters Biaxial experiments are required to calibrate the biaxial yield and flow parameters used to specify the failure ratios. If these are not available, the defaults can be used. Temperature dependence The calibration of temperature dependence requires the repetition of all the above experiments over the range of interest. Comparison with experimental results With proper calibration, the concrete model should produce reasonable results for mostly monotonic loadings. Comparison of the predictions of the model with the experimental results of Kupfer and Gerstle (1973) are shown in Figure 23.6.1–6 and Figure 23.6.1–7. Elements Abaqus/Standard offers a variety of elements for use with the smeared crack concrete model: beam, shell, plane stress, plane strain, generalized plane strain, axisymmetric, and three-dimensional elements. For general shell analysis more than the default number of five integration points through the thickness of the shell should be used; nine thickness integration points are commonly used to model progressive failure of the concrete through the thickness with acceptable accuracy. 30.0 25.0 20.0 15.0 10.0 5.0 0.0000 0.0005 30.0 25.0 20.0 15.0 10.0 5.0 5.0 4.0 3.0 2.0 1.0 / , Model Kupfer and Gerstle, 1973 0.0010 0.0015 Compressive strain in loaded direction 0.0020 0.0025 0.0030 5.0 4.0 3.0 2.0 1.0 / , Model Kupfer and Gerstle, 1973 / , / / , , 0.0000 0.0005 0.0010 0.0015 0.0020 0.0025 0.0030 Tensile strain normal to loaded direction Figure 23.6.1–6 Comparison of model prediction and Kupfer and Gerstle’s data for a uniaxial compression test. 5.0 4.0 3.0 2.0 1.0 / , Model Kupfer and Gerstle, 1973 30.0 25.0 20.0 15.0 10.0 5.0 / , 0.0000 0.0005 0.0010 0.0015 0.0020 0.0025 0.0030 Compressive strain in loaded plane 30.0 / 25.0 , 20.0 15.0 10.0 5.0 5.0 4.0 3.0 2.0 1.0 / , Model Kupfer and Gerstle, 1973 0.0000 0.0005 0.0010 0.0015 0.0020 0.0025 0.0030 Compressive strain normal to loaded plane Figure 23.6.1–7 Comparison of model prediction and Kupfer and Gerstle’s data for a biaxial compression test. Output In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables relate specifically to material points in the smeared crack concrete model: CRACK CONF Unit normal to cracks in concrete. Number of cracks at a concrete material point. Additional references • Crisfield, M. A., “Snap-Through and Snap-Back Response in Concrete Structures and the Dangers of Under-Integration,” International Journal for Numerical Methods in Engineering, vol. 22, pp. 751–767, 1986. • Hillerborg, A., M. Modeer, and P. E. Petersson, “Analysis of Crack Formation and Crack Growth in Concrete by Means of Fracture Mechanics and Finite Elements,” Cement and Concrete Research, vol. 6, pp. 773–782, 1976. • Kupfer, H. B., and K. H. Gerstle, “Behavior of Concrete under Biaxial Stresses,” Journal of Engineering Mechanics Division, ASCE, vol. 99, p. 853, 1973. 23.6.2 CRACKING MODEL FOR CONCRETE Products: Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *BRITTLE CRACKING • *BRITTLE FAILURE • *BRITTLE SHEAR • “Defining brittle cracking” in “Defining other mechanical models,” Section 12.9.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The brittle cracking model in Abaqus/Explicit: • provides a capability for modeling concrete in all types of structures: beams, trusses, shells and solids; • can also be useful for modeling other materials such as ceramics or brittle rocks; • is designed for applications in which the behavior is dominated by tensile cracking; • assumes that the compressive behavior is always linear elastic; • must be used with the linear elastic material model (“Linear elastic behavior,” Section 22.2.1), which also defines the material behavior completely prior to cracking; • is most accurate in applications where the brittle behavior dominates such that the assumption that the material is linear elastic in compression is adequate; • can be used for plain concrete, even though it is intended primarily for the analysis of reinforced concrete structures; • allows removal of elements based on a brittle failure criterion; and • is defined in detail in “A cracking model for concrete and other brittle materials,” Section 4.5.3 of the Abaqus Theory Manual. See “Inelastic behavior,” Section 23.1.1, for a discussion of the concrete models available in Abaqus. Reinforcement Rebars are in concrete structures is typically provided by means of rebars. Reinforcement one-dimensional strain theory elements (rods) that can be defined singly or embedded in oriented surfaces. Rebars are discussed in “Defining rebar as an element property,” Section 2.2.4. They are typically used with elastic-plastic material behavior and are superposed on a mesh of standard element types used to model the plain concrete. With this modeling approach, the concrete cracking behavior is considered independently of the rebar. Effects associated with the rebar/concrete interface, such as bond slip and dowel action, are modeled approximately by introducing some “tension stiffening” into the concrete cracking model to simulate load transfer across cracks through the rebar. Cracking Abaqus/Explicit uses a smeared crack model to represent the discontinuous brittle behavior in concrete. It does not track individual “macro” cracks: instead, constitutive calculations are performed independently at each material point of the finite element model. The presence of cracks enters into these calculations by the way in which the cracks affect the stress and material stiffness associated with the material point. For simplicity of discussion in this section, the term “crack” is used to mean a direction in which cracking has been detected at the single material calculation point in question: the closest physical concept is that there exists a continuum of micro-cracks in the neighborhood of the point, oriented as determined by the model. The anisotropy introduced by cracking is assumed to be important in the simulations for which the model is intended. Crack directions The Abaqus/Explicit cracking model assumes fixed, orthogonal cracks, with the maximum number of cracks at a material point limited by the number of direct stress components present at that material point of the finite element model (a maximum of three cracks in three-dimensional, plane strain, and axisymmetric problems; two cracks in plane stress and shell problems; and one crack in beam or truss problems). Internally, once cracks exist at a point, the component forms of all vector- and tensor-valued quantities are rotated so that they lie in the local system defined by the crack orientation vectors (the normals to the crack faces). The model ensures that these crack face normal vectors will be orthogonal, so that this local crack system is rectangular Cartesian. For output purposes you are offered results of stresses and strains in the global and/or local crack systems. Crack detection A simple Rankine criterion is used to detect crack initiation. This criterion states that a crack forms when the maximum principal tensile stress exceeds the tensile strength of the brittle material. Although crack detection is based purely on Mode I fracture considerations, ensuing cracked behavior includes both Mode I (tension softening/stiffening) and Mode II (shear softening/retention) behavior, as described later. As soon as the Rankine criterion for crack formation has been met, we assume that a first crack has formed. The crack surface is taken to be normal to the direction of the maximum tensile principal stress. Subsequent cracks may form with crack surface normals in the direction of maximum principal tensile stress that is orthogonal to the directions of any existing crack surface normals at the same point. Cracking is irrecoverable in the sense that, once a crack has occurred at a point, it remains throughout the rest of the calculation. However, crack closing and reopening may take place along the directions of the crack surface normals. The model neglects any permanent strain associated with cracking; that is, it is assumed that the cracks can close completely when the stress across them becomes compressive. Tension stiffening You can specify the postfailure behavior for direct straining across cracks by means of a postfailure stress-strain relation or by applying a fracture energy cracking criterion. Postfailure stress-strain relation In reinforced concrete the specification of postfailure behavior generally means giving the postfailure stress as a function of strain across the crack (Figure 23.6.2–1). In cases with little or no reinforcement, this introduces mesh sensitivity in the results, in the sense that the finite element predictions do not converge to a unique solution as the mesh is refined because mesh refinement leads to narrower crack bands. σ Ι Figure 23.6.2–1 Postfailure stress-strain curve. e ck nn In practical calculations for reinforced concrete, the mesh is usually such that each element contains rebars. In this case the interaction between the rebars and the concrete tends to mitigate this effect, provided that a reasonable amount of “tension stiffening” is introduced in the cracking model to simulate this interaction. This requires an estimate of the tension stiffening effect, which depends on factors such as the density of reinforcement, the quality of the bond between the rebar and the concrete, the relative size of the concrete aggregate compared to the rebar diameter, and the mesh. A reasonable starting point for relatively heavily reinforced concrete modeled with a fairly detailed mesh is to assume that the strain softening after failure reduces the stress linearly to zero at a total strain about ten times the strain at failure. Since the strain at failure in standard concretes is typically 10−4 , this suggests that tension stiffening that reduces the stress to zero at a total strain of about 10−3 is reasonable. This parameter should be calibrated to each particular case. In static applications too little tension stiffening will cause the local cracking failure in the concrete to introduce temporarily unstable behavior in the overall response of the model. Few practical designs exhibit such behavior, so that the presence of this type of response in the analysis model usually indicates that the tension stiffening is unreasonably low. Input File Usage: *BRITTLE CRACKING, TYPE=STRAIN Abaqus/CAE Usage: Property module: material editor: Mechanical→Brittle Cracking: Type: Strain Fracture energy cracking criterion When there is no reinforcement in significant regions of the model, the tension stiffening approach described above will introduce unreasonable mesh sensitivity into the results. However, it is generally accepted that Hillerborg’s (1976) fracture energy proposal is adequate to allay the concern for many practical purposes. Hillerborg defines the energy required to open a unit area of crack in Mode I ( ) as a material parameter, using brittle fracture concepts. With this approach the concrete’s brittle behavior is characterized by a stress-displacement response rather than a stress-strain response. Under tension a concrete specimen will crack across some section; and its length, after it has been pulled apart sufficiently for most of the stress to be removed (so that the elastic strain is small), will be determined primarily by the opening at the crack, which does not depend on the specimen’s length. Implementation In Abaqus/Explicit this fracture energy cracking model can be invoked by specifying the postfailure stress as a tabular function of displacement across the crack, as illustrated in Figure 23.6.2–2. σ Ι Figure 23.6.2–2 Postfailure stress-displacement curve. u ck , can be specified directly as a material property; in this Alternatively, the Mode I fracture energy, case, define the failure stress, , as a tabular function of the associated Mode I fracture energy. This model assumes a linear loss of strength after cracking (Figure 23.6.2–3). The crack normal displacement at which complete loss of strength takes place is, therefore, . Typical values of range from 40 N/m (0.22 lb/in) for a typical construction concrete (with a compressive strength of approximately 20 MPa, 2850 lb/in2 ) to 120 N/m (0.67 lb/in) for a high-strength concrete (with a compressive strength of approximately 40 MPa, 5700 lb/in2). Input File Usage: Use the following option to specify the postfailure stress as a tabular function of displacement: *BRITTLE CRACKING, TYPE=DISPLACEMENT σ Ι tu CRACKING MODEL tu u n u = 2G /σ no Figure 23.6.2–3 Postfailure stress-fracture energy curve. Use the following option to specify the postfailure stress as a tabular function of the fracture energy: *BRITTLE CRACKING, TYPE=GFI Property module: material editor: Mechanical→Brittle Cracking: Type: Displacement or GFI Abaqus/CAE Usage: Characteristic crack length The implementation of the stress-displacement concept in a finite element model requires the definition of a characteristic length associated with a material point. The characteristic crack length is based on the element geometry and formulation: it is a typical length of a line across an element for a first-order element; it is half of the same typical length for a second-order element. For beams and trusses it is a characteristic length along the element axis. For membranes and shells it is a characteristic length in the reference surface. For axisymmetric elements it is a characteristic length in the r–z plane only. For cohesive elements it is equal to the constitutive thickness. We use this definition of the characteristic crack length because the direction in which cracks will occur is not known in advance. Therefore, elements with large aspect ratios will have rather different behavior depending on the direction in which they crack: some mesh sensitivity remains because of this effect. Elements that are as close to square as possible are, therefore, recommended unless you can predict the direction in which cracks will form. Shear retention model An important feature of the cracking model is that, whereas crack initiation is based on Mode I fracture only, postcracked behavior includes Mode II as well as Mode I. The Mode II shear behavior is based on the common observation that the shear behavior depends on the amount of crack opening. More specifically, the cracked shear modulus is reduced as the crack opens. Therefore, Abaqus/Explicit offers a shear retention model in which the postcracked shear stiffness is defined as a function of the opening strain across the crack; the shear retention model must be defined in the cracking model, and zero shear retention should not be used. In these models the dependence is defined by expressing the postcracking shear modulus, , as a fraction of the uncracked shear modulus: where G is the shear modulus of the uncracked material and the shear retention factor, on the crack opening strain, Figure 23.6.2–4. , depends . You can specify this dependence in piecewise linear form, as shown in Figure 23.6.2–4 Piecewise linear form of the shear retention model. Alternatively, shear retention can be defined in the power law form: e ck nn are material parameters. This form, shown in Figure 23.6.2–5, satisfies the where p and requirements that as (corresponding to complete loss of aggregate interlock). See “A cracking model for concrete and other brittle materials,” Section 4.5.3 of the Abaqus Theory Manual, for a discussion of how shear retention is calculated in the case of two or more cracks. (corresponding to the state before crack initiation) and as Input File Usage: Use the following option to specify the piecewise linear form of the shear retention model: *BRITTLE SHEAR, TYPE=RETENTION FACTOR Use the following option to specify the power law form of the shear retention model: *BRITTLE SHEAR, TYPE=POWER LAW p = 1 e ck max e ck nn Figure 23.6.2–5 Power law form of the shear retention model. Abaqus/CAE Usage: Property module: material editor: Mechanical→Brittle Cracking: Suboptions→Brittle Shear Type: Retention Factor or Power Law Calibration One experiment, a uniaxial tension test, is required to calibrate the simplest version of the brittle cracking model. Other experiments may be required to gain accuracy in postfailure behavior. Uniaxial tension test This test is difficult to perform because it is necessary to have a very stiff testing machine to record the postcracking response. Quite often such equipment is not available; in this situation you must make an assumption about the tensile failure strength of the material and the postcracking response. For concrete the assumption usually made is that the tensile strength is 7–10% of the compressive strength. Uniaxial compression tests can be performed much more easily, so the compressive strength of concrete is usually known. Postcracking tensile behavior The values given for tension stiffening are a very important aspect of simulations using the Abaqus/Explicit brittle cracking model. The postcracking tensile response is highly dependent on the reinforcement present in the concrete. In simulations of unreinforced concrete, the tension stiffening models that are based on fracture energy concepts should be utilized. If reliable experimental data are not available, typical values that can be used were discussed before: common values of range from 40 N/m (0.22 lb/in) for a typical construction concrete (with a compressive strength of approximately 20 MPa, 2850 lb/in2 ) to 120 N/m (0.67 lb/in) for a high-strength concrete (with a compressive strength of approximately 40 MPa, 5700 lb/in2 ). In simulations of reinforced concrete the stress-strain tension stiffening model should be used; the amount of tension stiffening depends on the reinforcement present, as discussed before. A reasonable starting point for relatively heavily reinforced concrete modeled with a fairly detailed mesh is to assume that the strain softening after failure reduces the stress linearly to zero at a total strain about ten times the strain at failure. Since the strain at failure in standard concretes is typically 10−4 , this suggests that tension stiffening that reduces the stress to zero at a total strain of about 10−3 is reasonable. This parameter should be calibrated to each particular case. Postcracking shear behavior Calibration of the postcracking shear behavior requires combined tension and shear experiments, which are difficult to perform. If such test data are not available, a reasonable starting point is to assume that the shear retention factor, , goes linearly to zero at the same crack opening strain used for the tension stiffening model. Brittle failure criterion You can define brittle failure of the material. When one, two, or all three local direct cracking strain (displacement) components at a material point reach the value defined as the failure strain (displacement), the material point fails and all the stress components are set to zero. If all of the material points in an element fail, the element is removed from the mesh. For example, removal of a first-order reduced- integration solid element takes place as soon as its only integration point fails. However, all through- the-thickness integration points must fail before a shell element is removed from the mesh. If the postfailure relation is defined in terms of stress versus strain, the failure strain must be given as the failure criterion. If the postfailure relation is defined in terms of stress versus displacement or stress versus fracture energy, the failure displacement must be given as the failure criterion. The failure strain (displacement) can be specified as a function of temperature and/or predefined field variables. You can control how many cracks at a material point must fail before the material point is considered to have failed; the default is one crack. The number of cracks that must fail can only be one for beam and truss elements; it cannot be greater than two for plane stress and shell elements; and it cannot be greater than three otherwise. Input File Usage: Abaqus/CAE Usage: *BRITTLE FAILURE, CRACKS=n Property module: material editor: Mechanical→Brittle Cracking: Suboptions→Brittle Failure and select Failure Criteria: Unidirectional, Bidirectional, or Tridirectional to indicate the number of cracks that must fail for the material point to fail. Determining when to use the brittle failure criterion The brittle failure criterion is a crude way of modeling failure in Abaqus/Explicit and should be used with care. The main motivation for including this capability is to help in computations where not removing an element that can no longer carry stress may lead to excessive distortion of that element and subsequent premature termination of the simulation. For example, in a monotonically loaded structure whose failure mechanism is expected to be dominated by a single tensile macrofracture (Mode I cracking), it may be reasonable to use the brittle failure criterion to remove elements. On the other hand, the fact that the brittle material loses its ability to carry tensile stress does not preclude it from withstanding compressive stress; therefore, it may not be appropriate to remove elements if the material is expected to carry compressive loads after it has failed in tension. An example may be a shear wall subjected to cyclic loading as a result of some earthquake excitation; in this case cracks that develop completely under tensile stress will be able to carry compressive stress when load reversal takes place. Thus, the effective use of the brittle failure criterion relies on you having some knowledge of the structural behavior and potential failure mechanism. The use of the brittle failure criterion based on an incorrect user assumption of the failure mechanism will generally result in an incorrect simulation. Selecting the number of cracks that must fail before the material point is considered to have failed When you define brittle failure, you can control how many cracks must open to beyond the failure value before a material point is considered to have failed. The default number of cracks (one) should be used for most structural applications where failure is dominated by Mode I type cracking. However, there are cases in which you should specify a higher number because multiple cracks need to form to develop the eventual failure mechanism. One example may be an unreinforced, deep concrete beam where the failure mechanism is dominated by shear; in this case it is possible that two cracks need to form at each material point for the shear failure mechanism to develop. Again, the appropriate choice of the number of cracks that must fail relies on your knowledge of the structural and failure behaviors. Using brittle failure with rebar It is possible to use the brittle failure criterion in brittle cracking elements for which rebar are also defined; the obvious application is the modeling of reinforced concrete. When such elements fail according to the brittle failure criterion, the brittle cracking contribution to the element stress carrying capacity is removed but the rebar contribution to the element stress carrying capacity is not removed. However, if you also include shear failure in the rebar material definition, the rebar contribution to the element stress carrying capacity will also be removed if the shear failure criterion specified for the rebar is satisfied. This allows the modeling of progressive failure of an under-reinforced concrete structure where the concrete fails first followed by ductile failure of the reinforcement. Elements Abaqus/Explicit offers a variety of elements for use with the cracking model: shell; two-dimensional beam; and plane stress, plane strain, axisymmetric, and three-dimensional continuum elements. The model cannot be used with pipe and three-dimensional beam elements. Plane triangular, triangular prism, and tetrahedral elements are not recommended for use in reinforced concrete analysis since these elements do not support the use of rebar. truss; Output In addition to the standard output identifiers available in Abaqus/Explicit , the following output variables relate directly to material points that use the brittle cracking model: CKE CKLE All cracking strain components. All cracking strain components in local crack axes. CKEMAG Cracking strain magnitude. CKLS CRACK CKSTAT STATUS Additional reference All stress components in local crack axes. Crack orientations. Crack status of each crack. Status of element (brittle failure model). The status of an element is 1.0 if the element is active and 0.0 if the element is not. • Hillerborg, A., M. Modeer, and P. E. Petersson, “Analysis of Crack Formation and Crack Growth in Concrete by Means of Fracture Mechanics and Finite Elements,” Cement and Concrete Research, vol. 6, pp. 773–782, 1976. 23.6.3 CONCRETE DAMAGED PLASTICITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Inelastic behavior,” Section 23.1.1 • *CONCRETE DAMAGED PLASTICITY • *CONCRETE TENSION STIFFENING • *CONCRETE COMPRESSION HARDENING • *CONCRETE TENSION DAMAGE • *CONCRETE COMPRESSION DAMAGE • “Defining concrete damaged plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The concrete damaged plasticity model in Abaqus: • provides a general capability for modeling concrete and other quasi-brittle materials in all types of structures (beams, trusses, shells, and solids); • uses concepts of isotropic damaged elasticity in combination with isotropic tensile and compressive plasticity to represent the inelastic behavior of concrete; • can be used for plain concrete, even though it is intended primarily for the analysis of reinforced concrete structures; • can be used with rebar to model concrete reinforcement; • is designed for applications in which concrete is subjected to monotonic, cyclic, and/or dynamic loading under low confining pressures; • consists of the combination of nonassociated multi-hardening plasticity and scalar (isotropic) damaged elasticity to describe the irreversible damage that occurs during the fracturing process; • allows user control of stiffness recovery effects during cyclic load reversals; • can be defined to be sensitive to the rate of straining; • can be used in conjunction with a viscoplastic regularization of the constitutive equations in Abaqus/Standard to improve the convergence rate in the softening regime; • requires that the elastic behavior of the material be isotropic and linear ; and • is defined in detail in “Damaged plasticity model for concrete and other quasi-brittle materials,” Section 4.5.2 of the Abaqus Theory Manual. See “Inelastic behavior,” Section 23.1.1, for a discussion of the concrete models available in Abaqus. Mechanical behavior The model is a continuum, plasticity-based, damage model for concrete. It assumes that the main two failure mechanisms are tensile cracking and compressive crushing of the concrete material. The evolution of the yield (or failure) surface is controlled by two hardening variables, , linked to failure mechanisms under tension and compression loading, respectively. We refer to as tensile and compressive equivalent plastic strains, respectively. The following sections discuss the main assumptions about the mechanical behavior of concrete. and and Uniaxial tension and compression stress behavior The model assumes that the uniaxial tensile and compressive response of concrete is characterized by damaged plasticity, as shown in Figure 23.6.3–1. Under uniaxial tension the stress-strain response follows a linear elastic relationship until the value of the failure stress, , is reached. The failure stress corresponds to the onset of micro-cracking in the concrete material. Beyond the failure stress the formation of micro-cracks is represented macroscopically with a softening stress-strain response, which induces strain localization in the concrete structure. Under uniaxial compression the response is linear until the value of initial yield, . In the plastic regime the response is typically characterized by stress hardening followed by strain softening beyond the ultimate stress, . This representation, although somewhat simplified, captures the main features of the response of concrete. It is assumed that the uniaxial stress-strain curves can be converted into stress versus plastic-strain curves. (This conversion is performed automatically by Abaqus from the user-provided stress versus “inelastic” strain data, as explained below.) Thus, where the subscripts t and c refer to tension and compression, respectively; plastic strains, are other predefined field variables. are the equivalent plastic strain rates, and is the temperature, and and are the equivalent As shown in Figure 23.6.3–1, when the concrete specimen is unloaded from any point on the strain softening branch of the stress-strain curves, the unloading response is weakened: the elastic stiffness of the material appears to be damaged (or degraded). The degradation of the elastic stiffness is characterized by two damage variables, , which are assumed to be functions of the plastic strains, temperature, and field variables: and The damage variables can take values from zero, representing the undamaged material, to one, which represents total loss of strength. (a) (b) ε t σ t σ σ t0 E _ (1 d )Et 0 pl~ ε t ε el t σ c σ c u σ c 0 E0 _ (1 d )Ec 0 pl~ ε ε el ε c Figure 23.6.3–1 Response of concrete to uniaxial loading in tension (a) and compression (b). If is the initial (undamaged) elastic stiffness of the material, the stress-strain relations under uniaxial tension and compression loading are, respectively: We define the “effective” tensile and compressive cohesion stresses as The effective cohesion stresses determine the size of the yield (or failure) surface. Uniaxial cyclic behavior Under uniaxial cyclic loading conditions the degradation mechanisms are quite complex, involving the opening and closing of previously formed micro-cracks, as well as their interaction. Experimentally, it is observed that there is some recovery of the elastic stiffness as the load changes sign during a uniaxial cyclic test. The stiffness recovery effect, also known as the “unilateral effect,” is an important aspect of the concrete behavior under cyclic loading. The effect is usually more pronounced as the load changes from tension to compression, causing tensile cracks to close, which results in the recovery of the compressive stiffness. The concrete damaged plasticity model assumes that the reduction of the elastic modulus is given in terms of a scalar degradation variable d as where is the initial (undamaged) modulus of the material. This expression holds both in the tensile ( ) sides of the cycle. The stiffness degradation variable, d, is a function of the stress state and the uniaxial damage variables, ) and the compressive ( and . For the uniaxial cyclic conditions Abaqus assumes that where associated with stress reversals. They are defined according to and are functions of the stress state that are introduced to model stiffness recovery effects where and , which are assumed to be material properties, control the recovery of The weight factors the tensile and compressive stiffness upon load reversal. To illustrate this, consider the example in Figure 23.6.3–2, where the load changes from tension to compression. Assume that there was no previous compressive damage (crushing) in the material; that is, . Then and ε t σ t σ σ t0 E _ (1 d )Et 0 w = 1c w = 0c Figure 23.6.3–2 Illustration of the effect of the compression stiffness recovery parameter . • In tension ( • In compression ( ), ; therefore, as expected. ), ; therefore, the material fully recovers the compressive stiffness (which in this case is the initial undamaged stiffness, and there is no stiffness recovery. Intermediate values of result in partial recovery of the stiffness. ). If, on the other hand, , then , then , and . If Multiaxial behavior The stress-strain relations for the general three-dimensional multiaxial condition are given by the scalar damage elasticity equation: where is the initial (undamaged) elasticity matrix. The previous expression for the scalar stiffness degradation variable, d, is generalized to the with a multiaxial stress weight factor, multiaxial stress case by replacing the unit step function , defined as where are the principal stress components. The Macauley bracket is defined by . See “Damaged plasticity model for concrete and other quasi-brittle materials,” Section 4.5.2 of the Abaqus Theory Manual, for further details of the constitutive model. Reinforcement In Abaqus reinforcement in concrete structures is typically provided by means of rebars, which are one-dimensional rods that can be defined singly or embedded in oriented surfaces. Rebars are typically used with metal plasticity models to describe the behavior of the rebar material and are superposed on a mesh of standard element types used to model the concrete. With this modeling approach, the concrete behavior is considered independently of the rebar. Effects associated with the rebar/concrete interface, such as bond slip and dowel action, are modeled approximately by introducing some “tension stiffening” into the concrete modeling to simulate load transfer across cracks through the rebar. Details regarding tension stiffening are provided below. Defining the rebar can be tedious in complex problems, but it is important that this be done accurately since it may cause an analysis to fail due to lack of reinforcement in key regions of a model. See “Defining rebar as an element property,” Section 2.2.4, for more information regarding rebars. Defining tension stiffening The postfailure behavior for direct straining is modeled with tension stiffening, which allows you to define the strain-softening behavior for cracked concrete. This behavior also allows for the effects of the reinforcement interaction with concrete to be simulated in a simple manner. Tension stiffening is required in the concrete damaged plasticity model. You can specify tension stiffening by means of a postfailure stress-strain relation or by applying a fracture energy cracking criterion. Postfailure stress-strain relation In reinforced concrete the specification of postfailure behavior generally means giving the postfailure stress as a function of cracking strain, . The cracking strain is defined as the total strain minus the elastic strain corresponding to the undamaged material; that is, , as illustrated in Figure 23.6.3–3. To avoid potential numerical problems, Abaqus enforces a lower limit on the postfailure stress equal to one-hundreth of the initial failure stress: Tension stiffening data are given in terms of the cracking strain, available, the data are provided to Abaqus in terms of tensile damage curves, Abaqus automatically converts the cracking strain values to plastic strain values using the relationship . When unloading data are , as discussed below. , where . t σ σ t0 E E _ (1 d )Et 0 ck~ ε el ε 0t ~ ε pl ε el CONCRETE DAMAGED PLASTICITY ε t Figure 23.6.3–3 Illustration of the definition of the cracking strain used for the definition of tension stiffening data. Abaqus will issue an error message if the calculated plastic strain values are negative and/or decreasing with increasing cracking strain, which typically indicates that the tensile damage curves are incorrect. In the absence of tensile damage . In cases with little or no reinforcement, the specification of a postfailure stress-strain relation introduces mesh sensitivity in the results, in the sense that the finite element predictions do not converge to a unique solution as the mesh is refined because mesh refinement leads to narrower crack bands. This problem typically occurs if cracking failure occurs only at localized regions in the structure and mesh refinement does not result in the formation of additional cracks. If cracking failure is distributed evenly (either due to the effect of rebar or due to the presence of stabilizing elastic material, as in the case of plate bending), mesh sensitivity is less of a concern. In practical calculations for reinforced concrete, the mesh is usually such that each element contains rebars. The interaction between the rebars and the concrete tends to reduce the mesh sensitivity, provided that a reasonable amount of tension stiffening is introduced in the concrete model to simulate this interaction. This requires an estimate of the tension stiffening effect, which depends on such factors as the density of reinforcement, the quality of the bond between the rebar and the concrete, the relative size of the concrete aggregate compared to the rebar diameter, and the mesh. A reasonable starting point for relatively heavily reinforced concrete modeled with a fairly detailed mesh is to assume that the strain softening after failure reduces the stress linearly to zero at a total strain of about 10 times the strain at failure. The strain at failure in standard concretes is typically 10−4 , which suggests that tension stiffening that reduces the stress to zero at a total strain of about 10−3 is reasonable. This parameter should be calibrated to a particular case. The choice of tension stiffening parameters is important since, generally, more tension stiffening makes it easier to obtain numerical solutions. Too little tension stiffening will cause the local cracking failure in the concrete to introduce temporarily unstable behavior in the overall response of the model. Few practical designs exhibit such behavior, so that the presence of this type of response in the analysis model usually indicates that the tension stiffening is unreasonably low. Input File Usage: Abaqus/CAE Usage: *CONCRETE TENSION STIFFENING, TYPE=STRAIN (default) Property module: material editor: Mechanical→Plasticity→Concrete Damaged Plasticity: Tensile Behavior: Type: Strain Fracture energy cracking criterion When there is no reinforcement in significant regions of the model, the tension stiffening approach described above will introduce unreasonable mesh sensitivity into the results. However, it is generally accepted that Hillerborg’s (1976) fracture energy proposal is adequate to allay the concern for many practical purposes. Hillerborg defines the energy required to open a unit area of crack, , as a material parameter, using brittle fracture concepts. With this approach the concrete’s brittle behavior is characterized by a stress-displacement response rather than a stress-strain response. Under tension a concrete specimen will crack across some section. After it has been pulled apart sufficiently for most of the stress to be removed (so that the undamaged elastic strain is small), its length will be determined primarily by the opening at the crack. The opening does not depend on the specimen’s length. This fracture energy cracking model can be invoked by specifying the postfailure stress as a tabular function of cracking displacement, as shown in Figure 23.6.3–4. u ck Figure 23.6.3–4 Postfailure stress-displacement curve. Alternatively, the fracture energy, , can be specified directly as a material property; in this case, , as a tabular function of the associated fracture energy. This model assumes define the failure stress, a linear loss of strength after cracking, as shown in Figure 23.6.3–5. to G f u = 2G /σ to to u t Figure 23.6.3–5 Postfailure stress-fracture energy curve. . The cracking displacement at which complete loss of strength takes place is, therefore, Typical values of range from 40 N/m (0.22 lb/in) for a typical construction concrete (with a compressive strength of approximately 20 MPa, 2850 lb/in2 ) to 120 N/m (0.67 lb/in) for a high-strength concrete (with a compressive strength of approximately 40 MPa, 5700 lb/in2 ). If tensile damage, , is specified, Abaqus automatically converts the cracking displacement values to “plastic” displacement values using the relationship where the specimen length, , is assumed to be one unit length, . Implementation The implementation of this stress-displacement concept in a finite element model requires the definition of a characteristic length associated with an integration point. The characteristic crack length is based on the element geometry and formulation: it is a typical length of a line across an element for a first-order element; it is half of the same typical length for a second-order element. For beams and trusses it is a characteristic length along the element axis. For membranes and shells it is a characteristic length in the reference surface. For axisymmetric elements it is a characteristic length in the r–z plane only. For cohesive elements it is equal to the constitutive thickness. This definition of the characteristic crack length is used because the direction in which cracking occurs is not known in advance. Therefore, elements with large aspect ratios will have rather different behavior depending on the direction in which they crack: some mesh sensitivity remains because of this effect, and elements that have aspect ratios close to one are recommended. Input File Usage: Use the following option to specify the postfailure stress as a tabular function of displacement: *CONCRETE TENSION STIFFENING, TYPE=DISPLACEMENT Use the following option to specify the postfailure stress as a tabular function of the fracture energy: Abaqus/CAE Usage: *CONCRETE TENSION STIFFENING, TYPE=GFI Property module: material editor: Mechanical→Plasticity→Concrete Damaged Plasticity: Tensile Behavior: Type: Displacement or GFI Defining compressive behavior You can define the stress-strain behavior of plain concrete in uniaxial compression outside the elastic range. Compressive stress data are provided as a tabular function of inelastic (or crushing) strain, , and, if desired, strain rate, temperature, and field variables. Positive (absolute) values should be given for the compressive stress and strain. The stress-strain curve can be defined beyond the ultimate stress, into the strain-softening regime. Hardening data are given in terms of an inelastic strain, . The compressive inelastic strain is defined as the total strain minus the elastic strain corresponding to the undamaged material, , as illustrated in Figure 23.6.3–6. Unloading data are provided to Abaqus in terms of compressive damage curves, , as discussed below. Abaqus automatically converts the inelastic strain values to plastic strain values using the relationship , instead of plastic strain, , where Abaqus will issue an error message if the calculated plastic strain values are negative and/or decreasing with increasing inelastic strain, which typically indicates that the compressive damage curves are incorrect. In the absence of compressive damage . Input File Usage: Abaqus/CAE Usage: *CONCRETE COMPRESSION HARDENING Property module: material editor: Mechanical→Plasticity→Concrete Damaged Plasticity: Compressive Behavior Defining damage and stiffness recovery Damage, as a plasticity model; consequently, , can be specified in tabular form. (If damage is not specified, the model behaves .) and/or and In Abaqus the damage variables are treated as non-decreasing material point quantities. At any increment during the analysis, the new value of each damage variable is obtained as the maximum between the value at the end of the previous increment and the value corresponding to the current state (interpolated from the user-specified tabular data); that is, σ c σ c u σ c 0 E0 E0 _ (1 d )Ec 0 in~ ε el ε 0c pl~ ε el ε c ε c Figure 23.6.3–6 Definition of the compressive inelastic (or crushing) strain used for the definition of compression hardening data. The choice of the damage properties is important since, generally, excessive damage may have a critical effect on the rate of convergence. It is recommended to avoid using values of the damage variables above 0.99, which corresponds to a 99% reduction of the stiffness. Tensile damage You can define the uniaxial tension damage variable, cracking displacement. , as a tabular function of either cracking strain or Input File Usage: Use the following option to specify tensile damage as a function of cracking strain: *CONCRETE TENSION DAMAGE, TYPE=STRAIN (default) Use the following option to specify tensile damage as a function of cracking displacement: *CONCRETE TENSION DAMAGE, TYPE=DISPLACEMENT Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Concrete Damaged Plasticity: Tensile Behavior: Suboptions→Tension Damage: Type: Strain or Displacement Compressive damage You can define the uniaxial compression damage variable, strain. , as a tabular function of inelastic (crushing) Input File Usage: Abaqus/CAE Usage: *CONCRETE COMPRESSION DAMAGE Property module: material editor: Mechanical→Plasticity→Concrete Damaged Plasticity: Compressive Behavior: Suboptions→Compression Damage Stiffness recovery The experimental observation in most quasi-brittle materials, As discussed above, stiffness recovery is an important aspect of the mechanical response of concrete under cyclic loading. Abaqus allows direct user specification of the stiffness recovery factors . and is that the including concrete, compressive stiffness is recovered upon crack closure as the load changes from tension to compression. On the other hand, the tensile stiffness is not recovered as the load changes from compression to tension once crushing micro-cracks have developed. This behavior, which corresponds to , is the default used by Abaqus. Figure 23.6.3–7 illustrates a uniaxial load cycle assuming the default behavior. and Input File Usage: Use the following option to specify the compression stiffness recovery factor, : *CONCRETE TENSION DAMAGE, COMPRESSION RECOVERY= Use the following option to specify the tension stiffness recovery factor, : *CONCRETE COMPRESSION DAMAGE, TENSION RECOVERY= Property module: material editor: Mechanical→Plasticity→Concrete Damaged Plasticity: Tensile Behavior: Suboptions→Tension Damage: Compression recovery: Compressive Behavior: Suboptions→Compression Damage: Tension recovery: Abaqus/CAE Usage: Rate dependence The rate-sensitive behavior of quasi-brittle materials is mainly connected to the retardation effects that high strain rates have on the growth of micro-cracks. The effect is usually more pronounced under tensile loading. As the strain rate increases, the stress-strain curves exhibit decreasing nonlinearity as well as an increase in the peak strength. You can specify tension stiffening as a tabular function of cracking strain σ t σ t 0 E w = 1 t w = 0 t (1-d )Et 0 (1-d )Ec 0 (1-d )t (1-d )Ec 0 w = 0c w = 1c ε E Figure 23.6.3–7 Uniaxial load cycle (tension-compression-tension) assuming default values for the stiffness recovery factors: and . (or displacement) rate, and you can specify compression hardening data as a tabular function of inelastic strain rate. Input File Usage: Use the following options: Abaqus/CAE Usage: *CONCRETE TENSION STIFFENING *CONCRETE COMPRESSION HARDENING Property module: material editor: Mechanical→Plasticity→Concrete Damaged Plasticity: Tensile Behavior: Use strain-rate-dependent data Compressive Behavior: Use strain-rate-dependent data Concrete plasticity You can define flow potential, yield surface, and in Abaqus/Standard viscosity parameters for the concrete damaged plasticity material model. Input File Usage: Abaqus/CAE Usage: *CONCRETE DAMAGED PLASTICITY Property module: material editor: Mechanical→Plasticity→Concrete Damaged Plasticity: Plasticity Effective stress invariants The effective stress is defined as The plastic flow potential function and the yield surface make use of two stress invariants of the effective stress tensor, namely the hydrostatic pressure stress, and the Mises equivalent effective stress, where is the effective stress deviator, defined as Plastic flow The concrete damaged plasticity model assumes nonassociated potential plastic flow. The flow potential G used for this model is the Drucker-Prager hyperbolic function: where is the dilation angle measured in the p–q plane at high confining pressure; is the uniaxial tensile stress at failure, taken from the user- specified tension stiffening data; and is a parameter, referred to as the eccentricity, that defines the rate at which the function approaches the asymptote (the flow potential tends to a straight line as the eccentricity tends to zero). This flow potential, which is continuous and smooth, ensures that the flow direction is always uniquely defined. The function approaches the linear Drucker-Prager flow potential asymptotically at high confining pressure stress and intersects the hydrostatic pressure axis at 90°. See “Models for granular or polymer behavior,” Section 4.4.2 of the Abaqus Theory Manual, for further discussion of this potential. , which implies that the material has almost the The default flow potential eccentricity is same dilation angle over a wide range of confining pressure stress values. Increasing the value of provides more curvature to the flow potential, implying that the dilation angle increases more rapidly as the confining pressure decreases. Values of that are significantly less than the default value may lead to convergence problems if the material is subjected to low confining pressures because of the very tight curvature of the flow potential locally where it intersects the p-axis. Yield function The model makes use of the yield function of Lubliner et. al. (1989), with the modifications proposed by Lee and Fenves (1998) to account for different evolution of strength under tension and compression. The evolution of the yield surface is controlled by the hardening variables, . In terms of effective stresses, the yield function takes the form and with Here, is the maximum principal effective stress; is the ratio of initial equibiaxial compressive yield stress to initial uniaxial compressive yield stress (the default value is ); , to that on the compressive meridian, is the ratio of the second stress invariant on the tensile meridian, , at initial yield for any given value of the pressure invariant p such that the maximum principal stress is negative, ; it must satisfy the condition (the default value is is the effective tensile cohesion stress; and is the effective compressive cohesion stress. ); _ S2 K = 2/3 _ S1 K = 1 (T.M.) (C.M.) _ S3 Figure 23.6.3–8 Yield surfaces in the deviatoric plane, corresponding to different values of . Typical yield surfaces are shown in Figure 23.6.3–8 on the deviatoric plane and in Figure 23.6.3–9 for plane stress conditions. Nonassociated flow Because plastic flow is nonassociated, the use of concrete damaged plasticity results in a nonsymmetric material stiffness matrix. Therefore, to obtain an acceptable rate of convergence in Abaqus/Standard, the unsymmetric matrix storage and solution scheme should be used. Abaqus/Standard will automatically activate the unsymmetric solution scheme if concrete damaged plasticity is used in the analysis. If desired, you can turn off the unsymmetric solution scheme for a particular step . Viscoplastic regularization Material models exhibiting softening behavior and stiffness degradation often lead to severe convergence difficulties in implicit analysis programs, such as Abaqus/Standard. A common technique to overcome some of these convergence difficulties is the use of a viscoplastic regularization of the constitutive equations, which causes the consistent tangent stiffness of the softening material to become positive for sufficiently small time increments. The concrete damaged plasticity model can be regularized in Abaqus/Standard using viscoplasticity by permitting stresses to be outside of the yield surface. We use a generalization of the Duvaut-Lions regularization, according to which the viscoplastic strain rate tensor, , is defined as 1-α CONCRETE DAMAGED PLASTICITY uniaxial tension ∧ (q - 3α p + βσ ) = σ c0 ∧ uniaxial compression σ t0 ∧ biaxial tension 1-α (q - 3α p + βσ ) = σ c0 ∧ (σ ,σ ) b0 b0 σ c0 biaxial compression 1-α (q - 3α p ) = σ c0 Figure 23.6.3–9 Yield surface in plane stress. is the viscosity parameter representing the relaxation time of the viscoplastic system, and is Here the plastic strain evaluated in the inviscid backbone model. Similarly, a viscous stiffness degradation variable, , for the viscoplastic system is defined as where d is the degradation variable evaluated in the inviscid backbone model. The stress-strain relation of the viscoplastic model is given as Using the viscoplastic regularization with a small value for the viscosity parameter (small compared to the characteristic time increment) usually helps improve the rate of convergence of the model in the softening regime, without compromising results. The basic idea is that the solution of the viscoplastic system relaxes to that of the inviscid case as , where t represents time. You can specify the value of the viscosity parameter as part of the concrete damaged plasticity material behavior If the viscosity parameter is different from zero, output results of the plastic strain and definition. stiffness degradation refer to the viscoplastic values, . In Abaqus/Standard the default value of the viscosity parameter is zero, so that no viscoplastic regularization is performed. and Material damping The concrete damaged plasticity model can be used in combination with material damping . If stiffness proportional damping is specified, Abaqus calculates the damping stress based on the undamaged elastic stiffness. This may introduce large artificial damping forces on elements undergoing severe damage at high strain rates. Visualization of “crack directions” Unlike concrete models based on the smeared crack approach, the concrete damaged plasticity model does not have the notion of cracks developing at the material integration point. However, it is possible to introduce the concept of an effective crack direction with the purpose of obtaining a graphical visualization of the cracking patterns in the concrete structure. Different criteria can be adopted within the framework of scalar-damage plasticity for the definition of the direction of cracking. Following (1989), we can assume that cracking initiates at points where the tensile equivalent Lubliner et. al. plastic strain is greater than zero, , and the maximum principal plastic strain is positive. The direction of the vector normal to the crack plane is assumed to be parallel to the direction of the maximum principal plastic strain. This direction can be viewed in the Visualization module of Abaqus/CAE. Abaqus/CAE Usage: Visualization module: Result→Field Output: PE, Max. Principal Plot→Symbols Elements Abaqus offers a variety of elements for use with the concrete damaged plasticity model: truss, shell, plane stress, plane strain, generalized plane strain, axisymmetric, and three-dimensional elements. Most beam elements can be used; however, beam elements in space that include shear stress caused by torsion and do not include hoop stress (such as B31, B31H, B32, B32H, B33, and B33H) cannot be used. Thin-walled, open-section beam elements and PIPE elements can be used with the concrete damaged plasticity model in Abaqus/Standard. For general shell analysis more than the default number of five integration points through the thickness of the shell should be used; nine thickness integration points are commonly used to model progressive failure of the concrete through the thickness with acceptable accuracy. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables relate specifically to material points in the concrete damaged plasticity model: DAMAGEC DAMAGET PEEQ PEEQT SDEG DMENER ELDMD ALLDMD Compressive damage variable, . Tensile damage variable, . Compressive equivalent plastic strain, . Tensile equivalent plastic strain, Stiffness degradation variable, d. Energy dissipated per unit volume by damage. . Total energy dissipated in the element by damage. Energy dissipated in the whole (or partial) model by damage. The contribution from ALLDMD is included in the total strain energy ALLIE. EDMDDEN Energy dissipated per unit volume in the element by damage. SENER ELSE ALLSE The recoverable part of the energy per unit volume. The recoverable part of the energy in the element. The recoverable part of the energy in the whole (partial) model. ESEDEN The recoverable part of the energy per unit volume in the element. Additional references • Hillerborg, A., M. Modeer, and P. E. Petersson, “Analysis of Crack Formation and Crack Growth in Concrete by Means of Fracture Mechanics and Finite Elements,” Cement and Concrete Research, vol. 6, pp. 773–782, 1976. • Lee, J., and G. L. Fenves, “Plastic-Damage Model for Cyclic Loading of Concrete Structures,” Journal of Engineering Mechanics, vol. 124, no. 8, pp. 892–900, 1998. • Lubliner, J., J. Oliver, S. Oller, and E. Oñate, “A Plastic-Damage Model for Concrete,” International Journal of Solids and Structures, vol. 25, pp. 299–329, 1989. 23.7 Permanent set in rubberlike materials • “Permanent set in rubberlike materials,” Section 23.7.1 23.7.1 PERMANENT SET IN RUBBERLIKE MATERIALS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Combining material behaviors,” Section 21.1.3 • “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 • “Classical metal plasticity,” Section 23.2.1 • *HYPERELASTIC • *MULLINS EFFECT • *PLASTIC Overview This feature: • is intended for modeling permanent set observed in filled elastomers and thermoplastics; • is based on multiplicative split of the deformation gradient; • is based on the theory of incompressible isotropic hardening plasticity; • can be used with any isotropic hyperelasticity model; • can be combined with Mullins effects; and • cannot be used to model viscoelastic or hysteresis effects or with the steady-state transport procedure. Material behavior The real behavior of filled rubber elastomers under cyclic loading conditions is quite complex as shown in Figure 23.7.1–1. The observed mechanical behaviors are progressive damage resulting in a reduction of load carrying capacity with each cycle, stress softening (also known as Mullins effect) upon reloading after the first unloading from a previously attained maximum strain level, hysteretic dissipation of energy, and permanent set. This section is concerned with modeling permanent set; therefore, the idealized representation of permanent set is described below. Idealized material behavior From Figure 23.7.1–1 it is clear that the observed permanent set is different for each cycle, but the material has a tendency to stabilize after a number of cycles of loading between zero stress and a given level of strain. For a given load level along the primary loading path shown with the dashed line in Figure 23.7.1–1, the idealized representation of permanent set will be a single strain value after unloading has taken place. Since rate and time effects are ignored in this model, idealized loading and unloading take place along the same path, whether Mullins effect is included or not. Nominal Strain Figure 23.7.1–1 Typical behavior of a filled elastomer. The permanent set behavior is captured by isotropic hardening Mises plasticity with an associated flow rule. In the context of finite elastic strains associated with the underlying rubberlike material, plasticity is modeled using a multiplicative split of the deformation gradient into elastic and plastic components: where is the plastic part of the deformation gradient (representing the stress-free intermediate configuration). is the elastic part of the deformation gradient (representing the hyperelastic behavior) and An example of modeling permanent set along with Mullins effect for a rubberlike material can be found in “Analysis of a solid disc with Mullins effect and permanent set,” Section 3.1.7 of the Abaqus Example Problems Manual. Specifying permanent set The primary hyperelastic behavior can be defined by using any of the hyperelastic material models . the hyperelastic response of the material, the data must be specified with respect to the stress-free intermediate configuration after unloading has taken place. Permanent set can be defined through an isotropic hardening function in terms of the yield stress and the equivalent plastic strain. In this case the yield stress is the (effective) Kirchoff stress on the primary loading path from which unloading takes place, and the equivalent plastic strain is the corresponding logarithmic permanent set observed in the material. If is the true (Cauchy) stress, Kirchoff stress is defined as is the determinant of , where . Depending on what is being modeled, permanent set may be defined as the true permanent set seen in the material after recovery of viscoelastic strains or it may include viscoelastic strains. In either case, an initial yield stress is required, below which there will be no permanent set and the behavior of the material will be fully elastic. In the case of filled rubbers this initial yield stress may correspond to a small nonzero stress; whereas for the family of thermoplastic materials, there may be a more marked value of initial yield stress. Input File Usage: Abaqus/CAE Usage: *PLASTIC, HARDENING=ISOTROPIC Property module: material editor: Mechanical→Plasticity→Plastic Processing test data If you have uniaxial and/or biaxial test data, as shown in Figure 23.7.1–1, you can use an interactive Abaqus/CAE plug-in to obtain the hyperelasticity, plasticity, and Mullins effect data. For information about the plug-in and instructions about its usage, see “Abaqus/CAE plug-in application for processing cyclic test data of filled elastomers and thermoplastics” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com. Limitations The model is intended to capture permanent set under multiaxial stress states and mild reverse loading conditions, as illustrated by Govindarajan, Hurtado, and Mars (2007). This model is not intended to capture deformation under complete reverse loading. Any rate effects apply only to the plastic part of the material definition. Elements Permanent set can be modeled with all element types that support the use of the hyperelastic material model. Procedures Permanent set modeling can be carried out in all procedures that support the use of the hyperelastic material model with the exception of the steady-state transport procedure. In linear perturbation steps in Abaqus/Standard, the current material tangent stiffness corresponding to the elastic part is used to determine the response, while ignoring any plasticity effects. Output The standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2) corresponding to other isotropic hardening plasticity models can be obtained for permanent set models. Additional references • Govindarajan, S. M., J. A. Hurtado, and W. V. Mars, “Simulation of Mullins Effect in Filled Elastomers Using Multiplicative Decomposition,” European Conference for Constitutive Models for Rubber, September 2007, Paris, France. • Simo, J. C., “Algorithms for Static and Dynamic Multiplicative Plasticity that Preserve the Classical Return Mapping Schemes of the Infinitesimal Theory,” Computer Methods in Applied Mechanics and Engineering, vol. 99, p. 61–112, 1992. • Weber, G., and L. Anand, “Finite Deformation Constitutive Equations and Time Integration Isotropic Hyperelastic-Viscoplastic Solids,” Computer Methods in Applied Procedure for Mechanics and Engineering, vol. 79, p. 173–202, 1990. 24. Progressive Damage and Failure Progressive damage and failure: overview Damage and failure for ductile metals Damage and failure for fiber-reinforced composites Damage and failure for ductile materials in low-cycle fatigue analysis 24.1 24.2 24.3 24.1 Progressive damage and failure: overview • “Progressive damage and failure,” Section 24.1.1 PROGRESSIVE DAMAGE AND FAILURE PROGRESSIVE DAMAGE AND FAILURE Abaqus provides the following models to predict progressive damage and failure: • Progressive damage and failure for ductile metals: Abaqus offers a general capability for modeling progressive damage and failure in ductile metals. The functionality can be used in conjunction with the Mises, Johnson-Cook, Hill, and Drucker-Prager plasticity models (“Damage and failure for ductile metals: overview,” Section 24.2.1). The capability supports the specification of one or more damage initiation criteria, including ductile, shear, forming limit diagram (FLD), forming limit stress diagram (FLSD), Müschenborn-Sonne forming limit diagram (MSFLD), and Marciniak-Kuczynski (M-K) criteria. After damage initiation, the material stiffness is degraded progressively according to the specified damage evolution response. The progressive damage models allow for a smooth degradation of the material stiffness, which makes them suitable for both quasi-static and dynamic situations, a great advantage over the dynamic failure models (“Dynamic failure models,” Section 23.2.8). The Johnson-Cook and Marciniak-Kuczynski (M-K) damage initiation criteria are not available in Abaqus/Standard. • Progressive damage and failure for fiber-reinforced materials: Abaqus offers a capability to model anisotropic damage in fiber-reinforced materials (“Damage and failure for fiber-reinforced composites: overview,” Section 24.3.1). The response of the undamaged material is assumed to be linearly elastic, and the model is intended to predict behavior of fiber-reinforced materials for which damage can be initiated without a large amount of plastic deformation. The Hashin’s initiation criteria are used to predict the onset of damage, and the damage evolution law is based on the energy dissipated during the damage process and linear material softening. • Progressive for and failure damage ductile materials fatigue analysis: Abaqus/Standard offers a capability to model progressive damage and failure for ductile materials due to stress reversals and the accumulation of inelastic strain in a low-cycle fatigue analysis using the direct cyclic approach . The damage initiation criterion and damage evolution are characterized by the accumulated inelastic hysteresis energy per stabilized cycle . After damage initiation, the elastic material stiffness is degraded progressively according to the specified damage evolution response. low-cycle in In addition, Abaqus offers a concrete damaged model (“Concrete damaged plasticity,” Section 23.6.3), dynamic failure models (“Dynamic failure models,” Section 23.2.8), and specialized capabilities for modeling damage and failure in cohesive elements (“Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6) and in connectors (“Connector damage behavior,” Section 31.2.7). This section provides an overview of the progressive damage and failure capability and a brief description of the concepts of damage initiation and evolution. The discussion in this section is limited to damage models for ductile metals and fiber-reinforced materials. General framework for modeling damage and failure Abaqus offers a general framework for material failure modeling that allows the combination of multiple failure mechanisms acting simultaneously on the same material. Material failure refers to the complete loss of load-carrying capacity that results from progressive degradation of the material stiffness. The stiffness degradation process is modeled using damage mechanics. To help understand the failure modeling capabilities in Abaqus, consider the response of a typical metal specimen during a simple tensile test. The stress-strain response, such as that illustrated in Figure 24.1.1–1, will show distinct phases. The material response is initially linear elastic, , followed by plastic yielding with strain hardening, . Beyond point c there is a marked reduction of load-carrying capacity until rupture, . The deformation during this last phase is localized in a neck region of the specimen. Point c identifies the material state at the onset of damage, which is referred to as the damage initiation criterion. Beyond this point, the stress-strain response is governed by the evolution of the degradation of the stiffness in the region of strain localization. In the context of damage mechanics that the material can be viewed as the degraded response of the curve would have followed in the absence of damage. d’ d Figure 24.1.1–1 Typical uniaxial stress-strain response of a metal specimen. Thus, in Abaqus the specification of a failure mechanism consists of four distinct parts: • the definition of the effective (or undamaged) material response (e.g., Figure 24.1.1–1), in • a damage initiation criterion (e.g., c in Figure 24.1.1–1), • a damage evolution law (e.g., in Figure 24.1.1–1), and • a choice of element deletion whereby elements can be removed from the calculations once the material stiffness is fully degraded (e.g., d in Figure 24.1.1–1). These parts will be discussed separately for ductile metals (“Damage and failure for ductile metals: overview,” Section 24.2.1) and fiber-reinforced materials (“Damage and failure for fiber-reinforced composites: overview,” Section 24.3.1). Mesh dependency In continuum mechanics the constitutive model is normally expressed in terms of stress-strain relations. When the material exhibits strain-softening behavior, leading to strain localization, this formulation results in a strong mesh dependency of the finite element results in that the energy dissipated decreases upon mesh refinement. In Abaqus all of the available damage evolution models use a formulation intended to alleviate the mesh dependency. This is accomplished by introducing a characteristic length into the formulation, which in Abaqus is related to the element size, and expressing the softening part of the constitutive law as a stress-displacement relation. In this case the energy dissipated during the damage process is specified per unit area, not per unit volume. This energy is treated as an additional material parameter, and it is used to compute the displacement at which full material damage occurs. This is consistent with the concept of critical energy release rate as a material parameter for fracture mechanics. This formulation ensures that the correct amount of energy is dissipated and greatly alleviates the mesh dependency. 24.2 Damage and failure for ductile metals • “Damage and failure for ductile metals: overview,” Section 24.2.1 • “Damage initiation for ductile metals,” Section 24.2.2 • “Damage evolution and element removal for ductile metals,” Section 24.2.3 24.2.1 DAMAGE AND FAILURE FOR DUCTILE METALS: OVERVIEW Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Progressive damage and failure,” Section 24.1.1 • “Damage initiation for ductile metals,” Section 24.2.2 • “Damage evolution and element removal for ductile metals,” Section 24.2.3 • *DAMAGE INITIATION • *DAMAGE EVOLUTION • “Defining damage,” Section 12.9.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Abaqus/Standard and Abaqus/Explicit offer a general capability for predicting the onset of failure and a capability for modeling progressive damage and failure of ductile metals. In the most general case this requires the specification of the following: • the undamaged elastic-plastic response of the material (“Classical metal plasticity,” Section 23.2.1); • a damage initiation criterion (“Damage initiation for ductile metals,” Section 24.2.2); and • a damage evolution response, including a choice of element removal (“Damage evolution and element removal for ductile metals,” Section 24.2.3). A summary of the general framework for progressive damage and failure in Abaqus is given in “Progressive damage and failure,” Section 24.1.1. This section provides an overview of the damage initiation criteria and damage evolution law for ductile metals. In addition, Abaqus/Explicit offers dynamic failure models that are suitable for high-strain-rate dynamic problems (“Dynamic failure models,” Section 23.2.8). Damage initiation criterion Abaqus offers a variety of choices of damage initiation criteria for ductile metals, each associated with distinct types of material failure. They can be classified in the following categories: • Damage initiation criteria for the fracture of metals, including ductile and shear criteria. • Damage initiation criteria for the necking instability of sheet metal. These include forming limit diagrams (FLD, FLSD, and MSFLD) intended to assess the formability of sheet metal and the Marciniak-Kuczynski (M-K) criterion (available only in Abaqus/Explicit) to numerically predict necking instability in sheet metal taking into account the deformation history. These criteria are discussed in “Damage initiation for ductile metals,” Section 24.2.2. Each damage initiation criterion has an associated output variable to indicate whether the criterion has been met during the analysis. A value of 1.0 or higher indicates that the initiation criterion has been met. More than one damage initiation criterion can be specified for a given material. If multiple damage initiation criteria are specified for the same material, they are treated independently. Once a particular initiation criterion is satisfied, the material stiffness is degraded according to the specified damage evolution law for that criterion; in the absence of a damage evolution law, however, the material stiffness is not degraded. A failure mechanism for which no damage evolution response is specified is said to be inactive. Abaqus will evaluate the initiation criterion for an inactive mechanism for output purposes only, but the mechanism will have no effect on the material response. Input File Usage: Use the following option to define each damage initiation criterion (repeat as needed to define multiple criteria): Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=criterion 1 Property module: material editor: Mechanical→Damage for Ductile Metals→criterion Damage evolution The damage evolution law describes the rate of degradation of the material stiffness once the corresponding initiation criterion has been reached. For damage in ductile metals Abaqus assumes that the degradation of the stiffness associated with each active failure mechanism can be modeled using a scalar damage variable, represents the set of active mechanisms. At any given time during the analysis the stress tensor in the material is given by the scalar damage equation ), where ( where D is the overall damage variable and the current increment. material has lost its load-carrying capacity when mesh if all of the section points at any one integration location have lost their load-carrying capacity. is the effective (or undamaged) stress tensor computed in are the stresses that would exist in the material in the absence of damage. The . By default, an element is removed from the The overall damage variable, D, captures the combined effect of all active mechanisms and is computed in terms of the individual damage variables, , according to a user-specified rule. Abaqus supports different models of damage evolution in ductile metals and provides controls associated with element deletion due to material failure, as described in “Damage evolution and element removal for ductile metals,” Section 24.2.3. All of the available models use a formulation intended to alleviate the strong mesh dependency of the results that can arise from strain localization effects during progressive damage. Input File Usage: Use the following option immediately after the corresponding *DAMAGE INITIATION option to specify the damage evolution behavior: *DAMAGE EVOLUTION Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution Elements The failure modeling capability for ductile metals can be used with any elements in Abaqus that include mechanical behavior (elements that have displacement degrees of freedom). For coupled temperature-displacement elements the thermal properties of the material are not affected by the progressive damage of the material stiffness until the condition for element deletion is reached; at this point the thermal contribution of the element is also removed. The damage initiation criteria for sheet metal necking instability (FLD, FLSD, MSFLD, and M-K) are available only for elements that include mechanical behavior and use a plane stress formulation (i.e., plane stress, shell, continuum shell, and membrane elements). 24.2.2 DAMAGE INITIATION FOR DUCTILE METALS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Progressive damage and failure,” Section 24.1.1 • *DAMAGE INITIATION • “Defining damage,” Section 12.9.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The material damage initiation capability for ductile metals: • is intended as a general capability for predicting initiation of damage in metals, including sheet, extrusion, and cast metals as well as other materials; • can be used in combination with the damage evolution models for ductile metals described in “Damage evolution and element removal for ductile metals,” Section 24.2.3; • allows the specification of more than one damage initiation criterion; • includes ductile, shear, forming limit diagram (FLD), forming limit stress diagram (FLSD) and Müschenborn-Sonne forming limit diagram (MSFLD) criteria for damage initiation; • includes in Abaqus/Explicit the Marciniak-Kuczynski (M-K) and Johnson-Cook criteria for damage initiation; • can be used in Abaqus/Standard in conjunction with Mises, Johnson-Cook, Hill, and Drucker-Prager plasticity (ductile, shear, FLD, FLSD, and MSFLD criteria); and • can be used in Abaqus/Explicit in conjunction with Mises and Johnson-Cook plasticity (ductile, shear, FLD, FLSD, MSFLD, Johnson-Cook, and MK criteria) and in conjunction with Hill and Drucker-Prager plasticity (ductile, shear, FLD, FLSD, MSFLD, and Johnson-Cook criteria). Damage initiation criteria for fracture of metals Two main mechanisms can cause the fracture of a ductile metal: ductile fracture due to the nucleation, growth, and coalescence of voids; and shear fracture due to shear band localization. Based on phenomenological observations, these two mechanisms call for different forms of the criteria for the onset of damage (Hooputra et al., 2004). The functional forms provided by Abaqus for these criteria are discussed below. These criteria can be used in combination with the damage evolution models for ductile metals discussed in “Damage evolution and element removal for ductile metals,” Section 24.2.3, to model fracture of a ductile metal. Ductile criterion The ductile criterion is a phenomenological model for predicting the onset of damage due to nucleation, growth, and coalescence of voids. The model assumes that the equivalent plastic strain at the onset of damage, , is a function of stress triaxiality and strain rate: where is the stress triaxiality, p is the pressure stress, q is the Mises equivalent stress, and is the equivalent plastic strain rate. The criterion for damage initiation is met when the following condition is satisfied: where during the analysis the incremental increase in is computed as is a state variable that increases monotonically with plastic deformation. At each increment In Abaqus/Standard the ductile criterion can be used in conjunction with the Mises, Johnson-Cook, Hill, and Drucker-Prager plasticity models and in Abaqus/Explicit in conjunction with the Mises, Johnson-Cook, Hill, and Drucker-Prager plasticity models, including equation of state. Input File Usage: Abaqus/CAE Usage: Use the following option to specify the equivalent plastic strain at the onset of damage as a tabular function of stress triaxality, strain rate, and, optionally, temperature and predefined field variables: *DAMAGE INITIATION, CRITERION=DUCTILE, DEPENDENCIES=n Property module: material editor: Mechanical→Damage for Ductile Metals→Ductile Damage Defining dependency of ductile criterion on Lode angle in Abaqus/Explicit Recent experimental results for aluminum alloys and other metals (Bai and Wierzbicki, 2008) reveal that, in addition to stress triaxility and strain rate, ductile fracture can also depend on the third invariant of deviatoric stress, which is related to the Lode angle (or deviatoric polar angle). Abaqus/Explicit allows the definition of the equivalent plastic strain at the onset of ductile damage, , as a function of the Lode angle, , by way of the functional form where q is the Mises equivalent stress, and r is the third invariant of deviatoric stress, can take values from function stress states on the tensile meridian. , for stress states on the compressive meridian, to . The , for Input File Usage: Use the following option to indicate that the equivalent plastic strain at the onset of ductile damage is a function of the Lode angle: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=DUCTILE, LODE DEPENDENT Defining dependency of ductile criterion on Lode angle is not supported in Abaqus/CAE. Johnson-Cook criterion The Johnson-Cook criterion (available only in Abaqus/Explicit) is a special case of the ductile criterion in which the equivalent plastic strain at the onset of damage, , is assumed to be of the form – are failure parameters and where the original formula published by Johnson and Cook (1985) in the sign of the parameter difference is motivated by the fact that most materials experience a decrease in stress triaxiality; therefore, nondimensional temperature defined as is the reference strain rate. This expression differs from . This with increasing is the in the above expression will usually take positive values. is the current temperature, is the melting temperature, and where is the transition temperature defined as the one at or below which there is no temperature dependence on the expression of the damage strain . The material parameters must be measured at or below the transition temperature. The Johnson-Cook criterion can be used in conjunction with the Mises, Johnson-Cook, Hill, and Drucker-Prager plasticity models, including equation of state. When used in conjunction with the Johnson-Cook plasticity model, the specified values of the melting and transition temperatures should be consistent with the values specified in the plasticity definition. The Johnson-Cook damage initiation criterion can also be specified together with any other initiation criteria, including the ductile criteria; each initiation criterion is treated independently. Input File Usage: Use the following option to specify the parameters for the Johnson-Cook initiation criterion: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=JOHNSON COOK Property module: material editor: Mechanical→Damage for Ductile Metals→Johnson-Cook Damage Shear criterion The shear criterion is a phenomenological model for predicting the onset of damage due to shear band localization. The model assumes that the equivalent plastic strain at the onset of damage, , is a function of the shear stress ratio and strain rate: Here material parameter. A typical value of for damage initiation is met when the following condition is satisfied: is the shear stress ratio, for aluminum is is the maximum shear stress, and is a = 0.3 (Hooputra et al., 2004). The criterion where is a state variable that increases monotonically with plastic deformation proportional to the incremental change in equivalent plastic strain. At each increment during the analysis the incremental increase in is computed as In Abaqus/Explicit the shear criterion can be used in conjunction with the Mises, Johnson-Cook, Hill, and Drucker-Prager plasticity models, including equation of state. In Abaqus/Standard it can be used with the Mises, Johnson-Cook, Hill, and Drucker-Prager models. Input File Usage: and to specify the equivalent plastic Use the following option to specify strain at the onset of damage as a tabular function of the shear stress ratio, strain rate, and, optionally, temperature and predefined field variables: *DAMAGE INITIATION, CRITERION=SHEAR, KS= , DEPENDENCIES=n Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→Shear Damage Initial conditions Optionally, you can specify the initial work hardened state of the material by providing the initial equivalent plastic strain values and, if residual stresses are also present, the initial stress values . Abaqus uses this information to initialize the values of the ductile and shear damage initiation criteria, , assuming constant values of stress triaxiality and shear shear ratio (linear stress path). and Input File Usage: Abaqus/CAE Usage: Use the following options to specify that material hardening and residual stresses have occurred prior to the current analysis: *INITIAL CONDITIONS, TYPE=HARDENING *INITIAL CONDITIONS, TYPE=STRESS Use the following options to specify that material hardening and residual stresses have occurred prior to the current analysis: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening and Stress for the Types for Selected Step Damage initiation criteria for sheet metal instability Necking instability plays a determining factor in sheet metal forming processes: the size of the local neck region is typically of the order of the thickness of the sheet, and local necks can rapidly lead to fracture. Localized necking cannot be modeled with traditional shell elements used in sheet metal forming simulations because the size of the neck is of the order of the thickness of the element. Abaqus supports four criteria for predicting the onset of necking instability in sheet metals: forming limit diagram (FLD); forming limit stress diagram (FLSD); Müschenborn-Sonne forming limit diagram (MSFLD); and Marciniak-Kuczynski (M-K) criteria, which is available only in Abaqus/Explicit. These criteria apply only to elements with a plane stress formulation (plane stress, shell, continuum shell, and membrane elements); Abaqus ignores these criteria for other elements. The initiation criteria for necking instability can be used in combination with the damage evolution models discussed in “Damage evolution and element removal for ductile metals,” Section 24.2.3, to account for the damage induced by necking. Classical strain-based forming limit diagrams (FLDs) are known to be dependent on the strain path. Changes in the deformation mode (e.g., equibiaxial loading followed by uniaxial tensile strain) may result in major modifications in the level of the limit strains. Therefore, the FLD damage initiation criterion should be used with care if the strain paths in the analysis are nonlinear. In practical industrial applications, significant changes in the strain path may be induced by multistep forming operations, complex geometry of the tooling, and interface friction, among other factors. For problems with highly nonlinear strain paths Abaqus offers three additional damage initiation criteria: the forming limit stress diagram (FLSD) criterion, the Müschenborn-Sonne forming limit diagram (MSFLD) criterion, and in Abaqus/Explicit the Marciniak-Kuczynski (M-K) criterion; these alternatives to the FLD damage initiation criterion are intended to minimize load path dependence. The characteristics of each criterion available in Abaqus for predicting damage initiation in sheet metals are discussed below. Forming limit diagram (FLD) criterion The forming limit diagram (FLD) is a useful concept introduced by Keeler and Backofen (1964) to determine the amount of deformation that a material can withstand prior to the onset of necking instability. The maximum strains that a sheet material can sustain prior to the onset of necking are referred to as the forming limit strains. A FLD is a plot of the forming limit strains in the space of principal (in-plane) logarithmic strains. In the discussion that follows major and minor limit strains refer to the maximum and minimum values of the in-plane principal limit strains, respectively. The major limit strain is usually represented on the vertical axis and the minor strain on the horizontal axis, as illustrated in Figure 24.2.2–1. The line connecting the states at which deformation becomes unstable is referred to as the forming limit curve (FLC). The FLC gives a sense of the formability of a sheet of material. Strains computed numerically by Abaqus can be compared to a FLC to determine the feasibility of the forming process under analysis. major FLC ω = FLD ε A ε B major major Figure 24.2.2–1 Forming limit diagram (FLD). minor The FLD damage initiation criterion requires the specification of the FLC in tabular form by giving the major principal strain at damage initiation as a tabular function of the minor principal strain and, optionally, temperature and predefined field variables, . The damage initiation criterion for the FLD is given by the condition is a function of the current deformation state and is defined as the ratio of the current major principal strain, , to the major limit strain on the FLC evaluated at the current values of the minor principal strain, ; temperature, ; and predefined field variables, , where the variable : For example, for the deformation state given by point A in Figure 24.2.2–1 the damage initiation criterion is evaluated as If the value of the minor strain lies outside the range of the specified tabular values, Abaqus will extrapolate the value of the major limit strain on the FLC by assuming that the slope at the endpoint of the curve remains constant. Extrapolation with respect to temperature and field variables follows the standard conventions: the property is assumed to be constant outside the specified range of temperature and field variables . Experimentally, FLDs are measured under conditions of biaxial stretching of a sheet, without bending effects. Under bending loading, however, most materials can achieve limit strains that are much greater than those on the FLC. To avoid the prediction of early failure under bending deformation, Abaqus evaluates the FLD criterion using the strains at the midplane through the thickness of the element. For composite shells with several layers the criterion is evaluated at the midplane of each layer for which a FLD curve has been specified, which ensures that only biaxial stretching effects are taken into account. Therefore, the FLD criterion is not suitable for modeling failure under bending loading; other failure models (such as ductile and shear failure) are more appropriate for such loading. Once the FLD damage initiation criterion is met, the evolution of damage is driven independently at each material point through the thickness of the element based on the local deformation at that point. Thus, although bending effects do not affect the evaluation of the FLD criterion, they may affect the rate of evolution of damage. Input File Usage: Use the following option to specify the limit major strain as a tabular function of minor strain: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=FLD Property module: material editor: Mechanical→Damage for Ductile Metals→FLD Damage Forming limit stress diagram (FLSD) criterion When strain-based FLCs are converted into stress-based FLCs, the resulting stress-based curves have been shown to be minimally affected by changes to the strain path (Stoughton, 2000); that is, different strain-based FLCs, corresponding to different strain paths, are mapped onto a single stress-based FLC. This property makes forming limit stress diagrams (FLSDs) an attractive alternative to FLDs for the prediction of necking instability under arbitrary loading. However, the apparent independence of the stress-based limit curves on the strain path may simply reflect the small sensitivity of the yield stress to changes in plastic deformation. This topic is still under discussion in the research community. A FLSD is the stress counterpart of the FLD, with the major and minor principal in-plane stresses corresponding to the onset of necking localization plotted on the vertical and horizontal axes, respectively. In Abaqus the FLSD damage initiation criterion requires the specification of the major principal in-plane stress at damage initiation as a tabular function of the minor principal in-plane stress and, optionally, temperature and predefined field variables, . The damage initiation criterion for the FLSD is met when the condition is a function of the current stress state and is defined as the ratio of the current major principal stress, , to the major stress on the FLSD evaluated at the current values of minor stress, ; and predefined field variables, is satisfied, where the variable ; temperature, : If the value of the minor stress lies outside the range of specified tabular values, Abaqus will extrapolate the value of the major limit stress assuming that the slope at the endpoints of the curve remains constant. Extrapolation with respect to temperature and field variables follows the standard conventions: the property is assumed to be constant outside the specified range of temperature and field variables . For reasons similar to those discussed earlier for the FLD criterion, Abaqus evaluates the FLSD criterion using the stresses averaged through the thickness of the element (or the layer, in the case of composite shells with several layers), ignoring bending effects. Therefore, the FLSD criterion cannot be used to model failure under bending loading; other failure models (such as ductile and shear failure) are more suitable for such loading. Once the FLSD damage initiation criterion is met, the evolution of damage is driven independently at each material point through the thickness of the element based on the local deformation at that point. Thus, although bending effects do not affect the evaluation of the FLSD criterion, they may affect the rate of evolution of damage. Input File Usage: Abaqus/CAE Usage: Use the following option to specify the limit major stress as a tabular function of minor stress: *DAMAGE INITIATION, CRITERION=FLSD Property module: material editor: Mechanical→Damage for Ductile Metals→FLSD Damage Marciniak-Kuczynski (M-K) criterion Another approach available in Abaqus/Explicit for accurately predicting the forming limits for arbitrary loading paths is based on the localization analysis proposed by Marciniak and Kuczynski (1967). The approach can be used with the Mises and Johnson-Cook plasticity models, including kinematic hardening. In M-K analysis, virtual thickness imperfections are introduced as grooves simulating preexisting defects in an otherwise uniform sheet material. The deformation field is computed inside each groove as a result of the applied loading outside the groove. Necking is considered to occur when the ratio of the deformation in the groove relative to the nominal deformation (outside the groove) is greater than a critical value. Figure 24.2.2–2 shows schematically the geometry of the groove considered for M-K analysis. In the figure a denotes the nominal region in the shell element outside the imperfection, and b denotes the weak groove region. The initial thickness of the imperfection relative to the nominal thickness is given by the ratio , with the subscript 0 denoting quantities in the initial, strain-free state. The groove is oriented at a zero angle with respect to the 1-direction of the local material orientation. Abaqus/Explicit allows the specification of an anisotropic distribution of thickness imperfections as a function of angle with respect to the local material orientation, . Abaqus/Explicit first solves for the stress-strain field in the nominal area ignoring the presence of imperfections; then it considers the effect of each groove alone. The deformation field inside each groove is computed by enforcing the strain compatibility condition and the force equilibrium equations The subscripts n and t refer to the directions normal and tangential to the groove. In the above equilibrium equations are forces per unit width in the t-direction. and The onset of necking instability is assumed to occur when the ratio of the rate of deformation inside a groove relative to the rate of deformation if no groove were present is greater than a critical value. In t =f t 00 t a Figure 24.2.2–2 Imperfection model for the M-K analysis. addition, it may not be possible to find a solution that satisfies equilibrium and compatibility conditions once localization initiates at a particular groove; consequently, failure to find a converged solution is also an indicator of the onset of localized necking. For the evaluation of the damage initiation criterion Abaqus/Explicit uses the following measures of deformation severity: These deformation severity factors are evaluated on each of the specified groove directions and compared with the critical values. (The evaluation is performed only if the incremental deformation is primarily plastic; the M-K criterion will not predict damage initiation if the deformation increment is elastic.) The most unfavorable groove direction is used for the evaluation of the damage initiation criterion, which is given as , and are the critical values of the deformation severity indices. Damage initiation where , occurs when or when a converged solution to the equilibrium and compatibility equations cannot be found. By default, Abaqus/Explicit assumes ; you can specify different values. If one of these parameters is set equal to zero, its corresponding deformation severity factor is not included in the evaluation of the damage initiation criterion. If all of these parameters are set equal to zero, the M-K criterion is based solely on nonconvergence of the equilibrium and compatibility equations. You must specify the fraction, , equal to the initial thickness at the virtual imperfection divided by the nominal thickness , as well as the number of imperfections to be used for the evaluation of the M-K damage initiation criterion. It is assumed that these directions are equally spaced angularly. By default, Abaqus/Explicit uses four imperfections located at 0°, 45°, 90°, and 135° with respect to the local 1-direction of the material. The initial imperfection size can be defined as a tabular function of angular direction, ; this allows the modeling of an anisotropic distribution of flaws in the material. Abaqus/Explicit will use this table to evaluate the thickness of each of the imperfections that will be used for the evaluation of the M-K analysis method. In addition, the initial imperfection size can also be a function of initial temperature and field variables; this allows defining a nonuniform spatial distribution of imperfections. Abaqus/Explicit will compute the initial imperfection size based on the values of temperature and field variables at the beginning of the analysis. The initial size of the imperfection remains a constant property during the rest of the analysis. A general recommendation is to choose the value of such that the forming limit predicted numerically for uniaxial strain loading conditions ( ) matches the experimental result. The virtual grooves are introduced to evaluate the onset of necking instability; they do not influence the results in the underlying element. Once the criterion for necking instability is met, the material properties in the element are degraded according to the specified damage evolution law. Input File Usage: Use the following option to specify the initial imperfection thickness relative to the nominal thickness as a tabular function of the angle with respect to the 1-direction of the local material orientation and, optionally, initial temperature and field variables: *DAMAGE INITIATION, CRITERION=MK, DEPENDENCIES=n Use the following option to specify critical deformation severity factors: *DAMAGE INITIATION, CRITERION=MK, FEQ= FNT= , FNN= , Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→M-K Damage Performance considerations for the M-K criterion There can be a substantial increase in the overall computational cost when the M-K criterion is used. For example, the cost of processing a shell element with three section points through the thickness and four imperfections, which is the default for the M-K criterion, increases by approximately a factor of two compared to the cost without the M-K criterion. You can mitigate the cost of evaluating this damage initiation criterion by reducing the number of flaw directions considered or by increasing the number of increments between M-K computations, as explained below. Of course, the effect on the overall analysis cost depends on the fraction of the elements in the model that use this damage initiation criterion. The computational cost per element with the M-K criterion increases by approximately a factor of is the number of imperfections specified for the evaluation of the M-K criterion and where is the frequency, in number of increments, at which the M-K computations are performed. The coefficient of in the above formula gives a reasonable estimate of the cost increase in most cases, but the actual cost increase may vary from this estimate. By default, Abaqus/Explicit performs the M-K computations on each imperfection at each time increment, . Care must be taken to ensure that the M-K computations are performed frequently enough to ensure the accurate integration of the deformation field on each imperfection. Input File Usage: Use the following option to specify the number of imperfections and frequency of the M-K analysis: *DAMAGE INITIATION, CRITERION=MK, NUMBER IMPERFECTIONS= , FREQUENCY= Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→M-K Damage: Number of imperfections and Frequency Müschenborn-Sonne forming limit diagram (MSFLD) criterion Müschenborn and Sonne (1975) proposed a method to predict the influence of the deformation path on the forming limits of sheet metals on the basis of the equivalent plastic strain, by assuming that the forming limit curve represents the sum of the highest attainable equivalent plastic strains. Abaqus makes use of a generalization of this idea to establish a criterion of necking instability of sheet metals for arbitrary deformation paths. The approach requires transforming the original forming limit curve (without predeformation effects) from the space of major versus minor strains to the space of equivalent plastic strain, , versus ratio of principal strain rates, . For linear strain paths, assuming plastic incompressibility and neglecting elastic strains: As illustrated in Figure 24.2.2–3 , linear deformation paths in the FLD transform onto vertical paths in the – diagram (constant value of ). According to the MSFLD criterion, the onset of localized necking occurs when the sequence of deformation states in the diagram intersects the forming limit curve, as discussed below. It is emphasized that for linear deformation paths both FLD and MSFLD representations are identical and give rise to the same predictions. For arbitrary loading, however, the MSFLD representation takes into account the effects of the history of deformation through the use of the accumulated equivalent plastic strain. – For the specification of the MSFLD damage initiation criterion in Abaqus, you can directly provide and, optionally, equivalent . Alternatively, you the equivalent plastic strain at damage initiation as a tabular function of plastic strain rate, temperature, and predefined field variables, (a) FLD major (b) MSFLD plε minor Figure 24.2.2–3 Transformation of the forming limit curve from traditional FLD representation (a) to MSFLD representation (b). Linear deformation paths transform onto vertical paths. can specify the curve in the traditional FLD format (in the space of major and minor strains) by providing a tabular function of the form . In this case Abaqus will automatically transform the data into the Let – format. represent the ratio of the current equivalent plastic strain, ; strain rate, plastic strain on the limit curve evaluated at the current values of predefined field variables, : , to the equivalent ; and ; temperature, The MSFLD criterion for necking instability is met when the condition instability also occurs if the sequence of deformation states in the due to a sudden change in the straining direction. This situation is illustrated in Figure 24.2.2–4. As changes from to – diagram intersects , the line connecting the corresponding points in the with the forming limit curve. When this situation occurs, the MSFLD criterion is reached despite the fact that equal to one to indicate that the criterion has been met. is satisfied. Necking – diagram intersects the limit curve . For output purposes Abaqus sets the value of The equivalent plastic strain used for the evaluation of the MSFLD criterion in Abaqus is accumulated only over increments that result in an increase of the element area. Strain increments associated with a reduction of the element area cannot cause necking and do not contribute toward the evaluation of the MSFLD criterion. If the value of lies outside the range of specified tabular values, Abaqus extrapolates the value of equivalent plastic strain for initiation of necking assuming that the slope at the endpoints of the curve remains constant. Extrapolation with respect to strain rate, temperature, and field variables follows the plε Onset of necking MSFLD t +Δ t Figure 24.2.2–4 Illustration of how a sudden change in the straining direction, from to can produce a horizontal intersection with the limit curve and lead to onset of necking. , standard conventions: the property is assumed to be constant outside the specified range of strain rate, temperature, and field variables . As discussed in “Progressive damage and failure of ductile metals,” Section 2.2.21 of the Abaqus Verification Manual, predictions of necking instability based on the MSFLD criterion agree remarkably well with predictions based on the Marciniak and Kuczynski criterion, at significantly less computational cost than the Marciniak and Kuczynski criterion. There are some situations, however, in which the MSFLD criterion may overpredict the amount of formability left in the material. This occurs in situations when, sometime during the loading history, the material reaches a state that is very close to the point of necking instability and is subsequently strained in a direction along which it can sustain further deformation. In this case the MSFLD criterion may predict that the amount of additional formability in the new direction is greater than that predicted with the Marciniak and Kuczynski criterion. However, this situation is often not a concern in practical forming applications where safety factors in the forming limit diagrams are commonly used to ensure that the material state is sufficiently far away from the point of necking. Refer to “Progressive damage and failure of ductile metals,” Section 2.2.21 of the Abaqus Verification Manual, for a comparative analysis of these two criteria. For reasons similar to those discussed earlier for the FLD criterion, Abaqus evaluates the MSFLD criterion using the strains at the midplane through the thickness of the element (or the layer, in the case of composite shells with several layers), ignoring bending effects. Therefore, the MSFLD criterion cannot be used to model failure under bending loading; other failure models (such as ductile and shear failure) are more suitable for such loading. Once the MSFLD damage initiation criterion is met, the evolution of damage is driven independently at each material point through the thickness of the element based on the local deformation at that point. Thus, although bending effects do not affect the evaluation of the MSFLD criterion, they may affect the rate of evolution of damage. Input File Usage: Abaqus/CAE Usage: Use the following option to specify the MSFLD damage initiation criterion by providing the limit equivalent plastic strain as a tabular function of (default): *DAMAGE INITIATION, CRITERION=MSFLD, DEFINITION=MSFLD Use the following option to specify the MSFLD damage initiation criterion by providing the limit major strain as a tabular function of minor strain: *DAMAGE INITIATION, CRITERION=MSFLD, DEFINITION=FLD Property module: material editor: Mechanical→Damage for Ductile Metals→MSFLD Damage Numerical evaluation of the principal strain rates ratio The ratio of principal strain rates, , can jump in value due to sudden changes in the deformation path. Special care is required during explicit dynamic simulations to avoid nonphysical jumps in triggered by numerical noise, which may cause a horizontal intersection of the deformation state with the forming limit curve and lead to the premature prediction of necking instability. To overcome this problem, rather than computing as a ratio of instantaneous strain rates, Abaqus/Explicit periodically updates based on accumulated strain increments after small but significant changes in the equivalent plastic strain. The threshold value for the change in equivalent plastic strain triggering an update of is approximated as is denoted as , and where update of and are principal values of the accumulated plastic strain since the previous . The default value of is 0.002 (0.2%). In addition, Abaqus/Explicit supports the following filtering method for the computation of : represents the accumulated time over the analysis increments required to have an increase in ) facilitates filtering high-frequency where equivalent plastic strain of at least . The factor oscillations. This filtering method is usually not necessary provided that an appropriate value of is used. You can specify the value of directly. The default value is (no filtering). ( In Abaqus/Standard is computed at every analysis increment as , without using either of the above filtering methods. However, you can still specify values for and ; and these values can be imported into any subsequent analysis in Abaqus/Explicit. Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=MSFLD, PEINC= OMEGA= Property module: material editor: Mechanical→Damage for Ductile Metals→MSFLD Damage: Omega: , The value for cannot be specified directly in Abaqus/CAE. Initial conditions When we need to study the behavior of a material that has been previously subjected to deformations, such as those originated during the manufacturing process, initial equivalent plastic strain values can be provided to specify the initial work hardened state of the material . In addition, when the initial equivalent plastic strain is greater than the minimum value on the forming limit curve, the initial value of plays an important role in determining whether the MSFLD It is, therefore, important to damage initiation criterion will be met during subsequent deformation. specify the initial value of in these situations. To this end, you can specify initial values of the plastic strain tensor . Abaqus will use this information to compute the initial value of as the ratio of the minor and major principal plastic strains; that is, neglecting the elastic component of deformation and assuming a linear deformation path. Input File Usage: Use both of the following options to specify that material hardening and plastic strain have occurred prior to the current analysis: *INITIAL CONDITIONS, TYPE=HARDENING *INITIAL CONDITIONS, TYPE=PLASTIC STRAIN Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step Initial plastic strain conditions are not supported in Abaqus/CAE. Abaqus/CAE Usage: Elements The damage initiation criteria for ductile metals can be used with any elements in Abaqus that include mechanical behavior (elements that have displacement degrees of freedom) except for the pipe elements in Abaqus/Explicit. The models for sheet metal necking instability (FLD, FLSD, MSFLD, and M-K) are available only with elements that include mechanical behavior and use a plane stress formulation (i.e., plane stress, shell, continuum shell, and membrane elements). Output In addition to the standard output identifiers available in Abaqus (“Output variables,” Section 4.2), the following variables have special meaning when a damage initiation criterion is specified: ERPRATIO SHRRATIO TRIAX Ratio of principal strain rates, Shear stress ratio, initiation criterion. Stress triaxiality, with damage initiation). , used for the MSFLD damage initiation criterion. , used for the evaluation of the shear damage (available in Abaqus/Standard only in conjunction DMICRT DUCTCRT JCCRT SHRCRT FLDCRT FLSDCRT MSFLDCRT MKCRT All damage initiation criteria components listed below. Ductile damage initiation criterion, . Johnson-Cook damage initiation criterion (available only in Abaqus/Explicit). Shear damage initiation criterion, . Maximum value of the FLD damage initiation criterion, , during the analysis. Maximum value of the FLSD damage initiation criterion, analysis. Maximum value of the MSFLD damage initiation criterion, analysis. , during the , during the Marciniak-Kuczynski Abaqus/Explicit), . damage initiation criterion (available only in A value of 1 or greater for output variables associated with a damage initiation criterion indicates that the criterion has been met. Abaqus will limit the maximum value of the output variable to 1 if a damage evolution law has been prescribed for that criterion . However, if no damage evolution is specified, the criterion for damage initiation will continue to be computed beyond the point of damage initiation; in this case the output variable can take values greater than 1, indicating by how much the initiation criterion has been exceeded. Additional references • Hooputra, H., H. Gese, H. Dell, and H. Werner, “A Comprehensive Failure Model for Crashworthiness Simulation of Aluminium Extrusions,” International Journal of Crashworthiness, vol. 9, no. 5, pp. 449–464, 2004. • Bai, Y., and T. Wierzbicki, “A New Model of Metal Plasticity and Fracture with Pressure and Lode Dependence,” International Journal of Plasticity, vol. 24, no. 6, pp. 1071–1096, 2008. • Johnson, G. R., and W. H. Cook, “Fracture Characteristics of Three Metals Subjected to Various Strains, Strain rates, Temperatures and Pressures,” Engineering Fracture Mechanics, vol. 21, no. 1, pp. 31–48, 1985. • Keeler, S. P., and W. A. Backofen, “Plastic Instability and Fracture in Sheets Stretched over Rigid Punches,” ASM Transactions Quarterly, vol. 56, pp. 25–48, 1964. • Marciniak, Z., and K. Kuczynski, “Limit Strains in the Processes of Stretch Forming Sheet Metal,” International Journal of Mechanical Sciences, vol. 9, pp. 609–620, 1967. • Müschenborn, W., and H. Sonne, “Influence of the Strain Path on the Forming Limits of Sheet Metal,” Archiv fur das Eisenhüttenwesen, vol. 46, no. 9, pp. 597–602, 1975. • Stoughton, T. B., “A General Forming Limit Criterion for Sheet Metal Forming,” International Journal of Mechanical Sciences, vol. 42, pp. 1–27, 2000. 24.2.3 DAMAGE EVOLUTION AND ELEMENT REMOVAL FOR DUCTILE METALS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Progressive damage and failure,” Section 24.1.1 • *DAMAGE EVOLUTION • “Damage evolution” in “Defining damage,” Section 12.9.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The damage evolution capability for ductile metals: • assumes that damage is characterized by the progressive degradation of the material stiffness, leading to material failure; • must be used in combination with a damage initiation criterion for ductile metals (“Damage initiation for ductile metals,” Section 24.2.2); • uses mesh-independent measures (either plastic displacement or physical energy dissipation) to drive the evolution of damage after damage initiation; • takes into account the combined effect of different damage mechanisms acting simultaneously on the same material and includes options to specify how each mechanism contributes to the overall material degradation; and • offers options for what occurs upon failure, including the removal of elements from the mesh. Damage evolution Figure 24.2.3–1 illustrates the characteristic stress-strain behavior of a material undergoing damage. In the context of an elastic-plastic material with isotropic hardening, the damage manifests itself in two forms: softening of the yield stress and degradation of the elasticity. The solid curve in the figure represents the damaged stress-strain response, while the dashed curve is the response in the absence of damage. As discussed later, the damaged response depends on the element dimensions such that mesh dependency of the results is minimized. and In the figure are the yield stress and equivalent plastic strain at the onset of damage, and is the equivalent plastic strain at failure; that is, when the overall damage variable reaches the value . The overall damage variable, D, captures the combined effect of all active damage mechanisms , as discussed later in this section . The value of the equivalent plastic strain at failure, , depends on the characteristic length of the element and cannot be used as a material parameter for the specification of the damage evolution law. (D=0) D σ y0 (1-D)E ε pl ε pl Figure 24.2.3–1 Stress-strain curve with progressive damage degradation. Instead, the damage evolution law is specified in terms of equivalent plastic displacement, terms of fracture energy dissipation, ; these concepts are defined next. , or in Mesh dependency and characteristic length When material damage occurs, the stress-strain relationship no longer accurately represents the material’s behavior. Continuing to use the stress-strain relation introduces a strong mesh dependency based on strain localization, such that the energy dissipated decreases as the mesh is refined. A different approach is required to follow the strain-softening branch of the stress-strain response curve. Hillerborg’s (1976) fracture energy proposal is used to reduce mesh dependency by creating a stress-displacement response after damage is initiated. Using brittle fracture concepts, Hillerborg defines the energy required to open a unit area of crack, , as a material parameter. With this approach, the softening response after damage initiation is characterized by a stress-displacement response rather than a stress-strain response. The implementation of this stress-displacement concept in a finite element model requires the definition of a characteristic length, L, associated with an integration point. The fracture energy is then given as This expression introduces the definition of the equivalent plastic displacement, , as the fracture work conjugate of the yield stress after the onset of damage (work per unit area of the crack). Before damage initiation . The definition of the characteristic length depends on the element geometry and formulation: it is a typical length of a line across an element for a first-order element; it is half of the same typical length for ; after damage initiation a second-order element. For beams and trusses it is a characteristic length along the element axis. For membranes and shells it is a characteristic length in the reference surface. For axisymmetric elements it is a characteristic length in the r–z plane only. For cohesive elements it is equal to the constitutive thickness. This definition of the characteristic length is used because the direction in which fracture occurs is not known in advance. Therefore, elements with large aspect ratios will have rather different behavior depending on the direction in which they crack: some mesh sensitivity remains because of this effect, and elements that have aspect ratios close to unity are recommended. Each damage initiation criterion described in “Damage initiation for ductile metals,” Section 24.2.2, may have an associated damage evolution law. The damage evolution law can be specified in terms of equivalent plastic displacement, . Both of these options take into account the characteristic length of the element to alleviate mesh dependency of the results. , or in terms of fracture energy dissipation, Evaluating overall damage when multiple criteria are active The overall damage variable, D, captures the combined effect of all active mechanisms and is computed in terms of individual damage variables, , for each mechanism. You can choose to combine some of the damage variables in a multiplicative sense to form an intermediate variable, , as follows: Then, the overall damage variable is computed as the maximum of variables: and the remaining damage In the above expressions overall damage in a multiplicative and a maximum sense, respectively, with and represent the sets of active mechanisms that contribute to the . Input File Usage: Abaqus/CAE Usage: Use the following option to specify that the damage associated with a particular criterion contributes to the overall damage variable in a maximum sense (default): *DAMAGE EVOLUTION, DEGRADATION=MAXIMUM Use the following option to specify that the damage associated with a particular criterion contributes to the overall damage variable in a multiplicative sense: *DAMAGE EVOLUTION, DEGRADATION=MULTIPLICATIVE Use the following options to specify that the damage associated with a particular criterion contributes to the overall damage variable in a maximum sense (default) or in a multiplicative sense, respectively: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution: Degradation: Maximum or Multiplicative Defining damage evolution based on effective plastic displacement As discussed previously, once the damage initiation criterion has been reached, the effective plastic displacement, , is defined with the evolution equation where L is the characteristic length of the element. The evolution of the damage variable with the relative plastic displacement can be specified in tabular, linear, or exponential form. Instantaneous failure will occur if the plastic displacement at failure, , is specified as 0; however, this choice is not recommended and should be used with care because it causes a sudden drop of the stress at the material point that can lead to dynamic instabilities. Tabular form You can specify the damage variable directly as a tabular function of equivalent plastic displacement, , as shown in Figure 24.2.3–2(a). Input File Usage: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=TABULAR Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Type: Displacement: Softening: Tabular Evolution: Linear form Assume a linear evolution of the damage variable with effective plastic displacement, as shown in Figure 24.2.3–2(b). You can specify the effective plastic displacement, , at the point of failure (full degradation). Then, the damage variable increases according to , the This definition ensures that when the effective plastic displacement reaches the value material stiffness will be fully degraded ( ). The linear damage evolution law defines a truly linear stress-strain softening response only if the effective response of the material is perfectly plastic (constant yield stress) after damage initiation. Input File Usage: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=LINEAR Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Type: Displacement: Softening: Linear Evolution: u pl u pl u pl (a) tabular u pl (b) linear α=10 α=3 α=1 α=0 u pl (c) exponential Figure 24.2.3–2 Different definitions of damage evolution based on plastic displacement: (a) tabular, (b) linear, and (c) exponential. Exponential form Assume an exponential evolution of the damage variable with plastic displacement, as shown in Figure 24.2.3–2(c). You can specify the relative plastic displacement at failure, , and the exponent . The damage variable is given as Input File Usage: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=EXPONENTIAL Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Type: Displacement: Softening: Exponential Evolution: Defining damage evolution based on energy dissipated during the damage process , to be dissipated during the damage process directly. You can specify the fracture energy per unit area, Instantaneous failure will occur if is specified as 0. However, this choice is not recommended and should be used with care because it causes a sudden drop in the stress at the material point that can lead to dynamic instabilities. The evolution in the damage can be specified in linear or exponential form. Linear form Assume a linear evolution of the damage variable with plastic displacement. You can specify the fracture energy per unit area, . Then, once the damage initiation criterion is met, the damage variable increases according to where the equivalent plastic displacement at failure is computed as and is the value of the yield stress at the time when the failure criterion is reached. Therefore, the model becomes equivalent to that shown in Figure 24.2.3–2(b). The model ensures that the energy dissipated during the damage evolution process is equal to only if the effective response of the material is perfectly plastic (constant yield stress) beyond the onset of damage. Input File Usage: *DAMAGE EVOLUTION, TYPE=ENERGY, SOFTENING=LINEAR Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution: Type: Energy: Softening: Linear Exponential form Assume an exponential evolution of the damage variable given as The formulation of the model ensures that the energy dissipated during the damage evolution process is equal to In theory, the damage variable reaches a value of 1 only asymptotically at infinite equivalent plastic displacement (Figure 24.2.3–3(b)). In practice, Abaqus/Explicit will set d equal to one when the dissipated energy reaches a value of , as shown in Figure 24.2.3–3(a). . Input File Usage: *DAMAGE EVOLUTION, TYPE=ENERGY, SOFTENING=EXPONENTIAL Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile Metals→criterion: Suboptions→Damage Evolution: Type: Energy: Softening: Exponential yo u pl u pl (a) (b) Figure 24.2.3–3 Energy-based damage evolution with exponential law: evolution of (a) yield stress and (b) damage variable. Maximum degradation and choice of element removal You have control over how Abaqus treats elements with severe damage. You can specify an upper bound, , to the overall damage variable, D; and you can choose whether to delete an element once maximum degradation is reached. The latter choice also affects which stiffness components are damaged. Specifying the value of maximum degradation The default setting of depends on whether elements are to be deleted upon reaching maximum degradation (discussed next). For the default case of element deletion and in all cases for cohesive elements, . The output variable SDEG contains the value of D. No further damage is accumulated at an integration point once D reaches (except, of course, any remaining stiffness is lost upon element deletion). ; otherwise, Input File Usage: Use the following option to specify : *SECTION CONTROLS, MAX DEGRADATION= Removing the element from the mesh Elements are deleted by default upon reaching maximum degradation. Except for cohesive elements with traction-separation response , Abaqus applies damage to all stiffness components equally for elements that may eventually be removed: In Abaqus/Standard an element is removed from the mesh if D reaches at all of the section points at all the integration locations of an element except for cohesive elements (for cohesive elements the conditions for element deletion are that D reaches at all integration points and, for traction- separation response, none of the integration points are in compression). In Abaqus/Explicit an element is removed from the mesh if D reaches at all of the section points at any one integration location of an element except for cohesive elements (for cohesive elements the conditions for element deletion are that D reaches at all integration points and, for traction- separation response, none of the integration points are in compression). For example, removal of a solid element takes place, by default, when maximum degradation is reached at any one integration point. However, in a shell element all through-the-thickness section points at any one integration location of an element must fail before the element is removed from the mesh. In the case of second-order reduced- integration beam elements, reaching maximum degradation at all section points through the thickness at either of the two element integration locations along the beam axis leads, by default, to element removal. Similarly, in modified triangular and tetrahedral solid elements and fully integrated membrane elements D reaching at any one integration point leads, by default, to element removal. In a heat transfer analysis the thermal properties of the material are not affected by the progressive damage of the material stiffness until the condition for element deletion is reached; at this point the thermal contribution of the element is also removed. Input File Usage: Use the following option to delete the element from the mesh (default): *SECTION CONTROLS, ELEMENT DELETION=YES Keeping the element in the computations Optionally, you may choose not to remove the element from the mesh, except in the case of three- dimensional beam elements. With element deletion turned off, the overall damage variable is enforced to be if element deletion is turned off, which ensures that elements will remain active in the simulation with a residual stiffness of at least 1% of the original stiffness. The dimensionality of the stress state of the element affects which stiffness components can become damaged, as discussed below. . The default value is In a heat transfer analysis the thermal properties of the material are not affected by damage of the material stiffness. Input File Usage: Use the following option to keep the element in the computation: *SECTION CONTROLS, ELEMENT DELETION=NO Elements with three-dimensional stress states in Abaqus/Explicit For elements with three-dimensional stress states (including generalized plane strain elements) the shear stiffness will be degraded up to a maximum value, , leading to softening of the deviatoric stress components. The bulk stiffness, however, will be degraded only while the material is subjected to negative pressures (i.e., hydrostatic tension); there is no bulk degradation under positive pressures. This corresponds to a fluid-like behavior. Therefore, the degraded deviatoric, , and pressure, p, stresses are computed as where the deviatoric and volumetric damage variables are given as In this case the output variable SDEG contains the value of . Elements with three-dimensional stress states in Abaqus/Standard For elements with three-dimensional stress states (including generalized plane strain elements) the stiffness will be degraded uniformly until the maximum degradation, , is reached. Output variable SDEG contains the value of D. Elements with plane stress states For elements with a plane stress formulation (plane stress, shell, continuum shell, and membrane elements) the stiffness will be degraded uniformly until the maximum degradation, , is reached. Output variable SDEG contains the value of D. Elements with one-dimensional stress states For elements with a one-dimensional stress state (i.e., truss elements, rebar, and cohesive elements with gasket behavior) their only stress component will be degraded if it is positive (tension). The material stiffness will remain unaffected under compression loading. The stress is, therefore, given by , where the uniaxial damage variable is computed as In this case variable SDEG contains the value of . determines the maximum allowed degradation in uniaxial tension ( ). Output Convergence difficulties in Abaqus/Standard Material models exhibiting softening behavior and stiffness degradation often lead to severe convergence difficulties in implicit analysis programs, such as Abaqus/Standard. Some techniques are available in Abaqus/Standard to improve convergence for analyses involving these materials. Viscous regularization in Abaqus/Standard You can overcome some of the convergence difficulties associated with softening and stiffness degradation by using the viscous regularization scheme, which causes the tangent stiffness matrix of the softening material to be positive for sufficiently small time increments. In this regularization scheme a viscous damage variable is defined by the evolution equation: where is the viscosity coefficient representing the relaxation time of the viscous system and d is the damage variable evaluated in the inviscid base model. The damaged response of the viscous material is computed using the viscous value of the damage variable. Using viscous regularization with a small value of the viscosity parameter (small compared to the characteristic time increment) usually helps improve the rate of convergence of the model in the softening regime, without compromising results. The basic idea is that the solution of the viscous system relaxes to that of the inviscid case as , where t represents time. In Abaqus/Standard you can specify the viscous coefficients as part of a section controls definition. For more information, see “Using viscous regularization with cohesive elements, connector elements, and elements that can be used with the damage evolution models for ductile metals and fiber-reinforced composites in Abaqus/Standard” in “Section controls,” Section 27.1.4. Unsymmetric equation solver if any of the ductile evolution models is used, In general, the material Jacobian matrix will be nonsymmetric. To improve convergence, it is recommended that the unsymmetric equation solver is used in this case. Using the damage models with rebar It is possible to use material damage models in elements for which rebar are also defined. The base material contribution to the element stress-carrying capacity diminishes according to the behavior described previously in this section. The rebar contribution to the element stress-carrying capacity will not be affected unless damage is also included in the rebar material definition; in that case the rebar contribution to the element stress-carrying capacity will also be degraded after the damage initiation criterion specified for the rebar is met. For the default choice of element deletion, the element is removed from the mesh when at any one integration location all section points in the base material and rebar are fully degraded. Elements Damage evolution for ductile metals can be defined for any element that can be used with the damage initiation criteria for ductile metals in Abaqus (“Damage initiation for ductile metals,” Section 24.2.2). Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning when damage evolution is specified: STATUS SDEG Status of element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). Overall scalar stiffness degradation, D. Additional reference • Hillerborg, A., M. Modeer, and P. E. Petersson, “Analysis of Crack Formation and Crack Growth in Concrete by Means of Fracture Mechanics and Finite Elements,” Cement and Concrete Research, vol. 6, pp. 773–782, 1976. 24.3 Damage and failure for fiber-reinforced composites • “Damage and failure for fiber-reinforced composites: overview,” Section 24.3.1 • “Damage initiation for fiber-reinforced composites,” Section 24.3.2 • “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3 24.3.1 DAMAGE AND FAILURE FOR FIBER-REINFORCED COMPOSITES: OVERVIEW Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Progressive damage and failure,” Section 24.1.1 • “Damage initiation for fiber-reinforced composites,” Section 24.3.2 • “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3 • *DAMAGE INITIATION • *DAMAGE EVOLUTION • *DAMAGE STABILIZATION • “Hashin damage” in “Defining damage,” Section 12.9.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Abaqus offers a damage model enabling you to predict the onset of damage and to model damage evolution for elastic-brittle materials with anisotropic behavior. The model is primarily intended to be used with fiber-reinforced materials since they typically exhibit such behavior. This damage model requires specification of the following: • the undamaged response of the material, which must be linearly elastic ; • a damage initiation criterion ; and • a damage evolution response, including a choice of element removal . General concepts of damage in unidirectional lamina Damage is characterized by the degradation of material stiffness. It plays an important role in the analysis of fiber-reinforced composite materials. Many such materials exhibit elastic-brittle behavior; that is, damage in these materials is initiated without significant plastic deformation. Consequently, plasticity can be neglected when modeling behavior of such materials. The fibers in the fiber-reinforced material are assumed to be parallel, as depicted in Figure 24.3.1–1. You must specify material properties in a local coordinate system defined by the user. The lamina is in the 1–2 plane, and the local 1 direction corresponds to the fiber direction. You must specify the undamaged material response using one of the methods for defining an orthotropic linear elastic material (“Linear elastic behavior,” Section 22.2.1); the most convenient of which is the method for defining an orthotropic material in plane stress (“Defining orthotropic elasticity in plane stress” in “Linear elastic behavior,” Figure 24.3.1–1 Unidirectional lamina. Section 22.2.1). However, the material response can also be defined in terms of the engineering constants or by specifying the elastic stiffness matrix directly. The Abaqus anisotropic damage model is based on the work of Matzenmiller et. al (1995), Hashin and Rotem (1973), Hashin (1980), and Camanho and Davila (2002). Four different modes of failure are considered: • fiber rupture in tension; • fiber buckling and kinking in compression; • matrix cracking under transverse tension and shearing; and • matrix crushing under transverse compression and shearing. In Abaqus the onset of damage is determined by the initiation criteria proposed by Hashin and Rotem (1973) and Hashin (1980), in which the failure surface is expressed in the effective stress space (the stress acting over the area that effectively resists the force). These criteria are discussed in detail in “Damage initiation for fiber-reinforced composites,” Section 24.3.2. The response of the material is computed from where is the strain and is the elasticity matrix, which reflects any damage and has the form where current state of matrix damage, in the fiber direction, shear modulus, and and , reflects the current state of fiber damage, reflects the current state of shear damage, reflects the is the Young’s modulus is the is the Young’s modulus in the direction perpendicular to the fibers, are Poisson’s ratios. The evolution of the elasticity matrix due to damage is discussed in more detail in “Damage that section also evolution and element removal for fiber-reinforced composites,” Section 24.3.3; discusses: • options for treating severe damage (“Maximum degradation and choice of element removal” in “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3); and • viscous regularization (“Viscous regularization” in “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3). Elements The fiber-reinforced composite damage model must be used with elements with a plane stress formulation, which include plane stress, shell, continuum shell, and membrane elements. Additional references • Camanho, P. P., and C. G. Davila, “Mixed-Mode Decohesion Finite Elements for the Simulation of Delamination in Composite Materials,” NASA/TM-2002–211737, pp. 1–37, 2002. • Hashin, Z., “Failure Criteria for Unidirectional Fiber Composites,” Journal of Applied Mechanics, vol. 47, pp. 329–334, 1980. • Hashin, Z., and A. Rotem, “A Fatigue Criterion for Fiber-Reinforced Materials,” Journal of Composite Materials, vol. 7, pp. 448–464, 1973. • Matzenmiller, A., J. Lubliner, and R. L. Taylor, “A Constitutive Model for Anisotropic Damage in Fiber-Composites,” Mechanics of Materials, vol. 20, pp. 125–152, 1995. 24.3.2 DAMAGE INITIATION FOR FIBER-REINFORCED COMPOSITES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Progressive damage and failure,” Section 24.1.1 • “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3 • *DAMAGE INITIATION • “Hashin damage” in “Defining damage,” Section 12.9.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The material damage initiation capability for fiber-reinforced materials: • requires that the behavior of the undamaged material is linearly elastic ; • is based on Hashin’s theory (Hashin and Rotem, 1973, and Hashin, 1980); • takes into account four different failure modes: fiber tension, fiber compression, matrix tension, and matrix compression; and • can be used in combination with the damage evolution model described in “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3 . Damage Initiation Damage initiation refers to the onset of degradation at a material point. In Abaqus the damage initiation criteria for fiber-reinforced composites are based on Hashin’s theory . These criteria consider four different damage initiation mechanisms: fiber tension, fiber compression, matrix tension, and matrix compression. The initiation criteria have the following general forms: Fiber tension : Fiber compression : Matrix tension : Matrix compression : In the above equations denotes the longitudinal tensile strength; denotes the longitudinal compressive strength; denotes the transverse tensile strength; denotes the transverse compressive strength; denotes the longitudinal shear strength; denotes the transverse shear strength; is a coefficient that determines the contribution of the shear stress to the fiber tensile initiation criterion; and are components of the effective stress tensor, initiation criteria and which is computed from: , that is used to evaluate the where is the true stress and is the damage operator: , , and are internal (damage) variables that characterize fiber, matrix, and , shear damage, which are derived from damage variables , corresponding to the four modes previously discussed, as follows: , and , Prior to any damage initiation and evolution the damage operator, , is equal to the identity matrix, so . Once damage initiation and evolution has occurred for at least one mode, the damage operator becomes significant in the criteria for damage initiation of other modes (see “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3, for discussion of damage evolution). The effective stress, , is intended to represent the stress acting over the damaged area that effectively resists the internal forces. The initiation criteria presented above can be specialized to obtain the model proposed in Hashin or the model proposed in Hashin (1980) by and and Rotem (1973) by setting setting . An output variable is associated with each initiation criterion (fiber tension, fiber compression, matrix tension, matrix compression) to indicate whether the criterion has been met. A value of 1.0 or higher indicates that the initiation criterion has been met . If you define a damage initiation model without defining an associated evolution law, the initiation criteria will affect only output. Thus, you can use these criteria to evaluate the propensity of the material to undergo damage without modeling the damage process. Input File Usage: Use the following option to define the Hashin damage initiation criterion: *DAMAGE INITIATION, CRITERION=HASHIN, ALPHA= , , , , , Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Fiber- Reinforced Composites→Hashin Damage Elements The damage initiation criteria must be used with elements with a plane stress formulation, which include plane stress, shell, continuum shell, and membrane elements. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable the identifiers,” Section 4.2.1, and, “Abaqus/Explicit output variable identifiers,” Section 4.2.2), following variables relate specifically to damage initiation at a material point in the fiber-reinforced composite damage model: DMICRT HSNFTCRT HSNFCCRT HSNMTCRT HSNMCCRT All damage initiation criteria components. Maximum value of the fiber tensile initiation criterion experienced during the analysis. Maximum value of the fiber compressive initiation criterion experienced during the analysis. Maximum value of the matrix tensile initiation criterion experienced during the analysis. Maximum value of the matrix compressive initiation criterion experienced during the analysis. For the variables above that indicate whether an initiation criterion in a damage mode has been satisfied or not, a value that is less than 1.0 indicates that the criterion has not been satisfied, while a value of 1.0 or higher indicates that the criterion has been satisfied. If you define a damage evolution model, the maximum value of this variable does not exceed 1.0. However, if you do not define a damage evolution model, this variable can have values higher than 1.0, which indicates by how much the criterion has been exceeded. Additional references • Hashin, Z., “Failure Criteria for Unidirectional Fiber Composites,” Journal of Applied Mechanics, vol. 47, pp. 329–334, 1980. • Hashin, Z., and A. Rotem, “A Fatigue Criterion for Fiber-Reinforced Materials,” Journal of Composite Materials, vol. 7, pp. 448–464, 1973. 24.3.3 DAMAGE EVOLUTION AND ELEMENT REMOVAL FOR FIBER-REINFORCED COMPOSITES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Progressive damage and failure,” Section 24.1.1 • “Damage initiation for fiber-reinforced composites,” Section 24.3.2 • *DAMAGE EVOLUTION • “Damage evolution” in “Defining damage,” Section 12.9.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The damage evolution capability for fiber-reinforced materials in Abaqus: • assumes that damage is characterized by progressive degradation of material stiffness, leading to material failure; • requires linearly elastic behavior of the undamaged material ; • takes into account four different failure modes: fiber tension, fiber compression, matrix tension, and matrix compression; • uses four damage variables to describe damage for each failure mode; • must be used in combination with Hashin’s damage initiation criteria (“Damage initiation for fiber- reinforced composites,” Section 24.3.2); • is based on energy dissipation during the damage process; • offers options for what occurs upon failure, including the removal of elements from the mesh; and • can be used in conjunction with a viscous regularization of the constitutive equations to improve the convergence rate in the softening regime. Damage evolution The previous section (“Damage initiation for fiber-reinforced composites,” Section 24.3.2) discussed the damage initiation in plane stress fiber-reinforced composites. This section will discuss the post-damage initiation behavior for cases in which a damage evolution model has been specified. Prior to damage initiation the material is linearly elastic, with the stiffness matrix of a plane stress orthotropic material. Thereafter, the response of the material is computed from where is the strain and is the damaged elasticity matrix, which has the form where current state of matrix damage, in the fiber direction, and are Poisson’s ratios. The damage variables , reflects the current state of fiber damage, reflects the current state of shear damage, reflects the is the Young’s modulus is the Young’s modulus in the matrix direction, is the shear modulus, and , , and are derived from damage variables , , , and , corresponding to the four failure modes previously discussed, as follows: and are components of the effective stress tensor. The effective stress tensor is primarily used to evaluate damage initiation criteria; see “Damage initiation for fiber-reinforced composites,” Section 24.3.2, for a description of how the effective stress tensor is computed. Evolution of damage variables for each mode To alleviate mesh dependency during material softening, Abaqus introduces a characteristic length into the formulation, so that the constitutive law is expressed as a stress-displacement relation. The damage variable will evolve such that the stress-displacement behaves as shown in Figure 24.3.3–1 in each of the four failure modes. The positive slope of the stress-displacement curve prior to damage initiation corresponds to linear elastic material behavior; the negative slope after damage initiation is achieved by evolution of the respective damage variables according to the equations shown below. Equivalent displacement and stress for each of the four damage modes are defined as follows: Fiber tension : Fiber compression : equivalent stress σ eq δ eq δ eq equivalent displacement Figure 24.3.3–1 Equivalent stress versus equivalent displacement. Matrix tension : Matrix compression : The characteristic length, , is based on the element geometry and formulation: it is a typical length of a line across an element for a first-order element; it is half of the same typical length for a second-order element. For membranes and shells it is a characteristic length in the reference surface, computed as the square root of the area. The symbol in the equations above represents the Macaulay bracket operator, which is defined for every as . After damage initiation (i.e., ) for the behavior shown in Figure 24.3.3–1, the damage variable for a particular mode is given by the following expression is the initial equivalent displacement at which the initiation criterion for that mode was met is the displacement at which the material is completely damaged in this failure mode. The above where and relation is presented graphically in Figure 24.3.3–2. damage variable 1.0 δ eq δ eq equivalent displacement Figure 24.3.3–2 Damage variable as a function of equivalent displacement. for the various modes depend on the elastic stiffness and the strength parameters The values of specified as part of the damage initiation definition . For each failure mode you must specify the energy dissipated due to failure, for the various modes depend on the respective , which corresponds to the area of the triangle OAC in Figure 24.3.3–3. The values of values. Unloading from a partially damaged state, such as point B in Figure 24.3.3–3, occurs along a linear path toward the origin in the plot of equivalent stress vs. equivalent displacement; this same path is followed back to point B upon reloading as shown in the figure. equivalent stress δ eq δ eq equivalent displacement Figure 24.3.3–3 Linear damage evolution. Input File Usage: Use the following option to define the damage evolution law: *DAMAGE EVOLUTION, TYPE=ENERGY, SOFTENING=LINEAR , , , , , where are energies dissipated during damage for fiber tension, fiber compression, matrix tension, and matrix compression failure modes, respectively. , and Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Fiber- Reinforced Composites→Hashin Damage: Suboptions→Damage Evolution: Type: Energy: Softening: Linear Maximum degradation and choice of element removal You have control over how Abaqus treats elements with severe damage. By default, the upper bound to all damage variables at a material point is . You can reduce this upper bound as discussed in “Controlling element deletion and maximum degradation for materials with damage evolution” in “Section controls,” Section 27.1.4. By default, in Abaqus/Standard an element is removed (deleted) once damage variables for all failure modes at all material points reach . In Abaqus/Explicit a material point is assumed to fail when either of the damage variables associated with fiber failure modes (tensile or compressive) reaches and the element is removed from the mesh when this condition is satisfied at all of the section points at any one integration location of an element; for example, in the case of shell elements all through-the-thickness section points at any one integration location of the element must fail before the element is removed from the mesh. If an element is removed, the output variable STATUS is set to zero for the element, and it offers no resistance to subsequent deformation. Elements that have been removed are not displayed when you view the deformed model in the Visualization module of Abaqus/CAE (Abaqus/Viewer). However, the elements still remain in the Abaqus model. You can choose to display removed elements by suppressing use of the STATUS variable . Alternatively, you can specify that an element should remain in the model even after all of the . In this case, once all the damage variables reach the maximum value, the damage variables reach stiffness, , remains constant . Difficulties associated with element removal in Abaqus/Standard When elements are removed from the model, their nodes will still remain in the model even if they are not attached to any active elements. When the solution progresses, these nodes might undergo non-physical displacements due to the extrapolation scheme used in Abaqus/Standard to speed up the solution . These non-physical displacements can be prevented by turning off the extrapolation. In addition, applying a point load to a node that is not attached to an active element will cause convergence difficulties since there is no stiffness to resist the load. It is the responsibility of the user to prevent such situations. Viscous regularization Material models exhibiting softening behavior and stiffness degradation often lead to severe convergence difficulties in implicit analysis programs, such as Abaqus/Standard. You can overcome some of these convergence difficulties by using the viscous regularization scheme, which causes the tangent stiffness matrix of the softening material to be positive for sufficiently small time increments. In this regularization scheme a viscous damage variable is defined by the evolution equation: where is the viscosity coefficient representing the relaxation time of the viscous system and d is the damage variable evaluated in the inviscid backbone model. The damaged response of the viscous material is given as where the damaged elasticity matrix, , is computed using viscous values of damage variables for each failure mode. Using viscous regularization with a small value of the viscosity parameter (small compared to the characteristic time increment) usually helps improve the rate of convergence of the model in the softening regime, without compromising results. The basic idea is that the solution of the viscous system relaxes to that of the inviscid case as , where t represents time. Viscous regularization is also available in Abaqus/Explicit. Viscous regularization slows down the rate of increase of damage and leads to increased fracture energy with increasing deformation rates, which can be exploited as an effective method of modeling rate-dependent material behavior. In Abaqus/Standard the approximate amount of energy associated with viscous regularization over the whole model or over an element set is available using output variable ALLCD. Defining viscous regularization coefficients You can specify different values of viscous coefficients for different failure modes. Input File Usage: Use the following option to define viscous coefficients: *DAMAGE STABILIZATION , , , , , where are viscosity coefficients for fiber tension, fiber compression, matrix tension, and matrix compression failure modes, respectively. , Abaqus/CAE Usage: Use the following input to define the viscous coefficients for fiber-reinforced materials: Property module: material editor: Mechanical→Damage for Fiber-Reinforced Composites→Hashin Damage: Suboptions→Damage Stabilization Applying a single viscous coefficient in Abaqus/Standard Alternatively, in Abaqus/Standard you can specify the viscous coefficients as part of a section controls definition. In this case the same viscous coefficient will be applied to all failure modes. For more information, see “Using viscous regularization with cohesive elements, connector elements, and elements that can be used with the damage evolution models for ductile metals and fiber-reinforced composites in Abaqus/Standard” in “Section controls,” Section 27.1.4. Material damping If stiffness proportional damping is specified in combination with the damage evolution law for fiber- reinforced materials, Abaqus calculates the damping stresses using the damaged elastic stiffness. Elements The damage evolution law for fiber-reinforced materials must be used with elements with a plane stress formulation, which include plane stress, shell, continuum shell, and membrane elements. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables relate specifically to damage evolution in the fiber- reinforced composite damage model: STATUS Status of the element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). The value of this variable is set to 0.0 only if damage has occurred in all the damage modes. DAMAGEFT Fiber tensile damage variable. DAMAGEFC Fiber compressive damage variable. DAMAGEMT Matrix tensile damage variable. DAMAGEMC Matrix compressive damage variable. DAMAGESHR Shear damage variable. EDMDDEN Energy dissipated per unit volume in the element by damage. ELDMD DMENER ALLDMD ECDDEN ELCD CENER ALLCD Total energy dissipated in the element by damage. Energy dissipated per unit volume by damage. Energy dissipated in the whole (or partial) model by damage. Energy per unit volume in the element regularization. that is associated with viscous Total energy in the element that is associated with viscous regularization. Energy per unit volume that is associated with viscous regularization. The approximate amount of energy over the whole model or over an element set that is associated with viscous regularization. 24.4 Damage and failure for ductile materials in low-cycle fatigue analysis • “Damage and failure for ductile materials in low-cycle fatigue analysis: overview,” Section 24.4.1 • “Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2 • “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3 24.4.1 DAMAGE AND FAILURE FOR DUCTILE MATERIALS IN LOW-CYCLE FATIGUE ANALYSIS: OVERVIEW Product: Abaqus/Standard References • “Progressive damage and failure,” Section 24.1.1 • “Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2 • “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3 • “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7 • *DAMAGE INITIATION • *DAMAGE EVOLUTION Overview Abaqus/Standard offers a general capability for modeling progressive damage and failure of ductile materials due to stress reversals and the accumulation of inelastic strain energy in a low-cycle fatigue analysis using the direct cyclic approach. In the most general case this requires the specification of the following: • the undamaged ductile materials in any elements (including cohesive elements based on a continuum approach) whose response is defined in terms of a continuum-based constitutive model (“Material library: overview,” Section 21.1.1); • a damage initiation criterion (“Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2); and • a damage evolution response (“Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3). A summary of the general framework for progressive damage and failure in Abaqus is given in “Progressive damage and failure,” Section 24.1.1. This section provides an overview of the damage initiation criteria and damage evolution law for ductile materials in a low-cycle fatigue analysis using the direct cyclic approach. General concepts of damage of ductile materials in low-cycle fatigue Accurately and effectively predicting the fatigue life for an inelastic structure, such as a solder joint in an electronic chip packaging, subjected to sub-critical cyclic loading is a challenging problem. Cyclic thermal or mechanical loading often leads to stress reversals and the accumulation of inelastic strain, which may in turn lead to the initiation and propagation of a crack. The low-cycle fatigue analysis capability in Abaqus/Standard uses a direct cyclic approach (“Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7) to model progressive damage and failure based on a continuum damage approach. The damage initiation (“Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2) and evolution (“Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3) are characterized by the stabilized accumulated inelastic hysteresis strain energy per cycle proposed by Darveaux (2002) and Lau (2002). The damage evolution law describes the rate of degradation of the material stiffness per cycle once the corresponding initiation criterion has been reached. For damage in ductile materials Abaqus/Standard assumes that the degradation of the stiffness can be modeled using a scalar damage variable, . At any given cycle during the analysis the stress tensor in the material is given by the scalar damage equation where damage computed in the current increment. The material has lost its load carrying capacity when is the effective (or undamaged) stress tensor that would exist in the material in the absence of . Elements The failure modeling capability for ductile materials can be used with any elements (including cohesive elements based on a continuum approach) in Abaqus/Standard that include mechanical behavior (elements that have displacement degrees of freedom). Additional references • Darveaux, R., “Effect of Simulation Methodology on Solder Joint Crack Growth Correlation and Fatigue Life Prediction,” Journal of Electronic Packaging, vol. 124, pp. 147–154, 2002. • Lau, J., S. Pan, and C. Chang, “A New Thermal-Fatigue Life Prediction Model for Wafer Level Chip Scale Package (WLCSP) Solder Joints,” Journal of Electronic Packaging, vol. 124, pp. 212–220, 2002. 24.4.2 DAMAGE INITIATION FOR DUCTILE MATERIALS IN LOW-CYCLE FATIGUE Product: Abaqus/Standard References • “Progressive damage and failure,” Section 24.1.1 • *DAMAGE INITIATION Overview The material damage initiation capability for ductile materials based on inelastic hysteresis energy: • is intended as a general capability for predicting initiation of damage in ductile materials in a low- cycle fatigue analysis; • can be used in combination with the damage evolution law for ductile materials described in “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3; and • can be used only in a low-cycle fatigue analysis using the direct cyclic approach (“Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7). Damage initiation criteria for ductile materials The damage initiation criterion is a phenomenological model for predicting the onset of damage due to stress reversals and the accumulation of inelastic strain in a low-cycle fatigue analysis. It is characterized by the accumulated inelastic hysteresis energy per cycle, , in a material point when the structure response is stabilized in the cycle. The cycle number in which damage is initiated is given by where are working; some care is required to modify when converting to a different system of units. are material constants. The value of is dependent on the system of units in which you and The initiation criterion can be used in conjunction with any ductile material. Input File Usage: *DAMAGE INITIATION, CRITERION=HYSTERESIS ENERGY Elements The damage initiation criteria for ductile materials can be used with any elements in Abaqus/Standard that include mechanical behavior (elements that have displacement degrees of freedom). This includes cohesive elements based on a continuum approach (“Modeling of an adhesive layer of finite thickness” in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5). Output In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variable has special meaning when a damage initiation criterion is specified: CYCLEINI Number of cycles to initialize the damage at the material point. 24.4.3 DAMAGE EVOLUTION FOR DUCTILE MATERIALS IN LOW-CYCLE FATIGUE Product: Abaqus/Standard References • “Progressive damage and failure,” Section 24.1.1 • *DAMAGE EVOLUTION Overview The damage evolution capability for ductile materials based on inelastic hysteresis energy: • assumes that damage is characterized by the progressive degradation of the material stiffness, leading to material failure; • must be used in combination with a damage initiation criterion for ductile materials in low-cycle fatigue analysis (“Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2); • uses the inelastic hysteresis energy per stabilized cycle to drive the evolution of damage after damage initiation; and • must be used in conjunction with the linear elastic material model (“Linear elastic behavior,” the porous elastic material model (“Elastic behavior of porous materials,” Section 22.2.1), Section 22.3.1), or the hypoelastic material model (“Hypoelastic behavior,” Section 22.4.1). Damage evolution based on accumulated inelastic hysteresis energy Once the damage initiation criterion (“Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2) is satisfied at a material point, the damage state is calculated and updated based on the inelastic hysteresis energy for the stabilized cycle. The rate of the damage in a material point per cycle is given by are material constants, and and where point. The value of required to modify when converting to a different system of units. is the characteristic length associated with an integration is dependent on the system of units in which you are working; some care is For damage in ductile materials Abaqus/Standard assumes that the degradation of the elastic . At any given loading cycle during the stiffness can be modeled using the scalar damage variable, analysis the stress tensor in the material is given by the scalar damage equation where is the effective (or undamaged) stress tensor that would exist in the material in the absence of damage computed in the current increment. The material has completely lost its load carrying capacity when . You can remove the element from the mesh if all of the section points at all integration locations have lost their loading carrying capability. Input File Usage: *DAMAGE EVOLUTION, TYPE=HYSTERESIS ENERGY Mesh dependency and characteristic length The implementation of the damage evolution model requires the definition of a characteristic length associated with an integration point. The characteristic length is based on the element geometry and formulation: it is a typical length of a line across an element for a first-order element; it is half of the same typical length for a second-order element. For beams and trusses it is a characteristic length along the element axis. For membranes and shells it is a characteristic length in the reference surface. For axisymmetric elements it is a characteristic length in the r–z plane only. For cohesive elements it is equal to the constitutive thickness. This definition of the characteristic length is used because the direction in which fracture occurs is not known in advance. Therefore, elements with large aspect ratios will have rather different behavior depending on the direction in which the damage occurs: some mesh sensitivity remains because of this effect, and elements that are as close to square as possible are recommended. However, since the damage evolution law is energy based, mesh dependency of the results may be alleviated. Maximum degradation and element removal You can control how Abaqus/Standard treats elements with severe damage. Defining the upper bound to the damage variable . You can reduce By default, the upper bound to all damage variables at a material point is this upper bound as discussed in “Controlling element deletion and maximum degradation for materials with damage evolution” in “Section controls,” Section 27.1.4. Input File Usage: *SECTION CONTROLS, MAX DEGRADATION= Controlling element removal for damaged elements By default, in Abaqus/Standard an element is removed (deleted) once D reaches at all of the section points at all integration locations in the element. If an element is removed, the output variable STATUS is set to zero for the element, and it offers no resistance to subsequent deformation. However, the element still remains in the Abaqus/Standard model and may be visible during postprocessing. In the Visualization module of Abaqus/CAE, you can suppress the display of elements based on their status . Alternatively, you can specify that an element should remain in the model even after all of the . In this case, once all the damage variables reach the maximum value, the damage variables reach stiffness remains constant. Input File Usage: Use the following option to delete failed elements from the mesh (default): *SECTION CONTROLS, ELEMENT DELETION=YES Use the following option to keep failed elements in the mesh computations: *SECTION CONTROLS, ELEMENT DELETION=NO Difficulties associated with element removal in Abaqus/Standard When elements are removed from the model, their nodes remain in the model even if they are not attached to any active elements. When the solution progresses, these nodes might undergo non-physical displacements in Abaqus/Standard. In addition, applying a point load to a node that is not attached to an active element will cause convergence difficulties since there is no stiffness to resist the load. It is the responsibility of the user to prevent such situations. Elements Damage evolution for ductile materials can be defined for any element that can be used with the damage initiation criteria for a low-cycle fatigue analysis in Abaqus/Standard (“Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2). Output In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output the following variables have special meaning when damage variable identifiers,” Section 4.2.1), evolution is specified: STATUS SDEG Status of element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). Overall scalar stiffness degradation, D. 25. Hydrodynamic Properties Overview Equations of state 25.1 25.1 Overview • “Hydrodynamic behavior: overview,” Section 25.1.1 25.1.1 HYDRODYNAMIC BEHAVIOR: OVERVIEW library in Abaqus/Explicit The material includes several equation of state models to describe the hydrodynamic behavior of materials. An equation of state is a constitutive equation that defines the pressure as a function of the density and the internal energy (“Equation of state,” Section 25.2.1). The following equations of state are supported in Abaqus/Explicit: • Mie-Grüneisen equation of state: The Mie-Grüneisen equation of state (“Mie-Grüneisen equations of state” in “Equation of state,” Section 25.2.1) is used to model materials at high pressure. It is linear in energy and assumes a linear relationship between the shock velocity and the particle velocity. • Tabulated equation of state: The tabulated equation of state (“Tabulated equation of state” in “Equation of state,” Section 25.2.1) is used to model the hydrodynamic response of materials that exhibit sharp transitions in the pressure-density relationship, such as those induced by phase transformations. It is linear in energy. • P – α equation of state: The equation of state (“P – α equation of state” in “Equation of state,” Section 25.2.1) is designed for modeling the compaction of ductile porous materials. The constitutive model captures the irreversible compaction behavior at low stresses and predicts the correct thermodynamic behavior at high pressures for the fully compacted solid material. It is used in combination with either the Mie-Grüneisen equation of state or the tabulated equation of state to describe the solid phase. • JWL high explosive equation of state: The Jones-Wilkens-Lee (or JWL) equation of state (“JWL high explosive equation of state” in “Equation of state,” Section 25.2.1) models the pressure generated by the release of chemical energy in an explosive. This model is implemented in a form referred to as a programmed burn, which means that the reaction and initiation of the explosive is not determined by shock in the material. Instead, the initiation time is determined by a geometric construction using the detonation wave speed and the distance of the material point from the detonation points. • Ideal gas equation of state: The ideal gas equation of state (“Ideal gas equation of state” in “Equation of state,” Section 25.2.1) is an idealization to real gas behavior and can be used to model any gases approximately under appropriate conditions (e.g., low pressure and high temperature). Deviatoric behavior The material modeled by an equation of state may have no deviatoric strength or may have either isotropic elastic or viscous (both Newtonian and non-Newtonian) deviatoric behavior (“Deviatoric behavior” in “Equation of state,” Section 25.2.1). The elastic model can be used by itself or in conjunction with the Mises, the Johnson-Cook, or the extended Drucker-Prager plasticity models to model hydrodynamic materials with elastic-plastic deviatoric behavior. Thermal strain Thermal expansion cannot be introduced for any of the equation of state models. 25.2 Equations of state • “Equation of state,” Section 25.2.1 25.2.1 EQUATION OF STATE Products: Abaqus/Explicit Abaqus/CAE References • “Hydrodynamic behavior: overview,” Section 25.1.1 • “Material library: overview,” Section 21.1.1 • *EOS • *EOS COMPACTION • *ELASTIC • *VISCOSITY • *DETONATION POINT • *GAS SPECIFIC HEAT • *REACTION RATE • *TENSILE FAILURE • “Defining equations of state” in “Defining other mechanical models,” Section 12.9.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Equations of state: • provide a hydrodynamic material model in which the material’s volumetric strength is determined by an equation of state; • determine the pressure (positive in compression) as a function of the density, energy (the internal energy per unit mass), : ; • are available as Mie-Grüneisen equations of state (thus providing the linear • are available as tabulated equations of state linear in energy; • are available as equations of state for the compaction of ductile porous materials and must be used in conjunction with either the Mie-Grüneisen or the tabulated equation of state for the solid phase; , and the specific Hugoniot form); • are available as JWL high explosive equations of state; • are available as ignition and growth equations of state; • are available in the form of an ideal gas; • assume an adiabatic condition unless a dynamic fully coupled temperature-displacement analysis is used; • can be used to model a material that has only volumetric strength (the material is assumed to have no shear strength) or a material that also has isotropic elastic or viscous deviatoric behavior; • can be used with the Mises (“Classical metal plasticity,” Section 23.2.1) or the Johnson-Cook (“Johnson-Cook plasticity,” Section 23.2.7) plasticity models; • can be used with the extended Drucker-Prager (“Extended Drucker-Prager models,” Section 23.3.1) plasticity models (without plastic dilation); and • can be used with the tensile failure model (“Dynamic failure models,” Section 23.2.8) to model dynamic spall or a pressure cutoff. Energy equation and Hugoniot curve , to the The equation for conservation of energy equates the increase in internal energy per unit mass, rate at which work is being done by the stresses and the rate at which heat is being added. In the absence of heat conduction the energy equation can be written as where p is the pressure stress defined as positive in compression, viscosity, unit mass. is the deviatoric stress tensor, is the deviatoric part of strain rate, and is the pressure stress due to the bulk is the heat rate per The equation of state is assumed for the pressure as a function of the current density, , and the internal energy per unit mass, : which defines all the equilibrium states that can exist in a material. The internal energy can be eliminated from the above equation to obtain a p versus V relationship (where V is the current volume) or, equivalently, a p versus relationship that is unique to the material described by the equation of state model. This unique relationship is called the Hugoniot curve and is the locus of p–V states achievable behind a shock . pH pH|1 pH|0 Figure 25.2.1–1 A schematic representation of a Hugoniot curve. The Hugoniot pressure, experimental data. , is a function of density only and can be defined, in general, from fitting An equation of state is said to be linear in energy when it can be written in the form where and are functions of density only and depend on the particular equation of state model. Mie-Grüneisen equations of state A Mie-Grüneisen equation of state is linear in energy. The most common form is where density only, and and are the Hugoniot pressure and specific energy (per unit mass) and are functions of is the Grüneisen ratio defined as where is a material constant and The Hugoniot energy, is the reference density. , is related to the Hugoniot pressure by where above equations yields is the nominal volumetric compressive strain. Elimination of and from the The equation of state and the energy equation represent coupled equations for pressure and internal energy. Abaqus/Explicit solves these equations simultaneously at each material point. Linear Us − Up Hugoniot form A common fit to the Hugoniot data is given by where velocity, and s define the linear relationship between the linear shock velocity, , and the particle , as follows: With the above assumptions the linear Hugoniot form is written as where is equivalent to the elastic bulk modulus at small nominal strains. There is a limiting compression given by the denominator of this form of the equation of state or At this limit there is a tensile minimum; thereafter, negative sound speeds are calculated for the material. Input File Usage: Abaqus/CAE Usage: Initial state Use both of the following options: *DENSITY (to specify the reference density *EOS, TYPE=USUP (to specify the variables Property module: material editor: General→Density (to specify the reference density Mechanical→Eos: Type: Us - Up (to specify the variables , s, and ) ) ) , s, and ) , and pressure The initial state of the material is determined by the initial values of specific energy, stress, p. Abaqus/Explicit will automatically compute the initial density, , that satisfies the equation of state, . You can define the initial specific energy and initial stress state . The initial pressure used by the equation of state is inferred from the specified stress states. If no initial conditions are specified, Abaqus/Explicit will assume that the material is at its reference state: Input File Usage: Abaqus/CAE Usage: Use either or both of the following options, as required: *INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY *INITIAL CONDITIONS, TYPE=STRESS Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step Initial specific energy is not supported in Abaqus/CAE. Tabulated equation of state The tabulated equation of state provides flexibility in modeling the hydrodynamic response of materials that exhibit sharp transitions in the pressure-density relationship, such as those induced by phase transformations. The tabulated equation of state is linear in energy and assumes the form where and are functions of the logarithmic volumetric strain only, with , and is the reference density. You can specify the functions directly in tabular form. The tabular entries must be given in descending values of the volumetric strain (that is, from the most tensile to the most compressive states). Abaqus/Explicit will use a piecewise linear relationship between data points. Outside the range of specified values of volumetric strains, the functions are extrapolated based on the last slope computed from the data. and Input File Usage: Use both of the following options: *DENSITY (to specify the reference density *EOS, TYPE=TABULAR (to specify and The tabulated equation of state is not supported in Abaqus/CAE. as functions of ) ) Abaqus/CAE Usage: Initial state , and pressure The initial state of the material is determined by the initial values of specific energy, stress, p. Abaqus/Explicit automatically computes the initial density, , that satisfies the equation of state. You can define the initial specific energy and initial stress state . The initial pressure used by the equation of state is inferred from the specified stress states. If no initial conditions are specified, Abaqus/Explicit assumes that the material is at its reference state: Input File Usage: Use either or both of the following options, as required: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY *INITIAL CONDITIONS, TYPE=STRESS Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step Initial specific energy is not supported in Abaqus/CAE. P – α equation of state The equation of state is designed for modeling the compaction of ductile porous materials. The implementation in Abaqus/Explicit is based on the model proposed by Hermann (1968) and Carroll and Holt (1972). The constitutive model provides a detailed description of the irreversible compaction behavior at low stresses and predicts the correct thermodynamic behavior at high pressures for the fully compacted solid material. In Abaqus/Explicit the solid phase is assumed to be governed by either the Mie-Grüneisen equation of state or the tabulated equation of state. The relevant properties of the porous material in the virgin state, to be discussed later, and the material properties of the solid phase are specified separately. The porosity of the material, n, is defined as the ratio of pore volume, , to total volume, , where is the solid volume. The porosity remains in the range , with 0 indicating full compaction. It is convenient to introduce a scalar variable , sometimes referred to as “distension,” defined as the ratio of the density of the solid material, , both evaluated at the same temperature and pressure: , to the density of the porous material, For a fully compacted material pores is negligible compared to that of the solid phase, ; otherwise, is greater than 1. Assuming that the density of the can be expressed in terms of the porosity n as An equation of state is assumed for the pressure of the porous material as a function of ; current density, ; and internal energy per unit mass, , in the form Assuming that the pores carry no pressure, it follows from equilibrium considerations that when a pressure p is applied to the porous material, it gives rise to a volume-average pressure in the solid phase equal to . Assuming that the specific internal energies of the porous material and the solid matrix are the same (i.e., neglecting the surface energy of the pores), the equation of state of the porous material can be expressed as where is, when correct thermodynamic behavior at high pressures. is the equation of state of the solid material. For the fully compacted material (that equation of state reduces to that of the solid phase, therefore predicting the ), the The equation of state must be supplemented by an equation that describes the behavior of as a function of the thermodynamic state. This equation takes the form is a state variable corresponding to the minimum value attained by where (irreversible) compaction of the material. The state variable is initialized to the elastic limit material that is at its virgin state. The specific form of the function is illustrated in Figure 25.2.1–2 and is discussed next. during plastic for a used by Abaqus/Explicit α 0 α e α min α min A el (p, α )e A el (p, α )min A el (p, α )min A pl (p) pe p S Figure 25.2.1–2 elastic and plastic curves for the description of compaction of ductile porous materials. The function captures the general behavior to be expected in a ductile porous material. The unloaded virgin state corresponds to the value is the reference porosity of the material. Initial compression of the porous material is assumed to be elastic. Recall that decreasing porosity corresponds to a reduction in . As the pressure increases beyond the elastic limit, , the pores in the material start to crush, leading to irreversible compaction and permanent (plastic) volume change. Unloading from a partially compacted state follows a new elastic curve that depends on the maximum compaction (or, alternatively, the minimum value of ) ever attained during the deformation history of the material. The absolute value of the slope of the elastic curve decreases as decreases, as will be quantified later. The material becomes fully compacted when the pressure reaches the compaction pressure , a value that is retained forever. The function ; at that point , where therefore has multiple branches: a plastic branch, , corresponding to elastic unloading from partially compacted states. The appropriate branch of A is selected according to the following rule: , and multiple elastic branches, These expressions can be inverted to solve for p: The equation for the plastic curve takes the form or, alternatively, The elastic curve originally proposed by Hermann (1968) is given by the differential equation where the reference density of the solid; and (porous) materials, respectively. is the elastic bulk modulus of the solid material at small nominal strains; is are the reference sound speeds in the solid and virgin and the reference sound speed, equation of state, If the solid phase is modeled using the Mie-Grüneisen equation of state, is given directly by . On the other hand, if the solid phase is modeled using the tabulated is computed from the initial bulk modulus and reference density of the solid material, . In this case the reference density is required to be constant; it cannot be a function of temperature or field variables. Following Wardlaw et al. (1996), the above equation for the elastic curve in Abaqus/Explicit is simplified and replaced by the linear relations and Input File Usage: Use the following option to specify the reference density of the solid phase, : *DENSITY Use one of the following two options to specify additional material properties for the solid phase: *EOS, TYPE=USUP (if the solid phase is modeled using the Mie-Grüneisen equation of state) *EOS, TYPE=TABULAR (if the solid phase is modeled using the tabulated equation of state) Use the following option to specify the properties of the porous material (the reference sound speed, ; and the compaction pressure, ; the reference porosity, ; the elastic limit, ): Abaqus/CAE Usage: *EOS COMPACTION Only the Mie-Grüneisen equation of state is supported for the solid phase in Abaqus/CAE. Property module: material editor: General→Density (to specify the reference density Mechanical→Eos: Type: Us - Up (to specify the variables Mechanical→Eos: Suboptions→ Eos Compaction (to specify the reference sound speed, ; the porosity of the unloaded material, ) , s, and ) ; the pressure required to initialize plastic behavior, ; and the pressure at which all pores are crushed, ) Initial state , that satisfies the equation of state, The initial state of the porous material is determined from the initial values of porosity, specific energy, ; ; and pressure stress, p. Abaqus/Explicit automatically computes the initial density, . You can define the initial porosity, initial specific energy, and initial stress state . If no initial conditions are given, Abaqus/Explicit assumes that the material is at its virgin state: Abaqus/Explicit will issue an error message if the initial states . When initial conditions are specified only for p (or for will compute (or p) assuming that the state lies on the primary (monotonic loading) curve. state lies outside the region of allowed ), Abaqus/Explicit Input File Usage: Use some or all of the following options, as required: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY *INITIAL CONDITIONS, TYPE=STRESS *INITIAL CONDITIONS, TYPE=POROSITY Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step Initial specific energy and initial porosity are not supported in Abaqus/CAE. JWL high explosive equation of state The Jones-Wilkens-Lee (or JWL) equation of state models the pressure generated by the release of chemical energy in an explosive. This model is implemented in a form referred to as a programmed burn, which means that the reaction and initiation of the explosive is not determined by shock in the material. Instead, the initiation time is determined by a geometric construction using the detonation wave speed and the distance of the material point from the detonation points. The JWL equation of state can be written in terms of the internal energy per unit mass, , as where explosive; and and are user-defined material constants; is the user-defined density of the is the density of the detonation products. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *DENSITY (to specify the density of the explosive *EOS, TYPE=JWL (to specify the material constants Property module: material editor: General→Density (to specify the density of the explosive Mechanical→Eos: Type: JWL (to specify the material constants ) ) and ) and ) Arrival time of detonation wave Abaqus/Explicit calculates the arrival time of the detonation wave at a material point from the material point to the nearest detonation point divided by the detonation wave speed: as the distance is the position of the material point, is the where detonation delay time of the Nth detonation point, and is the detonation wave speed of the explosive material. The minimum in the above formula is over the N detonation points that apply to the material point. is the position of the Nth detonation point, To spread the burn wave over several elements, a burn fraction, , is computed as EOS is a constant that controls the width of the burn wave (set to a value of 2.5) and where characteristic length of the element. If the time is less than otherwise, the pressure is given by the product of above. is the , the pressure is zero in the explosive; and the pressure determined from the JWL equation Defining detonation points You can define any number of detonation points for the explosive material. Coordinates of the points must be defined along with a detonation delay time. Each material point responds to the first detonation point that it sees. The detonation arrival time at a material point is based upon the time that it takes a detonation wave (traveling at the detonation wave speed ) to reach the material point plus the detonation delay time for the detonation point. If there are multiple detonation points, the arrival time is based on the minimum arrival time for all the detonation points. In a body with curved surfaces care should be taken that the detonation arrival times are meaningful. The detonation arrival times are based on the straight line of sight from the material point to the detonation point. In a curved body the line of sight may pass outside of the body. Input File Usage: Use both of the following options to define the detonation points: *EOS, TYPE=JWL *DETONATION POINT Property module: material editor: Mechanical→Eos: Type: JWL: Suboptions→Detonation Point Abaqus/CAE Usage: Initial state Explosive materials generally have some nominal volumetric stiffness before detonation. It may be useful to incorporate this stiffness when elements modeled with a JWL equation of state are subjected to stress before initiation of detonation by the arriving detonation wave. You can define the pre-detonation bulk modulus, until detonation, at which time the pressure will be determined by the procedure outlined above. The initial relative density ( is assumed to be equal to the user-defined detonation energy ) used in the JWL equation is assumed to be unity. The initial specific energy . The pressure will be computed from the volumetric strain and . If you specify a nonzero value of , you can also define an initial stress state for the explosive materials. Input File Usage: Use the following option to define the initial stress: *INITIAL CONDITIONS, TYPE=STRESS Abaqus/CAE Usage: Optionally, you can also define the initial specific energy directly: *INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step Initial specific energy is not supported in Abaqus/CAE. Ignition and growth equation of state The ignition and growth equation of state models shock initiation and detonation wave propagation of solid high explosives. The heterogeneous explosive is modeled as a homogeneous mixture of two phases: the unreacted solid explosive and the reacted gas products. Separate JWL equations of state are prescribed for each phase: where and The subscript s refers to the unreacted solid explosive, and g refers to the reacted gas products. is the is the density of the are user-defined material constants used in the JWL equations; is the user-defined reference density of the explosive, and and detonation energy; unreacted explosive or the reacted products. Use both of the following options: *DENSITY(to specify the density of the explosive *EOS, TYPE=IGNITION AND GROWTH, DETONATION ENERGY= (to specify the material constants of the unreacted solid explosive and the reacted gas product) and ) Property module: material editor: General→Density (to specify the density of the explosive Mechanical→Eos: Type: Ignition and growth: Detonation energy: Solid Phase tabbed page and Gas Phase tabbed page (to specify the material constants of the unreacted solid explosive and the reacted gas product) and ) ; 25.2.1–12 Input File Usage: The mass fraction The mixture of unreacted solid explosive and reacted gas products is defined by the mass fraction where is the mass of the unreacted explosive, and assumed that the two phases are in thermo-mechanical equilibrium: is the mass of the reacted products. It is It is also assumed that the volumes are additive: Similarly, the internal energy is assumed to be additive: where Hence, the specific heat of the mixture is given by Input File Usage: Abaqus/CAE Usage: Use the following options to define the specific heat of the unreacted solid explosive: *EOS, TYPE=IGNITION AND GROWTH *SPECIFIC HEAT, DEPENDENCIES=n Use the following options to define the specific heat of the reacted gas product: *EOS, TYPE=IGNITION AND GROWTH *GAS SPECIFIC HEAT, DEPENDENCIES=n Use the following options to define the specific heat of the unreacted solid explosive: Property module: material editor: Mechanical→Eos: Type: Ignition and GrowthThermal→Specific Heat Use the following options to define the specific heat of the reacted gas product: Property module: material editor: Mechanical→Eos: Type: Ignition and growth: Gas Specific tabbed page: Specific Heat You can toggle on Use temperature-dependent data to define the specific heat as a function of temperature and/or select the Number of field variables to define the specific heat as a function of field variables. The reaction rate The conversion of unreacted solid explosive to reacted gas products is governed by the reaction rate. The reaction rate equation in the ignition and growth model is a pressure-driven rule, which includes three terms: These three terms are defined as follows: where , and z are reaction rate constants. The first term, , describes hot spot ignition by igniting some of the material relatively quickly , represents the growth but limiting it to a small proportion of the total solid of reaction from the hot spot sites into the material and describes the inward and outward grain burning phenomena; this term is limited to a proportion of the total solid , is used to describe the rapid transition to detonation observed in some energetic materials. . The second term, . The third term, Input File Usage: Use both of the following options to define the reaction rate: Abaqus/CAE Usage: *EOS, TYPE=IGNITION AND GROWTH *REACTION RATE Property module: material editor: Mechanical→Eos: Type: Ignition and growth: Reaction Rate tabbed page Initial state The initial mass fraction of the unreacted solid explosive is assumed to be one. The initial relative density ( ) used in the ignition and growth equation is assumed to be unity. The initial specific energy and initial stress can be defined for the unreacted explosive. Input File Usage: Abaqus/CAE Usage: Use the following option to define the initial stress: *INITIAL CONDITIONS, TYPE=STRESS Optionally, you can also define the initial specific energy directly: *INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step Initial specific energy is not supported in Abaqus/CAE. Ideal gas equation of state An ideal gas equation of state can be written in the form of is the ambient pressure, R is the gas constant, where is the absolute zero on the temperature scale being used. It is an idealization to real gas behavior and can be used to model any gases approximately under appropriate conditions (e.g., low pressure and high temperature). is the current temperature, and One of the important features of an ideal gas is that its specific energy depends only upon its temperature; therefore, the specific energy can be integrated numerically as is the initial specific energy at the initial temperature is the specific heat at constant where volume (or the constant volume heat capacity), which depends only upon temperature for an ideal gas. Modeling with an ideal gas equation of state is typically performed adiabatically; the temperature increase is calculated directly at the material integration points according to the adiabatic thermal energy increase caused by the work ). Therefore, unless a fully coupled temperature-displacement analysis is performed, an adiabatic condition is always assumed in Abaqus/Explicit. , where v is the specific volume (the volume per unit mass, and When performing a fully coupled temperature-displacement analysis, the pressure stress and specific energy are updated based on the evolving temperature field. The energy increase due to the change in state will be accounted for in the heat equation and will be subject to heat conduction. For the ideal gas model in Abaqus/Explicit you define the gas constant, R, and the ambient pressure, , and the molecular weight, . For an ideal gas R can be determined from the universal gas constant, , as follows: In general, the value R for any gas can be estimated by plotting as a function of state (e.g., pressure or temperature). The ideal gas approximation is adequate in any region where this value is constant. You must specify the specific heat at constant volume, is related to the specific heat at constant pressure, . For an ideal gas , by Input File Usage: Use both of the following options: *EOS, TYPE=IDEAL GAS *SPECIFIC HEAT, DEPENDENCIES=n Property module: material editor: Mechanical→Eos: Type: Ideal Gas Thermal→Specific Heat Abaqus/CAE Usage: Initial state , There are different methods to define the initial state of the gas. You can specify the initial density, and either the initial pressure stress, . The initial value of the unspecified , or the initial temperature, field (temperature or pressure) is determined from the equation of state. Alternatively, you can specify both the initial pressure stress and the initial temperature. In this case the user-specified initial density is replaced by that derived from the equation of state in terms of initial pressure and temperature. By default, Abaqus/Explicit automatically computes the initial specific energy, , from the initial temperature by numerically integrating the equation Optionally, you can override this default behavior by defining the initial specific energy for the ideal gas directly. Input File Usage: Use some or all of the following options, as required: *DENSITY, DEPENDENCIES=n *INITIAL CONDITIONS, TYPE=STRESS *INITIAL CONDITIONS, TYPE=TEMPERATURE Use the following option to specify the initial specific energy directly: *INITIAL CONDITIONS, TYPE=SPECIFIC ENERGY Abaqus/CAE Usage: Property module: material editor: General→Density Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step Initial specific energy is not supported in Abaqus/CAE. The value of absolute zero Input File Usage: When a non-absolute temperature scale is used, you must specify the value of absolute zero temperature. *PHYSICAL CONSTANTS, ABSOLUTE ZERO= Any module: Model→Edit Attributes→model_name: Absolute zero temperature Abaqus/CAE Usage: A special case In the case of an adiabatic analysis with constant specific heat (both energy is linear in temperature and are constant), the specific The pressure stress can, therefore, be recast in the common form of where is the ratio of specific heats and can be defined as where for a monatomic; for a diatomic; and for a polyatomic gas. Comparison with the hydrostatic fluid model The ideal gas equation of state can be used to model wave propagation effects and the dynamics of a spatially varying state of a gaseous region. For cases in which the inertial effects of the gas are not important and the state of the gas can be assumed to be uniform throughout a region, the hydrostatic fluid model (“Surface-based fluid cavities: overview,” Section 11.5.1) is a simpler, more computationally efficient alternative. Deviatoric behavior The equation of state defines only the material’s hydrostatic behavior. It can be used by itself, in which case the material has only volumetric strength (the material is assumed to have no shear strength). Alternatively, Abaqus/Explicit allows you to define deviatoric behavior, assuming that the deviatoric and volumetric responses are uncoupled. Two models are available for the deviatoric response: a linear isotropic elastic model and a viscous model. The material’s volumetric response is governed then by the equation of state model, while its deviatoric response is governed by either the linear isotropic elastic model or the viscous fluid model. Elastic shear behavior For the elastic shear behavior the deviatoric stress is related to the deviatoric strain as is the deviatoric stress and is the deviatoric elastic strain. See “Defining isotropic shear where elasticity for equations of state in Abaqus/Explicit” in “Linear elastic behavior,” Section 22.2.1, for more details. Input File Usage: Use both of the following options to define elastic shear behavior: *EOS *ELASTIC, TYPE=SHEAR Property module: material editor: Mechanical→Elasticity→Elastic; Type: Shear; Shear Modulus Abaqus/CAE Usage: Viscous shear behavior For the viscous shear behavior the deviatoric stress is related to the deviatoric strain rate as where is the engineering shear strain rate. is the deviatoric stress, is the deviatoric part of the strain rate, is the viscosity, and Abaqus/Explicit provides a wide range of viscosity models to describe both Newtonian and non- Newtonian fluids. These are described in “Viscosity,” Section 26.1.4. Input File Usage: Use both of the following options to define viscous shear behavior: Abaqus/CAE Usage: *EOS *VISCOSITY Property module: material editor: Mechanical→Viscosity Use with the Mises or the Johnson-Cook plasticity models An equation of state model can be used with the Mises (“Classical metal plasticity,” Section 23.2.1) or the Johnson-Cook (“Johnson-Cook plasticity,” Section 23.2.7) plasticity models to model elastic-plastic behavior. In this case you must define the elastic part of the shear behavior. The material’s volumetric response is governed by the equation of state model, while the deviatoric response is governed by the linear elastic shear and the plasticity model. Input File Usage: Use the following options: *EOS *ELASTIC, TYPE=SHEAR *PLASTIC Property module: material editor: Mechanical→Elasticity→Elastic; Type: Shear Mechanical→Plasticity→Plastic Abaqus/CAE Usage: Initial conditions You can specify initial conditions for the equivalent plastic strain, Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). (“Initial conditions in Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step Use with the extended Drucker-Prager plasticity models An equation of state model can be used in conjunction with the extended Drucker-Prager (“Extended Drucker-Prager models,” Section 23.3.1) plasticity models to model pressure-dependent plasticity behavior. This approach can be appropriate for modeling the response of ceramics and other brittle materials under high velocity impact conditions. In this case you must define the elastic part of the shear behavior. The material’s deviatoric response is governed by the linear elastic shear and the pressure-dependent plasticity model, while the volumetric response is governed by the equation of state model. In particular, no plastic dilation effects are taken into account (if you specify a dilation angle other than zero, the value is ignored and Abaqus/Explicit issues a warning message). “High-velocity impact of a ceramic target,” Section 2.1.18 of the Abaqus Example Problems Manual illustrates the use of an equation of state model with the extended Drucker-Prager plasticity models. Input File Usage: Use the following options: *EOS *ELASTIC, TYPE=SHEAR *DRUCKER PRAGER *DRUCKER PRAGER HARDENING Property module: material editor: Abaqus/CAE Usage: Initial conditions Mechanical→Elasticity→Elastic; Type: Shear Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker Prager Hardening You can specify initial conditions for the equivalent plastic strain, Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). (“Initial conditions in Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=HARDENING Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step Use with the tensile failure model An equation of state model (except the ideal gas equation of state) can also be used with the tensile failure model (“Dynamic failure models,” Section 23.2.8) to model dynamic spall or a pressure cutoff. The tensile failure model uses the hydrostatic pressure stress as a failure measure and offers a number of failure choices. You must provide the hydrostatic cutoff stress. You can specify that the deviatoric stresses should fail when the tensile failure criterion is met. In the case where the material’s deviatoric behavior is not defined, this specification is meaningless and is, therefore, ignored. The tensile failure model in Abaqus/Explicit is designed for high-strain-rate dynamic problems in which inertia effects are important. Therefore, it should be used only for such situations. Improper use of the tensile failure model may result in an incorrect simulation. Input File Usage: Abaqus/CAE Usage: Adiabatic assumption Use the following options: *EOS *TENSILE FAILURE The tensile failure model is not supported in Abaqus/CAE. An adiabatic condition is always assumed for materials modeled with an equation of state unless a dynamic coupled temperature-displacement procedure is used. The adiabatic condition is assumed irrespective of whether an adiabatic dynamic stress analysis step has been specified. The temperature increase is calculated directly at the material integration points according to the adiabatic thermal energy increase caused by the mechanical work where effect on the behavior of this model. is the specific heat at constant volume. Specifying temperature as a predefined field has no When performing a fully coupled temperature-displacement analysis, the specific energy is updated based on the evolving temperature field using Modeling fluids equation of state model can be used to model incompressible viscous and inviscid A linear laminar flow governed by the Navier-Stokes equation of motion. The volumetric response is governed by the equations of state, where the bulk modulus acts as a penalty parameter for the incompressible constraint. To model a viscous laminar flow that follows the Navier-Poisson law of a Newtonian fluid, use the Newtonian viscous deviatoric model and define the viscosity as the real linear viscosity of the fluid. To model non-Newtonian viscous flow, use one of the nonlinear viscosity models available in Abaqus/Explicit. Appropriate initial conditions for velocity and stress are essential to get an accurate solution for this class of problems. To model an incompressible inviscid fluid such as water in Abaqus/Explicit, it is useful to define a small amount of shear resistance to suppress shear modes that can otherwise tangle the mesh. Here the shear stiffness or shear viscosity acts as a penalty parameter. The shear modulus or viscosity should be small because flow is inviscid; a high shear modulus or viscosity will result in an overly stiff response. To avoid an overly stiff response, the internal forces arising due to the deviatoric response of the material should be kept several orders of magnitude below the forces arising due to the volumetric response. This can be done by choosing an elastic shear modulus that is several orders of magnitude lower than the bulk modulus. If the viscous model is used, the shear viscosity specified should be on the order of the shear modulus, calculated as above, scaled by the stable time increment. The expected stable time increment can be obtained from a data check analysis of the model. This method is a convenient way to approximate a shear resistance that will not introduce excessive viscosity in the material. If a shear model is defined, the hourglass control forces are calculated based on the shear resistance of the material. Thus, in materials with extremely low or zero shear strengths such as inviscid fluids, the hourglass forces calculated based on the default parameters are insufficient to prevent spurious hourglass modes. Therefore, a sufficiently high hourglass scaling factor is recommended to increase the resistance to such modes. Elements Equations of state can be used with any solid (continuum) elements in Abaqus/Explicit except plane stress elements. For three-dimensional applications exhibiting high confinement, the default kinematic formulation is recommended with reduced-integration solid elements . Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for the equation of state models: PALPH , of the Distension, minus the inverse of : porous material. The current porosity is equal to one PALPHMIN Minimum value, , of the distension attained during plastic compaction of the porous material. PEEQ Equivalent plastic strain, is the initial equivalent plastic strain (zero or user-specified; see “Initial conditions”). This is relevant only if the equation of state model is used in combination with the Mises, Johnson-Cook, or extended Drucker-Prage plasticity models. where Additional references • Carroll, M., and A. C. Holt, “Suggested Modification of the Journal of Applied Physics, vol. 43, no. 2, pp. 759–761, 1972. Model for Porous Materials,” • Dobratz, B. M., “LLNL Explosives Handbook, Properties of Chemical Explosives and Explosive Simulants,” UCRL-52997, Lawrence Livermore National Laboratory, Livermore, California, January 1981. • Herrmann, W., “Constitutive Equation for the Dynamic Compaction of Ductile Porous Materials,” Journal of Applied Physics, vol. 40, no. 6, pp. 2490–2499, 1968. • Lee, E., M. Finger, and W. Collins, “JWL Equation of State Coefficients for High Explosives,” UCID-16189, Lawrence Livermore National Laboratory, Livermore, California, January 1973. • Wardlaw, A. B., R. McKeown, and H. Chen, “Implementation and Application of the Equation of State in the DYSMAS Code,” Naval Surface Warfare Center, Dahlgren Division, Report Number: NSWCDD/TR-95/107, May 1996. Other Material Properties Mechanical properties Heat transfer properties Acoustic properties Mass diffusion properties Electromagnetic properties Pore fluid flow properties User materials OTHER MATERIAL PROPERTIES 26.1 26.2 26.3 26.4 26.5 26.6 26.1 Mechanical properties • “Material damping,” Section 26.1.1 • “Thermal expansion,” Section 26.1.2 • “Field expansion,” Section 26.1.3 • “Viscosity,” Section 26.1.4 26.1.1 MATERIAL DAMPING Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Dynamic analysis procedures: overview,” Section 6.3.1 • “Material library: overview,” Section 21.1.1 • *DAMPING • “Defining damping” in “Defining other mechanical models,” Section 12.9.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Material damping can be defined: • for direct-integration (nonlinear, implicit or explicit), subspace-based direct-integration, direct-solution steady-state, and subspace-based steady-state dynamic analysis; or • for mode-based (linear) dynamic analysis in Abaqus/Standard. Rayleigh damping In direct-integration dynamic analysis you very often define energy dissipation mechanisms—dashpots, inelastic material behavior, etc.—as part of the basic model. In such cases there is usually no need to introduce additional damping: it is often unimportant compared to these other dissipative effects. However, some models do not have such dissipation sources (an example is a linear system with chattering contact, such as a pipeline in a seismic event). In such cases it is often desirable to introduce some general damping. Abaqus provides “Rayleigh” damping for this purpose. It provides a convenient abstraction to damp lower (mass-dependent) and higher (stiffness-dependent) frequency range behavior. Rayleigh damping can also be used in direct-solution steady-state dynamic analyses and subspace-based steady-state dynamic analyses to get quantitatively accurate results, especially near natural frequencies. for stiffness proportional damping. To define material Rayleigh damping, you specify two Rayleigh damping factors: for mass proportional damping and In general, damping is a material property specified as part of the material definition. For the cases of rotary inertia, point mass elements, and substructures, where there is no reference to a material definition, the damping can be defined in conjunction with the property references. Any mass proportional damping also applies to nonstructural features . For a given mode i the fraction of critical damping, , can be expressed in terms of the damping factors and as: where proportional Rayleigh damping, damping, , damps the higher frequencies. is the natural frequency at this mode. This equation implies that, generally speaking, the mass , damps the lower frequencies and the stiffness proportional Rayleigh Mass proportional damping factor introduces damping forces caused by the absolute velocities of the model and so simulates The the idea of the model moving through a viscous “ether” (a permeating, still fluid, so that any motion of any point in the model causes damping). This damping factor defines mass proportional damping, in the sense that it gives a damping contribution proportional to the mass matrix for an element. If the element contains more than one material in Abaqus/Standard, the volume average value of is used to multiply the element’s mass matrix to define the damping contribution from this term. If the element contains more than one material in Abaqus/Explicit, the mass average value of is used to multiply the element’s lumped mass matrix to define the damping contribution from this term. has units of (1/time). Input File Usage: Abaqus/CAE Usage: *DAMPING, ALPHA= Property module: material editor: Mechanical→Damping: Alpha: Defining variable mass proportional damping in Abaqus/Explicit In Abaqus/Explicit you can define Therefore, mass proportional damping can vary during an Abaqus/Explicit analysis. *DAMPING, ALPHA=TABULAR Input File Usage: as a tabular function of temperature and/or field variables. Stiffness proportional damping factor introduces damping proportional to the strain rate, which can be thought of as damping The associated with the material itself. defines damping proportional to the elastic material stiffness. Since the model may have quite general nonlinear response, the concept of “stiffness proportional damping” must be generalized, since it is possible for the tangent stiffness matrix to have negative eigenvalues (which would imply negative damping). To overcome this problem, is interpreted as defining viscous material damping in Abaqus, which creates an additional “damping stress,” , proportional to the total strain rate: is the strain rate. For hyperelastic (“Hyperelastic behavior of rubberlike materials,” where Section 22.5.1) and hyperfoam (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2) materials is defined as the elastic stiffness in the strain-free state. For all other linear elastic materials is the material’s current elastic in Abaqus/Standard and all other materials in Abaqus/Explicit, stiffness. will be calculated based on the current temperature during the analysis. This damping stress is added to the stress caused by the constitutive response at the integration point when the dynamic equilibrium equations are formed, but it is not included in the stress output. As a result, damping can be introduced for any nonlinear case and provides standard Rayleigh damping for linear cases; for a linear case stiffness proportional damping is exactly the same as defining a damping matrix equal to times the (elastic) material stiffness matrix. Other contributions to the stiffness matrix (e.g., hourglass, transverse shear, and drill stiffnesses) are not included when computing stiffness proportional damping. has units of (time). Input File Usage: Abaqus/CAE Usage: *DAMPING, BETA= Property module: material editor: Mechanical→Damping: Beta: Defining variable stiffness proportional damping in Abaqus/Explicit In Abaqus/Explicit you can define Therefore, stiffness proportional damping can vary during an Abaqus/Explicit analysis. *DAMPING, BETA=TABULAR Input File Usage: as a tabular function of temperature and/or field variables. Structural damping Structural damping assumes that the damping forces are proportional to the forces caused by stressing of the structure and are opposed to the velocity. Therefore, this form of damping can be used only when the displacement and velocity are exactly 90° out of phase. Structural damping is best suited for frequency domain dynamic procedures . The damping forces are then are the damping forces, where are the forces caused by stressing of the structure. The damping forces due to structural damping are intended to represent frictional effects (as distinct from viscous effects). Thus, structural damping is suggested for models involving materials that exhibit frictional behavior or where local frictional effects are present throughout the model, such as dry rubbing of joints in a multi-link structure. , s is the user-defined structural damping factor, and Structural damping can be added to the model as mechanical dampers such as connector damping or as a complex stiffness on spring elements. Structural damping can be used in steady-state dynamic procedures that allow for nondiagonal damping. Input File Usage: Abaqus/CAE Usage: Use the following option to define structural damping: *DAMPING, STRUCTURAL= Property module: material editor: Mechanical→Damping: Structural: Artificial damping in direct-integration dynamic analysis In Abaqus/Standard the operators used for implicit direct time integration introduce some artificial damping in addition to Rayleigh damping. Damping associated with the Hilber-Hughes-Taylor and hybrid operators is usually controlled by the Hilber-Hughes-Taylor parameter , which is not the same as the and parameters of the Hilber-Hughes-Taylor and hybrid operators also affect numerical damping. The parameter controlling the mass proportional part of Rayleigh damping. The , , and parameters are not available for the backward Euler operator. See “Implicit dynamic analysis using direct integration,” Section 6.3.2, for more information about this other form of damping. Artificial damping in explicit dynamic analysis In Abaqus/Explicit a Rayleigh damping is meant to reflect physical damping in the actual material. small amount of numerical damping is introduced by default in the form of bulk viscosity to control high frequency oscillations; see “Explicit dynamic analysis,” Section 6.3.3, for more information about this other form of damping. Effects of damping on the stable time increment in Abaqus/Explicit As the fraction of critical damping for the highest mode ( Abaqus/Explicit decreases according to the equation ) increases, the stable time increment for where (by substituting , the frequency of the highest mode, into the equation for given previously) These equations indicate a tendency for stiffness proportional damping to have a greater effect on the stable time increment than mass proportional damping. To illustrate the effect that damping has on the stable time increment, consider a cantilever in bending modeled with continuum elements. The lowest frequency is 1 rad/sec, while for the particular mesh chosen, the highest frequency is 1000 rad/sec. The lowest mode in this problem corresponds to the cantilever in bending, and the highest frequency is related to the dilation of a single element. With no damping the stable time increment is If we use stiffness proportional damping to create 1% of critical damping in the lowest mode, the damping factor is given by This corresponds to a critical damping factor in the highest mode of The stable time increment with damping is, thus, reduced by a factor of and becomes Thus, introducing 1% critical damping in the lowest mode reduces the stable time increment by a factor of twenty. However, if we use mass proportional damping to damp out the lowest mode with 1% of critical damping, the damping factor is given by which corresponds to a critical damping factor in the highest mode of The stable time increment with damping is reduced by a factor of which is almost negligible. This example demonstrates that it is generally preferable to damp out low frequency response with mass proportional damping rather than stiffness proportional damping. However, mass proportional damping can significantly affect rigid body motion, so large is often undesirable. To avoid a dramatic drop in the stable time increment, the stiffness proportional damping factor, , should be less than or of the same order of magnitude as the initial stable time increment without damping. With , the stable time increment is reduced by about 52%. Damping in modal superposition procedures Damping can be specified as part of the step definition for modal superposition procedures. “Damping in a linear dynamic analysis” in “Dynamic analysis procedures: overview,” Section 6.3.1, describes the availability of damping types, which depends on the procedure type and the architecture used to perform the analysis, and provides details on the following types of damping: • Viscous modal damping (Rayleigh damping and fraction of critical damping) • Structural modal damping • Composite modal damping Use with other material models The factor applies to all elements that use a linear elastic material definition (“Linear elastic behavior,” Section 22.2.1) and to Abaqus/Standard beam and shell elements that use general sections. In the latter case, if a nonlinear beam section definition is provided, the factor is multiplied by the slope of the force-strain (or moment-curvature) relationship at zero strain or curvature. In addition, the factor applies to all Abaqus/Explicit elements that use a hyperelastic material definition (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1), a hyperfoam material definition (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2), or general shell sections (“Using a general shell section to define the section behavior,” Section 29.6.6). In the case of a no tension elastic material the factor is not used in tension, while for a no compression elastic material the factor is not used in compression . In other words, these modified elasticity models exhibit damping only when they have stiffness. Elements factor is applied to all elements that have mass including point mass elements (discrete The DASHPOTA elements in each global direction, each with one node fixed, can also be used to introduce this type of damping). For point mass and rotary inertia elements mass proportional or composite modal damping are defined as part of the point mass or rotary inertia definitions (“Point masses,” Section 30.1.1, and “Rotary inertia,” Section 30.2.1). The factor is not available for spring elements: discrete dashpot elements should be used in parallel with spring elements instead. The factor is also not applied to the transverse shear terms in Abaqus/Standard beams and shells. In Abaqus/Standard composite modal damping cannot be used with or within substructures. Rayleigh damping can be introduced for substructures. When Rayleigh damping is used within a substructure, for the substructure. These are weighted averages, using the mass as the weighting factor for and the volume as the weighting factor for . These averaged damping values can be superseded by providing them directly in a second damping definition. See “Using substructures,” Section 10.1.1. are averaged over the substructure to define single values of and and 26.1.2 THERMAL EXPANSION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “UEXPAN,” Section 1.1.29 of the Abaqus User Subroutines Reference Manual • *EXPANSION • “Defining other mechanical models,” Section 12.9.4 of the Abaqus/CAE User’s Manual • “Defining a fluid-filled porous material,” Section 12.12.3 of the Abaqus/CAE User’s Manual Overview Thermal expansion effects: • can be defined by specifying thermal expansion coefficients so that Abaqus can compute thermal strains and, in Abaqus/CFD, buoyancy forces; • can be isotropic, orthotropic, or fully anisotropic; • are defined as total expansion from a reference temperature; • can be specified as a function of temperature and/or field variables; • can be defined with a distribution for solid continuum elements in Abaqus/Standard; and • in Abaqus/Standard can be specified directly in user subroutine UEXPAN (if the thermal strains are complicated functions of field variables and state variables). Defining thermal expansion coefficients Thermal expansion is a material property included in a material definition except when it refers to the expansion of a gasket whose material properties are not defined as part of a material definition. In that case expansion must be used in conjunction with the gasket behavior definition . In an Abaqus/Standard analysis a spatially varying thermal expansion can be defined for homogeneous solid continuum elements by using a distribution (“Distribution definition,” Section 2.8.1). The distribution must include default values for the thermal expansion. If a distribution is used, no dependencies on temperature and/or field variables for the thermal expansion can be defined. Input File Usage: Use the following options to define thermal expansion for most materials: *MATERIAL *EXPANSION Abaqus/CAE Usage: Use the following options to define thermal expansion for gaskets whose constitutive response is defined directly as gasket behavior: *GASKET BEHAVIOR *EXPANSION Use the following option in conjunction with other material behaviors, including gasket behavior, to include thermal expansion effects: Property module: material editor: Mechanical→Expansion Computation of thermal strains Abaqus requires thermal expansion coefficients, reference temperature, , as shown in Figure 26.1.2–1. , that define the total thermal expansion from a εth εth εth θ0 θ1 θ2 Figure 26.1.2–1 Definition of the thermal expansion coefficient. They generate thermal strains according to the formula where is the thermal expansion coefficient; is the current temperature; is the initial temperature; are the current values of the predefined field variables; are the initial values of the field variables; and is the reference temperature for the thermal expansion coefficient. The second term in the above equation represents the strain due to the difference between the initial . This term is necessary to enforce the assumption that , and the reference temperature, temperature, there is no initial thermal strain for cases in which the reference temperature does not equal the initial temperature. Defining the reference temperature If the coefficient of thermal expansion, the reference temperature, define . , is not needed. If , is not a function of temperature or field variables, the value of is a function of temperature or field variables, you can Input File Usage: Abaqus/CAE Usage: *EXPANSION, ZERO= Property module: material editor: Mechanical→Expansion: Reference temperature: Converting thermal expansion coefficients from differential form to total form Total thermal expansion coefficients are commonly available in tables of material properties. However, sometimes you are given thermal expansion data in differential form: that is, the tangent to the strain-temperature curve is provided . To convert to the total thermal expansion form required by Abaqus, this relationship must be integrated from a suitably chosen reference temperature, : For example, suppose between and ; etc. Then, is a series of constant values: between and ; between and ; The corresponding total expansion coefficients required by Abaqus are then obtained as Defining increments of thermal strain in user subroutine UEXPAN Increments of thermal strain can be specified in Abaqus/Standard user subroutine UEXPAN as functions of temperature and/or predefined field variables. User subroutine UEXPAN must be used if the thermal strain increments depend on state variables. Input File Usage: Abaqus/CAE Usage: *EXPANSION, USER Property module: material editor: Mechanical→Expansion: Use user subroutine UEXPAN Defining the initial temperature and field variable values If the coefficient of thermal expansion, temperature and initial field variable values, in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. , is a function of temperature or field variables, the initial , are given as described in “Initial conditions and Element removal and reactivation If an element has been removed and subsequently reactivated in Abaqus/Standard (“Element and contact pair removal and reactivation,” Section 11.2.1), in the equation for the thermal strains represent and temperature and field variable values as they were at the moment of reactivation. Defining directionally dependent thermal expansion Isotropic or orthotropic thermal expansion can be defined in Abaqus. thermal expansion can be defined in Abaqus/Standard. In addition, fully anisotropic Orthotropic and anisotropic thermal expansion can be used only with materials where the material directions are defined with local orientations . Orthotropic thermal expansion in Abaqus/Explicit is allowed only with anisotropic elasticity (including orthotropic elasticity) and anisotropic yield . Only isotropic thermal expansion is allowed in Abaqus/CFD, for adiabatic stress analysis, and with the hyperelastic and hyperfoam material models. Isotropic expansion If the thermal expansion coefficient is defined directly, only one value of If user subroutine UEXPAN is used, only one isotropic thermal strain increment ( is needed at each temperature. ) must be defined. Input File Usage: Abaqus/CAE Usage: Use the following option to define the thermal expansion coefficient directly: *EXPANSION, TYPE=ISO Use the following option to define the thermal expansion with user subroutine UEXPAN: *EXPANSION, TYPE=ISO, USER Use the following input to define the thermal expansion coefficient directly: Property module: material editor: Mechanical→Expansion: Type: Isotropic Use the following input to define the thermal expansion with user subroutine UEXPAN: Property module: material editor: Mechanical→Expansion: Type: Isotropic, Use user subroutine UEXPAN THERMAL EXPANSION If the thermal expansion coefficients are defined directly, the three expansion coefficients in the principal material directions ( ) should be given as functions of temperature. If user subroutine UEXPAN is used, the three components of thermal strain increment in the principal material directions ( ) must be defined. , and , and , , Input File Usage: Use the following option to define the thermal expansion coefficient directly: *EXPANSION, TYPE=ORTHO Use the following option to define the thermal expansion with user subroutine UEXPAN: Abaqus/CAE Usage: *EXPANSION, TYPE=ORTHO, USER Use the following input to define the thermal expansion coefficient directly: Property module: material editor: Mechanical→Expansion: Type: Orthotropic Use the following input to define the thermal expansion with user subroutine UEXPAN: Property module: material editor: Mechanical→Expansion: Type: Orthotropic, Use user subroutine UEXPAN Anisotropic expansion If the thermal expansion coefficients are defined directly, all six components of , ) must be given as functions of temperature. If user subroutine UEXPAN is used, all six , , ( , , components of the thermal strain increment ( , , , , , ) must be defined. In an Abaqus/Standard analysis if a distribution is used to define the thermal expansion, the number of expansion coefficients given for each element in the distribution, which is determined by the associated distribution table (“Distribution definition,” Section 2.8.1), must be consistent with the level of anisotropy specified for the expansion behavior. For example, if orthotropic behavior is specified, three expansion coefficients must be defined for each element in the distribution. Input File Usage: Use the following option to define the thermal expansion coefficient directly: *EXPANSION, TYPE=ANISO Use the following option to define the thermal expansion with user subroutine UEXPAN: Abaqus/CAE Usage: *EXPANSION, TYPE=ANISO, USER Use the following input to define the thermal expansion coefficient directly: Property module: material editor: Mechanical→Expansion: Type: Anisotropic Thermal stress Use the following input to define the thermal expansion with user subroutine UEXPAN: Property module: material editor: Mechanical→Expansion: Type: Anisotropic, Use user subroutine UEXPAN When a structure is not free to expand, a change in temperature will cause stress. For example, consider a single two-node truss of length L that is completely restrained at both ends. The cross-sectional area; the Young’s modulus, E; and the thermal expansion coefficient, , are all constant. The stress in this one-dimensional problem can then be calculated from Hooke’s Law as is the total strain and element is fully restrained, is the thermal strain, where is the temperature change. Since the . If the temperature at both nodes is the same, we obtain the stress , where . Constrained thermal expansion can cause significant stress. For typical structural metals, temperature changes of about 150°C (300°F) can cause yield. Therefore, it is often important to define boundary conditions with particular care for problems involving thermal loading to avoid overconstraining the thermal expansion. Energy balance considerations Abaqus does not account for thermal expansion effects in the total energy balance equation, which can lead to an apparent imbalance of the total energy of the model. For example, in the example above of a two-node truss restrained at both ends, constraint thermal expansion introduces strain energy that will result in an equivalent increase in the total energy of the model. Use with other material models Thermal expansion can be combined with any other (mechanical) material behavior in Abaqus. Using thermal expansion with other material models For most materials thermal expansion is defined by a single coefficient or set of orthotropic or anisotropic coefficients or, in Abaqus/Standard, by defining the incremental thermal strains in user subroutine UEXPAN. For porous media in Abaqus/Standard, such as soils or rock, thermal expansion can be defined for the solid grains and for the permeating fluid (when using the coupled pore fluid diffusion/stress procedure—see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). In such a case the thermal expansion definition should be repeated to define the different thermal expansion effects. Using thermal expansion with gasket behaviors Thermal expansion can be used in conjunction with any gasket behavior definition. Thermal expansion will affect the expansion of the gasket in the membrane direction and/or the expansion in the gasket’s thickness direction. Elements Thermal expansion can be used with any stress/displacement or fluid element in Abaqus. 26.1.3 FIELD EXPANSION Product: Abaqus/Standard References • “Material library: overview,” Section 21.1.1 • “UEXPAN,” Section 1.1.29 of the Abaqus User Subroutines Reference Manual • *EXPANSION Overview Field expansion effects: • can be defined by specifying field expansion coefficients so that Abaqus/Standard can compute field expansion strains that are driven by changes in predefined field variables; • can be isotropic, orthotropic, or fully anisotropic; • are defined as total expansion from a reference value of the predefined field variable; • can be specified as a function of temperature and/or predefined field variables; • can be specified directly in user subroutine UEXPAN (if the field expansion strains are complicated functions of field variables and state variables); and • can be defined for more than one predefined field variable. Defining field expansion coefficients Field expansion is a material property included in a material definition except when it refers to the expansion of a gasket whose material properties are not defined as part of a material definition. In that case field expansion must be used in conjunction with the gasket behavior definition . Input File Usage: Use the following options to define field expansion associated with predefined field variable number n for most materials: *MATERIAL *EXPANSION, FIELD=n The *EXPANSION option can be repeated with different values of the predefined field variable number n to define field expansion associated with more than one field. Use the following options to define field expansion associated with predefined field variable number n for gaskets whose constitutive response is defined directly as gasket behavior: *GASKET BEHAVIOR *EXPANSION, FIELD=n The *EXPANSION option can be repeated with different values of the predefined field variable number n to define field expansion associated with more than one field. Computation of field expansion strains Abaqus/Standard requires field expansion coefficients, reference value of the predefined field variable n, , as shown in Figure 26.1.3–1. , that define the total field expansion from a εf εf εf (α ′ f)2 (α ′ f)1 (α f)2 (α f)1 0 fn 1 fn 2 fn fn Figure 26.1.3–1 Definition of the field expansion coefficient. The field expansion for each specified field generates field expansion strains according to the formula where is the field expansion coefficient; is the current value of the predefined field variable n; is the initial value of the predefined field variable n; are the current values of the predefined field variables; are the initial values of the predefined field variables; and is the reference value of the predefined field variable n for the field expansion coefficient. The second term in the above equation represents the strain due to the difference between the initial . This term is value of the predefined field variablen, necessary to enforce the assumption that there is no initial field expansion strain for cases in which the reference value of the predefined field variable n does not equal the corresponding initial value. , and the corresponding reference value, Defining the reference value of the predefined field variable If the coefficient of field expansion, value of the predefined field variable, variables, you can define . , is not a function of temperature or field variables, the reference is a function of temperature or field , is not needed. If Input File Usage: *EXPANSION, FIELD=n, ZERO= Converting field expansion coefficients from differential form to total form Total field expansion coefficients can be provided directly as outlined in the previous section. However, you may have field expansion data available in differential form: that is, the tangent to the strain-field variable curve is provided . To convert to the total field expansion form required by Abaqus, this relationship must be integrated from a suitably chosen reference value of the field variable, : For example, suppose between and ; is a series of constant values: and ; etc. Then, between and ; between The corresponding total expansion coefficients required by Abaqus are then obtained as Defining increments of field expansion strain in user subroutine UEXPAN Increments of field expansion strain can be specified in user subroutine UEXPAN as functions of temperature and/or predefined field variables. User subroutine UEXPAN must be used if the field expansion strain increments depend on state variables. You can use user subroutine UEXPAN only once within a single material definition. In particular, you cannot define both thermal and field expansions or multiple field expansions within the same material definition using user subroutine UEXPAN. Input File Usage: *EXPANSION, FIELD=n, USER Defining the initial temperature and field variable values If the coefficient of field expansion, the initial temperature and initial predefined field variable values, “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. , is a function of temperature and/or predefined field variables, , are given as described in and Element removal and reactivation If an element has been removed and subsequently reactivated (“Element and contact pair removal and reactivation,” Section 11.2.1), in the equation for the field expansion strains represent temperature and predefined field variable values as they were at the moment of reactivation. and Defining directionally dependent field expansion Isotropic, orthotropic, or fully anisotropic field expansion can be defined. Orthotropic and anisotropic field expansion can be used only with materials where the material directions are defined with local orientations . Only isotropic field expansion is allowed with the hyperelastic and hyperfoam material models. Isotropic expansion If the field expansion coefficient is defined directly, only one value of is needed at each temperature and/or predefined field variable. If user subroutine UEXPAN is used, only one isotropic field expansion strain increment ( ) must be defined. Input File Usage: Use the following option to define the field expansion coefficient directly: *EXPANSION, FIELD=n, TYPE=ISO Use the following option to define the field expansion with user subroutine UEXPAN: *EXPANSION, FIELD=n, TYPE=ISO, USER Orthotropic expansion If the field expansion coefficients are defined directly, the three expansion coefficients in the principal material directions ( ) should be given as functions of temperature and/or predefined , and , field variables. increment in the principal material directions ( If user subroutine UEXPAN is used, the three components of field expansion strain , and ) must be defined. , Input File Usage: Use the following option to define the field expansion coefficients directly: *EXPANSION, FIELD=n, TYPE=ORTHO Use the following option to define the field expansion with user subroutine UEXPAN: *EXPANSION, FIELD=n, TYPE=ORTHO, USER Anisotropic expansion If the field expansion coefficients are defined directly, all six components of , ) must be given as functions of temperature and/or predefined field variables. If user , subroutine UEXPAN is used, all six components of the field expansion strain increment ( , , ( , , , , , , ) must be defined. Input File Usage: Use the following option to define the field expansion coefficients directly: *EXPANSION, FIELD=n, TYPE=ANISO Use the following option to define the field expansion with user subroutine UEXPAN: *EXPANSION, FIELD=n, TYPE=ANISO, USER Field expansion stress When a structure is not free to expand, a change in a predefined field variable will cause stress if there is field expansion associated with that predefined field variable. For example, consider a single 2-node truss of length L that is completely restrained at both ends. The cross-sectional area; the Young’s modulus, E; and the field expansion coefficient, , are all constants. The stress in this one-dimensional problem can then be calculated from Hooke’s Law as is the field expansion strain, where n. Since the element is fully restrained, same, we obtain the stress is the change in the value of the predefined field variable number . If the values of the field variable at both nodes are the is the total strain and , where . Depending on the value of the field expansion coefficient and the change in the value of the corresponding predefined field variable, a constrained field expansion can cause significant stress and introduce strain energy that will result in an equivalent increase in the total energy of the model. Therefore, it is often important to define boundary conditions with particular care for problems involving this property to avoid overconstraining the field expansion. Use with other material models Field expansion can be combined with any other (mechanical) material behavior in Abaqus/Standard. Using field expansion with other material models For most materials field expansion is defined by a single coefficient or a set of orthotropic or anisotropic coefficients or by defining the incremental field expansion strains in user subroutine UEXPAN. Using field expansion with gasket behavior Field expansion can be used in conjunction with any gasket behavior definition. Field expansion will affect the expansion of the gasket in the membrane direction and/or the expansion in the gasket’s thickness direction. Elements Field expansion can be used with any stress/displacement element in Abaqus/Standard, except for beam and shell elements using a general section behavior. 26.1.4 VISCOSITY Products: Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Viscous shear behavior” in “Equation of state,” Section 25.2.1 • *VISCOSITY • *EOS • *TRS • “Defining viscosity” in “Defining other mechanical models,” Section 12.9.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Material shear viscosity is an internal property of a fluid that offers resistance to flow. It can be specified in Abaqus/Explicit and Abaqus/CFD. Material shear viscosity in Abaqus/Explicit: • can be a function of temperature and shear strain rate; and • must be used in combination with an equation of state (“Equation of state,” Section 25.2.1). Material shear viscosity in Abaqus/CFD: • can be a function of temperature only for the Newtonian model; • can be a function of shear strain rate; and • is not supported for field-dependent variants. Viscous shear behavior The resistance to flow of a viscous fluid is described by the following relationship between deviatoric stress and strain rate where is the engineering shear strain rate. is the deviatoric stress, is the deviatoric part of the strain rate, is the viscosity, and Newtonian fluids are characterized by a viscosity that only depends on temperature, . In the more general case of non-Newtonian fluids the viscosity is a function of the temperature and shear strain rate: where is the equivalent shear strain rate. In terms of the equivalent shear stress, , we have: Non-Newtonian fluids can be classified as shear-thinning (or pseudoplastic), when the apparent viscosity decreases with increasing shear rate, and shear-thickening (or dilatant), when the viscosity increases with strain rate. In addition to the Newtonian viscous fluid model, Abaqus/CFD and Abaqus/Explicit support several models of nonlinear viscosity to describe non-Newtonian fluids: power law, Carreau-Yasuda, Cross, Herschel-Bulkley, Powell-Eyring, and Ellis-Meter. Other functional forms of the viscosity can also be specified in tabular format. In addition, in Abaqus/Explicit user subroutine VUVISCOSITY can be used. Newtonian The Newtonian model is useful to model viscous laminar flow governed by the Navier-Poisson law of a Newtonian fluid, . Newtonian fluids are characterized by a viscosity that depends only on temperature, . You need to specify the viscosity as a tabular function of temperature when you define the Newtonian viscous deviatoric behavior. Input File Usage: Abaqus/CAE Usage: *VISCOSITY, DEFINITION=NEWTONIAN (default) Property module: material editor: Mechanical→Viscosity Power law The power law model is commonly used to describe the viscosity of non-Newtonian fluids. The viscosity is expressed as is the flow consistency index and , the fluid is where shear-thinning (or pseudoplastic): the apparent viscosity decreases with increasing shear rate. When , the fluid is Newtonian. Optionally, , on the value of the viscosity computed , the fluid is shear-thickening (or dilatant); and when is the flow behavior index. When , and/or an upper limit, you can place a lower limit, from the power law. Input File Usage: Abaqus/CAE Usage: *VISCOSITY, DEFINITION=POWER LAW The power law model is not supported in Abaqus/CAE. Carreau-Yasuda The Carreau-Yasuda model describes the shear thinning behavior of polymers. This model often provides a better fit than the power law model for both high and low shear strain rates. The viscosity is expressed as is the low shear rate Newtonian viscosity, is the natural time constant of the fluid ( where rates), from Newtonian to power law behavior), and regime. The coefficient is the infinite shear viscosity (at high shear strain is the critical shear rate at which the fluid changes represents the flow behavior index in the power law is a material parameter. The original Carreau model is recovered when =2. *VISCOSITY, DEFINITION=CARREAU-YASUDA The Carreau-Yasuda model is not supported in Abaqus/CAE. Input File Usage: Abaqus/CAE Usage: Cross The Cross model is commonly used when it is necessary to describe the low-shear-rate behavior of the viscosity. The viscosity is expressed as is the Newtonian viscosity, where the Cross model), fluid changes from Newtonian to power-law behavior), and law regime. is the natural time constant of the fluid ( is the infinite shear viscosity (usually assumed to be zero for is the critical shear rate at which the is the flow behavior index in the power Input File Usage: Abaqus/CAE Usage: *VISCOSITY, DEFINITION=CROSS The Cross model is not supported in Abaqus/CAE. Herschel-Bulkley The Herschel-Bulkley model can be used to describe the behavior of viscoplastic fluids, such as Bingham plastics, that exhibit a yield response. The viscosity is expressed as is the “yield” stress and Here low strain rate regime ( strain rates, the viscosity transitions into a power law model once the yield threshold is reached, The parameters respectively. Bingham plastics correspond to the case =1. is a penalty viscosity to model the “rigid-like” behavior in the very . With increasing . are the flow consistency and the flow behavior indexes in the power law regime, ), when the stress is below the yield stress, and Input File Usage: Abaqus/CAE Usage: *VISCOSITY, DEFINITION=HERSCHEL-BULKLEY The Herschel-Bulkley model is not supported in Abaqus/CAE. Powell-Eyring This model, which is derived from the theory of rate processes, is relevant primarily to molecular fluids but can be used in some cases to describe the viscous behavior of polymer solutions and viscoelastic suspensions over a wide range of shear rates. The viscosity is expressed as where time of the measured system. is the Newtonian viscosity, is the infinite shear viscosity, and represents a characteristic Input File Usage: Abaqus/CAE Usage: *VISCOSITY, DEFINITION=POWELL-EYRING The Powell-Eyring model is not supported in Abaqus/CAE. Ellis-Meter The Ellis-Meter model expresses the viscosity in terms of the effective shear stress, , as: where and the infinite shear viscosity, is the effective shear stress at which the viscosity is 50% between the Newtonian limit, , , and represents the flow index in the power law regime. Input File Usage: Abaqus/CAE Usage: *VISCOSITY, DEFINITION=ELLIS-METER The Ellis-Meter model is not supported in Abaqus/CAE. Tabular In Abaqus/Explicit the viscosity can be specified directly as a tabular function of shear strain rate and temperature. In Abaqus/CFD only shear strain rate dependence is supported. Input File Usage: Abaqus/CAE Usage: *VISCOSITY, DEFINITION=TABULAR Specifying the viscosity directly as a tabular function is not supported in Abaqus/CAE. User-defined (Abaqus/Explicit only) In Abaqus/Explicit you can specify a user-defined viscosity in user subroutine VUVISCOSITY . *VISCOSITY, DEFINITION=USER User-defined viscosity is not supported in Abaqus/CAE. Abaqus/CAE Usage: Input File Usage: Temperature dependence of viscosity (Abaqus/Explicit only) The temperature-dependence of the viscosity of many polymer materials of industrial interest obeys a time-temperature shift relationship in the form: is the shift function and where is the reference temperature at which the viscosity versus shear strain rate relationship is known. This concept for temperature dependence is usually referred to as thermo-rheologically simple (TRS) temperature dependence. In the Newtonian limit for low shear rates, when , we have Thus, the shift function is defined as the ratio of the Newtonian viscosity at the temperature of interest to that of the chosen reference state: . See “Thermo-rheologically simple temperature effects” in “Time domain viscoelasticity,” Section 22.7.1, for a description of the different forms of the shift function available in Abaqus. Input File Usage: Use the following options to define a thermo-rheologically simple (TRS) temperature-dependent viscosity: Abaqus/CAE Usage: *VISCOSITY *TRS Defining a thermo-rheologically simple temperature-dependent viscosity is not supported in Abaqus/CAE. Use with other material models Material shear viscosity in Abaqus/Explicit must be used in combination with an equation of state to define the material’s volumetric mechanical behavior . Elements Material shear viscosity can be used with any solid (continuum) elements in Abaqus/Explicit except plane stress elements and with any fluid (continuum) elements in Abaqus/CFD. 26.2 Heat transfer properties • “Thermal properties: overview,” Section 26.2.1 • “Conductivity,” Section 26.2.2 • “Specific heat,” Section 26.2.3 • “Latent heat,” Section 26.2.4 26.2.1 THERMAL PROPERTIES: OVERVIEW The following properties describe the thermal behavior of a material and can be used in heat transfer and thermal stress analyses : • Thermal conductivity: When heat flows by conduction, the thermal conductivity must be defined (“Conductivity,” Section 26.2.2). • Specific heat: In transient heat transfer analyses as well as adiabatic stress analyses the specific heat of a material must be defined (“Specific heat,” Section 26.2.3). • Latent heat: When a material changes phase, the change in internal energy can be significant. The amount of energy liberated or absorbed can be defined by specifying a latent heat for each phase change a material undergoes (“Latent heat,” Section 26.2.4). 26.2.2 CONDUCTIVITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Thermal properties: overview,” Section 26.2.1 • *CONDUCTIVITY • “Specifying thermal conductivity,” Section 12.10.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A material’s thermal conductivity: • must be defined for “Uncoupled heat transfer analysis,” Section 6.5.2; “Fully coupled thermal-stress analysis,” Section 6.5.3; and “Coupled thermal-electrical analysis,” Section 6.7.3; • must be defined for an Abaqus/CFD analysis when the energy equation is active (“Energy equation” in “Incompressible fluid dynamic analysis,” Section 6.6.2); • can be linear or nonlinear (by defining it as a function of temperature); • can be isotropic, orthotropic, or fully anisotropic; and • can be specified as a function of temperature and/or field variables. Directional dependence of thermal conductivity Isotropic, orthotropic, or fully anisotropic thermal conductivity can be defined. Only isotropic thermal conductivity can be defined for an incompressible fluid dynamic analysis that includes an energy equation. For orthotropic or anisotropic thermal conductivity, a local orientation (“Orientations,” Section 2.2.5) must be used to specify the material directions used to define the conductivity. Isotropic conductivity For isotropic conductivity only one value of conductivity is needed at each temperature and field variable value. Isotropic conductivity is the default. Input File Usage: Abaqus/CAE Usage: *CONDUCTIVITY, TYPE=ISO Property module: material editor: Thermal→Conductivity: Type: Isotropic Orthotropic conductivity For orthotropic conductivity three values of conductivity ( and field variable value. , , ) are needed at each temperature Input File Usage: *CONDUCTIVITY, TYPE=ORTHO Abaqus/CAE Usage: Property module: material editor: Thermal→Conductivity: Type: Orthotropic Anisotropic conductivity For fully anisotropic conductivity six values of conductivity ( each temperature and field variable value. , , , , , ) are needed at Input File Usage: Abaqus/CAE Usage: *CONDUCTIVITY, TYPE=ANISO Property module: material editor: Thermal→Conductivity: Type: Anisotropic Elements Thermal conductivity is active in all heat transfer, coupled temperature-displacement, coupled thermal- electrical-structural, and coupled thermal-electrical elements in Abaqus. Isotropic thermal conductivity is active in fluid (continuum) elements in Abaqus/CFD for incompressible fluid dynamic analyses that include an energy equation. 26.2.3 SPECIFIC HEAT Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Thermal properties: overview,” Section 26.2.1 • *SPECIFIC HEAT • “Defining specific heat,” Section 12.10.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A material’s specific heat: • is required for transient “Uncoupled heat transfer analysis,” Section 6.5.2; transient “Fully coupled thermal-stress analysis,” Section 6.5.3; transient “Coupled thermal-electrical analysis,” Section 6.7.3; and “Adiabatic analysis,” Section 6.5.4; • must be defined for an Abaqus/CFD analysis when the energy equation is active (“Energy equation” in “Incompressible fluid dynamic analysis,” Section 6.6.2); • must appear in conjunction with a density definition ; • can be linear or nonlinear (by defining it as a function of temperature); and • can be specified as a function of temperature and/or field variables. Defining specific heat The specific heat of a substance is defined as the amount of heat required to increase the temperature of a unit mass by one degree. Mathematically, this physical statement can be expressed as: is the infinitessimal heat added per unit mass and where is the entropy per unit mass. Since heat transfer depends on the conditions encountered during the whole process (a path function), it is necessary to specify the conditions used in the process to unambiguously characterize the specific heat. Thus, a process where the heat is supplied keeping the volume constant defines the specific heat as: where is the internal energy per unit mass. Whereas, a process where the heat is supplied keeping the pressure constant defines the specific heat as: is the enthalpy per unit mass. In general, the specific heats are functions of temperature. where For solids and liquids, are equivalent; thus, there is no need to distinguish between them. When possible, large changes in internal energy or enthalpy during a phase change should be modeled using “Latent heat,” Section 26.2.4, instead of specific heat. and Defining constant-volume specific heat The specific heat per unit mass is given as a function of temperature and field variables. By default, specific heat at constant volume is assumed. *SPECIFIC HEAT The following option can also be used in Abaqus/CFD: Input File Usage: Abaqus/CAE Usage: *SPECIFIC HEAT, TYPE=CONSTANT VOLUME Property module: material editor: Thermal→Specific Heat; Type: Constant Volume Defining constant-pressure specific heat In Abaqus/CFD the constant-pressure specific heat is required when the energy equation is used for thermal-flow problems. Input File Usage: Abaqus/CAE Usage: *SPECIFIC HEAT, TYPE=CONSTANT PRESSURE Property module: material editor: Thermal→Specific Heat; Type: Constant Pressure Elements Specific heat effects can be defined for all heat transfer, coupled thermal-electrical-structural, coupled temperature-displacement, coupled thermal-electrical, and fluid elements in Abaqus. Specific heat can also be defined for stress/displacement elements for use in adiabatic stress analysis. Specific heat must be defined for all transient thermal analyses even if the only elements in the model are user-defined elements (“User-defined elements,” Section 32.15.1), in which case a dummy specific heat must be specified. 26.2.4 LATENT HEAT Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • “Thermal properties: overview,” Section 26.2.1 • *LATENT HEAT • “Specifying latent heat data,” Section 12.10.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A material’s latent heat: • models large changes in internal energy during phase change of a material; • is active only during transient heat transfer, coupled thermal-stress, coupled thermal-electrical- structural and coupled thermal-electrical analysis in Abaqus ; • must appear in conjunction with a density definition ; and • always makes an analysis nonlinear. Defining latent heat Latent heat effects can be significant and must be included in many heat transfer problems involving phase change. When latent heat is given, it is assumed to be in addition to the specific heat effect . The latent heat is assumed to be released over a range of temperatures from a lower (solidus) temperature to an upper (liquidus) temperature. To model a pure material with a single phase change temperature, these limits can be made very close. As many latent heats as are necessary can be defined to model several phase changes in the material. Latent heat can be combined with any other material behavior in Abaqus, but it should not be included in the material definition unless necessary; it always makes the analysis nonlinear. Direct data specification If the phase change occurs within a known temperature range, the solidus and liquidus temperatures can be given directly. The latent heat should be given per unit mass. Input File Usage: Abaqus/CAE Usage: *LATENT HEAT Property module: material editor: Thermal→Latent Heat User subroutine In some cases it may be necessary to include a kinetic theory for the phase change to model the effect accurately in Abaqus/Standard; for example, the prediction of crystallization in a polymer casting process. In such cases you can model the process in considerable detail using solution-dependent state variables (“User subroutines: overview,” Section 18.1.1) and user subroutine HETVAL. Input File Usage: Use the following options: *HEAT GENERATION *DEPVAR Property module: material editor: Thermal→Heat Generation General→Depvar Abaqus/CAE Usage: Elements Latent heat effects can be used in all diffusive heat transfer, coupled temperature-displacement, coupled thermal-electrical-structural and coupled thermal-electrical elements in Abaqus but cannot be used with convective heat transfer elements. Strong latent heat effects are best modeled with first-order or modified second-order elements, which use integration methods designed to provide accurate results for such cases. See “Freezing of a square solid: the two-dimensional Stefan problem,” Section 1.6.2 of the Abaqus Benchmarks Manual, for an example of a heat conduction problem involving latent heat. 26.3 Acoustic properties • “Acoustic medium,” Section 26.3.1 26.3.1 ACOUSTIC MEDIUM Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1 • “Acoustic and shock loads,” Section 33.4.6 • “Material library: overview,” Section 21.1.1 • “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1 • *ACOUSTIC MEDIUM • *DENSITY • *INITIAL CONDITIONS • “Defining an acoustic medium,” Section 12.12.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview An acoustic medium: • is used to model sound propagation problems; • can be used in a purely acoustic analysis or in a coupled acoustic-structural analysis such as the calculation of shock waves in a fluid or noise levels in a vibration problem; • is an elastic medium (usually a fluid) in which stress is purely hydrostatic (no shear stress) and pressure is proportional to volumetric strain; • is specified as part of a material definition; • must appear in conjunction with a density definition ; • can include fluid cavitation in Abaqus/Explicit when the absolute pressure drops to a limit value; • can be defined as a function of temperature and/or field variables; • can include dissipative effects; • can model small pressure changes (small amplitude excitation); • can model waves in the presence of steady underlying flow of the medium; and • is active only during dynamic analysis procedures (“Dynamic analysis procedures: overview,” Section 6.3.1). Defining an acoustic medium The equilibrium equation for small motions of a compressible, inviscid fluid flowing through a resisting matrix material is taken to be where p is the dynamic pressure in the fluid (the pressure in excess of any initial static pressure), spatial position of the fluid particle, is the is the fluid particle acceleration, is the fluid particle velocity, is the density of the fluid, and is the “volumetric drag” (force per unit volume per velocity) caused by the fluid flowing through the matrix material. The d’Alembert term has been written without convection on the assumption that there is no steady flow of the fluid, which is usually considered to be sufficiently accurate for steady fluid velocities up to Mach 0.1. The constitutive behavior of the fluid is assumed to be inviscid and compressible, so that the bulk modulus of an acoustic medium relates the dynamic pressure in the medium to the volumetric strain by where an acoustic medium must be defined. is the volumetric strain. Both the bulk modulus and the density of The bulk modulus can be defined as a function of temperature and field variables but does not vary in value during an implicit dynamic analysis using the subspace projection method (“Implicit dynamic analysis using direct integration,” Section 6.3.2) or a direct-solution steady-state dynamic analysis (“Direct-solution steady-state dynamic analysis,” Section 6.3.4); for these procedures the value of the bulk modulus at the beginning of the step is used. Input File Usage: Abaqus/CAE Usage: Use both of the following options to define an acoustic medium: *ACOUSTIC MEDIUM, BULK MODULUS *DENSITY Property module: material editor: Other→Acoustic Medium: Bulk Modulus General→Density Volumetric drag Dissipation of energy (and attenuation of acoustic waves) may occur in an acoustic medium due to a variety of factors. Such dissipation effects are phenomenologically characterized in the frequency domain by the imaginary part of the propagation constant, which gives an exponential decay in amplitude as a function of distance. In Abaqus the simplest way to model this effect is through a “volumetric drag coefficient,” (force per unit volume per velocity). In frequency-domain procedures, may be frequency dependent. can be entered as a function of frequency— , where f is the frequency in cycles per time (usually Hz)—in addition to temperature and/or field variables only when the acoustic medium is used in a steady-state dynamics procedure. If the acoustic medium is used in a direct-integration dynamic procedure (including Abaqus/Explicit), the volumetric drag coefficient is assumed to be independent of frequency and the first value entered for the current temperature and/or field variable is used. In all procedures except direct steady-state dynamics the gradient of is assumed to be small. Input File Usage: Abaqus/CAE Usage: *ACOUSTIC MEDIUM, VOLUMETRIC DRAG Property module: material editor: Other→Acoustic Medium: Volumetric Drag: Include volumetric drag Porous acoustic material models Porous materials are commonly used to suppress acoustic waves; this attenuating effect arises from a number of effects as the acoustic fluid interacts with the solid matrix. For many categories of materials, the solid matrix can be approximated as either fully rigid compared to the acoustic fluid or fully limp. In these cases a mechanical model that resolves only acoustic waves will suffice. The acoustic behavior of porous materials can be modeled in a variety of ways in Abaqus/Standard. Craggs model The model discussed in Craggs (1978) is readily accommodated in Abaqus. Applying this model results in the dynamic equilibrium equation for the fluid expressed in this form: where “structure factor,” and is the real-valued resistivity, is the real-valued dimensionless porosity, is the dimensionless is the dimensionless wave number. This equation can be rewritten as This model, therefore, can be applied straightforwardly in Abaqus by setting the material density equal to . The Craggs model is , the volumetric drag equal to supported for all acoustic procedures in Abaqus. , and the bulk modulus equal to Delany-Bazley and Delany-Bazley-Miki models Abaqus/Standard supports the well-known empirical model proposed in Delany & Bazley (1970), which determines the material properties as a function of frequency and user-defined flow resistivity, ; density, . A variation on this model, proposed by Miki (1990) is also available. These ; and bulk modulus, models are supported only for steady-state dynamic procedures. Both models compute frequency-dependent material characteristic impedance, , according to the following formula: or propagation constant, , and wavenumber where and The constants are as given in the table below: Delany- Bazley Miki 0.0978 –0.7 0.189 –0.595 0.0571 –0.754 0.087 –0.732 0.1227 –0.618 0.1792 –0.618 0.0786 –0.632 0.1205 –0.632 The material characteristic impedance and the wavenumber are converted internally to complex density and complex bulk modulus for use in Abaqus. The signs of the imaginary parts in these formulae are consistent with the Abaqus sign convention for time-harmonic dynamics. Input File Usage: Abaqus/CAE Usage: Use the following options to use the Delany-Bazley model: *DENSITY *ACOUSTIC MEDIUM, BULK MODULUS *ACOUSTIC MEDIUM, POROUS MODEL=DELANY BAZLEY Use the following options to use the Miki model: *DENSITY *ACOUSTIC MEDIUM, BULK MODULUS *ACOUSTIC MEDIUM, POROUS MODEL=MIKI Porous acoustic material models are not supported in Abaqus/CAE. General frequency-dependent models For steady-state dynamic procedures, Abaqus/Standard supports general frequency-dependent complex bulk modulus and complex density. Using these parameters, data from a wide range of models can be accommodated in an analysis; for example, see Allard, et. al (1998), Attenborough (1982), Song & Bolton (1999), and Wilson (1993). These models are used in a variety of applications, such as ocean acoustics, aerospace, automotive, and architectural acoustic engineering. The signs of these parameters must be consistent with the sign conventions used in Abaqus, and with conservation of energy. Abaqus uses a Fourier transform pair formally equivalent to assuming time dependence. Consequently, the real parts of the density and bulk modulus are positive for all values of frequency, the imaginary part of the bulk modulus must be positive, and the imaginary part of the density must be negative. A linear isotropic acoustic material can be fully described with the two frequency-dependent . It is common, however, to encounter materials defined , wave number or propagation parameters: bulk modulus, in terms of other parameter pairs, such as characteristic impedance, , and density, . Data defined with the pair complex density and bulk modulus form, beginning from the following standard formulae: , or speed of sound, or can be converted into the ACOUSTIC MEDIUM Consistent with the Abaqus sign conventions, the real parts of and must be positive; the imaginary part of must be negative, and the imaginary part of must be positive. In commonly observed materials, the ratio of the magnitude of the imaginary part to the real part for each of these constants is usually much less than one. Input File Usage: Use the following option to use the general frequency-dependent model: *ACOUSTIC MEDIUM, COMPLEX BULK MODULUS *ACOUSTIC MEDIUM, COMPLEX DENSITY If desired, either complex material option can be used instead in conjunction with a real-valued, frequency-independent material option: *ACOUSTIC MEDIUM, COMPLEX BULK MODULUS *DENSITY or, alternatively, *ACOUSTIC MEDIUM, BULK MODULUS *ACOUSTIC MEDIUM, COMPLEX DENSITY Abaqus/CAE Usage: General frequency-dependent acoustic material models are not supported in Abaqus/CAE. Conversion from complex material impedance and wavenumber Since and the real and imaginary parts of are, respectively: and the real and imaginary parts of are, respectively: . Conversion from complex impedance and speed of sound Since and the real and imaginary parts of are, respectively: and the real and imaginary parts of are, respectively: . Fluid cavitation In general, fluids cannot withstand any significant tensile stress and are likely to undergo large volume expansion when the absolute pressure is close to or less than zero. Abaqus/Explicit allows modeling of this phenomenon through a cavitation pressure limit for the acoustic medium. When the fluid absolute pressure (sum of the dynamic and initial static pressures) reduces to this limit, the fluid undergoes free volume expansion (i.e., cavitation), without a further drop in the pressure. If this limit is not defined, the fluid is assumed not to undergo cavitation even under a tensile, negative absolute pressure, condition. The constitutive behavior for an acoustic medium capable of undergoing cavitation can be stated as where a pseudo-pressure , a measure of the volumetric strain, is defined as is the fluid cavitation limit and where is the initial acoustic static pressure. A total wave formulation is used for a nonlinear acoustic medium undergoing cavitation. This formulation is very similar to the scattered wave formulation except that the pseudo-pressure, defined as the product of the bulk modulus and the compressive volumetric strain, plays the role of the material state variable instead of the acoustic dynamic pressure and the acoustic dynamic pressure is readily available from this pseudo-pressure subject to the cavitation condition. Input File Usage: Abaqus/CAE Usage: *ACOUSTIC MEDIUM, CAVITATION LIMIT Fluid cavitation is not supported in Abaqus/CAE. Defining the wave formulation In the presence of cavitation in Abaqus/Explicit the fluid mechanical behavior is nonlinear. Hence, for an acoustic problem with incident wave loading and possible cavitation in the fluid, the scattered wave formulation, which provides a solution for only a scattered wave dynamic acoustic pressure, may not be appropriate. For these cases the total wave formulation, which solves for the total dynamic acoustic pressure, should be selected. See “Acoustic and shock loads,” Section 33.4.6, for details. *ACOUSTIC WAVE FORMULATION, TYPE=TOTAL WAVE Any module: Model→Edit Attributes→model_name. Toggle on Specify acoustic wave formulation: Total wave Abaqus/CAE Usage: Input File Usage: Defining the initial acoustic static pressure Cavitation occurs when the absolute pressure reaches the cavitation limit value. Abaqus/Explicit allows for an initial linearly varying hydrostatic pressure in the fluid medium . You can specify pressure values at two locations and a node set of the acoustic medium nodes. Abaqus/Explicit interpolates from these data to initialize the static pressure at all the nodes in the specified node set. If the pressure at only one location is specified, the hydrostatic pressure in the fluid is assumed to be uniform. The acoustic static pressure is used only for determining the cavitation status of the acoustic element nodes and does not apply any static loads to the acoustic or structural mesh at their common wetted interface. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=ACOUSTIC STATIC PRESSURE Initial acoustic pressures are not supported in Abaqus/CAE. Defining a steady flow field Acoustic finite elements can be used to simulate time-harmonic wave propagation and natural frequency analysis in the presence of a steady mean flow of the medium. For example, air may move at a speed large enough to affect the propagation speed of waves in the direction of flow and against it. These effects are modeled in Abaqus/Standard by specifying an acoustic flow velocity during the linear perturbation analysis step definition; you do not need to alter the acoustic material properties. See “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1, for details. Elements An acoustic material definition can be used only with the acoustic elements in Abaqus . In Abaqus/Standard second-order acoustic elements are more accurate than first-order elements. Use at least six nodes per wavelength in the acoustic medium to obtain accurate results. Output Nodal output variable POR (pressure magnitude) is available for an acoustic medium in Abaqus (in Abaqus/CAE this output variable is called PAC). When the scattered wave formulation is used with incident wave loading in Abaqus/Explicit, output variable POR represents only the scattered pressure response of the model and does not include the incident wave loading itself. When the total wave formulation is used, output variable POR represents the total dynamic acoustic pressure, which includes contributions from both incident and scattered waves as well as the dynamic effects of fluid cavitation. For either formulation output variable POR does not include the acoustic static pressure, which is used only to evaluate the cavitation status in the acoustic medium. In addition, in Abaqus/Standard nodal output variable PPOR (the pressure phase) is available for an acoustic medium. In Abaqus/Explicit nodal output variable PABS (the absolute pressure, equal to the sum of POR and the acoustic static pressure) is available for an acoustic medium. Additional references • Allard, J. F., M. Henry, J. Tizianel, L. Kelders, and W. Lauriks, “Sound Propagation in Air-Saturated Random Packings of Beads,” Journal of the Acoustical Society of America, vol. 104, no. 4, p. 2004, 1998. • Attenborough, K. F., “Acoustical Characterisitics of Rigid Fibrous Absorbents and Granular Materials,” Journal of the Acoustical Society of America, vol. 73, no. 3, p. 785, 1982. • Craggs, A., “A Finite Element Model for Rigid Porous Absorbing Materials,” Journal of Sound and Vibration, vol. 61, no. 1, p. 101, 1978. • Craggs, A., “Coupling of Finite Element Acoustic Absorption Models,” Journal of Sound and Vibration, vol. 66, no. 4, p. 605, 1979. • Delany, M. E., and E. N. Bazley, “Acoustic Properties of Fibrous Absorbent Materials,” Applied Acoustics, vol. 3, p. 105, 1970. • Miki, Y., “Acoustical Properties of Porous Materials - Modifications of Delany-Bazley Models,” Journal of the Acoustical Society of Japan (E), vol. 11, no. 1, p. 19, 1990. • Song, B. H., and J. S. Bolton, “A Transfer-Matrix Approach for Estimating the Characteristic Impedance and Wavenumbers of Limp and Rigid Porous Materials,” Journal of the Acoustical Society of America, vol. 107, no. 3, p. 1131, 1999. • Wilson, D. K., “Relaxation-Matched Modeling of Propagation through Porous Media, Including Fractal Pore Structure,” Journal of the Acoustical Society of America, vol. 94, no. 2, p. 1136, 1993. 26.4 Mass diffusion properties • “Diffusivity,” Section 26.4.1 • “Solubility,” Section 26.4.2 26.4.1 DIFFUSIVITY Products: Abaqus/Standard Abaqus/CAE References • “Mass diffusion analysis,” Section 6.9.1 • “Material library: overview,” Section 21.1.1 • *DIFFUSIVITY • *KAPPA • “Defining mass diffusion,” Section 12.12.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Diffusivity: • defines the diffusion or movement of one material through another, such as the diffusion of hydrogen through a metal; • must always be defined for mass diffusion analysis; • must be defined in conjunction with “Solubility,” Section 26.4.2; • can be defined as a function of concentration, temperature, and/or predefined field variables; • can be used in conjunction with a “Soret effect” factor to introduce mass diffusion caused by temperature gradients; • can be used in conjunction with a pressure stress factor to introduce mass diffusion caused by gradients of equivalent pressure stress (hydrostatic pressure); and • can produce a nonlinear mass diffusion analysis when dependence on concentration is included (the same can be said for the Soret effect factor and the pressure stress factor). Defining diffusivity Diffusivity is the relationship between the concentration flux, , of the diffusing material and the gradient of the chemical potential that is assumed to drive the mass diffusion process. Either general mass diffusion behavior or Fick’s diffusion law can be used to define diffusivity, as discussed below. General chemical potential Diffusive behavior provides the following general chemical potential: where is the diffusivity; is the solubility ; is the Soret effect factor, providing diffusion because of temperature gradient ; is the pressure stress factor, providing diffusion because of the gradient of the equivalent pressure stress ; is the normalized concentration; is the concentration of the diffusing material; is the temperature; is the temperature at absolute zero ; is the equivalent pressure stress; and are any predefined field variables. Input File Usage: Abaqus/CAE Usage: *DIFFUSIVITY, LAW=GENERAL (default) Property module: material editor: Other→Mass Diffusion→Diffusivity: Law: General Fick’s law An extended form of Fick’s law can be used as an alternative to the general chemical potential: Input File Usage: Abaqus/CAE Usage: *DIFFUSIVITY, LAW=FICK Property module: material editor: Other→Mass Diffusion→Diffusivity: Law: Fick Directional dependence of diffusivity Isotropic, orthotropic, or fully anisotropic diffusivity can be defined. For non-isotropic diffusivity a local orientation of the material directions must be specified . Isotropic diffusivity For isotropic diffusivity only one value of diffusivity is needed at each concentration, temperature, and field variable value. Input File Usage: Abaqus/CAE Usage: *DIFFUSIVITY, TYPE=ISO Property module: material editor: Other→Mass Diffusion→Diffusivity: Type: Isotropic Orthotropic diffusivity For orthotropic diffusivity three values of diffusivity ( temperature, and field variable value. , , ) are needed at each concentration, Input File Usage: Abaqus/CAE Usage: *DIFFUSIVITY, TYPE=ORTHO Property module: material editor: Other→Mass Diffusion→Diffusivity: Type: Orthotropic Anisotropic diffusivity For fully anisotropic diffusivity six values of diffusivity ( each concentration, temperature, and field variable value. *DIFFUSIVITY, TYPE=ANISO Property module: material editor: Other→Mass Diffusion→Diffusivity: Type: Anisotropic Abaqus/CAE Usage: Input File Usage: , , , , , ) are needed at Temperature-driven mass diffusion , governs temperature-driven mass diffusion. It can be defined as a function The Soret effect factor, of concentration, temperature, and/or field variables in the context of the constitutive equation presented above. The Soret effect factor cannot be specified in conjunction with Fick’s law since it is calculated automatically in this case . Input File Usage: Use both of the following options to specify general temperature-driven mass diffusion: *DIFFUSIVITY, LAW=GENERAL *KAPPA, TYPE=TEMP Use the following option to specify temperature-driven diffusion governed by Fick’s law: Abaqus/CAE Usage: *DIFFUSIVITY, LAW=FICK Use the following options to specify general temperature-driven mass diffusion: Property module: material editor: Other→Mass Diffusion→Diffusivity: Law: General: Suboptions→Soret Effect Use the following option to specify temperature-driven diffusion governed by Fick’s law: Property module: material editor: Other→Mass Diffusion→Diffusivity: Law: Fick Pressure stress-driven mass diffusion The pressure stress factor, , governs mass diffusion driven by the gradient of the equivalent pressure stress. It can be defined as a function of concentration, temperature, and/or field variables in the context of the constitutive equation presented above. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *DIFFUSIVITY, LAW=GENERAL *KAPPA, TYPE=PRESS Property module: material editor: Other→Mass Diffusion→Diffusivity: Law: General: Suboptions→Pressure Effect Mass diffusion driven by both temperature and pressure stress and causes gradients of temperature and equivalent pressure stress to drive mass Specifying both diffusion. Input File Usage: Abaqus/CAE Usage: Use all of the following options to specify general diffusion driven by gradients of temperature and pressure stress: *DIFFUSIVITY, LAW=GENERAL *KAPPA, TYPE=TEMP *KAPPA, TYPE=PRESS Use both of the following options to specify diffusion driven by the extended form of Fick’s law: *DIFFUSIVITY, LAW=FICK *KAPPA, TYPE=PRESS Use the following options to specify general diffusion driven by gradients of temperature and pressure stress: Property module: material editor: Other→Mass Diffusion→Diffusivity: Law: General: Suboptions→Soret Effect and Suboptions→Pressure Effect Use the following options to specify diffusion driven by the extended form of Fick’s law: Property module: material editor: Other→Mass Diffusion→Diffusivity: Law: Fick: Suboptions→Pressure Effect Specifying the value of absolute zero You can specify the value of absolute zero as a physical constant. Input File Usage: *PHYSICAL CONSTANTS, ABSOLUTE ZERO= Abaqus/CAE Usage: Any module: Model→Edit Attributes→model_name: Absolute zero temperature Elements The mass diffusion law can be used only with the two-dimensional, three-dimensional, and axisymmetric solid elements that are included in the heat transfer/mass diffusion element library. 26.4.2 SOLUBILITY Products: Abaqus/Standard Abaqus/CAE References • “Mass diffusion analysis,” Section 6.9.1 • “Material library: overview,” Section 21.1.1 • *SOLUBILITY • “Defining solubility” in “Defining mass diffusion,” Section 12.12.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Solubility: • is needed only for mass diffusion analysis; • is also known as Sievert’s parameter (in Sievert’s law); • must always accompany a diffusivity definition ; and • can be defined as a function of temperature and/or predefined field variables. Defining solubility Solubility, s, is used to define the “normalized concentration,” , of the diffusing phase in a mass diffusion process: where c is the concentration. The normalized concentration is often also referred to as the “activity” of the diffusing material, and the gradients of the normalized concentration, along with gradients of temperature and pressure stress, drive the diffusion process . Input File Usage: Abaqus/CAE Usage: *SOLUBILITY Property module: material editor: Other→Mass Diffusion→Solubility Elements The mass diffusion law can be used only with the two-dimensional, three-dimensional, and axisymmetric solid elements that are included in the heat transfer/mass diffusion element library. 26.5 Electromagnetic properties • “Electrical conductivity,” Section 26.5.1 • “Piezoelectric behavior,” Section 26.5.2 • “Magnetic permeability,” Section 26.5.3 26.5.1 ELECTRICAL CONDUCTIVITY Products: Abaqus/Standard Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • *ELECTRICAL CONDUCTIVITY • “Defining electrical conductivity,” Section 12.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A material’s electrical conductivity: • must be defined for “Coupled thermal-electrical analysis,” Section 6.7.3; • must be defined for “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4; • must be used to define the electromagnetic response of a conductor for “Eddy current analysis,” Section 6.7.5; • can be linear or nonlinear (by defining it as a function of temperature); • can be isotropic, orthotropic, or fully anisotropic; • can be specified as a function of temperature and/or field variables; and • can be specified as a function of frequency for “Eddy current analysis,” Section 6.7.5. Directional dependence of electrical conductivity Isotropic, orthotropic, or fully anisotropic electrical conductivity can be defined. For non-isotropic conductivity a local orientation for the material directions must be specified (“Orientations,” Section 2.2.5). Isotropic electrical conductivity For isotropic electrical conductivity only one value of electrical conductivity is needed at each temperature and field variable value. Isotropic electrical conductivity is the default. *ELECTRICAL CONDUCTIVITY, TYPE=ISOTROPIC Property module: material editor: Electrical/Magnetic→Electrical Conductivity: Type: Isotropic Abaqus/CAE Usage: Input File Usage: Orthotropic electrical conductivity For orthotropic electrical conductivity three values of electrical conductivity ( at each temperature and field variable value. , , ) are needed Input File Usage: *ELECTRICAL CONDUCTIVITY, TYPE=ORTHOTROPIC Abaqus/CAE Usage: Property module: material editor: Electrical/Magnetic→Electrical Conductivity: Type: Orthotropic Anisotropic electrical conductivity For fully anisotropic electrical conductivity six values ( temperature and field variable value. , , , , , ) are needed at each Input File Usage: Abaqus/CAE Usage: *ELECTRICAL CONDUCTIVITY, TYPE=ANISOTROPIC Property module: material editor: Electrical/Magnetic→Electrical Conductivity: Type: Anisotropic Frequency-dependent electrical conductivity Electrical conductivity can be defined as a function of frequency in an eddy current analysis. Input File Usage: Abaqus/CAE Usage: *ELECTRICAL CONDUCTIVITY, FREQUENCY Property module: material editor: Electrical/Magnetic→Electrical Conductivity: Toggle on Use frequency-dependent data Elements Electrical conductivity is active only in coupled thermal-electrical elements, coupled thermal-electrical- structural elements, and electromagnetic elements . 26.5.2 PIEZOELECTRIC BEHAVIOR Products: Abaqus/Standard Abaqus/CAE References • “Piezoelectric analysis,” Section 6.7.2 • “Material library: overview,” Section 21.1.1 • *DIELECTRIC • *PIEZOELECTRIC • “Defining dielectric material properties,” Section 12.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining piezoelectric properties,” Section 12.11.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A piezoelectric material: • is one in which an electrical field causes the material to strain, while stress causes an electric potential gradient; • provides linear relations between mechanical and electrical fields; and • is used in piezoelectric elements, which have both displacement and electrical potential as nodal variables. Defining a piezoelectric material A piezoelectric material responds to an electric potential gradient by straining, while stress causes an electric potential gradient in the material. This coupling between electric potential gradient and strain is the material’s piezoelectric property. The material will also have a dielectric property so that an electrical charge exists when the material has a potential gradient. Piezoelectric material behavior is discussed in “Piezoelectric analysis,” Section 2.10.1 of the Abaqus Theory Manual. The mechanical properties of the material must be modeled by linear elasticity (“Linear elastic behavior,” Section 22.2.1). The mechanical behavior can be defined by in terms of the piezoelectric stress coefficient matrix, , or by in terms of the piezoelectric strain coefficient matrix, . The electrical behavior is defined by where is the mechanical stress tensor; is the strain tensor; is the electric “displacement” vector; is the material’s elastic stiffness matrix defined at zero electrical potential gradient (short circuit condition); is the material’s piezoelectric stress coefficient matrix, defining the stress electrical potential gradient the electrical displacement gradient); is the material’s piezoelectric strain coefficient matrix, defining the strain electrical potential gradient is given later in this section); is the electrical potential; caused by the in a fully constrained material (it can also be interpreted as at a zero electrical potential caused by the in an unconstrained material (an alternative interpretation caused by the applied strain is the material’s dielectric property, defining the relation between the electric displacement and the electric potential gradient is the electrical potential gradient vector, . for a fully constrained material; and The material’s electrical and electro-mechanical coupling behaviors are, thus, defined by its , or its piezoelectric strain . These properties are defined as part of the material definition (“Material data , and its piezoelectric stress coefficient matrix, dielectric property, coefficient matrix, definition,” Section 21.1.2). Alternative forms of the constitutive equations Alternative forms of the piezoelectric constitutive equations are presented in this section. These forms of the equations involve material properties that cannot be used directly as input for Abaqus/Standard. However, they are related to the Abaqus/Standard input through simple relations that are presented in “Piezoelectric analysis,” Section 2.10.1 of the Abaqus Theory Manual. The intent of this section is to draw connections between the Abaqus/Standard terminology and input to that used commonly in the piezoelectricity community. The mechanical behavior can also be defined by in terms of the piezoelectric coefficient matrix , which defines the mechanical properties at zero electrical displacement (open circuit condition). Likewise, the electrical behavior can also be defined by , and the stiffness matrix in terms of the dielectric matrix for an unconstrained material or by where is the material’s elastic stiffness matrix defined at zero electrical displacement; at zero electrical potential gradient; is the material’s piezoelectric strain coefficient matrix used earlier, and based on the equations, may alternatively be interpreted as the electrical displacement caused by the stress is the material’s piezoelectric coefficient matrix, which can be interpreted as defining either the strain in an unconstrained material or the electrical potential gradient at zero electrical displacement; and caused by the electrical displacement caused by the stress is the material’s dielectric property, defining the relation between the electric displacement and the electric potential gradient for an unconstrained material. These are useful relationships that are often seen in the piezoelectric literature. analysis,” Section 2.10.1 of the Abaqus Theory Manual, the properties expressed in terms of the properties In “Piezoelectric are , that are used as input for Abaqus/Standard. , and , and , , Specifying dielectric material properties The dielectric matrix can be isotropic, orthotropic, or fully anisotropic. For non-isotropic dielectric materials a local orientation for the material directions must be specified (“Orientations,” Section 2.2.5). The entries of the dielectric matrix (what are referred to as “dielectric constants” in Abaqus) refer to what is more commonly known in the literature as the permittivity of the material. Isotropic dielectric properties The dielectric matrix can be fully isotropic, so that You specify the single value material. Isotropic behavior is the default. for the dielectric constant. must be determined for a constrained Input File Usage: Abaqus/CAE Usage: *DIELECTRIC, TYPE=ISO Property module: material editor: Electrical/Magnetic→Dielectric (Electrical Permittivity): Type: Isotropic Orthotropic dielectric properties For orthotropic behavior you must specify three values in the dielectric matrix ( , , and ). Input File Usage: *DIELECTRIC, TYPE=ORTHO Abaqus/CAE Usage: Property module: material editor: Electrical/Magnetic→Dielectric (Electrical Permittivity): Type: Orthotropic Anisotropic dielectric properties For fully anisotropic behavior you must specify six values in the dielectric matrix ( , , , , , and Input File Usage: Abaqus/CAE Usage: ). *DIELECTRIC, TYPE=ANISO Property module: material editor: Electrical/Magnetic→Dielectric (Electrical Permittivity): Type: Anisotropic Specifying piezoelectric material properties The piezoelectric material properties can be defined by giving the stress coefficients, default), or by giving the strain coefficients, following order (substitute d for e for strain coefficients): (this is the . In either case, 18 components must be given in the , , , , , , , , , , , , , , , , , . The first index on these coefficients refers to the component of electric displacement (sometimes called the electric flux), while the last pair of indices refers to the component of mechanical stress or strain. Thus, the piezoelectric components causing electrical displacement in the 1-direction are all given first, then those causing electrical displacement in the 2-direction, and then those causing electrical displacement in the 3-direction. (Some references list these coupling terms in a different order.) Input File Usage: Use the following option to give the stress coefficients: *PIEZOELECTRIC, TYPE=S Use the following option to give the strain coefficients: Abaqus/CAE Usage: *PIEZOELECTRIC, TYPE=E Property module: material editor: Electrical/Magnetic→Piezoelectric: Type: Stress or Strain Converting double index notation to triple index notation Industry-supplied piezoelectric data often use a double index notation. A double index notation can be converted easily to the required triple index notation in Abaqus/Standard by noting the convention followed in Abaqus for the correspondence between (second-order) tensor and vector notations: the 11, 22, 33, 12, 13, and 23 components of the tensor correspond to the 1, 2, 3, 4, 5, and 6 components, respectively, of the corresponding vector. Elements Piezoelectric coupling is active only in piezoelectric elements (those with displacement degrees of freedom and electrical potential degree of freedom 9). See “Choosing the appropriate element for an analysis type,” Section 27.1.3. 26.5.3 MAGNETIC PERMEABILITY Products: Abaqus/Standard Abaqus/CAE References • “Material library: overview,” Section 21.1.1 • *MAGNETIC PERMEABILITY • *NONLINEAR BH • “Defining magnetic permeability,” Section 12.11.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A material’s magnetic permeability: • must be defined for “Eddy current analysis,” Section 6.7.5, and “Magnetostatic analysis,” Section 6.7.6; • can be specified directly for linear magnetic behavior or through one or more B–H curves for nonlinear magnetic behavior; • can be isotropic, orthotropic, or (in the case of linear behavior) fully anisotropic; • can be specified as a function of temperature and/or field variables; and • can be specified as a function of frequency in a time-harmonic eddy current procedure. Linear magnetic behavior Linear magnetic behavior is defined by direct specification of magnetic permeability. Directional dependence of magnetic permeability Isotropic, orthotropic, or fully anisotropic magnetic permeability can be defined. For non-isotropic magnetic permeability a local orientation for the material directions must be specified (“Orientations,” Section 2.2.5). Isotropic magnetic permeability For isotropic magnetic permeability only one value of magnetic permeability is needed at each temperature and field variable value. Isotropic magnetic permeability is the default. Input File Usage: Abaqus/CAE Usage: *MAGNETIC PERMEABILITY, TYPE=ISOTROPIC Property module: material editor: Electrical/Magnetic→Magnetic Permeability: Type: Isotropic Orthotropic magnetic permeability For orthotropic magnetic permeability three values of magnetic permeability ( at each temperature and field variable value. , , ) are needed Input File Usage: Abaqus/CAE Usage: *MAGNETIC PERMEABILITY, TYPE=ORTHOTROPIC Property module: material editor: Electrical/Magnetic→Magnetic Permeability: Type: Orthotropic Anisotropic magnetic permeability For fully anisotropic magnetic permeability six values ( temperature and field variable value. , , , , , ) are needed at each Input File Usage: Abaqus/CAE Usage: *MAGNETIC PERMEABILITY, TYPE=ANISOTROPIC Property module: material editor: Electrical/Magnetic→Magnetic Permeability: Type: Anisotropic Frequency-dependent magnetic permeability Magnetic permeability can be defined as a function of frequency in a time-harmonic eddy current analysis. Input File Usage: Abaqus/CAE Usage: *MAGNETIC PERMEABILITY, FREQUENCY Property module: material editor: Electrical/Magnetic→Magnetic Permeability: Toggle on Use frequency-dependent data Nonlinear magnetic behavior Nonlinear magnetic behavior is characterized by magnetic permeability that depends on the strength of the magnetic field. The nonlinear magnetic material model in Abaqus is suitable for ideally soft magnetic materials (without any hysteresis effects) characterized by a monotonically increasing response in B–H space, where B and H refer to the strengths of the magnetic flux density vector and the magnetic field vector, respectively. Nonlinear magnetic behavior is defined through direct specification of one or more B–H curves that provide B as a function of H and, optionally, temperature and/or predefined field variables, in one or more directions. Nonlinear magnetic behavior can be isotropic, orthotropic, or transversely isotropic (which is a special case of the more general orthotropic behavior). More than one B–H curve is needed to define the nonlinear magnetic behavior if it is not isotropic. Directional dependence of nonlinear magnetic behavior Isotropic, orthotropic, or transversely isotropic nonlinear magnetic behavior can be defined. For non- isotropic nonlinear magnetic behavior a local orientation for the material directions must be specified (“Orientations,” Section 2.2.5). Isotropic nonlinear magnetic behavior For isotropic nonlinear magnetic response only one B–H curve is needed at each temperature and field variable value. Isotropic magnetic permeability is the default. Abaqus assumes that the nonlinear magnetic behavior is governed by Input File Usage: You define through a B–H curve: *MAGNETIC PERMEABILITY, NONLINEAR, TYPE=ISOTROPIC *NONLINEAR BH, DIR=direction The B–H curve in any direction (i.e., the nonlinear behavior in global direction 1, 2, or 3) will suffice as the nonlinear magnetic behavior is assumed to be the same in all directions. Abaqus/CAE Usage: Nonlinear magnetic behavior is not supported in Abaqus/CAE. Orthotropic nonlinear magnetic behavior For orthotropic nonlinear magnetic response three B–H curves (one curve to define the behavior in each of the local directions 1, 2, and 3) are needed at each temperature and field variable value. Abaqus assumes that the nonlinear magnetic behavior in the local material directions is governed by where refers to a diagonal matrix. Transversely isotropic nonlinear magnetic behavior is a special case of orthotropic behavior, in which the behavior in any two directions is the same and is different from that in the third direction. Input File Usage: You define independent B–H curves, one in each of the directions 1, 2, and 3: , and , respectively, through three , *MAGNETIC PERMEABILITY, NONLINEAR, TYPE=ORTHOTROPIC *NONLINEAR BH, DIR=1 … *NONLINEAR BH, DIR=2 … *NONLINEAR BH, DIR=3 … Abaqus/CAE Usage: Nonlinear magnetic behavior is not supported in Abaqus/CAE. Elements Magnetic material behavior is active only in electromagnetic elements . 26.6 Pore fluid flow properties • “Pore fluid flow properties,” Section 26.6.1 • “Permeability,” Section 26.6.2 • “Porous bulk moduli,” Section 26.6.3 • “Sorption,” Section 26.6.4 • “Swelling gel,” Section 26.6.5 • “Moisture swelling,” Section 26.6.6 26.6.1 PORE FLUID FLOW PROPERTIES Abaqus/Standard allows specific properties to be defined for a fluid-filled porous material. This type of porous medium is considered in a coupled pore fluid diffusion/stress analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). The following properties are available: • Permeability: Permeability defines the relationship between the flow rate of a liquid through a porous medium and the gradient of the piezometric head of that fluid . • Porous bulk moduli: The bulk moduli of the solid grains and of the fluid in a porous medium are defined such that their compressibility is considered in an analysis . • Sorption: Sorption defines the absorption/exsorption behavior of a porous material under partially saturated flow conditions . • Swelling gel: The swelling gel model is used to simulate the growth of gel particles that swell and trap wetting liquid in a partially saturated porous medium . • Moisture swelling: Moisture swelling defines the saturation-driven volumetric swelling of a porous medium’s solid skeleton under partially saturated flow conditions . Thermal expansion For porous media such as soils or rock, the thermal expansion of both the solid grains and the permeating fluid can be defined. See “Thermal expansion” in “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1, for more details. 26.6.2 PERMEABILITY Products: Abaqus/Standard Abaqus/CFD Abaqus/CAE References • “Pore fluid flow properties,” Section 26.6.1 • “Material library: overview,” Section 21.1.1 • *PERMEABILITY • “Defining permeability” in “Defining a fluid-filled porous material,” Section 12.12.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Permeability is the relationship between the volumetric flow rate per unit area of a particular wetting liquid through a porous medium and the gradient of the effective fluid pressure. It can be specified in Abaqus/Standard and Abaqus/CFD. Permeability in Abaqus/Standard: • must be specified for a wetting liquid for an effective stress/wetting liquid diffusion analysis ; • is defined, in general, by Forchheimer’s law, which accounts for changes in permeability as a function of fluid flow velocity; and • can be isotropic, orthotropic, or fully anisotropic and can be given as a function of void ratio, saturation, temperature, and field variables. Permeability in Abaqus/CFD: • must be specified for porous media flows ; and • can be isotropic and specified as a function of porosity only or can be specified through the Carman- Kozeny permeability-porosity relation. Permeability in Abaqus/Standard Permeability is defined for pore fluid flow. Forchheimer’s law According to Forchheimer’s law, high flow velocities have the effect of reducing the effective As the fluid flow velocity reduces, permeability and, Forchheimer’s law approximates the well-known Darcy’s law. Darcy’s law can, therefore, be used directly in Abaqus/Standard by omitting the velocity-dependent term in Forchheimer’s law. therefore, “choking” pore fluid flow. Forchheimer’s law is written as where for a completely for a fully saturated medium, is the volumetric flow rate of wetting liquid per unit area of the porous medium (the effective velocity of the wetting liquid); is the fluid saturation ( dry medium); is the porosity of the porous medium; is the void ratio; is the wetting fluid volume in the medium; is the void volume in the medium; is the volume of grains of solid material in the medium; is the volume of trapped wetting liquid in the medium; is the total volume of the medium; is the fluid velocity; is a “velocity coefficient,” which may be dependent on the void ratio of the material; is the dependence of permeability on saturation of the wetting liquid such that at ; is the density of the fluid; is the specific weight of the wetting liquid; is the magnitude of the gravitational acceleration; is the permeability of the fully saturated medium, which can be a function of void ratio (e, common in soil consolidation problems), temperature ( ), and/or field variables ( is the wetting liquid pore pressure; is position; and is the gravitational acceleration. ); Permeability definitions Permeability can be defined in different ways by different authors; caution should, therefore, be used to ensure that the specified input data are consistent with the definitions used in Abaqus/Standard. Permeability in Abaqus/Standard is defined as so that Forchheimer’s law can also be written as The fully saturated permeability, conditions. and/or temperature, , is typically obtained from experiments under low fluid velocity can be defined as a function of void ratio, e, (common in soil consolidation problems) . The void ratio can be derived from the porosity, n, using the relationship . Up to six variables may be needed to define the fully saturated permeability, depending on whether isotropic, orthotropic, or fully anisotropic permeability is to be modeled (discussed below). Alternative definition of permeability Some authors refer to the definition of permeability used in Abaqus/Standard, “hydraulic conductivity” of the porous medium and define the permeability as (units of LT ), as the is the kinematic viscosity of the wetting liquid (the ratio of the liquid’s dynamic viscosity to its (or Darcy). where mass density), g is the magnitude of the gravitational acceleration, and If the permeability is available in this form, it must be converted such that the appropriate values of are used in Abaqus/Standard. has dimensions Specifying the permeability Permeability in Abaqus/Standard can be isotropic, orthotropic, or fully anisotropic. For non-isotropic permeability a local orientation must be used to specify the material directions. Isotropic permeability For isotropic permeability in Abaqus/Standard define one value of the fully saturated permeability at each value of the void ratio. Input File Usage: Abaqus/CAE Usage: *PERMEABILITY, TYPE=ISOTROPIC Property module: material editor: Other→Pore Fluid→Permeability: Type: Isotropic Orthotropic permeability For orthotropic permeability in Abaqus/Standard define three values of the fully saturated permeability ( ) at each value of the void ratio. , and , Input File Usage: Abaqus/CAE Usage: *PERMEABILITY, TYPE=ORTHOTROPIC Property module: material editor: Other→Pore Fluid→Permeability: Type: Orthotropic Anisotropic permeability For fully anisotropic permeability in Abaqus/Standard define six values of the fully saturated permeability ( ) at each value of the void ratio. , and , , , , Input File Usage: Abaqus/CAE Usage: *PERMEABILITY, TYPE=ANISOTROPIC Property module: material editor: Other→Pore Fluid→Permeability: Type: Anisotropic Velocity coefficient Abaqus/Standard assumes that law is required ( Input File Usage: must be defined in tabular form. ), *PERMEABILITY, TYPE=VELOCITY by default, meaning that Darcy’s law is used. If Forchheimer’s This must be a repeated use of the *PERMEABILITY option for the same material, since must also be defined. Abaqus/CAE Usage: Property module: material editor: Other→Pore Fluid→Permeability: Suboptions→Velocity Dependence Saturation dependence In Abaqus/Standard you can define the dependence of permeability, ; . Abaqus/Standard assumes by default that for must specify definition of for . , on saturation, s, by specifying . The tabular for Input File Usage: *PERMEABILITY, TYPE=SATURATION This must be a repeated use of the *PERMEABILITY option for the same material, since must also be defined. Abaqus/CAE Usage: Property module: material editor: Other→Pore Fluid→Permeability: Suboptions→Saturation Dependence Specific weight of the wetting liquid In Abaqus/Standard the specific weight of the fluid, does not consider the weight of the wetting liquid (i.e., if excess pore fluid pressure is calculated). *PERMEABILITY, TYPE=type, SPECIFIC= , must be specified correctly even if the analysis Input File Usage: Abaqus/CAE Usage: The SPECIFIC parameter must be defined in conjunction with the fully saturated *PERMEABILITY option for a given medium. Property module: material editor: Other→Pore Fluid→Permeability: Specific weight of wetting liquid: Permeability in Abaqus/CFD For flows in fluid-saturated porous medium, the momentum equation in its simplest form can be written as where the first term on the right-hand side is the Darcy drag and the second term is the inertial drag (also called form drag or Forchheimer drag). In the above equation is the intrinsic average of the pressure (average taken over the fluid-phase only); is the extrinsic or superficial velocity vector, where the average is taken over a representative volume incorporating both the solid (matrix) and the fluid phases; is the density of the fluid; is the viscosity of the fluid; is the permeability of the porous medium (units of L2 ); and is the dimensionless inertial or form drag coefficient and, in general, is a function of the porosity . The inertial drag coefficient, relation is used, which is given by , is usually a function of the porosity . In Abaqus/CFD the Ergun’s where the constant is set by default as . A widely used model to specify the permeability as a function of porosity is the Carman-Kozeny relation, which is given by where represents the average radius of the porous particles/fibers. represents the Carman-Kozeny constant (parameter that is geometry dependent) and Specifying the permeability Permeability in Abaqus/CFD can be isotropic (with dependence only on porosity) or specified using a Carman-Kozeny relation. Isotropic permeability For isotropic permeability define one value of the fully saturated permeability at each value of the porosity. Input File Usage: *PERMEABILITY, TYPE=ISOTROPIC Abaqus/CAE Usage: Property module: material editor: Other→Pore Fluid→Permeability: Type: Isotropic (CFD) Carman-Kozeny model For the Carman-Kozeny relation, you can define the permeability Kozeny constant, and by specifying , the Carman- , the average pore-particle/fiber radius. *PERMEABILITY, TYPE=CARMAN KOZENY Property module: material editor: Other→Pore Fluid→Permeability: Type: Carman-Kozeny Input File Usage: Abaqus/CAE Usage: Inertial drag coefficient The value of the constant user-specified value. By default, the value of in the expression for the inertial drag coefficient, is 0.142887. , can be set to any Input File Usage: Abaqus/CAE Usage: *PERMEABILITY, TYPE=type, INERTIAL DRAG COEFFICIENT= Property module: material editor: Other→Pore Fluid→Permeability: Inertial drag coefficient: Elements In Abaqus/Standard permeability can be used only in elements that allow for pore pressure . Permeability can be used with any fluid element in Abaqus/CFD. 26.6.3 POROUS BULK MODULI Products: Abaqus/Standard Abaqus/CAE References • “Pore fluid flow properties,” Section 26.6.1 • “Material library: overview,” Section 21.1.1 • *POROUS BULK MODULI • “Defining porous bulk moduli” in “Defining a fluid-filled porous material,” Section 12.12.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The porous bulk moduli: • must be defined whenever the compressibility of the solid grains or the compressibility of the permeating fluid is to be considered in the analysis of a porous medium; and • must be defined when a swelling gel is modeled (“Moisture swelling,” Section 26.6.6). Defining porous bulk moduli You can specify the bulk modulus of the solid grains and the bulk modulus of the fluid as functions of temperature. If either modulus is omitted or set to zero, that phase of the material is assumed to be fully incompressible. Input File Usage: Abaqus/CAE Usage: *POROUS BULK MODULI Property module: material editor: Other→Pore Fluid→Porous Bulk Moduli Elements The porous bulk moduli can be defined only for elements that allow for pore pressure . 26.6.4 SORPTION Products: Abaqus/Standard Abaqus/CAE References • “Pore fluid flow properties,” Section 26.6.1 • “Material library: overview,” Section 21.1.1 • *SORPTION • “Defining sorption” in “Defining a fluid-filled porous material,” Section 12.12.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Sorption: • defines a porous material’s absorption/exsorption behavior under partially saturated flow conditions; and • is used in the analysis of coupled wetting liquid flow and porous medium stress (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). Sorption represent capillary effects in the medium. For A porous medium becomes partially saturated when the total pore liquid pressure, , becomes negative . Negative values of it is known that the saturation lies within certain limits that depend on the value of the capillary pressure, . Typical forms of these limits are shown in Figure 26.6.4–1. We write these limits as is the limit at which exsorption is the limit at which absorption will occur (so that will occur (so that ). The transition between absorption and exsorption and vice versa takes place along “scanning” curves (discussed below). These curves are approximated by the single straight line shown in Figure 26.6.4–1. , where ), and When partial saturation is included in the analysis of flow through a porous medium, the absorption behavior, the exsorption behavior, and the scanning behavior (between absorption and exsorption) should each be defined. Each of these behaviors is discussed below. If sorption is not defined at all, Abaqus/Standard assumes fully saturated flow ( ) for all values of . Strongly unsymmetric partially saturated flow coupled equations result from the definition of sorption. Therefore, Abaqus/Standard automatically uses its unsymmetric matrix storage and solution scheme if you request partially saturated analysis (i.e., if sorption is defined). pore pressure -uw exsorption absorption scanning 0.0 1.0 saturation Figure 26.6.4–1 Typical absorption and exsorption behaviors. Defining absorption and exsorption Absorption and exsorption behaviors are defined by specifying the pore liquid pressure, (negative “capillary tension”), as a function of saturation. In most physical cases the wetting liquid cannot be driven to zero saturation; to achieve zero saturation, the data would have to define . Absorption and exsorption data can be defined in either a tabular form or an analytical form. as Tabular form By default, you define the absorption and exsorption behaviors by specifying s, where . as a tabular function of Input File Usage: Use the following options: *SORPTION, TYPE=ABSORPTION, LAW=TABULAR *SORPTION, TYPE=EXSORPTION, LAW=TABULAR If the *SORPTION option is used only once, the behavior defined is taken as the behavior for absorption and exsorption. Abaqus/CAE Usage: Property module: material editor: Other→Pore Fluid→Sorption Absorption: Law: Tabular Exsorption: toggle on Include exsorption: Law: Tabular Analytical form The absorption and exsorption behaviors can be defined by the following analytical form: where the saturation values of interest . are positive material constants and are parameters used to define the lower bound of -uw -uw s0 -uw s1 duw ds s1 0.0 s0 s1 1.0 Figure 26.6.4–2 Logarithmic form of absorption and exsorption behaviors. Input File Usage: Use the following options: *SORPTION, TYPE=ABSORPTION, LAW=LOG *SORPTION, TYPE=EXSORPTION, LAW=LOG If the *SORPTION option is used only once, the behavior defined is taken as the behavior for absorption and exsorption. Abaqus/CAE Usage: Property module: material editor: Other→Pore Fluid→Sorption Absorption: Law: Log Exsorption: toggle on Include exsorption: Law: Log Defining the behavior between absorption and exsorption The behavior between absorption and exsorption is defined by a scanning line of user-specified constant slope, . This slope should be larger than the slope of any segment of the absorption or exsorption behaviors. If absorption and exsorption behaviors are defined with no scanning line, the slope of the scanning given in the absorption and exsorption behavior line is taken as 1.05 times the largest value of definitions. Input File Usage: Abaqus/CAE Usage: *SORPTION, TYPE=SCANNING This must be a repeated use of the *SORPTION option for the same material. Property module: material editor: Other→Pore Fluid→Sorption: Exsorption: toggle on Include exsorption and Include scanning: Slope Elements Sorption can be used only in elements that allow for pore pressure . 26.6.5 SWELLING GEL Products: Abaqus/Standard Abaqus/CAE References • “Pore fluid flow properties,” Section 26.6.1 • “Material library: overview,” Section 21.1.1 • *GEL • “Defining a swelling gel” in “Defining a fluid-filled porous material,” Section 12.12.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The swelling gel model: • allows for modeling of the growth of gel particles that swell and trap wetting liquid in a partially saturated porous medium; • is intended for use in moisture absorption problems, which typically involve polymeric materials, such as in the analysis of diapers; and • can be used in the analysis of coupled pore liquid flow and porous medium stress . Swelling gel model The simple swelling gel model is based on the idealization of a gel as a volume of individual spherical particles of equal radius, . The swelling evolution (discussed in detail in “Constitutive behavior in a porous medium,” Section 2.8.3 of the Abaqus Theory Manual) is assumed to be given by where the value of any grouping of terms in angled brackets result is not positive, and is set equal to zero if its mathematical is the fully swollen radius; is the relaxation time of the gel particles; is the saturation of the surrounding medium; is the radius of the gel particles when they are completely dry; is the maximum radius that the gel particles can achieve before they must touch; is the effective gel radius when the volume is entirely occupied with gel; is the initial porosity of the material; is the volume change in the material; and is the number of gel particles per unit volume. The second term in the definition of gel growth incorporates the assumption that the gel will swell only when the saturation of the surrounding medium, s, exceeds the effective saturation of the gel. The third term in the growth equation reduces the swelling rate when the surface of gel particles exposed to free fluid is limited by the combination of packing density and gel particle radius. The swelling gel model is defined by specifying the variables , , , and . Input File Usage: Abaqus/CAE Usage: *GEL Property module: material editor: Other→Pore Fluid→Gel Elements The swelling gel model can be used only in elements that allow for pore pressure . 26.6.6 MOISTURE SWELLING Products: Abaqus/Standard Abaqus/CAE References • “Pore fluid flow properties,” Section 26.6.1 • “Material library: overview,” Section 21.1.1 • *MOISTURE SWELLING • “Defining moisture swelling” in “Defining a fluid-filled porous material,” Section 12.12.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Moisture swelling: • defines the saturation-driven volumetric swelling of the solid skeleton of a porous medium in partially saturated flow conditions; • can be used in the analysis of coupled wetting liquid flow and porous medium stress ; and • can be either isotropic or anisotropic. Moisture swelling model The moisture swelling model assumes that the volumetric swelling of the porous medium’s solid skeleton is a function of the saturation of the wetting liquid in partially saturated flow conditions. The porous medium is partially saturated when the pore liquid pressure, , is negative . The swelling behavior is assumed to be reversible. The logarithmic measure of swelling strain is calculated with reference to the initial saturation so that (no sum on ) and where typical curve is shown in Figure 26.6.6–1. The ratios discussed below. are the volumetric swelling strains at the current and initial saturations. A allow for anisotropic swelling as , and , Defining volumetric swelling strain Define the volumetric swelling strain, swelling strain must be defined for the range . , as a tabular function of the wetting liquid saturation, s. The Input File Usage: *MOISTURE SWELLING εms εms(s) εms( sΙ) 0.0 sI 1.0 saturation Figure 26.6.6–1 Typical volumetric moisture swelling versus saturation curve. Abaqus/CAE Usage: Property module: material editor: Other→Pore Fluid→Moisture Swelling Defining initial saturation values You can define the initial saturation values as initial conditions. If no initial saturation values are given, the default is fully saturated conditions (saturation of 1.0). For partial saturation the initial saturation and pore fluid pressure must be consistent, in the sense that the pore fluid pressure must lie within the absorption and exsorption values for the initial saturation value . If this is not the case, Abaqus/Standard will adjust the saturation value as needed to satisfy this requirement. *INITIAL CONDITIONS, TYPE=SATURATION Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Saturation for the Types for Selected Step Abaqus/CAE Usage: Input File Usage: Defining anisotropic swelling Anisotropy can be included in moisture swelling behavior by defining the ratios that two or more of the three ratios differ. If the ratios that the swelling is isotropic and that strain directions depends on the user-specified local orientation . , such are not specified, Abaqus/Standard assumes . The orientation of the moisture swelling , and , Input File Usage: Use both of the following options: *MOISTURE SWELLING *RATIOS The *RATIOS option should immediately follow the *MOISTURE SWELLING option. Abaqus/CAE Usage: Property module: material editor: Other→Pore Fluid→Moisture Swelling: Suboptions→Ratios Elements The moisture swelling model can be used only in elements that allow for pore pressure . 26.7 User materials • “User-defined mechanical material behavior,” Section 26.7.1 • “User-defined thermal material behavior,” Section 26.7.2 26.7.1 USER-DEFINED MECHANICAL MATERIAL BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “UMAT,” Section 1.1.40 of the Abaqus User Subroutines Reference Manual • “VUMAT,” Section 1.2.17 of the Abaqus User Subroutines Reference Manual • *USER MATERIAL • *DEPVAR • “Specifying solution-dependent state variables,” Section 12.8.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining constants for a user material,” Section 12.8.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview User-defined mechanical material behavior in Abaqus: • is provided by means of an interface whereby any mechanical constitutive model can be added to the library; • requires that a constitutive model (or a library of models) is programmed in user subroutine UMAT (Abaqus/Standard) or VUMAT (Abaqus/Explicit); and • requires considerable effort and expertise: the feature is very general and powerful, but its use is not a routine exercise. Stress components and strain increments The subroutine interface has been implemented using Cauchy stress components (“true” stress). For soils problems “stress” should be interpreted as effective stress. The strain increments are defined by the symmetric part of the displacement increment gradient (equivalent to the time integral of the symmetric part of the velocity gradient). The orientation of the stress and strain components in user subroutine UMAT depends on the use of local orientations (“Orientations,” Section 2.2.5). In user subroutine VUMAT all strain measures are calculated with respect to the midincrement configuration. All tensor quantities are defined in the corotational coordinate system that rotates with the material point. To illustrate what this means in terms of stresses, consider the bar shown in Figure 26.7.1–1, which is stretched and rotated from its original configuration, , to its new position, . This deformation can be obtained in two stages; the bar is first stretched, as shown in Figure 26.7.1–2, and is then rotated by applying a rigid body rotation to it, as shown in Figure 26.7.1–3. The stress in the bar after it has been stretched is , and this stress does not change during the rigid body rotation. The coordinate system that rotates as a result of the rigid body rotation is the A Figure 26.7.1–1 Stretched and rotated bar. 11 11 Figure 26.7.1–2 Stretching of bar. 11 11 Figure 26.7.1–3 Rigid body rotation of bar. corotational coordinate system. The stress tensor and state variables are, therefore, computed directly and updated in user subroutine VUMAT using the strain tensor since all of these quantities are in the corotational system; these quantities do not have to be rotated by the user subroutine as is sometimes required in user subroutine UMAT. The elastic response predicted by a rate-form constitutive law depends on the objective stress rate employed. For example, the Green-Naghdi stress rate is used in VUMAT. However, the stress rate used for built-in material models may differ. For example, most material models used with solid (continuum) elements in Abaqus/Explicit employ the Jaumann stress rate. This difference in the formulation will cause significant differences in the results only if finite rotation of a material point is accompanied by finite shear. For a discussion of the objective stress rates used in Abaqus, see “Stress rates,” Section 1.5.3 of the Abaqus Theory Manual. Material constants Any material constants that are needed in user subroutine UMAT or VUMAT must be specified as part of a user-defined material behavior definition. Any other mechanical material behaviors included in the same material definition (except thermal expansion and, in Abaqus/Explicit, density) will be ignored; the user- defined material behavior requires that all mechanical material behavior calculations be programmed in subroutine UMAT or VUMAT. In Abaqus/Explicit the density (“Density,” Section 21.2.1) is required when using a user-defined material behavior. Input File Usage: In Abaqus/Standard use the following option to specify a user-defined material behavior: *USER MATERIAL, TYPE=MECHANICAL, CONSTANTS=number_of_constants In Abaqus/Explicit use both of the following options to specify a user-defined material behavior: *USER MATERIAL, CONSTANTS=number_of_constants *DENSITY In either case you must specify the number of material constants being entered. Abaqus/CAE Usage: In Abaqus/Standard use the following option to specify a user-defined material behavior: Property module: material editor: General→User Material: User material type: Mechanical In Abaqus/Explicit use both of the following options to specify a user-defined material behavior: Property module: material editor: General→User Material: User material type: Mechanical General→Density Unsymmetric equation solver in Abaqus/Standard If the user material’s Jacobian matrix, capability in Abaqus/Standard should be invoked . , is not symmetric, the unsymmetric equation solution Input File Usage: *USER MATERIAL, TYPE=MECHANICAL, CONSTANTS=number_of_constants, UNSYMM Abaqus/CAE Usage: Property module: material editor: General→User Material: User material type: Mechanical, toggle on Use unsymmetric material stiffness matrix Material state Many mechanical constitutive models require the storage of solution-dependent state variables (plastic strains, “back stress,” saturation values, etc. in rate constitutive forms or historical data for theories written in integral form). You should allocate storage for these variables in the associated material definition . There is no restriction on the number of state variables associated with a user-defined material. The user material subroutines are provided with the material state at the start of each increment, as described below. They must return values for the new stresses and the new internal state variables. State variables associated with UMAT and VUMAT can be output to the output database file (.odb) and results file (.fil) using the output identifiers SDV and SDVn . Material state in Abaqus/Standard User subroutine UMAT is called for each material point at each iteration of every increment. It is provided with the material state at the start of the increment (stress, solution-dependent state variables, temperature, and any predefined field variables) and with the increments in temperature, predefined state variables, strain, and time. In addition to updating the stresses and the solution-dependent state variables to their values at the end of the increment, subroutine UMAT must also provide the material Jacobian matrix, , for the mechanical constitutive model. This matrix will also depend on the integration scheme used if the constitutive model is in rate form and is integrated numerically in the subroutine. For any nontrivial constitutive model these will be challenging tasks. For example, the accuracy with which the Jacobian matrix is defined will usually be a major determinant of the convergence rate of the solution and, therefore, will have a strong influence on computational efficiency. Material state in Abaqus/Explicit User subroutine VUMAT is called for blocks of material points at each increment. When the subroutine is called, it is provided with the state at the start of the increment (stress, solution-dependent state variables). It is also provided with the stretches and rotations at the beginning and the end of the increment. The VUMAT user material interface passes a block of material points to the subroutine on each call, which allows vectorization of the material subroutine. The temperature is provided to user subroutine VUMAT at the start and the end of the increment. The temperature is passed in as information only and cannot be modified, even in a fully coupled thermal- stress analysis. However, if the inelastic heat fraction is defined in conjunction with the specific heat and conductivity in a fully coupled thermal-stress analysis in Abaqus/Explicit, the heat flux due to inelastic energy dissipation will be calculated automatically. If the VUMAT user subroutine is used to define an adiabatic material behavior (conversion of plastic work to heat) in an explicit dynamics procedure, you must specify both the inelastic heat fraction and the specific heat for the material, and you must store the temperatures and integrate them as user-defined state variables. Most often the temperatures are provided by specifying initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) and are constant throughout the analysis. Deleting elements from an Abaqus/Explicit mesh using state variables Element deletion in a mesh can be controlled during the course of an Abaqus/Explicit analysis through user subroutine VUMAT. Deleted elements have no ability to carry stresses and, therefore, have no contribution to the stiffness of the model. You specify the state variable number controlling the element deletion flag. For example, specifying a state variable number of 4 indicates that the fourth state variable is the deletion flag in VUMAT. The deletion state variable should be set to a value of one or zero in VUMAT. A value of one indicates that the material point is active, while a value of zero indicates that Abaqus/Explicit should delete the material point from the model by setting the stresses to zero. The structure of the block of material points passed to user subroutine VUMAT remains unchanged during the analysis; deleted material points are not removed from the block. Abaqus/Explicit will pass zero stresses and strain increments for all deleted material points. Once a material point has been flagged as deleted, it cannot be reactivated. An element will be deleted from the mesh only after all of the material points in the element are deleted. The status of an element can be determined by requesting output of the variable STATUS. This variable is equal to one if the element is active and equal to zero if the element is deleted. Input File Usage: Abaqus/CAE Usage: *DEPVAR, DELETE=variable number Property module: material editor: General→Depvar: Variable number controlling element deletion: variable number Hourglass control and transverse shear stiffness Normally the default hourglass control stiffness for reduced-integration elements in Abaqus/Standard and the transverse shear stiffness for shell, pipe, and beam elements are defined based on the elasticity associated with the material (“Section controls,” Section 27.1.4; “Shell section behavior,” Section 29.6.4; and “Choosing a beam element,” Section 29.3.3). These stiffnesses are based on a typical value of the initial shear modulus of the material, which may, for example, be given as part of an elastic material behavior (“Linear elastic behavior,” Section 22.2.1) included in the material definition. However, the shear modulus is not available during the preprocessing stage of input for materials defined with user subroutine UMAT or VUMAT. Therefore, you must provide the hourglass stiffness parameters when using UMAT to define the material behavior of elements with hourglassing modes; and you must specify the transverse shear stiffness when using UMAT or VUMAT to define the material behavior of beams and shells with transverse shear flexibility. Use of UMAT with other subroutines Various utility subroutines are also available in Abaqus/Standard for use with subroutine UMAT. These utility subroutines are discussed in “Obtaining stress invariants, principal stress/strain values and directions, and rotating tensors in an Abaqus/Standard analysis,” Section 2.1.11 of the Abaqus User Subroutines Reference Manual. User subroutine UMATHT can be used in conjunction with UMAT to define the constitutive thermal behavior of the material. The solution-dependent variables allocated in the material definition are accessible in both UMAT and UMATHT. In addition, user subroutines FRIC, GAPCON, and GAPELECTR are available for defining mechanical, thermal, and electrical interactions between surfaces. Use with other material models A number of material behaviors can be used in the definition of a material when its mechanical behavior is defined by user subroutine UMAT or VUMAT. These behaviors include density, thermal expansion, permeability, and heat transfer properties. Thermal expansion can alternatively be an integral part of the constitutive model implemented in UMAT or VUMAT. The temperature available in UMAT is always the interpolated temperature field at the element integration points. Naturally, if the thermal expansion behavior is implemented in UMAT, it is defined in terms of the integration point temperature. When the temperature field is interpolated differently within an element compared to the displacement field in Abaqus/Standard, implementing the thermal expansion behavior in UMAT may lead to differences compared to the built-in thermal expansion behavior. This situation commonly arises for coupled temperature-displacement elements. For example, for first-order coupled temperature-displacement elements, the built-in thermal expansion behavior uses a constant temperature field over the whole element , while the behavior in UMAT will be defined in terms of a linear temperature field. For a material defined by user subroutine UMAT or VUMAT, mass proportional damping can be included separately , but stiffness proportional damping must be defined in the user subroutine by the Jacobian (Abaqus/Standard only) and stress definitions. Stiffness proportional damping cannot be specified if the user material is used in the direct steady-state dynamics procedure. Elements User subroutines UMAT and VUMAT can be used with all elements in Abaqus that include mechanical behavior (elements that have displacement degrees of freedom). 26.7.2 USER-DEFINED THERMAL MATERIAL BEHAVIOR Products: Abaqus/Standard Abaqus/CAE References • “UMATHT,” Section 1.1.41 of the Abaqus User Subroutines Reference Manual • *USER MATERIAL • *DEPVAR • “Defining constants for a user material,” Section 12.8.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview User-defined thermal material behavior in Abaqus/Standard: • is provided by means of an interface whereby any thermal constitutive model can be added to the library; • requires that a constitutive model (or a library of models) is programmed in user subroutine UMATHT; and • requires considerable effort and expertise: the feature is very general and powerful, but its use is not a routine exercise. Material constants Any material constants that are needed in user subroutine UMATHT must be specified as part of a user- defined thermal material behavior definition. Any other thermal material behaviors included in the same material definition will be ignored: the user-defined thermal material behavior requires that all thermal behavior calculations are programmed in user subroutine UMATHT. Input File Usage: *USER MATERIAL, TYPE=THERMAL, CONSTANTS=number_of_constants You must specify the number of constants being entered. Abaqus/CAE Usage: Property module: material editor: General→User Material: User material type: Thermal Unsymmetric equation solver When the conductivity is defined in user subroutine UMATHT as a strong function of temperature, the heat transfer equilibrium equations become nonsymmetric and you may choose to invoke the unsymmetric equation solution capability; otherwise, convergence may be poor. Input File Usage: *USER MATERIAL, TYPE=THERMAL, CONSTANTS=number_of_constants, UNSYMM Abaqus/CAE Usage: Property module: material editor: General→User Material: User material type: Thermal, toggle on Use unsymmetric material stiffness matrix Material state Many thermal constitutive models require the storage of solution-dependent state variables. These state variables might include microstructure or phase content information when the material undergoes phase changes. You should allocate storage for these variables in the associated material definition . There is no restriction on the number of state variables associated with a user-defined material. User subroutine UMATHT is called for each material point at each iteration of every increment. It is provided with the thermal state of the material at the start of the increment (solution-dependent state variables, temperature, and any predefined field variables) and with the increments in temperature, predefined state variables, and time. Required calculations Subroutine UMATHT must perform the following functions: it must define the internal energy per unit mass and its variation with temperature and spatial gradients of temperature; it must define the heat flux vector and its variation with respect to temperature and spatial gradients of temperature; and it must update the solution-dependent state variables to their values at the end of the increment. The components of the heat flux and spatial gradients in user subroutine UMATHT are in directions that depend on the use of local orientations . Use with other user subroutines User subroutine UMAT can be used in conjunction with UMATHT to define the constitutive mechanical behavior of the material. The solution-dependent variables allocated in the material definition are accessible in both UMATHT and UMAT. In addition, user subroutines FRIC, GAPCON, and GAPELECTR are available for defining mechanical, thermal, and electrical interactions between surfaces. Use with other material models Density, mechanical properties, and electrical properties can be included in the definition of a material whose constitutive thermal behavior is defined by user subroutine UMATHT. Elements User subroutine UMATHT can be used with all elements in Abaqus/Standard that include thermal behavior (elements with temperature degrees of freedom such as pure heat transfer, coupled thermal-stress, and coupled thermal-electrical elements). SIMULIA is the Dassault Systèmes brand that delivers a scalable portfolio of Realistic Simulation solutions including the Abaqus product suite for Unified Finite Element Analysis; multiphysics solutions for insight into challenging engineering problems; and lifecycle management solutions for managing simulation data, processes, and intellectual property. By building on established technology, respected quality, and superior customer service, SIMULIA makes realistic simulation an integral business practice that improves product performance, reduces physical prototypes, and drives innovation. Headquartered in Providence, RI, USA, with R&D centers in Providence and in Vélizy, France, SIMULIA provides sales, services, and support through a global network of regional offices and distributors. For more information, visit www.simulia.com. About Dassault Systèmes As a world leader in 3D and Product Lifecycle Management (PLM) solutions, Dassault Systèmes brings value to more than 100,000 customers in 80 countries. A pioneer in the 3D software market since 1981, Dassault Systèmes develops and markets PLM application software and services that support industrial processes and provide a 3D vision of the entire lifecycle of products from conception to maintenance to recycling. The Dassault Systèmes portfolio consists of CATIA for designing the virtual product, SolidWorks for 3D mechanical design, DELMIA for virtual production, SIMULIA for virtual testing, ENOVIA for global collaborative lifecycle management, and 3DVIA for online 3D lifelike experiences. Dassault Systèmes’ shares are listed on Euronext Paris (#13065, DSY.PA), and Dassault Systèmes’ ADRs may be traded on the US Over-The-Counter (OTC) market (DASTY). For more information, visit www.3ds.com. fi , , , , , , , , . . , © . , , . / User’s Manual CAUTION: This documentation is intended for qualified users who will exercise sound engineering judgment and expertise in the use of the Abaqus Software. The Abaqus Software is inherently complex, and the examples and procedures in this documentation are not intended to be exhaustive or to apply to any particular situation. Users are cautioned to satisfy themselves as to the accuracy and results of their analyses. Dassault Systèmes and its subsidiaries, including Dassault Systèmes Simulia Corp., shall not be responsible for the accuracy or usefulness of any analysis performed using the Abaqus Software or the procedures, examples, or explanations in this documentation. Dassault Systèmes and its subsidiaries shall not be responsible for the consequences of any errors or omissions that may appear in this documentation. The Abaqus Software is available only under license from Dassault Systèmes or its subsidiary and may be used or reproduced only in accordance with the terms of such license. This documentation is subject to the terms and conditions of either the software license agreement signed by the parties, or, absent such an agreement, the then current software license agreement to which the documentation relates. This documentation and the software described in this documentation are subject to change without prior notice. No part of this documentation may be reproduced or distributed in any form without prior written permission of Dassault Systèmes or its subsidiary. The Abaqus Software is a product of Dassault Systèmes Simulia Corp., Providence, RI, USA. © Dassault Systèmes, 2012 Abaqus, the 3DS logo, SIMULIA, CATIA, and Unified FEA are trademarks or registered trademarks of Dassault Systèmes or its subsidiaries in the United States and/or other countries. Other company, product, and service names may be trademarks or service marks of their respective owners. For additional information concerning SIMULIA European Headquarters Fax: +1 401 276 4408, simulia.support@3ds.com, http://www.simulia.com Stationsplein 8-K, 6221 BT Maastricht, The Netherlands, Tel: +31 43 7999 084, Fax: +31 43 7999 306, simulia.europe.info@3ds.com Locations United States Australia Austria Benelux Canada China Finland France Germany India Italy Japan Korea Latin America Scandinavia United Kingdom Argentina Brazil Czech & Slovak Republics Greece Israel Malaysia Mexico New Zealand Poland Russia, Belarus & Ukraine Singapore South Africa Spain & Portugal Dassault Systèmes’ Centers of Simulation Excellence Fremont, CA, Tel: +1 510 794 5891, simulia.west.support@3ds.com West Lafayette, IN, Tel: +1 765 497 1373, simulia.central.support@3ds.com Northville, MI, Tel: +1 248 349 4669, simulia.greatlakes.info@3ds.com Woodbury, MN, Tel: +1 612 424 9044, simulia.central.support@3ds.com Mayfield Heights, OH, Tel: +1 216 378 1070, simulia.erie.info@3ds.com Mason, OH, Tel: +1 513 275 1430, simulia.central.support@3ds.com Warwick, RI, Tel: +1 401 739 3637, simulia.east.support@3ds.com Lewisville, TX, Tel: +1 972 221 6500, simulia.south.info@3ds.com Richmond VIC, Tel: +61 3 9421 2900, simulia.au.support@3ds.com Vienna, Tel: +43 1 22 707 200, simulia.at.info@3ds.com Maarssen, The Netherlands, Tel: +31 346 585 710, simulia.benelux.support@3ds.com Toronto, ON, Tel: +1 416 402 2219, simulia.greatlakes.info@3ds.com Beijing, P. R. China, Tel: +8610 6536 2288, simulia.cn.support@3ds.com Shanghai, P. R. China, Tel: +8621 3856 8000, simulia.cn.support@3ds.com Espoo, Tel: +358 40 902 2973, simulia.nordic.info@3ds.com Velizy Villacoublay Cedex, Tel: +33 1 61 62 72 72, simulia.fr.support@3ds.com Aachen, Tel: +49 241 474 01 0, simulia.de.info@3ds.com Munich, Tel: +49 89 543 48 77 0, simulia.de.info@3ds.com Chennai, Tamil Nadu, Tel: +91 44 43443000, simulia.in.info@3ds.com Lainate MI, Tel: +39 02 3343061, simulia.ity.info@3ds.com Tokyo, Tel: +81 3 5442 6302, simulia.jp.support@3ds.com Osaka, Tel: +81 6 7730 2703, simulia.jp.support@3ds.com Mapo-Gu, Seoul, Tel: +82 2 785 6707/8, simulia.kr.info@3ds.com Puerto Madero, Buenos Aires, Tel: +54 11 4312 8700, Horacio.Burbridge@3ds.com Stockholm, Sweden, Tel: +46 8 68430450, simulia.nordic.info@3ds.com Warrington, Tel: +44 1925 830900, simulia.uk.info@3ds.com Authorized Support Centers SMARTtech Sudamerica SRL, Buenos Aires, Tel: +54 11 4717 2717 KB Engineering, Buenos Aires, Tel: +54 11 4326 7542 Solaer Ingeniería, Buenos Aires, Tel: +54 221 489 1738 SMARTtech Mecânica, Sao Paulo-SP, Tel: +55 11 3168 3388 Synerma s. r. o., Psáry, Prague-West, Tel: +420 603 145 769, abaqus@synerma.cz 3 Dimensional Data Systems, Crete, Tel: +30 2821040012, support@3dds.gr ADCOM, Givataim, Tel: +972 3 7325311, shmulik.keidar@adcomsim.co.il WorleyParsons Services Sdn. Bhd., Kuala Lumpur, Tel: +603 2039 9000, abaqus.my@worleyparsons.com Kimeca.NET SA de CV, Mexico, Tel: +52 55 2459 2635 Matrix Applied Computing Ltd., Auckland, Tel: +64 9 623 1223, abaqus-tech@matrix.co.nz BudSoft Sp. z o.o., Poznań, Tel: +48 61 8508 466, info@budsoft.com.pl TESIS Ltd., Moscow, Tel: +7 495 612 44 22, info@tesis.com.ru WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com Finite Element Analysis Services (Pty) Ltd., Parklands, Tel: +27 21 556 6462, feas@feas.co.za Thailand Turkey Simutech Solution Corporation, Taipei, R.O.C., Tel: +886 2 2507 9550, camilla@simutech.com.tw WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com A-Ztech Ltd., Istanbul, Tel: +90 216 361 8850, info@a-ztech.com.tr Preface Support Both technical engineering support (for problems with creating a model or performing an analysis) and systems support (for installation, licensing, and hardware-related problems) for Abaqus are offered through a network of local support offices. Regional contact information is listed in the front of each Abaqus manual and is accessible from the Locations page at www.simulia.com. Support for SIMULIA products SIMULIA provides a knowledge database of answers and solutions to questions that we have answered, as well as guidelines on how to use Abaqus, SIMULIA Scenario Definition, Isight, and other SIMULIA products. You can also submit new requests for support. All support incidents are tracked. If you contact us by means outside the system to discuss an existing support problem and you know the incident or support request number, please mention it so that we can query the database to see what the latest action has been. Many questions about Abaqus can also be answered by visiting the Products page and the Support page at www.simulia.com. Anonymous ftp site To facilitate data transfer with SIMULIA, an anonymous ftp account is available at ftp.simulia.com. Login as user anonymous, and type your e-mail address as your password. Contact support before placing files on the site. Training All offices and representatives offer regularly scheduled public training classes. The courses are offered in a traditional classroom form and via the Web. We also provide training seminars at customer sites. All training classes and seminars include workshops to provide as much practical experience with Abaqus as possible. For a schedule and descriptions of available classes, see www.simulia.com or call your local office or representative. Feedback We welcome any suggestions for improvements to Abaqus software, the support program, or documentation. We will ensure that any enhancement requests you make are considered for future releases. If you wish to make a suggestion about the service or products, refer to www.simulia.com. Complaints should be made by contacting your local office or through www.simulia.com by visiting the Quality Assurance section of the 1.1.1 1.2.1 1.2.2 1.3.1 1.4.1 2.1.1 2.1.2 2.1.3 2.1.4 2.1.5 2.1.6 2.2.1 2.2.2 2.2.3 2.2.4 2.2.5 2.3.1 2.3.2 2.3.3 2.3.4 Contents Volume I PART I INTRODUCTION, SPATIAL MODELING, AND EXECUTION 1. Introduction Introduction: general Abaqus syntax and conventions Input syntax rules Conventions Abaqus model definition Defining a model in Abaqus Parametric modeling Parametric input 2. Spatial Modeling Node definition Node definition Parametric shape variation Nodal thicknesses Normal definitions at nodes Transformed coordinate systems Adjusting nodal coordinates Element definition Element definition Element foundations Defining reinforcement Defining rebar as an element property Orientations Surface definition Surfaces: overview Element-based surface definition Node-based surface definition Analytical rigid surface definition Eulerian surface definition Operating on surfaces Rigid body definition Rigid body definition Integrated output section definition Integrated output section definition Mass adjustment Adjust and/or redistribute mass of an element set Nonstructural mass definition Nonstructural mass definition Distribution definition Distribution definition Display body definition Display body definition Assembly definition Defining an assembly Matrix definition Defining matrices 3. Job Execution Execution procedures: overview Execution procedure for Abaqus: overview Execution procedures Obtaining information Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution SIMULIA Co-Simulation Engine controller execution Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution Abaqus/CAE execution Abaqus/Viewer execution Python execution Parametric studies Abaqus documentation Licensing utilities ASCII translation of results (.fil) files Joining results (.fil) files Querying the keyword/problem database ii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 2.3.5 2.3.6 2.4.1 2.5.1 2.6.1 2.7.1 2.8.1 2.9.1 2.10.1 2.11.1 3.1.1 3.2.1 3.2.2 3.2.3 3.2.4 3.2.5 3.2.6 3.2.7 3.2.8 3.2.9 3.2.10 Making user-defined executables and subroutines Input file and output database upgrade utility Generating output database reports Joining output database (.odb) files from restarted analyses Combining output from substructures Combining data from multiple output databases Network output database file connector Mapping thermal and magnetic loads Fixed format conversion utility Translating Nastran bulk data files to Abaqus input files Translating Abaqus files to Nastran bulk data files Translating ANSYS input files to Abaqus input files Translating PAM-CRASH input files to partial Abaqus input files Translating RADIOSS input files to partial Abaqus input files Translating Abaqus output database files to Nastran Output2 results files Translating LS-DYNA data files to Abaqus input files Exchanging Abaqus data with ZAERO Encrypting and decrypting Abaqus input data Job execution control Environment file settings Using the Abaqus environment settings Managing memory and disk resources Managing memory and disk use in Abaqus Parallel execution Parallel execution: overview Parallel execution in Abaqus/Standard Parallel execution in Abaqus/Explicit Parallel execution in Abaqus/CFD File extension definitions File extensions used by Abaqus FORTRAN unit numbers FORTRAN unit numbers used by Abaqus CONTENTS 3.2.14 3.2.15 3.2.16 3.2.17 3.2.18 3.2.19 3.2.20 3.2.21 3.2.22 3.2.23 3.2.24 3.2.25 3.2.26 3.2.27 3.2.28 3.2.29 3.2.30 3.2.31 3.2.32 3.2.33 3.3.1 3.4.1 3.5.1 3.5.2 3.5.3 3.5.4 3.6.1 3.7.1 4.1.2 4.1.3 4.1.4 4.2.1 4.2.2 4.2.3 4.3.1 5.1.1 5.1.2 5.1.3 5.1.4 CONTENTS 4. Output PART II OUTPUT Output Output to the data and results files Output to the output database Error indicator output Output variables Abaqus/Standard output variable identifiers Abaqus/Explicit output variable identifiers Abaqus/CFD output variable identifiers The postprocessing calculator The postprocessing calculator 5. File Output Format Accessing the results file Accessing the results file: overview Results file output format Accessing the results file information Utility routines for accessing the results file OI.1 Abaqus/Standard Output Variable Index OI.2 Abaqus/Explicit Output Variable Index OI.3 Abaqus/CFD Output Variable Index 6.1.1 6.1.2 6.1.3 6.1.4 6.1.5 6.1.6 6.2.1 6.2.2 6.2.3 6.2.4 6.2.5 6.2.6 6.2.7 6.3.1 6.3.2 6.3.3 6.3.4 6.3.5 6.3.6 6.3.7 6.3.8 6.3.9 6.3.10 6.3.11 6.4.1 6.5.1 6.5.2 Volume II PART III ANALYSIS PROCEDURES, SOLUTION, AND CONTROL 6. Analysis Procedures Introduction Solving analysis problems: overview Defining an analysis General and linear perturbation procedures Multiple load case analysis Direct linear equation solver Iterative linear equation solver Static stress/displacement analysis Static stress analysis procedures: overview Static stress analysis Eigenvalue buckling prediction Unstable collapse and postbuckling analysis Quasi-static analysis Direct cyclic analysis Low-cycle fatigue analysis using the direct cyclic approach Dynamic stress/displacement analysis Dynamic analysis procedures: overview Implicit dynamic analysis using direct integration Explicit dynamic analysis Direct-solution steady-state dynamic analysis Natural frequency extraction Complex eigenvalue extraction Transient modal dynamic analysis Mode-based steady-state dynamic analysis Subspace-based steady-state dynamic analysis Response spectrum analysis Random response analysis Steady-state transport analysis Steady-state transport analysis Heat transfer and thermal-stress analysis Heat transfer analysis procedures: overview Uncoupled heat transfer analysis 6.5.4 6.6.1 6.6.2 6.7.1 6.7.2 6.7.3 6.7.4 6.7.5 6.7.6 6.8.1 6.8.2 6.9.1 6.10.1 6.11.1 6.12.1 7.1.1 7.2.1 7.2.2 7.2.3 7.2.4 CONTENTS Fully coupled thermal-stress analysis Adiabatic analysis Fluid dynamic analysis Fluid dynamic analysis procedures: overview Incompressible fluid dynamic analysis Electromagnetic analysis Electromagnetic analysis procedures Piezoelectric analysis Coupled thermal-electrical analysis Fully coupled thermal-electrical-structural analysis Eddy current analysis Magnetostatic analysis Coupled pore fluid flow and stress analysis Coupled pore fluid diffusion and stress analysis Geostatic stress state Mass diffusion analysis Mass diffusion analysis Acoustic and shock analysis Acoustic, shock, and coupled acoustic-structural analysis Abaqus/Aqua analysis Abaqus/Aqua analysis Annealing Annealing procedure 7. Analysis Solution and Control Solving nonlinear problems Solving nonlinear problems Analysis convergence controls Convergence and time integration criteria: overview Commonly used control parameters Convergence criteria for nonlinear problems Time integration accuracy in transient problems ANALYSIS TECHNIQUES 8. Analysis Techniques: Introduction Analysis techniques: overview 9. Analysis Continuation Techniques Restarting an analysis Restarting an analysis Importing and transferring results Transferring results between Abaqus analyses: overview Transferring results between Abaqus/Explicit and Abaqus/Standard Transferring results from one Abaqus/Standard analysis to another Transferring results from one Abaqus/Explicit analysis to another 10. Modeling Abstractions Substructuring Using substructures Defining substructures Submodeling Submodeling: overview Node-based submodeling Surface-based submodeling Generating global matrices Generating matrices CONTENTS 8.1.1 9.1.1 9.2.1 9.2.2 9.2.3 9.2.4 10.1.1 10.1.2 10.2.1 10.2.2 10.2.3 10.3.1 Symmetric model generation, results transfer, and analysis of cyclic symmetry models Symmetric model generation Transferring results from a symmetric mesh or a partial three-dimensional mesh to a full three-dimensional mesh Analysis of models that exhibit cyclic symmetry Periodic media analysis Periodic media analysis Meshed beam cross-sections Meshed beam cross-sections vii 10.4.1 10.4.2 10.4.3 10.5.1 Modeling discontinuities as an enriched feature using the extended finite element method Modeling discontinuities as an enriched feature using the extended finite element 10.7.1 11.1.1 11.2.1 11.3.1 11.4.1 11.4.2 11.4.3 11.5.1 11.5.2 11.5.3 11.5.4 11.6.1 11.7.1 11.8.1 12.1.1 12.2.1 12.2.2 12.2.3 12.2.4 method 11. Special-Purpose Techniques Inertia relief Inertia relief Mesh modification or replacement Element and contact pair removal and reactivation Geometric imperfections Introducing a geometric imperfection into a model Fracture mechanics Fracture mechanics: overview Contour integral evaluation Crack propagation analysis Surface-based fluid modeling Surface-based fluid cavities: overview Fluid cavity definition Fluid exchange definition Inflator definition Mass scaling Mass scaling Selective subcycling Selective subcycling Steady-state detection Steady-state detection 12. Adaptivity Techniques Adaptivity techniques: overview Adaptivity techniques ALE adaptive meshing ALE adaptive meshing: overview Defining ALE adaptive mesh domains in Abaqus/Explicit ALE adaptive meshing and remapping in Abaqus/Explicit Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit 12.2.5 12.2.6 12.2.7 12.3.1 12.3.2 12.3.3 12.4.1 13.1.1 13.2.1 13.2.2 13.2.3 14.1.1 14.1.2 14.1.3 14.1.4 15.1.1 15.1.2 16.1.1 16.1.2 16.1.3 17.1.1 17.2.1 Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit Defining ALE adaptive mesh domains in Abaqus/Standard ALE adaptive meshing and remapping in Abaqus/Standard Adaptive remeshing Adaptive remeshing: overview Selection of error indicators influencing adaptive remeshing Solution-based mesh sizing Analysis continuation after mesh replacement Mesh-to-mesh solution mapping 13. Optimization Techniques Structural optimization: overview Structural optimization: overview Optimization models Design responses Objectives and constraints Creating Abaqus optimization models 14. Eulerian Analysis Eulerian analysis Defining Eulerian boundaries Eulerian mesh motion Defining adaptive mesh refinement in the Eulerian domain 15. Particle Methods Smoothed particle hydrodynamic analyses Smoothed particle hydrodynamic analysis Finite element conversion to SPH particles 16. Sequentially Coupled Multiphysics Analyses Predefined fields for sequential coupling Sequentially coupled thermal-stress analysis Predefined loads for sequential coupling 17. Co-simulation Co-simulation: overview Preparing an Abaqus analysis for co-simulation Preparing an Abaqus analysis for co-simulation Co-simulation between Abaqus solvers Abaqus/Standard to Abaqus/Explicit co-simulation Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation 18. Extending Abaqus Analysis Functionality User subroutines and utilities User subroutines: overview Available user subroutines Available utility routines 19. Design Sensitivity Analysis Design sensitivity analysis 20. Parametric Studies Scripting parametric studies Scripting parametric studies Parametric studies: commands aStudy.combine(): Combine parameter samples for parametric studies. aStudy.constrain(): Constrain parameter value combinations in parametric studies. aStudy.define(): Define parameters for parametric studies. aStudy.execute(): Execute the analysis of parametric study designs. aStudy.gather(): Gather the results of a parametric study. aStudy.generate(): Generate the analysis job data for a parametric study. aStudy.output(): Specify the source of parametric study results. aStudy=ParStudy(): Create a parametric study. aStudy.report(): Report parametric study results. aStudy.sample(): Sample parameters for parametric studies. 17.3.1 17.3.2 18.1.1 18.1.2 18.1.3 19.1.1 20.1.1 20.2.1 20.2.2 20.2.3 20.2.4 20.2.5 20.2.6 20.2.7 20.2.8 20.2.9 20.2.10 21.1.1 21.1.2 21.1.3 21.2.1 22.1.1 22.2.1 22.2.2 22.2.3 22.3.1 22.4.1 22.5.1 22.5.2 22.5.3 22.6.1 22.6.2 22.7.1 22.7.2 Volume III PART V MATERIALS 21. Materials: Introduction Introduction Material library: overview Material data definition Combining material behaviors General properties Density 22. Elastic Mechanical Properties Overview Elastic behavior: overview Linear elasticity Linear elastic behavior No compression or no tension Plane stress orthotropic failure measures Porous elasticity Elastic behavior of porous materials Hypoelasticity Hypoelastic behavior Hyperelasticity Hyperelastic behavior of rubberlike materials Hyperelastic behavior in elastomeric foams Anisotropic hyperelastic behavior Stress softening in elastomers Mullins effect Energy dissipation in elastomeric foams Viscoelasticity Time domain viscoelasticity Frequency domain viscoelasticity Nonlinear viscoelasticity Hysteresis in elastomers Parallel network viscoelastic model Rate sensitive elastomeric foams Low-density foams 23. Inelastic Mechanical Properties Overview Inelastic behavior Metal plasticity Classical metal plasticity Models for metals subjected to cyclic loading Rate-dependent yield Rate-dependent plasticity: creep and swelling Annealing or melting Anisotropic yield/creep Johnson-Cook plasticity Dynamic failure models Porous metal plasticity Cast iron plasticity Two-layer viscoplasticity ORNL – Oak Ridge National Laboratory constitutive model Deformation plasticity Other plasticity models Extended Drucker-Prager models Modified Drucker-Prager/Cap model Mohr-Coulomb plasticity Critical state (clay) plasticity model Crushable foam plasticity models Fabric materials Fabric material behavior Jointed materials Jointed material model Concrete Concrete smeared cracking Cracking model for concrete Concrete damaged plasticity xii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 22.8.1 22.8.2 22.9.1 23.1.1 23.2.1 23.2.2 23.2.3 23.2.4 23.2.5 23.2.6 23.2.7 23.2.8 23.2.9 23.2.10 23.2.11 23.2.12 23.2.13 23.3.1 23.3.2 23.3.3 23.3.4 23.3.5 23.4.1 23.5.1 23.7.1 24.1.1 24.2.1 24.2.2 24.2.3 24.3.1 24.3.2 24.3.3 24.4.1 24.4.2 24.4.3 25.1.1 25.2.1 26.1.1 26.1.2 26.1.3 26.1.4 26.2.1 26.2.2 26.2.3 26.2.4 Permanent set in rubberlike materials Permanent set in rubberlike materials 24. Progressive Damage and Failure Progressive damage and failure: overview Progressive damage and failure Damage and failure for ductile metals Damage and failure for ductile metals: overview Damage initiation for ductile metals Damage evolution and element removal for ductile metals Damage and failure for fiber-reinforced composites Damage and failure for fiber-reinforced composites: overview Damage initiation for fiber-reinforced composites Damage evolution and element removal for fiber-reinforced composites Damage and failure for ductile materials in low-cycle fatigue analysis Damage and failure for ductile materials in low-cycle fatigue analysis: overview Damage initiation for ductile materials in low-cycle fatigue Damage evolution for ductile materials in low-cycle fatigue 25. Hydrodynamic Properties Overview Hydrodynamic behavior: overview Equations of state Equation of state 26. Other Material Properties Mechanical properties Material damping Thermal expansion Field expansion Viscosity Heat transfer properties Thermal properties: overview Conductivity Specific heat Latent heat Acoustic properties Acoustic medium Mass diffusion properties Diffusivity Solubility Electromagnetic properties Electrical conductivity Piezoelectric behavior Magnetic permeability Pore fluid flow properties Pore fluid flow properties Permeability Porous bulk moduli Sorption Swelling gel Moisture swelling User materials User-defined mechanical material behavior User-defined thermal material behavior 26.3.1 26.4.1 26.4.2 26.5.1 26.5.2 26.5.3 26.6.1 26.6.2 26.6.3 26.6.4 26.6.5 26.6.6 26.7.1 26.7.2 27.1.1 27.1.2 27.1.3 27.1.4 28.1.1 28.1.2 28.1.3 28.1.4 28.1.5 28.1.6 28.1.7 28.2.1 28.2.2 28.3.1 28.3.2 28.4.1 28.4.2 28.5.1 28.5.2 29.1.1 29.1.2 29.1.3 Volume IV PART VI ELEMENTS 27. Elements: Introduction Element library: overview Choosing the element’s dimensionality Choosing the appropriate element for an analysis type Section controls 28. Continuum Elements General-purpose continuum elements Solid (continuum) elements One-dimensional solid (link) element library Two-dimensional solid element library Three-dimensional solid element library Cylindrical solid element library Axisymmetric solid element library Axisymmetric solid elements with nonlinear, asymmetric deformation Fluid continuum elements Fluid (continuum) elements Fluid element library Infinite elements Infinite elements Infinite element library Warping elements Warping elements Warping element library Particle elements Particle elements Particle element library 29. Structural Elements Membrane elements Membrane elements General membrane element library Cylindrical membrane element library Axisymmetric membrane element library Truss elements Truss elements Truss element library Beam elements Beam modeling: overview Choosing a beam cross-section Choosing a beam element Beam element cross-section orientation Beam section behavior Using a beam section integrated during the analysis to define the section behavior Using a general beam section to define the section behavior Beam element library Beam cross-section library Frame elements Frame elements Frame section behavior Frame element library Elbow elements Pipes and pipebends with deforming cross-sections: elbow elements Elbow element library Shell elements Shell elements: overview Choosing a shell element Defining the initial geometry of conventional shell elements Shell section behavior Using a shell section integrated during the analysis to define the section behavior Using a general shell section to define the section behavior Three-dimensional conventional shell element library Continuum shell element library Axisymmetric shell element library Axisymmetric shell elements with nonlinear, asymmetric deformation 29.1.4 29.2.1 29.2.2 29.3.1 29.3.2 29.3.3 29.3.4 29.3.5 29.3.6 29.3.7 29.3.8 29.3.9 29.4.1 29.4.2 29.4.3 29.5.1 29.5.2 29.6.1 29.6.2 29.6.3 29.6.4 29.6.5 29.6.6 29.6.7 29.6.8 29.6.9 29.6.10 30.1.1 30.1.2 30.2.1 30.2.2 30.3.1 30.3.2 30.4.1 30.4.2 31.1.1 31.1.2 31.1.3 31.1.4 31.1.5 31.2.1 31.2.2 31.2.3 31.2.4 31.2.5 31.2.6 31.2.7 31.2.8 31.2.9 31.2.10 32.1.1 32.1.2 30. Inertial, Rigid, and Capacitance Elements Point mass elements Point masses Mass element library Rotary inertia elements Rotary inertia Rotary inertia element library Rigid elements Rigid elements Rigid element library Capacitance elements Point capacitance Capacitance element library 31. Connector Elements Connector elements Connectors: overview Connector elements Connector actuation Connector element library Connection-type library Connector element behavior Connector behavior Connector elastic behavior Connector damping behavior Connector functions for coupled behavior Connector friction behavior Connector plastic behavior Connector damage behavior Connector stops and locks Connector failure behavior Connector uniaxial behavior 32. Special-Purpose Elements Spring elements Springs Spring element library Dashpot elements Dashpots Dashpot element library Flexible joint elements Flexible joint element Flexible joint element library Distributing coupling elements Distributing coupling elements Distributing coupling element library Cohesive elements Cohesive elements: overview Choosing a cohesive element Modeling with cohesive elements Defining the cohesive element’s initial geometry Defining the constitutive response of cohesive elements using a continuum approach Defining the constitutive response of cohesive elements using a traction-separation description Defining the constitutive response of fluid within the cohesive element gap Two-dimensional cohesive element library Three-dimensional cohesive element library Axisymmetric cohesive element library Gasket elements Gasket elements: overview Choosing a gasket element Including gasket elements in a model Defining the gasket element’s initial geometry Defining the gasket behavior using a material model Defining the gasket behavior directly using a gasket behavior model Two-dimensional gasket element library Three-dimensional gasket element library Axisymmetric gasket element library Surface elements Surface elements General surface element library Cylindrical surface element library Axisymmetric surface element library 32.2.1 32.2.2 32.3.1 32.3.2 32.4.1 32.4.2 32.5.1 32.5.2 32.5.3 32.5.4 32.5.5 32.5.6 32.5.7 32.5.8 32.5.9 32.5.10 32.6.1 32.6.2 32.6.3 32.6.4 32.6.5 32.6.6 32.6.7 32.6.8 32.6.9 32.7.1 32.7.2 32.7.3 32.7.4 32.8.1 32.8.2 32.9.1 32.9.2 32.10.1 32.10.2 32.11.1 32.11.2 32.12.1 32.12.2 32.13.1 32.13.2 32.14.1 32.14.2 32.15.1 32.15.2 Tube support elements Tube support elements Tube support element library Line spring elements Line spring elements for modeling part-through cracks in shells Line spring element library Elastic-plastic joints Elastic-plastic joints Elastic-plastic joint element library Drag chain elements Drag chains Drag chain element library Pipe-soil elements Pipe-soil interaction elements Pipe-soil interaction element library Acoustic interface elements Acoustic interface elements Acoustic interface element library Eulerian elements Eulerian elements Eulerian element library User-defined elements User-defined elements User-defined element library EI.1 Abaqus/Standard Element Index EI.2 Abaqus/Explicit Element Index EI.3 Abaqus/CFD Element Index Volume V PART VII PRESCRIBED CONDITIONS 33. Prescribed Conditions Overview Prescribed conditions: overview Amplitude curves Initial conditions Initial conditions in Abaqus/Standard and Abaqus/Explicit Initial conditions in Abaqus/CFD Boundary conditions Boundary conditions in Abaqus/Standard and Abaqus/Explicit Boundary conditions in Abaqus/CFD Loads Applying loads: overview Concentrated loads Distributed loads Thermal loads Electromagnetic loads Acoustic and shock loads Pore fluid flow Prescribed assembly loads Prescribed assembly loads Predefined fields Predefined fields PART VIII CONSTRAINTS 34. Constraints Overview Kinematic constraints: overview Multi-point constraints Linear constraint equations xx Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 33.1.1 33.1.2 33.2.1 33.2.2 33.3.1 33.3.2 33.4.1 33.4.2 33.4.3 33.4.4 33.4.5 33.4.6 33.4.7 33.5.1 34.2.2 34.2.3 34.3.1 34.3.2 34.3.3 34.3.4 34.4.1 34.5.1 34.6.1 35.1.1 35.2.1 35.2.2 35.2.3 35.2.4 35.2.5 35.2.6 35.3.1 35.3.2 35.3.3 35.3.4 35.3.5 35.3.6 35.3.7 35.3.8 General multi-point constraints Kinematic coupling constraints Surface-based constraints Mesh tie constraints Coupling constraints Shell-to-solid coupling Mesh-independent fasteners Embedded elements Embedded elements Element end release Element end release Overconstraint checks Overconstraint checks PART IX INTERACTIONS 35. Defining Contact Interactions Overview Contact interaction analysis: overview Defining general contact in Abaqus/Standard Defining general contact interactions in Abaqus/Standard Surface properties for general contact in Abaqus/Standard Contact properties for general contact in Abaqus/Standard Controlling initial contact status in Abaqus/Standard Stabilization for general contact in Abaqus/Standard Numerical controls for general contact in Abaqus/Standard Defining contact pairs in Abaqus/Standard Defining contact pairs in Abaqus/Standard Assigning surface properties for contact pairs in Abaqus/Standard Assigning contact properties for contact pairs in Abaqus/Standard Modeling contact interference fits in Abaqus/Standard Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs Adjusting contact controls in Abaqus/Standard Defining tied contact in Abaqus/Standard Extending master surfaces and slide lines Contact modeling if substructures are present Contact modeling if asymmetric-axisymmetric elements are present Defining general contact in Abaqus/Explicit Defining general contact interactions in Abaqus/Explicit Assigning surface properties for general contact in Abaqus/Explicit Assigning contact properties for general contact in Abaqus/Explicit Controlling initial contact status for general contact in Abaqus/Explicit Contact controls for general contact in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit Assigning surface properties for contact pairs in Abaqus/Explicit Assigning contact properties for contact pairs in Abaqus/Explicit Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit Contact controls for contact pairs in Abaqus/Explicit 36. Contact Property Models Mechanical contact properties Mechanical contact properties: overview Contact pressure-overclosure relationships Contact damping Contact blockage Frictional behavior User-defined interfacial constitutive behavior Pressure penetration loading Interaction of debonded surfaces Breakable bonds Surface-based cohesive behavior Thermal contact properties Thermal contact properties Electrical contact properties Electrical contact properties Pore fluid contact properties Pore fluid contact properties 37. Contact Formulations and Numerical Methods Contact formulations and numerical methods in Abaqus/Standard Contact formulations in Abaqus/Standard xxii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 35.3.9 35.3.10 35.4.1 35.4.2 35.4.3 35.4.4 35.4.5 35.5.1 35.5.2 35.5.3 35.5.4 35.5.5 36.1.1 36.1.2 36.1.3 36.1.4 36.1.5 36.1.6 36.1.7 36.1.8 36.1.9 36.1.10 36.2.1 37.1.2 37.1.3 37.2.1 37.2.2 37.2.3 38.1.1 38.1.2 38.2.1 38.2.2 39.1.1 39.2.1 39.2.2 39.3.1 39.3.2 39.4.1 39.4.2 39.5.1 39.5.2 40.1.1 Contact constraint enforcement methods in Abaqus/Standard Smoothing contact surfaces in Abaqus/Standard Contact formulations and numerical methods in Abaqus/Explicit Contact formulation for general contact in Abaqus/Explicit Contact formulations for contact pairs in Abaqus/Explicit Contact constraint enforcement methods in Abaqus/Explicit 38. Contact Difficulties and Diagnostics Resolving contact difficulties in Abaqus/Standard Contact diagnostics in an Abaqus/Standard analysis Common difficulties associated with contact modeling in Abaqus/Standard Resolving contact difficulties in Abaqus/Explicit Contact diagnostics in an Abaqus/Explicit analysis Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit 39. Contact Elements in Abaqus/Standard Contact modeling with elements Contact modeling with elements Gap contact elements Gap contact elements Gap element library Tube-to-tube contact elements Tube-to-tube contact elements Tube-to-tube contact element library Slide line contact elements Slide line contact elements Axisymmetric slide line element library Rigid surface contact elements Rigid surface contact elements Axisymmetric rigid surface contact element library 40. Defining Cavity Radiation in Abaqus/Standard Cavity radiation Printed on: • Chapter 6, “Analysis Procedures” Analysis Procedures Introduction Static stress/displacement analysis Dynamic stress/displacement analysis Steady-state transport analysis Heat transfer and thermal-stress analysis Fluid dynamic analysis Electromagnetic analysis Coupled pore fluid flow and stress analysis Mass diffusion analysis Acoustic and shock analysis Abaqus/Aqua analysis Annealing ANALYSIS PROCEDURES 6.1 6.2 6.3 6.4 6.5 6.6 6.7 6.8 6.9 6.10 6.11 6.1 Introduction • “Solving analysis problems: overview,” Section 6.1.1 • “Defining an analysis,” Section 6.1.2 • “General and linear perturbation procedures,” Section 6.1.3 • “Multiple load case analysis,” Section 6.1.4 • “Direct linear equation solver,” Section 6.1.5 • “Iterative linear equation solver,” Section 6.1.6 6.1.1 SOLVING ANALYSIS PROBLEMS: OVERVIEW Overview A large class of stress analysis problems can be solved with Abaqus/Standard and Abaqus/Explicit. A fundamental division of such problems is into static or dynamic response; dynamic problems are those in which inertia effects are significant. Abaqus/CFD solves a broad range of incompressible flow problems. An analysis problem history is defined using steps in Abaqus (“Defining an analysis,” Section 6.1.2). For each step you choose an analysis procedure, which defines the type of analysis to be performed during the step. The available analysis procedures are listed below and described in more detail in the referenced sections. Abaqus provides multiphysics capabilities using built-in fully coupled procedures, sequential coupling, and co-simulation as solution techniques for multiphysics simulation. An extensive selection of additional analysis techniques that provide powerful tools for performing your Abaqus analyses more efficiently and effectively is available; see Part IV, “Analysis Techniques.” Abaqus/Standard analysis Abaqus/Standard offers complete flexibility in making the distinction between static and dynamic response; the same analysis can contain several static and dynamic phases. Thus, a static preload might be applied, and then the linear or nonlinear dynamic response computed (as in the case of vibrations of a component of a rotating machine or the response of a flexible offshore system that is initially moved to an equilibrium position subject to buoyancy and steady current loads and then is excited by wave loading). Similarly, the static solution can be sought after a dynamic event (by following a dynamic analysis step with a step of static loading). See “Static stress/displacement analysis,” Section 6.2, and “Dynamic stress/displacement analysis,” Section 6.3, for information on these types of procedures. In addition to static and dynamic stress analysis, Abaqus/Standard offers the following analysis types: • “Steady-state transport analysis,” Section 6.4 • “Heat transfer and thermal-stress analysis,” Section 6.5 • “Electromagnetic analysis,” Section 6.7 • “Coupled pore fluid flow and stress analysis,” Section 6.8 • “Mass diffusion analysis,” Section 6.9 • “Acoustic and shock analysis,” Section 6.10 • “Abaqus/Aqua analysis,” Section 6.11 Abaqus/Explicit analysis Abaqus/Explicit solves dynamic response problems using an explicit direct-integration procedure. See “Dynamic stress/displacement analysis,” Section 6.3, for more information on the explicit dynamic procedures available in Abaqus. Abaqus/Explicit also provides heat transfer, acoustic, and annealing analysis capabilities: see “Heat transfer and thermal-stress analysis,” Section 6.5; “Acoustic and shock analysis,” Section 6.10; and “Annealing,” Section 6.12, for details. Abaqus/CFD analysis Abaqus/CFD solves a broad range of incompressible flow problems using a second-order projection method. See “Fluid dynamic analysis,” Section 6.6, for details on the incompressible flow procedures available in Abaqus. Multiphysics analyses Multiphysics is a coupled approach in the numerical solution of multiple interacting physical domains. Abaqus provides built-in fully coupled procedures, sequential coupling, and co-simulation as solution techniques for multiphysics simulation. Built-in fully coupled procedures Native Abaqus multiphysics capabilities solve the physics by adding degrees of freedom representing each of the physical fields and using a single solver. Abaqus provides the following built-in fully coupled procedures to solve multidisciplinary simulations, where all physics fields are computed by Abaqus: • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Coupled thermal-electrical analysis,” Section 6.7.3 • “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4 • “Piezoelectric analysis,” Section 6.7.2 (electrical and mechanical coupling) • “Eddy current analysis,” Section 6.7.5 (electromagnetic) • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 • “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1 • “Eulerian analysis,” Section 14.1.1 Sequential coupling A sequentially coupled multiphysics analysis can be used when the coupling between one or more of the physical fields in a model is only important in one direction. A common example is a thermal-stress analysis in which the temperature field does not depend strongly on the stress field. A typical sequentially coupled thermal-stress analysis consists of two Abaqus/Standard runs: a heat transfer analysis and a subsequent stress analysis. You can perform sequentially coupled multiphysics analyses in Abaqus/Standard as described in the following sections: • “Predefined fields for sequential coupling,” Section 16.1.1 • “Sequentially coupled thermal-stress analysis,” Section 16.1.2 • “Predefined loads for sequential coupling,” Section 16.1.3 Co-simulation The co-simulation technique is a multiphysics capability for run-time coupling of Abaqus and another analysis program. An Abaqus analysis can be coupled to another Abaqus analysis or to a third-party analysis program to perform multidisciplinary simulations and multidomain (multimodel) coupling. The co-simulation technique is described in the following sections: • “Co-simulation: overview,” Section 17.1.1 • “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1 • “Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 17.3.1 • “Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 17.3.2 6.1.2 DEFINING AN ANALYSIS Overview An analysis is defined in Abaqus by: • dividing the problem history into steps; • specifying an analysis procedure for each step; and • prescribing loads, boundary conditions, and output requests for each step. Abaqus distinguishes between general analysis steps and linear perturbation steps, and you can include multiple steps in your analysis. You can control how prescribed conditions are applied throughout each step. In addition, you can specify • the incrementation scheme used for controlling the solution, • the matrix storage and solution scheme in Abaqus/Standard, and • the precision level of the Abaqus/Explicit executable. Defining an analysis An analysis in Abaqus is defined using steps, analysis procedures, and optional history data. Defining steps A basic concept in Abaqus is the division of the problem history into steps. A step is any convenient phase of the history—a thermal transient, a creep hold, a dynamic transient, etc. In its simplest form a step can be just a static analysis in Abaqus/Standard of a load change from one magnitude to another. You can provide a description of each step that will appear in the data (.dat) file; this description is for convenience only. The step definition includes the type of analysis to be performed and optional history data, such as loads, boundary conditions, and output requests. Input File Usage: Abaqus/CAE Usage: Use the first option to begin a step and the second option to end a step: *STEP *END STEP The optional data lines on the *STEP option can be used to specify the step description. The first data line given appears in the data (.dat) file. Step module: Create Step: Description Specifying the analysis procedure For each step you choose an analysis procedure. This choice defines the type of analysis to be performed during the step: static stress analysis, dynamic stress analysis, eigenvalue buckling, transient heat transfer analysis, etc. The available analysis procedures are described in “Solving analysis problems: overview,” Section 6.1.1. Only one procedure is allowed per step. Input File Usage: The procedure definition option must immediately follow the *STEP option. Abaqus/CAE Usage: Step module: Create Step: choose the procedure type Prescribing loads, boundary conditions, and output requests The step definition includes optional history data, such as loads, boundary conditions, and output requests, as defined in “History data” in “Defining a model in Abaqus,” Section 1.3.1. For more information, see “Boundary conditions,” Section 33.3; “Loads,” Section 33.4; and “Output,” Section 4.1. Details for prescribing these conditions are discussed in the individual procedure sections. Input File Usage: Abaqus/CAE Usage: The optional history data are defined following the procedure definition within a *STEP block. You define history data (step-dependent objects) in the Interaction module, Load module, and Step module. General analysis steps versus linear perturbation steps There are two kinds of steps in Abaqus: general analysis steps, which can be used to analyze linear or nonlinear response, and linear perturbation steps, which can be used only to analyze linear problems. General analysis steps can be included in an Abaqus/Standard or Abaqus/Explicit analysis; linear perturbation analysis steps are available only in Abaqus/Standard. In Abaqus/Standard linear analysis is always considered to be linear perturbation analysis about the state at the time when the linear analysis procedure is introduced. This linear perturbation approach allows general application of linear analysis techniques in cases where the linear response depends on preloading or on the nonlinear response history of the model. See “General and linear perturbation procedures,” Section 6.1.3, for more details. Multiple load case analysis In general analysis steps Abaqus/Standard calculates the solution for a single set of applied loads. This is also the default for linear perturbation steps. However, for static, direct steady-state dynamic, and SIM-based steady-state dynamic linear perturbation steps it is possible to find solutions for multiple load cases. See “Multiple load case analysis,” Section 6.1.4, for a description of this capability. Multiple steps The analysis procedure can be changed from step to step in any meaningful way, so you have great flexibility in performing analyses. Since the state of the model (stresses, strains, temperatures, etc.) is updated throughout all general analysis steps, the effects of previous history are always included in the response in each new analysis step. Thus, for example, if natural frequency extraction is performed after a geometrically nonlinear static analysis step, the preload stiffness will be included. Linear perturbation steps have no effect on subsequent general analysis steps. The most obvious reason for using several steps in an analysis is to change analysis procedure type. However, several steps can also be used as a matter of convenience—for example, to change output requests, contact pairs in Abaqus/Explicit, boundary conditions, or loading (any information specified as history, or step-dependent, data). Sometimes an analysis may have progressed to a point where the present step definition needs to be modified. Abaqus provides for this contingency with the restart capability, whereby a step can be terminated prematurely and a new step can be defined for the problem continuation . Optional history data prescribing the loading, boundary conditions, output controls, and auxiliary controls will remain in effect for all subsequent general analysis steps, including those that are defined in a restart analysis, until they are modified or reset. Abaqus will compare all loads and boundary conditions specified in a step with the loads and boundary conditions in effect during the previous step to ensure consistency and continuity. This comparison is expensive if the number of individually specified loads and boundary conditions is very large. Hence, the number of individually specified loads and boundary conditions should be minimized, which can usually be done by using element and node sets instead of individual elements and nodes. For linear perturbation steps only the output controls are continued from one linear perturbation step to the next if there are no intermediate general analysis steps and the output controls are not redefined . Within Abaqus/Standard or Abaqus/Explicit, any combination of available procedures can be used from step to step. However, Abaqus/Standard and Abaqus/Explicit procedures cannot be used in the same analysis. See “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for information on importing results from one type of analysis to another. Defining time varying prescribed conditions By default, Abaqus assumes that external parameters, such as load magnitudes and boundary conditions, are constant (step function) or vary linearly (ramped) over a step, depending on the analysis procedure, as shown in Table 6.1.2–1. Some exceptions in Abaqus/Standard are discussed below. Table 6.1.2–1 Default amplitude variations for time domain procedures. Procedure Default amplitude variation Coupled pore fluid diffusion/stress (steady-state) Coupled pore fluid diffusion/stress (transient) Coupled thermal-electrical (steady-state) Coupled thermal-electrical (transient) Direct-integration dynamic Fully coupled thermal-electrical-structural in Abaqus/Standard (steady-state) Fully coupled thermal-electrical-structural in Abaqus/Standard (transient) Ramp Step Ramp Step Step (exception: Ramp if quasi-static application type is specified) Ramp Step Procedure Default amplitude variation Fully coupled thermal-stress in Abaqus/Standard (steady-state) Fully coupled thermal-stress in Abaqus/Standard (transient) Fully coupled thermal-stress in Abaqus/Explicit Incompressible flow Magnetostatic Mass diffusion (steady-state) Mass diffusion (transient) Quasi-static Static Steady-state transport Transient eddy current Transient modal dynamic Uncoupled heat transfer Uncoupled heat transfer (transient) Ramp Step Step Step Ramp Ramp Step Step Ramp Ramp Step Step Ramp Step No default amplitude variation is defined for a direct cyclic analysis step; for each applied load or boundary condition, the amplitude must be defined explicitly. Additional default amplitude variations in Abaqus/Standard For displacement or rotation degrees of freedom prescribed in Abaqus/Standard using displacement-type boundary conditions or displacement-type connector motions, the default amplitude variation is a ramp function for all procedure types; the default amplitude is a step function for all procedure types when using velocity-type boundary conditions or velocity-type connector motions. For motions prescribed using a predefined displacement field, the default amplitude variation is a ramp function for all procedure types; the default amplitude is a step function when using a predefined velocity field for all procedures except steady-state transport. The default amplitude variation is a step function for fluid flux loading in all procedure types. When a displacement or rotation boundary condition is removed, the corresponding reaction force or moment is reduced to zero according to the amplitude defined for the step. When film or radiation loads are removed, the variation is always a step function. Prescribing nondefault amplitude variations You can define complicated time variations of loadings, boundary conditions, and predefined fields by referring to an amplitude curve in the prescribed condition definition . User subroutines are also provided in Abaqus/Standard and Abaqus/Explicit for coding general loadings . In Abaqus/Standard you can change the default amplitude variation for a step (except the removal of film or radiation loads, as noted above). Input File Usage: In Abaqus/Standard use the following option to change the default amplitude variation for a step: Abaqus/CAE Usage: *STEP, AMPLITUDE=STEP or RAMP In Abaqus/Standard use the following input to change the default amplitude variation for a step: Step module: step editor: Other: Default load variation with time: Instantaneous or Ramp linearly over step Boundary conditions in Abaqus/Explicit Boundary conditions applied during an explicit dynamic response step should use appropriate amplitude references to define the time variation. If boundary conditions are specified for the step without amplitude references, they are applied instantaneously at the beginning of the step. Since Abaqus/Explicit does not admit jumps in displacement, the value of a nonzero displacement boundary condition that is specified without an amplitude reference will be ignored, and a zero velocity boundary condition will be enforced. Prescribing nondefault amplitude variations in transient procedures in Abaqus/Standard The default amplitude is a step function for transient analysis procedures (fully coupled thermal-stress, fully coupled thermal-electrical-structural, coupled thermal-electrical, direct-integration dynamic, uncoupled heat transfer, and mass diffusion). Care should be exercised when the nondefault ramp amplitude variation is specified for transient analysis procedures since unexpected results may occur. For example, if a step of a transient heat transfer analysis uses the ramp amplitude variation and temperature boundary conditions are removed in a subsequent step, the reaction fluxes generated in the previous step will be ramped to zero from their initial values over the duration of the step. Therefore, heat flux will continue to flow through the affected boundary nodes over the entire subsequent step even though the temperature boundary conditions were removed. Incrementation Each step in an Abaqus analysis is divided into multiple increments. In most cases you have two choices for controlling the solution: automatic time incrementation or user-specified fixed time incrementation. Automatic incrementation is recommended for most cases. The methods for selecting automatic or direct incrementation are discussed in the individual procedure sections. The issues associated with time incrementation in Abaqus/Standard, Abaqus/Explicit, and The time increments are generally much smaller in Abaqus/CFD analyses are quite different. Abaqus/Explicit than in Abaqus/Standard, while the time increments for Abaqus/CFD may be similar to those in Abaqus/Standard in many situations. Incrementation in Abaqus/Standard In nonlinear problems Abaqus/Standard will increment and iterate as necessary to analyze a step, depending on the severity of the nonlinearity. In transient cases with a physical time scale, you can provide parameters to indicate a level of accuracy in the time integration, and Abaqus/Standard will choose the time increments to achieve this accuracy. Direct user control is provided because it can sometimes save computational cost in cases where you are familiar with the problem and know a suitable incrementation scheme. Direct control can also occasionally be useful when automatic control has trouble with convergence in nonlinear problems. Specifying the maximum number of increments You can define the upper limit to the number of increments in an Abaqus/Standard analysis. In a direct cyclic analysis procedure, this upper limit should be set to the maximum number of increments in a single loading cycle. The default is 100. The analysis will stop if this maximum is exceeded before the complete solution for the step has been obtained. To arrive at a solution, it is often necessary to increase the number of increments allowed by defining a new upper limit. *STEP, INC=n Step module: step editor: Incrementation: Maximum number of increments Abaqus/CAE Usage: Input File Usage: Extrapolation of the solution In nonlinear analyses Abaqus/Standard uses extrapolation to speed up the solution. Extrapolation refers to the method used to determine the first guess to the incremental solution. The guess is determined by the size of the current time increment and by whether linear, displacement-based parabolic, velocity-based parabolic, or no extrapolation of the previously attained history of each solution variable is chosen. Displacement-based parabolic extrapolation is not relevant for Riks analyses, and velocity-based parabolic extrapolation is available only for direct-integration dynamic procedures. Linear extrapolation (the default for all procedures other than a direct-integration dynamic procedure using the transient fidelity application setting) uses 100% extrapolation (1% for the Riks method) of the previous incremental solution at the start of each increment to begin the nonlinear equation solution for the next increment. No extrapolation is used in the first increment of a step. In some cases extrapolation can cause Abaqus/Standard to iterate excessively; some common examples are abrupt changes in the load magnitudes or boundary conditions and if unloading occurs as a result of cracking (in concrete models) or buckling. In such cases you should suppress extrapolation. Displacement-based parabolic extrapolation uses two previous incremental solutions to obtain the first guess to the current incremental solution. This type of extrapolation is useful in situations when the local variation of the solution with respect to the time scale of the problem is expected to be quadratic, such as the large rotation of structures. If parabolic extrapolation is used in a step, it begins after the second increment of the step: the first increment employs no extrapolation, and the second increment employs linear extrapolation. Consequently, slower convergence rates may occur during the first two increments of the succeeding steps in a multistep analysis. Velocity-based parabolic extrapolation uses the previous displacement incremental solution to It is available only for direct-integration obtain the first guess to the current incremental solution. dynamic procedures, and it is the default if the transient fidelity application setting is specified as part of this procedure . This type of extrapolation is useful in situations with smooth solutions—i.e., when velocities do not display so called “saw tooth” patterns—and in such cases it may provide a better first guess than other extrapolations. If velocity-based parabolic extrapolation is used in a step, it begins after the first increment of the step; the first increment employs initial velocities. Input File Usage: Use the following option to choose linear extrapolation: *STEP, EXTRAPOLATION=LINEAR (default for all procedures other than a direct-integration dynamic procedure using the transient fidelity application setting) Use the following option to choose displacement-based parabolic extrapolation: *STEP, EXTRAPOLATION=PARABOLIC Use the following option to choose velocity-based parabolic extrapolation: *STEP, EXTRAPOLATION=VELOCITY PARABOLIC (default for a direct- integration dynamic procedure using the transient fidelity application setting) Use the following option to choose no extrapolation: *STEP, EXTRAPOLATION= NO Step module: step editor: Other: Extrapolation of previous state at start of each increment: Linear, Parabolic, Velocity parabolic, None, or Analysis product default Abaqus/CAE Usage: Incrementation in Abaqus/Explicit The time increment used in an Abaqus/Explicit analysis must be smaller than the stability limit of the central-difference operator ; failure to use a small enough time increment will result in an unstable solution. Although the time increments chosen by Abaqus/Explicit generally satisfy the stability criterion, user control over the size of the time increment is provided to reduce the chance of a solution going unstable. The small increments characteristic of an explicit dynamic analysis product make Abaqus/Explicit well suited for nonlinear analysis. Severe discontinuities in Abaqus/Standard Abaqus/Standard distinguishes between regular, equilibrium iterations (in which the solution varies smoothly) and severe discontinuity iterations (SDIs) in which abrupt changes in stiffness occur. The most common of such severe discontinuities involve open-close changes in contact and stick-slip changes in friction. By default, Abaqus/Standard will continue to iterate until the severe discontinuities are sufficiently small (or no severe discontinuities occur) and the equilibrium (flux) tolerances are satisfied. Alternatively, you can choose a different approach in which Abaqus/Standard will continue to iterate until no severe discontinuities occur. For contact openings with the default approach, a force discontinuity is generated when the contact force is set to zero, and this force discontinuity leads to force residuals that are checked against the time average force in the usual way, as described in “Convergence criteria for nonlinear problems,” Section 7.2.3. Similarly, in stick-to-slip transitions the frictional force is set to a lower value, which also leads to force residuals. For contact closures a severe discontinuity is considered sufficiently small if the penetration error is smaller than the contact compatibility tolerance times the incremental displacement. The penetration error is defined as the difference between the actual penetration and the penetration following from the contact pressure and pressure-overclosure relation. In cases where the displacement increment is essentially zero, a “zero penetration” check is used, similar to the check used for zero displacement increments . The same checks are used for slip-to-stick transitions in Lagrange friction. To make sure that sufficient accuracy is obtained for contact between hard bodies, it is also required that the estimated contact force error is smaller than the time average force times the contact force error tolerance. The estimated contact force error is obtained by multiplying the penetration by an effective stiffness. For hard contact this effective stiffness is equal to the stiffness of the underlying element, whereas for softened/penalty contact the effective stiffness is obtained by adding the compliance of the contact constraint and the underlying element. Forcing the iteration process to continue until no severe discontinuities occur is the more traditional, conservative method. However, this method can sometimes lead to convergence problems, particularly in large problems with many contact points or situations where contact conditions are only weakly determined. In such cases excessive iteration may occur and convergence may not be obtained Input File Usage: Abaqus/CAE Usage: *STEP, CONVERT SDI=NO Step module: step editor: Other: Convert severe discontinuity iterations: Off Matrix storage and solution scheme in Abaqus/Standard Abaqus/Standard generally uses Newton’s method to solve nonlinear problems and the stiffness method to solve linear problems. In both cases the stiffness matrix is needed. In some problems—for example, with Coulomb friction—this matrix is not symmetric. Abaqus/Standard will automatically choose whether a symmetric or unsymmetric matrix storage and solution scheme should be used based on the model and step definition used. In some cases you can override this choice; the rules are explained below. Usually it is not necessary to specify the matrix storage and solution scheme. The choice is available to improve computational efficiency in those cases where you judge that the default value is not the best choice. In certain cases where the exact tangent stiffness matrix is not symmetric, the extra iterations required by a symmetric approximation to the tangent matrix use less computer time than solving the nonsymmetric tangent matrix at each iteration. Therefore, for example, Abaqus/Standard invokes the symmetric matrix storage and solution scheme automatically in problems with Coulomb friction where every friction coefficient is less than or equal to 0.2, even though the resulting tangent matrix will have some nonsymmetric terms. However, if any friction coefficient is greater than 0.2, Abaqus/Standard will use the unsymmetric matrix storage and solution scheme automatically since it may significantly improve the convergence history. This choice of the unsymmetric matrix storage and solution scheme will consider changes to the friction model. Thus, if you modify the friction definition during the analysis to introduce a friction coefficient greater than 0.2, Abaqus/Standard will activate the unsymmetric matrix storage and solution scheme automatically. In cases in which the unsymmetric matrix storage and solution scheme is selected automatically, you must explicitly turn it off if so desired; it is recommended to do so if friction prevents any sliding motions. Input File Usage: Abaqus/CAE Usage: *STEP, UNSYMM=YES or NO Step module: step editor: Other: Storage: Use solver default or Unsymmetric or Symmetric Rules for using the unsymmetric matrix storage and solution scheme The following rules apply to matrix storage and solution schemes in Abaqus/Standard: 1. Since Abaqus/Standard provides eigenvalue extraction only for symmetric matrices, steps with eigenfrequency extraction or eigenvalue buckling prediction procedures always use the symmetric matrix storage and solution scheme. You cannot change this setting. In such steps Abaqus/Standard will symmetrize all contributions to the stiffness matrix. 2. In all steps except those with eigenfrequency extraction or eigenvalue buckling procedures, Abaqus/Standard uses the unsymmetric matrix storage and solution scheme when any of the following features are included in the model. You cannot change this setting. a. Heat transfer convection/diffusion elements (element types DCCxxx) b. General shell sections with unsymmetric section stiffness matrices (“Three-dimensional conventional shell element library,” Section 29.6.7) c. User-defined elements with unsymmetric element matrices (“User-defined elements,” Section 32.15.1) d. User-defined material models with unsymmetric material stiffness matrices (“User-defined mechanical material behavior,” Section 26.7.1, or “User-defined thermal material behavior,” Section 26.7.2) e. User-defined surface interaction models with unsymmetric interface stiffness matrices (“User- defined interfacial constitutive behavior,” Section 36.1.6) 3. The following features all trigger the unsymmetric matrix storage and solution scheme for the step. You cannot change this setting. a. Fully coupled thermal-stress analysis, except when a separated solution scheme is specified for the step (“Fully coupled thermal-stress analysis,” Section 6.5.3) b. Coupled thermal-electrical analysis, except when a separated solution scheme is specified for the step (“Coupled thermal-electrical analysis,” Section 6.7.3) c. Fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electrical- structural analysis,” Section 6.7.4) d. Coupled pore fluid diffusion/stress analysis with absorption or exsorption behavior (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1) e. Coupled pore fluid diffusion/stress analysis (steady-state) f. Coupled pore fluid diffusion/stress analysis (transient with gravity loading) g. Mass diffusion analysis (“Mass diffusion analysis,” Section 6.9.1) h. Radiation viewfactor calculation controls (“Cavity radiation,” Section 40.1.1) 4. By default, the unsymmetric matrix storage and solution scheme is used for the complex eigenvalue extraction procedure. You can change this setting. 5. In all other cases you can control whether a symmetric or a full matrix storage and arithmetic solution is chosen. If you do not specify the matrix storage and solution scheme, Abaqus/Standard utilizes the value used in the previous general analysis step. 6. If you do not specify the matrix storage and solution scheme in the first step of an analysis, Abaqus/Standard will choose the unsymmetric scheme when any of the following are used: a. Any Abaqus/Aqua load type b. The concrete damaged plasticity material model c. Friction with a friction coefficient greater than 0.2 The default value in the first step is the symmetric scheme for all other cases, except those covered by rules 2 and 3 above and for cases in which a friction coefficient is increased above 0.2 after the first step. 7. For radiative heat transfer surface interactions (“Thermal contact properties,” Section 36.2.1), certain follower forces (such as concentrated follower forces or moments), three-dimensional finite-sliding analyses, any finite sliding in coupled pore fluid diffusion/stress analyses, and certain material models (particularly nonassociated flow plasticity models and concrete) introduce unsymmetric terms in the model’s stiffness matrix. However, Abaqus/Standard does not automatically use the unsymmetric matrix storage and solution scheme when radiative heat transfer surface interactions are used. Specifying that the unsymmetric scheme should be used can sometimes improve convergence in such cases. 8. Coupled structural-acoustic and uncoupled acoustic analysis procedures in Abaqus/Standard generally use symmetric matrix storage and solution. Exceptions are the subspace-based steady-state dynamics or complex frequency procedures used for coupled structural-acoustic problems, where unsymmetric matrices are a consequence of the coupling procedure used in these cases. Using acoustic infinite elements or the acoustic flow velocity option triggers the unsymmetric matrix storage and solution scheme in Abaqus/Standard, except for natural frequency extraction using the Lanczos eigensolver, which uses symmetric matrix operations. Precision level of the Abaqus/Explicit executable You can choose a double-precision executable (with 64-bit word lengths) for Abaqus/Explicit on machines with a default, single-precision word length of 32 bits . Most new computers have 32-bit default word lengths even though they may have 64-bit memory addressing. The single-precision executable typically results in a CPU savings of 20% to 30% compared to the double-precision executable, and single precision provides accurate results in most cases. Exceptions in which single precision tends to be inadequate include analyses that require greater than approximately 300,000 increments, have typical nodal displacement increments less than 10−6 times the corresponding nodal coordinate values, include hyperelastic materials, or involve multiple revolutions of deformable parts; the double-precision executable is recommended in these cases (for example, see “Simulation of propeller rotation,” Section 2.3.15 of the Abaqus Benchmarks Manual). You can also run only a part of Abaqus/Explicit using double precision, while using single precision for the rest . These options are described below. • If double=explicit is used or the double option is specified without a value, the Abaqus/Explicit analysis will run in double precision, while the packager will run in single precision. While this choice would satisfy higher precision needs in most analyses, the data are written to the state (.abq) file in single precision. Moreover, analysis-related computations performed in the packager will still be executed in single precision. Thus, new steps, restart, and import analyses will commence from data that are stored/computed in single precision despite the fact that calculations during the step are performed in double precision. Thus, in general, one can expect somewhat noisy solutions at the beginning of the first step, at step transitions, upon restart, and after import. • If double=both is used, both the Abaqus/Explicit packager and analysis will run in double precision. This is the most expensive option but will ensure the highest overall execution precision. Analysis database floating point data will be written to the state (.abq) file at the end of packager or of a given step in double precision, thus ensuring in most cases the smoothest transition at step boundaries, upon restart, and after an import. • There may be cases where the default single precision analysis is inadequate, while the double=both option is too expensive. These are typically models that have complex links of constraints (such as a complex mechanism with connector elements, complex combinations of distributed/kinematic couplings, tie constraints and multi-point constraints, or interactions of such constraints with boundary conditions). For such models it is desirable to solve only the constraints in the model in double precision while the rest of the model is solved in single precision. This combination gives the desired accuracy of the solution while increasing performance compared to a full double precision analysis. • If double=constraint is used, the constraint packager and constraint solver are executed in double precision, while the remainder of the Abaqus/Explicit packager and analysis are executed in single precision. • If double=off is used or the double option is omitted (default), both the Abaqus/Explicit packager and the analysis will run in single precision. The double=off option is useful when you want to override the setting in the environment file. The significance of the precision level is indicated by comparing the solutions obtained with single and double precision. If no significant difference is found between single- and double-precision solutions for a particular model, the single-precision executable can be deemed adequate. 6.1.3 GENERAL AND LINEAR PERTURBATION PROCEDURES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Linear and nonlinear procedures,” Section 14.3.2 of the Abaqus/CAE User’s Manual Overview An analysis step during which the response can be either linear or nonlinear is called a general analysis step. An analysis step during which the response can be linear only is called a linear perturbation analysis step. General analysis steps can be included in an Abaqus/Standard or Abaqus/Explicit analysis; linear perturbation analysis steps are available only in Abaqus/Standard. A clear distinction is made in Abaqus/Standard between general analysis and linear perturbation analysis procedures. Loading conditions are defined differently for the two cases, time measures are different, and the results should be interpreted differently. These distinctions are defined in this section. Abaqus/Standard treats a linear perturbation analysis as a linear perturbation about a preloaded, predeformed state. Abaqus/Foundation, a subset of Abaqus/Standard, is limited entirely to linear perturbation analysis but does not allow preloading or predeformed states. General analysis steps A general analysis step is one in which the effects of any nonlinearities present in the model can be included. The starting condition for each general step is the ending condition from the last general step, with the state of the model evolving throughout the history of general analysis steps as it responds to the history of loading. If the first step of the analysis is a general step, the initial conditions for the step can be specified directly (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Abaqus always considers total time to increase throughout a general analysis. Each step also has its own step time, which begins at zero in each step. If the analysis procedure for the step has a physical time scale, as in a dynamic analysis, step time must correspond to that physical time. Otherwise, step time is any convenient time scale—for example, 0.0 to 1.0—for the step. The step times of all general analysis steps accumulate into total time. Therefore, if an option such as creep (available only in Abaqus/Standard) whose formulation depends on total time is used in a multistep analysis, any steps that do not have a physical time scale should have a negligibly small step time compared to the steps in which a physical time scale does exist. Sources of nonlinearity Nonlinear stress analysis problems can contain up to three sources of nonlinearity: material nonlinearity, geometric nonlinearity, and boundary nonlinearity. Material nonlinearity Abaqus offers models for a wide range of nonlinear material behaviors . Many of the materials are history dependent: the material’s response at any time depends on what has happened to it at previous times. Thus, the solution must be obtained by following the actual loading sequence. The general analysis procedures are designed with this in view. Geometric nonlinearity It is possible in Abaqus to define a problem as a “small-displacement” analysis, which means that geometric nonlinearity is ignored in the element calculations—the kinematic relationships are linearized. By default, large displacements and rotations are accounted for in contact constraints even if the small-displacement element formulations are used for the analysis; i.e., a large-sliding contact tracking algorithm is used . The elements in a small-displacement analysis are formulated in the reference (original) configuration, using original nodal coordinates. The errors in such an approximation are of the order of the strains and rotations compared to unity. The approximation also eliminates any possibility of capturing bifurcation buckling, which is sometimes a critical aspect of a structure’s response . You must consider these issues when interpreting the results of such an analysis. The alternative to a “small-displacement” analysis in Abaqus is to include large-displacement In this case most elements are formulated in the current configuration using current nodal effects. positions. Elements therefore distort from their original shapes as the deformation increases. With sufficiently large deformations, the elements may become so distorted that they are no longer suitable for use; for example, the volume of the element at an integration point may become negative. In this situation Abaqus will issue a warning message indicating the problem. In addition, Abaqus/Standard will cut back the time increment before making further attempts to continue the solution. Abaqus/Explicit also offers element failure models to allow elements that reach high strains to be removed from a model; see “Dynamic failure models,” Section 23.2.8, for details. For each step of an analysis you specify whether a small- or large-displacement formulation should be used (i.e., whether geometric nonlinearity should be ignored or included). By default, Abaqus/Standard uses a small-displacement formulation and Abaqus/Explicit uses a large-displacement formulation. The default value for the formulation in an import analysis is the same as the value at the time of import. If a large-displacement formulation is used during any step of an analysis, it will be used in all following steps in the analysis; there is no way to turn it off. Almost all of the elements in Abaqus use a fully nonlinear formulation. The exceptions are the cubic beam elements in Abaqus/Standard and the small-strain shell elements (those shell elements other than S3/S3R, S4, S4R, and the axisymmetric shells) in which the cross-sectional thickness change is ignored so that these elements are appropriate only for large rotations and small strains. Except for these elements, the strains and rotations can be arbitrarily large. The calculated stress is the “true” (Cauchy) stress. For beam, pipe, and shell elements the stress components are given in local directions that rotate with the material. For all other elements the stress components are given in the global directions unless a local orientation (“Orientations,” Section 2.2.5) is used at a point. For small-displacement analysis the infinitesimal strain measure is used, which is output with the strain output variable E; strain output specified with output variables LE and NE is the same as with E. Input File Usage: Use the following option to specify that a large-displacement formulation should be used for the step: *STEP, NLGEOM=YES (default in Abaqus/Explicit) Use the following option to specify that a small-displacement formulation should be used for the step: *STEP, NLGEOM=NO (default in Abaqus/Standard) Omitting the NLGEOM parameter is equivalent to using the default value. Abaqus/CAE Usage: Step module: Create Step: select any step type: Basic: Nlgeom: Off (for a small-displacement formulation) or On (for a large-displacement formulation) Boundary nonlinearity Contact problems are a common source of nonlinearity in stress analysis—see “Contact interaction analysis: overview,” Section 35.1.1. Other sources of boundary nonlinearity are nonlinear elastic springs, films, radiation, multi-point constraints, etc. Loading In a general analysis step the loads must be defined as total values. The rules for applying loads in a general, multistep analysis are defined in “Applying loads: overview,” Section 33.4.1. Incrementation The general analysis procedures in Abaqus offer two approaches for controlling incrementation. Automatic control is one choice: you define the step and, in some procedures, specify certain tolerances or error measures. Abaqus then automatically selects the increment size as it develops the response in the step. Direct user control of increment size is the alternative approach, whereby you specify the incrementation scheme. The direct approach is sometimes useful in repetitive analyses with Abaqus/Standard, where you have a good “feel” for the convergence behavior of the problem. The methods for selecting automatic or direct incrementation are discussed in the individual procedure sections. In nonlinear problems in Abaqus/Standard the challenge is always to obtain a convergent solution in the least possible computational time. In these cases automatic control of the time increment is usually more efficient because Abaqus/Standard can react to nonlinear response that you cannot predict ahead of time. Automatic control is particularly valuable in cases where the response or load varies widely through the step, as is often the case in diffusion-type problems such as creep, heat transfer, and consolidation. Ultimately, automatic control allows nonlinear problems to be run with confidence in Abaqus/Standard without extensive experience with the problem. Strong nonlinearities typically do not present difficulties in Abaqus/Explicit because of the small time increments that are characteristic of an explicit dynamic analysis product. Stabilization of unstable problems in Abaqus/Standard Some static problems can be naturally unstable, for a variety of reasons. Unconstrained rigid body motions Instability may occur because unconstrained rigid body motions exist. Abaqus/Standard may be able to handle this type of problem with automatic viscous damping when rigid body motions exist during the approach of two bodies that will eventually come into contact. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *CONTACT STABILIZATION *CONTACT CONTROLS, STABILIZE Automatic viscous damping is not supported in Abaqus/CAE. Localized buckling behavior or material instability Instability may also be caused by localized buckling behavior or by material instability; such instabilities are especially significant when no time-dependent behavior exists in the material modeling. The static, general analysis procedures in Abaqus/Standard can stabilize this type of problem if you request it . Input File Usage: Abaqus/CAE Usage: Use one of the following options: *STATIC, STABILIZE *VISCO, STABILIZE *STEADY STATE TRANSPORT, STABILIZE *COUPLED TEMPERATURE-DISPLACEMENT, STABILIZE *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, STABILIZE *SOILS, CONSOLIDATION, STABILIZE Step module: Create Step: General: any valid step type: Basic: Use stabilization with dissipated energy fraction Linear perturbation analysis steps Linear perturbation analysis steps are available only in Abaqus/Standard (Abaqus/Foundation is essentially the linear perturbation functionality in Abaqus/Standard). The response in a linear analysis step is the linear perturbation response about the base state. The base state is the current state of the model at the end of the last general analysis step prior to the linear perturbation step. If the first step of an analysis is a perturbation step, the base state is determined from the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). In Abaqus/Foundation the base state is always determined from the initial state of the model. Linear perturbation analyses can be performed from time to time during a fully nonlinear analysis by including the linear perturbation steps between the general response steps. The linear perturbation response has no effect as the general analysis is continued. The step time of linear perturbation steps, which is taken arbitrarily to be a very small number, is never accumulated into the total time. A simple example of this method is the determination of the natural frequencies of a violin string under increasing tension . The tension of the string is increased in several geometrically nonlinear analysis steps. After each of these steps, the frequencies can be extracted in a linear perturbation analysis step. If geometric nonlinearity is included in the general analysis upon which a linear perturbation study is based, stress stiffening or softening effects and load stiffness effects (from pressure and other follower forces) are included in the linear perturbation analysis. Load stiffness contributions are also generated for centrifugal and Coriolis loading. In direct steady- state dynamic analysis Coriolis loading generates an imaginary antisymmetric matrix. This contribution is accounted for currently in solid and truss elements only and is activated by using the unsymmetric matrix storage and solution scheme in the step. Linear perturbation procedures The following purely linear perturbation procedures are available in Abaqus/Standard: • “Eigenvalue buckling prediction,” Section 6.2.3 • “Direct-solution steady-state dynamic analysis,” Section 6.3.4 • “Natural frequency extraction,” Section 6.3.5 • “Complex eigenvalue extraction,” Section 6.3.6 • “Transient modal dynamic analysis,” Section 6.3.7 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 • “Subspace-based steady-state dynamic analysis,” Section 6.3.9 • “Response spectrum analysis,” Section 6.3.10 • “Random response analysis,” Section 6.3.11 • “Time-harmonic analysis” in “Eddy current analysis,” Section 6.7.5 In addition, the following analysis techniques are treated as linear perturbation steps in an analysis: • “Defining substructures,” Section 10.1.2 • “Generating matrices,” Section 10.3.1 Except for these procedures and the static procedure (explained below), all other procedures can be used only in general analysis steps (in other words, they are not available with Abaqus/Foundation). All linear perturbation procedures except for the complex eigenvalue extraction procedure are available with Abaqus/Foundation. Linear static perturbation analysis A linear static stress analysis (“Static stress analysis,” Section 6.2.2) can be conducted in Abaqus/Standard. Input File Usage: Use both of the following options to conduct a linear static perturbation analysis: *STEP, PERTURBATION *STATIC Omitting the PERTURBATION parameter on the *STEP option implies that a general static analysis is required. Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Static, Linear perturbation Loading Load magnitudes (including the magnitudes of prescribed boundary conditions) during a linear perturbation analysis step are defined as the magnitudes of the load perturbations only. Likewise, the value of any solution variable is output as the perturbation value only—the value of the variable in the base state is not included. Multiple load case analysis Multiple load cases can be analyzed simultaneously for static, direct-solution steady-state dynamic and SIM-based steady-state dynamic (including subspace projection) linear perturbation steps. See “Multiple load case analysis,” Section 6.1.4, for a description of this capability. Restrictions A linear perturbation analysis is subject to the following restrictions: • Since a linear perturbation analysis has no time period, amplitude references (“Amplitude curves,” Section 33.1.2) can be used meaningfully only to specify loads or boundary conditions as functions of frequency (in a steady-state dynamics analysis) or to define base motion (in mode-based dynamics procedures). If loads or boundary conditions are specified as functions of time, the amplitude value corresponding to time=0 will be used. • A general implicit dynamic analysis (“Implicit dynamic analysis using direct integration,” Section 6.3.2) cannot be interrupted to perform perturbation analyses: before performing the perturbation analysis, Abaqus/Standard requires that the structure be brought into static equilibrium. • During a linear perturbation analysis step, the model’s response is defined by its linear elastic (or viscoelastic) stiffness at the base state. Plasticity and other inelastic effects are ignored. For hyperelasticity (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1) or hypoelasticity (“Hypoelastic behavior,” Section 22.4.1), the tangent elastic moduli in the base state are used. If cracking has occurred—for example, in the concrete model (“Concrete smeared cracking,” Section 23.6.1)—the damaged elastic (secant) moduli are used. • Contact conditions cannot change during a linear perturbation analysis. The open/closed status of each contact constraint remains as it is in the base state. All points in contact (i.e., with a “closed” status) are assumed to be sticking if friction is present, except the contact nodes for which a velocity differential is imposed by the motion of the reference frame or the transport velocity. At those nodes, slipping conditions are assumed regardless of the friction coefficient. • The effects of temperature and field variable perturbations are ignored for materials that are dependent on temperature and field variables. However, temperature perturbations will produce perturbations of thermal strain. 6.1.4 MULTIPLE LOAD CASE ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • *LOAD CASE • *END LOAD CASE • Chapter 34, “Load cases,” of the Abaqus/CAE User’s Manual Overview A multiple load case analysis: • is used to study the linear responses of a structure subjected to distinct sets of loads and boundary conditions defined within a step (each set is referred to as a load case); • can be much more efficient than an equivalent multiple perturbation step analysis; • allows for the changing of mechanical loads and boundary conditions from load case to load case; • includes the effects of the base state; and • can be performed with static perturbation, direct-solution steady-state dynamic and SIM-based steady-state dynamic analyses. Load cases A load case refers to a set of loads, boundary conditions, and base motions comprising a particular loading condition. For example, in a simplified model the operational environment of an airplane might be broken into five load cases: (1) take-off, (2) climb, (3) cruise, (4) descent, and (5) landing. Often a load case is defined in terms of unit loads or prescribed boundary conditions, and a multiple load case analysis refers to the simultaneous solution for the responses of each load case in a set of such load cases. These responses can then be scaled and linearly combined during postprocessing to represent the actual loading environment. Other postprocessing manipulations on load cases are also common, such as finding the maximum Mises stress among all load cases. These types of load case manipulations can be requested in the Visualization module of Abaqus/CAE . Using multiple load cases A multiple load case analysis is conceptually equivalent to a multiple step analysis in which the load case definitions are mapped to consecutive perturbation steps. However, a multiple load case analysis is generally much more efficient than the equivalent multiple step analysis. The exception occurs when a large number of boundary conditions exist that are not common to all load cases (i.e., degrees of freedom are constrained in one load case but not others). It is difficult to define what “large” is since it is model dependent. The relative performance of the two analysis methods can be assessed by performing a data check analysis for both the multiple load case analysis and the equivalent multiple step analysis. The data check analysis writes resource information for each step to the data file, including the maximum wavefront, number of floating point operations, and minimum memory required. If these numbers are noticeably larger for the multiple load case step compared to those across all steps of the equivalent multiple step analysis (the number of floating point operations should be summed over all steps before comparing), the multiple step analysis will be more efficient. Although generally more efficient, the multiple load case analysis may consume more memory and disk space than an equivalent multiple step analysis. Thus, for large problems or problems with many load cases it is again advisable, as described above, to compare resource usage between the multiple load case analysis and the equivalent multiple step analysis. If resource requirements for the multiple load case analysis are deemed too large, consider dividing the load cases among a few steps. The resulting analysis (a hybrid of multiple load cases and multiple steps) will require fewer resources while retaining an efficiency advantage over an equivalent pure multiple step analysis. Defining load cases You define a load case within a static perturbation, direct-solution steady-state dynamic, and SIM-based steady-state dynamic analyses. Load case definitions do not propagate to subsequent steps. Only the following types of prescribed conditions can be specified within a load case definition: • Boundary conditions • Concentrated loads • Distributed loads • Distributed surface loads • Inertia-based loads • Base motions Additional rules governing these prescribed conditions are described in the sections that follow. No other types of prescribed conditions can appear in a step that contains load case definitions. All other valid analysis components, such as output requests, must be specified outside load case definitions. Each load case definition is assigned a name for postprocessing purposes. Input File Usage: Use the first option to begin a load case and the second option to end a load case: *LOAD CASE, NAME=name *END LOAD CASE Prescribed conditions specified within a load case definition apply only to that load case. In static perturbation and direct-solution steady-state dynamic analyses, prescribed conditions can be specified outside the load case definitions (in this case they apply to all load cases in the step). Abaqus/CAE Usage: Load module: Create Load Case: Name: name In Abaqus/CAE if a step contains load cases, all prescribed conditions in the step must be included in one or more load cases. Procedures Load cases can be defined only in perturbation steps with the following procedures: • Static • Direct-solution, steady-state dynamic • SIM-based, steady-state dynamic As with other perturbation steps, a multiple load case analysis will include the nonlinear effects of the previous general step (base state). The following analysis techniques are not supported in the context of a load case step: • Restart from a particular load case • Submodeling using results from other than the first load case in the global analysis • Importing and transferring results • Cyclic symmetry analysis • Contour integrals • Design sensitivity analysis Boundary conditions Boundary conditions can be specified both outside and inside load case definitions in the same step. Specifying a boundary condition outside the load case definitions in a step is equivalent to including it in all load case definitions in the step (i.e., the boundary condition will be applied to all load cases). Unless any boundary conditions are removed in the perturbation step, the boundary conditions that are active in the base state will propagate to all load cases in the perturbation step. If any boundary condition is removed in a step with load cases (either outside or inside load case definitions), the base state boundary conditions will not be propagated to any load case in the step. See “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1, for more information. Note: In Abaqus/CAE if a step contains load cases, all boundary conditions in the step must be included in one or more load cases. Boundary conditions can only be used with load cases in static perturbation and direct-solution steady-state dynamic analyses. Loads In static perturbation and direct-solution steady-state dynamic analyses concentrated, distributed, and distributed surface loads can be specified both outside and inside load case definitions in the same step. Inertia relief loads can be specified either outside load case definitions or inside load case definitions in the same step but not both simultaneously. Specifying one of these load types outside the load case definitions in a step is equivalent to including it in all load case definitions in the step (i.e., the loading will be applied to all load cases). In SIM-based steady-state dynamic analyses concentrated, distributed, distributed surface loads, and base motion can be specified only inside load case definitions in the same step. Inertia relief loads are not supported. Load cases cannot be used in models that include aqua loads . As with any perturbation step, perturbation loads must be defined completely within the perturbation step . Note: In Abaqus/CAE if a step contains load cases, all loads in the step must be included in one or more load cases. Predefined fields Field variables cannot be specified in a step with load cases. Elements Load cases cannot be used in models that include piezoelectric elements . Output In a step containing one or more load cases, field and history output requests to the output database and output requests to the data file are supported. Output requests to the results file are not supported. Output requests can be specified only outside load case definitions, and they apply to all load cases in a step. The step propagation rules for output requests are the same as for other perturbation steps . Most of the field and history output variables normally available within a particular procedure are also available during a multiple load case analysis . Additional restrictions apply for a SIM-based steady-state dynamic analysis; see “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1, for more information. The field output corresponding to each load case is stored in a separate frame on the output database with the load case name included as a frame attribute. To distinguish between load cases for history output variables, the name of the load case is appended to the history variable name. The Visualization module of Abaqus/CAE and the Abaqus Scripting Interface can be used to access and manipulate load case output. Abaqus/Standard does not perform consistency checks on the physical validity of the load case manipulations. For example, the linear superposition of two load cases, each with different boundary conditions, is allowed even though the combined results may not be physically meaningful. Input file template *HEADING … *STEP, PERTURBATION *STATIC or *STEADY STATE DYNAMICS, DIRECT … *OUTPUT, FIELD … *BOUNDARY Data lines to specify boundary conditions for all load cases. *DLOAD Data lines to specify distributed loads for all load cases. *CLOAD Data lines to specify point loads for all load cases. *DSLOAD Data lines to specify distributed surface loads for all load cases. *INERTIA RELIEF Data lines to specify inertia relief loading directions. (This option cannot be used inside load cases if it is used here.) … *LOAD CASE, NAME=name1 *BOUNDARY Data lines to specify boundary conditions for first load case. *DLOAD Data lines to specify distributed loads for first load case. *CLOAD Data lines to specify point loads for first load case. *DSLOAD Data lines to specify distributed surface loads for first load case. *INERTIA RELIEF Data lines to specify inertia relief loading directions. (This option cannot be used outside load cases if it is used here.) *END LOAD CASE *LOAD CASE, NAME=name2 Load and boundary condition options for second load case *END LOAD CASE … Subsequent load case definitions … *END STEP *STEP, PERTURBATION *FREQUENCY, SIM or *FREQUENCY, EIGENSOLVER=AMS *END STEP … *STEP, PERTURBATION *STEADY STATE DYNAMICS *LOAD CASE, NAME=name3 *BASE MOTION Data lines to specify base motion for first load case. *DLOAD Data lines to specify distributed loads for first load case. *CLOAD Data lines to specify point loads for first load case. *DSLOAD Data lines to specify distributed surface loads for first load case. *END LOAD CASE *LOAD CASE, NAME=name4 Load and base motion options for second load case. *END LOAD CASE … Subsequent load case definitions … *OUTPUT, HISTORY … *END STEP 6.1.5 DIRECT LINEAR EQUATION SOLVER Products: Abaqus/Standard Abaqus/CAE References • “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2 • “Using the Abaqus environment settings,” Section 3.3.1 • “Iterative linear equation solver,” Section 6.1.6 • “Parallel execution in Abaqus/Standard,” Section 3.5.2 • “Configuring analysis procedure settings,” Section 14.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Linear equation solution is used in linear and nonlinear analysis. In nonlinear analysis Abaqus/Standard uses the Newton method or a variant of it, such as the Riks method, within which it is necessary to solve a set of linear equations at each iteration. The direct linear equation solver finds the exact solution to this system of linear equations (up to machine precision). The direct linear equation solver in Abaqus/Standard: • uses a sparse, direct, Gauss elimination method; and • often represents the most time consuming part of the analysis (especially for large models)—the storage of the equations occupies the largest part of the disk space during the calculations. The sparse solver The direct sparse solver uses a “multifront” technique that can reduce the computational time to solve the equations dramatically if the equation system has a sparse structure. Such a matrix structure typically arises when the physical model is made from several parts or branches that are connected together; a spoked wheel is a good example of a structure that has a sparse stiffness matrix. Space frames and other structures modeled with beams, trusses, and shells often have sparse stiffness matrices. In contrast, a blocky structure—such as a single, solid, three-dimensional block —provides little opportunity for the sparse solver to reduce the computer time. For large blocky structures, the iterative linear equation solver may be more efficient . Input File Usage: Use the following option to use the default direct sparse solver: Abaqus/CAE Usage: *STEP Step module: step editor: Other: Method: Direct Setting controls for the direct linear solver The linear equation solver can optimize elimination of constraint equations associated with hard contact and hybrid elements. There are two potential undesirable side-effects associated with this option: • Possible small degradation of solution accuracy may adversely impact the nonlinear convergence behavior. • Possible minor performance degradation for models without hard contact constraints and/or hybrid elements. Input File Usage: Use the following option to turn on constraint optimization: Abaqus/CAE Usage: *SOLVER CONTROLS, CONSTRAINT OPTIMIZATION You cannot specify constraint optimization in Abaqus/CAE. 6.1.6 ITERATIVE LINEAR EQUATION SOLVER Products: Abaqus/Standard Abaqus/CAE References • *STEP • *SOLVER CONTROLS • “Parallel execution in Abaqus/Standard,” Section 3.5.2 • “Customizing solver controls,” Section 14.15.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The iterative linear equation solver in Abaqus/Standard: • can be used for linear and nonlinear static, quasi-static, heat transfer, geostatic, and coupled pore fluid diffusion and stress analysis solution procedures; • should be used only for large, well-conditioned models for which the direct sparse solver requires a prohibitively large number of floating point operations; • is likely to be dramatically faster than the direct equation solver for large, well-conditioned, blocky structures; • runs totally in-core and uses less storage than the direct sparse solver (memory and disk combined); • can be used only with three-dimensional models; • must be the only solver invoked in the analysis (i.e., you cannot use the iterative solver in one step and the direct solver in another); • cannot be used with automatic stabilization with an adaptive damping factor ; • can be used with a constant damping factor if stabilization is necessary ; • cannot be used if the system of equations includes Lagrange multiplier degrees of freedom (i.e., associated with distributing couplings, hybrid elements, connector elements, contact with direct enforcement); and • will degrade performance if used with models containing dense linear constraints (e.g., equations, kinematic couplings, MPCs) that eliminate a large number of slave degrees of freedom per master degree of freedom and/or eliminate some slave degrees of freedom in favor of a large number of master degrees of freedom. Iterative solver basics The iterative solver in Abaqus/Standard can be used to find the solution to a linear system of equations and can be invoked in a linear or nonlinear static, quasi-static, geostatic, pore fluid diffusion, or heat transfer analysis step. Since the technique is iterative, a converged solution to a given system of linear equations cannot be guaranteed. In cases where the iterative solver fails to converge to a solution, modifications to the model may be necessary to improve the convergence behavior. In some cases the only choice may be to use the direct solver to obtain a solution. When the iterative solver converges, the accuracy of this solution depends on the relative tolerance that is used; the default tolerance is sufficiently accurate for most purposes. However, tolerance adjustments for particular analyses may improve the overall performance of the simulation. In addition, the performance of the iterative solver relative to the direct sparse solver is highly sensitive to the model geometry, favoring blocky type structures (i.e., models that look more like a cube than a plate) with a high degree of mesh connectivity and a relatively low degree of sparsity. These types of models often demand the most computational and storage resources for the direct sparse solver. Models with a lesser degree of connectivity (often said to have a higher degree of sparsity), such as thin, shell-like structures, are much more suited to the direct sparse solver . Input File Usage: Abaqus/CAE Usage: Use the following option to invoke the iterative solver: *STEP, SOLVER=ITERATIVE Step module: step editor: Other: Method: Iterative The iterative solution technique The iterative solution technique in Abaqus/Standard is based on Krylov methods employing a preconditioner. This solver uses the following general strategy: 1. The Krylov method solver iterates on the system of equations generated by the finite element method while a preconditioner is applied at each iteration. 2. The preconditioner is calculated only once at the beginning of each linear system solve and is used to accelerate the convergence of the Krylov method. 3. In parallel, all components of the iterative solution process (including matrix assembly, preconditioner setup, and the actual solve using the Krylov method) are handled locally on each core with all necessary communication handled through an MPI-based implementation. The process outlined above is performed entirely internal to Abaqus/Standard, with no user intervention required. Convergence of the linear system of equations To generate the solution to the system of linear algebraic equations (denoted by the matrix equation , where K is the global stiffness matrix, f is the load vector, and u is the desired displacement solution), a sequence of Krylov solver iterations is performed, whereby an approximate solution gets closer to the exact solution at each iteration. The error in the approximate solution is measured by the relative residual of the linear system, defined by norm. , where is the The term “convergence” is used to describe this process, and the approximate solution is said to be converged when the relative residual is below a specified tolerance. By default, this tolerance is 10−3 for general nonlinear procedures. Linear perturbation procedures have the default tolerance of 10−6 . While the default tolerance may seem loose for general nonlinear procedures, it is important to note that the linear solver convergence tolerance is independent from the nonlinear convergence process (i.e., Newton-Raphson method) tolerances that are used to determine if analysis increments converge. The latter are the same regardless of the choice of linear equation solver, iterative or direct. The rate at which the approximate solution converges is directly related to the conditioning of the original system of equations. A linear system that is well conditioned will converge faster than an ill-conditioned system. If the residual does not converge to tolerance within the maximum number of iterations, the iterative solver is said to have encountered a non-convergence and Abaqus/Standard issues a warning message. However, the analysis will continue running and in some cases the Newton-Raphson iterations within increments may continue to converge. Setting controls for the iterative linear solver The default controls provided in Abaqus/Standard are usually sufficient. However, a method for overriding the default relative convergence tolerance and maximum number of solver iterations is provided. Resetting the solver controls You can specify that the solver controls be reset to their default values. Input File Usage: Abaqus/CAE Usage: *SOLVER CONTROLS, RESET Step module: Other→Solver Controls→Edit: Reset all parameters to their system-defined defaults Specifying the relative convergence tolerance By default, this tolerance is 10−3 for procedures other than linear perturbation. Linear perturbation procedures have the default tolerance of 10−6 . For nonlinear problems the accuracy of the linear solution can impact the convergence of the Newton method. In some cases it may be necessary to manually specify the iterative solver relative tolerance to improve the convergence of the Newton-Raphson method or to improve performance. Input File Usage: *SOLVER CONTROLS relative tolerance for convergence Abaqus/CAE Usage: Step module: Other→Solver Controls→Edit: Specify: Relative tolerance: Specify: relative tolerance for convergence Specifying the maximum number of solver iterations In rare instances the linear solver may require more than the default number of iterations to converge to the desired level of accuracy. In this case you can increase the maximum number of iterations allowed by the iterative solver (the default value is 300). Input File Usage: *SOLVER CONTROLS , max number of solver iterations Abaqus/CAE Usage: Step module: Other→Solver Controls→Edit: Specify: Max. number of iterations: Specify: max number of solver iterations Specifying the incomplete factorization fill-in levels for soils and geostatic analyses The preconditioner used for soils and geostatic analyses employs a factorization-based method, also In rare instances the linear solver may require more than the default number known as ILU(k). Incomplete of incomplete factorization fill-in levels to converge to the desired accuracy level. LU factorization of a matrix is a sparse approximation of the LU factorization. LU factorization typically changes the nonzero structure of the stiffness matrices by adding many nonzero entries; ILU factorization approximates the fully factorized matrices by limiting the number of nonzero entries introduced during the factorization. By default, the ILU factorization fill-in level used by the iterative solver is 0 and no nonzero entries are added. You can increase the fill-in level (maximum value is 3) to allow nonzero entries to be added based on the connectivity of the stiffness matrices and obtain a better approximation of the full factorization but with increased computational cost. *SOLVER CONTROLS , , ILU factorization fill-in level Input File Usage: Abaqus/CAE Usage: Step module: Other→Solver Controls→Edit: Specify: ILU factorization fill-in level: Specify: ILU factorization fill-in level Deciding to use the iterative solver Many factors must be carefully weighed before deciding to use the iterative solver in Abaqus/Standard, such as element type, contact and constraint equations, material and geometric nonlinearities, and material properties, all of which can impact robustness and performance. In cases where the model is ill-conditioned the iterative solver may converge very slowly or fail to converge. This may occur, for example, if many elements have poor aspect ratios. In addition to the robustness issues (relating mainly to the rate of convergence or stagnation), the iterative solver is expected to outperform the direct sparse solver only for blocky models (even when the model is well conditioned) that require a very large number of floating point operations for factorization. Typically, for a well-conditioned solid model, the number of degrees of freedom in the global model must be greater than one million before the iterative solver will be comparable to the direct solver in terms of run time. Element type and model geometry The most basic modeling issue that will affect the performance of the iterative solver is the model geometry, which must be carefully considered when deciding if the iterative solver is suited for a particular model. In general, models that are blocky in nature (i.e., look more like a cube than a plate) and are dominated by solid elements will behave well with the iterative solver. Although structural elements such as beams and shells are supported, models with structural elements will not perform optimally; the direct sparse solver should be used instead for such models. Common modeling techniques such as coating solid elements with a thin layer of membrane elements to recover accurate stresses on the boundary or fixing rigid body motion with weak springs may not work with the iterative solver. Applying loads or boundary conditions to large node sets using locally transformed coordinate systems can also cause convergence difficulties. All of these techniques are likely to lead to extremely slow convergence or stagnation. Another factor that can influence the convergence of the iterative solver is the quality of the elements. Blocky models, such as an engine block, that contain many poorly shaped elements with high aspect ratios can also lead to poor iterative solver convergence. It is a good idea to look for warning messages about poorly shaped elements when evaluating the performance of the iterative solver. Currently, hybrid elements and connectors are not supported with the iterative solver. Using cohesive elements with the iterative solver will likely lead to nonconvergence. Constraint equations Although the iterative solver can be used for models that include constraint equations (such as multi-point constraints, surface-based tie constraints, kinematic couplings, etc.), certain limitations may exist in the following situations: • linear or nonlinear multi-point constraints containing more than a few thousand degrees of freedom; • more than a few thousand linear or nonlinear multi-point constraints containing shared master degrees of freedom; • rigid body definition of elements containing more than a few thousand degrees of freedom; or • kinematic coupling constraints containing more than a few thousand slave degrees of freedom. If any of these conditions apply to a model, the solution cost of the linear system of equations will grow linearly with the number of such constraints. Furthermore, it is usually recommended to tighten the iterative solver tolerance and increase the number of maximum iterations in the linear iterative solver for nonlinear analysis to achieve convergence. Therefore, it is recommended to keep such constraints to a minimum if possible; otherwise, the increased cost may offset the performance gains that come from using the iterative solver. Distributing couplings are not supported with the iterative solver. Contact Since contact is a form of nonlinear analysis, special care must be taken in selecting the convergence tolerance for the iterative solver . Therefore, it is recommended to run the model through a static perturbation analysis before proceeding to the nonlinear problem. This will demonstrate how the iterative solver will perform for the specific model geometry without the added difficulty of nonlinear convergence. The iterative solver will work only with the penalty-based contact formulation with reasonable penalty stiffness. If contact with direct enforcement (i.e., the Lagrange multiplier method) or penalty contact with an extremely high penalty stiffness is used, Abaqus/Standard may fail to converge. The iterative solver does not support pore fluid contact, regardless of the contact formulation used. Material properties When deciding to use the iterative solver, the variation of material properties in the model should be considered. Models that have very large discontinuities in material behavior (many orders of magnitude) will most likely converge slowly and possibly stagnate. Nonlinear analysis The iterative solver can be used to solve the linear system of algebraic equations that arises at each iteration of the Newton procedure. However, the convergence of the nonlinear problem will be affected by the convergence of the iterative linear solver. The actual impact depends on the particular model and type of nonlinearities present. In some cases the default iterative solver tolerance of 10−3 is sufficient to maintain the convergence of the Newton method; in other cases a smaller linear solver tolerance (for example, 10−6) must be used. If a nonlinear analysis that uses the iterative solver fails to converge, it is often difficult to determine if this is due to the approximate linear equation solution of the iterative solver or if the Newton process itself is failing to converge. If nonlinear convergence problems occur, the direct solver can be used—given the problem is solvable using the direct solver due to solution cost—to eliminate the approximate linear solution as a possible source of the problem. 6.2 Static stress/displacement analysis • “Static stress analysis procedures: overview,” Section 6.2.1 • “Static stress analysis,” Section 6.2.2 • “Eigenvalue buckling prediction,” Section 6.2.3 • “Unstable collapse and postbuckling analysis,” Section 6.2.4 • “Quasi-static analysis,” Section 6.2.5 • “Direct cyclic analysis,” Section 6.2.6 • “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7 6.2.1 STATIC STRESS ANALYSIS PROCEDURES: OVERVIEW A static stress procedure is one in which inertia effects are neglected. Several static stress analysis procedures are available in Abaqus/Standard: • Static analysis: “Static stress analysis,” Section 6.2.2, is used for stable problems and can include linear or nonlinear response. • Eigenvalue buckling analysis: “Eigenvalue buckling prediction,” Section 6.2.3, is used to estimate the critical (bifurcation) load of “stiff” structures. It is a linear perturbation procedure. • Unstable collapse and postbuckling analysis: “Unstable collapse and postbuckling analysis,” Section 6.2.4, is used to estimate the unstable, geometrically nonlinear collapse of a structure. The method can also be helpful in obtaining a solution in other types of unstable problems, and it is often suitable for limit load analyses. • Quasi-static analysis: “Quasi-static analysis,” Section 6.2.5, is used to analyze the transient response of structures considering time-dependent material behavior (creep and swelling, viscoelasticity, and viscoplasticity). A quasi-static analysis can be linear or nonlinear. • Direct cyclic analysis: “Direct cyclic analysis,” Section 6.2.6, is used to calculate the stabilized cyclic response of the structure directly. It uses a combination of Fourier series and time integration of the nonlinear material behavior to obtain the stabilized cyclic solution iteratively. • Low-cycle fatigue analysis: “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7, is used to predict progressive damage and failure for ductile bulk materials and/or to predict delamination/debonding growth at the interfaces in laminated composites based on the direct cyclic approach in conjunction with the damage extrapolation technique. 6.2.2 STATIC STRESS ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Static stress analysis procedures: overview,” Section 6.2.1 • *STATIC • “Configuring a static, general procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A static stress analysis: • is used when inertia effects can be neglected; • can be linear or nonlinear; and • ignores time-dependent material effects (creep, swelling, viscoelasticity) but takes rate-dependent plasticity and hysteretic behavior for hyperelastic materials into account. Time period During a static step you assign a time period to the analysis. This is necessary for cross-references to the amplitude options, which can be used to determine the variation of loads and other externally prescribed parameters during a step . In some cases this time scale is quite real—for example, the response may be caused by temperatures varying with time based on a previous transient heat transfer run; or the material response may be rate dependent (rate-dependent plasticity), so that a natural time scale exists. Other cases do not have such a natural time scale; for example, when a vessel is pressurized up to limit load with rate-independent material response. If you do not specify a time period, Abaqus/Standard defaults to a time period in which “time” varies from 0.0 to 1.0 over the step. The “time” increments are then simply fractions of the total period of the step. Linear static analysis Linear static analysis involves the specification of load cases and appropriate boundary conditions. If all or part of a problem has linear response, substructuring is a powerful capability for reducing the computational cost of large analyses . Nonlinear static analysis Nonlinearities can arise from large-displacement effects, material nonlinearity, and/or boundary nonlinearities such as contact and friction (see “General and linear perturbation procedures,” Section 6.1.3) and must be accounted for. If geometrically nonlinear behavior is expected in a step, the large-displacement formulation should be used. In most nonlinear analyses the loading variations over the step follow a prescribed history such as a temperature transient or a prescribed displacement. Input File Usage: Use the following option to specify that a large-displacement formulation should be used for a static step: Abaqus/CAE Usage: *STEP, NLGEOM Step module: Create Step: General: Static, General: Basic: Nlgeom: On (to activate the large-displacement formulation) Unstable problems Some static problems can be naturally unstable, for a variety of reasons. Buckling or collapse In some geometrically nonlinear analyses, buckling or collapse may occur. In these cases a quasi- static solution can be obtained only if the magnitude of the load does not follow a prescribed history; it must be part of the solution. When the loading can be considered proportional (the loading over the complete structure can be scaled with a single parameter), a special approach—called the “modified Riks method”—can be used, as described in “Unstable collapse and postbuckling analysis,” Section 6.2.4. Input File Usage: Abaqus/CAE Usage: *STATIC, RIKS Step module: Create Step: General: Static, Riks Local instabilities In other unstable analyses the instabilities are local (e.g., surface wrinkling, material instability, or local buckling), in which case global load control methods such as the Riks method are not appropriate. Abaqus/Standard offers the option to stabilize this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1. Incrementation Abaqus/Standard uses Newton’s method to solve the nonlinear equilibrium equations. Many problems involve history-dependent response; therefore, the solution usually is obtained as a series of increments, with iterations to obtain equilibrium within each increment. Increments must sometimes be kept small (in the sense that rotation and strain increments must be small) to ensure correct modeling of history- dependent effects. Most commonly the choice of increment size is a matter of computational efficiency: if the increments are too large, more iterations will be required. Furthermore, Newton’s method has a finite radius of convergence; too large an increment can prevent any solution from being obtained because the initial state is too far away from the equilibrium state that is being sought—it is outside the radius of convergence. Thus, there is an algorithmic restriction on the increment size. Automatic incrementation In most cases the default automatic incrementation scheme is preferred because it will select increment sizes based on computational efficiency. Input File Usage: Abaqus/CAE Usage: *STATIC Step module: Create Step: General: Static, General: Incrementation: Type: Automatic (default) Direct incrementation Direct user control of the increment size is also provided because if you have considerable experience with a particular problem, you may be able to select a more economical approach. Input File Usage: Abaqus/CAE Usage: *STATIC, DIRECT Step module: Create Step: General: Static, General: Incrementation: Type: Fixed With direct user control, the solution to an increment can be accepted after the maximum number of iterations allowed has been completed (as defined in “Commonly used control parameters,” Section 7.2.2), even if the equilibrium tolerances are not satisfied. This approach is not recommended; it should be used only in special cases when you have a thorough understanding of how to interpret results obtained in this way. Very small increments and a minimum of two iterations are usually necessary if this option is used. Input File Usage: Abaqus/CAE Usage: *STATIC, DIRECT=NO STOP Step module: Create Step: General: Static, General: Other: Accept solution after reaching maximum number of iterations Steady-state frictional sliding In a static analysis procedure you can model steady-state frictional sliding between two deformable bodies or between a deformable and a rigid body that are moving with different velocities by specifying the motions of the bodies as predefined fields. In this case it is assumed that the slip velocity follows from the difference in the user-specified velocities and is independent of the nodal displacements, as described in “Coulomb friction,” Section 5.2.3 of the Abaqus Theory Manual. Since this frictional behavior is different from the frictional behavior used without steady-state frictional sliding, discontinuities may arise in the solutions between an analysis step in which relative velocity is determined from predefined motions and prior steps. An example is the discontinuity that occurs between the initial preloading of the disc pads in a disc brake system and the subsequent braking analysis where the disc spins with a prescribed rotation. To ensure a smooth transition in the solution, it is recommended that all analysis steps prior to the analysis step in which predefined motion is specified use a zero coefficient of friction. You can then modify the friction properties in the steady-state analysis to use the desired friction coefficient . Input File Usage: Abaqus/CAE Usage: *MOTION Predefined motion fields are not supported in Abaqus/CAE. Initial conditions Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified. “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the available initial conditions. Boundary conditions Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6); to warping degree of freedom 7 in open-section beam elements; or, if hydrostatic fluid elements are included in the model, to fluid pressure degree of freedom 8. If boundary conditions are applied to rotation degrees of freedom, you must understand how finite rotations are handled by Abaqus . During the analysis prescribed boundary conditions can be varied using an amplitude definition . Loads The following loads can be prescribed in a static stress analysis: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” Predefined fields The following predefined fields can be specified in a static stress analysis, as described in “Predefined fields,” Section 33.6.1: • Although temperature is not a degree of freedom in a static stress analysis, nodal temperatures can be specified as a predefined field. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any. • The values of user-defined field variables can be specified. These values only affect field-variable- dependent material properties, if any. Material options Most material models that describe mechanical behavior are available for use in a static stress analysis. The following material properties are not active during a static stress analysis: acoustic properties, properties, and pore fluid flow properties. STATIC STRESS ANALYSIS Rate-dependent yield (“Rate-dependent yield,” Section 23.2.3), (“Hysteresis in elastomers,” Section 22.8.1), and two-layer viscoplasticity (“Two-layer viscoplasticity,” Section 23.2.11) are the only time-dependent material responses that are active during a static analysis. The rate-dependent yield response is often important in rapid processes such as metal-working problems. The hysteresis model is useful in modeling the large-strain, rate-dependent response of elastomers that exhibit a pronounced hysteresis under cyclic loading. The two-layer viscoplasticity model is useful in situations where a significant time-dependent behavior as well as plasticity is observed, which for metals typically occurs at elevated temperatures. An appropriate time scale must be specified so that Abaqus/Standard can treat the rate dependence of the material responses correctly. hysteresis Static creep and swelling problems and time-domain viscoelastic models are analyzed by the quasi- static procedure (“Quasi-static analysis,” Section 6.2.5). When any of these time-dependent material models are used in a static analysis, a rate-independent elastic solution is obtained and the chosen time scale does not have an effect on the material response. For creep and swelling behavior this implies that the loading is applied instantaneously compared with the natural time scale over which creep effects take place. The same concept of instantaneous load application applies to time-domain viscoelastic behavior. You can also obtain the fully relaxed long-term viscoelastic solution directly in a static procedure without having to perform a transient analysis; this choice is meaningful only when time-domain viscoelastic material properties are defined. If the long-term viscoelastic solution is requested, the internal stresses associated with each of the Prony series terms are increased gradually from their values at the beginning of the step to their long-term values at the end of the step. For the two-layer viscoplastic material model, you can obtain the long-term response of the elastic- plastic network alone. When frequency-domain viscoelastic material properties are defined , the corresponding elastic moduli must be specified as long-term elastic moduli. This implies that the response corresponds to the long-term elastic solution, regardless of the time period specified for the step. Input File Usage: Abaqus/CAE Usage: Elements Use the following option to obtain the fully relaxed long-term elastic solution with time-domain viscoelasticity or the long-term elastic-plastic solution for two-layer viscoplasticity: *STATIC, LONG TERM Step module: Create Step: General: Static, General or Static, Riks: Other: Obtain long-term solution with time-domain material properties Any of the stress/displacement elements in Abaqus/Standard can be used in a static stress analysis . Although velocities are not available in a static stress analysis, dashpots can still be used (they can be useful in stabilizing an unstable problem). The relative velocity will be calculated as described in “Dashpots,” Section 32.2.1. Acoustic elements are not active in a static step. Consequently, if an acoustic-solid analysis includes a static step, only the solid elements will deform. If the deformations are large, the acoustic and solid meshes may not conform, and subsequent acoustic-structural analysis steps may produce misleading results. See “ALE adaptive meshing: overview,” Section 12.2.1, for information on using the adaptive meshing technique to deform the acoustic mesh. Output The element output available for a static stress analysis includes stress; strain; energies; the values of state, field, and user-defined variables; and composite failure measures. The nodal output available includes displacements, reaction forces, and coordinates. All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Input file template *HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS Data lines to specify initial conditions *AMPLITUDE Data lines to define amplitude variations ** *STEP (,NLGEOM) Once NLGEOM is specified, it will be active in all subsequent steps *STATIC, DIRECT Data line to define direct time incrementation *BOUNDARY Data lines to prescribe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD Data lines to specify loads *TEMPERATURE and/or *FIELD Data lines to specify values of predefined fields *END STEP ** *STEP *STATIC Data line to control automatic time incrementation *BOUNDARY, OP=MOD Data lines to modify or add zero-valued or nonzero boundary conditions *CLOAD, OP=NEW Data lines to specify new concentrated loads; all previous concentrated loads will be removed *DLOAD, OP=MOD Data lines to specify additional or modified distributed loads *TEMPERATURE and/or *FIELD Data lines to specify additional or modified values of predefined fields *END STEP 6.2.3 EIGENVALUE BUCKLING PREDICTION Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “General and linear perturbation procedures,” Section 6.1.3 • “Static stress analysis procedures: overview,” Section 6.2.1 • *BUCKLE • “Configuring a buckling procedure” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating and modifying prescribed conditions,” Section 16.4 of the Abaqus/CAE User’s Manual Overview Eigenvalue buckling analysis: • is generally used to estimate the critical (bifurcation) load of “stiff” structures; • is a linear perturbation procedure; • can be the first step in an analysis of an unloaded structure, or it can be performed after the structure has been preloaded—if the structure has been preloaded, the buckling load from the preloaded state is calculated; • can be used in the investigation of the imperfection sensitivity of a structure; • works only with symmetric matrices (hence, unsymmetric stiffness contributions such as the load stiffness associated with follower loads are symmetrized); and • cannot be used in a model containing substructures. General eigenvalue buckling In an eigenvalue buckling problem we look for the loads for which the model stiffness matrix becomes singular, so that the problem has nontrivial solutions. are nontrivial displacement solutions. The applied loads can consist of pressures, concentrated forces, nonzero prescribed displacements, and/or thermal loading. is the tangent stiffness matrix when the loads are applied, and the Eigenvalue buckling is generally used to estimate the critical buckling loads of stiff structures (classical eigenvalue buckling). Stiff structures carry their design loads primarily by axial or membrane action, rather than by bending action. Their response usually involves very little deformation prior to buckling. A simple example of a stiff structure is the Euler column, which responds very stiffly to a compressive axial load until a critical load is reached, when it bends suddenly and exhibits a much lower stiffness. However, even when the response of a structure is nonlinear before collapse, a general eigenvalue buckling analysis can provide useful estimates of collapse mode shapes. The base state The buckling loads are calculated relative to the base state of the structure. If the eigenvalue buckling procedure is the first step in an analysis, the initial conditions form the base state; otherwise, the base state is the current state of the model at the end of the last general analysis step . Thus, the base state can include preloads (“dead” loads), . The preloads are often zero in classical eigenvalue buckling problems. If geometric nonlinearity was included in the general analysis steps prior to the eigenvalue buckling analysis , the base state geometry is the deformed geometry at the end of the last general analysis step. If geometric nonlinearity was omitted, the base state geometry is the original configuration of the body. The eigenvalue problem An incremental loading pattern, magnitude of this loading is not important; it will be scaled by the load multipliers, eigenvalue problem: , is defined in the eigenvalue buckling prediction step. The , found in the where is the stiffness matrix corresponding to the base state, which includes the effects of the preloads, (if any); is the differential initial stress and load stiffness matrix due to the incremental loading pattern, ; are the eigenvalues; are the buckling mode shapes (eigenvectors); M and N refer to degrees of freedom M and N of the whole model; and refers to the ith buckling mode. The critical buckling loads are then preload pattern, thermal loading caused by temperature changes, while , and perturbation load pattern, . Normally, the lowest value of , may be different. For example, is caused by application of pressure. is of interest. The might be The buckling mode shapes, , are normalized vectors and do not represent actual magnitudes of deformation at critical load. They are normalized so that the maximum displacement component is 1.0. If all displacement components are zero, the maximum rotation component is normalized to 1.0. These buckling mode shapes are often the most useful outcome of the eigenvalue analysis, since they predict the likely failure mode of the structure. Abaqus/Standard can extract eigenvalues and eigenvectors for symmetric matrices only; therefore, are symmetrized. If the matrices have significant unsymmetric parts, the eigenproblem and may not be exactly what you expected to solve. Selecting the eigenvalue extraction method Abaqus/Standard offers the Lanczos and the subspace iteration eigenvalue extraction methods. The Lanczos method is generally faster when a large number of eigenmodes is required for a system with many degrees of freedom. The subspace iteration method may be faster when only a few (less than 20) eigenmodes are needed. By default, the subspace iteration eigensolver is employed. Subspace iteration and the Lanczos solver can be used for different steps in the same analysis; there is no requirement that the same eigensolver be used for all appropriate steps. For both eigensolvers you specify the desired number of eigenvalues; Abaqus/Standard will choose a suitable number of vectors for the subspace iteration procedure or a suitable block size for the Lanczos method (although you can override this choice, if needed). Significant overestimation of the actual number of eigenvalues can create very large files. If the actual number of eigenvalues is underestimated, Abaqus/Standard will issue a corresponding warning message. In general, the block size for the Lanczos method should be as large as the largest expected multiplicity of eigenvalues (that is, the largest number of modes with the same eigenvalue). A block size larger than 10 is not recommended. If the number of eigenvalues requested is n, the default block size is the minimum of (7, n). The number of block Lanczos steps is usually determined by Abaqus/Standard, but you can change it when you define the eigenvalue buckling prediction step. In general, if a particular type of eigenproblem converges slowly, providing more block Lanczos steps will reduce the analysis cost. On the other hand, if you know that a particular type of problem converges quickly, providing fewer block Lanczos steps will reduce the amount of in-core memory used. If the number of eigenvalues requested is n, the default is Block size n ≤ 10 n > 10 ≥ 4 40 40 30 30 70 60 60 30 If the subspace iteration technique is requested, you can also specify the maximum eigenvalue of interest; Abaqus/Standard will extract eigenvalues until either the requested number of eigenvalues has been extracted or the last eigenvalue extracted exceeds the maximum eigenvalue of interest. If the Lanczos eigensolver is requested, you can also specify the minimum and/or maximum eigenvalues of interest; Abaqus/Standard will extract eigenvalues until either the requested number of eigenvalues has been extracted in the given range or all the eigenvalues in the given range have been extracted. Input File Usage: Use the following option to perform an eigenvalue buckling analysis using the subspace iteration method: *BUCKLE, EIGENSOLVER=SUBSPACE (default) Use the following option to perform an eigenvalue buckling analysis using the Lanczos method: Abaqus/CAE Usage: *BUCKLE, EIGENSOLVER=LANCZOS Step module: Create Step: Linear perturbation: Buckle: Eigensolver: Lanczos or Subspace Limitations associated with applying the Lanczos eigensolver to a buckling analysis The Lanczos eigensolver cannot be used for buckling analyses in which the stiffness matrix is indefinite, as in the following cases: • A model containing hybrid elements or connector elements. • A model containing distributing coupling constraints, defined either directly (“Coupling constraints,” Section 34.3.2; “Shell-to-solid coupling,” Section 34.3.3; or “Mesh-independent fasteners,” Section 34.3.4) or by the distributing coupling elements (DCOUP2D and DCOUP3D). • A model containing contact pairs or contact elements. • A model that has been preloaded above the bifurcation (buckling) load. • A model that has rigid body modes. In such cases Abaqus/Standard will issue an error message and terminate the analysis. Order of calculation and formation of the stiffness matrices . , due to In an eigenvalue buckling prediction step Abaqus/Standard first does a static perturbation analysis to determine the incremental stresses, If the base state did not include geometric nonlinearity, the stiffness matrix used in this static perturbation analysis is the tangent elastic stiffness. If the base state did include geometric nonlinearity, initial stress and load stiffness terms (due to the preload, and In the eigenvalue extraction portion of the buckling step, the stiffness matrix corresponding to the base state geometry is formed. Initial stress and the load stiffness terms due to the preload, , are always included regardless of whether or not geometric nonlinearity is included and are calculated based on the geometry of the base state. When forming the stiffness matrices , all contact conditions are fixed in the base ) are included. The stiffness matrix corresponding to is then formed. and state. Buckling modes with closely spaced eigenvalues Some structures have many buckling modes with closely spaced eigenvalues, which can cause numerical problems. In these cases it often helps to apply enough preload, , to load the structure to just below the buckling load before performing the eigenvalue extraction. If is a scalar constant and the structure is “stiff” and elastic—and if the —where problem is linear, the structural stiffness changes to and the buckling loads are given by . The structure should not be preloaded above the buckling load. In that case the subspace iteration process may fail to converge or produce incorrect results; the Lanczos eigensolver cannot be used (as discussed earlier). . The process is equivalent to a dynamic eigenfrequency extraction with shift In many cases a series of closely spaced eigenvalues indicates that the structure is imperfection sensitive. An eigenvalue buckling analysis will not give accurate predictions of the buckling load for imperfection-sensitive structures; the static Riks procedure should be used instead . Understanding negative eigenvalues Sometimes, negative eigenvalues are reported in an eigenvalue buckling analysis. In most cases such negative eigenvalues indicate that the structure would buckle if the load were applied in the opposite direction. A classical example is a plate under shear loading; the plate will buckle at the same value for positive and negative applied shear load. Buckling under reverse loading can also occur in situations where it may not be expected. For example, a pressure vessel under external pressure may exhibit a negative eigenvalue (buckling under internal pressure) due to local buckling of a stiffener. Such “physical” negative buckling modes are usually readily understood once they are displayed and can usually be avoided by applying a preload before the buckling analysis. Negative eigenvalues sometimes correspond to buckling modes that cannot be understood readily in terms of physical behavior, particularly if a preload is applied that causes significant geometric nonlinearity. In this case a geometrically nonlinear load-displacement analysis should be performed (“Unstable collapse and postbuckling analysis,” Section 6.2.4). Including large geometry changes in a buckling analysis Because buckling analysis is usually done for “stiff” structures, it is not usually necessary to include the effects of geometry change in establishing equilibrium for the base state. However, if significant geometry change is involved in the base state and this effect is considered to be important, it can be included by specifying that geometric nonlinearity should be considered for the base state step . In such cases it is probably more realistic to perform a geometrically nonlinear load-displacement analysis (Riks analysis) to determine the collapse loads, especially for imperfection-sensitive structures. While large deformation can be included in the preload, the eigenvalue buckling theory relies on there being little geometric change due to the “live” buckling load, . If the live load produces significant geometric change, a nonlinear collapse (Riks) analysis must be used. The total buckling load predicted by the eigenvalue analysis, , may be a good estimate for the limit load in the nonlinear buckling analysis. The Riks method is described in “Unstable collapse and postbuckling analysis,” Section 6.2.4. Initial conditions The initial values of quantities such as stress, temperature, field variables, and solution-dependent If the buckling step is the first step variables can be specified for an eigenvalue buckling analysis. “Initial conditions in in the analysis, these initial conditions form the base state of the structure. Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the available initial conditions. Boundary conditions Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6) or to warping degree of freedom 7 in open-section beam elements (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). A nonzero prescribed boundary condition in a general analysis step preceding the eigenvalue buckling analysis can be used to preload the structure. Nonzero boundary conditions prescribed in an eigenvalue buckling step will contribute to the incremental stress and, thus, will contribute to the differential initial stress stiffness. When prescribing nonzero boundary conditions, you must interpret the resulting eigenproblem carefully. Nonzero prescribed boundary conditions will be treated as constraints (i.e., as if they were fixed) during the eigenvalue extraction. Therefore, unless the prescribed boundary conditions are removed for the eigenvalue extraction by specifying buckling mode boundary conditions , the mode shapes may be altered by these boundary conditions. Amplitude definitions (“Amplitude curves,” Section 33.1.2) cannot be used to vary the magnitudes of prescribed boundary conditions during an eigenvalue buckling analysis. You can define perturbation load and buckling mode boundary conditions in an eigenvalue buckling prediction step. Input File Usage: Abaqus/CAE Usage: Use either of the following two options to define perturbation load boundary conditions: *BOUNDARY *BOUNDARY, LOAD CASE=1 Use the following option to define buckling mode boundary conditions: *BOUNDARY, LOAD CASE=2, OP=NEW The OP=NEW parameter is required when you define buckling mode boundary conditions in an eigenvalue buckling prediction step; however, the perturbation load boundary conditions in the step can use either OP=NEW or OP=MOD. Load module: Create Boundary Condition: choose Mechanical for the Category and Symmetry/Antisymmetry/Encastre for the Types for Selected Step: toggle on Stress perturbation only to define a perturbation load boundary condition; toggle on Buckling mode calculation only to define a buckling mode boundary condition; toggle on Stress perturbation and buckling mode calculation to define both types of boundary conditions select region: Combining boundary conditions The buckling mode shapes depend on the stresses in the base state as well as the incremental stresses due to the perturbation loading in the buckling step. These stresses are influenced by the boundary conditions used in each step. In a general eigenvalue buckling analysis the following types of boundary conditions can influence the stresses: 1. The boundary conditions in the base state. 2. The boundary conditions used to calculate the linear perturbation stresses, . These boundary conditions will be: a. the perturbation load boundary conditions specified in the eigenvalue buckling step; or b. the base-state boundary conditions if no perturbation load boundary conditions are specified in the eigenvalue buckling step; or c. the buckling mode boundary conditions if neither perturbation load boundary conditions nor base-state boundary conditions exist. 3. The boundary conditions used for the eigenvalue extraction. These boundary conditions will be: a. the buckling mode boundary conditions; or b. the perturbation load boundary conditions if buckling mode boundary conditions are not specified in the eigenvalue buckling step; or c. the base-state boundary conditions if no boundary condition definition is used in the eigenvalue buckling step. Table 6.2.3–1 summarizes the use of boundary conditions during an eigenvalue buckling step. When buckling mode boundary conditions are specified, all boundary conditions to be imposed during eigenvalue extraction must be specified. Buckling of symmetric structures The buckling mode shapes of symmetric structures subjected to symmetric loadings are either symmetric or antisymmetric. In such cases it is often more efficient to model only part of the structure and then perform the buckling analysis twice for each symmetry plane: once with symmetric boundary conditions and once with antisymmetric boundary conditions. The live load pattern is usually symmetric, so symmetric boundary conditions are required for the calculation of the perturbation stresses used in the formation of the initial stress stiffness matrix. The boundary conditions must be switched to antisymmetric for the eigenvalue extraction to obtain the antisymmetric modes. “Buckling of a cylindrical shell under uniform axial pressure,” Section 1.2.3 of the Abaqus Benchmarks Manual, illustrates such a case. If the model includes more than one symmetry plane, it may be necessary to study all permutations of symmetric and antisymmetric boundary conditions for each symmetry plane. Table 6.2.3–1 Boundary conditions in effect during the different portions of an eigenvalue buckling analysis. User-defined boundary conditions Boundary conditions used by Abaqus Base state Eigenvalue buckling prediction step Linear perturbation Eigenvalue extraction 1, 2 1, 2 B = base-state boundary conditions; 0 = no boundary conditions specified 1 = perturbation load boundary conditions 2 = buckling mode boundary conditions Asymmetric buckling of axisymmetric structures Axisymmetric structures subjected to compressive loading often collapse in nonaxisymmetric modes. These modes cannot be found with purely axisymmetric modeling such as that provided by shell elements SAX1 and SAX2 (“Axisymmetric shell element library,” Section 29.6.9) or continuum elements CAX4 or CAX8 (“Axisymmetric solid element library,” Section 28.1.6). Such analyses must be done with three-dimensional shell or continuum elements. Loads The following types of loading can be prescribed in an eigenvalue buckling analysis: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” The load stiffness can have a significant effect on the critical buckling load; therefore, Abaqus/Standard will take the load stiffness due to preloads into account when solving the eigenvalue buckling problem. It is important that the structure not be preloaded above the critical buckling load. Any load applied during the eigenvalue buckling analysis is called a “live” load. This incremental , describes the load pattern for which buckling sensitivity is being investigated; its magnitude load, is not important. This incremental loading definition represents linear perturbation loads, as described in “Applying loads: overview,” Section 33.4.1. Follower forces (such as concentrated loads assumed to rotate with the nodal rotation or pressure loads) lead to an unsymmetric load stiffness. Since eigenvalue extraction in Abaqus/Standard can be performed only on symmetric matrices, eigenvalue analysis with follower loads may not yield correct results. Amplitude definitions cannot be used during an eigenvalue buckling analysis. “Applying loads: overview,” Section 33.4.1, describes all of the available loads. Prescribed boundary conditions can also be used to load the structure in an eigenvalue buckling analysis, as discussed earlier. Predefined fields In an eigenvalue buckling prediction step, nodal temperatures can be specified . The specified temperatures will cause thermal strain during the static perturbation analysis if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2), and incremental stresses will be generated. Hence, Abaqus/Standard can analyze buckling due to thermal stress. The specified temperature will not affect temperature-dependent material properties during the eigenvalue buckling prediction step; the material properties are based on the temperature in the base state. Amplitude definitions cannot be used to vary the magnitudes of prescribed temperatures during an eigenvalue buckling analysis. Material options During an eigenvalue buckling analysis, the model’s response is defined by its linear elastic stiffness in the base state. All nonlinear and/or inelastic material properties, as well as effects involving time or strain rate, are ignored during an eigenvalue buckling analysis. In classical eigenvalue buckling the response in the base state is also linear. If temperature-dependent elastic properties are used, the eigenvalue buckling analysis will not account for changes in the stiffness matrix due to temperature changes. The material properties of the base state will be used. Acoustic properties, thermal properties (except for thermal expansion), mass diffusion properties, electrical properties, and pore fluid flow properties are not active during an eigenvalue buckling analysis. Elements Any of the stress/displacement elements in Abaqus/Standard (including those with temperature or pressure degrees of freedom) can be used in an eigenvalue buckling analysis, with the exception that hybrid and contact elements cannot be used with the Lanczos eigensolver (as discussed earlier). See “Choosing the appropriate element for an analysis type,” Section 27.1.3. Output The values of the eigenvalues, , will be listed in the printed output file. If output of stresses, strains, reaction forces, etc. is requested, this information will be printed for each eigenvalue; these quantities are perturbation values and represent mode shapes, not absolute values. All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Buckling mode shapes can be plotted in the Visualization module of Abaqus/CAE. Input file template The following template describes a very general eigenvalue buckling problem, where as many eigenvalue buckling prediction steps as needed can be specified. Symmetric boundary conditions are specified in the model definition part of the Abaqus/Standard therefore, belong to the base state . In the first buckling step Abaqus/Standard uses the base-state boundary conditions to solve for the perturbation stresses as well as for the eigenvalue extraction. In the second buckling step the boundary conditions for the base state, the initial stress calculation, and the eigenvalue extraction are all different. Abaqus/Standard uses the specified symmetry boundary conditions to solve for the perturbation stresses but uses the specified antisymmetry boundary conditions for the eigenvalue extraction. *HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions contributing to the base state ** *STEP, NLGEOM The load stiffness terms will be included in the eigenvalue buckling steps since the NLGEOM parameter is used in this (optional) preload step *STATIC Data line to control incrementation *BOUNDARY Data lines to specify nonzero boundary conditions (dead loads) *CLOAD and/or *DLOAD and/or *TEMPERATURE Data lines to specify dead loads, *END STEP ** *STEP *BUCKLE Data line to request the desired number of symmetric modes *CLOAD and/or *DLOAD and/or *TEMPERATURE Data lines to specify perturbation loading, *END STEP ** *STEP *BUCKLE Data line to request the desired number of antisymmetric modes *CLOAD and/or *DLOAD and/or *TEMPERATURE Data lines to specify perturbation loading, *BOUNDARY, LOAD CASE=1 Data lines to specify all boundary conditions for perturbation loading *BOUNDARY, LOAD CASE=2, OP=NEW Data lines to specify all antisymmetric boundary conditions for eigenvalue extraction *END STEP 6.2.4 UNSTABLE COLLAPSE AND POSTBUCKLING ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Static stress analysis procedures: overview,” Section 6.2.1 • “Introducing a geometric imperfection into a model,” Section 11.3.1 • *STATIC • *IMPERFECTION • “Configuring a static, Riks procedure” in “Configuring general analysis procedures,” in the online HTML version of this Section 14.11.1 of the Abaqus/CAE User’s Manual, manual Overview The Riks method: • is generally used to predict unstable, geometrically nonlinear collapse of a structure; • can include nonlinear materials and boundary conditions; • often follows an eigenvalue buckling analysis to provide complete information about a structure’s collapse; and • can be used to speed convergence of ill-conditioned or snap-through problems that do not exhibit instability. Unstable response Geometrically nonlinear static problems sometimes involve buckling or collapse behavior, where the load-displacement response shows a negative stiffness and the structure must release strain energy to remain in equilibrium. Several approaches are possible for modeling such behavior. One is to treat the buckling response dynamically, thus actually modeling the response with inertia effects included as the structure snaps. This approach is easily accomplished by restarting the terminated static procedure (“Restarting an analysis,” Section 9.1.1) and switching to a dynamic procedure (“Implicit dynamic analysis using direct integration,” Section 6.3.2) when the static solution becomes unstable. In some simple cases displacement control can provide a solution, even when the conjugate load (the reaction force) is decreasing as the displacement increases. Another approach would be to use dashpots to stabilize the structure during a static analysis. Abaqus/Standard offers an automated version of this stabilization approach for the static analysis procedures . Alternatively, static equilibrium states during the unstable phase of the response can be found by using the “modified Riks method.” This method is used for cases where the loading is proportional; that is, where the load magnitudes are governed by a single scalar parameter. The method can provide solutions even in cases of complex, unstable response such as that shown in Figure 6.2.4–1. 1.0 Load, P Figure 6.2.4–1 Proportional loading with unstable response. Displacement The Riks method is also useful for solving ill-conditioned problems such as limit load problems or almost unstable problems that exhibit softening. The Riks method In simple cases linear eigenvalue analysis (“Eigenvalue buckling prediction,” Section 6.2.3) may be sufficient for design evaluation; but if there is concern about material nonlinearity, geometric nonlinearity prior to buckling, or unstable postbuckling response, a load-deflection (Riks) analysis must be performed to investigate the problem further. The Riks method uses the load magnitude as an additional unknown; it solves simultaneously for loads and displacements. Therefore, another quantity must be used to measure the progress of the solution; Abaqus/Standard uses the “arc length,” l, along the static equilibrium path in load-displacement space. This approach provides solutions regardless of whether the response is stable or unstable. See the “Modified Riks algorithm,” Section 2.3.2 of the Abaqus Theory Manual, for a detailed description of the method. Proportional loading If the Riks step is a continuation of a previous history, any loads that exist at the beginning of the step and are not redefined are treated as “dead” loads with constant magnitude. A load whose magnitude is defined in the Riks step is referred to as a “reference” load. All prescribed loads are ramped from the initial (dead load) value to the reference values specified. The loading during a Riks step is always proportional. The current load magnitude, , is defined by is the “dead load,” is the “load proportionality factor.” where The load proportionality factor is found as part of the solution. Abaqus/Standard prints out the current value of the load proportionality factor at each increment. is the reference load vector, and Incrementation Abaqus/Standard uses Newton’s method (as described in “Static stress analysis,” Section 6.2.2) to solve the nonlinear equilibrium equations. The Riks procedure uses only a 1% extrapolation of the strain increment. You provide an initial increment in arc length along the static equilibrium path, , when you define the step. The initial load proportionality factor, , is computed as where is a user-specified total arc length scale factor (typically set equal to 1). This value of is used during the first iteration of a Riks step. For subsequent iterations and increments the value is part of , can be used to control is computed automatically, so you have no control over the load magnitude. The value of of the solution. Minimum and maximum arc length increments, the automatic incrementation. and Input File Usage: Abaqus/CAE Usage: *STATIC, RIKS Step module: Create Step: General: Static, Riks Direct user control of the increment size is also provided; in this case the incremental arc length, , is kept constant. This method is not recommended for a Riks analysis since it prevents Abaqus/Standard from reducing the arc length when a severe nonlinearity is encountered. Input File Usage: Abaqus/CAE Usage: *STATIC, RIKS, DIRECT Step module: Create Step: General: Static, Riks: Incrementation: Type: Fixed Ending a Riks analysis step Since the loading magnitude is part of the solution, you need a method to specify when the step is completed. You can specify a maximum value of the load proportionality factor, , or a maximum displacement value at a specified degree of freedom. The step will terminate when either value is crossed. If neither of these finishing conditions is specified, the analysis will continue for the number of increments specified in the step definition . Bifurcation The Riks method works well in snap-through problems—those in which the equilibrium path in load-displacement space is smooth and does not branch. Generally you do not need take any special precautions in problems that do not exhibit branching (bifurcation). “Snap-through buckling analysis of circular arches,” Section 1.2.1 of the Abaqus Example Problems Manual, is an example of a smooth snap-through problem. The Riks method can also be used to solve postbuckling problems, both with stable and unstable postbuckling behavior. However, the exact postbuckling problem cannot be analyzed directly due to the discontinuous response at the point of buckling. To analyze a postbuckling problem, it must be turned into a problem with continuous response instead of bifurcation. This effect can be accomplished by introducing an initial imperfection into a “perfect” geometry so that there is some response in the buckling mode before the critical load is reached. Introducing geometric imperfections Imperfections are usually introduced by perturbations in the geometry. Unless the precise shape of an imperfection is known, an imperfection consisting of multiple superimposed buckling modes must be introduced (“Eigenvalue buckling prediction,” Section 6.2.3). Abaqus allows you to define imperfections; see “Introducing a geometric imperfection into a model,” Section 11.3.1. In this way the Riks method can be used to perform postbuckling analyses of structures that show linear behavior prior to (bifurcation) buckling. An example of this method of introducing geometric imperfections is presented in “Buckling of a cylindrical shell under uniform axial pressure,” Section 1.2.3 of the Abaqus Benchmarks Manual. By performing a load-displacement analysis, other important nonlinear effects, such as material inelasticity or contact, can be included. In contrast, all inelastic effects are ignored in a linear eigenvalue buckling analysis and all contact conditions are fixed in the base state. Imperfections based on linear buckling modes can also be useful for the analysis of structures that behave inelastically prior to reaching peak load. Introducing loading imperfections Perturbations in loads or boundary conditions can also be used to introduce initial imperfections. In this case fictitious “trigger” loads can be used to initiate the instability. The trigger loads should perturb the structure in the expected buckling modes. Typically, these loads are applied as dead loads prior to the Riks step so that they have fixed magnitudes. The magnitudes of trigger loads must be sufficiently small so that they do not affect the overall postbuckling solution. It is your responsibility to choose appropriate magnitudes and locations for such fictitious loads; Abaqus/Standard does not check that they are reasonable. Obtaining a solution at a particular load or displacement value The Riks algorithm cannot obtain a solution at a given load or displacement value since these are treated as unknowns—termination occurs at the first solution that satisfies the step termination criterion. To obtain solutions at exact values of load or displacement, the solution must be restarted at the desired point in the step (“Restarting an analysis,” Section 9.1.1) and a new, non-Riks step must be defined. Since the subsequent step is a continuation of the Riks analysis, the load magnitude in that step must be given appropriately so that the step begins with the loading continuing to increase or decrease according to its behavior at the point of restart. For example, if the load was increasing at the restart point and was positive, a larger load magnitude than the current magnitude should be given in the restart step to continue this behavior. If the load was decreasing but positive, a smaller magnitude than the current magnitude should be specified. Restrictions A Riks analysis is subject to the following restrictions: • A Riks step cannot be followed by another step in the same analysis. Subsequent steps must be analyzed by using the restart capability. • If a Riks analysis includes irreversible deformation such as plasticity and a restart using another Riks step is attempted while the magnitude of the load on the structure is decreasing, Abaqus/Standard will find the elastic unloading solution. Therefore, restart should occur at a point in the analysis where the load magnitude is increasing if plasticity is present. • For postbuckling problems involving loss of contact, the Riks method will usually not work; inertia or viscous damping forces (such as those provided by dashpots) must be introduced in a dynamic or static analysis to stabilize the solution. Initial conditions Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified; “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the available initial conditions. Boundary conditions Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6) or to warping degree of freedom 7 in open-section beam elements (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). Amplitude definitions (“Amplitude curves,” Section 33.1.2) cannot be used to vary the magnitudes of prescribed boundary conditions during a Riks analysis. Loads The following loads can be prescribed in a Riks analysis: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” Since Abaqus/Standard scales loading magnitudes proportionally based on the user-specified magnitudes, amplitude references are ignored when the Riks method is chosen. If follower loads are prescribed, their contribution to the stiffness matrix may be unsymmetric; the unsymmetric matrix storage and solution scheme can be used to improve computational efficiency in such cases . Predefined fields Nodal temperatures can be specified . Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The loads generated by the thermal strain contribute to the “reference” load specified for the Riks analysis and are ramped up with the load proportionality factor. Hence, the Riks procedure can analyze postbuckling and collapse due to thermal straining. The values of other user-defined field variables can be specified. These values affect only field- variable-dependent material properties, if any. Since the concept of time is replaced by arc length in a Riks analysis, the use of properties that change due to changes in temperatures and/or field variables is not recommended. Material options Most material models that describe mechanical behavior are available for use in a Riks analysis. The following material properties are not active during a Riks analysis: acoustic properties, thermal properties (except for thermal expansion), mass diffusion properties, electrical properties, and pore fluid flow properties. Materials with history dependence can be used; however, it should be realized that the results will depend on the loading history, which is not known in advance. The concept of time is replaced by arc length in a Riks analysis. Therefore, any effects involving time or strain rate (such as viscous damping or rate-dependent plasticity) are no longer treated correctly and should not be used. See Part V, “Materials,” for details on the material models available in Abaqus/Standard. Elements Any of the stress/displacement elements in Abaqus/Standard (including those with temperature or pressure degrees of freedom) can be used in a Riks analysis . Dashpots should not be used since velocities will be calculated as displacement increments divided by arc length, which is meaningless. Output Output options are provided to allow the magnitudes of individual load components (pressure, point loads, etc.) to be printed or to be written to the results file. The current value of the load proportionality factor, LPF, will be given automatically with any results or output database file output request. These output options are recommended when the Riks method is used so that load magnitudes can be seen directly. All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Input file template *HEADING … *INITIAL CONDITIONS Data lines to define initial conditions *BOUNDARY Data lines to specify zero-valued boundary conditions ** *STEP, NLGEOM *STATIC *CLOAD and/or *DLOAD and/or *TEMPERATURE Data lines to specify preload (dead load), *END STEP ** *STEP, NLGEOM *STATIC, RIKS Data line to define incrementation and stopping criteria *CLOAD and/or *DLOAD and/or *TEMPERATURE Data lines to specify reference loading, *END STEP 6.2.5 QUASI-STATIC ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Static stress analysis procedures: overview,” Section 6.2.1 • *VISCO • “Configuring a transient, static, stress/displacement analysis with time-dependent material response” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A quasi-static stress analysis in Abaqus/Standard: • is used to analyze problems with time-dependent material response (creep, swelling, viscoelasticity, and two-layer viscoplasticity); • is used when inertia effects can be neglected; and • can be linear or nonlinear. See “Mass scaling,” Section 11.6.1, and “Explicit dynamic analysis,” Section 6.3.3, for information on conducting quasi-static analysis in Abaqus/Explicit. See “Implicit dynamic analysis using direct integration,” Section 6.3.2, for information on conducting quasi-static analysis using a dynamic procedure in Abaqus/Standard. Incrementation You can control the time incrementation in a quasi-static analysis directly, or it can be controlled automatically by Abaqus/Standard. Automatic incrementation is preferred in almost all cases. Fixed incrementation If you specify the time increments in a quasi-static analysis directly, fixed time increments equal to the specified initial time increment will be used throughout the analysis. Input File Usage: Abaqus/CAE Usage: *VISCO Step module: Create Step: General: Visco Automatic incrementation If you select automatic incrementation, the size of the time increment is limited by the accuracy of the integration. The user-specified accuracy tolerance parameter limits the maximum inelastic strain rate change allowed over an increment: where t is the time at the beginning of the increment, at the end of the increment), and chosen for the accuracy tolerance parameter should be on the order of is the time is the time increment (so that is the equivalent creep strain rate. To achieve accuracy, the value for creep problems, where is an acceptable level of error in the stress and E is a typical elastic modulus, or on the order of the elastic strains for viscoelasticity problems. Input File Usage: Abaqus/CAE Usage: *VISCO, CETOL=tolerance Step module: Create Step: General: Visco: Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance Selecting explicit creep integration Nonlinear creep problems (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) that exhibit no other nonlinearities can be solved efficiently by forward-difference integration of the inelastic strains if the inelastic strain increments are smaller than the elastic strains. This explicit method is efficient computationally because, unlike implicit methods, iteration is not required. Although this method is only conditionally stable, the numerical stability limit of the explicit operator is in many cases sufficiently large to allow the solution to be developed in a reasonable number of time increments. For creep at very low stress levels, however, the unconditional stability of the backward difference In such cases Abaqus/Standard will invoke the implicit operator (implicit method) is desirable. integration scheme automatically. Explicit integration can be less expensive computationally and simplifies implementation of user- defined creep laws in user subroutine CREEP; you can restrict Abaqus/Standard to using this method for creep problems (with or without geometric nonlinearity included). See “Rate-dependent plasticity: creep and swelling,” Section 23.2.4, for further details. Input File Usage: Abaqus/CAE Usage: *VISCO, CETOL=tolerance, CREEP=EXPLICIT Step module: Create Step: General: Visco: Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance and Creep/swelling/viscoelastic integration: Explicit Integration scheme for viscoelasticity and rate-dependent yield Problems including “Time domain viscoelasticity,” Section 22.7.1, are always integrated with an unconditionally stable operator. The time step in these problems is limited only by the accuracy tolerance parameter defined above. Problems including “Rate-dependent yield,” Section 23.2.3, and “Parallel network viscoelastic model,” Section 22.8.2, are always integrated using an implicit, unconditionally stable method. The accuracy tolerance parameter does not limit the inelastic strain rate change and can be set equal to any nonzero value to activate automatic time incrementation. Unstable problems Some types of analyses may develop local instabilities, such as surface wrinkling, material instability, or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with the aid of automatic incrementation. Abaqus/Standard offers the ability to stabilize this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1. Initial conditions Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified, as described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. Boundary conditions Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6); to warping degree of freedom 7 in open-section beam elements; or, if hydrostatic fluid elements are included in the model, to fluid pressure degree of freedom 8. If boundary conditions are applied to rotation degrees of freedom, you must understand how Abaqus handles finite rotations. See “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Loads The following types of loading can be prescribed in a quasi-static analysis: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” Predefined fields The following predefined fields can be specified in a quasi-static analysis, as described in “Predefined fields,” Section 33.6.1: • Although temperature is not a degree of freedom in quasi-static analysis, nodal temperatures can be specified. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any. • The values of user-defined field variables can be specified. These values affect only field-variable- dependent material properties, if any. Material options The quasi-static procedure in Abaqus/Standard is generally used to analyze quasi-static creep and swelling problems, which occur over fairly long time periods (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4). This procedure can also be used to analyze viscoelastic materials (“Time domain viscoelasticity,” Section 22.7.1, and “Parallel network viscoelastic model,” Section 22.8.2) and two-layer viscoplastic materials (“Two-layer viscoplasticity,” Section 23.2.11). In addition, all material models that are valid in a static analysis procedure can be used. Elements Any of the stress/displacement elements in Abaqus/Standard (including those with temperature or pressure degrees of freedom) can be used in a quasi-static stress analysis—see “Choosing the appropriate element for an analysis type,” Section 27.1.3. Output In addition to the usual output variables available in Abaqus/Standard , the following variables are provided specifically for creep problems: Element integration point variables: CEEQ CESW Equivalent creep strain, . Magnitude of the swelling strain. CEMAG Magnitude of the creep strain, . CEP CE Principal creep strains. Output of all of the creep strain components and CEEQ, CESW, and CEMAG. Input file template *HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS Data lines to specify initial conditions *AMPLITUDE Data lines to define amplitude variations ** *STEP (,NLGEOM) *VISCO, CETOL=tolerance Data line to define time incrementation and a “real” time scale *BOUNDARY Data lines to describe nonzero boundary conditions *CLOAD and/or *DLOAD and/or *TEMPERATURE and/or *FIELD Data lines to specify loading *END STEP 6.2.6 DIRECT CYCLIC ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • *DIRECT CYCLIC • *TIME POINTS • *CONTROLS • “Configuring a direct cyclic procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A direct cyclic analysis: • is a quasi-static analysis; • uses a combination of Fourier series and time integration of the nonlinear material behavior to obtain the stabilized cyclic response of the structure iteratively; • avoids the considerable numerical expense associated with a transient analysis; • is ideally suited for very large problems in which many load cycles must be applied to obtain the stabilized response if transient analysis is performed; • can be performed with linear or nonlinear material with localized plastic deformation; • can be used to predict the likelihood of plastic ratchetting; • assumes geometrically linear behavior and fixed contact conditions; • uses the elastic stiffness, so the equation system is inverted only once; and • can also be used to predict progressive damage and failure for ductile bulk materials and/or to predict delamination/debonding growth at the interfaces in laminated composites in a low-cycle fatigue analysis. Introduction It is well known that after a number of repetitive loading cycles, the response of an elastic-plastic structure, such as an automobile exhaust manifold subjected to large temperature fluctuations and clamping loads, may lead to a stabilized state in which the stress-strain relationship in each successive cycle is the same as in the previous one. The classical approach to obtain the response of such a structure is to apply the periodic loading repetitively to the structure until a stabilized state is obtained. This approach can be quite expensive, since it may require the application of many loading cycles before the stabilized response is obtained. To avoid the considerable numerical expense associated with a transient analysis, a direct cyclic analysis can be used to calculate the cyclic response of the structure directly. The basis of this method is to construct a displacement function structure at all times t during a load cycle with period T as shown in Figure 6.2.6–1. that describes the response of the stabilized solution solution at iteration n+1 solution at iteration n t 1∇ t n∇ t n-1 t n t n+1 Figure 6.2.6–1 A displacement function at all times t during a load cycle with period T at different iterations. A truncated Fourier series is used for this purpose, , and is the angular frequency, where n stands for the number of terms in the Fourier series, and are unknown displacement coefficients associated with each degree of freedom in the problem. Abaqus/Standard solves for the unknown displacement coefficients by using a modified Newton method, with the elastic stiffness matrix at the beginning of the analysis step serving as the Jacobian in the scheme. We expand the residual vector in the modified Newton method using a Fourier series of the same form as the displacement solution: where each residual vector coefficient coefficient entire load cycle. At each instant in time in the cycle Abaqus/Standard obtains the residual vector in the Fourier series corresponds to a displacement , respectively. The residual coefficients are obtained by tracking through the by , and , and , the Fourier coefficients DIRECT CYCLIC ANALYSIS The displacement solution is obtained by solving for corrections to the displacement Fourier coefficients corresponding to each residual coefficient. The updated displacement solution is used in the next iteration to obtain the displacements at each instant in time. This process is repeated until convergence is obtained. Each pass through the complete load cycle can, therefore, be thought of as a single iteration of the solution to the nonlinear problem. Convergence is measured by ensuring that all entries of the residual coefficients are small. The algorithm to obtain a stabilized cycle is described in detail in “Direct cyclic algorithm,” Section 2.2.3 of the Abaqus Theory Manual. Direct cyclic analysis A direct cyclic step can be the only step in an analysis, can follow a general or linear perturbation step, or can be followed by a general or linear perturbation step. If a direct cyclic step is followed by a general step, the solution at the end of the direct cyclic step will be the initial state of the general step. If a direct cyclic step follows a general or linear perturbation step, the elastic stiffness matrix at the end of the last general analysis step prior to the direct cyclic step will serve as the Jacobian in the direct cyclic procedure. Any prior (non-cyclic) loads are simply included in the constant part of the Fourier expansion of the residual vectors, and the plastic strains at the end of the preloading step are used as initial conditions for the direct cyclic step. Multiple direct cyclic analysis steps can be included in a single analysis. In such a case the Fourier series coefficients obtained in the previous step can be used as starting values in the current step. By default, the Fourier coefficients are reset to zero, thus allowing application of cyclic loading conditions that are very different from those defined in the previous direct cyclic step. You can specify that a direct cyclic step in a restart analysis should use the Fourier coefficients from the previous step, thus allowing continuation of an analysis that has not reached a stabilized cycle. In a direct cyclic analysis a restart file is written at the end of the cycle or time period. Consequently, a restart analysis that is a continuation of a previous direct cyclic analysis will start with a new iteration at . Input File Usage: Use the following option to reset the Fourier series coefficients to zero: *DIRECT CYCLIC, CONTINUE=NO (default) Use the following option to specify that the current step is a continuation of the previous direct cyclic step: *DIRECT CYCLIC, CONTINUE=YES Abaqus/CAE Usage: Use the following option to reset the Fourier series coefficients to zero (default): Step module: Create Step: General: Direct cyclic Use the following option to specify that the current step is a continuation of the previous direct cyclic step: Step module: Create Step: General: Direct cyclic; Basic: Use displacement Fourier coefficients from previous direct cyclic step Using the direct cyclic approach to perform low-cycle fatigue analysis The direct cyclic procedure can also be used in conjunction with the damage extrapolation technique to predict progressive damage and failure for ductile bulk materials and/or to predict delamination/debonding at the interfaces in laminated composites in a low-cycle fatigue analysis. In this case multiple cycles can be included in a single direct cyclic analysis, as described in “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7. Input File Usage: Abaqus/CAE Usage: *DIRECT CYCLIC, FATIGUE Step module: Create Step: General: Direct cyclic; Fatigue: Include low-cycle fatigue analysis Controlling the solution accuracy Direct cyclic analysis combines a Fourier series approximation with time integration of the nonlinear material behavior to obtain the stabilized cyclic solution iteratively using a modified Newton method. The accuracy of the algorithm depends on the number of Fourier terms used, the number of iterations taken to obtain the stabilized solution, and the number of time points within the load period at which the material response and residual vector are evaluated. Abaqus/Standard allows you to control the solution in several ways, as described below. Controlling the iterations in the modified Newton method In the direct cyclic method global Newton iterations are performed to determine corrections to the displacement Fourier coefficients. During each global iteration Abaqus/Standard tracks through the entire time cycle to compute the residual vector at a suitable number of time points. This involves standard element-by-element finite element calculations in which history-dependent material variables are integrated. The residual vector is integrated over the period to obtain the Fourier residual coefficients, which in turn yield corrections in displacement coefficients when the system of equations is solved. Abaqus/Standard will continue with the iterative process until convergence is obtained or until the maximum number of iterations allowed has been reached. You can specify the maximum number of iterations when you define the direct cyclic step; the default is 200 iterations. Input File Usage: *DIRECT CYCLIC , , , , , , , max number of iterations Abaqus/CAE Usage: Step module: Create Step: General: Direct cyclic; Incrementation: Maximum number of iterations: max number of iterations Specifying convergence criteria Convergence is best measured by ensuring that all the residual coefficients are sufficiently small compared to the time averaged force and that all the corrections to displacement Fourier coefficients are sufficiently small compared to the displacement Fourier coefficients. The time averaged force is defined in “Convergence criteria for nonlinear problems,” Section 7.2.3. Abaqus/Standard requires that the ratio of the maximum residual coefficient to the time averaged force, , and the ratio of the maximum correction to the displacement coefficients to the largest displacement coefficient, , are less than the tolerances. The default values are = 0.005. To change these values, you must define direct cyclic controls. = 0.005 and plastic ratchetting occurs, the displacement and residual coefficients of all the periodic terms ( When a stabilized cyclic response does not exist, the method will not converge. In the case where , and ) in the Fourier series converge. However, the displacement and the residual coefficients of the ) in the Fourier series continue to grow from one iteration to another iteration. are used to detect the plastic ratchetting. The default values = 0.005. For more information, see “Controlling the solution accuracy in constant term ( The user-specified tolerances are direct cyclic analysis” in “Commonly used control parameters,” Section 7.2.2. = 0.005 and and and Input File Usage: Abaqus/CAE Usage: *CONTROLS, TYPE=DIRECT CYCLIC Step module: Other→General Solution Controls→Edit; Specify: Direct Cyclic Controlling the Fourier representations The number of Fourier terms required to obtain an accurate solution depends on the variation of the load as well as the variation of the structural response over the period. In determining the number of terms, keep in mind that the objective of this kind of analysis is to make low-cycle fatigue predictions. Hence, the goal is to obtain good approximation of the plastic strain cycle at each point; local inaccuracies in the stresses are less important. More Fourier terms usually provide a more accurate solution but at the expense of additional data storage and computational time. In addition, an accurate integration of the Fourier residual coefficients requires that the residual vector be evaluated at an adequate number of time points during the cycle. Abaqus/Standard uses a trapezoidal rule, which assumes a linear variation of the residual over a time increment, to integrate the residual coefficients. For accurate integration the number of time points must be larger than the number of Fourier coefficients (which is equal to , where n represents the number of Fourier terms). Abaqus/Standard will automatically reduce the number of Fourier coefficients used for the next iteration if it is found to be greater than the number of increments taken to complete an iteration. Abaqus/Standard uses an adaptive algorithm to determine the number of Fourier terms. By default, Abaqus/Standard starts with 11 terms and determines the response of the structure by using the iterative method described before. Once convergence is obtained (which is measured by ensuring that all the residual vector coefficients and all the corrections to displacement coefficients in the Fourier series are sufficiently small), Abaqus/Standard evaluates if a sufficient number of Fourier terms are used by determining if equilibrium was satisfied at all the time points during the cycle. If equilibrium is satisfied at all time points, the solution is accepted. Otherwise, Abaqus/Standard increases the number of Fourier terms (by default, 5 terms are added) and continues with the iterative scheme until convergence with the new number of Fourier terms is obtained. This process is repeated until equilibrium is reached or until the maximum number of Fourier terms has been used. This scheme is best illustrated in Figure 6.2.6–2, where both local equilibrium and overall convergence are obtained when the number of Fourier terms is equal to 21. A maximum number of 25 Fourier terms is used by default. You can specify the initial and maximum number of Fourier terms and the increment in the number of terms when you define the direct cyclic step. ratio of maximum residual to time average force equilibrium tolerance stabilized iteration with 11 terms stabilized iteration with 16 terms stabilized iteration with 21 terms equilibrium tolerance Figure 6.2.6–2 Stabilized iterations with different Fourier terms. You can also define the convergence criteria for determining convergence and for determining whether equilibrium is achieved at all time points through the period , with suitable defaults set by Abaqus/Standard. In a direct cyclic analysis that has not reached a stabilized cycle, you can increase the number of iterations or Fourier terms upon restart, thus allowing continuation of an analysis. Abaqus/Standard provides detailed output of the maximum residual at each time point, the maximum residual coefficient, the maximum displacement coefficient, the maximum correction to displacement coefficients, and the number of Fourier terms at the end of each iteration in the message (.msg) file. This output is described in more detail below. Input File Usage: *DIRECT CYCLIC , , , , initial number of terms, max number of terms, increment in number of terms Abaqus/CAE Usage: Step module: Create Step: General: Direct cyclic; Incrementation: Number of Fourier terms: Initial: initial number of terms, Maximum: max number of terms, Increment: increment in number of terms Controlling the incrementation during the cyclic time period To ensure an accurate solution, the material history as well as the residual vector must be evaluated at a sufficient number of time points during the cycle. The number of time points, , at which the response is computed must be larger than the number of Fourier coefficients; i.e., . Abaqus/Standard will automatically adjust the number of Fourier coefficients if such a condition is not satisfied. You can specify the time incrementation over the cycle directly, or it can be determined automatically by Abaqus/Standard. You should specify the maximum number of increments allowed in the time period as part of the step definition. The default is 100. Automatic incrementation There are several ways to choose the automatic incrementation scheme. If you specify only the maximum allowable nodal temperature change in an increment, the time increments are selected automatically based on this value. Abaqus/Standard will restrict the time increments to ensure that the maximum temperature change is not exceeded at any node during any increment of the analysis. For rate-dependent constitutive equations you can limit the size of the time increment by the accuracy of the integration. The user-specified accuracy tolerance parameter limits the maximum inelastic strain rate change allowed over an increment: where t is the time at the beginning of the increment, at the end of the increment), and value chosen for the accuracy tolerance parameter should be on the order of where of the elastic strains for viscoelasticity problems. is the time is the equivalent creep strain rate. To achieve sufficient accuracy, the for creep problems, is an acceptable level of error in the stress and E is a typical elastic modulus, or on the order is the time increment (so that If rate-dependent constitutive equations are used in combination with a varying temperature, both controls can be used simultaneously. Abaqus/Standard will then choose the increments that satisfy both criteria. If the time integration accuracy measure specified by either or both of the above controls is satisfied consecutive increments without cutbacks, the next time increment will be increased by a factor are user-defined parameters . The defaults are = 3 and = 1.5. . Both and Input File Usage: Abaqus/CAE Usage: Use the following option to specify the maximum allowable nodal temperature change: *DIRECT CYCLIC, DELTMX= Use the following option to specify the accuracy tolerance parameter: *DIRECT CYCLIC, CETOL=tolerance Use the following option to specify the maximum allowable nodal temperature change: Step module: Create Step: General: Direct cyclic; Incrementation: Max. allowable temperature change per increment: Use the following option to specify the accuracy tolerance parameter: Step module: Create Step: General: Direct cyclic; Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance Fixed time incrementation If neither the accuracy tolerance parameter nor the maximum allowable nodal temperature change is specified, the size of the time increment is fixed. You must specify the time increment and the time period T. Input File Usage: *DIRECT CYCLIC , T Abaqus/CAE Usage: Step module: Create Step: General: Direct cyclic; Basic: Cycle time period: T; Incrementation: Type: Fixed, Increment size: Defining the time points at which the response must be evaluated The user-defined time incrementation for a direct cyclic step can be augmented or superseded by specifying particular time points in the loading history at which the response of the structure should be evaluated. This feature is particularly useful if you know prior to the analysis at which time points in the analysis the load reaches a maximum and/or minimum value or when the response will change rapidly. An example is the analysis of the heating/cooling thermal cycle of an engine component where you typically know when the temperature reaches a maximum value. When time points are used with fixed time incrementation, the time incrementation specified for the direct cyclic step is ignored and instead the time incrementation precisely follows the specified time points. If time points are used with automatic incrementation, the time incrementation is variable; but the response of the structure will be evaluated at the specified time points. The time points can be listed individually, or they can be generated automatically by specifying the starting time point, ending time point, and increment in time between the two specified time points. Input File Usage: Abaqus/CAE Usage: Use the following options to list time points individually: *TIME POINTS, NAME=time points name *DIRECT CYCLIC, TIME POINTS=time points name Use the following options to generate time points automatically: *TIME POINTS, NAME=time points name, GENERATE *DIRECT CYCLIC, TIME POINTS=time points name Use the following options to list time points individually: Step module: Create Step: General: Direct cyclic; Incrementation: Evaluate structure response at time points: time points name Use the following options to generate time points automatically: Step module: Create Step: General: Direct cyclic; Incrementation: Evaluate structure response at time points: Create; Edit Time Points: Specify using delimiters: Start, End, Increment Controlling the application of periodicity conditions By default, Abaqus/Standard imposes periodic conditions during the iterative solution process by using the state obtained at the end of the previous iteration as the starting state for the current iteration; i.e., , where s is a solution variable such as plastic strain. In cases where the periodic solution is not easily found (for example, when the loading is close to causing ratchetting), the state around which the periodic solution is obtained may show considerably more “drift” than would be obtained in a transient analysis. In such cases you may wish to delay the application of periodic conditions as an artificial method to reduce this drift. Figure 6.2.6–3 compares the response of two identical structures subjected to the same set of cyclic loads and boundary conditions, where each structure experienced a different loading history prior to the application of the cyclic loads. Figure 6.2.6–3 shows that the prior loading history only affects the mean value of stress and strain; it does not affect the shape of the stress-strain curves or the amount of energy dissipated during the cycle. periodicity condition imposed from iteration 5 periodicity condition imposed from iteration 1 Figure 6.2.6–3 Influence of periodicity condition on mean value of the strains over a stabilized cycle. By delaying the application of periodicity conditions, you can influence the mean stress and strain level. However, this is rarely necessary since the average stress and strain levels are usually not needed for low-cycle fatigue life predictions. You can control when the periodicity conditions are applied by defining direct cyclic controls to . This variable defines from which iteration onward the application of periodic means that the periodicity conditions are specify the variable conditions will be activated. For example, setting applied from iteration 6 onwards. The default is , which is appropriate for most analyses. Input File Usage: *CONTROLS, TYPE=DIRECT CYCLIC Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit; Direct Cyclic: Initial conditions Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified . Boundary conditions Boundary conditions can be applied to any of the displacement or rotation degrees of freedom. During the analysis, prescribed boundary conditions must have an amplitude definition that is cyclic over the step: the start value must be equal to the end value . If the analysis consists of several steps, the usual rules apply . At each new step the boundary condition can either be modified or completely defined. All boundary conditions defined in previous steps remain unchanged unless they are redefined. Loads The following loads can be prescribed in a direct cyclic analysis: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” During the analysis each load must have an amplitude definition that is cyclic over the step where the start value must be equal to the end value . If the analysis consists of several steps, the usual rules apply . At each new step the loading can either be modified or completely defined. All loads defined in previous steps remain unchanged unless they are redefined. Predefined fields The following predefined fields can be specified in a direct cyclic analysis, as described in “Predefined fields,” Section 33.6.1: • Temperature is not a degree of freedom in a direct cyclic analysis, but nodal temperatures can be specified as a predefined field. The temperature values specified must be cyclic over the step: the start value must be equal to the end value . If the temperatures are read from the results file, you should specify initial temperature conditions equal to the temperature values at the end of the step . Alternatively, you can ramp the temperatures back to their initial condition values, as described in “Predefined fields,” Section 33.6.1. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any. • The values of user-defined field variables can be specified. These values affect only field-variable- dependent material properties, if any. The field variable values specified must be cyclic over the step. Material options Most material models, including user-defined materials (defined using user subroutine UMAT), that describe mechanical behavior are available for use in a direct cyclic analysis. The following material properties are not active during a direct cyclic analysis: acoustic properties, thermal properties (except for thermal expansion), mass diffusion properties, electrical conductivity properties, piezoelectric properties, and pore fluid flow properties. yield,” Section yield (“Rate-dependent plasticity: (“Two-layer viscoplasticity,” Section 23.2.11) can also be used during a direct cyclic analysis. (“Rate-dependent creep creep and swelling,” Section 23.2.4), and two-layer viscoplasticity Rate-dependent rate-dependent 23.2.3), Elements Any of the stress/displacement elements in Abaqus/Standard can be used in a direct cyclic analysis . Output Different types of output are available for postprocessing and for monitoring a direct cyclic analysis. Message file information Abaqus/Standard prints the residual force, time average force, and a flag to indicate if equilibrium was satisfied in the message (.msg) file at different time increments for each iteration. You can control the frequency in increments at which information is printed to the message file, and you can suppress the output; the default is to print output every 10 increments . Abaqus/Standard also prints the number of Fourier terms used, the maximum residual coefficient, the maximum correction to displacement coefficients, and the maximum displacement coefficient in the Fourier series in the message file at the end of each iteration. An example of the output is shown below: INC 10 TIME INC 0.250 ITERATION STEP TIME 2.50 26 STARTS LARG. RESI. FORCE 1.008E+01 TIME AVG. FORCE 50.9 FORCE EQUV. 20 30 0.250 0.250 5.00 7.50 1.622E+01 4.622E-02 76.8 99.8 ITERATION 26 SUMMARY NUMBER OF FOURIER TERMS USED 40, TOTAL NUMBER OF INCREMENTS CYCLE/STEP TIME AVERAGE FORCE TOTAL TIME COMPLETED TIME AVG. FORCE 30.0, 21.2 31.0 25.7 120 AT NODE 24 DOF 2 MAX. COEFFICIENT OF DISP. AT NODE 44 DOF 1 MAX. COEFF. OF RESI. FORCE ON CONST. TERM MAX. COEFF. OF RESI. FORCE ON PERI. TERMS 6 DOF 3 AT NODE MAX. CORR. TO COEFF. OF DISP. ON CONST. TERM 0.002 AT NODE 50 DOF 3 MAX. CORR. TO COEFF. OF DISP. ON PERI. TERMS 0.015 AT NODE 50 DOF 3 0.142 31.7 0.82 Results output Element and nodal output are written only when the stabilized cycle is reached. If a stabilized cycle has not been reached at the end of an analysis, output is written for the last iteration of the step. The element output available for a direct cyclic analysis includes stress; strain; energies; and the values of state, field, and user-defined variables. All the energies are set equal to zero at the beginning of each iteration since energies dissipated over an entire stabilized cycle are of interest in making fatigue life predictions in direct cyclic analysis. The nodal output available includes displacements, reaction forces, and coordinates. All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Recovering additional results for an iteration You may want to recover additional results for an iteration rather than for the stabilized cycle. You can extract these results from the restart data . This feature is particularly useful if you want to evaluate the shift of the strain from one iteration to another iteration when plastic ratchetting occurs. Input File Usage: Abaqus/CAE Usage: *POST OUTPUT, ITERATION=n Recovering additional results for an iteration is not supported in Abaqus/CAE. Specifying output at exact times Output at exact times is not supported for direct cyclic analysis. If output at exact times is requested, Abaqus will issue a warning message and change the output to an output at approximate times. Limitations A direct cyclic analysis is subject to the following limitations: • Contact conditions cannot change during a direct cyclic analysis; they remain as they were defined at the beginning of the analysis or at the end of any general step prior to the direct cyclic step. Frictional slipping is not allowed during direct cyclic analyses; all points in contact are assumed to be sticking if friction is present. • Geometric nonlinearity can be included only in any general step prior to a direct cyclic step; however, only small displacements and strains will be considered during the cyclic step. Input file template *HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS Data lines to specify initial conditions *AMPLITUDE Data lines to define amplitude variations ** *STEP (,INC=) Set INC equal to the maximum number of increments in a single loading cycle *DIRECT CYCLIC Data line to define time increment, cycle time, initial number of Fourier terms, maximum number of Fourier terms, increment in number of Fourier terms, and maximum number of iterations *TIME POINTS Data lines to list time points *BOUNDARY, AMPLITUDE= Data lines to prescribe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD, AMPLITUDE= Data lines to specify loads *TEMPERATURE and/or *FIELD, AMPLITUDE= Data lines to specify values of predefined fields *END STEP ** *STEP(,INC=) *DIRECT CYCLIC, DELTMX Data line to control automatic time incrementation and Fourier representations *BOUNDARY, OP=MOD,AMPLITUDE= Data lines to modify or add zero-valued or nonzero boundary conditions *CLOAD, OP=NEW, AMPLITUDE= Data lines to specify new concentrated loads; all previous concentrated loads will be removed *DLOAD, OP=MOD, AMPLITUDE= Data lines to specify additional or modified distributed loads *TEMPERATURE and/or *FIELD, AMPLITUDE= Data lines to specify additional or modified values of predefined fields *END STEP LOW-CYCLE FATIGUE ANALYSIS USING THE DIRECT CYCLIC APPROACH LOW-CYCLE FATIGUE ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Static stress analysis procedures: overview,” Section 6.2.1 • “Direct cyclic analysis,” Section 6.2.6 • “Crack propagation analysis,” Section 11.4.3 • “Damage and failure for ductile materials in low-cycle fatigue analysis,” Section 24.4 • “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1 • *DAMAGE EVOLUTION • *DAMAGE INITIATION • *DEBOND • *DIRECT CYCLIC • *FRACTURE CRITERION • *CONTROLS • “Configuring a direct cyclic procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A low-cycle fatigue analysis: • is characterized by states of stress high enough for inelastic deformation to occur in most cases; • is a quasi-static analysis on a structure subjected to sub-critical cyclic loading; • can be associated with thermal as well as mechanical loading; • uses the direct cyclic approach to obtain the stabilized cyclic response of the structure directly; • models progressive damage and failure in bulk ductile material based on a continuum damage mechanics approach, in which case damage initiation and evolution are characterized by the accumulated inelastic hysteresis strain energy per stabilized cycle; • models propagation of a discrete crack along an arbitrary, solution-dependent path without remeshing in the bulk material based on the principles of linear elastic fracture mechanics (LEFM) with the extended finite element method, in which case the onset and growth of fatigue crack are characterized by the relative fracture energy release rate; • models progressive delamination growth along a predefined path at the interfaces in laminated composites, in which case the onset and growth of fatigue delamination at the interfaces are characterized by the relative fracture energy release rate; • uses the damage extrapolation technique to accelerate the low-cycle fatigue analysis; and • assumes geometrically linear behavior and fixed contact conditions within each loading cycle. Approaches to low-cycle fatigue analysis The traditional approach for determining the fatigue limit for a structure is to establish the curves (load versus number of cycles to failure) for the materials in the structure. Such an approach is still used as a design tool in many cases to predict fatigue resistance of engineering structures. However, this technique is generally conservative, and it does not define a relationship between the cycle number and the degree of damage or crack length. One alternative approach is to predict the fatigue life by using a crack/damage evolution law based on the inelastic strain/energy when the structure’s response is stabilized after many cycles. Because the computational cost to simulate the slow progressive damage in a material over many load cycles is prohibitively expensive for all but the simplest models, numerical fatigue life studies usually involve modeling the response of the structure subjected to a small fraction of the actual loading history. This response is then extrapolated over many load cycles using empirical formulae such as the Coffin-Manson relationship to predict the likelihood of crack initiation and propagation. Since this approach is based on a constant crack/damage growth rate, it may not realistically predict the evolution of the crack or damage. Low-cycle fatigue analysis in Abaqus/Standard The direct cyclic analysis capability in Abaqus/Standard provides a computationally effective modeling technique to obtain the stabilized response of a structure subjected to periodic loading and is ideally suited to perform low-cycle fatigue calculations on a large structure. The capability uses a combination of Fourier series and time integration of the nonlinear material behavior to obtain the stabilized response of the structure directly. The theory and algorithm to obtain a stabilized response using the direct cyclic approach are described in detail in “Direct cyclic algorithm,” Section 2.2.3 of the Abaqus Theory Manual. The direct cyclic low-cycle fatigue procedure models the progressive damage and failure both in bulk materials (such as in solder joints in an electronic chip packaging or intra-laminar crack growth in laminated composites) and at material interfaces (such as delamination in laminated composites). The former can be based on either a continuum damage mechanics approach or the principles of linear elastic fracture mechanics with the extended finite element method. The response is obtained by evaluating the behavior of the structure at discrete points along the loading history . The solution at each of these points is used to predict the degradation and evolution of material properties that will take place during the next increment, which spans a number of load cycles, . The degraded material properties are then used to compute the solution at the next increment in the load history. Therefore, the crack/damage growth rate is updated continually throughout the analysis. The elastic material stiffness at a material point remains constant and contact conditions remain unchanged when the stabilized solution is computed at a given point in the loading history. Each of the Figure 6.2.7–1 Elastic stiffness degradation as a function of the cycle number. solutions along the loading history represents the stabilized response of the structure subjected to the applied period loads, with a level of material damage at each point in the structure computed from the previous solution. This process is repeated up to a point in the loading history at which a fatigue life assessment can be made. In bulk material, there are two approaches to modeling the progressive damage and failure. One approach is based on continuum damage mechanics. This approach is more appropriate for ductile material, in which the cyclic loading leads to stress reversals and the accumulation of plastic strains, which in turn cause the initiation and propagation of cracks. The damage initiation and evolution are characterized by the stabilized accumulated inelastic hysteresis strain energy per cycle as illustrated in Figure 6.2.7–2. The other approach is based on the principles of linear elastic fracture mechanics with the extended finite element method. This approach is more appropriate for brittle material or material with small scale yielding, in which the cyclic loading leads to material strength degradation causing fatigue crack growth along an arbitrary path. The onset and growth of the crack are characterized by the relative fracture energy release rate at the crack tip based on the Paris law (Paris, 1961). At interfaces of laminated composites the cyclic loading leads to interface strength degradation causing fatigue delamination growth. The onset and growth of delamination are also characterized by the relative fracture energy release rate at the crack tip based on the Paris law (Paris, 1961). Both the progressive damage mechanism in the bulk material and the progressive delamination growth mechanism at interfaces can be considered simultaneously, with the failure occurring first at the weakest link in a model. Defining a low-cycle fatigue analysis using the direct cyclic approach is similar to defining a direct cyclic analysis. See “Direct cyclic analysis,” Section 6.2.6, for details on how to specify the number of Fourier terms, number of iterations, and the increment sizes. You specify the maximum numbers of cycles, , when you define the low-cycle fatigue analysis step. *DIRECT CYCLIC, FATIGUE first data line , , Step module: Create Step: General: Direct cyclic; Fatigue: Include low-cycle fatigue analysis, Maximum number of cycles: Value: Abaqus/CAE Usage: Input File Usage: time stabilized plastic shakedown Figure 6.2.7–2 Plastic shakedown in a direct cyclic analysis. Determining whether to use the Fourier coefficients from the previous step A low-cycle fatigue step using the direct cyclic approach can be the only step in an analysis, can follow a general or linear perturbation step, or can be followed by a general or linear perturbation step. Multiple low-cycle fatigue analysis steps can be included in a single analysis. In such a case the Fourier series coefficients obtained in the previous step can be used as starting values in the current step. By default, the Fourier coefficients are reset to zero, thus allowing application of cyclic loading conditions that are very different from those defined in the previous low-cycle fatigue step. As in a direct cyclic analysis, you can specify that a low-cycle fatigue step in a restart analysis should use the Fourier coefficients from the previous step, thus allowing continuation of an analysis to simulate more loading cycles. In a low-cycle fatigue analysis a restart file is written at the end of the stabilized cycle. Consequently, a restart analysis that is a continuation of a previous low-cycle fatigue analysis will start with a new loading cycle at . Input File Usage: Use the following option to specify that the current step is a continuation of the previous low-cycle fatigue step using the direct cyclic approach: *DIRECT CYCLIC, FATIGUE, CONTINUE=YES Use the following option to reset the Fourier series coefficients to zero: *DIRECT CYCLIC, FATIGUE, CONTINUE=NO (default) Use the following option to specify that the current step is a continuation of the previous low-cycle fatigue step using the direct cyclic approach: Abaqus/CAE Usage: Step module: Create Step: General: Direct cyclic; Basic: Use displacement Fourier coefficients from previous direct cyclic step; Fatigue: Include low-cycle fatigue analysis Use the following option to reset the Fourier series coefficients to zero: Step module: Create Step: General: Direct cyclic; Fatigue: Include low-cycle fatigue analysis Progressive damage and damage extrapolation in bulk ductile material based on continuum damage mechanics approach Low-cycle fatigue analysis in Abaqus/Standard allows modeling of progressive damage and failure for ductile materials in any elements whose response is defined in terms of a continuum-based constitutive model (“Material library: overview,” Section 21.1.1). This includes cohesive elements modeled using a continuum approach (“Modeling of an adhesive layer of finite thickness” in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5). The inelastic definition in a material point must be used in conjunction with the linear elastic material model (“Linear elastic behavior,” Section 22.2.1), the porous elastic material model (“Elastic behavior of porous materials,” Section 22.3.1), or the hypoelastic material model (“Hypoelastic behavior,” Section 22.4.1). After damage initiation the elastic material stiffness is degraded progressively in each cycle (as shown in Figure 6.2.7–1) based on the accumulated stabilized inelastic hysteresis energy. It is impractical and computationally expensive to perform a cycle-by-cycle simulation for a low-cycle fatigue analysis; Instead, to accelerate the low-cycle fatigue analysis, each increment extrapolates the current damaged state in the bulk material forward over many cycles to a new damaged state after the current loading cycle is stabilized. Damage initiation and evolution Damage initiation refers to the beginning of degradation of the response of a material point. In a low-cycle fatigue analysis the damage initiation criterion is characterized by the accumulated inelastic hysteresis energy per cycle, and material constants are used to determine the number of the cycle in which damage is initiated, , Abaqus/Standard . At the end of a stabilized loading cycle, checks to see if the damage initiation criterion is satisfied in any material point; material stiffness at a material point will not be degraded unless this criterion is satisfied. The calculations and output associated with damage initiation are discussed in detail in “Damage initiation for ductile materials in low-cycle fatigue,” Section 24.4.2. . Once the damage initiation criterion is satisfied at a material point, the damage state is calculated and updated based on the inelastic hysteresis energy for the stabilized cycle. Abaqus/Standard assumes that the degradation of the elastic stiffness can be modeled using the scalar damage variable, . The rate of the damage in a material point per cycle, , is calculated based on the accumulated inelastic hysteresis energy, the characteristic length associated with an integration point, and material constants. For details, see “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3. Typically, a material has completely lost its load carrying capacity when . You can remove an element from the mesh if all of the section points at all integration locations of the element have lost their load carrying capability. Damage extrapolation technique in the bulk material If the damage initiation criterion is satisfied in any material point at the end of a stabilized cycle, Abaqus/Standard extrapolates the damage variable increment over a number of cycles, , from the current cycle forward to the next , is given by . The new damage state, is the characteristic length associated with an integration point, and are material where constants . and You specify the minimum ( ) number of cycles over which ) and maximum ( the damage is extrapolated forward in any given increment. The default values are 100 and 1000, respectively. Input File Usage: *DIRECT CYCLIC, FATIGUE first data line , Abaqus/CAE Usage: Step module: Create Step: General: Direct cyclic; Fatigue: Include low-cycle fatigue analysis, Cycle increment size: Minimum: , Maximum: Discrete crack propagation along an arbitrary path based on the principles of linear elastic fracture mechanics with the extended finite element method Low-cycle fatigue analysis in Abaqus/Standard allows the modeling of discrete crack growth along an arbitrary path based on the principles of linear elastic fracture mechanics with the extended finite element method. You complete the definition of the crack propagation capability by defining a fracture-based surface behavior and specifying the fracture criterion in enriched elements. The fracture energy release rates at the crack tips in enriched elements are calculated based on the modified virtual crack closure technique (VCCT). VCCT uses the principles of linear elastic fracture mechanics. Therefore, VCCT is appropriate for problems in which brittle fatigue crack growth occurs, although nonlinear material deformations can occur somewhere else in the bulk materials. For more information about defining fracture criteria and VCCT in enriched elements, see “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1. To accelerate the low-cycle fatigue analysis, the damage extrapolation technique is used, which advances the crack by at least one element length after each stabilized cycle. LOW-CYCLE FATIGUE ANALYSIS ; the other criterion is based on the maximum fracture energy release rate, The onset and growth of fatigue crack at an enriched element are characterized by using the Paris law, which relates the relative fracture energy release rate, , to crack growth rates. Two criteria must be met to initiate fatigue crack growth: one criterion is based on material constants, , and the current cycle number, , which corresponds to the cyclic energy release rate when the structure is loaded up to its maximum value. Once the onset of fatigue crack growth criterion is satisfied at the enriched elements, the crack growth rate, (the Paris law). The criteria for fatigue crack onset and growth are discussed in detail in “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1. , is a piecewise function based on material constants and Damage extrapolation technique and , Abaqus/Standard extends the crack length, If the onset of crack growth criterion is satisfied at any crack tip in the enriched element at the end of a stabilized cycle, , from the current cycle forward over a number of cycles, by fracturing at least one enriched element ahead of the crack tips. , to Given the material constants (as defined in “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1), combined with the known element length and likely propagation direction at the enriched elements ahead of the crack tips, the number of cycles necessary to fail each enriched element ahead of the crack tip can be calculated as , where represents the enriched element ahead of the th crack tip. The analysis is set up to advance the crack by at least one enriched element per increment after the loading cycle is stabilized. The element with the fewest cycles is identified to be fractured, and its is represented as the number of cycles to grow the crack equal to its element length, . The most critical element is completely fractured with a zero constraint and a zero stiffness at the cracked surfaces at the end of the stabilized cycle. As the enriched element is fractured, the load is redistributed, and a new relative fracture energy release rate must be calculated for the enriched elements ahead of the crack tips for the next cycle. This capability allows at least one enriched element ahead of the crack tips to be fractured after each stabilized cycle and precisely accounts for the number of cycles needed to cause fatigue crack growth over that length. Progressive delamination growth along a pre-defined path at interfaces Low-cycle fatigue analysis in Abaqus/Standard also allows the modeling of progressive delamination growth at the interfaces in laminated composites. The interface along which the delamination (or crack) propagates must be indicated in the model using a fracture criterion definition. The fracture energy release rates at the crack tips in the interface elements are calculated based on the virtual crack closure technique (VCCT). VCCT uses the principles of linear elastic fracture mechanics. Therefore, VCCT is appropriate for problems in which brittle fatigue delamination growth occurs along predefined surfaces, although nonlinear material deformations can occur in the bulk materials. For more information about defining fracture criteria and VCCT, see “Crack propagation analysis,” Section 11.4.3. To accelerate the low-cycle fatigue analysis, the damage extrapolation technique is used, which releases at least one element length at the crack tip along the interface after each stabilized cycle. When both brittle fatigue delamination at interfaces and ductile damage or discrete crack growth in bulk materials are considered in an analysis, failure occurs first at the weakest link. Onset and growth of fatigue delamination , and the current cycle number, The onset and growth of fatigue delamination at a defined crack interface are characterized by using the Paris law, which relates the relative fracture energy release rate, , to crack growth rates. Two criteria must be met to initiate fatigue delamination growth: one criterion is based on material constants, ; the other criterion is based on the maximum fracture energy release rate, , which corresponds to the cyclic energy release rate when the structure is loaded up to its maximum value. Once the onset of delamination growth criterion is satisfied at the interface, the delamination growth rate, (the Paris law). The criteria for fatigue delamination onset and growth are discussed in detail in “Low-cycle fatigue criterion” in “Crack propagation analysis,” Section 11.4.3. , is a piecewise function based on material constants and Damage extrapolation technique at the interface elements , to , Abaqus/Standard extends the crack length, If the onset of delamination growth criterion is satisfied at any crack tip in the interface at the end of a stabilized cycle, , from the current cycle forward over a number of cycles, by releasing at least one element at the interface. Given the material constants (as defined in “Low-cycle fatigue criterion” in “Crack propagation analysis,” and Section 11.4.3), combined with the known node spacing at the interface elements at the crack tips, the number of cycles necessary to fail each interface element at the crack tip can be calculated as , where j represents the node at the jth crack tip. The analysis is set up to release at least one interface element per increment after the loading cycle is stabilized. The element with the fewest cycles is identified to be released, and its is represented as the number of cycles to grow the crack equal to its element length, . The most critical element is completely released with a zero constraint and a zero stiffness at the end of the stabilized cycle. As the interface element is released, the load is redistributed, and a new relative fracture energy release rate must be calculated for the interface elements at the crack tips for the next cycle. This capability allows at least one interface element at the crack tips to be released after each stabilized cycle and precisely accounts for the number of cycles needed to cause fatigue crack growth over that length. Controlling the solution accuracy Low-cycle fatigue analysis utilizes the direct cyclic approach to obtain the stabilized cyclic solution iteratively by combining a Fourier series approximation with time integration of the nonlinear material behavior using a modified Newton method. The accuracy of the algorithm depends on the number of Fourier terms used, the number of iterations taken to obtain the stabilized solution, and the number of time points within the load period at which the material response and residual vector are evaluated. Some methods for controlling the solution accuracy in a direct cyclic analysis are described in detail in “Direct cyclic analysis,” Section 6.2.6. They all remain valid in a low-cycle fatigue analysis using the direct cyclic approach. In addition, the accuracy of a low-cycle fatigue analysis depends on the number of cycles over which the damage is extrapolated forward, as described below. Controlling the accuracy of damage extrapolation in the bulk material when using continuum damage mechanics approach To accelerate the low-cycle fatigue analysis, the damage extrapolation technique is used at the end of a stabilized cycle. In addition to specifying the minimum and maximum number of cycles over which the damage is extrapolated , you can specify the damage extrapolation tolerance, , to control the accuracy of damage extrapolation in the bulk material. The default is . Input File Usage: Use the following option to specify the damage extrapolation tolerance: *DIRECT CYCLIC, FATIGUE first data line , , , Abaqus/CAE Usage: Step module: Create Step: General: Direct cyclic; Fatigue: Include low-cycle fatigue analysis, Damage extrapolation tolerance: Determining the increment over which damage is extrapolated forward Abaqus/Standard uses an adaptive algorithm to determine the number of cycles over which the damage is extrapolated forward in each increment. By default, Abaqus/Standard starts with 500 cycles (half of the default value of maximum increment in number of cycles) and determines the maximum damage increment at any material points based on If the maximum damage increment, , is greater than the damage extrapolation tolerance that you specify, the number of cycles over which the damage is extrapolated forward is reduced accordingly to ensure the maximum damage increment is less than the damage extrapolation tolerance. On the other hand, if the maximum damage increment at all material points is less than half of the damage extrapolation tolerance that you specify, the number of cycles is increased accordingly to ensure the maximum damage increment is equal to the damage extrapolation tolerance. Initial conditions Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified . Boundary conditions Boundary conditions can be applied to any of the displacement or rotation degrees of freedom. During the analysis, prescribed boundary conditions must have an amplitude definition that is cyclic over the step: the start value must be equal to the end value . If the analysis consists of several steps, the usual rules apply . At each new step the boundary condition can either be modified or completely defined. All boundary conditions defined in previous steps remain unchanged unless they are redefined. Loads The following loads can be prescribed in a low-cycle fatigue analysis using the direct cyclic approach: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” During the analysis each load must have an amplitude definition that is cyclic over the step where the start value must be equal to the end value . If the analysis consists of several steps, the usual rules apply . At each new step the loading can either be modified or completely defined. All loads defined in previous steps remain unchanged unless they are redefined. Predefined fields The following predefined fields can be specified in a low-cycle fatigue analysis using the direct cyclic approach, as described in “Predefined fields,” Section 33.6.1: • Temperature is not a degree of freedom in a low-cycle fatigue analysis using the direct cyclic approach, but nodal temperatures can be specified as a predefined field. The temperature values specified must be cyclic over the step: the start value must be equal to the end value . If the temperatures are read from the results file, you should specify initial temperature conditions equal to the temperature values at the end of the step . Alternatively, you can ramp the temperatures back to their initial condition values, as described in “Predefined fields,” Section 33.6.1. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any. • The values of user-defined field variables can be specified. These values affect only field-variable- dependent material properties, if any. The field variable values specified must be cyclic over the step. Material options Most ductile material models that describe mechanical behavior are available for use in a low-cycle fatigue analysis. The inelastic definition in a material point must be used in conjunction with the linear elastic material model (“Linear elastic behavior,” Section 22.2.1), the porous elastic material model (“Elastic behavior of porous materials,” Section 22.3.1), or the hypoelastic material model (“Hypoelastic behavior,” Section 22.4.1). The following material properties are not active during a low-cycle fatigue analysis: acoustic properties, thermal properties (except for thermal expansion), mass diffusion properties, electrical conductivity properties, piezoeletric properties, and pore fluid flow properties. (“Rate-dependent creep 23.2.3), creep and swelling,” Section 23.2.4), and two-layer viscoplasticity yield (“Rate-dependent plasticity: (“Two-layer viscoplasticity,” Section 23.2.11) can also be used during a low-cycle fatigue analysis. yield,” Section Rate-dependent rate-dependent Elements Any of the stress/displacement elements in Abaqus/Standard can be used in a low-cycle fatigue analysis . This includes cohesive elements with finite thickness (“Modeling of an adhesive layer of finite thickness” in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5). However, when modeling fatigue crack growth based on the principles of linear elastic fracture mechanics with the extended finite element method, only first-order continuum stress/displacement elements and second- order stress/displacement tetrahedron elements can be associated with an enriched feature . Output Different types of output are available for postprocessing and for monitoring a low-cycle fatigue analysis using the direct cyclic approach. Message file information As in a direct cyclic analysis, low-cycle fatigue analysis using the direct cyclic approach in Abaqus/Standard prints the residual force, time average force, and a flag to indicate if equilibrium was satisfied in the message (.msg) file at different time increments for each iteration in each loading cycle. You can control the frequency in increments at which information is printed to the message file, and you can suppress the output; the default is to print output every 10 increments . Abaqus/Standard also prints the number of Fourier terms used, the maximum residual coefficient, the maximum correction to displacement coefficients, and the maximum displacement coefficient in the Fourier series in the message file at the end of each iteration in each cycle. An example of the output is shown below: INC 10 20 30 TIME INC 0.250 0.250 0.250 CYCLE 5 STARTS ITERATION STEP TIME 2.50 5.00 7.50 26 STARTS LARG. RESI. FORCE 1.008E+01 1.622E+01 4.622E-02 6.2.7–11 TIME AVG. FORCE 50.9 76.8 99.8 FORCE EQUV. ITERATION 26 SUMMARY NUMBER OF FOURIER TERMS USED 40, TOTAL NUMBER OF INCREMENTS CYCLE/STEP TIME AVERAGE FORCE TOTAL TIME COMPLETED TIME AVG. FORCE 30.0, 21.2 31.0 25.7 120 AT NODE 24 DOF 2 MAX. COEFFICIENT OF DISP. AT NODE 44 DOF 1 MAX. COEFF. OF RESI. FORCE ON CONST. TERM 6 DOF 3 AT NODE MAX. COEFF. OF RESI. FORCE ON PERI. TERMS MAX. CORR. TO COEFF. OF DISP. ON CONST. TERM 0.002 AT NODE 50 DOF 3 MAX. CORR. TO COEFF. OF DISP. ON PERI. TERMS 0.015 AT NODE 50 DOF 3 0.142 31.7 0.82 Results output Element and nodal output are written only when the stabilized cycle is reached. If a stabilized cycle has not been reached at the end of a cycle, output is written for the last iteration of the cycle. All standard output variables in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1) are In addition, the following variables are available for progressive damage in bulk ductile available. material based on the continuum damage mechanics approach: STATUS SDEG CYCLEINI Status of element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). Scalar stiffness degradation, D. Number of cycles to initialize the damage at the material point. The following variables are available for discrete crack propagation along an arbitrary path based on the principles of linear elastic fracture mechanics with the extended finite element method: STATUSXFEM Status of the enriched element. (The status of an enriched element is 1.0 if the element is completely cracked, 0.0 if the element is not. If the element is partially cracked, the value lies between 1.0 and 0.0.) CYCLEINIXFEM Number of cycles to initialize the crack at the enriched element. ENRRTXFEM All components of strain energy release rate range; i.e., the difference between the energy release rate at the maximum loading and at the minimum loading. Recovering additional results for a stabilized cycle You may want to recover additional results for a stabilized cycle. You can extract these results from the restart data . Input File Usage: Abaqus/CAE Usage: *POST OUTPUT, CYCLE=n Recovering additional results for a stabilized cycle is not supported in Abaqus/CAE. Specifying output at exact times Output at exact times is not supported for low-cycle fatigue analysis. If output at exact times is requested, Abaqus will issue a warning message and change the output to an output at approximate times. Limitations A low-cycle fatigue analysis using the direct cyclic approach is subject to the following limitations: • Contact conditions cannot change during a given cycle when direct cyclic analysis is used iteratively to obtain a stabilized solution. • Geometric nonlinearity can be included only in any general step prior to a direct cyclic step; however, only small displacements and strains will be considered during the cyclic step. Input file template The following is an example of modeling progressive damage and failure in the bulk material based on the continuum damage mechanics approach and progressive delamination growth at the interface: *HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS Data lines to specify initial conditions *AMPLITUDE Data lines to define amplitude variations ** *MATERIAL Options to define material properties *DAMAGE INITIATION, CRITERION=HYSTERESIS ENERGY Data lines to define material constants for bulk ductile material damage initiation *DAMAGE EVOLUTION, TYPE=HYSTERESIS ENERGY Data lines to define material constants for bulk ductile material damage evolution ** *SURFACE, NAME=slave Data lines to define slave surface at delamination interface *SURFACE, NAME=master Data lines to define master surface at delamination interface *CONTACT PAIR slave, master ** *STEP (,INC=) Set INC equal to the maximum number of increments in a single loading cycle *DIRECT CYCLIC, FATIGUE Data line to define time increment, cycle time, initial number of Fourier terms, maximum number of Fourier terms, increment in number of Fourier terms, and maximum number of iterations Data line to define minimum increment in number of cycles, maximum increment in number of cycles, total number of cycles, and damage extrapolation tolerance *DEBOND, SLAVE=slave, MASTER=master *FRACTURE CRITERION, TYPE=FATIGUE Data lines to define material constants used in Paris law and fracture criterion ** *BOUNDARY, AMPLITUDE= Data lines to prescribe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD, AMPLITUDE= Data lines to specify loads *TEMPERATURE and/or *FIELD, AMPLITUDE= Data lines to specify values of predefined fields ** *END STEP The following is an example of modeling discrete crack growth in the bulk material based on the principles of linear elastic fracture mechanics with the extended finite element method and progressive delamination growth at the interface: *HEADING … *ENRICHMENT, TYPE=PROPAGATION CRACK, INTERACTION=INTERACTION, ELSET=ENRICHED *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS Data lines to specify initial conditions *AMPLITUDE Data lines to define amplitude variations ** *MATERIAL Options to define material properties *SURFACE, INTERACTION=INTERACTION *SURFACE BEHAVIOR *FRACTURE CRITERION, TYPE=FATIGUE Data lines to define material constants used in the Paris law and fracture criterion in the bulk material for enriched elements ** *SURFACE, NAME=slave Data lines to define slave surface at delamination interface *SURFACE, NAME=master Data lines to define master surface at delamination interface *CONTACT PAIR slave, master ** *STEP (,INC=) Set INC equal to the maximum number of increments in a single loading cycle *DIRECT CYCLIC, FATIGUE Data line to define time increment, cycle time, initial number of Fourier terms, maximum number of Fourier terms, increment in number of Fourier terms, and maximum number of iterations Data line to define minimum increment in number of cycles, maximum increment in number of cycles, total number of cycles, and damage extrapolation tolerance *DEBOND, SLAVE=slave, MASTER=master *FRACTURE CRITERION, TYPE=FATIGUE Data lines to define material constants used in the Paris law and fracture criterion at the interface ** *BOUNDARY, AMPLITUDE= Data lines to prescribe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD, AMPLITUDE= Data lines to specify loads *TEMPERATURE and/or *FIELD, AMPLITUDE= Data lines to specify values of predefined fields ** *END STEP Additional references • Coffin, L., “A Study of the Effects of Cyclic Thermal Stresses on a Ductile Metal,” Transactions of the American Society of Mechanical Engineering, vol. 76, pp. 931–951, 1954. • Manson, S., “Behavior of Materials under Condition of Thermal Stress,” Heat Transfer Symposium, University of Michigan Engineering Research Institute, Ann Arbor, MI, pp. 9–75, 1953. • Paris, P., M. Gomaz, and W. Anderson, “A Rational Analytic Theory of Fatigue,” The Trend in Engineering, vol. 15, 1961. 6.3 Dynamic stress/displacement analysis • “Dynamic analysis procedures: overview,” Section 6.3.1 • “Implicit dynamic analysis using direct integration,” Section 6.3.2 • “Explicit dynamic analysis,” Section 6.3.3 • “Direct-solution steady-state dynamic analysis,” Section 6.3.4 • “Natural frequency extraction,” Section 6.3.5 • “Complex eigenvalue extraction,” Section 6.3.6 • “Transient modal dynamic analysis,” Section 6.3.7 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 • “Subspace-based steady-state dynamic analysis,” Section 6.3.9 • “Response spectrum analysis,” Section 6.3.10 • “Random response analysis,” Section 6.3.11 6.3.1 DYNAMIC ANALYSIS PROCEDURES: OVERVIEW Overview Abaqus offers several methods for performing dynamic analysis of problems in which inertia effects are considered. Direct integration of the system must be used when nonlinear dynamic response is being studied. Implicit direct integration is provided in Abaqus/Standard; explicit direct integration is provided in Abaqus/Explicit. Modal methods are usually chosen for linear analyses because in direct-integration dynamics the global equations of motion of the system must be integrated through time, which makes direct-integration methods significantly more expensive than modal methods. Subspace-based methods are provided in Abaqus/Standard and offer cost-effective approaches to the analysis of systems that are mildly nonlinear. In Abaqus/Standard dynamic studies of linear problems are generally performed by using the eigenmodes of the system as a basis for calculating the response. In such cases the necessary modes and frequencies are calculated first in a frequency extraction step. The mode-based procedures are generally simple to use; and the dynamic response analysis itself is usually not expensive computationally, although the eigenmode extraction can become computationally intensive if many modes are required for a large model. The eigenvalues can be extracted in a prestressed system with the “stress stiffening” effect included (the initial stress matrix is included if the base state step definition included nonlinear geometric effects), which may be necessary in the dynamic study of preloaded systems. It is not possible to prescribe nonzero displacements and rotations directly in mode-based procedures. The method for prescribing motion in mode-based procedures is explained in “Base motions in modal-based procedures,” Section 2.5.9 of the Abaqus Theory Manual. Density must be defined for all materials used in any dynamic analysis, and damping (both viscous and structural) can be specified either at the material or step level, as described below in “Damping in dynamic analysis.” Implicit versus explicit dynamics The direct-integration dynamic procedure provided in Abaqus/Standard offers a choice of implicit operators for integration of the equations of motion, while Abaqus/Explicit uses the central-difference operator. In an implicit dynamic analysis the integration operator matrix must be inverted and a set of nonlinear equilibrium equations must be solved at each time increment. In an explicit dynamic analysis displacements and velocities are calculated in terms of quantities that are known at the beginning of an increment; therefore, the global mass and stiffness matrices need not be formed and inverted, which means that each increment is relatively inexpensive compared to the increments in an implicit integration scheme. The size of the time increment in an explicit dynamic analysis is limited, however, because the central-difference operator is only conditionally stable; whereas the implicit operator options available in Abaqus/Standard are unconditionally stable and, thus, there is no such limit on the size of the time increment that can be used for most analyses in Abaqus/Standard (accuracy governs the time increment in Abaqus/Standard). The stability limit for the central-difference method (the largest time increment that can be taken without the method generating large, rapidly growing errors) is closely related to the time required for a stress wave to cross the smallest element dimension in the model; thus, the time increment in an explicit dynamic analysis can be very short if the mesh contains small elements or if the stress wave speed in the material is very high. The method is, therefore, computationally attractive for problems in which the total dynamic response time that must be modeled is only a few orders of magnitude longer than this stability limit; for example, wave propagation studies or some “event and response” applications. Many of the advantages of the explicit procedure also apply to slower (quasi-static) processes for cases in which it is appropriate to use mass scaling to reduce the wave speed . Abaqus/Explicit offers fewer element types than Abaqus/Standard. For example, only first-order, displacement method elements (4-node quadrilaterals, 8-node bricks, etc.) and modified second-order elements are used, and each degree of freedom in the model must have mass or rotary inertia associated with it. However, the method provided in Abaqus/Explicit has some important advantages: 1. The analysis cost rises only linearly with problem size, whereas the cost of solving the nonlinear equations associated with implicit integration rises more rapidly than linearly with problem size. Therefore, Abaqus/Explicit is attractive for very large problems. 2. The explicit integration method is often more efficient than the implicit integration method for solving extremely discontinuous short-term events or processes. 3. Problems involving stress wave propagation can be far more efficient computationally in Abaqus/Explicit than in Abaqus/Standard. In choosing an approach to a nonlinear dynamic problem you must consider the length of time for which the response is sought compared to the stability limit of the explicit method; the size of the problem; and the restriction of the explicit method to first-order, pure displacement method or modified second-order elements. In some cases the choice is obvious, but in many problems of practical interest the choice depends on details of the specific case. Experience is then the only useful guide. Direct-solution versus modal superposition procedures Direct solution procedures must be used for dynamic analyses that involve a nonlinear response. Modal superposition procedures are a cost-effective option for performing linear or mildly nonlinear dynamic analyses. Direct-solution dynamic analysis procedures The following direct-solution dynamic analyses procedures are available in Abaqus: • Implicit dynamic analysis: Implicit direct-integration dynamic analysis (“Implicit dynamic analysis using direct integration,” Section 6.3.2) is used to study (strongly) nonlinear transient dynamic response in Abaqus/Standard. • Subspace-based explicit dynamic analysis: The subspace projection method in integration of the dynamic equations of equilibrium Abaqus/Standard uses direct, explicit written in terms of a vector space spanned by a number of eigenvectors (“Implicit dynamic analysis using direct integration,” Section 6.3.2). The eigenmodes of the system extracted in a frequency extraction step are used as the global basis vectors. This method can be very effective for systems with mild nonlinearities that do not substantially change the mode shapes. It cannot be used in contact analyses. • Explicit dynamic analysis: Explicit direct-integration dynamic analysis (“Explicit dynamic analysis,” Section 6.3.3) is available in Abaqus/Explicit. • Direct-solution steady-state harmonic response analysis: The steady-state harmonic response of a system can be calculated in Abaqus/Standard directly in terms of the physical degrees of freedom of the model (“Direct-solution steady-state dynamic analysis,” Section 6.3.4). The solution is given as in-phase (real) and out-of-phase (imaginary) components of the solution variables (displacement, stress, etc.) as functions of frequency. The main advantage of this method is that frequency-dependent effects (such as frequency-dependent damping) can be modeled. The direct method is the most accurate but also the most expensive steady-state harmonic response procedure. The direct method can also be used if nonsymmetric terms in the stiffness are important or if model parameters depend on frequency. Modal superposition procedures Abaqus includes a full range of modal superposition procedures. Modal superposition procedures can be run using a high-performance linear dynamics software architecture called SIM. The SIM architecture offers advantages over the traditional linear dynamics architecture for some large-scale analyses, as discussed below in “Using the SIM architecture for modal superposition dynamic analyses.” Prior to any modal superposition procedure, the natural frequencies of a system must be extracted using the eigenvalue analysis procedure (“Natural frequency extraction,” Section 6.3.5). Frequency extraction can be performed using the SIM architecture. The following modal superposition procedures are available in Abaqus: • Mode-based steady-state harmonic response analysis: A steady-state dynamic analysis based on the natural modes of the system can be used to calculate a system’s linearized response to harmonic excitation (“Mode-based steady-state dynamic analysis,” Section 6.3.8). This mode-based method is typically less expensive than the direct method. The solution is given as in-phase (real) and out-of-phase (imaginary) components of the solution variables (displacement, stress, etc.) as functions of frequency. Mode-based steady-state harmonic analysis can be performed using the SIM architecture. • Subspace-based of Abaqus/Standard analysis the steady-state dynamic equations are written in terms of a vector space spanned by a number of eigenvectors (“Subspace-based steady-state dynamic analysis,” Section 6.3.9). The eigenmodes of the system extracted in a frequency extraction step are used as the global basis vectors. The method is attractive because it allows frequency-dependent effects to be modeled and is much cheaper than the direct analysis method (“Direct-solution steady-state dynamic analysis,” Section 6.3.4). Subspace-based steady-state harmonic response analysis can be used if the stiffness is nonsymmetric and can be performed using the SIM architecture. steady-state harmonic response analysis: type this In • Mode-based transient response analysis: The modal dynamic procedure (“Transient modal dynamic analysis,” Section 6.3.7) provides transient response for linear problems using modal superposition. Mode-based transient analysis can be performed using the SIM architecture. • Response spectrum analysis: A linear response spectrum analysis (“Response spectrum analysis,” Section 6.3.10) is often used to obtain an approximate upper bound of the peak significant response of a system to a user-supplied input spectrum (such as earthquake data) as a function of frequency. The method has a very low computational cost and provides useful information about the spectral behavior of a system. Response spectrum analysis can be performed using the SIM architecture. • Random response analysis: The linearized response of a model to random excitation can be calculated based on the natural modes of the system (“Random response analysis,” Section 6.3.11). This procedure is used when the structure is excited continuously and the loading can be expressed statistically in terms of a “Power Spectral Density” (PSD) function. The response is calculated in terms of statistical quantities such as the mean value and the standard deviation of nodal and element variables. Random response analysis can be performed using the SIM architecture. • Complex eigenvalue extraction: The complex eigenvalue extraction procedure performs eigenvalue extraction to calculate the complex eigenvalues and the corresponding complex mode shapes of a system (“Complex eigenvalue extraction,” Section 6.3.6). The eigenmodes of the system extracted in a frequency extraction step are used as the global basis vectors. The complex eigenvalue extraction can be performed using the SIM architecture. Using the SIM architecture for modal superposition dynamic analyses SIM is a high-performance software architecture available in Abaqus that can be used to perform modal superposition dynamic analyses. The SIM architecture is much more efficient than the traditional architecture for large-scale linear dynamic analyses (both model size and number of modes) with minimal output requests. SIM-based analyses can be used to efficiently handle nondiagonal damping generated from element or material contributions, as discussed below in “Damping in a mode-based steady-state and transient linear dynamic analysis using the SIM architecture.” Therefore, SIM-based procedures are an efficient alternative to subspace-based linear dynamic procedures for models with element damping or frequency- independent materials. Activating the SIM architecture To use the SIM architecture for a modal superposition dynamic analysis, activate SIM for the initial frequency extraction procedure. SIM-based frequency extraction procedures write the mode shapes and other modal system information to a special linear dynamics data (.sim) file. By default, this data file is written to the scratch directory and deleted upon job completion; however, if restart is requested, the file is saved in the user directory. All subsequent mode-based steady-state or transient dynamic steps in an analysis automatically use this linear dynamics data file (and by extension the SIM architecture). If you restart an analysis that uses the SIM architecture, you must include the linear dynamics data file. For more information about frequency extraction procedures, see “Natural frequency extraction,” Section 6.3.5. Input File Usage: *FREQUENCY, SIM Abaqus/CAE Usage: Step module: Step→Create: Frequency: Use SIM-based linear dynamics procedures Example The SIM architecture will be used for the entire linear dynamic analysis in the following input file template: *STEP *FREQUENCY, EIGENSOLVER=LANCZOS or AMS, SIM Data line to control eigenvalue extraction *END STEP ** *STEP *MODAL DYNAMIC Data line to control time incrementation *SELECT EIGENMODES Data lines to define the applicable mode ranges *END STEP ** *STEP *STEADY STATE DYNAMICS Data lines to specify frequency ranges and bias parameters *SELECT EIGENMODES Data lines to define the applicable mode ranges *END STEP ** *STEP *STEADY STATE DYNAMICS, SUBSPACE PROJECTION Data lines to specify frequency ranges and bias parameters *SELECT EIGENMODES Data lines to define the applicable mode ranges *END STEP Output in a SIM-based analysis Output is a fundamental factor in the performance of a linear dynamic analysis. Since it is difficult to predict the desired output quantities for a linear dynamic analysis, no output is written to the output database (.odb) file by default during a SIM-based linear dynamic analysis; output requests must be requested explicitly. Preselected output requests are ignored in SIM-based dynamic analysis procedures. There are several restrictions on available output requests that apply specifically to SIM-based analyses: • You cannot request output to the results (.fil) file. • Element variables cannot be output to the printed data (.dat) file except for random response analysis. • Output of “base motion” is not supported except for random response analysis. Limitations of the SIM architecture The SIM architecture cannot be used with frequency extractions using the subspace iteration eigensolver. Fully coupled structural-acoustic frequency extractions cannot be performed using the SIM architecture. However, projected coupling operators can be used to perform fully coupled structural-acoustic steady-state response analyses . The cyclic symmetry modeling feature cannot be used in SIM-based analyses. Nonphysical material properties in dynamic analyses Abaqus relies on user-supplied model data and assumes that the material’s physical properties reflect experimental results. Examples of meaningful material properties are a positive mass density per volume, a positive Young’s modulus, and a positive value for any available damping coefficients. However, in special cases you may want to “adjust” a value of density, mass, stiffness, or damping in a region or a part of the model to bring the overall mass, stiffness, or damping to the expected required levels. Certain material options in Abaqus allow you to introduce nonphysical material properties to achieve this adjustment. For example, to adjust the mass of the model, you can define a nonstructural mass with a negative mass value, use mass elements with a negative mass over a region of nodes, or introduce additional elements with negative density. Similarly, to adjust damping levels, you can use negative damping coefficients or introduce dashpot elements with a negative dashpot constant to reduce the overall damping levels. Springs with negative stiffness can be defined to adjust the model stiffness. If you specify nonphysical but allowed material properties, Abaqus issues a warning message. However, if you specify nonphysical material properties that are not allowed, Abaqus issues an error message. When introducing nonphysical material properties, you must be aware that the overall behavior should be “physical”; for example, the mass values at all nodes must be positive in an eigenvalue extraction procedure. There are consequences of using nonphysical material properties that are easy to check and interpret, and there are others beyond the control of Abaqus. Therefore, you should fully understand the stated problem and the consequences of using nonphysical material properties before you specify the properties. This is particularly important in Abaqus/Explicit analyses, where the size of the time increment depends on material properties. For example, distributed mass-dependent loads are calculated based on the overall mass density (positive and negative) provided. Damping in dynamic analysis Every nonconservative system exhibits some energy loss that is attributed to material nonlinearity, internal material friction, or to external (mostly joint) frictional behavior. Conventional engineering materials like steel and high strength aluminum alloys provide small amounts of internal material damping, not enough to prevent large amplification at or near resonant frequencies. Damping properties increase in modern composite fiber-reinforced materials, where the energy loss occurs through plastic or viscoelastic phenomena as well as from friction at the interfaces between the matrix and reinforcement. Still larger material damping is exhibited by thermoplastics. Mechanical dampers may be added to models to introduce damping forces to the system. In general, it is difficult to quantify the source of a system’s damping. It usually comes from several sources simultaneously; e.g., from energy loss during hysteretic loading, viscoelastic material properties, and external joint friction. Users that work with a specific system know the source of the energy loss from experience. A variety of methods are available in Abaqus to specify damping that accurately models the energy loss in a dynamic system. Sources of damping Abaqus has four categories of damping sources: material and element damping, global damping, modal damping, and damping associated with time integration. If necessary, you can include multiple damping sources and combine different damping sources in a model. Material and element damping Damping may be specified as part of a material definition that is assigned to a model . In addition, Abaqus has elements such as dashpots, springs with their complex stiffness matrix, and connectors that serve as dampers, all with viscous and structural damping factors. Viscous damping can be included in mass, beam, pipe, and shell elements with general section properties; and it can also be used in substructure elements . In direct steady-state dynamic analysis you can define the viscous and structural damping due to the interaction between the contacting surfaces by using user subroutine UINTER . Contact damping is not applicable for linear perturbation procedures. In acoustic elements, velocity proportional viscous damping is implemented using the volumetric drag parameter . Acoustic infinite elements and impedance conditions also add damping to a model. Global damping In situations where material or element damping is not appropriate or sufficient, you can apply abstract damping factors to an entire model. Abaqus allows you to specify global damping factors for both viscous (Rayleigh damping) and structural damping (imaginary stiffness matrix). Modal damping Modal damping applies only to mode-based linear dynamic analyses. This technique allows you to apply damping directly to the modes of the system. By definition, modal damping contributes only diagonal entries to the modal system of equations and can be defined several different ways. Damping associated with time integration Marching through a simulation with a finite time increment size causes some damping. This type of damping applies only to analyses using direct time integration. See “Implicit dynamic analysis using direct integration,” Section 6.3.2, for further discussion of this source of damping. Damping in a linear dynamic analysis Damping can be applied to a linear dynamic system in two forms: • velocity proportional viscous damping; and • displacement proportional structural damping, which is for use in frequency domain dynamics. The exception is SIM-based transient modal dynamic analysis, where the structural damping is converted to the equivalent diagonal viscous damping . An additional type of damping known as composite damping serves as a means to calculate a model average critical damping with the material density as the weight factor and is intended for use in mode- based dynamics (excluding subspace projection steady-state analysis and SIM-based dynamic analyses). For additional information, see “Damping options for modal dynamics,” Section 2.5.4 of the Abaqus Theory Manual. The types of damping available for linear dynamic analyses depend on the procedure type and the architecture (traditional or SIM) used to perform the analysis, as outlined in Table 6.3.1–1 and Table 6.3.1–2. For completeness, Table 6.3.1–1 also includes the damping options for a direct steady-state dynamic analysis. In addition to directly specified modal damping, global damping can be used in all linear dynamic procedures. Material and element damping can be used in subspace-based and SIM-based linear dynamic procedures. Table 6.3.1–1 Damping sources for traditional architecture. Damping Source Modal Global Material and Element 6.3.1–8 Traditional Architecture Mode-based steady-state dynamics Subspace-based steady-state dynamics Transient modal dynamics Random response analysis Complex frequency Response spectrum Table 6.3.1–2 Damping sources for SIM architecture. SIM Architecture Damping Source Modal Global Material and Element Mode-based steady-state dynamics Subspace-based steady-state dynamics Transient modal dynamics Random response analysis Complex frequency Response spectrum In a subspace-based or SIM-based linear dynamic analysis, material and element damping operators must first be projected onto the basis of mode shapes. This projection results in a full modal damping matrix for both viscous and structural damping; therefore, a modal steady-state response analysis requires the solution of a system of linear equations at each frequency point. The size of this system is equal to the number of modes used in the response calculation. In a mode-based transient analysis, the projected damping operator is treated explicitly in time by including it on the right-hand side of the system of equations. Frequency-dependent damping is supported only for the subspace-based and direct-integration steady-state dynamic procedures. Material and element damping is not supported for the response spectrum or the random response procedures. In these procedures, only modal and global damping are allowed, and material or element damping is ignored. Damping in a mode-based steady-state and transient linear dynamic analysis using the SIM architecture SIM-based linear dynamic analyses may include material and element damping contributions that introduce both diagonal and nondiagonal terms in the modal system of equations. The projection of material and element damping operators onto the basis of mode shapes is performed during the natural frequency extraction procedure, which enables a high-performance projection operation to be performed when used with the AMS eigensolver. If the damping operators depend on frequency, they will be evaluated at the frequency specified for property evaluation during the frequency extraction procedure. When the structural and viscous damping operators are projected onto the mode shapes, the full modal damping matrix is stored in the linear dynamics data (.sim) file. The full modal damping matrix is combined with any diagonal contributions from global damping or traditional modal damping. The combined damping operator matrix is included in subsequent mode-based transient or steady-state dynamics steps. If there are nondiagonal (i.e., projected) damping contributions and a large number of modes are included, performance of the linear dynamics calculations will be impacted since a direct solve must be performed at each frequency point. Acoustic damping due to impedance conditions is projected onto the subspace of acoustic eigenvectors. These contributions are taken into account in a subspace-based steady-state dynamics analysis that uses the SIM architecture. The default behavior for a SIM-based frequency extraction step is to project any element and material damping onto the mode shapes. You can turn off this damping projection if it is not desired; however, in this case only diagonal damping is available for subsequent modal superposition steps. If the projected damping matrices are not desired in a particular mode-based linear dynamic step for performance reasons, they can be deactivated in that step using the damping control techniques discussed above in “Damping in dynamic analysis.” Input File Usage: Use the following option to project material and element damping operators in a SIM-based analysis: Abaqus/CAE Usage: *FREQUENCY, SIM, DAMPING PROJECTION=ON (default) Use the following option to turn off damping projection in a SIM-based analysis: *FREQUENCY, SIM, DAMPING PROJECTION=OFF To control the projection of element and material damping in a SIM-based frequency extraction step that uses the Lanczos eigensolver: Step module: Step→Create: Frequency: Eigensolver: Lanczos, Use SIM-based linear dynamics procedures, toggle Project damping operators To control the projection of element and material damping in a frequency extraction step that uses the AMS eigensolver: Step module: Step→Create: Frequency: Eigensolver: AMS, toggle Project damping operators Defining viscous damping Abaqus allows you to choose a particular source of viscous damping, to add several sources, or to exclude viscous damping effects. Defining material/element viscous damping You can choose to model the viscous damping matrix, , by using material damping properties and/or damping elements (such as dashpot or mass elements). The viscous, mass, and/or stiffness proportional damping matrix will include the material Rayleigh damping factors, , as well as the element-oriented damping factor, (e.g., for mass elements). The material/element-based viscous damping matrix can be written as and where procedures projection of Input File Usage: Abaqus/CAE Usage: represents the viscous damping matrix for elements such as dashpots. In mode-based into the eigenmodes results in a non-diagonal matrix. , BETA= Use the following option to specify material viscous damping for elements with mechanical degrees of freedom: *DAMPING, ALPHA= Use the following option to specify material viscous damping for acoustic elements: *ACOUSTIC MEDIUM, VOLUMETRIC DRAG Property module: material editor: Mechanical→Damping: Alpha: or Beta: Property module: material editor: Other→Acoustic Medium: Volumetric Drag Defining global viscous damping You can supply global mass and stiffness proportional viscous damping factors, respectively, to create the global damping matrix using the global model mass and stiffness matrices, and , respectively: and , These parameters can be specified for the entire model (default), for the mechanical degree of freedom field (displacements and rotations) only, or for the acoustic field only. Input File Usage: Abaqus/CAE Usage: Use the following option to specify global viscous damping: *GLOBAL DAMPING, ALPHA= Global viscous damping is not supported in Abaqus/CAE. , BETA= Defining viscous modal damping Rayleigh damping introduces a damping matrix, , defined as where factors that you define. is the mass matrix of the model, is the stiffness matrix of the model, and and are In Abaqus/Standard you can define and independently for each mode, so that the above equation becomes (no sum on M) where the subscript M refers to the mode number and stiffness terms associated with the Mth mode. , , and are the damping, mass, and Input File Usage: Use the following option to define Rayleigh damping by specifying mode numbers: Abaqus/CAE Usage: *MODAL DAMPING, RAYLEIGH, DEFINITION=MODE NUMBERS Use the following option to define Rayleigh damping by specifying a frequency range: *MODAL DAMPING, RAYLEIGH, DEFINITION=FREQUENCY RANGE Use the following input to define Rayleigh damping by specifying mode numbers: Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Modes, Rayleigh: Use Rayleigh damping data Use the following input to define Rayleigh damping by specifying frequency ranges: Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Frequencies, Rayleigh: Use Rayleigh damping data Defining viscous modal damping as a fraction of the critical damping You can also specify the damping in each eigenmode in the model or for the specified frequency as a fraction of the critical damping. Critical damping is defined as where m is the mass of the system and k is the stiffness of the system. Typical values of the fraction of critical damping, ; but Abaqus/Standard accepts any positive value. The critical damping factors can be changed from step to step. , are from 1% to 10% of critical damping, Input File Usage: Use the following option to define the fraction of critical damping by specifying mode numbers: *MODAL DAMPING, MODAL=DIRECT, DEFINITION=MODE NUMBERS Use the following option to define the fraction of critical damping by specifying a frequency range: *MODAL DAMPING, MODAL=DIRECT, DEFINITION=FREQUENCY RANGE Abaqus/CAE Usage: Use the following input to define the fraction of critical damping by specifying mode numbers: Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Modes, Direct modal: Use direct damping data Use the following input to define the fraction of critical damping by specifying frequency ranges: Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Frequencies, Direct modal: Use direct damping data Viscous modal damping for uncoupled structural-acoustic frequency extractions For uncoupled structural-acoustic frequency extractions performed using the AMS eigensolver, you can apply different damping to the structural and acoustic modes. This technique can be used only when damping is specified for a range of frequencies. Input File Usage: Use the following option to apply the specified damping to only the structural modes: *MODAL DAMPING, MODAL=DIRECT, DEFINITION=FREQUENCY RANGE, FIELD=MECHANICAL Use the following option to apply the specified damping to only the acoustic modes: *MODAL DAMPING, MODAL=DIRECT, DEFINITION=FREQUENCY RANGE, FIELD=ACOUSTIC Use the following option to apply the specified damping to both structural and acoustic modes (default): *MODAL DAMPING, MODAL=DIRECT, DEFINITION=FREQUENCY RANGE, FIELD=ALL Abaqus/CAE Usage: The ability to specify different damping for structural and acoustic modes is not supported in Abaqus/CAE. Controlling the sources of viscous damping The material/element and global viscous damping sources can be controlled at the step level; controls are not available for modal damping. If both the material/element and global viscous damping matrices are supplied, both will be used as a combined damping matrix unless you request that only the element or global damping factor be used. The combined material/element and global viscous damping is Input File Usage: Use the following option to activate only the material/element viscous damping matrix: *DAMPING CONTROLS, VISCOUS=ELEMENT Use the following option to activate only the global viscous damping matrix: *DAMPING CONTROLS, VISCOUS=FACTOR Use the following option to activate the combined material/element and global viscous damping matrix: Abaqus/CAE Usage: *DAMPING CONTROLS, VISCOUS=COMBINED Damping controls are not supported in Abaqus/CAE. Excluding viscous damping effects You can choose to exclude the effects of viscous damping altogether at the step level. Input File Usage: Use the following option to exclude the viscous damping matrix: Abaqus/CAE Usage: *DAMPING CONTROLS, VISCOUS=NONE Damping controls are not supported in Abaqus/CAE. Defining structural damping Abaqus allows you to choose a particular source of structural damping, to add several sources, or to exclude structural damping effects. Defining material/element structural damping The material/element structural damping matrix (that represents the imaginary stiffness and is proportional to forces or displacements) is defined as represents the material structural damping, represents the structural damping coefficient for where elements such as springs with complex stiffnesses and connectors, and is the real element stiffness matrix. In mode-based procedures the projection of onto the mode shapes results in a full modal damping matrix. When using SIM-based modal procedures, the projected material and element damping matrix may be combined with global and modal damping . Material/element structural damping is not available for acoustic elements. Input File Usage: Use the following option to specify material structural damping: Abaqus/CAE Usage: *DAMPING, STRUCTURAL= Property module: material editor: Mechanical→Damping: Structural: Defining global structural damping You can define the global structural damping factor, , to get Global structural damping can be specified for the entire model (default), for the mechanical degree of freedom field (displacements and rotations) only, or for the acoustic field only. Input File Usage: Use the following option to specify global structural damping: Abaqus/CAE Usage: *GLOBAL DAMPING, STRUCTURAL= Global structural damping is not supported in Abaqus/CAE. Defining structural modal damping Structural damping assumes that the damping forces are proportional to the forces caused by stressing of the structure and are opposed to the velocity . This form of damping can be used only when the displacement and velocity are exactly 90° out of phase, as in steady-state and random response analyses where the excitation is purely sinusoidal. Structural damping can be defined as diagonal modal damping for mode-based steady-state dynamic and random response analyses. Input File Usage: Use the following option to define structural damping by specifying mode numbers: *MODAL DAMPING, STRUCTURAL, DEFINITION=MODE NUMBERS Use the following option to define structural damping by specifying a frequency range: *MODAL DAMPING, STRUCTURAL, DEFINITION=FREQUENCY RANGE Abaqus/CAE Usage: Use the following input to define structural damping by specifying mode numbers: Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Modes, Structural: Use structural damping data Use the following input to define structural damping by specifying frequency ranges: Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Frequencies, Structural: Use structural damping data Controlling the sources of structural damping The material/element and global structural damping sources can be controlled at the step level; controls are not available for modal damping. If both the material/element and global structural damping matrices are supplied, both will be combined unless you request that only the element or global damping factor be used. The combined structural damping matrix is Input File Usage: Use the following option to activate only the material/element structural damping matrix: *DAMPING CONTROLS, STRUCTURAL=ELEMENT Use the following option to activate only the global structural damping matrix: *DAMPING CONTROLS, STRUCTURAL=FACTOR Use the following option to activate the combined material/element and global structural damping matrix: Abaqus/CAE Usage: *DAMPING CONTROLS, STRUCTURAL=COMBINED Damping controls are not supported in Abaqus/CAE. Excluding structural damping effects You can choose to exclude the effects of structural damping altogether at the step level. Input File Usage: Use the following option to exclude structural damping matrix: Abaqus/CAE Usage: *DAMPING CONTROLS, STRUCTURAL=NONE Damping controls are not supported in Abaqus/CAE. Defining both viscous and structural damping The imaginary contribution to the frequency domain dynamics equation, which represents the effect of damping, may include both viscous and structural damping and can be written as where is the forcing frequency. Defining composite modal damping Composite modal damping allows you to define a damping factor for each material in the model as a fraction of critical damping. These factors are then combined into a damping factor for each mode as weighted averages of the mass matrix associated with each material: (no sum over ) where material m, is the critical damping fraction used in mode , is the mass matrix associated with material m, is the critical damping fraction defined for is the eigenvector of mode , and is the generalized mass associated with mode : (no sum on ) If you specify composite modal damping, Abaqus calculates the damping coefficients in the eigenfrequency extraction step from the damping factors that you defined for each material. Composite modal damping can be defined only by specifying mode numbers; it cannot be defined by specifying a frequency range. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *DAMPING, COMPOSITE= *MODAL DAMPING, MODAL=COMPOSITE Property module: material editor: Mechanical→Damping: Composite: Step module: Create Step: Linear perturbation: any valid step type: Damping: Composite modal: Use composite damping data Defining global damping for acoustic fields If your model contains acoustic elements, Abaqus applies any specified global damping to both the acoustic fields and the structural fields in the model by default. If desired, you can specify that a global damping definition applies only to the acoustic fields or only to the displacement and rotation fields. Input File Usage: Abaqus/CAE Usage: Use the following option to apply global damping to all of the displacement, rotation, and acoustic fields in a model: *GLOBAL DAMPING, FIELD=ALL (default) Use the following option to apply global damping only to the acoustic fields in a model: *GLOBAL DAMPING, FIELD=ACOUSTIC Use the following option to apply global damping only to the displacement and rotation fields in a model: *GLOBAL DAMPING, FIELD=MECHANICAL Global damping is not supported in Abaqus/CAE. Defining and using both global and modal diagonal damping Mode-based procedures—such as steady-state dynamics, transient modal dynamic, response spectrum, and random response analyses—can also use a step-dependent, modal damping definition that is specified per eigenmode. When multiple modal damping definitions are used with different damping types, the damping is additive. If the same damping type is specified more than once, the last specification is used. If modal damping is used with global damping, both types of damping will contribute to the damping matrix. Damping controls have no effect on modal damping. If damping controls are used to exclude certain global damping effects in a step, all modal damping effects are still included in the step. To exclude modal damping, the damping definition must be specifically removed from the step definition. 6.3.2 IMPLICIT DYNAMIC ANALYSIS USING DIRECT INTEGRATION Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Dynamic analysis procedures: overview,” Section 6.3.1 • *DYNAMIC • “Configuring a dynamic, Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual implicit procedure” in “Configuring general analysis procedures,” Overview A direct-integration dynamic analysis in Abaqus/Standard: • must be used when nonlinear dynamic response is being studied; • can be fully nonlinear (general dynamic analysis) or can be based on the modes of the linear system (subspace projection method); and • can be used to study a variety of applications, including: – dynamic responses requiring transient fidelity and involving minimal energy dissipation; – dynamic responses involving nonlinearity, contact, and moderate energy dissipation; and – quasi-static responses in which considerable energy dissipation provides stability and improved convergence behavior for determining an essentially static solution. General dynamic analysis General nonlinear dynamic analysis in Abaqus/Standard uses implicit time integration to calculate the transient dynamic or quasi-static response of a system. The procedure can be applied to a broad range of applications calling for varying numerical solution strategies, such as the amount of numerical damping required to obtain convergence and the way in which the automatic time incrementation algorithm proceeds through the solution. Typical dynamic applications fall into three categories: • Transient fidelity applications, such as an analysis of satellite systems, require minimal energy In these applications small time increments are taken to accurately resolve the dissipation. vibrational response of the structure, and numerical energy dissipation is kept at a minimum. These stringent requirements tend to degrade convergence behavior for simulations involving contact or nonlinearities. • Moderate dissipation applications encompass a more general range of dynamic events in which a moderate amount of energy is dissipated by plasticity, viscous damping, or other effects. Typical applications include various insertion, impact, and forming analyses. The response of these structures can be either monotonic or nonmonotonic. Accurate resolution of high-frequency vibrations is usually not of interest in these applications. Some numerical energy dissipation tends to reduce solution noise and improve convergence behavior in these applications without significantly degrading solution accuracy. • Quasi-static applications are primarily interested in determining a final static response. These problems typically show monotonic behavior, and inertia effects are introduced primarily to the statically unstable behavior may be due to regularize unstable behavior. temporarily unconstrained rigid body modes or “snap-through” phenomena. Large time increments are taken when possible to obtain the final solution at minimal computational cost. Considerable numerical dissipation may be required to obtain convergence during certain stages of the loading history. For example, An example of a transient fidelity application is available in “Modeling of an automobile suspension,” Section 2.1.7 of the Abaqus Example Problems Manual. An analysis that includes both a moderate dissipation step and a quasi-static step is described in “Impact analysis of a pawl-ratchet device,” Section 2.1.17 of the Abaqus Example Problems Manual. Specifying the application type Based on the classifications listed above, you should indicate the type of application you are studying when performing a general dynamic analysis. Abaqus/Standard assigns numerical settings based on your classification of the application type, and this classification can significantly affect a simulation. In some cases accurate results can be obtained with more than one application-type setting, in which case analysis efficiency should be considered. A general trend is that—among the three classifications—the high-dissipation quasi-static classification tends to result in the best convergence behavior and the low- dissipation transient fidelity classification tends to have the highest likelihood of convergence difficulty. Input File Usage: Abaqus/CAE Usage: Use the following option for transient fidelity applications: *DYNAMIC, APPLICATION=TRANSIENT FIDELITY (default for models without contact) Use the following option for moderate dissipation applications: *DYNAMIC, APPLICATION=MODERATE DISSIPATION (default for models with contact) Use the following option for quasi-static applications: *DYNAMIC, APPLICATION=QUASI-STATIC Step module: Create Step: General: Dynamic, Implicit The application type is specified in the Edit Step dialog box: Basic: Application: Transient fidelity, Moderate dissipation, Quasi-static, or Analysis product default Diagnostics for modeling errors associated with mass properties Accurate representation of inertia properties is necessary for accurate dynamic analyses. In some cases Abaqus/Standard provides diagnostic messages when it detects likely modeling errors associated with the specification of inertia properties. The most common way of specifying inertia properties is with material densities. Abaqus/Standard issues a warning message to the data (.dat) file if a material density is omitted in a dynamic analysis (this warning is not issued if the density is zero only for certain values of temperature or field variables). Other methods of specifying inertia properties include: • point mass and rotary inertia definitions, and • constraining nodes without inertia themselves to nodes having inertia properties defined. In some circumstances Abaqus/Standard attempts to solve systems of equations involving effective inversion of the global mass matrix to directly adjust velocities and accelerations during a general dynamic analysis as described in “Initial conditions” and “Intermittent contact/impact” below. These additional velocity and acceleration adjustments occur by default only for transient fidelity application types as defined above. If the global mass matrix is found to be singular, Abaqus/Standard issues an error message by default, because singular mass is an indication that the mass properties are not realistic due to a modeling error. Diagnostic feedback specific to the global mass matrix being singular is typically not provided for quasi-static and moderate dissipation application types, although warnings typically are issued regarding the lack of material density. Singular mass is not necessarily detrimental to a quasi-static analysis. For example, it would be reasonable to only define inertia properties (such as density) in components or regions with temporary static instabilities (such as initially unconstrained rigid body modes that become constrained once contact occurs) in a quasi-static analysis. You can control the course of action Abaqus/Standard takes upon detecting a singular global mass matrix. Input File Usage: Use the following default option to issue an error message and stop execution if a singular global mass matrix is detected when calculating velocity and acceleration adjustments: *DYNAMIC, SINGULAR MASS=ERROR Use the following option to issue a warning message and avoid velocity and acceleration adjustments (i.e., continue time integration using current velocities and accelerations) if a singular global mass matrix is detected: *DYNAMIC, SINGULAR MASS=WARNING Use the following option to adjust velocities and accelerations even if a singular mass matrix is detected. This setting can result in large, non-physical velocity and/or acceleration adjustments, which can, in turn, cause poor time integration solutions and artificial convergence difficulties. This approach is not generally recommended; it should be used only in special cases when the analyst has a thorough understanding of how to interpret results obtained in this way. Abaqus/CAE Usage: *DYNAMIC, SINGULAR MASS=MAKE ADJUSTMENTS The default singular mass setting cannot be modified in Abaqus/CAE. Numerical details The effect of the application-type classification on numerical aspects of general dynamic analyses is described below. In most cases the settings determined by the application type are sufficient to successfully perform an analysis. However, detailed user controls are provided to override settings on an individual basis. Time integration methods Abaqus/Standard uses the Hilber-Hughes-Taylor time integration by default unless you specify that the application type is quasi-static. The Hilber-Hughes-Taylor operator is an extension of the Newmark -method. Numerical parameters associated with the Hilber-Hughes-Taylor operator are tuned differently for moderate dissipation and transient fidelity applications (as discussed later in this section). The backward Euler operator is used by default if the application classification is quasi-static. These time integration operators are implicit, which means that the operator matrix must be inverted and a set of simultaneous nonlinear dynamic equilibrium equations must be solved at each time increment. This solution is done iteratively using Newton’s method. The principal advantage of these operators is that they are unconditionally stable for linear systems; there is no mathematical limit on the size of the time increment that can be used to integrate a linear system. An unconditionally stable integration operator is of great value when studying structural systems because a conditionally stable integration operator (such as that used in the explicit method) can lead to impractically small time steps and, therefore, a computationally expensive analysis. Marching through a simulation with a finite time increment size generally introduces some degree of numerical damping. This damping differs from the material damping discussed in “Material damping,” Section 26.1.1 (and in many cases these two forms of damping will work well together). The amount of damping associated with the time integration varies among the operator types (for example, the backward Euler operator tends to be more dissipative than the Hilber-Hughes-Taylor operator) and in many cases (such as with the Hilber-Hughes-Taylor operator) depends on settings of numerical parameters associated with the operator. The ability of the operator to effectively treat contact conditions is often of considerable importance with respect to their usefulness. For example, some changes in contact conditions can result in “negative damping” (nonphysical energy source) for many time integrators, which can be very undesirable. It is possible to override the time integrator implied by the application-type classification; for example, you can perform a moderate dissipation dynamic analysis using the backward Euler integrator. Changing the default integrator is not generally recommended but may be useful in special cases. Input File Usage: Use the following option to use the Hilber-Hughes-Taylor integrator with default integrator parameter settings corresponding to those for transient fidelity applications: *DYNAMIC, TIME INTEGRATOR=HHT-TF Use the following option to use the Hilber-Hughes-Taylor integrator with default integrator parameter settings corresponding to those for moderate dissipation applications: *DYNAMIC, TIME INTEGRATOR=HHT-MD Abaqus/CAE Usage: Use the following option to use the backward Euler integrator: *DYNAMIC, TIME INTEGRATOR=BWE The default time integrator cannot be modified in Abaqus/CAE. Additional control over integrator parameters Additional user controls enable modifications to settings of numerical parameters associated with the Hilber-Hughes-Taylor operator for descriptions of the numerical parameters). The default parameter settings depend on the specified application type, as indicated in Table 6.3.2–1 for the basis of these settings). Table 6.3.2–1 Default parameters for the Hilber-Hughes-Taylor integrator. Parameter Transient Fidelity Moderate Dissipation Application –0.05 0.275625 0.55 –0.41421 0.5 0.91421 These parameters can be adjusted or modified individually if the Hilber-Hughes-Taylor operator is being used. If the default settings of these parameters correspond to the transient fidelity settings shown in Table 6.3.2–1 and you explicitly modify the parameter alone, the other parameters will be adjusted automatically to . This relation provides control of the numerical damping associated with the time integrator while preserving desirable characteristics of the integrator. The numerical damping grows with the ratio of the time increment to the period of vibration of a mode. Negative values of results in no damping (energy preserving) and is exactly the trapezoidal rule (sometimes called the Newmark -method, with ). The setting provides the maximum numerical damping. It gives a damping ratio of about 6% when the time increment is 40% of the period of oscillation of the mode being studied. Allowable values of provide damping; whereas , and are: and and , , , Input File Usage: Abaqus/CAE Usage: . *DYNAMIC, ALPHA= , BETA= , GAMMA= Only the parameter can be modified in Abaqus/CAE: Step module: Create Step: General: Dynamic, Implicit: Other: Alpha: Specify: Default incrementation schemes Automatic time incrementation is used by default for nonlinear dynamic procedures. The main factors used to control adjustments to the time increment size for an implicit dynamic procedure are the convergence behavior of the Newton iterations and the accuracy of the time integration. The time increment size may vary considerably during an analysis. Details of the time increment control algorithm depend on the type of dynamic application you are studying. The following factors are considered by default in the time increment control algorithm if you specify a quasi-static–type application (the same factors control the time increment size for purely static analyses): • The time increment size is reduced if an increment appears to be diverging or if the convergence rate is slow. • The time increment size is fairly aggressively increased if rapid convergence occurs in previous increments. Analyses for moderate dissipation-type applications also use these same factors, as well as a default upper bound on the time increment size equal to one-tenth of the step duration. The following factors are considered by default in the time increment control algorithm if you specify a transient fidelity–type application: • The time increment size is reduced if an increment appears to be diverging or if the convergence rate is slow. • The time increment size is reduced if changes in contact status are detected during the first attempt of processing an increment. The new increment size is set such that the end of the increment corresponds to the average time of the contact status changes that were detected with the previous increment size. (In such cases an additional very small time increment is used to enforce compatibility of velocities and accelerations across active contact interfaces.) • The time increment size is reduced if the half-increment residual (out-of-balance force) halfway through a time increment exceeds the half-increment residual tolerance, which is 10,000 times the time average force for a contact analysis or 1000 times the time average force for an analysis without contact. • The time increment is gradually increased if rapid convergence occurs in previous increments. • The upper bound for the time increment size is equal to 1/100 of the step duration. Intermittent contact/impact The second and third factors described in the preceding list often result in very small time increment sizes for contact simulations that are performed as a transient fidelity application (and the time increment size tends to remain small due to the fourth factor). This problem can be avoided by specifying a different application type or by using more detailed user controls, as discussed below. General settings for the time increment controls A high level user control over which factors are considered by the time increment control algorithm can be used to override the defaults implied by the specified application type for the analysis. Regardless of the application type you have specified, you can enforce time increment controls associated with either quasi-static applications or transient fidelity applications. Input File Usage: Use the following option to obtain the aggressive time increment control settings associated with quasi-static applications: *DYNAMIC, INCREMENTATION=AGGRESSIVE Use the following option to obtain the more conservative time increment control settings associated with transient fidelity applications: *DYNAMIC, INCREMENTATION=CONSERVATIVE The default Abaqus/CAE. time incrementation control settings cannot be modified in Abaqus/CAE Usage: Controlling the half-increment residual Controls associated with the half-increment residual tolerance are provided for tuning the time incrementation. These controls are intended for advanced users and typically do not need to be modified. Input File Usage: Abaqus/CAE Usage: Use the following option to specify that no check of the half-increment residual should be performed: *DYNAMIC, NOHAF Use the following option to specify the half-increment residual tolerance as a scale factor of the time average force (moment): *DYNAMIC, HALFINC SCALE FACTOR=scale factor Use the following option to directly specify the half-increment residual force tolerance (the half-increment residual moment tolerance is the half-increment residual force tolerance times the characteristic element length automatically calculated): *DYNAMIC, HAFTOL=tolerance Use the following option to specify that no check of the half-increment residual should be performed: Step module: Create Step: General: Dynamic, Implicit: Incrementation: toggle on Suppress half-increment residual calculation Use the following option to specify the half-increment residual tolerance as a scale factor of the time average force (moment): Step module: Create Step: General: Dynamic, Implicit: Incrementation: Half-increment Residual: Specify scale factor: scale factor Use the following option to specify the half-increment residual force tolerance directly: Step module: Create Step: General: Dynamic, Implicit: Incrementation: Half-increment Residual: Specify value: tolerance Controlling incrementation involving contact By default, specifying a transient fidelity application typically results in reduced time increment sizes upon changes in contact status. An extra time increment with a very small size is subsequently performed to enforce compatibility of velocities and accelerations across active contact interfaces. Direct user control over these incrementation aspects is available. Input File Usage: Use the following option to avoid automatically cutting back the increment size and enforcing velocity and acceleration compatibility in the contact region upon changes in contact status: *DYNAMIC, IMPACT=NO Use the following option to automatically cut back the increment size and enforce velocity and acceleration compatibility in the contact region upon changes in contact status: *DYNAMIC, IMPACT=AVERAGE TIME Use the following option to enforce velocity and acceleration compatibility in the contact region without automatically cutting back the increment size upon changes in contact status: Abaqus/CAE Usage: *DYNAMIC, IMPACT=CURRENT TIME The default contact incrementation scheme cannot be modified in Abaqus/CAE. Direct time incrementation You may directly specify the time increment size to be used. This approach is not generally recommended but may be useful in special cases. The analysis will terminate if convergence tolerances are not satisfied within the maximum number of iterations allowed. It is possible to ignore convergence tolerances: the solution to an increment is accepted after the specified maximum number of iterations allowed even if convergence tolerances are not satisfied. Ignoring convergence tolerances can result in highly nonphysical results and is not recommended except by analysts with a thorough understanding of how to interpret results obtained this way. Input File Usage: Use the following option to directly specify the time increment: *DYNAMIC, DIRECT Use the following option to ignore convergence tolerances after the maximum number of iterations is reached: Abaqus/CAE Usage: *DYNAMIC, DIRECT=NO STOP Use the following option to specify the time increment directly: Step module: Create Step: General: Dynamic, Implicit: Incrementation: Fixed Use the following option to ignore convergence tolerances after the maximum number of iterations is reached: Step module: Create Step: General: Dynamic, Implicit: Other: Accept solution after reaching maximum number of iterations Default amplitude for loads Loads such as applied forces or pressures are ramped on by default if you have selected the quasi-static application classification; such ramping tends to enhance robustness because the load increment size is proportional to the time increment size. For example, if the Newton iterations are not able to converge for a particular time increment size, the automatic time incrementation algorithm will reduce the time increment size and restart the Newton iterations with a smaller load incremental considered. For the other application classifications the dynamic procedure applies loads with a step function by default such that the full load is applied in the first increment of the step (regardless of the time increment size) and the load magnitude remains constant over each step. Thus, if the first increment is unable to converge with the original time increment size, reducing the time increment will not reduce the load increment by default. In some cases the convergence behavior will still improve upon reducing the time increment because the regularizing effect of inertia on the integration operators is inversely proportional to the square of the time increment size. See “Defining an analysis,” Section 6.1.2, for more information on default amplitude types for the various procedures and how to override the default. The “subspace projection” method The alternative approach provided in Abaqus/Standard for nonlinear dynamic problems is the “subspace projection” method. See “Subspace dynamics,” Section 2.4.3 of the Abaqus Theory Manual, for the theory behind this method. In this method the modes of the linear system are extracted in an eigenfrequency extraction step (“Natural frequency extraction,” Section 6.3.5) prior to the dynamic analysis and are used as a small set of global basis vectors to develop the solution. These modes will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. The method works well when the system exhibits mildly nonlinear behavior, such as small regions of plastic yielding or rotations that are not small but not too large. This method can be very effective. As with the other direct integration methods, it is more expensive in terms of computer time than the modal methods of purely linear dynamic analysis, but it is often significantly less expensive than the direct integration of all of the equations of motion of the model. However, since the subspace projection method is based on the modes of the system, it will not be accurate if there is extreme nonlinear response that cannot be modeled well by the modes that form the basis of the solution. Input File Usage: Abaqus/CAE Usage: *DYNAMIC, SUBSPACE Step module: Create Step: General: Dynamic, Subspace Selecting the modes on which to project You can select the modes of the system on which the subspace projection will be performed. The mode numbers can be listed individually, or they can be generated automatically. If you choose not to select the modes, all modes extracted in the prior frequency extraction step, including residual modes if they were activated, are used in the subspace projection. Input File Usage: Use one of the following options: *SELECT EIGENMODES *SELECT EIGENMODES, GENERATE Step module: Create Step: General: Dynamic, Subspace: Basic: Number of modes to use: All or Specify Abaqus/CAE Usage: Numerical implementation The subspace projection method is implemented in Abaqus/Standard using the explicit (central difference) operator to integrate the equations of motion written in terms of the modes of the linear system. This integration method is particularly effective here because the modes are orthogonal with respect to the mass matrix so that the projected system always has a diagonal mass matrix. for the linear system, where A fixed time increment is used: this increment is the smaller of the time increment that you specify or 80% of the stable time increment, which is is the highest circular frequency of the modes that are used as the basis of the solution. The 80% factor is intended as a safety factor so that any increase in this highest frequency caused by nonlinear effects is less likely to cause the integration to become unstable. The 80% is rather arbitrary; in some cases it may be nonconservative. You must monitor the response—for example, the energy balance—to ensure that the time increment is not causing instability. Instability is a concern if the nonlinearities can stiffen the system significantly, although in many practical cases such stiffening effects are more prominent in increasing the lower frequencies of the system than in affecting the highest frequencies that are likely to be retained to represent the dynamic behavior accurately. Accuracy of the subspace projection method The effectiveness of the subspace projection method depends on the value of the modes of the linear system as a set of global interpolation functions for the problem, which is a matter of judgment on your part—the same sort of judgment as required when deciding if a particular mesh of finite elements is sufficient. The method is valuable for mildly nonlinear systems and for cases where it is easy to extract enough modes that you can be confident that they describe the system adequately. If nonlinear geometric effects are considered in the subspace dynamics step, it is possible to perform a dynamic simulation for some time, reextract the modes on the current stressed geometry by using another frequency extraction step, and then continue the analysis with the new modes as the subspace basis system. This procedure can improve the accuracy of the method in some cases. Material damping You can introduce Rayleigh damping, as explained in “Material damping,” Section 26.1.1. This damping will act in addition to numerical damping associated with the time integrator (discussed previously). Input File Usage: Abaqus/CAE Usage: *DAMPING, ALPHA= Property module: material editor: Mechanical→Damping: Alpha and Beta , BETA= Initial conditions “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the available initial conditions. Initial velocities must be defined in global directions regardless of the use of nodal transformations . If initial velocities are specified at nodes for which displacement boundary conditions are also specified, the initial velocities will be ignored at these nodes. However, if a displacement boundary condition refers to an amplitude curve with an analytically defined time variation (i.e., excluding the piecewise linear tabular and equally spaced definitions), Abaqus/Standard will compute the initial velocity for the nodes involved in the boundary condition as the time derivative (evaluated at time zero) of the analytic variation. When initial velocities are specified for dynamic analysis, they should be consistent with all of the constraints on the model, especially time-dependent boundary conditions. Abaqus/Standard will ensure that initial velocities are consistent with boundary conditions and with multi-point and equation constraints but will not check for consistency with internal constraints such as incompressibility of the material. In case of a conflict, boundary conditions and multi-point constraints take precedence over initial conditions. Specified initial velocities are used in a dynamic step only if it is the first dynamic step in an analysis. If a dynamic step is not the first dynamic step and there is an immediately preceding dynamic step, the velocities from the end of the preceding step are used as the initial velocities for the current step. If a dynamic step is not the first dynamic step and the immediately preceding step is not a dynamic step, zero initial velocities are assumed for the current step. Controlling calculation of accelerations at the beginning of a dynamic step By default, Abaqus/Standard will calculate accelerations at the beginning of the dynamic step for transient fidelity applications. You can choose to bypass these acceleration calculations, in which case Abaqus/Standard will assume that initial accelerations for the current step are zero unless there is an immediately preceding dynamic step. If the immediately preceding step is also a dynamic step, bypassing the acceleration calculations will cause Abaqus/Standard to use the accelerations from the end of the previous step to continue the new step. It is appropriate to bypass the acceleration calculations if the loading has not changed suddenly at the start of the dynamic step, but it is not correct if the loading at the beginning of the first increment is significantly different from that at the end of the previous step. In cases where large loads are applied suddenly, high-frequency noise due to the bypass of the acceleration calculations may greatly increase the half-increment residual. Input File Usage: Abaqus/CAE Usage: *DYNAMIC, INITIAL=NO Step module: Create Step: General: Dynamic, Implicit: Other: Initial acceleration calculations at beginning of step: Bypass Boundary conditions Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6), to warping degree of freedom 7 in open-section beam elements, to fluid pressure degree of freedom 8 for hydrostatic fluid elements, or to acoustic pressure degree of freedom 8 for acoustic elements (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). Amplitude references can be used to prescribe time-varying boundary conditions in a direct-integration dynamic step. Default amplitude variations are described in “Defining an analysis,” Section 6.1.2. In direct time integration dynamic analysis, when a node with a prescribed motion is used in an equation constraint or a multi-point constraint to control the motion of another node, the equation or multi-point constraint will be imposed correctly for the displacement and velocity of the dependent node. However, the acceleration will not be rigorously transmitted to the dependent node, which may cause some high-frequency noise. In the subspace projection method it is not currently possible to specify nonzero boundary conditions directly. Instead, acceleration boundary conditions can be approximated by using appropriate combinations of large point masses and concentrated loads. At the node where such a boundary condition is desired, attach a large point mass that is approximatively 105 –106 times larger than the mass of the original model. In addition, a concentrated load of magnitude equal to the product between the large point mass and the desired acceleration must be specified in the direction of the approximated boundary condition. Since the point mass is significantly larger than the mass of the model, the big mass–concentrated load combination will approximate the desired acceleration in the specified direction accurately. Boundary conditions other than accelerations must be converted into acceleration histories before they can be approximated. Loads The following loads can be prescribed in a dynamic analysis: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” • Distributed pressure or volumetric accelerations (on acoustic elements) can be applied; these are described in “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1. Predefined fields The following predefined fields can be specified in a dynamic analysis, as described in “Predefined fields,” Section 33.6.1: • Although temperature is not a degree of freedom in stress/displacement elements, nodal temperatures can be specified as a predefined field. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any. • The values of user-defined field variables can be specified. These values only affect field-variable- dependent material properties, if any. Material options Most material models that describe mechanical behavior are available for use in a dynamic analysis. The following material properties are not active during a dynamic analysis: thermal properties (except for thermal expansion), mass diffusion properties, electrical conductivity properties, and pore fluid flow properties. Rate-dependent material properties (“Time domain viscoelasticity,” Section 22.7.1; “Hysteresis in elastomers,” Section 22.8.1; “Rate-dependent yield,” Section 23.2.3; and “Two-layer viscoplasticity,” Section 23.2.11) can be included in a dynamic analysis. Elements Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in Abaqus/Standard (including those with temperature, pressure, and electrical potential degrees of freedom) can be used in a dynamic analysis. Inertia effects are ignored in hydrostatic fluid elements, and the inertia of the fluid in pore pressure elements is not taken into account. Output In addition to the usual output variables available in Abaqus/Standard , the following variables are provided specifically for implicit dynamic analysis: Variables for a specified element set or for the entire model: Current coordinates of the center of mass. Coordinate n of the center of mass ( ). ). Displacement of the center of mass. Displacement component n of the center of mass ( Rotation component n of the center of mass. Equivalent rigid body velocity components. Component n of the equivalent rigid body velocity ( Component n of the equivalent rigid body angular velocity ( Angular momentum about the center of mass. Component n of the angular momentum about the center of mass ( Angular momentum about the origin. Component n of the angular momentum about the origin ( Rotary inertia about the origin. ). -component of the rotary inertia about the origin ( ). Mass. Current volume. 6.3.2–13 ). ). ). XC XCn UC UCn URCn VC VCn VRCn HC HCn HO HOn RI RIij MASS Input file template *HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS Data lines to specify initial conditions *AMPLITUDE, NAME=name Data lines to define amplitude variations ** *STEP (,NLGEOM) Once NLGEOM is specified, it will be active in all subsequent steps. *DYNAMIC Data line to control automatic time incrementation *BOUNDARY Data lines to describe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD and/or *INCIDENT WAVE Data lines to specify loads *TEMPERATURE and/or *FIELD Data lines to prescribe predefined fields *CECHARGE and/or *DECHARGE (if electrical potential degrees of freedom are active) Data lines to specify charges *END STEP Additional references • Czekanski, A., N. El-Abbasi, and S. A. Meguid, “Optimal Time Integration Parameters for Elastodynamic Contact Problems,” Communications in Numerical Methods in Engineering, vol. 17, pp. 379–384, 2001. • Hilber, H. M., T. J. R. Hughes, and R. L. Taylor, “Improved Numerical Dissipation for Time Integration Algorithms in Structural Dynamics,” Earthquake Engineering and Structural Dynamics, vol. 5, pp. 283–292, 1977. 6.3.3 EXPLICIT DYNAMIC ANALYSIS Products: Abaqus/Explicit Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • *DYNAMIC • “Configuring a dynamic, explicit procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview An explicit dynamic analysis: • is computationally efficient for the analysis of large models with relatively short dynamic response times and for the analysis of extremely discontinuous events or processes; • allows for the definition of very general contact conditions (“Contact interaction analysis: overview,” Section 35.1.1); • uses a consistent, deformation; large-deformation theory—models can undergo large rotations and large • can use a geometrically linear deformation theory—strains and rotations are assumed to be small ; • can be used to perform an adiabatic stress analysis if inelastic dissipation is expected to generate heat in the material ; • can be used to perform quasi-static analyses with complicated contact conditions; and • allows for either automatic or fixed time incrementation to be used—by default, Abaqus/Explicit uses automatic time incrementation with the global time estimator. Explicit dynamic analysis The explicit dynamics procedure performs a large number of small time increments efficiently. An explicit central-difference time integration rule is used; each increment is relatively inexpensive (compared to the direct-integration dynamic analysis procedure available in Abaqus/Standard) because there is no solution for a set of simultaneous equations. The explicit central-difference operator satisfies the dynamic equilibrium equations at the beginning of the increment, t; the accelerations calculated at time t are used to advance the velocity solution to time and the displacement solution to time . Input File Usage: Abaqus/CAE Usage: *DYNAMIC, EXPLICIT Step module: Create Step: General: Dynamic, Explicit Numerical implementation The explicit dynamics analysis procedure is based upon the implementation of an explicit integration rule together with the use of diagonal (“lumped”) element mass matrices. The equations of motion for the body are integrated using the explicit central-difference integration rule where is a degree of freedom (a displacement or rotation component) and the subscript i refers to the increment number in an explicit dynamics step. The central-difference integration operator is explicit in the sense that the kinematic state is advanced using known values of from the previous increment. and The explicit integration rule is quite simple but by itself does not provide the computational efficiency associated with the explicit dynamics procedure. The key to the computational efficiency of the explicit procedure is the use of diagonal element mass matrices because the accelerations at the beginning of the increment are computed by is the mass matrix, is the applied load vector, and where is the internal force vector. A lumped mass matrix is used because its inverse is simple to compute and because the vector multiplication of the mass inverse by the inertial force requires only n operations, where n is the number of degrees of freedom in the model. The explicit procedure requires no iterations and no tangent stiffness matrix. The internal force vector, , is assembled from contributions from the individual elements such that a global stiffness matrix need not be formed. Nodal mass and inertia The explicit integration scheme in Abaqus/Explicit requires nodal mass or inertia to exist at all activated degrees of freedom unless constraints are applied using boundary conditions. More precisely, a nonzero nodal mass must exist unless all activated translational degrees of freedom are constrained and nonzero rotary inertia must exist unless all activated rotational degrees of freedom are constrained. Nodes that are part of a rigid body do not require mass, but the entire rigid body must possess mass and inertia unless constraints are used. Nodes that belong to Eulerian elements also do not require mass, since the surrounding Eulerian elements may be void at some time during the simulation. When degrees of freedom at a node are activated by elements with a nonzero mass density (e.g., solid, shell, beam) or mass and inertia elements, a nonzero nodal mass or inertia occurs naturally from the assemblage of lumped mass contributions. When degrees of freedom at a node are activated by elements with no mass (e.g., spring, dashpot, or connector elements), care must be taken either to constrain the node or to add mass and inertia as appropriate. Stability The explicit procedure integrates through time by using many small time increments. The central- difference operator is conditionally stable, and the stability limit for the operator (with no damping) is given in terms of the highest frequency of the system as With damping, the stable time increment is given by is the fraction of critical damping in the mode with the highest frequency. Contrary to our where usual engineering intuition, introducing damping to the solution reduces the stable time increment. In Abaqus/Explicit a small amount of damping is introduced in the form of bulk viscosity to control high frequency oscillations. Physical forms of damping, such as dashpots or material damping, can also be introduced. Bulk viscosity and material damping are discussed below. Estimating the stable time increment size An approximation to the stability limit is often written as the smallest transit time of a dilatational wave across any of the elements in the mesh where of is the smallest element dimension in the mesh and , defined below. and In general, for beams, conventional shells, and membranes the element thickness or cross-sectional dimensions are not considered in determining the smallest element dimension; the stability limit is based upon the midplane or membrane dimensions only. When the transverse shear stiffness is defined for shell elements , the stable time increment will also be based on the transverse shear behavior. is the dilatational wave speed in terms This estimate for is only approximate and in most cases is not a conservative (safe) estimate. In general, the actual stable time increment chosen by Abaqus/Explicit will be less than this estimate by a factor between and 1 in a three-dimensional model. The time increment chosen by Abaqus/Explicit also accounts for any stiffness behavior in a model associated with penalty contact. For further discussion, see “Computational cost” below. and 1 in a two-dimensional model and between Stable time increment report Abaqus/Explicit writes a report to the status (.sta) file during the data check phase of the analysis that contains an estimate of the minimum stable time increment and a listing of the elements with the smallest stable time increments and their values. The initial stable time increments listed do not include damping (bulk viscosity), mass scaling, or penalty contact effects. This listing is provided because often a few elements have much smaller stability limits than the rest of the elements in the mesh. The stable time increment can be increased by modifying the mesh to increase the size of the controlling element or by using appropriate mass scaling. Dilatational wave speed The current dilatational wave speed, hypoelastic material moduli from the material’s constitutive response. Effective Lamé’s constants, and , is determined in Abaqus/Explicit by calculating the effective , are determined in the following manner. Define as the increment of volumetric strain, and as the increment in the mean stress, as the as the increment in the deviatoric stress, deviatoric strain increment. We assume a hypoelastic stress-strain rule of the form The effective moduli can then be computed as For shell elements defined by a shell cross-section that requires numerical integration , the effective moduli for the section are computed by integrating the effective moduli at the section points through the thickness. These effective moduli represent the element stiffness and determine the current dilatational wave speed in the element as where is the density of the material. modulus, E, and Poisson’s ratio, , by EXPLICIT DYNAMIC ANALYSIS and Time incrementation The time increment used in an analysis must be smaller than the stability limit of the central-difference operator. Failure to use a small enough time increment will result in an unstable solution. When the solution becomes unstable, the time history response of solution variables such as displacements will usually oscillate with increasing amplitudes. The total energy balance will also change significantly. If the model contains only one material type, the initial time increment is directly proportional to the size of the smallest element in the mesh. If the mesh contains uniform size elements but contains multiple material descriptions, the element with the highest wave speed will determine the initial time increment. In nonlinear problems—those with large deformations and/or nonlinear material response—the highest frequency of the model will continually change, which consequently changes the stability limit. Abaqus/Explicit has two strategies for time incrementation control: fully automatic time incrementation (where the code accounts for changes in the stability limit) and fixed time incrementation. Scaling the time increment To reduce the chance of a solution going unstable, you can adjust the stable time increment computed by Abaqus/Explicit by a constant scaling factor. This factor can be used to scale the default global time estimate, the element-by-element estimate, or the fixed time increment based on the initial element-by- element estimate; it cannot be used to scale a fixed time increment specified directly by you. Input File Usage: Use the following option to scale the stable time increment based on the global time estimate: *DYNAMIC, EXPLICIT, SCALE FACTOR=f Use the following option to scale the stable time increment based on the element-by-element estimate: *DYNAMIC, EXPLICIT, ELEMENT BY ELEMENT, SCALE FACTOR=f Use the following option to scale the stable time increment based on the fixed time increment on the initial element-by-element estimate: *DYNAMIC, EXPLICIT, FIXED TIME INCREMENTATION, SCALE FACTOR=f Abaqus/CAE Usage: Step module: Create Step: General: Dynamic, Explicit: Incrementation: Time scaling factor: f Automatic time incrementation The default time incrementation scheme in Abaqus/Explicit is fully automatic and requires no user intervention. Two types of estimates are used to determine the stability limit: element by element and global. An analysis always starts by using the element-by-element estimation method and may switch to the global estimation method under certain circumstances, as explained below. Element-by-element estimation In an analysis Abaqus/Explicit initially uses a stability limit based on the highest element frequency in the whole model. This element-by-element estimate is determined using the current dilatational wave speed in each element. The element-by-element estimate is conservative; it will give a smaller stable time increment than the true stability limit that is based upon the maximum frequency of the entire model. In general, constraints such as boundary conditions and kinematic contact have the effect of compressing the eigenvalue spectrum, and the element-by-element estimates do not take this into account. The concept of the stable time increment as the time required to propagate a dilatational wave across the smallest element dimension is useful for interpreting how the explicit procedure chooses the time increment when element-by-element stability estimation controls the time increment. As the step proceeds, the global stability estimate, if used, will make the time increment less sensitive to element size. Input File Usage: Abaqus/CAE Usage: *DYNAMIC, EXPLICIT, ELEMENT BY ELEMENT Step module: Create Step: General: Dynamic, Explicit: Incrementation: Stable increment estimator: Element-by-element Global estimation The stability limit will be determined by the global estimator as the step proceeds unless the element-by- element estimation method is specified, fixed time incrementation is specified, or one of the conditions explained below prevents the use of global estimation. The switch to the global estimation method occurs once the algorithm determines that the accuracy of the global estimation method is acceptable. The adaptive, global estimation algorithm determines the maximum frequency of the entire model using the current dilatational wave speed. This algorithm continuously updates the estimate for the maximum frequency. The global estimator will usually allow time increments that exceed the element- by-element values. Abaqus/Explicit monitors the effectiveness of the global estimation algorithm. If the cost for computing the global time estimate is more than its benefit, the code will turn off the global estimation algorithm and simply use the element-by-element estimates to save computation time. Conditions that will prevent the use of the global time estimator The global estimation algorithm will not be used when any of the following capabilities are included in the model: • Fluid elements • Infinite elements • Dashpots • Thick shells (thickness to characteristic length ratio larger than 0.92) • Thick beams (thickness to length ratio larger than 1.0) • The JWL equation of state • Material damping • Nonisotropic elastic materials with temperature and field variable dependency • Distortion control • Adaptive meshing • Subcycling “Improved” stable time increment for three-dimensional continuum elements and elements with plane stress formulations For three-dimensional continuum elements and elements with plane stress formulations (shell, membrane, and two-dimensional plane stress elements) an “improved” estimate of the element characteristic length is used by default. This “improved” method usually results in a larger element stable time increment than a more traditional method. For analyses using variable mass scaling, the total mass added to achieve a given stable time increment will be less with the improved estimate. Input File Usage: Abaqus/CAE Usage: Fixed time incrementation Use the following option to activate the “improved” element time estimation method: *DYNAMIC, EXPLICIT, IMPROVED DT METHOD=YES Use the following option to deactivate the “improved” element time estimation method: *DYNAMIC, EXPLICIT, IMPROVED DT METHOD=NO The ability to deactivate the “improved” element time estimation method is not supported in Abaqus/CAE. A fixed time incrementation scheme is also available in Abaqus/Explicit. The fixed time increment size is determined either by the initial element-by-element stability estimate for the step or by a user-specified time increment. Fixed time incrementation may be useful when a more accurate representation of the higher mode response of a problem is required. In this case a time increment size smaller than the element-by-element estimates may be used. The element-by-element estimate can be obtained simply by running a data check analysis . When fixed time incrementation is used, Abaqus/Explicit will not check that the computed response is stable during the step. You should ensure that a valid response has been obtained by carefully checking the energy history and other response variables. Basing the fixed time increment size on the initial element-by-element stability limit You can use time increments the size of the initial element-by-element stability limit throughout a step. The dilatational wave speed in each element at the beginning of the step is used to compute the fixed time increment size. Input File Usage: Abaqus/CAE Usage: *DYNAMIC, EXPLICIT, FIXED TIME INCREMENTATION Step module: Create Step: General: Dynamic, Explicit: Incrementation: Type: Fixed: Use element-by-element time increment estimator Specifying the fixed time increment size directly Alternatively, you can specify a time increment size directly. Input File Usage: Abaqus/CAE Usage: *DYNAMIC, EXPLICIT, DIRECT USER CONTROL Step module: Create Step: General: Dynamic, Explicit: Incrementation: Type: Fixed: User-defined time increment Advantages of the explicit method The use of small increments (dictated by the stability limit) is advantageous because it allows the solution to proceed without iterations and without requiring tangent stiffness matrices to be formed. It also simplifies the treatment of contact. The explicit dynamics procedure is ideally suited for analyzing high-speed dynamic events, but many of the advantages of the explicit procedure also apply to the analysis of slower (quasi-static) processes. A good example is sheet metal forming, where contact dominates the solution and local instabilities may form due to wrinkling of the sheet. The results in an explicit dynamics analysis are not automatically checked for accuracy as they are in Abaqus/Standard (Abaqus/Standard uses the half-increment residual). In most cases this is not of concern because the stability condition imposes a small time increment such that the solution changes only slightly in any one time increment, which simplifies the incremental calculations. While the analysis may take an extremely large number of increments, each increment is relatively inexpensive, often resulting in an economical solution. It is not uncommon for Abaqus/Explicit to take over 105 increments for an analysis. The method is, therefore, computationally attractive for problems where the total dynamic response time that must be modeled is only a few orders of magnitude longer than the stability limit; for example, wave propagation studies or some “event and response” applications. Computational cost The computer time involved in running a simulation using explicit time integration with a given mesh is proportional to the time period of the event. The time increment based on the element-by-element stability estimate can be rewritten (ignoring damping) in the form where the minimum is taken over all elements in the mesh, element , of the material in the element, and element (defined above). is a characteristic length associated with an is the density are the effective Lamé’s constants for the material in the and The time increment from the global stability estimate may be somewhat larger, but for this discussion we will assume that the above inequality always holds (when the inequality does not hold, the solution time will be somewhat faster). For linear, nonisotropic elastic materials this stability limit is further scaled down by the square root of the ratio of the effective material stiffness to the maximum material stiffness in one particular direction. Since this effectively means that the time increment can be no larger than the time required to propagate a stress wave across an element, the computer time involved in running a quasi-static analysis can be very large: the cost of the simulation is directly proportional to the number of time increments required. The number of increments, n, required is remains constant, where T is the time period of the event being simulated. (Even the element-by-element approximation of will not remain constant in general, since element distortion will change and nonlinear material response will change the effective Lamé constants. But the assumption is sufficiently accurate for the purposes of this discussion.) Thus, if In a two-dimensional analysis refining the mesh by a factor of two in each direction will increase the run time in the explicit procedure by a factor of eight—four times as many elements and half the original time increment size. Similarly, in a three-dimensional analysis refining the mesh by a factor of two in each direction will increase the run time by a factor of sixteen. In a quasi-static analysis it is expedient to reduce the computational cost by either speeding up the simulation or by scaling the mass. In either case the kinetic energy should be monitored to ensure that the ratio of kinetic energy to internal energy does not get too large—typically less than 10%. Reducing the computational cost by speeding up the simulation To reduce the number of increments required, n, we can speed up the simulation compared to the time of the actual process—that is, we can artificially reduce the time period of the event, T. This will introduce two possible errors. If the simulation speed is increased too much, the increased inertia forces will change the predicted response (in an extreme case the problem will exhibit wave propagation response). The only way to avoid this error is to choose a speed-up that is not too large. The other error is that some aspects of the problem other than inertia forces—for example, material behavior—may also be rate dependent. In this case the actual time period of the event being modeled cannot be changed. Reducing the computational cost by using mass scaling Artificially increasing the material density, , just like decreasing T to . This concept, called “mass scaling,” reduces the ratio of the event time to the time for wave propagation across an element while leaving the event time fixed, which allows rate-dependent behavior to be included in the analysis. Mass scaling has exactly the same effect on inertia forces as speeding up the time of simulation. reduces n to , by a factor Mass scaling is attractive because it can be used in rate-dependent problems, but it must be used with care to ensure that the inertia forces do not dominate and change the solution. Either fixed or variable mass scaling can be invoked . Mass scaling can also be accomplished by altering the density; however, the fixed and variable mass scaling capabilities provide more versatile methods of scaling the mass of the entire model or specific element sets in the model. Reducing the computational cost by using selective subcycling One disadvantage in an explicit dynamic analysis is that a few very small elements will force the entire model to be integrated with a small time increment. You can use mixed time integration or “subcycling” methods to reduce this problem. In these methods the equations of motion for the body are still integrated using the explicit central-difference integration rule as shown above, but the different time increments are allowed for different groups of nodes in the finite element model. If most nodes are integrated with a large stable time increment and only a few nodes are integrated with a small time increment, the computational cost may be reduced significantly. Selective subcycling can be invoked by defining the subcycling zones. See “Selective subcycling,” Section 11.7.1 for details. Bulk viscosity Bulk viscosity introduces damping associated with volumetric straining. Its purpose is to improve the modeling of high-speed dynamic events . Abaqus/Explicit contains two forms of bulk viscosity: linear and quadratic. Linear bulk viscosity is included by default in an Abaqus/Explicit analysis. The bulk viscosity parameters defined below can be redefined and can be changed from step to step. If the default values are changed in a step, the new values will be used in subsequent steps until they are redefined. Bulk viscosities defined this way apply to the whole model. For an individual element set the linear and quadratic bulk viscosities can be scaled by a factor by defining section controls . and Input File Usage: Abaqus/CAE Usage: Use the following option to define bulk viscosity for the entire model: *BULK VISCOSITY Use the following options to define bulk viscosity for an individual element set: *BULK VISCOSITY *SECTION CONTROLS Use the following option to define bulk viscosity for the entire model: Step module: Create Step: General: Dynamic, Explicit: Other: Linear bulk viscosity parameter and Quadratic bulk viscosity parameter Defining bulk viscosity for an individual element set is not supported in Abaqus/CAE. Linear bulk viscosity Linear bulk viscosity is found in all elements and is introduced to damp “ringing” in the highest element frequency. This damping is sometimes referred to as truncation frequency damping. It generates a bulk viscosity pressure that is linear in the volumetric strain rate where dilatational wave speed, is a damping coefficient (default=.06), is the current material density, is the current is an element characteristic length, and is the volumetric strain rate. For acoustic elements, the bulk viscosity pressure can be obtained from the above equation by using the relationship of the fluid particle velocity and the pressure rate as where and c are the pressure rate and the speed of sound in the fluid, respectively. Quadratic bulk viscosity The second form of bulk viscosity pressure is found only in solid continuum elements (except the plane stress element CPS4R). This form is quadratic in the volumetric strain rate where viscosity. Quadratic bulk viscosity is applied only if the volumetric strain rate is compressive. is a damping coefficient (default=1.2) and all other quantities are as defined for the linear bulk The quadratic bulk viscosity pressure will smear a shock front across several elements and is introduced to prevent elements from collapsing under extremely high velocity gradients. Consider a simple one-element problem in which the nodes on one side of the element are fixed and the nodes on the other side have an initial velocity in the direction of the fixed nodes. If the initial velocity is equal to the dilatational wave speed of the material, without the quadratic bulk viscosity, the element would collapse to zero volume in one time increment (because the stable time increment size is precisely the transit time of a dilatational wave across the element). The quadratic bulk viscosity pressure will introduce a resisting pressure that will prevent the element from collapsing. Fraction of critical damping due to bulk viscosity The bulk viscosity pressure is not included in the material point stresses because it is intended as a numerical effect only—it is not considered part of the material’s constitutive response. The bulk viscosity pressures are based upon the dilatational mode of each element. The fraction of critical damping in the dilatational mode of each element is given by Rotational bulk viscosity for shell elements For the displacement degrees of freedom, bulk viscosity introduces damping associated with volumetric straining. Linear bulk viscosity or truncation frequency damping is used to damp the high frequency ringing that leads to unwanted noise in the solution or spurious overshoot in the response amplitude. For the same reason, in shells the high frequency ringing in the rotational degrees of freedom is damped with linear bulk viscosity acting on the mean curvature strain rate. This damping generates a bulk viscosity “pressure moment,” m, which is linear in the mean curvature strain rate is a damping coefficient (default = 0.06), where is the current dilatational wave speed, L is the characteristic length used for rotary inertia and transverse shear stiffness scaling , and , where h is the current thickness, is added to the direct components of the moment resultant. is twice the mean curvature strain rate. The resultant pressure moment is the original thickness, is the mass density, Material damping Defining inelastic material behavior, dashpots, etc. will introduce energy dissipation into a model. In addition to these mechanisms, general (“Rayleigh”) material damping can be introduced . Adding damping to a model, especially stiffness proportional damping, , may significantly reduce the stable time increment. Input File Usage: Abaqus/CAE Usage: *DAMPING, ALPHA= Property module: material editor: Mechanical→Damping: Alpha and Beta , BETA= Obtaining diagnostic information about critical elements Abaqus/Explicit writes critical elements (elements with the smallest stable time increments) and their stable time increment values to the output database at each summary increment for visualization in Abaqus/CAE. By default, the number of critical elements written to the output database is 10. Input File Usage: Abaqus/CAE Usage: *DIAGNOSTICS, CRITICAL ELEMENTS=value The ability to control the number of critical elements written to the output database is not supported in Abaqus/CAE. Obtaining diagnostic information about the deformation speed The deformation speed in an element is defined as the largest absolute value of all the deformation rate components of an element times the element characteristic length, . You can request diagnostic information about the deformation speed within a step definition, as described below. In a multistep analysis diagnostic requests remain in effect until they are explicitly redefined. Deformation speed warnings By default, Abaqus/Explicit will check for a relatively large deformation speed in all the elements since too high a value may cause the element to deform or collapse unrealistically. A warning message is issued if the ratio of deformation speed versus dilatational wave speed in an element reaches the value specified for the “warning ratio.” By default, the warning ratio is 0.3. You can redefine this limit. The first occurrence of the warning message is written to the status (.sta) file; subsequent occurrences are written to the message (.msg) file. See “Output,” Section 4.1.1, for a description of these output files. Generally when the ratio of deformation speed to dilatational wave speed is greater than 0.3, it is an indication that the purely mechanical material constitutive relationship is no longer valid and that a thermo-mechanical equation of state material is required. Input File Usage: Abaqus/CAE Usage: *DIAGNOSTICS, WARNING RATIO=ratio The ability to redefine the warning ratio limit is not supported in Abaqus/CAE. Deformation speed errors An error message is issued and the analysis is terminated when the maximum ratio of deformation speed versus current dilatational wave speed for any element is greater than the “cutoff ratio.” By default, the cutoff ratio is 1.0. You can redefine this limit. The check for this cutoff ratio is not applied to any model that has an equation of state material or a user-defined material . Input File Usage: Abaqus/CAE Usage: *DIAGNOSTICS, CUTOFF RATIO=ratio The ability to redefine the cutoff ratio limit is not supported in Abaqus/CAE. Obtaining a summary of the deformation speed information You can request summary diagnostic information to obtain warning and error messages for only the element with the largest ratio of deformation speed to dilatational wave speed. Input File Usage: Abaqus/CAE Usage: *DIAGNOSTICS, DEFORMATION SPEED CHECK=SUMMARY A summary of the deformation speed diagnostic information is output by default in Abaqus/CAE. Obtaining detailed deformation speed information You can request detailed diagnostic information to obtain warning and error messages for all elements with large deformation speed to dilatational wave speed ratios. Input File Usage: Abaqus/CAE Usage: *DIAGNOSTICS, DEFORMATION SPEED CHECK=DETAIL You cannot output detailed diagnostic information about the deformation speed in Abaqus/CAE. Disabling deformation speed checks You can choose to completely bypass the checks for large deformation speed. Input File Usage: Abaqus/CAE Usage: *DIAGNOSTICS, DEFORMATION SPEED CHECK=OFF You cannot disable the deformation speed checks in Abaqus/CAE. Monitoring output variables for extreme values There are some analyses in which it is useful to monitor the value of a variable at every increment. For example, in a force-driven analysis such as hydro-forming, the simulation time that is sufficient to model the completion of the physical process may depend on the magnitude of the displacement of a node or a group of nodes in the model. Another example is a drop test simulation where the postfailure response is not of interest. Monitoring the values of critical variables and halting the analysis when those variables exceed a given criterion can reduce computational expense and turnaround time. For such problems Abaqus/Explicit allows output variables to be monitored during an analysis to verify whether or not their values have exceeded or fallen below user-specified values in specified element or node sets. Comparisons of specified element integration point variables, element section variables, or nodal variables with user-specified values are performed at every increment. At the first occurrence of a variable exceeding the user-specified bounds, the variable name, the associated element or node number, and the increment number are written to the status (.sta) file. In addition, you can request that the analysis be stopped and/or the output state be written in the increment following the one in which the variable has exceeded the user-specified bound. At the end of each step in which variables are monitored, the maximum, minimum, or absolute maximum value that each variable attains during the course of the analysis, along with the number of the element or node where the extreme value occurred, will be written to the status file. Defining the element and nodal variables to be monitored The element output variables that can be monitored include all the element integration point variables and element section point variables that are available for history-type output to the output database. Similarly, the nodal output variables that can be monitored include all the nodal variables that are available for history output to the output database. The keys identifying the output variables are defined in “Abaqus/Explicit output variable identifiers,” Section 4.2.2. Input File Usage: Use the first option with one or both of the following options in the history portion of the input file: *EXTREME VALUE *EXTREME ELEMENT VALUE, ELSET=element_set_name *EXTREME NODE VALUE, NSET=nset_set_name The *EXTREME VALUE option can be repeated in the same step, and the *EXTREME ELEMENT VALUE and *EXTREME NODE VALUE options can be repeated as many times as necessary. Abaqus/CAE Usage: Extreme value output monitoring is not supported in Abaqus/CAE. Halting the analysis when the extreme value criterion is met You can choose to halt the analysis when the extreme value criterion is met. The analysis will stop at the end of the increment following the one in which any of the specified element or nodal variables exceeded the prescribed bounds. Input File Usage: Use the following options: Abaqus/CAE Usage: *EXTREME VALUE, HALT=YES *EXTREME ELEMENT VALUE and/or *EXTREME NODE VALUE Extreme value output monitoring is not supported in Abaqus/CAE. Obtaining output when the extreme value criterion is met You can obtain field-type output to the output database and an additional restart state when any of the selected variables fall outside the specified bounds for the first time during the analysis. The output will be written in the increment following the one in which such an occurrence took place. Since output is automatically written when the analysis terminates, this request has an effect only if you have not chosen to halt the analysis when the extreme value criterion is met as described above. Input File Usage: Use either or both of the following options in conjunction with the *EXTREME VALUE option: *EXTREME ELEMENT VALUE, ELSET=element_set_name, OUTPUT=YES *EXTREME NODE VALUE, NSET=node_set_name, OUTPUT=YES Extreme value output monitoring is not supported in Abaqus/CAE. Abaqus/CAE Usage: Monitoring variables in a multistep analysis In a multistep analysis the monitoring requests you specify remain in effect until they are redefined. You must redefine all requests to add or change any variables, element or node sets, or maxima or minima. Stopping the monitoring of variables in a new step You can stop monitoring variables in a new step. Input File Usage: Abaqus/CAE Usage: Use the *EXTREME VALUE option without the *EXTREME ELEMENT VALUE and *EXTREME NODE VALUE options. Extreme value output monitoring is not supported in Abaqus/CAE. Initial conditions “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the initial conditions that are available for an explicit dynamic analysis. Boundary conditions Boundary conditions can be defined as explained in “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Boundary conditions applied during an explicit dynamic response step should use appropriate amplitude references (“Amplitude curves,” Section 33.1.2). If boundary conditions are specified for the step without amplitude references, they are applied instantaneously at the beginning of the step. Since Abaqus/Explicit does not admit jumps in displacement, the value of a nonzero displacement boundary condition that is specified without an amplitude reference will be ignored, and a zero velocity boundary condition will be enforced. Loads The loading types available for an explicit dynamic analysis are explained in “Applying loads: overview,” Section 33.4.1. Concentrated nodal forces or moments can be applied to the displacement or rotation degrees of freedom (1–6). Distributed pressure forces or body forces can also be applied; the distributed load types available with particular elements are described in Part VI, “Elements.” As with boundary conditions, loads applied during a dynamic response step should use appropriate amplitude references (“Amplitude curves,” Section 33.1.2). If loads are specified for the step without amplitude references, they are applied instantaneously at the beginning of the step. Predefined fields The following predefined fields can be specified, as described in “Predefined fields,” Section 33.6.1: • Although temperature is not a degree of freedom in explicit dynamic analysis, nodal temperatures can be specified. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any. • The values of user-defined field variables can be specified. These values affect only field-variable- dependent material properties, if any. Material options Any of the material models in Abaqus/Explicit can be used in a general explicit dynamic analysis . Elements All of the elements available in Abaqus/Explicit can be used in an explicit dynamic analysis. The elements are listed in Part VI, “Elements.” If coupled temperature-displacement elements are used in an explicit dynamic analysis, the temperature degrees of freedom will be ignored. Output The element output available for a dynamic analysis includes stress; strain; energies; and the values of state, field, and user-defined variables. The nodal output available includes displacements, velocities, accelerations, reaction forces, and coordinates. All of the output variable identifiers are outlined in “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The types of output available are described in “Output,” Section 4.1.1. When an Abaqus/Explicit analysis encounters a fatal error, the preselected variables applicable to the current procedure are added automatically to the output database as field data for the last increment. Energy output is particularly important in checking the accuracy of the solution in an explicit dynamic analysis. In general, the total energy (ETOTAL) should be a constant or close to a constant; the “artificial” energies, such as the artificial strain energy (ALLAE), the damping dissipation (ALLVD), and the mass scaling work (ALLMW) should be negligible compared to “real” energies such as the strain energy (ALLSE) and the kinetic energy (ALLKE). In a quasi-static analysis the value of the kinetic energy (ALLKE) should not exceed a small fraction of the value of the strain energy (ALLIE). It is a good practice to output the constraint penalty work (ALLCW) and the contact penalty work (ALLPW) in analyses involving constraints (such as ties and fasteners) and contact. The value of these energies should be close to zero. Input file template *HEADING … *MATERIAL, NAME=name *ELASTIC … *DENSITY Data lines to define density *DAMPING, ALPHA = , BETA= Data lines to define Rayleigh damping … *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS, TYPE=type Data lines to specify initial conditions *AMPLITUDE, NAME=name Data lines to define amplitude variations ************************* *STEP *DYNAMIC, EXPLICIT Data line to specify the time period of the step *DIAGNOSTICS, DEFORMATION SPEED CHECK=SUMMARY *BOUNDARY, AMPLITUDE=name Data lines to describe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD Data lines to specify loading *TEMPERATURE and/or *FIELD Data lines to specify predefined fields *FILE OUTPUT, NUMBER INTERVAL=n *EL FILE Data line specifying element output variables *NODE FILE Data line specifying node output variables *ENERGY FILE *OUTPUT, FIELD, NUMBER INTERVAL=n *ELEMENT OUTPUT Data line specifying element output variables *NODE OUTPUT Data line specifying node output variables *OUTPUT, HISTORY, TIME INTERVAL=t *ELEMENT OUTPUT, ELSET=element set name Data line specifying element output variables *NODE OUTPUT, NSET=node set name Data line specifying node output variables *ENERGY OUTPUT Data line specifying energy output variables *END STEP ************************* *STEP *DYNAMIC, EXPLICIT, ELEMENT BY ELEMENT … *BULK VISCOSITY Data line to define linear and/or quadratic bulk viscosity in this step … *END STEP 6.3.4 DIRECT-SOLUTION STEADY-STATE DYNAMIC ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Dynamic analysis procedures: overview,” Section 6.3.1 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 • “Subspace-based steady-state dynamic analysis,” Section 6.3.9 • “Defining an analysis,” Section 6.1.2 • “General and linear perturbation procedures,” Section 6.1.3 • *STEADY STATE DYNAMICS • “Configuring a direct-solution steady-state dynamic procedure” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating and modifying prescribed conditions,” Section 16.4 of the Abaqus/CAE User’s Manual Overview A direct-solution steady-state dynamic analysis: • is used to calculate the steady-state dynamic linearized response of a system to harmonic excitation; • is a linear perturbation procedure; • calculates the response directly in terms of the physical degrees of freedom of the model; • is an alternative to mode-based steady-state dynamic analysis, in which the response of the system is calculated on the basis of the eigenmodes; • is more expensive computationally than mode-based or subspace-based steady-state dynamics; • is more accurate than mode-based or subspace-based steady-state dynamics, in particular if significant frequency-dependent material damping or viscoelastic material behavior is present in the structure; and • is able to bias the excitation frequencies toward the approximate values that generate a response peak. Introduction Steady-state dynamic analysis provides the steady-state amplitude and phase of the response of a system due to harmonic excitation at a given frequency. Usually such analysis is done as a frequency sweep by applying the loading at a series of different frequencies and recording the response; in Abaqus/Standard the direct-solution steady-state dynamic procedure conducts this frequency sweep. In a direct-solution steady-state analysis the steady-state harmonic response is calculated directly in terms of the physical degrees of freedom of the model using the mass, damping, and stiffness matrices of the system. When defining a direct-solution steady-state dynamic step, you specify the frequency ranges of interest and the number of frequencies at which results are required in each range (including the bounding frequencies of the range). In addition, you can specify the type of frequency spacing (linear or logarithmic) to be used, as described below (“Selecting the frequency spacing”). Logarithmic frequency spacing is the default. Frequencies are given in cycles/time. Those frequency points for which results are required can be spaced equally along the frequency axis (on a linear or a logarithmic scale), or they can be biased toward the ends of the user-defined frequency range by introducing a bias parameter (described below). The direct-solution steady-state analysis procedure can be used in the following cases for which the eigenvalues cannot be extracted (and, thus, the mode-based steady-state dynamics procedures are not applicable): • for nonsymmetric stiffness; • when any form of damping other than modal damping must be included; and • when viscoelastic material properties must be taken into account. While the response in this procedure is linear, the prior response can be nonlinear. Initial stress effects (stress stiffening) as well as load stiffness effects will be included in the steady-state dynamics response if nonlinear geometric effects (“General and linear perturbation procedures,” Section 6.1.3) were included in any general analysis step prior to the direct-solution steady-state dynamic procedure. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, DIRECT Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct Ignoring damping If damping terms can be ignored, you can specify that a real, rather than a complex, system matrix be factored, which can significantly reduce computational time. Damping is discussed below. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, DIRECT, REAL ONLY Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: Compute real response only Selecting the type of frequency interval for which output is requested Three types of frequency intervals are permitted for output from a direct-solution steady-state dynamic step. If an eigenvalue extraction step precedes the direct-solution steady-state dynamic step, you can select either the range or the eigenfrequency type of frequency interval; otherwise, only the range type can be used. Dividing the specified frequency range using the user-defined number of points and the optional bias function For the range type of frequency interval (the default), the specified frequency range of interest is divided using the user-defined number of points and the optional bias function. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, DIRECT, INTERVAL=RANGE Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: toggle off Use eigenfrequencies to subdivide each frequency range Specifying the frequency ranges by using the system’s eigenfrequencies If the direct-solution steady-state dynamic analysis is preceded by an eigenfrequency extraction step, you can select the eigenfrequency type of frequency interval. The following intervals then exist in each frequency range: • First interval: extends from the lower limit of the frequency range given to the first eigenfrequency in the range. • Intermediate intervals: extend from eigenfrequency to eigenfrequency. • Last interval: extends from the highest eigenfrequency in the range to the upper limit of the frequency range. For each of these intervals the frequencies at which results are calculated are determined using the user- defined number of points (which includes the bounding frequencies for the interval) and the optional bias function. Figure 6.3.4–1 illustrates the division of the frequency range for 5 calculation points and a bias parameter equal to 1. Input File Usage: *STEADY STATE DYNAMICS, DIRECT, INTERVAL=EIGENFREQUENCY Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: Use eigenfrequencies to subdivide each frequency range frequency points lower end of the range mode n mode n +1 mode n + 2 upper end of the range Figure 6.3.4–1 Division of range for the eigenfrequency type of interval and 5 calculation points. Specifying the frequency ranges by the frequency spread If the direct-solution steady-state dynamic analysis is preceded by an eigenfrequency extraction In this case intervals exist around each step, you can select the spread type of frequency interval. eigenfrequency in the frequency range. For each of the intervals the equally spaced frequencies at which results are calculated are determined using the user-defined number of points (which includes the bounding frequencies for the interval). The minimum number of frequency points is 3. If the user-defined value is less than 3 (or omitted), the default value of 3 points is assumed. Figure 6.3.4–2 illustrates the division of the frequency range for 5 calculation points. The bias parameter is not supported with the spread type of frequency interval. Frequency points Frequency points fn fn + 1 (1 – spread) · fn (1 + spread) · fn (1 – spread) · fn + 1 (1 + spread) · fn + 1 Figure 6.3.4–2 Division of range for the spread type of interval and 5 calculation points. and are eigenfrequencies of the system. Input File Usage: *STEADY STATE DYNAMICS, DIRECT, INTERVAL=SPREAD lwr_freq, upr_freq, numpts, bias_param, freq_scale_factor, spread Abaqus/CAE Usage: You cannot specify frequency ranges by frequency spread in Abaqus/CAE. Selecting the frequency spacing Two types of frequency spacing are permitted for a direct-solution steady-state dynamic step. For the logarithmic frequency spacing (the default), the specified frequency ranges of interest are divided using a logarithmic scale. Alternatively, a linear frequency spacing can be used if a linear scale is desired. Input File Usage: Use either of the following options: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, DIRECT, FREQUENCY SCALE=LOGARITHMIC *STEADY STATE DYNAMICS, DIRECT, FREQUENCY SCALE=LINEAR Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: Scale: Logarithmic or Linear Requesting multiple frequency ranges You can request multiple frequency ranges or multiple single frequency points for a direct-solution steady-state dynamic step. Input File Usage: *STEADY STATE DYNAMICS, DIRECT lwr_freq1, upr_freq1, numpts1, bias_param1, freq_scale_factor1 lwr_freq2, upr_freq2, numpts2, bias_param2, freq_scale_factor2 ... single_freq1 single_freq2 ... Repeat the data lines as often as necessary. Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: Data: enter data in table, and add rows as necessary The bias parameter The bias parameter can be used to provide closer spacing of the results points either toward the middle or toward the ends of each frequency interval. Figure 6.3.4–3 shows a few examples of the effect of the bias parameter on the frequency spacing. frequency points f1 Bias parameter = 1 f2 Bias parameter = 2 Bias parameter = 3 Bias parameter = 5 Figure 6.3.4–3 Effect of the bias parameter on the frequency spacing for a number of points . The bias formula used in direct-solution steady-state dynamics is where ; ); is the number of frequency points at which results are to be given; is one such frequency point ( is the lower limit of the frequency range; is the upper limit of the range; is the frequency at which the kth results are given; is the bias parameter value; and is the frequency or the logarithm of the frequency, depending on the value chosen for the frequency scale. A bias parameter, p, that is greater than 1.0 provides closer spacing of the results points toward the ends of the frequency interval, while values of p that are less than 1.0 provide closer spacing toward the middle of the frequency interval. The default bias parameter is 1.0 for a range frequency interval and 3.0 for an eigenfrequency interval. The frequency scale factor The frequency scale factor can be used to scale frequency points. All the frequency points, except the lower and upper limit of the frequency range, are multiplied by this factor. This scale factor can be used only when the frequency interval is specified by using the system’s eigenfrequencies . Damping If damping is absent, the response of a structure will be unbounded if the forcing frequency is equal to an eigenfrequency of the structure. To get quantitatively accurate results, especially near natural frequencies, accurate specification of damping properties is essential. The various damping options available are discussed in “Material damping,” Section 26.1.1. In direct-solution steady-state dynamics damping can be created by the following: • dashpots , • “Rayleigh” damping associated with materials and elements Section 26.1.1), , • structural damping , and • viscoelasticity included in the material definitions . When a real-only system matrix is factored, all forms of damping are ignored, including quiet boundaries on infinite elements and nonreflecting boundaries on acoustic elements. Contact conditions with sliding friction Abaqus/Standard automatically detects the contact nodes that are slipping due to velocity differences imposed by the motion of the reference frame or the transport velocity in prior steps. At those nodes the tangential degrees of freedom are not constrained and the effect of friction results in an unsymmetric contribution to the stiffness matrix. At other contact nodes the tangential degrees of freedom are constrained. Friction at contact nodes at which a velocity differential is imposed can give rise to damping terms. There are two kinds of friction-induced damping effects. The first effect is caused by the friction forces stabilizing the vibrations in the direction perpendicular to the slip direction. This effect exists only in three-dimensional analysis. The second effect is caused by a velocity-dependent friction coefficient. If the friction coefficient decreases with velocity (which is usually the case), the effect is destabilizing and is also known as “negative damping.” For more details, see “Coulomb friction,” Section 5.2.3 of the Abaqus Theory Manual. Direct-solution steady-state dynamics analysis allows you to include these friction-induced contributions to the damping matrix. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, DIRECT, FRICTION DAMPING=YES Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: Include friction-induced damping effects Initial conditions The base state is the current state of the model at the end of the last general analysis step prior to the steady-state dynamic step. If the first step of an analysis is a perturbation step, the base state is determined from the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Initial condition definitions that directly define solution variables, such as velocity, cannot be used in a steady-state dynamic analysis. Boundary conditions In a steady-state dynamic analysis the real and imaginary parts of any degree of freedom are either restrained or unrestrained simultaneously; it is physically impossible to have one part restrained and the other part unrestrained. Abaqus/Standard will automatically restrain both the real and imaginary parts of a degree of freedom even if only one part is prescribed specifically. The unspecified part will be assumed to have a perturbation magnitude of zero. Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6) in a direct-solution steady-state analysis. See “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. These boundary conditions will vary sinusoidally with time. You specify the real (in-phase) part of a boundary condition and the imaginary (out-of-phase) part of a boundary condition separately. Input File Usage: Use either of the following options to define the real (in-phase) part of the boundary condition: *BOUNDARY *BOUNDARY, REAL Abaqus/CAE Usage: Use the following option to define the imaginary (out-of-phase) part of the boundary condition: *BOUNDARY, IMAGINARY Load module: boundary condition editor: real (in-phase) part + imaginary (out-of-phase) part i Frequency-dependent boundary conditions An amplitude definition can be used to specify the amplitude of a boundary condition as a function of frequency (“Amplitude curves,” Section 33.1.2). Input File Usage: Abaqus/CAE Usage: Use both of the following options: *AMPLITUDE, NAME=name *BOUNDARY, REAL or IMAGINARY, AMPLITUDE=name Load or Interaction module: Create Amplitude: Name: name Load module: boundary condition editor: real (in-phase) part + imaginary (out-of-phase) part i: Amplitude: name Loads The following loads can be prescribed in a steady-state dynamic analysis: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” • Incident wave loads can be applied; see “Acoustic and shock loads,” Section 33.4.6. These loads are assumed to vary sinusoidally with time over a user-specified range of frequencies. Loads are given in terms of their real and imaginary components. Coriolis distributed loading adds an imaginary antisymmetric contribution to the overall system of equations. This contribution is currently accounted for in solid and truss elements only and is activated by using the unsymmetric matrix storage and solution scheme for the step (“Defining an analysis,” Section 6.1.2). Incident wave loads can be used to model sound waves from distinct planar or spherical sources or from diffuse fields. Fluid flux loading cannot be used in a steady-state dynamic analysis. Input File Usage: Use any of the following options to define the real (in-phase) part of the load: *CLOAD or *DLOAD *CLOAD or *DLOAD, REAL Use either of the following options to define the imaginary (out-of-phase) part of the load: *CLOAD or *DLOAD, IMAGINARY Abaqus/CAE Usage: Load module: part i load editor: real (in-phase) part + imaginary (out-of-phase) Frequency-dependent loading An amplitude definition can be used to specify the amplitude of a load as a function of frequency (“Amplitude curves,” Section 33.1.2). Input File Usage: Use both of the following options: *AMPLITUDE, NAME=name *CLOAD or *DLOAD, REAL or IMAGINARY, AMPLITUDE=name Load or Interaction module: Create Amplitude: Name: name Load module: part i: Amplitude: name load editor: real (in-phase) part + imaginary (out-of-phase) Abaqus/CAE Usage: Predefined fields Predefined temperature fields can be specified in direct-solution steady-state dynamic analysis and will produce harmonically varying thermal strains if thermal expansion is included in the material definition (“Thermal expansion,” Section 26.1.2). Other predefined fields are ignored. Material options As in any dynamic analysis procedure, mass or density (“Density,” Section 21.2.1) must be assigned to some regions of any separate parts of the model where dynamic response is required. If an analysis is desired in which the inertia effects are neglected, the density should be set to a very small number. The following material properties are not active during steady-state dynamic analyses: plasticity and other inelastic effects, thermal properties (except for thermal expansion), mass diffusion properties, electrical properties (except for the electrical potential, , in piezoelectric analysis), and pore fluid flow properties—see “General and linear perturbation procedures,” Section 6.1.3. Viscoelastic effects can be included in direct-solution steady-state harmonic response analysis. The linearized viscoelastic response is considered to be a perturbation about a nonlinear preloaded state, which is computed on the basis of purely elastic behavior (long-term response) in the viscoelastic components. Therefore, the vibration amplitude must be sufficiently small so that the material response in the dynamic phase of the problem can be treated as a linear perturbation about the predeformed state. Viscoelastic frequency domain response is described in “Frequency domain viscoelasticity,” Section 22.7.2. Elements Any of the following elements available in Abaqus/Standard can be used in a steady-state dynamic procedure: • stress/displacement elements (other than generalized axisymmetric elements with twist); • acoustic elements; • piezoelectric elements; or • hydrostatic fluid elements. See “Choosing the appropriate element for an analysis type,” Section 27.1.3. Output In direct-solution steady-state dynamic analysis the value of an output variable such as strain (E) or stress (S) is a complex number with real and imaginary components. In the case of data file output the first printed line gives the real components while the second lists the imaginary components. Results and data file output variables are also provided to obtain the magnitude and phase of many variables . In the case of data file output the first printed line gives the magnitudes while the second lists the phase angle. The following variables are provided specifically for steady-state dynamic analysis: Element integration point variables: PHS PHE PHEPG PHEFL PHMFL PHMFT Magnitude and phase angle of all stress components. Magnitude and phase angle of all strain components. Magnitude and phase angles of the electrical potential gradient vector. Magnitude and phase angles of the electrical flux vector. Magnitude and phase angle of the mass flow rate in fluid link elements. Magnitude and phase angle of the total mass flow in fluid link elements. For connector elements, the following element output variables are available: PHCTF PHCEF PHCVF PHCRF PHCSF PHCU PHCCU PHCV PHCA Nodal variables: PU PPOR PHPOT PRF PHCHG Magnitude and phase angle of connector total forces. Magnitude and phase angle of connector elastic forces. Magnitude and phase angle of connector viscous forces. Magnitude and phase angle of connector reaction forces. Magnitude and phase angle of connector friction forces. Magnitude and phase angle of connector relative displacements. Magnitude and phase angle of connector constitutive displacements. Magnitude and phase angle of connector relative velocities. Magnitude and phase angle of connector relative accelerations. Magnitude and phase angle of all displacement/rotation components at a node. Magnitude and phase angle of the fluid, pore, or acoustic pressure at a node. Magnitude and phase angle of the electrical potential at a node. Magnitude and phase angle of all reaction forces/moments at a node. Magnitude and phase angle of the reactive charge at a node. Element energy densities (such as the elastic strain energy density, SENER) and whole element energies (such as the total kinetic energy of an element, ELKE) are not available for output in a direct- solution steady-state dynamic analysis. Whole model variables such as ALLIE (total strain energy) are available for direct-solution steady- state dynamic analysis by requesting energy output to the data, results, or output database files . Input file template *HEADING … *AMPLITUDE, NAME=loadamp Data lines to define an amplitude curve as a function of frequency (cycles/time) ** *STEP, NLGEOM Include the NLGEOM parameter so that stress stiffening effects will be included in the steady-state dynamic step *STATIC **Any general analysis procedure can be used to preload the structure … *CLOAD and/or *DLOAD Data lines to prescribe preloads *TEMPERATURE and/or *FIELD Data lines to define values of predefined fields for preloading the structure *BOUNDARY Data lines to specify boundary conditions to preload the structure … *END STEP ** *STEP *STEADY STATE DYNAMICS, DIRECT Data lines to specify frequency ranges and bias parameters *BOUNDARY, REAL Data lines to specify real (in-phase) boundary conditions *BOUNDARY, IMAGINARY Data lines to specify imaginary (out-of-phase) boundary conditions *CLOAD, AMPLITUDE=loadamp Data lines to specify sinusoidally varying, frequency-dependent, concentrated loads *CLOAD and/or *DLOAD Data lines to specify sinusoidally varying loads … *END STEP 6.3.5 NATURAL FREQUENCY EXTRACTION Products: Abaqus/Standard Abaqus/CAE Abaqus/AMS References • “Defining an analysis,” Section 6.1.2 • “General and linear perturbation procedures,” Section 6.1.3 • “Dynamic analysis procedures: overview,” Section 6.3.1 • *FREQUENCY • “Configuring a frequency procedure” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The frequency extraction procedure: • performs eigenvalue extraction to calculate the natural frequencies and the corresponding mode shapes of a system; • will include initial stress and load stiffness effects due to preloads and initial conditions if geometric nonlinearity is accounted for in the base state, so that small vibrations of a preloaded structure can be modeled; • will compute residual modes if requested; • is a linear perturbation procedure; • can be performed using the traditional Abaqus software architecture or, if appropriate, the high- performance SIM architecture ; and • solves the eigenfrequency problem only for symmetric mass and stiffness matrices; the complex eigenfrequency solver must be used if unsymmetric contributions, such as the load stiffness, are needed. Eigenvalue extraction The eigenvalue problem for the natural frequencies of an undamped finite element model is where is the mass matrix (which is symmetric and positive definite); is the stiffness matrix (which includes initial stiffness effects if the base state included the effects of nonlinear geometry); is the eigenvector (the mode of vibration); and are degrees of freedom. M and N is positive definite, all eigenvalues are positive. Rigid body modes and instabilities When cause Instabilities produce to be indefinite. Rigid body modes produce zero eigenvalues. negative eigenvalues and occur when you include initial stress effects. Abaqus/Standard solves the eigenfrequency problem only for symmetric matrices. Selecting the eigenvalue extraction method Abaqus/Standard provides three eigenvalue extraction methods: • Lanczos • Automatic multi-level substructuring (AMS), an add-on analysis capability for Abaqus/Standard • Subspace iteration In addition, you must consider the software architecture that will be used for the subsequent modal superposition procedures. The choice of architecture has minimal impact on the frequency extraction procedure, but the SIM architecture can offer significant performance improvements over the traditional architecture for subsequent mode-based steady-state or transient dynamic procedures . The architecture that you use for the frequency extraction procedure is used for all subsequent mode-based linear dynamic procedures; you cannot switch architectures during an analysis. The software architectures used by the different eigensolvers are outlined in Table 6.3.5–1. Table 6.3.5–1 Software architectures available with different eigensolvers. Eigensolver Lanczos AMS Subspace Iteration Software Architecture Traditional SIM The Lanczos solver with the traditional architecture is the default eigenvalue extraction method because it has the most general capabilities. However, the Lanczos method is generally slower than the AMS method. The increased speed of the AMS eigensolver is particularly evident when you require a large number of eigenmodes for a system with many degrees of freedom. However, the AMS method has the following limitations: • All restrictions imposed on SIM-based linear dynamic procedures also apply to mode-based linear dynamic analyses based on mode shapes computed by the AMS eigensolver. See “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1, for details. • The AMS eigensolver does not compute composite modal damping factors, participation factors, or modal effective masses. However, if participation factors are needed for primary base motions, they will be computed but are not written to the printed data (.dat) file. • You cannot use the AMS eigensolver in an analysis that contains piezoelectric elements. • You cannot request output to the results (.fil) file in an AMS frequency extraction step. If your model has many degrees of freedom and these limitations are acceptable, you should use the AMS eigensolver. Otherwise, you should use the Lanczos eigensolver. The Lanczos eigensolver and the subspace iteration method are described in “Eigenvalue extraction,” Section 2.5.1 of the Abaqus Theory Manual. Lanczos eigensolver For the Lanczos method you need to provide the maximum frequency of interest or the number of eigenvalues required; Abaqus/Standard will determine a suitable block size (although you can override If you specify both the maximum frequency of interest and the number of this choice, if needed). eigenvalues required and the actual number of eigenvalues is underestimated, Abaqus/Standard will issue a corresponding warning message; the remaining eigenmodes can be found by restarting the frequency extraction. You can also specify the minimum frequencies of interest; Abaqus/Standard will extract eigenvalues until either the requested number of eigenvalues has been extracted in the given range or all the frequencies in the given range have been extracted. See “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1, for information on using the SIM architecture with the Lanczos eigensolver. Input File Usage: Abaqus/CAE Usage: *FREQUENCY, EIGENSOLVER=LANCZOS Step module: Step→Create: Frequency: Basic: Eigensolver: Lanczos Choosing a block size for the Lanczos method In general, the block size for the Lanczos method should be as large as the largest expected multiplicity of eigenvalues (that is, the largest number of modes with the same frequency). A block size larger than 10 is not recommended. If the number of eigenvalues requested is n, the default block size is the minimum of (7, n). The choice of 7 for block size proves to be efficient for problems with rigid body modes. The number of block Lanczos steps within each Lanczos run is usually determined by Abaqus/Standard but can be changed by you. In general, if a particular type of eigenproblem converges slowly, providing more block Lanczos steps will reduce the analysis cost. On the other hand, if you know that a particular type of problem converges quickly, providing fewer block Lanczos steps will reduce the amount of in-core memory used. The default values are Block size Maximum number of block Lanczos steps ≥ 4 80 50 45 35 Automatic multi-level substructuring (AMS) eigensolver For the AMS method you need only specify the maximum frequency of interest (the global frequency), and Abaqus/Standard will extract all the modes up to this frequency. You can also specify the minimum frequencies of interest and/or the number of requested modes. However, specifying these values will not affect the number of modes extracted by the eigensolver; it will affect only the number of modes that are stored for output or for a subsequent modal analysis. , , and The execution of the AMS eigensolver can be controlled by specifying three parameters: . These three parameters multiplied by the maximum (default value of 5) controls the cutoff frequency of interest define three cutoff frequencies. frequency for substructure eigenproblems in the reduction phase, while (default values of 1.7 and 1.1, respectively) control the cutoff frequencies used to define a starting subspace in the reduced eigensolution phase. Generally, increasing the value of and and improves the accuracy of the results but may affect the performance of the analysis. Requesting eigenvectors at all nodes By default, the AMS eigensolver computes eigenvectors at every node of the model. Input File Usage: Abaqus/CAE Usage: *FREQUENCY, EIGENSOLVER=AMS Step module: Step→Create: Frequency: Basic: Eigensolver: AMS Requesting eigenvectors only at specified nodes Alternatively, you can specify a node set, and eigenvectors will be computed and stored only at the nodes that belong to that node set. The node set that you specify must include all nodes at which loads are applied or output is requested in any subsequent modal analysis (this includes any restarted analysis). If element output is requested or element-based loading is applied, the nodes attached to the associated elements must also be included in this node set. Computing eigenvectors at only selected nodes improves performance and reduces the amount of stored data. Therefore, it is recommended that you use this option for large problems. Input File Usage: Abaqus/CAE Usage: *FREQUENCY, EIGENSOLVER=AMS, NSET=name Step module: Step→Create: Frequency: Basic: Eigensolver: AMS: Limit region of saved eigenvectors Controlling the AMS eigensolver The AMS method consists of the following three phases: • Reduction phase: In this phase Abaqus/Standard uses a multi-level substructuring technique to reduce the full system in a way that allows a very efficient eigensolution of the reduced system. The approach combines a sparse factorization based on a multi-level supernode elimination tree and a local eigensolution at each supernode. Starting from the lowest level supernodes, we use a Craig-Bampton substructure reduction technique to successively reduce the size of the system as we progress upward in the elimination tree. At each supernode a local eigensolution is obtained based on fixing the degrees of freedom connected to the next higher level supernode (these are the local retained or “fixed-interface” degrees of freedom). At the end of the reduction phase the full system has been reduced such that the reduced stiffness matrix is diagonal and the reduced mass matrix has unit diagonal values but contains off-diagonal blocks of nonzero values representing the coupling between the supernodes. The cost of the reduction phase depends on the system size and the number of eigenvalues extracted (the number of eigenvalues extracted is controlled indirectly by specifying the highest eigenfrequency desired). You can make trade-offs between cost and accuracy during the reduction phase through the parameter. This parameter multiplied by the highest eigenfrequency specified for the full model yields the highest eigenfrequency that is extracted in the local supernode eigensolutions. Increasing the value of increases the accuracy of the reduction since more local eigenmodes are retained. However, increasing the number of retained modes also increases the cost of the reduced eigensolution phase, which is discussed next. • Reduced eigensolution phase: In this phase Abaqus/Standard computes the eigensolution of the reduced system that comes from the previous phase. Although the reduced system typically is two orders of magnitude smaller in size than the original system, generally it still is too large to solve directly. Thus, the system is further reduced mainly by truncating the retained eigenmodes and then solved using a single subspace iteration step. The two AMS parameters, and , define a starting subspace of the subspace iteration step. The default values of these parameters are carefully chosen and provide accurate results in most cases. When a more accurate solution is needed, the recommended procedure is to increase both parameters proportionally from their respective default values. • Recovery phase: eigenvectors of the reduced problem and local substructure modes. specified nodes, the eigenvectors are computed only at those nodes. In this phase the eigenvectors of the original system are recovered using If you request recovery at Subspace iteration method For the subspace iteration procedure you need only specify the number of eigenvalues required; If the subspace iteration Abaqus/Standard chooses a suitable number of vectors for the iteration. technique is requested, you can also specify the maximum frequency of interest; Abaqus/Standard extracts eigenvalues until either the requested number of eigenvalues has been extracted or the last frequency extracted exceeds the maximum frequency of interest. Input File Usage: Abaqus/CAE Usage: *FREQUENCY, EIGENSOLVER=SUBSPACE Step module: Step→Create: Frequency: Basic: Eigensolver: Subspace Structural-acoustic coupling In Abaqus only the Structural-acoustic coupling affects the natural frequency response of systems. Lanczos eigensolver fully includes this effect. In Abaqus/AMS and the subspace eigensolver the effect of coupling is neglected for the purpose of computing the modes and frequencies; these are computed using natural boundary conditions at the structural-acoustic coupling surface. An intermediate degree of consideration of the structural-acoustic coupling operator is the default in Abaqus/AMS and the Lanczos eigensolver, which is based on the SIM architecture: the coupling is projected onto the modal space and stored for later use. Structural-acoustic coupling using the Lanczos eigensolver without the SIM architecture If structural-acoustic coupling is present in the model and the Lanczos method not based on the SIM architecture is used, Abaqus/Standard extracts the coupled modes by default. Because these modes fully account for coupling, they represent the mathematically optimal basis for subsequent modal procedures. The effect is most noticeable in strongly coupled systems such as steel shells and water. However, coupled structural-acoustic modes cannot be used in subsequent random response or response spectrum analyses. You can define the coupling using either acoustic-structural interaction elements or the surface-based tie constraint . It is possible to ignore coupling when extracting acoustic and structural modes; in this case the coupling boundary is treated as traction-free on the structural side and rigid on the acoustic side. Input File Usage: Use the following option to account for structural-acoustic coupling during the frequency extraction: *FREQUENCY, EIGENSOLVER=LANCZOS, ACOUSTIC COUPLING=ON (default if the SIM architecture is not used) Use the following option to ignore structural-acoustic coupling during the frequency extraction: *FREQUENCY, EIGENSOLVER=LANCZOS, ACOUSTIC COUPLING=OFF Abaqus/CAE Usage: Step module: Step→Create: Frequency: Basic: Eigensolver: Lanczos, toggle Include acoustic-structural coupling where applicable Structural-acoustic coupling using the AMS and Lanczos eigensolver based on the SIM architecture For frequency extractions that use the AMS eigensolver or the Lanczos eigensolver based on the SIM architecture, the modes are computed using traction-free boundary conditions on the structural side of the coupling boundary and rigid boundary conditions on the acoustic side. Structural-acoustic coupling operators are projected by default onto the subspace of eigenvectors. Contributions to these global operators, which come from surface-based tie constraints defined between structural and acoustic surfaces, are assembled into global matrices that are projected onto the mode shapes and used in subsequent SIM-based modal dynamic procedures. User-defined acoustic-structural interaction elements cannot be used in an AMS eigenvalue extraction analysis. Input File Usage: Use either of the following options to project structural-acoustic coupling operators onto the subspace of eigenvectors: Abaqus/CAE Usage: *FREQUENCY, EIGENSOLVER=AMS, ACOUSTIC COUPLING=PROJECTION (default for the AMS eigensolver) or *FREQUENCY, EIGENSOLVER=LANCZOS, SIM, ACOUSTIC COUPLING=PROJECTION (default in SIM-based analysis) Use the following option to disable the projection of structural-acoustic coupling operators: *FREQUENCY, ACOUSTIC COUPLING=OFF Use the following option to project structural-acoustic coupling operators onto the subspace of eigenvectors: Step module: Step→Create: Frequency: Basic: Eigensolver: AMS, toggle on Project acoustic-structural coupling where applicable Use the following option to disable the projection of structural-acoustic coupling operators: Step module: Step→Create: Frequency: Basic: Eigensolver: AMS, toggle off Project acoustic-structural coupling where applicable Projection of structural-acoustic coupling operators using the Lanczos eigensolver based on the SIM architecture is not supported in Abaqus/CAE. Specifying a frequency range for the acoustic modes Because structural-acoustic coupling is ignored during the AMS and SIM-based Lanczos eigenanalysis, the computed resonances will, in principle, be higher than those of the fully coupled system. This may be understood as a consequence of neglecting the mass of the fluid in the structural phase and vice versa. For the common metal and air case, the structural resonances may be relatively unaffected; however, some acoustic modes that are significant in the coupled response may be omitted due to the air’s upward frequency shift during eigenanalysis. Therefore, Abaqus allows you to specify a multiplier, so that the maximum acoustic frequency in the analysis is taken to be higher than the structural maximum. Input File Usage: Use either of the following options: *FREQUENCY, EIGENSOLVER=AMS , , , , , , acoustic range factor or *FREQUENCY, EIGENSOLVER=LANCZOS, SIM , , , , , , acoustic range factor Abaqus/CAE Usage: Step module: Step→Create: Frequency: Basic: Eigensolver: AMS, Acoustic range factor: acoustic range factor Specifying a frequency range for the acoustic modes when using the SIM-based Lanczos eigenanalysis is not supported in Abaqus/CAE. Effects of fluid motion on natural frequency analysis of acoustic systems To extract natural frequencies from an acoustic-only or coupled structural-acoustic system in which fluid motion is prescribed using an acoustic flow velocity, either the Lanczos method or the complex eigenvalue extraction procedure can be used. In the former case Abaqus extracts real-only eigenvalues and considers the fluid motion’s effects only on the acoustic stiffness matrix. Thus, these results are of primary interest as a basis for subsequent linear perturbation procedures. When the complex eigenvalue extraction procedure is used, the fluid motion effects are included in their entirety; that is, the acoustic stiffness and damping matrices are included in the analysis. Frequency shift For the Lanczos and subspace iteration eigensolvers you can specify a positive or negative shifted squared frequency, S. This feature is useful when a particular frequency is of concern or when the natural frequencies of an unrestrained structure or a structure that uses secondary base motions (large mass approach) are needed. In the latter case a shift from zero (the frequency of the rigid body modes) will avoid singularity problems or round-off errors for the large mass approach; a negative frequency shift is normally used. The default is no shift. If the Lanczos eigensolver is in use and the user-specified shift is outside the requested frequency range, the shift will be adjusted automatically to a value close to the requested range. Normalization For the Lanczos and subspace iteration eigensolvers both displacement and mass eigenvector normalization are available. Displacement normalization is the default. Mass normalization is the only option available for SIM-based natural frequency extraction. The choice of eigenvector normalization type has no influence on the results of subsequent modal dynamic steps . The normalization type determines only the manner in which the eigenvectors are represented. In addition to extracting the natural frequencies and mode shapes, the Lanczos and subspace iteration eigensolvers automatically calculate the generalized mass, the participation factor, the effective mass, and the composite modal damping for each mode; therefore, these variables are available for use in subsequent linear dynamic analyses. The AMS eigensolver computes only the generalized mass. Displacement normalization If displacement normalization is selected, the eigenvectors are normalized so that the largest displacement entry in each vector is unity. If the displacements are negligible, as in a torsional mode, the eigenvectors are normalized so that the largest rotation entry in each vector is unity. In a coupled acoustic-structural extraction, if the displacements and rotations in a particular eigenvector are small when compared to the acoustic pressures, the eigenvector is normalized so that the largest acoustic pressure in the eigenvector is unity. The normalization is done before the recovery of dependent degrees of freedom that have been previously eliminated with multi-point constraints or equation constraints. Therefore, it is possible that such degrees of freedom may have values greater than unity. Input File Usage: Abaqus/CAE Usage: *FREQUENCY, NORMALIZATION=DISPLACEMENT Step module: Step→Create: Frequency: Other: Normalize eigenvectors by: Displacement Mass normalization Alternatively, the eigenvectors can be normalized so that the generalized mass for each vector is unity. The “generalized mass” associated with mode is (no sum on ) is the structure’s mass matrix and where and M refer to degrees of freedom of the finite element model. is the eigenvector for mode . The superscripts N If the eigenvectors are normalized with respect to mass, all the eigenvectors are scaled so that =1. For coupled acoustic-structural analyses, an acoustic contribution fraction to the generalized mass is computed as well. Input File Usage: Abaqus/CAE Usage: *FREQUENCY, NORMALIZATION=MASS Step module: Step→Create: Frequency: Other: Normalize eigenvectors by: Mass Modal participation factors The participation factor for mode , is a variable that indicates how strongly motion in the global x-, y-, or z-direction or rigid body rotation about one of these axes is represented in the eigenvector of that mode. The six possible rigid body motions are indicated by , 6. The participation factor is defined as in direction i, , 2, where defines the magnitude of the rigid body response of degree of freedom N in the model to imposed rigid body motion (displacement or infinitesimal rotation) of type i. For example, at a node with three displacement and three rotation components, is (no sum on ) where is unity and all other are zero; x, y, and z are the coordinates of the node; and , and represent the coordinates of the center of rotation. The participation factors are, thus, defined for the translational degrees of freedom and for rotation around the center of rotation. For coupled acoustic- structural eigenfrequency analysis, an additional acoustic participation factor is computed as outlined in “Coupled acoustic-structural medium analysis,” Section 2.9.1 of the Abaqus Theory Manual. , Modal effective mass The effective mass for mode associated with kinematic direction i ( , 2, , 6) is defined as (no sum on ) If the effective masses of all modes are added in any global translational direction, the sum should give the total mass of the model (except for mass at kinematically restrained degrees of freedom). Thus, if the effective masses of the modes used in the analysis add up to a value that is significantly less than the model’s total mass, this result suggests that modes that have significant participation in a certain excitation direction have not been extracted. For coupled acoustic-structural eigenfrequency analysis, an additional acoustic effective mass is computed as outlined in “Coupled acoustic-structural medium analysis,” Section 2.9.1 of the Abaqus Theory Manual. Composite modal damping You can define composite damping factors for each material (“Material damping,” Section 26.1.1), which are assembled into fractions of critical damping values for each mode, , according to (no sum on ) where mass matrix made of material a. is the critical damping fraction given for material a and is the part of the structure’s A composite damping value will be calculated for each mode. These values are weighted damping values based on each material’s participation in each mode. Input File Usage: Abaqus/CAE Usage: *DAMPING, COMPOSITE Property module: Material→Create: Mechanical→Damping: Composite Obtaining residual modes for use in mode-based procedures Several analysis types in Abaqus/Standard are based on the eigenmodes and eigenvalues of the system. For example, in a mode-based steady-state dynamic analysis the mass and stiffness matrices and load vector of the physical system are projected onto a set of eigenmodes resulting in a diagonal system in terms of modal amplitudes (or generalized degrees of freedom). The solution to the physical system is obtained by scaling each eigenmode by its corresponding modal amplitude and superimposing the results (for more information, see “Linear dynamic analysis using modal superposition,” Section 2.5.3 of the Abaqus Theory Manual). Due to cost, usually only a small subset of the total possible eigenmodes of the system are extracted, with the subset consisting of eigenmodes corresponding to eigenfrequencies that are close to the excitation frequency. Since excitation frequencies typically fall in the range of the lower modes, it is usually the higher frequency modes that are left out. Depending on the nature of the loading, the accuracy of the modal solution may suffer if too few higher frequency modes are used. Thus, a trade-off exists between accuracy and cost. To minimize the number of modes required for a sufficient degree of accuracy, the set of eigenmodes used in the projection and superposition can be augmented with additional modes known as residual modes. The residual modes help correct for errors introduced In Abaqus/Standard a residual mode, R, represents the static response of the by mode truncation. structure subjected to a nominal (or unit) load, P, corresponding to the actual load that will be used in the mode-based analysis orthogonalized against the extracted eigenmodes, followed by an orthogonalization of the residual modes against each other. This orthogonalization is required to retain the orthogonality properties of the modes (residual and eigen) with respect to mass and stiffness. As a consequence of the mass and stiffness matrices being available, the orthogonalization can be done efficiently during the frequency extraction. Hence, if you wish to include residual modes in subsequent mode-based procedures, you must activate the residual mode calculations in the frequency extraction step. If the static responses are linearly dependent on each other or on the extracted eigenmodes, Abaqus/Standard automatically eliminates the redundant responses for the purpose of computing the residual modes. For the Lanczos eigensolver you must ensure that the static perturbation response of the load that will be applied in the subsequent mode-based analysis (i.e., ) is available by specifying that load in a static perturbation step immediately preceding the frequency extraction step. If multiple load cases are specified in this static perturbation analysis, one residual mode is calculated for each load case; otherwise, it is assumed that all loads are part of a single load case, and only one residual mode will be calculated. When residual modes are requested, the boundary conditions applied in the frequency extraction step must match those applied in the preceding static perturbation step. In addition, in the immediately preceding static perturbation step Abaqus/Standard requires that (1) if multiple load cases are used, the boundary conditions applied in each load case must be identical, and (2) the boundary condition magnitudes are zero. When generating dynamic substructures , residual modes usually will provide the most benefit if the loading patterns defined in each of the load cases in the preceding static perturbation step match the loading patterns defined under the corresponding substructure load cases in the substructure generation step. If you use the AMS eigensolver, you do not need to specify the loads in a preceding static perturbation step. Residual modes are computed at all degrees of freedom at which a concentrated load is applied in the following mode-based procedure. You can request additional residual modes by specifying degrees of freedom. One residual mode is computed for every requested degree of freedom. As an outcome of the orthogonalization process, a pseudo-eigenvalue corresponding to each residual mode, , is computed and given by (no sum on ) Henceforth, and in other Abaqus/Standard documentation, the term eigenvalue is used generally to refer to actual eigenvalues and pseudo-eigenvalues. All data (e.g., participation factors, etc.; see “Output”) associated with the modes (eigenmodes and residual modes) are ordered by increasing eigenvalue. Therefore, both eigenmodes and residual modes are assigned mode numbers. In the printed output file Abaqus/Standard clearly identifies which modes are eigenmodes and which modes are residual modes so that you can easily distinguish between them. By default, if you activate residual modes, all the calculated eigenmodes and residual modes will be used in subsequent mode-based procedures, unless: • You choose to obtain a new set of eigenmodes and residual modes in a new frequency extraction step. • You choose to select a subset of the available eigenmodes and residual modes in the mode-based procedure (selection of modes is described in each of the mode-based analysis type sections). Residual modes cannot be calculated if the cyclic symmetric modeling capability is used. In addition, the Lanczos or AMS eigensolver must be used if you wish to activate residual mode calculations. Input File Usage: Abaqus/CAE Usage: *FREQUENCY, RESIDUAL MODES Step module: Step→Create: Frequency: Basic: Include residual modes Evaluating frequency-dependent material properties When frequency-dependent material properties are specified, Abaqus/Standard offers the option of choosing the frequency at which these properties are evaluated for use in the frequency extraction procedure. This evaluation is necessary because the stiffness cannot be modified during the eigenvalue If you do not choose the frequency, Abaqus/Standard evaluates the stiffness extraction procedure. associated with frequency-dependent springs and dashpots at zero frequency and does not consider the stiffness contributions from frequency domain viscoelasticity. If you do specify a frequency, only the real part of the stiffness contributions from frequency domain viscoelasticity is considered. Evaluating the properties at a specified frequency is particularly useful in analyses in which the eigenfrequency extraction step is followed by a subspace projection steady-state dynamic step . In these analyses the eigenmodes extracted in the frequency extraction step are used as global basis functions to compute the steady-state dynamic response of a system subjected to harmonic excitation at a number of output frequencies. The accuracy of the results in the subspace projection steady-state dynamic step is improved if you choose to evaluate the material properties at a frequency in the vicinity of the center of the range spanned by the frequencies specified for the steady-state dynamic step. Input File Usage: Abaqus/CAE Usage: *FREQUENCY, PROPERTY EVALUATION=frequency Step module: Step→Create: Frequency: Other: Evaluate dependent properties at frequency Initial conditions If the frequency extraction procedure is the first step in an analysis, the initial conditions form the base state for the procedure (except for initial stresses, which cannot be included in the frequency extraction if it is the first step). Otherwise, the base state is the current state of the model at the end of the last general analysis step (“General and linear perturbation procedures,” Section 6.1.3). Initial stress stiffness effects (specified either through defining initial stresses or through loading in a general analysis step) will be included in the eigenvalue extraction only if geometric nonlinearity is considered in a general analysis procedure prior to the frequency extraction procedure. If initial stresses must be included in the frequency extraction and there is not a general nonlinear step prior to the frequency extraction step, a “dummy” static step—which includes geometric nonlinearity and which maintains the initial stresses with appropriate boundary conditions and loads—must be included before the frequency extraction step. “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the available initial conditions. Boundary conditions Nonzero magnitudes of boundary conditions in a frequency extraction step will be ignored; the degrees of freedom specified will be fixed (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). Boundary conditions defined in a frequency extraction step will not be used in subsequent general analysis steps (unless they are respecified). In a frequency extraction step involving piezoelectric elements, the electric potential degree of freedom must be constrained at least at one node to remove numerical singularities arising from the dielectric part of the element operator. Defining primary and secondary bases for modal superposition procedures If displacements or rotations are to be prescribed in subsequent dynamic modal superposition procedures, boundary conditions must be applied in the frequency extraction step; these degrees of freedom are grouped into “bases.” The bases are then used for prescribing motion in the modal superposition procedure—see “Transient modal dynamic analysis,” Section 6.3.7. Boundary conditions defined in the frequency extraction step supersede boundary conditions defined in previous steps. Hence, degrees of freedom that were fixed prior to the frequency extraction step will be associated with a specific base if they are redefined with reference to such a base in the frequency extraction step. The primary base By default, all degrees of freedom listed for a boundary condition will be assigned to an unnamed “primary” base. If the same motion will be prescribed at all fixed points, the boundary condition is defined only once; and all prescribed degrees of freedom belong to the primary base. Unless removed in the frequency extraction step, boundary conditions from the last general analysis step become fixed boundary conditions for the frequency step and belong to the primary base. If all rigid body motions are not suppressed by the boundary conditions that make up the primary base, you must apply a suitable frequency shift to avoid numerical problems. Input File Usage: *BOUNDARY The *BOUNDARY option without the BASE NAME parameter can appear only once in a frequency extraction step. Abaqus/CAE Usage: Load module: Create Boundary Condition Secondary bases If the modal superposition procedure will have more than one independent base motion, the driven nodes must be grouped together into “secondary” bases in addition to the primary base. The secondary bases must be named. Secondary bases are used only in modal dynamic and steady-state dynamic (not direct) procedures. The degrees of freedom associated with secondary bases are not suppressed; instead, a “big” mass is added to each of them. To provide six digits of numerical accuracy, Abaqus/Standard sets each “big” mass equal to 106 times the total mass of the structure and each “big” rotary inertia equal to 106 times the total moment of inertia of the structure. Hence, an artificial low frequency mode is introduced for every degree of freedom in a secondary base. To keep the requested range of frequencies unchanged, Abaqus/Standard automatically increases the number of eigenvalues extracted. Consequently, the cost of the eigenvalue extraction step will increase as more degrees of freedom are included in the secondary bases. To reduce the analysis cost, keep the number of degrees of freedom associated with secondary bases to a minimum. This can sometimes be done by reducing several secondary bases that all have the same prescribed motion to a single node by using BEAM type MPCs (“General multi-point constraints,” Section 34.2.2). For the Lanczos and subspace iteration methods a negative shift must be used with either the rigid body modes or secondary bases. The “big” masses are not included in the model statistics, and the total mass of the structure and the printed messages about masses and inertia for the entire model are not affected. However, the presence of the masses will be noticeable in the output tables printed for the eigenvalue extraction step, as well as in the information for the generalized masses and effective masses. See “Double cantilever subjected to multiple base motions,” Section 1.4.12 of the Abaqus Benchmarks Manual, for an example of the use of the base motion feature. More than one secondary base can be defined by repeating the boundary condition definition and assigning different base names. Input File Usage: Abaqus/CAE Usage: *BOUNDARY, BASE NAME=name Load module; Create Boundary Condition; Step: frequency_step; Category: Mechanical; Types for Selected Step: Secondary base; Constrained degrees-of-freedom: Region: select region, U1, U2, U3, UR1, UR2, and/or UR3 Loads Applied loads (“Applying loads: overview,” Section 33.4.1) are ignored during a frequency extraction analysis. If loads were applied in a previous general analysis step and geometric nonlinearity was considered for that prior step, the load stiffness determined at the end of the previous general analysis step is included in the eigenvalue extraction (“General and linear perturbation procedures,” Section 6.1.3). Predefined fields Predefined fields cannot be prescribed during natural frequency extraction. Material options The density of the material must be defined (“Density,” Section 21.2.1). The following material properties are not active during a frequency extraction: plasticity and other inelastic effects, rate-dependent material properties, thermal properties, mass diffusion properties, electrical properties (although piezoelectric materials are active), and pore fluid flow properties—see “General and linear perturbation procedures,” Section 6.1.3. Elements Other than generalized axisymmetric elements with twist, any of the stress/displacement or acoustic elements in Abaqus/Standard (including those with temperature, pressure, or electrical degrees of freedom) can be used in a frequency extraction procedure. Output The eigenvalues (EIGVAL), eigenfrequencies in cycles/time (EIGFREQ), generalized masses (GM), composite modal damping factors (CD), participation factors for displacement degrees of freedom 1–6 (PF1–PF6) and acoustic pressure (PF7), and modal effective masses for displacement degrees of freedom 1–6 (EM1–EM6) and acoustic pressure (EM7) are written automatically to the output database as history data. Output variables such as stress, strain, and displacement (which represent mode shapes) are also available for each eigenvalue; these quantities are perturbation values and represent mode shapes, not absolute values. The eigenvalues and corresponding frequencies (in both radians/time and cycles/time) will also be automatically listed in the printed output file, along with the generalized masses, composite modal damping factors, participation factors, and modal effective masses. The only energy density available in eigenvalue extraction procedures is the elastic strain energy density, SENER. All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. The AMS eigensolver does not compute composite modal damping factors, participation factors, or modal effective masses. In addition, you cannot request output to the results (.fil) file. You can restrict output to the results, data, and output database files by selecting the modes for which output is desired . Input File Usage: Use one of the following options: *EL FILE, MODE, LAST MODE *EL PRINT, MODE, LAST MODE *OUTPUT, MODE LIST Step module: Output→Field Output Requests→Create: Frequency: Specify modes Abaqus/CAE Usage: Input file template *HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS Data lines to specify initial conditions ** *STEP (,NLGEOM) If NLGEOM is used, initial stress and preload stiffness effects will be included in the frequency extraction step *STATIC … *CLOAD and/or *DLOAD Data lines to specify loads *TEMPERATURE and/or *FIELD Data lines to specify values of predefined fields *BOUNDARY Data lines to specify zero-valued or nonzero boundary conditions *END STEP ** *STEP, PERTURBATION *STATIC … *LOAD CASE, NAME=load case name Keywords and data lines to define loading for this load case *END LOAD CASE … *END STEP** *STEP *FREQUENCY, EIGENSOLVER=LANCZOS, RESIDUAL MODES Data line to control eigenvalue extraction *BOUNDARY *BOUNDARY, BASE NAME=name Data lines to assign degrees of freedom to a secondary base *END STEP 6.3.6 COMPLEX EIGENVALUE EXTRACTION Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “General and linear perturbation procedures,” Section 6.1.3 • *COMPLEX FREQUENCY • “Configuring a complex frequency procedure” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The complex eigenvalue extraction procedure: • performs eigenvalue extraction to calculate the complex eigenvalues and the corresponding complex mode shapes of a system; • is a linear perturbation procedure; • requires that an eigenfrequency extraction procedure (“Natural frequency extraction,” Section 6.3.5) be performed prior to the complex eigenvalue extraction; • can use the high-performance SIM software architecture ; • will include initial stress and load stiffness effects due to preloads and initial conditions if nonlinear geometric effects are included in the base state step definition (“General and linear perturbation procedures,” Section 6.1.3); • can include friction, damping, and unsymmetric load stiffness contributions; • can include unsymmetric damping and stiffness contributions in acoustic finite elements due to underlying mean flow (“Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1); and • cannot be used in a model defined as a cyclic symmetric structure (“Analysis of models that exhibit cyclic symmetry,” Section 10.4.3). Complex eigenvalue extraction the complex The complex eigenvalue extraction procedure uses a projection method to extract eigenvalues of the current system. The eigenvalue problem of the finite element model is formulated in the following manner: where M and N is the mass matrix (which is symmetric and, in general, is semi-positive definite); is the damping matrix; is the stiffness matrix (which can include initial stress stiffness and friction effects and, therefore, in general is unsymmetric); is the complex eigenvalue; is the complex eigenvector (the mode of vibration); and are degrees of freedom. The complex eigenvalue extraction procedure in Abaqus/Standard uses a subspace projection method; thus, the eigenmodes of the undamped system with the symmetrized stiffness matrix must be extracted using the eigenfrequency extraction procedure prior to the complex eigenvalue extraction step. By default, the entire subspace is used as the base vector; this subspace can be reduced as described below. Abaqus/Standard always computes all the complex eigenmodes available in the projection subspace (taking into account any user-specified modifications to the subspace). The user-specified number of requested eigenmodes and frequency range for the complex eigenvalue extraction procedure do not influence the number of computed complex eigenmodes. It determines only the number of reported modes, which cannot be higher than the dimension of the projected subspace. To modify the number of computed eigenmodes, reduce the projection subspace as described below or change the number of eigenmodes extracted in the prior natural frequency extraction step accordingly. If you do not specify the number of requested complex modes or the frequency range, all the computed modes will be reported. To take into account the unsymmetric effects, the unsymmetric matrix solution and storage scheme is used automatically for a complex eigenvalue extraction step. The unsymmetric effects will be disregarded if you specify that the symmetric solution and storage scheme should be used . Input File Usage: *COMPLEX FREQUENCY number of complex eigenmodes, frequency_min, frequency_max Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Complex frequency: Number of eigenvalues requested: All or Value, Minimum frequency of interest (cycles/time): value, Maximum frequency of interest (cycles/time): value Shift point You can specify a shift point, S, in cycles per time, for the complex eigenvalue extraction procedure (S ≥ 0). Abaqus/Standard reports the complex eigenmodes, so that the modes with the imaginary part closest to a given shift point are reported first. This feature is useful when a particular frequency range is of concern. The default is no shift. , in order of increasing Input File Usage: Abaqus/CAE Usage: *COMPLEX FREQUENCY , , , S Step module: Create Step: Linear perturbation: Complex frequency: Frequency shift (cycles/time): S Selecting the eigenmodes on which to project You can select eigenmodes of the undamped system with the symmetrized stiffness matrix on which the subspace projection will be performed. You can select them by specifying the mode numbers individually, by requesting that Abaqus/Standard generate the mode numbers automatically, or If you do not select the by requesting the eigenmodes that belong to specified frequency ranges. eigenmodes, all modes extracted in the prior eigenfrequency extraction step are used in the modal superposition. Input File Usage: Use one of the following options to select the eigenmodes by specifying mode numbers: *SELECT EIGENMODES, DEFINITION=MODE NUMBERS *SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS Use the following option to define the eigenmodes by specifying a frequency range: *SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE You cannot select the eigenmodes in Abaqus/CAE; all modes extracted are used in the subspace projection. Abaqus/CAE Usage: Evaluating frequency-dependent material properties When frequency-dependent material properties are specified, Abaqus/Standard offers the option of choosing the frequency at which these properties are evaluated for use in the complex eigenvalue extraction procedure. This evaluation is necessary because the operators cannot be modified during the eigenvalue extraction procedure. If you do not choose the frequency, Abaqus/Standard evaluates the stiffness and damping associated with frequency-dependent springs and dashpots at zero frequency and does not consider the stiffness and damping contributions from frequency-domain viscoelasticity. If you do specify a frequency, the stiffness and damping contributions from frequency-domain viscoelasticity are considered. Input File Usage: Abaqus/CAE Usage: *COMPLEX FREQUENCY, PROPERTY EVALUATION=frequency Step module: Create Step: Complex Frequency: Other: Evaluate dependent properties at frequency: value Contact conditions with sliding friction Abaqus/Standard automatically detects the contact nodes that are slipping due to velocity differences imposed by the motion of the reference frame or the transport velocity in prior steps. At those nodes the tangential degrees of freedom will not be constrained and the effect of friction will result in an unsymmetric contribution to the stiffness matrix. At other nodes in contact the tangential degrees of freedom will be constrained. Friction at contact nodes at which a velocity differential is imposed can give rise to damping terms. There are two kinds of friction-induced damping effects. The first effect is caused by the friction forces stabilizing the vibrations in the direction perpendicular to the slip direction. This effect exists only in three-dimensional analysis. The second effect is caused by a velocity-dependent friction coefficient. If the friction coefficient decreases with velocity (which is usually the case), the effect is destabilizing and is also known as “negative damping.” For more details, see “Coulomb friction,” Section 5.2.3 of the Abaqus Theory Manual. The complex eigensolver allows you to include these friction-induced contributions to the damping matrix. Input File Usage: Abaqus/CAE Usage: *COMPLEX FREQUENCY, FRICTION DAMPING=YES Step module: Create Step: Linear perturbation: Complex frequency: Include friction-induced damping effects Damping In complex eigenvalue extraction analysis damping can be defined by dashpots , by “Rayleigh” damping associated with materials and elements , and by quiet boundaries on infinite elements or acoustic elements. In addition, as described in “Contact conditions with sliding friction” above, friction-induced damping can be included. Structural damping, damping contributions from frequency-domain viscoelasticity, and all types of modal damping (except composite modal damping) are supported in complex eigenvalue extraction using the high-performance SIM architecture. Prescribing motion, transport velocity, and acoustic flow velocity Motion, transport velocity, and acoustic flow velocity affect complex frequency analyses. Motion and transport velocity must be specified in a preceding steady-state transport general step, and their effects are included in the complex frequency step. The acoustic flow velocity has no effect in steady-state transport steps, and acoustic flow velocities specified in a steady-state transport step are not propagated to perturbation steps. The acoustic flow velocity must be specified in each linear perturbation step where it is desired. Initial conditions Initial conditions cannot be specified for complex eigenvalue extraction. Boundary conditions Boundary conditions cannot be defined during complex eigenvalue extraction. The boundary conditions will be the same as in the prior natural frequency extraction analysis. Loads Applied loads (“Applying loads: overview,” Section 33.4.1) are ignored during a complex eigenvalue extraction. If loads were applied in a previous general analysis step in which nonlinear geometric effects were included, the load stiffness determined at the end of the previous general analysis step is included in the complex eigenvalue extraction . Coriolis distributed loading adds an unsymmetric contribution to the damping operator, which is currently accounted for only in solid and truss elements. Predefined fields Predefined fields cannot be prescribed during complex eigenvalue extraction. Material options The density of the material must be defined . The following material properties are not active during complex eigenvalue extraction: • plasticity and other inelastic effects; • rate-dependent material properties, excluding friction, which can be rate dependent if the velocity differential on the contact interface exists; • thermal properties; • mass diffusion properties; • electrical properties (although piezoelectric materials are active); and • pore fluid flow properties. Elements Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in Abaqus/Standard (including those with temperature or pressure degrees of freedom) can be used in complex eigenvalue extraction. Output ); frequencies The real (EIGREAL) and imaginary (EIGIMAG) parts of the eigenvalues, ( in cycles/time (EIGFREQ); and effective damping ratios (DAMPRATIO = ) are written automatically to the data (.dat) file and to the output database (.odb) file as history data. In addition, you can request that the generalized displacements (GU), which are the modes of the projected system, be written to the output database file . Output variables such as stress, strain, and displacement (which represent mode shapes) are also available for each eigenvalue; these quantities are perturbation values and represent mode shapes, not absolute values. and The only energy density available in eigenvalue extraction procedures is the elastic strain energy density, SENER. All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. You can restrict output to the data file and output database file by selecting the modes for which output is desired or “Output to the output database,” Section 4.1.3). Output to the results (.fil) file is not available for the complex eigenvalue extraction procedure. Setting the cutoff value for complex eigenmodes You can also set the cutoff value for complex eigenmodes, so only complex modes with the real part of the eigenvalue higher than the cutoff value are written to the output database file. The default cutoff value is 0.0. If the cutoff value is not set, all complex modes are output. Input File Usage: Use one of the following options to select complex eigenmodes for output: *COMPLEX FREQUENCY, UNSTABLE MODES ONLY *COMPLEX FREQUENCY, UNSTABLE MODES ONLY=value The SIM architecture The complex eigenvalue extraction analysis can be performed using the SIM architecture. The advantages of performing the complex eigenvalue extraction procedure using the SIM architecture are as follows: • structural damping, including damping defined with viscoelastic material, is taken into account; • modal damping can be specified; • matrices representing the stiffness, mass, and damping can be defined (both symmetric and unsymmetric matrices are supported); and • the AMS eigensolver can be used to generate the projection subspace for the complex eigenvalue extraction. When the AMS eigensolver is used for computing the projection subspace, you should increase the accuracy of the AMS eigensolution by increasing the values of the AMS parameters and by increasing the highest frequency of interest. The coupled structural-acoustic modes cannot be used in complex eigenvalue extraction analysis based on the SIM architecture. Input file template *HEADING … *SURFACE INTERACTION *FRICTION Specify zero friction coefficient *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS Data lines to specify initial conditions ** *STEP (,NLGEOM) If NLGEOM is used, initial stress and preload stiffness effects will be included in the eigenvalue extraction steps *STATIC … *CLOAD and/or *DLOAD Data lines to specify loads *TEMPERATURE and/or *FIELD Data lines to specify values of predefined fields *BOUNDARY Data lines to specify zero-valued or nonzero boundary conditions *END STEP ** *STEP(,NLGEOM) *STATIC Data line to define incrementation *CHANGE FRICTION *FRICTION Data lines to redefine friction coefficient *MOTION, ROTATION or TRANSLATION Data lines to define the velocity differential *END STEP ** *STEP *FREQUENCY Data line to control eigenvalue extraction *END STEP ** *STEP *COMPLEX FREQUENCY Data line to control complex eigenvalue extraction *SELECT EIGENMODES Data lines to define applicable mode ranges *END STEP 6.3.7 TRANSIENT MODAL DYNAMIC ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “General and linear perturbation procedures,” Section 6.1.3 • “Dynamic analysis procedures: overview,” Section 6.3.1 • *MODAL DYNAMIC • “Configuring a modal dynamics procedure” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A modal dynamic analysis: • is used to analyze transient linear dynamic problems using modal superposition; • can be performed only after a frequency extraction procedure since it bases the structure’s response on the modes of the system; • can use the high-performance SIM software architecture ; • can include nondiagonal damping effects (i.e., from material or element damping) only when using the SIM architecture; and • is a linear perturbation procedure. Modal dynamic analysis Transient modal dynamic analysis gives the response of the model as a function of time based on a given time-dependent loading. The structure’s response is based on a subset of the modes of the system, which must first be extracted using an eigenfrequency extraction procedure (“Natural frequency extraction,” Section 6.3.5). The modes will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. The number of modes extracted must be sufficient to model the dynamic response of the system adequately, which is a matter of judgment on your part. The modal amplitudes are integrated through time, and the response is synthesized from these modal responses. For linear systems the modal dynamic procedure is much less expensive computationally than the direct integration of the entire system of equations performed in the dynamic procedure (“Implicit dynamic analysis using direct integration,” Section 6.3.2). As long as the system is linear and is represented correctly by the modes being used (which are generally only a small subset of the total modes of the finite element model), the method is also very accurate because the integration operator used is exact whenever the forcing functions vary piecewise linearly with time. You should ensure that the forcing function definition and the choice of time increment are consistent for this purpose. For example, if the forcing is a seismic record in which acceleration values are given every millisecond and it is assumed that the acceleration varies linearly between these values, the time increment used in the modal dynamic procedure should be a millisecond. The user-specified maximum number of increments is ignored in a modal dynamic step. The number of increments is based on both the time increment and the total time chosen for the step. While the response in this procedure is for linear vibrations, the prior response can be nonlinear and stress stiffening (initial stress) effects will be included in the response if nonlinear geometric effects were included in the step definition for the base state of the eigenfrequency extraction procedure, as explained in “Natural frequency extraction,” Section 6.3.5. Selecting the modes and specifying damping You can select the modes to be used in modal superposition and specify damping values for all selected modes. Selecting the modes You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard generate the mode numbers automatically, or by requesting the modes that belong to specified frequency ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step, including residual modes if they were activated, are used in the modal superposition. Input File Usage: Use one of the following options to select the modes by specifying mode numbers: *SELECT EIGENMODES, DEFINITION=MODE NUMBERS *SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS Use the following option to select the modes by specifying a frequency range: *SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE You cannot select the modes in Abaqus/CAE; all modes extracted are used in the modal superposition. Abaqus/CAE Usage: Specifying modal damping Damping is almost always specified for a mode-based procedure; see “Material damping,” Section 26.1.1. You can define a damping coefficient for all or some of the modes used in the response calculation. The damping coefficient can be given for a specified mode number or for a specified frequency range. When damping is defined by specifying a frequency range, the damping coefficient for a mode is interpolated linearly between the specified frequencies. The frequency range can be discontinuous; the average damping value will be applied for an eigenfrequency at a discontinuity. The damping coefficients are assumed to be constant outside the range of specified frequencies. Input File Usage: Use the following option to define damping by specifying mode numbers: *MODAL DAMPING, DEFINITION=MODE NUMBERS Abaqus/CAE Usage: Use the following option to define damping by specifying a frequency range: *MODAL DAMPING, DEFINITION=FREQUENCY RANGE Use the following input to define damping by specifying mode numbers: Step module: Create Step: Linear perturbation: Modal dynamics: Damping Defining damping by specifying frequency ranges is not supported in Abaqus/CAE. Example of specifying damping Figure 6.3.7–1 illustrates how the damping coefficients at different eigenfrequencies are determined for the following input: *MODAL DAMPING, DEFINITION=FREQUENCY RANGE damping values d = d +2 d 3 f i d i eigenfrequencies frequencies damping values d 2 d 3 f 2 d 3 f 3 d 4 f 4 frequency Figure 6.3.7–1 Damping coefficients specified by frequency range. Rules for selecting modes and specifying damping coefficients The following rules apply for selecting modes and specifying modal damping coefficients: • No modal damping is included by default. • Mode selection and modal damping must be specified in the same way, using either mode numbers or a frequency range. • If you do not select any modes, all modes extracted in the prior frequency analysis, including residual modes if they were activated, will be used in the superposition. • If you do not specify damping coefficients for modes that you have selected, zero damping values will be used for these modes. • Damping is applied only to the modes that are selected. • Damping coefficients for selected modes that are beyond the specified frequency range are constant and equal to the damping coefficient specified for the first or the last frequency (depending which one is closer). This is consistent with the way Abaqus interprets amplitude definitions. Specifying global damping For convenience you can specify constant global damping factors for all selected eigenmodes for mass and stiffness proportional viscous factors, as well as stiffness proportional structural damping. Structural damping is a commonly used damping model that represents damping as complex stiffness. This representation causes no difficulty for frequency domain analysis such as steady-state dynamics for which the solution is already complex. However, the solution must remain real-valued in the time domain. To allow users to apply their structural damping model in the time domain, a method has been developed to convert structural damping to an equivalent viscous damping. This technique was designed so that the viscous damping applied in the frequency domain is identical to the structural damping if the projected damping matrix is diagonal. For further details, see “Modal dynamic analysis,” Section 2.5.5 of the Abaqus Theory Manual. Input File Usage: *GLOBAL DAMPING, ALPHA=factor, BETA=factor, STRUCTURAL=factor Abaqus/CAE Usage: Defining damping by global factors is not supported in Abaqus/CAE. Material damping Structural and viscous material damping is taken into account in a SIM-based transient modal analysis. Since the projection of damping onto the mode shapes is performed only one time during the frequency extraction step, significant performance advantages can be achieved by using the SIM-based transient modal procedure . If the damping operators depend on frequency, they will be evaluated at the frequency specified for property evaluation during the frequency extraction procedure. You can deactivate the structural or viscous damping in a transient modal procedure if desired. Input File Usage: Use the following option to deactivate structural and viscous damping in a specific transient modal dynamic step: Abaqus/CAE Usage: *DAMPING CONTROLS, STRUCTURAL=NONE, VISCOUS=NONE Damping controls are not supported in Abaqus/CAE. Initial conditions By default, the modal dynamic step will begin with zero initial displacements. If initial velocities have been defined (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1), they will be used; otherwise, the initial velocities will be zero. Alternatively, you can force the modal dynamic step to carry over the initial conditions from the immediately preceding step, which must be either another modal dynamic step or a static perturbation step: • In most cases if the immediately preceding step is a modal dynamic step, both the displacements and velocities are carried over from the end of that step and used as initial conditions for the current step. For a SIM-based analysis, you should use secondary base motion instead of primary base motion to carry over the initial conditions; Abaqus issues a warning message if primary base motion is used. • If the immediately preceding step is a static perturbation step, the displacements are carried over from that step. If initial velocities have been defined (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1), they will be used; otherwise, the initial velocities will be zero. Input File Usage: Use the following option to begin the modal dynamic step with zero initial displacements: Abaqus/CAE Usage: *MODAL DYNAMIC, CONTINUE=NO Use the following option to force the modal dynamic step to carry over the initial conditions from the immediately preceding step: *MODAL DYNAMIC, CONTINUE=YES Use the following option to begin the modal dynamic step with zero initial displacements: Step module: Create Step: Linear perturbation: Modal dynamics: Basic: Zero initial conditions Use the following option to force the modal dynamic step to carry over the initial conditions from the immediately preceding step: Step module: Create Step: Linear perturbation: Modal dynamics: Basic: Use initial conditions Boundary conditions It is not possible to prescribe nonzero displacements and rotations directly as boundary conditions (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) in mode-based dynamic response procedures. In these procedures the motion for nodes can be specified only as base motion, as described below. Nonzero displacement or acceleration history definitions given as boundary conditions are ignored in modal superposition procedures, and any changes in the support conditions from the eigenfrequency extraction step are flagged as errors. Prescribed motions in modal superposition procedures Boundary conditions must be applied during the eigenfrequency extraction step to the degrees of freedom that will be prescribed in the modal dynamic procedure. These degrees of freedom are grouped into one or more “bases” . The unnamed base is called the “primary” base. Named “secondary” bases must be defined by specifying boundary conditions in the frequency extraction step. A different motion can be prescribed for each base. Specifying the degree of freedom and the time history of the motion The displacements and rotations that are associated with a base are prescribed during the modal dynamic response procedure. The base motions are fully defined by at most three global translations and three global rotations. Thus, at most one base motion can be defined for each translation and rotation component. Base motions are always specified in global directions, regardless of the use of nodal transformations. You specify the global direction (1–6) for which the base motion is being defined. If a rotation is specified about an origin that is not the origin of the coordinates, you must specify the center of rotation. The time history of a motion must be defined by an amplitude curve (“Amplitude curves,” Section 33.1.2). Input File Usage: Abaqus/CAE Usage: *BASE MOTION, DOF=n, AMPLITUDE=name Load module; Create Boundary Condition; Step: modal_dynamic_step; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion; Basic tabbed page: Degree-of-freedom: U1, U2, U3, UR1, UR2, or UR3; Amplitude: name Scaling the amplitude of the base motion The amplitude curve used to define the time history of the motion can be scaled. By default, the scaling factor is 1.0. Input File Usage: Abaqus/CAE Usage: *BASE MOTION, DOF=n, AMPLITUDE=name, SCALE=n Load module; Create Boundary Condition; Step: modal_dynamic_step; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion; Basic tabbed page: Degree-of-freedom: U1, U2, U3, UR1, UR2, or UR3; Amplitude: name; Amplitude scale factor: n Specifying the type of base motion Base motions can be defined by a displacement, a velocity, or an acceleration history. If the prescribed excitation record is given in the form of a displacement or velocity history, Abaqus/Standard differentiates it to obtain the acceleration history. Furthermore, if the displacement or velocity histories have nonzero initial values, Abaqus/Standard will make corrections to the initial accelerations as described in “Modal dynamic analysis,” Section 2.5.5 of the Abaqus Theory Manual. The default is to give an acceleration history. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *BASE MOTION, DOF=n, AMPLITUDE=name, TYPE=ACCELERATION *BASE MOTION, DOF=n, AMPLITUDE=name, TYPE=VELOCITY *BASE MOTION, DOF=n, AMPLITUDE=name, TYPE=DISPLACEMENT Load module; Create Boundary Condition; Step: modal_dynamic_step; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion Specifying secondary base motion The primary base motion is specified by defining a base motion without referring to a base. If the base motion is to be applied to a secondary base, it must refer to the name of the base defined in the eigenfrequency extraction step. Input File Usage: *BASE MOTION, DOF=n, AMPLITUDE=name, BASE NAME=secondary base Abaqus/CAE Usage: Load module; Create Boundary Condition; Step: modal_dynamic_step; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion; toggle on Secondary base: boundary_condition_name Example To illustrate the concept of primary and secondary bases, consider a single-bay frame with supports at nodes 1 and 4. If the input prior to the eigenfrequency extraction step includes the following boundary conditions: • degrees of freedom 1 through 6 constrained at node 1 • degree of freedom 1 constrained at node 4 • degrees of freedom 3 through 6 constrained at node 4 and different base motions are assigned to degree of freedom 2 at nodes 1 and 4, the following step definitions could be used: • an eigenfrequency extraction step that includes a boundary condition associated with BASE2 constraining degree of freedom 2 at node 4; and • a modal dynamic step that includes two base motion definitions: the primary base motion assigned to degree of freedom 2 that does not refer to a base and the secondary base motion assigned to degree of freedom 2 that refers to BASE2. If boundary conditions were not given prior to the eigenfrequency extraction step, you would have to define them in the eigenfrequency extraction step. Again, the secondary base would be defined by a boundary condition with a base name. Calculating the response of the structure The degrees of freedom associated with the primary base are set to zero in the eigenfrequency extraction step, and primary base motions are introduced by multiplying the base acceleration with the modal participation factors. Hence, Abaqus/Standard calculates the response of the structure with respect to the primary base. If the rotational degrees of freedom are references in the primary base motion definition, the rotation is defined, as default, about the origin of the coordinate system unless you provide the center of rotation. The degrees of freedom associated with the secondary bases are not set to zero in the eigenfrequency extraction step; instead, a “big” mass is added to each of them. Any degree of freedom in a secondary base that was constrained by a regular boundary condition in a previous general step will be released, and a big mass will be added to that degree of freedom. Secondary base motions are introduced by nodal forces, obtained by multiplying the base acceleration with the big mass. Although the secondary base motions are defined in absolute terms, the response calculated at the secondary bases is relative to the motion of the primary base for the translational degrees of freedom. The rotational secondary bases are defined about the nodes included in the node sets specified in the base name definition. Therefore, you cannot change the center of rotation for secondary bases. For a more detailed description of the base motion procedure, see “Base motions in modal-based procedures,” Section 2.5.9 of the Abaqus Theory Manual. Loads The following loads can be prescribed in modal dynamic analysis, as described in “Concentrated loads,” Section 33.4.2: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6). • Distributed pressure forces or body forces can be applied; the distributed load types available with particular elements are described in Part VI, “Elements.” Predefined fields Predefined temperature fields are not allowed in transient modal dynamic analysis. Other predefined fields are ignored. Material options The density of the material must be defined (“Density,” Section 21.2.1). The following material properties are not active during a modal dynamic analysis: plasticity and other inelastic effects, rate-dependent material properties, thermal properties, mass diffusion properties, electrical properties (except for the electrical potential, , in piezoelectric analysis), and pore fluid flow properties. See “General and linear perturbation procedures,” Section 6.1.3. Elements Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in Abaqus/Standard (including those with temperature and pressure degrees of freedom) can be used in a modal dynamic analysis. Output All the output variables in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. The values of nodal solution variables U, V, and A in modal dynamics in the time domain are relative to the motion of the primary base. Hence, the sum of the relative motion and the base motion of the primary base yields the total motion; this total motion is available by requesting output variables TU, TV, and TA. In the absence of primary base motions, the relative and total motions are identical. The following modal variables can be output to the data or results files : GU GV GA SNE KE BM Generalized displacements for all modes. Generalized velocities for all modes. Generalized accelerations for all modes. Elastic strain energy for the entire model per each mode. Kinetic energy for the entire model per each mode. External work for the entire model per each mode. Base motion. Neither element energy densities (such as the elastic strain energy density, SENER) nor whole element energies (such as the total kinetic energy of an element, ELKE) are available for output in modal dynamic analysis. However, whole model variables such as ALLIE (total strain energy) are available for mode-based procedures as output to the data or results files . The computational expense of a modal dynamic analysis can be decreased significantly by reducing the amount of output requested. Input file template *HEADING … *AMPLITUDE, NAME=amplitude Data lines to define amplitude variations ** *STEP *FREQUENCY Data line to specify the number of modes to be extracted *BOUNDARY Data lines to assign degrees of freedom to the primary base *BOUNDARY, BASE NAME=base Data lines to assign degrees of freedom to a secondary base *END STEP ** *STEP *MODAL DYNAMIC Data line to control time incrementation *SELECT EIGENMODES Data lines to define the applicable mode ranges *MODAL DAMPING Data line to define modal damping *BASE MOTION, DOF=dof, AMPLITUDE=amplitude *BASE MOTION, DOF=dof, AMPLITUDE=amplitude, BASE NAME=base *END STEP 6.3.8 MODE-BASED STEADY-STATE DYNAMIC ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “General and linear perturbation procedures,” Section 6.1.3 • “Dynamic analysis procedures: overview,” Section 6.3.1 • “Direct-solution steady-state dynamic analysis,” Section 6.3.4 • “Natural frequency extraction,” Section 6.3.5 • “Subspace-based steady-state dynamic analysis,” Section 6.3.9 • *STEADY STATE DYNAMICS • “Configuring a mode-based steady-state dynamic analysis” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A mode-based steady-state dynamic analysis: • is used to calculate the steady-state dynamic linearized response of a system to harmonic excitation; • is a linear perturbation procedure; • calculates the response based on the system’s eigenfrequencies and modes; • requires that an eigenfrequency extraction procedure be performed prior to the steady-state dynamic analysis; • can use the high-performance SIM software architecture ; • can include nondiagonal damping effects (i.e., from material or element damping) only when using the SIM architecture; • is an alternative to direct-solution steady-state dynamic analysis, in which the system’s response is calculated in terms of the physical degrees of freedom of the model; • is computationally cheaper than direct-solution or subspace-based steady-state dynamics; • is less accurate than direct-solution or subspace-based steady-state analysis, in particular if significant material damping is present, and • is able to bias the excitation frequencies toward the values that generate a response peak. Introduction Steady-state dynamic analysis provides the steady-state amplitude and phase of the response of a system due to harmonic excitation at a given frequency. Usually such analysis is done as a frequency sweep by applying the loading at a series of different frequencies and recording the response; in Abaqus/Standard the steady-state dynamic analysis procedure is used to conduct the frequency sweep. In a mode-based steady-state dynamic analysis the response is based on modal superposition techniques; the modes of the system must first be extracted using the eigenfrequency extraction procedure. The modes will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. The number of modes extracted must be sufficient to model the dynamic response of the system adequately, which is a matter of judgment on your part. When defining a mode-based steady-state dynamic step, you specify the frequency ranges of interest and the number of frequencies at which results are required in each range (including the bounding frequencies of the range). In addition, you can specify the type of frequency spacing (linear or logarithmic) to be used, as described below (“Selecting the frequency spacing”). Logarithmic frequency spacing is the default. Frequencies are given in cycles/time. These frequency points for which results are required can be spaced equally along the frequency axis (on a linear or a logarithmic scale), or they can be biased toward the ends of the user-defined frequency range by introducing a bias parameter . While the response in this procedure is for linear vibrations, the prior response can be nonlinear. Initial stress effects (stress stiffening) will be included in the steady-state dynamics response if nonlinear geometric effects (“General and linear perturbation procedures,” Section 6.1.3) were included in any general analysis step prior to the eigenfrequency extraction step preceding the steady-state dynamic procedure. Input File Usage: *STEADY STATE DYNAMICS The DIRECT and SUBSPACE PROJECTION parameters must be omitted from the *STEADY STATE DYNAMICS option to conduct a mode-based steady-state dynamic analysis. Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal Selecting the type of frequency interval for which output is requested Three types of frequency intervals are permitted for output from a mode-based steady-state dynamic step. Specifying the frequency ranges by using the system’s eigenfrequencies By default, the eigenfrequency type of frequency interval is used; in this case the following intervals exist in each frequency range: • First interval: extends from the lower limit of the frequency range given to the first eigenfrequency in the range. • Intermediate intervals: extend from eigenfrequency to eigenfrequency. • Last interval: extends from the highest eigenfrequency in the range to the upper limit of the frequency range. For each of these intervals the frequencies at which results are calculated are determined using the user- defined number of points (which includes the bounding frequencies for the interval) and the optional bias function (which is discussed below and allows the sampling points on the frequency scale to be spaced closer together at eigenfrequencies in the frequency range). Thus, detailed definition of the response close to resonance frequencies is allowed. Figure 6.3.8–1 illustrates the division of the frequency range for 5 calculation points and a bias parameter equal to 1. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, INTERVAL=EIGENFREQUENCY Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal: Use eigenfrequencies to subdivide each frequency range frequency points lower end of the range mode n mode n +1 mode n + 2 upper end of the range Figure 6.3.8–1 Division of range for the eigenfrequency type of interval and 5 calculation points. Specifying the frequency ranges by the frequency spread If the spread type of frequency interval is selected, intervals exist around each eigenfrequency in the frequency range. For each of the intervals the equally spaced frequencies at which results are calculated are determined using the user-defined number of points (which includes the bounding frequencies for the interval). The minimum number of frequency points is 3. If the user-defined value is less than 3 (or omitted), the default value of 3 points is assumed. Figure 6.3.8–2 illustrates the division of the frequency range for 5 calculation points. The bias parameter is not supported with the spread type of frequency interval. Input File Usage: *STEADY STATE DYNAMICS, INTERVAL=SPREAD lwr_freq, upr_freq, numpts, bias_param, freq_scale_factor, spread Abaqus/CAE Usage: You cannot specify frequency ranges by frequency spread in Abaqus/CAE. Specifying the frequency ranges directly If the alternative range type of frequency interval is chosen, there is only one interval in the specified frequency range spanning from the lower to the upper limit of the range. This interval is divided using Frequency points Frequency points fn fn + 1 (1 – spread) · fn (1 + spread) · fn (1 – spread) · fn + 1 (1 + spread) · fn + 1 Figure 6.3.8–2 Division of range for the spread type of interval and 5 calculation points. and are eigenfrequencies of the system. the user-defined number of points and the optional bias function, which can be used to space the sampling frequency points closer to the range limits. For the range type of frequency interval, the peak responses around the system’s eigenfrequencies may be missed since the sampling frequencies at which output will be reported will not be biased toward the eigenfrequencies. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, INTERVAL=RANGE Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal: toggle off Use eigenfrequencies to subdivide each frequency range Selecting the frequency spacing Two types of frequency spacing are permitted for a mode-based steady-state dynamic step. For the logarithmic frequency spacing (the default), the specified frequency ranges of interest are divided using a logarithmic scale. Alternatively, a linear frequency spacing can be used if a linear scale is desired. Input File Usage: Abaqus/CAE Usage: Use either of the following options: *STEADY STATE DYNAMICS, FREQUENCY SCALE=LOGARITHMIC *STEADY STATE DYNAMICS, FREQUENCY SCALE=LINEAR Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal: Scale: Logarithmic or Linear Requesting multiple frequency ranges You can request multiple frequency ranges or multiple single frequency points for a mode-based steady- state dynamic step. Input File Usage: *STEADY STATE DYNAMICS lwr_freq1, upr_freq1, numpts1, bias_param1, freq_scale_factor1 lwr_freq2, upr_freq2, numpts2, bias_param2, freq_scale_factor2 ... single_freq1 single_freq2 ... Repeat the data lines as often as necessary. Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal: Data: enter data in table, and add rows as necessary The bias parameter The bias parameter can be used to provide closer spacing of the results points either toward the middle or toward the ends of each frequency interval. Figure 6.3.8–3 shows a few examples of the effect of the bias parameter on the frequency spacing. frequency points f1 Bias parameter = 1 f2 Bias parameter = 2 Bias parameter = 3 Bias parameter = 5 Figure 6.3.8–3 Effect of the bias parameter on the frequency spacing for a number of points . The bias formula used to calculate the frequency at which results are presented is as follows: where ; is the number of frequency points at which results are to be given within a frequency interval (discussed above); is one such frequency point ( is the lower limit of the frequency interval; is the upper limit of the frequency interval; is the frequency at which the kth results are given; ); is the bias parameter value; and is the frequency or the logarithm of the frequency, depending on the value used for the frequency scale parameter. A bias parameter, p, that is greater than 1.0 provides closer spacing of the results points toward the ends of the frequency interval, while values of p that are less than 1.0 provide closer spacing toward the middle of the frequency interval. The default bias parameter is 3.0 for an eigenfrequency interval and 1.0 for a range frequency interval. The frequency scale factor The frequency scale factor can be used to scale frequency points. All the frequency points, except the lower and upper limit of the frequency range, are multiplied by this factor. This scale factor can be used only when the frequency interval is specified by using the system’s eigenfrequencies . Selecting the modes and specifying damping You can select the modes to be used in modal superposition and specify damping values for all selected modes. Selecting the modes You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard generate the mode numbers automatically, or by requesting the modes that belong to specified frequency ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step, including residual modes if they were activated, are used in the modal superposition. Input File Usage: Abaqus/CAE Usage: Specifying modal damping Use one of the following options to select the modes by specifying mode numbers: *SELECT EIGENMODES, DEFINITION=MODE NUMBERS *SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS Use the following option to select the modes by specifying a frequency range: *SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE You cannot select the modes in Abaqus/CAE; all modes extracted are used in the modal superposition. Damping is almost always specified for a steady-state analysis . If damping is absent, the response of a structure will be unbounded if the forcing frequency is equal to an eigenfrequency of the structure. To get quantitatively accurate results, especially near natural frequencies, accurate specification of damping properties is essential. The various damping options available are discussed in “Material damping,” Section 26.1.1. You can define a damping coefficient for all or some of the modes used in the response calculation. The damping coefficient can be given for a specified mode number or for a specified frequency range. When damping is defined by specifying a frequency range, the damping coefficient for a mode is interpolated linearly between the specified frequencies. The frequency range can be discontinuous; the average damping value will be applied for an eigenfrequency at a discontinuity. The damping coefficients are assumed to be constant outside the range of specified frequencies. Input File Usage: Use the following option to define damping by specifying mode numbers: *MODAL DAMPING, DEFINITION=MODE NUMBERS Use the following option to define damping by specifying a frequency range: *MODAL DAMPING, DEFINITION=FREQUENCY RANGE Use the following option to define damping by global factors: Abaqus/CAE Usage: Use the following input to define damping by specifying mode numbers: Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal: Damping Defining damping by specifying frequency ranges is not supported in Abaqus/CAE. Example of specifying damping Figure 6.3.8–4 illustrates how the damping coefficients at different eigenfrequencies are determined for the following input: *MODAL DAMPING, DEFINITION=FREQUENCY RANGE Rules for selecting modes and specifying damping coefficients The following rules apply for selecting modes and specifying modal damping coefficients: • No modal damping is included by default. • Mode selection and modal damping must be specified in the same way, using either mode numbers or a frequency range. • If you do not select any modes, all modes extracted in the prior frequency analysis, including residual modes if they were activated, will be used in the superposition. • If you do not specify damping coefficients for modes that you have selected, zero damping values will be used for these modes. • Damping is applied only to the modes that are selected. • Damping coefficients for selected modes that are beyond the specified frequency range are constant and equal to the damping coefficient specified for the first or the last frequency (depending which one is closer). This is consistent with the way Abaqus interprets amplitude definitions. damping values d = d +2 d 3 f i d i eigenfrequencies frequencies damping values d 2 d 3 f 2 d 3 f 3 d 4 f 4 frequency Figure 6.3.8–4 Damping values specified by frequency range. Specifying global damping For convenience you can specify constant global damping factors for all selected eigenmodes for mass and stiffness proportional viscous factors, as well as stiffness proportional structural damping. For further details, see “Damping in dynamic analysis” in “Dynamic analysis procedures: overview,” Section 6.3.1. Input File Usage: *GLOBAL DAMPING, ALPHA=factor, BETA=factor, STRUCTURAL=factor Abaqus/CAE Usage: Defining damping by global factors is not supported in Abaqus/CAE. Material damping Structural and viscous material damping is taken into account in a SIM-based steady-state dynamic analysis. Since the projection of damping onto the mode shapes is performed only one time during the frequency extraction step, significant performance advantages can be achieved by using the SIM-based steady-state dynamic procedure . If the damping operators depend on frequency, they will be evaluated at the frequency specified for property evaluation during the frequency extraction procedure. You can deactivate the structural or viscous damping in a mode-based steady-state dynamic procedure if desired. Input File Usage: Abaqus/CAE Usage: Use the following option to deactivate structural and viscous damping in a specific steady-state dynamic step: *DAMPING CONTROLS, STRUCTURAL=NONE, VISCOUS=NONE Damping controls are not supported in Abaqus/CAE. Initial conditions The base state is the current state of the model at the end of the last general analysis step prior to the steady-state dynamic step. If the first step of an analysis is a perturbation step, the base state is determined from the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Initial condition definitions that directly define solution variables, such as velocity, cannot be used in a steady-state dynamic analysis. Boundary conditions In a mode-based steady-state dynamic analysis both the real and imaginary parts of any degree of freedom are either restrained or unrestrained; it is physically impossible to have one part restrained and the other part unrestrained. Abaqus/Standard will automatically restrain both the real and imaginary parts of a degree of freedom even if only one part is restrained. Base motion It is not possible to prescribe nonzero displacements and rotations directly as boundary conditions (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) in mode-based dynamic response procedures. Therefore, in a mode-based steady-state dynamic analysis, the motion of nodes can be specified only as base motion; nonzero displacement or acceleration history definitions given as boundary conditions are ignored, and any changes in the support conditions from the eigenfrequency extraction step are flagged as errors. The method for prescribing base motion in modal superposition procedures is described in “Transient modal dynamic analysis,” Section 6.3.7. When secondary bases are used, low frequency eigenmodes will be extracted for each “big” mass applied in the model. Use care when choosing the frequency lower limit range in such cases. The “big” mass modes are important in the modal superposition; however, the response at zero or arbitrarily low frequency level should not be requested since it forces Abaqus/Standard to calculate responses at frequencies between these “big” mass eigenfrequencies, which is not desirable. Frequency-dependent base motion An amplitude definition can be used to specify the amplitude of a base motion as a function of frequency (“Amplitude curves,” Section 33.1.2). Input File Usage: Use both of the following options: Abaqus/CAE Usage: *AMPLITUDE, NAME=name *BASE MOTION, REAL or IMAGINARY, AMPLITUDE=name Load module; Create Boundary Condition; Step: step_name; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion; Basic tabbed page: Degree-of-freedom: U1, U2, U3, UR1, UR2, or UR3; Amplitude: name Loads The following loads can be prescribed in a mode-based steady-state dynamic analysis, as described in “Concentrated loads,” Section 33.4.2: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6). • Distributed pressure forces or body forces can be applied; the distributed load types available with particular elements are described in Part VI, “Elements.” These loads are assumed to vary sinusoidally with time over a user-specified range of frequencies. Loads are given in terms of their real and imaginary components. Fluid flux loading cannot be used in a steady-state dynamic analysis. Input File Usage: Abaqus/CAE Usage: Use either of the following input lines to define the real (in-phase) part of the load: *CLOAD or *DLOAD *CLOAD or *DLOAD, REAL Use the following input line to define the imaginary (out-of-phase) part of the load: *CLOAD or *DLOAD, IMAGINARY Load module: part i load editor: real (in-phase) part + imaginary (out-of-phase) Frequency-dependent loading An amplitude definition can be used to specify the amplitude of a load as a function of frequency (“Amplitude curves,” Section 33.1.2). Input File Usage: Abaqus/CAE Usage: Use both of the following options: *AMPLITUDE, NAME=name *CLOAD or *DLOAD, REAL or IMAGINARY, AMPLITUDE=name Load or Interaction module: Create Amplitude: Name: name Load module: part i: Amplitude: name load editor: real (in-phase) part + imaginary (out-of-phase) Predefined fields Predefined temperature fields are not allowed in mode-based steady-state dynamic analysis. Other predefined fields are ignored. Material options As in any dynamic analysis procedure, mass or density (“Density,” Section 21.2.1) must be assigned to some regions of any separate parts of the model where dynamic response is required. The following material properties are not active during mode-based steady-state dynamic analyses: plasticity and other inelastic effects, viscoelastic effects, thermal properties, mass diffusion properties, electrical properties (except for the electrical potential, , in piezoelectric analysis), and pore fluid flow properties—see “General and linear perturbation procedures,” Section 6.1.3. Elements Any of the following elements available in Abaqus/Standard can be used in a steady-state dynamics procedure: • stress/displacement elements (other than generalized axisymmetric elements with twist); • acoustic elements; • piezoelectric elements; or • hydrostatic fluid elements. See “Choosing the appropriate element for an analysis type,” Section 27.1.3. Output In mode-based steady-state dynamic analysis the value of an output variable such as strain (E) or stress (S) is a complex number with real and imaginary components. In the case of data file output the first printed line gives the real components while the second lists the imaginary components. Results and data file output variables are also provided to obtain the magnitude and phase of many variables . In this case the first printed line in the data file gives the magnitude while the second gives the phase angle. The following variables are provided specifically for steady-state dynamic analysis: Element integration point variables: PHS PHE PHEPG PHEFL PHMFL PHMFT Magnitude and phase angle of all stress components. Magnitude and phase angle of all strain components. Magnitude and phase angles of the electrical potential gradient vector. Magnitude and phase angles of the electrical flux vector. Magnitude and phase angle of the mass flow rate in fluid link elements. Magnitude and phase angle of the total mass flow in fluid link elements. For connector elements, the following element output variables are available: PHCTF PHCEF PHCVF PHCRF PHCSF PHCU PHCCU Magnitude and phase angle of connector total forces. Magnitude and phase angle of connector elastic forces. Magnitude and phase angle of connector viscous forces. Magnitude and phase angle of connector reaction forces. Magnitude and phase angle of connector friction forces. Magnitude and phase angle of connector relative displacements. Magnitude and phase angle of connector constitutive displacements. Nodal variables: PU PPOR PHPOT PRF PHCHG Magnitude and phase angle of all displacement/rotation components at a node. Magnitude and phase angle of the fluid or acoustic pressure at a node. Magnitude and phase angle of the electrical potential at a node. Magnitude and phase angle of all reaction forces/moments at a node. Magnitude and phase angle of the reactive charge at a node. Element energy densities (such as the elastic strain energy density, SENER) and whole element energies (such as the total kinetic energy of an element, ELKE) are not available for output in a mode- based steady-state dynamic analysis. The standard output variables U, V, A, and the variable PU listed above correspond to motions relative to the motion of the primary base in a mode-based analysis. Total values, which include the motion of the primary base, are also available: TU TV TA PTU Magnitude of all components of total displacement/rotation at a node. Magnitude of all components of total velocity at a node. Magnitude of all components of total acceleration at a node. Magnitude and phase angle of all total displacement/rotation components at a node. The following modal variables are also available for mode-based steady-state dynamic analysis and can be output to the data, results, and/or output database files : GU GV GA GPU GPV GPA SNE KE BM Generalized displacements for all modes. Generalized velocities for all modes. Generalized accelerations for all modes. Phase angle of generalized displacements for all modes. Phase angle of generalized velocities for all modes. Phase angle of generalized acceleration for all modes. Elastic strain energy for the entire model per mode. Kinetic energy for the entire model per mode. External work for the entire model per mode. Base motion. Whole model variables such as ALLIE (total strain energy) are available for mode-based steady- state dynamics as output to the data, results, and/or output database files . Input file template *HEADING … *AMPLITUDE, NAME=loadamp Data lines to define an amplitude curve as a function of frequency (cycles/time) *AMPLITUDE, NAME=base Data lines to define an amplitude curve to be used to prescribe base motion ** *STEP, NLGEOM Include the NLGEOM parameter so that stress stiffening effects will be included in the steady-state dynamics step *STATIC **Any general analysis procedure can be used to preload the structure … *CLOAD and/or *DLOAD Data lines to prescribe preloads *TEMPERATURE and/or *FIELD Data lines to define values of predefined fields for preloading the structure *BOUNDARY Data lines to specify boundary conditions to preload the structure *END STEP ** *STEP *FREQUENCY Data line to control eigenvalue extraction *BOUNDARY Data lines to assign degrees of freedom to the primary base *BOUNDARY, BASE NAME=base2 Data lines to assign degrees of freedom to a secondary base *END STEP ** *STEP *STEADY STATE DYNAMICS Data lines to specify frequency ranges and bias parameters *SELECT EIGENMODES Data lines to define the applicable mode ranges *MODAL DAMPING Data lines to define the modal damping factors *BASE MOTION, DOF=dof, AMPLITUDE=base *BASE MOTION, DOF=dof, AMPLITUDE=base, BASE NAME=base2 *CLOAD and/or *DLOAD, AMPLITUDE=loadamp Data lines to specify sinusoidally varying, frequency-dependent loads … *END STEP 6.3.9 SUBSPACE-BASED STEADY-STATE DYNAMIC ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “General and linear perturbation procedures,” Section 6.1.3 • “Dynamic analysis procedures: overview,” Section 6.3.1 • “Direct-solution steady-state dynamic analysis,” Section 6.3.4 • “Natural frequency extraction,” Section 6.3.5 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 • *STEADY STATE DYNAMICS • “Configuring a subspace-based steady-state dynamic analysis” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A subspace-based steady-state dynamic analysis: • is used to calculate the steady-state dynamic linearized response of a system to harmonic excitation; • is based on projection of the steady-state dynamic equations on a subspace of selected modes of the undamped system; • is a linear perturbation procedure; • provides a cost-effective way to include frequency-dependent effects (such as frequency-dependent damping and viscoelastic effects) in the model; • allows for nonsymmetric stiffness; • requires that an eigenfrequency extraction procedure be performed prior to the steady-state dynamic analysis; • can use the high-performance SIM software architecture ; • is an alternative to direct-solution steady-state dynamic analysis, in which the system’s response is calculated in terms of the physical degrees of freedom of the model; • is computationally cheaper than direct-solution steady-state dynamics but more expensive than mode-based steady-state dynamics; • is less accurate than direct-solution steady-state analysis, damping or viscoelasticity with a high loss modulus is present; and in particular if significant material • is able to bias the excitation frequencies toward the values that generate a response peak. Introduction Steady-state dynamic analysis provides the steady-state amplitude and phase of the response of a system subjected to harmonic excitation at a given frequency. Usually such analysis is done as a frequency In sweep, by applying the loading at a series of different frequencies and recording the response. Abaqus/Standard the subspace-based steady-state dynamic analysis procedure is used to conduct the frequency sweep. In a subspace-based steady-state dynamic analysis the response is based on direct solution of the steady-state dynamic equations projected onto a subspace of modes. The modes of the undamped, symmetric system must first be extracted using the eigenfrequency extraction procedure. The modes will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. The procedure is based on the assumption that the forced steady-state vibration can be represented accurately by a number of modes of the undamped system that are in the range of the excitation frequencies of interest. The number of modes extracted must be sufficient to model the dynamic response of the system adequately, which is a matter of judgment on your part. The projection of the dynamic equilibrium equations onto a subspace of selected modes leads to a small system of complex equations that is solved for modal amplitudes, which are then used to compute nodal displacements, stresses, etc. When defining a subspace-based steady-state dynamic step, you specify the frequency ranges of interest and the number of frequencies at which results are required in each range (including the bounding frequencies of the range). In addition, you can specify the type of frequency spacing (linear or logarithmic) to be used, as described below (“Selecting the frequency spacing”). Logarithmic frequency If the spacing is the default if the frequency ranges are specified directly or by eigenfrequencies. frequency ranges are specified by the frequency spread, only linear spacing can be used. Frequencies should be given in cycles/time. The frequency points for which results are required can be spaced equally along the frequency axis (on a linear or a logarithmic scale), or they can be biased toward the ends of the user-defined frequency range by introducing a bias parameter . The subspace-based steady-state dynamic analysis procedure can be used: • for nonsymmetric stiffness; • when any form of damping (except modal damping) is included; and • when viscoelastic material properties must be taken into account. While the response in this procedure is for linear vibrations, the prior response can be nonlinear. Initial stress effects (stress stiffening) will be included in the steady-state dynamic response if nonlinear geometric effects (“General and linear perturbation procedures,” Section 6.1.3) were included in any general analysis step prior to the eigenfrequency extraction step preceding the subspace-based steady- state dynamic procedure. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace Ignoring damping If damping terms can be ignored, you can specify that a real, rather than a complex, system matrix be generated and projected, which can significantly reduce computational time, at the cost of ignoring the damping effects. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION, REAL ONLY Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: Compute real response only Selecting the type of frequency interval for which output is requested Three types of frequency intervals are permitted for output from a subspace-based steady-state dynamic step. Specifying the frequency ranges by using the system’s eigenfrequencies By default, the eigenfrequency type of frequency interval is used; in this case the following intervals exist in each frequency range: • First interval: extends from the lower limit of the frequency range given to the first eigenfrequency in the range. • Intermediate intervals: extend from eigenfrequency to eigenfrequency. • Last interval: extends from the highest eigenfrequency in the range to the upper limit of the frequency range. For each of these intervals the frequencies at which results are calculated are determined using the user- defined number of points (which includes the bounding frequencies for the interval) and the optional bias function (which is discussed below and allows the sampling points on the frequency scale to be spaced closer together at eigenfrequencies in the frequency range). Thus, detailed definition of the response close to resonance frequencies is allowed. Figure 6.3.9–1 illustrates the division of the frequency range for 5 calculation points and a bias parameter equal to 1. frequency points lower end of the range mode n mode n +1 mode n + 2 upper end of the range Figure 6.3.9–1 Division of range for the eigenfrequency type of interval and 5 calculation points. Input File Usage: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION, INTERVAL=EIGENFREQUENCY Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: Use eigenfrequencies to subdivide each frequency range Specifying the frequency ranges by the frequency spread If the spread type of frequency interval is selected, intervals exist around each eigenfrequency in the frequency range. For each of the intervals the equally spaced frequencies at which results are calculated are determined using the user-defined number of points (which includes the bounding frequencies for the interval). The minimum number of frequency points is 3. If the user-defined value is less than 3 (or omitted), the default value of 3 points is assumed. Figure 6.3.9–2 illustrates the division of the frequency range for 5 calculation points. The bias parameter is not supported with the spread type of frequency interval. Frequency points Frequency points fn fn + 1 (1 – spread) · fn (1 + spread) · fn (1 – spread) · fn + 1 (1 + spread) · fn + 1 Figure 6.3.9–2 Division of range for the spread type of interval and 5 calculation points. and are eigenfrequencies of the system. Input File Usage: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION, INTERVAL=SPREAD lwr_freq, upr_freq, numpts, bias_param, freq_scale_factor, spread Abaqus/CAE Usage: You cannot specify frequency ranges by frequency spread in Abaqus/CAE. Specifying the frequency ranges directly If the alternative range type of frequency interval is chosen, there is only one interval in the specified frequency range spanning from the lower to the upper limit of the range. This interval is divided using the user-defined number of points and the optional bias function, which can be used to space the sampling frequency points closer to the range limits. For the range type of frequency interval, the peak responses around the system’s eigenfrequencies may be missed since the sampling frequencies at which output will be reported will not be biased toward the eigenfrequencies. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION, INTERVAL=RANGE Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: toggle off Use eigenfrequencies to subdivide each frequency range Selecting the frequency spacing Two types of frequency spacing are permitted for a subspace-based steady-state dynamic step. For the logarithmic frequency spacing (the default), the specified frequency ranges of interest are divided using a logarithmic scale. Alternatively, a linear frequency spacing can be used if a linear scale is desired. Input File Usage: Use the following option to specify logarithmic frequency spacing: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION, FREQUENCY SCALE=LOGARITHMIC (default) Use the following option to specify linear frequency spacing: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION, FREQUENCY SCALE=LINEAR Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: Scale: Logarithmic or Linear Requesting multiple frequency ranges You can request multiple frequency ranges for a subspace-based steady-state dynamic step. When both frequency ranges and additional single frequency points are requested, the frequency ranges must be specified first. Input File Usage: Repeat the data lines as often as necessary to request multiple frequency ranges or multiple single frequency points: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION lwr_freq1, upr_freq1, numpts1, bias_param1, freq_scale_factor1 lwr_freq2, upr_freq2, numpts2, bias_param2, freq_scale_factor2 ... single_freq1 single_freq2 ... Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: Data: enter data in table, and add rows as necessary The bias parameter The bias parameter can be used to provide closer spacing of the results points either toward the middle or toward the ends of each frequency interval. Figure 6.3.9–3 shows a few examples of the effect of the bias parameter on the frequency spacing. frequency points f1 Bias parameter = 1 f2 Bias parameter = 2 Bias parameter = 3 Bias parameter = 5 Figure 6.3.9–3 Effect of the bias parameter on the frequency spacing for a number of points . The bias formula used in subspace-based steady-state dynamics is where ; is the number of frequency points at which results are to be given within a frequency interval (discussed above); is one such frequency point ( ); is the lower limit of the frequency interval; is the upper limit of the frequency interval; is the frequency at which the kth results are given; is the bias parameter value; and is the frequency or the logarithm of the frequency, depending on the value chosen for the frequency scale. A bias parameter, p, that is greater than 1.0 provides closer spacing of the results points toward the ends of the frequency interval, while values of p that are less than 1.0 provide closer spacing toward the middle of the frequency interval. The default bias parameter is 3.0 for an eigenfrequency interval and 1.0 for a range frequency interval. The frequency scale factor The frequency scale factor can be used to scale frequency points. All the frequency points, except the lower and upper limit of the frequency range, are multiplied by this factor. This scale factor can be used only when the frequency interval is specified by using the system’s eigenfrequencies . Damping If damping is absent, the response of a structure will be unbounded if the forcing frequency is equal to an eigenfrequency of the structure. To get quantitatively accurate results, especially near natural frequencies, accurate specification of damping properties is essential. The various damping options available are discussed in “Material damping,” Section 26.1.1. In subspace-based steady-state dynamic analysis damping can be created by the following: • dashpots , • “Rayleigh” damping associated with materials and elements Section 26.1.1), , • viscoelasticity included in the material definitions , • contributions from infinite elements or defined impedance conditions on acoustic elements, and • “volumetric drag” (viscous Rayleigh damping) in acoustic elements . If you specify that a real-only system matrix be generated and projected , all forms of damping are ignored, nonreflecting boundaries on acoustic elements. Contact conditions with sliding friction Abaqus/Standard automatically detects the contact nodes that are slipping due to velocity differences imposed by the motion of the reference frame or the transport velocity in prior steps. At those nodes the tangential degrees of freedom are not constrained and the effect of friction results in an unsymmetric contribution to the stiffness matrix. At other contact nodes the tangential degrees of freedom are constrained. Friction at contact nodes at which a velocity differential is imposed can give rise to damping terms. There are two kinds of friction-induced damping effects. The first effect is caused by the friction forces stabilizing the vibrations in the direction perpendicular to the slip direction. This effect exists only in three-dimensional analysis. The second effect is caused by a velocity-dependent friction coefficient. If the friction coefficient decreases with velocity (which is usually the case), the effect is destabilizing and is also known as “negative damping.” For more details, see “Coulomb friction,” Section 5.2.3 of the Abaqus Theory Manual. Subspace-based steady-state dynamics analysis allows you to include these friction-induced contributions to the damping matrix. Input File Usage: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION, FRICTION DAMPING=YES Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: Include friction-induced damping effects Selecting the modes on which to project You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard generate the mode numbers automatically, or by requesting the modes that belong to specified frequency ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step, including residual modes if they were activated, are used in the modal superposition. Input File Usage: Use the following option to select the modes by specifying mode numbers individually: *SELECT EIGENMODES, DEFINITION=MODE NUMBERS Use the following option to request that Abaqus/Standard generate the mode numbers automatically: *SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS Use the following option to select the modes by specifying a frequency range: *SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE You cannot select the modes in Abaqus/CAE; all modes extracted are used in the modal superposition. Abaqus/CAE Usage: Selecting the subspace projection frequency You can control the frequency of the subspace projections. By default, the dynamic equations are projected onto the subspace at each frequency you request. However, considerable computational savings can be obtained if the projection onto the subspace is performed only at selected frequency points. Projecting the subspace at each frequency requested By default, the dynamic equations are projected onto the subspace at each frequency you requested. This is the most computationally expensive method. If coupled acoustic-structural modes are extracted in the preceding eigenfrequency extraction step, this is the only method allowed. Input File Usage: Use either of the following options: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION *STEADY STATE DYNAMICS, SUBSPACE PROJECTION=ALL FREQUENCIES Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: Projection: Evaluate at each frequency Projecting the subspace using model properties at the center frequency of all ranges You can perform only one projection using model properties evaluated at the center frequency of all ranges and individual frequency points specified. The center frequency is determined on a logarithmic or linear scale depending on the spacing requested. This method is the least expensive. However, it should be chosen only when the material properties do not depend strongly on frequency. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION=CONSTANT Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: Projection: Constant Projecting the subspace at each extracted eigenfrequency You can perform the projections at each extracted eigenfrequency in the requested frequency range and at eigenfrequencies immediately outside the range. The projected mass, stiffness, and damping matrices are then interpolated at each frequency point requested. The interpolation is performed on a linear or logarithmic scale depending on the spacing requested. Input File Usage: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION=EIGENFREQUENCY Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: Projection: Interpolate at eigenfrequencies Projecting the subspace based on material property changes as a function of frequency You can select how often subspace projections are performed based on material property changes as a function of frequency. You specify the relative change in material stiffness and damping properties allowed before a new projection is performed. In the beginning of the subspace-based steady-state dynamic step Abaqus/Standard computes a table of relative changes in material stiffness and damping properties, and projections are performed based on the strictest of the two criteria. The projections are then interpolated at each requested frequency point as described above. The default value for the allowable stiffness or damping change is 0.1. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION=PROPERTY CHANGE, DAMPING CHANGE=percentage, STIFFNESS CHANGE=percentage Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: Projection: As a function of property changes, Max. damping change: percentage, Max. stiffness change: percentage Projecting the subspace at the limits of each frequency range You can select how often subspace projections are performed based on the limits of each frequency range. The projections onto the modal subspace of the dynamic equations are performed at the lower limit of each frequency range and at the upper limit of the last frequency range. The interpolation of the projected mass, stiffness, and damping matrices is performed on a linear scale. This method can be used only with the SIM architecture. This method should be chosen when the frequency dependence of material properties is close to linear within a frequency range. Input File Usage: Abaqus/CAE Usage: *STEADY STATE DYNAMICS, SUBSPACE PROJECTION=RANGE Step module: Create Step: Linear perturbation: Steady-state dynamics, Subspace: Projection: Interpolate at lower and upper frequency limits Initial conditions The base state is the current state of the model at the end of the last general analysis step prior to the steady-state dynamic step. If the first step of an analysis is a perturbation step, the base state is determined from the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Initial condition definitions that directly define solution variables, such as velocity, cannot be used in a steady-state dynamic analysis. Boundary conditions In a subspace-based steady-state dynamic analysis both the real and imaginary parts of any degree of freedom are either restrained or unrestrained; it is physically impossible to have one part restrained and the other part unrestrained. Abaqus/Standard will restrain both the real and imaginary parts of a degree of freedom automatically even if only one part is restrained. Base motion It is not possible to prescribe nonzero displacements and rotations directly as boundary conditions (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) in subspace-based Instead, prescribed motion can be specified as base motion; nonzero steady-state dynamic analysis. displacement or acceleration history definitions given as boundary conditions are ignored, and any changes in the support conditions from the eigenfrequency extraction step are flagged as errors. The method for prescribing base motion in modal superposition procedures is described in “Transient modal dynamic analysis,” Section 6.3.7. Frequency-dependent base motion An amplitude definition can be used to specify the amplitude of a base motion as a function of frequency (“Amplitude curves,” Section 33.1.2). Input File Usage: Use both of the following options: *AMPLITUDE, NAME=name *BASE MOTION, REAL or IMAGINARY, AMPLITUDE=name Abaqus/CAE Usage: Load module; Create Boundary Condition; Step: step_name; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion; Basic tabbed page: Degree-of-freedom: U1, U2, U3, UR1, UR2, or UR3; Amplitude: name Loads The following loads can be prescribed in a subspace-based steady-state dynamic analysis, as described in “Concentrated loads,” Section 33.4.2: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6). • Distributed pressure forces or body forces can be applied; the distributed load types available with particular elements are described in Part VI, “Elements.” • Incident wave loads can be applied; see “Acoustic and shock loads,” Section 33.4.6. Incident wave loads can be used to model sound waves from distinct planar or spherical sources or from diffuse fields. These loads are assumed to vary sinusoidally with time over a user-specified range of frequencies. Loads are given in terms of their real and imaginary components. Input File Usage: Use either of the following input lines to define the real (in-phase) part of the load: *CLOAD or *DLOAD *CLOAD or *DLOAD, REAL Use the following input line to define the imaginary (out-of-phase) part of the load: Abaqus/CAE Usage: *CLOAD or *DLOAD, IMAGINARY You can only define the real (in phase) part of the load in Abaqus/CAE. Load module: load editor: real (in-phase) part Frequency-dependent loading An amplitude definition can be used to specify the amplitude of a load as a function of frequency (“Amplitude curves,” Section 33.1.2). Input File Usage: Use both of the following options: Abaqus/CAE Usage: *AMPLITUDE, NAME=name *CLOAD or *DLOAD, REAL or IMAGINARY, AMPLITUDE=name Load or Interaction module: Create Amplitude: Name: name Load module: load editor: Amplitude: name Loading limitations Coriolis distributed loading adds an imaginary antisymmetric contribution to the overall system of equations. This contribution is currently accounted for in solid and truss elements only and is activated by requesting the unsymmetric matrix storage and solution scheme for the step. Fluid flux loading cannot be used in subspace-based steady-state dynamic analysis. Predefined fields Predefined temperature fields can be specified in subspace-based steady-state dynamic analysis and will produce harmonically varying thermal strains if thermal expansion is included in the material definition (“Thermal expansion,” Section 26.1.2). Other predefined fields are ignored. Material options As in any dynamic analysis procedure, mass or density (“Density,” Section 21.2.1) must be assigned to some regions of any separate parts of the model where dynamic response is required. If an analysis is desired in which the inertia effects are neglected, the density should be set to a very small number. Natural damping, as well as individual dashpots, can be included in this procedure. Viscoelastic effects can be included in subspace-based steady-state dynamic analysis. The linearized viscoelastic response is considered to be a perturbation about a nonlinear preloaded state, which is computed on the basis of purely elastic behavior (long-term response) in the viscoelastic components. Therefore, the vibration amplitude must be sufficiently small so that the material response in the dynamic phase of the problem can be treated as a linear perturbation about the predeformed state. Viscoelastic frequency domain response is described in “Frequency domain viscoelasticity,” Section 22.7.2. The following material properties are not active during subspace-based steady-state dynamic analyses: plasticity and other inelastic effects, thermal properties (except for thermal expansion), mass diffusion properties, electrical properties (except for the electrical potential, , in piezoelectric analysis), and pore fluid flow properties—see “General and linear perturbation procedures,” Section 6.1.3. Numerical investigations show that in general the accuracy of the results in the subspace-based steady-state dynamic step is improved if in the previous eigenfrequency extraction step the material properties are evaluated at a frequency in the vicinity of the center of the range spanned by the frequencies specified for the steady-state dynamic step . In this case the modes extracted in the previous eigenfrequency extraction step for the undamped system will reflect most accurately the modes of the damped system at frequencies located in the proximity of the frequency at which the material properties are evaluated. Thus, if the steady-state dynamic response is sought for a large span of frequencies and the specified material properties vary significantly over this span, the results will be more accurate if the range is divided into smaller ranges and several separate analyses are run over these smaller ranges with the material properties evaluated at appropriate frequencies. Elements Any of the following elements available in Abaqus/Standard can be used in a subspace-based steady-state dynamic analysis: • stress/displacement elements (other than generalized axisymmetric elements with twist); • acoustic elements; • piezoelectric elements; and • hydrostatic fluid elements. See “Choosing the appropriate element for an analysis type,” Section 27.1.3. Output In subspace-based steady-state dynamic analysis the value of an output variable such as strain (E) or stress (S) is a complex number with real and imaginary components. In the case of data file output the first printed line gives the real components while the second lists the imaginary components. Results and data file output variables are also provided to obtain the magnitude and phase of many variables . In this case the first printed line in the data file gives the magnitude while the second gives the phase angle. The following variables are provided specifically for subspace-based steady-state dynamic analysis: Element integration point variables: PHS PHE PHEPG PHEFL PHMFL PHMFT Magnitude and phase angle of all stress components. Magnitude and phase angle of all strain components. Magnitude and phase angles of the electrical potential gradient vector. Magnitude and phase angles of the electrical flux vector. Magnitude and phase angle of the mass flow rate in fluid link elements. Magnitude and phase angle of the total mass flow in fluid link elements. For connector elements, the following element output variables are available: PHCTF PHCEF PHCVF PHCRF PHCSF PHCU PHCCU PHCV PHCA Magnitude and phase angle of connector total forces. Magnitude and phase angle of connector elastic forces. Magnitude and phase angle of connector viscous forces. Magnitude and phase angle of connector reaction forces. Magnitude and phase angle of connector friction forces. Magnitude and phase angle of connector relative displacements. Magnitude and phase angle of connector constitutive displacements. Magnitude and phase angle of connector relative velocities. Magnitude and phase angle of connector relative accelerations. Nodal variables: PU PPOR PHPOT PRF PHCHG Magnitude and phase angle of all displacement/rotation components at a node. Magnitude and phase angle of the fluid or acoustic pressure at a node. Magnitude and phase angle of the electrical potential at a node. Magnitude and phase angle of all reaction forces/moments at a node. Magnitude and phase angle of the reactive charge at a node. Neither element energy densities (such as the elastic strain energy density, SENER) nor whole element energies (such as the total kinetic energy of an element, ELKE) are available for output in a subspace-based steady-state dynamic analysis. The standard output variables U, V, A, and the variable PU listed above correspond to motions relative to the motion of the primary base in a subspace-based steady-state dynamic analysis. Total values, which include the motion of the primary base, are also available: TU TV TA PTU Components of total displacement/rotation at a node. Components of total velocity at a node. Components of total acceleration at a node. Magnitude and phase angle of all total displacement/rotation components at a node. The specified base motion is available for subspace-based steady-state dynamic analysis and can be output to the data, results, and/or output database files . BM Base motion. Whole model variables such as ALLIE (total strain energy) are available for subspace-based steady- state dynamic analysis as output to the data, results, and/or output database files . Input file template *HEADING … *AMPLITUDE, NAME=loadamp Data lines to define an amplitude curve as a function of frequency (cycles/time) *AMPLITUDE, NAME=base Data lines to define an amplitude curve to be used to prescribe base motion ** *STEP, NLGEOM Include the NLGEOM parameter so that stress stiffening effects will be included in the steady-state dynamics step *STATIC **Any general analysis procedure can be used to preload the structure … *CLOAD and/or *DLOAD Data lines to prescribe preloads *TEMPERATURE and/or *FIELD Data lines to define values of predefined fields for preloading the structure *BOUNDARY Data lines to specify boundary conditions to preload the structure *END STEP ** *STEP *FREQUENCY Data line to control eigenvalue extraction *BOUNDARY Data lines to assign degrees of freedom to the primary base *BOUNDARY, BASE NAME=base2 Data lines to assign degrees of freedom to a secondary base *END STEP ** *STEP *STEADY STATE DYNAMICS, SUBSPACE PROJECTION Data lines to specify frequency ranges and bias parameters *SELECT EIGENMODES Data lines to define the applicable mode ranges *BASE MOTION, DOF=dof, AMPLITUDE=base *BASE MOTION, DOF=dof, AMPLITUDE=base, BASE NAME=base2 *CLOAD and/or *DLOAD, AMPLITUDE=loadamp Data lines to specify sinusoidally varying, frequency-dependent loads … *END STEP 6.3.10 RESPONSE SPECTRUM ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Dynamic analysis procedures: overview,” Section 6.3.1 • “Defining an analysis,” Section 6.1.2 • “General and linear perturbation procedures,” Section 6.1.3 • *RESPONSE SPECTRUM • *SPECTRUM • “Configuring a response spectrum procedure” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a spectrum,” Section 57.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A response spectrum analysis: • provides an estimate of the peak linear response of a structure to dynamic motion of fixed points (“base motion”) or dynamic force; • is typically used to analyze response to a seismic event; • assumes that the system’s response is linear so that it can be analyzed in the frequency domain using its natural modes, which must be extracted in a previous eigenfrequency extraction step (“Natural frequency extraction,” Section 6.3.5); • can use the high-performance SIM software architecture ; and • is a linear perturbation procedure and is, therefore, not appropriate if the excitation is so severe that nonlinear effects in the system are important. Response spectrum analysis Response spectrum analysis can be used to estimate the peak response (displacement, stress, etc.) of a structure to a particular base motion or force. The method is only approximate, but it is often a useful, inexpensive method for preliminary design studies. The response spectrum procedure is based on using a subset of the modes of the system, which must first be extracted by using the eigenfrequency extraction procedure. The modes will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. The number of modes extracted must be sufficient to model the dynamic response of the system adequately, which is a matter of judgment on your part. In cases with repeated eigenvalues and eigenvectors, the modal summation results must be interpreted with care. You should add insignificant mass to the structure or perturb the symmetric geometry such that the eigenvalues become unique. While the response in the response spectrum procedure is for linear vibrations, the prior response may be nonlinear. Initial stress effects (stress stiffening) will be included in the response spectrum analysis if nonlinear geometric effects (“General and linear perturbation procedures,” Section 6.1.3) were included in a general analysis step prior to the eigenfrequency extraction step. The problem to be solved can be stated as follows: given a set of base motions, ), ( ), estimate the peak value specified in orthogonal directions defined by direction cosines over all time of the response of any variable in a finite element model that is simultaneously subjected to these multiple base motions. The peak response is first computed independently for each direction of excitation for each natural mode of the system as a function of frequency and damping. These independent responses are then combined to create an estimate of the actual peak response of any variable chosen for output, as a function of frequency and damping. ( The acceleration history (base motion) is not given directly in a response spectrum analysis; it must first be converted into a spectrum. Specifying a spectrum , at each mode The response spectrum method is based on first finding the peak response to each base motion excitation of a one degree of freedom system that has a natural frequency equal to the frequency of interest. The single degree of freedom system is characterized by its undamped natural frequency, , and the fraction of critical damping present in the system, . The equations of motion of the system are integrated through time to find peak values of relative displacement, relative velocity, and relative or absolute acceleration for the linear, one degree of freedom system. This process is repeated for all frequency and damping values in the range of interest. Plots of these responses are known as displacement, velocity, and acceleration spectra: . The response spectrum can be obtained directly from measured data, as described in “Defining a spectrum using values of S as a function of frequency and damping,” below. You can also use a FORTRAN program to define a spectrum; an example of defining a spectrum from an acceleration record in this way is provided in “Analysis of a cantilever subject to earthquake motion,” Section 1.4.13 of the Abaqus Benchmarks Manual. , and , Alternatively, you can create the required spectrum by specifying an amplitude (time history record), the frequency range, and the damping values for which the spectrum will be built, as described in “Creating a spectrum from a given time history record,” below. The spectrum can be used in the subsequent response spectrum analysis, or it can be written to a file for future use. For each damping value the magnitude of the response spectrum must be given over the entire range of frequencies needed, in ascending value of frequency. Abaqus/Standard interpolates linearly between the values given on a log-log scale. Outside the extremes of the frequency range given, the magnitude is assumed to be constant, corresponding to the end value given. Any number of spectra can be defined, and each spectrum must be named. The response spectrum procedure allows up to three spectra to be applied simultaneously to the model in orthogonal physical directions defined by their direction cosines. Defining a spectrum using values of S as a function of frequency and damping You can define a spectrum by specifying values for the magnitude of the spectrum; frequency, in cycles per time, at which the magnitude is used; and associated damping, given as a ratio of critical damping. Input File Usage: To define the spectrum on the data lines: *SPECTRUM, NAME=spectrum name Repeat this option to define multiple spectra for an analysis. Abaqus/CAE Usage: To define a spectrum, do the following: Step, Interaction, or Load module: Tools→Amplitude→Create; Name: spectrum name, Type: Spectrum To apply a spectrum to the model, do the following: Step module: Create Step: Linear perturbation: Response spectrum: Use response spectrum: select spectrum name for each physical direction in which it should be applied Specifying the type of spectrum You can indicate whether a displacement, velocity, or acceleration spectrum is given. The default is an acceleration spectrum. Alternatively, an acceleration spectrum can be given in g-units. In this case you must also specify the value of the acceleration of gravity. Input File Usage: Use one of the following options to define a displacement, velocity, or acceleration spectrum: Abaqus/CAE Usage: *SPECTRUM, NAME=name, TYPE=DISPLACEMENT *SPECTRUM, NAME=name, TYPE=VELOCITY *SPECTRUM, NAME=name, TYPE=ACCELERATION Use the following option to define an acceleration spectrum given in g-units: *SPECTRUM, NAME=name, TYPE=G, G=g Use one of the following options to define a displacement, velocity, or acceleration spectrum: Step, Interaction, or Load module: Tools→Amplitude→Create; Type: Spectrum; Specification units: Displacement, Velocity, or Acceleration Use the following option to define an acceleration spectrum given in g-units: Step, Interaction, or Load module: Tools→Amplitude→Create; Type: Spectrum; Specification units: Gravity, Gravity: g Reading the data defining the spectrum from an alternate input file The data for the spectrum can be specified in an alternate input file and read into the Abaqus/Standard input file. Input File Usage: Abaqus/CAE Usage: *SPECTRUM, NAME=name, INPUT=file name Step, Interaction, or Load module: Tools→Amplitude→Create; Type: Spectrum; click mouse button 3 while holding the cursor over the data table, and select Read from File Creating a spectrum from a given time history record If you have a time history of a dynamic event (e.g., acceleration, velocity, displacement), you can build your own spectrum by specifying the record type and the amplitude name that this record represents. If the amplitude record is given with an arbitrarily changing time increment, linear interpolation will be needed for the implicit integration scheme for the dynamic equation of motion for a single degree of freedom system subjected to this record. You can specify the frequency range for the integration scheme and the frequency increment. You can build a spectrum for every fraction of critical damping indicated in the list of damping values. Input File Usage: *SPECTRUM, CREATE, AMPLITUDE=amplitude name, NAME=spectrum name, TIME INCREMENT=dt Abaqus/CAE Usage: Creating a spectrum from a given time history record is not supported in Abaqus/CAE. Specifying the type of spectrum to be created You can indicate whether a displacement, velocity, or acceleration spectrum is to be created. The default is an acceleration spectrum. Alternatively, an acceleration spectrum can be created in g-units. In this case you must also specify the value of the acceleration of gravity. Input File Usage: Use one of the following options to create a displacement, velocity, or acceleration spectrum: *SPECTRUM, CREATE, TYPE=DISPLACEMENT *SPECTRUM, CREATE, TYPE=VELOCITY *SPECTRUM, CREATE, TYPE=ACCELERATION Use the following option to create an acceleration spectrum in g-units: Abaqus/CAE Usage: *SPECTRUM, CREATE, TYPE=G, G=g Creating a spectrum from a given time history record is not supported in Abaqus/CAE. Specifying the record type that the time history represents You can indicate whether a displacement, velocity, or acceleration amplitude is specified. The default is an acceleration amplitude. Alternatively, an acceleration amplitude can be given in g-units. In this case you must also specify the value of the acceleration of gravity. Input File Usage: Use one of the following options to indicate that the amplitude is defined in displacement, velocity, or acceleration units: *SPECTRUM, CREATE, EVENT TYPE=DISPLACEMENT *SPECTRUM, CREATE, EVENT TYPE=VELOCITY *SPECTRUM, CREATE, EVENT TYPE=ACCELERATION Use the following option to indicate that an acceleration amplitude is given in g-units: *SPECTRUM, CREATE, EVENT TYPE=G, G=g Creating a spectrum from a given time history record is not supported in Abaqus/CAE. Abaqus/CAE Usage: Creating an absolute or relative acceleration spectrum When you create an acceleration spectrum from a given time history record, you can create an absolute or relative response spectrum. The default is an absolute spectrum. Input File Usage: Abaqus/CAE Usage: *SPECTRUM, CREATE, TYPE=ACCELERATION, ABSOLUTE *SPECTRUM, CREATE, TYPE=ACCELERATION, RELATIVE Creating a spectrum from a given time history record is not supported in Abaqus/CAE. Generating the list of damping values for the fraction of critical damping You must provide a list of damping values for the fraction of critical damping to create a spectrum. However, if the damping is evenly spaced between its lower and upper bound, you can automatically generate the list of damping values by providing the start value, end value, and increment for the fraction of critical damping. Input File Usage: Abaqus/CAE Usage: *SPECTRUM, CREATE, DAMPING GENERATE Creating a spectrum from a given time history record is not supported in Abaqus/CAE. Writing the generated spectra to an independent file You can write the generated spectra to an independent file. Otherwise, the generated spectra can be used only within the currently submitted job in subsequent response spectra procedures. You can inspect the generated spectra if you request that model definition data be printed to the data file . Input File Usage: Abaqus/CAE Usage: *SPECTRUM, CREATE, FILE=file name Creating a spectrum from a given time history record is not supported in Abaqus/CAE. Estimating the peak values of the modal responses Since the response spectrum procedure uses modal methods to define a model’s response, the value of any physical variable is defined from the amplitudes of the modal responses (the “generalized coordinates”), . The first stage in the response spectrum procedure is to estimate the peak values of these modal responses. For mode and spectrum k this is where ; ; is the modal amplitude for mode is a scaling parameter introduced as part of the response spectrum procedure definition for spectrum is the user-defined value of the spectrum in direction k interpolated, if necessary, at natural frequency and the fraction of critical damping in mode is the jth direction cosine for the kth spectrum; and is the participation factor for mode extraction,” Section 6.3.5). in direction j (see “Natural frequency ; Similar expressions for and can be obtained by substituting velocity or acceleration spectra in the above equation. Combining the individual peak responses The individual peak responses to the excitations in different directions will occur at different times and, therefore, must be combined into an overall peak response. Two combinations must be performed, and both introduce approximations into the results: 1. The multidirectional excitations must be combined into one overall response. This combination is controlled by the directional summation method, as described below in “Directional summation methods.” 2. The peak modal responses must be combined to estimate the peak physical response. This combination is controlled by the modal summation method, as described below in “Modal summation methods.” Depending on the type of base excitation, either modal responses or directional responses are combined first. Directional summation methods You choose the method for combining the multidirectional excitations depending on the nature of the excitations. The algebraic method If the input spectra in the different directions are components of a base excitation that is approximately in a single direction in space, then for each mode the peak responses in the different spatial directions are summed algebraically by After this summation is performed, the modal responses are summed. (Choosing the method used for modal summation is described below in “Modal summation methods.”) Since the directional components are summed first, the subscript k is not relevant and can be ignored in the modal summation equations that follow. Input File Usage: Abaqus/CAE Usage: *RESPONSE SPECTRUM, COMP=ALGEBRAIC, SUM=sum Step module: Create Step: Linear perturbation: Response spectrum: Excitations: Single direction or Multiple direction absolute sum The square root of the sum of the squares directional summation method If the spectra in different directions represent independent excitations, the modal summation is performed first, as explained below in “Modal summation methods.” Then, the responses in different excitation directions are combined by Input File Usage: Abaqus/CAE Usage: *RESPONSE SPECTRUM, COMP=SRSS, SUM=sum Step module: Create Step: Linear perturbation: Response spectrum: Excitations: Multiple direction square root of the sum of squares The forty-percent method If the spectra in different directions represent independent excitations, the modal summation is performed first, as explained below in “Modal summation methods.” Then, the responses in different excitation directions are combined by the 40% rule recommended by the ASCE 4–98 standard for Seismic Analysis of Safety-Related Nuclear Structures and Commentary, Section 3.2.7.1.2. This method combines the response for all possible combinations of the three components, including variations in sign (plus/minus), assuming that when the maximum response from one component occurs, the response from the other two components is 40% of their maximum value, using one of the following: Input File Usage: Abaqus/CAE Usage: *RESPONSE SPECTRUM, COMP=R40, SUM=sum Step module: Create Step: Linear perturbation: Response spectrum: Excitations: Multiple direction forty percent rule The thirty-percent method If the spectra in different directions represent independent excitations, the modal summation is performed first, as explained below in “Modal summation methods.” Then, the responses in different excitation directions are combined by the 30% rule recommended by the ASCE 4–98 standard for Seismic Analysis of Safety-Related Nuclear Structures and Commentary, Section 3.2.7.1.2. This method combines the response for all possible combinations of the three components, including variations in sign (plus/minus), assuming that when the maximum response from one component occurs, the response from the other two components is 30% of their maximum value, using one of the following: Input File Usage: Abaqus/CAE Usage: *RESPONSE SPECTRUM, COMP=R30, SUM=sum Step module: Create Step: Linear perturbation: Response spectrum: Excitations: Multiple direction thirty percent rule Modal summation methods The peak response of some physical variable reaction force, etc.) caused by the motion in the in direction k at frequency with damping (a component i of displacement, stress, section force, th natural mode excited by the given response spectra is given by where the subscript k is not relevant and can be ignored in this equation and in those that follow.) is the ith component of mode , and there is no sum on . (In the case of algebraic summation , into estimates of the total peak response, There are several methods for combining these peak physical responses in the individual modes, . Most of the methods implemented in Abaqus/Standard follow the ASCE 4–98 standard for Seismic Analysis of Safety Related Nuclear Structures and Commentary. The updated documents, “Reevaluation of Regulatory Guidance on Modal Response Combination Methods for Seismic Response Spectrum Analysis” issued in 1999 (NUREG/CR-6645, BNL-NUREG-52276) and “Draft Regulatory Guide” (DG-1127) issued in 2005 contain new recommendations. You are advised to read the new recommendations before choosing a modal summation method from among those described below. The absolute value method The absolute value method is the most conservative method for combining the modal responses. It is obtained by summing the absolute values resulting from each mode: This method implies that all of the responses peak simultaneously. It will overpredict the peak response of most systems; therefore, it may be too conservative to help in design. Input File Usage: Abaqus/CAE Usage: *RESPONSE SPECTRUM, COMP=comp, SUM=ABS Step module: Create Step: Linear perturbation: Response spectrum: Summations: Absolute values The square root of the sum of the squares modal summation method The square root of the sum of the squares method is less conservative than the absolute value method. It is also usually more accurate if the natural frequencies of the system are well separated. It uses the square root of the sum of the squares to combine the modal responses: Input File Usage: Abaqus/CAE Usage: *RESPONSE SPECTRUM, COMP=comp, SUM=SRSS Step module: Create Step: Linear perturbation: Response spectrum: Summations: Square root of the sum of squares The Naval Research Laboratory method The absolute value and square root of the sum of the squares methods can be combined to yield the Naval Research Laboratory method. It distinguishes the mode, , in which the physical variable has its maximum response and adds the square root of the sum of squares of the peak responses in all other modes to the absolute value of the peak response of that mode. This method gives the estimate: Input File Usage: Abaqus/CAE Usage: *RESPONSE SPECTRUM, COMP=comp, SUM=NRL Step module: Create Step: Linear perturbation: Response spectrum: Summations: Naval Research Laboratory The ten-percent method The ten-percent method recommended by Regulatory Guide 1.92 (1976) is no longer recommended according to the “Reevaluation of Regulatory Guidance on Modal Response Combination Methods for Seismic Response Spectrum Analysis” document issued in 1999. It is retained here because of its extensive prior use. The ten-percent method modifies the square root of the sum of the squares method by adding a contribution from all pairs of modes and whose frequencies are within 10% of each other, giving the estimate: The frequencies of modes and are considered to be within 10% of each other whenever The ten-percent method reduces to the square root of the sum of the squares method if the modes are well separated with no coupling between them. Input File Usage: Abaqus/CAE Usage: *RESPONSE SPECTRUM, COMP=comp, SUM=TENP Step module: Create Step: Linear perturbation: Response spectrum: Summations: Ten percent The complete quadratic combination method Like the ten-percent method, the complete quadratic combination method improves the estimation for structures with closely spaced eigenvalues. The complete quadratic combination method combines the modal response with the formula where frequencies and modal damping between the two modes: are cross-correlation coefficients between modes and , which depend on the ratio of where . If the modes are well spaced, their cross-correlation coefficient will be small ( method will give the same results as the square root of the sum of the squares method. ) and the This method is usually recommended for asymmetrical building systems since, in such cases, other methods can underestimate the response in the direction of motion and overestimate the response in the transverse direction. Input File Usage: Abaqus/CAE Usage: *RESPONSE SPECTRUM, COMP=comp, SUM=CQC Step module: Create Step: Linear perturbation: Response spectrum: Summations: Complete quadratic combination The grouping method This method, also known as the NRC grouping method, improves the response estimation for structures with closely spaced eigenvalues. The modal responses are grouped such that the lowest and highest frequency modes in a group are within 10% and no mode is in more than one group. The modal responses are summed absolutely within groups before performing a SRSS combination of the groups. Within the group responses are summed as for “n” frequencies within any “gr” group and then performing The above expression includes all the groups; in addition, the group can consist of just one frequency response if this frequency does not have another member that is within the 10% limit. Input File Usage: The ten-percent method will always produce results higher in value than the grouping method. *RESPONSE SPECTRUM, COMP=comp, SUM=GRP Step module: Create Step: Linear perturbation: Response spectrum: Summations: Grouping method Abaqus/CAE Usage: Double sum combination This method, also known as Rosenblueth’s double sum combination (Rosenblueth and Elorduy, 1969), is the first attempt to evaluate modal correlation based on random vibration theory. It utilizes the time duration , which depend also on the frequencies and damping coefficient of strong earthquake motion. The mode correlation coefficients , lead to the following mode combination: where where Input File Usage: Abaqus/CAE Usage: *RESPONSE SPECTRUM, COMP=comp, SUM=DSC Step module: Create Step: Linear perturbation: Response spectrum: Summations: Double sum combination Selecting the modes and specifying damping You can select the modes to be used in modal superposition and specify damping values for all selected modes. Selecting the modes You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard generate the mode numbers automatically, or by requesting the modes that belong to specified frequency ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step, including residual modes if they were activated, are used in the modal superposition. Input File Usage: Use one of the following options to select the modes by specifying mode numbers: *SELECT EIGENMODES, DEFINITION=MODE NUMBERS *SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS Use the following option to select the modes by specifying a frequency range: *SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE You cannot select the modes in Abaqus/CAE; all modes extracted are used in the modal superposition. Abaqus/CAE Usage: Specifying damping Damping is almost always specified for a mode-based procedure; see “Material damping,” Section 26.1.1. You can define a damping coefficient for all or some of the modes used in the response calculation. The damping coefficient can be given for a specified mode number or for a specified frequency range. When damping is defined by specifying a frequency range, the damping coefficient for an mode is interpolated linearly between the specified frequencies. The frequency range can be discontinuous; the average damping value will be applied for an eigenfrequency at a discontinuity. The damping coefficients are assumed to be constant outside the range of specified frequencies. Input File Usage: Abaqus/CAE Usage: Use the following option to define damping by specifying mode numbers: *MODAL DAMPING, DEFINITION=MODE NUMBERS Use the following option to define damping by specifying a frequency range: *MODAL DAMPING, DEFINITION=FREQUENCY RANGE Use the following input to define damping by specifying mode numbers: Step module: Create Step: Linear perturbation: Response spectrum: Damping: Specify damping over ranges of: Modes Use the following input to define damping by specifying a frequency range: Step module: Create Step: Linear perturbation: Response spectrum: Damping: Specify damping over ranges of: Frequencies Example of specifying damping Figure 6.3.10–1 illustrates how the damping coefficients at different eigenfrequencies are determined for the following input: *MODAL DAMPING, DEFINITION=FREQUENCY RANGE Rules for selecting modes and specifying damping coefficients The following rules apply for selecting modes and specifying modal damping coefficients: • No modal damping is included by default. • Mode selection and modal damping must be specified in the same way, using either mode numbers or a frequency range. • If you do not select any modes, all modes extracted in the prior frequency analysis, including residual modes if they were activated, will be used in the superposition. • If you do not specify damping coefficients for modes that you have selected, zero damping values will be used for these modes. damping values d = d +2 d 3 f i d i eigenfrequencies frequencies damping values d 2 d 3 f 2 d 3 f 3 d 4 f 4 frequency Figure 6.3.10–1 Damping values specified by frequency range. • Damping is applied only to the modes that are selected. • Damping coefficients for selected modes that are beyond the specified frequency range are constant and equal to the damping coefficient specified for the first or the last frequency (depending which one is closer). This is consistent with the way Abaqus interprets amplitude definitions. Initial conditions It is not appropriate to specify initial conditions in a response spectrum analysis. Boundary conditions All points constrained by boundary conditions and the ground nodes of connector elements are assumed to move in phase in any one direction. This base motion can use a different input spectrum in each of three orthogonal directions (two directions in a two-dimensional model). You define the input spectra, , as described earlier in , for different values of critical damping, , as functions of frequency, “Specifying a spectrum.” Secondary bases cannot be used in a response spectrum analysis. Loads The only “loading” that can be defined in a response spectrum analysis is that defined by the input spectra, as described earlier. No other loads can be prescribed in a response spectrum analysis. Predefined fields Predefined fields, including temperature, cannot be used in response spectrum analysis. Material options The density of the material must be defined (“Density,” Section 21.2.1). The following material properties are not active during a response spectrum analysis: plasticity and other inelastic effects, rate-dependent material properties, thermal properties, mass diffusion properties, electrical properties, and pore fluid flow properties—see “General and linear perturbation procedures,” Section 6.1.3. Elements Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in Abaqus/Standard can be used in a response spectrum analysis—see “Choosing the appropriate element for an analysis type,” Section 27.1.3. Output All the output variables in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. The value of an output variable such as strain, E; stress, S; or displacement, U, is its peak magnitude. In addition to the usual output variables available, the following modal variables are available for response spectrum analysis and can be output to the data and/or results files : GU GV GA SNE KE Generalized displacements for all modes. Generalized velocities for all modes. Generalized accelerations for all modes. Elastic strain energy for the entire model per each mode. Kinetic energy for the entire model per each mode. External work for the entire model per each mode. Neither element energy densities (such as the elastic strain energy density, SENER) nor whole element energies (such as the total kinetic energy of an element, ELKE) are available for output in response spectrum analysis. However, whole model variables such as ALLIE (total strain energy) are available for modal-based procedures as output to the data and/or results files . Reaction force output is not supported for response spectrum analysis using eigenmodes extracted using a SIM-based frequency extraction procedure with either the AMS or Lanczos eigensolver. Reaction force output in response spectrum analysis using eigenmodes extracted with the default Lanczos eigensolver provides directional combinations of so-called, modal reaction forces weighted with maximal absolute values of corresponding generalized displacements. Directional and modal combination rules used for the reaction force calculation are the same as for other nodal output variables. Modal reaction forces are calculated in the frequency extraction procedure. They represent static reaction forces calculated for the normal mode shapes. Generally, they cannot adequately represent reaction force in dynamic analysis. For models with diagonal mass and diagonal damping matrices the superposition of the modal reaction forces can provide a reasonable approximation of a nodal reaction force in mode-based analyses other than response spectrum analysis. In response spectrum analysis the model response can be better represented by requesting section stresses and section forces in structural elements containing supported nodes. Input file template , and *HEADING … *BOUNDARY Data lines to define points to be excited by the base motion controlled by the input spectra *SPECTRUM, NAME=name1, TYPE=type Data lines to define spectrum “name1” as a function of frequency, fraction of critical damping, *SPECTRUM, NAME=name2, TYPE=type Data lines to define spectrum “name2” as a function of frequency, fraction of critical damping, ** *STEP *FREQUENCY Data line to specify number of modes to be extracted *END STEP ** *STEP *RESPONSE SPECTRUM, COMP=comp, SUM=sum Data lines referring to response spectra and defining direction cosines *SELECT EIGENMODES Data lines to define the applicable mode ranges *MODAL DAMPING Data lines to define modal damping *END STEP , and Additional reference • Rosenblueth, E., and J. Elorduy, “Response of Linear Systems to Certain Transient Disturbances,” Proceedings of the Fourth World Conference on Earthquake Engineering, Santiago, Chile, 1969. 6.3.11 RANDOM RESPONSE ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “General and linear perturbation procedures,” Section 6.1.3 • “Dynamic analysis procedures: overview,” Section 6.3.1 • *RANDOM RESPONSE • *PSD-DEFINITION • *CORRELATION • “Configuring a random response procedure” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A random response analysis: • is a linear perturbation procedure that gives the linearized dynamic response of a model to user- defined random excitation; and • uses the set of modes extracted in a previous eigenfrequency extraction step to calculate the power spectral densities of response variables (stresses, strains, displacements, etc.) and the corresponding root mean square (RMS) values of these same variables. Random response analysis Random response analysis predicts the response of a system that is subjected to a nondeterministic continuous excitation that is expressed in a statistical sense by a cross-spectral density matrix. Since the loading is nondeterministic, it can be characterized only in a statistical sense; Abaqus/Standard assumes that the excitation is stationary and ergodic. These statistical measures are explained in detail in “Random response analysis,” Section 2.5.8 of the Abaqus Theory Manual. The random response procedure can, for example, be used to determine the response of an airplane to turbulence, the response of a car to road surface imperfections, the response of a structure to jet noise, or the response of a building to an earthquake. In the most general case the excitation is defined as a frequency-dependent cross-spectral density (CSD) matrix. Except in cases involving moving noise or user subroutine UCORR, it is assumed that for a given load case the CSD matrix can be separated into a product of a frequency-dependent, complex- valued scalar function and a frequency-independent, complex-valued, spatial correlation matrix. This assumption helps reduce both the computational time and the amount of required user input but implies that each element of the CSD matrix in a given load case has the same frequency dependence. You can define a different frequency dependence for each load case, but the loads in one load case will not be correlated with loads in another. Consequently, the system CSD matrix is assembled by simply summing (superimposing) the CSD matrices of the individual load cases. The frequency-dependent scalar function can be composed of a weighted sum of user-defined, complex-valued, frequency functions. These user-defined frequency functions are specified in units of power spectral density. You assign weights to each frequency function as well as specify properties of the spatial correlation matrix that defines the correlation between excitations at different locations and in different directions for a particular load case. Frequency functions and correlations are discussed below; see “Defining the frequency functions,” and “Defining the correlation.” The loads can be defined as concentrated point loads, as distributed loads, as connector element loads, or as base motion excitations, as described below in “Boundary conditions,” and “Loads.” Multiple, uncorrelated load cases can be defined for concentrated point loads, connector loads, and base motions. Load case 1 is reserved for all distributed loads defined in a particular step. In these steps load case 1 cannot be used for any concentrated point load, connector load, or base motion. Thus, there cannot be any correlation between distributed loads and any other load. Moreover, base motion excitations are assumed to be statistically independent (no correlation) with any other load type even when the same load case number is used. The concentrated point and connector element loads are assumed to be correlated if the same load case number is used. The random response procedure is based on using a subset of the modes of the system, which must first be extracted by using the eigenfrequency extraction procedure. The modes will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. The number of modes extracted must be sufficient to model the dynamic response of the system adequately, which is a matter of judgment on your part. The model can be preloaded prior to the eigenfrequency extraction. Initial stress effects are included in the stiffness used in the eigenfrequency extraction if geometric nonlinearities are included in the general analysis procedure used to apply the preloads (“General and linear perturbation procedures,” Section 6.1.3). The random response of the model is expressed as power spectral density values of nodal and element variables, as well as their root mean square values. Defining the frequency range You specify the frequency range of interest for the random response procedure. The response is calculated at multiple points between the lowest frequency of interest and the first eigenfrequency in the range, between each eigenfrequency in the range, and between the last eigenfrequency in the range and the highest frequency in the range as illustrated in Figure 6.3.11–1. The default number of calculation points in each interval is 20; you can change this number when you define the step. Accurate RMS values can be obtained only if enough points are used so that Abaqus/Standard can integrate accurately over the frequency range. The bias function allows the points on the frequency scale to be spaced closer together at the eigenfrequencies, thus allowing detailed definition of the response close to resonant frequencies and more accurate integration. Input File Usage: *RANDOM RESPONSE lower_freq_limit, upper_freq_limit, num_calc_pts, bias_parameter, freq_scale frequency points lower end of the range mode n mode n +1 mode n + 2 upper end of the range Figure 6.3.11–1 Division of range using modes and 5 calculation points. Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Random response The bias parameter The bias parameter can be used to provide closer spacing of the result points either toward the middle or toward the ends of each frequency interval. Figure 6.3.11–2 shows a few examples of the effect of the bias parameter on the frequency spacing. frequency points f1 Bias parameter = 1 f2 Bias parameter = 2 Bias parameter = 3 Bias parameter = 5 Figure 6.3.11–2 Effect of the bias parameter on the frequency spacing for a number of points . The bias formula used to calculate the frequency at which results are presented is as follows: where ; is the number of frequency points at which results are to be given; is one such frequency point ( is the lower limit of the frequency interval; is the upper limit of the interval; is the frequency at which the kth results are given; is the bias parameter value; and is the frequency or the logarithm of the frequency, depending on the chosen frequency scale. ); A bias parameter, p, that is greater than 1.0 provides closer spacing of the results points toward the ends of each frequency interval (as shown in the examples above), while values of p that are less than 1.0 provide closer spacing toward the middle of each frequency interval. The default value of the bias parameter for random response analysis is 3.0. Defining the frequency functions To define the random loading, you specify a frequency function and a cross-correlation definition that refers to the frequency function. The frequency functions are defined as model data (i.e., they are step independent) and must be named. A log-log scale is used in interpolating between the given values. The type of units in the CSD matrix of the excitation are specified as part of the frequency function definition. The default type is power units. If the CSD matrix of the excitation is due to base motion, the units must be in g units and you should define the acceleration of gravity. Alternatively, decibel units can be specified; this type of units is explained below. Input File Usage: Abaqus/CAE Usage: Use one of the following options to define the frequency function: *PSD-DEFINITION, NAME=name, TYPE=FORCE (default; power units) *PSD-DEFINITION, NAME=name, TYPE=BASE, G=g *PSD-DEFINITION, NAME=name, TYPE=DB, DB REFERENCE= Load module: Create Amplitude; Type: PSD Definition; Specification units: Power, Decibel, or Gravity Defining the cross-spectral density matrix in decibel units In Abaqus/Standard the decibel value full octave band conversion formula: is related to the frequency function by the following where Hence, the frequency function follows from the function defined in decibel units as is the user-specified reference power and is the midband frequency . Table 6.3.11–1 Standard octave bands. Band number Band center (frequency, Hz) 10 11 12 13 14 15 1.0 2.0 4.0 8.0 16.0 31.5 63.0 125.0 250.0 500.0 1000.0 2000.0 4000.0 8000.0 16000.0 If you have data in terms of an alternative frequency scale (e.g., one-third octave band), an equivalent full octave band power reference value can be obtained as described in “Random response analysis,” Section 2.5.8 of the Abaqus Theory Manual. in decibels must be specified as a function of the frequency band; the associated midband frequencies are given in Table 6.3.11–1. Alternate methods for defining frequency functions You can define a frequency function in an external file or in a user subroutine. Defining the frequency function in an external file The data to define a frequency function can be contained in an external file. Input File Usage: Abaqus/CAE Usage: *PSD-DEFINITION, NAME=name, TYPE=type, INPUT=file name Load module: Create Amplitude; Type: PSD Definition; Specification units: Power, Decibel, or Gravity; Real, Imaginary, Frequency Defining the frequency function in a user subroutine Complicated frequency functions can be more easily defined by user subroutine UPSD than by entering data directly. Input File Usage: *PSD-DEFINITION, NAME=name, TYPE=type, USER Any data lines given will be ignored if the USER parameter is specified. Abaqus/CAE Usage: Load module: Create Amplitude; Type: PSD Definition; Specification units: Power or Gravity; toggle on Specify data in an external user subroutine Defining the correlation You define the cross-correlation between the applied nodal loads or base motions. You can also assign scaling (weight) factors to the frequency functions through the cross-correlation definition. Distributed loads are converted to equivalent nodal loads, which are treated as individual point loads with respect to the cross-correlation. The cross-correlation is defined in the random response step and references a particular load case number and frequency function. Three types of correlation can be defined: correlated, uncorrelated, and moving noise. As many correlations as needed to define the random loading can be specified unless the moving noise type is chosen, in which case only one correlation can appear in the step definition. • For the correlated type all terms in the cross-spectral density matrix are considered, which implies that the loads on all degrees of freedom within the load case are fully correlated (statistically dependent on each other). • For the uncorrelated type only diagonal terms in the cross-spectral density matrix are considered, which implies that no correlation exists between the load on one degree of freedom and the load on another. You should exercise caution when choosing the uncorrelated type with distributed loads since the equivalent nodal forces would be uncorrelated with each other (statistically independent). • For the moving noise type the terms in the correlation matrix depend on the relative position of the points where the loads are applied. This type can be used only in conjunction with concentrated point loads and distributed loads. In addition, the moving noise formulation assumes that the frequency function referenced by the cross-correlation defines a reference power spectral density function of the noise source. (It is a reference power spectral density because it can later be scaled by the magnitude of the loadings specified as distributed, concentrated point, or connector element loads.) Since the power spectral density is real-valued for real-valued variables, the frequency function must not contain imaginary terms when used with the moving noise type of cross-correlation. Input File Usage: Use one of the following options to define the correlation: *CORRELATION, TYPE=CORRELATED, PSD=name *CORRELATION, TYPE=UNCORRELATED, PSD=name *CORRELATION, TYPE=MOVING NOISE For the moving noise type the reference to the power spectral density function must be given on each data line. Abaqus/CAE Usage: Load module; Create Boundary Condition; Step: random_response_step; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion; Correlation tabbed page: toggle on Specify correlation; Approach: Correlated or Uncorrelated; PSD: psd_amplitude_name Specifying whether the correlation matrix is complex For correlated or uncorrelated cross-correlations you can specify whether or not both real and imaginary terms will be included in the spatial correlation matrix. This specification does not affect the imaginary terms given for the power spectral density frequency function. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *CORRELATION, TYPE=CORRELATED, COMPLEX=YES or NO, PSD=name *CORRELATION, TYPE=UNCORRELATED, COMPLEX=YES or NO, PSD=name Load module; Create Boundary Condition; Step: random_response_step; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion; Correlation tabbed page: toggle on Specify correlation; Approach: Correlated or Uncorrelated; PSD: psd_amplitude_name; Real; Imaginary Alternate methods for defining a correlation You can define a correlation in an external input file or in a user subroutine. Defining the correlation in an external input file The data to define a correlation can be contained in an external input file. Input File Usage: Abaqus/CAE Usage: *CORRELATION, TYPE=type, PSD=name, INPUT=file_name You cannot define a correlation in an external file in Abaqus/CAE. Defining the correlation in a user subroutine Simple excitations, such as uncorrelated white noise, are easily defined. Excitations involving more complicated correlations, including cases where the elements of the CSD matrix have different frequency dependencies, can be defined through user subroutine UCORR. If the user subroutine is specified, only the load case number must be entered as part of the correlation definition. A user subroutine cannot be used to define a moving noise correlation. For uncorrelated cross-correlations only the diagonal terms of the correlation matrix specified in UCORR will be used. The combination of the cross-correlation with the various kinds of applied loads is discussed in more detail below. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *CORRELATION, TYPE=CORRELATED, USER, COMPLEX=YES or NO, PSD=name *CORRELATION, TYPE=UNCORRELATED, USER, PSD=name Load module; Create Boundary Condition; Step: random_response_step; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion; Correlation tabbed page: toggle on Specify correlation; Approach: User Selecting the modes and specifying damping You can select the modes to be used in modal superposition and specify damping values for all selected modes. Selecting the modes You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard generate the mode numbers automatically, or by requesting the modes that belong to specified frequency ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step, including residual modes if they were activated, are used in the modal superposition. Input File Usage: Use one of the following options to select the modes by specifying mode numbers: *SELECT EIGENMODES, DEFINITION=MODE NUMBERS *SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS Use the following option to select the modes by specifying a frequency range: *SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE You cannot select the modes in Abaqus/CAE; all modes extracted are used in the modal superposition. Abaqus/CAE Usage: Specifying damping Damping is almost always specified for a random response analysis . If damping is absent, the response of a structure will be unbounded if the forcing frequency is equal to an eigenfrequency of the structure. To get quantitatively accurate results, especially near natural frequencies, accurate specification of damping properties is essential. The various damping options available are discussed in “Material damping,” Section 26.1.1. You can define a damping coefficient for all or some of the modes used in the response calculation. The damping coefficient can be given for a specified mode number or for a specified frequency range. When damping is defined by specifying a frequency range, the damping coefficient for a mode is interpolated linearly between the specified frequencies. The frequency range can be discontinuous; the average damping value will be applied for an eigenfrequency at a discontinuity. The damping coefficients are assumed to be constant outside the range of specified frequencies. Input File Usage: Use the following option to define damping by specifying mode numbers: Abaqus/CAE Usage: *MODAL DAMPING, DEFINITION=MODE NUMBERS Use the following option to define damping by specifying a frequency range: *MODAL DAMPING, DEFINITION=FREQUENCY RANGE Use the following input to define damping by specifying mode numbers: Step module: Create Step: Linear perturbation: Random response: Damping Defining damping by specifying frequency ranges is not supported in Abaqus/CAE. Example of specifying damping Figure 6.3.11–3 illustrates how the damping coefficients at different eigenfrequencies are determined for the following input: *MODAL DAMPING, DEFINITION=FREQUENCY RANGE damping values d = d +2 d 3 f i d i eigenfrequencies frequencies damping values d 2 d 3 f 2 d 3 f 3 d 4 f 4 frequency Figure 6.3.11–3 Damping values specified by frequency range. Rules for selecting modes and specifying damping coefficients The following rules apply for selecting modes and specifying modal damping coefficients: • No modal damping is included by default. • Mode selection and modal damping must be specified in the same way, using either mode numbers or a frequency range. • If you do not select any modes, all modes extracted in the prior frequency analysis, including residual modes if they were activated, will be used in the superposition. • If you do not specify damping coefficients for modes that you have selected, zero damping values will be used for these modes. • Damping is applied only to the modes that are selected. • Damping coefficients for selected modes that are beyond the specified frequency range are constant and equal to the damping coefficient specified for the first or the last frequency (depending which one is closer). This is consistent with the way Abaqus interprets amplitude definitions. Initial conditions It is not appropriate to specify initial conditions in a random response analysis. Boundary conditions It is not possible to prescribe nonzero displacements and rotations directly as boundary conditions (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) in mode-based dynamic response procedures. Therefore, in a random response analysis the motion of nodes can be specified only as base motion; nonzero displacement, velocity, or acceleration history definitions given as boundary conditions are ignored, and any changes in the support conditions from the eigenfrequency extraction step are flagged as errors. In addition, any amplitude definitions are ignored in a random response analysis. The method for prescribing motion in modal superposition procedures is described in “Transient modal dynamic analysis,” Section 6.3.7. In random response analysis only a single (primary) base can be defined. Defining multiple load cases The excitation defined by the base motion is assigned to numbered load cases. These load cases are then referenced in the cross-correlation definition. The load cases are associated with frequency functions through the reference in the cross-correlation definition. Any number of load cases can be defined, but load case number 1 cannot be used if distributed loads are defined in the same step. Input File Usage: Abaqus/CAE Usage: *BASE MOTION, LOAD CASE=n Base motions with load cases are not supported in Abaqus/CAE. Converting base motion excitation to a cross-spectral density matrix When the excitation is provided by a base motion, it is converted directly into a cross-spectral density matrix projected onto the eigenspace through the modal participation factors , giving for for for , , , Re where the superscript * denotes complex conjugate and where is the modal participation factor for mode is the frequency function referenced by the Jth cross-correlation and defined as a function of the frequency f in g units; is a matrix of weight factors indicating the fraction of between base motion in directions i and j for load case I, as described below; to be associated with the correlation in excitation direction i (i=1–6); , 1, or 2, depending on whether the base motion corresponding to load case I is defined in terms of an acceleration spectrum, a velocity spectrum, or a displacement spectrum ; and is the user-specified acceleration of gravity for the same power spectral density frequency function that defines . If the cross-correlation is defined in user subroutine UCORR, Otherwise, is defined in the user subroutine. for all if the excitation is correlated or if the excitation is uncorrelated, where in load case I. is the (complex) value of the weight factor by which to scale the frequency function used Loads , where f is frequency in cycles per time and the subscripts The loading for random response analysis is defined in general terms by the cross-spectral density matrix refer to degree of freedom i at node N and degree of freedom j at node M, respectively. Distributed loads are converted to equivalent nodal loads, which—for the formulation of the correlation matrix—are treated are (force)2 or (moment)2 in the same way as concentrated point loads. The units of per frequency. In addition, any amplitude references on the concentrated point, connector element, or distributed load definitions are ignored in a random response analysis. and Defining multiple load cases Distributed loads will be assigned automatically to load case number 1. You assign a concentrated point load or connector element load to a numbered load case. Any number of concentrated point and connector element load cases can be specified, but load case number 1 cannot be used for a concentrated point or connector element load if a distributed load is present in the same step. The concentrated point, connector element, and distributed load cases are associated with frequency functions through the cross-correlation definition. Input File Usage: Use one or more of the following options: *CLOAD, LOAD CASE=n *CONNECTOR LOAD, LOAD CASE=m *DLOAD Correlated and uncorrelated loading For correlated or uncorrelated cross-correlations, the cross-spectral density matrix is defined as Re for for for , , , where the superscript * denotes complex conjugate and where is the load magnitude applied to degree of freedom i at node N for load case I; is the frequency function referenced by the Jth cross-correlation and defined as a function of the frequency f in power (force) or decibel units; and is a matrix of weight factors indicating the fraction of the cross-correlation term for load case I, as described below. to be associated with If the cross-correlation is defined in user subroutine UCORR, Otherwise, is defined in the user subroutine. for all if the excitation is correlated or if the excitation is uncorrelated, where in load case I. is the (complex) value of the weight factor by which to scale the frequency function used Moving noise loading For moving noise cross-correlations, the cross-spectral density matrix is defined as where is the load magnitude applied to degree of freedom i at node N for load case I; is the reference power spectral density function associated with load case I and defined as a function of the frequency f in power (force) or decibel units; is the velocity vector of noise propagation given for load case I; and are the coordinates of node N. This definition of moving noise implies that the different noise sources have no cross-correlation. Therefore, it is most generally used with only one noise source ( is the actual power spectral density of the moving noise source, it must be defined as a real-valued function. only). In addition, since Predefined fields Predefined fields, including temperature, cannot be used in random response analysis. Material options As in any dynamic analysis procedure, mass or density (“Density,” Section 21.2.1) must be assigned to some regions of any separate parts of the model where dynamic response is required. The following material properties are not active during a random response analysis: plasticity and other inelastic effects, rate-dependent properties, thermal properties, mass diffusion properties, electrical properties, and pore fluid flow properties . Elements Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in Abaqus/Standard can be used in a random response analysis . Output In random response analysis the value of a variable is its power spectral density; all of the output variables in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Power spectral density values are not available for concentrated and distributed loads and for SINV. Options are also provided in random response analysis to obtain root mean square values for certain variables, as listed below. Total values include base motion, while relative values are measured relative to the base motion. Element integration point variables: RS RE Root mean square of all stress components. Root mean square of all strain components. Element nodal point variables: MISES RMISES Mises equivalent stress.. Root mean square of Mises equivalent stress. For connector elements, the following element output variables are available: RCTF Root mean square of connector total forces. RCEF RCVF RCRF RCSF RCU RCCU Nodal variables: RU RTU RV RTV RA RTA RRF Root mean square of connector elastic forces. Root mean square of connector viscous forces. Root mean square of connector reaction forces. Root mean square of connector friction forces. Root mean square of connector relative displacements. Root mean square of connector constitutive displacements. Root mean square values of all components of the relative displacement/rotation at a node. Root mean square values of all components of the total displacement/rotation at a node. Root mean square values of all components of the relative velocity at a node. Root mean square values of all components of the total velocity at a node. Root mean square values of all components of the relative acceleration at a node. Root mean square values of all components of the total acceleration at a node. Root mean square values of all components of reaction forces and reaction moments at a node. No energy values are available for a random response analysis. To reduce the computational cost of random response analysis, you should request output only for selected element and node sets. Abaqus/Standard will calculate the response for only the element and nodal variables requested. When MISES or RMISES output is requested, Abaqus/Standard stores the needed data in the output database (.odb) file and Abaqus/Viewer does the actual computation of the responses. These computations require element stress output in the frequency step preceding the random response step. Note that specifying the name of the element set in the output request in the random response step has no effect on these two output variables. If MISES or RMISES output for a selected set of elements is desired, the name of that element set needs to be specified for the element stress output request in the preceding frequency step. Unlike in other procedures, MISES and RMISES output for random response analysis is computed at the element nodal points and not at the element integration points. Input file template *HEADING … *PSD-DEFINITION, NAME=name, TYPE=type Data lines to define a frequency function (or PSD function for moving noise) ** *STEP *FREQUENCY Data line to control eigenvalue extraction *BOUNDARY Data lines to assign degrees of freedom to the primary base *END STEP *STEP *RANDOM RESPONSE Data line to specify frequency range of interest *SELECT EIGENMODES Data lines to define the applicable mode ranges *MODAL DAMPING Data line to define modal damping *CORRELATION, PSD=name, TYPE=type Data lines to specify correlation for various excitation load cases (n, p) *DLOAD Data lines to define distributed loads *CLOAD, LOAD CASE=n Data lines to define concentrated loads in load case n *CONNECTOR LOAD, LOAD CASE=m Data lines to define connector loads in load case m *BASE MOTION, DOF=dof, LOAD CASE=p Data lines to define base motion p *END STEP 6.4 Steady-state transport analysis • “Steady-state transport analysis,” Section 6.4.1 6.4.1 STEADY-STATE TRANSPORT ANALYSIS Product: Abaqus/Standard References • “Defining an analysis,” Section 6.1.2 • “Symmetric model generation,” Section 10.4.1 • *STEADY STATE TRANSPORT • *SYMMETRIC MODEL GENERATION • *MOTION • *TRANSPORT VELOCITY • *ACOUSTIC FLOW VELOCITY Overview A steady-state transport analysis: • allows for steady-state rolling and sliding solutions including frictional effects and inertia effects; • allows for steady-state solutions to be obtained directly or by using a quasi-steady-state (pass-by- pass) technique; • is used to model the interaction between a deformable rolling object and one or more flat, convex, or concave surfaces; • is based on a specialized analysis capability where the rigid body motion is described in a spatial or Eulerian manner and the deformation in a material or Lagrangian manner; • allows for one element set in a model to be described in an Eulerian manner while the rest of the elements in the model are treated in a classical Lagrangian manner; • can be preceded by a static stress analysis or followed by a natural frequency extraction or a complex eigenvalue extraction step; • uses regular stress/displacement elements and special steady-state rolling and sliding contact pairs; • is currently available only for three-dimensional analysis with an axisymmetric geometry or a periodic geometry; and • allows rate-independent, rate-dependent, or history-dependent material behavior. Steady-state transport analysis It is cumbersome to model rolling and sliding contact, such as a tire rolling along a rigid surface or a disc rotating relative to a brake assembly, using a traditional Lagrangian formulation since the frame of reference in which motion is described is attached to the material. An observer in this reference frame views even steady-state rolling as a time-dependent process since each point undergoes a repeated history of deformation. Such an analysis is computationally expensive since a transient analysis must be performed and fine meshing is required along the entire surface of the cylinder. The steady-state transport analysis capability in Abaqus/Standard uses a reference frame that is attached to the axle of the rotating cylinder. An observer in this frame sees the cylinder as points that are not moving, although the material of which the cylinder is made is moving through those points. This removes the explicit time dependence from the problem—the observer sees a fixed point anywhere, with material moving through it. Thus, the finite element mesh describing the cylinder in this frame of reference does not undergo the large rigid body spinning motion. This means that a fine mesh is required only near the contact zone. This description can be viewed as a mixed Lagrangian/Eulerian method, where rigid body rotation is described in a spatial or Eulerian manner, and deformation, which is now measured relative to the rotating rigid body, is described in a material or Lagrangian manner. It is this kinematic description that converts the steady-state moving contact problem into a purely spatially dependent simulation. The steady-state rolling and sliding analysis capability provides solutions that include frictional effects, inertia effects, and material convection for most rate-independent, rate-dependent, and history- dependent material models. The theory is described in detail in “Steady-state transport analysis,” Section 2.7.1 of the Abaqus Theory Manual. Input File Usage: *STEADY STATE TRANSPORT Pass-by-pass analysis technique By default, the steady-state transport analysis procedure in Abaqus/Standard solves for a steady-state rolling and sliding solution directly as a series of increments, with iterations to obtain equilibrium within each increment. The solution in each increment is a steady-state solution corresponding to the loads acting on the structure at that instant. The steady-state transport analysis procedure also provides an alternative technique to obtain a quasi-steady-state rolling and sliding solution as a series of increments, with iterations to obtain equilibrium within each increment. However, the solution in each increment is usually not a steady-state solution corresponding to the loads acting on the structure at that instant. A steady-state solution is generally obtained in several increments, with each increment corresponding to a loading pass through the structure. Each loading pass through the structure can have a different magnitude. The pass-by-pass analysis technique is relevant only when used with plasticity/creep models. It has no effect on a viscoelastic material model. Input File Usage: *STEADY STATE TRANSPORT, PASS BY PASS Unstable problems Local instabilities (e.g., surface wrinkling, material instability, or local buckling), can occur in a steady- state transport analysis. Abaqus/Standard offers the option to stabilize this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1. Defining the model A steady-state transport analysis requires the definition of streamlines. The streamlines are the trajectories that the material follows during transport through the mesh. To meet this requirement, the mesh must be generated using the symmetric model generation capability, which is described in detail in “Symmetric model generation,” Section 10.4.1. The three-dimensional model can be created either by revolving an axisymmetric model about its axis of revolution or by revolving a single three-dimensional repetitive sector about its axis of symmetry. Revolving an axisymmetric cross-section to create a three-dimensional model You can generate a three-dimensional mesh by revolving a two-dimensional cross-section about In this case the symmetric model a symmetry axis, so that the streamlines follow the mesh lines. generation capability requires a two-dimensional cross-section of the body as a starting point. The cross-section, which must be discretized with axisymmetric finite elements, is defined in a separate input file. A data check analysis must be performed to write the model information to a restart file. The restart file is read in a subsequent run, and a three-dimensional model is generated by Abaqus/Standard by revolving the cross-section about the symmetry axis, starting at a reference plane. Both the symmetry axis and reference plane of the new three-dimensional model can be oriented in any direction in the global coordinate system. The symmetry axis also defines the axis of the spinning body. A nonuniform discretization in the circumferential direction can be specified to allow a finer mesh in the contact region than elsewhere in the model. Input File Usage: *SYMMETRIC MODEL GENERATION, REVOLVE Revolving a single three-dimensional sector to create a periodic model Alternatively, you can generate a periodic three-dimensional mesh by revolving a single To accurately account for the material three-dimensional sector about convection when the streamline integration is performed, the segment angle for the repetitive three-dimensional sector must be chosen small enough. its axis of symmetry. In this case the symmetric model generation capability requires a single three-dimensional sector as a starting point. The original three-dimensional sector is defined in a separate input file. A data check analysis must be performed to write the model information to a restart file. The restart file is read in a subsequent run, and a three-dimensional periodic model is generated by Abaqus/Standard by revolving the original three-dimensional sector about the symmetry axis. Both the symmetry axis and the original three-dimensional repetitive sector can be oriented in any direction in the global coordinate system. The symmetry axis also defines the axis of the spinning body. There is no restriction that the meshes on the two symmetry surfaces of the repetitive sector match in any way. If the surface meshes on either side of the original sector are not matched completely, constraints will be generated automatically to couple the opposing neighboring surfaces when revolving the original sector to create a periodic model. Input File Usage: *SYMMETRIC MODEL GENERATION, PERIODIC Identifying the elements being treated in an Eulerian manner By default, the rigid body motion in the whole model will be described in a spatial or Eulerian manner. In some cases you may want only part of the model to be treated with the Eulerian method while the rest should be treated with the classical Lagrangian method. One typical example is a disc brake where the disc itself can be treated with the Eulerian method while the brake assembly (brake pads and caliper) is treated with the Lagrangian method. In this case you can specify the name of an element set for which the rigid body motion will be described in an Eulerian manner. The elements that are not included in the element set will be treated with the classical Lagrangian method. Only one Eulerian element set can be specified in the whole model. In a new steady-state transport step or upon restart you can respecify a set of elements to be treated with the Eulerian method even after it has previously been treated with the Lagrangian method and vice versa. Elements treated with the Eulerian method and elements treated with the Lagrangian method cannot be mixed along a streamline. *STEADY STATE TRANSPORT, ELSET=name Input File Usage: Defining reference frame motions The deformable and rigid bodies can each be defined in their own moving reference frame in a steady- state rolling and sliding analysis. The motion of these reference frames can be defined quite generally and provides modeling of a spinning deformable body traveling along a straight line, or “cornering” or “precessing” around an axis. It is also possible to define reference frame motions for rigid bodies, including translations and rotations. The rigid body can be flat, convex, or concave, which allows for modeling of a deformable body in contact with a rotating drum, such as a tire rolling on a drum, or for modeling a tire mounted on a rigid rim. When defining different reference frame motions for bodies that interact, you must make sure that the interactions are indeed steady. For example, for a planar rigid surface the relative reference frame motion must be tangential to the rigid surface, and for a body of revolution the relative reference frame motion must be rotation around its axis. Spinning motion The spinning motion of the deformable body around its own axis is described by a user-specified angular velocity, . This angular velocity defines the transport of material through the mesh; you define the magnitude of the spinning rotation, . The axis of revolution is the symmetry axis used for generating the mesh as described in “Defining the model.” The transport velocity must be defined for all nodes on the spinning body. The magnitude of the angular velocity can also be defined with user subroutine UMOTION. The transport velocity can also be applied to a rigid body based on a three-dimensional surface of revolution. In that case the velocity is applied to the rigid body reference node to describe the transport of the (rigid) material relative to the reference node. Abaqus/Standard assumes that the rigid body spins around the axis of revolution of the rigid body. This option can, for example, be applied to the rigid body representing the rim on which a tire is mounted. Abaqus/Standard will automatically update the position and orientation of the rotation axis to the current configuration in a large-displacement analysis, such as in the case where a prescribed load applied to the reference node of a rotating rigid drum maintains the contact pressure between the tire and drum or the case where a camber angle is applied to the axle of the deformable body. Input File Usage: Use either of the following options: *TRANSPORT VELOCITY *TRANSPORT VELOCITY, USER Defining a reference frame for translational or rotational motion The rotating deformable body is also associated with a reference frame. This reference frame can either translate or rotate with respect to the fixed global reference frame. Similarly, each rigid body must be defined in a reference frame that is either fixed, translates, or rotates. For example, to associate straight line travel at ground velocity, , with a spinning deformable body, the deformable body can be defined in a reference frame translating at velocity and the rigid surface can be defined in a fixed reference frame. Alternatively, the deformable body can be defined in a reference frame that does not translate and the rigid body can be defined in a frame translating at velocity . Another example is a deformable body precessing along a circular path. In such a case a rotating frame is associated with the deformable body that defines the precession axis and angular velocity, while the rigid body is defined in a fixed reference frame. For this purpose you can apply a specified motion of the reference frame to all nodes of the deformable body or to the reference node of a rigid body. A translating reference frame is defined by specifying the components of the velocity vector, . A rotating reference frame is defined by specifying the magnitude of an angular rotation velocity, , and the position and orientation of the axis of rotation in the current configuration. The position and orientation of the axis are applied at the beginning of the step and remain fixed during the step. Input File Usage: Use the following option to define the motion of a translating reference frame: *MOTION, TRANSLATION Use the following option to define the motion of a rotating reference frame: *MOTION, ROTATION Contact conditions Abaqus/Standard provides contact between a rigid surface and deformable body moving with different velocities, such as contact between a rolling tire and the ground, as well as contact between surfaces moving with the same velocity, such as the contact between the bead and rim in a tire analysis. Abaqus/Standard also provides contact between two deformable bodies moving with the same velocity, such as the contact between the tread blocks on a tire surface, as well as contact between two deformable bodies moving with different velocities, such as the contact between a disc and brake assembly. Contact between a rigid surface and a deformable body moving with different velocities The rigid surface can be either an analytical surface or made from rigid elements. When the master and slave surfaces move with different velocities, you will normally select to use a Coulomb friction law that assumes that slip occurs if the frictional stress is equal to the critical stress the friction coefficient, and p is the contact pressure. No slip occurs when transport the condition of no slip is approximated in Abaqus/Standard by stiff “viscous” behavior are the shear stresses on the contact plane, is . For steady-state , where and where are the tangential slip velocities that depend on deformation along a streamline and is the “stick viscosity,” R is the radius of the cylinder, and is a user-defined slip tolerance for which the default is 0.005. Using a larger slip tolerance makes convergence of the solution more rapid at the expense of solution accuracy. Using a smaller slip tolerance imposes the “no relative motion” constraint more accurately but may slow convergence. The default value provides a conservative balance between efficiency and accuracy for rolling contact problems. Since this frictional model used for steady-state rolling is different from the frictional models used with other analysis procedures in Abaqus/Standard, discontinuities may arise in the solutions between a steady-state transport analysis and any other analysis procedure, such as a static footprint analysis. To ensure a smooth transition in the solution, it is recommended that all analysis steps prior to a steady- state rolling analysis use a zero coefficient of friction. You can then modify the friction properties in the steady-state transport analysis step to use the desired friction coefficient . This frictional model is more relevant in a tire analysis since the velocity of the rotating tire strongly depends on the deformation gradients along a streamline on the contact surface. The solution state at a material point depends on the solution of neighboring points, and convective effects must be considered. However, since the deformation gradients along a streamline on the contact surface are small in a disc brake analysis, a simplified frictional model, which ignores the convective effect on the contact surface, can be used. Such a frictional model is discussed in the following section. Contact between two deformable bodies moving with different velocities When the slave and master surfaces rotate with different velocities, such as contact between a disc and brake assembly, slip will develop between the two deformable surfaces. The transport velocity (“Spinning motion”) and the motion of a reference frame (“Defining a reference frame for translational or rotational motion”) can be defined in a steady-state transport analysis procedure to model the steady-state frictional sliding between two deformable bodies that are moving with different velocities. In this case it is assumed that the slip rate simply follows from the difference in velocities specified by the transport velocity and the motion of the reference frame and is independent of the deformation gradient along a streamline or the nodal displacements on the contact surface. No convective effects are considered between the contact surfaces, and the frictional stress does not depend on any history effects. Hence, the frictional stress is given by is the friction coefficient, p is the contact pressure, are the slip where velocities that are defined by the transport velocity and the motion of the reference frame. If no velocity or the same velocity are defined at contact nodes with friction, sticking conditions are applied automatically. The friction model is described in detail in “Coulomb friction,” Section 5.2.3 of the Abaqus Theory Manual. are the slip directions, and Such a simplified frictional model is relevant only in a disc brake analysis. It should be used with care in a rolling tire analysis where deformation gradients on the contact surface are significant. Since this frictional behavior is different from the frictional models used with other analysis procedures in Abaqus/Standard, discontinuities may arise in the solutions between a steady-state transport analysis and any other analysis procedure. An example is the discontinuity that occurs between the initial preloading of the disc pads in a disc brake system and the subsequent braking analysis where the disc spins with a prescribed rotation. To ensure a smooth transition in the solution, it is recommended that all analysis steps prior to a steady-state analysis use a zero coefficient of friction . You can then increase the friction coefficient to the desired value in the steady-state transport analysis . Contact between surfaces spinning with the same angular velocity When the slave and master surfaces rotate with the same angular velocity, such as the surface between In such a the bead and rim in a tire analysis, no relative velocity develops between the surfaces. case, frictional stresses develop as a reaction between the bodies. Abaqus/Standard will automatically determine that the slave and master surface rotate with the same speed and apply the standard Coulomb friction model, which is described in detail in “Frictional behavior,” Section 36.1.5. When the standard Coulomb friction model is used in a reference frame that implies flow of material through the mesh, convective effects must be considered. However, Abaqus/Standard assumes that no convective effects are present between surfaces during steady-state transport analysis. In other words, Abaqus/Standard assumes that the frictional stress at a point depends on the history of deformation in the Lagrangian reference frame and ignores any history effects that may occur as a result of the deformation that the point experiences during the spinning motion. The assumption that the frictional stress does not depend on history effects during rolling is valid for modeling contact between a tire bead and rim where relative slip occurs only during rim mounting in a static analysis prior to the steady-state transport analysis. When slip occurs during the steady-state transport analysis, the solution obtained is no longer the correct steady-state solution because convective effects are ignored. To ensure that no slip takes place between the surfaces during steady-state rolling, it is recommended that you modify the friction properties in the steady-state transport analysis step to activate rough friction . Incrementation Abaqus/Standard uses Newton’s method to solve the nonlinear equilibrium equations. The nonlinearities in a steady-state transport analysis arise from large-displacement effects, material nonlinearity, and boundary nonlinearities such as contact and friction. If geometrically nonlinear behavior is expected other than the large rigid body rotation associated with the steady-state motion, the step definition should include nonlinear geometric effects. The steady-state rolling and sliding solution must often be obtained as a series of increments, with iterations to obtain equilibrium within each increment. If the direct steady-state solution technique is used, the solution in each increment is a steady-state solution corresponding to the loads acting on the structure at that instant. If the pass-by-pass steady-state solution technique is used, the solution in each increment is usually not a steady-state solution corresponding to the loads acting on the structure at that instant. In this case a steady-state solution is generally obtained in several increments, with each increment corresponding to a loading pass through the structure. Since Newton’s method has a finite radius of convergence, too large an increment in the applied load can prevent any solution from being obtained because the current steady-state solution is too far away from the new steady-state equilibrium solution that is being sought: it is outside the radius of convergence. Thus, there is an algorithmic restriction on the increment size. Automatic incrementation In most cases the default automatic incrementation scheme is preferred because it will select increment sizes based on computational efficiency. Input File Usage: *STEADY STATE TRANSPORT Direct incrementation Direct user control of the increment size is also provided because if you have considerable experience with a particular problem, you may be able to select a more economical approach. Input File Usage: *STEADY STATE TRANSPORT, DIRECT Using the maximum number of iterations to determine the increment size The solution to an increment can be accepted after the maximum number of iterations allowed has been completed (as defined in “Commonly used control parameters,” Section 7.2.2), even if the equilibrium tolerances are not satisfied. This approach is not recommended; it should be used only in special cases when you have a thorough understanding of how to interpret results obtained in this way. Very small increments and a minimum of two iterations are usually necessary in this case. Input File Usage: *STEADY STATE TRANSPORT, DIRECT=NO STOP Convergence in a steady-state transport analysis The steady-state transport procedure may experience convergence difficulties in certain situations that are described below. Convergence issues with friction , and the traveling straight line velocity, The frictional forces that develop on the contact surface as a result of steady-state rolling are functions of the spinning angular velocity, . When these frictional forces are large, convergence of Newton’s method becomes difficult. Convergence problems in Abaqus/Standard are usually resolved by taking a smaller load increment. However, contact forces due to steady-state rolling usually do not reduce when the magnitudes of the velocities are reduced. For example, if a spinning object is prevented from moving ( ), full slipping conditions will develop over the entire contact zone for all values of spinning angular velocity . Consequently, the frictional force remains constant for all (provided that the normal force remains constant), so that smaller increments in the velocities ( ) do not reduce the magnitude of the frictional forces and, hence, do not overcome convergence difficulties. , or cornering velocity, To provide for convergence through the use of smaller increments in such cases, the friction coefficient can be increased from zero to the desired value over the analysis step. This is accomplished by setting the initial friction coefficient for the model to zero , then increasing the friction coefficient to its final value in the steady-state transport analysis step . Convergence issues with the Mullins effect material model If the Mullins effect material model is included in the material definition , there could be a strong discontinuity in the response of a structure in transitioning from a static (non-rolling) state to a steady-state rolling state. This discontinuity is due to the damage that occurs during the transient response (such as the damage that occurs as the structure undergoes its first revolution after static preloading). Since the transient response is not modeled during a steady-state transport analysis, the resulting discontinuity in the response can lead to convergence problems. The damage associated with the Mullins effect is independent of the angular speed of rotation: as a result, time increment cutbacks do not resolve the convergence problems. The Mullins effect can be ramped up over the time period of the step in these situations to obtain a converged solution. In such a case the change in response due to damage is applied gradually over the step. The solution at the end of the step corresponds to the fully damaged material; solutions during the step correspond to a partially damaged material and are, therefore, physically meaningless. Thus, it is recommended that in going from a static to a steady-state rolling solution, a do-nothing step at a low angular speed of rotation be first carried out with the Mullins effect ramped on. This facilitates resolution of the discontinuity in a gradual manner. The do-nothing step can then be followed by the regular steady-state transport step with the Mullins effect applied instantaneously at the beginning of the step. This approach is illustrated in “Analysis of a solid disc with Mullins effect and permanent set,” Section 3.1.7 of the Abaqus Example Problems Manual. Input File Usage: *STEADY STATE TRANSPORT, MULLINS=RAMP or STEP (default) Convergence issues with streamline integration in plasticity/creep models Although in principle any material point along a streamline can be used as a starting point for the streamline integration when material convective calculations are performed, Abaqus/Standard always uses the material points in the original sector or the material points in the original cross-section as starting points for the streamline integration in a model with periodic geometry or axisymmetric geometry, respectively. If the pass-by-pass solution technique is used, after an increment has been performed for all the streamlines, Abaqus/Standard will automatically use the state obtained at the end of the streamline as the starting state for the streamline integration in the subsequent increment. This iterative process is repeated for each increment until a steady-state solution is reached. If the direct steady-state solution technique is used, several local iterations are usually required for each streamline, with a local iteration corresponding to an integration over a closed loop streamline. After a local iteration has been performed for a streamline, Abaqus/Standard will check to see if the steady-state condition is satisfied for the streamline. This is best measured by ensuring the differences between the stresses/strains at the starting point of the streamline obtained before and after the iteration are sufficiently small. If the steady-state condition is not satisfied for the streamline, Abaqus/Standard will automatically use the state obtained at the end of the previous local iteration as the starting state for the streamline integration in the subsequent local iteration. This iterative process is repeated until a steady-state solution is reached for all the streamlines. To improve the rate of convergence, it is recommended that you apply loads on elements or nodes away from the starting points of the streamlines. Initial conditions Initial values of stresses, temperatures, field variables, solution-dependent state variables, etc. can be specified. “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the available initial conditions. Boundary conditions Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6). During the analysis prescribed boundary conditions can be varied using an amplitude definition . Loads Loading in a steady-state transport analysis includes the motion of the structure, inertia (d’Alembert) forces due to motion, concentrated loads, distributed pressures, and body forces. Inertia effects The motion of the deformable body gives rise to inertia (d’Alembert) forces that can be included. These forces include centrifugal and Coriolis effects. The density of the material must be defined in the material description. At higher rotational velocities, inertia forces can give rise to instabilities in the form of standing waves, which are likely to prevent convergence of the Newton algorithm. Input File Usage: Use the following option to include inertia forces: *STEADY STATE TRANSPORT, INERTIA=YES Inertia loads for tetrahedral elements Inertia loads for tetrahedral elements C3D4, C3D10, C3D10I, and C3D10M are not taken into account in a steady-state transport analysis. Tetrahedral elements will appear only in a periodic model created by revolving a three-dimensional sector that contains tetrahedral elements. Tetrahedral elements will not appear in an axisymmetric model created by revolving a two-dimensional cross-section about a symmetry axis. See “Symmetric model generation,” Section 10.4.1, for details. Other prescribed loads The following loads can be prescribed in a steady-state transport analysis, as described in “Concentrated loads,” Section 33.4.2: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6). • Distributed pressure forces or body forces can be applied; the distributed load types available with particular elements are described in Part VI, “Elements.” In most cases such loads should be applied around the whole circumference of the body; a load on a single point or element corresponds to a spatially fixed load, which in most cases is not realistic. Predefined fields The following predefined fields can be specified in a steady-state transport analysis, as described in “Predefined fields,” Section 33.6.1: • Although temperature is not a degree of freedom in a steady-state transport analysis, nodal temperatures can be specified as a predefined field. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any. • The values of user-defined field variables can be specified. These values only affect field-variable- dependent material properties, if any. Material options Since the steady-state transport capability uses a kinematic description that implies flow of material through the mesh, convective effects must be considered for the material response. Most material models that describe mechanical behavior (including user-defined materials) are available for use in a steady-state transport analysis. In particular, history-dependent viscoelasticity (“Time domain viscoelasticity,” Section 22.7.1), history-dependent Mullins effect (“Mullins effect,” Section 22.6.1), classical metal plasticity (“Classical metal plasticity,” Section 23.2.1), rate-dependent yield (“Rate-dependent yield,” Section 23.2.3), rate-dependent creep (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4), and two-layer viscoplasticity (“Two-layer viscoplasticity,” Section 23.2.11) can all be used during a steady-state transport analysis. The following material properties are not active during a steady-state transport analysis: thermal properties (except for thermal expansion), mass diffusion properties, electrical properties, and pore fluid flow properties. Abaqus/Standard also provides the ability to obtain the fully relaxed long-term elastic or elastic- plastic solution during a steady-state transport analysis if the material description includes viscoelastic or viscoplastic material properties. If the material description includes viscoelastic material properties, the long-term solution will ignore the material convection calculations. If the two-layer viscoplastic material model is used, the long-term solution will include only the material convection calculations based on the long-term response of the elastic-plastic network. Input File Usage: *STEADY STATE TRANSPORT, LONG TERM Choosing an appropriate material model Since material points in a spinning and sliding body undergo repeated loading/unloading cycles, an appropriate material model must be chosen to characterize the response correctly under such loading conditions. The use of plasticity material models with isotropic type hardening is generally not recommended since they will continue to harden during cyclic loading, which may lead to a large number of iterations until the steady-state solution is reached. Kinematic hardening plasticity models should be used to model the inelastic behavior of materials that are subjected to repeated loading. For rate-dependent creep, is recommended (“Two-layer the two-layer viscoplasticity model viscoplasticity,” Section 23.2.11) for modeling the response of materials with significant time-dependent behavior as well as plasticity at elevated temperatures. For history-dependent viscoelasticity, it is more appropriate to use cyclic (frequency domain) test data to calibrate the time-domain viscoelastic material model for steady-state transport analysis. The cyclic experiments should be performed in the frequency range anticipated in the rolling simulation. Abaqus/Standard internally converts the frequency domain storage and loss modulus data into a time- domain (Prony series) representation. This data conversion capability is described in detail in “Time domain viscoelasticity,” Section 22.7.1. Analysis steps prior to a steady-state transport analysis It is recommended that the solutions in any analysis step prior to a steady-state transport analysis, such as a static footprint or preloading solution, be based on the long-term elastic moduli or the long-term elastic-plastic response if viscoelastic or viscoplastic material properties are used (for example, see “Static stress analysis,” Section 6.2.2). The long-term solution provides a smooth transition between a static analysis and a slow rolling or sliding steady-state transport analysis. Material convection in nonlinear analysis When material convection is included in the steady-state transport solution, Abaqus/Standard uses an approximate Jacobian matrix in the Newton solution of the nonlinear equilibrium equations. The rate of convergence in such a case is no longer quadratic but depends strongly on the severity of the nonlinearities. It is often necessary to adjust the default solution controls (“Commonly used control parameters,” Section 7.2.2) to obtain a steady-state transport solution when material convection is considered. Elements the three-dimensional stress/displacement elements in Abaqus/Standard can be used Most of in a steady-state transport analysis . When the three-dimensional model is generated from an axisymmetric cross-section, the element type used in the two-dimensional model determines the element type in the three-dimensional The correspondence between the two-dimensional and three-dimensional element types model. is described in “Symmetric model generation,” Section 10.4.1. If the three-dimensional periodic model is generated from a single three-dimensional sector, any of the stress/displacement elements in Abaqus/Standard can be used. Output The element output available for a steady-state transport analysis includes stress, strain, energies, and the values of state, field, and user-defined variables. The nodal output available includes displacements, velocities, reaction forces, and coordinates. The contact output variable CSLIP contains steady-state slip rates for the steady-state transport procedure, unlike the usual definition of this variable. All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Limitations The steady-state transport analysis capability has several limitations. • The deformable structure must be a full 360° cylindrical body of revolution. Convective boundary conditions are not available to model segments of a cylinder. • The capability is not available in two dimensions. • Only one deformable spinning body is permitted. The symmetric model generation capability must be used to generate the deformable body (“Symmetric model generation,” Section 10.4.1). Input file template *HEADING … *SYMMETRIC MODEL GENERATION, REVOLVE Data lines to define model generation *SURFACE INTERACTION *FRICTION Specify zero friction coefficient ** *STEP *STATIC Data lines to define analysis steps prior to transport analysis *END STEP … *STEP *STEADY STATE TRANSPORT Data line to define incrementation *CHANGE FRICTION *FRICTION Data lines to redefine friction coefficient *BOUNDARY Data lines to define boundary conditions *TRANSPORT VELOCITY Data lines to define spinning angular velocity *MOTION, TRANSLATION or ROTATION Data lines to define traveling velocity or cornering rotational velocity *EL PRINT and/or *NODE PRINT Data lines to request output variables *END STEP 6.5 Heat transfer and thermal-stress analysis • “Heat transfer analysis procedures: overview,” Section 6.5.1 • “Uncoupled heat transfer analysis,” Section 6.5.2 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Adiabatic analysis,” Section 6.5.4 6.5.1 HEAT TRANSFER ANALYSIS PROCEDURES: OVERVIEW Abaqus can solve the following types of heat transfer problems: • Uncoupled heat transfer analysis: Heat forced convection, and boundary radiation can be analyzed in Abaqus/Standard. See “Uncoupled heat transfer analysis,” Section 6.5.2. In these analyses the temperature field is calculated without knowledge of the stress/deformation state or the electrical field in the bodies being studied. Pure heat transfer problems can be transient or steady-state and linear or nonlinear. transfer problems involving conduction, • Sequentially coupled thermal-stress analysis: If the stress/displacement solution is dependent on a temperature field but there is no inverse dependency, a sequentially coupled thermal-stress analysis can be conducted in Abaqus/Standard. Sequentially coupled thermal-stress analysis is performed by first solving the pure heat transfer problem, then reading the temperature solution into a stress analysis as a predefined field. See “Sequentially coupled thermal-stress analysis,” Section 16.1.2. In the stress analysis the temperature can vary with time and position but is not changed by the stress analysis solution. Abaqus allows for dissimilar meshes between the heat transfer analysis model and the thermal-stress analysis model. Temperature values will be interpolated based on element interpolators evaluated at nodes of the thermal-stress model. • Fully coupled thermal-stress analysis: A coupled temperature-displacement procedure is used to solve simultaneously for the stress/displacement and the temperature fields. A coupled analysis is used when the thermal and mechanical solutions affect each other strongly. For example, in rapid metalworking problems the inelastic deformation of the material causes heating, and in contact problems the heat conducted across gaps may depend strongly on the gap clearance or pressure. Both Abaqus/Standard and Abaqus/Explicit provide coupled temperature-displacement analysis procedures, but the algorithms used by each program differ considerably. In Abaqus/Standard the heat transfer equations are integrated using a backward-difference scheme, and the coupled system is solved using Newton’s method. These problems can be transient or steady-state and linear or nonlinear. In Abaqus/Explicit the heat transfer equations are integrated using an explicit forward-difference time integration rule, and the mechanical solution response is obtained using an explicit central-difference integration rule. Fully coupled thermal-stress analysis in Abaqus/Explicit is always transient. Cavity radiation effects cannot be included in a fully coupled thermal-stress analysis. See “Fully coupled thermal-stress analysis,” Section 6.5.3, for more details. • Fully coupled thermal-electrical-structural analysis: A coupled thermal-electrical-structural procedure is used to solve simultaneously for the stress/displacement, the electrical potential, and the temperature fields. A coupled analysis is used when the thermal, electrical, and mechanical solutions affect each other strongly. An example of such a process is resistance spot welding, where two or more metal parts are joined by fusion at discrete points at the material interface. The fusion is caused by heat generated due to the current flow at the contact points, which depends on the pressure applied at these points. These problems can be transient or steady-state and linear or nonlinear. Cavity radiation effects cannot be included in a fully coupled thermal-electrical-structural analysis. This procedure is available only in Abaqus/Standard. See “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4, for more details. • Adiabatic analysis: An adiabatic mechanical analysis can be used in cases where mechanical deformation causes heating, but the event is so rapid that this heat has no time to diffuse through the material. Adiabatic analysis can be performed in Abaqus/Standard or Abaqus/Explicit; see “Adiabatic analysis,” Section 6.5.4. An adiabatic analysis can be static or dynamic and linear or nonlinear. • Coupled thermal-electrical analysis: A fully coupled thermal-electrical analysis capability is provided in Abaqus/Standard for problems where heat is generated due to the flow of electrical current through a conductor. See “Coupled thermal-electrical analysis,” Section 6.7.3. • Cavity radiation: In Abaqus/Standard cavity radiation effects can be included (in addition to prescribed boundary radiation) in uncoupled heat transfer problems. See “Cavity radiation,” Section 40.1.1. The cavities can be open or closed. Symmetries and blocking within cavities can be modeled. Viewfactors are calculated automatically, and motion of objects bounding a cavity can be prescribed during the analysis. Cavity radiation problems are nonlinear and can be transient or steady-state. 6.5.2 UNCOUPLED HEAT TRANSFER ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Heat transfer analysis procedures: overview,” Section 6.5.1 • *HEAT TRANSFER • “Including volumetric heat generation in heat Abaqus/CAE User’s Manual, in the online HTML version of this manual transfer analyses,” Section 12.10.2 of the • “Configuring a heat transfer procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Uncoupled heat transfer problems: • are those in which the temperature field is calculated without consideration of the stress/deformation or the electrical field in the bodies being studied; • can include conduction, boundary convection, and boundary radiation; • can include cavity radiation effects—see “Cavity radiation,” Section 40.1.1; • can include forced convection through the mesh if forced convection/diffusion heat transfer elements are used; • can include thermal interactions such as gap radiation, conductance, and heat generation between contact surfaces—see “Thermal contact properties,” Section 36.2.1; • can include thermal material behavior defined in user subroutine UMATHT—see “User-defined thermal material behavior,” Section 26.7.2; • can be transient or steady-state; • can be linear or nonlinear; and • require the use of heat transfer elements. Heat transfer analysis Uncoupled heat transfer analysis is used to model solid body heat conduction with general, temperature- dependent conductivity, internal energy (including latent heat effects), and quite general convection and radiation boundary conditions, including cavity radiation. Forced convection of a fluid through the mesh can be modeled by using forced convection/diffusion elements. Sources of nonlinearity in a heat transfer analysis Heat transfer problems can be nonlinear because the material properties are temperature dependent or because the boundary conditions are nonlinear. Usually the nonlinearity associated with temperature- dependent material properties is mild because the properties do not change rapidly with temperature. However, when latent heat effects are included, the analysis may be severely nonlinear . Boundary conditions are very often nonlinear; for example, film coefficients can be functions of surface temperature. Again, the nonlinearities are often mild and cause little difficulty. An exception is the “boiling” film condition, in which the film coefficient can change very rapidly because the fluid adjacent to the surface boils. A rapidly changing film condition (within a step or from one step to another) can be modeled easily using temperature-dependent and field-variable-dependent film coefficients. Radiation effects always make heat transfer problems nonlinear. Nonlinearities in radiation grow as temperatures increase. Abaqus/Standard uses an iterative scheme to solve nonlinear heat transfer problems. The scheme uses the Newton method with some modification to improve stability of the iteration process in the presence of highly nonlinear latent heat effects. Steady-state cases involving severe nonlinearities are sometimes more effectively solved as transient cases because of the stabilizing influence of the heat capacity terms. The required steady-state solution can be obtained as the very long transient time response; the transient will simply stabilize the solution for that long time response. Matrix storage and solution scheme In heat transfer analyses involving cavity radiation or forced convection/diffusion elements, the system of equations is unsymmetric. The nonsymmetric matrix storage and solution scheme is invoked automatically in these cases . Steady-state analysis Steady-state analysis means that the internal energy term (the specific heat term) in the governing heat transfer equation is omitted. The problem then has no intrinsic physically meaningful time scale. Nevertheless, you can assign an initial time increment, a total time period, and maximum and minimum allowed time increments to the analysis step, which is often convenient for output identification and for specifying prescribed temperatures and fluxes with varying magnitudes. Any fluxes or boundary condition changes to be applied during a steady-state heat transfer step should be given within the step, using appropriate amplitude references to specify their “time” variations (“Amplitude curves,” Section 33.1.2). If fluxes and boundary conditions are specified for the step without amplitude references, they are assumed to change linearly with “time” during the step, from their magnitudes at the end of the previous step (or zero, if this is the beginning of the analysis) to their newly specified magnitudes at the end of the heat transfer step. Input File Usage: *HEAT TRANSFER, STEADY STATE Abaqus/CAE Usage: Step module: Create Step: General: Heat transfer: Response: Steady state Automatic incrementation When steady-state analysis is chosen, you suggest an initial “time” increment and define a “time” period for the step; Abaqus/Standard then increments through the step accordingly. By default, Abaqus/Standard automatically determines a suitable increment size for each increment of the step. Fixed incrementation You can also use a fixed incrementation scheme, in which Abaqus/Standard uses the same increment size for the duration of the step. The suggested initial “time” increment, , defines the increment size. Input File Usage: Set the initial increment, minimum increment size, and maximum increment size to the same value: *HEAT TRANSFER, STEADY STATE , , , Abaqus/CAE Usage: Step module: Create Step: General: Heat transfer: Response: Steady-state: Incrementation: Type: Fixed: Increment size: Transient analysis Time integration in transient problems is done with the backward Euler method (sometimes also referred to as the modified Crank-Nicholson operator) in the pure conduction elements. This method is unconditionally stable for linear problems. The forced convection/diffusion elements use the trapezoidal rule for time integration. They include numerical diffusion control (the “upwinding” Petrov-Galerkin method) and, optionally, numerical dispersion control. The elements with dispersion control offer improved solution accuracy in cases where the transient response of the fluid is important. Artificial dispersion control introduces a stability limit on the size of the time increment such that the local Courant number is the time increment, is the magnitude of the velocity vector, and must be less than 1, where is a characteristic element length in the direction of flow; that is, heat cannot be convected across more than one element length, , in a single increment of time. In a uniform velocity field the smallest element will dictate the stable time increment. Approximate calculation of the Courant number, C, is helpful during the mesh design stages so that excessively small stable time increments can be avoided. The elements without dispersion control have no such stability limit; therefore, it may be more economical to use the elements without this feature in transient cases where transient effects in the fluid itself are not a critical part of the solution (for example, when the important solution is the temperature field in the solid bodies that are included in the model, and when characteristic transient times in the fluid are very much shorter than characteristic transient times in the solids). Time incrementation in a transient heat transfer analysis can be controlled directly by you or automatically by Abaqus/Standard. Automatic time incrementation is generally preferred. Automatic incrementation The time increments can be selected automatically based on the user-prescribed maximum allowable nodal temperature change in an increment, . Abaqus/Standard will restrict the time increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the analysis . Input File Usage: Abaqus/CAE Usage: *HEAT TRANSFER, DELTMX= Step module: Create Step: General: Heat transfer: Response: Transient: Incrementation: Type: Automatic: Max. allowable temperature change per increment: Fixed incrementation If you select direct incrementation and do not specify specified initial time increment, , will then be used throughout the analysis. , fixed time increments equal to the user- Input File Usage: *HEAT TRANSFER Abaqus/CAE Usage: Step module: Create Step: General: Heat transfer: Response: Transient: Incrementation: Type: Fixed: Increment size: Spurious oscillations due to small time increments In transient heat transfer analysis with second-order elements there is a relationship between the minimum usable time increment and the element size. A simple guideline is is the time increment, is the density, c is the specific heat, k is the thermal conductivity, where and is a typical element dimension (such as the length of a side of an element). If time increments smaller than this value are used in a mesh of second-order elements, spurious oscillations can appear in the solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations are nonphysical and may cause problems if temperature-dependent material properties are present. Abaqus/Standard provides no check on the user-defined initial time increment; you must ensure that the given value does not violate the above criterion. In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates such oscillations but can lead to locally inaccurate solutions especially in terms of the heat flux for small time increments. If smaller time increments are required, a finer mesh should be used in regions where the temperature changes occur. Unless you specify a maximum allowable time increment size as part of the heat transfer step definition, there is no upper limit on the time increment size (the integration procedure is unconditionally stable, at least for linear problems). However, if forced convection/diffusion elements including numerical dispersion control (element types DCCxxD) are included in the model, there is a numerical stability limit on the allowable time increment. The requirement is that , where is a characteristic element length in the direction of is the magnitude of the fluid velocity and flow. Abaqus/Standard will adjust the time increment automatically to satisfy this stability limit. Ending a transient analysis A transient analysis can be terminated by completing a specified time period, or it can be continued until steady-state conditions are reached. By default, the analysis will end when the given time period has been completed. Alternatively, you can specify that the analysis will end when steady state is reached or after the given time period, whichever comes first. Steady state is defined by the temperature change rate: when the temperature at every temperature degree of freedom changes at a rate that is less than the user-specified rate (given as part of the step definition), the analysis terminates. Input File Usage: Use the following option to end the analysis when the time period is reached: *HEAT TRANSFER, END=PERIOD (default) Use the following option to end the analysis based on the temperature change rate: *HEAT TRANSFER, END=SS Step module: Create Step: General: Heat transfer: Response: Transient: Incrementation: End step when temperature change is less than Abaqus/CAE Usage: Internal heat generation Volumetric heat generation within a material can be defined either in user subroutine HETVAL or user subroutine UMATHT. These user subroutines are mutually exclusive. Defining internal heat generation in user subroutine HETVAL If user subroutine HETVAL is used to define internal heat generation, heat generation must be included in the material definition with the other thermal property definitions. Heat generation might be associated with (relatively low) energy phase changes occurring during the solution. Such heat generation usually depends on state variables (such as the fraction transformed), which themselves evolve with the solution and are stored as solution-dependent state variables . The heat generation is computed in user subroutine HETVAL, where any associated state variables can also be updated. The subroutine will be called at all material calculation points for which the material definition includes heat generation. *HEAT GENERATION Property module: material editor: Thermal: Heat Generation Abaqus/CAE Usage: Input File Usage: Defining internal heat generation in user subroutine UMATHT If user subroutine UMATHT is used to define internal heat generation, all other thermal properties must also be defined within the subroutine. Input File Usage: Abaqus/CAE Usage: *USER MATERIAL Property module: material editor: General: User Material: User material type: Thermal Forced convection through the mesh The velocity of a fluid moving through the mesh can be prescribed if forced convection/diffusion heat transfer elements are used. Conduction between the fluid and adjacent forced convection/diffusion heat transfer elements will be affected by the mass flow rate of the fluid. For example, if a pipe is filled with a fluid with an initial temperature profile that contains a temperature pulse, the initial temperature pulse will not only diffuse (because of conduction in the fluid and the pipe), but it will also be transported (or convected) down the pipe. Since the fluid velocity is prescribed, it is called forced convection. Natural convection occurs when differences in fluid density created by thermal gradients cause motion of the fluid (bouyancy-driven flow). The forced convection/diffusion elements are not designed to handle this phenomenon; the flow must be prescribed. You can specify the mass flow rates per unit area (or through the entire section for one-dimensional elements) at the nodes. Abaqus/Standard interpolates the mass flow rates to the material points. The numerical solution of the transient heat transfer equation including convection becomes increasingly difficult as convection dominates diffusion. The Peclet number, , is a dimensionless parameter that indicates the degree of convection dominance over diffusion: is the magnitude of the velocity vector, where conductivity, and that convection dominates over diffusion on the spatial scale defined by the element size, Peclet numbers greater than about 1000 should not be used. is the density, c is the specific heat, k is the thermal indicate . In general, is a characteristic element length in the direction of flow. Large values of Petrov-Galerkin finite elements are used in Abaqus/Standard to model systems with high Peclet numbers accurately; these elements use nonsymmetric, upwinded weighting functions to control numerical diffusion and dispersion and, thus, stabilize results. The upwinding term is partly a function of the element Peclet number, as described in “Convection/diffusion,” Section 2.11.3 of the Abaqus Theory Manual. If the fluid flows along a boundary along which a rapid change of temperature is prescribed, it is, in fact, subjected to a thermal transient, even for steady-state analysis. This transient can give rise to the same kind of spurious temperature oscillations that are observed in transient heat transfer analysis, as discussed earlier in this section. Since Abaqus/Standard uses first-order elements for convective heat transfer, the oscillation can be eliminated by lumping the heat capacity terms. However, the upwinded weighting functions prevent lumping in the direction of the flow. Hence, spurious oscillations may still occur, in particular if the flow is not precisely tangential to the boundary along which the temperature change occurs. Input File Usage: Use the following option within the heat transfer step definition to prescribe the fluid velocity: *MASS FLOW RATE Abaqus/CAE Usage: Mass flow rate is not supported in Abaqus/CAE. Modifying or removing mass flow rates By default, the mass flow rates given are modifications of existing flow rates or are to be applied in addition to any mass flow rates defined previously. You can remove all previously defined mass flow rates and, optionally, specify new mass flow rates. Input File Usage: Use the following option to modify an existing flow rate or to specify an additional flow rate: *MASS FLOW RATE, OP=MOD (default) Use the following option to release all previously applied flow rates and to specify new flow rates: *MASS FLOW RATE, OP=NEW Abaqus/CAE Usage: Mass flow rate is not supported in Abaqus/CAE. Specifying time-dependent mass flow rates Mass flow rates can be given in combination with an amplitude definition, if required, to control the magnitude of the flow rate as a function of time (“Amplitude curves,” Section 33.1.2). Input File Usage: Use both of the following options to define a time-dependent mass flow rate: *AMPLITUDE, NAME=name *MASS FLOW RATE, AMPLITUDE=name Abaqus/CAE Usage: Mass flow rate is not supported in Abaqus/CAE. Defining mass flow rates in a user subroutine Mass flow rates can be defined by user subroutine UMASFL. UMASFL will be called for each specified node. Any mass flow rate values given directly will be ignored. Input File Usage: *MASS FLOW RATE, USER Abaqus/CAE Usage: Mass flow rate is not supported in Abaqus/CAE. Reading the mass flow rate data from an alternate file The data for the mass flow rate can be contained in an alternate file. See “Input syntax rules,” Section 1.2.1, for the syntax of the file name. Input File Usage: *MASS FLOW RATE, INPUT=file_name Abaqus/CAE Usage: Mass flow rate is not supported in Abaqus/CAE. Cavity radiation Cavity radiation can be activated in a heat transfer step. This feature involves interacting heat transfer between all of the facets of the cavity surface, dependent on the facet temperatures, facet emissivities, and the geometric viewfactors between each facet pair. When the thermal emissivity is a function of temperature or field variables, you can specify the maximum allowable emissivity change during an increment in addition to the maximum temperature change to control the time incrementation. See “Cavity radiation,” Section 40.1.1, for more information. Input File Usage: Use the following option in the step definition to activate cavity radiation: *RADIATION VIEWFACTOR Use the following option to specify the maximum allowable emissivity change: *HEAT TRANSFER, MXDEM=max_delta_emissivity You can specify the maximum allowable emissivity change for a heat transfer step. Step module: Create Step: General: Heat transfer: Incrementation: Max. allowable emissivity change per increment Abaqus/CAE Usage: Initial conditions By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures . Forced convection through the mesh In a heat transfer analysis involving forced convection through the mesh, you can define nonzero initial mass flow rates at the nodes of the forced convection/diffusion heat transfer elements in the model, as described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. For element types DCC1D2 and DCC1D2D the mass flow rate is positive from the first to the second node of the element. For two- and three-dimensional elements the direction of the mass flow rate is defined by giving the components in the x-, y-, and z-directions. Input File Usage: *INITIAL CONDITIONS, TYPE=MASS FLOW RATE Abaqus/CAE Usage: Mass flow rate is not supported in Abaqus/CAE. Boundary conditions Boundary conditions can be used to prescribe temperatures (degree of freedom 11) at nodes in a heat transfer analysis . Shell elements have additional temperature degrees of freedom 12, 13, etc. through the thickness . Boundary conditions can be specified as functions of time by referring to amplitude curves . For purely diffusive heat transfer elements a boundary without any prescribed boundary conditions (natural boundary condition) corresponds to an insulated surface. For forced convection/diffusion elements only the flux associated with conduction is zero; energy is free to convect across an unconstrained surface. This natural boundary condition correctly models areas where fluid is crossing a surface (as, for example, at the upstream and downstream boundaries of the mesh) and prevents spurious reflections of energy back into the mesh. Loads The following types of loading can be prescribed in a heat transfer analysis, as described in “Thermal loads,” Section 33.4.4: • Concentrated heat fluxes. • Body fluxes and distributed surface fluxes. • Average-temperature radiation conditions. • Convective film conditions and radiation conditions; film properties can be made a function of temperature. Cavity radiation effects can also be included, as described in “Cavity radiation,” Section 40.1.1. Predefined fields Predefined temperature fields are not allowed in heat transfer analyses. Boundary conditions should be used instead to specify temperatures, as described earlier. Other predefined field variables can be specified in a heat transfer analysis. These values will affect field-variable-dependent material properties, if any. See “Predefined fields,” Section 33.6.1. Material options The thermal conductivity of the materials in a heat transfer analysis must be defined. The specific heat and density of the materials must also be defined for transient heat transfer problems. Latent heat can be defined for diffusive heat transfer elements if changes in internal energy due to phase changes are important. Latent heat cannot be defined directly for forced convection/diffusion elements. See “Thermal properties: overview,” Section 26.2.1, for details on defining thermal properties in Abaqus. Alternatively, user subroutine UMATHT can be used to define the thermal constitutive behavior of the material, including internal heat generation. For example, if a material modeled can go through a complex phase change, the specific heat can be defined in user subroutine UMATHT in sufficient detail to capture the phase change. Thermal expansion coefficients are not meaningful in an uncoupled heat transfer analysis problem since deformation of the structure is not considered. Elements The heat transfer element library in Abaqus/Standard includes diffusive heat transfer elements, which allow for heat storage (specific heat and latent heat effects) and heat conduction. Forced convection/diffusion heat transfer elements are also available: in addition to heat storage and heat conduction these elements allow for forced convection caused by fluid flowing through the mesh. These elements cannot be used with latent heat—see “Solid (continuum) elements,” Section 28.1.1, for additional details. Forced convection/diffusion elements with dispersion control are available for problems where the temperature transient in the fluid must be calculated accurately. See “Choosing the appropriate element for an analysis type,” Section 27.1.3. Multiple temperatures are available through the thickness of shell heat transfer elements. See “Choosing a shell element,” Section 29.6.2. The first-order heat transfer elements (such as the 2-node link, 4-node quadrilateral, and 8-node brick) use a numerical integration rule with the integration stations located at the corners of the element for the heat capacitance terms and for the calculations of the distributed surface fluxes. First-order diffusive elements are preferred in cases involving latent heat effects since they use such a special integration technique to provide accurate solutions with large latent heats. The forced convection/diffusion elements cannot use this special integration technique and, therefore, are unsuitable for problems with latent heat effects. The second-order heat transfer elements use conventional Gaussian integration. Thus, the second-order elements are to be preferred for problems when the solution will be smooth (without latent heat effects), and usually give more accurate results for the same number of nodes in the mesh. Thermal interactions between adjacent surfaces and thermal gap elements are also provided to model heat transfer across the boundary layer between a solid and a fluid or between two closely adjacent solids. See “Thermal contact properties,” Section 36.2.1. Output The following heat transfer output variables are available: Element integration point variables: HFL HFLn HFLM TEMP MFR MFRn Magnitude and components of the heat flux vector. Component n of the heat flux vector (n=1, 2, 3). Magnitude of the heat flux vector. Integration point temperatures. User-specified mass flow rates. Component n of the mass flow rate (n=1, 2, 3). Whole element variables: FLUXS NFLUX FILM RAD Nodal variables: NT NTn RFL RFLn CFL CFLn Current values of uniform distributed heat fluxes. Fluxes at the nodes caused by heat conduction (internal fluxes). Current values of film conditions. Current values of radiation conditions. Nodal point temperatures. Temperature degree of freedom n at a node (n=11, 12, …). Reaction flux values due to prescribed temperature. Reaction flux value n at a node (n=11, 12, …). Concentrated flux values. Concentrated flux value n at a node (n=11, 12, …). RFLE Total flux at a node, including flux convected through the node in forced convection/diffusion elements but excluding external fluxes due to user-defined concentrated fluxes, distributed fluxes, film conditions, radiation conditions, and cavity radiation. Since RFLE is a scalar nodal output variable, care should be taken when summing it over on two surfaces with shared nodes. If node sets on both surfaces include the shared nodes, the output of RFLE on the common nodes will contribute to the sums of this output quantity on both surfaces. RFLEn Total flux value n at a node (n=11, 12, …). All of the output variables available in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Input file template *HEADING … *PHYSICAL CONSTANTS, ABSOLUTE ZERO= *INITIAL CONDITIONS, TYPE=TEMPERATURE Data lines to prescribe initial temperatures at the nodes *AMPLITUDE, NAME=trefamp Data lines to define amplitude curve to be used for radiation reference temperature, *FILM PROPERTY, NAME=film Data lines to define the convection film coefficient, h, as a function of temperature ** *STEP Transient analysis including forced convection through the mesh *HEAT TRANSFER, END=SS, DELTMX= Data line to define incrementation and steady state ** *CFLUX and/or *DFLUX Data lines to define concentrated and/or distributed fluxes *FILM Data lines referring to film property table film *RADIATE, AMPLITUDE=trefamp Data lines to define boundary radiation ** *EL PRINT TEMP, HFL NFLUX, FILM, RAD *NODE PRINT NT11, RFL *END STEP 6.5.3 FULLY COUPLED THERMAL-STRESS ANALYSIS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Heat transfer analysis procedures: overview,” Section 6.5.1 • *COUPLED TEMPERATURE-DISPLACEMENT • *DYNAMIC TEMPERATURE-DISPLACEMENT • “Specifying an inelastic heat fraction,” Section 12.10.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Configuring a fully coupled, simultaneous heat transfer and stress procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Configuring a dynamic fully coupled thermal-stress procedure using explicit integration” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A fully coupled thermal-stress analysis: • is performed when the mechanical and thermal solutions affect each other strongly and, therefore, must be obtained simultaneously; • requires the existence of elements with both temperature and displacement degrees of freedom in the model; • can be used to analyze time-dependent material response; • cannot include cavity radiation effects but may include average-temperature radiation conditions ; and • takes into account temperature dependence of material properties only for the properties that are assigned to elements with temperature degrees of freedom. In Abaqus/Standard a fully coupled thermal-stress analysis: • neglects inertia effects; and • can be transient or steady-state. In Abaqus/Explicit a fully coupled thermal-stress analysis: • includes inertia effects; and • models transient thermal response. Fully coupled thermal-stress analysis Fully coupled thermal-stress analysis is needed when the stress analysis is dependent on the temperature distribution and the temperature distribution depends on the stress solution. For example, metalworking problems may include significant heating due to inelastic deformation of the material which, in In addition, contact conditions exist in some problems where turn, changes the material properties. the heat conducted between surfaces may depend strongly on the separation of the surfaces or the pressure transmitted across the surfaces . For such cases the thermal and mechanical solutions must be obtained simultaneously rather than sequentially. Coupled temperature-displacement elements are provided for this purpose in both Abaqus/Standard and Abaqus/Explicit; however, each program uses different algorithms to solve coupled thermal-stress problems. Fully coupled thermal-stress analysis in Abaqus/Standard In Abaqus/Standard the temperatures are integrated using a backward-difference scheme, and the nonlinear coupled system is solved using Newton’s method. Abaqus/Standard offers an exact as well as an approximate implementation of Newton’s method for fully coupled temperature-displacement analysis. Exact implementation An exact implementation of Newton’s method involves a nonsymmetric Jacobian matrix as is illustrated in the following matrix representation of the coupled equations: and where are submatrices of the fully coupled Jacobian matrix, and residual vectors, respectively. are the respective corrections to the incremental displacement and temperature, and are the mechanical and thermal Solving this system of equations requires the use of the unsymmetric matrix storage and solution scheme. Furthermore, the mechanical and thermal equations must be solved simultaneously. The method provides quadratic convergence when the solution estimate is within the radius of convergence of the algorithm. The exact implementation is used by default. Approximate implementation Some problems require a fully coupled analysis in the sense that the mechanical and thermal solutions evolve simultaneously, but with a weak coupling between the two solutions. In other words, the components in the off-diagonal submatrices are small compared to the components in the diagonal submatrices . An example of such a situation is the disc brake problem (“Thermal-stress analysis of a disc brake,” Section 5.1.1 of the Abaqus Example Problems Manual). For these problems a less costly solution may be obtained by setting the off-diagonal submatrices to zero so that we obtain an approximate set of equations: , , As a result of this approximation the thermal and mechanical equations can be solved separately, with fewer equations to consider in each subproblem. The savings due to this approximation, measured as solver time per iteration, will be of the order of a factor of two, with similar significant savings in solver storage of the factored stiffness matrix. Further, in many situations the subproblems may be fully symmetric or approximated as symmetric, so that the less costly symmetric storage and solution scheme can be used. The solver time savings for a symmetric solution is an additional factor of two. Unless you explicitly choose the unsymmetric matrix storage and solution scheme, selection of the scheme will depend on other details of the problem . This modified form of Newton’s method does not affect solution accuracy since the fully coupled effect is considered through the residual vector at each increment in time. However, the rate of convergence is no longer quadratic and depends strongly on the magnitude of the coupling effect, so more iterations are generally needed to achieve equilibrium than with the exact implementation of Newton’s method. When the coupling is significant, the convergence rate becomes very slow and may prohibit obtaining a solution. In such cases the exact implementation of Newton’s method is required. In cases where it is possible to use this approximation, the convergence in an increment will depend strongly on the quality of the first guess to the incremental solution, which you can control by selecting the extrapolation method used for the step . Input File Usage: Abaqus/CAE Usage: Use the following option to specify a separated solution scheme: *SOLUTION TECHNIQUE, TYPE=SEPARATED Step module: Create Step: General: Coupled temp-displacement: Other: Solution technique: Separated Steady-state analysis A steady-state coupled temperature-displacement analysis can be performed in Abaqus/Standard. In steady-state cases you should assign an arbitrary “time” scale to the step: you specify a “time” period and “time” incrementation parameters. This time scale is convenient for changing loads and boundary conditions through the step and for obtaining solutions to highly nonlinear (but steady-state) cases; however, for the latter purpose, transient analysis often provides a natural way of coping with the nonlinearity. Frictional slip heat generation is normally neglected in for the steady-state case. However, it can still be accounted for if motions are used to specify translational or rotational nodal velocities in disk brake- type problems or if user subroutine FRIC provides the incremental frictional dissipation through the variable SFD. If frictional heat generation is present, the heat flux into the two contact surfaces depends on the slip rate of the surfaces. The “time” scale in this case cannot be described as arbitrary, and a transient analysis should be performed. Input File Usage: Abaqus/CAE Usage: *COUPLED TEMPERATURE-DISPLACEMENT, STEADY STATE Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Steady state Transient analysis Alternatively, you can perform a transient coupled temperature-displacement analysis. You can control the time incrementation in a transient analysis directly, or Abaqus/Standard can control it automatically. Automatic time incrementation is generally preferred. Automatic incrementation controlled by a maximum allowable temperature change The time increments can be selected automatically based on a user-prescribed maximum allowable nodal temperature change in an increment, . Abaqus/Standard will restrict the time increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the analysis . Input File Usage: Abaqus/CAE Usage: *COUPLED TEMPERATURE-DISPLACEMENT, DELTMX= Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient; Incrementation: Type: Automatic, Max. allowable temperature change per increment: Fixed incrementation If you do not specify , fixed time increments equal to the user-specified initial time increment, , will be used throughout the analysis. Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT Abaqus/CAE Usage: Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient; Incrementation: Type: Fixed: Increment size: Spurious oscillations due to small time increments In transient analysis with second-order elements there is a relationship between the minimum usable time increment and the element size. A simple guideline is where is the time increment, is the density, c is the specific heat, k is the thermal conductivity, and is a typical element dimension (such as the length of a side of an element). If time increments smaller than this value are used in a mesh of second-order elements, spurious oscillations can appear in the solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations are nonphysical and may cause problems if temperature-dependent material properties are present. In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time increments are required, a finer mesh should be used in regions where the temperature changes rapidly. There is no upper limit on the time increment size (the integration procedure is unconditionally stable) unless nonlinearities cause convergence problems. Automatic incrementation controlled by the creep response The accuracy of the integration of time-dependent (creep) material behavior is governed by the user-specified accuracy tolerance parameter, . This parameter is used to prescribe the maximum strain rate change allowed at any point during an increment, as described in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4. The accuracy tolerance parameter can be specified together with the maximum allowable nodal temperature change in an increment, (described above); however, specifying the accuracy tolerance parameter activates automatic incrementation even if is not specified. Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT, DELTMX= CETOL=tolerance , Abaqus/CAE Usage: Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient, Include creep/swelling/viscoelastic behavior; Incrementation: Type: Automatic, Max. allowable temperature change per increment: strain error tolerance: tolerance , Creep/swelling/viscoelastic Selecting explicit creep integration Nonlinear creep problems (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) that exhibit no other nonlinearities can be solved efficiently by forward-difference integration of the inelastic strains if the inelastic strain increments are smaller than the elastic strains. This explicit method is efficient computationally because, unlike implicit methods, iteration is not required as long as no other nonlinearities are present. Although this method is only conditionally stable, the numerical stability limit of the explicit operator is in many cases sufficiently large to allow the solution to be developed in a reasonable number of time increments. For most coupled thermal-stress analyses, however, the unconditional stability of the backward difference operator (implicit method) is desirable. In such cases the implicit integration scheme may be invoked automatically by Abaqus/Standard. Explicit integration can be less expensive computationally and simplifies implementation of user- defined creep laws in user subroutine CREEP; you can restrict Abaqus/Standard to using this method for creep problems (with or without geometric nonlinearity included). See “Rate-dependent plasticity: creep and swelling,” Section 23.2.4, for further details. Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT, CETOL=tolerance, CREEP=EXPLICIT Abaqus/CAE Usage: Step module: Create Step: General: Coupled temp-displacement: Basic: Response: Transient, Include creep/swelling/viscoelastic behavior; Incrementation: Type: Automatic, Creep/swelling/viscoelastic strain error tolerance: tolerance, Creep/swelling/viscoelastic integration: Explicit Excluding creep and viscoelastic response You can specify that no creep or viscoelastic response will occur during a step even if creep or viscoelastic material properties have been defined. Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT, DELTMX= CREEP=NONE , Abaqus/CAE Usage: Step module: Create Step: General: Coupled temp- displacement: Basic: Response: Transient, toggle off Include creep/swelling/viscoelastic behavior Unstable problems Some types of analyses may develop local instabilities, such as surface wrinkling, material instability, In such cases it may not be possible to obtain a quasi-static solution, even with or local buckling. the aid of automatic incrementation. Abaqus/Standard offers a method of stabilizing this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1. Units In coupled problems where two different fields are active, take care when choosing the units of the problem. If the choice of units is such that the terms generated by the equations for each field are different by many orders of magnitude, the precision on some computers may be insufficient to resolve the numerical ill-conditioning of the coupled equations. Therefore, choose units that avoid ill-conditioned matrices. For example, consider using units of Mpascal instead of pascal for the stress equilibrium equations to reduce the disparity between the magnitudes of the stress equilibrium equations and the heat flux continuity equations. Fully coupled thermal-stress analysis in Abaqus/Explicit In Abaqus/Explicit the heat transfer equations are integrated using the explicit forward-difference time integration rule is the temperature at node N and the subscript i refers to the increment number in an explicit where dynamic step. The forward-difference integration is explicit in the sense that no equations need to be solved when a lumped capacitance matrix is used. The current temperatures are obtained using known are computed at the beginning of the values of increment by from the previous increment. The values of where internal flux vector. is the lumped capacitance matrix, is the applied nodal source vector, and is the The mechanical solution response is obtained using the explicit central-difference integration rule with a lumped mass matrix as described in “Explicit dynamic analysis,” Section 6.3.3. Since both the forward-difference and central-difference integrations are explicit, the heat transfer and mechanical solutions are obtained simultaneously by an explicit coupling. Therefore, no iterations or tangent stiffness matrices are required. Explicit integration can be less expensive computationally and simplifies the treatment of contact. For a comparison of explicit and implicit direct-integration procedures, see “Dynamic analysis procedures: overview,” Section 6.3.1. Stability The explicit procedure integrates through time by using many small time increments. The central- difference and forward-difference operators are conditionally stable. The stability limit for both operators (with no damping in the mechanical solution response) is obtained by choosing where is the highest frequency in the system of equations of the mechanical solution response and is the largest eigenvalue in the system of equations of the thermal solution response. Estimating the time increment size An approximation to the stability limit for the forward-difference operator in the thermal solution response is given by where material. The parameters k, heat, respectively. is the smallest element dimension in the mesh and is the thermal diffusivity of the , and c represent the material’s thermal conductivity, density, and specific In most applications of explicit analysis the mechanical response will govern the stability limit. The thermal response may govern the stability limit when material parameter values are non-physical or a very large amount of mass scaling is used. The calculation of the time increment size for the mechanical solution response is discussed in “Explicit dynamic analysis,” Section 6.3.3. Stable time increment report Abaqus/Explicit writes a report to the status (.sta) file during the data check phase of the analysis that contains an estimate of the minimum stable time increment and a listing of the elements with the smallest stable time increments and their values. The initial minimum stable time increment accounts for the stability requirements of both the thermal and mechanical solution responses. The initial stable time increments listed do not include damping (bulk viscosity), mass scaling, or penalty contact effects in the mechanical solution response. This listing is provided because often a few elements have much smaller stability limits than the rest of the elements in the mesh. The stable time increment can be increased by modifying the mesh to increase the size of the controlling element or by using appropriate mass scaling. Time incrementation The time increment used in an analysis must be smaller than the stability limits of the central- and forward-difference operators. Failure to use such a time increment will result in an unstable solution. When the solution becomes unstable, the time history response of solution variables, such as displacements, will usually oscillate with increasing amplitudes. The total energy balance will also change significantly. Abaqus/Explicit has two strategies for time incrementation control: fully automatic time incrementation (where the code accounts for changes in the stability limit) and fixed time incrementation. Scaling the time increment To reduce the chance of a solution going unstable, the stable time increment computed by Abaqus/Explicit can be adjusted by a constant scaling factor. This factor can be used to scale the default global time estimate, the element-by-element estimate, or the fixed time increment based on the initial element-by- element estimate; it cannot be used to scale a fixed time increment that you specified directly. Input File Usage: Use any of the following options: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, SCALE FACTOR=f *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, ELEMENT BY ELEMENT, SCALE FACTOR=f *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, FIXED TIME INCREMENTATION, SCALE FACTOR=f Abaqus/CAE Usage: Step module: Create Step: General: Dynamic, Temp-disp, Explicit: Incrementation: Time scaling factor: f Automatic time incrementation The default time incrementation scheme in Abaqus/Explicit is fully automatic and requires no user intervention. Two types of estimates are used to determine the stability limit: element-by-element for both the thermal and mechanical solution responses and global for the mechanical solution response. An analysis always starts by using the element-by-element estimation method and may switch to the global estimation method under certain circumstances, as explained in “Explicit dynamic analysis,” Section 6.3.3. In an analysis Abaqus/Explicit initially uses a stability limit based on the thermal and mechanical solution responses in the whole model. This element-by-element estimate is determined using the smallest time increment size due to the thermal and mechanical solution responses in each element. The element-by-element estimate is conservative; it will give a smaller stable time increment than the true stability limit, which is based upon the maximum frequency of the entire model. In general, constraints such as boundary conditions and kinematic contact have the effect of compressing the eigenvalue spectrum, and the element-by-element estimates do not take this into account The stable time increment size due to the mechanical solution response will be determined by the global estimator as the step proceeds unless the element-by-element estimator is chosen, fixed time incrementation is specified, or one of the conditions explained in “Explicit dynamic analysis,” Section 6.3.3, prevents the use of global estimation. The stable time increment size due to the thermal solution response will always be determined by using an element-by-element estimation method. The switch to the global estimation method in mechanical solution response occurs once the algorithm determines that the accuracy of the global estimation method is acceptable. For details, see “Explicit dynamic analysis,” Section 6.3.3 For three-dimensional continuum elements and elements with plane stress formulations (shell, membrane, and two-dimensional plane stress elements) an “improved” estimate of the element characteristic length is used by default. This “improved” method usually results in a larger element stable time increment than a more traditional method. For analyses using variable mass scaling, the total mass added to achieve a given stable time increment will be less with the improved estimate. Input File Usage: Use the following option to specify the element-by-element estimation method: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, ELEMENT BY ELEMENT Use the following option to activate the “improved” element time estimation method: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, IMPROVED DT METHOD=YES Use the following option to deactivate the “improved” element time estimation method: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, IMPROVED DT METHOD=NO Step module: Create Step: General: Dynamic, Temp-disp, Explicit: Incrementation: Type: Automatic, Stable increment estimator: Element-by-element The ability to deactivate the “improved” element time estimation method is not supported in Abaqus/CAE. Abaqus/CAE Usage: Fixed time incrementation A fixed time incrementation scheme is also available in Abaqus/Explicit. The fixed time increment size is determined either by the initial element-by-element stability estimate for the step or by a user-specified time increment. Fixed time incrementation may be useful when a more accurate representation of the higher mode response of a problem is required. In this case a time increment size smaller than the element-by-element estimates may be used. The element-by-element estimate can be obtained simply by running a data check analysis . When fixed time incrementation is used, Abaqus/Explicit will not check that the computed response is stable during the step. You should ensure that a valid response has been obtained by carefully checking the energy history and other response variables. If you choose to use time increments the size of the initial element-by-element stability limit throughout a step, the dilatational wave speed and the thermal diffusivity in each element at the beginning of the step are used to compute the fixed time increment size. To reduce the chance of a solution going unstable, the initial stable time increment that Abaqus/Explicit computes can be adjusted by a constant scaling factor, as described above in “Scaling the time increment.” Alternatively, you can specify a time increment size directly. Input File Usage: Use the following option to request time increments the size of the element-by- element stability limit: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, FIXED TIME INCREMENTATION Use the following option to specify the time increment size directly: *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT, DIRECT USER CONTROL Abaqus/CAE Usage: Step module: Create Step: General: Dynamic, Temp-disp, Explicit: Incrementation: Type: Fixed, Use element-by-element time increment estimator or User-defined time increment: Reducing the computational cost by using selective subcycling The selective subcycling method can be used in a coupled thermal-stress analysis exactly as in a pure mechanical analysis, as described in “Explicit dynamic analysis,” Section 6.3.3 and “Selective subcycling,” Section 11.7.1. Monitoring output variables for extreme values The extreme values defined as the element and nodal variables in a coupled thermal-stress analysis can be monitored exactly as described in “Explicit dynamic analysis,” Section 6.3.3, for a pure mechanical analysis. Initial conditions By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures. Initial stresses, field variables, etc. can also be defined; “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the initial conditions that are available for a fully coupled thermal-stress analysis. Boundary conditions Boundary conditions can be used to prescribe both temperatures (degree of freedom 11) and displacements/rotations (degrees of freedom 1–6) at nodes in fully coupled thermal-stress analysis . Shell elements in Abaqus/Standard have additional temperature degrees of freedom 12, 13, etc. through the thickness . Boundary conditions can be specified as functions of time by referring to amplitude curves (“Amplitude curves,” Section 33.1.2). Boundary conditions applied during a dynamic coupled temperature-displacement response step should use appropriate amplitude references (“Amplitude curves,” Section 33.1.2). If boundary conditions are specified for the step without amplitude references, they are applied instantaneously at the beginning of the step. Since Abaqus/Explicit does not admit jumps in displacement, the value of a nonzero displacement boundary condition that is specified without an amplitude reference will be ignored, and a zero velocity boundary condition will be enforced. Loads The following types of thermal loads can be prescribed in a fully coupled thermal-stress analysis, as described in “Thermal loads,” Section 33.4.4: • Concentrated heat fluxes. • Body fluxes and distributed surface fluxes. • Node-based film and radiation conditions. • Average-temperature radiation conditions. • Element and surface-based film and radiation conditions. The following types of mechanical loads can be prescribed: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” Predefined fields Predefined temperature fields are not allowed in a fully coupled thermal-stress analysis. Boundary conditions should be used instead to prescribe temperature degree of freedom 11 (and 12, 13, etc. in Abaqus/Standard shell elements), as described earlier. Other predefined field variables can be specified in a fully coupled thermal-stress analysis. These values will affect only field-variable-dependent material properties, if any. See “Predefined fields,” Section 33.6.1. Material options The materials in a fully coupled thermal-stress analysis must have both thermal properties, such as conductivity, and mechanical properties, such as elasticity, defined. See Part V, “Materials,” for details on the material models available in Abaqus. In Abaqus/Standard internal heat generation can be specified; see “Uncoupled heat transfer analysis,” Section 6.5.2. Thermal strain will arise if thermal expansion (“Thermal expansion,” Section 26.1.2) is included in the material property definition. In Abaqus/Standard a fully coupled temperature-displacement analysis can be used to analyze static creep and swelling problems, which generally occur over fairly long time periods (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4); viscoelastic materials (“Time domain viscoelasticity,” Section 22.7.1); or viscoplastic materials (“Rate-dependent yield,” Section 23.2.3). Inelastic energy dissipation as a heat source You can specify an inelastic heat fraction in a fully coupled thermal-stress analysis to provide for inelastic energy dissipation as a heat source. Plastic straining gives rise to a heat flux per unit volume of where constant), is the heat flux that is added into the thermal energy balance, is a user-defined factor (assumed is the stress, and is the rate of plastic straining. Inelastic heat fractions are typically used in the simulation of high-speed manufacturing processes involving large amounts of inelastic strain, where the heating of the material caused by its deformation significantly influences temperature-dependent material properties. The generated heat is treated as a volumetric heat flux source term in the heat balance equation. An inelastic heat fraction can be specified for materials with plastic behavior that use the Mises or Hill yield surface (“Inelastic behavior,” Section 23.1.1). It cannot be used with the combined isotropic/kinematic hardening model. The inelastic heat fraction can be specified for user-defined material behavior in Abaqus/Explicit and will be multiplied by the inelastic energy dissipation coded in the user subroutine to obtain the heat flux. In Abaqus/Standard the inelastic heat fraction cannot be used with user-defined material behavior; in this case the heat flux that must be added to the thermal energy balance is computed directly in the user subroutine. In Abaqus/Standard an inelastic heat fraction can also be specified for hyperelastic material definitions that include time-domain viscoelasticity (“Time domain viscoelasticity,” Section 22.7.1). The default value of the inelastic heat fraction is 0.9. If you do not include the inelastic heat fraction behavior in the material definition, the heat generated by inelastic deformation is not included in the analysis. Input File Usage: *INELASTIC HEAT FRACTION Abaqus/CAE Usage: Property module: material editor: Thermal: Inelastic Heat Fraction: Fraction: Elements Coupled temperature-displacement elements that have both displacements and temperatures as nodal variables are available in both Abaqus/Standard and Abaqus/Explicit . In Abaqus/Standard simultaneous temperature/displacement solution requires the use of such elements; pure displacement elements can be used in part of the model in the fully coupled thermal-stress procedure, but pure heat transfer elements cannot be used. In Abaqus/Explicit any of the available elements, except Eulerian elements, can be used in the fully coupled thermal-stress procedure; however, the thermal solution will be obtained only at nodes where the temperature degree of freedom has been activated (i.e., at nodes attached to coupled temperature-displacement elements). The first-order coupled temperature-displacement elements in Abaqus use a constant temperature over the element to calculate thermal expansion. The second-order coupled temperature-displacement elements in Abaqus/Standard use a lower-order interpolation for temperature than for displacement (parabolic variation of displacements and linear variation of temperature) to obtain a compatible variation of thermal and mechanical strain. Output See “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2, for a complete list of output variables. The types of output available are described in “Output,” Section 4.1.1. Input file template *HEADING … ** Specify the coupled temperature-displacement element type *ELEMENT, TYPE=CPS4T … ** *STEP *COUPLED TEMPERATURE-DISPLACEMENT or *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT Data line to define incrementation *BOUNDARY Data lines to define nonzero boundary conditions on displacement or temperature degrees of freedom *CFLUX and/or *CFILM and/or *CRADIATE and/or *DFLUX and/or *DSFLUX and/or *FILM and/or *SFILM and/or *RADIATE and/or *SRADIATE Data lines to define thermal loads *CLOAD and/or *DLOAD and/or *DSLOAD Data lines to define mechanical loads *FIELD Data lines to define field variable values *END STEP 6.5.4 ADIABATIC ANALYSIS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Heat transfer analysis procedures: overview,” Section 6.5.1 • *DYNAMIC • *STATIC • *DENSITY • *INELASTIC HEAT FRACTION • *SPECIFIC HEAT • “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining thermal material models,” Section 12.10 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview An adiabatic stress analysis: • is used in cases where mechanical deformation causes heating but the event is so rapid that this heat has no time to diffuse through the material—for example, a very high-speed forming process; • can be conducted as part of a dynamic analysis (“Implicit dynamic analysis using direct integration,” Section 6.3.2, or “Explicit dynamic analysis,” Section 6.3.3) or as part of a static analysis (“Static stress analysis,” Section 6.2.2); • in Abaqus/Standard is available only for the isotropic hardening metal plasticity models with a Mises yield surface (“Classical metal plasticity,” Section 23.2.1); • in Abaqus/Explicit is relevant only for the metal plasticity models (including both Mises and Hill yield surfaces); • can be conducted if parts of the model are elastic only—no change in temperature occurs in the elastic regions; and • requires that a material’s density, specific heat, and inelastic heat fraction (fraction of inelastic dissipation rate that appears as heat flux) be specified. Adiabatic analysis Adiabatic thermal-stress analysis is typically used to simulate high-speed manufacturing processes involving large amounts of inelastic strain, where the heating of the material caused by its deformation is an important effect because of temperature-dependent material properties. The temperature increase is calculated directly at the material integration points according to the adiabatic thermal energy increases caused by inelastic deformation; temperature is not a degree of freedom in the problem. No allowance is made for conduction of heat in an adiabatic analysis. For problems where both inelastic heating and conduction of the heat are important, a fully coupled temperature-displacement analysis must be performed (“Fully coupled thermal-stress analysis,” Section 6.5.3). In an adiabatic analysis plastic straining gives rise to a heat flux per unit volume of is the heat flux that is added into the thermal energy balance, where heat fraction (assumed constant; discussed below), The heat equation solved at each integration point is is the stress, and is the user-specified inelastic is the rate of plastic straining. is the material density and where heat,” Section 26.2.3). is the specific heat . In this case the temperatures at the end of the adiabatic analysis must be written to the Abaqus/Standard results file as element variables averaged at the nodes. Since temperature values in an adiabatic analysis can be written to the results file as element quantities only by using the TEMP output variable identifier, they cannot be read directly into a subsequent thermal diffusion analysis as initial conditions. However, if you postprocess the results file to produce a second results file in which the temperature data are provided as nodal quantities, a subsequent heat transfer analysis can be performed with these temperatures as initial conditions. See “Predefined fields,” Section 33.6.1, and “Accessing the results file information,” Section 5.1.3, for details. Alternatively, you could postprocess the results file to produce a data list containing data pairs consisting of nodes and temperatures. The temperatures, NT, obtained from the heat transfer analysis can then be used to drive a continuation of the previous stress analysis. This stress analysis should be restarted from the end of the adiabatic analysis and will provide the response to the change of the temperature field obtained during the heat transfer analysis. In this case Abaqus/Standard will automatically read the temperatures from the results file that was obtained from the heat transfer analysis and apply them in the restarted analysis. Example The following input options could be used to perform a heat transfer analysis using the temperatures from an adiabatic analysis and then continue the stress analysis: **Static adiabatic analysis … *STEP *STATIC, ADIABATIC … **Write the temperatures to the results file as element **variables averaged at the nodes *EL FILE, POSITION=AVERAGED AT NODES TEMP *END STEP **Heat transfer analysis using the temperatures from the **static analysis as initial conditions … *INITIAL CONDITIONS, TYPE=TEMPERATURE, FILE=new results file, STEP=step, INC=increment *STEP *HEAT TRANSFER … *NODE FILE NT *END STEP **Restart from the adiabatic analysis using temperatures **obtained from the heat transfer analysis *RESTART, WRITE, READ, STEP=k, INC=i, END STEP … *STEP *STATIC … *TEMPERATURE, FILE=heat_transfer_results_file … *END STEP Fully coupled temperature-displacement analysis If the continuation of the analysis into thermal diffusion requires a fully coupled temperature- displacement analysis , the simplest (but more expensive) approach is to use coupled temperature-displacement elements throughout the adiabatic analysis. At the end of the static or the dynamic adiabatic calculations, the temperatures must be written to the results file as element variables averaged at the nodes. In addition, you must constrain all temperature degrees of freedom since they are not used in the adiabatic analysis. The adiabatic analysis can then be restarted to apply the correct temperature distribution obtained from the adiabatic analysis to the temperature degree of freedom of each node in the model. To create the input for the boundary conditions, you must postprocess the results file obtained from the adiabatic analysis and extract the value of TEMP at each node in the model . The temperature boundary conditions can be released as needed in subsequent coupled temperature-displacement analysis steps. Example The following input options could be used to perform a coupled temperature-displacement analysis using the temperatures from an adiabatic analysis: **Static adiabatic analysis, coupled temperature-displacement **plane stress elements … *ELEMENT, TYPE=CPS4T, ELSET=EALL … *BOUNDARY nodes, 11, 11, 0.0 *STEP *STATIC, ADIABATIC … **Write the temperatures to the results file as element **variables averaged at the nodes *EL FILE, POSITION=AVERAGED AT NODES TEMP *END STEP **Restart from the adiabatic analysis *RESTART, WRITE, READ, STEP=k, INC=i, END STEP … *STEP *STATIC **Dummy step to associate the temperature variable TEMP with **the temperature degree of freedom at each node 1.0, 1.0 … *BOUNDARY, OP=NEW node, 11, 11, temperature … *END STEP **Coupled temperature displacement run for cool down of **structure: continuation of the restart analysis … *STEP *COUPLED TEMPERATURE-DISPLACEMENT 0.1, 1.0 … *BOUNDARY, OP=NEW **no temperature boundary condition specified *END STEP Initial conditions Initial temperatures can be prescribed at nodes as initial conditions. Initial values of stresses, field variables, solution-dependent state variables, etc. can also be specified . Boundary conditions Boundary conditions can be applied to displacement degrees of freedom in an adiabatic analysis in the same way that they are applied in nonadiabatic dynamic, explicit dynamic, or static analysis steps . Temperature is not a degree of freedom in an adiabatic analysis. Loads The loading options available for an adiabatic analysis are the same as those available for nonadiabatic dynamic, explicit dynamic, or static analysis steps . The following types of mechanical loads can be prescribed: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” Predefined fields Predefined temperature fields cannot be used during an adiabatic analysis step. The values of user-defined field variables can be specified; these values affect only field-variable- dependent material properties, if any. See “Predefined fields,” Section 33.6.1. Material options In Abaqus/Standard only Mises plasticity with isotropic elasticity and isotropic hardening (“Inelastic behavior,” Section 23.1.1) is allowed in adiabatic stress analysis. Kinematic or combined hardening is not available, but rate effects can be included. However, portions of the model can include only elastic material; no change in temperature occurs in the elastic regions, since there is no source of heat generation. In Abaqus/Explicit both Mises and Hill plasticity are allowed in adiabatic stress analysis. You must specify the density, the inelastic heat fraction, and the specific heat as part of the material definition for the material in which heat will be generated by plastic dissipation. You can also specify latent heat if necessary (“Latent heat,” Section 26.2.4). The inelastic heat fraction is the amount of inelastic dissipation used to calculate the increase in temperature. The default value of the inelastic heat fraction is 0.9. If the inelastic heat fraction is not included in the material definition, the heat generated by inelastic deformation is not included in the analysis. In Abaqus/Standard adiabatic analyses can also be carried out with user subroutine UMAT. In this case the temperature must be defined as a solution-dependent state variable, and all coupling terms must be included in the user subroutine. If conductivity (“Conductivity,” Section 26.2.2) is defined for the material, it will be ignored during adiabatic analysis steps. Input File Usage: All of the following options must be included in the material definition: *DENSITY *INELASTIC HEAT FRACTION *SPECIFIC HEAT The following option can be included if latent heat effects are important: Abaqus/CAE Usage: *LATENT HEAT All of the following must be included in the material definition: Property module: Material editor: General→Density Material editor: Thermal→Inelastic Heat Fraction Material editor: Thermal→Specific Heat The following can be included if latent heat effects are important: Property module: material editor: Thermal→Latent Heat Temperature-dependent material properties Material properties can be temperature dependent. Since the only source of temperature change in adiabatic analysis is inelastic deformation, the temperature can only rise. This temperature rise may cause thermal expansion (usually a small effect) and localization of the deformation if the flow stress is reduced by the temperature rise. Since the adiabatic assumption applies only in rapid events and inelastic deformation usually causes significant temperature rises only if the deformation is substantial, the strain rates are often large in adiabatic analysis. The softening of the material caused by the temperature rise may, thus, be offset somewhat by strengthening associated with rate dependence if the material is rate sensitive. Elements Any of the stress/displacement or coupled temperature-displacement elements in Abaqus can be used in an adiabatic analysis . Mass or spring elements will not contribute to the heating of the material since they cannot generate plastic strains. If coupled temperature-displacement elements are used in an adiabatic analysis, the temperature degrees of freedom will be ignored. Output Since temperatures are updated at the material calculation points, output of temperature is available with output variable TEMP, not with output variable NT. The element output available for an adiabatic analysis includes stress; strain; energies; the values of state, field, and user-defined variables; and composite failure measures. The nodal output available includes displacements, reaction forces, and coordinates. All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. Input file template *HEADING … *MATERIAL, NAME=name *ELASTIC, TYPE=ISOTROPIC Data lines to define isotropic linear elasticity *PLASTIC Data lines to define metal plasticity *DENSITY Data lines to define density *INELASTIC HEAT FRACTION Data line to define inelastic heat fraction *SPECIFIC HEAT Data lines to define specific heat … *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS, TYPE=type Data lines to specify initial conditions *AMPLITUDE, NAME=name Data lines to define amplitude variations ** *STEP, NLGEOM The NLGEOM parameter is used in Abaqus/Standard to include geometric nonlinearity *DYNAMIC, ADIABATIC or *DYNAMIC, EXPLICIT, ADIABATIC or *STATIC, ADIABATIC Data line to control time incrementation or to specify the time period of the step *BOUNDARY, AMPLITUDE=name Data lines to describe nonzero or zero-valued boundary conditions *CLOAD and/or *DLOAD and/or *DSLOAD Data lines to specify loads *FIELD Data lines to specify field variable values *END STEP 6.6 Fluid dynamic analysis • “Fluid dynamic analysis procedures: overview,” Section 6.6.1 • “Incompressible fluid dynamic analysis,” Section 6.6.2 6.6.1 FLUID DYNAMIC ANALYSIS PROCEDURES: OVERVIEW Overview Abaqus/CFD provides advanced computational fluid dynamics capabilities with extensive support for preprocessing and postprocessing provided in Abaqus/CAE. These scalable parallel CFD simulation capabilities address a broad range of nonlinear coupled fluid-thermal and fluid-structural problems. Abaqus/CFD can solve the following types of incompressible flow problems: • Laminar and turbulent: Internal or external flows that are steady-state or transient, span a broad Reynolds number range, and involve complex geometry may be simulated with Abaqus/CFD. This includes flow problems induced by spatially varying distributed body forces. • Thermal convective: Problems that involve heat transfer and require an energy equation and that may involve buoyancy-driven flows (i.e., natural convection) can also be solved with Abaqus/CFD. This type of problem includes turbulent heat transfer for a broad range of Prandtl numbers. • Deforming-mesh ALE: Abaqus/CFD includes the ability to perform deforming-mesh analyses using an arbitrary Lagrangian-Eulerian (ALE) description of the equations of motion, heat transfer, and turbulent transport. Deforming-mesh problems may include prescribed boundary motion that induces fluid flow or FSI problems where the boundary motion is relatively independent of the fluid flow. For more details, see “Incompressible fluid dynamic analysis,” Section 6.6.2. Activation of fields in Abaqus/CFD In Abaqus/CFD the active fields (degrees of freedom) are determined by the analysis procedure and the options specified, such as turbulence models and auxiliary transport equations. For example, using the energy equation in conjunction with the incompressible flow procedure activates the velocity, pressure, and temperature degrees of freedom. For a complete listing of the available degrees of freedom, see “Active degrees of freedom” in “Boundary conditions in Abaqus/CFD,” Section 33.3.2. 6.6.2 INCOMPRESSIBLE FLUID DYNAMIC ANALYSIS Products: Abaqus/CFD Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Fluid dynamic analysis procedures: overview,” Section 6.6.1 Overview An incompressible fluid dynamics analysis: • is one where the velocity field is divergence-free and the pressure does not contain a thermodynamic component; • is one where the energy contained in acoustic waves is small relative to the energy transported by advection (i.e., when the Mach number is in the range ); • can be either laminar or turbulent, steady or time-dependent; • can be used to study either internal or external flows; • can include energy transport and buoyancy forces; • can be used with a deforming mesh for ALE calculations; and • can be performed with conjugate heat transfer or fluid-structure interaction. Incompressible fluid dynamic analysis Incompressible flow is one of the most frequently encountered flow regimes encompassing a diverse set of problems that include: atmospheric dispersal, food processing, aerodynamic design of automobiles, biomedical flows, electronics cooling, and manufacturing processes such as chemical vapor deposition, mold filling, and casting. Input File Usage: Abaqus/CAE Usage: *CFD, INCOMPRESSIBLE NAVIER STOKES Step module: Create Step: General: Flow; Flow type: Incompressible Governing equations The momentum equations in integral form for an arbitrary control volume can be written as where is an arbitrary control volume with surface area is the outward normal to , , is the fluid density, is the pressure, is the velocity vector, is the velocity of the moving mesh, is the body force, and is the viscous shear stress. The viscous shear stress, information, see “Viscosity,” Section 26.1.4. , is also referred to as the deviatoric stress, Incompressibility requires a solenoidal velocity field expressed by , where . For more Numerical implementation The solution of the incompressible Navier-Stokes equations poses a number of algorithmic issues due to the divergence-free velocity condition and the concomitant spatial and temporal resolution required to achieve solutions in complex geometries for engineering applications. The Abaqus/CFD incompressible solver uses a hybrid discretization built on the integral conservation statements for an arbitrary deforming domain. For time-dependent problems, an advanced second-order projection method is used with a node-centered finite-element discretization for the pressure. This hybrid approach guarantees accurate solutions and eliminates the possibility of spurious pressure modes while retaining the local conservation properties associated with traditional finite volume methods. An edge-based implementation is used for all transport equations permitting a single implementation that spans a broad variety of element topologies ranging from simple tetrahedral and hexahedral elements to arbitrary polyhedral. In Abaqus/CFD tetrahedral, wedge, and hexahedral elements are supported. Projection method The basic concept for projection methods is the legitimate segregation of pressure and velocity fields for efficient solution of the incompressible Navier-Stokes equations. Over the past two decades, projection methods have found broad application for problems involving laminar and turbulent fluid dynamics, large density variations, chemical reactions, free surfaces, mold filling, and non-Newtonian behavior. In practice, the projection is used to remove the part of the velocity field that is not divergence- free (“div-free”). The projection is achieved by splitting the velocity field into div-free and curl-free components using a Helmholtz decomposition. The projection operators are constructed so that they satisfy prescribed boundary conditions and are norm-reducing, resulting in a robust solution algorithm for incompressible flows. Least-squares gradient estimation The solution methods in Abaqus/CFD use a linearly complete second-order accurate least-squares gradient estimation. This permits accurate evaluation of dual-edge fluxes for both advective and diffusive processes. All transport equations in Abaqus/CFD make use of the second-order least-squares operators. Advection methods The advection treatment in Abaqus/CFD is edge-based, monotonicity-preserving, and preserves smooth variations to second order in space. The advection algorithm relies on a least-squares gradient estimation with unstructured-grid slope limiters that are topology independent. Sharp gradients are captured within approximately 2–3 elements; i.e., , and the use of slope limiting in conjunction with a local diffusive limiter precludes over-/under-shoots in advected fields. The advection terms in the momentum and transport equations can be treated either explicitly or implicitly . Energy equation The energy transport equation is optionally activated in Abaqus/CFD for non-isothermal flows. For small density variations, the Boussinesq approximation provides the coupling between momentum and energy equations. In turbulent flows, the energy transport includes a turbulent heat flux based on the turbulent eddy viscosity and turbulent Prandtl number. Abaqus/CFD provides a temperature-based energy equation. The energy equation, in temperature form, can be obtained from the first law of thermodynamics and is given by is the constant pressure specific heat, where is heat flux due to conduction defined by Fourier’s law, and is the heat supplied externally into the body per unit volume. The energy equation is solved in terms of temperature in Abaqus/CFD. is the temperature, Input File Usage: Use the following option to specify an isothermal flow problem (default): *CFD, ENERGY EQUATION=NO ENERGY Use the following option to specify a thermal (heat) transport problem with temperature as the primary transport scalar variable: Abaqus/CAE Usage: *CFD, ENERGY EQUATION=TEMPERATURE Use the following option to specify an isothermal flow problem: Step module: Create Step: General: Flow; Basic tabbed page: Energy equation: None Use the following option to specify a thermal (heat) transport problem with temperature as the primary transport scalar variable: Step module: Create Step: General: Flow; Basic tabbed page: Energy equation: Temperature Turbulence models Turbulence modeling is a pacing technology for computational fluid dynamics. There is no single universal turbulence model that can adequately handle all possible flow conditions and geometrical configurations. This is complicated by the plethora of turbulence models and modeling approaches that are currently available; e.g., Reynolds Averaged Navier-Stokes (RANS), Unsteady Reynolds Averaged Navier-Stokes (URANS), Large-Eddy Simulation (LES), Implicit Large-Eddy Simulation (ILES), and hybrid RANS/LES (HRLES). Ultimately, you must ensure that the approximations made in a given turbulence model are consistent with the physical problem being modeled. The following turbulent flow models are available: ILES, Spalart-Allmaras (SA), and RNG k– . These models span a relatively broad set of flow problems that include time-dependent flows, fluid- structure interaction (FSI), and conjugate heat transfer (CHT). Implicit Large-Eddy Simulation (ILES) Large-eddy simulation relies on a segregation of length and time scales in turbulent flows and a modeling approach that permits the direct simulation of grid-resolved flow structures and the modeling of unresolved subgrid features. Implicit LES is a methodology for modeling high Reynolds number flows that combines computational efficiency and ease of implementation with predictive calculations and flexible application. In Abaqus/CFD ILES relies on the discrete monotonicity-preserving form of the advective operator to implicitly define the subgrid-scale model. This model is inherently time-dependent requiring time-accurate solutions to the incompressible Navier-Stokes equations where the time scale is approximately that of an eddy-turnover time for resolve-scale flow features. In addition, this model must be run in full three dimensions, which typically imposes larger grid densities and stringent grid resolution criteria relative to more traditional steady-state RANS simulations. However, this approach is extremely flexible and can be applied to a broad range of flows and FSI problems. There are no user settings required for ILES. Input File Usage: Abaqus/CAE Usage: Use the *CFD option without the *TURBULENCE MODEL option. Step module: Create Step: General: Flow; Turbulence tabbed page: None Spalart-Allmaras (SA) turbulence model The Spalart-Allmaras (SA) model is a one-equation turbulence model that uses an eddy-viscosity variable with a nonlinear transport equation. The model was developed based on empiricism, dimensional analysis, and a requirement for Galilean invariance. The model has found broad use and has been calibrated for two-dimensional mixing layers, wakes, and flat-plate boundary layers. The model produces reasonably accurate predictions of turbulent flows in the presence of adverse pressure gradients and may be used for flows where separation occurs. This model is spatially local and requires only moderate resolution in boundary layers. Although initially designed for external and free-shear flows, the Spalart-Allmaras model can also be used for internal flows. The basic form of the one-equation Spalart-Allmaras model consists of one transport equation for the turbulent eddy viscosity, . The model requires the normal distance from the wall used in the damping functions needed to control the turbulent viscosity in the near-wall region. Abaqus/CFD automatically computes the normal distance function, permitting simple specification of the model boundary conditions. The turbulent viscosity transport equation for the Spalart-Allmaras model is given by where the damping functions and model coefficients are defined as: where is the normal distance from the wall, and the effective turbulent viscosity is defined as The Spalart-Allmaras model coefficients are shown in Table 6.6.2–1. In addition, a turbulent Prandtl number ( ) can be specified. Table 6.6.2–1 Spalart-Allmaras model coefficients. 0.1355 0.622 7.1 0.6667 0.3 0.41 The Spalart-Allmaras model can provide very accurate boundary layer results if the near-wall region is resolved (near-wall resolution such that the nondimensional wall distance is approximately 3). However, the implementation of boundary conditions for the Spalart-Allmaras model in Abaqus/CFD permits the use of coarser meshes as well. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *CFD *TURBULENCE MODEL, TYPE=SPALART ALLMARAS Step module: Create Step: General: Flow; Turbulence tabbed page: Spalart-Allmaras RNG k–epsilon turbulence model The RNG k– model is a two-equation turbulence model that evolves an equation for the turbulent kinetic energy, k, and the energy dissipation rate, . The model equations are developed from fundamental physical principles and dimensional analysis. In general, the coefficients of the model are usually calibrated using canonical flows and experimental data. However, the RNG version of the model computes the coefficients using Renormalization Group theory (Yakhot et al., 1992). The model equations are where the turbulent viscosity is and The second and third terms on the right-hand-side of the k– transport equations above represent the production and dissipation of k and , respectively. The RNG k– model coefficients are shown in Table 6.6.2–2. In addition, a turbulent Prandtl number ) can be specified. ( Table 6.6.2–2 RNG k– model coefficients. 0.085 1.42 1.68 0.72 0.72 0.012 4.38 Input File Usage: Use both of the following options: *CFD *TURBULENCE MODEL, TYPE=RNG KEPSILON Step module: Create Step: General: Flow; Turbulence tabbed page: k-epsilon renormalization group (RNG) Abaqus/CAE Usage: Wall functions It is well known that the k– model has limitations, especially on wall-bounded flows where high values of eddy viscosity in the near-wall region are usually reproduced. For high Reynolds number flows often encountered in many industrial applications, a full resolution of the thin viscous sub-layer that occurs near a wall using a fine mesh may not be economical. Consequently, for meshes that cannot resolve the viscous sub-layer, wall functions are used to represent the effects of the viscous sub-layer on the transport processes. In Abaqus/CFD wall functions are used to avoid the need for highly resolved boundary layer meshes. This approach relies on the law of the wall to obtain the wall shear stress. The law of the wall is a universal velocity profile that wall-bounded flows develop in the absence of pressure gradients. The law of the wall is where if if , is the wall tangent velocity, is the kinematic viscosity, is the density, is the shear stress at the wall, and and are constants. The standard law of the wall profile is limited in its usage. For example, in recirculating flows the turbulent kinetic energy k becomes zero at separation and reattachment points, where, by definition, is zero. This singular behavior causes the predicted results to be erroneous. To overcome this, the standard law of the wall is modified based on a new scale for the friction velocity following the method proposed by Launder and Spalding (1974). The modified friction velocity is given by which does not suffer from a singular behavior at flow reattachment, separation, and at points of flow impingement. Correspondingly, the wall distances are re-scaled as follows: The modified law of the wall reduces to the standard law of the wall under the conditions of uniform wall shear stress, and when the generation and dissipation of turbulent kinetic energy are in balance (i.e., when the turbulence structure is in equilibrium). Under such conditions, and thus, . The wall shear stress for the modified law of the wall can be evaluated as (Albets-Chico, et al., 2008) if if , where the subscript p denotes the wall element center at which all the quantities of interest are evaluated. The use of the wall function requires the modification of the transport equations for k and for the wall layer of elements. Specifically, the production and dissipation terms in the governing transport equation for the turbulent kinetic energy k are modified to account for the presence of the wall. Following the procedure outlined in (Craft et al., 2002), an average value of the production of k as given below is used in the transport equation. Such an average is obtained based on a two-layer model of the wall element (i.e., the wall element is divided into a partly viscous sub-layer region and a partly turbulent log-layer or inertial layer region). if if , where is the maximum of the wall normal distances of all the vertices of a given wall element, and is the wall normal distance of the edge of the viscous sub-layer, where Similarly, an average value of the dissipation rate for k is also prescribed for the wall elements based on a two-layer integration and is given by The transport equation for is not solved for the wall layer elements. Instead, the value of is directly prescribed at the point p as follows: if if . if if . Therefore, integration of the k and transport equations is performed with a zero-flux (i.e., homogeneous Neumann boundary conditions) at the walls. Guidelines on wall functions The main advantage of wall functions is the relaxed requirement on mesh resolution at walls. However, the main disadvantage of using wall functions is the dependence on the near-wall mesh resolution. Wall functions based on the law of the wall approach usually work best for wall elements whose centers lie in the fully turbulent layer (inertial or log layer) for which such functions are designed. This effectively imposes a lower limit on the value of the scaled wall coordinate, . For complex geometries, ensuring that all the near wall cells are outside the viscous sublayer is difficult. The precise location of the logarithmic region is solution dependent and may vary with time. To accommodate a more flexible mesh, a resolution-insensitive wall function (Durbin, 2009) has been implemented. Briefly, this wall function is based on limiting the minimum value of such that the value of the velocity gradient at the first wall-attached element is the same as if it was located on the edge of the viscous sub-layer. A best practice for wall-bounded flows is to have at least 8–10 points in the boundary layer region where . Deforming-mesh ALE Many industrial CFD/FSI/CHT problems involve moving boundaries or deforming geometries. This class of problem includes prescribed boundary motion that induces fluid flow or where the boundary motion is relatively independent of the fluid flow. Abaqus/CFD uses an arbitrary Lagrangian-Eulerian (ALE) formulation and automated mesh deformation method that preserves element size in boundary layers. The ALE and deforming-mesh algorithms are activated automatically for problems that involve a moving boundary prescribed by the user or identified as a moving boundary in an FSI co-simulation. Abaqus/CFD offers distortion control to prevent elements from inverting or distorting excessively in fluid mesh movement . To properly control the mesh motion during a simulation, it is the user’s responsibility to prescribe appropriate displacement boundary conditions on the computational mesh. Porous media flows Flows through fluid-saturated porous media occur in a wide range of industrial and environmental applications. Such flows can be isothermal (no heat transfer) or non-isothermal in nature. Examples include packed-bed heat exchangers, heat pipes, thermal insulation, petroleum reservoirs, nuclear waste repositories, geothermal engineering, thermal management of electronic devices, metal alloy casting, and flow past porous scaffolds in bioreactors. Isothermal flows For isothermal flows in porous media, many studies are usually carried out using the Darcy flow model, which is an empirical law for creeping flow through an infinitely extended uniform medium. However, non-Darcian effects such as fluid inertial effects are quite important for certain applications. The model implemented in Abaqus/CFD is based on the volume-averaged Darcy-Brinkman-Forchheimer equations that account for both Darcian and inertial non-Darcian effects. The following assumptions are made in deriving the governing equations: • the porosity of the medium does not vary with time or the time scale of variation of the porosity is considered to be much larger than the dominant time scales of the fluid motion; and • the permeability of the porous medium is isotropic and dependent only on the porosity of the medium. Based on the above assumptions, the volume-averaged mass conservation and the Darcy-Brinkman- Forchheimer momentum equations governing the flow of an incompressible fluid in a fluid-saturated porous media can be written as follows (Nield and Bejan, 2010): where is the extrinsic average or the superficial velocity vector, where the average is taken over a representative volume incorporating both the solid (matrix) and the fluid phases; is the intrinsic average of the pressure (average taken only over the fluid-phase); is the density of the fluid; is the viscosity of the fluid; is the porosity (volume fraction of the fluid phase) of the porous medium; and is the permeability of the porous medium. The second term on the right-hand side of the momentum equation is the Brinkman term accounting for the presence of solid boundaries, the third term represents the Darcy drag term (linear in velocity), and the last term represents the inertial (quadratic in velocity) or the Forchheimer drag. The parameter is the inertial drag coefficient (also referred to as the form drag coefficient). Based on Ergun’s equation (Nield and Bejan, 2010), . The porous drag forces (namely, the Darcy and Forchheimer drag forces) are activated for a prescribed element set by specifying them as distributed loads . is a constant that is set to a default value of , where Thus, , of the porous medium. The default value of the porous media flow problem requires the specification of the porosity, , and the permeability, can also be changed in the material property definition . For the case of turbulent flow within a porous medium, the fluid viscosity includes the contribution of both the molecular and the turbulent eddy viscosities. For conjugate flows involving domains consisting of both pure fluid regions and fluid-saturated porous media, the pure fluid porosity is set to a value of 1 by default. Permeability-Porosity relationships The permeability of a porous medium is generally a function of the physical properties of the interconnected pore system such as porosity and tortuosity. Determination of the appropriate permeability-porosity relationship requires a detailed knowledge of the size distribution and spatial arrangement of the pore channels in the porous medium. The permeability-porosity relation can be specified directly in Abaqus/CFD using the material property definition. Another permeability-porosity relation supported in Abaqus/CFD is the widely accepted Carman- Kozeny model. This relation is given as follows: where particles/fibers. represents the Carman-Kozeny constant and represents the average radius of the porous Limitations • While turbulence can be activated for a porous media flow problem, a rigorous volume-averaging procedure has not been implemented in Abaqus/CFD to account for turbulence transport within the porous media. The equations governing the transport of the turbulence variables are solved by neglecting the effects of the presence of porous medium. In other words, the porous medium remains transparent (fully open) to the transport of turbulence variables. • When the arbitrary Lagrangian-Eulerian (ALE) and deforming mesh algorithms are activated for a porous flow problem, changes in the porosity of the medium associated with large mesh/domain deformations are not taken into account. The model is strictly valid only for the case of undeformable porous media. Non-isothermal flows (heat transfer) The following assumptions are made in the implementation of the volume-averaged energy equation for porous media in Abaqus/CFD: • The medium is isotropic. • Radiative effects, viscous dissipation, and work done by the changes in pressure are negligible. • Local thermal equilibrium is valid (i.e., solid and fluid phase temperatures are the same). • No net heat transfer takes place between the different phases in the porous media. Based on the above assumptions, the effective energy equation for the porous medium can be given as follows (Nield and Bejan, 2010): where and Here, , , and is the extrinsic average or the superficial velocity vector, and denote the fluid phase, solid (matrix) phase, and effective medium, respectively. the specific heat capacity at constant pressure, heat production per unit volume or the heat source ( heat transfer within a porous medium, the fluid conductivity molecular and turbulent eddy conductivities. is the thermal conductivity, and is the temperature. The subscripts is is the effective ). For the case of turbulent includes the contribution of both the As seen from the above equation, the porous media heat transfer problem requires the specification of the following input: • The thermal properties of the solid (matrix) phase: the density, ; and specific heat capacity, ; the conductivity, ; and the • The thermal properties of the fluid (matrix) phase: the molecular conductivity, capacity, , apart from the specification of other fluid properties such as the density, ; and specific heat , viscosity, , and permeability, . Linear equation solvers The solution methods for the momentum and auxiliary transport equations in Abaqus/CFD rely on scalable parallel preconditioned Krylov solvers. The pressure, pressure-increment, and distance function equations are solved with user-selectable Krylov solvers and a robust algebraic multigrid preconditioner. A set of preselected default convergence criteria and iteration limits are prescribed for all linear equation solvers. The default solver settings should provide computationally efficient and robust solutions across a spectrum of CFD problems. However, full access to diagnostic information, In practice, the pressure-increment equation convergence criteria, and optional solvers is provided. may be the most sensitive linear system and could require user intervention based on knowledge of the specific flow problem. Input File Usage: Use the following option to specify parameters for solving the momentum transport equations: *MOMENTUM EQUATION SOLVER Use the following option to specify parameters for solving other transport equations, such as the energy or turbulence transport equations: *TRANSPORT EQUATION SOLVER Use the following option to specify parameters for solving the pressure equation: *PRESSURE EQUATION SOLVER Convergence criteria and diagnostics Iterative solvers compute an approximate solution to a given set of equations; therefore, convergence criteria are required to determine if the solution is acceptable. While default settings should be adequate for most problems, you can modify the convergence criteria. In addition to the option of setting convergence criteria, convergence history output is available that may be useful for some advanced users to tune the solvers for performance or robustness. For the algebraic multigrid preconditioner, diagnostic information such as the number of grids, grid sparsity, and largest eigenvalue and condition number estimates are available upon request. The diagnostic information for the algebraic multigrid preconditioner is printed every time the preconditioner is computed. Specifying convergence criteria The linear convergence limit (also commonly referred to as the convergence tolerance), the frequency of convergence checking, and the maximum number of iterations can be set. The iterative solver will stop when the relative residual norm of the system of equations and the relative correction of the solution norm fall below the convergence limit. Input File Usage: Abaqus/CAE Usage: Use the following options to specify convergence criteria for the momentum and auxiliary transport equations: *MOMENTUM EQUATION SOLVER max iterations, frequency check, convergence limit *TRANSPORT EQUATION SOLVER max iterations, frequency check, convergence limit *PRESSURE EQUATION SOLVER max iterations, frequency check, convergence limit Step module: Create Step: General: Flow; Solvers tabbed page: Momentum Equation, Pressure Equation, or Transport Equation tabbed page; enter values for Iteration limit, Convergence checking frequency, and Linear convergence limit Accessing convergence output You can monitor the convergence of the iterative solver by accessing convergence output. When you activate the convergence output, the current relative residual norm and the relative solution correction norm are output each time the convergence is checked. Input File Usage: Abaqus/CAE Usage: Use the following options to write convergence output to the log file for the linear equation solvers: *MOMENTUM EQUATION SOLVER, CONVERGENCE=ON *TRANSPORT EQUATION SOLVER, CONVERGENCE=ON *PRESSURE EQUATION SOLVER, CONVERGENCE=ON Step module: Create Step: General: Flow; Solvers tabbed page: Momentum Equation, Pressure Equation, or Transport Equation tabbed page; toggle on Include convergence output Accessing diagnostic information Diagnostic output is useful only for the algebraic multigrid preconditioner. For other preconditioners, only a solver initialization message is printed for diagnostic output. For the algebraic multigrid preconditioner, the number of grids, grid sparsity, and largest eigenvalue and condition number estimates are output each time the preconditioner is computed. Input File Usage: Use the following option to write diagnostic output to the log file for the pressure equation solver using the algebraic multigrid preconditioner: *PRESSURE EQUATION SOLVER, TYPE=AMG, DIAGNOSTICS=ON Abaqus/CAE Usage: Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page; toggle on Include diagnostic output Specifying a solver for the pressure equation Three solver types are available for the solving the pressure equation. The default AMG solver uses an algebraic multigrid preconditioner and offers the choice of three Krylov solvers: conjugate gradient, bi-conjugate gradient stabilized, and flexible generalized minimal residual. The SSORCG solver uses a symmetric successive over-relaxation preconditioner and conjugate gradient Krylov solver. The DSCG solver uses a diagonally scaled preconditioner and conjugate gradient Krylov solver. The AMG solver provides many additional options that are intended for advanced usage and in cases where convergence difficulties are encountered. Input File Usage: Abaqus/CAE Usage: Use one of the following options to specify the solver type: *PRESSURE EQUATION SOLVER, TYPE=AMG (default) *PRESSURE EQUATION SOLVER, TYPE=SSORCG *PRESSURE EQUATION SOLVER, TYPE=DSCG Use the following option to specify the AMG solver: Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page: Solver options: Use analysis defaults Use the following option to specify the SSORCG solver: Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page: Solver options: Specify, Preconditioner Type: Symmetric successive over-relaxation The DSCG solver is not supported in Abaqus/CAE. Specifying the complexity level For the AMG solver, you can choose from three preset levels or you can specify the Krylov solver and smoother settings directly. The presets are provided for convenience. Preset level 1 is primarily intended for use with meshes with good element aspect ratios and in some cases may provide a performance benefit over the default preset level 2. Preset level 3 is intended for problems that encounter convergence difficulties, which typically have elements with high aspect ratios or highly distorted elements. Input File Usage: Preset level 1 corresponds to the following: *PRESSURE EQUATION SOLVER, TYPE=AMG 250, 2, 10−5 CHEBYCHEV, 2, 2, CG Preset level 2 (default) corresponds to the following: *PRESSURE EQUATION SOLVER, TYPE=AMG 250, 2, 10−5 ICC, 1, 1, CG Abaqus/CAE Usage: Preset level 3 corresponds to the following: *PRESSURE EQUATION SOLVER, TYPE=AMG 250, 2, 10−5 ICC, 2, 2, BCGS Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page: Solver options: Specify, Preconditioner Type: Algebraic multi-grid Use one of the following options to choose a preset complexity level: Complexity Level: Preset: 1, 2, or 3 Use the following option to specify the Krylov solver and smoother settings directly: Complexity Level: User defined Specifying the solver type Three Krylov solver options are provided for the AMG solver. The default conjugate gradient solver is the fastest; however, in some cases where convergence difficulties are observed, the bi-conjugate gradient stabilized or flexible generalized minimal residual solvers are recommended. These two solvers are more robust but computationally more expensive than the conjugate gradient solver. Input File Usage: Use the following option to specify the Krylov solver type: *PRESSURE EQUATION SOLVER, TYPE=AMG first data line , , , solver type Abaqus/CAE Usage: where solver type is CG for the conjugate gradient solver (default), BCGS for the bi-conjugate gradient squared solver, and FGMRES for the flexible generalized minimum residual solver. Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page: Solver options: Specify, Preconditioner Type: Algebraic multi-grid Use one of the following options to specify the Krylov solver: Solver Type: Conjugate gradient, Bi-conjugate gradient, stabilized, or Flexible generalized minimal residual Specifying the residual smoother settings You can choose between incomplete factorization and polynomial residual smoothers that are used within the AMG preconditioner. While incomplete factorization is computationally more expensive than polynomial smoothing, in many cases this cost is amortized by fast convergence and robustness. Polynomial smoothing is recommended for problems with a very good mesh quality (i.e., no skewed or large aspect ratio elements). The number of pre- and post-smoothing sweeps can also be specified. It is recommended that you apply the same number of pre- and post-sweeps. For the polynomial smoother, a minimum of two pre- and post-sweeps are recommended. Input File Usage: Use the following option to specify the residual smoother settings: *PRESSURE EQUATION SOLVER, TYPE=AMG first data line smoother, pre-smoothing sweeps, post-smoothing sweeps Abaqus/CAE Usage: Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page: Solver options: Specify, Preconditioner Type: Algebraic multi-grid, Residual Smoother: Incomplete factorization or Polynomial, Pre-sweeps: select number, Post-sweeps: select number Time incrementation Abaqus/CFD uses second-order time-accurate integration by default, where all diffusive terms, advective terms, and body forces are integrated with the trapezoidal rule (Crank-Nicolson method). The default method is “second-order accurate” in that truncation errors within a time increment are proportional to the time increment squared, thus they decrease by a factor of four if the time increment is halved. You can individually select alternative time integrators for each of these terms. A fully implicit advection treatment is also available, which is particularly useful for quickly advancing toward steady-state solutions. Time increment size control By default, Abaqus/CFD uses an automatic time incrementation algorithm that continually adjusts the time increment size to satisfy the Courant-Friedrichs-Lewy (CFL) stability condition for advection. The default value, CFL=0.45, guarantees the solution’s stability. You can further limit the automatically computed time increment size by specifying a maximum value. You can also specify an initial time increment size. This value is automatically decreased as necessary to satisfy a maximum initial CFL value of 0.45 based on the starting conditions of the flow. Alternatively, you can select fixed time incrementation and specify the time increment size. In this case the time increment size remains constant throughout the step, but stability is not guaranteed. Input File Usage: Use the following option to specify automatic time incrementation (default): *CFD, INCREMENTATION=FIXED CFL time increment, time period, scale factor, suggested CFL, check increment, max allowable time increment divergence tolerance, , , , Use the following option to specify fixed time step incrementation: *CFD, INCREMENTATION=FIXED STEP SIZE time increment, time period, divergence tolerance, , , , For both options above, can be set to 0.5 for the Crank-Nicolson method (default), 0.6667 for the Galerkin method, or 1 for the first-order backward- Euler method. Abaqus/CAE Usage: Use the following options to specify automatic time incrementation: Step module: Create Step: General: Flow; Basic tabbed page: enter a value for Time period; Incrementation tabbed page: Type: Automatic (Fixed CFL); enter values for Initial time increment, Maximum CFL number, Increment adjustment frequency, Time step growth scale factor, Divergence tolerance Use the following option to specify fixed time step incrementation: Step module: Create Step: General: Flow; Basic tabbed page: enter a value for Time period; Incrementation tabbed page: Type: Fixed, enter values for Time increment and Divergence tolerance Use the following options to specify the time integration method for viscous/diffusive terms, boundary conditions, and advective terms: Viscous, Load/Boundary condition, or Advective: Trapezoid (1/2), Galerkin (2/3), or Backward-Euler (1) Time-accurate analysis The time integration parameters are all set by default to , which produces a second order–accurate semi-implicit method suitable for time-accurate transient analysis. When automatic time incrementation is used, you should specify CFL to maintain stability and time accuracy. Steady-state analysis In analyses where the goal is to reach a steady-state solution, the fully implicit (backward-Euler) method can be activated by setting all time integration parameters to . This method is unconditionally stable, allowing you to specify large CFL values to significantly increase the time increment size. Strict guidelines for selecting the maximum allowable CFL number are not available, and this maximum value may vary for different flows and meshes. CFL values of 10 or more have been used successfully for some analyses where only the final result is of interest. Monitoring output variables Abaqus/CFD provides a number of output variables that are useful for monitoring the health of a calculation and are good indicators for situations where the flow has reached a steady-state condition. These variables are written to the status (.sta) file and can be examined as the analysis job is executing. The RMS divergence output variable is useful for determining if a calculation is proceeding normally. Values of the RMS divergence output variable that are O(1) can indicate that the problem is incorrectly specified or that the calculation has become unstable. The global kinetic energy (KE) provides a good indicator for when the flow has reached a steady state; i.e., when the kinetic energy asymptotically approaches a constant value, the flow is typically achieving a steady-state condition where the velocities and pressure do not vary in time. Alternatively, the global kinetic energy can indicate a steady-periodic or chaotic flow situation as well. Initial conditions Initial conditions for the density, velocity, temperature, turbulent eddy viscosity, turbulent kinetic energy, and dissipation rate can be specified . If the density is omitted, the specified material density is used for incompressible flow simulations. For a well-posed incompressible flow problem, the initial velocity must satisfy the boundary conditions and also the imposed divergence-free condition; i.e., the solvability conditions. Abaqus/CFD automatically uses the user-defined boundary conditions and tests the specified velocity initial conditions to be sure the solvability conditions are satisfied. If they are not, the initial velocity is projected onto a divergence-free subspace, yielding initial conditions that define a well-posed incompressible Navier-Stokes problem. Therefore, in some circumstances, user-specified velocity initial conditions may be overridden with velocity conditions that satisfy solvability. Boundary conditions temperature, pressure, and eddy viscosity can be defined . During the analysis prescribed boundary conditions can be varied using an amplitude definition . All amplitude definitions except smooth step and solution-dependent amplitudes are available. By default, all boundary conditions are applied instantaneously. Velocity and pressure boundary conditions can be specified via user subroutines . Displacement and velocity boundary conditions at FSI interfaces are prescribed automatically by the definition of a co-simulation region; therefore, you should not prescribe these conditions at an FSI interface. Similarly, you should not define the temperature at a CHT interface; the temperature is automatically prescribed by the definition of a co-simulation region. For more information, see “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1. The specification of no-slip/no-penetration boundary conditions at walls requires the specification of the turbulent eddy viscosity and normal-distance function, which is handled automatically by Abaqus/CFD. Hydrostatic pressure condition In incompressible flows, the pressure is only known within an arbitrary additive constant value or the hydrostatic pressure. In many practical situations, the pressure at an outflow boundary may be prescribed, which, in effect, sets the hydrostatic pressure level. In cases where there is no pressure prescribed, it is necessary to set the hydrostatic pressure level at a minimum of one node in the mesh. The fluid reference pressure can be used to specify the hydrostatic pressure level. When there are no prescribed pressure boundary conditions, the fluid reference pressure establishes the hydrostatic pressure level and makes the pressure-increment equation non-singular. If pressure boundary conditions are prescribed in addition to the reference pressure level, the reference pressure simply adjusts the output pressures according to the specified pressure level. For more information, see “Specifying a fluid reference pressure” in “Concentrated loads,” Section 33.4.2. Loads The loading types for Abaqus/CFD include applied heat flux, volumetric heat-generation sources, general body forces, and gravity loading. Gravity loading defines the gravity vector used with a Boussinesq-type body force in buoyancy driven flow . Gravity loading can be used only in conjunction with the energy equation and will be ignored if used without the energy equation. During the analysis prescribed loads can be varied using an amplitude definition . All amplitude definitions except smooth step and solution-dependent amplitudes are available. Material options Material definitions in Abaqus/CFD follow the Abaqus conventions but also present several material properties specific to fluid dynamics. In Abaqus/CFD the typical material properties include viscosity, constant-pressure specific heat, density, and coefficient of thermal expansion. The thermal expansion is used with a Boussinesq-type body force in buoyancy driven flow. In contrast to Abaqus/Standard and Abaqus/Explicit, which use the constant-volume specific heat, the constant-pressure specific heat is required when the energy equation is used for thermal-flow problems. For problems involving an ideal gas, the user may optionally specify constant-volume specific heat and the ideal gas constant. Elements Abaqus/CFD supports three element types: the 8-node hexahedral element, FC3D8; the 6-node triangular prism element, FC3D6; and the 4-node tetrahedral element, FC3D4 elements,” Section 28.2.1). These elements cannot be mixed in a single connected fluid domain. However, a single flow model can contain multiple domains, each with a different element type. Output The output available from Abaqus/CFD for an incompressible fluid dynamic analysis includes both nodal and surface field data and element and surface time-history data. For the nodal and element output, the preselected field and history data include velocity (V), temperature (TEMP), pressure (PRESSURE), and turbulent eddy viscosity (TURBNU). In addition, preselected field data include displacement (U). Preselected data are not available for surface output. In addition to the preselected output, you can request several derived and auxiliary variables. All of the output variable identifiers are outlined in “Abaqus/CFD output variable identifiers,” Section 4.2.3. Input file template *HEADING … *NODE … *ELEMENT, TYPE=FC3D4 … *MATERIAL, NAME=matname *CONDUCTIVITY Data lines to define the thermal conductivity *DENSITY Data lines to define the fluid density *SPECIFIC HEAT, TYPE=CONSTANT PRESSURE Data lines to define the specific heat *VISCOSITY Data lines to define the fluid viscosity *INITIAL CONDITIONS, TYPE=TEMPERATURE, ELEMENT AVERAGE Data lines to prescribe initial temperatures at the elements *INITIAL CONDITIONS, TYPE=VELX, ELEMENT AVERAGE Data lines to prescribe initial x-velocity at the elements *INITIAL CONDITIONS, TYPE=VELY, ELEMENT AVERAGE Data lines to prescribe initial y-velocity at the elements *INITIAL CONDITIONS, TYPE=VELY, ELEMENT AVERAGE Data lines to prescribe initial y-velocity at the elements … *AMPLITUDE, NAME=velxamp, DEFINITION=TABULAR Data lines to define amplitude curve to be used for inlet x-velocity ** *STEP ** Incompressible flow example *CFD, INCOMPRESSIBLE NAVIER STOKES, INCREMENTATION=FIXED CFL Data lines to define incrementation ** ** Boundary conditions ** *FLUID BOUNDARY, TYPE=SURFACE inlet_surface, VELX, value for x-velocity inlet_surface, VELY, value for y-velocity inlet_surface, VELZ, value for z-velocity ** *FLUID BOUNDARY, TYPE=SURFACE temperature_surface, TEMP, value for temperature ** *FLUID BOUNDARY, TYPE=SURFACE outlet_surface, P, value for pressure ** ** Field output ** *OUTPUT, FIELD, TIME INTERVAL=interval for field output *ELEMENT OUTPUT PRESSURE, TEMP, TURBNU, V *NODE OUTPUT PRESSURE, TEMP, TURBNU, V ** ** History output ** *OUTPUT, HISTORY, FREQUENCY=interval for history output *ELEMENT OUTPUT, ELSET=element set for history output, FREQUENCY=SURFACE … *END STEP Additional references • Albets-Chico, X., C. D. Perez-Segarra, A. Olivia, and J. Bredberg, “Analysis of Wall-Function Approaches using Two-Equation Turbulence Models,” International Journal of Heat and Mass Transfer, vol. 51, p. 4940–4957, 2008. • Casey, M., and T. Wintergerste, ERCOFTAC Special Interest Group on “Quality and Trust in Industrial CFD”, European Research Community on Flow, Turbulence and Combustion (ERCOFTAC), 2000. • Craft, T. J., A. V. Gerasimov, H. Iacovides, and B. E. Launder, “Progress in the Generalization of Wall-Function Treatments,” International Journal of Heat and Fluid Flow, vol. 23, p. 148–160, 2002. • Durbin, P. A., “Limiters and wall treatments in applied turbulence modeling,” Fluid Dynamics research, vol. 41, p. 1–17, 2009. • Launder, B. E., and D. B. Spalding, “The Numerical Computation of Turbulent Flows,” Computer Methods in Applied Mechanics and Engineering, vol. 3, p. 269–289, 1974. • Nield, D.A., and A. Bejan, Convection in Porous Media, Springer, New York, Third edition, 2010. • Yakhot, V., S. A. Orszag, S. Thangam, T. B. Gatski, and C. G. Speziale, “Development of Turbulence Models for Shear Flows by a Double Expansion Technique,” Physics of Fluids A, vol. 4, no. 7, p. 1510–1520, 1992. 6.7 Electromagnetic analysis • “Electromagnetic analysis procedures,” Section 6.7.1 • “Piezoelectric analysis,” Section 6.7.2 • “Coupled thermal-electrical analysis,” Section 6.7.3 • “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4 • “Eddy current analysis,” Section 6.7.5 • “Magnetostatic analysis,” Section 6.7.6 6.7.1 ELECTROMAGNETIC ANALYSIS PROCEDURES Overview Abaqus/Standard offers several analysis procedures to model piezoelectric, electrical conduction, and electromagnetic phenomena. The distinct electrical phenomena modeled by these procedures is described first, followed by a brief overview of each procedure. Electrostatic, electrical conduction, magnetostatic, and electromagnetic analyses Piezoelectric effect is the electromechanical interaction exhibited by some materials. This coupled electrostatic-structural response is modeled using piezoelectric analysis in Abaqus/Standard. In this procedure the electric potential is a degree of freedom and its conjugate is the electric charge. Coupled thermal-electrical conduction, with or without structural coupling, is modeled using electrical procedures. In these procedures the electric potential is a degree of freedom and its conjugate is the electric current. While transient effects are ignored in electrical conduction, thus making it steady state, thermal fields can be modeled either as transient or steady state. Magnetostatic analysis is used to compute the magnetic fields due to direct currents. It solves the magnetostatic approximation to Maxwell’s equations. The magnetic vector potential is a degree of freedom in a magnetostatic analysis, and its conjugate is the surface current. Electromagnetic analysis is used to model the full coupling between time-varying electric and magnetic fields by solving Maxwell’s equations. In such an analysis the magnetic vector potential is a degree of freedom and its conjugate is the surface current. Electrostatic procedure The following electrostatic analysis procedure is available in Abaqus/Standard: • Piezoelectric analysis: In a piezoelectric material an electric potential gradient causes straining, while stress causes an electric potential in the material (“Piezoelectric analysis,” Section 6.7.2). This coupling is provided by defining the piezoelectric and dielectric coefficients of a material and can be used in natural frequency extraction, transient dynamic analysis, both linear and nonlinear static stress analysis, and steady-state dynamic analysis procedures. In all procedures, including nonlinear statics and dynamics, the piezoelectric behavior is always assumed to be linear. Steady electrical conduction procedures The following electrical conduction analyses procedures are available in Abaqus/Standard: • Coupled thermal-electrical analysis: The electric potential and temperature fields can be solved simultaneously by performing a coupled thermal-electrical analysis (“Coupled In these problems the energy dissipated by an thermal-electrical analysis,” Section 6.7.3). electrical current flowing through a conductor is converted into thermal energy, and the electrical conductivity can, in turn, be temperature dependent. Thermal loads can be applied, but deformation of the structure is not considered. Coupled thermal-electrical problems can be linear or nonlinear. • Fully coupled thermal-electrical-structural analysis: A coupled thermal-electrical-structural analysis is used to solve simultaneously for the stress/displacement, the electric potential, and the temperature fields. A coupled analysis is used when the thermal, electrical, and mechanical solutions affect each other strongly. An example of such a process is resistance spot welding, where two or more metal parts are joined by fusion at discrete points at the material interface. The fusion is caused by heat generated due to the current flow at the contact points, which depends on the pressure applied at these points. These problems can be transient or steady state and linear or nonlinear. Cavity radiation effects cannot be included in a fully coupled thermal-electrical-structural analysis. See “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4, for more details. Magnetostatic procedure The following magnetostatic analysis procedure is available in Abaqus/Standard: • Magnetostatic analysis: A magnetostatic analysis is used to solve for the magnetic vector potential, from which the magnetic field is computed in the entire domain. For example, the magnetic field due to the flow of direct current can be modeled. The procedure supports linear as well as nonlinear magnetic material properties. See “Magnetostatic analysis,” Section 6.7.6, for more details. Electromagnetic procedures Electromagnetic analyses are used to solve for the magnetic vector potential, from which both electric and magnetic fields are computed in the entire domain. The following electromagnetic analysis procedures are available in Abaqus/Standard: • Time-harmonic eddy current analysis: This procedure assumes time-harmonic excitation and It supports linear electrical conductivity and linear magnetic material behavior. For response. example, eddy currents induced in a workpiece that is in the vicinity of a source of excitation (such as a coil carrying alternating current) can be modeled. See “Time-harmonic analysis” in “Eddy current analysis,” Section 6.7.5, for more details. • Transient eddy current analysis: This procedure assumes general time variation of the excitation and response. It supports linear electrical conductivity and both linear and nonlinear magnetic material behavior. For example, eddy currents induced in a workpiece that is in the vicinity of a source of excitation (such as a coil carrying time-varying current) can be modeled. See “Transient analysis” in “Eddy current analysis,” Section 6.7.5, for more details. 6.7.2 PIEZOELECTRIC ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Piezoelectric behavior,” Section 26.5.2 • “Defining an analysis,” Section 6.1.2 • “Electromagnetic analysis procedures,” Section 6.7.1 • “Defining a concentrated charge,” Section 16.9.30 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a surface charge,” Section 16.9.31 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a body charge,” Section 16.9.32 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Coupled piezoelectric problems: • are those in which an electric potential gradient causes straining, while stress causes an electric potential gradient in the material; • are solved using an eigenfrequency extraction, modal dynamic, static, dynamic, or steady-state dynamic procedure; • require the use of piezoelectric elements and piezoelectric material properties; • can be performed for continuum problems in one, two, and three dimensions; and • can be used in both linear and nonlinear analysis (however, in nonlinear analysis the piezoelectric part of the constitutive behavior is assumed to be linear). Piezoelectric response The electrical response of a piezoelectric material is assumed to be made up of piezoelectric and dielectric effects: where is the electrical potential, is the component of the electric flux vector (also known as the electric displacement) in the ith material direction, is the piezoelectric stress coupling, is a small-strain component, is the material’s dielectric matrix for a fully constrained material, and is the gradient of the electrical potential along the ith material direction, . Defining piezoelectric and dielectric properties is discussed in “Piezoelectric behavior,” Section 26.5.2. The theoretical basis of the piezoelectric analysis capability in Abaqus is defined in “Piezoelectric analysis,” Section 2.10.1 of the Abaqus Theory Manual. Procedures available for piezoelectric analysis Piezoelectric analysis can be carried out with the following procedures: • “Static stress analysis,” Section 6.2.2 • “Implicit dynamic analysis using direct integration,” Section 6.3.2 • “Direct-solution steady-state dynamic analysis,” Section 6.3.4 • “Natural frequency extraction,” Section 6.3.5 • “Transient modal dynamic analysis,” Section 6.3.7 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 • “Subspace-based steady-state dynamic analysis,” Section 6.3.9 Initial conditions Initial conditions of piezoelectric quantities cannot be specified. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, for a description of the initial conditions that can be applied in static or dynamic procedures. Boundary conditions The electric potential at a node (degree of freedom 9) can be prescribed using a boundary condition . Displacement and rotation degrees of freedom can also be prescribed by using boundary conditions as described in the relevant static and dynamic analysis procedure sections. See “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Boundary conditions can be prescribed as functions of time by referring to amplitude curves (“Amplitude curves,” Section 33.1.2). In an eigenfrequency extraction step (“Natural frequency extraction,” Section 6.3.5 ) involving piezoelectric elements, the electric potential degree of freedom must be constrained at least at one node to remove singularities from the dielectric part of the element operator. Loads Both mechanical and electrical loads can be applied in a piezoelectric analysis. Applying mechanical loads The following types of mechanical loads can be prescribed in a piezoelectric analysis: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. Applying electrical loads The following types of electrical loads can be prescribed, as described in “Electromagnetic loads,” Section 33.4.5: • Concentrated electric charge. • Distributed surface electric charge and body electric charge. Loading in mode-based and subspace-based procedures Electrical charge loads should be used only in conjunction with residual modes in the eigenvalue extraction step, due to the “massless” mode effect. Since the electrical potential degrees of freedom do not have any associated mass, these degrees of freedom are essentially eliminated (similar to Guyan reduction or mass condensation) during the eigenvalue extraction. The residual modes represent the static response corresponding to the electrical charge loads, which will adequately represent the potential degree of freedom in the eigenspace. Predefined fields The following predefined fields can be specified in a piezoelectric analysis, as described in “Predefined fields,” Section 33.6.1: • Although temperature is not a degree of freedom in piezoelectric elements, nodal temperatures can be specified. The specified temperature affects only temperature-dependent material properties, if any. • The values of user-defined field variables can be specified. These values affect only field-variable- dependent material properties, if any. Material options The piezoelectric coupling matrix and the dielectric matrix are specified as part of the material definition for piezoelectric materials, as described in “Piezoelectric behavior,” Section 26.5.2. They are relevant only when the material definition is used with coupled piezoelectric elements. The mechanical behavior of the material can include linear elasticity only (“Linear elastic behavior,” Section 22.2.1). Elements Piezoelectric elements must be used in a piezoelectric analysis . The electric potential, , is degree of freedom 9 at each node of these elements. In addition, regular stress/displacement elements can be used in parts of the model where piezoelectric effects do not need to be considered. Output The following output variables are applicable to the electrical solution in a piezoelectric analysis: Element integration point variables: EENER EPG EPGM EPGn EFLX EFLXM EFLXn Electrostatic energy density. Magnitude and components of the electrical potential gradient vector, Magnitude of the electrical potential gradient vector. Component n of the electrical potential gradient vector (n=1, 2, 3). Magnitude and components of the electrical flux (displacement) vector, Magnitude of the electrical flux (displacement) vector. Component n of the electrical flux (displacement) vector (n=1, 2, 3). . . Whole element variables: CHRGS ELCTE Values of distributed electrical charges. Total electrostatic energy in the element, . Nodal variables: EPOT RCHG CECHG Input file template Electrical potential degree of freedom at a node. Reactive electrical nodal charge (conjugate to prescribed electrical potential). Concentrated electrical nodal charge. *HEADING … *MATERIAL, NAME=matl *ELASTIC Data lines to define linear elasticity *PIEZOELECTRIC Data lines to define piezoelectric behavior *DIELECTRIC Data lines to define dielectric behavior … *AMPLITUDE, NAME=name Data lines to define amplitude curve for defining concentrated electric charge ** *STEP, (optionally NLGEOM) *STATIC ** or *DYNAMIC, *FREQUENCY, *MODAL DYNAMIC, ** *STEADY STATE DYNAMICS (, DIRECT or , SUBSPACE PROJECTION) *BOUNDARY Data lines to define boundary conditions on electrical potential and displacement (rotation) degrees of freedom *CECHARGE, AMPLITUDE=name Data lines to define time-dependent concentrated electric charges *DECHARGE and/or *DSECHARGE Data lines to define distributed electric charges *CLOAD and/or *DLOAD and/or *DSLOAD Data lines to define mechanical loading *END STEP 6.7.3 COUPLED THERMAL-ELECTRICAL ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Electromagnetic analysis procedures,” Section 6.7.1 • “Electrical conductivity,” Section 26.5.1 • *COUPLED THERMAL-ELECTRICAL • *JOULE HEAT FRACTION • “Specifying a joule heat fraction,” Section 12.10.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Configuring a fully coupled, simultaneous heat transfer and electrical procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Coupled thermal-electrical problems: • are those in which coupling between the electrical potential and temperature fields make it necessary to solve both fields simultaneously; • require the use of coupled thermal-electrical elements, although pure heat transfer elements can also be used in the model; • can include a specification of the fraction of electrical energy that will be released as heat; • can include thermal interactions such as gap radiation, gap conductance, and heat generation between surfaces ; • can include cavity radiation effects ; • can include electrical interactions such as electrical current flowing across surfaces ; • allow for transient or steady-state thermal solutions and for steady-state electrical solutions; and • can be linear or nonlinear. Coupled thermal-electrical analysis Joule heating arises when the energy dissipated by an electrical current flowing through a conductor is converted into thermal energy. Abaqus/Standard provides a fully coupled thermal-electrical procedure for analyzing this type of problem: the coupled thermal-electrical equations are solved simultaneously for both temperature and electrical potential at the nodes. The capability includes the analysis of the electrical problem, the thermal problem, and the temperature-dependent coupling between the two problems. Coupling arises from two sources: electrical conductivity and internal heat generation, which is a function of the electrical current density. The thermal part of the problem can include heat conduction and heat storage (“Thermal properties: overview,” Section 26.2.1) as well as cavity radiation effects (“Cavity radiation,” Section 40.1.1). Forced convection caused by fluid flowing through the mesh is not considered. The thermal-electrical equations are unsymmetric; therefore, the unsymmetric solver is invoked automatically if you request coupled thermal-electrical analysis. For problems where coupling between the thermal and electrical solutions is weak or where a pure electrical conduction analysis is required for the entire model, the unsymmetric terms resulting from the interfield coupling may be small or zero. In these problems you can invoke the less costly symmetric storage and solution scheme by solving the thermal and electrical equations separately. The separated technique uses the symmetric solver by default. The thermal-electrical solution schemes are discussed below. The theoretical basis of coupled thermal-electrical analysis is described in detail in “Coupled thermal-electrical analysis,” Section 2.12.1 of the Abaqus Theory Manual. Governing electric field equation The electric field in a conducting material is governed by Maxwell’s equation of conservation of charge. Assuming steady-state direct current, the equation reduces to where V is any control volume whose surface is S, density (current per unit area), and is the outward normal to S, is the electrical current is the internal volumetric current source per unit volume. The flow of electrical current is described by Ohm’s law: where ) , is the electrical field intensity, defined as the negative of the gradient of the electrical potential is the electrical potential, is the electrical conductivity matrix, is the temperature, and are predefined field variables. Using Ohm’s law in the conservation equation, written in variational form, provides the governing equation of the finite element model: where is the current density entering the control volume across S. Defining the electrical conductivity The electrical conductivity, , can be isotropic, orthotropic, or fully anisotropic . Ohm’s law assumes that the electrical conductivity is independent of the electrical field, . The coupled thermal-electrical problem is nonlinear when the electrical conductivity depends on temperature. Specifying the amount of thermal energy generated due to electrical current Joule’s law describes the rate of electrical energy, as , dissipated by current flowing through a conductor The amount of this energy released as internal heat within the body is conversion factor. You specify is converted into heat ( The fraction given can include a unit conversion factor, if required. is an energy in the material definition. It is assumed that all the electrical energy ) if you do not include the joule heat fraction in the material description. , where Input File Usage: Abaqus/CAE Usage: *JOULE HEAT FRACTION Property module: material editor: Thermal→Joule Heat Fraction Steady-state analysis Steady-state analysis provides the steady-state solution directly. Steady-state thermal analysis means that the internal energy term (the specific heat term) in the governing heat transfer equation is omitted. Only direct current is considered in the electrical problem, and it is assumed that the system has negligible capacitance. (Electrical transient effects are so rapid that they can be neglected.) Input File Usage: Abaqus/CAE Usage: *COUPLED THERMAL-ELECTRICAL, STEADY STATE Step module: Create Step: General: Coupled thermal-electric: Basic: Response: Steady state Assigning a “time” scale to the analysis A steady-state analysis has no intrinsic physically meaningful time scale. Nevertheless, you can assign a “time” scale to the analysis step, which is often convenient for output identification and for specifying prescribed temperatures, electrical potential, and fluxes (heat flux and current density) with varying magnitudes. Thus, when steady-state analysis is chosen, you specify a “time” period and “time” incrementation parameters for the step; Abaqus/Standard then increments through the step accordingly. Any fluxes or boundary condition changes to be applied during a steady-state step should be given using appropriate amplitude references to specify their “time” variations (“Amplitude curves,” If fluxes and boundary conditions are specified for the step without amplitude Section 33.1.2). references, they are assumed to change linearly with “time” during the step—from their magnitudes at the end of the previous step (or zero, if this is the beginning of the analysis) to their newly specified magnitudes at the end of this step . Transient analysis Alternatively, the thermal portion of the coupled thermal-electrical problem can be considered transient. As in steady-state analysis, electrical transient effects are neglected. See “Uncoupled heat transfer analysis,” Section 6.5.2, for a more detailed description of the heat transfer capability in Abaqus/Standard. Input File Usage: Abaqus/CAE Usage: *COUPLED THERMAL-ELECTRICAL Step module: Create Step: General: Coupled thermal-electric: Basic: Response: Transient Time incrementation Time integration in the transient heat transfer problem is done with the same backward Euler method used in uncoupled heat transfer analysis. This method is unconditionally stable for linear problems. You can specify the time increments directly, or Abaqus can select them automatically based on a user- prescribed maximum nodal temperature change in an increment. Automatic time incrementation is generally preferred. Automatic incrementation The time increment size can be selected automatically based on a user-prescribed maximum allowable nodal temperature change in an increment, . Abaqus/Standard will restrict the time increments to ensure that these values are not exceeded at any node (except nodes with boundary conditions) during any increment of the analysis . Input File Usage: Abaqus/CAE Usage: *COUPLED THERMAL-ELECTRICAL, DELTMX= Step module: Create Step: General: Coupled thermal-electric: Basic: Response: Transient; Incrementation: Type: Automatic: Max. allowable temperature change per increment: Fixed incrementation If you select fixed time incrementation and do not specify user-specified initial time increment, , will then be used throughout the analysis. , fixed time increments equal to the Input File Usage: *COUPLED THERMAL-ELECTRICAL Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electric: Basic: Response: Transient; Incrementation: Type: Fixed: Increment size: Spurious oscillations due to small time increments In transient heat transfer analysis with second-order elements there is a relationship between the minimum usable time increment and the element size. A simple guideline is where is the time increment, is the density, c is the specific heat, k is the thermal conductivity, and is a typical element dimension (such as the length of a side of an element). If time increments smaller than this value are used in a mesh of second-order elements, spurious oscillations can appear in the solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations are nonphysical and may cause problems if temperature-dependent material properties are present. In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time increments are required, a finer mesh should be used in regions where the temperature changes rapidly. There is no upper limit on the time increment size (the integration procedure is unconditionally stable) unless nonlinearities cause convergence problems. Ending a transient analysis By default, a transient analysis will end when the specified time period has been completed. Alternatively, you can specify that the analysis should continue until steady-state conditions are reached. Steady state is defined by the temperature change rate; when the temperature changes at a rate that is less than the user-specified rate (given as part of the step definition), the analysis terminates. Input File Usage: Use the following option to end the analysis when the time period is reached: *COUPLED THERMAL-ELECTRICAL, END=PERIOD (default) Use the following option to end the analysis based on the temperature change rate: *COUPLED THERMAL-ELECTRICAL, END=SS Step module: Create Step: General: Coupled thermal-electric: Basic: Response: Transient; Incrementation: End step when temperature change is less than Abaqus/CAE Usage: Fully coupled solution schemes Abaqus/Standard offers an exact as well as an approximate implementation of Newton’s method for coupled thermal-electrical analysis. Exact implementation An exact implementation of Newton’s method involves a nonsymmetric Jacobian matrix as is illustrated in the following matrix representation of the coupled equations: where and are submatrices of the fully coupled Jacobian matrix, and are the respective corrections to the incremental electrical potential and temperature, are the electrical and thermal and residual vectors, respectively. Solving this system of equations requires the use of the unsymmetric matrix storage and solution scheme. Furthermore, the electrical and thermal equations must be solved simultaneously. The method provides quadratic convergence when the solution estimate is within the radius of convergence of the algorithm. The exact implementation is used by default. Approximate implementation Some problems require a fully coupled analysis in the sense that the electrical and thermal solutions In other words, the evolve simultaneously, but with a weak coupling between the two solutions. components in the off-diagonal submatrices are small compared to the components in the diagonal submatrices . For these problems a less costly solution may be obtained by setting the off-diagonal submatrices to zero, so that we obtain an approximate set of equations: , , As a result of this approximation the electrical and thermal equations can be solved separately, with fewer equations to consider in each subproblem. The savings due to this approximation, measured as solver time per iteration, will be of the order of a factor of two, with similar significant savings in solver storage of the factored stiffness matrix. Further, in situations without strong thermal loading due to cavity radiation, the subproblems may be fully symmetric or approximated as symmetric, so that the less costly symmetric storage and solution scheme can be used. The solver time savings for a symmetric solution is an additional factor of two. Unless you explicitly select the unsymmetric solver for the step (“Defining an analysis,” Section 6.1.2), the symmetric solver will be used with this separated technique. This modified form of Newton’s method does not affect solution accuracy since the fully coupled effect is considered through the residual vector at each increment in time. However, the rate of convergence is no longer quadratic and depends strongly on the magnitude of the coupling effect, so more iterations are generally needed to achieve equilibrium than with the exact implementation of Newton’s method. When the coupling is significant, the convergence rate becomes very slow and may prohibit the attainment of a solution. In such cases the exact implementation of Newton’s method is required. In cases where it is possible to use this approximation, the convergence in an increment will depend strongly on the quality of the first guess to the incremental solution, which you can control by selecting the extrapolation method used for the step . Input File Usage: Abaqus/CAE Usage: Use the following option to specify a separated solution scheme: *SOLUTION TECHNIQUE, TYPE=SEPARATED Step module: Create Step: General: Coupled thermal-electric: Other: Solution technique: Separated Uncoupled electric conduction and heat transfer analysis The coupled thermal-electrical procedure can also be used to perform uncoupled electric conduction analysis for the whole model or just part of the model (using coupled thermal-electrical elements). Uncoupled electrical analysis is available by omitting the thermal properties from the material description, in which case only the electric potential degrees of freedom are activated in the element and all heat transfer effects are ignored. If heat transfer effects are ignored in the entire model, you should invoke the separated solution technique described above. Use of this technique will then invoke the symmetric storage and solution scheme, which is an exact representation of a purely electrical problem. Similarly, coupled thermal-electrical elements can be used in an uncoupled heat transfer analysis (“Uncoupled heat transfer analysis,” Section 6.5.2), in which case all electric conduction effects are ignored. This feature is useful if a thermal-electrical analysis is followed by a pure heat conduction analysis. A typical example is a welding process, where the electric current is applied instantaneously, followed by a cooldown period during which no electrical effects need to be considered. The symmetric solver is activated by default in an uncoupled heat transfer analysis. Cavity radiation Cavity radiation can be activated in a heat transfer step. This feature involves interacting heat transfer between all of the facets of the cavity surface, dependent on the facet temperatures, facet emissivities, and the geometric viewfactors between each facet pair. When the thermal emissivity is a function of temperature or field variables, you can specify the maximum allowable emissivity change during an increment in addition to the maximum temperature change to control the time incrementation. See “Cavity radiation,” Section 40.1.1, for more information. Input File Usage: Use the following option in the step definition to activate cavity radiation: *RADIATION VIEWFACTOR Use the following option to specify the maximum allowable emissivity change: *HEAT TRANSFER, MXDEM=max_delta_emissivity You can specify the maximum allowable emissivity change for a heat transfer step. Step module: Create Step: General: Heat transfer: Incrementation: Max. allowable emissivity change per increment Abaqus/CAE Usage: Initial conditions By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures or field variables . Since only steady-state electrical currents are considered, the initial value of the electrical potential is not relevant. Boundary conditions Boundary conditions can be used to prescribe the electrical potential, 9), and the temperature, Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. (degree of freedom (degree of freedom 11), at the nodes. See “Boundary conditions in Boundary conditions can be specified as functions of time by referring to amplitude curves . A boundary without any prescribed boundary conditions corresponds to an insulated surface. Loads Both thermal and electrical loads can be applied in a coupled thermal-electrical analysis. Applying thermal loads The following types of thermal loads can be prescribed in a coupled thermal-electrical analysis, as described in “Thermal loads,” Section 33.4.4: • Concentrated heat fluxes. • Body fluxes and distributed surface fluxes. • Average-temperature radiation conditions. • Convective film conditions and radiation conditions. Applying electrical loads The following types of electrical loads can be prescribed, as described in “Electromagnetic loads,” Section 33.4.5: • Concentrated current. • Distributed surface current densities and body current densities. Predefined fields Predefined temperature fields are not allowed in coupled thermal-electrical analyses. Boundary conditions should be used instead to specify temperatures, as described above. Other predefined field variables can be specified in a coupled thermal-electrical analysis. These See “Predefined fields,” values affect only field-variable-dependent material properties, Section 33.6.1. if any. Material options Both thermal and electrical properties are active in coupled thermal-electrical analyses. properties are omitted, an uncoupled electrical analysis will be performed. If thermal All mechanical behavior material models (such as elasticity and plasticity) are ignored in a coupled thermal-electrical analysis. Thermal material properties For the heat transfer portion of the analysis, the thermal conductivity must be defined . The specific heat must also be defined for transient heat transfer problems . If changes in internal energy due to phase changes are important, latent heat can be defined . Thermal expansion coefficients (“Thermal expansion,” Section 26.1.2) are not meaningful in a coupled thermal-electrical analysis since deformation of the structure is not considered. Internal heat generation can be specified . Electrical material properties For the electrical portion of the analysis, the electrical conductivity must be defined . The electrical conductivity can be a function of temperature and user-defined field variables. The fraction of electrical energy dissipated as heat can also be defined, as explained above. Elements The simultaneous solution in a coupled thermal-electrical analysis requires the use of elements that have both temperature (degree of freedom 11) and electrical potential (degree of freedom 9) as nodal variables. The finite element model can also include pure heat transfer elements (so that a pure heat transfer analysis is provided for that part of the model) and coupled thermal-electrical elements for which no thermal properties are given (so that a pure electrical conduction solution is provided for that part of the model). Coupled thermal-electrical elements are available in Abaqus/Standard in one dimension, two dimensions (planar and axisymmetric), and three dimensions. See “Choosing the appropriate element for an analysis type,” Section 27.1.3. Output The following output variables can be used to request output relating to the electric conduction solution: Element integration point variables: EPG EPGM EPGn ECD JENER Magnitude and components of the electrical potential gradient vector, Magnitude of the electrical potential gradient vector. Component n of the electrical potential gradient vector (n=1, 2, 3). Magnitude and components of the electrical current density vector, J. Electrical energy dissipated due to flow of current, . . Whole element variables: ECURS NCURS ELJD Distributed applied electrical current. Electrical current at nodes due to electric conduction. Total electrical energy dissipated due to flow of current, . Nodal variables: EPOT RECUR CECUR Electrical potential, Reactive electrical current. Concentrated applied electrical current. . Whole model variables: ALLJD Electrical energy summed over the model. Surface interaction variables : ECD ECDA ECDT ECDTA SJD SJDA SJDT SJDTA WEIGHT Electrical current density. ECD multiplied by area. Time integrated ECD. Time integrated ECDA. Heat flux per unit area generated by the electrical current. SJD multiplied by area. Time integrated SJD. Time integrated SJDA. Heat distribution between interface surfaces, f. Considerations for steady-state coupled thermal-electrical analysis In a steady-state coupled thermal-electrical analysis the electrical energy dissipated due to flow of electrical current at an integration point (output variable JENER) is computed using the following relationship: denotes the electrical energy dissipated due to flow of electrical current and where step time. In the above relationship it is assumed that the rate of the electrical energy dissipation, has a constant value in the step that is equal to the value currently computed. is the current , The output variable JENER and the derived output variables ELJD and ALLJD contain the values of electrical energies dissipated in the current step only. Similarly, the contribution from the electrical current flow to the output variable ALLWK includes only the external work performed in the current step. Input file template *HEADING … *MATERIAL, NAME=mat1 *CONDUCTIVITY Data lines to define thermal conductivity *ELECTRICAL CONDUCTIVITY Data lines to define electrical conductivity * HEAT FRACTION Data lines to define the fraction of electric energy released as heat ** *STEP *COUPLED THERMAL-ELECTRICAL Data line to define incrementation and steady state *BOUNDARY Data lines to define boundary conditions on electrical potential and temperature degrees of freedom *CECURRENT Data lines to define concentrated currents *DECURRENT and/or *DSECURRENT Data lines to define distributed current densities *CFLUX and/or *DFLUX and/or *DSFLUX Data lines to define thermal loading *FILM and/or *SFILM and/or *RADIATE and/or *SRADIATE Data lines to define convective film and radiation conditions … *CONTACT PRINT or *CONTACT FILE Data lines to request output of surface interaction variables *END STEP 6.7.4 FULLY COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Coupled thermal-electrical analysis,” Section 6.7.3 • *COUPLED TEMPERATURE-DISPLACEMENT • “Configuring a fully coupled, simultaneous heat transfer, electrical, and structural procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A fully coupled thermal-electrical-structural analysis: • is performed when coupling between the displacement, temperature, and electrical potential fields makes it necessary to obtain solutions for all three fields simultaneously; • requires the existence of elements with displacement, temperature, and electrical potential degrees of freedom in the model; • allows for transient or steady-state thermal solutions, static displacement solutions, and steady-state electrical solutions; • can include thermal interactions such as gap radiation, gap conductance, and gap heat generation between surfaces ; • can include electrical interactions such as gap electrical conductance ; • cannot include cavity radiation effects but may include radiation boundary conditions ; • takes into account temperature dependence of material properties only for the properties that are assigned to elements with temperature degrees of freedom; • neglects inertia effects; and • can be transient or steady state. Fully coupled thermal-electrical-structural analysis A fully coupled thermal-electrical-structural analysis is the union of a coupled thermal-displacement analysis and a coupled thermal-electrical analysis . Coupling between the temperature and electrical degrees of freedom arises from temperature- dependent electrical conductivity and internal heat generation (Joule heating), which is a function of the electrical current density. The thermal part of the problem can include heat conduction and heat storage (“Thermal properties: overview,” Section 26.2.1). Forced convection caused by fluid flowing through the mesh is not considered. Coupling between the temperature and displacement degrees of from and internal heat generation, temperature-dependent material properties, which is a function of inelastic deformation of the material. In addition, contact conditions exist in some problems where the heat conducted between surfaces may depend strongly on the separation of the surfaces and/or the pressure transmitted across the surfaces as well as friction . thermal expansion, freedom arises Coupling between the electrical and displacement degrees of freedom arises in problems where electricity flows between contact surfaces. The electrical conduction may depend strongly on the separation of the surfaces and/or the pressure transmitted across the surfaces . An example of a simulation that requires a fully coupled thermal-electrical-structural analysis is resistance spot welding. In a typical spot welding process two or more thin metal sheets are pinched between two electrodes. A large current is passed between the electrodes, which melts the metal between the electrodes and forms a weld. The integrity of the weld depends on many parameters including the electrical conductance between the sheets (which can be a function of contact pressure and temperature). Steady-state analysis Steady-state analysis provides the steady-state solution directly. Steady-state thermal analysis means that the internal energy term (the specific heat term) in the governing heat transfer equation is omitted. A static displacement solution is assumed. Only direct current is considered in the electrical problem, and it is assumed that the system has negligible capacitance. Electrical transient effects are so rapid that they can be neglected. Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, STEADY STATE Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electrical- structural: Basic: Response: Steady state Assigning a “time” scale to the analysis In steady-state cases you should assign an arbitrary “time” scale to the step: you specify a “time” period and “time” incrementation parameters. This time scale is convenient for changing loads and boundary conditions through the step and for obtaining solutions to highly nonlinear (but steady-state) cases; however, for the latter purpose, transient analysis often provides a natural way of coping with the nonlinearity. Accounting for frictional slip heat generation Frictional slip heat generation is normally neglected in the steady-state case. However, it can still be accounted for if motions are used to specify translational or rotational nodal velocities in disk brake-type problems or if user subroutine FRIC provides the incremental frictional dissipation through the variable SFD. If frictional heat generation is present, the heat flux into the two contact surfaces depends on the slip rate of the surfaces. The “time” scale in this case cannot be described as arbitrary, and a transient analysis should be performed. Transient analysis Alternatively, you can perform a transient coupled thermal-electrical-structural analysis. As in steady- state analysis, electrical transient effects are neglected and a static displacement solution is assumed. You can control the time incrementation in a transient analysis directly, or Abaqus/Standard can control it automatically. Automatic time incrementation is generally preferred. Automatic incrementation controlled by a maximum allowable temperature change The time increments can be selected automatically based on a user-prescribed maximum allowable nodal temperature change in an increment, . Abaqus/Standard will restrict the time increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the analysis . Input File Usage: Abaqus/CAE Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, DELTMX= Step module: Create Step: General: Coupled thermal-electrical- structural: Basic: Response: Transient; Incrementation: Type: Automatic: Max. allowable temperature change per increment: Fixed incrementation If you do not specify , fixed time increments equal to the user-specified initial time increment, , will be used throughout the analysis. Input File Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electrical- structural: Basic: Response: Transient; Incrementation: Type: Fixed: Increment size: Spurious oscillations due to small time increments In transient analysis with second-order elements there is a relationship between the minimum usable time increment and the element size. A simple guideline is where is the time increment, is the density, c is the specific heat, k is the thermal conductivity, and is a typical element dimension (such as the length of a side of an element). If time increments smaller than this value are used in a mesh of second-order elements, spurious oscillations can appear in the solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations are nonphysical and may cause problems if temperature-dependent material properties are present. In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time increments are required, a finer mesh should be used in regions where the temperature changes rapidly. There is no upper limit on the time increment size (the integration procedure is unconditionally stable) unless nonlinearities cause convergence problems. Automatic incrementation controlled by the creep response The accuracy of the integration of time-dependent (creep) material behavior is governed by the user-specified accuracy tolerance parameter, . This parameter is used to prescribe the maximum strain rate change allowed at any point during an increment, as described in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4. The accuracy tolerance parameter can be specified together with the maximum allowable nodal temperature change in an increment, (described above); however, specifying the accuracy tolerance parameter activates automatic incrementation even if is not specified. Input File Usage: Abaqus/CAE Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, DELTMX= , CETOL=tolerance Step module: Create Step: General: Coupled thermal-electrical- structural: Basic: Response: Transient, toggle on Include creep/swelling/viscoelastic behavior; Incrementation: Type: Automatic: Max. allowable temperature change per increment: Creep/swelling/viscoelastic strain error tolerance: tolerance , Selecting explicit creep integration Nonlinear creep problems (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) that exhibit no other nonlinearities can be solved efficiently by forward-difference integration of the inelastic strains if the inelastic strain increments are smaller than the elastic strains. This explicit method is efficient computationally because, unlike implicit methods, iteration is not required as long as no other nonlinearities are present. Although this method is only conditionally stable, the numerical stability limit of the explicit operator is in many cases sufficiently large to allow the solution to be developed in a reasonable number of time increments. For most coupled thermal-electrical-structural analyses, however, the unconditional stability of the backward difference operator (implicit method) is desirable. In such cases the implicit integration scheme may be invoked automatically by Abaqus/Standard. Explicit integration can be less expensive computationally and simplifies implementation of user- defined creep laws in user subroutine CREEP; you can restrict Abaqus/Standard to using this method for creep problems (with or without geometric nonlinearity included). See “Rate-dependent plasticity: creep and swelling,” Section 23.2.4, for further details. Input File Usage: Abaqus/CAE Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, CETOL=tolerance, CREEP=EXPLICIT Step module: Create Step: General: Coupled thermal-electrical- structural: Basic: Response: Transient, toggle on Include creep/swelling/viscoelastic behavior; Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance, Creep/swelling/viscoelastic integration: Explicit Excluding creep and viscoelastic response You can specify that no creep or viscoelastic response will occur during a step even if creep or viscoelastic material properties have been defined. Input File Usage: Abaqus/CAE Usage: *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, DELTMX= , CREEP=NONE Step module: Create Step: General: Coupled thermal-electrical- structural: Basic: Response: Transient, toggle off Include creep/swelling/viscoelastic behavior Unstable problems Some types of analyses may develop local instabilities, such as surface wrinkling, material instability, or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with the aid of automatic incrementation. Abaqus/Standard offers a method of stabilizing this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1. Units In coupled problems where two or three different fields are active, take care when choosing the units of the problem. If the choice of units is such that the terms generated by the equations for each field are different by many orders of magnitude, the precision on some computers may be insufficient to resolve the numerical ill-conditioning of the coupled equations. Therefore, choose units that avoid ill-conditioned matrices. For example, consider using units of Mpascal instead of pascal for the stress equilibrium equations to reduce the disparity between the magnitudes of the stress equilibrium equations, the heat flux continuity equations, and the conservation of charge equations. Initial conditions By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures. Initial stresses, field variables, etc. can also be defined; “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the initial conditions that are available for a fully coupled thermal-electrical-structural analysis. Boundary conditions can be used to prescribe freedom 11), Boundary conditions displacements/rotations (degrees of freedom 1–6), or electrical potentials (degree of freedom 9) at nodes in a fully coupled thermal-electrical-structural analysis . temperatures (degree of Boundary conditions can be specified as functions of time by referring to amplitude curves (“Amplitude curves,” Section 33.1.2). Loads The following types of thermal loads can be prescribed in a fully coupled thermal-electrical-structural analysis, as described in “Thermal loads,” Section 33.4.4: • Concentrated heat fluxes. • Body fluxes and distributed surface fluxes. • Node-based film and radiation conditions. • Average-temperature radiation conditions. • Element and surface-based film and radiation conditions. The following types of mechanical loads can be prescribed: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The following types of electrical loads can be prescribed, as described in “Electromagnetic loads,” Section 33.4.5: • Concentrated current. • Distributed surface current densities and body current densities. Predefined fields Predefined temperature fields are not allowed in a fully coupled thermal-electrical-structural analysis. Boundary conditions should be used instead to prescribe temperature degree of freedom 11, as described earlier. Other predefined field variables can be specified in a fully coupled thermal-electrical-structural analysis. These values will affect only field-variable-dependent material properties, if any. See “Predefined fields,” Section 33.6.1. Material options The materials in a fully coupled thermal-electrical-structural analysis must have thermal properties (such as conductivity), mechanical properties (such as elasticity), and electrical properties (such as electrical conductivity) defined. See Part V, “Materials,” for details on the material models available in Abaqus. Internal heat generation can be specified; see “Uncoupled heat transfer analysis,” Section 6.5.2. Thermal strain will arise if thermal expansion (“Thermal expansion,” Section 26.1.2) is included in the material property definition. A fully coupled thermal-electrical-structural analysis can be used to analyze static creep and swelling problems, which generally occur over fairly long time periods (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4); viscoelastic materials (“Time domain viscoelasticity,” Section 22.7.1); or viscoplastic materials (“Rate-dependent yield,” Section 23.2.3). Inelastic energy dissipation as a heat source You can specify an inelastic heat fraction in a fully coupled thermal-electrical-structural analysis to provide for inelastic energy dissipation as a heat source. Plastic straining gives rise to a heat flux per unit volume of where constant), is the heat flux that is added into the thermal energy balance, is a user-defined factor (assumed is the stress, and is the rate of plastic straining. Inelastic heat fractions are typically used in the simulation of high-speed manufacturing processes involving large amounts of inelastic strain, where the heating of the material caused by its deformation significantly influences temperature-dependent material properties. The generated heat is treated as a volumetric heat flux source term in the heat balance equation. An inelastic heat fraction can be specified for materials with plastic behavior that use the Mises or Hill yield surface (“Inelastic behavior,” Section 23.1.1). It cannot be used with the combined isotropic/kinematic hardening model. The inelastic heat fraction can be specified for user-defined material behavior in Abaqus/Explicit and will be multiplied by the inelastic energy dissipation coded in the user subroutine to obtain the heat flux. In Abaqus/Standard the inelastic heat fraction cannot be used with user-defined material behavior; in this case the heat flux that must be added to the thermal energy balance is computed directly in the user subroutine. In Abaqus/Standard an inelastic heat fraction can also be specified for hyperelastic material definitions that include time-domain viscoelasticity (“Time domain viscoelasticity,” Section 22.7.1). The default value of the inelastic heat fraction is 0.9. If you do not include the inelastic heat fraction behavior in the material definition, the heat generated by inelastic deformation is not included in the analysis. Input File Usage: *INELASTIC HEAT FRACTION Specifying the amount of thermal energy generated due to electrical current Joule’s law describes the rate of electrical energy, as , dissipated by current flowing through a conductor The amount of this energy released as internal heat within the body is conversion factor. You specify is converted into heat ( The fraction given can include a unit conversion factor, if required. is an energy in the material definition. It is assumed that all the electrical energy ) if you do not include the joule heat fraction in the material description. , where Input File Usage: *JOULE HEAT FRACTION Elements Coupled thermal-electrical-structural elements that have displacements, temperatures, and electrical potentials as nodal variables are available. Simultaneous temperature/electrical potential/displacement solution requires the use of such elements; pure displacement and temperature-displacement elements can be used in part of the model in a fully coupled thermal-electrical-structural analysis, but pure heat transfer elements cannot be used. The first-order coupled thermal-electrical-structural elements in Abaqus use a constant temperature over the element to calculate thermal expansion. The second-order coupled thermal-electrical-structural elements in Abaqus use a lower-order interpolation for temperature than for displacement (parabolic variation of displacements and linear variation of temperature) to obtain a compatible variation of thermal and mechanical strain. Output See “Abaqus/Standard output variable identifiers,” Section 4.2.1, for a complete list of output variables. The types of output available are described in “Output,” Section 4.1.1. Considerations for steady-state coupled thermal-electrical-structural analysis In a steady-state coupled thermal-electrical-structural analysis the electrical energy dissipated due to flow of electrical current at an integration point (output variable JENER) is computed using the following relationship: denotes the electrical energy dissipated due to flow of electrical current and where step time. In the above relationship it is assumed that the rate of the electrical energy dissipation, has a constant value in the step that is equal to the value currently computed. is the current , The output variable JENER and the derived output variables ELJD and ALLJD contain the values of electrical energies dissipated in the current step only. Similarly, the contribution from the electrical current flow to the output variable ALLWK includes only the external work performed in the current step. Input file template *HEADING … ** Specify the coupled thermal-electrical-structural element type *ELEMENT, TYPE=Q3D8 … ** *STEP *COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL Data line to define incrementation *BOUNDARY Data lines to define nonzero boundary conditions on displacement, temperature or electrical potential degrees of freedom *CFLUX and/or *CFILM and/or *CRADIATE and/or *DFLUX and/or *DSFLUX and/or *FILM and/or *SFILM and/or *RADIATE and/or *SRADIATE Data lines to define thermal loads *CLOAD and/or *DLOAD and/or *DSLOAD Data lines to define mechanical loads *CECURRENT Data lines to define concentrated currents *DECURRENT and/or *DSECURRENT Data lines to define distributed current densities *FIELD Data lines to define field variable values *END STEP 6.7.5 EDDY CURRENT ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Mapping thermal and magnetic loads,” Section 3.2.22 • “Electromagnetic analysis procedures,” Section 6.7.1 • “Electrical conductivity,” Section 26.5.1 • “Magnetic permeability,” Section 26.5.3 • “Electromagnetic loads,” Section 33.4.5 • “Predefined loads for sequential coupling,” Section 16.1.3 • *ELECTROMAGNETIC • *D EM POTENTIAL • *DECURRENT • *DSECURRENT • “UDECURRENT,” Section 1.1.23 of the Abaqus User Subroutines Reference Manual • “UDEMPOTENTIAL,” Section 1.1.24 of the Abaqus User Subroutines Reference Manual • “UDSECURRENT,” Section 1.1.26 of the Abaqus User Subroutines Reference Manual • “Configuring a time-harmonic electromagnetic analysis” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a magnetic vector potential boundary condition,” Section 16.10.17 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Eddy current problems: • involve coupling between electric and magnetic fields, which are solved for simultaneously; • solve Maxwell’s equations describing electromagnetic phenomena under the low-frequency assumption that neglects the effects of displacement currents; • require the use of electromagnetic elements in the whole domain; • require that magnetic permeability is specified in the whole domain and electrical conductivity is specified in the conducting regions; • allows for both time-harmonic and transient electromagnetic solutions; • calculate as output variables, rate of Joule heating and intensity of magnetic body forces associated with eddy currents, and these output variables can be transferred from a time-harmonic electromagnetic solution to drive a subsequent heat transfer, coupled temperature-displacement, or stress/displacement analysis, thereby allowing for the coupling of electromagnetic fields with thermal and/or mechanical fields in a sequentially coupled manner; and • can be solved using continuum elements in two- and three-dimensional space. Eddy current analysis Eddy currents are generated in a metal workpiece when it is placed within a time-varying magnetic field. Joule heating arises when the energy dissipated by the eddy currents flowing through the workpiece is converted into thermal energy. This heating mechanism is usually referred to as induction heating; the induction cooker is an example of a device that uses this mechanism. The time-varying magnetic field is usually generated by a coil that is placed close to the workpiece. The coil carries either a known amount of total current or an unknown amount of current under a known potential (voltage) difference. The current in the coil is assumed to be alternating at a known frequency for a time-harmonic eddy current analysis but may have an arbitrary variation in time for a transient eddy current analysis. The time-harmonic eddy current analysis procedure is based on the assumption that a time-harmonic excitation with a certain frequency results in a time-harmonic electromagnetic response with the same frequency everywhere in the domain. In other words, both the electric and the magnetic fields oscillate at the same frequency as that of the alternating current in the coil. The transient eddy current analysis does not make any assumption regarding the time-variation of the current in the coil; in fact any arbitrary time variation can be specified, and the electric and magnetic fields follow from the solution to Maxwell’s equations in the time domain. The eddy current analysis provides output, such as Joule heat dissipation or magnetic body force intensity, that can be transferred, from a time-harmonic eddy current analysis only, to drive a subsequent heat transfer, coupled temperature-displacement, or stress/displacement analysis. This allows for modeling the interactions of the electromagnetic fields with thermal and/or mechanical fields in a sequentially coupled manner. See “Mapping thermal and magnetic loads,” Section 3.2.22, and “Predefined loads for sequential coupling,” Section 16.1.3, for details. Electromagnetic elements must be used to model the response of all the regions in an eddy current analysis including the coil, the workpiece, and the space in between and surrounding them. To obtain accurate solutions, the outer boundary of the space (surrounding the coil and the workpiece) being modeled must be at least a few characteristic length scales away from the device on all sides. The electromagnetic elements use an element edge-based interpolation of the fields instead of the standard node-based interpolation. The user-defined nodes only define the geometry of the elements; and the degrees of freedom of the element are not associated with these nodes, which has implications for applying boundary conditions . Governing field equations The electric and magnetic fields are governed by Maxwell’s equations describing electromagnetic phenomena. The formulation is based on the low-frequency assumption, which neglects the displacement current correction term in Ampere’s law. This assumption is appropriate when the wavelength of the electromagnetic waves corresponding to the excitation frequency is large compared to typical length scales over which the response is computed. In the following discussion, the governing equations are written for a linear medium. Time-harmonic analysis It is convenient to introduce a magnetic vector potential, . The solution procedure seeks a time-harmonic electromagnetic response, , such that the magnetic flux density vector , radians/sec when the system is subjected to a time-harmonic excitation of the same . In the represent the amplitudes of the magnetic vector potential ) with frequency frequency; for example, through an impressed oscillating volume current density, preceding expressions the vectors and and applied volume current density vector, respectively, while the exponential factors (with represent the corresponding phases. Under these assumptions, Maxwell’s equations reduce to in terms of the amplitudes of the field quantities, the electrical conductivity tensor, to the magnetic field, conductivity relates the volume current density, , through a constitutive equation of the form: and ; the magnetic permeability tensor, . The magnetic permeability relates the magnetic flux density, ; and , , while the electrical . , and the electric field, , by Ohm’s law: The variational form of the above equation is where tangential surface current density, if any, at the external surfaces. represents the variation of the magnetic vector potential, and represents the applied Abaqus/Standard solves the variational form of Maxwell’s equations for the in-phase (real) and out-of-phase (imaginary) components of the magnetic vector potential. The other field quantities are derived from the magnetic vector potential. Transient analysis It is convenient to introduce a magnetic vector potential, and time, such that the magnetic flux density vector time-dependent electromagnetic response, excitation; for example, through an impressed distribution of volume current density, these assumptions, Maxwell’s equations reduce to , assumed to be a function of spatial position . The solution procedure seeks a , when the system is subjected to a time-dependent . Under in terms of the field quantities, conductivity tensor, and ; the magnetic permeability tensor, . The magnetic permeability relates the magnetic flux density, ; and the electrical , to the magnetic field, conductivity relates the volume current density, , through a constitutive equation of the form: , and the electric field, , while the electrical . , by Ohm’s law: The variational form of the above equation is where tangential surface current density, if any, at the external surfaces. represents the variation of the magnetic vector potential, and represents the applied Abaqus/Standard solves the variational form of Maxwell’s equations for the components of the magnetic vector potential. The other field quantities are derived from the magnetic vector potential. Defining the magnetic behavior The magnetic behavior of the electromagnetic medium can be linear or nonlinear. However, only linear magnetic behavior is available for time-harmonic eddy current analysis. Linear magnetic behavior is characterized by a magnetic permeability tensor that is assumed to be independent of the magnetic field. It is defined through direct specification of the absolute magnetic permeability tensor, , which can be isotropic, orthotropic, or fully anisotropic . The magnetic permeability can also depend on temperature and/or predefined field variables. For a time-harmonic eddy current analysis, the magnetic permeability can also depend on frequency. Nonlinear magnetic behavior, which is available only for transient eddy current analysis, is characterized by magnetic permeability that depends on the strength of the magnetic field. The nonlinear magnetic material model in Abaqus is suitable for ideally soft magnetic materials characterized by a monotonically increasing response in B–H space, where B and H refer to the strengths of the magnetic flux density vector and the magnetic field vector, respectively. Nonlinear magnetic behavior is defined through direct specification of one or more B–H curves that provide B as a function of H and, optionally, temperature and/or predefined field variables, in one or more directions. Nonlinear magnetic behavior can be isotropic, orthotropic, or transversely isotropic (which is a special case of the more general orthotropic behavior). Defining the electrical conductivity The electrical conductivity, , can be isotropic, orthotropic, or fully anisotropic . The electrical conductivity can also depend on temperature and/or predefined field variables. For a time-harmonic eddy current analysis, the electrical conductivity can also depend on frequency. Ohm’s law assumes that the electrical conductivity is independent of the electrical field, . Time-harmonic analysis The eddy current analysis procedure provides the time-harmonic solution directly at a given excitation frequency. You can specify one or more excitation frequencies, one or more frequency ranges, or a combination of excitation frequencies and ranges. Input File Usage: *ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC lower_freq1, upper_freq1, num_pts1 lower_freq2, upper_freq2, num_pts2 ... single_freq1 single_freq2 ... For example, the following input illustrates the simplest case of specifying excitation at a single frequency: *ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC single_freq1 Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Electromagnetic, Time harmonic; enter data in table, and add rows as necessary Transient analysis The eddy current analysis procedure provides the transient solution to a given arbitrary time-dependent excitation. Input File Usage: Abaqus/CAE Usage: *ELECTROMAGNETIC, LOW FREQUENCY, TRANSIENT A transient eddy current analysis is not supported in Abaqus/CAE. Tme incrementation Time integration in the transient eddy current analysis is done with the backward Euler method. This method is unconditionally stable for linear problems but may lead to inaccuracies if time increments are too large. The resulting system of equations can be nonlinear in general, and Abaqus/Standard uses Newton’s method to solve the system. The solution usually is obtained as a series of increments, with iterations to obtain equilibrium within each increment. Increments must sometimes be kept small to ensure accuracy of the time integration procedure. The choice of increment size is also a matter of computational efficiency: if the increments are too large, more iterations are required. Furthermore, Newton’s method has a finite radius of convergence; too large an increment can prevent any solution from being obtained because the initial state is too far away from the equilibrium state that is being sought—it is outside the radius of convergence. Thus, there is an algorithmic restriction on the increment size. Automatic incrementation In most cases the default automatic incrementation scheme is preferred because it will select increment sizes based on computational efficiency. However, you must ensure that the time increments are such that the time integration results in an accurate solution. Abaqus/Standard does not have any built in checks to ensure integration accuracy. Input File Usage: Abaqus/CAE Usage: *ELECTROMAGNETIC, LOW FREQUENCY, TRANSIENT A transient eddy current analysis is not supported in Abaqus/CAE. Direct incrementation Direct user control of the increment size is also provided; if you have considerable experience with a particular problem, you may be able to select a more economical approach. Input File Usage: Abaqus/CAE Usage: *ELECTROMAGNETIC, LOW FREQUENCY, TRANSIENT, DIRECT A transient eddy current analysis is not supported in Abaqus/CAE. Ill-conditioning in eddy current analyses with electrically nonconductive regions In an eddy current analysis it is very common that large portions of the model consist of electrically nonconductive regions, such as air and/or a vacuum. In such cases it is well known that the associated stiffness matrix can be very ill-conditioned; i.e., it can have many singularities (Bíró, 1999). Abaqus uses a special iterative solution technique to prevent the ill-conditioned matrix from negatively impacting the computed electric and magnetic fields. The default implementation works well for many problems. However, there can be situations in which the default numerical scheme fails to converge or results in a noisy solution. In such cases adding a “small” amount of artificial electrical conductivity to the nonconductive domain may help regularize the problem and allow Abaqus to converge to the correct solution. The artificial electrical conductivity should be chosen such that the electromagnetic waves propagating through these regions undergo little modification and, in particular, do not experience the sharp exponential decay that is typical when such fields impinge upon a real conductor. It is recommended that you set the artificial conductivity to be about five to eight orders of magnitude less than that of any of the conductors in the model. As an alternative to specifying electrical conductivity in the nonconductive domain, Abaqus also provides a stabilization scheme to help mitigate the effects of the ill-conditioning. You can provide input to this stabilization algorithm by specifying the stabilization factor, which is assumed to be 1.0 by default if the stabilization scheme is used. Higher values of the stabilization factor lead to more stabilization, while lower values of the stabilization factor lead to less stabilization. Input File Usage: Use the following to use stabilization in a time-harmonic procedure: *ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC, STABILIZATION=stabilization factor Use the following to use stabilization in a transient procedure: *ELECTROMAGNETIC, LOW FREQUENCY, TRANSIENT, STABILIZATION=stabilization factor Initial conditions Initial values of temperature and/or predefined field variables can be specified. These values affect only temperature and/or field-variable-dependent material properties, if any. Initial conditions on the electric and/or magnetic fields cannot be specified in an eddy current analysis. Boundary conditions Electromagnetic elements use an element edge-based interpolation of the fields. The degrees of freedom of the element are not associated with the user-defined nodes, which only define the geometry of the element. Consequently, the standard node-based method of specifying boundary conditions cannot be used with electromagnetic elements. The method used for specifying boundary conditions for electromagnetic elements is described in the following paragraphs. Boundary conditions in Abaqus typically refer to what are traditionally known as Dirichlet-type boundary conditions in the literature, where the values of the primary variable are known on the whole boundary or on a portion of the boundary. The alternative, Neumann-type boundary conditions, refer to situations where the values of the conjugate to the primary variable are known on portions of the boundary. In Abaqus Neumann-type boundary conditions are represented as surface loads in the finite- element formulation. For electromagnetic boundary value problems, Dirichlet boundary conditions on an enclosing surface must be specified as is the outward normal to the surface, as discussed in this section. Neumann boundary conditions must be specified as the surface current density vector, , where , as discussed in “Loads” below. for the representative surfaces. In Abaqus Dirichlet boundary conditions are specified as magnetic vector potential, , on (element-based) surfaces that represent symmetry planes and/or external boundaries in the model; Abaqus computes In applications where the electromagnetic fields are driven by a current-carrying coil that is close to the workpiece, the model may span a domain that is up to 10 times the characteristic length scale associated with the coil/workpiece assembly. In such cases, the electromagnetic fields are assumed to have decayed sufficiently in the far-field, and the value of the magnetic vector potential can be set to zero in the far-field boundary. On the other hand, in applications such as one where a conductor is embedded in a uniform (but varying time-harmonically in a time-harmonic eddy current analysis or with a more general time variation in a transient eddy current analysis) far-field magnetic field, it may be necessary to specify nonzero values of the magnetic vector potential on some portions of the external boundary. In this case an alternative method to model the same physical phenomena is to specify the corresponding unique value of surface current density, can be computed based on known values of the , on the far-field boundary . far-field magnetic field. A surface without any prescribed boundary condition corresponds to a surface with zero surface currents, or no loads. Nonuniform boundary conditions can be defined with user subroutine UDEMPOTENTIAL. Prescribing boundary conditions in a time-harmonic eddy current analysis In a time-harmonic eddy current analysis the boundary conditions are assumed to be time harmonic and are applied simultaneously to both the real and imaginary parts of the magnetic vector potential. It is not possible to specify Dirichlet boundary conditions on the real parts and Neumann boundary conditions on the imaginary parts and vice versa. Abaqus automatically restrains both the real and imaginary parts even if only one part is prescribed explicitly. The unspecified part is assumed to have a magnitude of zero. When you prescribe the boundary condition on an element-based surface for a time-harmonic eddy current analysis , you must specify the surface name, the region type label (S), the boundary condition type label, an optional orientation name, the magnitude of the real part of the boundary condition, the direction vector for the real part of the boundary condition, the magnitude of the imaginary part of the boundary condition, and the direction vector for the imaginary part of the boundary condition. The optional orientation name defines the local coordinate system in which the components of the magnetic vector potential are defined. By default, the components are defined with respect to the global directions. The specified direction vector components are normalized by Abaqus and, thus, do not contribute to the magnitude of the boundary condition. During a time-harmonic eddy current analysis, frequency-dependent boundary conditions can be prescribed as described in “Frequency-dependent boundary conditions in a time-harmonic eddy current analysis” below. Input File Usage: Use the following option in a time-harmonic eddy current analysis to define both the real (in-phase) and imaginary (out-of-phase) parts of the boundary condition on element-based surfaces: *D EM POTENTIAL surface name, S, bc type label, orientation, magnitude of real part, direction vector of real part, magnitude of imaginary part, direction vector of imaginary part where the boundary condition type label (bc type label) can be MVP for a uniform boundary condition or MVPNU for a nonuniform boundary condition. Load module: Create Boundary Condition: choose Electrical/Magnetic for the Category and Magnetic vector potential for the Types for Selected Step; Distribution: Uniform or User-defined; real components + imaginary components Abaqus/CAE Usage: Prescribing boundary conditions in a transient eddy current analysis The method of specification of the boundary condition for a transient eddy current analysis is substantially similar to that of the time-harmonic eddy current analysis, except that the concepts of real and imaginary are not relevant any more. In this case you specify the magnitude of the magnetic vector potential, followed by its direction vector. The specified direction vector components are normalized by Abaqus and, thus, do not contribute to the magnitude of the boundary condition. During a transient eddy current analysis, prescribed boundary conditions can be varied using an amplitude definition . Input File Usage: Use the following option in a transient eddy current analysis to define the boundary condition on element-based surfaces: *D EM POTENTIAL surface name, S, bc type label, orientation, magnitude, direction vector where the boundary condition type label (bc type label) can be MVP for a uniform boundary condition or MVPNU for a nonuniform boundary condition. Abaqus/CAE Usage: Transient eddy current analysis is not supported in Abaqus/CAE. Frequency-dependent boundary conditions in a time-harmonic eddy current analysis An amplitude definition can be used to specify the amplitude of a boundary condition as a function of frequency (“Amplitude curves,” Section 33.1.2). Input File Usage: Use both of the following options: *AMPLITUDE, NAME=name *D EM POTENTIAL, AMPLITUDE=name Load or Interaction module: Create Amplitude: Name: amplitude_name Load module: Create Boundary Condition: choose Electrical/Magnetic for the Category and Magnetic vector potential for the Types for Selected Step; Amplitude: amplitude_name Abaqus/CAE Usage: Loads The following types of electromagnetic loads can be applied in an eddy current analysis : analysis, and • Element-based distributed volume current density vector: in a transient eddy current analysis • Surface-based distributed surface current density vector: in a transient eddy current analysis analysis, and in a time-harmonic eddy current in a time-harmonic eddy current All loads in a time-harmonic eddy current analysis are assumed to be time-harmonic with the excitation frequency. During a transient eddy current analysis all loads can be varied using an amplitude definition . Nonuniform loads can be specified using user subroutines UDECURRENT and UDSECURRENT. Frequency-dependent loading in a time-harmonic eddy current analysis In a time-harmonic eddy current analysis, an amplitude definition can be used to specify the amplitude of a load as a function of frequency (“Amplitude curves,” Section 33.1.2). Predefined fields Predefined temperature and field variables can be specified in an eddy current analysis. These values affect only temperature and/or field-variable-dependent material properties, if any. See “Predefined fields,” Section 33.6.1. Material options Magnetic material behavior must be specified everywhere in the model. Only linear magnetic behavior is supported in a time-harmonic eddy current analysis, but nonlinear magnetic behavior is also supported in a transient eddy current analysis. Linear magnetic behavior can be defined by specifying the magnetic permeability directly, while nonlinear magnetic behavior is defined in terms of one or more B–H curves. Electrical conductivity must be specified in conductor regions. All other material properties are ignored in an eddy current analysis. Both magnetic permeability and electrical conductivity can be functions of frequency, predefined temperature, and field variables in a time-harmonic eddy current analysis. In a transient eddy current analysis, all material behavior can be functions of predefined temperature and/or field variables. Elements Electromagnetic elements must be used to model all regions in an eddy current analysis. Unlike conventional finite elements, which use node-based interpolation, these elements use edge-based interpolation with the tangential components of the magnetic vector potential along element edges serving as the primary degrees of freedom. Electromagnetic elements are available in Abaqus/Standard in two dimensions (planar only) and three dimensions . The planar elements are formulated in terms of an in-plane magnetic vector potential, thereby the magnetic flux density and magnetic field vectors only have an out-of-plane component. The electric field and the current density vectors are in-plane for the planar elements. Output Eddy current analysis provides output only to the output database (.odb) file . Output to the data (.dat) file and to the results (.fil) file is not available. For the first four vector quantities listed below (which are derived from the magnetic vector potential and the constitutive equations), the magnitude and components of the real and imaginary parts are output in a time-harmonic eddy current procedure. Element centroidal variables: EMB EMH EME EMCD Magnitude and components of the magnetic flux density vector, Magnitude and components of the magnetic field vector, . . Magnitude and components of the electric field vector, Magnitude and components of the eddy current vector, . , in conducting regions. EMBF EMBFC EMJH Magnetic body force intensity vector (force per unit volume per unit time) due to flow of current. Complex magnetic body force intensity vector (real and imaginary parts of the force per unit volume) due to flow of current. Only available in a time-harmonic eddy current analysis. Rate of Joule heating (amount of heat per unit volume per unit time) due to flow of current. Whole element variables: ELJD Total rate of Joule heating (amount of heat per unit time) due to flow of current in an element. Whole model variables: ALLJD Rate of Joule heating (amount of heat per unit time) summed over the model or an element set. Input file template The following is an input file template that makes use of linear magnetic material behavior in a time- harmonic eddy current analysis: *HEADING … *MATERIAL, NAME=mat1 *MAGNETIC PERMEABILITY Data lines to define magnetic permeability *ELECTRICAL CONDUCTIVITY Data lines to define electrical conductivity in the conductor region ** *STEP *ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC Data line to specify excitation frequencies *D EM POTENTIAL Data lines to define boundary conditions on magnetic vector potential *DECURRENT Data lines to define element-based distributed volume current density vector *DSECURRENT Data lines to define surface-based distributed surface current density vector *OUTPUT, FIELD or HISTORY Data lines to request element-based output *ENERGY OUTPUT Data line to request whole model Joule heat dissipation output *END STEP The following is an input file template that makes use of nonlinear magnetic material behavior in a transient eddy current analysis: *HEADING … *MATERIAL, NAME=mat1 *MAGNETIC PERMEABILITY, NONLINEAR *NONLINEAR BH, DIR=direction Data lines to define nonlinear B-H curve *ELECTRICAL CONDUCTIVITY Data lines to define electrical conductivity in the conductor region ** *STEP *ELECTROMAGNETIC, LOW FREQUENCY, TRANSIENT *D EM POTENTIAL Data lines to define boundary conditions on magnetic vector potential *DECURRENT Data lines to define element-based distributed volume current density vector *DSECURRENT Data lines to define surface-based distributed surface current density vector *OUTPUT, FIELD or HISTORY Data lines to request element-based output *ENERGY OUTPUT Data line to request whole model Joule heat dissipation output *END STEP Additional reference • Bíró, O., “Edge Element Formulation of Eddy Current Problems,” Computer Methods in Applied Mechanics and Engineering, vol. 169, pp. 391–405, 1999. 6.7.6 MAGNETOSTATIC ANALYSIS Product: Abaqus/Standard References • “Electromagnetic analysis procedures,” Section 6.7.1 • “Magnetic permeability,” Section 26.5.3 • “Electromagnetic loads,” Section 33.4.5 • *MAGNETOSTATIC • *D EM POTENTIAL • *DECURRENT • *DSECURRENT • “UDECURRENT,” Section 1.1.23 of the Abaqus User Subroutines Reference Manual • “UDEMPOTENTIAL,” Section 1.1.24 of the Abaqus User Subroutines Reference Manual • “UDSECURRENT,” Section 1.1.26 of the Abaqus User Subroutines Reference Manual Overview Magnetostatic problems: • solve the magnetostatic approximation of Maxwell’s equations describing electromagnetic phenomena and compute the magnetic fields due to direct currents; • involve only magnetic fields, which are assumed to be vary slowly in time such that electromagnetic coupling can be neglected; • require the use of electromagnetic elements in the whole domain; • require that magnetic permeability is specified in the whole domain; • can be solved with nonlinear magnetic behavior; and • can be solved using continuum elements in two- and three-dimensional space. Magnetostatic analysis A direct current creates a static magnetic field in the space surrounding the current carrying region. For applications where the magnitude of the direct current can be assumed to be a constant or to vary slowly with time, coupling between magnetic and electric fields can be neglected. The magnetostatic approximation to Maxwell’s equations involves the magnetic fields only. Magnetostatic analysis provides a solution for applications where the above assumptions are valid. Electromagnetic elements must be used to model the response of all the regions in a magnetostatic analysis, including regions such as current carrying coils and the surrounding space. To obtain accurate solutions, the outer boundary of the space being modeled must be at least a few characteristic length scales away from the region of interest on all sides. Electromagnetic elements use an element edge-based interpolation of the fields instead of the standard node-based interpolation. The user-defined nodes only define the geometry of the elements; and the degrees of freedom of the element are not associated with these nodes, which has implications for applying boundary conditions . Governing field equations The magnetic fields are governed by the magnetostatic approximation to Maxwell’s equations describing electromagnetic phenomena. It is convenient to introduce a magnetic vector potential, , such that the magnetic flux density . The solution procedure seeks a static magnetic response due to, for example, an in some regions of the model. The magnetostatic vector impressed direct volume current density distribution, approximation to Maxwell’s equations is given by in terms of the field quantities, permeability relates the magnetic flux density, equation of the form: and . and the magnetic permeability tensor, , to the magnetic field, . The magnetic , through a constitutive The variational form of the above equation is where tangential surface current density, if any, at the external surfaces. represents the variation of the magnetic vector potential, and represents the applied Abaqus/Standard solves the variational form of Maxwell’s equations for the components of the magnetic vector potential. The other field quantities are derived from the magnetic vector potential. In the following discussion, the governing equations are written for a linear medium. Defining the magnetic behavior The magnetic behavior of the electromagnetic medium can be linear or nonlinear. Linear magnetic behavior is characterized by a magnetic permeability tensor that is assumed to be independent of the magnetic field. It is defined through direct specification of the absolute magnetic permeability tensor, , which can be isotropic, orthotropic, or fully anisotropic . The magnetic permeability can also depend on temperature and/or predefined field variables. Nonlinear magnetic behavior is characterized by magnetic permeability that depends on the strength of the magnetic field. The nonlinear magnetic material model in Abaqus is suitable for ideally soft magnetic materials characterized by a monotonically increasing response in B–H space, where B and H refer to the strengths of the magnetic flux density vector and the magnetic field vector, respectively. Nonlinear magnetic behavior is defined through direct specification of one or more B–H curves that provide B as a function of H and, optionally, temperature and/or predefined field variables, in one or more directions. Nonlinear magnetic behavior can be isotropic, orthotropic, or transversely isotropic (which is a special case of the more general orthotropic behavior). Magnetostatic analysis Magnetostatic analysis provides the magnetic flux density and the magnetic field at a given value of the impressed direct current. Input File Usage: *MAGNETOSTATIC Ill-conditioning in magnetostatic analyses In magnetostatic analysis the stiffness matrix can be very ill-conditioned; i.e., it can have many singularities. Abaqus uses a special iterative solution technique to prevent the ill-conditioned matrix from negatively impacting the computed magnetic fields. The default implementation works well for many problems. However, there can be situations in which the default numerical scheme fails to converge. Abaqus provides a stabilization scheme to help mitigate the effects of the ill-conditioning. You can provide input to this stabilization algorithm by specifying the stabilization factor, which is assumed to be 1.0 by default if the stabilization scheme is used. Higher values of the stabilization factor lead to more stabilization, while lower values of the stabilization factor lead to less stabilization. Input File Usage: *MAGNETOSTATIC, STABILIZATION=stabilization factor Initial conditions Initial values of temperature and/or predefined field variables can be specified. These values affect only temperature and/or field-variable-dependent material properties, if any. Initial conditions on magnetic fields cannot be specified in a magnetostatic analysis. Boundary conditions Electromagnetic elements use an element edge-based interpolation of the fields. The degrees of freedom of the element are not associated with the user-defined nodes, which only define the geometry of the element. Consequently, the standard node-based method of specifying boundary conditions cannot be used with electromagnetic elements. Boundary conditions in Abaqus typically refer to what are traditionally known as Dirichlet-type boundary conditions in the literature, where the values of the primary variable are known on the whole boundary or on a portion of the boundary. The alternative, Neumann-type boundary conditions, refer to situations where the values of the conjugate to the primary variable are known on portions of the boundary. In Abaqus, Neumann-type boundary conditions are represented as surface loads in the finite element formulation. For electromagnetic boundary value problems, including magnetostatic problems, Dirichlet boundary conditions on an enclosing surface must be specified as is the outward , where normal to the surface, as discussed in this section. Neumann boundary conditions must be specified as the surface current density vector, , as discussed in “Loads” below. In Abaqus, Dirichlet boundary conditions are specified as magnetic vector potential, , on (element-based) surfaces that represent symmetry planes and/or external boundaries in the model; Abaqus computes for the representative surfaces. The model may span a domain that is up to 10 times some characteristic length scale for the problem. In such cases the magnetic fields are assumed to have decayed sufficiently in the far-field, and the value of the magnetic vector potential can be set to zero in the far-field boundary. On the other hand, in applications such as one where a magnetic material is embedded in a uniform far-field magnetic field, it may be necessary to specify nonzero values of the magnetic vector potential on some portions of the external boundary. In this case an alternative method to model the same physical phenomena is to specify the corresponding unique value of surface current density, can be computed based on known values of the far-field magnetic field. , on the far-field boundary . In a magnetostatic analysis the boundary conditions are assumed to be either constant or varying slowly with time. The time variation can be specified using an amplitude definition (“Amplitude curves,” Section 33.1.2) A surface without any prescribed boundary condition corresponds to a surface with zero surface currents or no loads. When you prescribe the boundary condition on an element-based surface , you must specify the surface name, the region type label (S), the boundary condition type label, an optional orientation name, the magnitude of the magnetic vector potential, and the direction vector for the magnetic vector potential. The optional orientation name defines the local coordinate system in which the components of the magnetic vector potential are defined. By default, the components are defined with respect to the global directions. The specified vector components are normalized by Abaqus and, thus, do not contribute to the magnitude of the boundary condition. Nonuniform boundary conditions can be defined with user subroutine UDEMPOTENTIAL. Input File Usage: Use the following option to define both the real (in-phase) and imaginary (out- of-phase) parts of the boundary condition on element-based surfaces: *D EM POTENTIAL surface name, S, bc type label, orientation, magnitude, direction vector where the boundary condition type label (bc type label) can be MVP for a uniform boundary condition or MVPNU for a nonuniform boundary condition. Loads The following types of electromagnetic loads can be applied in a magnetostatic analysis : • Element-based distributed volume current density vector, • Surface-based distributed surface current density vector, During the analysis the prescribed load can be varied using an amplitude definition (“Amplitude curves,” Section 33.1.2). Predefined fields Predefined temperature and field variables can be specified in a magnetostatic analysis. These values affect only temperature and/or field-variable-dependent material properties, if any. See “Predefined fields,” Section 33.6.1. Material options The magnetic behavior must be defined everywhere in the model, either by specifying the absolute magnetic permeability tensor for linear magnetic behavior or by specifying the B–H curve-based response for nonlinear magnetic behavior. All other material properties, including electrical conductivity, are ignored in a magnetostatic analysis. The magnetic behavior can be functions of predefined temperature and/or field variables. Elements Electromagnetic elements must be used to model all regions in a magnetostatic analysis. Unlike conventional finite elements, which use node-based interpolation, these elements use edge-based interpolation with the tangential components of the magnetic vector potential along element edges serving as the primary degrees of freedom. Electromagnetic elements are available in Abaqus/Standard in two dimensions (planar only) and three dimensions . The planar elements are formulated in terms of an in-plane magnetic vector potential, thereby the magnetic flux density and magnetic field vectors have only an out-of-plane component. Output Magnetostatic analysis provides output only to the output database (.odb) file . Output to the data (.dat) file and to the results (.fil) file is not available. Element centroidal variables: EMB EMH Magnitude and components of the magnetic flux density vector, Magnitude and components of the magnetic field vector, . . Input file template *HEADING … *MATERIAL, NAME=mat1 *MAGNETIC PERMEABILITY, NONLINEAR Data lines to define magnetic permeability for linear magnetic behavior; no data required here for nonlinear magnetic behavior *NONLINEAR BH, DIR=direction Data lines to define nonlinear B-H curve ** *STEP *MAGNETOSTATIC Data line to define time incrementation *D EM POTENTIAL Data lines to define boundary conditions on magnetic vector potential *DECURRENT Data lines to define element-based distributed volume current density vector *DSECURRENT Data lines to define surface-based distributed surface current density vector *OUTPUT, FIELD or HISTORY Data lines to request element-based output *END STEP 6.8 Coupled pore fluid flow and stress analysis • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 • “Geostatic stress state,” Section 6.8.2 6.8.1 COUPLED PORE FLUID DIFFUSION AND STRESS ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Pore fluid flow properties,” Section 26.6.1 • *SOILS • “Defining pore fluid expansion” in “Defining a fluid-filled porous material,” Section 12.12.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Configuring an effective stress analysis for fluid-filled porous media” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A coupled pore fluid diffusion/stress analysis: • is used to model single phase, partially or fully saturated fluid flow through porous media; • can be performed in terms of either total pore pressure or excess pore pressure by including or excluding the pore fluid weight; • requires the use of pore pressure elements with associated pore fluid flow properties defined; • can, optionally, also model heat transfer due to conduction in the soil skeleton and the pore fluid, and convection due to the flow of the pore fluid, through the use of coupled temperature–pore pressure displacement elements; • can be transient or steady-state; • can be linear or nonlinear; and • can include pore pressure contact between bodies . Typical applications Some of the more common coupled pore fluid diffusion/stress (and, optionally, thermal) analysis problems that can be analyzed with Abaqus/Standard are: • Saturated flow: Soil mechanics problems generally involve fully saturated flow, since the solid is fully saturated with ground water. Typical examples of saturated flow include consolidation of soils under foundations and excavation of tunnels in saturated soil. • Partially saturated flow: Partially saturated flow occurs when the wetting liquid is absorbed into or exsorbed from the medium by capillary action. Irrigation and hydrology problems generally include partially saturated flow. • Combined flow: Combined fully saturated and partially saturated flow occurs in problems such as seepage of water through an earth dam, where the position of the phreatic surface (the boundary between fully saturated and partially saturated soil) is of interest. • Moisture migration: Although not normally associated with soil mechanics, moisture migration problems can also be solved using the coupled pore fluid diffusion/stress procedure. These problems may involve partially saturated flow in polymeric materials such as paper towels and sponge-like materials; in the biomedical industry they may also involve saturated flow in hydrated soft tissues. In some applications, such as a source of heat buried in soil, it is important to model the coupling between the mechanical deformation, pore fluid flow, and heat transfer. In such problems the difference in the thermal expansion coefficients between the soil and the pore fluid often plays an important role in determining the rate of diffusion of the pore fluid and heat from the source. • Combined heat transfer and pore fluid flow: Flow through porous media A porous medium is modeled in Abaqus/Standard by a conventional approach that considers the medium as a multiphase material and adopts an effective stress principle to describe its behavior. The porous medium modeling provided considers the presence of two fluids in the medium. One is the “wetting liquid,” which is assumed to be relatively (but not entirely) incompressible. Often the other is a gas, which is relatively compressible. An example of such a system is soil containing ground water. When the medium is partially saturated, both fluids exist at a point; when it is fully saturated, the voids are completely filled with the wetting liquid. The elementary volume, , is made up of a volume of grains of solid material, , that is free ; a volume of voids, to move through the medium if driven. In some systems (for example, systems containing particles that absorb the wetting liquid and swell in the process) there may also be a significant volume of trapped wetting liquid, ; and a volume of wetting liquid, . The porous medium is modeled by attaching the finite element mesh to the solid phase; fluid can flow through this mesh. The mechanical part of the model is based on the effective stress principle defined in “Effective stress principle for porous media,” Section 2.8.1 of the Abaqus Theory Manual. The model also uses a continuity equation for the mass of wetting fluid in a unit volume of the medium. This equation is described in “Continuity statement for the wetting liquid phase in a porous medium,” Section 2.8.4 of the Abaqus Theory Manual. It is written with pore pressure (the average pressure in the wetting fluid at a point in the porous medium) as the basic variable (degree of freedom 8 at the nodes). The conjugate flux variable is the volumetric flow rate at the node, . The porous medium is partially saturated when the pore liquid pressure, , is negative. Coupled flow and heat transfer through porous media Optionally, heat transfer due to conduction in the soil skeleton and pore fluid, as well as convection in the pore fluid, can also be modeled. This capability represents an enhancement to the basic pore fluid flow capabilities discussed in the earlier paragraphs and requires the use of coupled temperature–pore pressure elements that have temperature as an additional degree of freedom (degree of freedom 11 at the nodes) in addition to the pore pressure and the displacement components. When you use the coupled temperature–pore pressure elements, Abaqus solves the heat transfer equation in addition to and in a fully coupled manner with the continuity equation and the mechanical equilibrium equations. Only linear brick, first-order axisymmetric, and second-order modified tetrahedrons are available for modeling coupled heat transfer with pore fluid flow and mechanical deformation. Coupled temperature–pore pressure elements are not supported in Abaqus/CAE. Total and excess pore fluid pressure The coupled pore fluid diffusion/stress analysis capability can provide solutions either in terms of total or “excess” pore fluid pressure. The excess pore fluid pressure at a point is the pore fluid pressure in excess of the hydrostatic pressure required to support the weight of pore fluid above the elevation of the material point. The difference between total and excess pore pressure is relevant only for cases in which gravitational loading is important; for example, when the loading provided by the hydrostatic pressure in the pore fluid is large or when effects like “wicking” (transient capillary suction of liquid into a dry column) are being studied. Total pore pressure solutions are provided when the gravity distributed load is used to define the gravity load on the model. Excess pore pressure solutions are provided in all other cases; for example, when gravity loading is defined with body force distributed loads. Steady-state analysis Steady-state coupled pore pressure/effective stress analysis assumes that there are no transient effects in the wetting liquid continuity equation; that is, the steady-state solution corresponds to constant wetting liquid velocities and constant volume of wetting liquid per unit volume in the continuum. Thus, for example, thermal expansion of the liquid phase has no effect on the steady-state solution: it is a transient effect. Therefore, the time scale chosen during steady-state analysis is relevant only to rate effects in the constitutive model used for the porous medium (excluding creep and viscoelasticity, which are disabled in steady-state analysis). Mechanical loads and boundary conditions can be changed gradually over the step by referring to an amplitude curve to accommodate possible geometric nonlinearities in the response. The steady-state coupled equations are strongly unsymmetric; therefore, the unsymmetric matrix solution and storage scheme is used automatically for steady-state analysis steps . If heat transfer is modeled using the coupled temperature–pore pressure elements, the steady-state solution neglects all transient effects in the heat transfer equation and provides only the steady-state temperature distribution. Input File Usage: Abaqus/CAE Usage: *SOILS Step module: Create Step: General: Soils: Basic: Pore fluid response: Steady state Incrementation You can specify a fixed time increment size in a coupled pore fluid diffusion/stress analysis, or Abaqus/Standard can select the time increment size automatically. Automatic incrementation is recommended because the time increments in a typical diffusion analysis can increase by several orders of magnitude during the simulation. If you do not activate automatic incrementation, fixed time increments will be used. Input File Usage: Use the following option to activate automatic incrementation in steady-state analysis: *SOILS, UTOL=any arbitrary nonzero value The solution does not depend on the value specified for UTOL; this value is simply a flag for automatic incrementation. Abaqus/CAE Usage: Step module: Create Step: General: Soils: Basic: Pore fluid response: Steady state; Incrementation: Type: Automatic Transient analysis In a transient coupled pore pressure/effective stress analysis the backward difference operator is used to integrate the continuity equation and the heat transfer equation (if heat transfer is modeled): this operator provides unconditional stability so that the only concern with respect to time integration is accuracy. You can provide the time increments, or they can be selected automatically. The coupled partially saturated flow equations are strongly unsymmetric, so the unsymmetric solver is used automatically if you request partially saturated analysis (by including absorption/exsorption behavior in the material definition). The unsymmetric solver is also activated automatically when gravity distributed loading is used during a soils consolidation analysis. For fully saturated flow analyses in which finite-sliding coupled pore pressure-displacement contact is modeled using contact pairs, certain contributions to the model’s stiffness matrix are unsymmetric. Using the unsymmetric solver can sometimes improve convergence in such cases since Abaqus does not automatically do so. For fully saturated flow analyses in which heat transfer is also modeled, the contributions to the model’s stiffness matrix arising from convective heat transfer due to pore fluid flow are unsymmetric. Using the unsymmetric solver can sometimes improve convergence in such cases since Abaqus does not automatically do so. Spurious oscillations due to small time increments The integration procedure used in Abaqus/Standard for consolidation analysis introduces a relationship between the minimum usable time increment and the element size, as shown below for fully saturated and partially saturated flows. If time increments smaller than these values are used, spurious oscillations may appear in the solution (except for partially saturated cases when linear elements or modified triangular elements are used; in these cases Abaqus/Standard uses a special integration scheme for the wetting liquid storage term to avoid the problem). These nonphysical oscillations may cause problems if pressure- sensitive plasticity is used to model the porous medium and may lead to convergence difficulties in partially saturated analyses. If the problem requires analysis with smaller time increments than the relationships given below allow, a finer mesh is required. Generally there is no upper limit on the time step except accuracy, since the integration procedure is unconditionally stable unless nonlinearities cause convergence problems. Fully saturated flow A simple guideline that can be used for the minimum usable time increment in the case of fully saturated flow is where is the time increment, is the specific weight of the wetting liquid, is the Young’s modulus of the soil, is the permeability of the soil , is the magnitude of the velocity of the pore fluid, is the velocity coefficient in Forchheimer’s flow law ( in the case of Darcy flow), is the bulk modulus of the solid grains , and is a typical element dimension. Partially saturated flow In partially saturated flow cases the corresponding guideline for the minimum time increment is where is the saturation; is the permeability-saturation relationship; is the rate of change of saturation with respect Section 26.6.4); is the initial porosity of the material; and the other parameters are as defined for the case of fully saturated flow. to pore pressure (see “Sorption,” Fixed incrementation If you choose fixed time incrementation, fixed time increments equal to the size of the user-specified initial time increment, , will be used. Fixed incrementation is not generally recommended because the time increments in a typical diffusion analysis can increase over several orders of magnitude during the simulation; automatic incrementation is usually a better choice. Input File Usage: *SOILS, CONSOLIDATION Abaqus/CAE Usage: Step module: Create Step: General: Soils: Basic: Pore fluid response: Transient consolidation; Incrementation: Type: Fixed, Increment size: Automatic incrementation If you choose automatic time incrementation, you must specify two (three if heat transfer is also modeled) tolerance parameters. The accuracy of the time integration of the flow continuity equations is governed by the maximum wetting liquid pore pressure change, , allowed in an increment. Abaqus/Standard restricts the time increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment in the analysis. If heat transfer is modeled, the accuracy of time integration is also governed by the maximum temperature change, , allowed in an increment. Abaqus/Standard restricts the time increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the analysis. The accuracy of the integration of the time-dependent (creep) material behavior is governed by the , as maximum strain rate change allowed at any point during an increment, described in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4. Input File Usage: If heat transfer is not modeled: Abaqus/CAE Usage: *SOILS, CONSOLIDATION, UTOL= , , CETOL=errtol If heat transfer is modeled: *SOILS, CONSOLIDATION, UTOL= CETOL=errtol , DELTMX= , Step module: Create Step: General: Soils: Basic: Pore fluid response: Transient consolidation; Incrementation: Type: Automatic, Max. pore pressure change per increment: Creep/swelling/viscoelastic strain error tolerance: errtol , Specifying the maximum temperature change per increment is not supported in Abaqus/CAE. Ending a transient analysis Transient soils analysis can be terminated by completing a specified time period, or it can be continued until steady-state conditions are reached. By default, the analysis will end when the given time period has been completed. Alternatively, you can specify that the analysis will end when steady state is reached or the time period ends, whichever comes first. When heat transfer is not modeled, steady state is defined by a maximum permitted rate of change of pore pressure with time: when all pore pressures are changing at less than the user-defined rate, the analysis terminates. However, with heat transfer included, the analysis terminates only when both the pore pressure and temperature are changing at less than the user-defined rates. Input File Usage: Use the following option to end the analysis when the time period is reached: Abaqus/CAE Usage: *SOILS, CONSOLIDATION, END=PERIOD (default) Use the following option to end the analysis based on the pore pressure and, if heat transfer is modeled, temperature change rate: *SOILS, CONSOLIDATION, END=SS Step module: Create Step: General: Soils: Basic: Pore fluid response: Transient consolidation; Incrementation: End step when pore pressure change rate is less than If heat transfer is modeled, directly specifying the temperature change rate to define steady state is not supported in Abaqus/CAE. Neglecting creep during a transient analysis You can specify that creep or viscoelastic response should be neglected during a consolidation analysis, even if creep or viscoelastic material properties have been defined. Input File Usage: Abaqus/CAE Usage: *SOILS, CONSOLIDATION, CREEP=NONE Step module: Create Step: General: Soils: Basic: Pore fluid response: Transient consolidation, toggle off Include creep/swelling/viscoelastic behavior Unstable problems Some types of analyses may develop local instabilities, such as surface wrinkling, material instability, or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with the aid of automatic incrementation. Abaqus/Standard offers the option to stabilize this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in “Automatic stabilization of unstable problems” in “Solving nonlinear problems,” Section 7.1.1. Optional modeling of coupled heat transfer When coupled temperature–pore pressure elements are used, heat transfer is modeled in these elements by default. However, you may optionally choose to switch off heat transfer within these elements during some steps in the analysis. This feature may be helpful in reducing computation time during certain phases in the analysis when heat transfer is not an important part of the overall physics of the problem. Input File Usage: Use the following option either during a transient or a steady-state procedure to suppress heat transfer modeling: *SOILS, CONSOLIDATION, HEAT=NO Abaqus/CAE Usage: Switching off the heat Abaqus/CAE. transfer part of the physics is not supported in Units In coupled problems where two or more different fields are being solved, you must be careful when choosing the units of the problem. If the choice of units is such that the numbers generated by the equations for the different fields differ by many orders of magnitude, the precision on some computers may be insufficient to resolve the numerical ill-conditioning of the coupled equations. Therefore, choose units that avoid badly conditioned matrices. For example, consider using units of Mpascal instead of pascal for the stress equilibrium equations to reduce the disparity between the magnitudes of the stress equilibrium equations and the pore flow continuity equations. Initial conditions Initial conditions can be applied as defined in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. Defining initial pore fluid pressures Initial values of pore fluid pressures, , can be defined at the nodes. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=PORE PRESSURE Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Pore pressure for the Types for Selected Step Defining initial void ratios Initial values of the void ratio, e, can be given at the nodes. The void ratio is defined as the ratio of the volume of voids to the volume of solid material . The evolution of void ratio is governed by the deformation of the different phases of the material, as discussed in detail in “Constitutive behavior in a porous medium,” Section 2.8.3 of the Abaqus Theory Manual. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=RATIO Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step Defining initial saturation Initial saturation values, s, can be given at the nodes. Saturation is defined as the ratio of wetting fluid volume to void volume . Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=SATURATION Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Saturation for the Types for Selected Step Defining initial stresses An initial (effective) stress field can be specified . Most geotechnical problems begin from a geostatic state, which is a steady-state equilibrium configuration of the undisturbed soil or rock body under geostatic loading and usually includes both horizontal and vertical components. It is important to establish these initial conditions correctly so that the problem begins from an equilibrium state. The geostatic procedure can be used to verify that the user-defined initial stresses are indeed in equilibrium with the given geostatic loads and boundary conditions . Input File Usage: Use one of the following options: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=STRESS *INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress or Geostatic stress for the Types for Selected Step Defining initial temperature Initial temperature values can be defined at the nodes. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=TEMPERATURE Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step Boundary conditions Boundary conditions can be applied to displacement degrees of freedom 1–6 and to pore pressure degree of freedom 8 (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). In addition, boundary conditions can also be applied to temperature degree of freedom 11 if heat transfer is modeled using coupled temperature–pore pressure elements. During the analysis prescribed boundary conditions can be varied by referring to an amplitude curve (“Amplitude curves,” Section 33.1.2). If no amplitude reference is given, the default variation of a boundary condition in a coupled pore fluid diffusion/stress analysis step is as defined in “Defining an analysis,” Section 6.1.2. If the pore pressure is prescribed with a boundary condition, fluid is assumed to enter and leave through the node as needed to maintain the prescribed pressure. Likewise, if the temperature is prescribed with a boundary condition, heat is assumed to enter and leave through the node as needed to maintain the prescribed temperature. Loads The following loading types can be prescribed in a coupled pore fluid diffusion/stress analysis: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” The magnitude and direction of gravitational loading are usually defined by using the gravity distributed load type. • Pore fluid flow is controlled as described in “Pore fluid flow,” Section 33.4.7. If heat transfer is modeled, the following types of thermal loading can also be prescribed (“Thermal loads,” Section 33.4.4). These loads are not supported in Abaqus/CAE during a coupled thermal pore pressure/stress analysis. • Concentrated heat fluxes. • Body fluxes and distributed surface fluxes. • Convective film conditions and radiation conditions; film properties can be made a function of temperature. Predefined fields The following predefined fields can be prescribed, as described in “Predefined fields,” Section 33.6.1: • For a coupled pore fluid diffusion/stress analysis that does not model heat transfer and uses regular pore pressure elements, temperature is not a degree of freedom and nodal temperatures can be specified. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any. • Predefined temperature fields are not allowed in coupled pore fluid diffusion/stress analysis that also models heat transfer. Boundary conditions should be used instead to specify temperatures, as described earlier. • The values of user-defined field variables can be specified; these values affect only field-variable- dependent material properties, if any. Material options Any of the mechanical constitutive models available in Abaqus/Standard can be used to model the porous material. In problems formulated in terms of total pore pressure, you must include the density of the dry material in the material definition . You can use a permeability material property to define the specific weight of the wetting liquid, ; the permeability, . , and its dependence on the void ratio, e, and saturation, ; and the flow velocity, You can define the compressibility of the solid grains and of the permeating fluid in both fully and partially saturated flow problems . If you do not specify the porous bulk moduli, the materials are assumed to be fully incompressible. For partially saturated flow you must define the porous medium’s absorption/exsorption behavior . Gel swelling (“Swelling gel,” Section 26.6.5) and volumetric moisture swelling of the solid skeleton (“Moisture swelling,” Section 26.6.6) can be included in partially saturated cases. These effects are usually associated with modeling of moisture migration in polymeric systems rather than with geotechnical systems. Thermal properties if heat transfer is modeled In problems that model heat transfer, the thermal conductivity for either the solid material or the permeating fluid, or more commonly for both phases, must be defined. Only isotropic conductivity can be specified for the pore fluid. The specific heat and density of the phases must also be defined for transient heat transfer problems. Latent heat for the phases can be defined if changes in internal energy due to phase changes are important. See “Thermal properties: overview,” Section 26.2.1, for details on defining thermal properties in Abaqus. Examples of problems that model fully coupled heat transfer along with pore fluid diffusion and mechanical deformation can be found in “Consolidation around a cylindrical heat source,” Section 1.15.7 of the Abaqus Benchmarks Manual, and “Permafrost thawing–pipeline interaction,” Section 10.1.6 of the Abaqus Example Problems Manual. The thermal properties can be defined separately for the solid material and the permeating fluid. Input File Usage: To define the conductivity, specific heat, density, and latent heat of the permeating fluid, use the following options: *CONDUCTIVITY, TYPE=ISO, PORE FLUID *SPECIFIC HEAT, PORE FLUID *LATENT HEAT, PORE FLUID *DENSITY, PORE FLUID To define the conductivity, specific heat, density, and latent heat of the solid material, use the following options: *EXPANSION, TYPE=ISO or ORTHO or ANISO *SPECIFIC HEAT *DENSITY *LATENT HEAT Defining the thermal properties and the density of the permeating fluid is not supported in Abaqus/CAE. To define the conductivity, specific heat, density, and latent heat of the solid material, use the following options: Property module: material editor: Thermal→Conductivity: Type: Isotropic Thermal→Specific Heat General→Density Thermal→Latent Heat 6.8.1–11 Thermal expansion Thermal expansion can be defined separately for the solid material and for the permeating fluid. In such a case you should repeat the expansion material property, with the necessary parameters, to define the different thermal expansion effects . Thermal expansion will be active only in a consolidation (transient) analysis. Input File Usage: Abaqus/CAE Usage: To define the thermal expansion of the permeating fluid: *EXPANSION, TYPE=ISO, PORE FLUID To define the thermal expansion of the solid material: *EXPANSION, TYPE=ISO or ORTHO or ANISO To define the thermal expansion of the permeating fluid: Property module: material editor: Other→Pore Fluid→Pore Fluid Expansion To define the thermal expansion of the solid material: Property module: material editor: Mechanical→Expansion Elements The analysis of flow through porous media in Abaqus/Standard is available for plane strain, axisymmetric, and three-dimensional problems. The modeling of coupled heat transfer effects is available only for axisymmetric and three-dimensional problems. Continuum pore pressure elements are provided for modeling fluid flow through a deforming porous medium in a coupled pore fluid diffusion/stress analysis. These elements have pore pressure degree of freedom 8 in addition to displacement degrees of freedom 1–3. Heat transfer through the porous medium can also be modeled using continuum coupled temperature–pore pressure elements. These elements have temperature degree of freedom 11 in addition to pore pressure degree of freedom 8 and displacement degrees of freedom 1–3. Stress/displacement elements can be used in parts of the model without pore fluid flow. See “Choosing the appropriate element for an analysis type,” Section 27.1.3, for more information. Output The element output available for a coupled pore fluid diffusion/stress analysis includes the usual mechanical quantities such as (effective) stress; strain; energies; and the values of state, field, and user-defined variables. In addition, the following quantities associated with pore fluid flow are available: . Void ratio, e. Pore pressure, Saturation, s. Gel volume ratio, Total fluid volume ratio, Magnitude and components of the pore fluid effective velocity vector, . . . 6.8.1–12 VOIDR POR SAT GELVR FLUVR FLVELM FLVELn Magnitude, , of the pore fluid effective velocity vector. Component n of the pore fluid effective velocity vector (n=1, 2, 3). If heat transfer is modeled, the following element output variables associated with heat transfer are also available: HFL HFLn HFLM TEMP Magnitude and components of the heat flux vector. Component n of the heat flux vector (n=1, 2, 3). Magnitude of the heat flux vector. Integration point temperatures. The nodal output available includes the usual mechanical quantities such as displacements, reaction forces, and coordinates. In addition, the following quantities associated with pore fluid flow are available: CFF POR RVF RVT Concentrated fluid flow at a node. Pore pressure at a node. Reaction fluid volume flux due to prescribed pressure. This flux is the rate at which fluid volume is entering or leaving the model through the node to maintain the prescribed pressure boundary condition. A positive value of RVF indicates that fluid is entering the model. Reaction total fluid volume (computed only in a transient analysis). This value is the time integrated value of RVF. If heat transfer is modeled, the following nodal output variables associated with heat transfer are also available: NT RFL RFLn CFL CFLn Nodal point temperatures. Reaction flux values due to prescribed temperature. Reaction flux value n at a node (n=11, 12, …). Concentrated flux values. Concentrated flux value n at a node (n=11, 12, …). All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Input file template *HEADING … *********************************** ** ** Material definition ** *********************************** , as a function of the void ratio, e *MATERIAL, NAME=soil Data lines to define mechanical properties of the solid material … *EXPANSION Data lines to define the thermal expansion coefficient of the solid grains *EXPANSION, TYPE=ISO, PORE FLUID Data lines to define the thermal expansion coefficient of the permeating fluid *PERMEABILITY, SPECIFIC= Data lines to define permeability, *PERMEABILITY, TYPE=SATURATION Data lines to define the dependence of permeability on saturation, *PERMEABILITY, TYPE=VELOCITY Data lines to define the velocity coefficient, *POROUS BULK MODULI Data line to define the bulk moduli of the solid grains and the permeating fluid *SORPTION, TYPE=ABSORPTION Data lines to define absorption behavior *SORPTION, TYPE=EXSORPTION Data lines to define exsorption behavior *SORPTION, TYPE=SCANNING Data lines to define scanning behavior (between absorption and exsorption) *GEL Data line to define gel behavior in partially saturated flow *MOISTURE SWELLING Data lines to define moisture swelling strain as a function of saturation in partially saturated flow *CONDUCTIVITY Data lines to define thermal conductivity of the solid grains if heat transfer is modeled *CONDUCTIVITY,TYPE=ISO, PORE FLUID Data lines to define thermal conductivity of the permeating fluid if heat transfer is modeled *SPECIFIC HEAT Data lines to define specific heat of the solid grains if transient heat transfer is modeled *SPECIFIC HEAT,PORE FLUID Data lines to define specific heat of the permeating fluid if transient heat transfer is modeled *DENSITY Data lines to define density of the solid grains if transient heat transfer is modeled *DENSITY,PORE FLUID Data lines to define density of the permeating fluid if transient heat transfer is modeled *LATENT HEAT Data lines to define latent heat of the solid grains if phase change due to temperature change is modeled *LATENT HEAT,PORE FLUID Data lines to define latent heat of the permeating fluid if phase change due to temperature change is modeled … *********************************** ** ** Boundary conditions and initial conditions ** *********************************** *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC Data lines to specify initial stresses *INITIAL CONDITIONS, TYPE=PORE PRESSURE Data lines to define initial values of pore fluid pressures *INITIAL CONDITIONS, TYPE=RATIO Data lines to define initial values of the void ratio *INITIAL CONDITIONS, TYPE=SATURATION Data lines to define initial saturation *INITIAL CONDITIONS, TYPE=TEMPERATURE Data lines to define initial saturation *AMPLITUDE, NAME=name Data lines to define amplitude variations *********************************** ** ** Step 1: Optional step to ensure an equilibrium ** geostatic stress field ** *********************************** *STEP *GEOSTATIC *CLOAD and/or *DLOAD and/or *TEMPERATURE and/or *FIELD Data lines to specify mechanical loading *FLOW and/or *SFLOW and/or *DFLOW and/or *DSFLOW Data lines to specify pore fluid flow *CFLUX and/or *DFLUX Data lines to define concentrated and/or distributed heat fluxes if heat transfer is modeled *BOUNDARY Data lines to specify displacements or pore pressures *END STEP *********************************** ** ** Step 2: Coupled pore diffusion/stress analysis step ** *********************************** *STEP (,NLGEOM) ** Use NLGEOM to include geometric nonlinearities *SOILS Data line to define incrementation *CLOAD and/or *DLOAD and/or *DSLOAD Data lines to specify mechanical loading *FLOW and/or *SFLOW and/or *DFLOW and/or *DSFLOW Data lines to specify pore fluid flow *CFLUX and/or *DFLUX Data lines to define concentrated and/or distributed heat fluxes if heat transfer is modeled *FILM Data lines referring to film property table if heat transfer is modeled *BOUNDARY Data lines to specify displacements, pore pressures, or temperatures *END STEP 6.8.2 GEOSTATIC STRESS STATE Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 • *GEOSTATIC • “Configuring a geostatic stress field procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A geostatic stress field procedure: • is used to verify that the initial geostatic stress field is in equilibrium with applied loads and boundary conditions and to iterate, if necessary, to obtain equilibrium; • accounts for pore pressure degrees of freedom when pore pressure elements are used, and accounts for temperature degrees of freedom when coupled temperature–pore pressure elements are used; • is usually the first step of a geotechnical analysis, followed by a coupled pore fluid diffusion/stress (with or without heat transfer) or static analysis procedure; and • can be linear or nonlinear. Establishing geostatic equilibrium The geostatic procedure is normally used as the first step of a geotechnical analysis; in such cases gravity loads are applied during this step. Ideally, the loads and initial stresses should exactly equilibrate and produce zero deformations. However, in complex problems it may be difficult to specify initial stresses and loads that equilibrate exactly. Abaqus/Standard provides two procedures for establishing the initial equilibrium. The first procedure is applicable to problems for which the initial stress state is known at least approximately. The second, enhanced, procedure is also applicable for cases in which the initial stresses are not known; it is supported for only a limited number of elements and materials. Establishing equilibrium when the initial stress state is approximately known The geostatic procedure requires that the initial stresses are close to the equilibrium state; otherwise, the displacements corresponding to the equilibrium state might be large. Abaqus/Standard checks for equilibrium during the geostatic procedure and iterates, if needed, to obtain a stress state that equilibrates the prescribed boundary conditions and loads. This stress state, which is a modification of the stress field defined by the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1), is then used as the initial stress field in a subsequent static or coupled pore fluid diffusion/stress (with or without heat transfer) analysis. If the stresses given as initial conditions are far from equilibrium under the geostatic loading and there is some nonlinearity in the problem definition, this iteration process may fail. Therefore, you should ensure that the initial stresses are reasonably close to equilibrium. If the deformations produced during the geostatic step are significant compared to the deformations caused by subsequent loading, the definition of the initial state should be reexamined. If heat transfer is modeled during the geostatic step through the use of coupled temperature–pore pressure elements, the initial temperature field and thermal loads, if specified, must be such that the system is relatively close to a state of thermal equilibrium. Steady-state heat transfer is assumed during a geostatic step. Input File Usage: Abaqus/CAE Usage: *GEOSTATIC Step module: Create Step: General: Geostatic Establishing equilibrium when the initial stress state is unknown To obtain equilibrium in cases when the initial stress state is unknown or is known only approximately, you can invoke an enhanced procedure. Abaqus automatically computes the equilibrium corresponding to the initial loads and the initial configuration, allowing only small displacements within user-specified tolerances. (The default tolerance is .) The procedure is available with a limited number of elements and materials and is intended to be used in analyses in which the material response is primarily elastic; that is, inelastic deformations are small. The procedure is supported for both geometrically linear and geometrically nonlinear analyses. However, in general, the performance in the geometrically linear case will be better. Therefore, it might be advantageous to obtain the initial equilibrium in a geometrically linear step, even though a geometrically nonlinear analysis is performed in subsequent steps. Input File Usage: Use the following option to invoke the enhanced procedure: Abaqus/CAE Usage: *GEOSTATIC, UTOL=displacement tolerance Step module: Create Step: General: Geostatic: Incrementation tabbed page: Automatic: Max. displacement change Limitations The following limitations apply to the enhanced procedure: • It is supported only for a limited number of elements and materials . When the procedure is used with nonsupported elements or material models, Abaqus issues a warning message. In this case it is the user’s responsibility to ensure that the displacement tolerances are larger than the displacements in the analysis; otherwise, convergence problems may occur. • It can be used in a restart analysis only if it had been used in the previous analysis. Optional modeling of coupled heat transfer When coupled temperature–pore pressure elements are used, heat transfer is modeled in these elements by default. However, you may optionally choose to switch off heat transfer within these elements during a geostatic step. This feature may be helpful in reducing computation time if temperature and associated heat flow effects are not important. Input File Usage: Use the following option to suppress heat transfer modeling: Abaqus/CAE Usage: *GEOSTATIC, HEAT=NO Switching off the heat Abaqus/CAE. transfer part of the physics is not supported in Vertical equilibrium in a porous medium Most geotechnical problems begin from a geostatic state, which is a steady-state equilibrium configuration of the undisturbed soil or rock body under geostatic loading. The equilibrium state usually includes both horizontal and vertical stress components. It is important to establish these initial conditions correctly so that the problem begins from an equilibrium state. Since such problems often involve fully or partially saturated flow, the initial void ratio of the porous medium, , the initial pore pressure, , and the initial effective stress must all be defined. If the magnitude and direction of the gravitational loading are defined by using the gravity distributed load type, a total, rather than excess, pore pressure solution is used . This discussion is based on the total pore pressure formulation. The z-axis points vertically in this discussion, and atmospheric pressure is neglected. We assume that the pore fluid is in hydrostatic equilibrium during the geostatic procedure so that where is the user-defined specific weight of the pore fluid . (The pore fluid is not in hydrostatic equilibrium if there is significant steady-state flow of pore fluid through the porous medium: in that case a steady-state coupled pore fluid diffusion/stress analysis must be performed to establish the initial conditions for any subsequent transient calculations—see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1.) If we also take to be independent of z (which is usually the case, since the fluid is almost incompressible), this equation can be integrated to define where fluid is only partially saturated. is the height of the phreatic surface, at which and above which and the pore We usually assume that there are no significant shear stresses , . Then, equilibrium in the vertical direction is is the dry density of the porous solid material (the dry mass per unit volume), g is the where gravitational acceleration, . Since porosity is the ratio of pore volume to total volume and the void ratio is the ratio of pore volume to solids volume, is the initial porosity of the material, and s is the saturation, is defined from the initial void ratio by Abaqus/Standard requires that the initial value of the effective stress, , be given as an initial condition (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Effective stress is defined from the total stress, , by is a unit matrix. Combining this definition with the equilibrium statement in the z-direction and where hydrostatic equilibrium in the pore fluid gives again using the assumption that the dry soil from the partially saturated soil. The soil is assumed to be dry ( assumed to be partially saturated for and fully saturated for is independent of z. In many cases s is constant. For example, in fully saturated flow phreatic surface. If we further assume that the initial porosity, medium, , are also constant, the above equation is readily integrated to give is the position of the surface that separates , and it is ) for . everywhere below the , and the dry density of the porous where is the position of the surface of the porous medium, . In more complicated cases where s, , and/or vary with height, the equation must be integrated in the vertical direction to define the initial values of . Horizontal equilibrium in a porous medium In many geotechnical applications there is also horizontal stress, typically caused by tectonic action. If the pore fluid is under hydrostatic equilibrium and , equilibrium in the horizontal directions requires that the horizontal components of effective stress do not vary with horizontal position: only, where is any horizontal component of effective stress. Initial conditions The initial effective geostatic stress field, , is given by defining initial stress conditions. Unless the enhanced procedure is used, the initial state of stress must be close to being in equilibrium with the applied loads and boundary conditions. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. You can specify that the initial stresses vary only with elevation, as described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. In this case the horizontal stress is typically assumed to be a fraction of the vertical stress: those fractions are defined in the x- and y-directions. In problems involving partially or fully saturated porous media, initial pore fluid pressures, , void , and saturation values, s, must be given . In partially saturated cases the initial pore pressure and saturation values must lie on or between the absorption and exsorption curves . A partially saturated problem is illustrated in “Wicking in a partially saturated porous medium,” Section 1.9.3 of the Abaqus Benchmarks Manual. You may also specify initial temperatures in the model if heat transfer is modeled during the geostatic procedure. Boundary conditions Boundary conditions can be applied to displacement degrees of freedom 1–6 and to pore pressure degree of freedom 8 (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). If coupled temperature–pore pressure elements are used, boundary conditions on temperature degree of freedom 11 can also be applied to nodes belonging to these elements. If the enhanced procedure is used and nonzero boundary conditions are applied, it is the user’s responsibility to ensure that the displacements corresponding to the tolerances specified are larger than the displacements in the analysis; otherwise, the displacements at the nonzero boundary nodes will be reset to zero with the tolerances specified. The boundary conditions should be in equilibrium with the initial stresses and applied loads. If the horizontal stress is nonzero, horizontal equilibrium must be maintained by fixing the boundary conditions on any nonhorizontal edges of the finite element model in the horizontal direction or by using infinite elements (“Infinite elements,” Section 28.3.1). If heat transfer is modeled, the temperature boundary conditions should be in equilibrium with the initial temperature field and applied thermal loads. Loads The following loading types can be prescribed in a geostatic stress field procedure: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can also be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” The magnitude and direction of gravitational loading are defined by using the gravity or body force distributed load types. • Pore fluid flow is controlled as described in “Pore fluid flow,” Section 33.4.7. If heat transfer is modeled, the following types of thermal loading can also be prescribed (“Thermal loads,” Section 33.4.4). These loads are not supported in Abaqus/CAE during a geostatic analysis. • Concentrated heat fluxes. • Body fluxes and distributed surface fluxes. • Convective film conditions and radiation conditions; film properties can be made a function of temperature. Predefined fields The following predefined fields can be specified in a geostatic stress field procedure, as described in “Predefined fields,” Section 33.6.1: • For a geostatic analysis that does not model heat transfer and uses regular pore pressure elements, temperature is not a degree of freedom and nodal temperatures can be specified. • Predefined temperature fields are not allowed in a geostatic analysis that also models heat transfer. Boundary conditions should be used instead to specify temperatures, as described earlier. • The values of user-defined field variables can be specified; these values affect only field-variable- dependent material properties, if any. Material options Any of the mechanical constitutive models available in Abaqus/Standard can be used to model the porous solid material. However, the enhanced procedure can be used only with the elastic, porous elastic, extended Cam-clay plasticity, and Mohr-Coulomb plasticity models. Use of a nonsupported material model with this procedure may lead to poor convergence or no convergence if displacements are larger than the displacements corresponding to the tolerances specified. Abaqus will issue a warning message if the procedure is used with a nonsupported material model. If a porous medium will be analyzed subsequent to the geostatic procedure, pore fluid flow quantities such as permeability and sorption should be defined . If heat transfer is modeled, thermal properties such as conductivity, specific heat, and density should be defined for both the solid and the pore fluid phases (see “Thermal properties if heat transfer is modeled” in “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1, for details on how to specify separate thermal properties for the two phases). Elements Any of the stress/displacement elements in Abaqus/Standard can be used in a geostatic procedure. Continuum pore pressure elements can also be used for modeling fluid in a deforming porous medium. These elements have pore pressure degree of freedom 8 in addition to displacement degrees of freedom 1–3. However, the enhanced procedure can be used only with continuum and cohesive elements with pore pressure degrees of freedom and the corresponding stress/displacements elements. Use of nonsupported elements with this procedure may lead to poor convergence or no convergence if displacements are larger than the displacements corresponding to the tolerances specified. Abaqus will issue a warning message if the procedure is used with a nonsupported element. Continuum elements that couple temperature, pore pressure, and displacement can be used if heat transfer needs to be modeled. These elements have temperature degree of freedom 11 in addition to pore pressure degree of freedom 8 and displacement degrees of freedom 1–3. See “Choosing the appropriate element for an analysis type,” Section 27.1.3, for more information. Output The element output available for a coupled pore fluid diffusion/stress analysis includes the usual mechanical quantities such as (effective) stress; strain; energies; and the values of state, field, and user-defined variables. In addition, the following quantities associated with pore fluid flow are available: VOIDR POR SAT GELVR FLUVR FLVEL FLVELM FLVELn . Void ratio, e. Pore pressure, Saturation, s. Gel volume ratio, Total fluid volume ratio, Magnitude and components of the pore fluid effective velocity vector, , of the pore fluid effective velocity vector. Magnitude, Component n of the pore fluid effective velocity vector (n=1, 2, 3). . . . If heat transfer is modeled, the following element output variables associated with heat transfer are also available: HFL HFLn HFLM TEMP Magnitude and components of the heat flux vector. Component n of the heat flux vector (n=1, 2, 3). Magnitude of the heat flux vector. Integration point temperatures. The nodal output available includes the usual mechanical quantities such as displacements, reaction forces, and coordinates. In addition, the following quantities associated with pore fluid flow are available: POR RVF Pore pressure at a node. Reaction fluid volume flux due to prescribed pressure. This flux is the rate at which fluid volume is entering or leaving the model through the node to maintain the prescribed pressure boundary condition. A positive value of RVF indicates fluid is entering the model. If heat transfer is modeled, the following nodal output variables associated with heat transfer are also available: NT RFL RFLn CFL CFLn Nodal point temperatures. Reaction flux values due to prescribed temperature. Reaction flux value n at a node (n=11, 12, …). Concentrated flux values. Concentrated flux value n at a node (n=11, 12, …). All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Input file template , as a function of the void ratio, e *HEADING … *MATERIAL, NAME=mat1 Data lines to define mechanical properties of the solid material … *DENSITY Data lines to define the density of the dry material *PERMEABILITY, SPECIFIC= Data lines to define permeability, *CONDUCTIVITY Data lines to define thermal conductivity of the solid grains if heat transfer is modeled *CONDUCTIVITY,TYPE=ISO, PORE FLUID Data lines to define thermal conductivity of the permeating fluid if heat transfer is modeled *SPECIFIC HEAT Data lines to define specific heat of the solid grains if transient heat transfer is modeled in a subsequent step *SPECIFIC HEAT,PORE FLUID Data lines to define specific heat of the permeating fluid if transient heat transfer is modeled in a subsequent step *DENSITY Data lines to define density of the solid grains if transient heat transfer is modeled in a subsequent step *DENSITY,PORE FLUID Data lines to define density of the permeating fluid if transient heat transfer is modeled in a subsequent step *LATENT HEAT Data lines to define latent heat of the solid grains if phase change due to temperature change is modeled *LATENT HEAT,PORE FLUID Data lines to define latent heat of the permeating fluid if phase change due to temperature change is modeled … *INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC Data lines to define the initial stress state *INITIAL CONDITIONS, TYPE=PORE PRESSURE Data lines to define initial values of pore fluid pressures *INITIAL CONDITIONS, TYPE=RATIO Data lines to define initial values of the void ratio *INITIAL CONDITIONS, TYPE=SATURATION Data lines to define initial saturation *INITIAL CONDITIONS, TYPE=TEMPERATURE Data lines to define initial temperature *BOUNDARY Data lines to define zero-valued boundary conditions ** *STEP *GEOSTATIC *CLOAD and/or *DLOAD and/or *DSLOAD Data lines to specify mechanical loading *FLOW and/or *SFLOW and/or *DFLOW and/or *DSFLOW Data lines to specify pore fluid flow *CFLUX and/or *DFLUX Data lines to define concentrated and/or distributed heat fluxes if heat transfer is modeled *BOUNDARY Data lines to specify displacements or pore pressures *END STEP 6.9 Mass diffusion analysis • “Mass diffusion analysis,” Section 6.9.1 6.9.1 MASS DIFFUSION ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • *MASS DIFFUSION • “Configuring a mass diffusion procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating and modifying prescribed conditions,” Section 16.4 of the Abaqus/CAE User’s Manual • “Defining a concentrated concentration flux,” Section 16.9.33 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a body concentration flux,” Section 16.9.35 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a surface concentration flux,” Section 16.9.34 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A mass diffusion analysis: • models the transient or steady-state diffusion of one material through another, such as the diffusion of hydrogen through a metal; • requires the use of mass diffusion elements; and • can be used to model temperature and/or pressure-driven mass diffusion. Governing equations The governing equations for mass diffusion are an extension of Fick’s equations: they allow for nonuniform solubility of the diffusing substance in the base material and for mass diffusion driven by gradients of temperature and pressure. The basic solution variable (used as the degree of freedom at the nodes of the mesh) is the “normalized concentration” (often also referred to as the “activity” of the diffusing material), , where c is the mass concentration of the diffusing material and s is its solubility in the base material. Therefore, when the mesh includes dissimilar materials that share nodes, the normalized concentration is continuous across the interface between the different materials. For example, a diatomic gas that dissociates during diffusion can be described using Sievert’s law: , where p is the partial pressure of the diffusing gas. Combining Sievert’s law with the definition of normalized concentration given earlier, . Equilibrium requires the partial pressure to be continuous across an interface, so normalized concentration will be continuous as well. If an expression other than Sievert’s law defines the relationship between concentration and partial pressure for a diffusing material, solubility should be defined accordingly. The diffusion problem is defined from the requirement of mass conservation for the diffusing phase: where V is any volume whose surface is S, of the diffusing phase, and is the concentration flux leaving S. is the outward normal to S, is the flux of concentration Diffusion is assumed to be driven by the gradient of a general chemical potential, which gives the behavior is the solubility; where is the diffusivity; providing diffusion because of temperature gradient; zero on the temperature scale being used; driven by the gradient of the equivalent pressure stress, predefined field variables. , or is the temperature; is the “Soret effect” factor, is the value of absolute is the pressure stress factor, providing diffusion are any is stress; and ; Whenever D, depends on concentration, the problem becomes nonlinear and the system of equations becomes nonsymmetric. In practical cases the dependence on concentration is quite strong, so the nonsymmetric matrix storage and solution scheme is invoked automatically when a mass diffusion analysis is performed . Fick’s law Mass diffusion behavior is often described by Fick’s law (Crank, 1956): Fick’s law is offered in Abaqus/Standard as a special case of the general chemical potential relation. To establish the relationship between Fick’s law and the general chemical potential, we write Fick’s law as In most practical cases , and we can write The two terms in this equation describe the normalized concentration and temperature-driven diffusion, respectively. The normalized concentration-driven diffusion term is identical to that given in relation if MASS DIFFUSION This conversion is done automatically in Abaqus/Standard when you request Fick’s law . An extended form of Fick’s law can also be chosen by specifying a nonzero value for : In this case Abaqus/Standard will still define automatically as discussed earlier. Units The units of concentration are commonly given as parts per million (P). On the basis of the applicability of Sievert’s law to the mass diffusion, the units of solubility are , where F is force and L is length. The units of the Soret effect factor are . The units of the pressure stress factor are , ; and the concentration volumetric , and the units of equivalent pressure stress are , then has units of . The diffusivity, , has units of where T is time. The concentration flux, flux, , has units of . Steady-state analysis Steady-state mass diffusion analysis provides the steady-state solution directly: the rate of change of concentration with respect to time is omitted from the governing diffusion equation in steady-state analysis. In nonlinear cases iteration may be necessary to achieve a converged solution. Since the rate term is removed from the governing equations, the steady-state problem has no intrinsic physically meaningful time scale; nevertheless, you may assign a “time” scale to the analysis step. This time scale is often convenient for output identification and for specifying prescribed normalized concentrations and fluxes with varying magnitudes. Thus, when steady-state analysis is chosen, you specify a “time” increment and a “time” period for the step; Abaqus/Standard then increments through the step accordingly. If a steady-state analysis step is to be followed by a transient analysis step and total time is used in amplitude definitions (“Amplitude curves,” Section 33.1.2), the time period should be defined to be negligibly small in the steady-state step. For more details on time scales and time stepping, see “Defining an analysis,” Section 6.1.2. *MASS DIFFUSION, STEADY STATE Step module: Create Step: General: Mass diffusion: Basic: Response: Steady state Abaqus/CAE Usage: Input File Usage: Transient analysis Time integration in transient diffusion analysis is done with the backward Euler method (also referred to as the modified Crank-Nicholson operator). This method is unconditionally stable for linear problems. Automatic or fixed time incrementation can be used for transient analysis. The automatic time incrementation scheme is generally preferred because the response is usually simple diffusion: the rate of change of normalized concentration varies widely during the step and requires different time increments to maintain accuracy in the time integration. Spurious oscillations due to small time increments In transient mass diffusion analysis with second-order elements there is a relationship between the minimum usable time step and the element size. A simple guideline is is the time increment, D is the diffusivity, and where is a typical element dimension (such as the length of a side of an element). If time increments smaller than this value are used, spurious oscillations can appear in the solution. Abaqus/Standard provides no check on the initial time increment defined for a mass diffusion analysis; you must ensure that the given value does not violate the above criterion. In transient analysis using first-order elements the solubility terms are lumped, which eliminates such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time increments are required, a finer mesh should be used in regions where the normalized concentration changes occur. Generally there is no upper limit on the time increment because the integration procedure is unconditionally stable unless nonlinearities cause numerical problems. Automatic incrementation Input File Usage: The automatic time incrementation scheme for mass diffusion problems is based on the user-specified maximum normalized concentration change allowed at any node during an increment, *MASS DIFFUSION, DCMAX= Step module: Create Step: General: Mass diffusion: Basic: Response: Transient; Incrementation: Type: Automatic: Max. allowable normalized concentration change: Abaqus/CAE Usage: . Fixed time incrementation If you choose fixed time incrementation, fixed time increments equal to the size of the user-specified initial time increment, , will be used. Input File Usage: *MASS DIFFUSION Abaqus/CAE Usage: Step module: Create Step: General: Mass diffusion: Basic: Response: Transient; Incrementation: Type: Fixed, Increment size: Ending a transient analysis Transient mass diffusion analysis can be terminated by completing a specified time period, or it can be continued until steady-state conditions are reached. By default, the analysis will end when the given time period has been completed. Alternatively, you can specify that the analysis will end when steady state is reached or the time period ends, whichever comes first. Steady state is defined as the point in time when all normalized concentrations change at less than a user-defined rate. Input File Usage: Abaqus/CAE Usage: Initial conditions Use the following option to end the analysis when the time period is reached: *MASS DIFFUSION, END=PERIOD (default) Use the following option to end the analysis based on the concentration change rate: *MASS DIFFUSION, END=SS Step module: Create Step: General: Mass diffusion: Basic: Response: Transient; Incrementation: Type: Automatic: End step when normalized concentration change rate is less than An initial normalized concentration of the diffusing material at specific nodes that belong to mass diffusion elements can be defined (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). For an analysis in which mass diffusion is driven by gradients of temperature and/or pressure (“Diffusivity,” Section 26.4.1), the initial temperature and pressure stress fields in a model can also be defined. Input File Usage: Use the following options: *INITIAL CONDITIONS, TYPE=CONCENTRATION for initial concentrations *INITIAL CONDITIONS, TYPE=TEMPERATURE for initial temperatures *INITIAL CONDITIONS, TYPE=PRESSURE STRESS for initial equivalent pressure stress Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step Initial concentration and equivalent pressure stress are not supported in Abaqus/CAE. Boundary conditions Boundary conditions can be applied to nodal degree of freedom 11 in any mass diffusion element to prescribe values of normalized concentration (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). Such values can be specified as functions of time. Any boundary condition changes to be applied during a mass diffusion step should be given in the respective step using appropriate amplitude definitions to specify their “time” variations (“Amplitude curves,” Section 33.1.2). If boundary conditions are specified for the step without amplitude references, they are assumed to change either linearly with “time” during the step or instantly at the start of the step, according to the user-specified or default time variation associated with the step . Loads Concentration fluxes are the only loads that can be applied in a mass diffusion analysis step. Input File Usage: Use the following option to specify a concentrated concentration flux at a node: *CFLUX node number or node set name, degree of freedom, concentrated flux magnitude Use the following option to specify a distributed concentration flux acting on entire elements (body flux) or just on element faces (surface flux): *DFLUX element number or element set name, BF or Sn, distributed flux magnitude Abaqus/CAE Usage: Use the following input to define a concentrated concentration flux at a node: Load module: Create Load: choose Mass diffusion for the Category and Concentrated concentration flux for the Types for Selected Step: select region: Magnitude: concentrated flux magnitude Use the following input to define a distributed concentration flux acting on entire elements (body flux) or just on element faces (surface flux): Load module: Create Load: choose Mass diffusion for the Category and Body concentration flux or Surface concentration flux for the Types for Selected Step: Distribution: Uniform or select an analytical field, Magnitude: distributed flux magnitude Modifying or removing concentration fluxes Concentrated or distributed concentration fluxes can be added, modified, or removed as described in “Applying loads: overview,” Section 33.4.1. Specifying time-dependent concentration fluxes The magnitude of a concentrated or a distributed concentration flux can be controlled by referring to an amplitude curve . If different magnitude variations are needed for different fluxes, the flux definitions can be repeated, with each referring to its own amplitude curve. Defining nonuniform distributed concentration fluxes in a user subroutine To define nonuniform distributed concentration fluxes, the variation of the flux magnitude throughout a step can be defined in user subroutine DFLUX. If a reference flux magnitude is specified directly, it will be ignored. As a result, any amplitude reference in the flux definition is also ignored. Input File Usage: Use the following option to define a nonuniform distributed concentration body flux: *DFLUX element number or element set, BFNU Use the following option to define a nonuniform distributed concentration surface flux: *DFLUX element number or element set, SnNU Abaqus/CAE Usage: Use the following input to define a nonuniform distributed concentration body flux: Load module: Create Load: choose Mass diffusion for the Category and Body concentration flux for the Types for Selected Step: select region: Distribution: User-defined Use the following input to define a nonuniform distributed concentration surface flux: Load module: Create Load: choose Mass diffusion for the Category and Surface concentration flux for the Types for Selected Step: select region: Distribution: User-defined Predefined fields Predefined temperatures, equivalent pressure stresses, and field variables can be specified in a mass diffusion analysis. Prescribing temperatures Temperatures are applied to nodes in temperature-driven mass diffusion analyses by defining a temperature field; absolute zero on the temperature scale used is defined as described in “Specifying the value of absolute zero” in “Thermal loads,” Section 33.4.4. Alternatively, the temperature field can be obtained from a previous heat transfer analysis. Time-dependent temperature variations are possible with either approach. A simple interface is provided that uses the Abaqus/Standard results file from the heat transfer analysis to define the temperature field at different times in the mass diffusion analysis. Abaqus/Standard assumes that the nodes in the mass diffusion analysis have the same numbers as the nodes in the previous heat transfer analysis. Values in the results file are ignored at nodes that exist in the heat transfer analysis but not in the mass diffusion analysis, and the temperatures at nodes that did not exist in the heat transfer analysis will not be set by reading the results file. For specific details on prescribing temperatures, see “Predefined temperature” in “Predefined fields,” Section 33.6.1. Prescribing equivalent pressure stresses Equivalent pressure stress values can be given at nodes by specifying them directly as a predefined field in the mass diffusion analysis or indirectly by reading the equivalent pressure stresses from the results file of a previous stress/displacement, fully coupled temperature-displacement, or fully coupled thermal- electrical-structural analysis. Regardless of the manner in which they are specified, pressures should be entered according to the Abaqus convention that equivalent pressure stresses are positive when they are compressive. A simple interface is provided that uses the Abaqus/Standard results file from a mechanical analysis to define the equivalent pressure stresses at different times in the mass diffusion analysis. Abaqus/Standard assumes that the nodes in the mass diffusion analysis have the same numbers as the nodes in the previous mechanical analysis. Values in the results file are ignored at nodes that exist in the mechanical analysis but not in the mass diffusion analysis, and the pressures at nodes that did not exist in the mechanical analysis will not be set by reading the results file. For specific details on prescribing equivalent pressure stresses, see “Predefined pressure stress” in “Predefined fields,” Section 33.6.1. Specifying predefined field variables You can specify values of predefined field variables during a mass diffusion analysis. These values affect only field-variable-dependent material properties, if any. See “Predefined field variables” in “Predefined fields,” Section 33.6.1. Material options Both diffusivity (“Diffusivity,” Section 26.4.1) and solubility (“Solubility,” Section 26.4.2) must be defined in a mass diffusion analysis. Optionally, a Soret effect factor and a pressure stress factor can be defined to introduce mass diffusion caused by temperature and pressure gradients, respectively. The use of Fick’s law also introduces temperature-driven mass diffusion since a Soret effect factor is calculated automatically. Elements Mass diffusion analysis can be performed using only the two-dimensional, three-dimensional, and axisymmetric solid elements that are included in the Abaqus/Standard heat transfer/mass diffusion element library. Output In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables have special meaning in mass diffusion analyses: Element integration point variables: CONC ISOL MFL MFLM MFLn TEMP Mass concentration. Amount of solute at the integration point, calculated as the product of the mass concentration and the integration point volume. Magnitude and components of the concentration flux vector (excluding the terms due to pressure and temperature gradients). Magnitude of the concentration flux vector. Component n of the concentration flux vector (n = 1, 2, 3). Magnitude of the applied temperature field. Whole element variables: ESOL NFLUX FLUXS Amount of solute in the element, calculated as the sum of ISOL over all the element integration points. Fluxes at the nodes of the element caused by mass diffusion in the element. Distributed mass flux applied to an element. Whole or partial model variables: SOL Amount of solute in the model or specified element set, calculated as the sum of ESOL over all the elements in the model or set. Nodal variables: CFL CFLn NNC NNCn RFL RFLn Input file template All concentrated flux values. Concentrated flux value n at a node (n = 11). All normalized concentration values at a node. Normalized concentration degree of freedom n at a node (n = 11). All reaction flux values (conjugate to normalized concentration). Reaction flux value n at a node (n = 11) (conjugate to normalized concentration). The following template is representative of a three-step mass diffusion analysis. The first step establishes an initial steady-state concentration distribution of a diffusing material. In the second step equivalent pressure stresses are read from a fully coupled temperature-displacement analysis and the transient mass diffusion response is obtained for the case of mechanical loading of the body. In the final step a temperature field is read from a fully coupled temperature-displacement analysis and the transient mass diffusion response is calculated for the case of heating and cooling the body in which diffusion occurs. An example problem that follows this template is “Thermo-mechanical diffusion of hydrogen in a bending beam,” Section 1.10.1 of the Abaqus Benchmarks Manual. *HEADING … *MATERIAL,NAME=mat1 *SOLUBILITY Data lines to define solubility *DIFFUSIVITY Data lines to define diffusivity *KAPPA,TYPE=TEMP Data lines to define diffusion driven by temperature gradients *KAPPA,TYPE=PRESS Data lines to define diffusion driven by gradients of equivalent pressure stress *INITIAL CONDITIONS,TYPE=TEMPERATURE Data lines to define an initial temperature field *INITIAL CONDITIONS,TYPE=CONCENTRATION Data lines to define initial nodal values of normalized concentration *INITIAL CONDITIONS,TYPE=PRESSURE STRESS Data lines to define initial nodal values of equivalent pressure stress *AMPLITUDE,NAME=name Data lines to define amplitude variations ** *STEP Step 1 - steady-state solution *MASS DIFFUSION,STEADY STATE Data line to define incrementation *BOUNDARY Data lines to prescribe nodal values of normalized concentration *EL FILE Data lines to define element integration output to the results file *NODE FILE Data lines to define nodal output to the results file *END STEP ** *STEP Step 2 - transient analysis driven by pressure stress gradients *MASS DIFFUSION,DCMAX=dcmax,END=SS Data line to define incrementation *BOUNDARY Data lines to prescribe nodal values of normalized concentration *PRESSURE STRESS,FILE=name *EL FILE Data lines to define element integration output to the results file *NODE FILE Data lines to define nodal output to the results file *END STEP ** *STEP Step 3 - transient analysis driven by temperature gradients *MASS DIFFUSION,DCMAX=dcmax,END=SS Data line to define incrementation *BOUNDARY Data lines to prescribe nodal values of normalized concentration *TEMPERATURE,FILE=name *EL FILE Data lines to define element integration output to the results file *NODE FILE Data lines to define nodal output to the results file *END STEP Additional reference • Crank, J., The Mathematics of Diffusion, Clarendon Press, Oxford, 1956. 6.10 Acoustic and shock analysis • “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1 6.10.1 ACOUSTIC, SHOCK, AND COUPLED ACOUSTIC-STRUCTURAL ANALYSIS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Acoustic medium,” Section 26.3.1 • “Acoustic and shock loads,” Section 33.4.6 • “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1 • “ALE adaptive meshing: overview,” Section 12.2.1 • “Steady-state transport analysis,” Section 6.4.1 • *ACOUSTIC FLOW VELOCITY • *ACOUSTIC WAVE FORMULATION • *ADAPTIVE MESH • *BEAM FLUID INERTIA • *CONWEP CHARGE PROPERTY • *IMPEDANCE • *IMPEDANCE PROPERTY • *INCIDENT WAVE • *INCIDENT WAVE INTERACTION • *INITIAL CONDITIONS • *SIMPEDANCE • *TIE • “Defining an acoustic pressure boundary condition,” Section 16.10.19 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating the submodel boundary condition,” Section 38.4 of the Abaqus/CAE User’s Manual Overview Analyses performed using acoustic elements, an acoustic medium, and a dynamic procedure can simulate a variety of engineering phenomena including low-amplitude wave phenomena involving fluids such as air and water and “shock” analysis involving higher amplitude waves in fluids interacting with structures. An acoustic analysis: • is used to model sound propagation, emission, and radiation problems; • can include incident wave loading to model effects such as underwater explosion (UNDEX) on structures interacting with fluids, airborne blast loading on structures, or sound waves impinging on a structure; • in Abaqus/Explicit can include fluid undergoing cavitation when the absolute pressure drops to a limit value; • is performed using one of the dynamic analysis procedures (“Dynamic analysis procedures: overview,” Section 6.3.1); • can be used to model an acoustic medium alone, as in the study of the natural frequencies of vibration of a cavity containing an acoustic fluid; • can be used to model a coupled acoustic-structural system, as in the study of the noise level in a vehicle; • can be used to model the sound transmitted through a coupled acoustic-structural system; • requires the use of acoustic elements and, for coupled acoustic-structural analysis, a surface-based interaction using a tie constraint or, in Abaqus/Standard, acoustic interface elements; • can be used to obtain the scattered wave solution directly under incident wave loading when the mechanical behavior of the fluid is linear; • can be used to obtain a total wave solution (sum of the incident and the scattered waves) by selecting the total wave formulation, particularly when nonlinear fluid behavior such as cavitation is present in the acoustic medium; • can be used to model problems where the acoustic medium interacts with a structure subjected to large static deformation; • in Abaqus/Standard can be used with symmetric model generation (“Symmetric model generation,” Section 10.4.1) and symmetric results transfer (“Transferring results from a symmetric mesh or a partial three-dimensional mesh to a full three-dimensional mesh,” Section 10.4.2); • in Abaqus/Standard can be used with steady-state transport (“Steady-state transport analysis,” Section 6.4.1) and an acoustic flow velocity (“*ACOUSTIC FLOW VELOCITY,” Section 1.1 of the Abaqus Keywords Reference Manual) to model acoustic perturbations of a moving fluid; • in Abaqus/Standard can include a coupled structural-acoustic substructure that was previously defined (“Defining substructures,” Section 10.1.2); • can be used to model both interior problems, where a structure surrounds one or more acoustic cavities, and exterior problems, where a structure is located in a fluid medium extending to infinity; and • is applicable to any vibration or dynamic problem in a medium where the effects of shear stress are negligible. A shock analysis: • is used to model blast effects on structures; • often requires double precision to avoid roundoff error when Abaqus/Explicit is used; • may include acoustic elements to model the effects of fluid inertia and compressibility; • may include virtual mass effects to model the effect of an incompressible fluid interacting with a pipe structure; • is performed using one of the dynamic analysis procedures (“Dynamic analysis procedures: overview,” Section 6.3.1); • can be used to model both interior problems, where a structure surrounds one or more fluid cavities, and exterior problems, where a structure is located in a fluid medium extending to infinity; and • in Abaqus/Explicit can include air blast loading on structures using the CONWEP model. Procedures available for acoustic analysis Acoustic elements model the propagation of acoustic waves and are active only in dynamic analysis procedures. They are most commonly used in the following procedures: • Direct solution, steady-state, harmonic analysis. analysis,” Section 6.3.4. See “Direct-solution steady-state dynamic • Frequency analysis. See “Natural frequency extraction,” Section 6.3.5. • Subspace-based steady-state dynamic analysis. See “Subspace-based steady-state dynamic analysis,” Section 6.3.9. • Explicit dynamic analysis. See “Explicit dynamic analysis,” Section 6.3.3. Acoustic analysis can also be performed using: • Direct time integration analysis. Section 6.3.2. See “Implicit dynamic analysis using direct integration,” • Complex frequency analysis. See “Natural frequency extraction,” Section 6.3.5. • Mode-based transient dynamic analysis. See “Transient modal dynamic analysis,” Section 6.3.7. • Mode-based steady-state dynamic analysis. See “Mode-based steady-state dynamic analysis,” Section 6.3.8. • Dynamic fully coupled temperature-displacement analysis. See “Fully coupled thermal-stress analysis,” Section 6.5.3. In general, analysis with acoustic elements should be thought of as small-displacement linear perturbation analysis, in which the strain in the acoustic elements is strictly (or overwhelmingly) volumetric and small. In many applications the base state for the linear perturbation is simply ignored: for solid structures interacting with air or water, the initial stress (if any) in the air or water has negligible physical effect on the acoustic waves. Most engineering acoustic analyses, transient or steady state, are of this type. An important exception is when the acoustic perturbation occurs in a gas or liquid with high-speed underlying flow. If the magnitude of the flow velocity is significant compared to the speed of sound in the fluid (i.e., the Mach number is much greater than zero), the propagation of waves is facilitated in the direction of flow and impeded in the direction against the flow. This phenomenon is the source of the well-known “Doppler effect.” In Abaqus/Standard underlying flow effects are prescribed for nodes making up acoustic elements by specifying an acoustic flow velocity. Acoustic elements can be used in a static analysis, but all acoustic effects will be ignored. A typical example is the air cavity in a tire/wheel assembly. In such a simulation the tire is subjected to inflation, rim mounting, and footprint loads prior to the coupled acoustic-structural analysis in which the acoustic response of the air cavity is determined. See “Defining ALE adaptive mesh domains in Abaqus/Standard,” Section 12.2.6, and “ALE adaptive meshing and remapping in Abaqus/Standard,” Section 12.2.7, for more information. Acoustic elements also can be used in a substructure generation procedure to generate coupled structural-acoustic substructures. Only structural degrees of freedom can be retained. The retained eigenmodes must be selected when an acoustic-structural substructure is generated. In a static analysis involving a substructure containing acoustic elements, the results will differ from the results obtained in an equivalent static analysis without substructures. The reason is that the acoustic-structural coupling is taken into account in the substructure (leading to hydrostatic contributions of the acoustic fluid), while the coupling is ignored in a static analysis without substructures. More details on coupled structural-acoustic substructures can be found in “Defining substructures,” Section 10.1.2. A volumetric drag coefficient, , can be defined to simulate fluid velocity-dependent pressure amplitude losses. These occur, for example, when the acoustic medium flows through a porous matrix that causes some resistance , such as a sound-deadening material like fiberglass insulation. For direct time integration dynamic analysis we assume there are no significant spatial discontinuities in the quantity is the density of the fluid (acoustic medium), and that the volumetric drag is small at acoustic-structural boundaries. These assumptions, which can limit the applicability of the analysis, are discussed further in “Coupled acoustic-structural medium analysis,” Section 2.9.1 of the Abaqus Theory Manual. , where The direct-solution steady-state dynamic harmonic response procedure is advantageous for acoustic-structural sound propagation problems, because the gradient of need not be small and because acoustic-structural coupling and damping are not restricted in this formulation. If there is no damping or if damping can be neglected, factoring a real-only matrix can reduce computational time significantly; see “Direct-solution steady-state dynamic analysis,” Section 6.3.4, for details. Some fluid-solid interaction analyses involve long-duration dynamic effects that more closely resemble structural dynamic analysis than wave propagation; that is, the important dynamics of the structure occur at a time scale that is long compared to the compressional wave speed of the solid medium and the acoustic wave speed of the fluid. Equivalently, in such cases, disturbances of interest in the structure propagate very slowly in comparison to waves in the fluid and compressional waves in the structure. In such instances, modeling of the structure using beams is common. When these structural elements interact with a surrounding fluid, the important fluid effect is due to motions associated with incompressible flow . These motions result in a perceived inertia added to the structural beam; therefore, this case is usually referred to as the “virtual mass approximation.” For this case Abaqus allows you to modify the inertia properties of beam and pipe elements, as described below. Loads on the structure associated with incident waves in the fluid can be accommodated under this approximation as well. Natural frequency extraction Abaqus can compute both real and complex eigensolutions for purely acoustic or structural-acoustic systems, with or without damping. Exterior acoustic problems may also be solved. Selecting an eigensolver In a coupled acoustic-structural model, real-valued coupled modes are extracted by default using the Lanczos eigenfrequency extraction procedure. Coupling may be suppressed in the frequency extraction step; in this case the structural elements behave as though the interface with the acoustic elements were free (as though this surface were “in vacuo”), and the acoustic elements behave as though the boundary with the structural elements were rigid. Structural-acoustic coupling is ignored if the subspace iteration eigensolver is used. When applying the AMS eigensolver or the Lanczos eigensolver based on the SIM architecture to a coupled structural-acoustic model, Abaqus by default projects and stores the acoustic coupling matrix during the natural frequency extraction, for later use in coupled forced response analyses. The structural and acoustic regions are not actually coupled during the eigenanalysis; Abaqus solves the two regions separately but computes and stores the projected coupling operator for use in subsequent steady-state dynamic steps. Only structural-acoustic coupling defined using tied contact is supported. You can suppress this coupling if desired. Damping due to acoustic volumetric drag is also projected by default during an eigenanalysis and is restored by default in subsequent steady-state dynamic steps. Damping and inertia effects in an acoustic natural frequency extraction Since damping is not taken into account in real-valued modal extraction, the volumetric drag effect is not considered, except for its small contribution to any nonreflecting boundaries . The damping contributions due to any impedance boundary conditions (element-based or surface-based) or acoustic infinite elements are not included in an eigenfrequency extraction step, but the contributions to the acoustic element mass and stiffness matrices are included. Similarly, the (symmetrized) stiffness and mass contributions of acoustic infinite elements are included in an eigenfrequency extraction step, but the damping effects are neglected. Modal analysis of damped and radiating acoustic systems can be performed in Abaqus as well. Using the complex eigenvalue extraction procedure, the damping contributions of acoustic infinite elements, nonreflecting impedance conditions, and general impedance layers are restored to the element operators. If an underlying flow field is defined for the acoustic region by specifying an acoustic flow velocity, the natural frequencies and modes are affected. However, in real-valued frequency extraction only the acoustic element mass and stiffness matrices contribute to the solution. Since the formulation for acoustics in the presence of a flow field requires a complex part in the element operator (damping matrix), the real-valued procedure can include the effects of flow only to a limited degree. The complex frequency procedure in Abaqus/Standard includes the damping matrix contribution and is, therefore, required when modes of a system with moving fluid are sought. The complex frequency procedure can be used only following the Lanczos real-valued frequency procedure. Virtual mass effects defined for beams by adding inertia (“Additional inertia due to immersion in fluid” in “Beam section behavior,” Section 29.3.5) are included in modal analysis: their effect is simply to add inertia to a beam element. Interpreting the extracted modes in a coupled structural-acoustic natural frequency analysis While all the modes extracted in a coupled Lanczos structural-acoustic natural frequency analysis include the effects of fluid-solid interaction, some of them may have predominantly structural contributions while others may have predominantly acoustic contributions. Coupled structural-acoustic eigenmodes can be categorized as follows: • Most generally, an individual mode may exhibit participation in both the fluid and the solid media; this is referred to as a “coupled mode.” • Second, there are the “structural resonance” modes. These are modes corresponding to the eigenmodes of the structure without the presence of the acoustic fluid. The presence of the acoustic fluid has a relatively small effect on these eigenfrequencies and the mode shapes. • Third, there are the “acoustic cavity resonance” modes. These are nonzero eigenfrequency coupled modes that have a significant contribution in the resulting dynamics of the acoustic pressure in mode-based dynamic procedures. • Fourth, if insufficient boundary conditions are specified on the structural part of a model, the frequency extraction procedure will extract rigid body modes. These modes have zero eigenfrequencies (sometimes they appear as either small positive or even negative eigenvalues). However, if sufficient structural degrees of freedom are constrained, these rigid body modes disappear. • Finally, there are the singular acoustic modes, which have zero eigenfrequencies and constant acoustic pressure; they are mathematically analogous to structural rigid body modes. The structural part of the singular acoustic modes corresponds to the quasi-static structural response to constant pressure in unconstrained acoustic regions. These eigenmodes are predominantly acoustic and are important in representing the (low-frequency) acoustic response in mode-based analysis in the presence of acoustic loads, in the same way that rigid body modes are important in the representation of structural motion. As is true for the structural rigid body modes, if a sufficient number of constrained acoustic degrees of freedom is specified (one degree of freedom 8 per acoustic region is enough), the singular acoustic modes will disappear. In models with only one unconstrained acoustic region (the most common case) only one singular acoustic mode will In general there are as many singular acoustic modes as there are independent be computed. unconstrained acoustic regions. If these modes are present, they are always reported first by the Lanczos eigensolver; and a note at the bottom of the eigenfrequency table in the data file provides information about the number of singular acoustic modes. The generalized masses and effective masses can help distinguish between the various types of modes and can be used to assess which modes are important for subsequent mode-based analyses. In addition, the acoustic contribution to the generalized masses is reported as a fraction for each eigenmode. The closer the value of this fraction is to unity, the more pronounced is the acoustic component of this eigenmode. An acoustic effective mass is also computed for each eigenmode. This scalar quantity is scaled such that when all eigenmodes in a model are extracted, the sum of all acoustic effective masses is equal to 1.0 (minus the contributions from nodes with restrained acoustic degrees of freedom). The the higher the acoustic effective acoustic effective mass can be compared between different modes: mass, the more important (typically) the mode is for accurate representation of the acoustic pressure. For example, the fluid cavity acoustic resonance modes will have larger acoustic effective masses compared to the other modes. Modal superposition procedures In Abaqus acoustic domains are handled quite similarly to solid and structural domains. Real-valued eigenmodes, resulting from a previous real-valued eigenfrequency extraction procedure with or without coupling effects included, are used as a basis for modal solutions. The mode-based steady-state dynamic procedure is the most computationally efficient alternative to compute the steady-state response of structural-acoustic systems. Structural-acoustic coupling and damping effects in these analyses depend on the type of modal procedure and the eigensolver that was used to compute the eigenfrequencies. Structural-acoustic coupling in modal analyses using the Lanczos eigensolver without the SIM architecture If coupled modes are computed using the Lanczos eigensolver, both the mode-based and subspace projection steady-state dynamic procedures will If uncoupled Lanczos modes are computed, coupling can be restored only by using subspace projection. It is sufficient to project at a single frequency (constant subspace) to resolve the acoustic coupling for all frequencies. include structural-acoustic coupled effects. Acoustic medium damping in modal analyses using the Lanczos eigensolver without the SIM architecture In subspace-based steady-state dynamic analysis, acoustic medium damping and structural material infinite element, and impedance damping are considered, and the structural-acoustic interaction, boundary terms are also included. Acoustic medium damping is not considered in the procedures that base the response prediction directly on the system’s eigenmodes, such as transient modal dynamic analysis or the mode-based steady- state dynamic procedure. These methods should, therefore, be used with caution for problems with impedance boundary conditions. Modal damping can be used in these procedures (“Material damping,” Section 26.1.1) to model material damping and volumetric drag effects; however, modal damping usually cannot be used to model the fluid-solid coupling or the impedance boundary effects accurately. Structural-acoustic coupling and damping in modal analyses using the subspace iteration eigensolver The subspace iteration eigensolver neglects the effects of structural-acoustic coupling; coupling effects are not included in subsequent modal procedures. therefore, As with analyses using the Lanczos eigensolver, acoustic medium damping and structural material damping are considered in subsequent subspace-based steady-state dynamic procedures, but these damping effects are not considered in subsequent transient modal or mode-based steady-state dynamic procedures. Structural-acoustic coupling and damping in modal analyses using the AMS eigensolver or the Lanczos eigensolver based on the SIM architecture When modes are computed using the AMS eigensolver or the Lanczos eigensolver based on the SIM architecture, the structural-acoustic coupling and acoustic damping operators are projected and stored by default during the natural frequency extraction. Subsequent coupled forced response analyses using modal steady-state dynamics automatically restore the effects of structural-acoustic coupling and damping by automatically using these projected matrices; if the matrices were not projected, the steady-state dynamic step would not include these effects. A mode-based steady-state dynamic step cannot use nonsymmetric damping, such as from acoustic flow velocity or infinite element effects. To take these effects into account, a subspace-based steady-state dynamic analysis should be used. Defining translational or rotational underlying flow velocity in Abaqus/Standard As described above, acoustic analysis in Abaqus/Standard can be performed as a linear perturbation of a high-speed flow field. The flow velocity field affects the propagation of acoustic waves in the medium through the effect of the flow velocity on the speed of the wave propagation. Waves travel faster along the direction of the local flow vector and are correspondingly impeded in the direction against the flow direction. It is sufficient for you to define the velocity field in the affected acoustic region; the accelerations do not play a role in the formulation. You specify the flow in the acoustic finite element region as history data within a dynamic linear perturbation step. The flow field can be described either by direct input of the velocity components or by defining rotating motion associated with a reference frame. In the former case, each node in the acoustic region where flow occurs is assigned a Cartesian velocity defined by specifying the components of the velocity vector, . In the latter case, the rotational velocity for the nodes in the acoustic region is defined by specifying the magnitude of an angular rotation velocity, , and the position and orientation of the axis of rotation in the current configuration. The position and orientation of the axis are applied at the beginning of the step and remain fixed during the step. The specified underlying flow is active only for acoustic finite elements; other elements with acoustic degrees of freedom, such as acoustic infinite and interface elements, are unaffected by the specified flow velocity. The effect of underlying flow on the acoustic finite elements depends also on the procedure used: the effects are present only in frequency-domain dynamic procedures and natural frequency extraction. For complex-valued procedures, such as complex frequency extraction and steady-state dynamics, the presence of underlying flow affects the acoustic finite element stiffness matrices and adds a significant contribution to the element damping matrix. For real-valued procedures, such as eigenfrequency extraction and steady-state dynamics analysis in which a real-only system matrix is factored, the presence of underlying flow affects only the acoustic finite element stiffness matrices; the damping matrix is ignored. Consequently, the effect of flow on the acoustic field is fully realized only in complex-valued procedures. For rotating systems, solid and acoustic materials are treated differently in Abaqus. Flow of solid material through a mesh may induce significant deformation and is handled by using steady-state transport; subsequent linear perturbation steps are analyzed about this deformed state . Flow of material through an acoustic mesh is handled entirely within linear perturbation steps by specifying an acoustic flow velocity; a preliminary nonlinear steady-state transport analysis is not required. For coupled acoustic-structural systems undergoing rotation, such as tires, the model may be subjected to a steady-state transport step, which deforms the solid medium, followed by linear perturbation dynamic steps. The effect of the rotation of the solid is included in the linear perturbation steps in this case; to include the effect of the rotation of the acoustic fluid, specify an acoustic flow velocity in the linear perturbation steps. Input File Usage: Abaqus/CAE Usage: Use the following option to define a translating fluid velocity: *ACOUSTIC FLOW VELOCITY, TRANSLATION Use the following option to define a rotating fluid velocity: *ACOUSTIC FLOW VELOCITY, ROTATION Acoustic flow velocity is not supported in Abaqus/CAE. Updating the acoustic domain during a large-displacement Abaqus/Standard analysis By default, the acoustic-structural coupling calculations are based on the original configuration of the fluid domain. However, acoustic elements can also be used in an analysis where the structural domain experiences large deformation prior to the coupled analysis. A typical example is the interior cavity of a tire subjected to structural loads such as inflation, rim mounting, and footprint pressure. the deformation of The acoustic elements in Abaqus do not have displacement degrees of freedom and, therefore, cannot model the fluid when the structure undergoes large deformation. Abaqus/Standard solves the problem of computing the current configuration of the acoustic domain by periodically creating a new acoustic mesh. The new mesh uses the same topology (elements and connectivity) throughout the simulation, but the nodal locations are adjusted so that the acoustic domain conforms to the structural domain on the boundary. A new acoustic mesh is computed when adaptive meshing is specified and nonlinear geometric effects are considered in any non-perturbation Abaqus/Standard analysis procedure in which acoustic effects are ignored. The adaptive meshing features for acoustic analysis are described in detail in “Defining ALE adaptive mesh domains in Abaqus/Standard,” Section 12.2.6, and “ALE adaptive meshing and remapping in Abaqus/Standard,” Section 12.2.7. Initial conditions In Abaqus/Standard the initial acoustic static pressure (hydrostatic or ambient) is not modeled by the acoustic formulation and cannot be specified as an initial condition. In Abaqus/Explicit the initial acoustic pressure corresponding to the initial static equilibrium (hydrostatic or ambient) can be specified and is meaningful only when the acoustic fluid is capable of undergoing cavitation. In problems with possible fluid cavitation the initial acoustic static pressure is taken into account in the cavitation condition; i.e., the sum of the dynamic and static acoustic pressures needs to drop to the cavitation pressure limit for the cavitation to occur. The specified acoustic static pressure is used only in the cavitation condition and does not apply any static loads to the acoustic or structural meshes at their common wetted interface. In addition, the acoustic static pressure is not included in the nodal acoustic pressure degree of freedom. The initial temperature and field variable values can be specified (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) for the direct time integration dynamic, explicit dynamic, dynamic fully coupled temperature-displacement, and mode-based transient dynamic analysis procedures. Changes in these variables during the analysis will affect any temperature-dependent or field-variable-dependent acoustic medium properties. Boundary conditions The various boundary conditions that can be applied to an acoustic medium are described below. These include acoustic domain boundaries with stationary rigid walls or symmetry planes, prescribed pressure values such as a free surface with zero dynamic pressure, specified impedance , and structural interfaces such as the interface with a ship or a submarine. The radiating (nonreflecting) boundary condition for exterior problems (such as a structure vibrating in an acoustic medium of infinite extent) is implemented as a special case of the impedance boundary condition . On any given part of the acoustic domain boundary only one boundary condition type should be applied, except for the combination of the impedance boundary condition and the acoustic-structural interface condition. Boundary with a stationary rigid wall or a symmetry plane The default boundary condition for an acoustic medium is a boundary with a stationary rigid wall or a symmetry plane. The “force” conjugate to pressure in the acoustics formulation in Abaqus is the normal pressure gradient at the surface divided by the mass density; dimensionally this is equal to a force per unit mass. In the absence of volumetric drag this force per unit mass is equal to the inward acceleration of the acoustic medium. The conjugate variable at a node on the surface is the inward volume acceleration, which is the integral of the inward acceleration of the acoustic medium evaluated over the surface area associated with the node. A “traction-free” surface (one with no boundary conditions, no applied loads, no surface impedance conditions, and no interface elements) is a surface normal to which the acoustic medium undergoes no motion and, thus, corresponds to a rigid, stationary surface adjacent to the fluid. A symmetry plane for the acoustic medium is another “traction-free” surface. Prescribed pressure The basic variable in the acoustic medium is pressure (degree of freedom 8). Therefore, this variable can be prescribed at any node in the acoustic model by applying a boundary condition (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). Setting the pressure to zero represents a “free surface,” where the pressure does not vary because of the motion of the surface (to account for surface motion effects, see the discussion of impedance below). Prescribing a nonzero value for the pressure represents a sound source. An amplitude variation can be used to specify the value of the pressure. In a steady-state analysis you can specify both the in-phase (real) part of the pressure (default) and the out-of-phase (imaginary) part of the pressure. Input File Usage: Abaqus/CAE Usage: Boundary with a structure Use either of the following options to define the real (in-phase) part of the boundary condition: *BOUNDARY *BOUNDARY, REAL Use the following option to define the imaginary (out-of-phase) part of the boundary condition: *BOUNDARY, IMAGINARY Load module: Create Boundary Condition: choose Other for the Category and Acoustic pressure for the Types for Selected Step: select regions: Magnitude: real (in-phase) part + imaginary (out-of-phase) part i If the acoustic medium is adjacent to a structure, there will be a transfer of momentum and energy between the media at the boundary. The pressure field modeled with acoustic elements creates a normal surface traction on the structure, and the acceleration field modeled with structural elements creates the natural forcing term at the fluid boundary (for details, see “Coupled acoustic-structural medium analysis,” Section 2.9.1 of the Abaqus Theory Manual). The surface-based coupling procedure and the user-defined acoustic interface elements differ slightly in their theoretical implementation. In essence, the interface elements computed internally by the surface-based procedure are discrete point elements computed at the nodes of the slave surface. A user-defined acoustic interface element, on the other hand, distributes coupling effects across all of its nodes. Generally, the results obtained using the two coupling methods will be very similar, but the difference in discretization at the coupling boundary may create small differences in results. Defining acoustic-structural coupling with user-defined acoustic interface elements In Abaqus/Standard, if the structural and acoustic meshes share nodes at the boundary, lining this boundary with acoustic-structural library,” Section 32.13.2) will enforce the required physical coupling condition. The interface element normals must point into the acoustic medium, which forces continuity of the normal accelerations of the acoustic medium and of the structure at the boundary and ensures that the pressure of the acoustic elements is applied to the structure. Displacements can also be prescribed at such a boundary. interface elements . No additional element definitions are required. The slave surface, the first of the two surfaces specified for the tie constraint, must be element-based; whereas the master surface can be either element- or node-based. A surface based on rigid element types (R3D4, etc.) or an analytical rigid surface cannot be used as a master surface; instead, use a deformable surface made rigid. For surface-based tie constraints Abaqus automatically computes the region of influence for each internally generated acoustic-structural interface element. If the user-defined slave surface overhangs the master surface significantly, the regions of influence may include parts of the overhang. Consequently, the overhanging part of the slave surface may exhibit nonphysical coupled degrees of freedom: displacements if the slave surface is acoustic and acoustic pressures if the slave surface is solid or structural. These nonphysical results on the overhang do not affect the remainder of the solution, and it should be understood that they are not meaningful. Input File Usage: Use the following option in an analysis with the fluid mesh surface as the slave: *TIE, NAME=fluidslave fluid_surf, struct_surface Use the following option in an analysis with the solid mesh surface as the slave: *TIE, NAME=solidslave struct_surf, fluid_surf Abaqus/CAE Usage: Interaction module: Create Constraint: Tie Coupling surfaces to structures using acoustic infinite elements Acoustic infinite elements may form surfaces that can be coupled to structures by using a tie constraint in two different ways. The acoustic infinite element surface may consist of the base (first) facets of the acoustic infinite elements; in this case this surface should be tied to a topologically similar structural surface. The acoustic infinite element edges may also be used to define surfaces , which can be tied to solid elements. This approach couples the semi-infinite sides of acoustic infinite elements to solid elements. Mesh refinement Although the meshes may be nodally nonconforming at the tied surfaces, mesh refinement affects the accuracy of the coupled solution. In acoustic-solid problems the mesh refinement depends on the wave speeds in the two media. The mesh for the medium with the lower wave speed should generally be more refined and, therefore, should be the slave surface. If the details of the wave field in the vicinity of the fluid-solid interface are important, the meshes should be of equally high refinement, with the refinement corresponding to the lower wave speed medium. In this case the choice of the master surface is arbitrary. An exception is the case where the acoustic medium must be updated to follow the structure during a large-deformation analysis. In such a case the slave surface must be defined on the acoustic domain. Another exception is the case of fluids coupled to both sides of shell or beam elements (as described below). Solving the structural system sequentially using the submodeling technique In some applications the normal surface traction on the structure created by the acoustic fluid may be negligible compared to other forces in the structural system. For example, a metal motor housing may radiate sound into the surrounding air, but the reaction pressure of the air on the motor may be insignificant to the dynamics of the housing. In these cases the submodeling technique can be used to solve the system sequentially; that is, the structural analysis (uncoupled from the fluid) is followed by the acoustic analysis (driven by the structure). Usually, this decoupling of the analysis reduces computational cost. The structural system plays the role of the “global” model, and the acoustic fluid is the submodel. The structural displacements on the boundary of the acoustic fluid must be saved to the results file in the global analysis. Since Abaqus interpolates the fields between the global and submodels, acoustic-structural interface elements can be used. They should be applied to the fluid boundary to be driven by the global structural model. Input File Usage: Use the following options in the global (structural) analysis to be followed by a submodeling analysis: *NSET, NSET=solid_boundary_driving_the_fluid *NODE FILE, NSET=solid_boundary_driving_the_fluid Use the following options in the subsequent submodeling (fluid) analysis that uses acoustic interface elements on the fluid boundary to be driven: *NSET, NSET=fluid_boundary_to_be_driven *SUBMODEL, EXTERIOR TOLERANCE=tolerance fluid_boundary_to_be_driven *BOUNDARY, SUBMODEL, STEP=1 fluid_boundary_to be_driven, 1, 3, Abaqus/CAE Usage: Use the following input in the submodeling (fluid) analysis that uses an acoustic interface on the fluid boundary to be driven: Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select regions for fluid_boundary_to _be_driven: Exterior tolerance: relative: tolerance; Degrees of freedom: 1, 3; Global step number: 1 Defining acoustic-structural coupling on both sides of a beam or shell In Abaqus/Standard there are two alternatives available for modeling a beam (in two dimensions) or shell interacting with fluid on both sides: a surface-based procedure and an element-based procedure. In Abaqus/Explicit the surface-based procedure must be used. Use of the surface-based procedure is straightforward. Two surfaces must be defined on the beam or shell: one on the SPOS side and one on the SNEG side. Each surface is then coupled to the fluid using a tie constraint. At least one of the two surfaces on the beam or shell must be a master surface. In Abaqus/Standard, if the same nodes are used for the fluid and the beam or shell, acoustic interface elements must be used in the following manner to define acoustic-structural coupling on both sides of a beam or shell element: 1. Define a second set of nodes coincident with the beam or shell nodes, and constrain the motions of the two sets of nodes together using a PIN-type MPC (“General multi-point constraints,” Section 34.2.2). 2. Use the first set of nodes to line one side of the beam or shell elements with acoustic interface elements (with the normals of the acoustic interface elements pointing into the fluid). 3. Use the second set of nodes to line the other side of the beam or shell elements with acoustic interface elements (with the normals pointing into the fluid on the opposite side of the structure, as in Step 2). 4. The acoustic elements on the first side of the beam or shell elements should be defined using the first set of nodes, and the acoustic elements on the second side of the beam or shell elements should be defined using the second set of nodes. Defining the virtual mass effect (fluid-structural coupling) for beam and pipe elements In Abaqus virtual mass effects on submerged Timoshenko beam elements can be modeled by specifying additional inertia for the beam. The virtual mass effects are specified as part of the section definition of the beam. 1. Define the beam section (“Using a beam section integrated during the analysis to define the section behavior,” Section 29.3.6, or “Using a general beam section to define the section behavior,” Section 29.3.7), any additional internal inertia (“Adding inertia to the beam section behavior for Timoshenko beams” in “Beam section behavior,” Section 29.3.5), and the beam material properties. 2. Define the virtual mass effect (“Additional inertia due to immersion in fluid” in “Beam section behavior,” Section 29.3.5). 3. If the model is to be loaded using an incident wave (“Incident wave loading due to external sources” in “Acoustic and shock loads,” Section 33.4.6), define a surface or surfaces on the beam elements. Loads The following types of loading can be prescribed in an acoustic analysis, as described in “Acoustic and shock loads,” Section 33.4.6: • Concentrated pressure-conjugate loading. • An impedance condition that specifies the relationship between the pressure of the acoustic medium and the normal motion at the boundary (either element-based or surface-based). Such a condition is applied, for example, to include the effect of small-amplitude “sloshing” in a gravity field or to include the effect of a compressible, possibly dissipative, lining (such as a carpet) between the acoustic medium and a fixed, rigid wall or a structure. This type of condition can also be applied to edge facets of acoustic infinite elements. • Nonreflecting radiation conditions on acoustic boundaries (either element-based or surface-based). An impedance can be defined to select the appropriate radiating boundary condition taking the radiating surface shape into consideration. • Incident wave loading such as that caused by an underwater explosion or a sound field. Since this type of loading is usually applied in conjunction with semi-infinite acoustic regions, two alternative modeling formulations are available in Abaqus. A total pressure-based formulation is provided when the incident wave loading is applied to the exterior of a semi-infinite acoustic mesh. This formulation must be used to handle the incident wave loading when the acoustic medium is capable of cavitation, rendering the fluid material behavior nonlinear. The scattered pressure formulation is typically used when cavitation is not part of the fluid mechanical behavior and when the loads are applied to fluid-solid interfaces. Sound transmission loss and acoustic scattering problems usually fall into the latter category. For both formulations, when incident wave loading is applied to a given surface, a mathematical jump occurs between the pressures on both sides of the surface because the side from which the incident pressure arrives is implicitly a region of scattered pressure. This jump is handled automatically when the incident wave load is applied to a surface with a nonreflecting impedance condition and when the incident wave load is applied to a fluid-solid interface. However, if the incident wave load is applied to a surface lying between acoustic finite or infinite elements, the jump will not be modeled properly because pressures are continuous between acoustic elements. For this case, low-mass and low-stiffness membrane, shell, or surface elements should be interposed between the acoustic elements to permit the jump in pressure to exist. Incident wave loading can be applied in time-harmonic problems, using the direct solution steady-state dynamics and the subspace-based, steady-state dynamic procedures. You can define individual spherical or planar sources emitting waves, or you can use the deterministic diffuse field model in Abaqus. In the former case, usage is quite similar to transient analysis: the defined sources correspond to distinct sound sources. The latter case models the sound field incident on a surface exposed to a reverberant chamber: the field is assumed to be equivalent to a number of plane waves arriving from directions distributed on a hemisphere. Only the scattered wave formulation is supported when using incident wave loading in steady-state dynamics. See “Acoustic and shock loads,” Section 33.4.6, for several examples of incident wave loading. • Loading due to an incident shock wave caused by an air explosion. Although this type of wave is highly nonlinear and complex, the pressure loading due to the shock wave can be calculated readily from empirical data provided by the CONWEP model available in Abaqus/Explicit. The main advantage of this model is that the loading is applied directly to the structure subject to the blast; there is no need to include the fluid medium in the computational domain. In the CONWEP model, empirical data for two types of waves are available: spherical waves for explosions in mid- air and hemispherical waves for explosions at ground level in which ground effects are included. The CONWEP model does not account for effects of shadowing by intervening objects. In addition, it does not account for effects due to confinement and, thereby, excludes incorporation of any reflecting surfaces in the analysis. The model does account for the angle of incident of the blast wave; see “Acoustic and shock loads,” Section 33.4.6, for incorporation of the incident angle in the pressure load calculation. Predefined fields The following predefined fields can be specified in an acoustic analysis, as described in “Predefined fields,” Section 33.6.1: • Although temperature is not a degree of freedom in acoustic elements, nodal temperatures can be specified. The specified temperature affects temperature-dependent material properties. • The values of user-defined field variables can be specified. These values affect field-variable- dependent material properties. Material options Only the acoustic medium material model (“Acoustic medium,” Section 26.3.1) is valid for use in an acoustic analysis. The structure in a coupled acoustic-structural analysis can be modeled using any material model. Since acoustic analyses are always performed using a dynamic procedure, the structure’s density (“Density,” Section 21.2.1) should usually be defined. Porous materials are often modeled using an acoustic formulation when the dilatational waves in the porous medium dominate the shear effects. A large number of models exist for this category of phenomenon. In Abaqus, two categories of models are available for porous media modeled with acoustic elements: phenomenological models and general frequency-dependent models. Phenomenological models describe the dynamic characteristics using material data related to the porous structure, such as porosity itself, tortuosity, etc. Alternatively, you can specify the dynamic properties directly for the material; usually, this is done using a table of frequency-dependent data. See “Acoustic medium,” Section 26.3.1, for details on specifying acoustic materials in Abaqus. When the acoustic medium is capable of cavitation and the analysis includes incident wave loading, a total pressure-based formulation must be used. Either the default scattered wave formulation or the total wave formulation can be used if the cavitation is absent or the problem has no incident wave loading. For beam elements using the virtual mass approximation, the relevant data are specified as part of the beam section definition. Elements Abaqus provides a set of elements for modeling an acoustic medium undergoing small pressure changes. In addition, Abaqus/Standard provides interface elements to couple these acoustic elements to a structural model . If interface elements are used, only direct-solution steady-state harmonic (linear) response analysis (“Direct-solution steady- state dynamic analysis,” Section 6.3.4) and transient response analysis (“Implicit dynamic analysis using direct integration,” Section 6.3.2) can be performed. In Abaqus/Standard the second-order acoustic elements are generally considerably more accurate than first-order acoustic elements for a given number of degrees of freedom. The acoustic elements in Abaqus/Explicit are limited to first-order interpolations. Acoustic elements cannot be used together with hydrostatic fluid elements. With the CONWEP model provided in Abaqus/Explicit, the analysis must be three-dimensional. In addition, The loading surface must be comprised of solid, shell, or membrane elements only. CONWEP loading cannot be applied to acoustic elements. Exterior problems We often need to model an exterior problem, such as a structure vibrating in an acoustic medium of infinite extent. Impedance-type radiation boundary conditions can be used to model the motions of waves out of the mesh. In addition, Abaqus provides acoustic infinite elements for this class of problems. Impedance-type radiation conditions In this case acoustic elements are used to model the region between the structure and a simple geometric surface (located away from the structure), and a radiating (nonreflecting) boundary condition is applied at that surface. The radiating boundary conditions are approximate, so that the error in an exterior acoustic analysis is controlled not only by the usual finite element discretization error but also by the error in the approximate radiation condition. In Abaqus the radiation boundary conditions converge to the exact condition in the limit as they become infinitely distant from the radiating structure. In practice, these radiation conditions provide accurate results when the distance between the surface and the structure is at least one-half of the longest characteristic or responsive structural wavelength. For details, see “Acoustic and shock loads,” Section 33.4.6. Acoustic infinite elements Acoustic infinite elements are provided for modeling exterior problems (“Infinite elements,” Section 28.3.1). These elements have surface topology: line and quadratic segments in two-dimensional and axisymmetric problems and triangles and quadrilaterals in three-dimensional problems. Generally, the acoustic infinite elements are defined on a terminating surface of a region of acoustic finite elements. The infinite element formulation is considerably more accurate than the impedance-type radiation boundary conditions in cases where the wave field impinging on the terminating surface has many complex features. The radiation boundary conditions are relatively simple, equivalent to a “zeroth-order” infinite element; the acoustic infinite elements implemented in Abaqus are of variable order, up to ninth. Acoustic infinite elements can be coupled directly to structural surfaces by using a surface-based tie constraint: this may provide adequate accuracy in some applications. In general cases the acoustic infinite elements are defined on the terminating surface of the acoustic finite element mesh. The diameter of the acoustic finite element mesh can be considerably smaller, for a given solution accuracy, than is the case when using radiation boundary conditions. The nodal connectivity on the acoustic infinite element defines the element’s surface topology. To complete the element formulation, the surface topology must be mapped into the infinite domain. This mapping requires a reference point, given in the element section property definition. The reference point serves to define a characteristic length used in the coordinate mapping. In the ideal case of acoustic radiation from a spherical surface, the correct placement of the reference point is the center of the sphere. In general, the acoustic infinite elements produce the most accurate results when the reference node is located near the center of the region enclosed by the infinite elements. Nodal normal vectors are required for an accurate mapping of the infinite domain. The nodal normal vectors must point into the infinite domain and are used to define the portion of the infinite domain treated by a particular infinite element. To cover the infinite domain without overlap, each node attached to an infinite element must have a unique normal. The nodal normal vectors are specified or calculated as follows. User-specified alternative nodal normals (“Normal definitions at nodes,” Section 2.1.4) are ignored for acoustic infinite elements and, therefore, cannot be used to define normal directions for acoustic elements. Over the element’s surface topology, the normal vectors must be divergent; that is, the area mapped (in two dimensions) or the volume mapped (in three dimensions) must increase with distance into the infinite domain. To ensure this criteria, the normal vectors at each acoustic infinite element node are defined to lie along the vector between that node and the reference point given in the element section property definition. See “Infinite elements,” Section 28.3.1, for more information. Mesh refinement Inadequate mesh refinement is the most common source of difficulties in acoustic and vibration analysis. For reasonable accuracy, at least six representative internodal intervals of the acoustic mesh should fit into the shortest acoustic wavelength present in the analysis; accuracy improves substantially if ten or more internodal intervals are used at the shortest wavelength. In steady-state analyses the shortest wavelength will occur in the medium with the lowest speed of sound, at the highest frequency analyzed. In transient analyses the shortest wavelength present is more difficult to determine before an analysis: it is reasonable to estimate this wavelength using the highest frequency present in the loads or prescribed boundary conditions. An “internodal interval” is defined as the distance from a node to its nearest neighbor in an element; that is, the element size for a linear element or half of the element size for a quadratic element. At a fixed internodal interval, quadratic elements are more accurate than linear elements. The level of refinement chosen for the acoustic medium should be reflected in the solid medium as well: the solid mesh should be sufficiently refined to accurately model flexural, compressional, and shear waves. The level of mesh refinement required depends on the application. Any finite element discretization of a domain in which waves propagate introduces a certain amount of error per wavelength. In meshes that are small in terms of wavelengths, relatively coarse (for example, six internodal intervals per wavelength) meshes may be adequate. For meshes that contain many wavelengths at the frequency of interest, the per-wavelength finite element discretization error accumulates, generally necessitating In these larger meshes the accumulated per-wavelength error may be greater levels of refinement. present throughout the mesh if refinement is inadequate. The acoustic wavelength decreases with increasing frequency, so there is an upper frequency limit for a given mesh. Let the number of internodal intervals we desire per acoustic wavelength ( represent the maximum internodal interval of an element in a mesh, the cyclical frequency of excitation, and the speed of sound, where is recommended), is the bulk modulus of the acoustic medium and is its density. The requirements are then expressed as The above expressions can be used to estimate the maximum allowable element length if the frequency is given or the maximum frequency for which a given mesh size is valid. For example, in air at room temperature, meters per second. The following table gives some values for maximum internodal distances to model given maximum frequencies accurately: Maximum Frequency of Interest, Maximum Internodal Interval, , Maximum Internodal Interval, , 100 Hz 500 Hz 1000 Hz 20 kHz < 430 mm < 86 mm < 43 mm < 2.1 mm < 286 mm < 57 mm <29mm < 1.4mm For exterior problems the accuracy of an analysis also depends on the accuracy of the absorbing boundary condition. As mentioned above, the absorbing boundary impedance conditions implemented in Abaqus are used with a standoff thickness of acoustic finite elements between the acoustic sources and the radiating boundary. Since the approximate radiation conditions converge to the exact condition in the limit of infinite standoff, a greater standoff thickness improves the accuracy of the solution. The standoff thickness wavelengths at the minimum frequency to be analyzed: is expressed as Continuing the example using the properties of air, we can calculate the recommended minimum standoff thicknesses corresponding to a specified minimum frequency of interest, using : Minimum Frequency of Interest, Radiation Boundary Standoff, 100 Hz 500 Hz 1000 Hz 20 kHz > 1140 mm > 230 mm > 114 mm > 5.7 mm The computational requirements for an exterior problem thus depend on both the radiation boundary standoff and the internodal distance. The number of nodes N in a model depends on the volume of the mesh, controlled by . The exact number of nodes depends on the details of the model, but the expression and the spatial dimension d, and the mesh density, controlled by indicates the size of the model with respect to the ratio of the maximum to minimum frequencies in a given analysis. Because the mesh size for an exterior problem exhibits such strong dependence on the bandwidth, , you can control the size of an analysis by splitting the band. For example, if the overall frequency range of interest is 100 to 10000 Hz, a single spherical mesh covering this band in three dimensions has size However, splitting the problem into two bands, mesh for each band, results in two analyses of size and , and creating an exterior In coupled acoustic-structural systems there usually exist different wave speeds for the fluid and solid media. In the region of the acoustic-structural interface, the wave phenomena in both media may exhibit length scales characteristic of the slower medium; that is, the length scale of the wave dynamics may be as short as the shorter wavelength, corresponding to the lower wave speed. This result follows from the fact that the two media are coupled at the boundary. The region near the acoustic-structural interface where these effects are important is usually no thicker than the shorter wavelength. For example, in an analysis involving water interacting with rubber, the wave speed in the rubber may be much lower than that of water. A finite element mesh used to model this problem in detail would require refinement down to six (or more) nodes per shorter wavelength, on both sides of the interface. On the water side (faster, longer wavelength) accuracy will probably not be compromised significantly if this region of high refinement extends no further into the water than one short wavelength. Of course, in some analyses the effects in the vicinity of the interface may be unimportant. Then, the two meshes can be refined only so far as to represent their own characteristic wavelengths accurately. Output Nodal output variable POR (pressure magnitude at the nodes of the acoustic elements) is available for an acoustic medium (in Abaqus/CAE this output variable is called PAC). When the scattered wave formulation (default) is used with incident wave loading, output variable POR represents only the scattered pressure response of the model and does not include the incident wave loading itself. When the total wave formulation is used, output variable POR represents the total dynamic acoustic pressure, which includes contributions from both incident and scattered waves as well as the dynamic effects of fluid cavitation. For either formulation output variable POR does not include the acoustic static pressure. In Abaqus/Explicit an additional nodal output variable PABS (the absolute pressure, equal to the sum of POR and the acoustic static pressure) is available. When the dynamic effects of fluid cavitation are of interest, you can specify the acoustic static pressure in an acoustic analysis that uses the total wave formulation. If the acoustic static pressure is not specified in an acoustic region, it is assumed to be large; thus precluding cavitation in that region. For general steps, including implicit and explicit dynamic steps, no energy quantities are computed for acoustic elements. Consequently, these elements will not contribute to the total energy balance. Steady-state dynamic output For steady-state dynamic analysis POR is complex and can be displayed in several forms in the Visualization module of Abaqus/CAE. The phase angle (PPOR) is available as output to the data (.dat) and results (.fil) files. in direct-solution steady-state dynamic or subspace-based steady-state dynamic analysis. The “sound pressure level” is defined as: ACOUSTIC ANALYSIS where and the is defined as a physical constant in the model , at any point using the formula: is computed from the complex-valued acoustic pressure The acoustic particle velocity at any material point is The acoustic intensity vector, a measure of the rate of flow of energy at a material point, is In an acoustic medium the stress tensor is simply the acoustic pressure times the identity tensor, so this expression simplifies to The hats denote complex conjugation. The real part of the intensity is referred to as the “active intensity,” and the imaginary part is the “reactive intensity.” The acoustic pressure gradient is also available for acoustic finite elements in steady-state dynamic analysis. In steady-state dynamic analysis, additional nodal output quantities are available for acoustic infinite elements. PINF denotes the complex pressure coefficients of the infinite element shape functions. These coefficients can be used to visualize the exterior acoustic field (i.e., within the volume of the acoustic infinite elements) using scripting in the Visualization module of Abaqus/CAE; see “Using infinite elements to compute and view the results of an acoustic far-field analysis,” Section 9.10.11 of the INFN is the normal vector used by the acoustic infinite element Abaqus Scripting User’s Manual. to define the element volume. INFR denotes the radius used for the element at that node, and INFC denotes the element cosine; that is, the minimum dot product between the nodal normal vector and the acoustic infinite element facet normal vectors attached to that node. See “Acoustic infinite elements,” Section 3.3.2 of the Abaqus Theory Manual, for more complete descriptions of these quantities. INFN, INFR, INFC are useful in debugging a model using acoustic infinite elements; consequently, it is sometimes valuable to perform a steady-state dynamics, direct analysis on a model to visualize this information. For steady-state dynamic steps, energy quantities are available for acoustic elements. These elements contribute to the total energy balance in steady-state dynamics. Defining the reference pressure You must define the reference pressure, default value for the reference pressure. , used to compute the sound pressure level; there is no Input File Usage: Abaqus/CAE Usage: *PHYSICAL CONSTANTS, SPL REFERENCE PRESSURE= You cannot define a reference pressure in Abaqus/CAE. Input file template The following is an example of the step definition for a direct-solution steady-state dynamic acoustic analysis that looks for the response of a model at six frequencies ranging linearly from to cycles/time. The pressure at node set INPUT (nodes at the boundary) is prescribed to have an in- ). An phase component of 3.0 and an out-of-phase component of −4.0 (i.e., a complex value of in-phase inward volume acceleration of 40.0 is specified at node 10. On the surface LINER1 an impedance is defined based on the impedance property named CARPET1. On the second face of all of the elements in element set PAD, another surface impedance based on CARPET1 is defined. On the fourth face of all of the elements in element set END, the default plane wave boundary condition is specified. Printed output of pressure magnitude and phase is requested for node set OUTPUT. Acoustic pressure and displacement are written to the output database. All output is written once for each of the six excitation frequencies. *HEADING … *SURFACE, NAME=LINER1 10, S3 *IMPEDANCE PROPERTY, NAME=CARPET1 Data describing impedance properties as a function of frequency ** *STEP *STEADY STATE DYNAMICS, DIRECT 10, 100, 6 *SIMPEDANCE, PROPERTY=CARPET1 LINER1, ** *IMPEDANCE, PROPERTY=CARPET1 PAD, I2 *IMPEDANCE END, I4 ** Apply complex pressure at node set INPUT *BOUNDARY, REAL INPUT, 8, 8, 3. *BOUNDARY, IMAGINARY INPUT, 8, 8, -4. ** Apply an in-phase inward volume acceleration at node 10 *CLOAD 10, 8, 40. ** Output requests *NODE PRINT, NSET=OUTPUT, TOTALS=YES POR, PPOR *OUTPUT, FIELD *NODE OUTPUT U, PU, POR *END STEP The following is a template of the step definition for an Abaqus/Explicit acoustic analysis. On the surface SURF an impedance is defined based on the impedance property named IPROP. In addition, impedance is defined on elements or element sets. *HEADING … *ELEMENT, TYPE=AC2D4R … ** *SURFACE, NAME=SURF Data line to define surface *IMPEDANCE PROPERTY, NAME=IPROP Data describing impedance properties ** *STEP *DYNAMIC, EXPLICIT or *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT Data line to define incrementation *SIMPEDANCE, PROPERTY=IPROP SURF, ** *IMPEDANCE Data lines to define impedance on elements or element sets *CLOAD Data line to define acoustic loads *FIELD Data line to define field variable values *END STEP The following template is representative of a coupled acoustic-structural shock problem using the preferred interface for applying incident wave loading : *HEADING … *ELEMENT, TYPE=…, ELSET=ACOUSTIC Data lines to define acoustic elements *ELEMENT, TYPE=…, ELSET=SOLID Data lines to define solid elements *ELEMENT, TYPE=…, ELSET=BEAM Data lines to define beam elements *BEAM SECTION,ELSET=BEAM,MATERIAL=... Data lines to define the beam stiffness section properties *BEAM FLUID INERTIA Data line to define the beam virtual mass property *SURFACE, NAME=IW_LOAD_ACOUSTIC Data lines to define the acoustic surface loaded by the incident wave *SURFACE, NAME=IW_LOAD_SOLID Data lines to define the solid surface loaded by the incident wave *SURFACE, NAME=IW_LOAD_BEAM Data lines to define the beam surface loaded by the incident wave *SURFACE, NAME=TIE_ACOUSTIC Data lines to define the acoustic surface interface with the solid mesh *SURFACE, NAME=TIE_SOLID Data lines to define the solid surface interface with the acoustic mesh *INCIDENT WAVE INTERACTION PROPERTY, NAME=IWPROP, TYPE=SPHERE Data lines to define a spherical incident wave field *UNDEX CHARGE PROPERTY Data lines to define the underwater explosion parameters ** Tie the acoustic mesh to the solid mesh *TIE, NAME=COUPLING TIE_ACOUSTIC, TIE_SOLID *STEP *DYNAMIC, EXPLICIT or *DYNAMIC ** Load the acoustic surface *INCIDENT WAVE INTERACTION, PROPERTY=IWPROP IW_LOAD_ACOUSTIC, source node, standoff node, reference magnitude ** Load the solid surface *INCIDENT WAVE INTERACTION, PROPERTY=IWPROP IW_LOAD_SOLID, source node, standoff node, reference magnitude ** Load the beam surface *INCIDENT WAVE INTERACTION, PROPERTY=IWPROP IW_LOAD_BEAM, source node, standoff node, reference magnitude *END STEP The following template is representative of a coupled acoustic-structural shock problem using the alternative interface for applying incident wave loading: *HEADING … *ELEMENT, TYPE=…, ELSET=ACOUSTIC Data lines to define acoustic elements *ELEMENT, TYPE=…, ELSET=SOLID Data lines to define solid elements *ELEMENT, TYPE=…, ELSET=BEAM Data lines to define beam elements *BEAM SECTION,ELSET=BEAM,MATERIAL=... Data lines to define the beam stiffness section properties *BEAM FLUID INERTIA Data line to define the beam virtual mass property *SURFACE, NAME=IW_LOAD_ACOUSTIC Data lines to define the acoustic surface loaded by the incident wave *SURFACE, NAME=IW_LOAD_SOLID Data lines to define the solid surface loaded by the incident wave *SURFACE, NAME=IW_LOAD_BEAM Data lines to define the beam surface loaded by the incident wave *SURFACE, NAME=TIE_ACOUSTIC Data lines to define the acoustic surface interface with the solid mesh *SURFACE, NAME=TIE_SOLID Data lines to define the solid surface interface with the acoustic mesh *INCIDENT WAVE PROPERTY, NAME=IWPROP, TYPE=SPHERE Data lines to define a spherical incident wave field *INCIDENT WAVE FLUID PROPERTY Data lines to define the fluid properties for the incident wave field *AMPLITUDE, DEFINITION=BUBBLE, NAME=PRESSUREVTIME Data lines to define the underwater explosion parameters ** Tie the acoustic mesh to the solid mesh *TIE, NAME=COUPLING TIE_ACOUSTIC, TIE_SOLID *STEP *DYNAMIC or *DYNAMIC, EXPLICIT ** Load the acoustic surface *INCIDENT WAVE, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP IW_LOAD_ACOUSTIC, {amplitude} ** Load the solid surface and the beam surface *INCIDENT WAVE, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP IW_LOAD_SOLID, {amplitude} IW_LOAD_BEAM, {amplitude} *END STEP The following template is representative of a coupled acoustic-structural sound transmission problem using the preferred interface for applying incident wave loading : *HEADING … *ELEMENT, TYPE=…, ELSET=ACOUSTIC Data lines to define acoustic elements *ELEMENT, TYPE=…, ELSET=SOLID Data lines to define solid elements *SURFACE, NAME=IW_LOAD_ACOUSTIC Data lines to define the acoustic surface loaded by the incident wave *SURFACE, NAME=IW_LOAD_SOLID Data lines to define the solid surface loaded by the incident wave *SURFACE, NAME=TIE_ACOUSTIC Data lines to define the acoustic surface interface with the solid mesh *SURFACE, NAME=TIE_SOLID Data lines to define the solid surface interface with the acoustic mesh *INCIDENT WAVE INTERACTION PROPERTY, NAME=FIRST, TYPE=SPHERE Data lines to define a spherical incident wave field *INCIDENT WAVE INTERACTION PROPERTY, NAME=SECOND, TYPE=PLANE Data lines to define a planar incident wave field ** Tie the acoustic mesh to the solid mesh *TIE, NAME=COUPLING TIE_ACOUSTIC, TIE_SOLID *STEP *STEADY STATE DYNAMICS, DIRECT or SUBSPACE PROJECTION ** Define the load on the acoustic and solid surfaces due to ** the first loading case: *LOAD CASE, NAME=FIRST_SOURCE ** Load the acoustic surface: define the real part at the ** standoff point *INCIDENT WAVE INTERACTION, PROPERTY=FIRST, REAL IW_LOAD_ACOUSTIC, first source node, first standoff node, reference magnitude ** Load the acoustic surface: define the imaginary part at the ** standoff point *INCIDENT WAVE INTERACTION, PROPERTY=FIRST, IMAGINARY IW_LOAD_ACOUSTIC, first source node, first standoff node, reference magnitude ** Load the solid surface: define the real part at the ** standoff point *INCIDENT WAVE INTERACTION, PROPERTY=FIRST, REAL IW_LOAD_SOLID, first source node, first standoff node, reference magnitude ** Load the solid surface: define the imaginary part at the ** standoff point *INCIDENT WAVE INTERACTION, PROPERTY=FIRST, IMAGINARY IW_LOAD_SOLID, first source node, first standoff node, reference magnitude *END LOAD CASE ** Define the load on the acoustic and solid surfaces due to ** the next loading case: *LOAD CASE, NAME=SECOND_SOURCE ** Load the acoustic surface: define the real part at the ** standoff point *INCIDENT WAVE INTERACTION, PROPERTY=SECOND, REAL IW_LOAD_ACOUSTIC, second source node, second standoff node, reference magnitude ** Load the acoustic surface: define the imaginary part at the ** standoff point *INCIDENT WAVE INTERACTION, PROPERTY=SECOND, IMAGINARY IW_LOAD_ACOUSTIC, second source node, second standoff node, reference magnitude ** Load the solid surface: define the real part at the ** standoff point *INCIDENT WAVE INTERACTION, PROPERTY=SECOND, REAL IW_LOAD_SOLID, second source node, second standoff node, reference magnitude ** Load the solid surface: define the imaginary part at the ** standoff point *INCIDENT WAVE INTERACTION, PROPERTY=SECOND, IMAGINARY IW_LOAD_SOLID, second source node, second standoff node, reference magnitude *END LOAD CASE *END STEP 6.11 Abaqus/Aqua analysis • “Abaqus/Aqua analysis,” Section 6.11.1 6.11.1 Abaqus/AQUA ANALYSIS Product: Abaqus/Aqua References • “UWAVE,” Section 1.1.54 of the Abaqus User Subroutines Reference Manual • “Defining an analysis,” Section 6.1.2 • *AQUA • *CLOAD • *C ADDED MASS • *DLOAD • *D ADDED MASS • *WAVE • *WIND Overview An Abaqus/Aqua analysis: • is used to apply steady current, wave, and wind loading to submerged or partially submerged structures in problems such as the modeling of offshore piping installations or the analysis of marine risers; • can be performed using the static (“Static stress analysis,” Section 6.2.2), direct-integration dynamic (“Implicit dynamic analysis using direct integration,” Section 6.3.2), explicit dynamics (“Explicit dynamic analysis,” Section 6.3.3), or eigenfrequency extraction (“Natural frequency extraction,” Section 6.3.5) procedures; • will calculate drag, buoyancy, and inertia loading only for beam, pipe, elbow, truss, and certain rigid elements; • can include elements that model spud cans for jack-up foundation analysis in Abaqus/Standard; and • can be linear or nonlinear. Procedures available for Aqua analysis Aqua loading can be applied in static steps (“Static stress analysis,” Section 6.2.2), direct-integration dynamic steps (“Implicit dynamic analysis using direct integration,” Section 6.3.2), and explicit dynamic steps (“Explicit dynamic analysis,” Section 6.3.3). During these steps fluid particle velocity is assumed to consist of two superposed effects: steady currents, which can vary with elevation and location, and gravity waves. Fluid particle accelerations are associated with gravity waves only. The fluid particle velocities and accelerations are used to calculate drag and inertia loading on the immersed body. Abaqus/Aqua also computes the fluid surface elevation and allows for partial immersion; drag and buoyancy loadings are omitted for those parts of the structure that are above the fluid surface or below the seabed level. An eigenfrequency extraction step (“Natural frequency extraction,” Section 6.3.5) can be used to extract the natural frequencies of a structure prestressed by the Aqua loading in a static or direct-integration dynamic step (if that step included the effects of nonlinear geometry). The added-mass effect due to fluid inertia loads can be included in an eigenfrequency extraction step. Defining an Abaqus/Aqua problem Aqua loads are applied in the following manner: 1. The fluid properties and steady current velocity are defined for the model. 2. Gravity waves and wind velocity are defined for the model. 3. Drag, buoyancy, and fluid inertia loads are applied to elements and nodes of the structure using distributed or concentrated load definitions within the static or direct-integration dynamic step definition. The magnitudes of the loads applied are determined by the fluid properties, steady current, wave, and wind definitions. 4. In an eigenfrequency extraction step concentrated and distributed added mass definitions are used (instead of concentrated and distributed loads) to include the effects of fluid inertia. The load-stiffness terms from Abaqus/Aqua loads, which are important in geometrically nonlinear analysis, are fundamentally unsymmetric. Therefore, the unsymmetric matrix solution and storage scheme should be used for the step when nonlinear geometric effects are included (“Defining an analysis,” Section 6.1.2). It is essential to use the unsymmetric solver when the structure being analyzed is flexible (see, for example, “Slender pipe subject to drag: the “reed in the wind”,” Section 1.13.3 of the Abaqus Benchmarks Manual). On the other hand, if a relatively stiff structure is subject to Aqua loads or if a dynamic step uses small time increments, the unsymmetric load-stiffness terms may not be dominant and you may be able to obtain a convergent solution with the symmetric solver (see, for example, “Riser dynamics,” Section 12.1.2 of the Abaqus Example Problems Manual). Coordinate system The z-coordinate axis must point vertically for three-dimensional cases, and the y-coordinate axis must point vertically for two-dimensional cases. For the three-dimensional case the still fluid surface (when there is no wave motion) lies in a plane that is parallel to the x–y plane. For the two-dimensional case it lies parallel to the x-axis. The position of the still fluid surface is specified as part of the fluid property data. Defining the fluid properties Aqua loadings require the definition of fluid density, seabed and free surface elevation, and the gravitational constant. Input File Usage: *AQUA seabed elevation, free surface elevation, gravitational constant, fluid density The *AQUA option must be included in the model data portion of the input file. Defining a steady current Steady currents are defined by giving steady fluid velocity as a function of elevation and location. Elevation is defined in the positive z-direction for three-dimensional models and in the positive y-direction for two-dimensional models. For two-dimensional cases the z-component of the steady current velocity is ignored. See “Input syntax rules,” Section 1.2.1, for an explanation of how to define one property (in this case steady current velocity) as a function of multiple independent variables. If the fluid velocity is not a function of elevation or location (for example, when modeling a problem in a coordinate system that moves uniformly through the still fluid, such as a tow-out analysis), only one fluid velocity need be specified. The steady current velocities can be scaled by referring to an amplitude curve (“Amplitude curves,” Section 33.1.2) from the concentrated or distributed load definitions used to apply drag loads, as described later. Input File Usage: *AQUA fluid properties on first data line (described above) X-velocityfluid, Y-velocityfluid , Z-velocityfluid , elevation, X-coord, Y-coord ... Defining gravity waves Gravity waves are defined by specifying a wave theory. The wave theory determines fluid acceleration, velocity, and pressure field fluctuations. The fluid acceleration and velocity field fluctuations contribute to the drag loads. The fluid pressure field fluctuations contribute to the buoyancy loads. Choosing the type of wave theory to be used Using Abaqus/Aqua in an Abaqus/Standard analysis, you can choose Airy linear wave theory, Stokes fifth-order wave theory, wave data read from a gridded mesh, or fluid kinematics defined in user subroutine UWAVE. For Airy and Stokes waves the fluid surface elevation and the fluid particle velocities and accelerations will be calculated as functions of time and location based on the wave definition. If wave data are provided in the form of a gridded mesh, you must specify these quantities. If user subroutine UWAVE is used, the fluid kinematics must be defined in that routine. Similarly, using Abaqus/Aqua in an Abaqus/Explicit analysis, you can choose Airy linear wave theory, Stokes fifth-order wave theory, or fluid kinematics defined in user subroutine VWAVE. All of the built-in wave theories assume a series of waves in the horizontal plane (the plane of the fluid surface) that are unaffected by any fluid-structural interaction. The Airy and Stokes theories are based on irrotational flow of an inviscid, incompressible fluid, where the wave height H is small compared to the still water depth d. The bottom of the fluid is assumed to be flat (the still water depth is constant). The Ursell parameter, is the wavelength, should be much less than 1.0 for Airy wave theory to be applicable and should where be less than 10.0 for Stokes theory to be applicable. For ratios of H/ greater than 0.142, the crest of the wave is predicted to break. The assumed boundary conditions on the free surface are then no longer valid in either theory, which limits the maximum wave amplitude for either theory. Airy wave theory , is less Linear Airy wave theory is generally used when the ratio of wave height to water depth, than 0.03, provided that the water is deep (ratio of water depth to wavelength, , is greater than 20). Convective acceleration terms are neglected in the Airy theory as part of the linearization. The Airy wave theory is described in detail in “Airy wave theory,” Section 6.2.2 of the Abaqus Theory Manual. Since the Airy wave theory is linear, any number of wave trains traveling in different directions across the water can be defined; the fluid particle velocities and accelerations sum by linear superposition. The direction of each wave component is given by specifying the direction cosines of a vector, , lying in the plane defined by the still fluid surface. By default, Airy waves are defined in terms of wavelength, . Alternatively, you can define the . For Airy wave theory the wavelength and period of each component waves in terms of wave period, are related by where is the period of this component, is the gravitational acceleration, is the wavelength, and is the undisturbed (still) water depth. Input File Usage: Use the following option to define an Airy wave in terms of wavelength: *WAVE, TYPE=AIRY amplitude, wavelength, phase angle, x-direction cosine, y-direction cosine Use the following option to define an Airy wave in terms of wave period: *WAVE, TYPE=AIRY, WAVE PERIOD amplitude, wave period, phase angle, x-direction cosine, y-direction cosine In either case repeat the data line to define multiple wave trains. Stokes fifth-order wave theory The Stokes fifth-order wave theory is a deep-water wave theory that is valid for relatively large wavelengths. Convective terms are included in the fluid particle acceleration calculations for Stokes fifth-order theory and can be significant for larger ratios. The Stokes wave theory is described in detail in “Stokes wave theory,” Section 6.2.3 of the Abaqus Theory Manual. Because the Stokes fifth-order wave theory is nonlinear, only one wave train is allowed in an analysis. The relationship between wavelength and period of the waves in Stokes fifth-order theory is not as simple as that for the Airy theory, although the formula given above is a first-order approximation. Stokes waves can be defined only in terms of the wave period, . Input File Usage: *WAVE, TYPE=STOKES wave height, wave period, phase angle, direction of travel cosines Gridded wave data You can choose to provide wave surface elevations, particle velocities and accelerations, and the dynamic pressure at points in a user-defined grid through a binary data file. The binary file contains information about the wave definition, the location of the grid points where wave information is specified, and the wave kinematics at user-defined times. At spatial locations within the user-defined grid, Abaqus/Aqua will interpolate the wave kinematics from the nearest grid points, using either linear or quadratic interpolation. When a point on the structure is above the user-defined grid, Abaqus/Aqua assumes that the point is above the free surface elevation. Hence, no fluid loads are applied. If a point on the structure falls outside the user-defined spatial grid without being above the grid, Abaqus/Aqua finds the wave kinematics at the nearest point within the grid and uses those values at the point on the structure. Input File Usage: *WAVE, TYPE=GRIDDED, DATA FILE=file_name Binary data file requirements for gridded wave data The data file must contain the following unformatted (binary) records . The data for the FORTRAN WRITE statement are given for each record: First record: NCOMP, DTG, NWGX, NWGY, NWGZ, IPDYN where NCOMP is the number of wave components to be read in the data file; DTG is the time increment at which wave data are given on the grid; NWGX NWGY is the number of grid points in the grid’s x-direction; is the number of grid points in the grid’s y-direction—if this number is one, Abaqus/Aqua assumes that the wave data are constant with respect to the local y-direction; NWGZ is the number of grid points in the grid’s z-direction—if this number is zero or one, the analysis is two-dimensional and the y-direction is vertical; and IPDYN is an integer flag indicating whether dynamic pressure information is stored (IPDYN=1) or not stored (IPDYN=0) in the gridded wave file. Second record: (AMP(K1), WXL(K1), PHI(K1), K1=1,NCOMP) where NCOMP is read on the first record, above; AMP WXL PHI contains the wave component amplitude, contains the wavelength of this component, contains the phase angle of this component, ; ; and (in degrees). The second record of this file contains the wave component data used to generate the gridded wave data; it is not used by Abaqus/Aqua. This record is provided only for information in user subroutine UEL by using the GETWAVE interface . The meaning of the arrays AMP and WXL is left to you; however, PHI is converted to radians. Third record: (WGX(K1),K1=1,NWGX), (WGY(K1),K1=1,NWGY), (WGZ(K1),K1=1,NWGZ) where NWGi WGX WGY WGZ are read on the first record, above; contains the local x-coordinates of the grid points; contains the local y-coordinates of the grid points; and contains the local z-coordinates of the grid points (not included in the gridded wave file for two-dimensional analyses). Remaining records if IPDYN=0: For three dimensions: (((WGVX(K1,K2,K3), WGVY(K1,K2,K3), WGVZ(K1,K2,K3), WGAX(K1,K2,K3), WGAY(K1,K2,K3), WGAZ(K1,K2,K3), K3=1,NWGZ), WZCRST(K1,K2), NCRST(K1,K2), K1=1,NWGX), K2=1,NWGY) For two dimensions: ((WGVX(K1,K2), WGVY(K1,K2), WGAX(K1,K2), WGAY(K1,K2), K2=1,NWGY), WZCRST(K1), NCRST(K1), K1=1,NWGX) Remaining records if IPDYN=1: For three dimensions: (((WGVX(K1,K2,K3), WGVY(K1,K2,K3), WGVZ(K1,K2,K3), WGAX(K1,K2,K3), WGAY(K1,K2,K3), WGAZ(K1,K2,K3), P(K1,K2,K3), DPDZ(K1,K2,K3), K3=1,NWGZ), WZCRST(K1,K2), NCRST(K1,K2), K1=1,NWGX), K2=1,NWGY) For two dimensions: ((WGVX(K1,K2), WGVY(K1,K2), WGAX(K1,K2), WGAY(K1,K2), P(K1,K2), DPDZ(K1,K2), K2=1,NWGY), WZCRST(K1), NCRST(K1), K1=1,NWGX) where WGVX WGVY WGVZ WGAX WGAY WGAZ WZCRST NCRST DPDZ contains the local x-components of the wave particle velocity, contains the local y-components of the wave particle velocity, contains the local z-components of the wave particle velocity, contains the local x-components of the wave particle acceleration, contains the local y-components of the wave particle acceleration, contains the local z-components of the wave particle acceleration, contains the wave surface elevation, contains the index for the vertical grid level just above the instantaneous water surface, contains the dynamic pressure, and contains the gradient of the dynamic pressure in the vertical direction. User-defined wave theory in Abaqus/Standard A user-defined wave theory can be coded in user subroutine UWAVE in an Abaqus/Aqua analysis in Abaqus/Standard. You can define the fluid particle velocity, acceleration, free surface elevation, and fluid pressure field in the user subroutine. For stochastic analysis, you can specify a random number seed, r, and define frequency/amplitude pairs that define the wave spectrum. During the analysis Abaqus/Aqua stores an intermediate configuration that can be used in the user subroutine to compute the stochastic description of the waves. The intermediate configuration is initialized as the reference configuration and is replaced by the current configuration only when requested by the user subroutine. In this way the stochastic description of the wave field can be stored in an external database and recalculated only when necessary. Input File Usage: Use the following option to specify the wave kinematics in user subroutine UWAVE: *WAVE, TYPE=USER Use the following option for stochastic analysis to make the intermediate configuration available in user subroutine UWAVE: *WAVE, TYPE=USER, STOCHASTIC=r frequency, amplitude ... User-defined wave theory in Abaqus/Explicit A user-defined wave theory can be coded in user subroutine VWAVE in an Abaqus/Aqua analysis in Abaqus/Explicit. You can define the fluid particle velocity, acceleration, free surface elevation, and fluid pressure field in the user subroutine. The quantities required to define the wave kinematics can be specified as properties and passed into the user subroutine. For example, in the case of stochastic wave kinematics, any required seed variable and/or frequency-amplitude data pairs can be specified as properties. You can also declare and use state variables for user-defined wave calculations, which will be provided at the nodes and initialized to zero at the beginning of the step. You have to update the state variables within the user subroutine. For example, the state variables can be used to store any intermediate configuration of the structure that is used to describe a stochastic wave field. Input File Usage: Use the following option to specify the wave kinematics in user subroutine VWAVE: *WAVE, TYPE=USER Use the following option to specify properties available as a real-array argument PROPS of size NPROPS in user subroutine VWAVE: *WAVE, TYPE=USER, PROPERTIES=nprops prop_1, prop_2, ..., prop_8 ..., prop_nprops Use the following option to specify state variables available as a real-array argument STATEVAR of size NSTATEVAR in user subroutine VWAVE: *WAVE, TYPE=USER, DEPVAR=nstatevar Wave position as a function of time can be chosen by specifying the phase For Airy and Stokes waves the position of the wave at time angle of the wave (or wave components for Airy waves). By default, the waves are chosen such that they have a trough (vertical displacement of the fluid surface is a minimum) at the origin of the horizontal axes at time for the waves. A positive phase angle shifts the waves backward in their travel direction . . You can change this trough by introducing a phase angle The time t used in the wave theory is the total time in the analysis. Therefore, if the direct-integration dynamic steps in which Airy or Stokes waves are applied are preceded by any steps other than direct- integration dynamic steps (such as static steps), it is usually convenient to make the time period in these steps very small compared to the period of the wave. Because total time is used, the phase of the wave will be continuous from the end of one dynamic step to the beginning of the next dynamic step. Defining a minimum wave trough elevation For computational efficiency Abaqus/Aqua uses a minimum wave trough elevation below which the structure is assumed to be immersed. Below this elevation no calculation of the fluid surface need be done Vertical axis (Z-direction in 3-D cases, Y-direction in 2-D cases) Direction of wave travel H, wave height Wave of zero phase angle has a trough at the origin of the horizontal axis at time t=0. λ, wavelength Figure 6.11.1–1 Wave of zero phase angle. horizontal position to determine if the point of interest is above the instantaneous free surface. Similarly, a maximum wave elevation is used: any point above the maximum wave elevation is assumed to have no fluid loading. For Airy and Stokes waves the minimum and maximum wave elevations are calculated from the wave theory. For gridded waves Abaqus/Aqua allows the definition of a minimum wave trough elevation: in two-dimensional analysis. The structure is always assumed to in three-dimensional analysis or be immersed below this elevation. The maximum wave elevation is calculated as the still water elevation plus the difference between this elevation and the minimum wave trough elevation. If the minimum wave trough elevation is not specified for gridded waves, Abaqus/Aqua will compare the elevation of every point on the structure with the instantaneous fluid surface as defined by the gridded data. When defining this elevation, make sure that no wave trough ever drops below the minimum wave trough elevation specified. Input File Usage: *WAVE, TYPE=GRIDDED, DATA FILE=file_name, MINIMUM=elevation Wave kinematics, dynamic pressure, and extrapolation for Airy waves A spatial (Eulerian) description of the wave field is used for all wave types; therefore, a structural point’s coordinates are used to evaluate the wave kinematics. In geometrically nonlinear analysis the structural point’s coordinates are its current coordinates. In geometrically linear analysis the wave kinematics are evaluated using the structural point’s reference coordinates. In both geometrically linear and nonlinear analysis for both static and direct-integration dynamic procedures, submergence is calculated to the instantaneous water level at the current value of total time for the analysis. Fluid loading is applied only to those points on the structure below the instantaneous water level. When buoyancy loading is applied in conjunction with a gravity wave, the dynamic pressure due to the disturbance of the still surface is added to the hydrostatic pressure (measured to the still water level) to obtain the total buoyancy loading, except when the buoyancy loading described by a distributed or concentrated load definition overrides the fluid properties given for the Abaqus/Aqua analysis. Dynamic pressure is included for both static and dynamic procedures for Airy, Stokes, and gridded wave types; however, with gridded wave data you can choose to suppress this effect. See “Airy wave theory,” Section 6.2.2 of the Abaqus Theory Manual, and “Stokes wave theory,” Section 6.2.3 of the Abaqus Theory Manual, for a definition of dynamic pressure. Although the linearized Airy wave theory assumes that the fluid displacements are small with respect to the wavelength and the fluid depth, these displacements may not be small with respect to the dimensions of the structure immersed in the fluid. As a result of the linearizing approximations special treatment is necessary to calculate the wave kinematics for points below the instantaneous water level but above the still water line. Abaqus/Aqua uses extrapolation with Airy wave theory: the wave velocity, acceleration, and dynamic pressure for points above the still water level but below the instantaneous free surface are taken to be the values evaluated from the wave theory at the still water level. See “Airy wave theory,” Section 6.2.2 of the Abaqus Theory Manual, for more details. Reading the data that define gravity waves from an alternate file The data for the gravity wave can be contained in an alternate file. See “Input syntax rules,” Section 1.2.1, for the syntax of the file name. Input File Usage: *WAVE, INPUT=file_name Defining a wind velocity profile You can define a wind velocity profile. Wind loading is applied only to elements above the still water surface elevation (defined in the fluid properties). If an element is above the still water depth but is submerged due to a wave, the wind loading will still be applied. The wind profile is assumed to vary with height (the positive z-direction in three-dimensional models, the positive y-direction in two-dimensional models) according to the power law wind profile and has no variation in the horizontal plane. The power law wind velocity profile is given by where is the local wind velocity ( is a unit vector along the local x-axis of the wind field, and is a unit vector along the local y-axis of the wind field); is the time-varying wind velocity at the reference height, is a user-defined constant (default value 1/7); is the distance above the still water surface (i.e., , as described below; is the still water surface); and is the reference distance above the still water surface where the time variation of the wind velocity is given. The wind local system is defined by giving the direction cosines of the unit vector . Input File Usage: *WIND air density, , , , x-direction cosine for , y-direction cosine for , Prescribing the time variation of wind velocity at the reference height The variation in time of the wind profile is defined by reference height : , the wind velocity vector time history at a The wind velocity component time histories and are given by and are user-defined as described above (with default values of 1.0) and where are time-dependent functions defined by referring to amplitude curves from the concentrated or distributed load definitions used to apply the wind loading to the model. If no amplitude curve is referenced, the wind velocity components are the constant values and and . Geometrically linear versus geometrically nonlinear analysis In geometrically linear analysis wind velocities are calculated based on the original coordinates of the structure. In geometrically nonlinear analysis the current coordinates of a point on the structure are used to calculate the wind velocity at that point. Initial conditions Initial conditions can be applied to the structure in an Abaqus/Aqua analysis in the same way as in static and dynamic analyses without Aqua loads. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. Boundary conditions Boundary conditions can be applied to the structure in an Abaqus/Aqua analysis in the same way as in static and dynamic analyses without Aqua loads. See “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Defining contact at the seabed Aqua loads are applied only above the seabed. To model the bottom of the sea using a contact plane, the elevation of the contact plane must be slightly higher than the seabed level to avoid ambiguity between the contact condition and applied loading. If the contact plane is at the same level as the seabed, there is a risk that round-off problems will cause Aqua loads not to be applied to nodes in contact with the seabed. Loads Steady current, wave, and wind loads are applied to nodes or elements of the structure using concentrated and/or distributed load definitions. Wind loads are applied only if the point is currently above the still fluid surface; fluid loads are applied only if the point is currently below the instantaneous fluid surface and above the seabed. Distributed loads are applied to partly immersed elements. Concentrated and distributed load definitions cannot be used in eigenfrequency extraction steps, so the loads described below can be applied only in static and direct-integration dynamic steps. Controlling the time variation and magnitude of Aqua loading You have three ways to control the magnitude of an Aqua load as a function of time: 1. You can reference a user-defined amplitude curve (“Amplitude curves,” Section 33.1.2) from the concentrated or distributed load definition to scale the entire load. 2. You can specify a magnitude factor, M, for the concentrated or distributed load definition, which is used to scale all the load. This magnitude factor allows normalized amplitude curves to be defined and used for multiple loads. The default magnitude factor is always . 3. You can reference individual user-defined amplitude curves to scale different components of the loading separately. For example, steady current velocity and wave velocity can be scaled separately by referencing different amplitude curves. All of these scaling factors are cumulative. Buoyancy loads The calculated buoyancy of a structure depends on the orientation of the exposed surface area with respect to the vertical direction. This surface area is calculated automatically by Abaqus/Aqua for distributed buoyancy loading; however, you must specify the exposed area and direction cosines of the outward normal at a node for concentrated buoyancy loading. Abaqus/Aqua uses a closed-end loading condition while computing the distributed buoyancy forces on all line elements. To obtain an open-end loading condition, concentrated buoyancy loading can be used to counteract the buoyancy load applied to the ends of the elements. The buoyancy loads require the definition of fluid density, seabed and free surface elevation, and the gravitational constant. The default external fluid properties are defined for the model as described in “Defining the fluid properties.” You can override some of these properties by specifying them directly in the distributed or concentrated load definition. This provides for modeling situations where different parts of the structure are subjected to different buoyancy loads, such as a pipe inside another pipe where the static fluid surrounding the inner pipe is different from the fluid surrounding the outer pipe. Gravity waves (“Wave kinematics, dynamic pressure, and extrapolation for Airy waves”) do not affect the buoyancy loading when any external fluid property is overridden. Specifying distributed buoyancy loads To apply distributed buoyancy loads to elements immersed in a fluid, the effective outer diameter of beam, truss, and one-dimensional rigid elements must be specified. Provide the external fluid density, free surface elevation, and additional pressure to override the default fluid properties to model the situations described above. For situations where it is necessary to model the fluid inside an element, the effective inner diameter of the element must also be given, along with the density and free surface elevation of the fluid inside the element. Distributed buoyancy loading can be applied to rigid surface elements. However, the effects of waves are ignored for these elements; the buoyancy loading is calculated to the still water level only. For proper application of a positive buoyancy force, the positive normal of R3D3 and R3D4 elements must point into the fluid. Input File Usage: *DLOAD element number or set, PB, M, effective outer diameter, internal fluid density, effective inner diameter, internal free surface elevation, external fluid density, external free surface elevation, additional pressure Specifying concentrated buoyancy loads For concentrated buoyancy loads applied to nodes immersed in a fluid, the load is calculated based on the sum of the hydrostatic pressure (measured to the still water level) and the dynamic pressure due to wave action. The total pressure is multiplied by the exposed area associated with the node. The loading is automatically considered to be a follower force in geometrically nonlinear analysis (for elements that have rotational degrees of freedom); therefore, it is not necessary to specify that the load is a follower force. Provide the external fluid density, free surface elevation, and additional pressure to override the default fluid properties to model the situations described above. Input File Usage: *CLOAD node number or set, TSB, M, exposed area, local coordinate system data, external fluid density, external free surface elevation, additional pressure Drag loads Both waves and wind can cause drag loading on a structure. Fluid drag refers to drag caused by the structural member being immersed in the fluid defined by the fluid properties and the gravity waves and, thus, subject to steady current and wave loading. Fluid drag loading is provided by Morison’s equation. Fluid drag loads must be specified in terms of a normal (transverse) load and a tangential load. Wind drag is generated on the portions of a structure that are above the still fluid surface defined by the fluid properties because these portions are exposed to the user-defined wind velocity profile. Specifying distributed transverse fluid or wind drag loads Distributed transverse drag is defined as follows : where is the force per unit length, transverse to the member; is the current value of the amplitude curve referred to by the distributed load definition, multiplied by the user-defined magnitude factor, M; is the mass density of the fluid (given in the fluid properties) for fluid distributed drag or is the mass density of the air (given in the wind velocity profile) for wind distributed drag; is the drag coefficient; and is the effective outer diameter of the member. The relative fluid particle velocity in the normal direction, , is given by where is the fluid particle velocity ; is the velocity of this point on the structure (zero during static steps); is the structural velocity factor; and is the unit vector along the axis of the element. The effective outer diameter of the element, D; the drag coefficient, factor, distributed drag or wind distributed drag). ; and the structural velocity , must be defined in the distributed load definition together with the distributed load type (fluid The velocities due to steady current and waves can be scaled individually for fluid distributed drag by referring to different amplitude curves. Thus, the fluid particle velocity, , at any time is where is the current value of the first amplitude curve listed in the load definition or 1.0 if the amplitude reference is omitted, is the steady current velocity defined in the fluid properties, is the current value of the second amplitude curve listed in the load definition or 1.0 if the amplitude reference is omitted, and is the user-defined wave velocity. The wind velocity is defined in components relative to the local axes and defined for the wind velocity profile. Each velocity component can be scaled independently by referring to different amplitude curves. The total wind velocity at any time, , is and where components in the local x- and y-directions, respectively. The values of , the wind velocity profile; and z is the distance above the still fluid surface. are the amplitude references provided in the load definition for the velocity are defined by , and , Input File Usage: Use the following option to define fluid distributed drag: *DLOAD element number or set, FDD, M, D, , , , Use the following option to define wind distributed drag: *DLOAD element number or set, WDD, M, D, , , , Specifying distributed tangential fluid drag loads Distributed tangential fluid loading is a load in the tangential direction of an element due to skin friction. This type of loading is defined as follows : where is the force per unit length, tangent to the member; is the amplitude curve referred to by the distributed load definition, multiplied by the user- defined magnitude factor, M; is the mass density of the fluid (given in the fluid properties); is the tangential drag coefficient; is the effective outer diameter of the member; and is a constant (by default, , for quadratic dependence of force on velocity). The relative fluid particle velocity in the tangential direction, , is given by where is the fluid particle velocity (as defined above for distributed transverse fluid drag loading), is the velocity of this point on the structure (zero during static steps), is the structural velocity factor, and is the unit vector along the axis of the element. The effective outer diameter of the element, D; the drag coefficient, ; the structural velocity factor, ; and the exponent, h, must be defined in the distributed load definition together with the distributed load type (fluid drag tangential). As with distributed transverse fluid loading, the velocities due to steady current and waves ( and ) can be scaled individually by referring to different amplitude curves. Input File Usage: Use the following option to define fluid drag tangential: *DLOAD element number or set, FDT, M, D, , , h, , Specifying concentrated fluid or wind drag loads using a concentrated load definition Concentrated fluid or wind drag loading applies a load normal to the end of an element. Such loading is automatically considered to be a follower force in geometrically nonlinear analysis (for elements that have rotational degrees of freedom). The drag theory uses Morison’s equation . The drag force is nonzero when the net flow is in the opposite direction of the outward normal to the exposed area and is zero when the net flow is in the direction of the normal: drag where for for is the amplitude curve referenced by the concentrated load definition multiplied by the user- defined magnitude factor, M; is the mass density of the fluid (given in the fluid properties) for transition section fluid drag or is the mass density of the air (given in the wind velocity profile) for transition section wind drag; is the drag coefficient; is the exposed area; and is the relative velocity between the structural member and the fluid particle along is given by , where tangential fluid drag loading. and as defined above for distributed The exposed area, , must be defined in the concentrated load definition together with the concentrated load type (transition section fluid drag or transition section wind drag). ; and the structural velocity factor, ; the drag coefficient, As with distributed transverse fluid loading, the velocities due to steady current and waves ( ) and the velocity components of the wind in the and individually by referring to different amplitude curves. and directions ( and ) can be scaled Input File Usage: Use the following option to define transition section fluid drag: *CLOAD node number or set, TFD, M, , , , , Use the following option to define transition section wind drag: *CLOAD node number or set, TWD, M, , , , , Specifying concentrated fluid or wind drag loads using a distributed load definition You can apply concentrated fluid or wind drag loading on the ends of elements. These loads have the same effect as specifying a concentrated load at a node using a concentrated load definition with concentrated load type transition section fluid drag or transition section wind drag, except that the normal to the exposed area cannot be specified when a distributed load definition is used; the normal to the end of the element is defined by the tangent to the element. The load can be applied to the first end (node) of the element or to the second end (node 2 or 3, as appropriate) of the element. These loads are nonzero only when the net flow is in the opposite direction of the outward normal to the exposed area. The loading is exactly the same as that described for the concentrated fluid or wind drag loading applied with a concentrated load definition. The “distributed” form of the loading is provided for convenience. Input File Usage: Use the following option to define fluid drag on the first end of the element: *DLOAD element number or set, FD1, M, , C, , , Use the following option to define fluid drag on the second end of the element: *DLOAD element number or set, FD2, M, , C, , , Use the following option to define wind drag on the first end of the element: *DLOAD element number or set, WD1, M, , C, , , Use the following option to define wind drag on the second end of the element: *DLOAD element number or set, WD2, M, , C, , , Neglecting the wave’s contribution to drag and inertia loading during a step If the wave’s contribution to the drag and inertia loading should not be applied during a step, the concentrated or distributed load component definition must explicitly refer to an amplitude curve with a value of zero. This is the only way to prevent waves from contributing to the fluid velocities and accelerations used in the calculation of these concentrated or distributed load types. Fluid inertia loads (added-mass effects) Fluid inertia loading causes a structure to have increased inertial resistance to acceleration. This fluid “added-mass” effect is included automatically in a direct-integration dynamic step when fluid inertia loading is applied. Concentrated or distributed added mass must be defined to include the added-mass effect in an eigenfrequency extraction step. Specifying distributed fluid inertia loads in a direct-integration dynamic step Distributed fluid inertia loading is defined as follows : where is the force per unit length, transverse to the member, caused by fluid inertia; is the amplitude curve referred to by the distributed load definition multiplied by the user- defined magnitude factor, M; is the mass density of the fluid (given in the fluid properties); is the effective outer diameter of the member; is the transverse fluid inertia coefficient; is the transverse added-mass coefficient; is the transverse component of the fluid acceleration; and is the transverse component of the beam acceleration (zero during static steps). The effective outer diameter, D; transverse fluid inertia coefficient, coefficient, (distributed fluid inertia). ; and transverse added-mass , must be defined in the distributed load definition together with the distributed load type The fluid acceleration, scaled by the amplitude curve, , is calculated according to the user-defined gravity wave and is further , referred to by the distributed load definition. Input File Usage: Use the following option to define distributed fluid inertia in a dynamic step: *DLOAD element number or set, FI, M, D, , , Specifying distributed fluid inertia loads in an eigenfrequency extraction step The added mass contribution due to distributed fluid inertia loading is per unit length of the member in the directions transverse to the axis of the member only, where is the mass density of the fluid (given in the fluid properties), is the effective outer diameter of the member, and is the transverse added-mass coefficient. Input File Usage: *D ADDED MASS element number or set, FI, D, Specifying concentrated fluid inertia loads in a direct-integration dynamic step using a concentrated load definition Concentrated fluid inertia loading is automatically considered to be a follower force (for elements that have rotational degrees of freedom). The inertia term is calculated as a force in the current direction of the outward normal to the exposed surface area: where is the point force caused by fluid inertia; is the amplitude curve referenced by the concentrated load definition multiplied by the user- defined magnitude factor, M; is the mass density of the fluid (given in the fluid properties); is the tangential inertia coefficient; is the fluid acceleration shape factor (of dimension ); is the tangential added-mass coefficient; is the structural acceleration shape factor (of dimension ); is the fluid acceleration in the direction of the outward normal to the exposed surface; and is the structural acceleration in the direction of the outward normal to the exposed surface (zero during static steps). The tangential inertia coefficient, coefficient, ; and the structural acceleration shape factor, definition together with the concentrated load type (transition section inertia). ; the fluid acceleration shape factor, ; the tangential added-mass , are given in the concentrated load The fluid acceleration, scaled by the amplitude curve, , is calculated according to the user-defined gravity wave and is further , referred to by the concentrated load definition. Input File Usage: Use the following option to define transition section inertia in a dynamic step: *CLOAD node number or set, TSI, M, , , , , Specifying concentrated fluid inertia loads in a direct-integration dynamic step using a distributed load definition You can apply concentrated fluid inertia loading at the ends of elements. These loads have the same effect as specifying a concentrated fluid added-inertia loading using a concentrated load definition with concentrated load type transition section inertia, except that the normal to the exposed area cannot be specified when a distributed load definition is used; the normal to the end of the element is defined by the tangent to the element. The inertia loading can be applied to the first end (node) of the element or to the second end (node 2 or 3, as appropriate) of the element. The loading is exactly the same as that described for the concentrated fluid inertia loading applied with a concentrated load definition. The “distributed” form of the loading is provided for convenience. Input File Usage: Use the following option to define fluid inertia on the first end of the element in a dynamic step: *DLOAD element number or set, FI1, M, , , , , Use the following option to define fluid inertia on the second end of the element in a dynamic step: *DLOAD element number or set, FI2, M, , , , , Specifying concentrated fluid inertia effects in an eigenfrequency extraction step using a concentrated added mass definition The added mass contribution due to concentrated fluid inertia loading in an eigenfrequency extraction step is in the direction normal to the transition section area, where is the mass density of the fluid (given in the fluid properties), is the tangential added-mass coefficient, and is the structural acceleration shape factor (of dimension ). Input File Usage: *C ADDED MASS node number or set, TSI, direction cosines defining the outward normal of the exposed area , Specifying concentrated fluid inertia effects in an eigenfrequency extraction step using a distributed added mass definition You can apply concentrated fluid inertia effects at the ends of elements. These loads have the same effect as specifying concentrated fluid inertia effects using a concentrated added mass definition with concentrated load type transition section inertia, but in this case the normal to the exposed area cannot be specified; the normal to the end of the element is defined by the tangent to the element. The added mass can be applied to the first end (node) of the element or to the second end (node 2 or 3, as appropriate) of the element. The effect is exactly the same as that described for the concentrated fluid inertia effects applied with a concentrated added mass definition. The “distributed” form of the loading is provided for convenience. Input File Usage: Use the following option to define fluid inertia on the first end of the element in an eigenfrequency extraction step: *D ADDED MASS element number or set, FI1, , Use the following option to define fluid inertia on the second end of the element in an eigenfrequency extraction step: *D ADDED MASS element number or set, FI2, , Applying non-Aqua loads to the structure Concentrated and distributed load definitions can also be used to apply concentrated and distributed forces that are not associated with wind, waves, or steady current to the structure. See “Concentrated loads,” Section 33.4.2, and “Distributed loads,” Section 33.4.3. Predefined fields The following predefined fields can be specified for the structure (not the fluid) in an Abaqus/Aqua analysis, as described in “Predefined fields,” Section 33.6.1: • Temperatures of nodes in the structure can be specified. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature- dependent material properties, if any. • The values of user-defined field variables can be specified. These values affect only field-variable- dependent material properties, if any. Material options Any of the mechanical constitutive models in Abaqus can be used for modeling the structure in an Abaqus/Aqua analysis . Elements The fluid loads in an Abaqus/Aqua analysis cannot be applied to all element types. Only the beam, pipe, elbow, truss, and rigid beam elements in Abaqus/Standard and linear beam and pipe elements in Abaqus/Explicit can be used to subject a structure to general Abaqus/Aqua loading. The only load that can be applied to two-dimensional rigid surfaces (R3D3 and R3D4 elements) is hydrostatic buoyancy; and this loading can be applied only in Abaqus/Standard. Current, wave, and wind loading have no effect on rigid surfaces. Jack-up foundation analysis Abaqus/Standard provides element types JOINT2D and JOINT3D, which can be used to model elastic- plastic interaction between spud cans and the sea floor . Output In addition to the usual output variables available in Abaqus/Standard and in Abaqus/Explicit , element section output variable ESF1 can be used to request output of the effective axial force in a beam subjected to pressure loading . The velocities and accelerations of the fluid cannot be output. Input file template *HEADING … *AQUA Data lines defining the fluid properties and steady current velocity *WAVE, TYPE=wave theory Data lines defining gravity waves ** *STEP (, NLGEOM) Use the NLGEOM parameter to include nonlinear geometric effects *DYNAMIC (or *STATIC or *DYNAMIC, EXPLICIT) … *CLOAD Data lines defining concentrated buoyancy, fluid/wind drag, and fluid inertia loads *DLOAD Data lines defining distributed buoyancy, fluid/wind drag, and fluid inertia loads *END STEP ** *STEP The NLGEOM parameter must have been included in the previous step to obtain the natural frequencies of the prestressed structure *FREQUENCY … *C ADDED MASS Data lines to define concentrated added-mass effects *D ADDED MASS Data lines to define distributed added-mass effects *END STEP 6.12 Annealing • “Annealing procedure,” Section 6.12.1 6.12.1 ANNEALING PROCEDURE Products: Abaqus/Explicit Abaqus/CAE References • *ANNEAL • “Configuring an annealing procedure” Section 14.11.1 of the Abaqus/CAE User’s Manual, manual in “Configuring general analysis procedures,” in the online HTML version of this Overview The anneal procedure: • is used to anneal a structure by setting all appropriate state variables and velocities to zero; and • is intended only for metal plasticity and user-defined material models; it has no effect on other material models. The annealing process The anneal procedure is intended to simulate the relaxation of stresses and plastic strains that occurs as metals are heated to high temperatures. Physically, annealing is the process of heating a metal part to a high temperature to allow the microstructure to recrystallize, removing dislocations caused by cold working of the material. During the anneal procedure Abaqus/Explicit sets all appropriate state variables to zero. These variables include stresses, backstresses, plastic strains, and velocities. In the case of metal porous plasticity, the void volume fraction is also set to zero, such that the material becomes fully dense. There is no time scale in an annealing step; therefore, time does not advance. The annealing process occurs instantaneously. No data are required for the anneal procedure. Input File Usage: Abaqus/CAE Usage: *ANNEAL Step module: Create Step: General: Anneal Temperatures Thermal strains are set to zero, and the temperature at all nodes in the model will be set to a uniform temperature or will be maintained at the current temperature during the anneal procedure. By default, the temperature at all nodes is maintained at the current temperature. You can specify a different final temperature, . Input File Usage: Abaqus/CAE Usage: *ANNEAL, TEMPERATURE= Step module: Create Step: General: Anneal: Post-anneal reference temperature: Value Initial conditions The initial state for the anneal step is the state of the model at the end of the last explicit dynamic analysis step. Boundary conditions It is not appropriate to specify new boundary conditions or to modify boundary conditions in an anneal procedure; all boundary conditions in effect prior to this procedure will remain fixed. Loads It is not meaningful to specify loads in an anneal procedure. Predefined fields It is not meaningful to specify predefined fields in an anneal procedure. Material options The annealing procedure is intended only for metal plasticity models (“Classical metal plasticity,” Section 23.2.1) and user-defined materials modeled with user subroutines VFABRIC and VUMAT. The metal plasticity models in Abaqus/Explicit include Mises, Johnson-Cook, Hill, and metal porous plasticity. Abaqus/Explicit also allows annealing of elastic materials (“Linear elastic behavior,” Section 22.2.1), including isotropic, orthotropic, and anisotropic elasticity. The annealing procedure has no effect on other material models. Elements All of the elements that are available in Abaqus/Explicit can be used in an anneal procedure. The elements are listed in Part VI, “Elements.” Output There is no output associated with an anneal step. Input file template *HEADING … ** *STEP *DYNAMIC, EXPLICIT (,ADIABATIC) or *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT Data line to specify the time period of the step *BOUNDARY, AMPLITUDE=name Data lines to describe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD Data lines to specify loads *TEMPERATURE and/or *FIELD Data lines to specify values of predefined fields *END STEP ** *STEP *ANNEAL (,TEMPERATURE= ) *END STEP ** *STEP *DYNAMIC, EXPLICIT (,ADIABATIC) Data line to specify the time period of the step *BOUNDARY, AMPLITUDE=name Data lines to describe zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD and/or *DSLOAD Data lines to specify loads *TEMPERATURE and/or *FIELD Data lines to specify values of predefined fields *END STEP 7. Analysis Solution and Control Solving nonlinear problems Analysis convergence controls 7.1 7.1 Solving nonlinear problems • “Solving nonlinear problems,” Section 7.1.1 7.1.1 SOLVING NONLINEAR PROBLEMS Products: Abaqus/Standard Abaqus/CAE References • “Convergence and time integration criteria: overview,” Section 7.2.1 • “Commonly used control parameters,” Section 7.2.2 • “Convergence criteria for nonlinear problems,” Section 7.2.3 • “Time integration accuracy in transient problems,” Section 7.2.4 • “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Solving nonlinear problems in Abaqus/Standard involves: • a combination of incremental and iterative procedures; • using the Newton method to solve the nonlinear equations; • determining convergence; • defining loads as a function of time; and • choosing suitable time increments automatically. Some static problems may become unstable because of severe nonlinearity. Abaqus/Standard offers a set of automatic stabilization mechanisms to handle such problems. The solution of nonlinear problems The nonlinear load-displacement curve for a structure is shown in Figure 7.1.1–1. Load Displacement Figure 7.1.1–1 Nonlinear load-displacement curve. The objective of the analysis is to determine this response. In a nonlinear analysis the solution cannot be calculated by solving a single system of linear equations, as would be done in a linear problem. Instead, the solution is found by specifying the loading as a function of time and incrementing time to obtain the nonlinear response. Therefore, Abaqus/Standard breaks the simulation into a number of time increments and finds the approximate equilibrium configuration at the end of each time increment. Using the Newton method, it often takes Abaqus/Standard several iterations to determine an acceptable solution to each time increment. Steps, increments, and iterations • The time history for a simulation consists of one or more steps. You define the steps, which generally consist of an analysis procedure, loading, and output requests. Different loads, boundary conditions, analysis procedures, and output requests can be used in each step. For example: Step 1: Hold a plate between rigid jaws. Step 2: Add loads to deform the plate. Step 3: Find the natural frequencies of the deformed plate. • An increment is part of a step. In nonlinear analyses each step is broken into increments so that the nonlinear solution path can be followed. You suggest the size of the first increment, and Abaqus/Standard automatically chooses the size of the subsequent increments. At the end of each increment the structure is in (approximate) equilibrium and results are available for writing to the restart, data, results, or output database files. • An iteration is an attempt at finding an equilibrium solution in an increment. If the model is not in equilibrium at the end of the iteration, Abaqus/Standard tries another iteration. With every iteration the solution that Abaqus/Standard obtains should be closer to equilibrium; however, sometimes the iteration process may diverge—subsequent iterations may move away from the equilibrium state. In that case Abaqus/Standard may terminate the iteration process and attempt to find a solution with a smaller increment size. Convergence Consider the external forces, P, and the internal (nodal) forces, I, acting on a body and Figure 7.1.1–2(b), respectively). The internal loads acting on a node are caused by the stresses in the elements that are attached to that node. For the body to be in equilibrium, the net force acting at every node must be zero. Therefore, the basic statement of equilibrium is that the internal forces, I, and the external forces, P, must balance each other: The nonlinear response of a structure to a small load increment, Abaqus/Standard uses the structure’s tangent stiffness, , which is based on its configuration at , is shown in Figure 7.1.1–3. , and , the structure’s configuration to calculate a displacement correction, , for the structure. Using is updated to . Id Ia Ic Ib (a) External loads in a simulation. (b) Internal forces acting at a node. Figure 7.1.1–2 Internal and external loads on a body. Load Ra Ia ΔP K0 Ka ca u0 ua Displacement Figure 7.1.1–3 First iteration in an increment. Abaqus/Standard then calculates the structure’s internal forces, , in this updated configuration. The difference between the total applied load, P, and can now be calculated as where If is the force residual for the iteration. is zero at every degree of freedom in the model, point a in Figure 7.1.1–3 would lie on the load-deflection curve and the structure would be in equilibrium. In a nonlinear problem will never be exactly zero, so Abaqus/Standard compares it to a tolerance value. If is less than this force residual tolerance at all nodes, Abaqus/Standard accepts the solution as being in equilibrium. By default, this tolerance value is set to 0.5% of an average force in the structure, averaged over time. Abaqus/Standard automatically calculates this spatially and time-averaged force throughout the simulation. You can change this, and all other such tolerances, by specifying solution controls . If is less than the current tolerance value, P and are considered to be in equilibrium and is a valid equilibrium configuration for the structure under the applied load. However, before Abaqus/Standard accepts the solution, it also checks that the last displacement correction, , is small relative to the total incremental displacement, is greater than a fraction (1% by default) of the incremental displacement, Abaqus/Standard performs another iteration. Both convergence checks must be satisfied before a solution is said to have converged for that time increment. If the solution from an iteration is not converged, Abaqus/Standard performs another iteration to try to bring the internal and external forces into balance. First, Abaqus/Standard forms the new stiffness, . This stiffness, together with the residual , that brings the system closer to equilibrium (point , for the structure based on the updated configuration, , determines another displacement correction, . If b in Figure 7.1.1–4). Ia ΔP K0 u0 ua Ka Load Rb Ib Ia K0 cb ua ub Displacement Figure 7.1.1–4 Second iteration. Abaqus/Standard calculates a new force residual, . Again, the largest force residual at any degree of freedom, , using the internal forces from the structure’s new configuration, , is compared against the force residual tolerance, and the displacement correction for the second iteration, , is compared to the increment of displacement, . If necessary, Abaqus/Standard performs further iterations. For more details on convergence in Abaqus/Standard, see “Convergence criteria for nonlinear problems,” Section 7.2.3. For each iteration in a nonlinear analysis Abaqus/Standard forms the model’s stiffness matrix and solves a system of equations. Therefore, the computational cost of each iteration is close to the cost of conducting a complete linear analysis, making the computational expense of a nonlinear analysis potentially many times greater than the cost of a linear analysis. Since it is possible with Abaqus/Standard to save results at each converged increment, the amount of output data available from a nonlinear simulation can also be much greater than that available from a linear analysis of the same geometry. Automatic incrementation control By default, Abaqus/Standard automatically adjusts the size of the time increments to solve nonlinear problems efficiently. You need to suggest only the size of the first increment in each step of the simulation, after which Abaqus/Standard automatically adjusts the size of the increments. If you do not provide a suggested initial increment size, Abaqus/Standard will attempt to apply all of the loads defined in the step in a single increment. For highly nonlinear problems Abaqus/Standard will have to reduce the increment size repeatedly to obtain a solution, resulting in wasted CPU time. It is advantageous to provide a reasonable initial increment size because only in mildly nonlinear problems can all of the loads in a step be applied in a single increment. The number of iterations needed to find a converged solution for a time increment will vary depending on the degree of nonlinearity in the system. With the default incrementation control, the procedure works as follows. If the solution has not converged within 16 iterations or if the solution appears to diverge, Abaqus/Standard abandons the increment and starts again with the increment size set to 25% of its previous value. It then attempts to find a converged solution with this smaller time increment. If the solution still fails to converge, Abaqus/Standard reduces the increment size again. This process is continued until a solution is found. If the time increment becomes smaller than the minimum you defined or more than 5 attempts are needed, Abaqus/Standard stops the analysis. If the increment converges in fewer than 5 iterations, this indicates that the solution is being found fairly easily. Therefore, Abaqus/Standard automatically increases the increment size by 50% if 2 consecutive increments require fewer than 5 iterations to obtain a converged solution. While the default automatic incrementation control is suitable for most analyses, you can change all the defaults when necessary by specifying solution controls; see “Commonly used control parameters,” Section 7.2.2, and “Time integration accuracy in transient problems,” Section 7.2.4. Automatic stabilization of unstable problems Nonlinear static problems can be unstable. Such instabilities may be of a geometrical nature, such as buckling, or of a material nature, such as material softening. If the instability manifests itself in a global load-displacement response with a negative stiffness, the problem can be treated as a buckling or collapse problem as described in “Unstable collapse and postbuckling analysis,” Section 6.2.4. However, if the instability is localized, there will be a local transfer of strain energy from one part of the model to neighboring parts, and global solution methods may not work. This class of problems has to be solved either dynamically or with the aid of (artificial) damping; for example, by using dashpots. Abaqus/Standard provides an automatic mechanism for stabilizing unstable quasi-static problems through the automatic addition of volume-proportional damping to the model. The applied damping factors can be constant over the duration of a step, or they can vary with time to account for changes over the course of a step. The latter, adaptive approach is typically preferred. Automatic stabilization of static problems with a constant damping factor Automatic stabilization with a constant damping factor is triggered by including automatic stabilization in any nonlinear quasi-static procedure. Viscous forces of the form are added to the global equilibrium equations is an artificial mass matrix calculated with unity density, c is a damping factor, where is the vector of nodal velocities, and meaning in the context of the problem being solved). is the increment of time (which may or may not have a physical For the case of static stabilization the mass matrix for Timoshenko beams is always calculated assuming isotropic rotary inertia, regardless of the type of rotary inertia specified for the beam section definition (“Rotary inertia for Timoshenko beams” in “Beam section behavior,” Section 29.3.5). Automatic stabilization does not carry over automatically to subsequent steps. It needs to be declared for any step in which you want it to be active. Abaqus/Standard recalculates new values for the damping factor, based on the declared damping intensity and on the solution of the first increment of the step. Therefore, unless you specify the same damping factor directly , an analysis with an unstable step may produce slightly different results from the same analysis with the original step split into two steps. Moreover, if the instabilities in the model have not subsided by the end of a step, viscous forces may be terminated abruptly or modified at the beginning of subsequent steps, potentially causing convergence difficulties if automatic stabilization is not used in the subsequent step. If such a situation arises, it is recommended that the problem be restarted with the damping factor set equal to the value chosen by Abaqus/Standard (or to the value you specified) in the previous step. This value is printed in the message (.msg) file for the previous step. If it is necessary to have an accurate static equilibrium solution after an instability has occurred (and the model’s behavior has returned to a stable regime), the step with automatic stabilization can be followed by a step without such stabilization. Calculating the damping factor based on the dissipated energy fraction It is assumed that the problem is stable at the beginning of the step and that instabilities may develop in the course of the step. While the model is stable, viscous forces and, therefore, the viscous energy dissipated are very small. Thus, the additional artificial damping has no effect. If a local region goes unstable, the local velocities increase and, consequently, part of the strain energy then released is dissipated by the applied damping. Abaqus/Standard can, if necessary, reduce the time increment to permit the process to occur without the unstable response causing very large displacements. Abaqus/Standard calculates and prints to the message file the damping factor, c, based on the solution of the first increment of a step. In most applications the first increment of the step is stable without the need to apply damping. The damping factor is then determined in such a way that the dissipated energy for a given increment with characteristics similar to the first increment is a small fraction of the extrapolated strain energy. The fraction is called the dissipated energy fraction and has a default value of 2.0 × 10−4 . If the default value for the dissipated energy fraction is used, the adaptive automatic stabilization scheme discussed in the next section will be activated automatically by default in the step. Alternatively, you can specify the non-default dissipated energy fraction for automatic stabilization directly. Input File Usage: Abaqus/CAE Usage: Use any of the following options to specify a nondefault dissipated energy fraction: *COUPLED TEMPERATURE-DISPLACEMENT, STABILIZE=dissipated energy fraction *SOILS, STABILIZE=dissipated energy fraction *STATIC, STABILIZE=dissipated energy fraction *STEADY STATE TRANSPORT, STABILIZE=dissipated energy fraction *VISCO, STABILIZE=dissipated energy fraction Step module: Create Step: General: any valid step type: Basic: select Specify dissipated energy fraction from the Automatic stabilization field Considerations when the first increment is unstable or singular There are cases where the first increment is either unstable or singular (due to a rigid body mode). In such cases it is not possible to obtain a solution to the first increment without applying some damping. Therefore, some damping is already applied during the first increment. The damping factor used for the initial increment is chosen such that the average element damping matrix component, divided by the step time, is equal to the average element stiffness matrix component multiplied by the dissipated energy fraction. If the calculated strain energy change in this increment indicates that the solution without damping is stable, the damping factor is recalculated based upon the energy method described previously. However, if the strain energy change indicates that the solution is unstable or singular, the initially calculated damping factor is maintained, and a warning message is issued indicating that the amount of damping applied may not be appropriate. In many cases the amount of damping may actually be rather large, which can affect the solution in ways that are not desirable. Therefore, if the above mentioned warning message is issued, check the viscous forces (VF) and compare them with the expected nodal forces to make sure that the viscous forces do not dominate the solution. If necessary, follow the stabilized step with another step in which stabilization is not used or with a step in which a much smaller damping factor is used. Directly specifying the damping factor You can also specify the damping factor directly. Unfortunately, it is generally quite difficult to make a reasonable estimate for the damping factor unless a value is known from the output of previous runs; the damping factor depends not only on the amount of damping but also on mesh size and material behavior. Input File Usage: Use any of the following options to specify the damping factor directly: *COUPLED TEMPERATURE-DISPLACEMENT, STABILIZE, FACTOR=damping factor *SOILS, STABILIZE, FACTOR=damping factor Abaqus/CAE Usage: *STATIC, STABILIZE, FACTOR=damping factor *STEADY STATE TRANSPORT, STABILIZE, FACTOR=damping factor *VISCO, STABILIZE, FACTOR=damping factor Step module: Create Step: General: Coupled temp-displacement, Soils, Static, General, or Visco: Basic: select Specify damping factor from the Automatic stabilization field Adaptive automatic stabilization scheme As discussed above, the automatic stabilization scheme with a constant damping factor typically works well to subside instabilities and to eliminate rigid body modes without having a major effect on the solution. However, there is no guarantee that the value of the damping factor is optimal or even suitable in some cases. This is particularly true for thin shell models, in which the damping factor may be too high when a poor estimation of the extrapolated strain energy is made during the first increment. For such models you may have to increase the damping factor if the convergence behavior is problematic or to decrease the damping factor if it distorts the solution. The former case would require you to rerun the analysis with a larger damping factor, while the latter case would require you to perform post-analysis comparison of the energy dissipated by viscous damping (ALLSD) to the total strain energy (ALLIE). Therefore, obtaining an optimal value for the damping factor is a manual process requiring trial and error until a converged solution is obtained and the dissipated stabilization energy is sufficiently small. The adaptive automatic stabilization scheme, in which the damping factor can vary spatially and with time, provides an effective alternative approach. In this case the damping factor is controlled by the convergence history and the ratio of the energy dissipated by viscous damping to the total strain energy. If the convergence behavior is problematic because of instabilities or rigid body modes, Abaqus/Standard automatically increases the damping factor. For example, the damping factor may increase if an analysis takes extra severe discontinuity or equilibrium iterations per increment or requires time increment cutbacks. On the other hand, Abaqus/Standard may reduce the damping factor automatically if instabilities and rigid body modes subside. The ratio of the energy dissipated by viscous damping to the total strain energy is limited by an accuracy tolerance that you specify. Such an accuracy tolerance is imposed on the global level for the whole model. If the ratio of the energy dissipated by viscous damping to the total strain energy for the whole model exceeds the accuracy tolerance, the damping factor at each individual element is adjusted to ensure that the ratio of the stabilization energy to the strain energy is less than the accuracy tolerance on both the global and local element level. The stabilization energy always increases, while the strain energy may decrease. Therefore, Abaqus/Standard restricts the ratio of the incremental value of the stabilization energy to the incremental value of the strain energy for each increment to ensure that this value has not exceeded the accuracy tolerance if the ratio of the total stabilization energy to the total strain energy exceeds the accuracy tolerance. The accuracy tolerance is a targeted value and can be exceeded in some situations, such as when there is rigid body motion or when significant non-local instability occurs. The default accuracy tolerance used by the adaptive automatic stabilization scheme is 0.05. The default tolerance is suitable for most applications, but you have the option of specifying a nondefault accuracy tolerance if necessary. If the accuracy tolerance is set equal to zero, the adaptive automatic stabilization scheme is not activated and the automatic stabilization scheme with a constant damping factor will be used in the step. If the accuracy tolerance is not specified but the dissipated energy fraction with the default value of 2.0 × 10−4 is used, the adaptive automatic damping algorithm will be activated automatically with an accuracy tolerance of 0.05. Input File Usage: Use any of the following options to activate adaptive automatic stabilization with the default stabilization energy tolerance: *COUPLED TEMPERATURE-DISPLACEMENT, STABILIZE *SOILS, STABILIZE *STATIC, STABILIZE *STEADY STATE TRANSPORT, STABILIZE *VISCO, STABILIZE Use any of the following options to activate adaptive automatic stabilization with a nondefault stabilization energy tolerance: *COUPLED TEMPERATURE-DISPLACEMENT, STABILIZE, ALLSDTOL=accuracy tolerance *SOILS, STABILIZE, ALLSDTOL=accuracy tolerance *STATIC, STABILIZE, ALLSDTOL=accuracy tolerance *STEADY STATE TRANSPORT, STABILIZE, ALLSDTOL=accuracy tolerance *VISCO, STABILIZE, ALLSDTOL=accuracy tolerance Step module: Create Step: General: Coupled temp-displacement, Soils, Static, General, or Visco: Basic: select an Automatic stabilization method: toggle on Use adaptive stabilization with max. ratio of stabilization to strain energy: accuracy tolerance Abaqus/CAE Usage: Default value of the initial damping factor By default, the initial value of the damping factor is typically equal to the value that would be used for automatic stabilization with a constant damping factor . In some cases additional factors that are considered with adaptive automatic stabilization cause some differences in the initial damping factor. Specifying the initial damping factor directly Alternatively, you can specify the initial damping factor directly. The damping factor is adjusted based on the convergence history and the accuracy tolerance through the step. Input File Usage: Use any of the following options to specify the initial damping factor directly with the default stabilization energy tolerance: *COUPLED TEMPERATURE-DISPLACEMENT, STABILIZE, FACTOR=damping factor, ALLSDTOL *SOILS, STABILIZE, FACTOR=damping factor, ALLSDTOL Abaqus/CAE Usage: *STATIC, STABILIZE, FACTOR=damping factor, ALLSDTOL *STEADY STATE TRANSPORT, STABILIZE, FACTOR=damping factor, ALLSDTOL *VISCO, STABILIZE, FACTOR=damping factor, ALLSDTOL Step module: Create Step: General: Coupled temp-displacement, Soils, Static, General, or Visco: Basic: from the Automatic stabilization field, select Specify damping factor: damping factor: toggle on Use adaptive stabilization with max. ratio of stabilization to strain energy: maximum ratio Propagating the damping factors from the immediately preceding general step into the current step Adaptive automatic stabilization provides an option to propagate the damping factors from the immediately preceding general step to the subsequent steps. The default is to not propagate the damping factors from the results of the preceding general step. In this case Abaqus recalculates the initial damping factors based on the declared dissipated energy faction and on the solution of the first increment of the step, or you can specify the initial damping factors directly. Input File Usage: Use any of the following options to indicate that the damping factors in the current step are propagated from the immediately preceding general step: *COUPLED TEMPERATURE-DISPLACEMENT, STABILIZE, ALLSDTOL, CONTINUE=YES *SOILS, STABILIZE, ALLSDTOL, CONTINUE=YES *STATIC, STABILIZE, ALLSDTOL, CONTINUE=YES *STEADY STATE TRANSPORT, STABILIZE, ALLSDTOL, CONTINUE=YES *VISCO, STABILIZE, ALLSDTOL, CONTINUE=YES Step module: Create Step: General: Coupled temp-displacement, Soils, Static, General, or Visco: Basic: select Use damping factors from previous general step from the Automatic stabilization field: Use adaptive stabilization with max. ratio of stabilization to strain energy: accuracy tolerance Abaqus/CAE Usage: Ensuring that an accurate solution is obtained with automatic stabilization Whenever automatic stabilization is applied to a problem, check the following to ensure that accurate solutions are obtained: • For a damping factor calculated using the dissipated energy fraction, check the factor printed to the message (.msg) file at the end of the first increment to ensure that a reasonable amount of damping is applied. Unfortunately, the damping factor is problem dependent; therefore, you must rely on experience from previous runs. • Compare the viscous forces (VF) with the overall forces in the analysis, and ensure that the viscous forces are relatively small compared with the overall forces in the model. • Compare the viscous damping energy (ALLSD) with the total strain energy (ALLIE), and ensure that the ratio does not exceed the dissipated energy fraction or any reasonable amount. The viscous damping energy may be large if the structure undergoes a large amount of motion. The automated procedure of computing damping factors works well for many applications. However, there are cases where the computed damping factor is either too small, thus not controlling the instability, or too high, thus leading to inaccurate results. These problems are more likely to occur when using a constant damping factor—the damping factor is computed in the first increment, which may not be representative of behavior in the rest of the step. For example, consider a sequentially coupled thermal- stress analysis in which a mechanical analysis reads temperatures from a previous transient thermal analysis. Typically the thermal analysis exhibits a diffusive process, where rapid changes in temperature occurs early in the analysis and minor changes in temperature occur once steady state is reached. In such a case Abaqus will compute the extrapolated strain energy based on the temperatures corresponding to the time of the first increment (in this case there may be a significant change in temperature for the first increment), thus yielding a larger then expected extrapolated strain energy. This in turn leads to a damping factor that is too large, resulting in inaccurate results. If one of the automatic stabilization methods is not working appropriately, you can try using the other automatic stabilization method; the adaptive stabilization scheme is generally preferred. Alternatively, you can try directly specifying the damping factor. 7.2 Analysis convergence controls • “Convergence and time integration criteria: overview,” Section 7.2.1 • “Commonly used control parameters,” Section 7.2.2 • “Convergence criteria for nonlinear problems,” Section 7.2.3 • “Time integration accuracy in transient problems,” Section 7.2.4 7.2.1 CONVERGENCE AND TIME INTEGRATION CRITERIA: OVERVIEW Numerous control parameters are associated with the convergence and integration accuracy algorithms in Abaqus/Standard. These parameters are assigned default values that are chosen to optimize the accuracy and efficiency of the solution for a wide spectrum of nonlinear problems. You can change the solution control parameters, as described in the following sections: • A brief synopsis of the more important solution control parameters, together with a description of the circumstances in which they can be used effectively, is provided in “Commonly used control parameters,” Section 7.2.2. This section is likely to be the most useful for the general user and should be read first. • Abaqus/Standard incorporates an empirical algorithm designed to solve the equilibrium equations of nonlinear systems accurately and economically. The criteria used to establish convergence of nonlinear increments and the automatic adjustment of increment size based on the convergence rate are described in “Convergence criteria for nonlinear problems,” Section 7.2.3. • Abaqus/Standard allows you to choose “time integration accuracy parameters” in problems that have a physical time scale. The algorithms that use these parameters for automatically controlling time increment sizes are described in “Time integration accuracy in transient problems,” Section 7.2.4. • Abaqus/CFD allows you to choose the control parameters used in an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation to alleviate instability and mesh distortion during the analysis. Modifying the default solution controls The default values for the solution control parameters need not be adjusted for most cases. You can reset them, however, within a step definition. Values given for the solution control parameters remain in effect for the remainder of the analysis or until they are reset. Input File Usage: *CONTROLS The *CONTROLS option can be repeated, parameters. if necessary, with different Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify Resetting all default solution controls You can restore all solution control parameters to their default values. Input File Usage: Abaqus/CAE Usage: *CONTROLS, RESET Step module: Other→General Solution Controls→Edit: toggle on Reset all parameters to their system-defined defaults 7.2.2 COMMONLY USED CONTROL PARAMETERS Products: Abaqus/Standard Abaqus/CFD Abaqus/CAE References • “Convergence and time integration criteria: overview,” Section 7.2.1 • *CONTROLS • “Customizing general solution controls,” Section 14.15.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Solution control parameters can be used to control: • nonlinear equation solution accuracy; • time increment adjustment; and • FSI stabilization and mesh distortion in an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation. These solution control parameters need not be changed for most analyses. In difficult cases, however, the solution procedure may not converge with the default controls or may use an excessive number of increments and iterations. After it has been established that such problems are not due to modeling errors, it may be useful to change certain control parameters. This section presents a brief synopsis of the more important solution control parameters, together with a description of the circumstances in which they can be used effectively. Values given for the solution control parameters remain in effect for the remainder of the analysis or until they are reset. You can restore all solution control parameters to their default values . Terminology In this section the word “flux” means the variable whose discretized equilibrium is being sought and for which the equilibrium equations may be nonlinear: force, moment, heat flux, concentration volumetric flux, or pore liquid volumetric flux. The word “field” refers to the basic variables of the system, such as the components of the displacement in a continuum stress analysis or temperature in a heat transfer analysis. The superscript refers to one such type of equation. The fields and corresponding fluxes available in Abaqus/Standard are listed in “Convergence criteria for nonlinear problems,” Section 7.2.3. Defining tolerances for field equations Solution control parameters can be used to define tolerances for field equations. You can select the type of equation for which the solution control parameters are being defined, as shown in Table 7.2.2–1. The default tolerances can be reset if the analysis does not require high accuracy in the convergence criteria. Table 7.2.2–1 Selecting the field equation. Equilibrium equation Input file Abaqus/CAE All active fields FIELD=GLOBAL Apply to all applicable fields Force and bimoment FIELD=DISPLACEMENT Displacement Moment Heat transfer Hydrostatic fluid Pore fluid pressure FIELD=ROTATION Rotation FIELD=TEMPERATURE Temperature 11, 12, 13, ... FIELD=HYDROSTATIC FLUID PRESSURE Hydrostatic Fluid Pressure FIELD=PORE FLUID PRESSURE Pore Fluid Pressure Mass diffusion FIELD=CONCENTRATION Concentration Electrical conduction FIELD=ELECTRICAL POTENTIAL Electrical Potential FIELD=MATERIAL FLOW Unsupported DOF all 1, 2, 3, 7 4, 5, 6 11 10 FIELD=PRESSURE LAGRANGE MULTIPLIER Unsupported N/A FIELD=VOLUMETRIC LAGRANGE MULTIPLIER Unsupported N/A 7.2.2–2 Mechanism analysis (connector elements with material flow degree of freedom) Analysis containing C3D4H elements (all materials, except compressible hyperelastic elastomers and elastomeric foams). Analysis containing C3D4H elements with compressible hyperelastic The most significant solution control parameters for field equation tolerances— , , and —may have to be modified in cases where the residuals are large relative to the fluxes or in cases , where the incremental solution is essentially zero. Input File Usage: Abaqus/CAE Usage: *CONTROLS, PARAMETERS=FIELD, FIELD=field Step module: Other→General Solution Controls→Edit: toggle on Specify: Field Equations: Apply to all applicable fields or Specify individual fields: field Modifying the residual control is the convergence criterion for the ratio of the largest residual to the corresponding average flux norm, is defined in “Convergence criteria for nonlinear problems,” Section 7.2.3. The , for convergence. = 5 × 10−3, which is rather strict by engineering standards but in all but exceptional default value is cases will guarantee an accurate solution to complex nonlinear problems. The value for this ratio can be increased to a larger number if some accuracy can be sacrificed for computational speed. Modifying the solution correction control is the convergence criterion for the ratio of the largest solution correction to the largest corresponding = 10−2. In addition to sufficiently small residuals, incremental solution value. The default value is Abaqus/Standard requires that the largest correction to the solution value be small in comparison to the largest corresponding incremental solution value. Some analyses may not require such accuracy, thus permitting this ratio to be increased. Specifying the average flux is the value of average flux used by Abaqus/Standard for checking residuals. The default value is the time average flux calculated by Abaqus/Standard, as defined in “Convergence criteria for nonlinear problems,” Section 7.2.3. You may, however, define a constant value, , for the average flux, in which case throughout the step. You may wish to use absolute tolerances for your residual checks. The absolute tolerance value is . To avoid testing the magnitude of the , and the ratio then equal to the product of the average flux, solution correction, you can set to 1.0. Modifying the initial time average flux is the initial value of the time average flux for the current step. The default value is the time average flux from the previous step or 10−2 if this is Step 1. Redefining is sometimes helpful when a coupled problem is analyzed and some of the fields in the problem are not active in the first step; for example, if a static step is carried out before a fully coupled thermal-stress step. Redefinition of can also be useful if the first step is essentially a null step; for example, in a contact problem before any contact occurs, the initial fluxes (forces) generated are zero. In such cases should be given as a typical flux magnitude that will occur when field first becomes active. The initial value of is retained until an iteration is completed for which time we redefine criteria for nonlinear problems,” Section 7.2.3). . The criterion for zero flux compared to is If you specify the average flux, , directly, the value given for is ignored. , at which and message (.msg) files. Nondefault controls are marked by ***. For example, specifying the following controls: Field Equation Displacement Rotation 0.01 0.02 1.0 2.0 10.0 20.0 – 2.E3 – – 1.E−4 – would result in the following output: CONVERGENCE TOLERANCE PARAMETERS FOR FORCE *** CRIT. FOR RESIDUAL FORCE FOR A NONLINEAR PROBLEM *** CRITERION FOR DISP. CORRECTION IN A NONLINEAR PROBLEM *** INITIAL VALUE OF TIME AVERAGE FORCE AVERAGE FORCE IS TIME AVERAGE FORCE ALT. CRIT. FOR RESIDUAL FORCE FOR A NONLINEAR PROBLEM *** CRIT. FOR ZERO FORCE RELATIVE TO TIME AVRG. FORCE CRIT. FOR DISP. CORRECTION WHEN THERE IS ZERO FLUX CRIT. FOR RESIDUAL FORCE WHEN THERE IS ZERO FLUX FIELD CONVERSION RATIO CONVERGENCE TOLERANCE PARAMETERS FOR MOMENT *** CRIT. FOR RESIDUAL MOMENT FOR A NONLINEAR PROBLEM *** CRIT. FOR ROTATION CORRECTION IN A NONLINEAR PROBLEM *** INITIAL VALUE OF TIME AVERAGE MOMENT *** USER DEFINED VALUE OF AVERAGE MOMENT NORM ALT. CRIT. FOR RESID. MOMENT FOR A NONLINEAR PROBLEM CRIT. FOR ZERO MOMENT RELATIVE TO TIME AVRG. MOMENT CRIT. FOR ROTATION CORRECTION WHEN ZERO FLUX CRIT. FOR RESIDUAL MOMENT WHEN ZERO FLUX FIELD CONVERSION RATIO 1.000E-02 1.00 10.0 2.000E-02 1.000E-04 1.000E-03 1.000E-08 1.00 2.000E-02 2.00 20.0 2.000E+03 2.000E-02 1.000E-05 1.000E-03 1.000E-08 1.00 Controlling the time incrementation scheme Solution control parameters can be used to alter both the convergence control algorithm and the time incrementation scheme. The time incrementation parameters are the most significant since they have a direct effect on convergence. They may have to be modified if convergence is (initially) nonmonotonic or if convergence is nonquadratic. and Nonmonotonic convergence may occur if various nonlinearities interact; the combination of friction, nonlinear material behavior, and geometric nonlinearity may lead to nonmonotonically decreasing residuals. for example, Nonquadratic convergence will occur if the Jacobian is not exact, which may occur for complex material models. It may also occur if the Jacobian is nonsymmetric but the symmetric equation solver is used. In that case the unsymmetric equation solver should be specified for the step . Input File Usage: Abaqus/CAE Usage: *CONTROLS, PARAMETERS=TIME INCREMENTATION Step module: Other→General Solution Controls→Edit: toggle on Specify: Time Incrementation Specifying the equilibrium iteration for a residual check is the number of equilibrium iterations after which the check is made that the residuals are not If the initial convergence is increasing in two consecutive iterations. The default value is nonmonotonic, it may be necessary to increase this value. . Specifying the equilibrium iteration for a logarithmic rate of convergence check is the number of equilibrium iterations after which the logarithmic rate of convergence check begins. The default value is . In cases where convergence is nonquadratic and this cannot be corrected by using the unsymmetric equation solver for the step, the logarithmic convergence check should be eliminated by setting this parameter to a high value. Avoiding premature cutbacks in difficult analyses . For example, in a difficult analysis involving both Sometimes it is useful to increase both friction and the concrete material model, it may be helpful to set to avoid premature cutbacks of the time increment. These two parameters can be raised to more appropriate values for severely discontinuous problems by increasing them individually. and and Automatically setting the time incrementation parameters . In this You can automatically set the parameters described above to the values case any values that you specified previously for are specified multiple times in a step with different solution control settings, the last definition will be used. *CONTROLS, ANALYSIS=DISCONTINUOUS Step module: Other→General Solution Controls→Edit: toggle on Specify: Time Incrementation: Discontinuous analysis are overridden. However, if Abaqus/CAE Usage: Input File Usage: and and and Improving solution efficiency in a problem that involves a high coefficient of friction The solution efficiency can sometimes be improved in an analysis that involves a high coefficient of friction by automatically setting the time incrementation parameters and using the unsymmetric equation solver. Abaqus/Standard output The controls in effect for an analysis are listed in the data (.dat) and message (.msg) files. Nondefault controls are marked by **. For example, specifying the time incrementation parameters =7 and =10 would result in the following output: TIME INCREMENTATION CONTROL PARAMETERS: *** FIRST EQUIL. ITERATION FOR CONSECUTIVE DIVERGENCE CHECK *** EQUIL. ITER. AT WHICH LOG. CONVERGENCE RATE CHECK BEGINS EQUIL. ITER. AFTER WHICH ALTERNATE RESIDUAL IS USED MAXIMUM EQUILIBRIUM ITERATIONS ALLOWED EQUIL. ITERATION COUNT FOR CUT-BACK IN NEXT INCREMENT MAX EQUIL. ITERS IN TWO INCREMENTS FOR TIME INC. INCREASE MAXIMUM ITERATIONS FOR SEVERE DISCONTINUITIES MAXIMUM CUT-BACKS ALLOWED IN AN INCREMENT MAX DISCON. ITERS IN TWO INCS FOR TIME INC. INCREASE CUT-BACK FACTOR AFTER DIVERGENCE CUT-BACK FACTOR FOR TOO SLOW CONVERGENCE CUT-BACK FACTOR AFTER TOO MANY EQUILIBRIUM ITERATIONS 10 16 10 12 0.250 0.500 0.750 Activating the “line search” algorithm In strongly nonlinear problems the Newton algorithms used in Abaqus/Standard may sometimes diverge during equilibrium iteration. The line search algorithm (discussed in “Improving the efficiency of the solution by using the line search algorithm” in “Convergence criteria for nonlinear problems,” Section 7.2.3) detects these situations automatically and applies a scale factor to the computed solution correction, which helps to prevent divergence. The line search algorithm is particularly useful when the quasi-Newton method is used. By default, the line search algorithm is enabled only during steps where the quasi-Newton method , to a reasonable value (such as 5) to is used. Set the maximum number of line search iterations, activate the line search procedure or to zero to forcibly deactivate the line search. Input File Usage: *CONTROLS, PARAMETERS=LINE SEARCH Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Line Search Control: Defining tolerances for constraint equations Solution control parameters can be used to set tolerances for constraint equations. You can set strain compatibility tolerances for hybrid elements, displacement and rotation compatibility tolerances for distributing coupling constraints (specified as surface-based constraints or using DCOUP2D/DCOUP3D elements), and compatibility tolerances for softened contact. See “Convergence criteria for nonlinear problems,” Section 7.2.3, for details. Controlling the solution accuracy in direct cyclic analysis Solution control parameters can be used in direct cyclic analysis to specify when to impose the periodicity conditions and to set tolerances for stabilized state and plastic ratchetting detections. Input File Usage: *CONTROLS, TYPE=DIRECT CYCLIC , , , , Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Direct Cyclic: , , , , Imposing the periodicity condition You can specify the iteration number at which the periodicity condition is first imposed, value is of an analysis. This solution control parameter rarely needs to be reset from its default value. . The default = 1, in which case the periodicity condition is imposed for all iterations from the beginning Defining tolerances for stabilized state and plastic ratchetting detections You can specify the stabilized state detection criteria, is the maximum allowable ratio of the largest residual coefficient on any terms in the Fourier series to the corresponding average flux norm, and is the maximum allowable ratio of the largest correction to the displacement coefficient on any terms in the Fourier series to the largest displacement coefficient. The default values are = 5 × 10−3 and satisfied. = 5 × 10−3 . The solution converges to a stabilized state if both these criteria are and . If plastic ratchetting occurs, the shape of the stress-strain curves remains unchanged but the mean value of the plastic strain over a cycle continues to shift from one iteration to the next. In that case it is desirable to use separate tolerances for the constant term in the Fourier series to detect the plastic ratchetting. You can also specify the plastic ratchetting detection criteria, is the maximum allowable ratio of the largest residual coefficient on the constant term in the Fourier series to the corresponding average flux norm, and is the maximum allowable ratio of the largest correction to the displacement coefficient on the constant term in the Fourier series to the largest displacement = 5 × 10−3 . Plastic ratchetting is expected coefficient. The default values are if the residual coefficients and the corrections to the displacement coefficients on any of the periodic terms are within the tolerances set by , respectively, but the maximum residual coefficient on the constant term and the maximum correction to the displacement coefficient on the constant term exceed the tolerances set by , respectively. = 5 × 10−3 and and and and . Abaqus/Standard output The controls in effect for an analysis are listed in the data (.dat) and message (.msg) files. Nondefault controls are marked by **. For example, specifying the following controls: 1.0E−4 1.0E−4 1.0E−4 1.E−4 would result in the following output: STABILIZED STATE AND PLASTIC RATCHETTING DETECTION PARAMETERS FOR FORCE 1.0E-04 ** CRIT. FOR RESI. COEFF. ON ANY FOURIER TERMS 1.0E-04 ** CRIT. FOR CORR. TO DISP. COEFF. ON ANY FOURIER TERMS 1.0E-04 ** CRIT. FOR RESI. COEFF. ON CONSTANT FOURIER TERM ** CRIT. FOR CORR. TO DISP. COEFF. ON CONST. FOURIER TERM 1.0E-04 PERIODICITY CONDITION CONTROL PARAMETER: ** ITERATION NUMBER AT WHICH PERIODICITY CONDITION ** STARTS TO IMPOSE Controlling the solution accuracy in an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation Solution control parameters can be used in an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation to control the FSI stabilization and the mesh distortion. Controlling FSI stabilization You can specify the minimum number of remesh increments, maximum number of remesh increments, FSI penalty scale factor, and solid/fluid density ratio to control the FSI stabilization. The minimum and maximum number of remesh increments controls the number of mesh smoothing steps taken during the ALE process for FSI or deforming mesh problems. Reducing the minimum and maximum number of mesh smoothing increments can help reduce the computational time. Similarly, increasing the minimum/maximum number of smoothing increments helps to ensure that the mesh quality remains good and avoids potential element collapse during the evolution of an FSI problem. The FSI penalty scale factor has a default value of 1.0. Increasing this parameter in increments of 0.1 may be necessary for extremely flexible structures in high density fluids when the structural accelerations are high. When multiple solid-fluid interfaces are present, you should choose the smallest solid/fluid density ratio. Input File Usage: Use the following option to control the FSI stabilization: *CONTROLS, TYPE=FSI minimum number of remesh increments, maximum number of remesh increments, FSI penalty scale factor, solid/fluid density ratio Abaqus/CAE Usage: Controlling FSI stabilization in an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation is not supported in Abaqus/CAE. Controlling mesh distortion Similar to the distortion control used in Abaqus/Explicit , Abaqus/CFD offers distortion control to prevent elements from inverting or distorting excessively in fluid mesh movement. By default, distortion control is turned off during the co-simulation. Input File Usage: Use the following option to deactivate distortion control (default): *CONTROLS, TYPE=FSI, DISTORTION CONTROL=OFF Use the following option to activate distortion control: Abaqus/CAE Usage: *CONTROLS, TYPE=FSI, DISTORTION CONTROL=ON Controlling mesh distortion in an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation is not supported in Abaqus/CAE. 7.2.3 CONVERGENCE CRITERIA FOR NONLINEAR PROBLEMS Products: Abaqus/Standard Abaqus/CAE WARNING: The information in this section is provided for users who may wish to adjust the convergence criteria for the solution of nonlinear systems. In most cases these criteria need not be adjusted. References • “Convergence and time integration criteria: overview,” Section 7.2.1 • *CONTROLS • “Customizing general solution controls,” Section 14.15.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview In nonlinear problems the governing balance equations must be solved iteratively. This section describes: • the solution method for nonlinear problems (Newton’s method); • the field equations that can be solved by Abaqus/Standard; • the criteria used to establish convergence of each iteration during the solution; • “severe discontinuity” iterations; and • the line search algorithm, which can be used to improve the robustness of the Newton method. Solution method Where possible, Abaqus/Standard uses Newton’s method to solve nonlinear problems. In some cases it uses an exact implementation of Newton’s method, in the sense that the Jacobian of the system is defined exactly, and quadratic convergence is obtained when the estimate of the solution is within the radius of convergence of the algorithm. In other cases the Jacobian is approximated so that the iterative method is not an exact Newton method. For example, some material and surface interface models (such as nonassociated flow plasticity models or Coulomb friction) create a nonsymmetric Jacobian matrix, but you may choose to approximate this matrix by its symmetric part. Many problems exhibit discontinuous behavior. A common example is contact: at a particular point on a surface, the contact constraint is either present or absent. Another (usually less severe) example is strain reversal in plasticity at a point where the material is yielding. Specifying the quasi-Newton method You can choose to use the quasi-Newton technique for a particular step (described in “Quasi-Newton solution technique,” Section 2.2.2 of the Abaqus Theory Manual) instead of the standard Newton method for solving nonlinear equations. The quasi-Newton technique can save substantial computational cost in some cases by reducing the number of times the Jacobian matrix is factorized. Generally it is most successful when the system is large and many iterations are needed per increment or when the stiffness matrix is not changing much from iteration to iteration (such as in a dynamic analysis using implicit time integration or in a small-displacement analysis with local plasticity). It can be used only for symmetric systems of equations; therefore, it cannot be used when the unsymmetric solver is specified for a step , nor can it be used for procedures that always produce an unsymmetric system of equations, such as “Fully coupled thermal-stress analysis,” Section 6.5.3, and “Abaqus/Aqua analysis,” Section 6.11.1. In addition, it cannot be used for a static Riks procedure . The quasi-Newton method works well in combination with the line search method . Line searches help to prevent divergence of equilibrium iterations resulting from the inexact Jacobian produced by the quasi-Newton method. The line search method is activated by default for steps that use the quasi-Newton method. You can override this action by specifying line search controls. You can specify the number of quasi-Newton iterations allowed before the kernel matrix is reformed. The default number of iterations is 8. Additional matrix reformations may occur automatically during the iteration process depending on the convergence behavior. Since quadratic convergence is not expected during quasi-Newton iterations, the logarithmic rate of convergence check is not applied during the time incrementation. Furthermore, the iteration count used in the time incrementation is a weighted sum of quasi-Newton iterations, with the weight factor depending on whether or not a kernel matrix has been reformed. Input File Usage: *SOLUTION TECHNIQUE, TYPE=QUASI-NEWTON, REFORM KERNEL=n Abaqus/CAE Usage: Step module: step editor: Other: Solution technique: Quasi-Newton, Number of iterations allowed before the kernel matrix is reformed: n Specifying the separated method Alternatively, you can choose to use the separated technique instead of the standard Newton method for solving nonlinear equations for fully coupled thermal-stress and coupled thermal-electrical procedures. The separated technique (described in “Fully coupled thermal-stress analysis,” Section 6.5.3, and “Coupled thermal-electrical analysis,” Section 6.7.3) approximates the Jacobian by eliminating interfield coupling terms and can save substantial computational cost in cases where there is relatively weak coupling between the fields. Input File Usage: Abaqus/CAE Usage: *SOLUTION TECHNIQUE, TYPE=SEPARATED Step module: step editor: Other: Solution technique: Separated Field equations Field equations can be modeled separately or fully coupled. Some fields in Abaqus/Standard can only have linear response. Each field is discretized by using basic nodal variables (the degrees of freedom at the nodes of the finite element model) such as the components of the displacement in a continuum stress analysis problem. Each field has a conjugate “flux.” Available fields and their conjugate fluxes The fields and conjugate fluxes available in Abaqus/Standard are as follows: Basic problem Stress analysis: Force equilibrium Structural stress analysis: Moment equilibrium Field Conjugate flux Displacement, ; Force, ; Warping, w Rotation, Bimoment, W Moment, Heat transfer analysis Temperature, Heat flux, q Acoustic analysis (linear only) Acoustic pressure, u Rate of change of fluid volumetric flux Pore liquid flow analysis Pore liquid pressure, u Pore liquid volumetric flux, q Hydrostatic fluid modeling Fluid pressure, p Fluid volume, V Mass diffusion analysis Normalized concentration, Mass concentration volumetric flux, Q Piezoelectric analysis Electrical potential, Electrical charge, q Electric conduction analysis Electrical potential, Electrical current, J Mechanism analysis (connector elements with material flow degree of freedom) Analysis containing C3D4H elements (all materials, except compressible hyperelastic elastomers and elastomeric foams). Analysis containing C3D4H elements with compressible hyperelastic or hyperfoam materials. Material flow Material flux Pressure Lagrange multiplier Volumetric flux Volumetric Lagrange multiplier Pressure flux Constraint equations In some cases the problem also involves constraint equations. constraints are included by using Lagrange multipliers: In Abaqus/Standard the following Problem Constraint variable Constraint Hybrid solid (except C3D4H elements) Hybrid beam Hybrid beam Distributing coupling Distributing coupling Contact Pressure stress Volumetric strain compatibility Axial force Axial strain compatibility Transverse shear force Transverse shear strain compatibility Force Moment Coupling displacement compatibility Coupling rotation compatibility Normal pressure Surface penetration Contact with Lagrange friction Shear stress Relative shear sliding If the penalty method is used, the contact Lagrange multipliers may not be present. Solving coupled field equations In a general problem several (possibly nonlinear) coupled field equations of types be solved and several different (possibly nonlinear) constraints of type simultaneously. For example, in a structural problem in which hybrid beam elements are used, might represent the displacement field and the equilibrium equations for the conjugate force and might represent the rotation field and the equilibrium equations for the conjugate moment, while represents axial strain compatibility and represents transverse shear strain compatibility. must must be satisfied Controlling the accuracy of the solution The default solution control parameters defined in Abaqus/Standard are designed to provide reasonably optimal solution of complex problems involving combinations of nonlinearities as well as efficient solution of simpler nonlinear cases. However, the most important consideration in the choice of the control parameters is that any solution accepted as “converged” is a close approximation to the exact solution of the nonlinear equations. In this context “close approximation” is interpreted rather strictly by engineering standards when the default value is used, as described below. You can reset many solution control parameters related to the tolerances used for field equations. If you define less strict convergence criteria, results may be accepted as converged when they are not sufficiently close to the exact solution of the system. Use caution when resetting solution control parameters. Lack of convergence is often due to modeling issues, which should be resolved before changing the accuracy controls. You can select the type of equation for which the solution control parameters are being defined; for example, you can redefine the default controls for the displacement field and warping degree of freedom equilibrium equations only. By default, the solution control parameters will apply to all active fields in the model. See “Defining tolerances for field equations” in “Commonly used control parameters,” Section 7.2.2, for details. Input File Usage: *CONTROLS, PARAMETERS=FIELD, FIELD=field , , , , , , , , , Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Field Equations: Apply to all applicable fields or Specify individual fields: field Terminology Each field, measures are used in deciding if an increment has converged: , that is active in the problem is tested for convergence of the field equations. The following The largest residual in the balance equation for field . The largest change in a nodal variable of type The largest correction to any nodal variable of type iteration. The largest error in a constraint of type j. The instantaneous magnitude of the flux for field at time t, averaged over the entire model (spatial average flux). This average is by default defined by the fluxes that the elements apply to their nodes and any externally defined fluxes: provided by the current Newton in the increment. at its th node at time t, Here, E is the number of elements in the model, is the number of degrees of freedom of type is the number of nodes in element e, is the of element e, at node magnitude of the total flux component that element e applies at its ith degree of freedom of type (depends is the number of external fluxes for field on element type, loading type, and number of loads applied to an element), and is the magnitude of the ith external flux for field . An overall time-averaged value of the typical flux for field the current increment. Normally, the step in which iteration of the current increment. so far during this step including is defined as averaged over all the increments in for the current increment is recalculated after every is nonzero. The where in which number. The default for is the total number of increments so far in the step, including the current increment, is a small is the value of . Here is 10−5, but in rare cases, you can change this default. at increment i and Alternatively, you can define a value for the average flux in the step, . In this case, throughout the step. At the start of the step, is normally the value from the previous step (except for by default). Alternatively, you can define an initial value for , as described in “Modifying the initial time average flux” in retains its initial value until an is Step 1, when the time average flux, “Commonly used control parameters,” Section 7.2.2. iteration is completed for which defined, the value defined for The time-averaged value of the largest flux corresponding to the field excluding the current increment. The largest flux corresponding to the field during the current iteration. , at which time we redefine during this step, is ignored.) . (If Average flux ) is computed from the spatial average of the flux ( The time-averaged value of the flux ( ) at various instants in time. In some situations where only a small part of the model is active (the fluxes over the rest of the model are zero or very small), the spatial average of a flux over the entire model can be very small when compared to the spatial average over the active part of the model. Over a period of time this can result in a small value for the time-averaged value of the flux and in turn may lead to a convergence criterion that is very strict by engineering standards. To avoid such an excessively strict convergence criterion, Abaqus/Standard uses an algorithm to determine the active parts of a model at any given instant. During an iteration any flux freedom is also marked inactive. the current step. The default value of is treated as inactive, and the corresponding degree of is the time-averaged value of the largest flux in the model during is 10−5; you can redefine this parameter. At the end of an iteration the largest flux in the model during the current iteration ( ) is compared with the time-averaged value of the largest flux ( , the spatial average is computed over only the active parts of the model; if , all inactive parts of the model are reclassified as active and the spatial average is computed over the entire model. The appropriate spatial average of the flux obtained in this manner is then used to compute the time-averaged flux that is used in the convergence criterion. Setting computed over the entire model. forces the spatial averages of a flux to be always If ). If you specify a value for the average flux in the step, , throughout the step. Residuals Most nonlinear engineering calculations will be sufficiently accurate if the error in the residuals is less than %. Therefore, Abaqus/Standard normally uses as the residual check, where you can define convergence is accepted if the largest correction to the solution, largest incremental change in the corresponding solution variable, (it is 0.005 by default). If this inequality is satisfied, , is also small compared to the , estimated as CONVERGENCE CRITERIA satisfies the same criterion: You can define ; the default value is 10−2. , and The superscripts i, residual in field parameters,” Section 7.2.2, for more details on specifying refers to the largest at the start of the first iteration of the increment. See “Commonly used control . refer to the iteration number, and Zero flux In some cases there may be zero flux in the equations of type increments. Zero flux is defined as 10−5 and the solution for field convergence for field redefine this parameter. is accepted when is accepted if , where, as discussed earlier, anywhere in the model during some has a default value of , and is 10−3 ; you can . If not, . The default value of is compared to Negligible response in some fields Cases may arise where more than one field is active in the model yet there is negligible response in some of the fields in some increments. If some type of physical conversion factor, , exists between active for those particular increments fields ) to be used realistically as part of the convergence where criteria for field . An example of is a characteristic length to convert between force and moment. in the above paragraph can be replaced by is deemed too small ( and , Here, is a factor calculated by Abaqus/Standard based on the problem definition and the fields involved and is 1.0. Currently, this concept is used only for converting between the fields associated with forces and moments, when is a field conversion ratio that you can define. The default value for represents a characteristic element length. Linear increments Linear cases do not require more than one equilibrium iteration per increment. If for all , the increment is considered to be linear. You can define is 10−8 . Any case that passes such a stringent comparison of the largest residual with the average flux magnitude in each field is ; it is intended to be very small. The default value of considered linear and does not require further iteration. If this requirement is satisfied at some iteration after the first, the solution is accepted without any check on the size of the correction to the solution. Nonquadratic convergence In some cases quadratic convergence of the iterations is not possible because the Jacobian of the Newton scheme is approximated. If after iterations the convergence rate is only linear, Abaqus/Standard uses a looser tolerance, as the residual check. This tolerance modification is not applied when the quasi-Newton method is used, since it is normal for this method to require a larger number of iterations to converge. You can define “Controlling iteration”). , which is 2 × 10−2 by default. You can also define (by default, ; see Convergence also requires that Iteration continues until both criteria are satisfied for all active fields or the increment is abandoned. When the active field is the displacement, the convergence criterion requiring the largest displacement correction to be small relative to the maximum displacement increment ( ) is ignored when the maximum displacement increment itself is very small, as defined by is 10−8; you is the characteristic element length. The default value for , where can redefine this parameter. Controlling iteration Each increment of a nonlinear solution will usually be solved by multiple equilibrium iterations. The number of iterations may become excessive, in which case the increment size should be reduced and the increment attempted again. On the other hand, if successive increments are solved with a minimum number of iterations, the increment size may be increased. You can specify a number of time incrementation control parameters; some of them are described in this section, while the remainder are described in “Time integration accuracy in transient problems,” Section 7.2.4. Input File Usage: *CONTROLS, PARAMETERS=TIME INCREMENTATION , , , , , , , , , , , , , , , , , , , , , , , , , , Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Time Incrementation; click More to see additional data tables CONVERGENCE CRITERIA Abaqus/Standard may have trouble with the element calculations because of excessive distortion in large- displacement problems or because of very large plastic strain increments. If this occurs and automatic time incrementation has been chosen, the increment will be attempted again with a time increment of . If fixed time times the current time increment, where you can define . By default, stepping has been chosen, the analysis will terminate with an error message. Reattempting a diverging increment Sometimes the increment is too large for the solution to converge at all—the initial state is outside the “radius of convergence” of the Newton method. This condition can be detected by observing the behavior of the largest residuals, . In some cases these will not decrease from iteration to iteration throughout an iteration sequence that leads to convergence, but we assume that, if they fail to decrease over two consecutive iterations, the iterations should be abandoned. Thus, if where i is the iteration counter, the iterations are abandoned. This check is first made after following a solution discontinuity. You can define If fixed time stepping has been chosen, the analysis will terminate with an error message. With automatic time stepping the increment is begun again, using a time increment of times the previous attempt, where you can define . This subdivision continues until a successful time increment is found or the minimum time increment allowed has failed, in which case the job ends with an error message. Using the line search algorithm with sometimes helps in such cases . ; it must be at least 3. The default value of iterations is 4. . By default, Reattempting an increment when too many equilibrium iterations are required In case quadratic convergence cannot be obtained, the logarithmic rate of convergence, will often be maintained throughout the iteration process. This rate can be established during the early iterations. If convergence has not been achieved after or more iterations following a solution discontinuity, if automatic time incrementation has been selected, and if the slowest convergence rate over all fields total iterations subsequent to the last solution discontinuity are expected to be required, the increment is begun again with a time increment of times the If fixed time incrementation has been chosen, the iterations are continued; but if one abandoned. convergence is not achieved within iterations after the last solution discontinuity in the increment, the analysis will terminate with an error message. suggests that more than You can define the values of , , and . By default, , , and =0.5. Increasing or reducing the size of the time increment for efficiency When automatic time incrementation is chosen, the effectiveness of the nonlinear equation solution is used in the selection of the next time increment (in addition to the time integration accuracy criteria discussed in “Time integration accuracy in transient problems,” Section 7.2.4). iterations are required in two consecutive increments, the time increment may be increased by a factor of iterations, the next time increment is reduced to . By default, . If an increment converges but takes more than times the current time increment. You can define the values of , If no more than , and , and , , . , Extrapolation At each increment after the first increment of a nonlinear analysis step Abaqus/Standard estimates the solution to the increment by extrapolating the solution from the previous increment (or increments). By default, 100% linear extrapolation is used (1% for the Riks method). Extrapolation is abandoned if where define the value of ; it is 0.1 by default. is the proposed new time increment, and is the last successful time increment. You can You can turn this extrapolation scheme off for a particular step—see “Defining an analysis,” Section 6.1.2. Convergence of strain constraints in hybrid elements , with an absolute tolerance for the corresponding error, Strain constraint convergence in “hybrid” elements is checked by comparing the largest error in each strain constraint, . The magnitudes of these errors are reported in the message (.msg) file after each iteration as “compatibility errors.” For example, the volumetric compatibility error is a measure of the accuracy with which the incompressibility constraint is satisfied. Since nonlinearity in constraint equations is generally reflected in the field equations in the same problem, no attempt is made to estimate convergence rates in these constraint equations: we assume that the measures of convergence rate in the field equations are sufficient. You can define the Input File Usage: , ( ). By default, all of the *CONTROLS, PARAMETERS=CONSTRAINTS , and = 10−5. , , Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Constraint Equations Severe discontinuity iterations Abaqus/Standard distinguishes between regular, equilibrium iterations (in which the solution varies smoothly) and severe discontinuity iterations (SDIs) in which abrupt changes in stiffness occur. By default, Abaqus/Standard will continue to iterate until the severe discontinuities are sufficiently small (or no severe discontinuities occur) and the equilibrium (flux) tolerances are satisfied. For more information on the criteria used for the severe discontinuity checks, see “Severe discontinuities in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2. Alternatively, Abaqus/Standard will continue to iterate until no severe discontinuities occur and the equilibrium (flux) tolerances are satisfied. This more traditional method can cause convergence difficulties if the contact conditions are only weakly determined and contact “chattering” occurs or if a large number of severe discontinuity iterations are required to settle the contact conditions. You can define the contact and slip compatibility tolerance, the soft contact compatibility tolerance for low pressure, and the contact force error tolerance. Input File Usage: *CONTROLS, PARAMETERS=CONSTRAINTS , , , , , , , Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Constraint Equations Defining the contact force error tolerance is not supported in Abaqus/CAE. Severe discontinuity iterations in implicit dynamic analysis In implicit dynamic analysis, the average time of all contact changes in the increment is estimated and the time incrementation is interrupted to solve impact equations at that time. With augmented Lagrange or penalty constraint enforcement methods or with softened contact, no contact constraints are imposed when impact equations are solved. However, if the contact constraints are not satisfied within given tolerances, a severe discontinuity iteration is forced. See “Intermittent contact/impact,” Section 2.4.2 of the Abaqus Theory Manual, for details on intermittent contact in dynamic problems. Controlling the number of severe discontinuity iterations By default, Abaqus applies sophisticated criteria involving changes in penetration, changes in the residual force, and the number of severe discontinuities from one iteration to the next to determine whether iteration should be continued or terminated. Hence, it is in principle not necessary to limit the number of severe discontinuity iterations. This makes it possible to run contact problems that require large numbers of contact changes without having to change the control parameters. It is still possible to set a limit, , for the maximum number of severe discontinuity iterations; by default, , which in practice should always be more than the actual number of iterations in an increment. Input File Usage: *CONTROLS, PARAMETERS=TIME INCREMENTATION , , , , , , , , , , Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Time Incrementation; click More to see additional data tables Controlling the number of severe discontinuity iterations when severe discontinuities always force iterations In this case a limit, an increment. If more than started over with a time increment size of , is placed on the number of iterations caused by severe discontinuities in iterations are required for severe discontinuities, the increment is times the abandoned increment size (for automatic time incrementation). If fixed time incrementation was chosen, the analysis terminates with an error message. You can define the values of . and . By default, *CONTROLS, PARAMETERS=TIME INCREMENTATION , , , , , , , , , , and Input File Usage: Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Time Incrementation; click More to see additional data tables Improving the efficiency of the solution by using the line search algorithm Abaqus/Standard provides the option of including a “line search” algorithm. The purpose of the line search is to improve the robustness of the Newton or quasi-Newton methods. By default, the line search is active only for steps that use the quasi-Newton method. During equilibrium iterations where residuals are large, the line search algorithm scales the correction to the solution by a line search scale factor, . An iterative process is used to find the value of that minimizes the component of the residual vector in the direction of the correction vector; this component is called , where j is the line search iteration number. Each line search iteration requires one pass through the Abaqus/Standard element loop but does not require any operations using the global stiffness matrix. It is usually sufficient to determine limit this accuracy. A maximum of allowable range of : The line search ceases when only to modest accuracy. There are several controls used to line search iterations are performed. There is a limit on the where line search ceases, cease when the change in is evaluated before the first equilibrium iteration. The residual reduction factor at which the , is typically set to a rather loose tolerance. The line search algorithm will also provided by a line search iteration is less than , , and , times . = 1.0, You can define the values of , =5 with the quasi-Newton method. Set . By default, = 0 with the Newton method, and to a nonzero value to activate the line search algorithm or to zero to forcibly deactivate line search. Default values for the additional line search parameters are = 0.10. These defaults are chosen to achieve modest accuracy for the line search scale factor, while minimizing the additional cost of line search iterations. More agressive line searching can be beneficial in some simulations, especially when many nonlinear iterations and/or cutbacks are needed to resolve sharp discontinuities in the solution. In these cases you could try allowing more line search iterations ( =10) and requiring more accuracy in the line search scale factor ( =0.01). This may result in more line search iterations but fewer nonlinear iterations and cutbacks and an overall reduction in solution cost. = 0.25, and = 0.0001, Input File Usage: *CONTROLS, PARAMETERS=LINE SEARCH , , , , Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Line Search Control TIME INTEGRATION ACCURACY IN TRANSIENT PROBLEMS TIME INTEGRATION ACCURACY Products: Abaqus/Standard Abaqus/CAE References • “Convergence and time integration criteria: overview,” Section 7.2.1 • “Implicit dynamic analysis using direct integration,” Section 6.3.2 • “Uncoupled heat transfer analysis,” Section 6.5.2 • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 • “Rate-dependent plasticity: creep and swelling,” Section 23.2.4 • *CONTROLS • “Customizing general solution controls,” Section 14.15.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Abaqus/Standard usually uses automatic time stepping schemes for the solution of transient problems. Factors influencing the increment size for transient problems include convergence aspects related to the degree of geometric, material, and contact nonlinearity (which also influence non-transient problems and are discussed in “Convergence criteria for nonlinear problems,” Section 7.2.3) and the ability of the time integration operator to accurately resolve variations in the accelerations, velocities, and displacements over an increment. This section discusses tolerance parameters and adjustments to the time increment size related to the latter aspect. Time incrementation parameters and adjustment criteria Table 7.2.4–1 lists tolerance parameters available for specific analysis procedures. Descriptions of time integrators for the transient procedure types and, in the case of implicit dynamics, discussion of additional factors influencing the time increment size related to accuracy of time integration are provided in the respective sections referenced in Table 7.2.4–1. Table 7.2.4–1 Time integration accuracy measures for various procedures. Procedure Accuracy measure Tolerance Implicit dynamics (“Implicit dynamic analysis using direct integration,” Section 6.3.2) Half-increment residual Half-increment residual tolerance Transient heat transfer analysis (“Uncoupled heat transfer analysis,” Section 6.5.2) Consolidation analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1) Creep and viscoelastic material behavior (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) Temperature increment, Pore pressure increment, Creep tolerance , will be active. Corresponding measures of the integration accuracy, In any transient analysis where automatic time incrementation is used, some of these tolerances, , , will be calculated for each increment in the step. Abaqus/Standard will use these values to adjust the time incrementation using the criteria described in this section. The smallest time increment required by all criteria is used if more than one accuracy measure is active. Reducing the time increment size for any control, J, that is active in the step, the time increment If is too large to satisfy that time integration accuracy requirement. The increment is, therefore, begun again with a time increment of where you can define the value of . By default, = 0.85. Input File Usage: Abaqus/CAE Usage: *CONTROLS, PARAMETERS=TIME INCREMENTATION first data line , , , Step module: Other→General Solution Controls→Edit: toggle on Specify: Time Incrementation; click More to see additional data tables Increasing the time increment size If at the current time increment, , for all J in each of because of nonlinearity, the next time increment will be increased to consecutive increments, i, and if no cut-back has occurred within those increments = 3, = 0.75, and = 0.8. is You can define the values of the proposed new time increment, which is defined as , and . By default, , for transient heat transfer and transient mass diffusion problems and which is defined as for other transient problems. A limit, , is placed on the time increment increase factor. The default value of depends on the type of analysis: • • • = 1.25 for dynamic analysis = 2.0 for diffusion-dominated processes: creep, transient heat transfer, coupled temperature- displacement, soils consolidation, and transient mass diffusion = 1.5 for all other cases You can redefine for each analysis type. If the problem is nonlinear, the time increment may be restricted by the rate of convergence of the nonlinear equations. The time incrementation controls used with nonlinear problems are described in “Convergence criteria for nonlinear problems,” Section 7.2.3. Input File Usage: *CONTROLS, PARAMETERS=TIME INCREMENTATION , , , , , , , , , , , , , , , , , , , Abaqus/CAE Usage: Step module: Other→General Solution Controls→Edit: toggle on Specify: Time Incrementation; click More to see additional data tables Avoiding small changes to the time increment size during implicit integration procedures In linear transient problems when Abaqus/Standard uses implicit integration, the system of equations must be reformed and decomposed whenever the time increment changes even though the stiffness matrix does not change. Therefore, to reduce the number of increments at which the system matrix changes, Abaqus/Standard makes use of the factor , where The definition of increments: results in the following inequality between the proposed and the current time Based on this inequality the time increment is allowed to increase only when its value computed by the criteria described earlier in this section, or computed using the value of PNEWDT specified in certain user subroutines (UMAT, for example), is greater than or equal to is 1.0, but you can redefine it to be a smaller number. Reducing to a value less than 1.0 allows the time increment to increase by a factor that is smaller than , thereby forcing a time increment change, even if the change is small. Otherwise, the solution continues with the same . The default value of . Input File Usage: Abaqus/CAE Usage: *CONTROLS, PARAMETERS=TIME INCREMENTATION first data line second data line , , , , Step module: Other→General Solution Controls→Edit: toggle on Specify: Time Incrementation; click More to see additional data tables • Chapter 8, “Analysis Techniques: Introduction” • Chapter 9, “Analysis Continuation Techniques” • Chapter 10, “Modeling Abstractions” • Chapter 11, “Special-Purpose Techniques” • Chapter 12, “Adaptivity Techniques” • Chapter 13, “Optimization Techniques” • Chapter 14, “Eulerian Analysis” • Chapter 15, “Particle Methods” • Chapter 16, “Sequentially Coupled Multiphysics Analyses” • Chapter 17, “Co-simulation” • Chapter 18, “Extending Abaqus Analysis Functionality” • Chapter 19, “Design Sensitivity Analysis” 8. Analysis Techniques: Introduction Introduction 8.1 Introduction • “Analysis techniques: overview,” Section 8.1.1 8.1.1 ANALYSIS TECHNIQUES: OVERVIEW Abaqus provides an extensive selection of analysis techniques. These techniques provide powerful tools for performing your analysis more efficiently and effectively. Analysis continuation techniques In many cases your analysis results represent a significant investment of computational effort. As a result, you will often want to reduce computation costs by utilizing results from an analysis that has already been performed. In other cases your overall analysis history will be comprised of distinct Abaqus jobs, each representing a portion of the response history of the model. Abaqus provides the following analysis continuation techniques: • Abaqus allows you to restart an analysis, as long as you request that certain files containing model and state data be saved in the original analysis. See “Restarting an analysis,” Section 9.1.1. • You can perform part of an analysis with Abaqus/Standard or Abaqus/Explicit and continue the analysis with the other product. You can transfer results from Abaqus/Standard to Abaqus/Explicit, from Abaqus/Explicit to Abaqus/Standard, and from Abaqus/Standard to Abaqus/Standard. See “Transferring results between Abaqus analyses: overview,” Section 9.2.1. Modeling abstractions All Abaqus models involve certain abstractions. In addition to the traditional abstractions associated with the finite element method, you can include techniques in your model to obtain more cost-effective solutions. Abaqus provides the following techniques for modeling abstractions: • You can create substructures by grouping a number of elements together and retaining only the degrees of freedom needed to interface with adjacent structures. This technique is particularly useful when a substructure is to be reused in the same analysis, in different analyses, or by different analysts. See “Using substructures,” Section 10.1.1. • You can analyze local regions of a model in greater detail and interpolate the solution results from a larger coarser global model. See “Submodeling: overview,” Section 10.2.1. • You can allow for the mathematical abstraction of model data such as mesh and material information by generating global or element matrices representing the stiffness, mass, viscous See “Generating matrices,” damping, structural damping, and load vectors in a model. Section 10.3.1. • You can create a three-dimensional model in Abaqus/Standard by revolving various forms of axisymmetric and three-dimensional model sectors about an axis of symmetry . You can also transfer the solution obtained in an original axisymmetric model to the new model . In addition, for models that exhibit cyclic symmetry you can extract eigenmodes and perform mode-based steady-state dynamic analysis by modeling only a single repetitive sector of the model . • Using the periodic media analysis technique, you can effectively model systems that are repetitive in nature, such as manufacturing processes involving conveyor belts or continuous forming operations. See “Periodic media analysis,” Section 10.5.1. • You can define a complex beam cross-section, including multiple materials and complex geometry, and automatically generate beam element cross-section properties. See “Meshed beam cross-sections,” Section 10.6.1. • Using the extended finite element method, you can model discontinuities, such as cracks, as an enriched feature without creating a mesh to match the geometry of the discontinuity. See “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1. Special-purpose techniques Certain analysis techniques do not fall into a general classification and are grouped here as special- purpose techniques. Abaqus provides the following special-purpose techniques: • You can use the inertia relief technique as an inexpensive alternative to performing a full dynamic analysis on a free or partially constrained body subjected to loads derived from rigid body accelerations. See “Inertia relief,” Section 11.1.1. • You can selectively remove, and later reintroduce, parts of a model. See “Element and contact pair removal and reactivation,” Section 11.2.1. • You can introduce small imperfections into a model, typically for postbuckling analysis. See “Introducing a geometric imperfection into a model,” Section 11.3.1. • You can evaluate fracture performance through contour integral evaluation, through crack propagation modeling techniques, or by using line spring elements in conjunction with shell elements. See “Fracture mechanics: overview,” Section 11.4.1. • You can model coupling between the deformation of a fluid-filled structure and the pressure exerted by a contained fluid . • In Abaqus/Explicit you can use the mass scaling technique to control the stable time increment and increase computational efficiency. See “Mass scaling,” Section 11.6.1. • You can use selective subcycling to allow different time increments to be used for different groups of elements, which can reduce the run time for an analysis when a small region of elements in the model controls the stable time increment. See “Selective subcycling,” Section 11.7.1. • You can use steady-state detection to detect the time in a quasi-static uni-directional Abaqus/Explicit simulation when a steady-state condition has been reached and then terminate the simulation. See “Steady-state detection,” Section 11.8.1. Adaptivity techniques Adaptivity techniques enable modification of your mesh to obtain a better solution. Abaqus provides the following adaptivity techniques: • You can use ALE adaptive meshing to control mesh distortion or to model material loss. See “ALE adaptive meshing: overview,” Section 12.2.1. • You can use adaptive remeshing with Abaqus/Standard and Abaqus/CAE to iteratively improve your mesh to obtain a more accurate solution. See “Adaptive remeshing: overview,” Section 12.3.1. • You can use mesh-to-mesh solution mapping as part of a mesh replacement strategy for distortion control. See “Mesh-to-mesh solution mapping,” Section 12.4.1. See “Adaptivity techniques,” Section 12.1.1, for a comparison of the adaptivity methods. Optimization techniques You can use structural optimization, an iterative process that helps you refine your designs, to perform topology and shape optimization. In Abaqus/CAE you create the model to be optimized and define, configure, and execute the structural optimization. See “Structural optimization: overview,” Section 13.1.1. Eulerian analysis You can use Abaqus/Explicit to simulate extreme deformation, up to and including fluid flow, in an Eulerian analysis. Eulerian materials can be coupled to Lagrangian structures to analyze fluid-structure interactions. See “Eulerian analysis,” Section 14.1.1. Particle methods Using the smoothed particle hydrodynamics technique, you can model violent free-surface fluid flow (such as wave impact) and extremely high deformation/obliteration of solid structures (such as ballistics). See “Smoothed particle hydrodynamic analysis,” Section 15.1.1. Sequentially coupled multiphysics analyses In Abaqus/Standard you can perform sequentially coupled multiphysics analyses when the coupling between one or more of the physical fields in a model is only important in one direction. See “Sequentially coupled multiphysics analyses,” Section 16.1. Co-simulation You can use the co-simulation technique for run-time coupling of two Abaqus analyses or of Abaqus with third-party analysis programs to perform multiphysics simulation. See “Co-simulation: overview,” Section 17.1.1. Extending Abaqus analysis functionality You can use the flexibility of user subroutines to increase the functionality of Abaqus. See “User subroutines and utilities,” Section 18.1. Design sensitivity analysis You can use design sensitivity analysis (DSA) techniques to determine sensitivities of responses with respect to specified design parameters. You can use these techniques for design studies within Abaqus/Standard or in conjunction with third-party design optimization tools. See “Design sensitivity analysis,” Section 19.1.1. Parametric studies You can use parametric studies to perform multiple analyses in which you can systematically vary modeling parameters that you define. See “Scripting parametric studies,” Section 20.1.1, and “Parametric studies: commands,” Section 20.2. Availability of analysis techniques The availability of the analysis techniques provided in Abaqus is summarized in Table 8.1.1–1. In addition, optimization techniques are available in Abaqus/CAE . Table 8.1.1–1 Availability of analysis techniques in Abaqus. Technique Abaqus/Standard Abaqus/Explicit Abaqus/CFD “Restarting an analysis,” Section 9.1 “Importing and transferring results,” Section 9.2 “Substructuring,” Section 10.1 “Submodeling,” Section 10.2 “Generating global matrices,” Section 10.3 “Symmetric model generation, results transfer, and analysis of cyclic symmetry models,” Section 10.4 “Periodic media analysis,” Section 10.5 “Meshed beam cross-sections,” Section 10.6 “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7 “Inertia relief,” Section 11.1 Abaqus/Standard Abaqus/Explicit Abaqus/CFD ANALYSIS TECHNIQUES OVERVIEW “Mesh modification or replacement,” Section 11.2 “Geometric imperfections,” Section 11.3 “Fracture mechanics,” Section 11.4 “Surface-based fluid modeling,” Section 11.5 “Mass scaling,” Section 11.6 “Selective subcycling,” Section 11.7 “Steady-state detection,” Section 11.8 “ALE adaptive meshing,” Section 12.2 “Adaptive remeshing,” Section 12.3 “Analysis continuation after mesh replacement,” Section 12.4 “Eulerian analysis,” Section 14.1 “Smoothed particle hydrodynamic analyses,” Section 15.1 “Sequentially coupled multiphysics analyses,” Section 16.1 “Co-simulation,” Section 17.1 “User subroutines and utilities,” Section 18.1 “Design sensitivity analysis,” Section 19.1 “Scripting parametric studies,” Section 20.1 9. Analysis Continuation Techniques Restarting an analysis Importing and transferring results 9.1 9.1 Restarting an analysis • “Restarting an analysis,” Section 9.1.1 9.1.1 RESTARTING AN ANALYSIS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Output,” Section 4.1.1 • *RESTART • “Restarting an analysis,” Section 19.6 of the Abaqus/CAE User’s Manual Overview When you run an analysis, you can write the model definition and state to the files required for restart. Scenarios for using the restart capability include: • Continuing an interrupted run: If an analysis is interrupted by a computer malfunction, the Abaqus restart analysis capability allows the analysis to complete as originally defined. • Continuing with additional steps: After viewing results from a successful analysis, you may decide to append steps to the load history. • Changing an analysis: Sometimes, having viewed the results of the previous analysis, you may want to restart the analysis from an intermediate point and change the remaining load history data in some manner. In addition, you may want to add additional steps to the load history if the previous analysis completed successfully. “Output,” Section 4.1.1, describes the process of obtaining results output from an Abaqus/Standard restart file. Writing restart files If you want to be able to restart an analysis, you must request restart output. This output will be written to files that can be used to restart the analysis. If you do not request that restart data be written, restart files will not be created in Abaqus/Standard, while in Abaqus/Explicit and Abaqus/CFD a state file will be created with results at only the beginning and end of each step. In Abaqus/Standard these files are the restart (job-name.res; file size limited to 16 gigabytes), analysis database (.mdl and .stt), part (.prt), output database (.odb), and linear dynamics and substructure database (.sim) files. In Abaqus/Explicit these files are the restart (job-name.res; file size limited to 16 gigabytes), analysis database (.abq, .mdl, .pac, and .stt), part (.prt), selected results (.sel), and output database (.odb) files. In Abaqus/CFD these files are the restart and analysis database (job-name.sim) and output database (.odb) files. These files, collectively referred to as the restart files, allow an analysis to be completed up to a certain point in a particular run and restarted and continued in a subsequent run. The output database file only needs to contain the model data; results data are not required and can be suppressed. You can control the amount of data written to the restart files, as described below. The amount of data written to the restart file can be changed from step to step if you include the restart request in each step definition. Restart information is not written during the following linear perturbation steps: • “Static stress analysis,” Section 6.2.2 (perturbation) • “Eigenvalue buckling prediction,” Section 6.2.3 • “Direct-solution steady-state dynamic analysis,” Section 6.3.4 • “Complex eigenvalue extraction,” Section 6.3.6 • “Transient modal dynamic analysis,” Section 6.3.7 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 • “Subspace-based steady-state dynamic analysis,” Section 6.3.9 • “Response spectrum analysis,” Section 6.3.10 • “Random response analysis,” Section 6.3.11 • “Eddy current analysis,” Section 6.7.5 Input File Usage: Use the following option to request that restart data be written for an analysis: *RESTART, WRITE The *RESTART, WRITE option can be used as either model data or history data. Abaqus/CAE Usage: Step module: Output→Restart Requests In Abaqus/CAE restart requests are always associated with a particular step; you cannot define a restart request for the entire analysis. Restart requests are created by default for every step; restart requests for Abaqus/Standard and Abaqus/CFD steps have a default frequency of 0, while restart requests for Abaqus/Explicit steps have a default number of intervals of 1. Controlling the frequency of output to the restart files You can specify the frequency at which data will be written to the Abaqus/Standard restart file and the Abaqus/Explicit and Abaqus/CFD state files. The variables to be written cannot be specified; a complete set of data is written each time. Therefore, the restart files can be quite large unless you control the frequency with which restart information is written. If restart information is requested for an Abaqus/Standard analysis at exact time intervals, Abaqus/Standard will obtain a solution each time data are written. In this case if the frequency of output to the restart file is high, the number of increments and, consequently, the computational cost of the analysis may increase considerably. Specifying the frequency of output to the Abaqus/Standard restart file in increments By default, Abaqus/Standard will write data to the restart file after each increment at which the increment number is exactly divisible by a user-specified frequency value, N, and at the end of each step of the analysis (regardless of the increment number at that time). In a direct cyclic or a low-cycle fatigue analysis Abaqus/Standard will write data to the restart file only at the end of a loading cycle; therefore, Abaqus/Standard will write data to the restart file after each iteration (or cycle in a low-cycle fatigue analysis) at which the iteration number (or cycle number in a low-cycle fatigue analysis) is exactly divisible by N and at the end of each step of the analysis. Input File Usage: Abaqus/CAE Usage: *RESTART, WRITE, FREQUENCY=N By default, N=1. Step module: Output→Restart Requests: enter N in the Frequency column for each step By default, N=0 (no restart information is written). Specifying the frequency of output to the Abaqus/Standard restart file in time intervals Abaqus/Standard can divide the step into a user-specified number of time intervals, n, and write the results at the end of each interval, for a total of n points for the step. If n is specified, by default data will be written to the results file at the exact times calculated by dividing the step into n equal intervals. Alternatively, you can choose to write the information at the increment ending immediately after the time dictated by each interval. You can specify the frequency of restart output in time intervals only for the procedures listed in Table 9.1.1–1. In addition, this capability is not supported for linear perturbation analyses. Input File Usage: Use the following option to request results at the exact time intervals: *RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=YES Use the following option to request immediately after each time interval: results at the increments ending Abaqus/CAE Usage: *RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=NO Step module: Output→Restart Requests: enter n in the Intervals column; toggle on the Time Marks column for each step if you want the results written at the exact time intervals Table 9.1.1–1 List of Abaqus/Standard procedures that support restart at time intervals. Procedure Time incrementation Restart at exact time intervals Restart at approximate time intervals “Static stress analysis,” Section 6.2.2 (except if the Riks method is used) “Implicit dynamic analysis using direct integration,” Section 6.3.2 Automatic Fixed Automatic Fixed 9.1.1–3 — Procedure Time incrementation Restart at exact time intervals Restart at approximate time intervals “Uncoupled heat transfer analysis,” Section 6.5.2 (except if you specify that the analysis end when steady state is reached) “Mass diffusion analysis,” Section 6.9.1 (except if you specify that the analysis end when steady state is reached) “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 (except if you specify that the analysis end when steady state is reached) “Fully coupled thermal-stress analysis,” Section 6.5.3 “Fully coupled thermal-electrical- structural analysis,” Section 6.7.4 “Coupled thermal-electrical analysis,” Section 6.7.3 (except if you specify that the analysis end when steady state is reached) “Steady-state transport analysis,” Section 6.4.1 “Subspace-based steady-state dynamic analysis,” Section 6.3.9 “Quasi-static analysis,” Section 6.2.5 Automatic Fixed Automatic Fixed Automatic Fixed Automatic Fixed Automatic Fixed Automatic Fixed Automatic Fixed Fixed Automatic Fixed — — — — — — — — — Time incrementation If the output frequency is specified in terms of the number of intervals, Abaqus/Standard will adjust the time increments to ensure that data are written at the exact time points specified. In some cases Abaqus may use a time increment smaller than the minimum time increment allowed in the step in the increment directly before a time point. However, Abaqus will not violate the minimum time increment allowed for consolidation, transient mass diffusion, transient heat transfer, transient couple thermal-electrical, transient coupled temperature-displacement, and transient coupled thermal-electrical-structural analyses. For these procedures if a time increment smaller than the minimum time increment is required, Abaqus will use the minimum time increment allowed in the step and will write restart data at the first increment after the time point. When the output frequency is specified in terms of the number of intervals, the number of increments necessary to complete the analysis might increase, which might adversely affect performance. Specifying the frequency of output to the Abaqus/Explicit state file Abaqus/Explicit will divide the step into a user-specified number of time intervals, n, and write the results at the beginning of the step and at the end of each interval, for a total of n+1 points for the step. By default, the results will be written to the state file at the increment ending immediately after the time dictated by each interval. Alternatively, you can choose to write the results at the exact times calculated by dividing the step into n equal intervals. Results are always written at the end of the step, so it is not necessary to request results at the exact time intervals if results are required only at the end of a step. If a problem precludes the analysis from continuing to completion, such as if an element becomes excessively distorted, Abaqus/Explicit will attempt to save the last completed increment in the state file. Input File Usage: Use the following option to request immediately after each time interval: results at the increments ending *RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=NO Use the following option to request results at the exact time intervals: *RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=YES By default, n=1. Abaqus/CAE Usage: Step module: Output→Restart Requests: enter n in the Intervals column; toggle on the Time Marks column for each step if you want the results written at the exact time intervals By default, n=1. Specifying the frequency of output to the Abaqus/CFD state file in increments Abaqus/CFD will write data to the restart file after each increment at which the increment number is exactly divisible by a user-specified frequency value, N, and at the end of each step of the analysis (regardless of the increment number at that time). Input File Usage: *RESTART, WRITE, FREQUENCY=N Abaqus/CAE Usage: By default, N=1. Step module: Output→Restart Requests: enter N in the Frequency column for each step By default, N=0 (no restart information is written). Specifying the frequency of output to the Abaqus/CFD state file in time intervals Abaqus/CFD will divide the step into a user-specified number of time intervals, n, and write the results at the beginning of the step and at the end of each interval, for a total of n+1 points for the step. By default, the results will be written to the state file at the increment ending immediately after the time dictated by each interval. If a problem precludes the analysis from continuing to completion, such as if the solution does not converge, Abaqus/CFD will attempt to save the last completed increment in the state file. Input File Usage: Abaqus/CAE Usage: *RESTART, WRITE, NUMBER INTERVAL=n Step module: Output→Restart Requests: enter n in the Intervals column By default, n=0. Synchronizing restart information written in a co-simulation Restart output must be synchronized between co-simulation analyses for a co-simulation restart to be successful. To achieve this synchronization, it is recommended that you request that restart data are written at a specified number of time intervals, n. In this case Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD will write restart information at the co-simulation target time immediately after the time dictated by each interval. If you specify the frequency of output for restart data in increments, it is very difficult to synchronize the writing of restart information, and the restart analysis may start from two different time points, possibly leading to an imbalance. Input File Usage: Use the following option to synchronize restart information written in a co- simulation: *RESTART, WRITE, NUMBER INTERVAL=n When using the NUMBER INTERVAL parameter for a co-simulation, the TIME MARKS parameter on the *RESTART option is always set to NO. Step module: Output→Restart Requests: enter n in the Intervals column Abaqus/CAE Usage: Controlling the precision of output to the Abaqus/Explicit state file By default, Abaqus/Explicit writes to the state file in double precision when the analysis is run in double precision. Alternatively, you can choose to write data to the state file in single precision if you want to reduce the size of the state file. This option may cause noisy results between step boundaries or for the first step of a restart analysis. If Abaqus/Explicit is run in single precision, this control parameter is ignored and single precision is always used. Input File Usage: Abaqus/CAE Usage: *RESTART, WRITE, SINGLE Single precision state file output is not supported by Abaqus/CAE. Overlaying results in the restart files For an Abaqus/Standard or Abaqus/Explicit analysis, you can specify that only one increment (or one iteration in the case of a direct cyclic analysis) per step should be retained in the Abaqus/Standard restart file or Abaqus/Explicit state file, thus minimizing the size of the files. As the data are written, they overlay the data from the previous increment (or iteration), if any, written for the same step. You can specify whether or not the data should be overlaid for each step individually. Since in Abaqus/Explicit the results are written by default only at the end of the step, it is recommended to overlay the data in conjunction with specifying a number of time intervals at which data are written; in this way the data in the restart file are advanced as dictated by the number of intervals used. To protect you from losing data if your system crashes, when Abaqus/Standard writes a frame from a given increment, it does not strictly overwrite the frame from the last saved increment. Instead, it always keeps a reserve frame and only frees a given saved frame for overwriting when the next frame is secured on the file. This reserve frame is not deleted unless the space is required for later increments. This process produces a bonus frame in the last step of an analysis if overlaying is occurring in that step and if the analysis completes successfully; users will observe that the penultimate restart frame is also retained for the last step, even though overlay is being used. The advantage of overlaying the restart data is that it minimizes the space required to store the restart files. Input File Usage: Abaqus/CAE Usage: Restarting an analysis Use the following option in Abaqus/Standard: *RESTART, WRITE, OVERLAY Use the following option in Abaqus/Explicit: *RESTART, WRITE, OVERLAY, NUMBER INTERVAL=n Step module: Output→Restart Requests: click to check the Overlay column for each step You restart (continue) an analysis by specifying that the restart or state, analysis database, and part files created by the original analysis be read into the new analysis. The restart files must be saved upon completion of the first job. In Abaqus/Explicit the package (.pac) file and the selected results (.sel) file are also used for restarting an analysis and must be saved upon completion of the first job. Since restart files can be very large, sufficient disk space must be provided (in Abaqus/Standard the analysis input file processor estimates the space that is required for the restart file). You can specify the point at which the analysis is continued in the new run, as discussed below. An analysis cannot be restarted from the linear perturbation steps listed in “Writing restart files.” In addition, if an Abaqus/Standard or Abaqus/Explicit analysis is terminated abruptly by an operating system command or due to a power failure, it is unlikely that the job can be recovered or restarted. In this situation, files that are open during the analysis process are not closed properly, which may result in loss of data and incomplete files. Input File Usage: Use the following option to restart an analysis: *RESTART, READ When the READ parameter is included, the *RESTART option must appear as model data. It is normally the first option in the input file after the *HEADING option. Abaqus/CAE Usage: Job module: job editor: toggle on Restart as the Job Type Identifying the analysis to be restarted In an Abaqus/Standard restart analysis you must specify the name of the restart file that contains the specified step and increment, iteration (for a direct cyclic analysis), or cycle (for a low-cycle fatigue analysis). In an Abaqus/Explicit or an Abaqus/CFD restart analysis you must specify the name of the state file that contains the specified step and interval. Abaqus issues an error message if the step and increment, iteration, cycle, or interval number at which restart is requested do not exist in the specified restart or state file. Input File Usage: Enter the following input on the command line: abaqus job=job-name oldjob=oldjob-name Abaqus/CAE Usage: Any module: Model→Edit Attributes→model_name: Restart: toggle on Read data from job and enter the oldjob-name Specifying the restart point You can specify the point (step and increment, iteration, cycle, or interval) in the previous analysis from which to restart. Truncating a step in the previous analysis when you restart is discussed below. Specifying the restart point for an Abaqus/Standard analysis (except when restarting from a direct cyclic or a low-cycle fatigue analysis) An Abaqus/Standard analysis restarted from any analysis other than a direct cyclic or a low-cycle fatigue analysis will continue the analysis immediately after the user-specified step and increment. If you do not specify a step or increment, the analysis will restart at the last available step and increment found in the restart file. Input File Usage: Abaqus/CAE Usage: *RESTART, READ, STEP=step, INC=increment Any module: Model→Edit Attributes→model_name: Restart: toggle on Read data from job, Step name: step, toggle on Restart from increment, interval, iteration, or cycle, and enter the increment Specifying the restart point for an Abaqus/Standard analysis restarted from a direct cyclic analysis An Abaqus/Standard analysis restarted from a previous direct cyclic analysis can be restarted only from the end of a loading cycle. In this case you should specify the step and iteration number at which the new analysis will be resumed. In a direct cyclic analysis that has not reached a stabilized cycle upon restart, you can increase the number of iterations or Fourier terms, thus allowing continuation of an analysis . Input File Usage: Abaqus/CAE Usage: *RESTART, READ, STEP=step, ITERATION=iteration Any module: Model→Edit Attributes→model_name: Restart: toggle on Read data from job, Step name: step, toggle on Restart from increment, interval, iteration, or cycle, and enter the iteration Specifying the restart point for an Abaqus/Standard analysis restarted from a low-cycle fatigue analysis An Abaqus/Standard analysis restarted from a previous low-cycle fatigue analysis can be restarted only from the end of a loading cycle. In this case you should specify the step and cycle number at which the new analysis will be resumed. Input File Usage: Abaqus/CAE Usage: *RESTART, READ, STEP=step, CYCLE=cycle Any module: Model→Edit Attributes→model_name: Restart: toggle on Read data from job, Step name: step, toggle on Restart from increment, interval, iteration, or cycle, and enter the cycle Specifying the restart point for an Abaqus/Explicit analysis An Abaqus/Explicit restart analysis will continue the analysis immediately after the user-specified step and interval. You must specify the step from which an Abaqus/Explicit restart analysis will continue. If you do not specify an interval from which to restart or that the current step should be terminated at a specified interval, the analysis is restarted from the last interval available in the state file for the specified step. Input File Usage: Abaqus/CAE Usage: *RESTART, READ, STEP=step, INTERVAL=interval Any module: Model→Edit Attributes→model_name: Restart: toggle on Read data from job, Step name: step, toggle on Restart from increment, interval, iteration, or cycle, and enter the interval Specifying the restart point for an Abaqus/CFD analysis An Abaqus/CFD restart analysis will continue the analysis immediately after the user-specified step and increment. You must specify the step and increment from which an Abaqus/CFD restart analysis will continue. If you do not specify a step or increment, an error message will be issued. Input File Usage: Abaqus/CAE Usage: *RESTART, READ, STEP=step, INC=increment Any module: Model→Edit Attributes→model_name: Restart: toggle on Read data from job, Step name: step, toggle on Restart from increment, interval, iteration, or cycle, and enter the increment Continuing an analysis without changes To continue an analysis without changes, only the steps subsequent to the step at which restart is being made should be defined in the restart analysis. All other information has been saved to the restart files. This feature cannot be used for an Abaqus analysis that uses the co-simulation technique and cannot be used for an Abaqus/CFD analysis. Continuing an Abaqus/Standard analysis without changes In Abaqus/Standard, in cases where restart is being performed simply to continue a long step (which might have been terminated because the time limit for the job was exceeded, for example), the data for the restart run may simply consist of the request to read restart data from another analysis. Input File Usage: Abaqus/CAE Usage: *RESTART, READ Any module: Model→Edit Attributes→model_name: Restart: toggle on Read data from job Continuing an Abaqus/Explicit analysis without changes In Abaqus/Explicit, in cases where restart is being performed simply to continue a long step (which might have been terminated because a CPU time limit was exceeded, for example), do not use a restart analysis; instead, use a recover analysis. In this case no data are needed (unless user subroutines are being used). Input File Usage: Enter the following input on the command line: abaqus job=job-name recover Abaqus/CAE Usage: Job module: job editor: toggle on Recover (Explicit) as the Job Type Truncating a step You can truncate an analysis step prior to its completion when you restart the analysis. For example, by default, if the previous analysis is an Abaqus/Standard procedure and you specify that the restart point is Step p, the restart analysis will restart from the last saved increment of Step p and continue the step to completion. However, if you specify that the restart point is increment n of Step p and that the step should be terminated before restart, the restart analysis will restart from increment n of Step p, end Step p at that point, and continue with newly defined steps. In this case the step from which the analysis is being restarted will be truncated at the time of restart, regardless of the step end time that had been given in the previous analysis. Thus, the step is considered to be completed even though all of the loading may not have been applied. Continuation of the analysis will be defined by history data provided in the restart run. When you truncate an analysis step in an Abaqus/Explicit restart analysis, you must specify the interval after which the analysis should be restarted. When you truncate an analysis step in an Abaqus/CFD restart analysis, you must specify the increment after which the analysis should be restarted. If the step from which the restart is being made completed normally, you can truncate the step to restart within the step so that you can request additional output, write to the restart file with a higher frequency, etc. In Abaqus/Explicit it may be necessary to truncate an analysis step when an unforeseen event occurs within a step; for example, if contact surface definitions require modification due to unforeseen displacements. If the step from which the restart is being made completed normally and the restart is being made from the last increment, iteration, or interval, truncating the analysis step will have no effect. If the restart is being made from a job that was truncated by the operating system (for example, because of insufficient disk space, run-time limit exceeded, etc.), you will usually not choose to truncate the analysis step, so that the old step will first be completed before a new step—if any exists—is started. If restart is being made from the end of a step that terminated prematurely inside Abaqus (for example, because it ran out of increments or it failed to converge), you must truncate the step and include a new step definition. If you do not truncate the step, Abaqus will try to continue the old step upon restart and will terminate the analysis in the same manner as before. Use the following option in Abaqus/Standard to restart from any analysis step other than a direct cyclic step: RESTART *RESTART, READ, STEP=p, INC=n, END STEP Use the following option in Abaqus/Standard to restart from a direct cyclic analysis step: *RESTART, READ, STEP=p, ITERATION=n, END STEP Use the following option in Abaqus/Standard to restart from a low-cycle fatigue analysis step: *RESTART, READ, STEP=p, CYCLE=n, END STEP Use the following option in Abaqus/Explicit: *RESTART, READ, STEP=p, INTERVAL=n, END STEP Any module: Model→Edit Attributes→model_name: Restart: toggle on Read data from job; Step name: step; toggle on Restart from increment, interval, iteration, or cycle, enter the increment, interval, iteration, or cycle; and toggle on and terminate the step at this point Abaqus/CAE Usage: Amplitude references Care should be taken if loads and boundary conditions refer to amplitude curves (“Amplitude curves,” Section 33.1.2). If the amplitude is given in terms of total time, the loads and boundary conditions will continue to be applied according to the amplitude definition. However, if the amplitude is given in terms of step time (default), the loads and boundary conditions will be held constant at their values at the time the step is terminated. Temperatures, field variables, and mass flow rates applied in the old step will remain in the new step if they are not redefined. If an amplitude curve was not specified, these quantities will continue to be applied according to the default amplitude for the procedure. Automatic stabilization in Abaqus/Standard In Abaqus/Standard care should be exercised when automatic stabilization is active at the point at which a step is truncated. This may happen either in the middle of quasi-static procedures using automatic stabilization or during contact analyses using automatic viscous damping . In such cases viscous forces may be present, which will not be carried over to the subsequent step, therefore causing convergence difficulties. In the case of quasi-static procedures using automatic stabilization it is recommended that the stabilization continue to be enforced during the following step and that you specify the damping factor directly, using the last value printed out by Abaqus/Standard in the message file. In the case of automatic viscous damping in a contact pair when contact has not yet been fully established, it is recommended that the damping be applied again, although there is no guarantee that the amount of damping applied will be the same as in the original step. Choosing the initial time increment for an Abaqus/Standard restart analysis In Abaqus/Standard take care in choosing the time period and initial time increment for the new step if the previous step was truncated. In transient analyses the initial time increment for the new step should be similar to the time increment that was used at the point of restart in the old step. In quasi-static analyses choose the initial time increment of the new step so that the increments in loads or prescribed boundary conditions are similar to those at the point of restart in the old step. In a nonlinear analysis the increment of load applied in the first increment of the restart run should be similar to that applied in the last converged increment of the previous run. Let = the load to be applied in the first increment of the restart run, = the remaining load to be applied in the restart run, = the initial time increment for the restart run, and = the total step time for the first step of the restart run. The following equation can then be used to determine the initial time increment for the restart run: Example Suppose an Abaqus/Standard job stopped running because it reached the maximum number of increments specified for the step. The original input file was as follows: *HEADING … *STEP, INC=4 *STATIC, DIRECT 0.1, 1.0 *CLOAD 1, 2, 20.0 *RESTART, WRITE, FREQUENCY=2 *END STEP This run ended at Step 1, increment 4 with a load of 8.0 applied. The following input file could be used to restart this job and to complete the loading: *HEADING *RESTART, READ, STEP=1, INC=4, END STEP *STEP, INC=120 *STATIC, DIRECT 0.1, 0.6 *CLOAD 1, 2, 20.0 *END STEP Notice that the concentrated load applied is the same as in the previous step. In this example assume that a load increment of 2.0 was applied in the last converged increment of the previous run. Therefore, the initial time increment for the restart run is chosen such that the load increment applied during the first increment is also 2.0. The remaining load to be applied in the restart run is 12.0 (20.0 total − 8.0 applied in the previous run). Substitution into the equation for the initial time increment yields , is chosen to be 0.6 so that the total accumulated time is 1.0 when the applied load is 20.0 (at the end of the step). Thus, the initial time increment for the restart run, /6. The step time for the first step of the restarted job, , is set equal to 0.1. = Supplying additional data in the restart analysis It is possible to define steps subsequent to the step at which restart is being made. It is also possible to supply new amplitude definitions, new surfaces, new node sets, and new element sets during the restart analysis. Existing sets cannot be modified. In Abaqus/Standard additional surfaces defined in the model part of a restart analysis have the restriction that they can be referenced only from surface-based loading definitions or output requests for user-defined surface sections . Example For example, suppose a one-step Abaqus/Explicit job stopped prior to completion because a CPU time limit was exceeded and you have decided that a second step should be added with new boundary condition definitions. The following input file could be used to restart this job, complete the remaining part of Step 1, and complete Step 2: *HEADING *RESTART, READ, STEP=1 ** ** This defines Step 2 ** *STEP *DYNAMIC, EXPLICIT , .003 *BOUNDARY, OP=NEW … *END STEP Continuation of optional history data in restart analyses The rules governing the continuation of optional analysis history data—loading, boundary conditions, output controls, and auxiliary controls —are the same for the steps defined in the restart analysis and the original analysis. For a discussion of the rules governing the continuation of optional history data, see “Defining an analysis,” Section 6.1.2. Prescribing predefined fields in the restart analysis It is possible to prescribe predefined fields in the restart analysis. To specify predefined temperatures or field variables in an Abaqus/Standard restart analysis, the corresponding predefined field must have been specified in the original analysis as initial temperatures or field variables (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) or as predefined temperatures or field variables (“Predefined fields,” Section 33.6.1). Restarting with user subroutines User subroutines are not written to the Abaqus/Standard restart file or to the Abaqus/Explicit state file. Therefore, if the original analysis contained any user subroutines, these subroutines must be included again in the restart run or when recovering additional results output from restart data . These subroutines can be modified on restart; however, modifications should be made with caution because they may invalidate the solution from which the restart is being made. Simultaneously reading and writing a restart file You can continue a previous analysis as a restart analysis and write the results from the restart analysis to a new restart file or state file. For example, if the previous analysis is an Abaqus/Explicit procedure and in the current analysis you specify that the restart point is Step p and the restart output frequency is n, the analysis will be restarted from the last saved interval of Step p and restart states will be written in subsequent steps based on the new value of n. To discontinue the writing of a restart file in Abaqus/Standard when you are restarting a previous analysis, specify a restart output frequency of 0; if you do not specify a frequency, the file will continue to be written at the frequency defined for the previous analysis. The new restart file Restart files can be very large for large models or for jobs involving many restart increments (unless you choose to overlay the restart data—see “Overlaying results in the restart files”). Therefore, the previous restart file is not copied to the beginning of the new restart file when a job is restarted: only the data at restart increments requested in the current run are saved to the new restart file. However, if an eigenfrequency extraction step (“Natural frequency extraction,” Section 6.3.5) is restarted and additional eigenvalues are requested, the new restart file will contain those eigenvalues that converged during the first run as well as the additional eigenvalues. Example: Abaqus/Standard Suppose an Abaqus/Standard job stopped running because it ran out of disk space. The last complete information for an increment in the restart file is from Step 2, increment 4. The following two-line input file could be used to restart this job and continue writing the restart file: *HEADING *RESTART, READ, STEP=2, INC=4, WRITE Example: Abaqus/Explicit Suppose you stopped an Abaqus/Explicit job because too much output was being generated. The last information in the state file is from Step 2, Interval 4 at a time of .004. Step 2 has a time period of .010 and restart results were requested at 10 intervals. The following input file could be used to restart this job and redefine the remainder of the step with reduced output requests: *HEADING *RESTART, READ, END STEP, STEP=2, INTERVAL=4 *STEP *DYNAMIC, EXPLICIT , .006 *RESTART, WRITE, NUMBER INTERVAL=2 *END STEP Continuation of output upon restart When you restart an analysis, Abaqus creates a new output database file (job-name.odb) and a new results file (job-name.fil; this file is not created in Abaqus/CFD) and writes output data to those files according to the criteria described below. Output database (.odb) files The Abaqus output database file (job-name.odb) contains results that can be used for postprocessing in Abaqus/CAE. By default, the output database file is not made continuous across restarts; Abaqus creates a new output database file each time a job is run. You can combine X–Y data extracted from multiple output database files in the Visualization module of Abaqus/CAE. Alternatively, you can also join field and history results from an original analysis and a restart analysis by running the abaqus restartjoin execution procedure. For more information, see “Joining output database (.odb) files from restarted analyses,” Section 3.2.18. Results (.fil) files The Abaqus results file created in Abaqus/Standard and Abaqus/Explicit (job-name.fil) contains user-specified results that can be used for postprocessing in external postprocessing packages. In Abaqus/Explicit results are also written to the selected results file (job-name.sel), which is then converted to the results file for postprocessing. See “Output,” Section 4.1.1, for details. Upon restart Abaqus/Standard will copy the information from the old results file into the results file for the new job up to the restart point and begin writing the new results to the new file following that point. Abaqus/Explicit will copy the information from the old selected results file into the selected results file for the new job up to the restart point and begin writing the new results to the new file following that point. If the old results file is not provided, Abaqus/Standard will continue the analysis, writing the results of the restart analysis only to the new results file. Therefore, you will have segments of the analysis results in different files, which should be avoided in most cases since postprocessing programs assume that the results are in a single continuous file. You can merge such segmented results files, if necessary, by using the abaqus append execution procedure (“Joining results (.fil) files,” Section 3.2.12). Restart compatibility A restart analysis in Abaqus/Standard can use the restart files generated from the same or any previous maintenance delivery of the same general release. For example, if the original analysis is executed with the Abaqus 6.12-3 maintenance delivery, all subsequent Abaqus 6.12 maintenance deliveries can be used to launch the restart analysis. Restart is not compatible between general releases (for example, between Abaqus 6.11 and Abaqus 6.12). In Abaqus/Explicit and Abaqus/CFD the original analysis and the restart analysis must use precisely the same release. For example, if the original analysis is executed with the Abaqus 6.12-3 maintenance delivery, only this exact release can be used to launch the restart analysis. A restart analysis in Abaqus and a recover analysis in Abaqus/Explicit must be run on a computer that is binary compatible with the computer used to generate the restart files. 9.2 Importing and transferring results • “Transferring results between Abaqus analyses: overview,” Section 9.2.1 • “Transferring results between Abaqus/Explicit and Abaqus/Standard,” Section 9.2.2 • “Transferring results from one Abaqus/Standard analysis to another,” Section 9.2.3 • “Transferring results from one Abaqus/Explicit analysis to another,” Section 9.2.4 TRANSFERRING RESULTS BETWEEN Abaqus ANALYSES: OVERVIEW TRANSFERRING RESULTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Transferring results between Abaqus/Explicit and Abaqus/Standard,” Section 9.2.2 • “Transferring results from one Abaqus/Standard analysis to another,” Section 9.2.3 • “Transferring results from one Abaqus/Explicit analysis to another,” Section 9.2.4 • *IMPORT • *IMPORT ELSET • *IMPORT NSET • *IMPORT CONTROLS • *INSTANCE • “Transferring results between Abaqus analyses,” Section 16.6 of the Abaqus/CAE User’s Manual Overview Abaqus provides the capability to import a deformed mesh and its associated material state from Abaqus/Standard into Abaqus/Explicit and vice versa. in manufacturing problems; for example, the entire sheet metal forming process (which requires an initial preloading, forming, and subsequent springback) can be analyzed. In this case the initial preloading can be simulated with Abaqus/Standard using a static procedure and the subsequent forming process can be simulated with Abaqus/Explicit. Finally, the springback analysis can be performed with Abaqus/Standard. This capability is particularly useful Abaqus also provides the capability to transfer desired results and model information from an Abaqus/Standard analysis to a new Abaqus/Standard analysis or from an Abaqus/Explicit analysis to a new Abaqus/Explicit analysis, where additional model definitions may be specified before the analysis is continued. For example, during an assembly process an analyst may first be interested in the local behavior of a particular component but later is concerned with the behavior of the assembled product. In this case the local behavior can first be analyzed in an Abaqus/Standard or Abaqus/Explicit analysis. Subsequently, the model information and results from this analysis can be transferred to a second Abaqus/Standard or Abaqus/Explicit analysis, where additional model definitions for the other components can be specified, and the behavior of the entire product can then be analyzed. For this capability to work, the same release of Abaqus/Explicit and Abaqus/Standard must be run on computers that are binary compatible. In addition, you can transfer model and results only from one previous analysis; transfer from multiple analyses is not supported. Saving the analysis results The restart files from the original analysis contain the analysis results that are transferred from Abaqus/Standard or Abaqus/Explicit. Obtaining restart files is described in more detail in “Writing restart files” in “Restarting an analysis,” Section 9.1.1; brief summaries are provided below. By default, Abaqus/Standard does not write any restart information and Abaqus/Explicit writes results at the beginning and end of each step. Saving results from Abaqus/Standard If the results are to be imported from an Abaqus/Standard analysis, the results from the original Abaqus/Standard job must be written to the restart (.res), analysis database (.mdl and .stt), part (.prt), and output database (.odb) files. You can specify the increments at which restart information will be written. Restart information is always written at the end of a step in addition to the requested increments whenever you request restart data in Abaqus/Standard. *RESTART, WRITE, FREQUENCY=n Step module: Output→Restart Requests: enter n in the Frequency column for each step Abaqus/CAE Usage: Input File Usage: Saving results from Abaqus/Explicit If the results are to be imported from an Abaqus/Explicit analysis, the results from the original Abaqus/Explicit job must be written to the state (.abq) file at the time when transfer of the state of the deformed body is required. The state (.abq), restart (.res), analysis database (.stt), package (.pac), part (.prt), and output database (.odb) files will be used for importing the results from Abaqus/Explicit. You can specify whether the results are to be written at the exact time dictated by the specified time interval, n, during a step of an Abaqus/Explicit analysis or at the increment ending after the time dictated by the specified time interval. Results are always written at the end of a step, so it is not necessary to request results at the exact time intervals if results will be read only from the end of a step. Input File Usage: Use the following option to request immediately after each time interval: results at the increments ending Abaqus/CAE Usage: *RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=NO Use the following option to request results at the exact time intervals: *RESTART, WRITE, NUMBER INTERVAL=n, TIME MARKS=YES Step module: Output→Restart Requests: enter n in the Number Interval column; click to check the Time Marks column for each step if you want the results written at the exact time intervals Specifying the transfer of model data and results The import capability is used to transfer model data and results from one analysis to another. The following sections describe how to specify the import request. You can import element sets from models that are not defined as assemblies of part instances, or you can import part instances from models that are defined as assemblies of part instances. In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Specifying the transfer of model data and results for models that are not defined as assemblies of part instances You can import element sets from a previous analysis to specify the transfer of model data and results for models that are not defined as assemblies of part instances. This import capability is illustrated in “Springback of two-dimensional draw bending,” Section 1.5.1 of the Abaqus Example Problems Manual, and “Axisymmetric forming of a circular cup,” Section 1.3.7 of the Abaqus Example Problems Manual. Input File Usage: Use the following option to import element sets from a previous analysis: *IMPORT list of element sets that are to be imported To prevent any ambiguity regarding element and node definitions, the *IMPORT option must be specified before any options that define additional model data in the input file. In addition, the *IMPORT option can be specified only once. Each element set name specified on the data line of the *IMPORT option must have been used in a section definition option (e.g., *SOLID SECTION) in the original analysis. An element set can contain no more than three different types of elements. Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Specifying the transfer of model data and results for models that are defined as assemblies of part instances You can import part instances from a previous analysis to specify the transfer of model data and results for models that are defined as assemblies of part instances. If you import more than one part instance, the part instances must be from the same output database (.odb) file and all import parameters must be the same for each imported part instance. Each instance name that you specify must be the same as the instance name in the original analysis. Only sets that are defined within the imported instance will be imported. Sets defined at the assembly level must be redefined in the import analysis. New set definitions and surface definitions can be added upon import. You cannot assign new sections, material orientations, normals, or beam orientations to the imported part instance. Input File Usage: Use the following options to import a part instance from a previous analysis: *INSTANCE, INSTANCE=instance-name Abaqus/CAE Usage: Additional set and surface definitions (optional) *IMPORT *END INSTANCE In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: select the instances to which the initial state should be assigned Identifying the analysis from which the data will be obtained You must specify the name of the job from which the model and results data will be obtained. Input File Usage: For all models you can enter the following input on the command line: abaqus job=job-name oldjob=oldjob-name If the oldjob parameter is omitted, Abaqus will prompt for the job name even if the current job is an Abaqus/Explicit analysis that uses the recover option to restart from the last available step and increment in the state file. Alternatively, for models defined as assemblies of part instances, you can use the following option: *INSTANCE, LIBRARY=oldjob-name If you import more than one part instance, the oldjob-name specified by the LIBRARY parameter must be the same for each imported part instance. If the job name is specified on the command line using the oldjob option, the command line specification will take precedence over the LIBRARY parameter. Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: Job name: output-database-name Importing model data Element property definitions of imported elements can be redefined only if the reference configuration is updated and the material state is not imported . In this case the material orientation definitions (“Orientations,” Section 2.2.5), hourglass stiffness but not hourglass control definitions, and transverse shear stiffness definitions (in the case of shell elements) of the imported elements can also be redefined. For other reference configuration and material state combinations, the information required to define the section for each imported element will be imported from the original analysis. Material orientations cannot be redefined in the import analysis; orientation names cannot be reused in the import analysis. For imported elements, the material orientations will be transferred from the original analysis. Transverse shear stiffness for imported shell elements cannot be redefined; the values will be transferred from the original analysis. Hourglass stiffness for the imported elements cannot be redefined in an Abaqus/Standard import analysis; the default values will be used. The section control definitions (kinematic formulation, order of accuracy in the element formulation, and hourglass control approach) to be used for imported elements cannot be redefined . Only nodes associated with the imported elements are imported. New nodes can be defined in the import analysis. Nodes or elements that use the same numbers as nodes or elements being imported can be defined provided that the reference configuration is updated, the material state is not imported, and the import is not done from an instance library. The new definitions will overwrite the imported definitions. If the reference configuration is not updated, new nodes or elements cannot use the imported node and element numbers irrespective of whether or not the material state is imported. During results transfer from an Abaqus/Standard analysis to another Abaqus/Standard analysis or from an Abaqus/Explicit to another Abaqus/Explicit analysis, the coordinates of imported nodes can be modified from their imported values by respecifying the nodal definitions if the reference configuration is updated and the material state is not imported. This modification of the coordinates of imported nodes is not allowed during transfer of results from Abaqus/Explicit to Abaqus/Standard or vice versa. Importing model data defined by a distribution While transferring results from one Abaqus/Standard analysis to another Abaqus/Standard analysis, most element or material properties defined by a distribution are imported along with the elements. The only exceptions are spatially varying thicknesses and orientation angles defined on the layers of composite shells and solids; in this case Abaqus issues an error message during input file preprocessing. While transferring results from an Abaqus/Explicit analysis to an Abaqus/Standard analysis, the only spatially varying element properties defined by a distribution that can be imported are shell thicknesses and section orientations for shell and solid elements. If any other element or material properties are defined with a distribution, Abaqus issues an error message during input file preprocessing. While transferring results from an Abaqus/Standard analysis to an Abaqus/Explicit analysis or from an Abaqus/Explicit analysis to another Abaqus/Explicit analysis, the only spatially varying element properties defined by a distribution that can be imported are shell thicknesses, section orientations for shell and solid elements, orientation angles defined for shell sections on the layers of composite shells, and section stiffness matrices specified directly for general shell sections. If any other element or material properties are defined with a distribution, Abaqus issues an error message during input file preprocessing. Section and material properties of imported elements can be redefined with distributions only if the reference configuration is updated and the material state is not imported . In this case the material orientation definitions (“Orientations,” Section 2.2.5), hourglass stiffness but not hourglass control definitions, and transverse shear stiffness definitions (in the case of shell elements) of the imported elements can also be redefined. Importing results from an Abaqus/Standard analysis (other than a direct cyclic analysis) If the results are imported from an Abaqus/Standard analysis, you can specify the step and increment in the restart file for which the results are to be imported. By default, the results written at the end of the analysis are imported. Input File Usage: *IMPORT, STEP=step, INCREMENT=increment For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition. Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: select instances: Step: select Specify: step and Frame: select Specify: increment Importing results from an Abaqus/Standard direct cyclic analysis If the results are imported from a direct cyclic analysis, you can specify the step and iteration number in the restart file for which the results are to be imported. By default, the results written at the end of the analysis are imported. Input File Usage: *IMPORT, STEP=step, ITERATION=iteration For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition. Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: select instances: Step: select Specify: step and Frame: select Specify: iteration Importing results from an Abaqus/Explicit analysis If the results are imported from an Abaqus/Explicit analysis, you can specify the step and interval in the state file for which the results are to be imported. By default, the results written at the end of the analysis are imported. Input File Usage: *IMPORT, STEP=step, INTERVAL=interval For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition. Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: select instances: Step: select Specify: step and Frame: select Specify: interval Updating the reference configuration Once the current model configuration of an Abaqus analysis is imported into Abaqus/Explicit or Abaqus/Standard, the analysis can be continued with or without updating the reference configuration If the reference configuration is not updated to be the imported to be the imported configuration. configuration, the displacements and strains are reported as total values relative to the original reference configuration and will, hence, be continuous. If the reference configuration is updated to be the imported configuration, displacements and strains reported in the import analysis are the total values relative to the updated reference configuration. This choice is useful if results need to be displayed relative to the imported configuration, such as may be desirable in springback analysis. The reference configuration cannot be updated if the imported analysis is geometrically linear. The choice of whether or not to update the reference configuration can influence strain-free nodal adjustments associated with contact initialization in Abaqus/Standard. Strain-free adjustments can be used to resolve penetrations or gaps that exist in the reference configuration in Abaqus/Standard, so prior displacements are not considered by the strain-free adjustment algorithm upon import if the reference configuration is not updated. Strain-free nodal adjustments in Abaqus/Explicit are based on the current configuration rather than the reference configuration, so these adjustments are not sensitive to whether the reference configuration is updated in Abaqus/Explicit. Further details on strain-free adjustments are provided in “Default contact initialization method” in “Controlling initial contact status in Abaqus/Standard,” Section 35.2.4; “Controlling initial contact status in Abaqus/Standard,” Section 35.2.4; “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 35.4.4; and “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 35.5.4. If connector elements are imported, the configuration can be updated provided that the state is not imported. Input File Usage: Use the following option to specify that the reference configuration is to be updated to the imported configuration: *IMPORT, STEP=step, UPDATE=YES Use the following option to specify that the reference configuration should not be updated to the imported configuration: *IMPORT, STEP=step, UPDATE=NO For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition. Abaqus/CAE Usage: In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Initial State for the Types for Selected Step: toggle Update reference configuration on or off Importing the material state You can specify whether or not the associated material state should be imported. If you choose to import the material state, the following are imported: • stresses; • equivalent plastic strains; • back stresses for the kinematic hardening models; • user-defined state variables; • damage-related state variables for the concrete damaged plasticity model; • damage-related state-variables for traction-separation response with cohesive elements; • damage-related state variables for ductile metals; • damage-related state variables for fiber-reinforced composites; • maximum deviatoric strain energy density during deformation history for Mullins effect; • internal strains and stresses for viscoelastic material models; and • connector state variables such as plastic strains, frictional slip, and damage state. Thus, the state is imported correctly for further analysis only for the following: • linear elasticity, • Mises plasticity (including the kinematic hardening models), • extended Drucker-Prager plasticity, • crushable foam plasticity, • Mohr-Coulomb plasticity, • critical state (clay) plasticity, • cast iron plasticity, • concrete damaged plasticity, • hyperelasticity (including Mullins effect), • hyperfoam, • viscoelasticity, • traction-separation response with damage for cohesive elements, • damage for ductile metals, • damage for fiber-reinforced composites, • connector behavior, and • materials defined in user subroutines UMAT and VUMAT. For all other material models only stresses will be imported. No other state variables will be imported. If the material behavior is defined in a user subroutine, you must ensure that the UMAT and VUMAT are consistent. If connector elements are imported, the state can be imported provided that the configuration is not updated. Input File Usage: Use the following option to specify that the material state should be imported: Abaqus/CAE Usage: *IMPORT, STATE=YES Use the following option to specify that the material state should not be imported: *IMPORT, STATE=NO For models that are defined as assemblies of part instances, the *IMPORT option must appear within a part instance definition. In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. Abaqus/CAE always imports the material state. If you want to import only the deformed mesh, you can import an orphan mesh from a selected step and increment of an output database; see “What kinds of files can be imported and exported from Abaqus/CAE?,” Section 10.1.1 of the Abaqus/CAE User’s Manual. Defining constraints upon import Most constraints (such as multi-point constraints and surface-based tie constraints) are not imported from the original analysis and must be redefined in the import analysis. Using the reference configuration of the original analysis without update ensures identical reproduction of these constraints in the import analysis. If a new constraint is defined in the import analysis, it is important to ensure that the constraint is not in violation either in the reference configuration or in the starting configuration of the import analysis. These two configurations are one and the same for newly introduced nodes. If a new constraint involves nodes of the original analysis, it is appropriate to update the reference configuration for the import analysis . In an Abaqus/Standard analysis with adaptive meshing and acoustic-to-structure tie constraints, the structural as well as the acoustic nodes may move from their initial positions. When such acoustic and structure meshes are imported from Abaqus/Standard into Abaqus/Explicit without updating the reference configuration, the acoustic elements at the interface may appear distorted when viewed in the undeformed plot mode in the Visualization module of Abaqus/CAE. This distortion appears because the reference configuration for the acoustic nodes is updated automatically while the configuration for the non-acoustic nodes is not. The deformed plot at time=0 displays the correct mesh. Importing element set and node set definitions All element set and node set definitions associated with the imported elements are imported by default. For models that are not defined as assemblies of part instances, you can also selectively import only specified element set or node set definitions. This capability provides a convenient way of selectively reusing the element or node sets defined in the original analysis. However, any members of such sets that do not belong to the imported elements are removed from the specified sets. For example, suppose three element sets—SHELL3D, MEMB, and ALL—are defined in the original analysis. Element set ALL contains all of the elements in element sets SHELL3D and MEMB, as well as other elements. You choose to import only the element sets SHELL3D and MEMB (i.e., the elements in these sets as well as the element set definitions). In addition, you selectively import the element set definition ALL (but not the elements in this set). If element 100 belongs to element set ALL but not to either element set SHELL3D or element set MEMB, it will not be imported and will be removed from the list of elements belonging to element set ALL. The imported element set definitions are processed before any node or element definitions; therefore, even if element 100 is subsequently redefined in the import analysis, it will not belong to element set ALL (unless it is explicitly assigned to element set ALL in the import analysis). Only node and element sets defined in the original or previous import analysis are available for importing. New sets defined during a restart run cannot be imported. Input File Usage: Abaqus/CAE Usage: Use either or both of the following options immediately following the *IMPORT option to import selected element or node set definitions: *IMPORT ELSET *IMPORT NSET For models that are defined as assemblies of part instances, you cannot selectively import element and node set definitions. All element and node set definitions are imported automatically. In Abaqus/CAE you can import model data and results only from models that are defined as assemblies of part instances. You cannot selectively import element and node set definitions in Abaqus/CAE. All element and node set definitions are imported automatically. Specifying a tolerance for shell normals in the updated configuration When the imported configuration is updated upon import, the mesh discretization may not satisfy the mesh geometry checks imposed in Abaqus/Explicit or Abaqus/Standard to evaluate whether or not a mesh is reasonable. In the case of highly warped shell elements it is possible that the normal at the center of the element that is calculated from the midsurface interpolation may differ from the normal that is interpolated from the rotated normals at the nodes. If the difference exceeds the tolerance specified, the analysis will terminate. This suggests that a fine mesh may be required to model areas of high curvature change to achieve a successful analysis. The unit normal computed from the midsurface interpolation, , and that predicted by the interpolation of the rotated normals at the nodes, , must satisfy the condition: where you can specify the tolerance, = 0.1 is used. . If you do not specify a tolerance value, a default value of Input File Usage: If you update the reference configuration to be the imported configuration, you can specify a tolerance for error checking on shell normals: Abaqus/CAE Usage: *IMPORT CONTROLS, NORMAL TOL= The shell normal tolerance is not supported in Abaqus/CAE. 9.2.2 TRANSFERRING RESULTS BETWEEN Abaqus/Explicit AND Abaqus/Standard Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Transferring results between Abaqus analyses: overview,” Section 9.2.1 • *IMPORT • *IMPORT ELSET • *IMPORT NSET • *IMPORT CONTROLS • *INSTANCE • “Transferring results between Abaqus analyses,” Section 16.6 of the Abaqus/CAE User’s Manual Overview Abaqus provides the capability to import a deformed mesh and its associated material state from Abaqus/Standard into Abaqus/Explicit and vice versa. In addition, new model information can be specified during the import analysis. This capability is useful for problems that involve several analysis stages. For example, in manufacturing processes the preloading can be analyzed using Abaqus/Standard and the subsequent forming operation can be simulated using Abaqus/Explicit. Finally, the springback of the material can be performed in Abaqus/Standard. For this capability to work, the same release of Abaqus/Explicit and Abaqus/Standard must be run on computers that are binary compatible. Information about how to transfer results between Abaqus analyses is provided in “Transferring results between Abaqus analyses: overview,” Section 9.2.1. Specifying new data in an import analysis Additional model definitions such as new elements, nodes, surfaces, etc. can be defined during the import analysis. Initial conditions can also be specified during the import analysis. New model definitions New nodes, elements, and material properties can be added to the model in an import analysis once import has been specified. Nodal coordinates must be defined in the updated configuration, regardless of whether or not the reference configuration is updated on import . The usual Abaqus input can be used. Imported material definitions can be used with the new elements (which will need new section property definitions). Nodal transformation transformations (“Transformed coordinate systems,” Section 2.1.5) are not Nodal imported; transformations can be defined independently in the import analysis. Continuous displacements, velocities, etc. are obtained only if the nodal transformations in the import analysis are the same as those in the original analysis. Use of the same transformations is also recommended for nodes with boundary conditions or point loads defined in a local system. Specifying geometric nonlinearity in an import analysis By default, Abaqus/Standard uses a small-strain formulation (i.e., geometric nonlinearity is ignored) and Abaqus/Explicit uses a large-deformation formulation (i.e., geometric nonlinearity is included). For each step of an analysis you can specify which formulation should be used; see “Geometric nonlinearity” in “General and linear perturbation procedures,” Section 6.1.3, for details. The default value for the formulation in an import analysis is the same as the value at the time of import. Once the large-displacement formulation is used during a given step in any analysis, it will remain active in all the subsequent steps, whether or not the analysis is imported. If the small-displacement formulation is used at the time of import, the reference configuration cannot be updated. Specifying initial conditions for imported elements and nodes Initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) can be specified on the imported elements or nodes only under certain conditions. Table 9.2.2–1 lists the initial conditions that are allowed depending on whether or not the material state is imported . The reference configuration can be updated or not, as desired. Table 9.2.2–1 Valid initial conditions. Initial condition Hardening Relative density Rotational velocity Solution-dependent state variables Stress Velocity Void ratio Material state imported? No No Yes or No No No Yes or No No Procedures Results can be imported into Abaqus/Explicit only from a general analysis step involving static stress analysis, dynamic stress analysis, or steady-state transport analysis in Abaqus/Standard. Results transfer from linear perturbation procedures (“General and linear perturbation procedures,” Section 6.1.3) is not allowed. Abaqus/Standard offers several analysis procedures that can be used in an import analysis. These procedures can be used to perform an eigenvalue analysis, static or dynamic stress analysis, buckling analysis, etc. See “Solving analysis problems: overview,” Section 6.1.1, for a discussion of the available procedures. For springback analysis of a formed component the first step in the Abaqus/Standard analysis usually consists of a static analysis procedure so that the initial out-of-balance forces can be removed gradually from the system. The removal of these forces is performed automatically by Abaqus/Standard during the first static analysis step, as described below. If the first step in the Abaqus/Standard analysis is not a static step (such as a dynamic step), the analysis proceeds directly from the state imported from the Abaqus/Explicit analysis. Achieving static equilibrium when importing into Abaqus/Standard When the current state of a deformed body in an explicit dynamic analysis is imported into a static analysis, the model will not initially be in static equilibrium. Initial out-of-balance forces must be applied to the deformed body in dynamic equilibrium to achieve static equilibrium. Both dynamic forces (inertia and damping) and boundary interaction forces contribute to the initial out-of-balance forces. The boundary forces are the result of interactions from fixed boundary and contact conditions. Any changes in the boundary and contact conditions from the Abaqus/Explicit analysis to the Abaqus/Standard analysis will contribute to the initial out-of-balance forces. In general the instantaneous removal of the initial out-of-balance forces in a static analysis will lead to convergence problems. Hence, these forces need to be removed gradually until complete static equilibrium is achieved. During this process of removing the out-of-balance forces, the body will deform further and a redistribution of internal forces will occur, resulting in a new stress state. (This is essentially what occurs during “springback,” when a formed product is removed from the worktools.) When the first step in the Abaqus/Standard import analysis is a static procedure, the following algorithm is used to remove the initial out-of-balance forces automatically: 1. The imported stresses are defined at the start of the analysis as the initial stresses in the material. 2. An additional set of artificial stresses is defined at each material point. These stresses are equal in magnitude to the imported stresses but are of opposite sign. The sum of the material point stresses and these artificial stresses, thus, creates zero internal forces at the beginning of the step. 3. The internal artificial stresses are ramped off linearly in time during the first step. Thus, at the end of the step the artificial stresses have been removed completely and the remaining stresses in the material will be the residual stress state associated with static equilibrium. Once static equilibrium has been obtained, subsequent steps can be defined using any analysis procedure that would normally follow a static analysis in Abaqus. When the first step is not a static analysis, no artificial stress state is applied and the imported stresses are used in the internal force computations for the element. Boundary conditions Boundary conditions, including any connector motion, specified in the original analysis are not imported. They must be defined again in the import analysis. In some cases nonzero boundary conditions imposed in the original analysis need to be maintained at the same values in the import analysis when the imported configuration is not updated. In such cases you can prescribe a constant (step function) amplitude variation for the analysis step so that the newly applied boundary conditions are applied instantaneously and held at that value for the duration of the step. Alternatively, you can refer to an amplitude curve in the boundary condition definition . If boundary conditions in the original analysis are applied in a transformed coordinate system , the same coordinate system should be defined and used in the import analysis. For a discussion of applying boundary conditions, see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Loads Loads, including those applied for connector actuation, defined in the original analysis are not imported. Loads may, therefore, need to be redefined in the import analysis. There are no restrictions on the loads that can be applied when results are imported from one analysis to the other. In cases when the loads need to be maintained at the same values as in the original analysis, you can prescribe a constant (step function) amplitude variation for the analysis step to apply the loads instantaneously at the start of the step and hold them for the duration of the step. Alternatively, you can refer to an amplitude curve in the load definition . If point loads in the original analysis are applied in a transformed coordinate system and the loads must be maintained in the import analysis, the load application is simplified if the same coordinate system is defined and used in the import analysis. See “Applying loads: overview,” Section 33.4.1, for an overview of the loading types available in Abaqus. Predefined fields The field variables at nodes are not imported. If the elements being imported are coupled temperature- displacement elements, the temperature is imported if the associated material state is imported. The temperature is also imported for an adiabatic analysis if the associated material state is imported. For all other cases the temperatures at nodes are not imported. If the original analysis uses predefined temperature fields (“Predefined temperature” in “Predefined fields,” Section 33.6.1) to vary the temperatures at nodes, the import analysis will not be allowed to continue. If the original analysis uses predefined field variable definitions (“Predefined field variables” in “Predefined fields,” Section 33.6.1) to vary the field variables at nodes, the import analysis will be allowed to continue only if all the elements being imported are coupled temperature-displacement elements; however, the field variables are not imported. If the original analysis uses initial temperature (“Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) and field variable (“Defining initial values of predefined field variables” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) conditions, the import analysis will be allowed to continue only if all the elements being imported are coupled temperature-displacement elements. In addition, specification of initial conditions for temperatures and field variables is not allowed in an import analysis, unless all the elements being imported are coupled temperature-displacement elements. In this case initial conditions for temperatures and field variables can be specified on the imported nodes if the reference configuration is updated and the material state is not imported. Initial temperatures can be specified in the import analysis if it is an adiabatic analysis. Material options All material property definitions and the orientations associated with imported elements are imported by default. Material properties can be changed by respecifying the material property definitions with the same material name. All relevant material properties must be redefined since the old definitions that were imported by default will be overwritten. Material orientations associated with imported elements can be changed only if the reference configuration is updated and the material state is not imported; the material orientations associated with imported elements cannot be redefined for other combinations of the reference configuration and material state. When connector elements are imported, any associated connector behavior definitions are imported by default. The imported connector behavior definitions can be modified only if the state is not imported. If mass scaling (“Mass scaling,” Section 11.6.1) is used in Abaqus/Explicit, the scaled masses will not be transferred to the subsequent import analysis in Abaqus/Standard. The mass of the model for the Abaqus/Standard analysis will be based on either the imported or the redefined density definitions. The material model must be redefined in the import analysis if changes to material damping are required. When material definitions are changed, care must be taken to ensure that a consistent material state is maintained. It may sometimes be possible to simplify the material definition. For example, if a Mises plasticity model was used in the Abaqus/Explicit analysis and no further plastic yielding is expected in the Abaqus/Standard analysis (as is generally the case for springback simulations), a linear elastic material can be used for the Abaqus/Standard analysis. However, if further nonlinear material behavior is expected, no changes to the existing material definitions should be made. The history of the state variables will not be maintained if the material models are not the same in both the original analysis and the import analysis. Elements The import capability is available for first-order continuum, modified triangular and tetrahedral elements, conventional shell, continuum shell, membrane, beam (both linear and quadratic), pipe (linear), truss, connector, rigid, and surface elements that are common to both Abaqus/Explicit and Abaqus/Standard, as defined in Table 9.2.2–2. Table 9.2.2–2 Common element types that can be transferred between Abaqus/Explicit and Abaqus/Standard. Common element types CPS3, CPS3T, CPS4R, CPS4RT, CPS6M, CPS6MT CPE3, CPE3T, CPE4R, CPE4RT, CPE6M, CPE6MT CAX3, CAX3T, CAX4R, CAX4RT, CAX6M, CAX6MT C3D4, C3D4T, C3D6, C3D6T, C3D8, C3D8R, C3D8T, C3D8RT, C3D10M, C3D10MT M3D3, M3D4, M3D4R R2D2 R3D3, R3D4 RAX2 S4, S4R, S3R, S4RT, S3RT SC8R, SC8RT, SC6R, SC6RT SAX1 SFM3D3, SFM3D4R T2D2 T3D2 B21, B22, PIPE21 B31, B32, PIPE31 CONN2D21 , CONN3D21 AC2D3, AC2D4R, AC2D4, ACIN2D2 AC3D4, AC3D6, AC3D8R, AC3D8, ACIN3D3, ACIN3D4 ACAX3, ACAX4R, ACAX4, ACINAX2 COH2D4, COHAX4, COH3D6, COH3D8 1 Connector elements can be imported from Abaqus/Standard to Abaqus/Explicit; but not vice versa. When S3R shell elements are imported from Abaqus/Explicit into Abaqus/Standard, they are converted into degenerated S4R elements automatically. However, when S3R shell elements are imported from Abaqus/Standard into Abaqus/Explicit, they remain S3R elements. When C3D6 and C3D6T solid elements are imported from Abaqus/Explicit into Abaqus/Standard, the results at the single point integration are applied to both integration points in Abaqus/Standard and the full integration is used automatically. However, when C3D6 and C3D6T solid elements are imported from Abaqus/Standard into Abaqus/Explicit, only the results at the first integration point are imported and are used in the reduced integration. When quadrilateral and hexahedral acoustic finite elements are imported between Abaqus/Explicit and Abaqus/Standard, they are converted to or from reduced-integration types, as required. The following restrictions apply to the import capability: • Connector elements can be imported from Abaqus/Standard to Abaqus/Explicit but not vice versa. Further, if connector elements are imported, the configuration can be updated provided that the state is not imported and the state can be imported provided that the configuration is not updated. • Rebars defined using rebar layers (“Defining reinforcement,” Section 2.2.3) are imported provided the underlying elements are also imported. Rebar reinforcements defined using the embedded element technique (“Embedded elements,” Section 34.4.1) are imported if the host and embedded elements used in this definition are also imported. Rebars defined as an element property (“Defining rebar as an element property,” Section 2.2.4) cannot be imported. • Infinite elements and fluid elements cannot be imported. • Rigid elements for which the thickness is interpolated from the nodes in an Abaqus/Explicit analysis will not be imported into Abaqus/Standard. • A rigid body containing both deformable and rigid elements cannot be imported. A rigid body that includes rigid elements is imported when the element set used to define the rigid body is specified for import. A rigid body that includes deformable elements is imported into Abaqus/Explicit when the element set used to define the rigid body is specified for import. The imported rigid body definition is overwritten if it is respecified using the same element set. When the model is defined in terms of an assembly of part instances, the reference node of an imported rigid body must belong to an imported instance. • When a rigid body is imported, any associated data such as pin node sets and tie node sets are part of the imported definition. However, these sets as imported contain only those nodes that are connected to the imported elements. • Failed elements in Abaqus/Explicit will not be imported into Abaqus/Standard. • Elements that are being removed or are inactive in Abaqus/Standard will not be imported into Abaqus/Explicit. • Rigid surfaces will not be imported. When importing results from an Abaqus/Explicit analysis to an Abaqus/Standard analysis, each element set specified can contain only compatible element types listed in Table 9.2.2–3 and can contain at most three different element types. Table 9.2.2–3 Compatible element types. ACINAX2, ACIN2D2, ACIN3D3, ACIN3D4 CPE4R, CPE3, AC2D3, AC2D4 CPS4R, CPS3 CAX4R, CAX3, ACAX3, ACAX4 AC3D4, AC3D6, AC3D8, C3D8, C3D8R, C3D4, C3D6 M3D4R, M3D3, M3D4 R3D3, R3D4 S4R, S3R, SC6R, SC8R, S4 SFM3D3, SFM3D4R CAX6M, C3D10M C3D8T, C3D4T, C3D6T SC6RT, SC8RT, S4T, S4RT, S3T, S3RT Using section controls in an import analysis it is important that the When transferring results between Abaqus/Standard and Abaqus/Explicit, hourglass forces are computed consistently. The enhanced hourglass control formulation is recommended for computing hourglass forces in the original as well as all subsequent import analyses. Once section controls have been defined in the original analysis, they cannot be modified in any subsequent Abaqus/Standard or Abaqus/Explicit analysis. Therefore, if section controls are to be used in any one analysis in a series of import analyses, they must be specified in the very first analysis. The section controls specified for an element set in the original analysis will be used for the elements belonging to that element set in all subsequent import analyses. Section controls other than the hourglass control formulation have appropriate defaults depending on the type of analysis and, generally, do not need to be changed. Nondefault values can be chosen subject to certain restrictions. In an Abaqus/Standard analysis only the average strain kinematic formulation and second-order accurate element formulation are available; other kinematic formulations, element formulations, or section controls that are relevant only in an Abaqus/Explicit analysis can be specified in the Abaqus/Standard analysis. Such controls will be ignored in the Abaqus/Standard analysis but retained for the subsequent Abaqus/Explicit import analysis. If a kinematic formulation other than average strain is used for solid elements in the Abaqus/Explicit analysis, the differences in the kinematic formulations may lead to errors in Abaqus/Standard if the elements are distorted or undergo large rotations. Using the first-order accurate element in Abaqus/Explicit and the second-order accurate element formulation (the only available formulation) in Abaqus/Standard is not expected to cause significant errors, since the time increment size in Abaqus/Explicit is inherently small. One exception to this is when the Abaqus/Explicit analysis involves components undergoing several revolutions, in which case it is recommended that the second-order accurate element formulation be used in Abaqus/Explicit. formulation (default) Input File Usage: Use the following options in the original analysis: *MEMBRANE SECTION, CONTROLS=name1, ELSET=elset1 *SHELL SECTION, CONTROLS=name2, ELSET=elset2 *SHELL GENERAL SECTION, CONTROLS=name3, ELSET=elset3 *SOLID SECTION, CONTROLS=name4, ELSET=elset4 Use options similar to the following one in the original analysis: *SECTION CONTROLS, NAME=name1 Define section controls when you assign the element type in the original analysis: Mesh module: Mesh→Element Type: Element Controls Abaqus/CAE Usage: Membrane and shell element thickness computation The computations for membrane and shell element thicknesses are described below. Shell elements defined using a general shell section For shells defined using a general shell section, the current thickness is computed based on the effective Poisson’s ratio, which is 0.5 by default, in both Abaqus/Explicit and Abaqus/Standard. Input File Usage: Abaqus/CAE Usage: *SHELL GENERAL SECTION, POISSON= Property module: homogeneous or composite shell section editor: Section integration: Before analysis: Advanced: Section Poisson's ratio Shell elements defined using shell sections integrated during analysis and membrane elements For shells defined using shell sections integrated during analysis and for membranes in Abaqus/Standard, the current thickness is computed based on the effective Poisson’s ratio, which is 0.5 by default. In Abaqus/Explicit, on the other hand, the computation of the thickness could be based either on the effective Poisson’s ratio or the through-thickness strains, with the computation based on the through-thickness strains used by default. If you do not specify a section Poisson’s ratio for shell sections integrated during analysis or for membrane sections in an original Abaqus/Explicit or Abaqus/Standard analysis, the thickness computations in the original and all subsequent import analyses are carried out using the default methods. In other words, the thicknesses in all Abaqus/Standard analyses are computed using the default effective Poisson’s ratio of 0.5, while the thicknesses in all Abaqus/Explicit analyses are computed using the through-thickness strains. When the section Poisson’s ratio is assigned a numerical value in an original Abaqus/Standard or Abaqus/Explicit analysis, the thickness computations in the original analysis and all subsequent import analyses are performed using the specified value for the effective Poisson’s ratio. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *SHELL SECTION, POISSON= *SHELL SECTION, POISSON=MATERIAL *MEMBRANE SECTION, POISSON= *MEMBRANE SECTION, POISSON=MATERIAL Property module: Homogeneous or composite shell section editor: Section integration: During analysis: Advanced: Section Poisson's ratio Membrane section editor: Section Poisson's ratio Contact angle computation in SLIPRING-type connector elements The contact angle, , made by the belt wrapping around node b is computed automatically in Abaqus/Explicit, ignoring the value specified within the Abaqus/Standard analysis. Constraints Most types of kinematic constraints (including multi-point constraints and surface-based tie constraints) specified in the original analysis are not imported and must be defined again in the import analysis; however, embedded element constraints are imported by default. See “Kinematic constraints: overview,” Section 34.1.1, for a discussion of the various types of kinematic constraints. Interactions Contact definitions specified in the original analysis and the contact state are not imported. Contact can be defined again in the import analysis by specifying the surfaces and contact pairs; however, you may not be able to use the exact contact definitions that were used in the original analysis because of differences in the contact capabilities between Abaqus/Standard and Abaqus/Explicit. The contact constraint enforcement may be different in Abaqus/Standard and Abaqus/Explicit. Examples of potential causes for differences include: • Abaqus/Standard typically uses a “pure master-slave” approach, whereas Abaqus/Explicit typically uses a “balanced master-slave” approach. • Depending on the contact formulations used, Abaqus/Standard and Abaqus/Explicit sometimes treat shell thicknesses and midsurface offsets differently. Thus, when the contact conditions are defined in the import analysis, the contact state that existed in the previous analysis may not be reproduced at the beginning of the import analysis. This could lead to a redistribution of stresses and an analysis that differs from what you desire. In some cases this problem can be mitigated by using nondefault options, such as ignoring shell thicknesses in the contact calculations, to match behaviors in Abaqus/Standard and Abaqus/Explicit. For a detailed description of the contact capabilities in Abaqus and the differences in the contact capabilities between Abaqus/Standard and Abaqus/Explicit, see “Contact interaction analysis: overview,” Section 35.1.1. Output Output can be requested for an import analysis in the same way as for an analysis in which the results are not imported. The output variables available in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. The output variables available in Abaqus/Explicit are listed in “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The values of the following material point output variables will be continuous in an import analysis when the material state is imported: stress, equivalent plastic strain (PEEQ), and solution-dependent state variables (SDV) for UMAT and VUMAT. Similarly, for a connector behavior, the plastic relative displacement (CUP), kinematic hardening shift force (CALPHAF), overall damage (CDMG), damage initiation criteria (CDIF, CDIM, CDIP), friction accumulated slip (CASU), and connector status (CSLST, CFAILST) will be continuous. If the reference configuration is not updated, the displacements, strains, whole element variables, section variables, and energy quantities will be reported relative to the original configuration. Accelerations are recomputed at the start of an import analysis in Abaqus/Explicit and may be different from those obtained at the end of an Abaqus/Standard analysis. The differences in accelerations arise from the recalculation of the internal forces created by the imported stresses using the Abaqus/Explicit element formulation algorithms. If the reference configuration is updated, displacements, strains, whole element variables, section variables, and energy quantities will not be continuous in an import analysis and will be reported relative to the updated reference configuration. Time and step number will not be continuous between the original and the import analyses if the reference configuration is updated. Time and step number will be continuous only if the reference configuration is not updated. Limitations The import capability has the following known limitations. Where applicable, details are given in the relevant sections. • The same release of Abaqus/Explicit and Abaqus/Standard must be run on computers that are binary compatible. • The capability is not available for fluid elements; infinite elements; and spring, mass, dashpot, and rotary inertia elements. Connector elements can be imported from Abaqus/Standard to Abaqus/Explicit but not vice versa. See the discussion on “Elements” earlier in this section for further details. • If connector elements are imported, the configuration can be updated provided that the state is not imported and the state can be imported provided that the configuration is not updated. • All elements and nodes must be included in at least one set in the original analysis when importing part instances. • Node sets that are generated from existing element sets must be defined in the original analysis. • Surface definitions, contact pair definitions, and general contact definitions are not imported. Analytical rigid surfaces will not be imported. • If the material state is imported, only stresses will be imported for material models other than those defined by linear elasticity, hyperelasticity, Mullins effect, hyperfoam, viscoelasticity, Mises plasticity (including the kinematic hardening models), extended Drucker-Prager plasticity, crushable foam plasticity, Mohr-Coulomb plasticity, critical state (clay) plasticity, cast iron plasticity, concrete damaged plasticity, damage for cohesive elements, damage for ductile metals, or damage for fiber-reinforced composites. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details. • If the state is imported for connector elements with behavior defined, the plastic displacements, the frictional slip, and the damage state are imported and the connector forces are recomputed. Some of the connector output variables, such as CU, are also recomputed on import. The recomputed variables may differ slightly at the point of import due to precision and algorithmic differences between the two solvers across import. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details. • Temperatures and field variables at nodes are not imported. If the temperature is a state variable (as in an adiabatic analysis where temperature is an integration point quantity), it will be imported if the material state is imported. See the discussion on “Predefined fields” for details. • Loads, boundary conditions, multi-point constraints, and equations are not imported. • Kinematic and distributing coupling constraints are not imported. In addition, the reference node of a coupling constraint will not be imported unless the reference node is part of another element definition that is imported. • Element and contact pair removal and reactivation,” Section 11.2.1) cannot be used in the first step of an import analysis in Abaqus/Standard. It can be used in the subsequent steps. removal/reactivation (“Element and contact pair • In a series of Abaqus/Standard and Abaqus/Explicit import analyses in the order Abaqus/Explicit(1) → Abaqus/Standard(1) → Abaqus/Explicit(2) →Abaqus/Standard(2), if elements in an element set are removed in the Abaqus/Standard(1) analysis, the subsequent Abaqus/Standard(2) import analysis does not recognize that this element set was removed in a previous analysis and fails with an error message stating that the element set is not found in the restart file. Such failures can be avoided by using flattened input files and requesting only the active element sets for import. • Section controls must be defined in the original analysis if any of a series of import analyses uses nondefault element formulations since section controls cannot be changed in an import analysis. See the discussion on “Using section controls in an import analysis” earlier in this section. • The symmetric model generation capability (“Symmetric model generation,” Section 10.4.1) cannot be used in an import analysis in Abaqus/Standard. • The results file, restart file, or output database file generated during the import analysis is not appended to the results file, restart file, or output database file of the original analysis. • An Abaqus/Standard import analysis where the reference configuration is not updated is not allowed if the adaptive meshing capability (“ALE adaptive meshing: overview,” Section 12.2.1) was used in the previous Abaqus/Explicit analysis. • Mesh-independent spot welds and tie constraints are not imported. These constraints can be redefined in the import analysis and are formed using the reference configuration of the import model. If the reference configuration is updated, the redefined constraints may not match the old constraints exactly due to the differences in geometry. If new constraints are defined and the reference configuration of the import model is not updated, they may not initially be in compliance if the nodes involved in the constraint have nonzero displacements. This may cause numerical difficulty and potential abort of the import analysis. In this case it is recommended that you update the reference configuration upon import. • The first step after an import when the reference conference is updated should not be used to generate a substructure. • For beam structures that have acute curvatures and undergo large permanent changes in curvatures, slightly different equilibrated configurations will be seen when using import depending on whether or not the reference configuration is to be updated to the imported configuration . This configuration difference is due to beam element formulation differences between Abaqus/Standard and Abaqus/Explicit. Input file template Transferring results between Abaqus/Explicit and Abaqus/Standard using models that are not defined as assemblies of part instances: Abaqus/Explicit analysis: *HEADING … *MATERIAL, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP *DYNAMIC, EXPLICIT … *RESTART, WRITE, NUMBER INTERVAL=n *END STEP Abaqus/Standard analysis: *HEADING *IMPORT, STEP=step, INTERVAL=interval, STATE=YES, UPDATE=NO Data lines to specify element sets to be imported *IMPORT ELSET Data lines to specify element set definitions to be imported *IMPORT NSET Data lines to specify node set definitions to be imported ** *** Optionally redefine the material block ** *MATERIAL, NAME=mat1 *ELASTIC Data lines to redefine linear elasticity *PLASTIC Data lines to redefine Mises plasticity … *BOUNDARY Data lines to redefine boundary conditions *STEP, NLGEOM=YES *STATIC … *END STEP Transferring results between Abaqus/Standard and Abaqus/Explicit using models that are not defined as assemblies of part instances: Abaqus/Standard analysis: *HEADING … *MATERIAL, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP *STATIC … *RESTART, WRITE, FREQUENCY=n *END STEP Abaqus/Explicit analysis: *HEADING *IMPORT, STEP=step, INCREMENT=increment, STATE=YES, UPDATE=NO Data lines to specify element sets to be imported *IMPORT ELSET Data lines to specify element set definitions to be imported *IMPORT NSET Data lines to specify node set definitions to be imported ** *** Optionally redefine the material block ** *MATERIAL, NAME=mat1 *ELASTIC Data lines to redefine linear elasticity *PLASTIC Data lines to redefine Mises plasticity … *BOUNDARY Data lines to redefine boundary conditions *STEP *DYNAMIC, EXPLICIT … *END STEP Transferring results between Abaqus/Explicit and Abaqus/Standard using models defined as assemblies of part instances: Abaqus/Explicit analysis: *HEADING *PART, NAME=Part-1 Node, element, section, set, and surface definitions *END PART *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=i1, PART=Part-1 Additional set and surface definitions (optional) *END INSTANCE Assembly level set and surface definitions … *END ASSEMBLY *MATERIAL, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP *DYNAMIC, EXPLICIT … *RESTART, WRITE, NUMBER INTERVAL=n *END STEP Abaqus/Standard analysis: *HEADING Part definitions (optional) *ASSEMBLY, NAME=Assembly-1 *INSTANCE, INSTANCE=i1, LIBRARY=oldjob-name Additional set and surface definitions (optional) *IMPORT, STEP=step, INTERVAL=interval, STATE=YES, UPDATE=NO *END INSTANCE Additional part instance definitions (optional) Assembly level set and surface definitions … *END ASSEMBLY ** *** Optionally redefine the material block ** *MATERIAL, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP, NLGEOM=YES *STATIC … *END STEP Transferring results between Abaqus/Standard and Abaqus/Explicit using models defined as assemblies of part instances: Abaqus/Standard analysis: *HEADING *PART, NAME=Part-1 Node, element, section, set, and surface definitions *END PART *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=i1, PART=Part-1 Additional set and surface definitions (optional) *END INSTANCE Assembly level set and surface definitions … *END ASSEMBLY *MATERIAL, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP *STATIC … *RESTART, WRITE, FREQUENCY=n *END STEP Abaqus/Explicit analysis: *HEADING Part definitions (optional) *ASSEMBLY, NAME=Assembly-1 *INSTANCE, INSTANCE=i1, LIBRARY=oldjob-name Additional set and surface definitions (optional) *IMPORT, STEP=step, INCREMENT=increment, STATE=YES, UPDATE=NO *END INSTANCE Additional part instance definitions (optional) Assembly level set and surface definitions *END ASSEMBLY ** *** Optionally redefine the material block ** *MATERIAL, NAME=mat1 *ELASTIC Data lines to redefine linear elasticity *PLASTIC Data lines to redefine Mises plasticity … *BOUNDARY Data lines to redefine boundary conditions *STEP *DYNAMIC, EXPLICIT … *END STEP 9.2.3 TRANSFERRING RESULTS FROM ONE Abaqus/Standard ANALYSIS TO ANOTHER Products: Abaqus/Standard Abaqus/CAE References • “Transferring results between Abaqus analyses: overview,” Section 9.2.1 • *IMPORT • *IMPORT ELSET • *IMPORT NSET • *IMPORT CONTROLS • *INSTANCE • “Transferring results between Abaqus analyses,” Section 16.6 of the Abaqus/CAE User’s Manual Overview information from an Abaqus provides the capability to transfer desired results and model Abaqus/Standard analysis to a new Abaqus/Standard analysis, where additional model definitions may be specified before the analysis is continued. For example, during an assembly process an analyst may first be interested in the local behavior of a particular component but later is concerned with the behavior of the assembled product. In this case the local behavior can first be analyzed in an Abaqus/Standard analysis. Subsequently, the model information and results from this analysis can be transferred to a second Abaqus/Standard analysis, where additional model definitions for the other components can be specified, and the behavior of the entire product can then be analyzed. For this capability to work, the same release of Abaqus/Standard must be run on computers that are binary compatible. Information about how to transfer results between Abaqus analyses is provided in “Transferring results between Abaqus analyses: overview,” Section 9.2.1. Comparison with the restart capability Both the import and restart capabilities in Abaqus/Standard allow for the transfer of results and model information from one Abaqus/Standard analysis to another Abaqus/Standard analysis. However, the two capabilities have been designed for different applications. The restart capability allows a completed Abaqus/Standard analysis to be restarted and continued. The entire model and results from the original analysis are transferred to the restart run, where additional analysis steps can be defined. Not much new model data can be specified in the restarted analysis; only model information such as new amplitude definitions, new node sets, and new element sets are allowed. Detailed information on the restart capability is given in “Restarting an analysis,” Section 9.1.1. The import capability also allows a completed Abaqus/Standard analysis to be continued. In addition, this capability allows for the analysis to be continued with only desired components from the original analysis; the entire model need not be transferred. New model data—such as elements, nodes, surfaces, contact pairs, etc.—can be specified during the import analysis. During the import analysis it is possible to choose whether only model information from the previous analysis is to be transferred or if the results associated with that model also are to be transferred. For situations where the goal is to continue the original analysis with no change to the model information, it is recommended that the restart capability be used. For situations where the model information requires changes, or for cases where you require control over the transfer of results, the import capability should be used. Specifying new data in an import analysis Additional model definitions such as new elements, nodes, surfaces, etc. can be defined during the import analysis. Initial conditions can also be specified during the import analysis. New model definitions New nodes, elements, and material properties can be added to the model in an import analysis once import has been specified. Nodal coordinates must be defined in the updated configuration, regardless of whether or not the reference configuration is updated on import . The usual Abaqus/Standard input can be used. Imported material definitions can be used with the new elements (which will need new section property definitions). Nodal transformation transformations (“Transformed coordinate systems,” Section 2.1.5) are not Nodal imported; transformations can be defined independently in the import analysis. Continuous displacements, velocities, etc. are obtained only if the nodal transformations in the import analysis are the same as those in the original analysis. Use of the same transformations is also recommended for nodes with boundary conditions or point loads defined in a local system. Specifying geometric nonlinearity in an import analysis By default, Abaqus/Standard uses a small-strain formulation (i.e., geometric nonlinearity is ignored). For each step of an analysis you can specify whether or not geometric nonlinearity should be included; see “Geometric nonlinearity” in “General and linear perturbation procedures,” Section 6.1.3, for details. The default value for the formulation in an import analysis is the same as the value at the time of import. Once the large-displacement formulation is used during a given step in any analysis, it will remain active in all the subsequent steps, whether or not the analysis is imported. If the small-displacement formulation is used at the time of import, the reference configuration cannot be updated. Specifying initial conditions for imported elements and nodes Initial conditions can be specified on the imported elements or nodes only under certain conditions. Table 9.2.3–1 lists the initial conditions that are allowed depending on whether or not the material state is imported . The reference configuration can be updated or not, as desired, with one exception: for initial temperature or field variable conditions, the reference configuration must be updated. Table 9.2.3–1 Valid initial conditions. Initial condition Field variable Hardening Relative density Rotational velocity Solution-dependent state variables Stress Temperature Velocity Void ratio Material state imported? No No No Yes or No No No No Yes or No No Procedures Results can be imported only from a general analysis step involving static stress analysis, dynamic stress analysis, steady-state transport analysis, coupled temperature-displacement analysis, or thermal- electrical-structural analysis in Abaqus/Standard. Results transfer from linear perturbation procedures (“General and linear perturbation procedures,” Section 6.1.3) is not allowed. Abaqus/Standard offers several analysis procedures that can be used in an import analysis. These procedures can be used to perform an eigenvalue analysis, static or dynamic stress analysis, buckling analysis, etc. See “Solving analysis problems: overview,” Section 6.1.1, for a discussion of the available procedures. When results are transferred from an Abaqus/Standard dynamic analysis to another Abaqus/Standard analysis where the first step is a static procedure, the initial out-of-balance forces must be removed gradually from the system. The removal of these forces is performed automatically by Abaqus/Standard during the first static analysis step, as described below. If the first step in the Abaqus/Standard analysis is not a static step (such as a dynamic step), the analysis proceeds directly from the state imported from the previous Abaqus/Standard analysis. Achieving static equilibrium when importing from a dynamic analysis to a static analysis When the current state of a deformed body in a dynamic analysis is imported into a static analysis, the model will not initially be in static equilibrium. Initial out-of-balance forces must be applied to the deformed body in dynamic equilibrium to achieve static equilibrium. Both dynamic forces (inertia and damping) and boundary interaction forces contribute to the initial out-of-balance forces. The boundary forces are the result of interactions from fixed boundary and contact conditions. Any changes in the boundary and contact conditions will contribute to the initial out-of-balance forces. In general, the instantaneous removal of the initial out-of-balance forces in a static analysis will lead to convergence problems. Hence, these forces need to be removed gradually until complete static equilibrium is achieved. During this process of removing the out-of-balance forces, the body will deform further and a redistribution of internal forces will occur, resulting in a new stress state. (This is essentially what occurs during “springback,” when a formed product is removed from the worktools.) When the first step in the Abaqus/Standard import analysis is a static procedure, the following algorithm is used to remove the initial out-of-balance forces automatically: 1. The imported stresses are defined at the start of the analysis as the initial stresses in the material. 2. An additional set of artificial stresses is defined at each material point. These stresses are equal in magnitude to the imported stresses but are of opposite sign. The sum of the material point stresses and these artificial stresses, thus, creates zero internal forces at the beginning of the step. 3. The internal artificial stresses are ramped off linearly in time during the first step. Thus, at the end of the step the artificial stresses have been removed completely and the remaining stresses in the material will be the residual stress state associated with static equilibrium. Once static equilibrium has been obtained, subsequent steps can be defined using any analysis procedure that would normally follow a static analysis. When the first step is not a static analysis, no artificial stress state is applied and the imported stresses are used in the internal force computations for the element. Boundary conditions Boundary conditions specified in the original analysis are not imported; they must be redefined in the import analysis. In some cases nonzero boundary conditions imposed in the original analysis need to be maintained at the same values in the import analysis when the imported configuration is not updated. In such cases you can prescribe a constant (step function) amplitude variation for the analysis step so that the newly applied boundary conditions are applied instantaneously and held at that value for the duration of the step. Alternatively, you can refer to an amplitude curve in the boundary condition definition . If boundary conditions in the original analysis are applied in a transformed coordinate system , the same coordinate system should be defined and used in the import analysis. For discussions on applying boundary conditions and multi-point constraints, see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1, and “Kinematic constraints: overview,” Section 34.1.1. Loads Loads defined in the original analysis are not imported. Therefore, loads may need to be redefined in the import analysis. There are no restrictions on the loads that can be applied when results are imported from one analysis to the other. In cases when the loads need to be maintained at the same values as in the original analysis, you can prescribe a constant (step function) amplitude variation for the analysis step to apply the loads instantaneously at the start of the step and hold them for the duration of the step. Alternatively, you can refer to an amplitude curve in the load definition . If point loads in the original analysis are applied in a transformed coordinate system and the loads must be maintained in the import analysis, the load application is simplified if the same coordinate system is defined and used in the import analysis. See “Applying loads: overview,” Section 33.4.1, for an overview of the loading types available in Abaqus/Standard. Predefined fields Temperatures, whether they are prescribed or are degrees of freedom (as in a coupled thermal-stress analysis), and field variables at nodes are imported if the material state is imported. If the reference configuration is updated and the material state is imported, the initial conditions for temperatures and field variables at the imported nodes will be reset to the imported values; for example, the thermal strains will now be measured relative to the imported temperatures. If the reference configuration is updated but the material state is not imported, the initial conditions are reset to zero. In this case you can respecify the initial conditions on the imported nodes. If the temperature is a state variable (as in an adiabatic analysis where temperature is an integration point quantity), it will be imported if the material state is imported. Material options All material property definitions and orientations associated with imported elements are imported by default. Material properties can be changed by respecifying the material property definitions with the same material name. In this case all relevant material properties must be redefined since the old definitions that were imported by default will be overwritten. Material orientations associated with imported elements can be changed only if the reference configuration is updated and the material state is not imported; the material orientations associated with imported elements cannot be redefined for other combinations of the reference configuration and material state. The material model must be redefined in the import analysis if changes to material damping are required. When material definitions are changed, care must be taken to ensure that a consistent material state is maintained. It may sometimes be possible to simplify the material definition. For example, if a Mises plasticity model was used in the first Abaqus/Standard analysis and no further plastic yielding is expected in a subsequent Abaqus/Standard analysis, a linear elastic material can be used for the Abaqus/Standard analysis. However, if further nonlinear material behavior is expected, no changes to the existing material definitions should be made. The history of the state variables will not be maintained if the material models are not the same in both the original analysis and the import analysis. Elements The import capability is available for thermal-electrical-structural elements and a subset of the stress/displacement and coupled temperature-displacement continuum, shell, membrane, truss, rigid, and surface elements available in Abaqus/Standard. The complete list of supported elements is provided in Table 9.2.3–2. If elements that are removed are imported, they become active in the import analysis and should be removed in the first step of the import analysis. Table 9.2.3–2 Element types that can be transferred from one Abaqus/Standard analysis to another. Element Type Supported Elements Plane strain continuum CPE3, CPE3H, CPE3T, CPE4, CPE4H, CPE4HT, CPE4I, CPE4IH, CPE4R, CPE4RHT, CPE4RT, CPE4T CPE6, CPE6H, CPE6M, CPE6MH, CPE6MHT, CPE6MT, CPE8, CPE8H, CPE8HT, CPE8R, CPE8RH, CPE8RHT, CPE8RT, CPE8T Plane stress continuum CPS3, CPS3T, CPS4, CPS4I, CPS4R, CPS4T CPS6, CPS6M, CPS6MT, CPS8, CPS8R, CPS8RT, CPS8T Three-dimensional continuum Axisymmetric continuum C3D4, C3D4H, C3D4T, C3D6, C3D6H, C3D6T, C3D8, C3D8H, C3D8HT, C3D8I, C3D8IH, C3D8R, C3D8RH, C3D8RHT, C3D8RT, C3D8T, Q3D4, Q3D6, Q3D8, Q3D8H, Q3D8R, Q3D8RH C3D10, C3D10H, C3D10I, C3D10M, C3D10MH, C3D10MHT, C3D10MT, C3D15, C3D15H, C3D15V, C3D15VH, C3D20, C3D20H, C3D20HT, C3D20R, C3D20RHT, C3D20RT, C3D20T, C3D27, C3D27H, C3D27RH, Q3D10M, Q3D10MH, Q3D20, Q3D20H, Q3D20R, Q3D20RH CAX3, CAX3H, CAX3T, CAX4, CAX4H, CAX4HT, CAX4I, CAX4IH, CAX4R, CAX4RH, CAX4RHT, CAX4RT, CAX4T CAX6, CAX6M, CAX6MH, CAX6MHT, CAX6MT, CAX8, CAX8H, CAX8HT, CAX8R, CAX8RH, CAX8RHT, CAX8RT, CAX8T Membrane M3D3, M3D4R Element Type Supported Elements Two-dimensional rigid R2D2 Three-dimensional rigid R3D3, R3D4 Axisymmetric rigid RAX2 Three-dimensional shell S4R, S3R, S4RT, S3RT, S4T, S3T Axisymmetric shell SAX1 Continuum shell SC6RT, SC8RT Surface SFM3D3, SFM3D4R Two-dimensional truss T2D2, T2D2T Three-dimensional truss T3D2, T3D2T Cohesive COH2D4, COHAX4, COH3D6, COH3D8 The following element types cannot be imported: • Acoustic elements • Axisymmetric-asymmetric continuum and shell elements • Beam elements • Connector elements • Coupled thermal-electrical elements • Diffusive heat transfer/mass diffusion elements and forced convection/diffusion elements • Generalized plane strain elements • Gasket elements • Heat capacitance elements • Inertial elements (mass and rotary inertia) • Infinite elements • Piezoelectric elements • Special-purpose elements • Substructures • User-defined elements In addition, the following restrictions apply to the import capability: • Rebars defined using rebar layers (“Defining reinforcement,” Section 2.2.3) are imported provided the underlying elements are also imported. Rebar reinforcements defined using the embedded element technique (“Embedded elements,” Section 34.4.1) are imported if the host and embedded elements used in this definition are also imported. Rebars defined as an element property (“Defining rebar as an element property,” Section 2.2.4) cannot be imported. • A rigid body containing both deformable and rigid elements cannot be imported. A rigid body that includes rigid elements is imported when the element set used to define the rigid body is specified for import. A rigid body that includes deformable elements is imported when the element set used to define the rigid body is specified for import. The imported rigid body definition is overwritten if it is respecified using the same element set. When the model is defined in terms of an assembly of part instances, the reference node of an imported rigid body must belong to an imported instance. • When a rigid body is imported, any associated data such as pin node sets and tie node sets are part of the imported definition. However, these sets as imported contain only those nodes that are connected to the imported elements. Constraints Most types of kinematic constraints specified in the original analysis are not imported and must be defined again in the import analysis; however, surface-based tie constraints are imported by default. See “Kinematic constraints: overview,” Section 34.1.1, for a discussion of the various types of kinematic constraints. Interactions The various aspects of most surface-based mechanical contact definitions (including the surface, contact pair, and contact property definitions) can be imported. Thermal interactions, electrical interactions, and pore fluid surface interactions cannot be imported. Certain types of mechanical contact aspects—pressure, penetration loads, and debonded surfaces—cannot be imported. The most commonly used mechanical contact aspects—pressure-overclosure behavior, frictional behavior, and damping—can be imported. The ability to import element-based and node-based surfaces is determined by whether or not the underlying elements and nodes defining these surfaces are imported. If the underlying elements or nodes of a surface are not imported, that surface will not be imported. If only some of the underlying nodes or elements used in the original definition of the surface are imported, only that part of the surface corresponding to the imported elements will be imported. Rigid surface definitions are imported when the associated slave surface is also imported. Contact pair definitions are imported provided that all the slave and master surfaces used in the original definition of the contact pair are also imported. Contact conditions modeled with contact elements will be ignored during the transfer process. The contact state associated with a stress/displacement analysis is imported if the material state is imported. If the reference configuration is updated, the accumulated contact strains will be set to zero. The contact state associated with thermal, electrical, or pore fluid surface interactions is not imported. The contact state associated with a crack propagation analysis is not imported; initially bonded contact surface definitions are not transferred. If a contact pair was inactive in the step from which the import was done due to the use of contact pair removal , it must be deactivated again in the first step of the import analysis. Additional contact information can be defined in the import analysis by specifying new surfaces, contact pairs, and interactions. New contact pair definitions can use the imported surface interaction definitions. For a detailed description of the contact capabilities in Abaqus/Standard, refer to “Contact interaction analysis: overview,” Section 35.1.1. Output Output can be requested for an import analysis in the same way as for an analysis in which the results are not imported. Output requests in the original analysis are not transferred to the import analysis; output requests in the import analysis have to be respecified. The output variables available in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. The values of the following material point output variables will be continuous in an import analysis when the material state is imported: stress, equivalent plastic strain (PEEQ), and solution-dependent state variables (SDV) for UMAT. If the reference configuration is not updated, the displacements, strains, whole element variables, section variables, and energy quantities will be reported relative to the original configuration. If the reference configuration is updated, displacements, strains, whole element variables, section variables, and energy quantities will not be continuous in an import analysis and will be reported relative to the updated reference configuration. Time and step number will not be continuous between the original and the import analyses if the reference configuration is updated. Time and step number will be continuous only if the reference configuration is not updated. Limitations The import capability has the following known limitations. Where applicable, details are given in the relevant sections. • The same release of Abaqus/Standard must be run on computers that are binary compatible. • The capability is not available for fluid elements; infinite elements; and spring, mass, dashpot, rotary inertia, and connector elements. See the discussion on “Elements” earlier in this section for further details. • Surfaces are not imported when the model is defined as an assembly of part instances. • All elements and nodes must be included in at least one set in the original analysis when importing part instances. • The contact state associated with thermal, electrical, and pore fluid surface interactions is not imported; the contact state associated with crack propagation is not imported. • General contact definitions are not imported. • If the material state is imported, only stresses will be imported for material models other than those defined by linear elasticity, hyperelasticity, hyperfoam, viscoelasticity, Mises plasticity, and damage for cohesive elements. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details. • Loads, boundary conditions, multi-point constraints, and equations are not imported. • Kinematic and distributing coupling constraints are not imported. In addition, the reference node of a coupling constraint will not be imported unless the reference node is part of another element definition that is imported. • When you import part instances individually from a previous analysis that was defined as an assembly of part instances, reference nodes associated with rigid body or coupling constraints defined on the imported instances will not be available in the import analysis for load or boundary condition application. • Pre-tension section definitions are not imported; they have to be redefined in the import analysis. • The capability is not available for elements with composite solid section definitions. • If the elements that are removed in the original analysis are imported, they become active in the import analysis and should be removed in the first step of the import analysis. • The symmetric model generation capability cannot be used in an import analysis in Abaqus/Standard. • The results file, restart file, or output database file generated during the import analysis is not appended to the results file, restart file, or output database file of the original analysis. • There may be a slight discontinuity during the transfer of state variables for analyses using fully integrated, first-order continuum elements if the elements are significantly deformed and the reference configuration is updated. • Mesh-independent spot welds are not imported. However, the spot weld reference nodes are imported and can be used to redefine spot welds in the import analysis. The locations of the spot weld reference nodes and projection points are computed based upon the reference configuration of the import analysis. Therefore, if the deformed configuration of the imported model is significantly different from its reference configuration, it is recommended that the reference configuration be updated. • If the value of the friction coefficient is changed from the value given in the model data of the original analysis, the changed value must be respecified in the first step of the import analysis . • The capability is not available if adaptive meshing is used in the original analysis. • Enriched features are not imported. • Restart files from the original analysis are used in the analysis preprocessor and in the Abaqus/Standard execution in the import analysis. When the import job is run in parallel on computer clusters by using MPI-based parallelization, these restart files are copied to each host machine. The original job restart files are not decomposed to match the import analysis parallel domain and may be large relative to the local disk space available on the host machines. You can minimize this file size by requesting restart output only for the increment from which import will occur. Input file template Transferring results using models that are not defined as assemblies of part instances: First Abaqus/Standard analysis: *HEADING … *MATERIAL, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP, NLGEOM=YES *STATIC … *RESTART, WRITE *END STEP Abaqus/Standard import analysis: *HEADING *IMPORT, STEP=step, INCREMENT=increment, STATE=YES, UPDATE=NO Data lines to specify element sets to be imported *IMPORT ELSET Data lines to specify element set definitions to be imported *IMPORT NSET Data lines to specify node set definitions to be imported ** *** Optionally define additional model information ** *BOUNDARY Data lines to redefine boundary conditions *STEP, NLGEOM=YES *STATIC … *END STEP Transferring results using models defined as assemblies of part instances: First Abaqus/Standard analysis: *HEADING *PART, NAME=Part-1 Node, element, section, set, and surface definitions *END PART *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=i1, PART=Part-1 Additional set and surface definitions (optional) *END INSTANCE Assembly level set and surface definitions … *END ASSEMBLY *MATERIAL, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP *STATIC … *RESTART, WRITE, FREQUENCY=n *END STEP Abaqus/Standard import analysis: *HEADING Part definitions (optional) *ASSEMBLY, NAME=Assembly-1 *INSTANCE, INSTANCE=i1, LIBRARY=oldjob-name Additional set and surface definitions (optional) *IMPORT, STEP=step, INCREMENT=increment, STATE=YES, UPDATE=NO *END INSTANCE Additional part instance definitions (optional) Assembly level set and surface definitions … *END ASSEMBLY ** *** Optionally define additional model information ** *BOUNDARY Data lines to define boundary conditions *STEP, NLGEOM=YES *STATIC … *END STEP 9.2.4 TRANSFERRING RESULTS FROM ONE Abaqus/Explicit ANALYSIS TO ANOTHER Products: Abaqus/Explicit Abaqus/CAE References • “Transferring results between Abaqus analyses: overview,” Section 9.2.1 • *IMPORT • *IMPORT ELSET • *IMPORT NSET • *IMPORT CONTROLS • *INSTANCE • “Transferring results between Abaqus analyses,” Section 16.6 of the Abaqus/CAE User’s Manual Overview Abaqus provides the capability to transfer desired results and model information from an Abaqus/Explicit analysis to a new Abaqus/Explicit analysis, where additional model definitions may be specified before the analysis is continued. For example, during an assembly process an analyst may first be interested in the local behavior of a particular component but later is concerned with the behavior of the assembled product. In this case the local behavior can first be analyzed in an Abaqus/Explicit analysis. Subsequently, the model information and results from this analysis can be transferred to a second Abaqus/Explicit analysis, where additional model definitions for the other components can be specified, and the behavior of the entire product can then be analyzed. For this capability to work, the same release of Abaqus/Explicit must be run on computers that are binary compatible. Information about how to transfer results between Abaqus analyses is provided in “Transferring results between Abaqus analyses: overview,” Section 9.2.1. Comparison with the restart capability Both the import and restart capabilities in Abaqus/Explicit allow for the transfer of results and model information from one Abaqus/Explicit analysis to another Abaqus/Explicit analysis. However, the two capabilities have been designed for different applications. The restart capability allows a completed Abaqus/Explicit analysis to be restarted and continued. The entire model and results from the original analysis are transferred to the restart run, where additional analysis steps can be defined. Not much new model data can be specified in the restarted analysis; only model information such as new amplitude definitions, new node sets, and new element sets are allowed. Detailed information on the restart capability is given in “Restarting an analysis,” Section 9.1.1. The import capability also allows a completed Abaqus/Explicit analysis to be continued. In addition, this capability allows for the analysis to be continued with only desired components from the original analysis; the entire model need not be transferred. New model data—such as elements, nodes, surfaces, contact pairs, etc.—can be specified during the import analysis. During the import analysis it is possible to choose whether only model information from the previous analysis is to be transferred or if the results associated with that model also are to be transferred. For situations where the goal is to continue the original analysis with no change to the model information, it is recommended that the restart capability be used. For situations where the model information requires changes, or for cases where you require control over the transfer of results, the import capability should be used. Specifying new data in an import analysis Additional model definitions such as new elements, nodes, surfaces, etc. can be defined during the import analysis. Initial conditions can also be specified during the import analysis. New model definitions New nodes, elements, and material properties can be added to the model in an import analysis once import has been specified. Nodal coordinates must be defined in the updated configuration, regardless of whether or not the reference configuration is updated on import . The usual Abaqus/Explicit input can be used. Imported material definitions can be used with the new elements (which will need new section property definitions). Nodal transformation transformations (“Transformed coordinate systems,” Section 2.1.5) are not Nodal imported; transformations can be defined independently in the import analysis. Continuous displacements, velocities, etc. are obtained only if the nodal transformations in the import analysis are the same as those in the original analysis. Use of the same transformations is also recommended for nodes with boundary conditions or point loads defined in a local system. Specifying geometric nonlinearity in an import analysis By default, Abaqus/Explicit uses a large-strain formulation. For each step of an analysis you can specify whether or not geometric nonlinearity should be included; see “Geometric nonlinearity” in “General and linear perturbation procedures,” Section 6.1.3, for details. The default value for the formulation in an import analysis is the same as the value at the time of import. Once the large-displacement formulation is used during a given step in any analysis, it will remain active in all the subsequent steps, whether or not the analysis is imported. If the small-displacement formulation is used at the time of import, the reference configuration cannot be updated. Specifying initial conditions for imported elements and nodes Initial conditions can be specified on the imported elements or nodes only under certain conditions. Table 9.2.4–1 lists the initial conditions that are allowed depending on whether or not the material state is imported . The reference configuration can be updated or not, as desired, with one exception: for initial temperature or field variable conditions, the reference configuration must be updated. Table 9.2.4–1 Valid initial conditions. Initial condition Field variable Hardening Relative density Rotational velocity Solution-dependent state variables Stress Temperature Velocity Void ratio Material state imported No No No Yes or No No No No Yes or No No Boundary conditions Boundary conditions (including connector motion) specified in the original analysis are not imported. They must be redefined in the import analysis. In some cases nonzero boundary conditions imposed in the original analysis need to be maintained at the same values in the import analysis when the imported configuration is not updated. In such cases you can prescribe a constant (step function) amplitude variation for the analysis step so that the newly applied boundary conditions are applied instantaneously and held at that value for the duration of the step. Alternatively, you can refer to an amplitude curve in the boundary condition definition . If boundary conditions in the original analysis are applied in a transformed coordinate system , the same coordinate system should be defined and used in the import analysis. For discussions on applying boundary conditions and multi-point constraints, see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1, and “Kinematic constraints: overview,” Section 34.1.1. Loads Loads, including those applied for connector actuation, defined in the original analysis are not imported. Therefore, loads may need to be redefined in the import analysis. There are no restrictions on the loads that can be applied when results are imported from one analysis to the other. In cases when the loads need to be maintained at the same values as in the original analysis, you can prescribe a constant (step function) amplitude variation for the analysis step to apply the loads instantaneously at the start of the step and hold them for the duration of the step. Alternatively, you can refer to an amplitude curve in the load definition . If point loads in the original analysis are applied in a transformed coordinate system and the loads must be maintained in the import analysis, the load application is simplified if the same coordinate system is defined and used in the import analysis. See “Applying loads: overview,” Section 33.4.1, for an overview of the loading types available in Abaqus/Explicit. Predefined fields Temperatures, whether they are prescribed or are degrees of freedom (as in a coupled thermal-stress analysis), and field variables at nodes are imported if the material state is imported. If the reference configuration is updated and the material state is imported, the initial conditions for temperatures and field variables at the imported nodes will be reset to the imported values; for example, the thermal strains will now be measured relative to the imported temperatures. If the reference configuration is updated but the material state is not imported, the initial conditions are reset to zero. In this case you can respecify the initial conditions on the imported nodes. If the temperature is a state variable (as in an adiabatic analysis where temperature is an integration point quantity), it will be imported if the material state is imported. Material options All material property definitions and orientations associated with imported elements are imported by default. Material properties can be changed by respecifying the material property definitions with the same material name. In this case all relevant material properties must be redefined since the old definitions that were imported by default will be overwritten. Material orientations associated with imported elements can be changed only if the reference configuration is updated and the material state is not imported; the material orientations associated with imported elements cannot be redefined for other combinations of the reference configuration and material state. When connector elements are imported, any associated connector behavior definitions are imported by default. The imported connector behavior definitions can be modified only if the state is not imported. The material model must be redefined in the import analysis if changes to material damping are required. When material definitions are changed, care must be taken to ensure that a consistent material state It may sometimes be possible to simplify the material definition. For example, if a is maintained. Mises plasticity model was used in the first Abaqus/Explicit analysis and no further plastic yielding is expected in a subsequent Abaqus/Explicit analysis, a linear elastic material can be used for the subsequent Abaqus/Explicit analysis. However, if further nonlinear material behavior is expected, no changes to the existing material definitions should be made. The history of the state variables will not be maintained if the material models are not the same in both the original analysis and the import analysis. Elements The import capability is available for a subset of the stress/displacement and coupled temperature- displacement continuum, shell, membrane, truss, connector, rigid, and surface elements available in Abaqus/Explicit. The complete list of supported elements is provided in Table 9.2.4–2. If elements that are removed are imported, they become active in the import analysis and should be removed in the first step of the import analysis. Table 9.2.4–2 Element types that can be transferred from one Abaqus/Explicit analysis to another. Element Type Supported Elements Plane strain continuum CPE3, CPE4R, CPE4RT, CPE6M, CPE6MT, CPE3T Plane stress continuum CPS3, CPS4R, CPS4RT, CPS6M, CPS6MT, CPS3T Three-dimensional continuum C3D4, C3D4T, C3D6, C3D6T, C3D8R, C3D8RT, C3D10M, C3D10MT, C3D8, C3D8T, C3D8I Axisymmetric continuum CAX3, CAX4R, CAX3T, CAX4RT, CAX6M, CAX6MT Membrane M3D3, M3D4 M3D4R Two-dimensional rigid R2D2 Three-dimensional rigid R3D3, R3D4 Axisymmetric rigid RAX2 Three-dimensional shell S4R, S3R, S3, S4, S4RS, S4RSW, S3RS, S3T, S3RT, S4T, S4RT Continuum shell elements SC6R, SC8R, SC6RT, SC8RT Axisymmetric shell SAX1 Surface SFM3D3, SFM3D4R Two-dimensional truss Three-dimensional truss T2D2 T3D2 Two-dimensional beam B21, B22 Three-dimensional beam B31, B32 Connector elements CONN2D2, CONN3D2 Element Type Supported Elements Cohesive COH2D4, COHAX4, COH3D6, COH3D8 Infinite elements CINPS4, CINPE4, CINAX4, CIN3D8, ACIN2D2, ACIN3D3, ACINAX2 Acoustic elements AC2D3, AC2D4R, AC3D4, AC3D6, ACAX3, ACAX4R, AC3D8R The following element types cannot be imported: • Heat capacitance elements • Inertial elements (mass and rotary inertia) • Eulerian elements (EC3D8R and EC3D8RT) In addition, the following restrictions apply to the import capability: • Rebars defined using rebar layers (“Defining reinforcement,” Section 2.2.3) are imported provided the underlying elements are also imported. Rebar reinforcements defined using the embedded element technique (“Embedded elements,” Section 34.4.1) are imported if the host and embedded elements used in this definition are also imported. Rebars defined as an element property (“Defining rebar as an element property,” Section 2.2.4) cannot be imported. • If connector elements are imported, the configuration can be updated provided that the state is not imported and the state can be imported provided that the configuration is not updated. • A rigid body containing both deformable and rigid elements cannot be imported. A rigid body that includes rigid elements is imported when the element set used to define the rigid body is specified for import. A rigid body that includes deformable elements is imported when the element set used to define the rigid body is specified for import. The imported rigid body definition is overwritten if it is respecified using the same element set. When the model is defined in terms of an assembly of part instances, the reference node of an imported rigid body must belong to an imported instance. • When a rigid body is imported, any associated data such as pin node sets and tie node sets are part of the imported definition. However, these sets as imported contain only those nodes that are connected to the imported elements. Constraints Kinematic constraints (including multi-point constraints and surface-based tie constraints) specified in the original analysis are not imported and must be defined again in the import analysis. See “Kinematic constraints: overview,” Section 34.1.1, for a discussion of the various types of kinematic constraints. Interactions For general contact, the contact state is imported if general contact is defined in both analyses. For contact defined by contact pairs, contact definitions specified in the original analysis and the contact state are not imported. Contact can be defined again in the import analysis by specifying the surfaces and contact pairs. Additional contact information can be defined in the import analysis by specifying new surfaces, contact pairs, and interactions. For a detailed description of the contact capabilities in Abaqus/Explicit, refer to “Contact interaction analysis: overview,” Section 35.1.1. Output Output can be requested for an import analysis in the same way as for an analysis in which the results are not imported. Output requests in the original analysis are not transferred to the import analysis; output requests in the import analysis have to be respecified. The output variables available in Abaqus/Explicit are listed in “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The values of the following material point output variables will be continuous in an import analysis when the material state is imported: stress, equivalent plastic strain (PEEQ), and solution-dependent state variables (SDV) for VUMAT. Similarly, for a connector behavior, the plastic relative displacement (CUP), kinematic hardening shift force (CALPHAF), overall damage (CDMG), damage initiation criteria (CDIF, CDIM, CDIP), friction accumulated slip (CASU), and connector status (CSLST, CFAILST) will be continuous. If the reference configuration is not updated, the displacements, strains, whole element variables, section variables, and energy quantities will be reported relative to the original configuration. If the reference configuration is updated, displacements, strains, whole element variables, section variables, and energy quantities will not be continuous in an import analysis and will be reported relative to the updated reference configuration. Time and step number will not be continuous between the original and the import analyses if the reference configuration is updated. Time and step number will be continuous only if the reference configuration is not updated. Limitations The import capability has the following known limitations. Where applicable, details are given in the relevant sections. • The same release of Abaqus/Explicit must be run on computers that are binary compatible. • The capability is not available for spring, mass, dashpot, and rotary inertia. See the discussion on “Elements” earlier in this section for further details. • If connector elements are imported, the configuration can be updated provided that the state is not imported and the state can be imported provided that the configuration is not updated. • Surfaces are not imported when the model is defined as an assembly of part instances. • All elements and nodes must be included in at least one set in the original analysis when importing part instances. • The contact state for contact pairs is not imported. • If the material state is imported, only stresses will be imported for material models other than those defined by linear elasticity, hyperelasticity, hyperfoam, viscoelasticity, Mises plasticity, and damage for cohesive elements. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details. For a connector behavior, the plastic displacements, the frictional slip, and the damage state are imported and the connector forces are recomputed. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details. • Loads, boundary conditions, multi-point constraints, equations, and surface-based tie constraints are not imported. • Kinematic and distributing coupling constraints are not imported. In addition, the reference node of a coupling constraint will not be imported unless the reference node is part of another element definition that is imported. • The results file, restart file, or output database file generated during the import analysis is not appended to the results file, restart file, or output database file of the original analysis. • Mesh-independent spot welds and tie constraints are not imported. These constraints can be redefined in the import analysis and are formed using the reference configuration of the import model. If the reference configuration is updated, the redefined constraints may not match the old constraints exactly due to the differences in geometry. If new constraints are defined and the reference configuration of the import model is not updated, they may not initially be in compliance if the nodes involved in the constraint have nonzero displacements. This may cause numerical difficulty and potential abort of the import analysis. In this case it is recommended that you update the reference configuration upon import. Input file template Transferring results using models that are not defined as assemblies of part instances: First Abaqus/Explicit analysis: *HEADING … *MATERIAL, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP *DYNAMIC, EXPLICIT … *RESTART, WRITE, NUMBER INTERVAL=n *END STEP Abaqus/Explicit import analysis: *HEADING *IMPORT, STEP=step, INTERVAL=interval, STATE=YES, UPDATE=NO Data lines to specify element sets to be imported *IMPORT ELSET Data lines to specify element set definitions to be imported *IMPORT NSET Data lines to specify node set definitions to be imported ** *** Optionally define additional model information ** *BOUNDARY Data lines to redefine boundary conditions *STEP *DYNAMIC, EXPLICIT … *END STEP Transferring results using models defined as assemblies of part instances: First Abaqus/Explicit analysis: *HEADING *PART, NAME=Part-1 Node, element, section, set, and surface definitions *END PART *ASSEMBLY, NAME=Assembly-1 *INSTANCE, NAME=i1, PART=Part-1 Additional set and surface definitions (optional) *END INSTANCE Assembly level set and surface definitions … *END ASSEMBLY *MATERIAL, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP *DYNAMIC, EXPLICIT … *RESTART, WRITE, NUMBER INTERVAL=n *END STEP Abaqus/Explicit import analysis: *HEADING Part definitions (optional) *ASSEMBLY, NAME=Assembly-1 *INSTANCE, INSTANCE=i1, LIBRARY=oldjob-name Additional set and surface definitions (optional) *IMPORT, STEP=step, INTERVAL=interval, STATE=YES, UPDATE=NO *END INSTANCE Additional part instance definitions (optional) Assembly level set and surface definitions … *END ASSEMBLY ** *** Optionally define additional model information ** *BOUNDARY Data lines to define boundary conditions *STEP *DYNAMIC, EXPLICIT … *END STEP 10. Modeling Abstractions Substructuring Submodeling Generating global matrices Symmetric model generation, results transfer, and analysis of cyclic symmetry models Periodic media analysis Meshed beam cross-sections Modeling discontinuties as an enriched figure using extended finite element method 10.1 10.2 10.3 10.4 10.5 10.6 10.1 Substructuring • “Using substructures,” Section 10.1.1 • “Defining substructures,” Section 10.1.2 10.1.1 USING SUBSTRUCTURES Products: Abaqus/Standard Abaqus/CAE References • “Defining substructures,” Section 10.1.2 • *SLOAD • *SUBSTRUCTURE PATH • *SUBSTRUCTURE PROPERTY Overview Substructures: • allow a collection of elements to be grouped together and all but the retained degrees of freedom eliminated on the basis of linear response within the group; • are used in the same manner as any of the standard element types in the Abaqus element library once created as described in “Defining substructures,” Section 10.1.2; • can be used in stress/displacement and in coupled acoustic-structural analyses; • have linear response but allow for large translations and large rotations; • are particularly useful in cases where identical pieces appear several times in a structure (such as the teeth of a gear) since a single substructure can be used repeatedly; • can be translated, rotated with respect to the global system, and reflected in a plane when they are used; • are connected to the rest of the model by the retained degrees of freedom at the retained nodes; • may contain a set of internal load cases and boundary conditions that can be activated and scaled; • can include dynamic effects by including retained eigenmodes; and • appear to the rest of the model as a stiffness, optional mass, damping, and a set of scalable load vectors. Substructures Substructures are collections of elements from which the internal degrees of freedom have been eliminated. Retained nodes and degrees of freedom are those that will be recognized externally at the usage level (when the substructure is used in an analysis), and they are defined during generation of the substructure. Factors that determine how many and which nodes and degrees of freedom should be retained are discussed below and in “Defining substructures,” Section 10.1.2. Substructures versus superelements In the finite element literature substructures are also referred to as superelements. In earlier releases of Abaqus a distinction was made between substructures and superelements. The term “substructure” was used when it was needed to make clear that results were recovered within the substructure. Otherwise, both terms were used interchangeably. To avoid confusion, the term “superelement” will no longer be used. Why use substructures? There are a number of good reasons to use substructures. Computational advantages • System matrices (stiffness, mass) are small as a result of substructuring. Subsequent to the creation of the substructure, only the retained degrees of freedom and the associated reduced stiffness (and mass) matrix are used in the analysis until it is necessary to recover the solution internal to the substructure. • Efficiency is improved when the same substructure is used multiple times. The stiffness calculation and substructure reduction are done only once; however, the substructure itself can be used many times, resulting in a significant savings in computational effort. • Substructuring can isolate possible changes outside substructures to save time during reanalysis. During the design process large portions of the structure will often remain unchanged; these portions can be isolated in a substructure to save the computational effort involved in forming the stiffness of that part of the structure. • In a problem with local nonlinearities, such as a model that includes interfaces with possible separation or contact, the iterations to resolve these local nonlinearities can be made on a very much reduced number of degrees of freedom if the substructure capability is used to condense the model down to just those degrees of freedom involved in the local nonlinearity. Organizational advantages • Substructuring provides a systematic approach to complex analyses. The design process often begins with independent analyses of naturally occurring substructures. Therefore, it is efficient to perform the final design analysis with the use of substructure data obtained during these independent analyses. • Substructure libraries allow analysts to share substructures. In large design projects large groups of engineers must often conduct analyses using the same structures. Substructure libraries provide a clean and simple way of sharing structural information. • Many practical structures are so large and complex that a finite element model of the complete structure places excessive demands on available computational resources. Such a large linear problem can be solved by building the model, substructure by substructure, and stacking these level by level until the whole structure is complete and then recovering the displacements and stresses locally, as required. Valid procedures Substructures can be used without restriction in the following procedures: • “Static stress analysis,” Section 6.2.2 • “Implicit dynamic analysis using direct integration,” Section 6.3.2 • “Direct-solution steady-state dynamic analysis,” Section 6.3.4 • “Natural frequency extraction,” Section 6.3.5 • “Complex eigenvalue extraction,” Section 6.3.6 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 Substructures can also be used in the following procedures, but recovery of eliminated degrees of freedom is not supported: • “Transient modal dynamic analysis,” Section 6.3.7 • “Response spectrum analysis,” Section 6.3.10 • “Random response analysis,” Section 6.3.11 Using substructures in static analysis Substructuring introduces no additional approximation in linear static structural analysis: the substructure is an exact representation of the linear, static behavior of its members. The principal drawback to the use of substructures in stress/displacement analyses is that a substructure’s stiffness matrix is fully populated (no zero terms) and, therefore, may be very large if the substructure has a large number of retained degrees of freedom. This, in turn, may mean that the wavefront of the model within which substructures are used may be large, thus leading to long computer times to solve the equations. This difficulty can often be avoided by choosing the substructure’s boundaries carefully or by reusing several smaller substructures rather than a single larger substructure. In some cases it is possible to take advantage of the fact that Abaqus/Standard allows individual degrees of freedom to be retained, rather than the whole set of degrees of freedom at a node. For example, in contact problems without friction only the displacement component normal to the surface need be retained for the contact solution. Nodal transformations can be helpful in orienting the displacement components at surface nodes for this purpose . In a static analysis involving a substructure containing acoustic elements, the results will differ from the results obtained in an equivalent static analysis without substructures. The acoustic-structural coupling is taken into account in the substructure (leading to hydrostatic contributions of the acoustic fluid), while the coupling is ignored in a static analysis without substructures. Using substructures in dynamic analysis Substructures introduce approximations in dynamic analysis. The default approach to the dynamic representation of a substructure is to reduce its mass and damping matrix with the same transformation as is used for its stiffness matrix, which is known as “Guyan reduction.” This approach assumes that the response between the eliminated and retained degrees of freedom is correctly represented by the static modes only. This representation may not be accurate if dynamic modes within the substructure are important. The dynamic representation may be improved for Guyan reduction by retaining additional physical degrees of freedom that are not required to connect the substructure to the rest of the model. For example, if the substructure is a plate or a beam, some transverse displacements (and, perhaps, in-surface rotation components) might be included as retained degrees of freedom for this purpose. For more details regarding Guyan reduction, see “Substructuring and substructure analysis,” Section 2.14.1 of the Abaqus Theory Manual. “Dynamic mode addition” can be used as an alternative to Guyan reduction. This approach involves adding generalized degrees of freedom associated with the eigenmodes extracted for the substructure, with all of the physical retained degrees of freedom automatically constrained. This improves dynamic behavior, but it introduces the additional cost of extracting the eigenmodes for the constrained substructure. For more details regarding dynamic mode addition, see “Substructuring and substructure analysis,” Section 2.14.1 of the Abaqus Theory Manual. The reduction methods can be applied simultaneously to different substructures within the same structure. Definition of the reduced mass matrix is discussed further in “Defining substructures,” Section 10.1.2. Using substructures in geometrically nonlinear stress/displacement analysis Substructures may undergo large motions if geometric nonlinearities are considered in a particular overview,” Section 6.2.1). stress/displacement analysis deformations at all times during the geometrically nonlinear analysis. An equivalent rigid body rotation for each substructure is computed during each equilibrium iteration using the retained nodes of the substructure. The substructure’s mass, damping, stiffness matrix (including the retained eigenmodes), and force vectors are then rotated appropriately using the equivalent rigid body rotation. Appropriate (rotated) linear perturbation displacements (strain-inducing displacements relative to the rotating reference configuration) are used to compute the internal force associated with the substructure. Degrees of freedom at a node should not be retained selectively if the substructure is to be used in geometrically nonlinear analysis. Coupled acoustic-structural substructures should not be used in geometrically nonlinear analyses. Comparison with component mode synthesis The component mode synthesis method (also known as the Craig-Bampton method) has been developed to permit the structure to be subdivided into components (substructures), with most of the analysis being done on the smaller components to develop an approximate model for the entire structure. The substructures in Abaqus/Standard are, in fact, a particular case of the Craig-Bampton method extended to allow for large rotations and translations of the substructure (component). The component mode synthesis method is based on the assumption that the small deformations of a substructure can be modeled using a collection of modes. The most frequently used modes in the literature are typically referred to as follows: • constraint modes, which are static shapes obtained by giving each retained degree of freedom in the substructure a unit displacement while holding all other retained degrees of freedom fixed; and • fixed-interface normal modes, which are obtained by fixing the retained degrees of freedom and computing the eigenmodes of the substructure. The constraint modes are precisely the static modes used by Abaqus/Standard. You include these modes in the substructure’s representation by specifying the degrees of freedom that are to be retained . The fixed-interface normal modes are the eigenmodes extracted in the eigenfrequency extraction step at the generation level, and these modes represent a particular case of substructure dynamic modes allowed in Abaqus . You include the dynamic modes in the substructure’s representation by specifying the eigenmodes to be retained. Including substructures in a model When a substructure is used in a model, it is assigned an element number and defined by nodes just like any other element. Use an element definition (“Element definition,” Section 2.2.1) with a substructure identifier to include substructures in the definition of another substructure (nested substructure) or in an analysis model. The substructure can be read from a substructure library. A maximum of 500 libraries can be accessed to read substructure data within a given analysis. In the element definition you define the substructure’s element number at the usage level and assign node numbers to the substructure’s retained nodes. More than one substructure can be defined per element definition. Once a substructure has been introduced by an element definition, it is treated like any other element in the model, except that its response can be linear only (although it can be used as a part of a model that includes nonlinear effects, including large displacements). Using substructures requires that the substructure database be available. All the files generated for a substructure including the .sup and .sim files and/or the .prt, .stt, and .mdl files must be available. Input File Usage: Abaqus/CAE Usage: Use the following option to include one or more substructures in a model: *ELEMENT, TYPE=Zn Use the following option to include one substructure in a model: All modules: File→Import→Part: File Filter: Substructure Repeat the import process for each substructure that you want to include in the model. Ordering of the substructure nodes on the usage level The node numbers that are used when a substructure is created and the node numbers that are associated with the substructure when it is used are entirely independent. The ordering of the retained nodes when the substructure is used can be defined in two different ways: 1. The nodes can be provided in the same order that they were listed in the substructure definition. In this case you must prevent the sorting of the retained nodes when you specify the retained degrees of freedom (see “Preventing the degrees of freedom from being sorted” in “Defining substructures,” Section 10.1.2). Duplicate nodes are not combined if the retained nodes are not sorted. Therefore, if the same nodes are specified more than once in the list of retained degrees of freedom to retain different degrees of freedom, the corresponding nodes at the usage level must appear the same number of times. 2. The substructure nodes must be specified in the same order as the retained nodes sorted into ascending numerical order according to their numbers used within the substructure. This approach is the default when you specify the retained degrees of freedom. In either case you must ensure that the nodes match up properly whenever a substructure is used. Reading the substructure definition from a substructure library You can read the substructure definition from a substructure library. Input File Usage: Abaqus/CAE Usage: *ELEMENT, TYPE=Zn, FILE=substructure_library_name Substructure libraries are not supported in Abaqus/CAE. Interpreting the model output in the data file If model definition data are written to the data file (“Controlling the amount of analysis input file processor information written to the data file” in “Output,” Section 4.1.1), substructure instances are identified in the data (.dat) file by the substructure identifier followed by an F and two digits that indicate the substructure library number. The full name of the substructure library associated with this number is also contained in the model output. Defining the substructure’s properties You associate a property definition with each substructure in the model. The property definition serves the following purposes: 1. It defines any translation, rotation, and reflection of the substructure at the usage level. 2. It allows a tolerance to be set to ensure that the coordinates of the usage level nodes match the coordinates of the nodes used to generate the substructure. 3. It controls using various sources of substructure damping in the dynamic analysis at the usage level. Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE PROPERTY, ELSET=name Use the following options to define translation and rotation of the substructure: Assembly module: Instance→Translate or Instance→Rotate Reflection of the substructure is not supported in Abaqus/CAE. Use the following option to apply constraints that connect the retained nodes with the usage level nodes: Interaction module: Constraint→Create Translating, rotating, and reflecting a substructure Translation, rotation, and/or reflection (in that order) of a substructure can be specified in a substructure property definition. Specify a translation by giving a translation vector. Specify a rotation by giving two points, a and b, defining a rotation axis plus a right-handed angular rotation around that axis. Specify a reflection by giving three non-colinear points in the reflection plane. A translation does not affect the substructure’s stiffness or mass: the principal reason to apply a translation is to enable the tolerance check on nodal coordinates as discussed later. Rotation and/or reflection of a substructure affect the substructure’s stiffness and mass. The substructure load case definitions are rotated and/or reflected in the same way as the substructure’s stiffness and mass; therefore, all loads within substructure load cases are applied in the local directions associated with the substructure when it was created. For distributed loads (for example, pressure loading of a surface) this application is precisely what is desired. However, distributed body forces in coordinate directions (BX, BY, BZ) are applied in the substructure’s local directions instead of in the global directions, which may not be what is needed. Similarly, distributed loadings that depend on position (for example, hydrostatic pressure or centrifugal loads) are based on the substructure’s local coordinates and not on the substructure position during usage. Be careful to ensure that loading of a rotated or shifted substructure is correct for its usage. Whenever a substructure is translated, rotated, and/or reflected, the degrees of freedom at any retained nodes are with respect to the coordinate directions at the usage level. Therefore, if all of the degrees of freedom of a node are not retained or if a two-dimensional substructure is used in a three-dimensional model with rotation out of the x–y plane, additional degrees of freedom may be activated due to rotation and/or reflection. Be careful to check the validity of the substructure usage in such cases. Setting a tolerance on the substructure nodes One difficulty with using large substructures is ensuring that the retained nodes in the substructure are connected to the correct nodes on the usage level (after substructure translation, rotation, and/or reflection, if applicable). Therefore, Abaqus/Standard checks that the coordinates of the retained nodes match the coordinates of the corresponding nodes on the usage level. A substructure does not require any coordinates on the usage level because it consists only of a stiffness matrix, a mass matrix, and a number of load cases. Nevertheless, it is usually a good check of a model’s validity to verify that the substructure and the model into which it is introduced are geometrically consistent. To check the coordinates, you can set a tolerance on the distance between usage level nodes and the corresponding substructure nodes. This tolerance indicates the largest deviation allowable before a warning is issued. If you do not specify this tolerance, the default is to use a tolerance of 10−4 times the largest overall dimension within the substructure. If you specify a tolerance of 0.0, the position of the retained nodes is not checked. The geometric check is based on the coordinates of the retained nodes after translation, rotation, and/or reflection of the substructure at the usage level; motions of these nodes that occur as a result of geometrically nonlinear preloading during generation of the substructure are not considered in this check. Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE PROPERTY, ELSET=name, POSITION TOL=tolerance Assembly module: Instance→Translate and Instance→Rotate Defining substructure damping Abaqus allows you to choose a particular source of damping for a substructure, to add several sources, or to exclude the damping effects for a substructure at the usage level. Sources of substructure damping You can choose to model the damping of a substructure at the usage stage by using the condensed viscous damping matrix, , computed during the , and the condensed structural damping matrix, generation stage and stored on the substructure data base. Alternatively, you can use stiffness and mass proportional damping factors to create a substructure damping matrix using the condensed stiffness and mass matrices, , respectively. You can also request that both damping sources be combined or exclude the effects of damping altogether at the usage level. and Input File Usage: Use the following option to control the sources of the substructure damping: *DAMPING CONTROLS, VISCOUS=viscousDampingSource, STRUCTURAL=structuralDampingSource Abaqus/CAE Usage: Use the following option to control the sources of the substructure damping: Step module: Create Step: Linear perturbation: Substructure generation: Damping tabbed page Controlling the sources of viscous damping In the general case the substructure viscous damping is defined by the following matrix: Input File Usage: To activate only the generated condensed viscous damping matrix of the substructure (the first term on the right hand side), use the following option: *DAMPING CONTROLS, VISCOUS=ELEMENT To activate only the Rayleigh viscous damping, use the following option: *DAMPING CONTROLS, VISCOUS=FACTOR To activate the combined generated and Rayleigh viscous damping matrix, use the following option: *DAMPING CONTROLS, VISCOUS=COMBINED To exclude the effects of viscous damping altogether at the usage level, use the following option: *DAMPING CONTROLS, VISCOUS=NONE To activate only the generated condensed viscous damping matrix of the substructure (the first term on the right hand side), use the following option: USING SUBSTRUCTURES Step module: Create Step: Linear perturbation: Substructure generation: Damping tabbed page: Viscous damping: Element To activate only the Rayleigh viscous damping, use the following option: Step module: Create Step: Linear perturbation: Substructure generation: Damping tabbed page: Viscous damping: Factor To activate the combined generated and Rayleigh viscous damping matrix, use the following option: Step module: Create Step: Linear perturbation: Substructure generation: Damping tabbed page: Viscous damping: Combined To exclude the effects of viscous damping altogether at the usage level, use the following option: Step module: Create Step: Linear perturbation: Substructure generation: Damping tabbed page: Viscous damping: None Controlling the sources of structural damping In the general case the substructure structural damping is defined by the following matrix: Input File Usage: Abaqus/CAE Usage: To activate only the generated condensed structural damping matrix of the substructure (the first term on the right hand side), use the following option: *DAMPING CONTROLS, STRUCTURAL=ELEMENT To activate only the stiffness proportional structural damping matrix, use the following option: *DAMPING CONTROLS, STRUCTURAL=FACTOR To activate the combined generated and stiffness proportional structural damping matrix, use the following option: *DAMPING CONTROLS, STRUCTURAL=COMBINED To exclude the structural damping matrix, use the following option: *DAMPING CONTROLS, STRUCTURAL=NONE To activate only the generated condensed structural damping matrix of the substructure (the first term on the right hand side), use the following option: Step module: Create Step: Linear perturbation: Substructure generation: Damping tabbed page: Structural damping: Element To activate only the stiffness proportional structural damping matrix, use the following option: Defining damping ratios Step module: Create Step: Linear perturbation: Substructure generation: Damping tabbed page: Structural damping: Factor To activate the combined generated and stiffness proportional structural damping matrix, use the following option: Step module: Create Step: Linear perturbation: Substructure generation: Damping tabbed page: Structural damping: Combined To exclude the structural damping matrix, use the following option: Step module: Create Step: Linear perturbation: Substructure generation: Damping tabbed page: Structural damping: None By default, the Rayleigh damping ratios, stiffness proportional and mass proportional damping for a substructure are zeros. , and the structural damping ratio, and , used to define Input File Usage: Abaqus/CAE Usage: Use the following options to define the values of the substructure damping ratios at the usage level: *DAMPING, ALPHA= Use the following option to define the values of the substructure damping ratios at the usage level: , STRUCTURAL= , BETA= Step module: Create Step: Linear perturbation: Substructure generation: Damping tabbed page: Alpha: : Beta: : Structural: Defining damping for modal dynamic analysis To define damping for linear dynamic analysis based on the structure’s modes, specify modal damping when using the substructure. The damping in each eigenmode can be given as a fraction of the critical damping. Alternatively, Rayleigh damping can be defined. Composite modal damping cannot be used inside substructures. See “Transient modal dynamic analysis,” Section 6.3.7, for more information about the modal damping procedure. Input File Usage: Use the following option to define the damping in each eigenmode as a fraction of the critical damping: *MODAL DAMPING, MODAL=DIRECT Use the following option to define Rayleigh damping: *MODAL DAMPING, RAYLEIGH Abaqus/CAE Usage: Modal damping for substructures is not supported in Abaqus/CAE. Defining kinematic constraints and transformations All kinematic boundary conditions, MPCs, and transformations can be applied to retained degrees of freedom at the usage level. These specifications can be changed from step to step in the usual way. In this respect substructures and their retained nodes act in an identical manner to regular elements and their nodes. Defining transformations at retained nodes If a nodal transformation (“Transformed coordinate systems,” Section 2.1.5) is used during substructure generation at a retained node, the transformations are built into the substructure. This creates an inconsistency when the substructure node is attached to a standard Abaqus element since Abaqus/Standard uses the retained degrees of freedom directly without checking their directions. Therefore, it is suggested that this situation be avoided. If a nodal transformation must be used, the resulting inconsistency can be resolved by retaining all degrees of freedom at the node and applying a linear constraint equation (“Linear constraint equations,” Section 34.2.1) as follows. At any point where such a transformed substructure node is attached to a global model, define two coincident nodes on the usage level, P and Q, for example. Use node P for the substructure at the usage level (defined with an element definition); the local directions of the degrees of freedom are already built in at this node. Use node Q for all standard Abaqus elements attached to this point. Use a local transformation at node Q to transform the degrees of freedom to the same local directions that are built-in for node P. Now use a linear constraint equation to equate the individual degrees of freedom at nodes P and Q. Applying loads to a substructure Loads or boundary conditions that are to be applied to a substructure within an analysis (at the usage level) must be specified during the substructure generation step by defining a substructure load case or by requesting that the substructure’s gravity load vectors be calculated . A load case can be made up of any combination of loadings and nonzero boundary conditions, and multiple load cases can be defined for any given substructure. When you activate load cases created for a substructure, you specify the element number or element set name of the substructures, the associated substructure load case names, and the scaling multipliers for the specified substructure load case loads and/or boundary conditions. To reproduce the loading conditions defined during substructure generation exactly, use a magnitude of 1.0. Boundary conditions specified during a substructure’s generation are always present, whether the substructure load case that they are part of is active or not. They are effectively built into the substructure and can only be scaled if desired but not removed. See “Defining substructures,” Section 10.1.2, for further information about defining boundary conditions in substructures. Input File Usage: Use the following option to activate a substructure load case: Abaqus/CAE Usage: *SLOAD Use the following option to activate a substructure load case: Load module: load editor: Category: Mechanical: Types for Selected Step: Substructure load Modifying or removing load cases By default, substructure loads are applied as modifications of existing loads or in addition to any loads previously defined. You can remove all previously defined loads and, optionally, specify new loads when you activate a load case. Boundary conditions cannot be removed. Input File Usage: Use the following option to modify load cases: Abaqus/CAE Usage: *SLOAD, OP=MOD Use the following option to remove load cases: *SLOAD, OP=NEW Use the following option to modify load cases: Load module: Load Case Manager: click Edit Use the following option to remove load cases: Load module: Load Case Manager: click Delete Specifying time-dependent load cases The magnitude of substructure loads can be varied with time by referring to an amplitude definition (“Amplitude curves,” Section 33.1.2). Input File Usage: Use the following options to define time-dependent load cases: Abaqus/CAE Usage: *AMPLITUDE, NAME=amplitude *SLOAD, AMPLITUDE=amplitude Use the following options to define time-dependent load cases: Load module: amplitude editor: Create Amplitude: Amplitude: amplitude Load module: load editor: Category: Mechanical: Types for Selected Step: Substructure load: Amplitude: amplitude Load cases in geometrically nonlinear analyses All substructure loads and boundary conditions are applied in a local system associated with the substructure. Since this local system rotates with the substructure when large motions are present, these loads and boundary conditions will rotate as well. As a consequence, you should be careful when using substructure loads in geometrically nonlinear analyses to ensure that the loading is in the appropriate direction at the usage level. This situation is similar to rotating the substructure via a substructure property definition. Gravity loading A distributed load definition can be used to apply gravity loading to a substructure with a user-defined magnitude, scaled by an amplitude definition, and acting in a specifed direction. To enable gravity the calculation of the substructure’s gravity load loading for a substructure, you must request vectors during the substructure generation step . In this case gravity loading should not be defined as part of a substructure load case. Input File Usage: Use the following option to define gravity loading: *DLOAD, AMPLITUDE=amplitude element set or element number, GRAV, magnitude, direction Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Gravity for the Types for Selected Step Obtaining output of results within a substructure You can obtain output within substructures used in static, dynamic, eigenfrequency extraction, and steady-state and transient modal dynamic analyses. The recovery of output is not possible for substructures used in response spectrum and random response analyses. Output within a substructure does not include the displacements, stresses, etc. resulting from the preload deformation of a substructure. Output within substructures is available in the data (.dat) file, in the results (.fil) file, and in output database (.odb) files. Separate output database files are created for each substructure using the naming convention inputfile-name_substructure-number.odb. If a substructure contains a nested substructure, a file called inputfile-name_substructure-number_nested-substructure-number.odb is created containing the output for the nested substructure. The abaqus substructurecombine execution procedure can combine model and results data from two substructure output databases into a single output database. For more information, see “Combining output from substructures,” Section 3.2.19. Recovery of the solution within substructures requires that the information for recovering the data within a substructure be available from the .sup, .sim, .prt, .stt, and .mdl files. Output is organized substructure by substructure: you direct Abaqus/Standard to go inside a particular substructure and then request output for that substructure. Results can be recovered within nested multilevel substructures only if the substructure libraries for all substructures in the chain are available. Substructure output requests are most easily pictured by thinking of substructures as “levels” of detailed modeling. At the global (top) level we have the analysis model (for example, an airplane). Dropping down from this level to the first substructure level, we have the main components of the model defined as substructures (wings, stabilizer, fuselage, etc.). Dropping down to the second substructure level, we have other substructures (flaps, tanks, floors, etc.), which, in turn, may contain third level substructures (spars, stringers, etc.), and so on. To obtain output, you move down and back up through these various levels using substructure paths, similar to the way you navigate a tree structure for file directories. Each substructure path definition consists of entering into a substructure at the next level down or leaving the current substructure and moving up one level in the tree. At the start of the output requests, Abaqus/Standard is at the global model level. You must always enter and leave a substructure consistently, so that after a set of substructure output requests Abaqus/Standard is left at the global model level. You must return to the global level (outside all substructures) before the end of the step definition. If you enter and leave in the same substructure path definition, the effect is to leave the substructure and enter another substructure at the same level. Entering a substructure for output To enter a particular substructure for output, you identify the substructure by the element number n chosen for it in the model. All subsequent output requests are for output within that substructure and must be given in terms of its internal node and element numbers (the node and element numbers used when the substructure was created). Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE PATH, ENTER ELEMENT=n Step module: field output request editor: Domain: Substructure: click and select substructure sets Leaving a substructure after obtaining output After you have obtained output for a substructure, you must return to the level of the model of which the substructure forms a part, thus indicating the end of the output requests for variables within that substructure. Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE PATH, LEAVE Step module: field output request editor: Domain: Substructure: click and select substructure sets Obtaining output if substructures are nested You must enter several substructures if substructures are used at multiple levels and output is required several levels down. Nesting of substructures is not supported in Abaqus/CAE. Example: obtaining output within nested substructures For example, suppose that a model includes several substructures at two levels. Printed output of stress components is required in some elements within two substructures at the second level, as well as printed output of the displacements at some of the nodes of one of the first-level substructures. (Recall that “first-level” refers to substructures used directly in the analysis model; “second-level” substructures are used as components of first-level substructures.) The data might be as follows: *SUBSTRUCTURE PATH, ENTER ELEMENT=N ** This option takes us into element number N, which must be a substructure. *SUBSTRUCTURE PATH, ENTER ELEMENT=M ** We now drop down into element number M of this substructure. ** M is the element number used for this substructure when N was created. ** M must refer to a substructure.*EL PRINT, ELSET=A1 ** This option requests stress output in element set A1 of this substructure. ** This element set must have been defined during the creation of substructure M. *SUBSTRUCTURE PATH, LEAVE ** This option takes us back up into first-level substructure N. *SUBSTRUCTURE PATH, ENTER ELEMENT=P ** This option takes us down into element P, which must again be a substructure in element N. *EL PRINT, ELSET=A1 ** This option requests the printing of stress output in element set A1. It is possible that ** this is the same set of elements in the same substructure as was used in the request above ** because substructures M and P may both be copies of the same substructure. ** However, the stresses will presumably be different because they represent the same ** component in different locations in the model. *SUBSTRUCTURE PATH, LEAVE ** Back to N. *SUBSTRUCTURE PATH, LEAVE ** We are now back at the global level. *SUBSTRUCTURE PATH, ENTER ELEMENT=R ** Enter element R at the global level: this element is the substructure in which we want ** to print the displacements. *NODE PRINT, NSET=FLANGE ** This option prints the displacements at all nodes in node set ** FLANGE of the substructure. ** Again, FLANGE must have been defined when the substructure was ** created. *SUBSTRUCTURE PATH, LEAVE ** Back to the global level. Interpreting nodal variable output The nodal displacements within the substructure do not include the displacements resulting from the preload deformation if it exists. If a substructure is rotated and/or reflected, nodal variables are output relative to the global coordinate system of the analysis. In a geometrically nonlinear analysis, the nodal displacements will include the large motions associated with the translation and rotation of the substructure in addition If a nodal transformation (“Transformed coordinate systems,” to the small-strain displacements. Section 2.1.5) has been used, nodal output will be in either the local or the global directions, depending on the nodal output request . If a nodal transformation has been used during substructure generation, the transformed directions are rotated with the substructure. Interpreting element variable output Element output variables within a substructure do not include the values of the variable resulting from the preload deformation if it exists. Element variables in continuum elements are output relative to the global coordinate system of the analysis model or in the local (material) coordinate system if one has been used (“Orientations,” Section 2.2.5). Element output for structural elements is always given with respect to the element coordinate system used during substructure generation. Integration point coordinates and local material directions are given with respect to the global coordinate system. Element quantities associated with nonlinear preload response (plastic strains, creep strains, etc.) can be output during a substructure recovery. Since the response in a substructure during its usage is entirely linear, these quantities, which are part of the base state, do not change from the values computed during the preload. If a substructure was reflected, the element connectivities of continuum elements written to the substructure instance output database are adjusted so as not to violate the Abaqus convention for counterclockwise element numbering. You cannot directly obtain the element output for the element centroidal values or the element output at the element nodes when you recover results within substructures. This output data can be calculated from the substructure-related data in the output database file using commands in the Abaqus Scripting Interface. Interpreting results written to the results file Results within substructures can be written to the results file. Substructure path records are inserted in the results file to indicate the switch into a substructure: all records following such a record belong to the substructure defined on that record until the next substructure path record appears in the file. Requests for output to the results file will cause Abaqus/Standard to write the definitions of elements and nodes at the global level and within all substructures in the model to the file. As with the results records themselves, these records for nodes and elements within substructures will be preceded and followed by substructure path records to indicate that they belong to that substructure. Node and element numbers within each substructure are local to that substructure, so that the same node and element numbers may appear in several substructures and in the global level model. In such a case the substructure path records must be used to identify the location of a particular node or element within the model. If you can ensure that node and element numbers are unique throughout the entire model, including all substructures, the substructure path records in the results file can be ignored. Visualizing substructure results While Abaqus/CAE does not support substructures directly, you can view substructure results by combining all of the substructure instance output database (.odb) files into a single file. See “Combining output from substructures,” Section 3.2.19, for details. You can also load and view each individual substructure instance output database (.odb) file separately in Abaqus/CAE. Substructure library compatibility A substructure usage analysis can use the substructure libraries generated from the same or any previous maintenance delivery of the same general release. For example, if a substructure is generated with the Abaqus 6.12-3 maintenance delivery, it can be used in all subsequent Abaqus 6.12 maintenance deliveries. The substructure library is not compatible between general releases (for example, between Abaqus 6.11 and Abaqus 6.12). A substructure usage analysis must be run on a computer that is binary compatible with the computer used to generate the substructure library. Input file template The following template can be used to generate a substructure: *HEADING … *NODE,NSET=N1 Data lines to define the nodes. … *NSET,NSET=N3 Data lines to define the node set members. … *ELEMENT, TYPE=CPE8, ELSET=E1 Data lines to define the elements that make up the substructure. … *ELSET,ELSET=E3 Data lines to define the element set members. … *SOLID SECTION, ELSET=E1, MATERIAL=M1 *MATERIAL, NAME=M1 *ELASTIC 30.E6, 0.3 *DENSITY 0.0007324 *STEP *FREQUENCY Data line to specify the number of modes ( m). The *FREQUENCY option is required if modes are requested using the *SELECT EIGENMODES option. *END STEP *STEP *STATIC … Options to define a linear or nonlinear static preload. … *END STEP *STEP *SUBSTRUCTURE GENERATE, TYPE=Z101, OVERWRITE, MASS MATRIX=YES, VISCOUS DAMPING MATRIX=YES, STRUCTURAL DAMPING MATRIX=YES, RECOVERY MATRIX=YES, NSET=N3, ELSET=E3 *RETAINED NODAL DOFS Data lines to define the retained degrees of freedom. *SELECT EIGENMODES, GENERATE 1, m, 1 *SUBSTRUCTURE LOAD CASE, NAME=BOUND *BOUNDARY Data lines to define the boundary conditions. *SUBSTRUCTURE LOAD CASE, NAME=LOADS *CLOAD Data lines to define concentrated loading. *DLOAD Data lines to define distributed loading. *END STEP The following template can be used to define substructure instances: *HEADING … *ELEMENT, TYPE=Z101, ELSET=E2 Data line to define the element. *SUBSTRUCTURE PROPERTY, ELSET=E2 *BOUNDARY … *RESTART, WRITE *STEP *STATIC … *BOUNDARY … *SLOAD E2, LOADS, scale factor *SUBSTRUCTURE PATH, ENTER ELEMENT=n *EL PRINT S, *NODE PRINT U, *SUBSTRUCTURE PATH, LEAVE *END STEP *STEP *DYNAMIC … *BOUNDARY … *SUBSTRUCTURE PATH, ENTER ELEMENT=n *EL PRINT S, *NODE PRINT U, V *SUBSTRUCTURE PATH, LEAVE *END STEP 10.1.2 DEFINING SUBSTRUCTURES Products: Abaqus/Standard Abaqus/CAE References • “Using substructures,” Section 10.1.1 • *RETAINED NODAL DOFS • *SELECT EIGENMODES • *SUBSTRUCTURE COPY • *SUBSTRUCTURE DELETE • *SUBSTRUCTURE DIRECTORY • *SUBSTRUCTURE GENERATE • *SUBSTRUCTURE LOAD CASE • *SUBSTRUCTURE MATRIX OUTPUT Overview This section describes how individual substructures are defined. Section 10.1.1, for information regarding how they are used in a model. See “Using substructures,” Substructures are defined using the substructure generation procedure. The substructure creation and usage cannot be included in the same analysis. Multiple substructures can be generated in an analysis. Any substructure can consist of one or more other substructures; if this is the case, the nested-level substructures must be defined first. The substructure library is not organized in terms of part instances; therefore, substructures cannot be generated from models that have an assembly defined. None of the substructure options are supported in models that have an assembly defined. To define a typical substructure generation step, do the following: • Invoke the substructure generation procedure. • Define the nodes and degrees of freedom that are to be retained as external degrees of freedom when the substructure is used. • Optionally, retain extra dynamic modes to improve the dynamic behavior of the substructure during usage. • Optionally, specify substructure load cases. • Optionally, write the recovery matrix, substructure’s stiffness matrix, mass matrix, and/or load case vectors to a file. Generating a substructure When you generate a substructure, you specify an identifier that will be assigned to this substructure in a substructure library. The identifier must begin with the letter Z followed by a number that cannot exceed 9999. Substructure identifiers must be unique within a library. If a substructure with this same identifier already exists in the library, the analysis will terminate with an error message unless you have specified that the existing substructure should be overwritten, as described below. *SUBSTRUCTURE GENERATE, TYPE=Zn Step module: Create Step: Linear perturbation: Substructure generation: n Abaqus/CAE Usage: Input File Usage: Substructure database A substructure database is the set of files that describe the geometry of a substructure, and Abaqus writes all substructure data to the substructure database during the analysis. The substructure database can include files with the following extensions: .sup, .sim, .prt, .mdl, and .stt; the .sup file is called the substructure library. By default, substructure data are written to a substructure database named jobname, and the substructure files are named jobname.sup, jobname_Zn.sim, jobname_Zn.prt, jobname_Zn.mdl, and jobname_Zn.stt. Files with the extensions .sup and .sim are generated for all substructures. Files with the extensions .prt, .mdl, and .stt are generated only if the solution within the substructure can be fully or partially recovered. Several substructures can share a substructure library file, but other files are individual for each substructure. It is strongly recommended that the substructure library name be different for different substructures. You can choose to write the data to a user-specified substructure database. If you specify the substructure library name, the files will be named library_name_Zn.sim, library_name_Zn.prt, library_name_Zn.mdl, and library_name_Zn.stt. Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE GENERATE, TYPE=Zn, LIBRARY=library_name Definition of substructure libraries is not supported in Abaqus/CAE. Overwriting the substructure data in a library If a substructure generation analysis is rerun using the same jobname without deleting the substructure library and one substructure or more will be regenerated, you must specify that the existing substructures can be overwritten. This requirement also holds true if the jobname is different for the second analysis but the same library_name is specified. Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE GENERATE, TYPE=Zn, LIBRARY=library_name, OVERWRITE Definition of substructure libraries is not supported in Abaqus/CAE. Recovery within a substructure By default, the solution at any degree of freedom in the substructure can be recovered. Abaqus must have access to the substructure’s .mdl, .prt, and .stt files to perform a full recovery. These files all reside in the substructure database. You can specify that a recovery of element or nodal information will not be required within this substructure. This reduces the size of the substructure database significantly for a large substructure because the information that is needed to recover eliminated variables is not stored. However, this information cannot be recreated at a later time except by regenerating the entire substructure with recovery enabled. Input File Usage: Use the following option to enable recovery for a substructure: *SUBSTRUCTURE GENERATE, TYPE=Zn, RECOVERY MATRIX=YES (default) Use the following option to disable recovery for a substructure: Abaqus/CAE Usage: *SUBSTRUCTURE GENERATE, TYPE=Zn, RECOVERY MATRIX=NO Use the following option to enable recovery for a substructure: Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Whole model Use the following option to disable recovery for a substructure: Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle off Evaluate recovery matrix for Using the selective recovery method If results recovery is desired only at a subset of the internal degrees of freedom, disk usage can be reduced substantially by using the selective recovery method. To enable selective recovery, the region where recovery is desired can be specified directly. Input File Usage: Use the following option to define the node set for selective recovery: *SUBSTRUCTURE GENERATE, RECOVERY MATRIX=YES, NSET=Node set name Use the following option to define the element set for selective recovery: *SUBSTRUCTURE GENERATE, RECOVERY MATRIX=YES, ELSET=Element set name Abaqus/CAE Usage: Use the following option to define the node set for selective recovery: Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Region: Node set name Use the following option to define the element set for selective recovery: Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Region: Element set name Evaluating frequency-dependent material properties When frequency-dependent material properties are specified, Abaqus/Standard offers the option of choosing the frequency at which these properties are evaluated for use in substructure generation. If you do not choose the frequency, Abaqus/Standard evaluates the stiffness at zero frequency and does not consider the stiffness contributions from frequency-domain viscoelasticity. If you do specify a frequency, only the real part of the stiffness contributions from frequency-domain viscoelasticity is considered. Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE GENERATE, PROPERTY EVALUATION=frequency Step module: Step editor: Substructure generate: Options tabbed page: toggle on Evaluate frequency-dependent properties at frequency: frequency Defining the retained degrees of freedom The degrees of freedom at a node can be divided into retained degrees of freedom (for use at the usage level of the substructure) and eliminated degrees of freedom (internal to the substructure). Abaqus/Standard allows any of the degrees of freedom at any of the nodes of a substructure to be retained with one exception: if an acoustic-structural substructure is generated, based on coupled or uncoupled modes, only structural degrees of freedom can be retained. You must make sure that the choice of retained degrees of freedom is reasonable so that the substructure can be connected correctly to the rest of the model. Any degrees of freedom where kinematic constraints may have to be respecified during usage of the substructure should be kept as retained degrees of freedom. If any degrees of freedom of nodes used to define distributing coupling elements are retained, the degrees of freedom of an internal node associated with the Lagrange multipliers are added automatically to the list of the retained degrees of freedom of the substructure. To define the retained degrees of freedom, specify the node number or node set label and, optionally, the first and the last degree of freedom to be retained. By default, the nodes associated with the retained degrees of freedom will be sorted into ascending numerical order. Input File Usage: Abaqus/CAE Usage: *RETAINED NODAL DOFS Load module: boundary condition editor: Category: Mechanical: Types for Selected Step: Retained nodal dofs Preventing the degrees of freedom from being sorted You can prevent the degrees of freedom from being sorted. The ordering of the nodes when using a substructure is then the same as the ordering used when specifying the retained nodes. Input File Usage: Abaqus/CAE Usage: *RETAINED NODAL DOFS, SORTED=NO You cannot prevent retained nodes from being sorted in Abaqus/CAE. Retaining degrees of freedom when the substructure is intended for geometrically nonlinear analysis at the usage level When the substructure is intended for use in geometrically nonlinear analyses, it is recommended to retain all translational and/or all rotational degrees of freedom from a particular node. Even in the case when only a single translational/rotational degree of freedom of a particular node is deemed as needed at the usage level, you should retain all translational/rotational degrees of freedom associated with that node. Otherwise, as the substructure rotates during a geometrically nonlinear analysis, local numerical instabilities (negative eigenvalues) may occur since the rotated substructure may have no stiffness in particular degrees of freedom. You must choose an appropriate number of nodes that will allow for the computation of an equivalent rigid body motion of the substructure. In two-dimensional or axisymmetric analyses, retaining two nodes with all translational degrees of freedom or one node with all translational and rotational degrees of freedom is sufficient to compute an equivalent rigid body motion of the substructure at the usage level. In three-dimensional analysis, three non-colinear nodes with all translational degrees of freedom retained or one node with all translations and rotations are needed. If the retained nodes are colinear or fewer than three nodes are retained, you must retain at least one node with all rotational degrees of freedom. When Abaqus/Standard cannot compute an equivalent rigid body motion for the substructure during the analysis at the usage level because the number of retained degrees of freedom is not appropriate, a warning message is issued and any geometrically nonlinear effects associated with the substructure are ignored. Defining kinematic constraints Kinematic constraints are defined as described in “Kinematic constraints: overview,” Section 34.1.1. The following rules apply: • All kinematic boundary conditions associated with degrees of freedom that are not retained must be specified when the substructure is generated. The conditions are built into the substructure and remain imposed any time that it is used. Once the substructure is generated, kinematic constraints on internal variables cannot be respecified; they can be modified or removed only by erasing and recreating the substructure in the library. The magnitude of a prescribed boundary condition applied to an internal degree of freedom can be associated with a substructure load case and can be changed at the usage level. The restraint itself is built into the substructure and cannot be removed by omitting a reference to the load case. • During substructure generation, multi-point constraints in which some of the substructure’s retained degrees of freedom are eliminated in favor of internal degrees of freedom must be avoided. If it is desirable to retain certain degrees of freedom that are eliminated by the multi-point constraints, you must reassign all of the variables appearing in the multi-point constraints as retained degrees of freedom and impose the constraints at the usage level. Defining the generalized degrees of freedom An effective technique for modeling the dynamic behavior of a substructure is to augment the response within the substructure by including some generalized degrees of freedom associated with the dynamic modes. You can select the modes to retain, which must be calculated in a previous frequency extraction step (“Natural frequency extraction,” Section 6.3.5). The selected modes have to be fully recovered: if they were computed with the AMS eigensolver and only partially recovered, an error message will be issued. The modes will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. If all retained degrees of freedom of the substructure are constrained in the frequency extraction step, this technique is commonly referred to as the Craig-Bampton method. If all retained degrees of freedom of the substructure are not constrained in the frequency extraction step, this technique is commonly referred to as the Craig-Chang method. The substructure dynamic modes in the Craig- Bampton method are commonly referred to as the fixed-interface modes, and the substructure dynamic modes in the Craig-Chang method are commonly referred to as the free-interface modes. If some retained degrees of freedom of the substructure are constrained and other retained degrees of freedom are not constrained in the frequency extraction step, the dynamic modes are called mixed-interface modes. If the free-interface or mixed-interface dynamic modes are selected, the substructure generation time can increase substantially compared to the case when the same number of fixed-interface dynamic modes is used. Abaqus issues a warning message in this case. However, better solution accuracy can sometimes be achieved with a significantly smaller number of free- or mixed-interface dynamic modes than by using fixed-interface modes. A sufficient number of the dynamic modes should be selected to provide adequate dynamic representation of the substructure. Examine loading frequencies and frequency content of the structure to determine this range. Specify a shift point and/or a cutoff frequency in the eigenfrequency extraction step definition to obtain modes in the desired frequency range only. Inclusion of generalized degrees of freedom adds the cost of the frequency extraction to the substructure generation step but greatly improves the accuracy of the solution if the substructure is used in a subsequent dynamic (“Implicit dynamic analysis using direct integration,” Section 6.3.2), steady-state dynamic (“Direct-solution steady-state dynamic analysis,” Section 6.3.4), or frequency extraction (“Natural frequency extraction,” Section 6.3.5) analysis. In the case of the displacement normalization of the eigenvectors in a frequency extraction analysis, a substructure must have at least one physical degree of freedom active on the usage level; otherwise, the modes cannot be normalized properly. See “Substructuring and substructure analysis,” Section 2.14.1 of the Abaqus Theory Manual, for additional details. The retained eigenmodes must be selected when an acoustic-structural substructure is generated. The effect of acoustic-structural coupling can be included in the retained eigenmodes during the natural frequency extraction procedure. To calculate the coupled structural-acoustic eigenmodes, use a frequency extraction analysis with the default Lanczos eigensolver and include the effect of acoustic- structural coupling during the natural frequency extraction procedure (“Natural frequency extraction,” Section 6.3.5). Abaqus can also use uncoupled eigenmodes, generated from either SIM-based Lanczos or AMS eigensolver, to generate a coupled acoustic-structural substructure. In this case the effect of acoustic-structural coupling is included during the substructure generation. Both structural and acoustic eigenmodes have to be retained for the substructure generation, and the selection of the acoustic zero-frequency modes, if such modes are present, is required to get an accurate substructure. Selecting the modes to be used in a substructure generation analysis by their mode numbers You can directly specify the eigenmodes to be used in a substructure generation analysis by their mode numbers. Input File Usage: *SELECT EIGENMODES eigenmode 1, eigenmode 2, etc. Abaqus/CAE Usage: Use the following option to generate the list of eigenmodes by mode range, with each row in the data table specifying a single mode number. The starting mode number and ending mode number in each row should be equal, and the increment value should be zero. Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Specify retained eigenmodes by: Mode range: Start Mode: eigenmode 1: End Mode: eigenmode 1: Increment: 0 Start Mode: eigenmode 2: End Mode: eigenmode 2: Increment: 0 etc. Generating a list of the eigenmodes by mode range Instead of listing all the retained eigenmode numbers, you can generate the list of eigenmodes. Input File Usage: Use the following option to generate the list of eigenmodes by mode range, with each data line specifying the start mode number, the end mode number, and the increment in mode numbers between these two values: *SELECT EIGENMODES, GENERATE first mode number, last mode number, increment Abaqus/CAE Usage: Use the following option to generate the list of eigenmodes by mode range, with each row in the data table specifying the start mode number, the end mode number, and the increment in mode numbers between these two values: Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Specify retained eigenmodes by: Mode range: Start Mode: first mode number: End Mode: last mode number: Increment: increment Generating a list of the eigenmodes by frequency range You can select all the modes from the specified frequency range including frequency boundaries. Input File Usage: Abaqus/CAE Usage: Use the following option to generate the list of eigenmodes by frequency range, with each data line specifying the lower boundary of the frequency range and the upper boundary of the frequency range: *SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE lower boundary of the frequency range, upper boundary of the frequency range Use the following option to generate the list of eigenmodes by frequency range, with each row in the data table specifying the lower boundary of the frequency range and the upper boundary of the frequency range: Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Specify retained eigenmodes by: Frequency range: Lower Frequency: lower boundary of the frequency range: Upper Frequency: upper boundary of the frequency range Preloading a substructure Substructures can be used in models that exhibit nonlinear response (associated with standard Abaqus elements or with contact definitions), but the response within a substructure assumes linear small deformations. However, a substructure’s response may be a linear perturbation about a predeformed (possibly rotating and translating) base state, defined on the basis of nonlinear response within the substructure during its preload history. When the substructure is intended for use in geometrically nonlinear analyses, the substructure preloading should be limited to loads that generate self-equilibrating stresses only (such as thermal stresses or interference fits). In most cases, preload stresses are not self-equilibrating (such as stresses from specified boundary conditions or applied loads). If non-self-equilibrating prestress exists and the substructure undergoes a rigid body motion at the usage level, additional stress is generated in the substructure. Such usage level stresses are non-physical and will lead to convergence problems and results that are difficult to interpret. Therefore, you should use extreme care when preloading a substructure intended for use in geometrically nonlinear analyses. This preloading concept allows such effects as stress stiffening to be included in a substructure. Preloading is a part of the state of the substructure: the preload is self-equilibrating and so does not generate a load vector when the substructure is used. Any loading of the substructure during its use in a model is in addition to the preload. It is important to distinguish the difference between a preload and a load case. Both are allowed during a substructure generation analysis, but only the preloads are actually applied to the substructure during generation. Load cases, defined during substructure generation, can only be applied at the usage level . Load cases are discussed in more detail later. Computation of the total response of a variable Any recovered response variable within a substructure (such as stress or displacement) is defined to be a perturbation (with some exceptions for geometrically nonlinear analyses) from the preloaded base state. For geometrically nonlinear analyses, the displacement output includes both the equivalent rigid body rotation and translation associated with the substructure and the strain-inducing small-displacement perturbation. If the total response of a variable is desired, it can be computed by adding the perturbation result to the final result computed during the substructure preload. Computation of the tangent stiffness of a preloaded substructure The rules for calculating the stiffness matrix of a preloaded substructure are the same as those for a static linear perturbation step. See “General and linear perturbation procedures,” Section 6.1.3, for a detailed description of the rules. Defining a preloading history Specify the loading history that defines the preload state for a substructure. Input File Usage: Abaqus/CAE Usage: Use the following options: *STEP Options to define the preloading history. *END STEP Any number of steps can be defined. *STEP *SUBSTRUCTURE GENERATE Options to define the substructure. *END STEP The Substructure generation step must be defined after the preloading steps in an Abaqus/CAE analysis. Prescribing boundary conditions at retained degrees of freedom during preloading steps During substructure preloading, boundary conditions can be prescribed at retained degrees of freedom. When the preloaded substructure is subsequently created in a substructure generation step, you must release all the retained degrees of freedom . An error message will be issued if some of the retained degrees of freedom are not released. The reaction forces at the released degrees of freedom become concentrated loads that are in equilibrium with the stresses within the substructure. These concentrated loads cannot be removed without changing the preload. The preloaded substructure is, thus, in equilibrium. If the preload in a substructure must effectively apply loading to other parts of the structure, a substructure load case corresponding to the loads applied in the preload history must be created. The technique is demonstrated in “Analysis of a rotating fan using substructures and cyclic symmetry,” Section 2.2.1 of the Abaqus Example Problems Manual. Generating a reduced mass matrix for a substructure You can generate a reduced mass matrix for a substructure. A reduced mass matrix is calculated by projecting the global mass matrix to the subspace of the substructure modes. This technique is known as Guyan reduction if only the static modes associated with the nodal retained degrees of freedom are used. Using only the static modes may not be sufficient to define the dynamic response of the substructure accurately. Additional dynamic modes must be used to improve the response inside the substructure. Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE GENERATE, TYPE=Zn, MASS MATRIX=YES Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute reduced mass matrix Generating a reduced viscous damping matrix for a substructure You can generate a reduced viscous damping matrix for a substructure. The reduced viscous damping matrix is calculated in a manner similar to that used for the reduced mass matrix. Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE GENERATE, TYPE=Zn, VISCOUS DAMPING MATRIX=YES Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute reduced viscous damping matrix Generating a reduced structural damping matrix for a substructure You can generate a reduced structural damping matrix for a substructure. The reduced structural damping matrix is calculated in a manner similar to that used for the reduced mass matrix. Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE GENERATE, TYPE=Zn, STRUCTURAL DAMPING MATRIX=YES Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute reduced structural damping matrix Generating substructures with unsymmetric damping matrices When a coupled acoustic-structural substructure, generated from coupled or uncoupled modes, is generated from a model with damping specified on the acoustic domain, the substructure damping matrices are unsymmetric. The substructure viscous damping matrix will be unsymmetric if a substructure is generated from the rolling tire. Abaqus does not automatically generate an unsymmetric substructure in these cases. You must explicitly select the unsymmetric solver for the substructure generation step to obtain correct substructure damping matrices with unsymmetric contributions. Defining substructure load cases for subsequent loading in an analysis The load cases defined during the generation of a substructure and activated at the usage level are the equivalent of the elemental loading types available for the regular elements in Abaqus. They can be made up of any combination of loadings (distributed loads, concentrated nodal loads, thermal expansion, and load cases defined for any substructures that may be used as part of the definition of this substructure). The load cases are needed so that, when the substructure is subsequently used in a model, the consistent loads on the retained degrees of freedom need be scaled only by the appropriate magnitudes of the particular loads applied: it is not necessary to go inside the substructure and repeat the basic element calculations to distribute the loads. Each such load case can be applied when the substructure is used by associating it with an amplitude/time curve and a magnitude (“Amplitude curves,” Section 33.1.2). When a substructure is used, the substructure load case loadings that were created when the substructure was generated are the only loads that can be used in that substructure. Except for gravity loading, when using the substructure, you cannot apply distributed loads, temperature loads, etc. to the elements that make up any substructure. These loads must be built into the substructure during its creation. You can define multiple substructure load cases during the substructure generation to define different loadings for the substructure. Each load case is assigned a name that will be used when the load case is applied on the usage level. You can use any combination of concentrated load, distributed load, substructure load, and temperature fields (“Concentrated loads,” Section 33.4.2; and “Distributed loads,” Section 33.4.3) to define each load case. You assign each basic loading a reference magnitude, which will then be scaled by the actual magnitude specified when the substructure load is applied. The reference magnitude assigned to each basic loading must be defined as the change in load or boundary condition from the base state, not the total of the base state plus the perturbation value. Initial conditions applied within the substructure generation are not included as part of a load case definition. For temperature loads, the load vector for the substructure load case will contain only the contributions due to thermal expansion. If temperature-dependent properties are present, they are evaluated at the temperatures specified in the preloaded state. Consequently, to take into account nonzero initial temperature fields prescribed as initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1), it is necessary to preload the structure before creating the substructure. When using temperature loading in a substructure load case, the data cannot be read from a results file. The temperatures specified must be defined as the change in the temperatures from the base state. Abaqus/Standard currently has a limitation when a substructure load case definition includes acoustic loading during a substructure generation procedure in which retained modes are specified: the contribution of the singular (constant pressure) acoustic modes (“Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1) is not taken into account in the generated load case. Since the contribution of this mode is significant for low frequency response, the generated load case will inadequately represent the specified acoustic load in these cases. If there are no singular acoustic regions in the coupled acoustic-structure substructure, the acoustic loads are represented accurately. It is important to distinguish the difference between a load case and a preload. Both are defined during substructure generation, but only the preloads are actually applied to the substructure on the generation level; load cases, defined on the generation level, can only be applied on the usage level, and they act on a preloaded base state if one has been specified. (Preloads were discussed earlier.) In general analysis steps and perturbation steps substructure loads are treated in the same way as other loads, such as concentrated loads and distributed loads (“Concentrated loads,” Section 33.4.2, and “Distributed loads,” Section 33.4.3). For example, if a general analysis step is followed by another general analysis step, the substructure loads will be retained in the second step with their magnitude equal to that at the end of the previous general analysis step, unless the substructure load is modified or removed. In a linear perturbation step the substructure load represents an incremental load. If a substructure load is used to apply Coriolis loading in a direct-solution steady-state dynamic analysis, the unsymmetric load stiffness contribution is not taken into account. Input File Usage: Use the following options: *SUBSTRUCTURE LOAD CASE, NAME=name *CLOAD and/or *DLOAD and/or *DSLOAD and/or *TEMPERATURE The load case defined via the *SUBSTRUCTURE LOAD CASE option ends when an option other than *CLOAD, *DLOAD, *DSLOAD, or *TEMPERATURE is encountered. The load definitions can be specified in any order. Abaqus/CAE Usage: Use the following option to define a substructure load case and the loads included in it: Load module: Create Load Case: click : select loads Defining boundary conditions All boundary conditions to be built into the substructure matrices must be specified using a boundary condition definition. These cannot be part of a substructure load case specification. Once a kinematic boundary condition is specified on a particular nodal degree of freedom, it is built into the substructure matrices, is in effect for all load cases, and cannot be removed (or redefined at the usage level). The boundary conditions specified as part of the preloading history are built into the substructure matrices. If there is any doubt whether a restraint is permanent or not, it is better to make the degree of freedom a retained degree of freedom and not specify any restraint in the substructure definition. The restraint can then be included as needed in each analysis step. Load cases when the substructure is used in geometrically nonlinear analyses All loads and boundary conditions included in a substructure load case at the generation level and applied as a substructure load at the usage level are applied in a local system associated with the substructure. Since this system rotates with the substructure when large motions are present, these loads and boundary conditions will rotate as well. As a consequence, you should be careful when using substructure load cases in geometrically nonlinear analyses to ensure that the loading is in the appropriate direction at the usage level. This situation is similar to rotating the substructure using a substructure property definition. Gravity loading To apply gravity loading, density must be defined for at least some of the elements included in the substructure. A gravity load can be applied to a substructure in two different ways with two different interpretations. If a distributed load definition is used as a part of a substructure load case during substructure generation (as described in “Defining substructure load cases for subsequent loading in an analysis” above), the gravity loading becomes part of the substructure load case and, hence, rotates to follow the substructure’s local system during usage (the local system may rotate by rotating the substructure via a substructure property definition or due to geometrically nonlinear response). To define gravity loading that acts in a fixed global direction during usage, you can request that the substructure’s gravity load vectors be calculated during substructure generation. In this case gravity loading should not be defined as part of a substructure load case. When the gravity load vectors are calculated, Abaqus/Standard generates a gravity load vector for each global direction (three for three-dimensional analyses and two for two-dimensional/axisymmetric analyses). At the usage level, a distributed load definition can be used to specify gravity loading on the substructure that acts in a fixed global direction with the specified magnitude. Input File Usage: Abaqus/CAE Usage: Use the following option to calculate the substructure’s gravity load vectors during substructure generation: *SUBSTRUCTURE GENERATE, GRAVITY LOAD=YES Step module: Create Step: Linear perturbation: Substructure generation: Options tabbed page: toggle on Compute gravity load vectors Writing the recovery matrix, reduced stiffness matrix, mass matrix, load case vectors, and gravity vectors to a file You can write a substructure’s recovery matrix, reduced stiffness matrix, mass matrix, and load case vectors to a file. This output is useful when the substructure is to be used in another program. The output records can be written either to the Abaqus/Standard results file, to a user-defined file, or to the output database file . In each case you must specify which output to write out: the mass matrix, the recovery matrix, the load case vectors, the stiffness matrix, and/or the gravity load vectors. By default, no output will be generated. Repeat the substructure matrix output request in the substructure generation file of each substructure for which the substructure matrix output is required. If substructure load case vector output is requested for a preloaded substructure, the output will contain a record with a load case number that is equal to zero. This load vector contains the forces that were necessary to equilibrate any stresses that were generated during the previous steps. Input File Usage: *SUBSTRUCTURE MATRIX OUTPUT, MASS=YES, RECOVERY MATRIX=YES, SLOAD=YES, STIFFNESS=YES, GRAVITY LOAD=YES Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Whole model or Region Writing the records to the Abaqus/Standard results file By default, the requested matrices are written to the Abaqus/Standard results file corresponding to the substructure generation input file name. The record formats for the results file are described in “Results file output format,” Section 5.1.2. The file can be written in either binary or ASCII format (“Output,” Section 4.1.1). Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE MATRIX OUTPUT, OUTPUT FILE=RESULTS FILE Abaqus/CAE automatically writes the requested matrices to the Abaqus results file when you run an analysis with a Substructure generation step. Writing the records to the output database file You can specify that the matrices should be written to the output database (.odb) file. Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE MATRIX OUTPUT, OUTPUT FILE=ODB Abaqus/CAE automatically writes the requested matrices to the output database file when you run an analysis with a Substructure generation step. Writing the records to a user-defined file You can specify the name of the file (without an extension) to which the data will be written. The records are written to be compatible with a linear user-defined element. The record formats are described in “User-defined elements,” Section 32.15.1. An .mtx extension will be added to the file name specified. Input File Usage: *SUBSTRUCTURE MATRIX OUTPUT, OUTPUT FILE=USER DEFINED, FILE NAME=file_name Abaqus/CAE Usage: Job module: job editor: Name Managing substructures inside libraries Substructures are stored in a collection of libraries. Housekeeping functions are provided to help maintain extensive libraries; for example, substructures can be deleted from a library or moved to a different library. Once a substructure library has been generated, the disk files can be made read-only to protect the library from accidental deletion or modification. A substructure library must be write-accessible during a substructure’s generation and when substructures are added or deleted from a library using the substructure housekeeping functions. When multiple analyses are used to generate a substructure library, these analyses must be run one after another; they cannot be run simultaneously. Abaqus may not be able to provide any indication that the substructure library being written may already be in use by another Abaqus analysis. If several analyses write to the same library simultaneously, the library may get corrupted. If this occurs and the library is used in a subsequent analysis, the result may be a large preprocessor memory demand. Input File Usage: Use any of the following options (described in detail below) to perform housekeeping functions on substructure libraries: *SUBSTRUCTURE COPY *SUBSTRUCTURE DELETE *SUBSTRUCTURE DIRECTORY The housekeeping options can appear anywhere within the model portion of the input file (“Defining a model in Abaqus,” Section 1.3.1). An input file can consist of merely the *HEADING option and one or more of the housekeeping options. In this case the files and substructures to which the housekeeping options refer must exist at the start of the analysis. Abaqus/CAE Usage: Substructure libraries are not supported in Abaqus/CAE. Listing the substructures stored in a substructure library You can obtain a summary of information about the substructures stored in a substructure library. If necessary, you can identify a nondefault name for the library (the default name is jobname). Input File Usage: Abaqus/CAE Usage: *SUBSTRUCTURE DIRECTORY, LIBRARY=substructure_library_name Substructure libraries are not supported in Abaqus/CAE. Removing a substructure from a substructure library You can remove a specified substructure from a substructure library. If necessary, you can identify the name of the library. Input File Usage: *SUBSTRUCTURE DELETE, TYPE=Zn, LIBRARY=substructure_library_name Abaqus/CAE Usage: Substructure libraries are not supported in Abaqus/CAE. Copying or moving a substructure definition You can copy a substructure definition from one library to another or from one substructure to another within the same library. You must identify the substructure being copied and assign a name to the substructure being created. When copying substructures from library to library, you can identify the name of the library containing the substructure being copied. Similarly, you can identify the name of the new library to which the substructure will be copied. This new library need not exist prior to the substructure being copied; it will be created in this case. If the original substructure is to be deleted, you can follow the copy with a delete . Input File Usage: *SUBSTRUCTURE COPY, OLD TYPE=Zn, NEW TYPE=Zn, OLD LIBRARY=substructure_library_name, NEW LIBRARY=substructure_library_name Abaqus/CAE Usage: Substructure libraries are not supported in Abaqus/CAE. Renaming substructure libraries Once a substructure library has been generated, the disk file should not be renamed manually. To rename a substructure library, copy the existing substructures to a new library. The new library need not exist prior to the first substructure being copied. You can then delete the original disk file manually if you do not need it anymore. 10.2 Submodeling • “Submodeling: overview,” Section 10.2.1 • “Node-based submodeling,” Section 10.2.2 • “Surface-based submodeling,” Section 10.2.3 10.2.1 SUBMODELING: OVERVIEW Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Node-based submodeling,” Section 10.2.2 • “Surface-based submodeling,” Section 10.2.3 • *SUBMODEL • Chapter 38, “Submodeling,” of the Abaqus/CAE User’s Manual Overview The submodeling technique: • is used to study a local part of a model with a refined mesh based on interpolation of the solution from an initial (undeformed), relatively coarse, global model; • is most useful when it is necessary to obtain an accurate, detailed solution in a local region and the detailed modeling of that local region has negligible effect on the overall solution; • can be used to drive a local part of the model by nodal results, such as displacements , or by the element stress results from the global mesh; • can be used to analyze an acoustic model driven by displacements from a structural, global model when the acoustic fluid has negligible effect on the structural solution; • can be used for the analysis of a structure driven by acoustic pressures from an acoustic or coupled acoustic-structural, global model; • can use a combination of Abaqus/Explicit and Abaqus/Standard procedures; • can use a combination of linear and nonlinear procedures; and • cannot be used in an import analysis. Terminology The model whose solution is interpolated onto the relevant parts of the boundary of the submodel is referred to as the “global” model (even though it may itself be a submodel of a larger “global” model). Driven variables are defined as those variables in the submodel that are constrained to match results from the global model. Driven variables can be degrees of freedom at nodes in the node-based technique, or they can be components of stress tensor at the integration points of element faces in the surface-based technique. Submodeling techniques Submodeling can be applied quite generally in Abaqus. The material response defined for the submodel may be different from that defined for the global model. Both the global model and the submodel can have nonlinear response. See “Shell-to-solid submodeling and shell-to-solid coupling of a pipe joint,” Section 1.1.10 of the Abaqus Example Problems Manual, for an example application of the submodeling technique. Submodeling is classified first according to which of two basic techniques is used. The most common, and more general technique, is node-based submodeling, which uses a nodal results field (including displacement, temperature, or pressure degrees of freedom) to interpolate global model results onto the submodel nodes. The alternative surface-based technique uses the stress field to interpolate global model results onto the submodel integration points on the driven element-based surface facets. You can choose either the node-based or surface-based technique or a combination of the two in your submodel. The following factors should be considered in deciding on the technique to be used: • Whether you are performing solid-to-solid submodeling in a general static analysis in Abaqus/Standard: – Surface-based submodeling is available only for solid models and static analyses. – For all other procedures use the node-based technique. • Whether the global model and submodel differ significantly in their average stiffness in the region of the submodel: – When the stiffness of the models is comparable, node-based submodeling of displacements will provide comparable results to the surface-based technique with a lesser likelihood of numerical issues associated with rigid-body modes. – When the stiffness of the models differs and the global model is exposed primarily to a load-controlled environment, the surface-based technique will generally provide more accurate stress results. Stiffness differences may arise due to additional detail in the submodel, such as explicit modeling of a fillet or a hole. In other cases stiffness changes may result from minor geometry changes for which a reanalysis of the global model is not warranted. • Whether your model is subjected to large deformations or rotations: – Node-based submodeling of displacements will result in more accurate transmission of large deformation and rotation to the submodel. • Whether the displacement response of the global model corresponds to the displacement response of the submodel: – When the displacements in the global model correspond closely with the expected displacements in the submodel, node-based submodeling is generally preferable. – Surface-based submodeling should be used when the submodel displacement response is expected to differ from the global model response. This situation can occur when thermal strains are modeled and the temperature history of the submodel differs from that of the global model; for example, when heat transfer submodeling is performed as part of a sequential thermal-structural analysis. • The stiffness of the structure: – Surface-based submodeling may provide more accurate results for very stiff structures. When the structure is so stiff that only a small component of the global model displacement field contributes to the stress response, numerical roundoff in the displacement results can become significant; for example, when the global model displacement is dominated by a rigid-body motion component. • The type of output you are interested in from the submodel: – Node-based submodeling of displacements will result in more accurate transmission of a displacement field. – Surface-based submodeling will result in more accurate transmission of a stress field, and determination of reaction forces in the submodel. You can use both node-based submodeling and stress-based submodeling in the same model. Node-based submodeling Node-based submodeling is the more general combinations and procedures in both Abaqus/Explicit and Abaqus/Standard. technique, supporting a variety of element type Input File Usage: Abaqus/CAE Usage: *SUBMODEL, TYPE=NODE Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: Driving region: Specify Element types supported Different element types can be used in the submodel than those used to model the corresponding region in the global model. The following types of submodeling are provided for the node-based approach (global-to- submodel): • Two-dimensional models: – Solid-to-solid – Acoustic-to-structure • Three-dimensional models: – Solid-to-solid – Shell-to-shell – Membrane-to-membrane – Shell-to-solid – Acoustic-to-structure A global or submodel is meshed with continuum shell elements constitutes a three-dimensional solid region in the submodeling technique. Hence, the use of the submodeling technique for models involving continuum shell elements is the same as with models involving continuum solid elements such as C3D8R or C3D6. region that Procedures supported Both the global model and the submodel can have nonlinear response and can be analyzed for any sequence of analysis procedures. These procedures do not have to be the same for both models. For example, the linear or nonlinear dynamic response of the global model can be used to drive the static, nonlinear response of the submodel on the grounds that the submodel is too small for dynamic effects to be significant in that local region. The global procedure can be performed in Abaqus/Standard to drive a submodeling procedure in Abaqus/Explicit and vice versa. For example, a static analysis performed in Abaqus/Standard can drive a quasi-static Abaqus/Explicit analysis in the submodel. The step time used in these analyses can be different; the time variable of the amplitude functions generated at the driven nodes can be scaled to the step time used in the submodel. Your submodel cannot refer to a global model step that includes multiple load cases . You must perform the global analysis with a single load definition for the step that will drive the submodel. Surface-based submodeling Surface-based submodeling is provided as a complement to the node-based technique, enabling you to drive the submodel with stresses from the global model. Input File Usage: Abaqus/CAE Usage: *SUBMODEL, TYPE=SURFACE Load module: Create Load: choose Mechanical for the Category and Submodel for the Types for Selected Step: Driving region: Specify Element types supported The following types of submodeling are provided for the surface-based approach (global-to-submodel): • Two-dimensional models: – Solid-to-solid • Three-dimensional models: – Solid-to-solid Different element types can be used in the submodel than those used to model the corresponding region in the global model. Continuum elements supported for the static analysis procedure are supported for surface-based submodeling, with the following exceptions: • Cylindrical elements are not supported. • Continuum shell elements are not supported. Procedures supported The surface-based technique is implemented only for static analysis in Abaqus/Standard. Your submodel cannot refer to a global model step that includes multiple load cases . You must perform the global analysis with a single load definition for the step that will drive the submodel. Performing a submodeling analysis A submodeling analysis consists of: • running a global analysis and saving the results in the vicinity of the submodel boundary; • defining the total set of driven nodes or driven surfaces in the submodel; • defining the time variation of the driven variables in the submodel analysis by specifying the actual nodes and degrees of freedom or element-based surfaces to be driven in each step; and • running the submodel analysis using the “driven variables” to drive the solution. Linking the global model and the submodel The submodel is run as a separate analysis from the global analysis. The only link between the submodel and the global model is the transfer of the time-dependent values of variables saved in the global analysis to the relevant boundary nodes of the submodel or to the relevant boundary surfaces. This transfer is accomplished by saving the results from the global model either in the results (.fil) file or in the output database (.odb) for the node-based technique or in the output database (.odb) for the stress-based technique, then reading these results into the submodel analysis. If the global model is defined in terms of an assembly of part instances, the part (.prt) file from the global model is required for the submodel analysis. Since the submodel is a separate analysis, submodeling can be used to any number of levels; a submodel can be used as the global model for a subsequent submodel. Accuracy The global model in a submodeling analysis must define the submodel boundary response with sufficient accuracy. It is your responsibility to ensure that any particular use of the submodeling technique provides physically meaningful results. In general, the solution at the boundary of the submodel must not be altered significantly by the different local modeling. There is no built-in check of this criterion in Abaqus; it is a matter of judgment on your part. In general, accuracy can be checked by comparing contour plots of important variables near the boundaries of the submodeled region. Specifying the global elements used to drive the submodel By default, the global model in the vicinity of the submodel is searched for elements that encompass the locations of driven nodes or driven surfaces’ faces; the submodel is then driven by the response of these elements. In some cases more than one element can encompass the location of a driven node. For example, adjacent bodies in the global model may have temporarily coincident nodes or surfaces, as depicted in Figure 10.2.1–1. Global model Local model A B contact interface driven node Figure 10.2.1–1 A global model with coincident surfaces in the area of the local model’s driven nodes. In this case the location of the driven node in the corresponding global model is touching both element A and element C; however, only the results from element A should drive the node in the submodel. To preclude certain elements from driving the submodel, you have the option of specifying a global element set to limit the search to an appropriate subset of the global model. Input File Usage: *SUBMODEL, GLOBAL ELSET=name If the global model is defined in terms of an assembly of part instances, give the complete name—including the assembly and part instance names—when specifying the global element set. For example, an element set named top in part instance I-1 of assembly Assembly-1 must be referred to by Assembly-1.I-1.top. If the submodel is not defined in terms of an assembly of part instances, the dots in the global element set name must be replaced by underscores: Assembly- 1_I-1_top. If the global element set is defined at the assembly level, you may provide the element set name without qualifying it with the assembly name in a submodel analysis. Abaqus/CAE Usage: Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: Driving region: Specify Minimizing file sizes The size of the results file or the output database can be minimized for a submodeling analysis by requesting output for only those global nodes and global elements that are used to drive the submodel. To determine which global nodes and/or elements are used to drive the submodel, do the following: 1. Run a data check analysis on the global model with any combination of results file or output database file output requests. A data check analysis is performed by using the datacheck parameter in the command for running Abaqus (“Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2). 2. Run a data check analysis on the submodel. A listing of the global nodes and/or elements that will be used to drive the submodel is output to the data file during the submodeling data check analysis. Frequency of output Pay special attention to the frequency at which you request output in the global model . It is possible to define the results file output or nodal and element output to the output database file such that the information is written at different frequencies for different nodes and elements, although that should not be done for nodes and elements involved in the interpolation to define values at driven variables since Abaqus will take values at the coarsest frequency only. To avoid this problem, write the nodal and elemental output to the output database or the results file using the same frequency for all nodes and elements involved in the interpolation and choose a frequency that will allow the history in the submodel to be reproduced accurately. Input File Usage: To control the output frequency to the Abaqus/Standard results file, use the following option: *NODE FILE, FREQUENCY To control the output frequency to the Abaqus/Explicit results file, use the following option: *FILE OUTPUT, NUMBER INTERVAL To control the output frequency to the output database, use the following option: Abaqus/CAE Usage: *OUTPUT, FIELD, FREQUENCY Step module: Output→Field Output Requests→Create: Frequency Material options Any of the material models described in Part V, “Materials,” can be used in the global and submodel analyses. The material response defined for the submodel may be different from that defined for the global model. Elements The dimensionality of the submodel must be the same as that of the global model: both models must be either two-dimensional or three-dimensional. The following limitations apply: • The boundary nodes of the submodel must lie within regions of the global model where Abaqus is able to perform spatial interpolation to define the values of the driven variables. Therefore, they must lie within (or, as allowed by the exterior tolerance, near to) two- or three-dimensional geometrically defined elements in the global model. Such geometrically defined elements are: – first- or second-order triangles or quadrilaterals in two dimensions; – first- or second-order triangular or quadrilateral shells; and – first- or second-order tetrahedra, wedges, or bricks in three dimensions. • The boundary nodes cannot lie in regions of the global model where there are only one-dimensional elements (beams, trusses, links, axisymmetric shells) since Abaqus does not provide the necessary interpolation of results for such elements. • The boundary nodes cannot lie in regions of the global model where there are only user elements, substructures, springs, dashpots, cohesive elements, etc. since those element types do not allow for geometric interpolation. • The boundary nodes cannot lie in regions of the global model where there are only axisymmetric solid elements with nonlinear, asymmetric deformation (CAXA elements). The submodeling capability is currently not supported for these elements. • The reference node associated with generalized plane strain elements (CPEG) cannot be used as a driven boundary node in a submodeling analysis. Output Any of the output normally available within a particular procedure is also available during a submodeling analysis . As described above, nodal output requests to the results file or output database file must be used in the global analysis to save the values of the driven variables at the submodel boundary. 10.2.2 NODE-BASED SUBMODELING Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Submodeling: overview,” Section 10.2.1 • *SUBMODEL • *BOUNDARY • Chapter 38, “Submodeling,” of the Abaqus/CAE User’s Manual Overview The following types of node-based submodeling are available: • Same-to-same (e.g., solid-to-solid, shell-to-shell); • Shell-to-solid; and • Acoustic-to-structure. These submodel types support the following nodal-driven variables: • Displacement, • Rotation, • Temperature, • Pore pressure, and • Acoustic pressure. Performing a node-based submodeling analysis For an overview of submodeling that includes some details common to both node-based and surface- based submodeling, see “Submodeling: overview,” Section 10.2.1. Your submodel analysis is driven, either partly or completely, from the results obtained from a global model analysis. The results from the global model are interpolated onto the nodes on the appropriate parts of the boundary of the submodel . Thus, the response at the boundary of the local region is defined by the solution for the global model. The driven nodes and any loads applied to the local region determine the solution in the submodel. Different types of node-based submodeling Three different techniques are available for nodal-based submodeling. Solid-to-solid submodeling The linear or nonlinear response of a global solid model can be used to drive the submodel response of a solid submodel. The driven variables can be displacements or temperatures. symmetry submodel boundaries nodes where global model solution must be stored for interpolation Figure 10.2.2–1 The global model. Shell-to-solid submodeling The linear or nonlinear response of a global shell model can be used to drive the submodel response of a solid submodel. The driven variables are displacements, which are determined from global model displacements and rotations. Acoustic submodeling The linear or nonlinear response of a global, structural model can be used to drive the acoustic response of a fluid region of any size if the forces exerted on the structure by the fluid are small. This is often the case for metal structures in air, building interiors, or for sound propagation from a liquid to air. In the case of a liquid and a gas, no special procedures need be followed; the pressure degrees of freedom couple straightforwardly. In the case of a structure driving a fluid, you must ensure that the degrees of freedom to be driven in the submodel exist among the global model results. Several alternatives exist. A thin layer of fluid elements, with the same properties as the submodel fluid, can be added to the global model; this element set and its nodes can then be used to drive the submodel in the usual manner. Alternatively, you can create acoustic interface elements on the surface of the submodel and drive the corresponding nodes with the structural nodes . In problems where the fluid exerts large pressures on the structure, the mechanical response of the structure may be of interest. Acoustic-to-structure submodeling can be used in such problems. The submodel in these problems is a part of the structural component of the global model. The acoustic pressure obtained from solving a coupled acoustic-structural global analysis is used to drive the submodel on the surface it shares with the fluid medium. Other boundaries of the submodel may be driven using the displacements of the structural component of the global model via solid-to-solid submodeling. The acoustic-to-structure submodel analysis solves an uncoupled structural force-displacement problem. The acoustic pressure from the global model is interpolated to the submodel driven nodes. The tributary area and the outward normal associated with the driven node are used to convert the interpolated acoustic pressure to a concentrated load acting at that location . Saving the results from the global model The results from the global analysis must be saved at all nodes required for the interpolation of the driven variables to the boundary of the submodel . The results (.fil) file or the output database (.odb) file can be used for this purpose. Saving the results to the results file In each step of the global model whose solution will be used to drive the submodel, write the nodal results for all driven variables to the results file . These results must be written in the global coordinate system of the model. The submodel can refer only to a global model results file that is from a binary compatible platform. When the global model is run in Abaqus/Explicit and results file output is requested, the results are written to the selected results (.sel) file; this file needs to be converted into a results (.fil) file using the convert option . Input File Usage: Abaqus/CAE Usage: *NODE FILE (In Abaqus/Standard GLOBAL=NO should not be used on the *NODE FILE option.) You cannot write output to the results file in Abaqus/CAE. Saving the results to the output database In each step of the global model whose solution will be used to drive the submodel, write the nodal results for all driven variables to the output database . Unlike the results file, nodal output to the output database is always written in the global directions. The output database can be transferred to any platform since it is binary neutral. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *OUTPUT, FIELD *NODE OUTPUT Step module: Output→Field Output Requests→Create Saving results with higher precision By default, the nodal output to the output database is written using single precision, which may not be sufficient for certain classes of problems; for example, submodels undergoing large rigid body motions (consider also surface-based submodeling in these cases—see “Surface-based submodeling,” Section 10.2.3). For such analyses request the nodal output to the fullest possible precision . Input File Usage: Abaqus/CAE Usage: abaqus job=global_model_input_file output_precision=full Job module: Create Job: Precision: Nodal output precision: Full Saving results from a global model with a physical time scale If the global analysis in Abaqus/Standard involves a physical time scale and the results file is to be used in the submodel analysis, request that the results file output be written at the beginning of the step (the zero increment) for all steps in the global analysis . Abaqus will then have the complete solution history (including the solution state at the beginning of a step) from which a submodel may be driven. If the zero increment results are not requested, incorrect results will be obtained if the step time in the submodel is less than the step time of the first increment on the results file. Instead of interpolating between the results at the start of the step and the results of the first increment on the results file, Abaqus will simply use the results of the first increment as long as the submodel step time is less than the step time of the first increment on the results file. The zero increment request is not required in Abaqus/Explicit, because the results are always written to the results file at the beginning of each step. Similarly, the results will always be correctly interpolated when using the output database to transfer the results from the global model to the submodel, because the zero increment is always written to the output database. Input File Usage: Abaqus/CAE Usage: *FILE FORMAT, ZERO INCREMENT You cannot write output to the results file in Abaqus/CAE. Referring to the global model results from the submodel analysis You must define the source of the global solution results. Provide the name of the global results file or output database file; the file extension is optional. If the file extension is omitted, Abaqus will correctly choose the extension if only the results file or the output database file exists. If the file extension is omitted and both results and output database files exist, the results file will be used. Input File Usage: abaqus job=submodel_input_file globalmodel=global_results_file or global_output_database Abaqus/CAE Usage: Any module: Model→Edit Attributes→submodel: Submodel: Read data from job: global_results_file or global_output_database Specifying the driven nodes in the submodel Specifying the driven nodes does not activate the driven variables: they must be activated by specifying the appropriate submodel boundary conditions. All nodes of the submodel where variables will be driven in any step must be specified as driven nodes since the list of nodes cannot be extended subsequent to its initial definition (even at restart). However, variables at the nodes given do not have to be driven in all steps: the choice of which variables are driven in a particular step is made as part of a submodel boundary condition definition, as discussed later. NODE-BASED SUBMODELING boundary nodes of the submodel driven by global model solution Figure 10.2.2–2 The magnified submodel. Input File Usage: *SUBMODEL list of nodes or node set labels or, for acoustic-to-structure submodeling, the name of an element-based structural surface The *SUBMODEL option must be included in the model definition portion of the input file for the submodel analysis. Multiple *SUBMODEL options are allowed; however, in this case you must ensure that the driven nodes specified on the data line of one option are separate and distinct from the nodes specified on the data lines of all the other options. Abaqus/CAE Usage: Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region Specifying the driven nodes in shell-to-solid submodeling In shell-to-solid submodeling, the submodel is made up of solid elements and replaces a region where conventional shell elements are used in the global model. In this case Abaqus expects that all the driven nodes on the submodel belong to solid elements and are driven from a global model region that is entirely made up of shell elements. The boundary where the submodel is driven is a set of surfaces in the submodel but is a set of lines in the shell reference surface in the global model, as shown in Figure 10.2.2–3. The dashed line on the shell model is replaced by the shaded surfaces of the solid element submodel. a) Shell global model with submodel boundaries A, B, C - shell reference surface - driven nodes b) Magnified solid element submodel Figure 10.2.2–3 Shell-to-solid submodeling. Whenever shell-to-solid submodeling is used, you must define the maximum shell thickness in the global model, given in the units used for the models. If a shell offset is defined in the global model, the shell thickness must be set equal to twice the maximum distance from the top or bottom shell surface to the shell reference surface. Input File Usage: Abaqus/CAE Usage: *SUBMODEL, SHELL TO SOLID, SHELL THICKNESS=thickness If more than one *SUBMODEL option is used, parameter must be included on every option. the SHELL TO SOLID Any module: Model→Edit Attributes→submodel: Submodel: Shell global model drives a solid submodel Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region: Shell thickness: thickness Specifying the driven nodes in acoustic-to-structure submodeling The global analysis for acoustic-to-structure submodeling problems is performed as a coupled acoustic- structural analysis. The acoustic nodal pressures from the global analysis must be written to the results file for the acoustic mesh in contact with the structural surface of interest. In the submodel analysis acoustic pressures from the global analysis drive the user-specified structural surface of interest. The driven nodes for the submodel are the nodes lying on the specified surface. Only element-based surfaces are allowed in acoustic-to-structure submodeling. Input File Usage: *SUBMODEL, ACOUSTIC TO STRUCTURE, ABSOLUTE EXTERIOR TOLERANCE=value Abaqus/CAE Usage: Acoustic-to-structure submodeling is not supported in Abaqus/CAE. Specifying driven nodes for shells with acoustic pressures on both sides In certain problems the acoustic pressure may act on both sides of a shell structure. Figure 10.2.2–4 shows a section of a global model consisting of a shell structure that is sandwiched between two acoustic media. acoustic region 1 SPOS SNEG acoustic region 2 ELSET = Acoustic_SPOS ELSET = Acoustic_SNEG shell structure Figure 10.2.2–4 A cross-section of the acoustic-to-structure global model with acoustic regions on both sides of the shell. Separate element sets consisting of acoustic elements on the positive and negative sides of the shell are defined, respectively. The nodal pressures for nodes attached to elements in these sets are written to the selected results file. Figure 10.2.2–5 shows the submodel that consists only of the refined shell structure. surface Shell_SPOS surface Shell_SNEG driven node shell structure Figure 10.2.2–5 The acoustic-to-structure submodel with acoustic pressure on both sides of the shell. Two separate surfaces are defined on the SPOS and SNEG sides, respectively. To apply the acoustic pressure from the global analysis on each side of the shell correctly, you must specify the surface name along with the corresponding acoustic element set. Input File Usage: *SUBMODEL, ACOUSTIC TO STRUCTURE, GLOBAL ELSET=Acoustic_SPOS Shell_SPOS *SUBMODEL, ACOUSTIC TO STRUCTURE, GLOBAL ELSET=Acoustic_SNEG Shell_SNEG Abaqus/CAE Usage: Acoustic-to-structure submodeling is not supported in Abaqus/CAE. Defining geometric tolerances A geometric tolerance is used to define how far a boundary node in the submodel can lie outside the exterior surface of the global model, as that surface is interpolated in the global, undeformed finite element model. By default, nodes in the submodel must lie within a distance calculated by multiplying the average element size in the global model by 0.05. You can change the tolerance, which is useful in cases where submodel driven nodes lie to a greater extent outside the global model exterior surface. Tolerances larger than this default value, however, may result in significantly greater computation times and lower accuracy in the driven solution for driven nodes significantly outside the global model exterior surface. You can define the geometric tolerance as a fraction of the size of the average element in the global model or as an absolute distance in the length units chosen for the model. If both tolerances are defined, Abaqus uses the tighter tolerance. Input File Usage: Abaqus/CAE Usage: Use the following option to define the geometric tolerance as an absolute distance: *SUBMODEL, ABSOLUTE EXTERIOR TOLERANCE=tolerance Use the following option to define the geometric tolerance as a fraction of the size of the average element in the global model: *SUBMODEL, EXTERIOR TOLERANCE=tolerance Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region: Exterior tolerance: absolute: or relative: tolerance The exterior tolerance in solid-to-solid submodeling The exterior tolerance for a solid-to-solid submodel analysis is indicated by the shaded region in If the distance between the driven nodes and the free surface of the global model Figure 10.2.2–6. falls within the specified tolerance, the solution variables from the global model are extrapolated to the submodel. The exterior tolerance in shell-to-shell submodeling In a shell-to-shell submodel analysis Abaqus checks whether the driven nodes of the submodel lie sufficiently close to the reference surface of the shell elements in the global model. To simplify calculations, the closest point in the global model is calculated as the intersection of a line drawn exterior surface in global model exterior surface in submodel nodes in global model nodes in submodel actual geometric surface Figure 10.2.2–6 The exterior tolerance in solid-to-solid submodeling. through the node on the submodel with the reference surface of the shell in the global model. The direction of the line is normal to a flat surface approximation to each shell element. The normal to the flat surface is the average of the normals at the nodes of the shell element. The distance checked against the specified exterior tolerance is shown in Figure 10.2.2–7. The exterior tolerance in shell-to-solid submodeling For shell-to-solid submodeling Abaqus uses two kinds of tolerances to determine the relationship between the submodel and the global model. First, the closest point on the shell reference surface of the global model is determined. This point, the “image node,” is shown in Figure 10.2.2–8. The user-specified exterior tolerance is used to check if the image node lies within the domain of the global model. Then the distance, , between the driven node and its image is checked; if the distance is less than half the value of the specified shell thickness plus the exterior tolerance, it is accepted. This check is only approximate if the global model has varying shell thickness or if the shell reference surface is offset from the midsurface. interpolated position on shell reference surface plane approximation global model shell reference surface submodel's driven node distance checked against exterior tolerance Figure 10.2.2–7 Flat surface approximation in shell-to-shell submodeling. exterior tolerance AI global model shell elements shell reference surface t = shell thickness A - driven node AI - driven node image on the shell reference surface solid element submodel mesh Figure 10.2.2–8 The exterior tolerance in shell-to-solid submodeling. Permitting driven nodes to be excluded from submodeling In some cases (such as when your submodel geometry is more detailed than the global model in regions near a free surface) you may specify driven nodes that Abaqus will find, even when accounting for the search tolerance, to be outside the region of the global model elements. By default, these cases result in an error message. In solid-to-solid submodeling you can, however, specify that Abaqus ignore driven nodes that cannot be found. Use this option with caution and always evaluate the list of nodes that are labeled as not found. Most cases where Abaqus finds driven nodes to lie outside the global model reflect a modeling error and use of the intersection only option may lead to incorrect results in these cases. Input File Usage: Use the following option to specify that Abaqus ignore driven nodes that cannot be found in the global model elements: *SUBMODEL, INTERSECTION ONLY list of nodes or node set labels The driven nodes ignored through the use of the INTERSECTION ONLY parameter are then ignored in all subsequent submodel boundary condition references. Defining the driven variables in the submodel The actual driven variables are defined in any step as a submodel boundary condition. The boundary conditions are “driven variables” obtained from the results or output database file of the global analysis. The degrees of freedom on the driven nodes of the submodel must exist at the forcing nodes of the global model. In a problem involving an acoustic fluid submodel driven by a structural global model, for example, acoustic interface elements should be created on the submodel’s driven boundary with the structure. For solid-to-solid and shell-to-shell submodeling specify the individual degrees of freedom to be driven. In most cases all components of the solution variables (displacements, rotations, temperatures, etc.) at these nodes are driven by the global solution, although you may choose to drive only some components at any of the driven nodes. For shell-to-solid submodeling the driven degrees of freedom are chosen automatically based on a user-specified zone around the shell reference surface, as explained later. Abaqus/Explicit does not admit jumps in displacement and rotation boundary conditions ; any jumps in the driven displacements and rotations will be ignored. It is not recommended to have all the variables at all the nodes in the submodel driven by the global solution. For acoustic-to-structure submodeling, the loads due to acoustic pressure acting at the driven nodes of the submodel are activated by specifying pressure (degree of freedom 8) along with the driven node set. Only one submodel boundary condition can be specified in each step of the analysis. Input File Usage: Abaqus/CAE Usage: *BOUNDARY, SUBMODEL Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region: Degrees of freedom: degrees of freedom Specifying the step number from the global analysis You specify the step of the global model history that is to be used for the driven variables in the current submodel analysis step. When the global solution is obtained from the results file, the zero increment is included if it was requested in the global analysis . In a general analysis step or a direct-solution steady-state dynamic analysis step, Abaqus calculates the amplitudes for the driven variables as functions of time or frequency from the results of the global model. Input File Usage: Abaqus/CAE Usage: *BOUNDARY, SUBMODEL, STEP=step Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region: Global step number: step Scaling the global time period to the submodel time period The global analysis and submodel analysis can have different time steps. You can scale the time variable of the driven nodes from the global analysis to the step time of the submodel analysis. This technique is useful when the analyses are static or quasi-static in nature; the use of this technique in dynamic analyses with significant inertial effects is not recommended. If the same step time is used in both the global model and the submodel, the time scale has no effect. The time scale cannot be specified in frequency domain analyses or in linear perturbation steps. Abaqus will determine the values that the driven variables will follow throughout the step in the submodel analysis by using the points in time at which the global solution results or output database file was written. When the time variable of the driven nodes of the global analysis is scaled and if the step time is different from the submodel step time, the points in time of the driven variables are scaled to the submodel step time. Input File Usage: Abaqus/CAE Usage: *BOUNDARY, SUBMODEL, STEP=step, TIMESCALE Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region: Scale time period of global step to time period of submodel step Scaling the magnitude of driven variables For displacement-based submodeling the magnitude values of driven variables are obtained by multiplying the displacement history as obtained from the global analysis by a scaling parameter. You can scale the driven variables by setting the scaling parameter in the definition of the submodel boundary conditions. This technique is useful in scaling the submodel boundary conditions in a multiple-step analysis without rerunning the global model. It can be used in Abaqus/Standard and Abaqus/Explicit for the same-to-same and shell-to-solid cases except for acoustic-to-structure submodeling. *BOUNDARY, SUBMODEL, STEP=step, SCALE=scalarValue Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region: Scale: scale Abaqus/CAE Usage: Input File Usage: Modifying the set of driven variables You can modify the submodel boundary condition to add new variables to the list of driven variables, you can remove variables from the driven variable set, and you can reintroduce them later . New nodes cannot be added to the total set of driven nodes defined for the submodel; this set of driven nodes is a fixed part of the model definition. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *BOUNDARY, SUBMODEL, OP=MOD *BOUNDARY, SUBMODEL, OP=NEW Load module: boundary condition editor: Degrees of freedom Automatically selecting the driven variables in shell-to-solid submodeling For shell-to-solid submodeling the driven degrees of freedom at the driven nodes are chosen automatically, depending on the distance between the driven node and the global model shell reference surface. All displacement components are driven at nodes that lie on the reference surface or within a “center zone,” as shown in Figure 10.2.2–9. The size of the center zone is specified as part of the submodel boundary condition definition, as described below. For nodes that lie further away from the reference surface, only the displacement components parallel to the shell reference surface are driven. At least one layer of nodes in the submodel must be within the center zone; if no nodes are found this close to the reference surface, Abaqus issues an error message. Specifying the size of the center zone in shell-to-solid submodeling The center zone method of prescribing driven variables usually provides a reasonable transfer of the plane stress assumption in the shell model. The width of this zone around the reference surface where all displacement components are driven may be different for various driven nodes or node sets. If you do not provide values for the center zone size, a default value of 10% of the maximum of the specified shell thicknesses is assumed. For complicated geometries it can be advantageous to assign a different center zone size to different nodes or node sets. You can view the driven nodes lying inside and outside the center zone in Abaqus/CAE by displaying Input File Usage: the model boundary conditions (View→ODB Display Options) in the Visualization module. *BOUNDARY, SUBMODEL, STEP=step nodes, center zone size Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region: Center zone size: center zone size Abaqus/CAE Usage: Transferring transverse shear stresses in shell-to-solid submodeling Usually it is enough for the layer of nodes closest to the shell reference surface to lie inside the center zone. If a very fine solid mesh is used in the thickness direction and substantial transverse shear stresses If this distance is small enough, all displacement components are driven. center zone shell nodes boundary nodes on solid submodel (driven nodes) For most solid nodes only tangential displacement components are driven u t tangent to shell reference surface Figure 10.2.2–9 Center zone choice in shell-to-solid submodeling. are transferred, it may be necessary to make the center zone size large enough that multiple layers of nodes lie inside the zone. However, if the transverse shear stresses at the submodel boundary are high and the submodel is highly refined in the thickness direction, high local stresses may develop since the shear force at the submodel boundary is transferred only at the driven nodes within the center zone. High transverse shear stresses occur only in regions where bending moments vary rapidly; it is better not to locate the submodel boundary in such regions. It is best to locate the submodel boundary in areas of low transverse shear stress in the global model. Special considerations There are several special considerations that are worth noting. Specifying the shell thickness in shell-to-shell submodeling For shell-to-shell submodeling the shell thickness generally is not changed between the models. You can specify different shell thicknesses if, for example, a local thickness change is being investigated; however, Abaqus does not check the validity of these differences. Limitations in shell-to-solid submodeling The following limitations and special cases apply to the shell-to-solid capability: • The global model can contain both solid and shell elements; however, when the shell-to-solid capability is used, all driven nodes must lie within shell elements in the global model. If the driven boundary lies at the border between a solid and a shell region, the driven nodes must be moved a small distance away from the solid region . • Corners or kinks may exist in global models made of shell elements. At such corners or kinks the shell elements only approximate the distribution of the material away from the midsurface of the shell . Because of such approximations, it is not possible to drive a submodel correctly if the driven nodes of the submodel lie within a shell thickness from a corner or a kink. If necessary, use the approach shown in Figure 10.2.2–11. A better approach is to include the corner or kink as part of the submodel and drive it from nodes well away from corners or kinks since they are a source of stress concentration and high stress gradients . • Temperature degrees of freedom cannot be driven in shell-to-solid submodeling. Alternative to shell-to-solid submodeling An alternative to shell-to-solid submodeling is the surface-based shell-to-solid coupling capability discussed in “Shell-to-solid coupling,” Section 34.3.3. Procedures Neither the coupled thermal-electrical procedure nor any of the mode-based dynamics procedures can be used on the submodel level. In addition, submodeling cannot be used in conjunction with symmetric model generation or symmetric results transfer. Adaptive meshes should not be used in the global model. However, they can be used in the submodel analysis; Abaqus will always treat the driven nodes in the submodel as Lagrangian nodes. Both general (possibly nonlinear) and linear perturbation steps can be used in submodeling . Submodeling in dynamic procedures The submodeling capability can be used in the dynamic procedures using explicit integration (in Abaqus/Explicit) and in the dynamic procedures using direct integration (in Abaqus/Standard). The following combinations of procedures between the global model and the submodel can be considered: explicit dynamic, implicit dynamic, dynamic coupled thermal-stress, and coupled thermal-stress. In dynamic problems in which inertial forces are significant, the global model and the submodel need to be run for the same step time intervals. In Abaqus/Explicit a quasi-static analysis is performed as a dynamic procedure. For this case and for the static analyses performed in Abaqus/Standard, the time step of the global model and submodel can be different. The time variable of the driven nodes from the global analysis must be scaled to the step time of the submodel analysis to match the time variable of the amplitude functions generated at the driven nodes to the step time used in the submodel. For significantly dynamic problems in Abaqus/Explicit, a sufficiently large number of intervals need to be written to the results or output database file for the global model. Preferably the displacement results solid elements shell elements Global model =driven node (1) (2) Two possible submodels Incorrect submodel (driven nodes in both shell and solid regions of the global model) Figure 10.2.2–10 A limitation of shell-to-solid submodeling. =driven node solid submodel overlap of material in submodel shell reference surface ε << thickness global model Figure 10.2.2–11 Shell-to-solid submodeling around corners. driven nodes away from kinks or corners Figure 10.2.2–12 Solid submodel of a shell intersection. shell reference surface for the nodes that are used to drive the submodel should be saved for each increment. This caution is necessary in particular for problems with elastic material properties to avoid possible aliasing (under sampling), which can cause solution distortion in the submodel. These requirements do not apply to quasi-static problems. Interpreting acceleration results When you drive a submodel boundary with global model displacement results, the displacements are interpreted as a smoothed piecewise linear function in time, similar to how you would apply a displacement boundary condition using a tabular amplitude definition . This smoothed function typically results in displacements and velocities at the driven nodes that agree reasonably with the global model. Acceleration results at the driven boundary, however, are generally not in good agreement with the global model as they reflect the shape of the displacement history smoothing rather than the global model acceleration results (information that is not available from a piecewise linear global-model displacement history). The submodel acceleration results away from the submodel driven nodes are less affected by this smoothing and are typically in good agreement with the global model response. Obtaining a solution at a particular point in time using linear perturbation analysis In Abaqus/Standard it is possible to study the submodel’s linearized response corresponding to a particular point in time in the global solution by using a static, linear perturbation procedure in the submodel analysis. You can select the increment in the global analysis step that is to be used as the basis for calculating the values for the driven variables. If you do not select an increment in a static linear perturbation step, the last increment of the selected step in the global analysis is used as the basis for calculating the values for the driven variables. You cannot select an increment in a general submodel step. Input File Usage: Abaqus/CAE Usage: *BOUNDARY, SUBMODEL, STEP=step, INC=increment Load module: Create Boundary Condition: choose Other for the Category and Submodel for the Types for Selected Step: select region: Global step number: step, Global increment: increment Submodeling in the frequency domain The submodeling capability can be used in the frequency domain by using the direct-solution steady-state dynamics procedure. Mode-based steady-state dynamics cannot be used at the submodel level. The only restriction on the specification of the frequency range in the submodel is that the minimum and maximum frequency should lie within the range of calculated frequencies in the global model. Abaqus will interpolate the solution variables from the global model in the frequency domain, as well as spatially, before applying them to the submodel. The results will be most accurate if the frequencies at which the response in the submodel is requested match the frequencies at which the response was calculated in the global model. This is particularly true in the vicinity of the eigenfrequencies of the global model. In the global model you must write both the amplitude and the phase of the nodal displacements to the results file so that Abaqus can apply the real and imaginary parts of the solution at the driven nodes in the submodel. If you are using the output database to drive the submodel, you need to request only nodal displacement output since displacement output to the output database includes both real and imaginary parts. Mixing general and linear perturbation steps It is possible to mix general steps and linear perturbation steps in both the global and the submodel analyses. Abaqus allows general analysis steps to be treated as linear perturbation steps during submodeling, and vice versa. Example: Submodeling with general and linear perturbation steps For an example of submodeling that uses both general and linear perturbation steps, consider the following situation. The global analysis consists of a static preload—done as a general, nonlinear, 5 seconds of modal dynamic response analysis: NODE-BASED SUBMODELING *STEP ** Apply preload *STATIC 0.1, 1.0 … ** Write out results for nodes needed to ** interpolate to the submodel's boundary *NODE FILE, NSET=DETAIL *END STEP *STEP ** Calculate modes and frequencies *FREQUENCY … ** The *NODE FILE option is repeated because ** this is the first linear perturbation step *NODE FILE, NSET=DETAIL *END STEP *STEP ** Dynamic response of preloaded system *MODAL DYNAMIC 0.01, 5.0 … *END STEP We wish to study the local, possibly nonlinear, response of a part of this model that is so small that we do not need to model dynamic effects locally and can, thus, perform two steps of static analysis: ** Define submodel boundary (driven nodes) *SUBMODEL PERIM *STEP ** Preload *STATIC 0.1, 1.0 *BOUNDARY, SUBMODEL, STEP=1 … *END STEP *STEP ** Local static response to global dynamic step *STATIC 0.01, 5.0 *BOUNDARY, SUBMODEL, STEP=3 … *END STEP It is perfectly acceptable that the submodel analysis requests general, possibly nonlinear, analysis for both steps, while in the global analysis the dynamic step was a linear perturbation step (modal dynamics is always a linear perturbation analysis). It is your responsibility to judge that this use of the submodeling feature is reasonable. For example, suppose that the global analysis were continued with a fourth step of general, nonlinear static response: *RESTART, READ, STEP=3 ** Read state at end of initial preload ** (could equally well use *RESTART, READ, STEP=1) *STEP ** Add more preload *STATIC 0.2, 1.0 … *END STEP This fourth general analysis step starts with the state at the end of general analysis Step 1 because the frequency extraction and the modal dynamic steps are both linear perturbation steps. However, if we restart the submodel analysis in the same way, the solution may not be comparable with the global model solution: *RESTART, READ, STEP=2 ** Read state at end of step 2 *STEP ** Add more preload *STATIC 0.2, 1.0 *BOUNDARY, SUBMODEL, STEP=4 … *END STEP The second step in the submodel is a general analysis step, to which the response may be nonlinear, thus changing the state of the model. A valid alternative would be to apply the Step 4 response to the submodel immediately after the first step: *RESTART, READ, STEP=1 ** Read state at end of preload step *STEP ** Add more preload *STATIC 0.2, 1.0 *BOUNDARY, SUBMODEL, STEP=4 … *END STEP Reinterpreting solution variables in the submodel analysis During general analysis steps Abaqus works in terms of total solution variables such as the displacements, , about a base . When general analysis steps and linear perturbation steps are reinterpreted in the submodel . In linear perturbation steps Abaqus works in terms of the displacement perturbation, state, analysis, the global analysis results are treated as defined in Table 10.2.2–1. Table 10.2.2–1 Reinterpreting solution variables in the submodel analysis. Driven variable basis Global increment specified in definition of submodel boundary condition none none Global analysis step basis Submodel step basis General Linear perturbation General Linear perturbation General General Static, linear perturbation Static, linear perturbation In this table is the current value of a driven variable in the submodel at any time during a general, nonlinear, analysis step; is the value of the perturbation of a driven variable in the submodel during a linear perturbation step; and are the corresponding values of the same (geometrically interpolated) variable in the global model; is the “base state” value of the variable during a linear perturbation step in the global analysis; is the “base state” value of the variable during a linear perturbation step in the submodel analysis; is the value of at increment i of the global analysis step; and is the value of at increment i of the global analysis step. Mixing general and linear perturbation steps in shell-to-solid submodeling Additional assumptions must be made for the shell-to-solid case when a general procedure on the global model drives a linear perturbation procedure on the submodel and vice versa. The assumptions depend on the geometric formulation used (linear or nonlinear) and on the procedure combination. For details and governing equations for these cases, see “Submodeling analysis,” Section 2.15.1 of the Abaqus Theory Manual. Initial conditions The definition of initial conditions should be consistent between the global model and the submodel. Boundary conditions Boundary conditions (other than submodel boundary conditions) prescribed on the degrees of freedom that are driven will replace those prescribed using submodel boundary conditions. When this replacement occurs, Abaqus reports the change in the data file. A node can be driven from the global model in some steps and have user-prescribed boundary In these cases all relevant boundary conditions must be respecified . Any other boundary conditions that are applied in the submodel region should be imposed in the submodel analysis in the usual way. It is your responsibility to apply such prescribed boundary conditions to the submodel correctly so that they correspond to the loading of the global model. Be careful with submodel boundary nodes that are also on planes of symmetry, where both forms of boundary conditions can be applied. It may be helpful in such cases to apply boundary conditions in a local coordinate system . The local coordinate system should be applied only to the boundary conditions that are intended to override the submodel boundary conditions, since the submodel boundary conditions are always output in the global coordinate directions by the global model. Loads Any loads that are applied in the submodel region must be imposed in the submodel analysis in the usual way. It is your responsibility to apply such loads to the submodel correctly so that they correspond to the loading of the global model. See “Applying loads: overview,” Section 33.4.1, for an overview of the loads available in Abaqus. Predefined fields The following predefined fields can be specified in a submodeling analysis, as described in “Predefined fields,” Section 33.6.1: • Nodal temperatures can be specified. Any difference between the applied and initial temperatures will cause thermal strain if a thermal expansion coefficient is given for the material (“Thermal expansion,” Section 26.1.2). The specified temperature also affects temperature-dependent material properties, if any. • The values of user-defined field variables can be specified. These values affect only field-variable- dependent material properties, if any. Abaqus interpolates solution variables onto the submodel driven nodes. It can also interpolate temperatures as field variables . Other predefined fields will not be interpolated to the nodes of the submodel; they must be available from the input data for all nodes of the submodel where they are required. Abaqus/Standard provides multiple approaches for cases where a submodel thermal-stress analysis must be performed using temperature solutions from a global heat transfer analysis. • Run a heat transfer analysis of the global model, and write the nodal temperatures to the results or output database file. Run a sequentially coupled thermal-stress analysis of the global model. The temperatures obtained from the results or output database file of the global heat transfer analysis are field variables in this case. If the mesh used in the thermal-stress analysis is different from the mesh in the heat transfer analysis, specify that Abaqus/Standard should interpolate the temperature field from the heat transfer analysis mesh to the thermal-stress analysis mesh. Run a thermal- stress analysis of the submodel using the results or output database file for the global thermal-stress analysis to read the driven variables (displacement field) and using the results or output database file from either the global heat transfer analysis or the global thermal-stress analysis to read the temperatures as field variables. In either case the temperature field will have to be interpolated to the current submodel nodes. If interpolation between dissimilar meshes is necessary, the global output database file must be used to read the temperatures. For details, see Figure 10.2.2–13 and Figure 10.2.2–14. Global model (mesh1) Heat transfer analysis Field variables Global.odb Interpolate from mesh1 to mesh 3 Field variables Global.odb Interpolate from mesh1 to mesh4 Global model (mesh3) Static analysis Read temperatures from Global.odb Driven variables Global_u.fil or Global_u.odb Submodel (mesh4) Static analysis Read temperatures from Global.odb Figure 10.2.2–13 Sequentially coupled thermal-stress analysis for the global model with only a thermal-stress analysis for the submodel. • Run a heat transfer analysis of the global model, and write the nodal temperatures to the results or output database file. Run a sequentially coupled thermal-stress analysis (the global thermal-stress Global model (mesh1) Heat transfer analysis Field variable Global_1.odb Interpolate from mesh1 to mesh2 Global model (mesh2) Static analysis Read temperatures from Global_1.odb Driven variable Global_2.fil or Global_2.odb Field variable Global_2.odb Interpolate from mesh2 to mesh3 Submodel (mesh3) Static analysis Read temperatures from Global_2.odb Figure 10.2.2–14 Sequentially coupled thermal-stress analysis for the global model with only a thermal-stress analysis for the submodel. analysis) using the same mesh (mesh1) as the global heat transfer analysis and the temperatures from the results or output database file for the global heat transfer analysis. Next, run a submodel heat transfer analysis using the mesh (mesh2) that is required for the final submodel thermal-stress analysis, and write the nodal temperatures to the results or output database file. Use the temperature solution from the global heat transfer analysis to drive the solution of the submodel heat transfer analysis. Finally, run the submodel thermal-stress analysis using the temperatures (as field variables) obtained from the results or output database file for the submodel heat transfer analysis and the displacements (as driven variables) obtained from the global thermal-stress analysis. See the detailed flow chart in Figure 10.2.2–15. Material options Any of the material models described in Part V, “Materials,” can be used in the global and submodel analyses. The material response defined for the submodel may be different from that defined for the global model. Elements The dimensionality of the submodel must be the same as that of the global model: both models must be either two-dimensional or three-dimensional. The following limitations apply: Submodel (mesh2) Submodel Heat transfer analysis Field variables Submodel_heat.fil or Submodel_heat.odb Global model (mesh1) Heat transfer analysis Driven variables Global.fil Global.odb Field variables Global.fil or Global.odb Global model (mesh1) Static analysis Read temperatures from Global.fil or Global.odb Driven variables Global_u.fil Global_u.odb Submodel (mesh2) Static analysis Read temperatures from Submodel_heat.fil or Submodel_heat.odb Figure 10.2.2–15 Sequentially coupled thermal-stress analysis for both the global model and submodel. • The boundary nodes of the submodel must lie within regions of the global model where Abaqus is able to perform spatial interpolation to define the values of the driven variables. Therefore, they must lie within (or, as allowed by the exterior tolerance, near to) two- or three-dimensional geometrically defined elements in the global model. Such geometrically defined elements are: – first- or second-order triangles or quadrilaterals in two dimensions; – first- or second-order triangular or quadrilateral shells; and – first- or second-order tetrahedra, wedges, or bricks in three dimensions. • When shell elements with five degrees of freedom per node (S4R5, S8R5, STRI65, etc.) are used in the global model, the rotations are not written to the results file or the output database; therefore, only the displacement degrees of freedom can be driven. This restriction suggests that submodeling should not be used with these elements or that the submodel should include a set of narrow elements around its driven edges so that the interpolated displacements at these nodes effectively transfer the rotation. Five degree of freedom shells cannot be used in shell-to-solid submodeling. • The boundary nodes cannot lie in regions of the global model where there are only one-dimensional elements (beams, trusses, links, axisymmetric shells) since Abaqus does not provide the necessary interpolation of results for such elements. • The boundary nodes cannot lie in regions of the global model where there are only user elements, substructures, springs, dashpots, etc. since those element types do not allow for geometric interpolation. • The boundary nodes cannot lie in regions of the global model where there are only axisymmetric solid elements with nonlinear, asymmetric deformation (CAXA elements). The submodeling capability is currently not supported for these elements. • The reference node associated with generalized plane strain elements (CPEG) cannot be used as a driven boundary node in a submodeling analysis. Output Any of the output normally available within a particular procedure is also available during a submodeling analysis . As described above, nodal output requests to the results file or output database file must be used in the global analysis to save the values of the driven variables at the submodel boundary. Input file template Global analysis: *HEADING … *STEP Step 1 *STATIC (or *DYNAMIC, etc.) Data line to define step time and control incrementation … *NODE FILE List of solution variables to be used to drive the submodel *OUTPUT, FIELD *NODE OUTPUT List of solution variables to be used to drive the submodel *END STEP Submodel analysis: *HEADING … *SUBMODEL, EXTERIOR TOLERANCE=tolerance List of all nodes to be driven ** *STEP *STATIC (or any other allowable procedure) Data line to define step time (must be the same as the step time in the global analysis unless the TIMESCALE parameter is used on the *BOUNDARY option) and control incrementation … *BOUNDARY, SUBMODEL, STEP=1 Data lines listing nodes and degrees of freedom to be driven in this step … *END STEP 10.2.3 SURFACE-BASED SUBMODELING Products: Abaqus/Standard References • “Submodeling: overview,” Section 10.2.1 • *SUBMODEL • *DSLOAD • Chapter 38, “Submodeling,” of the Abaqus/CAE User’s Manual Overview The surface-based submodeling technique: • may not provide the same level of accuracy as node-based submodeling; • should be used only when the node-based technique cannot provide adequate results; • is limited to stress-based solid-to-solid submodeling for general static procedures in Abaqus/Standard; • applies surface tractions to submodel surfaces based on a stress field interpolated from the global model; and • can be combined with node-based submodeling of displacements . Performing a surface-based submodeling analysis Your submodel analysis is driven, either partly or completely, from the results obtained from a global model analysis. The results from the global model are interpolated onto the surfaces on the appropriate parts of the boundary of the submodel. Thus, the response at the boundary of the local region is defined by the solution for the global model. The driven surfaces and any loads applied to the local region determine the solution in the submodel. Surface-based submodeling should be used only when the node-based technique cannot provide adequate results. For a comparison of the two submodeling techniques and recommendations for their application, refer to “Submodeling: overview,” Section 10.2.1. Saving the results from the global model The results from the global analysis must be saved at all elements required for the interpolation of the driven variables to the boundary surface of the submodel. Only the output database can be used for this purpose. In each step of the global model whose solution will be used to drive the submodel, write the stress results to the output database . Input File Usage: Use both of the following options: Abaqus/CAE Usage: *OUTPUT, FIELD *ELEMENT OUTPUT Step module: Output→Field Output Requests→Create Referring to the global model results from the submodel analysis You must define the source of the global solution results and provide the name of the output database file; the file extension is optional. If the file extension is omitted, Abaqus will correctly choose the extension if the output database file exists. Input File Usage: abaqus job=submodel_input_file globalmodel= global_output_database Abaqus/CAE Usage: Any module: Model→Edit Attributes→submodel: Submodel: Read data from job: global_output_database Specifying the driven surfaces in the submodel Specifying the driven element-based surfaces does not activate the driven surface loads: they must be activated by specifying the appropriate submodel distributed surface loads. All surface facets of the submodel to be driven by stresses in any step must be specified as driven surfaces since the list of surfaces cannot be extended subsequent to its initial definition (even at restart). However, variables at the surfaces given do not have to be driven in all steps: the choice of which surfaces are driven in a particular step is made as part of a submodel distributed surface load definition, as discussed in “Defining the driven surface tractions in the submodel,” later in this section. boundary surface of the submodel driven by the global model solution Figure 10.2.3–1 The magnified submodel. Input File Usage: *SUBMODEL list of element-based structural surfaces The *SUBMODEL option must be included in the model definition portion of the input file for the submodel analysis. Multiple *SUBMODEL options are allowed; however, in this case you must ensure that the driven surfaces specified on the data line of one option are separate and distinct from the other surfaces specified on the data lines of all the other options. Abaqus/CAE Usage: Load module: Create Load: choose Other for the Category and Submodel for the Types for Selected Step: Driving region: select region Defining geometric tolerances A geometric tolerance is used to define how far driven element-based surface nodes in the submodel can lie outside the exterior surface of the global model, as that surface is interpolated in the global, undeformed finite element model. By default, surface nodes in the submodel must lie within a distance calculated by multiplying the average element size in the global model by 0.05. You can change the tolerance, which is useful in cases where submodel driven surfaces lie to a greater extent outside the global model exterior surface. Tolerances larger than this default value, however, can result in significantly greater computation times and lower accuracy in the driven solution for driven surface regions significantly outside the global model exterior surface. You can define the geometric tolerance as a fraction of the size of the average element in the global model or as an absolute distance in the length units chosen for the model. If both tolerances are defined, Abaqus uses the tighter tolerance. Input File Usage: Use the following option to define the geometric tolerance as an absolute distance: *SUBMODEL, TYPE=SURFACE, ABSOLUTE EXTERIOR TOLERANCE=tolerance Use the following option to define the geometric tolerance as a fraction of the size of the average element in the global model: *SUBMODEL, TYPE=SURFACE, EXTERIOR TOLERANCE=tolerance Load module: Create Load choose Other for the Category and Submodel for the Types for Selected Step: select region: Exterior tolerance: absolute: or relative: tolerance Abaqus/CAE Usage: The exterior tolerance in solid-to-solid submodeling The exterior tolerance for a solid-to-solid submodel analysis is indicated by the shaded region in Figure 10.2.3–2. If the distance between the driven surface nodes and the free surface of the global model falls within the specified tolerance, the solution variables from the global model are extrapolated to the submodel. exterior surface in global model driven surface in submodel nodes in global model nodes in submodel actual geometric surface Figure 10.2.3–2 The exterior tolerance in surface-based submodeling. Defining the driven surface tractions in the submodel The actual driven surface tractions are defined in any step as submodel distributed surface loads. The stresses resulting in these tractions are “driven variables” obtained from the output database file of the global analysis. All stress components from the global model elements that will drive the submodel boundary surface must have been written to the output database. They will be used to create traction, shear, and normal stresses at integration points of driven surfaces (as non-uniform distributed surface loads). All applicable stress components are calculated and applied to the surface integration points at each time increment. Input File Usage: Abaqus/CAE Usage: *DSLOAD, SUBMODEL Load module: Create load: choose Other for the Category and Submodel for the Types for Selected Step Specifying the step number from the global analysis You specify the step of the global model history that is to be used for the driven variables in the current submodel analysis step. Input File Usage: Abaqus/CAE Usage: *DSLOAD, SUBMODEL, STEP=step Load module: Create load: choose Other for the Category and Submodel for the Types for Selected Step: select region: Global step number: step Modifying the set of driven surface tractions You can modify the submodel distributed surface load definitions from step to step to change the global step reference, you can remove surface load definitions, and you can reintroduce them later . New surfaces cannot be added to the total set of driven surface defined for the submodel; this set of driven surfaces is a fixed part of the model definition. Input File Usage: Use one of the following options: *DSLOAD, SUBMODEL, OP=MOD *DSLOAD, SUBMODEL, OP=NEW Guidelines for obtaining adequate solution accuracy Unlike node-based submodeling, surface-based submodeling can in many cases provide incorrect or misleading submodel results. This risk follows from the methods used to interpolate stresses from the global model to the submodel: • The global model material point stresses are smoothed and associated with the global model nodes. • These global model node-located stresses are then interpolated to the submodel surface integration points and applied as tractions. This process is generally nonconservative, resulting in a submodel traction field that is not equivalent to the global model stress field in an equilibrium sense. Modeling guidelines You can improve accuracy and achieve reasonable submodel solutions by observing the following guidelines: • Design your models so that your submodel surface intersects the global model in regions of relatively low stress gradients. • Design your models so that your submodel surface intersects the global model in regions of uniform element size. A warning message is provided in the data (.dat) file in cases where significant nonuniform element size distributions are seen. Checking your results To understand whether your modeling approach results in a reasonably accurate solution, the following guidelines are recommended: • Compare the stress distributions on the submodel-driven surfaces with the stress distributions in the global model. You can view the stress distributions in the global model by using tools such as cutting planes and path plots in the Visualization module of Abaqus/CAE. The degree to which the global model’s stress distributions agree with those in the submodel-driven surface is generally an indication of the level of accuracy of your submodel solution. • When using inertia relief in the submodel for cases where submodeling does not remove all rigid body modes, compare the inertia relief forces to the prevailing force level in your submodel. If the inertia relief force is large compared to the prevailing force level, your submodel results may be inaccurate. Special considerations There are several special considerations that are worth noting. Handling of rigid-body modes When you use surface-based submodeling exclusively to drive your submodel response, your displacement solution will not be unique; you will generally encounter rigid-body modes and accompanying numerical issues. You can address these rigid-body modes by • providing sufficient node-based submodel displacement boundary condition definitions in the submodel analysis, • providing sufficient boundary condition definitions in the submodel analysis, or • providing an inertia relief load definition in the submodel analysis . You can combine these definitions, as necessary and appropriate to your model, to address all rigid body modes. Cases of finite rotation Global model stress results are stored in the output database in the global coordinate system. Submodel tractions are calculated from these stresses and the current configuration surface normal in the submodel. Hence, when your global model result involves significant finite rotation, your submodel results will generally be inaccurate unless you provide sufficient node-based submodel displacement boundary condition definitions to impart similar rigid-body rotations to the submodel; exclusive use of surface-based submodeling definitions is not adequate to provide these rigid-body motions. You may also experience convergence difficulties in the submodel when it is not properly rotated. Inelastic behavior When surface-based submodeling is used to drive a submodel region with an inelastic material definition, you may encounter rigid-body modes and accompanying numerical issues. For example, numerical issues will prevent convergence if the submodel material definition includes plasticity and the submodel loading results in a shear band formation beyond the material hardening definition, such that unconstrained motion can occur (i.e., if the submodel loads exceed the limit load capacity). In these cases node-based submodeling should be used. Procedures Only the static procedure is allowed. Both general (possibly nonlinear) and linear perturbation steps can be used in submodeling . Obtaining a solution at a particular point in time using linear perturbation analysis In Abaqus/Standard it is possible to study the submodel’s linearized response corresponding to a particular point in time in the global solution by using a static, linear perturbation procedure in the submodel analysis. You can select the increment in the global analysis step that is to be used as the basis for calculating the values for the driven variables. If you do not select an increment in a static linear perturbation step, the last increment of the selected step in the global analysis is used as the basis for calculating the values for the driven variables. You cannot select an increment in a general submodel step. Input File Usage: Abaqus/CAE Usage: *DSLOAD, SUBMODEL, STEP=step, INC=increment Selection of a specific global model increment is not supported in Abaqus/CAE. Mixing general and linear perturbation steps It is possible to mix general steps and linear perturbation steps in both the global and the submodel analyses. Abaqus allows general analysis steps to be treated as linear perturbation steps during submodeling, and vice versa. Example: Submodeling with general and linear perturbation steps For an example of submodeling that uses both general and linear perturbation steps, consider the following situation. The global analysis consists of a static preload—done as a general, nonlinear, analysis step—followed by extraction of the eigenmodes of the preloaded structure, then a step of 5 seconds of modal dynamic response analysis: *STEP ** Apply preload *STATIC 0.1, 1.0 … ** Write out stress results for elements needed to ** interpolate to the submodel's surfaces *ELEMENT OUTPUT, ELSET=DETAIL *END STEP *STEP ** Calculate modes and frequencies *FREQUENCY … ** The *ELEMENT OUTPUT option is repeated because ** this is the first linear perturbation step *ELEMENT OUTPUT, ELSET=DETAIL *END STEP *STEP ** Dynamic response of preloaded system *MODAL DYNAMIC 0.01, 5.0 … *END STEP We wish to study the local, possibly nonlinear, response of a part of this model that is so small that we do not need to model dynamic effects locally and can, thus, perform two steps of static analysis: ** Define submodel surfaces (driven surfaces) *SUBMODEL,TYPE=SURFACE PERIM *STEP ** Preload *STATIC 0.1, 1.0 *DSLOAD, SUBMODEL, STEP=1 … *END STEP *STEP ** Local static response to global dynamic step *STATIC 0.01, 5.0 *DSLOAD, SUBMODEL, STEP=3 … *END STEP It is perfectly acceptable that the submodel analysis requests general, possibly nonlinear, analysis for both steps, while in the global analysis the dynamic step was a linear perturbation step (modal dynamics is always a linear perturbation analysis). It is your responsibility to judge that this use of the submodeling feature is reasonable. For example, suppose that the global analysis were continued with a fourth step of general, nonlinear static response: *RESTART, READ, STEP=3 ** Read state at end of initial preload ** (could equally well use *RESTART, READ, STEP=1) *STEP ** Add more preload *STATIC 0.2, 1.0 … *END STEP This fourth general analysis step starts with the state at the end of general analysis Step 1 because the frequency extraction and the modal dynamic steps are both linear perturbation steps. However, if we restart the submodel analysis in the same way, the solution may not be comparable with the global model solution: *RESTART, READ, STEP=2 ** Read state at end of step 2 *STEP ** Add more preload *STATIC 0.2, 1.0 *DSLOAD, SUBMODEL, STEP=4 … *END STEP The second step in the submodel is a general analysis step, to which the response may be nonlinear, thus changing the state of the model. A valid alternative would be to apply the Step 4 response to the submodel immediately after the first step: *RESTART, READ, STEP=1 ** Read state at end of preload step *STEP ** Add more preload *STATIC 0.2, 1.0 *DSLOAD, SUBMODEL, STEP=4 … *END STEP Loads Any loads that are applied in the submodel region of the global analysis must be imposed in the submodel analysis in the usual way. It is your responsibility to apply such loads to the submodel correctly so that they correspond to the loading of the global model. See “Applying loads: overview,” Section 33.4.1, for an overview of the loads available in Abaqus. Output Any of the output normally available within a particular procedure is also available during a submodeling analysis . As described above, element stress output requests to the output database file must be used in the global analysis to save the values of the driven variables at the submodel boundary. Input file template Global analysis: *HEADING … *STEP Step 1 *STATIC (or *STATIC, etc.) Data line to define step time and control incrementation … *ELEMENT OUTPUT *OUTPUT, FIELD *ELEMENT OUTPUT *END STEP Submodel analysis: *HEADING … *SUBMODEL,TYPE=SURFACE, EXTERIOR TOLERANCE=tolerance List of all surfaces to be driven ** *STEP *STATIC (or any other allowable procedure) Data line to define step time and control incrementation. …*DSLOAD, SUBMODEL, STEP=1 Data lines listing surfaces to be driven in this step … *END STEP 10.3 Generating global matrices • “Generating matrices,” Section 10.3.1 10.3.1 GENERATING MATRICES Product: Abaqus/Standard References • “Defining matrices,” Section 2.11.1 • “Defining an analysis,” Section 6.1.2 • *MATRIX GENERATE • *MATRIX OUTPUT • *MATRIX INPUT • *CLOAD Overview Matrix generation: • is a linear perturbation procedure; • allows for the mathematical abstraction of model data such as mesh and material information by generating global or element matrices representing the stiffness, mass, viscous damping, structural damping, and load vectors in a model; • generally creates matrices identical to those used in a subspace-based steady-state dynamic procedure . • includes initial stress and load stiffness effects due to preloads and initial conditions if nonlinear geometric effects are included in the analysis; • writes matrix data to a binary .sim file that can be read as input by Abaqus; and • can output matrix data to text files that can be read as input in other analyses by Abaqus or other simulation software. Generating global matrices A linearized finite element model can be summarized in terms of matrices representing the stiffness, mass, damping, and loads in the model. Using these matrices, you can exchange model data between other users, vendors, or software packages without exchanging mesh or material data. Matrix representations of a model prevent the transfer of proprietary information and minimize the need for data manipulation. The matrix generation procedure is a linear perturbation step that accounts for all current boundary conditions, loads, and material response in a model. You can also specify new boundary conditions, loads, and predefined fields within the matrix generation step. The generated matrices are input to a matrix usage model. The matrix generation procedure uses SIM, which is a high-performance database available in Abaqus. The generated matrices are stored in a file named jobname_Xn.sim, where jobname is the name of the input file or analysis job and n is the number of the Abaqus step that generates the matrices. Specifying the matrix type You can generate matrices representing the following model features: • stiffness, • mass, • viscous damping, • structural damping, and • loads. The load matrix contains integrated nodal load vectors (right-hand sides) for the load cases defined in the matrix generation step. Load cases can be made up of any combination of loadings—distributed loads, concentrated nodal loads, thermal expansion, and load cases defined for any substructures that may be used as part of the model. Input File Usage: Use the following option to generate the stiffness matrix: *MATRIX GENERATE, STIFFNESS Use the following option to generate the mass matrix: *MATRIX GENERATE, MASS Use the following option to generate the viscous damping matrix: *MATRIX GENERATE, VISCOUS DAMPING Use the following option to generate the structural damping matrix: *MATRIX GENERATE, STRUCTURAL DAMPING Use the following option to generate the load matrix: *MATRIX GENERATE, LOAD Generating element matrices By default, the matrix generation procedure generates global matrices for a model in assembled form. The generated global matrices are assembled from the local element matrices and include contributions from matrix input data. Abaqus/Standard offers an option to generate global matrices in element-by- element form. Instead of global (assembled) matrices, local element matrices are generated. If you choose to generate local element matrices for a model containing matrix input data, Abaqus/Standard calculates and stores only element matrices; the matrix input data are ignored. Input File Usage: *MATRIX GENERATE, ELEMENT BY ELEMENT Generating matrices for a part of the model By default, the matrix generation procedure generates matrices for a whole model. Abaqus/Standard can generate matrices for a part of the model defined by an element set. Input File Usage: *MATRIX GENERATE, ELSET=element set name Evaluating frequency-dependent material properties When frequency-dependent material properties are specified in the model definition, Abaqus/Standard offers the option of choosing the frequency at which these properties are evaluated for use in global matrix generation. If you do not choose the frequency, Abaqus/Standard evaluates the matrices at zero frequency and does not consider the contributions from frequency-domain viscoelasticity. Input File Usage: *MATRIX GENERATE, PROPERTY EVALUATION=frequency Specifying public nodes An Abaqus/Standard model may contain user-defined nodes and internal nodes. Internal nodes are nodes with internal degrees of freedom associated with them (for example, Lagrange multipliers and generalized displacements) that are created internally by Abaqus/Standard. You can use the matrix generation procedure to specify some of the user-defined nodes as “public nodes.” These nodes will be visible in the matrix usage model. The remaining user-defined nodes in the matrix data are designated as internal nodes and are effectively hidden in the matrix usage model . By default, all user-defined nodes in the matrix data are public nodes. By specifying public nodes, you can reduce the number of user-defined nodes in the matrix usage analysis, which simplifies the remapping process . For example, you may want to identify the nodes for attaching a subcomponent (matrix) to the matrix usage model or the nodes for the output of results as public nodes. Input File Usage: *MATRIX GENERATE, PUBLIC NODES=node set name Initial conditions Matrix generation is a linear perturbation procedure. Therefore, the initial state for the matrix generation step is the state of the model at the end of the last general analysis step. The generated matrix includes initial stress and load stiffness effects due to preloads and initial conditions if nonlinear geometric effects are included in the analysis. Boundary conditions Boundary conditions can be defined or modified in a matrix generation step. For more information on defining boundary conditions, see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Any boundary conditions that are defined in a matrix generation step will not be used in subsequent general analysis steps (unless they are respecified). Loads All types of loads can be applied in the load cases for a matrix generation step. Real and imaginary parts of the load vectors will be generated for the complex loads. For more information on applying loads, see “Applying loads: overview,” Section 33.4.1. Any loads that are defined in a matrix generation step will not be used in subsequent general analysis steps (unless they are respecified). Predefined fields All types of predefined fields can be specified in a matrix generation procedure. For more information on specifying predefined fields, see “Predefined fields,” Section 33.6.1. Any predefined fields that are defined in a matrix generation step will not be used in subsequent general analysis steps (unless they are respecified). Material options All types of materials that are available in Abaqus/Standard can be used in a matrix generation procedure. Elements All types of elements that are available in Abaqus/Standard can be used in the matrix generation procedure. Generating matrices for models containing solid continuum infinite elements Solid continuum infinite elements (CIN-type elements) have different formulations in static and dynamic analyses. Therefore, when generating matrices for a model containing solid continuum infinite elements, you must specify whether to use the static or dynamic formulation. Input File Usage: Use the following option to select the static formulation for solid infinite elements: *MATRIX GENERATE, SOLID INFINITE FORMULATION=STATIC Use the following option to select the dynamic formulation for solid infinite elements: *MATRIX GENERATE, SOLID INFINITE FORMULATION=DYNAMIC Output In a matrix generation analysis, you can output the stiffness, mass, viscous damping, structural damping, and load matrices to text files. Several formats are available for the matrix output, as discussed below. Matrices are copied from the .sim file and output in text files that use the following naming convention: jobname_matrixN.mtx where jobname is the name of the input file or analysis job, matrix is a four-letter identifier indicating the matrix type (as outlined in Table 10.3.1–1), and N is the number associated with the Abaqus analysis step generating the matrices. Table 10.3.1–1 Identifiers used in the generated matrix file name. Identifier Matrix Type STIF MASS DMPV DMPS LOAD Stiffness matrix Mass matrix Viscous damping matrix Structural damping matrix Load matrix For example, if a stiffness matrix generation is performed in the third step of an analysis job named VehicleFrame, the matrix is output to a file named VehicleFrame_STIF3.mtx. Input File Usage: Use the following option to output the stiffness matrix: *MATRIX OUTPUT, STIFFNESS Use the following option to output the mass matrix: *MATRIX OUTPUT, MASS Use the following option to output the viscous damping matrix: *MATRIX OUTPUT, VISCOUS DAMPING Use the following option to output the structural damping matrix: *MATRIX OUTPUT, STRUCTURAL DAMPING Use the following option to output the load matrix: *MATRIX OUTPUT, LOAD Matrix input text format This default text format creates matrix files consistent with the format used by the matrix definition technique in Abaqus/Standard . This format does not convert any of the internal Abaqus node labels. A negative number or zero can be used as a label for an internal node. Input File Usage: *MATRIX OUTPUT, FORMAT=MATRIX INPUT Format of the operator matrix The assembled sparse matrix operator data are written to the text file as a series of comma-separated lists. Each row in the file represents a single matrix entry; a row is written as a comma-separated list with the following elements: 1. Row node label 2. Degree of freedom for row node 3. Column node label 4. Degree of freedom for column node 5. Matrix entry Format of the load matrix Nonzero entries in load matrices, which represent right-hand-side vector data, are written to the text file as a comma-separated list with the following elements: 1. Node label 2. Degree of freedom 3. Right-hand-side vector entry The format of the load vectors and heading labels is based on the Abaqus keyword interface, which allows the generated loads to be easily applied in other Abaqus analyses. Each load vector uses the following headings to indicate the real and imaginary portions of the load: *CLOAD, REAL *CLOAD, IMAGINARY If the matrix generation step has multiple load cases, the load matrices for each load case are wrapped by the following labels in the generated text file: *LOAD CASE … *END LOAD CASE Including generated matrix data and generated loads in another Abaqus model The generated sparse matrix data and generated loads that are output in matrix input text format can be included in another Abaqus model. Input File Usage: Use the following options: *MATRIX INPUT *INCLUDE, INPUT=matrix or load file Labeling text format You can generate text files in which the matrix is formatted according to the standard labeling format. Internal Abaqus node labels are converted into large positive numbers that are acceptable for Abaqus matrix input data. This is the only difference between the labeling text format and the default matrix input text format. All nodes of the matrix generated in the labeling text format are treated as user-defined nodes if the matrix is used in an Abaqus/Standard analysis. Input File Usage: *MATRIX OUTPUT, FORMAT=LABELS Coordinate text format You can generate text files in which the matrix is formatted according to the common mathematical coordinate format. This format is commonly used in mathematics programs such as MATLAB. separated list with the following elements: GENERATING MATRICES 1. Row number 2. Column number 3. Matrix entry For load matrices, which represent right-hand-side vector data, each row in the text file is written with the following elements: 1. Equation (row) number 2. Right-hand-side vector entry Commented load case options are written to the output file to indicate the load cases. Input File Usage: *MATRIX OUTPUT, FORMAT=COORDINATE Outputting matrices in element-by-element form If matrices are generated in element-by-element form, you can write them in element-by-element form. When you generate text files using the matrix input or labeling format, each row in the file represents a single matrix entry; a row is written as a comma-separated list with the following elements: 1. Element label 2. Row node label 3. Degree of freedom for row node 4. Column node label 5. Degree of freedom for column node 6. Matrix entry For load matrices, which represent right-hand-side vector data, each row in the text file is written with the following elements: 1. Element label 2. Node label 3. Degree of freedom 4. Right-hand-side vector entry Coordinate format is also available for element-by-element global matrix generation. Each row in a coordinate-formatted file corresponds to a matrix entry; a row is written as a comma-separated list with the following elements: 1. Element number 2. Row number 3. Column number 4. Matrix entry For load matrices each row in the text file is written with the following elements: 1. Element number 2. Equation (row) number 3. Right-hand-side vector entry Input file template *HEADING … ** *STEP Options to define the preloading history for the model. *END STEP ** *STEP *MATRIX GENERATE, STIFFNESS, MASS, VISCOUS DAMPING, STRUCTURAL DAMPING, LOAD *MATRIX OUTPUT, STIFFNESS, MASS, VISCOUS DAMPING, STRUCTURAL DAMPING, LOAD, FORMAT=MATRIX INPUT *BOUNDARY Options to define the boundary conditions for the matrix generation step. ** *LOAD CASE, NAME=LC1 Options to define the loading for the first load case. *END LOAD CASE ** *LOAD CASE, NAME=LC2 Options to define the loading for the second load case. *END LOAD CASE Any number of load cases can be defined. *END STEP OF CYCLIC SYMMETRY MODELS 10.4 Symmetric model generation, results transfer, and analysis of cyclic symmetry models • “Symmetric model generation,” Section 10.4.1 • “Transferring results from a symmetric mesh or a partial three-dimensional mesh to a full three- dimensional mesh,” Section 10.4.2 • “Analysis of models that exhibit cyclic symmetry,” Section 10.4.3 10.4.1 SYMMETRIC MODEL GENERATION Product: Abaqus/Standard Reference • *SYMMETRIC MODEL GENERATION Overview A three-dimensional model can be created in Abaqus/Standard by: • revolving an axisymmetric model about its axis of revolution; • revolving a single three-dimensional sector about its axis of symmetry; or • combining two parts of a symmetric three-dimensional model, where one of the parts is the original model and the other part is obtained by reflecting the original model through either a symmetry line or a symmetry plane. Abaqus/Standard also provides for the transfer of the solution obtained in the original analysis onto the new model . Only stress/displacement, heat transfer, coupled temperature-displacement, and acoustic elements can be used to generate a new model. Model generation The symmetric model generation capability can be used to create a three-dimensional model by revolving an axisymmetric model about its axis of revolution, by revolving a single three-dimensional sector about its axis of symmetry, or by combining two parts of a symmetric model, where one part is the original model and the other part is the original model reflected through a line or a plane. The original model must have been saved to a restart file. The symmetric model generation capability is not available for models defined in terms of an assembly of part instances. Therefore, an element set name or a node set name containing quotation marks is not supported. An entire three-dimensional model—including nodes, elements, section definitions, material and orientation definitions, rebar, and contact pair definitions—is generated from the original model. Symmetric model generation from a model with general contact is not allowed. You must redefine most types of kinematic constraints (“Kinematic constraints: overview,” Section 34.1.1). However, surface-based constraints (“Mesh tie constraints,” Section 34.3.1) and embedded element constraints (“Embedded elements,” Section 34.4.1) defined in the original model will be generated automatically in the new three-dimensional model. Changes made to the model as part of the history data—element or contact pair removal/reactivation (“Element and contact pair removal and reactivation,” Section 11.2.1) or changes to friction properties (“Changing friction properties during an Abaqus/Standard analysis” in “Frictional behavior,” Section 36.1.5)—will not be transferred to the new model. Such changes will have to be redefined in the history data of the new model. All element and node sets defined in the original model will be used in the new model. These sets will contain all of the new elements and nodes that originated from the original sets. Additional nodes, elements, contact surfaces, etc. can also be defined to create parts of the model that were not specified in the original model. You must ensure that the numbering of these nodes and elements does not conflict with those used by the symmetric model generation capability. You can control the node and element numbering in the new model (as described below for each type of revolved model) so that you can define additional parts of the model without the risk of conflicting element and node labels. The smallest node/element number used in defining additional parts of the new model should be greater than the largest node/element number generated by the symmetric model generation capability. Eliminating duplicate nodes Duplicate nodes will be generated in certain situations. Such nodes can be eliminated to ensure that the mesh is connected properly. Duplicate nodes can be generated on the axis of revolution of a revolved model, on the connection planes between sectors of a periodic model, and on the connection plane between the two parts of a reflected model. You can specify the tolerance distance, d, to be used in the search for duplicate nodes. The default distance is 1.0% of the average element dimension. In some cases a tolerance distance that is smaller than the default value needs to be specified if, for example, the distance between two nodes on one of the connection planes in the original sector of a periodic model is smaller than the default tolerance distance. Closely spaced nodes elsewhere in the model, such as between interface surfaces or on parts of the model that are generated with any of the other model definition options, will not be eliminated. Input File Usage: Use one of the following options to specify the tolerance to be used in the search for duplicate nodes: *SYMMETRIC MODEL GENERATION, PERIODIC, TOLERANCE=d *SYMMETRIC MODEL GENERATION, REVOLVE, TOLERANCE=d *SYMMETRIC MODEL GENERATION, REFLECT, TOLERANCE=d Writing the new model definition to an external file You can specify the name of an external file (without an extension) to which the data for the new model definition will be written. The extension .axi will be added to the file name provided. The file can be edited to modify or to extend the model generated by Abaqus/Standard. Input File Usage: Use one of the following options: *SYMMETRIC MODEL GENERATION, PERIODIC, FILE NAME=name *SYMMETRIC MODEL GENERATION, REVOLVE, FILE NAME=name *SYMMETRIC MODEL GENERATION, REFLECT, FILE NAME=name Identifying the restart files The symmetric model generation capability uses the restart (.res), analysis database (.stt and .mdl), and part (.prt) files from the old model to generate the new model. The name of the restart files from the old model must be specified when the new analysis is executed by using the oldjob parameter in the command for running Abaqus or by answering a request made by the command procedure . Verifying the new model It is recommended that you verify the new model carefully before an analysis is performed. The symmetric model generation capability requires only information stored in the restart file during a data check run to generate the new model, which allows you to verify the new model before the analysis of the original model is performed. A data check analysis is performed by using the datacheck parameter in the command for running Abaqus . Revolving an axisymmetric cross-section You can create a three-dimensional model by revolving the cross-section of a two-dimensional axisymmetric model about a symmetry axis starting at a prescribed reference plane, . Both the symmetry axis and reference plane of the new three-dimensional model can be oriented in any direction with respect to the global coordinate system . A nonuniform discretization in the circumferential direction can be specified. reference cross-section at θ = 0 Figure 10.4.1–1 Revolving an axisymmetric cross-section. Specify the coordinates of points a, b, and c shown in Figure 10.4.1–1, followed by a list that defines the discretization in the circumferential direction containing the segment angle, number of elements per segment, and the bias ratio of the segment. Several segment angles, each with a different number of element subdivisions and a different bias ratio, can be used to define the complete discretization around the circumference of the revolved model. The endpoint of a cross-section revolved through 360.0° will always be connected to the origin of revolution, , regardless of the value specified for the duplicate node tolerance. Input File Usage: *SYMMETRIC MODEL GENERATION, REVOLVE Local orientation system A local cylindrical orientation system is always used for element output of stress, strain, etc. A default local orientation definition is provided if the material in the original axisymmetric model does not contain an orientation definition. This default orientation is defined with the polar axis of the system along the axis of revolution, with an additional 90.0° rotation about the local 1-direction so that the local axes are 1=radial, 2=axial, and 3=circumferential. If shells or membranes are used, the projections of the local 2- and 3-axes onto the surface of the shell or membrane are taken as the local directions on the surface. This orientation system is always provided, even if an orientation is specified in the original axisymmetric model. However, if the results of the axisymmetric analysis are mapped onto the new three-dimensional model and an orientation definition is associated with the material in the original model, the original orientation revolved about the axis of symmetry replaces this default orientation definition. Controlling the new node and element numbering You can define the increments in numbers between each node and element around the circumference of the three-dimensional model. The numbering starts at the reference cross-section . The reference cross-section uses the same numbering as the original axisymmetric model. The defaults are the largest node and element numbers used in the original axisymmetric model. Control over the numbering allows you to define additional parts of the model without the risk of conflicting element and node labels. Each offset value should be greater than or equal to the maximum node or element label, respectively, used in the original model. When specifying the offset value, care must be taken that the generated node or element does not exceed the maximum value allowed, which is 999,999,999. Input File Usage: *SYMMETRIC MODEL GENERATION, REVOLVE, NODE OFFSET=offset, ELEMENT OFFSET=offset Correspondence between axisymmetric and three-dimensional elements The element type used in the original two-dimensional model determines the element type in the new three-dimensional model. You can specify whether the new element should be either a general three- dimensional element or a cylindrical element. General and cylindrical elements can be used in the same model. Input File Usage: *SYMMETRIC MODEL GENERATION, REVOLVE coordinates of points a and b coordinates of point c segment angle, number of elements per segment, bias ratio, CYLINDRICAL or GENERAL For example, the following input specifies 4 cylindrical elements in a 300° segment and 10 general elements in a 60° segment: *SYMMETRIC MODEL GENERATION, REVOLVE ax , ay , az , bx , by , bz cx , cy , cz 300.0, 4, 1.0, CYLINDRICAL 60.0, 10, 1.0, GENERAL Regular axisymmetric elements (CAX), axisymmetric elements with twist (CGAX), shell elements, membrane elements, rigid elements, and surface elements can be used in the two-dimensional model; however, nonlinear axisymmetric elements (CAXA) cannot be used. A two-dimensional model that contains incompatible mode elements; first-order, reduced-integration, continuum elements; shell elements; or rigid elements cannot be used to generate cylindrical elements. The correspondence between the axisymmetric element type and the equivalent three-dimensional element type (general or cylindrical) is shown in Table 10.4.1–1. Table 10.4.1–1 Correspondence between axisymmetric and three-dimensional (general and cylindrical) element types. Axisymmetric element General three- dimensional element Cylindrical element ACAX3 CAX3 CAX3H CGAX3 CGAX3H CGAX3T DCAX3 ACAX4 CAX4 CAX4H CAX4I CAX4R CAX4RH CGAX4 AC3D6 C3D6 C3D6H C3D6 C3D6H C3D6T DC3D6 AC3D8 C3D8 C3D8H C3D8I C3D8R C3D8RH C3D8 10.4.1–5 CCL9 CCL9H CCL9 CCL9H CCL12 CCL12H Axisymmetric element General three- dimensional element Cylindrical element CGAX4H CGAX4R CGAX4RH CAX4T CAX4RT CAX4HT CAX4RHT CGAX4T CGAX4RT CGAX4HT CGAX4RHT DCAX4 DCCAX4 DCCAX4D ACAX6 CAX6 CAX6H CGAX6 CGAX6H DCAX6 ACAX8 CAX8 CAX8H CAX8R CAX8RH CGAX8 CGAX8H CGAX8R CCL12H CCL18 CCL18H CCL18 CCL18H CCL24 CCL24H CCL24R CCL24RH CCL24 CCL24H CCL24R C3D8H C3D8R C3D8RH C3D8T C3D8RT C3D8HT C3D8RHT C3D8T C3D8RT C3D8HT C3D8RHT DC3D8 DCC3D8 DCC3D8D AC3D15 C3D15 C3D15H C3D15 C3D15H DC3D15 AC3D20 C3D20 C3D20H C3D20R C3D20RH C3D20 C3D20H C3D20R Axisymmetric element General three- dimensional element Cylindrical element CGAX8RH CAX8T CAX8RT CAX8HT CAX8RHT CGAX8T CGAX8RT CGAX8HT CGAX8RHT DCAX8 SAX1 DSAX1 SAX2 DSAX2 MAX1 MGAX1 MAX2 MGAX2 RAX2 SFMAX1 SFMGAX1 SFMAX2 SFMGAX2 C3D20RH C3D20T C3D20RT C3D20HT C3D20RHT C3D20T C3D20RT C3D20HT C3D20RHT DC3D20 S4R DS4 S8R DS8 M3D4R M3D4R M3D8R M3D8R R3D4 SFM3D4R SFM3D4R SFM3D8R SFM3D8R CCL24RH MCL6 MCL6 MCL9 MCL9 SFMCL6 SFMCL6 SFMCL9 SFMCL9 Limitations • First- and second-order elements cannot be used together in the axisymmetric model. • Nonaxisymmetric elements such as springs, dashpots, beams, and trusses will be ignored in the model generation. • Only surface-based contact pairs can be revolved. Models using general contact cannot be revolved. Contact conditions modeled with contact elements will be ignored in the model generation. • A two-dimensional model reduced- integration, continuum elements; shell elements; or rigid elements cannot be used to generate cylindrical elements. includes incompatible mode elements; first-order, that • Rebar with nonuniform spacing in the radial direction of an axisymmetric element cannot be revolved. • Most types of kinematic constraints cannot be revolved. However, surface-based constraints (“Mesh tie constraints,” Section 34.3.1) and embedded element constraints (“Embedded elements,” Section 34.4.1) defined in the original model will be generated automatically in the new three-dimensional model. • Only stress/displacement, heat transfer, coupled temperature-displacement, and acoustic elements can be revolved. Revolving a three-dimensional sector to create a periodic model You can create a three-dimensional periodic model by revolving a single three-dimensional sector about a symmetry axis. Each generated sector in the periodic model can span the same angle in the circumferential direction, such as in a vented disc, or alternatively, can have a variable angle, such as in a treaded tire. In both cases, each sector always has the same geometry and mesh. Both the symmetry axis and the original three-dimensional sector can be oriented in any direction with respect to the global coordinate system . Mismatched surface meshes can be used between sectors. Both open (the structure has end edges) or closed loop periodic structures can be generated. If a closed loop periodic structure needs to be created, the sum of the segment angles over all the sectors must be equal to 360°. Defining a periodic model with a constant angle To define a periodic model with a constant angle, you must specify the coordinates of points a and b shown in Figure 10.4.1–2 to define the symmetry axis. You then define the segment angle, (in degrees), of the original sector and the number of three-dimensional repetitive sectors, N, including the original sector, in the generated periodic model. Input File Usage: *SYMMETRIC MODEL GENERATION, PERIODIC=CONSTANT coordinates of points a and b θ, N Defining a periodic model with a variable angle To define a periodic model with a variable angle, the surfaces on both sides of the original sector must be completely planar. You specify the coordinates of points a and b shown in Figure 10.4.1–2 to define the symmetry axis. You then define the segment angle, (in degrees), of the original sector and the number of three-dimensional repetitive sectors, N, including the original sector, in the generated periodic model. Next, you specify an additional number of three-dimensional sectors to be generated, M, and the angular Figure 10.4.1–2 Revolving a three-dimensional sector to form a periodic model. scaling factor, f, in the circumferential direction with respect to the original sector to be applied to these additional sectors. You can define pairs of additional sectors and scaling factors as needed. Input File Usage: *SYMMETRIC MODEL GENERATION, PERIODIC=VARIABLE coordinates of points a and b θ, N M1 , f1 M2 , f2 Etc. For example, the following input creates a 210° three-dimensional model with 7 sectors with the angles of 20°, 20°, 30°, 30°, 30°, 40°, and 40°, respectively: *SYMMETRIC MODEL GENERATION, PERIODIC=VARIABLE ax , ay , az , bx , by , bz 20.0,2 3,1.5 2,2.0 Applying constraints to symmetric surfaces with mismatched meshes If the symmetric surfaces in the original sector have precisely matched meshes, as shown in Figure 10.4.1–3, any duplicate nodes that are generated will be eliminated automatically to ensure that the mesh is connected properly between the neighboring sectors when revolving the original sector about the symmetry axis to create a periodic model. Figure 10.4.1–3 Surfaces with precisely matching meshes on the original sector. In all other cases you must define one or more pairs of corresponding surfaces on each side of the original sector in the original model and specify the pairs of corresponding surfaces in the symmetric model generation definition. Optionally, you can also specify the tolerance distance within which nodes on one surface of a sector must lie from the corresponding surface of the neighboring sector to be constrained. Nodes on the surface of the sector that are further away from the corresponding surface of the neighboring sector than this distance are not constrained. The default value for the tolerance distance is 5% or 10% of the typical element size in the surfaces of the original sector, depending on whether node-to-surface or surface-to-surface type constraints are used, respectively. You can also specify whether surface-to-surface (default) or node-to-surface constraints should be used. Constraints between the automatically generated neighboring pairs of corresponding surfaces are then applied with an automatically generated surface-based tie constraint (“Mesh tie constraints,” Section 34.3.1) when revolving the original sector about the symmetry axis to create a periodic model. The first surface of each specified pair is the slave surface, and all degrees of freedom of the nodes in the surface will be eliminated by internally generated multi-point constraints. MODEL GENERATION Use the following options in the original model: *SURFACE, NAME=master *SURFACE, NAME=slave Use the following option in the new model with a constant angle for each sector: *SYMMETRIC MODEL GENERATION, PERIODIC=CONSTANT ax , ay , az , bx , by , bz θ, N slave, master, tolerance distance, SURFACE or NODE Use the following option in the new model with a variable angle for each sector: *SYMMETRIC MODEL GENERATION, PERIODIC=VARIABLE ax , ay , az , bx , by , bz θ, N M, f slave, master, tolerance distance, SURFACE or NODE Local orientation system If an A local cylindrical orientation system is always used for element output of stress, strain, etc. orientation is specified in the original three-dimensional sector , the orientation system in the new model is defined by revolving the original orientation system about the symmetry axis. If shells or membranes are used, the projections of the local 2- and 3-axes onto the surface of the shell or membrane are taken as the local directions on the surface. If the material in the original three-dimensional sector does not contain an orientation definition, a default local orientation definition is provided. This default orientation is defined by revolving the global coordinate system in the original model about the axis of symmetry in the new model. Controlling the new node and element numbering You can define the increments in numbers between each node and element around the circumference of the three-dimensional model. The numbering starts at the original three-dimensional repetitive sector. The original three-dimensional repetitive sector uses the same numbering as the original model. The defaults are the largest node and element numbers used in the original model. Control over the numbering allows you to define additional parts of the model without the risk of conflicting element and node labels. Each offset value should be greater than or equal to the maximum node or element label, respectively, used in the original model. When specifying the offset value, care must be taken that the generated node or element does not exceed the maximum value allowed, which is 999,999,999. *SYMMETRIC MODEL GENERATION, PERIODIC, NODE OFFSET=offset, ELEMENT OFFSET=offset Input File Usage: Limitations • Only surface-based contact pairs can be revolved. Models using general contact cannot be revolved. Contact conditions modeled with contact elements will be ignored in the model generation. • Most types of kinematic constraints cannot be revolved. However, surface-based constraints (“Mesh tie constraints,” Section 34.3.1) and embedded element constraints (“Embedded elements,” Section 34.4.1) defined in the original model will be generated automatically in the new three-dimensional model. One exception is that surface-based ties for enforcing cyclic symmetric constraints are not revolved. • Surface-based distributed coupling constraints—e.g., (“Coupling constraints,” Section 34.3.2), shell-to-solid couplings (“Shell-to-solid coupling,” Section 34.3.3), and fasteners (“Mesh-independent fasteners,” Section 34.3.4)—cannot be revolved and must be redefined. • Only stress/displacement, heat transfer, coupled temperature-displacement, and acoustic elements couplings can be revolved. Beam and frame elements cannot be revolved. Reflecting a partial three-dimensional model You can create a three-dimensional model by combining two parts of a symmetric three-dimensional model. One of the parts is the original model, and the other part is obtained by reflecting the original model through a symmetry line (Figure 10.4.1–4) or plane (Figure 10.4.1–5). Specify the coordinates of points a, b, and (if required) c shown in Figure 10.4.1–4 and Figure 10.4.1–5. reflection line 6 + n 5 + n 7 + n 8 + n 2 + n 1 + n 3 + n 4 + n Figure 10.4.1–4 Reflecting a three-dimensional model through line with node offset n. reflection plane 7 + n 8 + n 6 + n 5 + n 3 + n 4 + n 2 + n 1 + n Figure 10.4.1–5 Reflecting a three-dimensional model through a plane with node offset n. Input File Usage: Use one of the following options: *SYMMETRIC MODEL GENERATION, REFLECT=LINE *SYMMETRIC MODEL GENERATION, REFLECT=PLANE Controlling the new node and element numbering You can specify constants that must be added to the original node and element numbers for numbering the reflected part of the three-dimensional model. The defaults are the maximum node and element numbers used in the original model. Control over the numbering allows you to define additional parts of the model without the risk of conflicting element and node labels. Input File Usage: *SYMMETRIC MODEL GENERATION, REFLECT, NODE OFFSET=offset, ELEMENT OFFSET=offset Limitations • Only surface-based contact pairs can be reflected. Models using general contact cannot be reflected. Contact conditions modeled with contact elements will be ignored in the model generation. • You must ensure that master surfaces remain continuous after reflection. A discontinuous surface is created when the surface in the original model does not intersect the connection plane between the two parts of the symmetric structure. • Rigid surfaces cannot be reflected. The rigid surface definition of the original model is simply repeated in the new model. You must, therefore, specify the complete rigid surface in the original model. • Most types of kinematic constraints cannot be reflected. However, surface-based constraints (“Mesh tie constraints,” Section 34.3.1) and embedded element constraints (“Embedded elements,” Section 34.4.1) defined in the original model will be generated automatically in the new three-dimensional model. • Only stress/displacement, heat transfer, coupled temperature-displacement, and acoustic elements can be reflected. • Nonaxisymmetric elements such as springs, dashpots, beams, and trusses cannot be reflected. TRANSFERRING RESULTS FROM A SYMMETRIC MESH OR A PARTIAL THREE- DIMENSIONAL MESH TO A FULL THREE-DIMENSIONAL MESH SYMMETRIC RESULTS TRANSFER Product: Abaqus/Standard References • “Symmetric model generation,” Section 10.4.1 • *SYMMETRIC RESULTS TRANSFER Overview Symmetric results transfer: • reduces the analysis cost of structures that may first undergo symmetric deformation followed by nonsymmetric deformation later during the loading history; • can be used to transfer the solution of an axisymmetric model to a three-dimensional model; • can be used to transfer the solution of the symmetric part of a three-dimensional model to a full three-dimensional model; • must be used in conjunction with the symmetric model generation capability ; and • can be used only to transfer the solution of a stress/displacement, heat transfer, coupled temperature- displacement, or coupled acoustic-structural analysis to a new model. Transferring the solution from a symmetric mesh or a partial three-dimensional mesh to a full three-dimensional mesh The symmetric results transfer capability can be used to transfer the solution of an axisymmetric model to a three-dimensional model or to transfer the solution of the symmetric part of a three-dimensional model to a full three-dimensional model. The symmetric model generation capability described in “Symmetric model generation,” Section 10.4.1, must be used to generate the three-dimensional model. The symmetric results transfer capability is not available for models defined in terms of an assembly of part instances. The solution that is transferred to the new model consists of the deformed configuration and corresponding material state, which includes strains and all state variables. The nodes are imported with their original coordinates. This solution becomes the initial or base state in the new analysis. Specifying the time at which the solution obtained in the original model must be read You specify the time at which the solution obtained in the original model must be read. The required step and increment or iteration must have been written to the restart files during the original analysis. Input File Usage: Use the following option if the solution is transferred from any analysis other than a direct cyclic procedure: *SYMMETRIC RESULTS TRANSFER, STEP=step, INC=increment Use the following option if the solution is transferred from a previous direct cyclic analysis: *SYMMETRIC RESULTS TRANSFER, STEP=step, ITERATION=iteration Obtaining equilibrium You must ensure that the model is in equilibrium at the beginning of the analysis. It is recommended that an initial step definition be included using boundary conditions and loading that match the state of the model from which the results are transferred. An initial time increment equal to the total time should be used for this step to allow Abaqus/Standard to try and achieve the equilibrium in one increment. If needed, Abaqus/Standard can resolve the stress unbalance linearly over the step such that more than one increment is used. You can choose to have the stress unbalance resolved in the first increment of the step instead. Input File Usage: Use the following option to have Abaqus/Standard resolve the stress unbalance linearly over the step: *SYMMETRIC RESULTS TRANSFER, UNBALANCED STRESS=RAMP Use the following option to have Abaqus/Standard resolve the stress unbalance in the first increment of the step: *SYMMETRIC RESULTS TRANSFER, UNBALANCED STRESS=STEP Identifying the restart files The symmetric results transfer capability uses the restart (.res), analysis database (.stt and .mdl), part (.prt), and output database (.odb) files from the old analysis to transfer the solution data to the new mesh. The name of the restart files from the old analysis must be specified when the new analysis is executed by using the oldjob parameter in the command for running Abaqus or by answering a request made by the command procedure . Verifying the new model It is recommended that you verify that the new model is generated correctly before results are transferred or any analysis is performed. The model generation capability requires only information stored in the restart files during a data check run to generate the new model, which allows you to verify the new model before the analysis of the original model is performed. A data check analysis is performed by using the datacheck parameter in the command for running Abaqus . Once the model has been verified, the analysis of the original model can be performed and the results can be transferred to the new model. The transferred solution can be written to the results files by requesting output at the beginning of a step (the zero increment; see “Output,” Section 4.1.1). This solution can also be viewed in Abaqus/CAE. Orientation system When results are transferred from an axisymmetric model to a three-dimensional model, a local cylindrical orientation system is used for element output of stress, strain, etc. A default local orientation definition (“Orientations,” Section 2.2.5) is provided if the material in the original axisymmetric model does not contain an orientation definition. This default orientation is defined with the polar axis of the system along the axis of revolution with an additional 90° rotation about the local 1-direction so that the local axes are 1=radial, 2=axial, and 3=circumferential. If shells or membranes are used, the projections of the local 2- and 3-axes onto the surface of the shell or membrane are taken as the local directions on the surface. It is assumed that the material properties are specified in this system. If, on the other hand, an orientation definition is associated with the material in the original model, the orientation in the new three-dimensional model will be that orientation definition revolved about the axis of symmetry. When results are transferred from a partial three-dimensional model to a full three-dimensional model by reflecting the partial three-dimensional model, a local material orientation is created in the full three-dimensional model based on the corresponding orientation definition in the partial three-dimensional model. However, if the material does not contain an orientation definition in the partial three-dimensional model and the partial three-dimensional model is not created by revolving an axisymmetric model, no local orientation definition is created in the full three-dimensional model. The full three-dimensional model uses a global coordinate system. When results are transferred from a three-dimensional sector to a periodic three-dimensional model by revolving the three-dimensional sector about its symmetry axis, a local cylindrical orientation system is always used for element output of stress, strain, etc. If an orientation is specified in the original three-dimensional sector, the orientation system in the new model is defined by revolving the original orientation system about the symmetry axis. If shells or membranes are used, the projections of the local 2- and 3-axes onto the surface of the shell or membrane are taken as the local directions on the surface. If the material in the original three-dimensional sector does not contain an orientation definition, a default local orientation definition is provided. This default orientation is defined by revolving the global coordinate system in the original model about the axis of symmetry in the new model. Coordinate system at nodes The displacement and rotational components obtained from the original model are first transformed into a global, rectangular Cartesian axis system before the results are transferred. If local coordinate directions are required in the new model, a nodal transformation (“Transformed coordinate systems,” Section 2.1.5) must be specified in the new model to define this coordinate system. Limitations The following limitations exist for result transfer from an axisymmetric model to a 3-D model: • Result transfer is not available from 8-node reduced-integration axisymmetric elements (CAX8R and CAX8RH) to the corresponding 20-node brick elements (C3D20R and C3D20RH) when the elements are underlying the slave surface in a contact pair. • SAX2 is a finite-strain shell, while S8R is a small-strain shell. Do not use this combination when deformations are large in the original analysis. The following limitation exists for result transfer from a symmetric 3-D model to a full 3-D model: • Result transfer is not supported for shells with five degrees of freedom per node (STRI65, S8R5, and S9R5). Initial conditions Initial conditions can be specified on all nodes and elements, including the part of the model generated using symmetric model generation . However, in most cases the symmetric results transfer capability will overwrite the initial condition values with the solution obtained from the original model. An exception is initial temperatures and field variables. Initial temperatures and field variables are overwritten only when temperatures and field variables are specified in the original model. If only part of the original model contains a specification for temperatures or field variables, the remaining part of the model is assumed to have initial conditions with a magnitude of zero. This distribution of the field will be transferred to the new model. If temperatures and/or field variables are not defined anywhere in the original model, the initial conditions specified in the new model are applied. Boundary conditions All boundary conditions must be redefined; the symmetric result transfer capability ignores the boundary conditions specified in the original model. You must ensure that the model is in equilibrium at the beginning of the analysis; therefore, an initial step definition should be included using boundary conditions and loading that match the state of the model from which the results are transferred. Loads All loads must be redefined; the symmetric result transfer capability ignores the loads specified in the original model. You must ensure that the model is in equilibrium at the beginning of the analysis; therefore, an initial step definition should be included using boundary conditions and loading that match the state of the model from which the results are transferred. Material options All of the material definitions defined in the original model will be transferred to the new model. Elements Any element or contact pair removal/reactivation definition that was active in the original model should be respecified. Output All of the standard output variables available for stress/displacement elements can be used with the symmetric results transfer capability. The solution that is transferred to the new model can be written to the results (.fil) file by requesting output at the beginning of a step (the zero increment; see “Output,” Section 4.1.1). It can also be displayed in Abaqus/CAE. 10.4.3 ANALYSIS OF MODELS THAT EXHIBIT CYCLIC SYMMETRY Products: Abaqus/Standard Abaqus/CAE References • “Natural frequency extraction,” Section 6.3.5 • “Mode-based steady-state dynamic analysis,” Section 6.3.8 • *CYCLIC SYMMETRY MODEL • *SELECT CYCLIC SYMMETRY MODES • *SURFACE • *TIE • “Defining cyclic symmetry,” Section 15.13.19 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The cyclic symmetry analysis technique in Abaqus/Standard: • makes it possible to analyze the behavior of a 360° structure with cyclic symmetry based on a model of a repetitive sector; • can determine the response to cyclic symmetric loading in static, quasi-static, and heat transfer analyses; • can calculate all eigenfrequencies and eigenmodes of the 360° structure with the block Lanczos eigenfrequency extraction procedure; • can determine the response to loading corresponding to a given cyclic symmetry mode in modal- based steady-state dynamic analysis; and • does not require that matched meshes be used on the symmetry surfaces. Introduction Structures that exhibit cyclic symmetry provide the analyst with an opportunity to model an entire 360° structure at considerably reduced computational expense by analyzing only a single repetitive sector of the model. Typically, this is the smallest sector that can be identified, although this is not necessary. For example, if a structure consists of 16 repetitive sectors it is possible to use a 45° model containing two repetitive sectors. The sectors are numbered in the counterclockwise direction to the axis of cyclic symmetry (as described further below). Of course this is less efficient than using a 22.5° model with one sector. There is no restriction that the meshes on the two symmetry surfaces of a repetitive sector match in any way. There are two basic cases that must be considered in such an analysis: a model that has a cyclic symmetric initial state and a cyclic symmetric response, and a model with a cyclic symmetric initial state but a nonsymmetric response. The cyclic symmetry capability in Abaqus/Standard provides for linear and nonlinear analysis of cyclic symmetric structures with cyclic symmetric response. The condition that the structure be cyclic symmetric holds throughout the analysis, so in a loading step it is not possible to have any nonsymmetric deformation in the structure at any time. Therefore, only cyclic symmetric loads can be applied for this situation. Analysis of cyclic symmetric structures that exhibit nonsymmetric response requires additional consideration. Such an analysis can be performed only in a linear perturbation step, since the nonsymmetric deformation invalidates the assumption of a cyclic symmetric “base state” for any subsequent step in a general nonlinear analysis. The full response of an entire cyclic symmetric structure, such as the structure illustrated in Figure 10.4.3–1, can be represented as a linear combination of several independent basic responses, each of which corresponds to some k-fold cyclic symmetry mode. Finite element model of this sector only Figure 10.4.3–1 Cyclic symmetric structure. The cyclic symmetry mode number, which is sometimes also referred to as the “nodal diameter,” indicates the number of waves along the circumference in a basic response. Figure 10.4.3–2, Figure 10.4.3–3, and Figure 10.4.3–4 illustrate basic responses corresponding to the 0-, 1-, and 2-fold modes (nodal diameters 0, 1, and 2) in a cyclic symmetric structure containing four repetitive sectors. A full linear perturbation analysis can be performed by solving a sequence of corresponding linear analyses for a symmetric single sector. Cyclic symmetric boundary conditions (associated with various cyclic symmetry modes) on the single sector give rise to Hermitian stiffness and mass matrices (complex matrices with symmetric real parts and skew-symmetric imaginary parts). The kth linear analysis in the sequence is performed using symmetry conditions that correspond to the k-fold cyclic symmetry mode of the structural response. For a structure exhibiting N-fold cyclic symmetry, only (N odd) such analyses are required. This results in a solution for the response of the entire structure at a relatively low computational expense. (N even) or Figure 10.4.3–2 Response corresponding to the 0-fold cyclic symmetry mode. Figure 10.4.3–3 Response corresponding to the 1-fold cyclic symmetry mode. Figure 10.4.3–4 Response corresponding to the 2-fold cyclic symmetry mode. To perform a general linear analysis of a cyclic symmetric structure, the external forces should be represented as a linear combination of basic loads, each of which corresponds to a symmetry mode and excites a structural response corresponding to the same mode. In static analysis a capability to define loads on any mode other than the 0-fold mode has not yet been implemented. As the response of the 0-fold mode preserves cyclic symmetry, analysis of this type of structure can be done in a general nonlinear step, as well as in a linear perturbation step (as described above). For the same reason, such a step can be used as a preload step for a cyclic symmetric linear perturbation step. Extraction of a nonsymmetrical response for a cyclic symmetric structure is currently available only for eigenfrequency extraction analysis (“Natural frequency extraction,” Section 6.3.5) using the block Lanczos method and for frequency domain, modal-based steady-state dynamic analysis (“Mode-based steady-state dynamic analysis,” Section 6.3.8). Natural frequencies corresponding to both symmetric and nonsymmetric eigenmodes can be extracted for a specific cyclic symmetry mode, for a group of cyclic symmetry modes, or for all cyclic symmetry modes. They can be used within the subsequent steady-state dynamic analysis. The eigenmodes onto which the solution is projected are chosen as described in “Selecting the modes and specifying damping” in “Mode-based steady-state dynamic analysis,” Section 6.3.8. In a steady-state modal-based dynamic analysis, concentrated, distributed, and surface loads can be defined as projected onto a specific cyclic symmetry mode. Within the same steady-state dynamics step all applied loads have to be given as projected onto the same cyclic symmetry mode. This limitation implies that the specified cyclic symmetry mode must be the same for all loads within the given steady- state dynamics step. Defining a cyclic symmetric model Define the mesh for a single sector of the model, the so called “datum sector.” Specify the number of sectors, n, in the 360° model. Define the axis of symmetry by specifying the coordinates (in the global coordinate system) of two points lying on the axis. The axis direction is from the first point to the second point, and the sectors are numbered counterclockwise around the axis, with the datum sector as sector number 1. For a two-dimensional model only a single point needs to be given on the axis. The axis direction is assumed to be in the positive z-direction; hence, the sectors are numbered counterclockwise in the x–y plane. Input File Usage: *CYCLIC SYMMETRY MODEL, N=n In a model defined in terms of an assembly of part instances, the *CYCLIC SYMMETRY MODEL option must appear within the model definition . Abaqus/CAE Usage: Interaction module: Interaction→Create: Cyclic symmetry: Total number of sectors: n Applying cyclic symmetry constraints To apply the cyclic symmetry constraints, you must define one or more pairs of corresponding surfaces on each side of the datum sector . You can then apply the cyclic symmetry constraints between the pairs of corresponding surfaces using a cyclic symmetry surface-based tie constraint . The first surface of each pair specified in the tie constraint definition is the slave surface, and all degrees of freedom of the nodes in the surface will be eliminated by internally generated multi-point constraints. The second surface of each pair is a master surface. If more than one pair of slave/master surfaces is defined, the rotation direction from the slave surface to the master surface must be the same for all pairs (i.e., clockwise or counterclockwise). Input File Usage: Use the following options to apply a cyclic symmetry constraint between two surfaces: *SURFACE, NAME=master *SURFACE, NAME=slave *TIE, CYCLIC SYMMETRY, NAME=cyclic slave, master Abaqus/CAE Usage: Interaction module: Interaction→Create: Cyclic symmetry: click Surface in the prompt area Using mismatched surface meshes In the case of mismatched surface meshes, as shown in Figure 10.4.3–5, the finer mesh should typically be the slave surface. Mismatched meshes may cause some local inaccuracies in the stress field. The magnitude of the inaccuracies depends on the degree of mismatch between the meshes as well as on the element type used: the inaccuracies are typically most pronounced for second-order (modified) tetrahedral elements. Hence, if mismatched surface meshes are used, it is recommended that the sector boundaries be chosen in areas where accuracy of the local stress field is not critical. datum sector symmetry axis symmetry surfaces Figure 10.4.3–5 Cyclic symmetry surfaces with mismatched nodes. For shells the cyclic symmetry condition has to be applied to the nodes on the edges of the shell elements. Currently cyclic symmetry is not supported for element-based surfaces defined on the edges of shells. Therefore, if mismatched meshes are used for shell elements, an element-based surface should be defined on the top or bottom of the shell elements adjacent to the edges that form the master surface. A node-based surface can be defined on the edge that forms the slave surface. Applying node-to-node cyclic symmetry constraints In the case of matched meshes, either surface can be chosen as the slave surface. If the surfaces have matched meshes, as shown in Figure 10.4.3–6, it is possible to use a node-based master surface to obtain node-to-node cyclic symmetry constraints. The advantage of this is that Abaqus/Standard will adjust the positions of the nodes on the slave surface so that they precisely match the positions of the nodes on the master surface. This yields the most accurate results and minimizes the computational cost. In this case the slave surface will typically be chosen as a node-based surface as well, although computationally it does not matter since in either case a strict node-to-node constraint is applied. datum sector symmetry axis corresponding nodes on the symmetry surfaces symmetry surfaces Figure 10.4.3–6 Cyclic symmetry surfaces with node-to-node matching. For discrete members (such as trusses or beams) the cyclic symmetry condition can be enforced only using node-based surfaces. Input File Usage: Use the following options to apply a cyclic symmetry constraint between two node-based surfaces: *SURFACE, TYPE=NODE, NAME=master *SURFACE, TYPE=NODE, NAME=slave *TIE, CYCLIC SYMMETRY, NAME=cyclic slave, master Abaqus/CAE Usage: Interaction module: Interaction→Create: Cyclic symmetry: click Node Region in the prompt area Applying cyclic symmetry conditions on the symmetry axis If a node is located on the symmetry axis, special cyclic symmetry constraints must be applied for the 0-fold and 1-fold cyclic symmetry modes; whereas all degrees of freedom must be constrained for the other cyclic symmetry modes. For the 0-fold cyclic symmetry mode the degrees of freedom in the plane orthogonal to the symmetry axis are constrained; for the 1-fold cyclic symmetry mode the degrees of freedom along the symmetry axis are constrained. Abaqus/Standard will create these constraints automatically as long as the node is included in the definition of the slave surface, the master surface, or both the slave and master surfaces. Obtaining all eigenfrequencies of a cyclic symmetric structure The natural frequencies and corresponding eigenmodes of a cyclic symmetric structure can be extracted using the eigenfrequency extraction procedure with the Lanczos eigensolver . No additional information is required for the eigenfrequency extraction procedure. All the natural frequencies are sorted in the conventional (ascending) order. For each natural frequency the cyclic symmetry mode number is reported. The eigenmodes are written in the order corresponding to natural frequencies to the data (.dat), results (.fil), and output database (.odb) files for the user-specified datum sector only. These modes can be expanded in Abaqus/CAE to the entire structure depending on the cyclic symmetry mode number. There are two different types of eigenmodes: single and paired. The eigenmodes for 0-fold cyclic symmetry are always single. For even N the eigenmodes for the -fold cyclic symmetry are also single. The eigenmodes for the remaining (odd N) cyclic symmetry modes are paired. The natural frequencies corresponding to the paired eigenmodes are equal and always appear together in the table of the natural frequencies in the data file. The expansion of the eigenmodes with k-fold cyclic symmetry ( can be done in the following manner: ) to the sector (even N) or where Here (datum) sector and on the ith sectors, respectively; and and are paired eigenmodes corresponding to double natural frequencies on the first . From the expressions above it is clear that eigenmodes with 0-fold cyclic symmetry are always -fold cyclic symmetry are . Similarly, for even N the eigenmodes with symmetric; i.e., single, since . Selecting the cyclic symmetry modes You can select the cyclic symmetry modes for which the eigenfrequency analysis will be performed by specifying the lowest cyclic symmetry mode to be used in the analysis, nmin, and the highest cyclic symmetry mode to be used in the analysis, nmax. By default, nmin is 0. By default, nmax is (even N) or (odd N). The value of nmin cannot be greater than the value of nmax, and the value of nmax cannot be greater than the default value. If you do not select the cyclic symmetry modes, all possible cyclic symmetry modes are considered in the analysis. You can choose to use only the even cyclic symmetry modes. Input File Usage: Use the following option to specify the cyclic symmetry modes: Abaqus/CAE Usage: *SELECT CYCLIC SYMMETRY MODES, NMIN=nmin, NMAX=nmax Use the following option to request only the even cyclic symmetry modes: *SELECT CYCLIC SYMMETRY MODES, EVEN Use the following option to specify the cyclic symmetry modes: Interaction module: Interaction→Create: Cyclic symmetry: toggle on Specified range and specify the Lowest nodal diameter and Highest nodal diameter You cannot request only the even cyclic symmetry modes in Abaqus/CAE. Selecting the cyclic symmetry mode for a steady-state dynamic step Only a single cyclic mode can be excited in a steady-state dynamic step. You specify the cyclic symmetry mode associated with the loading in the load definition. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *CLOAD, CYCLIC MODE=k, REAL or IMAGINARY *DLOAD, CYCLIC MODE=k, REAL or IMAGINARY *DSLOAD, CYCLIC MODE=k, REAL or IMAGINARY Interaction module: Interaction→Create: Cyclic symmetry: Excited nodal diameter Comparison of the cyclic symmetry analysis technique and MPC type CYCLSYM MPC type CYCLSYM (“General multi-point constraints,” Section 34.2.2) provides a subset of the functionality provided by the cyclic symmetry analysis capability. For an eigenvalue analysis MPC type CYCLSYM will allow extraction of the symmetric (0-fold) modes only. The cyclic symmetry analysis capability allows the use of surfaces (“Surfaces: overview,” Section 2.3.1) to define the symmetry surfaces for the model, which enables the use of mismatched meshes on the symmetry surfaces, whereas MPC type CYCLSYM can be applied only on a node-to-node basis. Limitations The following limitations exist: • A continuation capability is not available for the cyclic symmetry eigenvalue extraction procedure. Each eigenvalue extraction step will not reuse any eigenmodes obtained in the previous eigenvalue extraction steps. • The specified cyclic symmetry mode must be the same for all loads defined within a given steady- state dynamic step. • Base motion is not implemented for cyclic symmetry models. • Cyclic symmetry conditions are applied to the mechanical degrees of freedom in stress/displacement analysis and temperature degrees of freedom in heat transfer analysis. Cyclic symmetry conditions are not applied to acoustic pressure, pore pressure, and electrical degrees of freedom. • Cavity radiation cannot be used in cyclic symmetric models. Initial conditions All applied initial conditions must be cyclic symmetric. Boundary conditions Only cyclic symmetric boundary conditions can be applied. Boundary conditions cannot be applied to the nodes on the slave cyclic symmetry surface. Loads In static analysis only cyclic symmetric loads can be applied. Coriolis loads cannot be applied, and the effect of the Coriolis load stiffness is not considered in the frequency analysis. In modal-based steady-state dynamic analysis the loads are defined on the datum sector for a specific cyclic symmetry mode, which is indicated in the loading definition. For the k-fold cyclic symmetry mode (corresponding to real and imaginary components, respectively) on the sector are obtained in the following manner: the complex loads and where and F and G are real and imaginary components of loads specified for the datum sector, respectively. For the 0-fold cyclic symmetry mode ( ) this type of loading corresponds to a cyclic symmetric load pattern with this type of loading is generated when . For a spatially constant load pattern is applied to a rotating structure (or when a constant load pattern rotates around the structure). For the and -fold mode the complex loads on the sector i are: and . Predefined fields Only cyclic symmetric predefined fields can be applied. Hence, the predefined fields should have the same values at each side of the datum sector. Material options No specific restrictions apply to material models for cyclic symmetry models of general procedures. For the frequency analysis procedure, see the remarks in “Natural frequency extraction,” Section 6.3.5. Elements Axisymmetric elements should not be used in cyclic symmetry models. Output Nodal displacements and element output variables such as stress, strain, and section force are only available for the datum sector. The mass listed in the data file is computed for the whole model. In the eigenvalue extraction procedure the following special conditions apply: • If displacement eigenvector normalization is chosen (the default), the largest displacement entry in each eigenvector on the datum sector is unity. If mass eigenvector normalization is chosen, the eigenvectors are normalized so that the generalized mass computed on the datum sector is unity. See “Natural frequency extraction,” Section 6.3.5, for details. • The eigenvalue numbers, cyclic symmetry mode numbers, and corresponding frequencies (in both radians/time and cycles/time) are listed in the data file, along with the generalized masses, composite modal damping factors, participation factors, and modal effective masses. The generalized masses are calculated on the datum sector; composite modal damping factors, participation factors, and modal effective masses are calculated for the entire model. • You can restrict output to the results and data files by selecting the modes for which output is desired . • With Abaqus/CAE static displacements and eigenmodes can be displayed for any sector. The results of steady-state, modal-based dynamic analysis can also be animated for any number of sectors, including the entire model. Input file template *HEADING … ** *CYCLIC SYMMETRY MODEL, N=integer N denotes the number of sectors in the entire 360° model. … ** *SURFACE, NAME=name, TYPE=ELEMENT *SURFACE, NAME=name, TYPE=NODE Surface description for the slave and master nodes that will be referenced in the *TIE option. … ** *TIE, CYCLIC SYMMETRY Indicates the internal MPCs that tie the master and slave surfaces using the cyclic symmetry condition in the cyclic symmetry models only. Data lines to specify surface names that will be tied with this option. … ** *STEP (,NLGEOM) If NLGEOM is used, initial stress and preload stiffness effects will be included in subsequent linear perturbation steps, including the frequency extraction step *STATIC ... *DLOAD Data lines to specify element or element set, load type, value, (direction). ... ** *END STEP *STEP *FREQUENCY, EIGENSOLVER=LANCZOS … *SELECT CYCLIC SYMMETRY MODES, NMAX=integer, NMIN=integer, EVEN … ** *END STEP *STEP *STEADY STATE DYNAMICS … *SELECT EIGENMODES Use this option to specify the list of eigenmodes used in the response. *MODAL DAMPING Data lines to specify damping coefficients associated with eigenmodes. … *CLOAD, CYCLIC MODE=integer, REAL or IMAGINARY Data lines to specify node or node set, degree of freedom, value *DLOAD, CYCLIC MODE=integer, REAL or IMAGINARY Data lines to specify element or element set, load type, value, (direction) … *DSLOAD, CYCLIC MODE=integer, REAL or IMAGINARY Data lines to specify element or element set, load type, value, (direction) … ** *END STEP 10.5 Periodic media analysis • “Periodic media analysis,” Section 10.5.1 10.5.1 PERIODIC MEDIA ANALYSIS Product: Abaqus/Explicit References • *PERIODIC MEDIA • *MEDIA TRANSPORT Overview The periodic media analysis technique in Abaqus/Explicit: • is a Lagrangian technique that offers an Eulerian-like view into a moving structure; • can be used to effectively model systems that are repetitive in nature, such as manufacturing processes involving conveyor belts or continuous forming operations; • leads to significant analysis time speedup when compared to traditional modeling techniques that may require excessively large meshes; and • requires topologically identical meshed parts to create the model, which can be accomplished via the parts and instances modeling paradigm. Introduction Quite often industrial processes that need to be analyzed involve sections that repeat in a simple pattern and move through a process zone. A prominent example is a conveyor belt with regularly spaced packages, as illustrated schematically in Figure 10.5.1–1 and exemplified with a finite element mesh in Figure 10.5.1–2. Continuous forming operations such as metal rolling are also good examples because the deforming material can be broken up into an arbitrary number of identical sections. Trigger plane Moving belt direction Re-instantiate exiting building block Figure 10.5.1–1 Schematic representation of periodic media. Step: Step−1, pre−tensioning of belt Increment 0: Step Time = 0.0 Figure 10.5.1–2 Conveyor belt with packages on top. For the sake of clarity we will use the conveyor belt example throughout this discussion to illustrate many of the concepts associated with the periodic media analysis technique. Figure 10.5.1–1 shows a conceptual decomposition of the conveyor belt; in reality, the belt is a continuous entity. Conceptually, the overall model can be decomposed into blocks (topologically identical meshed structures) that are connected together and span the process zone. You create a part that defines a “building block” (the meshed structure that is repeated to model the entire periodic media) and then construct the whole model via a chain of appropriately positioned instances. The periodic media analysis technique provides a simple way to automatically connect these instances together at the front and back ends of adjacent blocks. This technique also provides a convenient way to define loads and boundary conditions that represent the physical system at the unconnected ends of the first and last blocks in the chain. The first block of the chain is referred to as the inlet, and the last block is referred to as the outlet. Finally, when the periodic media moves through the process zone, blocks from the outlet are automatically shuffled to the inlet. The blocks (meshed structures) defined with this technique can interact via contact with other modeling features that are not periodic in nature, such as the rollers depicted in Figure 10.5.1–1. At the core of the periodic media analysis technique lies the concept of shuffling blocks from the outlet back to the inlet. A dedicated algorithm is used to detect when the inlet has moved too far into the process zone and to shuffle a block from the outlet directly to the inlet. The dashed arrow in Figure 10.5.1–1 illustrates the shuffling process. To ensure a smooth transition, the necessary nodal and element state data from the inlet block are stored at the beginning of the current step. When shuffling occurs, the stored nodal and element state data are mapped to the new inlet block and any inlet/outlet loads or boundary conditions are transferred to the newly exposed block ends. Thus, the periodic media analysis technique offers a convenient way for an Eulerian-like view into the moving repetitive structure. For example, you may be interested in assessing the package dynamics on the belt at a location somewhere between the rollers in both transient and steady-state conditions. You define several blocks around that location, you define contact with the rollers as necessary, and you provide appropriate inlet and outlet loading conditions. The periodic media analysis technique provides a convenient and economical way to create and analyze this system. By re-using elements that have left the process zone via this shuffling process, you can avoid the large meshes at the inlet end required for purely Lagrangian simulations. Constructing a periodic media model The first step in constructing a periodic media model is to identify the portion of the model that constitutes the building block of the repetitive structure. In Figure 10.5.1–2 one square belt patch together with one asymmetrically shaped package on top constitute such a building block. If you string together several blocks, the entire belt with packages can be modeled as shown. Defining a building block The following requirements must be observed when defining each building block: • an unsorted element set must be defined to include all elements in the building block, and • an unsorted node set must be defined to include all nodes in the building block. To ensure the proper transfer of information as the periodic media advances, these unsorted sets must be topologically identical between all blocks. The easiest way to achieve this requirement is to use the parts and instances modeling paradigm. You define one part corresponding to the building block and define unsorted element and node sets as discussed above. You then instantiate the part as many times as needed with the appropriate translations and rotations to generate the periodic media mesh. Constraints such as ties, couplings, and rigid bodies are allowed within a building block. You must ensure that these constraints are defined in a topologically identical fashion in all blocks. The periodic media analysis technique connects together these otherwise unconnected blocks to create a continuous model. If structural elements (e.g., shells) are used in the connecting regions of the blocks, the nodes on the edges of these regions are connected to the adjacent regions. If continuum elements are used, the nodes on the faces of these regions are connected. For these constraints to be constructed reliably, the following additional requirements must be observed: • the nodal arrangements at the front and back connecting ends of blocks must be topologically identical, • the front and back end nodes of adjacent blocks must be coincident, • the nodal arrangements at the front and back end of the initial inlet block must have coordinates that differ only by a rigid body translation, and • two node-based surfaces created using unsorted node sets at the front and back end of each block must be defined. The node-based surfaces are used to automatically generate node-to-node tie constraints between adjacent blocks such that the whole assembly behaves as a continuous entity. Input File Usage: Use the following option to define the sequence of blocks using unsorted sets and surfaces as described above: *PERIODIC MEDIA, NAME=name elset1, nodeset1, frontsurf1, backsurf1 elset2, nodeset2, frontsurf2, backsurf2 ... elsetn, nodesetn, frontsurfn, backsurfn Each data line provides the set and surface names associated with a given block. Applying loads and boundary conditions at media ends In the schematic belt shown in Figure 10.5.1–1, you usually need to apply loads or boundary conditions at both ends of the assembly. At the inlet point I it is often useful to apply a pre-tension load that keeps the belt taut, while at the outlet point O the belt velocity is usually prescribed. As the belt advances and exiting blocks are being shuffled from the outlet to the inlet, the nodes requiring the boundary conditions will change. Therefore, these boundary conditions and loads cannot be prescribed directly at nodes belonging to the block. The periodic media analysis technique allows for the application of such loading features via two control nodes that are associated with the current inlet and outlet node-based surfaces. The control nodes are similar to reference nodes used in other features (such as kinematic couplings) and impose automatically defined rigid body–like constraints on the nodes at the extreme ends of the assembly. You apply loads and boundary conditions at these control nodes. A rigid body–like constraint is also imposed on the front end nodes of the inlet block, but no loads or boundary conditions can be applied. When exiting blocks are being shuffled back to the inlet, the control points will enforce these rigid body–like constraints on the new extreme end surfaces and remove the rigid body–like constraints from the previous locations. The process is automatic and fully managed by the periodic media analysis technique. Input File Usage: Use the following option to define control nodes for the inlet and outlet conditions: *PERIODIC MEDIA, INLET CONTROL NODE=node, OUTLET CONTROL NODE=node Defining the process zone When the inlet block moves completely into the process zone, the outlet block is shuffled back to the inlet, as the dashed arrow indicates in Figure 10.5.1–1. A trigger plane controls the precise timing for when the shuffling occurs. When the nodes located at the current inlet point I cross the trigger plane, the shuffling process is launched. The trigger plane is defined using the coordinates of a (usually) stationary node and the z-axis of a user-defined orientation. The local z-axis direction points from the inlet toward the process zone. Input File Usage: Use the following option to define the trigger plane via a trigger node and orientation: *PERIODIC MEDIA, TRIGGER NODE=node, ORIENTATION=orientation Activating a periodic media The shuffling process can be activated on a step-by-step basis. By default, the shuffling process is inactive. In many cases the configuration of the periodic media in the operating condition can be determined only via simulation. This allows any number of analysis steps to be carried out prior to activating the shuffling process. The example illustrated in Figure 10.5.1–2 and in “Media transport,” Section 3.25.1 of the Abaqus Verification Manual, shows a conveyor belt transporting asymmetrical packages placed initially at regular intervals. In its operating condition the belt will be tensioned. You can pre-stretch the belt assembly in either Abaqus/Standard or Abaqus/Explicit. If the pre-stretch analysis is conducted in Abaqus/Standard, all ties between adjacent blocks as well as boundary conditions at the inlet and outlet ends nodes need to be defined explicitly as the periodic media analysis technique is available only in Abaqus/Explicit. If the pre-stretching step is conducted in Abaqus/Explicit, the shuffling process should remain inactive during the pre-stretching step. Input File Usage: Use the following option to activate or deactivate the periodic media shuffling process: *MEDIA TRANSPORT periodic_media_name1, ACTIVE periodic_media_name2, INACTIVE ... Modeling tips The periodic media analysis technique is a powerful feature; however, you must exercise good engineering judgement when using it. The following comments and recommendations will help you avoid common pitfalls when using this technique: • The block shuffling process is inherently noisy as chunks of elements are detached at one end and reattached at the other. Although the process uses appropriate material and kinematic states, small shocks are inherent to the process. A small amount of mass proportional damping is recommended to dampen out this excitation. • The combination of boundary conditions at the inlet control node and any loads applied in the process zone should ensure that the inlet block moves across the trigger plane without a change in direction. In the conveyor belt example, a good modeling practice would be to place a fixed guide roller at least two blocks away from the trigger plane. • For more complex geometries (such as belts that change direction between rollers or package wrapping analyses when the belt is the wrapping material itself), it may be necessary to start with a straight sequence of blocks and move the belt rollers (which are not part of the periodic media definition) into the desired locations. Contact interaction between the belt and the rollers would deform the belt in the desired configuration. This additional analysis step can greatly simplify the definition of the initial mesh. • Sometimes it may be necessary to model the process of threading a belt wrapping through rollers, just as in physical reality at the start of a manufacturing process. If this leading segment is followed by periodic blocks that include actual packages, you can attach the periodic media mesh to a regular mesh to execute the threading. The periodic media part of the mesh can then be imported into a separate model without the leading mesh, and the analysis of the periodic media consisting only of the wrapper and packages can be executed. Initial conditions Initial conditions can be specified at all nodes in the periodic media mesh. Velocity initial boundary conditions can be used to minimize the solution time needed to reach a steady-state operating condition. In cases where pre-stretching is required, importing from the prior analysis rather than performing a multistep analysis allows for initial conditions to be applied to the stretched configuration. Since periodic media definitions are not imported, they must be respecified in every analysis in which they are required. Boundary conditions The inlet and outlet control nodes are the only two nodes associated with a periodic media definition at which boundary conditions can be specified. Furthermore, only velocity boundary conditions are permitted. You must not specify boundary conditions at any other node associated with the periodic media mesh. While the periodic media is active and if a steady-state solution is sought, these boundary conditions should be kept constant in both direction and magnitude to mitigate solution noise. Loads Only concentrated loads can be applied to the inlet and outlet control nodes to either drive or stretch the periodic media. While the periodic media is active, these loads should be kept constant in both direction and magnitude. Gravity loads can be applied as desired. Other distributed loads can also be specified; however, you must keep in mind that the loads will travel with the blocks as they are shuffled. Material options Only the following material models can be used in association with a periodic media: • elasticity, • viscoelasticity, • Mises plasticity, • lamina elasticity, • hyperfoams, • crushable foams, and • user-defined materials. Limitations Periodic media analyses are subject to the following limitations: • Only membranes, shells, trusses, continuum elements, and rigid elements are allowed within blocks. Rebar layers can also be used, if applicable. • No explicitly defined constraints are allowed between nodes belonging to different blocks. • Mass scaling must be defined in the same fashion for all blocks. The periodic media should not be involved in • general contact that defines thermal contact properties or coupled Eulerian-Lagrangian contact or • contact defined via the contact pair algorithm. Input file template The following example illustrates a model with two periodic media defined: *HEADING … *PERIODIC MEDIA, NAME=belt1, CONTROL NODE=10, OUTLET CONTROL NODE=110, ORIENTATION=ori1, TRIGGER NODE=210 elset1, nodeset1, frontedgesurf1, backedgesurf1 elset2, nodeset1, frontedgesurf2, backedgesurf2 elset3, nodeset1, frontedgesurf3, backedgesurf3 *PERIODIC MEDIA, NAME=belt2, CONTROL NODE=11, OUTLET CONTROL NODE=111, ORIENTATION=ori2, TRIGGER NODE=211 elset1, nodeset1, frontedgesurf1, backedgesurf1 elset2, nodeset1, frontedgesurf2, backedgesurf2 elset3, nodeset1, frontedgesurf3, backedgesurf3 *STEP *DYNAMIC, EXPLICIT *MEDIA TRANSPORT belt1, ACTIVE belt2, INACTIVE *END STEP 10.6 Meshed beam cross-sections • “Meshed beam cross-sections,” Section 10.6.1 10.6.1 MESHED BEAM CROSS-SECTIONS Products: Abaqus/Standard Abaqus/Explicit References • *BEAM GENERAL SECTION • *BEAM SECTION GENERATE • *SECTION ORIGIN • *SECTION POINTS Overview Meshed cross-sections: • allow for the description of a beam cross-section including multiple materials and complex geometry; • are meshed in Abaqus/Standard with two-dimensional warping elements, which have an out-of- plane warping displacement as the only degree of freedom; • generate beam cross-section properties that can be used in a subsequent beam element analysis in either Abaqus/Standard or Abaqus/Explicit; • allow only isotropic linear elastic material behavior (“Defining isotropic elasticity” in “Linear elastic behavior,” Section 22.2.1) or orthotropic linear elastic material behavior for warping elements (“Defining orthotropic elasticity for warping elements” in “Linear elastic behavior,” Section 22.2.1); and • allow stress and strain postprocessing on the beam element model or the two-dimensional warping element model. Introduction The response of some structures is beam-like, yet the beam cross-section geometry or multi-material makeup of the cross-section do not permit the use of a predefined library beam cross-section. In these cases a meshed cross-section can be used to model the beam cross-section and to generate beam cross- section properties appropriate for subsequent use in a Timoshenko beam analysis. The beam properties are generated assuming a thick-walled (solid) cross-section with unconstrained out-of-plane warping, so open-section beam elements cannot use the beam cross-section properties generated from the meshed section . The generated beam cross-section properties include axial, bending, torsional, and transverse shear stiffnesses; mass, rotary inertia, and damping properties; and the centroid and shear center of the cross-section. In addition, the equivalent beam cross-section properties include information on stress recovery, such as the warping function and its derivatives. A typical example of a structure that requires a meshed cross-section is the hull of a ship for whipping analysis, where the ship’s hull has a multi-cell and multi-material construction. Other examples include an airfoil-shaped rotor blade or wing, a layered composite I-beam (with fibers running along the length of the beam axis or perpendicular to it), etc. Modeling approach As shown in Figure 10.6.1–1, a meshed cross-section allows for a complex description of a beam cross- section: one which may include an arbitrary shape, multiple materials, multiple cells, and non-structural mass. The basic idea is to create a two-dimensional finite element model of the beam cross-section. The meshed cross-section is used in Abaqus/Standard to numerically calculate the properties required to characterize the structural response of the cross-section in a subsequent beam element analysis. The two- dimensional Abaqus/Standard analysis writes the cross-sectional properties to an input-file-ready text file (jobname.bsp). In the subsequent Abaqus/Standard or Abaqus/Explicit beam element analysis the beam elements requiring the meshed cross-section properties include the text file jobname.bsp as the general beam section data. Once the beam element analysis is complete, the Visualization module of Abaqus/CAE is used to visualize results at preselected points along the beam length or to examine detailed stress and strain results displayed directly on the two-dimensional meshed cross-section. Y global foam fluid steel or composite media X global Figure 10.6.1–1 An example of a meshed section profile. In summary, the procedure for analyzing and postprocessing a beam analysis using a meshed cross- section is as follows: 1. Mesh and analyze a two-dimensional Abaqus/Standard model of the beam cross-section. 2. Use the generated cross-sectional properties in an Abaqus/Standard or Abaqus/Explicit beam analysis. 3. Using the beam analysis results, postprocess from the beam model or the two-dimensional cross- section model. Meshing and analyzing a two-dimensional model of the beam cross-section The cross-section is meshed using special-purpose two-dimensional elements: WARP2D3 (3-node triangular) and WARP2D4 (4-node quadrilateral). These elements have one degree of freedom per node representing the value of the out-of-plane warping function and use a solid section definition; no section data are required. Adjacent elements in the cross-sectional mesh must share common nodes; mesh refinement using multi-point constraints is not allowed. Each element in the cross-sectional mesh can refer to a different elastic material, using either isotropic linear elastic material behavior or orthotropic linear elastic material behavior for warping elements . Alternatively, density (“Density,” Section 21.2.1) can be the only material property specified, which is useful for modeling non-structural masses such as fuel in a tank. The model is then analyzed by using the beam section property generation procedure within the step definition. This cross-section analysis will numerically calculate geometric, stiffness, and inertial properties of the section, including the warping function and shear center and will write the calculated properties to the jobname.bsp text file. The contents of this text file, which can be used in a subsequent Abaqus/Standard or Abaqus/Explicit beam analysis, are described in detail below. Input File Usage: Use the following option to generate beam section properties for a meshed cross-section: *BEAM SECTION GENERATE Defining the origin of the cross-section By default, the origin of the cross-section is the origin of the coordinate system used to define the mesh. You can override this default and input the coordinates of the origin directly or specify that the origin coincides with the shear center or centroid of the cross-section. A nondefault origin is particularly useful when the beam node to be used in the actual analysis does not coincide with the origin of the two-dimensional coordinate system. Input File Usage: Use both of the following options to input the coordinates of the origin directly: *BEAM SECTION GENERATE *SECTION ORIGIN Use both of the following options to locate the origin at either the centroid or shear center: *BEAM SECTION GENERATE *SECTION ORIGIN, ORIGIN=CENTROID or SHEAR CENTER Requesting output at particular integration points Output to the output database can be recovered during the actual analysis at particular integration points on the cross-section. Requesting output at a large number of cross-sectional points may degrade performance. Input File Usage: Use both of the following options to request output at particular integration points: *BEAM SECTION GENERATE *SECTION POINTS Contents of the jobname.bsp text file After the analysis to generate the cross-sectional properties completes, the jobname.bsp text file contains the following lines of data: , , , , , , , , , *TRANSVERSE SHEAR STIFFNESS , , *CENTROID , *SHEAR CENTER , *DAMPING, ALPHA= , BETA= , COMPOSITE= The first two lines of data in the jobname.bsp text file correspond to the section property data for an arbitrarily shaped solid general beam cross-section meshed with warping elements . If you requested output at particular integration points in the two-dimensional cross-section model generation, the jobname.bsp text file contains the following additional lines: *SECTION POINTS section point label, 2-D element number, integration point number E, , ... , , , , , where the set of two data lines is repeated for as many section points as requested. The cross-sectional property information written to the jobname.bsp text file will be read into the general beam section definition in the subsequent beam analysis as described below. Using the generated cross-section properties in a beam analysis the section properties calculated and stored in the jobname.bsp text file As discussed above, can be used in an actual beam analysis to define cross-sections for beam elements. The data stored in jobname.bsp correspond to the section property data for an arbitrarily shaped solid general beam cross-section meshed with warping elements . Consequently, a simple method of inserting these data is to include the jobname.bsp text file in the beam analysis. Input File Usage: Use the following options to generate section properties in a beam analysis: *BEAM GENERAL SECTION, SECTION=MESHED , , (direction cosines for ) *INCLUDE, INPUT=jobname.bsp Postprocessing from the beam model or the two-dimensional cross-section model A tickmark contour plot can be used to visualize stress and strain output along the length of the beam model. All stress and strain components requested for the two-dimensional cross-section model generation will be available. Contour plots of stress and strain on the two-dimensional cross-section are also available. The section geometry is read from the output database generated by the two-dimensional cross-section analysis, while the generalized section results are read from the output database generated by the beam analysis. Initial conditions Initial conditions are not meaningful when generating beam section properties and are ignored. Boundary conditions Boundary conditions are not meaningful when generating beam section properties and are ignored. Loads Loads are not meaningful when generating beam section properties and are ignored. Predefined fields Temperature and field variables are not allowed for meshed sections. Material options Only the following material behaviors are allowed for meshed sections: • isotropic linear elasticity (“Defining isotropic elasticity” in “Linear elastic behavior,” Section 22.2.1) • orthotropic linear elasticity for warping elements (“Defining orthotropic elasticity for warping elements” in “Linear elastic behavior,” Section 22.2.1) • density (“Density,” Section 21.2.1) Elements Warping elements must be used to mesh the two-dimensional cross-section. See “Warping elements,” Section 28.4.1, for details. Output Element output is calculated during the actual beam analysis at the integration points on the meshed cross-section that are selected in the property generation analysis as described above. Output from the property generation analysis is available only on the output database. The Visualization module of Abaqus/CAE can be used to generate contour plots of element output on the cross-section, which requires the output databases from both the section property generation analysis (the cross-section model) and the actual beam analysis. For more information, see the example Python script in “Viewing the analysis of a meshed beam cross-section,” Section 9.10.10 of the Abaqus Scripting User’s Manual. Input file template Generating the cross-section properties in an Abaqus/Standard analysis *HEADING Meshed cross section ... *NODE, NSET=ALL ... *ELEMENT, TYPE=WARP2D3, ELSET=TRI ... *ELEMENT, TYPE=WARP2D4, ELSET=QUAD ... *SOLID SECTION, MATERIAL=COMPOSITE, ELSET=TRI *MATERIAL,NAME=COMPOSITE *ELASTIC, TYPE=TRACTION E, G1, G2 *DENSITY ... *SOLID SECTION, MATERIAL=MASS_ONLY, ELSET=QUAD *MATERIAL, NAME=MASS_ONLY *DENSITY ... *STEP *BEAM SECTION GENERATE *SECTION ORIGIN X, Y *SECTION POINTS section point label, element number, integration point number *END STEP Using the generated cross-section properties in a subsequent Abaqus/Standard or Abaqus/Explicit beam analysis *HEADING Beam analysis ) , , ... *NODE, NSET=NALL ... *ELEMENT, TYPE=B31, ELSET=BEAM1 ... *BEAM GENERAL SECTION, SECTION=MESHED (direction cosines for *INCLUDE, INPUT=jobname.bsp ... *STEP *DYNAMIC ... *BOUNDARY ... *CLOAD ... *OUTPUT *ELEMENT OUTPUT ... *END STEP EXTENDED FINITE ELEMENT METHOD 10.7 Modeling discontinuities as an enriched feature using the extended finite element method • “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1 10.7.1 MODELING DISCONTINUITIES AS AN ENRICHED FEATURE USING THE EXTENDED FINITE ELEMENT METHOD Products: Abaqus/Standard Abaqus/CAE Abaqus/Viewer References • *ENRICHMENT • *ENRICHMENT ACTIVATION • “Using the extended finite element method to model fracture mechanics,” Section 31.3 of the Abaqus/CAE User’s Manual Overview Modeling discontinuities, such as cracks, as an enriched feature: • is commonly referred to as the extended finite element method (XFEM); • is an extension of the conventional finite element method based on the concept of partition of unity; • allows the presence of discontinuities in an element by enriching degrees of freedom with special displacement functions; • does not require the mesh to match the geometry of the discontinuities; • is a very attractive and effective way to simulate initiation and propagation of a discrete crack along an arbitrary, solution-dependent path without the requirement of remeshing in the bulk materials; • can be simultaneously used with the surface-based cohesive behavior approach or the Virtual Crack Closure Technique , which are best suited for modeling interfacial delamination; • can be performed using the static procedure , the implicit dynamic procedure , or the low-cycle fatigue analysis using the direct cyclic approach ; • can also be used to perform contour integral evaluations for an arbitrary stationary surface crack without the need to refine the mesh around the crack tip; • allows contact interaction of cracked element surfaces based on a small-sliding formulation; • allows both material and geometrical nonlinearity; and • is currently available only for first-order stress/displacement solid continuum elements and second- order stress/displacement tetrahedron elements. Modeling approach Modeling stationary discontinuities, such as a crack, with the conventional finite element method requires that the mesh conforms to the geometric discontinuities. Therefore, considerable mesh refinement is needed in the neighborhood of the crack tip to capture the singular asymptotic fields adequately. Modeling a growing crack is even more cumbersome because the mesh must be updated continuously to match the geometry of the discontinuity as the crack progresses. The extended finite element method (XFEM) alleviates the shortcomings associated with meshing crack surfaces. The extended finite element method was first introduced by Belytschko and Black (1999). It is an extension of the conventional finite element method based on the concept of partition of unity by Melenk and Babuska (1996), which allows local enrichment functions to be easily incorporated into a finite element approximation. The presence of discontinuities is ensured by the special enriched functions in conjunction with additional degrees of freedom. However, the finite element framework and its properties such as sparsity and symmetry are retained. Introducing nodal enrichment functions For the purpose of fracture analysis, the enrichment functions typically consist of the near-tip asymptotic functions that capture the singularity around the crack tip and a discontinuous function that represents the jump in displacement across the crack surfaces. The approximation for a displacement vector function with the partition of unity enrichment is where are the usual nodal shape functions; the first term on the right-hand side of the above equation, , is the usual nodal displacement vector associated with the continuous part of the finite element solution; the second term is the product of the nodal enriched degree of freedom vector, , and the associated discontinuous jump function across the crack surfaces; and the third term is the product of the nodal enriched degree of freedom vector, , and the associated elastic asymptotic crack-tip functions, . The first term on the right-hand side is applicable to all the nodes in the model; the second term is valid for nodes whose shape function support is cut by the crack interior; and the third term is used only for nodes whose shape function support is cut by the crack tip. Figure 10.7.1–1 illustrates the discontinuous jump function across the crack surfaces, , which is given by where normal to the crack at is a sample (Gauss) point, . is the point on the crack closest to , and is the unit outward Figure 10.7.1–1 illustrates the asymptotic crack tip functions in an isotropic elastic material, , which are given by Crack tip X* X* Figure 10.7.1–1 Illustration of normal and tangential coordinates for a smooth crack. where at the tip. is a polar coordinate system with its origin at the crack tip and is tangent to the crack These functions span the asymptotic crack-tip function of elasto-statics, and takes into account the discontinuity across the crack face. The use of asymptotic crack-tip functions is not restricted to crack modeling in an isotropic elastic material. The same approach can be used to represent a crack along a bimaterial interface, impinged on the bimaterial interface, or in an elastic-plastic power law hardening material. However, in each of these three cases different forms of asymptotic crack-tip functions are required depending on the crack location and the extent of the inelastic material deformation. The different forms for the asymptotic crack-tip functions are discussed by Sukumar (2004), Sukumar and Prevost (2003), and Elguedj (2006), respectively. Accurately modeling the crack-tip singularity requires constantly keeping track of where the crack propagates and is cumbersome because the degree of crack singularity depends on the location of the crack in a non-isotropic material. Therefore, we consider the asymptotic singularity functions only when modeling stationary cracks in Abaqus/Standard. Moving cracks are modeled using one of the two alternative approaches described below. Modeling moving cracks with the cohesive segments method and phantom nodes One alternative approach within the framework of XFEM is based on traction-separation cohesive behavior. This approach is used in Abaqus/Standard to simulate crack initiation and propagation. This is a very general interaction modeling capability, which can be used for modeling brittle or ductile fracture. The other crack initiation and propagation capabilities available in Abaqus/Standard are based on cohesive elements (“Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6) or on surface-based cohesive behavior (“Surface-based cohesive behavior,” Section 36.1.10). Unlike these methods, which require that the cohesive surfaces align with element boundaries and the cracks propagate along a set of predefined paths, the XFEM-based cohesive segments method can be used to simulate crack initiation and propagation along an arbitrary, solution-dependent path in the bulk materials, since the crack propagation is not tied to the element boundaries in a mesh. In this case the near-tip asymptotic singularity is not needed, and only the displacement jump across a cracked element is considered. Therefore, the crack has to propagate across an entire element at a time to avoid the need to model the stress singularity. Phantom nodes, which are superposed on the original real nodes, are introduced to represent the discontinuity of the cracked elements, as illustrated in Figure 10.7.1–2. When the element is intact, each phantom node is completely constrained to its corresponding real node. When the element is cut through by a crack, the cracked element splits into two parts. Each part is formed by a combination of some real and phantom nodes depending on the orientation of the crack. Each phantom node and its corresponding real node are no longer tied together and can move apart. original nodes phantom nodes Ω− crack crack Ω+ Ω− crack Ω+ Ω− + Ω− Ω− Ω− Ω− Figure 10.7.1–2 The principle of the phantom node method. The magnitude of the separation is governed by the cohesive law until the cohesive strength of the cracked element is zero, after which the phantom and the real nodes move independently. To have a set of full interpolation bases, the part of the cracked element that belongs in the real domain, , is extended to the phantom domain, , can be interpolated by using the degrees of freedom for the nodes in the phantom domain, . The jump in the displacement field is realized by simply integrating only over the area from the side of the real nodes up to the crack; i.e., and . This method provides an effective and attractive engineering approach and has been used for simulation of the initiation and growth of multiple cracks in solids by Song (2006) and Remmers (2008). It has been proven to exhibit almost no mesh dependence if the mesh is sufficiently refined. . Then the displacement in the real domain, Modeling moving cracks based on the principles of linear elastic fracture mechanics (LEFM) and phantom nodes Another alternative approach to modeling moving cracks within the framework of XFEM is based on the principles of linear elastic fracture mechanics (LEFM). Therefore, it is more appropriate for problems in which brittle crack propagation occurs. Similar to the XFEM-based cohesive segments method described above, the near-tip asymptotic singularity is not considered, and only the displacement jump across a cracked element is considered. Therefore, the crack has to propagate across an entire element at a time to avoid the need to model the stress singularity. The strain energy release rate at the crack tip is calculated based on the modified Virtual Crack Closure Technique (VCCT), which has been used to model delamination along a known and partially bonded surface (see “Crack propagation analysis,” Section 11.4.3). However, unlike this method, the XFEM-based LEFM approach can be used to simulate crack propagation along an arbitrary, solution-dependent path in the bulk material without the requirement of a pre-existing crack in the model. The modeling technique is very similar to the XFEM-based cohesive segment approach described above where phantom nodes are introduced to represent the discontinuity of the cracked element when the fracture criterion is satisfied. The real node and the corresponding phantom node will separate when the equivalent strain energy release rate exceeds the critical strain energy release rate at the crack tip in an enriched element. The traction is initially carried as equal and opposite forces on the two surfaces of the cracked element. The traction is ramped down linearly over the separation between the two surfaces with the dissipated strain energy equal to either the critical strain energy required to initiate the separation or the critical strain energy required to propagate the crack depending on whether the VCCT or the enhanced VCCT criterion is specified. Modeling low-cycle fatigue crack propagation based on the principles of LEFM The XFEM-based LEFM approach can also be used to simulate a discrete crack growth subjected to sub- critical cyclic loading in a low-cycle fatigue analysis using the direct cyclic approach (“Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7). The fracture energy release rates at the crack tips in the enriched elements are calculated based on the above mentioned modified VCCT technique. The onset and crack growth are characterized by using the Paris law, which relates the relative fracture energy release rates to crack growth rates as illustrated in Figure 10.7.1–3. This approach has been used to model progressive delamination under a sub-critical cyclic loading along a known and partially bonded surface . However, unlike this method, the XFEM-based LEFM approach can be used to simulate fatigue crack propagation along an arbitrary, solution-dependent path in the bulk material. Using the level set method to describe discontinuous geometry A key development that facilitates treatment of cracks in an extended finite element analysis is the description of crack geometry, because the mesh is not required to conform to the crack geometry. The level set method, which is a powerful numerical technique for analyzing and computing interface motion, fits naturally with the extended finite element method and makes it possible to model arbitrary crack growth without remeshing. The crack geometry is defined by two almost-orthogonal signed distance functions, as illustrated in Figure 10.7.1–4. The first, , describes the crack surface, while the second, , is used to construct an orthogonal surface so that the intersection of the two surfaces gives the crack front. indicates the positive normal to the crack front. No explicit representation of the boundaries or interfaces is needed because they are entirely described by the nodal data. Two signed distance functions per node are generally required to describe a crack geometry. indicates the positive normal to the crack surface; da dN Paris Regime Gthresh Gpl GC Figure 10.7.1–3 Fatigue crack growth governed by the Paris law. crack surface ( = 0) φ orthogonal surface ( = 0) Ψ + + crack front (intersection of and ) Ψ φ Figure 10.7.1–4 Representation of a nonplanar crack in three dimensions by two signed distance functions and . Defining an enriched feature and its properties You must specify an enriched feature and its properties. One or multiple pre-existing cracks can be associated with an enriched feature. In addition, during an analysis one or multiple cracks can initiate in an enriched feature without any initial defects. However, multiple cracks can nucleate in a single enriched feature only when the damage initiation criterion is satisfied in multiple elements in the same time increment. Otherwise, additional cracks will not nucleate until all the pre-existing cracks in an enriched feature have propagated through the boundary of the given enriched feature. If several crack nucleations are expected to occur at different locations sequentially during an analysis, multiple enriched features can be specified in the model. Enriched degrees of freedom are activated only when an element is intersected by a crack. Only stress/displacement solid continuum elements can be associated with an enriched feature. Input File Usage: Abaqus/CAE Usage: *ENRICHMENT Interaction module: Special→Crack→Create→XFEM Defining the type of enrichment You can choose to model an arbitrary stationary crack or a discrete crack propagation along an arbitrary, solution-dependent path. The former requires that the elements around the crack tips are enriched with asymptotic functions to catch the singularity and that the elements intersected by the crack interior are enriched with the jump function across the crack surfaces. The latter infers that crack propagation is modeled with either the cohesive segments method or the linear elastic fracture mechanics approach in conjunction with phantom nodes. However, the options are mutually exclusive and cannot be specified simultaneously in a model. Input File Usage: Abaqus/CAE Usage: Use the following option to specify a crack propagation analysis (default): *ENRICHMENT, TYPE=PROPAGATION CRACK Use the following option to specify an analysis with stationary cracks: *ENRICHMENT, TYPE=STATIONARY CRACK Use the following input to specify a crack propagation analysis: Interaction module: crack editor: toggle on Allow crack growth Use the following input to specify an analysis with stationary cracks: Interaction module: crack editor: toggle off Allow crack growth Assigning a name to the enriched feature You must assign a name to an enriched feature, such as a crack. This name can be used in defining the initial location of the crack surfaces, in identifying a crack for contour integral output, and in activating or deactivating the crack propagation analysis. Input File Usage: Abaqus/CAE Usage: *ENRICHMENT, NAME=name Interaction module: Special→Crack→Create: XFEM: Name: name Identifying an enriched region You must associate the enrichment definition with a region of your model. Only degrees of freedom in elements within these regions are potentially enriched with special functions. The region should consist of elements that are presently intersected by cracks and those that are likely to be intersected by cracks as the cracks propagate. Input File Usage: Abaqus/CAE Usage: *ENRICHMENT, ELSET=element set name Interaction module: Special→Crack→Create→: XFEM: Select the crack domain: select region Defining contact of cracked element surfaces using a small-sliding formulation When an element is cut by a crack, the compressive behavior of the crack surfaces has to be considered. The formulae that govern behavior are very similar to those used for surface-based small-sliding penalty contact (“Mechanical contact properties: overview,” Section 36.1.1). For an element intersected by a stationary crack or a moving crack with the linear elastic fracture mechanics approach, it is assumed that the elastic cohesive strength of the cracked element is zero. Therefore, compressive behavior of the crack surfaces is fully defined with the above options when the crack surfaces come into contact. For a moving crack with the cohesive segments method, the situation is more complex; traction-separation cohesive behavior as well as compressive behavior of the crack surfaces are involved in a cracked element. In the contact normal direction, the pressure-overclosure relationship governing the compressive behavior between the surfaces does not interact with the cohesive behavior, since they each describe the interaction between the surfaces in a different contact regime. The pressure-overclosure relationship governs the behavior only when the crack is “closed”; the cohesive behavior contributes to the contact normal stress only when the crack is “open” (i.e., not in contact). If the elastic cohesive stiffness of an element is undamaged in the shear direction, it is assumed that the cohesive behavior is active. Any tangential slip is assumed to be purely elastic in nature and is resisted by the elastic cohesive strength of the element, resulting in shear forces. If damage has been defined, the cohesive contribution to the shear stresses starts degrading with damage evolution. Once maximum degradation has been reached, the cohesive contribution to the shear stresses is zero. The friction model activates and begins contributing to the shear stresses. Input File Usage: Use the following options to define contact of crack surfaces using a small- sliding formulation: *ENRICHMENT, INTERACTION=interaction_property_name *SURFACE INTERACTION, NAME=interaction_property_name *SURFACE BEHAVIOR Interaction module: crack editor: toggle on Specify contact property Abaqus/CAE Usage: Applying cohesive material concepts to XFEM-based cohesive behavior The formulae and laws that govern the behavior of XFEM-based cohesive segments for a crack propagation analysis are very similar to those used for cohesive elements with traction-separation constitutive behavior (“Defining the constitutive response of cohesive elements using a traction- separation description,” Section 32.5.6) and those used for surface-based cohesive behavior (“Surface-based cohesive behavior,” Section 36.1.10). The similarities extend to the linear elastic traction-separation model, damage initiation criteria, and damage evolution laws. Linear elastic traction-separation behavior The available traction-separation model in Abaqus assumes initially linear elastic behavior followed by the initiation and evolution of damage. The elastic behavior is written in terms of an elastic constitutive matrix that relates the normal and shear stresses to the normal and shear separations of a cracked element. , and (in three- , which represent the normal and the two shear tractions, respectively. The , consists of the following components: The nominal traction stress vector, , dimensional problems) corresponding separations are denoted by , , and . The elastic behavior can then be written as The normal and tangential stiffness components will not be coupled: pure normal separation by itself does not give rise to cohesive forces in the shear directions, and pure shear slip with zero normal separation does not give rise to any cohesive forces in the normal direction. The terms are calculated based on the elastic properties for an enriched element. Specifying the elastic properties of the material in an enriched region is sufficient to define both the elastic stiffness and the traction-separation behavior. , and , Damage modeling Damage modeling allows you to simulate the degradation and eventual failure of an enriched element. The failure mechanism consists of two ingredients: a damage initiation criterion and a damage evolution law. The initial response is assumed to be linear as discussed in the previous section. However, once a damage initiation criterion is met, damage can occur according to a user-defined damage evolution law. Figure 10.7.1–5 shows a typical linear and a typical nonlinear traction-separation response with a failure mechanism. The enriched elements do not undergo damage under pure compression. Damage of the traction-separation response for cohesive behavior in an enriched element is defined within the same general framework used for conventional materials . However, unlike cohesive elements with traction-separation behavior, you do not have to specify the undamaged traction-separation behavior in an enriched element. Crack initiation and direction of crack extension Crack initiation refers to the beginning of degradation of the cohesive response at an enriched element. The process of degradation begins when the stresses or the strains satisfy specified crack initiation criteria. Crack initiation criteria are available based on the following Abaqus/Standard built-in models: • the maximum principal stress criterion, • the maximum principal strain criterion, Tmax Tmax max max Crack opening (a) Crack opening (b) Figure 10.7.1–5 Typical linear (a) and nonlinear (b) traction-separation response. • the maximum nominal stress criterion, • the maximum nominal strain criterion, • the quadratic traction-interaction criterion, and • the quadratic separation-interaction criterion. In addition, a user-defined damage initiation criterion can be specified in user subroutine UDMGINI. An additional crack is introduced or the crack length of an existing crack is extended after an equilibrium increment when the fracture criterion, f, reaches the value 1.0 within a given tolerance: You can specify the tolerance initiation criterion is satisfied. The default value of . If , the time increment is cut back such that the crack is 0.05. Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, TOLERANCE= Property module: material editor: Mechanical: Damage for Traction Separation Laws: Quade Damage, Maxe Damage, Quads Damage, Maxs Damage, Maxpe Damage, or Maxps Damage: Tolerance: Specifying the crack direction When the maximum principal stress or the maximum principal strain criterion is specified, the newly introduced crack is always orthogonal to the maximum principal stress/strain direction when the fracture criterion is satisfied. However, when one of the other Abaqus/Standard built-in crack initiation criteria is used, you have to specify if the newly introduced crack will be orthogonal to the element local 1- direction or orthogonal to the element local 2-direction when the fracture criterion is satisfied. By default, the crack is orthogonal to the element local 1-direction. If a user-defined damage initiation criterion is specified, the normal direction to the crack plane or the crack line can be defined in user subroutine UDMGINI. Input File Usage: Abaqus/CAE Usage: Use one of the following options to specify the crack direction when the maximum nominal stress, the quadratic traction-interaction, or the quadratic separation-interaction criterion is specified: the maximum nominal strain, *DAMAGE INITIATION, NORMAL DIRECTION=1 (default) *DAMAGE INITIATION, NORMAL DIRECTION=2 Property module: material editor: Mechanical→Damage for Traction Separation Laws: Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Direction relative to local 1-direction (for XFEM): Normal or Parallel Maximum principal stress criterion The maximum principal stress criterion can be represented as represents the maximum allowable principal stress. The symbol represents the Macaulay Here, bracket with the usual interpretation (i.e., ). if The Macaulay brackets are used to signify that a purely compressive stress state does not initiate damage. Damage is assumed to initiate when the maximum principal stress ratio (as defined in the expression above) reaches a value of one. and if Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=MAXPS Property module: material editor: Mechanical: Damage for Traction Separation Laws: Maxps Damage Maximum principal strain criterion The maximum principal strain criterion can be represented as Here, represents the maximum allowable principal strain, and the Macaulay brackets signify that a purely compressive strain does not initiate damage. Damage is assumed to initiate when the maximum principal strain ratio (as defined in the expression above) reaches a value of one. Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=MAXPE Property module: material editor: Mechanical: Damage for Traction Separation Laws: Maxpe Damage Maximum nominal stress criterion The maximum nominal stress criterion can be represented as The nominal traction stress vector, is the component normal to the likely cracked surface, and , consists of three components (two in two-dimensional problems). are the two shear components on the likely cracked surface. Depending on what you specify , the likely cracked surface will be orthogonal either to the element local 1-direction or to the element local 2-direction. Here, represent the peak values of the nominal stress. The symbol represents the Macaulay bracket with the usual interpretation. The Macaulay brackets are used to signify that a purely compressive stress state does not initiate damage. Damage is assumed to initiate when the maximum nominal stress ratio (as defined in the expression above) reaches a value of one. , and and , Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=MAXS Property module: material editor: Mechanical: Damage for Traction Separation Laws: Maxs Damage Maximum nominal strain criterion The maximum nominal strain criterion can be represented as Damage is assumed to initiate when the maximum nominal strain ratio (as defined in the expression above) reaches a value of one. Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=MAXE Property module: material editor: Mechanical: Damage for Traction Separation Laws: Maxe Damage Quadratic nominal stress criterion The quadratic nominal stress criterion can be represented as Damage is assumed to initiate when the quadratic interaction function involving the stress ratios (as defined in the expression above) reaches a value of one. Input File Usage: *DAMAGE INITIATION, CRITERION=QUADS Abaqus/CAE Usage: Property module: material editor: Mechanical: Damage for Traction Separation Laws: Quads Damage Quadratic nominal strain criterion The quadratic nominal strain criterion can be represented as Damage is assumed to initiate when the quadratic interaction function involving the nominal strain ratios (as defined in the expression above) reaches a value of one. Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=QUADE Property module: material editor: Mechanical: Damage for Traction Separation Laws: Quade Damage User-defined damage initiation criterion User subroutine UDMGINI provides a general capability for implementing a user-defined damage initiation criterion. You can define several damage initiation mechanisms in user subroutine UDMGINI. You represent each damage initiation mechanism by a fracture criterion, , and its associated normal direction to the crack plane or the crack line. Although you can define several damage initiation mechanisms, the actual damage initiation for an enriched element is governed by the most severe damage initiation mechanism: Damage is assumed to initiate when f, as defined in the expression above, reaches a value of one. You must specify any material constants that are needed in user subroutine UDMGINI as part of a user-defined damage initiation criterion definition. Input File Usage: Use the following option to define a user-defined damage initiation criterion: *DAMAGE INITIATION, CRITERION=USER Use the following option to specify the total number of failure mechanisms in the user-defined damage initiation criterion: *DAMAGE INITIATION, CRITERION=USER, FAILURE MECHANISMS= Use the following option to define properties for a user-defined damage initiation criterion: *DAMAGE INITIATION, CRITERION=USER, PROPERTIES=number_of_constants Abaqus/CAE Usage: Defining a user-defined damage initiation criterion is not supported in Abaqus/CAE. Damage evolution The damage evolution law describes the rate at which the cohesive stiffness is degraded once the corresponding initiation criterion is reached. The general framework for describing the evolution of damage is conceptually similar to that used for damage evolution in surface-based cohesive behavior (“Surface-based cohesive behavior,” Section 36.1.10). A scalar damage variable, D, represents the averaged overall damage at the intersection between the crack surfaces and the edges of cracked elements. It initially has a value of 0. If damage evolution is modeled, D monotonically evolves from 0 to 1 upon further loading after the initiation of damage. The normal and shear stress components are affected by the damage according to otherwise (no damage to compressive stiffness); where separation behavior for the current separations without damage. , and , are the normal and shear stress components predicted by the elastic traction- To describe the evolution of damage under a combination of normal and shear separations across the interface, an effective separation is defined as Input File Usage: Use the following option to specify a damage evolution law: Abaqus/CAE Usage: *DAMAGE EVOLUTION Property module: editor: for Traction Separation Laws: Maxpe Damage or Maxps Damage: Suboptions→Damage Evolution Mechanical→Damage material Use in conjunction with user-defined damage initiation criterion A separate damage evolution law should be specified for each damage initiation criterion defined in user subroutine UDMGINI. Each combination of a damage initiation criterion and a corresponding damage evolution law is referred to as a failure mechanism. Damage will accumulate for only one failure mechanism per element, corresponding to the mechanism whose damage initiation criterion was achieved first. Input File Usage: Abaqus/CAE Usage: Use the following options to specify damage evolution laws for multiple user- defined damage initiation criteria: *DAMAGE INITIATION, CRITERION=USER, FAILURE MECHANISMS= *DAMAGE EVOLUTION, FAILURE INDEX=1 *DAMAGE EVOLUTION, FAILURE INDEX=2 ... *DAMAGE EVOLUTION, FAILURE INDEX= Defining a user-defined damage initiation criterion is not supported in Abaqus/CAE. Viscous regularization in Abaqus/Standard Models exhibiting various forms of softening behavior and stiffness degradation often lead to severe convergence difficulties in Abaqus/Standard. Viscous regularization of the constitutive equations defining cohesive behavior in an enriched element can be used to overcome some of these convergence difficulties. Viscous regularization damping causes the tangent stiffness matrix to be positive definite for sufficiently small time increments. The approximate amount of energy associated with viscous regularization over the whole model is available using output variable ALLVD. Input File Usage: Abaqus/CAE Usage: Use the following option to specify viscous regularization: *DAMAGE STABILIZATION Property module: material editor: Mechanical→Damage for Traction Separation Laws: Quade Damage, Maxe Damage, Quads Damage, Maxs Damage, Maxpe Damage, or Maxps Damage: Suboptions→Damage Stabilization Cohesive Applying the VCCT technique to the XFEM-based LEFM approach The formulae and laws that govern the behavior of the XFEM-based linear elastic fracture mechanics approach for crack propagation analysis are very similar to those used for modeling delamination along a known and partially bonded surface , where the strain energy release rate at the crack tip is calculated based on the modified Virtual Crack Closure Technique (VCCT). However, unlike this method, the XFEM-based LEFM approach can be used to simulate crack propagation along an arbitrary, solution-dependent path in the bulk material with or without an initial crack. You complete the definition of the crack propagation capability by defining a fracture-based surface behavior and specifying the fracture criterion in enriched elements. Crack nucleation and direction of crack extension By definition, the XFEM-based LEFM approach inherently requires the presence of a crack in the model since it is based on the principles of linear elastic fracture mechanics. The crack can be pre-existing, or it can nucleate during the analysis. If there is no pre-existing crack for a given enriched region, the XFEM- based LEFM approach is not activated until a crack nucleates. The crack nucleation is governed by one of the six built-in stress- or strain-based crack initiation criteria or a user-defined crack initiation criterion discussed in “Crack initiation and direction of crack extension,” above. After a crack is nucleated in an enriched region, subsequent propagation of the crack is governed by the XFEM-based LEFM criterion. Input File Usage: Use the following option to specify the crack nucleation criterion as part of the material definition when there is no pre-existing crack in an enriched region: Abaqus/CAE Usage: *DAMAGE INITIATION, TOLERANCE= Property module: material editor: Mechanical: Damage for Traction Separation Laws: Quade Damage, Maxe Damage, Quads Damage, Maxs Damage, Maxpe Damage, or Maxps Damage: Specifying when a pre-existing crack will extend If there is a pre-existing crack in an enriched region, the crack extends after an equilibrium increment when the fracture criterion, f, reaches the value 1.0 within a given tolerance: You can specify the tolerance extension criterion is satisfied. The default value of . If is 0.2. , the time increment is cut back such that the crack Input File Usage: Use both of the following options: Abaqus/CAE Usage: Interaction→Property→Create, Contact, *SURFACE BEHAVIOR *FRACTURE CRITERION, TOLERANCE= Interaction module: Mechanical→Fracture Criterion, Tolerance: , TYPE=VCCT Specifying the crack propagation direction You must specify the crack propagation direction when the fracture criterion is satisfied. The crack can extend at a direction normal to the direction of the maximum tangential stress, orthogonal to the element local 1-direction , or orthogonal to the element local 2-direction. By default, the crack propagates normal to the direction of the maximum tangential stress. Input File Usage: Use one of the following options to specify the crack direction when the fracture criterion is satisfied: Abaqus/CAE Usage: *FRACTURE CRITERION, NORMAL DIRECTION=MTS (default) *FRACTURE CRITERION, NORMAL DIRECTION=1 *FRACTURE CRITERION, NORMAL DIRECTION=2 Interaction module: contact property editor: Mechanical→Fracture Criterion: Direction of crack growth relative to local 1-direction: Maximum tangential stress, Normal, or Parallel Mixed mode behavior Abaqus provides three common mode-mix formulae for computing the equivalent fracture energy release rate : the BK law, the power law, and the Reeder law models. The choice of model is not always clear in any given analysis; an appropriate model is best selected empirically. BK law The BK law model is described in Benzeggagh and Kenane (1996) by the following formula: To define this model, you must provide and . This model provides a power law relationship combining energy release rates in Mode I, Mode II, and Mode III into a single scalar fracture criterion. Input File Usage: *FRACTURE CRITERION, TYPE=VCCT, MIXED MODE BEHAVIOR=BK Abaqus/CAE Usage: contact property editor: Mechanical→Fracture Interaction module: Criterion: Mixed mode behavior: BK, and enter the critical energy release rates in the data table Power law The power law model is described in Wu and Reuter (1965) by the following formula: To define this model, you must provide and . Input File Usage: *FRACTURE CRITERION, TYPE=VCCT, MIXED MODE BEHAVIOR=POWER Abaqus/CAE Usage: contact property editor: Mechanical→Fracture Interaction module: Criterion: Mixed mode behavior: Power, and enter the critical energy release rates in the data table Reeder law The Reeder law model is described in Reeder et al. (2002) by the following formula: To define this model, you must provide ; when when applies only to three-dimensional problems. and . The Reeder law is best applied , the Reeder law reduces to the BK law. The Reeder law Input File Usage: *FRACTURE CRITERION, TYPE=VCCT, MIXED MODE BEHAVIOR=REEDER Abaqus/CAE Usage: contact property editor: Mechanical→Fracture Interaction module: Criterion: Mixed mode behavior: Reeder, and enter the critical energy release rates in the data table Defining variable critical energy release rates You can define a VCCT criterion with varying energy release rates by specifying the critical energy release rates at the nodes. If you indicate that the nodal critical energy rates will be specified, any constant critical energy release rates you specify are ignored and the critical energy release rates are interpolated from the nodes. The critical energy release rates must be defined at all nodes in the enriched region. Input File Usage: Use both of the following options: *FRACTURE CRITERION, TYPE=VCCT, NODAL ENERGY RATE *NODAL ENERGY RATE Defining a VCCT criterion with varying energy release rates is not supported in Abaqus/CAE. Abaqus/CAE Usage: Enhanced VCCT criterion The formulae and laws governing the behavior of the enhanced VCCT criterion are very similar to those used for the VCCT criterion. However, unlike the VCCT criterion, the onset and growth of a crack can be controlled by two different critical fracture energy release rates: . In a general case and involving Mode I, II, and III fracture, when the fracture criterion is satisfied; i.e, the traction on the two surfaces of the cracked element is ramped down over the separation with the dissipated strain energy equal to the critical equivalent strain energy required to propagate the crack, . , rather than the critical equivalent strain energy required to initiate the separation, for different mixed-mode are identical to those used for The formulae for calculating fracture criteria. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *SURFACE BEHAVIOR *FRACTURE CRITERION, TYPE=ENHANCED VCCT Specifying the enhanced VCCT criterion is not supported in Abaqus/CAE. Low-cycle fatigue criterion based on the principles of LEFM If you specify the low-cycle fatigue criterion, progressive crack growth at the enriched elements subjected to sub-critical cyclic loading can be simulated. This criterion can be used only in a low-cycle fatigue analysis using the direct cyclic approach (“Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7). A low-cycle fatigue step can be the only step, can follow a general static step, or can be followed by a general static step. You can include multiple low-cycle fatigue analysis steps in a single analysis. If you perform a fatigue analysis in a model without a pre-existing crack, you must precede the fatigue step with a static step that nucleates a crack, as discussed in “Crack nucleation and direction of crack extension.” The onset and fatigue crack growth are characterized by using the Paris law, which relates the relative fracture energy release rate to crack growth rates as illustrated in Figure 10.7.1–3. The fracture energy release rates at the crack tips in the enriched elements are calculated based on the above mentioned VCCT technique. The Paris regime is bounded by the energy release rate threshold, , below which there is no consideration of fatigue crack initiation or growth, and the energy release rate upper limit, , above which the fatigue crack will grow at an accelerated rate. is the critical equivalent strain energy release rate calculated based on the user-specified mode-mix criterion and the fracture strength of the bulk material. The formulae for calculating have been provided above for different mixed mode fracture criteria. You can specify the ratio of . The default values are . and the ratio of over over and Input File Usage: Use both of the following options: Abaqus/CAE Usage: *SURFACE BEHAVIOR *FRACTURE CRITERION, TYPE=FATIGUE Specifying a low-cycle fatigue criterion is not supported in Abaqus/CAE. Onset of fatigue crack growth The onset of fatigue crack growth refers to the beginning of fatigue crack growth at the crack tip in the enriched elements. In a low-cycle fatigue analysis the onset of the fatigue crack growth criterion is characterized by , which is the relative fracture energy release rate when the structure is loaded between its maximum and minimum values. The fatigue crack growth initiation criterion is defined as and are material constants and is the cycle number. The enriched elements ahead of the where crack tips will not be fractured unless the above equation is satisfied and the maximum fracture energy release rate, , which corresponds to the cyclic energy release rate when the structure is loaded up to its maximum value, is greater than . Fatigue crack growth using the Paris law Once the onset of the fatigue crack growth criterion is satisfied at the enriched element, the crack growth rate, . The rate of the crack growth per cycle is given by the Paris law if , can be calculated based on the relative fracture energy release rate, where and are material constants. and At the end of cycle , from the current cycle , Abaqus/Standard extends the crack length, forward over an incremental number of cycles, by fracturing at least one enriched element to ahead of the crack tips. Given the material constants , combined with the known element length and the likely crack propagation direction at the enriched elements ahead of the crack tips, the number of cycles necessary to fail each enriched element ahead of the crack tip can be calculated as , where j represents the enriched element ahead of the th crack tip. The analysis is set up to advance the crack by at least one enriched element after the loading cycle is stabilized. The element with the fewest cycles is identified to be fractured, and its is represented as the number of cycles to grow the crack equal to its element length, . The most critical element is completely fractured with a zero constraint and a zero stiffness at the end of the stabilized cycle. As the enriched element is fractured, the load is redistributed and a new relative fracture energy release rate must be calculated for the enriched elements ahead of the crack tips for the next cycle. This capability allows at least one enriched element ahead of the crack tips to be fractured completely after each stabilized cycle and precisely accounts for the number of cycles needed to cause fatigue crack growth over that length. If , the enriched elements ahead of the crack tips will be fractured by increasing the cycle number count, , by one only. Viscous regularization for the XFEM-based LEFM approach The simulation of structures with unstable propagating cracks is challenging and difficult. Nonconvergent behavior may occur from time to time. Localized damping is included for the XFEM-based LEFM approach by using the viscous regularization technique. Viscous regularization damping causes the tangent stiffness matrix of the softening material to be positive for sufficiently small time increments. Input File Usage: Use one of the following options Abaqus/CAE Usage: *FRACTURE CRITERION, TYPE=VCCT, VISCOSITY= *FRACTURE CRITERION, TYPE=ENHANCED VCCT, VISCOSITY= Interaction module: Criterion: Viscosity: contact property editor: Mechanical→Fracture Specifying the initial location of an enriched feature Because the mesh is not required to conform to the geometric discontinuities, the initial location of a pre-existing crack must be specified in the model. The level set method is provided for this purpose. Two signed distance functions per node are generally required to describe a crack geometry. The first describes the crack surface, while the second is used to construct an orthogonal surface so that the intersection of the two surfaces gives the crack front . The first signed distance function must be either greater or less than zero and cannot be equal to zero. If an initial crack has to be defined at the boundaries of an element, a very small positive or negative value for the first signed distance function must be specified. Input File Usage: Abaqus/CAE Usage: Use the following option to specify the initial location of an enriched feature: *INITIAL CONDITIONS, TYPE=ENRICHMENT Interaction module: crack editor: Crack location: Select: select region Activating and deactivating the enriched feature The crack propagation capability can be activated or deactivated within the step definition. Input File Usage: Abaqus/CAE Usage: Contour integral Use the following option to activate the crack propagation capability within the step definition: *ENRICHMENT ACTIVATION, NAME=name, ACTIVATE=ON (default) Use the following option to deactivate the crack propagation capability within the step definition: *ENRICHMENT ACTIVATION, NAME=name, ACTIVATE=OFF Use the following option to deactivate the crack propagation capability automatically once all the pre-existing cracks (or if there are no pre-existing cracks, all the allowable newly nucleated cracks) have propagated through the boundary of the given enriched feature within the step definition: *ENRICHMENT ACTIVATION, NAME=name, ACTIVATE=AUTO OFF To modify the status of the crack propagation capability in a step, you must first create an XFEM crack growth interaction: Interaction module: Create Interaction: select initial step: XFEM Crack Growth: select crack: Interaction manager: select interaction in step: Edit: toggle on/off Allow crack growth in this step When you evaluate the contour integrals using the conventional finite element method (“Contour integral evaluation,” Section 11.4.2), you must define the crack front explicitly and specify the virtual crack extension direction in addition to matching the mesh to the cracked geometry. Detailed focused meshes are generally required and obtaining accurate contour integral results for a crack in a three-dimensional curved surface can be cumbersome. The extended finite element in conjunction with the level set method alleviates these shortcomings. The adequate singular asymptotic fields and the discontinuity are ensured by the special enrichment functions in conjunction with additional degrees of freedom. In addition, the crack front and the virtual crack extension direction are determined automatically by the level set signed distance functions. Input File Usage: Use the following option to obtain contour integral for a named enriched feature with the extended finite element method: Abaqus/CAE Usage: *CONTOUR INTEGRAL, XFEM, CRACK NAME=name Step module: history output request editor: Domain: Crack: crack name Specifying the enrichment radius Although XFEM has alleviated the shortcomings associated with refining the mesh in the neighborhood of the crack front due to the added asymptotic fields, you must generate a sufficient number of elements around the crack front to obtain path-independent contours. The group of elements within a small radius from the crack front are enriched and become involved in the contour integral calculations. The default enrichment radius is three times the typical element characteristic length in the enriched area. You must include the elements inside the enrichment radius in the element set used to define the enriched region. Input File Usage: Use the following option to specify an enrichment radius: Abaqus/CAE Usage: *ENRICHMENT, ENRICHMENT RADIUS Interaction module: crack editor: Enrichment radius: Analysis default or Specify Procedures Modeling discontinuities as an enriched feature can be performed using any of the following: • static analysis ; • implicit dynamic analysis ; or • low-cycle fatigue analysis using the direct cyclic approach (“Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7). Initial conditions Initial conditions to identify initial boundaries or interfaces of an enriched feature can be specified . Boundary conditions Boundary conditions can be applied to any of the displacement degrees of freedom . Loads The following types of loading can be prescribed in a model with an enriched feature: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–3); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” Predefined fields The following predefined fields can be specified in a model with an enriched feature, as described in “Predefined fields,” Section 33.6.1: • Nodal temperatures (although temperature is not a degree of freedom in stress/displacement elements). The specified temperature affects temperature-dependent critical stress and strain failure criteria. • The values of user-defined field variables. The specified value affects field-variable-dependent material properties. Material options Any of the mechanical constitutive models in Abaqus/Standard, including user-defined materials (defined using user subroutine “UMAT,” Section 1.1.40 of the Abaqus User Subroutines Reference Manual) can be used to model the mechanical behavior of the enriched element in a crack propagation analysis. See Part V, “Materials.” The inelastic definition at a material point must be used in conjunction with the linear elastic material model (“Linear elastic behavior,” Section 22.2.1) or the hypoelastic material model (“Hypoelastic behavior,” Section 22.4.1). Only isotropic elastic materials are supported when evaluating the contour integral for a stationary crack. Elements Only first-order solid continuum stress/displacement elements and second-order stress/displacement tetrahedron elements can be associated with an enriched feature. For propagating cracks these include bilinear plane strain and plane stress elements, bilinear axisymmetric elements, linear brick elements, linear tetrahedron elements, and second-order tetrahedron elements. For stationary cracks, these include linear brick elements, linear tetrahedron elements, and second-order tetrahedron elements. For an incompatible mode element, Abaqus/Standard discards the contribution due to the incompatible deformation mode immediately after the element is fractured under a tensile loading. Therefore, the stress level at the cracked element may not return completely to its originally unloaded state even when this cracked element is unloaded completely and the contact of the cracked element surfaces is reestablished. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables have special meaning for a model with an enriched feature: PHILSM PSILSM STATUSXFEM ENRRTXFEM Signed distance function to describe the crack surface. Signed distance function to describe the initial crack front. Status of the enriched element. (The status of an enriched element is 1.0 if the element is completely cracked and 0.0 if the element contains no crack. If the element is partially cracked, the value of STATUSXFEM lies between 1.0 and 0.0.) All components of strain energy release rate when linear elastic fracture mechanics with the extended finite element method is used. Visualization A crack can be visualized through the iso-surface for the signed distance function PHILSM. If a crack cuts through a very tiny corner of an enriched element, the displacements along the crack front in the enriched element may be distorted in rare cases in the Visualization module of Abaqus/CAE (Abaqus/Viewer) when displaying the contours. The distortion, however, is not present when viewing only the deformed shape. Limitations The following limitations exist with an enriched feature: • An enriched element cannot be intersected by more than one crack. • A crack is not allowed to turn more than 90° in one increment during an analysis. • Only asymptotic crack-tip fields in an isotropic elastic material are considered for a stationary crack. • Adaptive remeshing is not supported. Input file template The following is an example of modeling crack propagation with the XFEM-based cohesive segments method: *HEADING ... *NODE, NSET=ALL ... *ELEMENT, TYPE=C3D8, ELSET=REGULAR *ELEMENT, TYPE=C3D8, ELSET=ENRICHED ... *SOLID SECTION, MATERIAL=STEEL1, ELSET=REGULAR *SOLID SECTION, MATERIAL=STEEL12, ELSET=ENRICHED *ENRICHMENT, TYPE=PROPAGATION CRACK, ELSET=ENRICHED, NAME=ENRICHMENT, INTERACTION=INTERACTION *MATERIAL, NAME=STEEL1 ... *MATERIAL, NAME=STEEL2 *DAMAGE INITIATION, CRITERION=MAXPS, TOLERANCE=0.05 *DAMAGE EVOLUTION, TYPE=ENERGY Data lines to specify the failure mechanism ... *SURFACE INTERACTION, NAME=INTERACTION *SURFACE BEHAVIOR Data lines to specify the contact of cracked element surfaces ... *STEP *STATIC ... *END STEP *STEP *STATIC ... *ENRICHMENT ACTIVATION, TYPE=PROPAGATION CRACK, NAME=ENRICHMENT, ACTIVATE=OFF ... *END STEP The following is an example of modeling crack propagation with the XFEM-based LEFM approach: *HEADING ... *NODE, NSET=ALL ... *ELEMENT, TYPE=C3D8, ELSET=REGULAR *ELEMENT, TYPE=C3D8, ELSET=ENRICHED ... *SOLID SECTION, MATERIAL=STEEL1, ELSET=REGULAR *SOLID SECTION, MATERIAL=STEEL12, ELSET=ENRICHED *ENRICHMENT, TYPE=PROPAGATION CRACK, ELSET=ENRICHED, NAME=ENRICHMENT, INTERACTION=INTERACTION *MATERIAL, NAME=STEEL1 ... *MATERIAL, NAME=STEEL2 *DAMAGE INITIATION, CRITERION=MAXPS, TOLERANCE=0.05 Data lines to specify the crack nucleation mechanism ... *SURFACE INTERACTION, NAME=INTERACTION *SURFACE BEHAVIOR *FRACTURE CRITERION, TYPE=VCCT, TOLERANCE=0.05,VISCOSITY=0.00001 Data lines to specify the crack propagation criterion ... *END STEP The following is an example of calculating contour integrals in stationary cracks with the extended finite element method: *HEADING ... *NODE, NSET=ALL ... *ELEMENT, TYPE=C3D8, ELSET=REGULAR *ELEMENT, TYPE=C3D8, ELSET=ENRICHED ... *SOLID SECTION, MATERIAL=STEEL1, ELSET=REGULAR *SOLID SECTION, MATERIAL=STEEL12, ELSET=ENRICHED *ENRICHMENT, TYPE=STATIONARY CRACK, ELSET=ENRICHED, NAME=ENRICHMENT, ENRICHMENT RADIUS *MATERIAL, NAME=STEEL1 ... *MATERIAL, NAME=STEEL2 ... *STEP *STATIC ... *CONTOUR INTEGRAL, CRACK NAME=ENRICHMENT, XFEM *END STEP Additional references • Belytschko, T., and T. Black, “Elastic Crack Growth in Finite Elements with Minimal Remeshing,” International Journal for Numerical Methods in Engineering, vol. 45, pp. 601–620, 1999. • Benzeggagh, M., and M. Kenane, “Measurement of Mixed-Mode Delamination Fracture Toughness of Unidirectional Glass/Epoxy Composites with Mixed-Mode Bending Apparatus,” Composite Science and Technology, vol. 56, p. 439, 1996. • Elguedj, T., A. Gravouil, and A. Combescure, “Appropriate Extended Functions for X-FEM Simulation of Plastic Fracture Mechanics,” Computer Methods in Applied Mechanics and Engineering, vol. 195, pp. 501–515, 2006. • Melenk, J., and I. Babuska, “The Partition of Unity Finite Element Method: Basic Theory and Applications,” Computer Methods in Applied Mechanics and Engineering, vol. 39, pp. 289–314, 1996. • Reeder, “Postbuckling and and D. R.. Ambur, Growth of Delaminations in Composite Plates Subjected to Axial Compression” 43rd AIAA/ASME/ASCE/AHS/ASC Structures, Structural Dynamics, and Materials Conference, Denver, Colorado, vol. 1746, p. 10, 2002. P. B. Chunchu, S. Kyongchan, J., • Remmers, J. J. C., R. de Borst, and A. Needleman, “The Simulation of Dynamic Crack Propagation using the Cohesive Segments Method,” Journal of the Mechanics and Physics of Solids, vol. 56, pp. 70–92, 2008. • Song, J. H., P. M. A. Areias, and T. Belytschko, “A Method for Dynamic Crack and Shear Band Propagation with Phantom Nodes,” International Journal for Numerical Methods in Engineering, vol. 67, pp. 868–893, 2006. • Sukumar, N., Z. Y. Huang, J.-H. Prevost, and Z. Suo, “Partition of Unity Enrichment for Bimaterial Interface Cracks,” International Journal for Numerical Methods in Engineering, vol. 59, pp. 1075–1102, 2004. • Sukumar, N., and J.-H. Prevost, “Modeling Quasi-Static Crack Growth with the Extended Finite Element Method Part I: Computer Implementation,” International Journal for Solids and Structures, vol. 40, pp. 7513–7537, 2003. • Wu, E. M., and R. C. Reuter Jr., “Crack Extension in Fiberglass Reinforced Plastics,” T and M Report, University of Illinois, vol. 275, 1965. 11. Special-Purpose Techniques Inertia relief Mesh modification or replacement Geometric imperfections Fracture mechanics Surface-based fluid modeling Mass scaling Selective subcycling Steady-state detection 11.1 11.2 11.3 11.4 11.5 11.6 11.7 11.1 Inertia relief • “Inertia relief,” Section 11.1.1 11.1.1 INERTIA RELIEF Products: Abaqus/Standard Abaqus/CAE References • “Distributed loads,” Section 33.4.3 • “Defining an analysis,” Section 6.1.2 • *INERTIA RELIEF • “Defining an inertia relief load,” Section 16.9.16 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Inertia relief: • involves balancing externally applied forces on a free or partially constrained body with loads derived from constant rigid body accelerations; • requires material density or mass and/or rotary inertia values to be specified for computing inertia relief loads; • can be performed for static, dynamic, and buckling analyses in Abaqus/Standard; • varies the inertia relief loading with the applied loading in static analysis; • applies inertia relief load corresponding to the static preload in dynamic analysis; • can be used to balance applied perturbation loads when used with buckling analysis; • uses rigid body accelerations consistent with the specified boundary conditions to compute the inertia relief loads; • can be geometrically linear or nonlinear; • may require the use of the unsymmetric solver if there are large inertia relief moments in a geometrically nonlinear analysis; • is an inexpensive alternative to doing a full dynamic free body analysis when applied loads vary slowly compared to the eigenfrequencies of the body; and • can be used with multiple load cases. Typical applications Inertia relief loading can be applied in static (“Static stress analysis,” Section 6.2.2), dynamic (“Implicit dynamic analysis using direct integration,” Section 6.3.2), and eigenvalue buckling prediction steps (“Eigenvalue buckling prediction,” Section 6.2.3). In a static step the inertia relief loading varies with the applied external loading. An example of using an inertia relief load is modeling a rocket undergoing constant or slowly varying acceleration during lift-off (i.e., a free body subjected to a constant or slowly varying external force) with a static analysis procedure. The inertia forces experienced by the body are included in the static solution through inertia relief loading that balances the external loading. In a dynamic step the inertia relief loading is calculated based on the static preload and is held constant during the step. The following is an example of using an inertia relief load in a dynamic analysis procedure: Consider a free body submerged in water and subjected to shock wave loading due to an explosion. A dynamic analysis is needed to compute the transient solution. If it is known that initially the body is stationary under gravity and hydrostatic pressure from the fluid, the gravity load should exactly balance the buoyancy force. However, if the finite element model does not include all the mass existing in the body (for example, ballast), without additional loading, the body would accelerate due to out-of- balance external forces. Applying inertia relief loading exactly balances these unbalanced external loads, placing the body in static equilibrium. The dynamic analysis then provides the transient response of the body to the shock wave loading as deformation of the body relative to its static equilibrium position. In a buckling analysis the inertia relief load can be applied in the static preload step, in the eigenvalue buckling prediction step, or in both steps. In the eigenvalue buckling prediction step the inertia relief load is calculated based on the perturbation loads. Consider the static analysis rocket example. If we use inertia relief in a buckling analysis of the rocket with the rocket thrust as the perturbation load, we can predict the critical thrust that causes the rocket to buckle. Basic formulation In inertia relief the total response, due to rigid body motion of a reference point, , of the body is written as a combination of a rigid body response , and a relative response, : with corresponding expressions for velocities and accelerations. The reference point is the center of mass except when you must specify the reference point. Then, the finite element approximation to the dynamic equilibrium equation becomes is the mass matrix, where is the external force vector. The is the internal force vector, and response of interest in a static analysis involving inertia relief is the rigid body response corresponding to the dynamic motion of the reference point and the static response relative to the rigid body motion. Hence, the relative acceleration term drops from the equilibrium equation. The rigid body response can be expressed in terms of the acceleration of the reference point, , and rigid body mode vectors, , (in three dimensions): represents the acceleration vector corresponding to a unit imposed acceleration (displacement or rotation) in the j-direction at the reference point. For example, at a node with the usual three displacements and three rotations is INERTIA RELIEF is unity; all other where represent the coordinates of the reference point that is the center of rotation. If the system undergoes finite changes in geometry, are zero; x, y, and z are the coordinates of the node; and will both be functions of time. , and and , Projecting the dynamic equilibrium equation onto the rigid body modes, we have where is the rigid body acceleration associated with the rigid body mode j. The actual number of rigid body modes will be less than 6 in the presence of symmetry planes as well as for two-dimensional and axisymmetric analyses. Thus, the rigid body response can be evaluated directly from the external loads. is the “rigid body inertia” and The relative response of the body can be obtained by solving the equilibrium equation with the moved to the right hand side; that is, applied as a body force. The static known inertial term equilibrium equation then becomes where . In a dynamic analysis involving inertia relief the rigid body mode vectors are calculated in the configuration at the start of the dynamic analysis, and the reference point accelerations are calculated to balance the static preloads in this configuration. The relative acceleration term is not dropped, so the dynamic equilibrium equation becomes where . In a geometrically nonlinear analysis the rigid body mode vectors are recomputed during the analysis using the current configuration but the reference point accelerations are kept constant. This keeps the total magnitude of inertia relief loads constant during the analysis but allows the loads to be proportional to the spatial mass distribution, which changes with geometry. Input File Usage: *INERTIA RELIEF Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Inertia relief for the Types for Selected Step Inertia relief loading directions By default, all rigid body motion directions in a model can be loaded by inertia relief loading (in this discussion we use the word “direction” to mean any rigid body translation or rotation). In models with symmetry planes or models that are allowed to move freely in only specific directions, the free directions for which inertia relief loading is applied can be specified. For example, in a three-dimensional analysis with one symmetry plane only three free directions exist—two translations and one rotation. Add an additional symmetry plane and only one free translation remains. A cylinder-piston arrangement is an example where the only free direction considered is motion along the cylinder’s axis. In these situations you specify the free directions that are loaded by inertia relief loading by indicating the degrees of freedom. The case of two free rotation directions is not permitted. For cyclic symmetric models with inertia relief only translation in the Z-direction and rotation about the Z-direction are considered for computing inertia relief loading. Input File Usage: *INERTIA RELIEF integer list of global degrees of freedom identifying the free directions Abaqus/CAE Usage: For example, the list 1, 3, 5 implies that translations in the X- and Z-directions and rotation about the Y-axis are free directions. Load module: Create Load: choose Mechanical for the Category and Inertia relief for the Types for Selected Step: toggle on the degrees of freedom to define the Free Directions (the degrees of freedom displayed are dependent on the modeling space) Defining the free directions in a local coordinate system If the free directions are not global directions, an orientation can be used to define the local coordinate system to which the integer list of degree of freedom identifiers refers. Input File Usage: *INERTIA RELIEF, ORIENTATION=orientation_name integer list of local degrees of freedom identifying the free directions Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Inertia relief for the Types for Selected Step: click Edit, and choose a local CSYS Defining free direction combinations that require a user-specified reference point Not all user-chosen combinations of free directions admit unconstrained rigid body motion; that is, there are certain combinations of free directions for which an additional point is required to define the rigid body motion vectors. For example, in three dimensions the choice 4, 5, 6 corresponds to free rotations about a fixed point. The fixed point must be given to define the rigid body motion vectors. In other examples the free directions include rotation about a fixed axis. Consider a turbine blade rotating about its axis, as shown in Figure 11.1.1–1. turbine blade surfaces with cyclic symmetry constraints rigid body rotation chosen as free direction hub reference point on axis of rotation Figure 11.1.1–1 Inertia relief for a turbine blade with rotation about the axis as the only free direction. To find the angular acceleration of the blade as it rotates under an applied force couple or moment, you should specify the coordinates of the point on the shaft about which the blade is rotating. The free direction combinations for which you must specify a reference point are given in Table 11.1.1–1. Input File Usage: Abaqus/CAE Usage: *INERTIA RELIEF, ORIENTATION=orientation_name integer list of local degrees of freedom identifying the free directions X, Y, Z coordinates of the reference point for defining the rigid body vectors Load module: Create Load: choose Mechanical for the Category and Inertia relief for the Types for Selected Step: toggle on Global position of reference point, and enter the X, Y, and (if available) Z coordinates Table 11.1.1–1 Free direction combinations requiring a reference point. Degree of freedom identifiers defining free directions Reference point definition Fixed rotation point Point on rotation axis Point on symmetry line 4, 5, 6 1, 4, 5, 6 2, 4, 5, 6 3, 4, 5, 6 1, 2, 4, 5, 6 1, 3, 4, 5, 6 2, 3, 4, 5, 6 2, 4 3, 4 1, 5 3, 5 1, 6 2, 6 1, 2, 4 1, 2, 5 1, 3, 4 1, 3, 6 2, 3, 5 2, 3, 6 1, 4 2, 5 3, 6 Initial conditions Initial conditions can be specified in the same way as in static and dynamic analyses without inertia relief loads. If inertia relief is used in the first step in the analysis, these initial conditions form the base state of the body. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. Boundary conditions Boundary conditions are specified in the same way as in analyses without inertia relief loads . In theory, a statically determinate set of restraints is needed when inertia relief is used in a static step. By “statically determinate” we mean a set of restraints that restrain all rigid body modes but no deformation modes. Such a set provides a unique displacement solution and ensures that the inertia relief loading exactly balances the user-specified external loading: zero reaction forces with no rigid body motion of the center of mass. Table 11.1.1–2 summarizes the restraint requirements for various cases. Table 11.1.1–2 Necessary and sufficient statically determinate restraints. Problem dimensionality Free directions Number of required restraints 2-D 2 Translations and 1 Rotation Axisymmetric Axisymmetric with twist 1 Translation 1 Translation and 1 Rotation 3-D 3 Translations and 3 Rotations However, it is not necessary for the user to explicitly specify boundary conditions (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1) with inertia relief except in the case of buckling analysis. If no boundary conditions or insufficient boundary conditions are specified, a warning message will be issued and boundary conditions necessary to restrain the rigid body modes will be imposed internally at the point in the model that corresponds to the original location of the reference point. On the other hand, if too many boundary conditions are specified in certain directions, a warning message will be issued to indicate that the reaction forces may be nonzero at the nodes with overspecified boundary conditions. If there are insufficient boundary conditions in certain directions and too many boundary conditions in other directions, the problem will be treated as a combination of these cases. If a model has no boundary conditions or insufficient boundary conditions, a particular number of numerical singularity warnings can be issued during each equilibrium iteration in the analysis. The displacement solution is postprocessed to remove unconstrained rigid body motion. However, the number of numerical singularities should not exceed the number of unconstrained rigid body modes; any extra numerical singularity messages may indicate other problems. Similarly, a model with no boundary conditions or insufficient boundary conditions may produce negative eigenvalue messages. If the number of negative eigenvalues at each equilibrium iteration in the analysis does not exceed the maximum reasonable number of numerical singularities associated with the boundary conditions for inertia relief, the results can be trusted, but extra negative eigenvalues may indicate other problems. If a model contains symmetry planes or is constrained to move freely in specific directions, inertia relief loading should be applied only in those free directions. No boundary conditions should be specified in the free directions; however, sufficient boundary conditions must be specified in the other directions. Any boundary conditions that violate the above requirements will be flagged as an error. An error will also be issued if the combination of free directions includes only two free rotations or if a reference point is required but not specified. In a buckling analysis, proper boundary conditions are important for getting the correct mode shape. Sufficient boundary conditions must be specified when inertia relief loading is applied in such an analysis. See “Eigenvalue buckling prediction,” Section 6.2.3, for details on how to apply boundary conditions in a buckling analysis. Loads An analysis that uses inertia relief can include concentrated nodal forces at displacement degrees of freedom (1–6), distributed pressure forces or body forces, and user-defined loading. Inertia relief loads are used to balance the external loads. They are computed and applied when inertia relief is included in the step definition. The rules for propagating load definitions between steps hold for inertia relief loads. See “Applying loads: overview,” Section 33.4.1. The inertia relief loads will not be propagated to steps where inertia relief is not valid for the specified procedure. If there are large inertia relief moments in a geometrically nonlinear analysis, their contribution to the stiffness matrix may be unsymmetric. In such cases unsymmetric equation solution may improve the computational efficiency . Computing inertia relief loads The nodal force vector corresponding to the inertia relief loads is calculated as follows. The applied loads are projected onto the rigid body modes, . These force and moment components (six components in three dimensions) are used with the “rigid body inertia” to solve for the rigid body accelerations, . Only the rigid body acceleration components corresponding to the inertia relief loading directions are nonzero. The nodal force vector is calculated using the assembled mass matrix as Fixed inertia relief loads You can specify that the inertia relief loads should be held fixed in magnitude and direction at the values calculated at the end of the previous step. Input File Usage: Abaqus/CAE Usage: *INERTIA RELIEF, FIXED Load module: Create Load: choose Mechanical for the Category and Inertia relief for the Types for Selected Step: Method: Fix at current loading Removing inertia relief loads You can specify that the inertia relief loads that were applied in the previous general analysis step should be removed in the current step. Input File Usage: Abaqus/CAE Usage: *INERTIA RELIEF, REMOVE Load module: Load Manager: Deactivate Predefined fields User-defined field variables can be specified in the same way as in static and dynamic analyses without inertia relief loads. See “Predefined fields,” Section 33.6.1. Material options Any of the mechanical constitutive models that are available in Abaqus/Standard for use in static, dynamic, or buckling analyses can be used with inertia relief . Since inertia relief loading is calculated using the inertia properties of the model, the density must be specified to define the model’s inertia properties. Elements Most of the stress/displacement elements that are available in Abaqus/Standard for use in static, dynamic, and buckling analyses (including mass and rotary inertia elements and user elements) can be used. A warning will be issued when the model contains elements that do not have associated mass or inertia (for example, hydrostatic fluid elements and pore pressure elements). An error will be issued if the model contains elements that do not allow finite boundaries (for example, infinite elements and elastic element foundations). Although five degree of freedom shell elements can be used in a step with inertia relief loads, they may cause convergence difficulties if the model has no boundary conditions or insufficient boundary conditions. To improve convergence, these elements should be replaced with other conventional shell elements. In the case of a substructure you must generate a reduced mass matrix for the substructure . The reduced mass matrix is included in the global mass matrix of the entire model to compute rigid body accelerations and inertia relief loads. Inertia relief can be used only with substructures in a geometrically linear analysis. An error message is issued if inertia relief is used with substructures in a geometrically nonlinear analysis. Output In addition to the usual output variables available in Abaqus/Standard , the following variables are provided specifically for inertia relief: Variables for the entire model: IRX IRXn IRA IRAn IRARn IRF IRFn IRMn IRRI IRRIij IRMASS ). Current coordinates of the reference point. Coordinate n of the reference point ( Equivalent rigid body acceleration components. Component n of the equivalent rigid body acceleration ( Component n of the equivalent rigid body angular acceleration with respect to the reference point ( Inertia relief load corresponding to the equivalent rigid body acceleration. Component n of the inertia relief load corresponding to the equivalent rigid body acceleration ( Component n of the inertia relief moment corresponding to the equivalent rigid body angular acceleration with respect to the reference point ( Rotary inertia about the reference point. ). ). ). ). -component of the rotary inertia about the reference point ( ). Whole model mass. For most cases inertia relief loads correspond to the product of “rigid body inertia” and the equivalent rigid body acceleration vector. However, when only a few rigid body directions are chosen as free directions for inertia relief, inertia relief loads are computed in all rigid body directions for output purposes, but equivalent rigid body accelerations are computed in only the free directions with the equivalent rigid body angular accelerations computed from the diagonal entries of the “rigid body inertia.” Limitations You need to be aware of limitations that may be encountered in analyses with inertia relief loads. Internal boundary conditions and convergence in geometrically linear and nonlinear analysis In a model containing internal boundary conditions that generate unbalanced internal forces or moments, such as is possible from certain elements (for example, SPRING1, DASHPOT1, SPRING2, DASHPOT2, or GAPUNI elements) or kinematic constraints (for example, coupling constraints, linear constraint equations, multi-point constraints, or surface-based tie constraints), inertia relief loads will If the model contains sufficient boundary conditions, not balance these internal forces or moments. these internal forces or moments will appear as nonzero reaction forces or moments. If the model does not contain sufficient boundary conditions, these internal forces or moments will appear as unconverged residual fluxes in the message file for geometrically linear as well as nonlinear analyses. The model should be treated as having internal boundary conditions, with the unconverged residuals representing the reaction forces or moments needed to impose the internal boundary conditions. Ideally, the internal boundary conditions should be removed or sufficient boundary conditions should be added to the model. Unconnected regions and analyses with contact Inertia relief is not supported for models consisting of multiple unconnected regions, even if contact is defined between them. An exception is when tied contact is defined between the regions. In this case it is the user’s responsibility to ensure that different parts are tied in such a way that no rigid body motion is possible between them. In addition, models involving contact with inertia relief loads may show poor convergence or fail to converge in cases when the surfaces are not in contact or when contact stabilization is used. Mass and stiffness defined using matrices Mass and stiffness cannot be defined using matrices in analyses with inertia relief loads. Input file template *HEADING … *DENSITY Data line to specify material density *BOUNDARY Data lines to specify zero-valued boundary conditions ** *STEP (, NLGEOM) (, PERTURBATION) Use the NLGEOM parameter to include nonlinear geometric effects; it will remain active in all subsequent steps. *STATIC (or *DYNAMIC) … *CLOAD and/or *DLOAD Data lines to specify loads *INERTIA RELIEF, ORIENTATION=orientation_name Data lines to specify global (or local, if the ORIENTATION parameter is used) degrees of freedom that define free directions and to provide coordinates of a reference point *END STEP ** *STEP *STATIC(or *DYNAMIC) … *INERTIA RELIEF, FIXED or REMOVE Include the FIXED parameter to keep inertia relief loads fixed at their current values from the beginning of the step; include the REMOVE parameter to remove inertia relief loads from the beginning of the step. *END STEP 11.2 Mesh modification or replacement • “Element and contact pair removal and reactivation,” Section 11.2.1 11.2.1 ELEMENT AND CONTACT PAIR REMOVAL AND REACTIVATION Products: Abaqus/Standard Abaqus/CAE References • “Removing and reactivating contact pairs” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1 • *MODEL CHANGE • “Defining a model change interaction,” Section 15.13.13 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Element and contact pair removal/reactivation: • can be used to simulate removal of part of the model, either temporarily or for the remainder of the analysis; • allows reactivation of elements strain-free or with strain; • can be used to save computational time when a contact pair is not needed; • can be used only in general analysis steps; and • can be used in a restart analysis only if it was used or activated in the original analysis. Removing elements You can remove specified elements from the model in a general analysis step. Just prior to the removal step, Abaqus/Standard stores the forces/fluxes that the region to be removed is exerting on the remaining part of the model at the nodes on the boundary between them. These forces are ramped down to zero during the removal step; therefore, the effect of the removed region on the rest of the model is completely absent only at the end of the removal step. The forces are ramped down gradually to ensure that element removal has a smooth effect on the model. No further element calculations are performed for elements being removed, starting from the beginning of the step in which they are removed. The removed elements remain inactive in subsequent steps unless you reactivate them as described below. Input File Usage: Use the following option to remove elements from the model: Abaqus/CAE Usage: *MODEL CHANGE, TYPE=ELEMENT, REMOVE Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Deactivated in this step Removing elements in transient procedures Care must be taken in removing elements in transient procedures. The nodal flux that the removed elements apply at the boundary with the rest of the model is ramped down over the step. In transient heat transfer, fully coupled temperature-displacement, or fully coupled thermal-electrical-structural analysis if the fluxes are high and the step is long, this ramping down may have the effect of cooling down or heating up the rest of the body. In dynamic analysis if the forces are high and the step is long, kinetic energy can be imparted to the remaining portion of the model. This problem can be avoided by removing the elements in a very short transient step prior to the rest of the analysis. This step can be done in a single increment. Reactivating stress/displacement elements types of reactivation are provided for stress/displacement elements (including Two distinct substructures): strain-free reactivation and reactivation with strain. Strain-free reactivation resets the initial configuration; reactivation with strain does not. Although elements cannot be created within an analysis, a similar effect can be achieved by creating elements in the model definition, removing them in the first step, and subsequently reactivating them. Strain-free reactivation When stress/displacement elements are reactivated in a strain-free state, they become fully active immediately at the moment of reactivation (the start of the step in which they are reactivated). They are reset to an “annealed” state (zero stress, strain, plastic strain, etc.) in the configuration in which they lie at the start of the reactivation step. This configuration depends on whether a small- or large-displacement analysis is being conducted. Alternatively, reactivation in a nonvirgin state can be specified, as described below. Since these elements are reactivated in a virgin state (i.e., with zero stress), they exert zero nodal forces on the rest of the model. This result allows reactivation to be done immediately, without an adverse effect on the smoothness of the solution. After reactivation the strains and the deformation gradients are based on the displacements subsequent to the moment of reactivation, rather than on their total displacements. Thus, the current configuration at the start of the reactivation step is the new initial configuration for the element. This kind of reactivation usually is used to model the creation of an undeformed and unstrained region of the model that is sharing a boundary with another, possibly stressed, deformed region. For example, in tunnel excavation an unstressed tunnel liner is added to line the walls of an already deformed tunnel . Input File Usage: Use the following option to reactivate elements in a strain-free state: Abaqus/CAE Usage: *MODEL CHANGE, ADD=STRAIN FREE (default) Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Reactivated in this step Small-displacement analysis In small-displacement analysis the displacements at reactivation are considered to be small; therefore, volume, mass, initial length, and orientation directions do not change. Large-displacement analysis In large-displacement analysis the new configuration can be significantly different from the original configuration specified in the model definition. The change in configuration may result from large deformation or rigid body motion. For the nodes of the reactivated elements to be in the correct position upon reactivation, these nodes must be shared by elements that are not removed. Otherwise, the nodes of the removed elements remain at the location occupied at the time of removal. For cases where an enclosed region of material is reactivated, the shared-node restriction may require that a duplicate set of elements whose material properties do not influence the stress solution be defined on top of the removed elements. These duplicate elements provide a means of tracking the position of the nodes of the removed elements. Upon reactivation an element can have a significantly different volume or mass, so the mass matrix is reformed for the element. Any local orientations applicable to the element are redefined on the new configuration. For shell and membrane elements, however, the thickness of the reactivated elements is the thickness as specified at the start of the analysis by the element’s section definition, a nodal thickness definition (“Nodal thicknesses,” Section 2.1.3), or an import definition (“Transferring results between Abaqus analyses: overview,” Section 9.2.1). The current normals on structural elements at the moment of reactivation become new initial normals for that element. The current normal is the element’s original normal (as specified in the model definition) rotated by the nodal rotation at the moment of reactivation. This scheme preserves the angle between the normals of reactivated elements and those of the elements with which they share nodes. (Usually, this angle should be zero and the normals should be identical, such as when a strain-free layer is added to an already deformed shell or beam. This can be achieved by ensuring that the normals are identical in the model definition.) If the reactivated structural elements share nodes with only non-structural elements (elements that do not provide stiffness to rotational degrees of freedom), duplicate structural elements are required so that the rotational degrees of freedom at the shared nodes will follow the deformation and rigid body motion before reactivation. In a large-displacement analysis an element that is being reactivated strain free fits into whatever configuration is given by its nodes at the moment of reactivation. You must ensure that this configuration is meaningful and is not severely distorted. Abaqus/Standard will apply geometry checks on the reactivated elements; these checks are the same as the checks that are done in the analysis input file processor. Warnings are printed in the message file if the elements seem inappropriately distorted; and error messages are given if the distortion is severe, in which case the analysis will be stopped. If a geometry check on an element produces a warning or an error message, its current coordinates—and normals if applicable—are printed to the message file for your inspection. The current coordinates can be printed for all elements being reactivated by requesting detailed printout for element removal/reactivation, as explained in “The Abaqus/Standard message file” in “Output,” Section 4.1.1. Reactivating axisymmetric elements Abaqus/Standard will not stop the analysis if an axisymmetric element has a very small negative radial coordinate at reactivation (if the magnitude of the radial coordinate is less than 10−4 times the average element length). In this case a warning is printed, and a radial coordinate of zero is assumed. If the radial coordinate is negative and larger than 10−4 times the average element length in magnitude, the analysis will stop. For axisymmetric-asymmetric elements (SAXA and CAXA) the displacements at reactivation are considered small even in large-displacement analysis because these elements require an axisymmetric original configuration, but the configuration given by the nodes of these elements at reactivation would not, in general, be axisymmetric. Therefore, the original configuration is assumed not to change for these elements. Reactivating coupled temperature-displacement and coupled thermal-electrical-structural elements In a fully coupled temperature-displacement analysis and a fully coupled thermal-electrical-structural analysis, continuum elements attain their full mechanical stiffness immediately upon strain-free reactivation; however, to ensure smoothness of the solution, thermal conductivity is ramped up from zero over the step. Reactivating spring elements and substructures If spring elements or substructures are reactivated “without strain,” the configuration at the moment of reactivation represents the zero-displacement state of the element; the forces in the spring or substructures are based on relative displacements subsequent to the moment of reactivation. Reactivation with strain Elements reactivated with strain start in an annealed state unless reactivation in a nonvirgin state is specified, as described below. The following scheme is implemented for the elements during the reactivation step: Let represent the displacements of the nodes of this element, which are the displacements as shared by the rest of the model or as specified by boundary conditions. In general, these displacements can vary with time over the reactivation step. At any time in the reactivation step Abaqus/Standard enforces displacements, , for the element: where is a parameter that ramps linearly from 0 to 1 during the step. Thus, during the step the displacements felt by the reactivated elements ramp up to their actual values. To produce a consistent stiffness matrix, the element stiffness is also multiplied by therefore, the rest of the model experiences the reactivated elements as though their stiffnesses were ramped up during the step. ; This ramping up of displacements instead of direct ramping up of element forces ensures that the strain in the element ramps up from zero to the strain given by the displacement of its nodes. This gradual ramping up of strains is desirable so that the response of history-dependent materials can be integrated gradually. Subsequent to the end of the reactivation step, the strains in reactivated elements correspond to the displacements of their nodes from their initial configuration, rather than to their displacements since the moment of reactivation. This is appropriate, for example, in the refueling of a nuclear reactor, where the new fuel assembly must conform to the distortion of its old neighbors. This reactivation scheme does not work for the rotations of shell elements that have five degrees of freedom per node because a total rotation is not stored at those nodes. Consequently, reactivation with strain is not allowed for these elements. If an element is reactivated with strain after having been previously reactivated strain free, the strains are based on the displacements from the configuration in which the element was reactivated strain free (because this defined the new initial configuration for the element). In this case the in the formula above should be interpreted as the displacement of the node relative to the position in which the element was reactivated strain free. Input File Usage: Use the following option to reactivate elements with strain: Abaqus/CAE Usage: *MODEL CHANGE, ADD=WITH STRAIN Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Reactivated in this step; toggle on Reactivated elements with strain (when applicable) Reactivating elements with rebar Rebars are reactivated strain free or with strain exactly like the element in which they are defined. The annealing that takes place upon reactivation is also applied to rebars in the model. Reactivation of rebars can also be done in a nonvirgin state. Reactivating other element types During reactivation of all element types other than stress/displacement elements, substructures, and contact elements, the nodal forces caused by stress in the element and by distributed loads are scaled by a value that ramps from zero to one during the reactivation step. (The nodal fluxes are scaled similarly for heat transfer elements.) In effect this scaling ramps the element stiffness up from zero during the step; for elements with mass or damping this scaling also ramps up the mass or damping during the step. During the reactivation step the thermal conductivity of heat transfer elements and the permeability of pore pressure elements are ramped up from zero over the step. User-defined elements can be removed and reactivated. User subroutine UEL is not called in steps in which the element is being removed or has already been removed. Input File Usage: Abaqus/CAE Usage: *MODEL CHANGE, ADD Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Reactivated in this step Removing and reactivating contact pairs You can remove specified slave and master surfaces from the model in a general analysis step. Contact pair removal and reactivation is explained in “Removing and reactivating contact pairs” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1. Input File Usage: Abaqus/CAE Usage: *MODEL CHANGE, TYPE=CONTACT PAIR, REMOVE or ADD Use the following option to remove contact pairs: Interaction module: Create Interaction: Surface-to-surface contact (Standard) or Self-contact (Standard): toggle off Active in this step Use the following option to reactivate contact pairs: Interaction module: Create Interaction: Surface-to-surface contact (Standard) or Self-contact (Standard): toggle on Active in this step Removing and reactivating contact elements Contact elements are removed and reactivated by Abaqus/Standard in the same way as contact pairs, as described in “Removing and reactivating contact pairs” in “Defining contact pairs in Abaqus/Standard,” Section 35.3.1. Input File Usage: Abaqus/CAE Usage: *MODEL CHANGE, TYPE=ELEMENT, REMOVE or ADD Use the following option to remove contact elements: Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Deactivated in this step Use the following option to reactivate contact elements: Interaction module: Create Interaction: Model Change: Definition: Region, Activation state of region elements: Reactivated in this step Modeling issues In some cases element removal/reactivation may cause numerical problems. The following guidelines can be used to reduce the chance of difficulty: • If elements are removed in a static stress analysis and this removal leaves a region of the model with an unconstrained rigid body mode, solver problems will occur and the analysis most likely will fail to converge. Therefore, ensure that the remainder of the model is constrained sufficiently. • If elements that are connected to a contact pair are removed, the contact pair should also be removed to avoid solver problems. • If all elements attached to a node constrained with a multi-point constraint or a linear constraint equation are being removed, this node should be the dependent node of the multi-point constraint or linear constraint equation. In some cases element removal may cause Abaqus/Standard to report extra unconnected regions in the message file. These messages can be safely ignored. Removing or reactivating elements and contact pairs in a restart analysis Elements or contact pairs can be removed or reactivated in a restart analysis (“Restarting an analysis,” Section 9.1.1) only if elements or contact pairs were removed or reactivated in the original analysis. In situations where it is expected that the addition or removal of elements or contact pairs will be required in a restart analysis, but there is no such need in the original analysis, you must activate element or contact pair removal/reactivation in the original analysis. Activating this capability does not add or remove any elements or contact pairs; it only prepares Abaqus/Standard to allow for these changes in a subsequent restart analysis. Input File Usage: the Use following removal/reactivation: option to activate element or contact pair Abaqus/CAE Usage: *MODEL CHANGE, ACTIVATE Interaction module: Create Interaction: Model Change: Definition: Restart Procedures Elements or contact pairs cannot be removed or reactivated in a linear perturbation step or in a static Riks step . For elements to be absent in such steps, they must have been inactive at the end of the previous general analysis (nonperturbation) step. Initial conditions When elements are added back into the model, they are usually assumed to be “annealed”; that is, they have zero plastic strain, creep strain, etc. and zero stress at the start of the step in which they are reactivated. It is possible to reactivate an element so that it starts with a nonzero stress, equivalent plastic strain, and, if relevant, backstress (in a nonvirgin state). Reactivation in a nonvirgin state To reactivate elements with nonzero stress, define initial stress conditions to specify the required stress in the model definition. Then the elements must be removed in the first step of the analysis. When reactivated, they will have the initial stress specified. The reactivation is done immediately, so the initial stress (which is applied in full during the first increment) must be self-equilibrating to avoid convergence issues. If the elements were not removed in the first step, if they were removed again after the first step, or if initial conditions were not specified for them, they will have zero stresses when reactivated. In a similar manner a material can be reactivated with a nonzero initial equivalent plastic strain and, if relevant, backstress. When elements are reactivated, any applied initial stress is not displayed in the zero increment frame. Input File Usage: Abaqus/CAE Usage: Use the following option to specify initial stress conditions: *INITIAL CONDITIONS, TYPE=STRESS Use the following option to specify initial equivalent plastic strain and backstress: *INITIAL CONDITIONS, TYPE=HARDENING Use the following options to specify the initial stress conditions: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Stress for the Types for Selected Step Use the following options to specify the initial equivalent plastic strain and backstress: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step Boundary conditions The nodal variables of removed elements are not changed when the elements are removed. You can reset these variables by defining a boundary condition while the elements are inactive . Loads Distributed and concentrated loads that are applied in an area where elements are removed or reactivated may need to be modified. Distributed loads Any distributed loads, fluxes, flows, and foundations specified for inactive elements are also inactive. However, unless you explicitly remove them, records of these loads are still kept and are listed in the data (.dat) file as though the elements were still present. Continuation of loads across steps is not affected by removal; on element reactivation unremoved distributed loads are also reactivated. By default, if a distributed load is applied to an element that is being reactivated in a step, the distributed load magnitude is scaled up linearly from zero to its end-of-step value during the step. If such a load is applied with an amplitude reference, the magnitude value given by the amplitude reference is scaled again by a value that ramps from zero to one throughout the step. This scheme ensures that reactivation has a smooth effect on the solution, even in cases where a distributed load with an amplitude reference on a reactivated element is carried over from a previous step. Concentrated loads Concentrated loads or fluxes are not removed when the surrounding elements are removed; therefore, you must ensure that any concentrated loads or fluxes that are carried solely by removed elements are also removed. Otherwise, a solver problem will occur during the removal step (a force is applied to a degree of freedom with zero stiffness). Concentrated loads or fluxes should be ramped up when they are reintroduced along with reactivated elements. Predefined fields The nodal variables of removed elements are not changed directly when the elements are removed. You can reset these variables by defining temperature or other predefined field variables while the elements are inactive . For example, elements that are removed in a stress/displacement analysis can be reintroduced at a different temperature by setting the temperatures at the nodes on these elements to the desired value while the elements are inactive due to removal. Temperatures The temperatures at the start of the reactivation step become the initial temperatures for reactivated elements; thermal strains (and, thus, also the thermal stresses) are based on the temperature change subsequent to the instant of reactivation . Material options On annealing, compaction-related quantities—such as the yield stress in hydrostatic compression, , in crushable foam plasticity (“Crushable foam plasticity models,” Section 23.3.5); the yield stress in hydrostatic compression, , in cap plasticity (“Modified Drucker-Prager/Cap model,” Section 23.3.2); and the void volume fraction, f, in porous metal plasticity (“Porous metal plasticity,” Section 23.2.9)—are reset to the values they had at the start of the analysis. For porous materials the porosity, n, is reset to its initial value and the saturation, s, retains its value from the instant of removal . Elements with a user-defined material type can be removed and reactivated; user subroutines UMAT and UMATHT are not called while the elements are inactive. On reactivation the stresses and strains in user subroutine UMAT are set to zero, and conductivity and heat fluxes defined in user subroutine UMATHT are ramped up from zero during the reactivation step. Solution-dependent state variables must be reset in user subroutine UMAT, UMATHT, or SDVINI, which will be called on reactivation. Elements Removal is not currently supported for rigid, cohesive, gasket, and piezoelectric elements. All other element types in Abaqus/Standard can be removed and reactivated. See “Choosing the appropriate element for an analysis type,” Section 27.1.3. Output Output is not available for elements or contact surfaces that have been removed. Inactive elements and contact surfaces are visible in Abaqus/CAE. Input file template *HEADING … *STEP *STATIC … ** Remove all elements in element set SIDE *MODEL CHANGE, REMOVE SIDE, ** Remove contact pair (SLAVE1, MASTER1) *MODEL CHANGE, TYPE=CONTACT PAIR, REMOVE SLAVE1, MASTER1 … *END STEP ** *STEP *STATIC … ** Reactivate elements in element set SIDE *MODEL CHANGE, ADD=STRAIN FREE SIDE, ** Reactivate contact pair (SLAVE1, MASTER1) *MODEL CHANGE, TYPE=CONTACT PAIR, ADD SLAVE1, MASTER1 … *END STEP 11.3 Geometric imperfections • “Introducing a geometric imperfection into a model,” Section 11.3.1 INTRODUCING A GEOMETRIC IMPERFECTION INTO A MODEL GEOMETRIC IMPERFECTIONS Products: Abaqus/Standard Abaqus/Explicit References • “Unstable collapse and postbuckling analysis,” Section 6.2.4 • *IMPERFECTION Overview A geometric imperfection pattern: • is generally introduced in a model for a postbuckling load-displacement analysis; • can be defined as a linear superposition of buckling eigenmodes obtained from a previous eigenvalue buckling prediction or eigenfrequency extraction analysis performed with Abaqus/Standard; • can be based on the solution obtained from a previous static analysis performed with Abaqus/Standard; or • can be specified directly. General postbuckling analysis In Abaqus/Standard the Riks method (“Unstable collapse and postbuckling analysis,” Section 6.2.4) can be used to solve postbuckling problems, both with stable and unstable postbuckling behavior. However, the exact postbuckling problem often cannot be analyzed directly due to the discontinuous response (bifurcation) at the point of buckling. To analyze a postbuckling problem, you must turn it into a problem with continuous response instead of bifurcation, which can be accomplished by introducing a geometric imperfection pattern in the “perfect” geometry so that there is some response in the buckling mode before the critical load is reached. Introducing geometric imperfections Imperfections are usually introduced by perturbations in the geometry. Abaqus offers three ways to define an imperfection: as a linear superposition of buckling eigenmodes, from the displacements of a static analysis, or by specifying the node number and imperfection values directly. Only the translational degrees of freedom are modified. Abaqus will then calculate the normals using the usual algorithm based on the perturbed coordinates. Unless the precise shape of an imperfection is known, an imperfection consisting of multiple superimposed buckling modes can be introduced (“Eigenvalue buckling prediction,” Section 6.2.3). The usual approach involves two analysis runs with the same model definition, using Abaqus/Standard to establish the probable collapse modes and either Abaqus/Standard or Abaqus/Explicit to perform the postbuckling analysis: 1. In the first analysis run perform an eigenvalue buckling analysis with Abaqus/Standard on the “perfect” structure to establish probable collapse modes and to verify that the mesh discretizes those modes accurately. Write the eigenmodes in the default global system to the results file as nodal data (“Output to the data and results files,” Section 4.1.2). 2. In the second analysis run use Abaqus/Standard or Abaqus/Explicit to introduce an imperfection in the geometry by adding these buckling modes to the “perfect” geometry. The lowest buckling modes are frequently assumed to provide the most critical imperfections, so usually these are scaled and added to the perfect geometry to create the perturbed mesh. The imperfection thus has the form where is the mode shape and is the associated scale factor. You must choose the scale factors of the various modes; usually (if the structure is not imperfection sensitive) the lowest buckling mode should have the largest factor. The magnitudes of the perturbations used are typically a few percent of a relative structural dimension such as a beam cross-section or shell thickness. 3. Use either Abaqus/Standard or Abaqus/Explicit to perform the postbuckling analysis. • In Abaqus/Standard perform a geometrically nonlinear load-displacement analysis of the structure containing the imperfection using the Riks method. In this way the Riks method can be used to perform postbuckling analyses of “stiff” structures that show linear behavior prior to buckling, if perfect. By performing a load-displacement analysis, other important nonlinear effects, such as material inelasticity or contact, can be included. • In Abaqus/Explicit perform a postbuckling analysis on the perturbed structure. Abaqus imports imperfection data through the user node labels. Abaqus does not check model compatibility between both analysis runs. Node set definitions in the original model and the model with the imperfection may be different. Care must be taken for models in which Abaqus generates additional nodes (for example, the nodes generated for contact surfaces on 20-node brick elements). In such cases you have to ensure that the models for both analysis runs are identical and that the nodal information for the generated nodes is written to the results file. If the model is defined in terms of an assembly of part instances, the part (.prt) file from the original analysis is required to read the eigenmodes from the results file. Both the original model and the subsequent model must be defined consistently in terms of an assembly of part instances. Defining an imperfection based on eigenmode data To define an imperfection based on the superposition of weighted mode shapes, specify the results file and step from a previous eigenfrequency extraction or eigenvalue buckling prediction analysis. Optionally, you can import eigenmode data for a specified node set. Input File Usage: *IMPERFECTION, FILE=results_file, STEP=step, NSET=name Defining an imperfection based on static analysis data To define an imperfection based on the deformed geometry of a previous static analysis (“Unstable collapse and postbuckling analysis,” Section 6.2.4), specify the results file and step (and, optionally, the increment number) from a previous static analysis. (If the increment number is not specified, Abaqus will read data from the last increment available for the specified step in the results file.) Optionally, you can import modal data for a specified node set. Input File Usage: *IMPERFECTION, FILE=results_file, STEP=step, INC=inc, NSET=name Defining an imperfection directly You can specify the imperfection directly as a table of node numbers and coordinate perturbations in the global coordinate system or, optionally, in a cylindrical or spherical coordinate system. Alternatively, you can read the imperfection data from a separate input file. Input File Usage: *IMPERFECTION, SYSTEM=name, INPUT=input file If no input file is specified, Abaqus assumes that the data follow the option. Imperfection sensitivity The response of some structures depends strongly on the imperfections in the original geometry, particularly if the buckling modes interact after buckling occurs. Hence, imperfections based on a single buckling mode tend to yield nonconservative results. By adjusting the magnitude of the scaling factors of the various buckling modes, the imperfection sensitivity of the structure can be assessed. Normally, a number of analyses should be conducted to investigate the sensitivity of a structure to imperfections. Structures with many closely spaced eigenmodes tend to be imperfection sensitive, and imperfections with shapes corresponding to the eigenmode for the lowest eigenvalue may not give the worst case. The imperfect structure will be easier to analyze if the imperfection is large. If the imperfection is small, the deformation will be quite small (relative to the imperfection) below the critical load. The response will grow quickly near the critical load, introducing a rapid change in behavior. On the other hand, if the imperfection is large, the postbuckling response will grow steadily before the critical load is reached. In this case the transition into postbuckled behavior will be smooth and relatively easy to analyze. Input file template The following example illustrates a postbuckling analysis of a structure with an imperfection defined by a linear superposition of the buckling eigenmodes and involves two analysis runs with the same model definition. The initial analysis run performs an eigenvalue buckling analysis with Abaqus/Standard to establish the probable collapse modes and writes them to the results file. *HEADING Initial analysis run to write the buckling modes to the results file *NODE Data lines to define initial “perfect” geometry … ** *STEP *BUCKLE Data lines to define the number of buckling eigenmodes *CLOAD and/or *DLOAD and/or *DSLOAD and/or *TEMPERATURE Data lines to specify the reference load, *NODE FILE, GLOBAL=YES, LAST MODE=n *END STEP The second analysis run introduces the imperfection and performs a postbuckling analysis employing the modified Riks method in Abaqus/Standard. *HEADING Second analysis run to define the imperfection and perform the postbuckling analysis *NODE Data lines to define initial “perfect” geometry … *IMPERFECTION, FILE=results_file, STEP=step Data lines specifying the mode number and its associated scale factor … ** *STEP, NLGEOM *STATIC, RIKS Data line to define incrementation and stopping criteria *CLOAD and/or *DLOAD and/or *DSLOAD and/or *TEMPERATURE Data lines to specify reference loading, *END STEP An alternative second analysis run introduces the imperfection and performs a postbuckling analysis with Abaqus/Explicit. *HEADING Second analysis run to define the imperfection and perform the postbuckling analysis *NODE Data lines to define initial “perfect” geometry … *IMPERFECTION, FILE=results_file, STEP=step Data lines specifying the mode number and its associated scale factor … ** *STEP *DYNAMIC, EXPLICIT Data line to define the time period of the step. *CLOAD and/or *DLOAD and/or *DSLOAD and/or *TEMPERATURE *END STEP 11.4 Fracture mechanics • “Fracture mechanics: overview,” Section 11.4.1 • “Contour integral evaluation,” Section 11.4.2 • “Crack propagation analysis,” Section 11.4.3 11.4.1 FRACTURE MECHANICS: OVERVIEW Abaqus/Standard provides the following methods for performing fracture mechanics studies: • Onset of cracking: The onset of cracking can be studied in quasi-static problems by using contour integrals (“Contour integral evaluation,” Section 11.4.2). The J-integral, the -integral (for creep), the stress intensity factors for both homogeneous materials and interfacial cracks, the crack propagation direction, and the T-stress are calculated by Abaqus/Standard. Contour integrals can be used in two- or three-dimensional problems. In these types of problems focused meshes are generally required and the propagation of a crack is not studied. • Crack propagation: The crack propagation capability allows quasi-static, including low-cycle fatigue, crack growth along predefined paths to be studied (“Crack propagation analysis,” Section 11.4.3). Cracks debond along user-defined surfaces. Several crack propagation criteria are available, and multiple cracks can be included in the analysis. Contour integrals can be requested in crack propagation problems. • Line spring elements: Part-through cracks in shells can be modeled inexpensively by using line spring elements in a static procedure, as explained in “Line spring elements for modeling part-through cracks in shells,” Section 32.9.1. • Extended finite element method (XFEM): XFEM models a crack as an enriched feature by adding degrees of freedom in elements with special displacement functions (“Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1). XFEM does not require the mesh to match the geometry of the discontinuities. It can be used to simulate initiation and propagation of a discrete crack along an arbitrary, solution-dependent path without the requirement of remeshing. XFEM can also be used to perform contour integral evaluation without the need to refine the mesh around the crack tip. 11.4.2 CONTOUR INTEGRAL EVALUATION Products: Abaqus/Standard Abaqus/CAE References • “Fracture mechanics: overview,” Section 11.4.1 • *CONTOUR INTEGRAL • “Using contour integrals to model fracture mechanics,” Section 31.2 of the Abaqus/CAE User’s Manual Overview Abaqus/Standard offers the evaluation of several parameters for fracture mechanics studies based on either the conventional finite element method or the extended finite element method (XFEM, see “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1): • the J-integral, which is widely accepted as a quasi-static fracture mechanics parameter for linear material response and, with limitations, for nonlinear material response; • the -integral, which has an equivalent role to the J-integral in the context of time-dependent creep behavior (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) in a quasi-static step (“Quasi-static analysis,” Section 6.2.5); • the stress intensity factors, which are used in linear elastic fracture mechanics to measure the strength of the local crack-tip fields; • the crack propagation direction—i.e., the angle at which a preexisting crack will propagate; and • the T-stress, which represents a stress parallel to the crack faces and is used as an indicator of the extent to which parameters like the J-integral are useful characterizations of the deformation field around the crack. Contour integrals: • are output quantities—they do not affect the results; • can be requested only in general analysis steps; • can be used only with two-dimensional quadrilateral elements or three-dimensional brick elements when used with the conventional finite element method; • can be evaluated without requiring a detailed refined mesh around the crack tips when used with XFEM; and • are currently available only for first-order or second-order tetrahedron and first-order brick elements with isotropic elastic material when used with XFEM. Contour integral evaluation Abaqus/Standard offers two different ways to evaluate the contour integral. The first approach is based on the conventional finite element method, which typically requires you to conform the mesh to the cracked geometry, to explicitly define the crack front, and to specify the virtual crack extension direction. Detailed focused meshes are generally required, and obtaining accurate contour integral results for a crack in a three-dimensional curved surface can be quite cumbersome. The extended finite element method (XFEM) alleviates these shortcomings. XFEM does not require the mesh to match the cracked geometry. The presence of a crack is ensured by the special enriched functions in conjunction with additional degrees of freedom. This approach also removes the requirement for explicitly defining the crack front or specifying the virtual crack extension direction when evaluating the contour integral. The data required for the contour integral are determined automatically based on the level set signed distance functions at the nodes in an element . Several contour integral evaluations are possible at each location along a crack. In a finite element model each evaluation can be thought of as the virtual motion of a block of material surrounding the crack tip (in two dimensions) or surrounding each node along the crack line (in three dimensions). Each block is defined by contours, where each contour is a ring of elements completely surrounding the crack tip or the nodes along the crack line from one crack face to the opposite crack face. These rings of elements are defined recursively to surround all previous contours. Abaqus/Standard automatically finds the elements that form each ring from the regions defined as the crack tip or crack line. Each contour provides an evaluation of the contour integral. The possible number of evaluations is the number of such rings of elements. You must specify the number of contours to be used in calculating contour integrals. In addition, you must specify the type of contour integral to be calculated, as described below. By default, Abaqus/Standard calculates the J-integral. You can assign a name to a crack that is used to identify the contour integral values in the data file and in the output database file. The name is also used by Abaqus/CAE to request contour integral output. If you are using the conventional finite element method and do not specify a crack name, by default Abaqus/Standard generates crack numbers that follow the order in which the cracks are defined. If you are using XFEM, you must set the crack name equal to the name assigned to the enriched feature. Input File Usage: Use the follow option to evaluate the contour integral with the conventional finite element method: *CONTOUR INTEGRAL, CRACK NAME=crack name, CONTOURS=n, TYPE=integral_type Abaqus/CAE Usage: Use the following option to evaluate the contour integral with XFEM: *CONTOUR INTEGRAL, CRACK NAME=crack name, XFEM, CONTOURS=n, TYPE=integral_type Interaction module: Special→Crack→Create: Name: crack name, Type: Contour integral or XFEM Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: integral_type The domain integral method Using the divergence theorem, the contour integral can be expanded into an area integral in two dimensions or a volume integral in three dimensions, over a finite domain surrounding the crack. This domain integral method is used to evaluate contour integrals in Abaqus/Standard. The method is quite robust in the sense that accurate contour integral estimates are usually obtained even with quite coarse meshes. The method is robust because the integral is taken over a domain of elements surrounding the crack and because errors in local solution parameters have less effect on the evaluated quantities such as J, , the stress intensity factors, and the T-stress. Requesting multiple contour integrals Contour integrals at several different crack tips in two dimensions or along several different crack lines in three dimensions can be evaluated at any time by repeating the contour integral request as often as needed in the step definition. When you are using the conventional finite element method, you must specify the crack front and the direction of virtual crack extension (or the normal to the crack plane if this normal is constant) for each crack tip or crack line, as described below. When you are using XFEM, you do not need to specify the crack front or the virtual crack extension direction because they will be determined by Abaqus/Standard. However, you must set each crack name equal to the corresponding enriched feature, with each enriched feature consisting of only one crack. In addition, regardless of whether you are using either the conventional finite element method or XFEM, you must specify the number of contours to be calculated for each integral. The J -integral The J-integral is usually used in rate-independent quasi-static fracture analysis to characterize the energy release associated with crack growth. It can be related to the stress intensity factor if the material response is linear. The J-integral is defined in terms of the energy release rate associated with crack advance. For a in the plane of a three-dimensional fracture, the energy release rate is given virtual crack advance by where line, is a surface element along a vanishing small tubular surface enclosing the crack tip or crack is given by is the local direction of virtual crack extension. is the outward normal to , and For elastic material behavior W is the elastic strain energy; for elastic-plastic or elasto-viscoplastic material behavior W is defined as the elastic strain energy density plus the plastic dissipation, thus representing the strain energy in an “equivalent elastic material.” Therefore, the J-integral calculated is suitable only for monotonic loading of elastic-plastic materials. Input File Usage: Abaqus/CAE Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=J Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: J-integral Domain dependence The J-integral should be independent of the domain used provided that the crack faces are parallel to each other, but J-integral estimates from different rings may vary because of the approximate nature of the finite element solution. Strong variation in these estimates, commonly called domain dependence or contour dependence, typically indicates an error in the contour integral definition. Gradual variation in these estimates may indicate that a finer mesh is needed or, if plasticity is included, that the contour integral domain does not completely include the plastic zone. If the “equivalent elastic material” is not a good representation of the elastic-plastic material, the contour integrals will be domain independent only if they completely include the plastic zone. Since it is not always possible to include the plastic zone in three dimensions, a finer mesh may be the only solution. If the first contour integral is defined by specifying the nodes at the crack tip, the first few contours may be inaccurate. To check the accuracy of these contours, you can request more contours and determine the value of the contour integral that appears approximately constant from one contour to the next. The contour integral values that are not approximately equal to this constant should be discarded. In linear elastic problems the first and second contours typically should be ignored as inaccurate. For some three-dimensional models with an open crack front, the J-integral estimates may be inaccurate from the node sets (or elements in the case with XFEM) at the crack front ends. The resolution difficulty is compounded by the skewness of the outmost layer of elements. This accuracy loss is confined only to the contour integrals at the front ends and has no effect on the accuracy of the contour integral values at the neighboring node sets (or elements in the case with XFEM) along the crack front. Including the effect of a residual stress field on J-integral evaluation A residual stress field often occurs in a structure; for example, as a result of service loads that produce plasticity, a metal forming process in the absence of an anneal treatment, thermal effects, or swelling effects. When the residual stresses are significant, the standard definition of the J-integral as described above may lead to a path-dependent value. To ensure its path independence, the J-integral evaluation must include an additional term that accounts for the residual stress field. In Abaqus/Standard the problem with a residual stress field is treated as an initial strain problem. If the total strain is written as the sum of mechanical strain, , and initial strain, ; i.e., a path-independent energy release rate in the presence of a residual stress field is given by where V is the domain volume enclosing the crack tip or crack line, W is defined as the mechanical strain energy density only, and remains constant during the entire deformation. The residual stress field can be specified by reading the stress data from a previous analysis step or by defining an initial condition . You specify the step number from which the stress data in the last available increment of the specified step will be considered as residual stresses. If the step number is set equal to zero (default), the residual stress field is defined by the initial condition definition. When XFEM is used, the residual stress field can be defined only with an initial condition definition. *CONTOUR INTEGRAL, RESIDUAL STRESS STEP=n, TYPE=J Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Step for residual stress initialization values: step, Type: J-integral Abaqus/CAE Usage: Input File Usage: The Ct -integral The Ct -integral is supported with the conventional finite element method; however, it is not supported with XFEM. The -integral can be used for time-dependent creep behavior, where it characterizes creep crack deformation under certain creep conditions, including transient crack growth. is, for example, proportional to the rate of growth of the crack-tip/crack-line creep zone for a stationary crack under small-scale creep conditions. Under steady-state creep conditions, when creep dominates throughout the specimen, -integrals should be requested only in a quasi-static step. becomes path independent and is known as . The -integral is obtained by replacing the displacements with velocities and the strain energy density with the strain energy rate density in the J-integral expansion. The strain energy rate density is defined as is not uniquely defined if multiple deformation mechanisms contribute to the strain rate. However, the creep mechanism will dominate within a zone surrounding a crack tip or crack line, so elastic and plastic contributions to are negligible. The size of that zone depends on the extent of creep relaxation: the zone is initially small but eventually encompasses the entire specimen when steady-state creep is reached. Abaqus/Standard considers only creep in the calculation of . Neglecting elastic and plastic strain rates, the strain energy density for the power law creep model with time hardening form in Abaqus/Standard is where n is the power law exponent, q is the equivalent Mises stress, and is the equivalent uniaxial strain rate. For the hyperbolic-sine law an analytical expression of is obtained by numerical integration; a five-point Gauss quadrature scheme gives reasonable accuracy in the range of realistic creep strain rates. is not available. For this law The domain integral method is used for For user-defined creep laws the strain energy rate density must be defined in user subroutine CREEP. *CONTOUR INTEGRAL, CONTOURS=n, TYPE=C Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: Ct-integral -integrals as described above for J-integrals. Abaqus/CAE Usage: Input File Usage: Domain dependence Prior to steady state -integral estimates will exhibit domain dependence, even if the finite element mesh is sufficiently refined, because of the assumption of creep dominance within the domain specified. These estimate corresponding to a contour shrunk onto the crack tip or crack line . estimates should be extrapolated to zero radius to obtain an improved Including the effect of a residual stress field on -integral evaluation An additional term is included to account for the residual stress field when calculating the as described in “Including the effect of a residual stress field on J-integral evaluation.” -integral, Input File Usage: Abaqus/CAE Usage: *CONTOUR INTEGRAL, RESIDUAL STRESS STEP=n, TYPE=C Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Step for residual stress initialization values: step, Type: Ct-integral The stress intensity factors The stress intensity factors are usually used in linear elastic fracture mechanics to characterize the local crack-tip/crack-line stress and displacement fields. They are related to the energy release rate (the J-integral) through , and , where factor matrix. For homogeneous, isotropic materials are the stress intensity factors and is called the pre-logarithmic energy is diagonal, and the above equation simplifies to where For an interfacial crack between two dissimilar isotropic materials, for plane stress and for plane strain, axisymmetry, and three dimensions. where for plane strain, axisymmetry, and three dimensions; and for plane stress. Unlike their analogues in a homogeneous material, are no longer the pure Mode I and Mode II stress intensity factors for an interfacial crack. They are simply the real and imaginary parts of a complex stress intensity factor. and Although the energy release rate is calculated directly in Abaqus/Standard, it is usually not straightforward to compute stress intensity factors from a known J-integral for mixed-mode problems. Abaqus/Standard provides an interaction integral method to compute the stress intensity factors directly for a crack under mixed-mode loading. This capability is available for linear isotropic and anisotropic materials. The theory is described in detail in “Stress intensity factor extraction,” Section 2.16.2 of the Abaqus Theory Manual. In this case the J-integrals calculated from the stress intensity factors will also be output. These J-integral values may be slightly different from those estimated by requesting the J-integral directly, due to the different algorithms used for the calculations. Input File Usage: Abaqus/CAE Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=K FACTORS Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: Stress intensity factors Domain dependence The stress intensity factors have the same domain dependence features as the J-integral. Including the effect of a residual stress field on stress intensity factor evaluation An additional term is included to account for the residual stress field when calculating the stress intensity factors, as described in “Including the effect of a residual stress field on J-integral evaluation.” Input File Usage: *CONTOUR INTEGRAL, RESIDUAL STRESS STEP=n, TYPE=K FACTORS Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Step for residual stress initialization values: step, Type: Stress intensity factors The crack propagation direction For homogeneous, isotropic elastic materials the direction of cracking initiation can be calculated using one of the following three criteria: the maximum tangential stress criterion, the maximum energy release rate criterion, or the is not taken into account in any of these criteria. criterion. The maximum tangential stress criterion Using either the condition (where r and crack tip in a plane orthogonal to the crack line), we can obtain or are polar coordinates centered at the where the crack propagation angle the crack propagation in the “straight-ahead” direction. The crack propagation angle is measured from to ; i.e., it is measured about the direction counterclockwise measured from in Figure 11.4.2–1. The crack propagation angle will be output. is measured with respect to the crack plane and , while if if represents . , or Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=K FACTORS, DIRECTION=MTS Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: Stress intensity factors, Crack initiation criterion: Maximum tangential stress The maximum energy release rate criterion This criterion postulates that a crack initially propagates in the direction that maximizes the energy release rate. The crack propagation angle will be output. Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=K FACTORS, DIRECTION=MERR Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: Stress intensity factors, Crack initiation criterion: Maximum energy release rate The KII = 0 criterion This criterion assumes that a crack initially propagates in the direction that makes . The crack propagation angle will be output. Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=K FACTORS, DIRECTION=KII0 Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: Stress intensity factors, Crack initiation criterion: K11=0 The T -stress The T-stress component represents a stress parallel to the crack faces at the crack tip. Its magnitude can alter not only the size and shape of the plastic zone but also the stress triaxiality ahead of the crack tip. It is, therefore, a useful indicator of whether measures of the strength of the crack-tip singularity (such as the J-integral or the stress intensity factors) are useful in characterizing a crack under a particular loading. In a linear elastic analysis the T-stress should be calculated using loads equal to the loads in the elastic-plastic analysis. See “T -stress extraction,” Section 2.16.3 of the Abaqus Theory Manual, for more information. Input File Usage: Abaqus/CAE Usage: *CONTOUR INTEGRAL, CONTOURS=n, TYPE=T-STRESS Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Type: T-stress Domain dependence In general, the T-stress has larger domain dependence or contour dependence than the J-integral and the stress intensity factors. Numerical tests suggest that the estimates from the first two rings of elements abutting the crack tip or crack line generally do not provide accurate results. Sufficient contours extending from the crack tip or crack line should be chosen so that the T-stress can be determined to be independent of the number of contours, within engineering accuracy. Particularly for axisymmetric models, the closer the crack tip is to the symmetry axis, the more refined the mesh in the domain should be to achieve path independence of the contour integral. Including the effect of a residual stress field on T -stress evaluation An additional term is included to account for the residual stress field when calculating the T -stress, as described in “Including the effect of a residual stress field on J-integral evaluation.” Input File Usage: Abaqus/CAE Usage: *CONTOUR INTEGRAL, RESIDUAL STRESS STEP=n, TYPE=T-STRESS Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Step for residual stress initialization values: step, Type: T-stress Defining the data required for a contour integral with the conventional finite element method To request contour integral output with the conventional finite element method, you must define the crack front and specify the virtual crack extension direction. Defining the crack front You must specify the crack front; i.e., the region that defines the first contour. Abaqus/Standard uses this region and one layer of elements surrounding it to compute the first contour integral. An additional layer of elements is used to compute each subsequent contour. The crack front can be equivalent to the crack tip in two dimensions or the crack line in three dimensions; or it can be a larger region surrounding the crack tip or crack line, in which case it must include the crack tip or crack line. If blunted crack tips are modeled, the crack front should include all the nodes going from one crack face to the other that would collapse onto the crack tip if the radius of the blunted tip were reduced to zero. Otherwise, the contour integral value will depend on the path until the contour region reaches the parallel crack faces. Input File Usage: *CONTOUR INTEGRAL, CONTOURS=n Specify the crack front node set name on the data line; the format depends on the method you use to specify the virtual crack extension direction. For two-dimensional cases only one crack front node set (the crack front at the crack tip) must be specified. For three-dimensional cases you must repeat the data line to specify the crack front for each node (or cluster of focused nodes) along the crack line in order from one end of the crack to the other, including the midside nodes of second-order elements; it is not permissible to skip nodes along the crack line. Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front Defining the crack tip or crack line By default, Abaqus/Standard defines the crack tip as the first node specified for the crack front and the crack line as the sequence of first nodes specified for the crack front. The first node is the node with the smallest node number, unless the node set is generated as unsorted. Alternatively, you can specify the crack-tip node or crack-line nodes directly. This specification plays a critical role for a three-dimensional crack with a blunt crack tip. Abaqus/CAE cannot determine the crack tip or crack line automatically based on the specified crack front. However, if you select a point to define the crack front in two dimensions, the same point defines the crack tip; likewise, if you select edges to define the crack front in three dimensions, the same edges define the crack line. For all other cases you must define the crack tip or crack line directly. Input File Usage: Use the following option to specify the crack-tip nodes directly: *CONTOUR INTEGRAL, CONTOURS=n, CRACK TIP NODES Specify the crack front node set name and the crack tip node number or node set name on the data line; the format depends on the method you use to specify the virtual crack extension direction. Repeat the data line for three-dimensional cases. Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front, then select the crack tip (in two dimensions) or crack line (in three dimensions) Defining a closed-loop crack line Sometimes a crack line may form a closed loop (for example, when modeling a full penny-shaped crack without invoking symmetry conditions). In such cases the finite element mesh in the crack-tip region can be created with or without seams; i.e., linear constraint equations (“Linear constraint equations,” Section 34.2.1) or multi-point constraints (“General multi-point constraints,” Section 34.2.2) may or may not be used to tie two layers of nodes together. If a crack line forms a closed loop, the starting node set of the crack front can be chosen arbitrarily and the other node sets defining the crack front must go around the crack front sequentially. The last node set defining the crack front must be the same as the first node set. If a closed loop is formed by creating coincident nodes that are then tied together by linear constraint equations and multi-point constraints, the node sets must be specified in order starting from one of the node sets involved in the constraint equation or multi-point constraint and terminating with the other node set. Specifying the virtual crack extension direction You must specify the direction of virtual crack extension at each crack tip in two dimensions or at each node along the crack line in three dimensions by specifying either the normal to the crack plane, , or the virtual crack extension direction, . If the virtual crack extension direction is specified to point into the material (parallel to the crack faces), the J-integral values calculated will be positive. Negative J-integral values are obtained when the virtual crack extension direction is specified in the opposite direction. Specifying the normal to the crack plane The virtual crack extension direction can be defined by specifying the normal, this case Abaqus/Standard will calculate a virtual crack extension direction, crack front tangent, crack; for a two-dimensional crack, we simply have implies that the crack plane is flat since only one value of . As shown in Figure 11.4.2–1, and , and the normal, , to the crack plane. In , that is orthogonal to the for a three-dimensional . Specifying the normal can be given per contour integral. Input File Usage: Abaqus/CAE Usage: *CONTOUR INTEGRAL, CONTOURS=n, NORMAL ), ), -direction cosine (or -direction cosine (or -direction cosine (or blank) crack front node set name (2-D) or names (3-D) Interaction module: Special→Crack→Create: select the crack front: Specify crack extension direction using: Normal to crack plane Specifying the virtual crack extension direction , can be specified directly. In three dimensions the Alternatively, the virtual crack extension direction, virtual crack extension direction, , will be corrected to be orthogonal to any normal defined at a node or in other cases to the tangent to the crack line itself. The tangent, , to the crack line at a particular point is obtained by parabolic interpolation through the crack front for which the virtual crack extension 1/4 point nodes crack plane Crack front node set Crack front node set. See section A-A below. Figure 11.4.2–1 Typical focused mesh for fracture mechanics evaluation. vector is defined and the nearest node sets on either side of this region. Abaqus/Standard will normalize the virtual crack extension direction, . Section A-A *CONTOUR INTEGRAL, CONTOURS=n crack front node set name, cosine (or ), -direction cosine (or blank) -direction cosine (or ), -direction 11.4.2–12 Repeat the data line for three-dimensional cases to specify the crack front and virtual crack extension vector for each node (or cluster of focused nodes) along the crack line. Abaqus/CAE Usage: Interaction module: Special→Crack→Create: select the crack front: Specify crack extension direction using: q vectors Defining surface normals In a case where the crack front intersects the external surface of a three-dimensional solid, where there is a surface of material discontinuity in the model, or where the crack is in a curved shell, the virtual crack extension direction, , must lie in the plane of the surface for accurate contour integral evaluation. Surface normals should be specified at all nodes that lie on such surfaces within the contours requested for this purpose (these nodes are printed out under the “Contour Integral” information in the data file). For shell element models the normals can be specified with the nodal coordinates if the normals calculated by Abaqus/Standard are not adequate. For solid element models the normals can be specified either directly or using the nodal coordinates (the fourth–sixth coordinates). If surface normals are not specified for the nodes on the crack surfaces and the external surfaces at the ends of a crack line, Abaqus/Standard will calculate the normals automatically for these nodes to correct any inadequate virtual crack extension directions, . Defining the data required for a contour integral with XFEM If you are using XFEM to evaluate the contour integral, both the crack front and the virtual crack extension direction are determined by Abaqus/Standard. Symmetry with the conventional finite element method If the crack is defined on a symmetry plane, only half the structure needs to be modeled. The change in potential energy calculated from the virtual crack front advance is doubled to compute the correct contour integral values. Input File Usage: Use the following option to indicate that the crack is defined on a symmetry plane: Abaqus/CAE Usage: *CONTOUR INTEGRAL, CONTOURS=n, SYMM Interaction module: Special→Crack→Create: select the crack front and crack tip or crack line, and specify the crack extension direction: General: toggle on On symmetry plane (half-crack model) Constructing a fracture mechanics mesh for small-strain analysis with the conventional finite element method Sharp cracks (where the crack faces lie on top of one another in the undeformed configuration) are usually modeled using small-strain assumptions. Focused meshes, as shown in Figure 11.4.2–1, should normally be used for small-strain fracture mechanics evaluations. However, for a sharp crack the strain field becomes singular at the crack tip. This result is obviously an approximation to the physics; however, the large-strain zone is very localized, and most fracture mechanics problems can be solved satisfactorily using only small-strain analysis. The crack-tip strain singularity depends on the material model used. Linear elasticity, perfect plasticity, and power-law hardening are commonly used in fracture mechanics analysis. Power-law hardening has the form is the equivalent total strain, where stress, n is the power-law hardening exponent (typically in the range of 3 to 8; perfect plasticity for large ), and is a reference strain, is a material constant (typically in the range 0.5 to 1.0). is the Mises stress, is the initial yield is very close to Results for pure power-law nonlinear elastic materials in a body under traction loading are proportional to the load to some power. Therefore, the fracture parameters for one geometry under a particular load can be scaled to any other load of the same distribution but different magnitude. If the loading is proportional (the direction of the stress increase in stress space is approximately constant) and monotonically increasing, power-law hardening deformation plasticity and incremental plasticity are essentially equivalent. However, deformation plasticity is a nonlinear elastic material for which more analytical results are available. Abaqus uses the Ramberg-Osgood form of deformation plasticity ; this model is not a pure power law model, which must be considered. Creating the singularity In most cases the singularity at the crack tip should be considered in small-strain analysis (when geometric nonlinearities are ignored). Including the singularity often improves the accuracy of the J-integral, the stress intensity factors, and the stress and strain calculations because the stresses and strains in the region close to the crack tip are more accurate. If r is the distance from the crack tip, the strain singularity in small-strain analysis is for linear elasticity, for perfect plasticity, and for power-law hardening. Modeling the crack-tip singularity in two dimensions The square root and crack tip is modeled with a ring of collapsed quadrilateral elements, as shown in Figure 11.4.2–2. singularity can be built into a finite element mesh using standard elements. The -1 -1 a, b, c isoparametric space physical space Figure 11.4.2–2 Collapsed two-dimensional element. To obtain a mesh singularity, generally second-order elements are used and the elements are collapsed as follows: 1. Collapse one side of an 8-node isoparametric element (CPE8R, for example) so that all three nodes—a, b, and c—have the same geometric location (on the crack tip). 2. Move the midside nodes on the sides connected to the crack tip to the 1/4 point nearest the crack tip. You can create “quarter point” spacing with second-order isoparametric elements when you generate nodes for a region of a mesh; see “Creating quarter-point spacing” in “Node definition,” Section 2.1.1. This procedure will create the strain singularity The singularity cannot be created using Abaqus elements, but the combination of the and terms can provide a reasonable approximation for . collapsed, and the two coincident nodes are free to displace independently, a If 4-node isoparametric elements (for example, CPE4R) are used, one side of the element is singularity is created. If the crack region is meshed with linear elements, the position specified for the midside nodes is ignored. Creating a square root singularity If nodes a, b, and c are constrained to move together, singular (suitable for linear elasticity). and the strains and stresses are square root Input File Usage: *NFILL, SINGULAR Constrain the collapsed nodes to move together by specifying the same node number in the list of nodes forming the element or by using a linear constraint equation or multi-point constraint to tie them together. Interaction module: Special→Crack→Create: select the crack front and crack tip, and specify the crack extension direction: Singularity: Midside node parameter: 0.25, Collapsed element side, single node Abaqus/CAE Usage: Creating a 1/r singularity If the midside nodes remain at the midside points rather than being moved to the 1/4 points and nodes a, b, and c are allowed to move independently, only the singularity in strain is created (suitable for perfect plasticity). Input File Usage: Abaqus/CAE Usage: *NFILL Interaction module: Special→Crack→Create: select the crack front and crack tip, and specify the crack extension direction: Singularity: Midside node parameter: 0.5, Collapsed element side, duplicate nodes Creating a combined square root and 1/r singularity If the midside nodes are moved to the 1/4 points but nodes a, b, and c are allowed to move independently, the singularity created is a combination of the square root and singularities. This combination is usually best for a power-law hardening material. However, since the singularity dominates, moving the midside nodes to the 1/4 points gives only slightly better results than if the nodes are left at the midside points. Since creating a mesh with the midside nodes moved to the quarter points can be difficult, it is often best to simply use the singularity. Input File Usage: Abaqus/CAE Usage: *NFILL, SINGULAR Interaction module: Special→Crack→Create: select the crack front and crack tip, and specify the crack extension direction: Singularity: Midside node parameter: 0.25, Collapsed element side, duplicate nodes Modeling the crack-tip singularity in three dimensions To create singular fields, 20-node bricks and 27-node bricks can be used with a collapsed face .The planes of the three-dimensional elements perpendicular to the crack line should be planar for the best accuracy. If they are not planar, the element Jacobian may become negative at some integration points when the midside nodes are moved to the 1/4 points. To correct this problem, move the midside nodes slightly away from the 1/4 points toward the midpoint position (the distance moved is not critical). See “Meshing the crack region and assigning elements,” Section 31.2.7 of the Abaqus/CAE User’s Manual, for information on creating a three-dimensional fracture mechanics mesh in Abaqus/CAE. C3D20(RH) midplane edge plane 2 nodes collapsed to the same location crack line 3 nodes collapsed to the same location midside nodes moved to 1/4 pts. Figure 11.4.2–3 Collapsed three-dimensional element. Creating a square root singularity To obtain a square root singularity, constrain the nodes on the collapsed face of the edge planes to move together and move the nodes to the 1/4 points. If the nodes at the midplane of a collapsed 20-node brick are constrained to move together, ; therefore, the singularity is not the same on the midplane as on an edge plane. This difference causes local oscillations in the solution about the crack tip along the crack line, although normally the oscillations are not significant. If all midface nodes and the centroid node are included in a 27-node brick and the midside and midface nodes are moved to the 1/4 points closest to the crack line, the oscillation in the local stress and strain fields can be reduced. Input File Usage: Abaqus/CAE Usage: *NFILL, SINGULAR Constrain the collapsed nodes to move together by specifying the same node number in the list of nodes forming the element or by using a linear constraint equation or multi-point constraint to tie them together. Interaction module: Special→Crack→Create: select the crack front and crack line, and specify the crack extension direction: Singularity: Midside node parameter: 0.25, Collapsed element side, single node Creating a 1/r singularity To obtain a keep the midside nodes at the midpoints. singularity, allow the three nodes on the collapsed face to displace independently and Input File Usage: Abaqus/CAE Usage: *NFILL Interaction module: Special→Crack→Create: select the crack front and crack line, and specify the crack extension direction: Singularity: Midside node parameter: 0.5, Collapsed element side, duplicate nodes Creating a combined square root and 1/r singularity To obtain a combined square root and singularity, allow the nodes on the collapsed face to displace independently and move the midside nodes to the 1/4 points. As in the two-dimensional case, if it is difficult to create the mesh with the nodes moved to the 1/4 points, simply use the singularity. Input File Usage: Abaqus/CAE Usage: *NFILL, SINGULAR Interaction module: Special→Crack→Create: select the crack front and crack line, and specify the crack extension direction: Singularity: Midside node parameter: 0.25, Collapsed element side, duplicate nodes Mesh refinement the smaller the radial The size of the crack-tip elements influences the accuracy of the solutions: dimension of the elements from the crack tip, the better the stress, strain, etc. results will be and, therefore, the better the contour integral calculations will be. The angular strain dependence is not modeled with the singular elements. Reasonable results are obtained if typical elements around the crack tip subtend angles in the range of 10° (accurate) to 22.5° (moderately accurate). Since the crack tip causes a stress concentration, the stress and strain gradients are large as the crack tip is approached. Path dependence in the evaluation of the J-integral may be an indication that the mesh is not sufficiently refined, but path independence does not prove mesh convergence. The finite element mesh must be refined in the vicinity of the crack to get accurate stresses and strains; however, accurate J-integral results can frequently be obtained even with a relatively coarse mesh. In many cases if sufficiently fine meshes are used, accurate contour integral values can be obtained without using singular elements. Modeling the crack-tip region in shells Focused meshes can be used, but not all of the three-dimensional shell elements in Abaqus/Standard can be collapsed. Elements S8R and S8RT cannot be degenerated into triangles; element types S4, S4R, S4R5, S8R5, and S9R5 can. The quarter-point technique (moving the midside nodes to the quarter points to give a singularity for elastic fracture mechanics applications) can be used with S8R5 and S9R5 elements but not with S8R(T) elements. When the quarter-point technique is used with S9R5 elements, the midface node should be moved to the quarter-point position along with the two midside nodes. If S8R(T) elements are used, a keyhole should be introduced at the crack tip. Flaws lying in the plane through the thickness of a shell can be modeled using line spring elements; see “Line spring elements for modeling part-through cracks in shells,” Section 32.9.1. In many cases line spring elements provide accurate J-integral and stress intensity values, but these elements are limited to modeling small strain and rotations. Limited modeling of plasticity is also allowed with line springs. Constructing a fracture mechanics mesh for finite-strain analysis with the conventional finite element method In large-strain analysis (when geometric nonlinearities are included) singular elements should not normally be used. The mesh must be sufficiently refined to model the very high strain gradients around the crack tip if details in this region are required. Even if only the J-integral is required, the deformation around the crack tip may dominate the solution and the crack-tip region will have to be modeled with sufficient detail to avoid numerical problems. , where Physically, the crack tip is not perfectly sharp. Therefore, it is normally modeled as a blunted notch with a radius of is a characteristic dimension of the plastic zone ahead of the crack tip. The notch must be small enough that, at the loads of interest, the deformed shape of the notch no longer depends on the original geometry. Typically, the notch must blunt out to more than four times its original radius for the deformed shape to be independent of the original geometry. The size of the elements around the notch should be about 1/10 the notch-tip radius to obtain accurate results. If a crack is modeled as sharp, the finite elements near the crack tip may not be able to approximate the high gradients, resulting in convergence problems. The stress and strain results around the crack tip will probably be inaccurate even if convergence is achieved. However, if the solution converges, the contour integral results should be reasonably accurate. The convergence difficulties will probably be greater in three dimensions than in two dimensions. In situations involving finite rotations but small strains, such as bending of slender structures, a small “keyhole” around the crack tip should be modeled. If the hole is small, the results will not be affected significantly and problems in dealing with the singular strains at the crack tip will be avoided. Using constraints with the conventional finite element method General multi-point constraints and linear constraint equations (“Kinematic constraints: overview,” Section 34.1.1) should not be used on nodes in the mesh regions where contour integrals are calculated unless the nodes involved in the constraint are located at the same point. The nodes at the crack tip of a focused mesh can be tied together using multi-point constraints without adversely affecting the contour integral calculations. Tying these nodes will change the singularity at the crack tip, but path independence of the contour integral will be maintained. In addition, path independence of the contour integrals will not be affected if two faces of a model are joined using MPC type TIE or a linear constraint equation, provided that all nodes of the two faces are coincident. Using multi-point constraints for mesh refinement or for applying symmetry/antisymmetry boundary conditions within the contour integral region will result in path dependence of the contour integrals. No warning or error messages are provided if this rule is violated. Procedures You can request contour integrals in fracture mechanics problems that were modeled using the following procedures: • static (“Static stress analysis,” Section 6.2.2) with both XFEM and the conventional finite element methods; • quasi-static (“Quasi-static analysis,” Section 6.2.5) with the conventional finite element method only; • steady-state transport (“Steady-state transport analysis,” Section 6.4.1) with the conventional finite element method only; • coupled thermal-stress procedures (“Fully coupled thermal-stress analysis,” Section 6.5.3) with the conventional finite element method only; and • crack propagation (“Crack propagation analysis,” Section 11.4.3) with the conventional finite element method only. Contour integrals can be requested only in general analysis steps: they are not calculated in linear perturbation analyses (“General and linear perturbation procedures,” Section 6.1.3). A crack analysis with pressure applied on the crack surfaces may give inaccurate contour integral values if geometric nonlinearity is included in a step. Loads Contour integral calculations include the following distributed load types: • thermal loads; • distributed loads, including crack face pressure and traction loads on continuum elements as well as those applied using user subroutine DLOAD and UTRACLOAD; • distributed loads, including surface traction loads and crack face edge loads on shell elements as well as those applied using user subroutine UTRACLOAD; • uniform and nonuniform body forces; and • centrifugal loads on continuum and shell elements. Contributions to the contour integral due to concentrated loads in the domain are not included; instead, the mesh must be modified to include a small element and a distributed load must be applied to this element. Contributions due to contact forces are not included. Material options J-integral calculations are valid for linear elastic, nonlinear elastic, and elastic-plastic materials. Plastic behavior can be modeled as nonlinear elastic (“Deformation plasticity,” Section 23.2.13), but the results are generally best if the material is modeled by incremental plasticity and is subject to proportional, monotonic traction loading. If unloading has taken place in the plastic zone around the crack tip, the J-integral will not be valid except in very limited cases. The -integral is valid for problems involving creep (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4). The stress intensity factor calculation is valid for cracks in homogeneous, linear elastic materials. It is also valid for an interfacial crack between two different isotropic linear elastic materials. It is not valid for any other types of materials, including user-defined materials. The crack propagation direction is valid only for homogeneous, isotropic linear elastic materials. The T-stress is valid only for homogeneous, isotropic linear elastic materials. Although the T-stress is calculated using the linear elastic material properties of the body with a crack, it is usually used with the J-integral calculated using the elastic-plastic material properties of the body . If there is material discontinuity, the normal to the material discontinuity line must be specified for all nodes on the material discontinuity that will lie in a contour integral domain. The normal can be specified by defining user-specified normals for the elements on both sides of the discontinuity or by using nodal normal coordinates for the nodes on the discontinuity. Contour integral calculations cannot be performed for a crack with a material discontinuity line passing through its tip (except for an interfacial crack between two different materials). Therefore, you should be careful when specifying a normal that is not perpendicular to the virtual crack extension direction, , for the nodes at the crack tip. Elements When used with XFEM, the contour integral can be evaluated only in first-order or second-order tetrahedron and first-order brick elements. The following paragraphs apply only to the conventional finite element method. The contour integral evaluation capability in Abaqus/Standard assumes that the elements that lie within the domain used for the calculations are quadrilaterals in two-dimensional or shell models or bricks in continuum three-dimensional models. Triangles, tetrahedra, or wedges should not be used in the mesh that is included in the contour integral regions. When the elements around the crack tip are generated in Abaqus/CAE, triangular elements (in two dimensions) or wedge elements (in three dimensions) are converted to collapsed quadrilateral or hexahedral elements. The elements within the contour domain should be of the same type. In shell structures the contour integrals calculated by Abaqus/Standard will be contour independent only if the deformation mode around the crack tip is primarily membrane. If there are significant bending or transverse shear effects in the domain, the contour integrals may not be contour independent and contour integral values should be obtained directly from the displacements and/or the stresses. Generalized plane strain elements, generalized axisymmetric elements with twist, asymmetric- axisymmetric elements, membrane elements, and cylindrical elements should not be used in the contour integral regions. The contribution of rebar is included only in the calculations of the J-integral and the -integral for shell elements defined with a shell section integrated during the analysis . Output The domain associated with each contour is calculated automatically. The nodes belonging to each domain can be printed in the data file; see “Controlling the amount of analysis input file processor information written to the data file” in “Output,” Section 4.1.1. If you are using the conventional contour integral method, for each domain Abaqus/Standard creates a new node set in the output database to In addition, new node sets are include these nodes; you can view these node sets in Abaqus/CAE. created in the output database for nodes on crack surfaces and on free surfaces whose nodal normals are calculated by Abaqus/Standard. Contour integrals cannot be recovered from the restart file as described in “Output,” Section 4.1.1. You should not request element output extrapolated to the nodes (“Element output” in “Output to the data and results files,” Section 4.1.2) for second-order elements with one collapsed side in two dimensions or one collapsed face in three dimensions. Default contour integral output By default, the contour integral values are written to the data file and to the output database file. The following naming convention is used for contour integrals written to the output database: integral-type: abbrev-integral-type at history-output-request-name_crack-name_internal- crack-tip-node-set-name__Contour_contour-number where integral-type can be • Crack propagation direction (Cpd) • J-integral (J) • J-integral estimated from Ks (JKs) • Stress intensity factor K1 (K1) • Stress intensity factor K2 (K2) • T-stress (T) For example, J-integral: J at JINT_CRACK_CRACKTIP-1__Contour_1 Writing the contour integrals to the results file You can choose to write the contour integral values to the results file in addition to the data file. Input File Usage: Abaqus/CAE Usage: Use the following option to write the contour integrals to the results file instead of the data file: *CONTOUR INTEGRAL, CONTOURS=n, OUTPUT=FILE Use the following option to write the contour integrals to the results file in addition to the data file: *CONTOUR INTEGRAL, CONTOURS=n, OUTPUT=BOTH You cannot write contour integrals to the results file from Abaqus/CAE. Controlling the output frequency You can control the output frequency, in increments, of contour integrals. By default, the crack-tip location and associated quantities will be printed every increment. Specify an output frequency of 0 to suppress contour integral output. The output frequency for contour integral output to the output database is controlled by the larger of the frequency values specified for history output to the output database (see “Output to the output database,” Section 4.1.3) or for contour integral output. If you specify an output frequency of 0 for the history output to the output database, contour integral values will not be written to the output database. Input File Usage: *CONTOUR INTEGRAL, CRACK NAME=crack name, CONTOURS=n, FREQUENCY=f Abaqus/CAE Usage: Step module: history output request editor: Domain: Crack: crack name, Number of contours: n, Save output at 11.4.3 CRACK PROPAGATION ANALYSIS Products: Abaqus/Standard Abaqus/Explicit References • “Defining an analysis,” Section 6.1.2 • “Fracture mechanics: overview,” Section 11.4.1 • “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7 • “Surface-based cohesive behavior,” Section 36.1.10 • *COHESIVE BEHAVIOR • *CONTACT CLEARANCE • *DEBOND • *DIRECT CYCLIC • *FRACTURE CRITERION • *NODAL ENERGY RATE • “Defining surface-to-surface contact in an Abaqus/Standard analysis” in “Defining surface-to- surface contact,” Section 15.13.7 of the Abaqus/CAE User’s Manual Overview Crack propagation analysis: • allows for six types of fracture criteria in Abaqus/Standard—critical stress at a certain distance ahead of the crack tip, critical crack opening displacement, crack length versus time, VCCT (the Virtual Crack Closure Technique), enhanced VCCT, and the low-cycle fatigue criterion based on the Paris law; • allows for the VCCT fracture criterion in Abaqus/Explicit; • in Abaqus/Standard models quasi-static crack growth in two dimensions (planar and axisymmetric) for all types of fracture criteria and in three dimensions (solid, shells, and continuum shells) for VCCT, enhanced VCCT, and the low-cycle fatigue criteria; and • in Abaqus/Explicit models crack growth in three dimensions (solid, shells, and continuum shells) for VCCT criterion; and • requires that you define two distinct initially bonded contact surfaces between which the crack will propagate. Defining initially bonded crack surfaces in Abaqus/Standard Potential crack surfaces are modeled as slave and master contact surfaces . Any contact formulation except the finite-sliding, surface-to-surface formulation can be used. The predetermined crack surfaces are assumed to be initially partially bonded so that the crack tips can be identified explicitly by Abaqus/Standard. Initially bonded crack surfaces cannot be used with self-contact. Define an initial condition to identify which part of the crack is initially bonded. You specify the slave surface, the master surface, and a node set that identifies the initially bonded part of the slave surface. The unbonded portion of the slave surface will behave as a regular contact surface. Either the slave surface or the master surface must be specified; if only the master surface is given, all of the slave surfaces associated with this master surface that have nodes in the node set will be bonded at these nodes. If a node set is not specified, the initial contact conditions will apply to the entire contact pair; in this case, no crack tips can be identified, and the bonded surfaces cannot separate. If a node set is specified, the initial conditions apply only to the slave nodes in the node set. Abaqus/Standard checks to ensure that the node set defined includes only slave nodes belonging to the contact pair specified. By default, the nodes in the node set are considered to be initially bonded in all directions. *INITIAL CONDITIONS, TYPE=CONTACT Input File Usage: Bonding only in the normal direction For fracture criteria based on the critical stress, critical crack opening displacement, or crack length versus time, it is possible to bond the nodes in the node set (or the contact pair if a node set is not defined) only in the normal direction. In this case the nodes are allowed to move freely tangential to the contact surfaces. Friction (“Frictional behavior,” Section 36.1.5) cannot be specified if the nodes are bonded only in the normal direction. Bonding only in the normal direction is typically used to model bonded contact conditions in Mode I crack problems where the shear stress ahead of the crack along the crack plane is zero. Input File Usage: *INITIAL CONDITIONS, TYPE=CONTACT, NORMAL Activating the crack propagation capability in Abaqus/Standard The crack propagation capability must be activated within the step definition to specify that crack propagation may occur between the two surfaces that are initially partially bonded. You specify the surfaces along which the crack propagates. If the crack propagation capability is not activated for partially bonded surfaces, the surfaces will not separate; in this case the specified initial contact conditions would have the same effect as that provided by the tied contact capability, which generates a permanent bond between two surfaces during the entire analysis . Input File Usage: *DEBOND, SLAVE=slave_surface_name, MASTER=master_surface_name Propagation of multiple cracks Cracks can propagate from either a single crack tip or multiple crack tips. The crack propagation capability in Abaqus/Standard requires that the surfaces be initially partially bonded so that the crack tips can be identified. A contact pair can have crack propagation from multiple crack tips. However, only one crack propagation criterion is allowed for a given contact pair. Crack propagation along several contact pairs can be modeled by specifying multiple crack propagation definitions. Defining and activating crack propagation in Abaqus/Explicit In Abaqus/Explicit potential crack surfaces are modeled as bonded general contact surfaces . Hence, the capability is available in three-dimensional analyses only and is implemented using a pure master-slave formulation. As is the case in Abaqus/Standard, the predetermined crack surfaces are assumed to be initially partially bonded so that the crack tips can be identified explicitly. interactions in Abaqus/Explicit,” Section 35.4.1) To identify which pair of surfaces determine the crack and which part of the crack is initially bonded, you must define and assign a contact clearance . You first define a contact clearance to specify the node set that is initially bonded, and then you assign this contact clearance to a pair of two single-sided surfaces that define the crack. The unbonded portion behaves as a regular contact surface. The nodes in the node set are considered to be initially bonded in all directions. The crack tip is identified only from the specified two surfaces and the node set. No attempt is made to determine a crack tip from all surfaces included in the general contact domain. Consequently, to be able to identify the crack tip, the surface including the specified node set must extend past the node set. Otherwise, the surfaces will not debond, and the crack cannot propagate. You complete the definition of the crack propagation capability by defining a fracture-based cohesive behavior surface interaction. You activate the crack propagation by assigning it to the pair of surfaces that are initially partially bonded. If the fracture criterion is met, crack propagation occurs between these two surfaces. Cohesive behavior is also used to specify the elastic behavior of the bonds . If a fracture-based surface interaction is not assigned to a pair of surfaces, the crack definition is incomplete. Unlike Abaqus/Standard where the identified nodes will stay bonded if the crack is not activated, in Abaqus/Explicit the nodes identified by the contact clearance definition will separate without generating any interface stress. Similar to Abaqus/Standard, cracks can propagate from single or multiple crack tips for the same pair of surfaces. Input File Usage: Use the following options: *CONTACT CLEARANCE, NAME=clearance_name, SEARCH NSET=bonded_nset_name ** *SURFACE INTERACTION, NAME=interaction_name *COHESIVE BEHAVIOR *FRACTURE CRITERION ..** *CONTACT *CONTACT CLEARANCE ASSIGNMENT slave_surface, master_surface, clearance_name *CONTACT PROPERTY ASSIGNMENT slave_surface, master_surface, interaction_name Specifying a fracture criterion You can specify the crack propagation criteria, as discussed below. Table 11.4.3–1 shows which criteria are supported by Abaqus/Standard and Abaqus/Explicit. Only one crack propagation criterion is allowed per contact pair even if multiple cracks are present. Table 11.4.3–1 Crack propagation criterion Abaqus/Standard Abaqus/Explicit Critical stress Critical crack opening displacement Crack length versus time VCCT Enhanced VCCT Low-cycle fatigue Yes Yes Yes Yes Yes Yes No No No Yes No No Crack propagation analysis is carried out on a nodal basis. The crack-tip node debonds when the fracture criterion, f, reaches the value 1.0 within a given tolerance: and where for other fracture criteria. You can specify the tolerance for VCCT, enhanced VCCT, and low-cycle fatigue criteria or . In Abaqus/Standard, if , the time increment is cut back such that the crack propagation criterion is satisfied except in the case of an unstable crack growth problem where multiple nodes at and ahead of a crack tip are allowed to debond without the cut back of increment size in one increment. The default value of is 0.1 for the critical stress, critical crack opening displacement, and crack length versus time criteria and is 0.2 for the VCCT, enhanced VCCT, and low-cycle fatigue criteria. Input File Usage: *FRACTURE CRITERION, TOLERANCE= , TYPE=type Critical stress criterion This criterion is available only in Abaqus/Standard. If you specify a critical stress criterion at a critical distance ahead of the crack tip, the crack-tip node debonds when the local stress across the interface at a specified distance ahead of the crack tip reaches a critical value. This criterion is typically used for crack propagation in brittle materials. The critical stress criterion is defined as is the normal component of stress carried across the interface at the distance specified; are the shear stress components in the interface; and where and stresses, which you must specify. The second component of the shear failure stress, a two-dimensional analysis; therefore, the value of when the fracture criterion, f, reaches the value 1.0. are the normal and shear failure , is not relevant in need not be specified. The crack-tip node debonds and If the value of is not given or is specified as zero, it will be taken to be a very large number so that the shear stress has no effect on the fracture criterion. The distance ahead of the crack tip is measured along the slave surface, as shown in Figure 11.4.3–1. The stresses at the specified distance ahead of the crack tip are obtained by interpolating the values at the adjacent nodes. The interpolation depends on whether first-order or second-order elements are used to define the slave surface. unbonded portion bonded portion slave surface master surface current crack tip distance ahead of the crack tip Figure 11.4.3–1 Distance specification for the critical stress criterion. Input File Usage: *FRACTURE CRITERION, TYPE=CRITICAL STRESS, DISTANCE=n Critical crack opening displacement criterion This criterion is available only in Abaqus/Standard. If you base the crack propagation analysis on the crack opening displacement criterion, the crack-tip node debonds when the crack opening displacement at a specified distance behind the crack tip reaches a critical value. This criterion is typically used for crack propagation in ductile materials. The crack opening displacement criterion is defined as is the measured value of crack opening displacement and where is the critical value of the crack opening displacement (user-specified). The crack-tip node debonds when the fracture criterion reaches the value 1.0. You must supply the crack opening displacement versus cumulative crack length data. In Abaqus/Standard the cumulative crack length is defined as the distance between the initial crack tip and the current crack tip measured along the slave surface in the current configuration. The crack opening displacement is defined as the normal distance separating the two faces of the crack at the given distance. You specify the position, n, behind the crack tip where the critical crack opening displacement is calculated. The value of this position must be specified as the length of the straight line joining the current crack tip and points on the slave and master surfaces (Figure 11.4.3–2). Distance, n, from crack tip to point x on the slave surface Measured crack opening displacement value, δ crack tip Figure 11.4.3–2 Distance specification for the critical crack opening displacement criterion. Abaqus/Standard computes the crack opening displacement at that point by interpolating the values at the adjacent nodes. The interpolation depends on whether first-order or second-order elements are used to define the slave surface. An error message will be issued if the value of n is not within the end points of the contact pair. Input File Usage: *FRACTURE CRITERION, TYPE=COD, DISTANCE=n Modeling symmetry In problems where the debonding surfaces lie on a symmetry plane, you can specify that Abaqus/Standard should consider only half of the user-specified crack opening displacement values. In this case the initial bonding must be in the normal direction only . *FRACTURE CRITERION, TYPE=COD, DISTANCE=n, SYMMETRY Input File Usage: Crack length versus time criterion This criterion is available only in Abaqus/Standard. To specify the crack propagation explicitly as a function of total time, you must provide a crack length versus time relationship and a reference point from which the crack length is measured. This reference point is defined by specifying a node set. Abaqus/Standard finds the average of the current positions of the nodes in the set to define the reference point. During crack propagation the crack length is measured from this user-specified reference point along the slave surface in the deformed configuration. The time specified must be total time, not step time. The fracture criterion, f, is stated in terms of the user-specified crack length and the length of the current crack tip. The length of the current crack tip from the reference point is measured as the sum of the straight line distance of the initial crack tip from the reference point and the distance between the initial crack tip and the current crack tip measured along the slave surface. Referring to Figure 11.4.3–3, let node 1 be the initial location of the crack tip and node 3 be the current location of the crack tip. The distance of the current crack tip located at node 3 is given by where between nodes 1 and 2, and is the length of the straight line joining node 1 and the reference point, is the distance is the distance between nodes 2 and 3 measured along the slave surface. The fracture criterion, f, is given by where l is the length at the current time obtained from the user-specified crack length versus time curve. Crack-tip node 3 will debond when the failure function f reaches the value of 1.0 (within the user-defined tolerance). If geometric nonlinearity is considered in the step (“Defining an analysis,” Section 6.1.2), the reference point may move as the body deforms; you must ensure that this movement does not invalidate the crack length versus time criterion. Abaqus/Standard does not extrapolate beyond the end points of your crack data. Therefore, if the first crack length specified is greater than the distance from the crack reference point to the first slave surface master surface length ±ftol Δl23 Δl23 Δl12 l1 reference point reference node set Figure 11.4.3–3 Crack propagation as a function of time. time bonded node, the first bonded node will never debond and the crack will not propagate. In this case Abaqus/Standard will print warning messages in the message (.msg) file. Input File Usage: *FRACTURE CRITERION, TYPE=CRACK LENGTH, NSET=name VCCT criterion This criterion is available in both Abaqus/Standard and Abaqus/Explicit. The Virtual Crack Closure Technique (VCCT) criterion uses the principles of linear elastic fracture mechanics (LEFM) and, therefore, is appropriate for problems in which brittle crack propagation occurs along predefined surfaces. VCCT is based on the assumption that the strain energy released when a crack is extended by a certain amount is the same as the energy required to close the crack by the same amount. For example, Figure 11.4.3–4 illustrates the similarity between crack extension from i to j and crack closure at j. In Figure 11.4.3–5 nodes 2 and 5 will start to release when is the Mode I energy release rate, where is the length of the elements at the crack front, is the vertical displacement between nodes 1 and 6. Assuming that the crack closure is governed by linear elastic behavior, the energy to close the crack (and, thus, the energy to open the crack) is calculated from the previous equation. Similar arguments and equations can be written in two dimensions for Mode II and for three-dimensional crack surfaces including Mode III. is the critical Mode I energy release rate, b is the width, d is the vertical force between nodes 2 and 5, and δ a crack closed i j δ a i j Figure 11.4.3–4 Mode I: The energy released when a crack is extended by a certain amount is the same as the energy required to close the crack. In the general case involving Mode I, II, and III the fracture criterion is defined as is the equivalent strain energy release rate calculated at a node, and is the critical where equivalent strain energy release rate calculated based on the user-specified mode-mix criterion and the bond strength of the interface. The crack-tip node will debond when the fracture criterion reaches the value of 1.0. v1,6 y, v 1 x, u Fv,2,5 crit Load Fv,2,5 Load Fv,2,5 5 4 2 3 Area = G dbIC V2,5 crit Displacement V2,5 Figure 11.4.3–5 Pure Mode I modified. Abaqus provides three common mode-mix formulae for computing : the BK law, the power law, and the Reeder law models. The choice of model is not always clear in any given analysis; an appropriate model is best selected empirically. BK law The BK law model is described in Benzeggagh (1996) by the following formula: To define this model, you must provide and . This model provides a power law relationship combining energy release rates in Mode I, Mode II, and Mode III into a single scalar fracture criterion. Input File Usage: *FRACTURE CRITERION, TYPE=VCCT, MIXED MODE BEHAVIOR=BK Power law The power law model is described in Wu (1965) by the following formula: To define this model, you must provide and . Input File Usage: *FRACTURE CRITERION, TYPE=VCCT, MIXED MODE BEHAVIOR=POWER Reeder law The Reeder law model is described in Reeder (2002) by the following formula: To define this model, you must provide when applies only to three-dimensional problems. . When and . The Reeder law is best applied , the Reeder law reduces to the BK law. The Reeder law Input File Usage: *FRACTURE CRITERION, TYPE=VCCT, MIXED MODE BEHAVIOR=REEDER Releasing multiple nodes in one increment in Abaqus/Standard For an unstable crack growth problem, sometimes it is more efficient to allow multiple nodes at and ahead of a crack tip to debond in one increment without cutting back the increment size when the VCCT fracture criterion is satisfied. This capability is activated automatically if you specify an unstable growth tolerance, . In this case if the fracture criterion, f, is within the given unstable growth tolerance: where is the tolerance described earlier in this section, rather than cut back the increment size, more nodes at and ahead of the crack tip are allowed to debond in one increment until for all the nodes ahead of the crack tip. The forces at those debonded nodes are completely released immediately during the following increment. If you do not specify a value for the unstable growth tolerance, the default value is infinity. In this case the fracture criterion, f, for unstable crack growth is not limited by any upper-bound value in the above equation. Input File Usage: *FRACTURE CRITERION, TYPE=VCCT, UNSTABLE GROWTH TOLERANCE= Defining variable critical energy release rates You can define a VCCT criterion with varying energy release rates by specifying the critical energy release rates at the nodes. If you indicate that the nodal critical energy rates will be specified, any constant critical energy release rates you specify are ignored, and the critical energy release rates are interpolated from the nodes. The critical energy release rates must be defined at all nodes on the slave surface. Input File Usage: Use both of the following options: *FRACTURE CRITERION, TYPE=VCCT, NODAL ENERGY RATE *NODAL ENERGY RATE Enhanced VCCT criterion This criterion is available only in Abaqus/Standard. The enhanced VCCT criterion is very similar to the original VCCT criterion described above. As in the original VCCT criterion, the fracture criterion in the general case involving Mode I, II, and III is defined as The crack-tip node debonds when the fracture criterion reaches the value of 1.0. However, unlike the original VCCT criterion, you can specify two different critical fracture energy release rates: for the onset of a crack and for the growth of a crack. When the enhanced VCCT criterion is used in the general case involving Mode I, II, and III fracture, the amount of energy dissipated associated with the release of the debonding force is controlled by the critical equivalent strain energy release rate required to propagate the crack, , rather than by the critical equivalent strain energy release rate required to initiate the crack, for different mixed-mode fracture criteria. are identical to those used for The formulae for calculating Input File Usage: *FRACTURE CRITERION, TYPE=ENHANCED VCCT Low-cycle fatigue criterion This criterion is available only in Abaqus/Standard. If you specify the low-cycle fatigue criterion, progressive delamination growth at the interfaces in laminated composites subjected to sub-critical cyclic loadings can be simulated. This criterion can be used only in a low-cycle fatigue analysis using the direct cyclic approach (“Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7). The onset and delamination growth are characterized by using the Paris law, which relates the relative fracture energy release rate to crack growth rates as illustrated in Figure 11.4.3–6. The fracture energy release rates at the crack tips in the interface elements are calculated based on the above mentioned VCCT technique. The Paris regime is bounded by the energy release rate threshold, , below which there is no consideration of fatigue crack initiation or growth, and the energy release rate upper limit, , above which the fatigue crack will grow at an accelerated rate. is the critical equivalent strain energy release rate calculated based on the user-specified mode-mix criterion and the bond strength of the interface. The formulae for calculating have been provided above for different mixed mode fracture criteria. You can specify the ratio of . The default values are and the ratio of over over and . Input File Usage: *FRACTURE CRITERION, TYPE=FATIGUE Onset of delamination growth The onset of delamination growth refers to the beginning of fatigue crack growth at the crack tip along the interface. In a low-cycle fatigue analysis the onset of the fatigue crack growth criterion is characterized by , which is the relative fracture energy release rate when the structure is loaded between its maximum and minimum values. The fatigue crack growth initiation criterion is defined as da dN Paris Regime Gthresh Gpl GC Figure 11.4.3–6 Fatigue crack growth govern by Paris law. and are material constants and where is the cycle number. The interface elements at the crack tips will not be released unless the above equation is satisfied and the maximum fracture energy release rate, , which corresponds to the cyclic energy release rate when the structure is loaded up to its maximum value, is greater than . Fatigue delamination growth using the Paris law Once the onset of delamination growth criterion is satisfied at the interface, the delamination growth rate, . The rate of the delamination growth per cycle is given by the Paris law if , can be calculated based on the relative fracture energy release rate, where and are material constants. At the end of cycle , Abaqus/Standard extends the crack length, , from the current cycle by releasing at least one element at forward over an incremental number of cycles, to the interface. Given the material constants and , combined with the known node spacing at the interface elements at the crack tips, the number of cycles necessary to fail each interface element at the crack tip can be calculated as , where j represents the node at the jthe crack tip. The analysis is set up to release at least one interface element after the loading cycle is stabilized. The element with the fewest cycles is identified to be released, and its is represented as the number of cycles to grow the crack equal to its element length, . The most critical element is completely released with a zero constraint and a zero stiffness at the end of the stabilized cycle. As the interface element is released, the load is redistributed and a new relative fracture energy release rate must be calculated for the interface elements at the crack tips for the next cycle. This capability allows at least one interface element at the crack tips to be released after each stabilized cycle and precisely accounts for the number of cycles needed to cause fatigue crack growth over that length. , the interface elements at the crack tips will be released by increasing the cycle If number count, , by one only. Specifying how a debonding force is released after a fracture criterion is met in Abaqus/Standard After debonding, the traction between two surfaces is initially carried as equal and opposite forces at the slave node and the corresponding point on the master surface. The debonding force is released as the crack opens and advances. Once complete debonding has occurred at a point, the bond surfaces act like standard contact surfaces with associated interface characteristics. There are two different ways to release the debonding force, depending on the fracture criterion that you specify. Specifying a debonding amplitude curve When you use the critical stress, critical crack opening displacement, or crack length versus time fracture criteria, you can define how this force is to be reduced to zero with time after debonding starts at a particular node on the bonded surface. You specify a relative amplitude, a, as a function of time after debonding starts at a node. Thus, suppose the force transmitted between the surfaces at slave node N is . Then, for any time the force . The relative amplitude must be 1.0 at when that node starts to debond, which occurs at time transmitted between the surfaces at node N is the relative time 0.0 and must reduce to 0.0 at the last relative time point given. The best choice of the amplitude curve depends on the material properties, specified loading, and the crack propagation criterion. If the stresses are removed too rapidly, the resulting large changes in the strains near the crack tip can cause convergence difficulties. For large-strain problems severe mesh distortion can also occur. For problems with rate-independent materials a linear amplitude curve is normally adequate. For problems with rate-dependent materials the stresses should be ramped off more slowly at the beginning of debonding to avoid convergence and mesh distortion difficulties. To reduce the likelihood of convergence and mesh distortion difficulties, you can reduce the value of the debond stress by 25% in 50% of the time to debond. The solution should not be strongly influenced by the details of the unloading procedure; if it is, this usually indicates that the mesh should be refined in the debond region. Input File Usage: *DEBOND, SLAVE=slave, MASTER=master Data lines to define debonding amplitude curve Ramping down debonding force for the VCCT and the enhanced VCCT criteria For the VCCT and the enhanced VCCT criteria, when the energy release rate exceeds the critical value at a crack tip, you can either release the traction between the two surfaces at the crack tip immediately during the following increment or release the traction gradually during succeeding increments with the reduction of the magnitude of the debonding force being governed by the critical fracture energy release rate. The latter approach is sometimes recommended to avoid sudden loss of stability when the crack tip is advanced. The enhanced VCCT criterion is meaningful only when used in conjunction with the latter approach. When the former approach is used, the results obtained by using the enhanced VCCT criterion are identical to those obtained by using the original VCCT criterion. Input File Usage: Use the following option to release the traction immediately: *DEBOND, SLAVE=slave, MASTER=master, DEBONDING FORCE=STEP Use the following option to release the traction gradually: *DEBOND, SLAVE=slave, MASTER=master, DEBONDING FORCE=RAMP Procedures Crack propagation analysis can be performed for static or dynamic overloadings using the following procedures: • “Static stress analysis,” Section 6.2.2 • “Quasi-static analysis,” Section 6.2.5 • “Implicit dynamic analysis using direct integration,” Section 6.3.2 • “Explicit dynamic analysis,” Section 6.3.3 • “Fully coupled thermal-stress analysis,” Section 6.5.3 It can also be performed for sub-critical cyclic fatigue loadings using the following procedure: • “Low-cycle fatigue analysis using the direct cyclic approach,” Section 6.2.7 Controlling time incrementation during debonding in Abaqus/Standard When automatic incrementation is used for any criteria other than VCCT, enhanced VCCT, or low-cycle fatigue, you can specify the size of the time increment used just after debonding starts. By default, the time increment is equal to the last relative time specified. However, if a fracture criterion is met at the beginning of an increment, the size of the time increment used just after debonding starts will be set equal to the minimum time increment allowed in this step. For fixed time incrementation the specified time increment value will be used as the time increment size after debonding starts if Abaqus/Standard finds it needs a smaller time increment than the fixed time increment size. The time increment size will be modified as required until debonding is complete. *DEBOND, SLAVE=slave, MASTER=master, TIME INCREMENT=t Input File Usage: Viscous regularization for VCCT in Abaqus/Standard The simulation of structures with unstable propagating cracks is challenging and difficult. Nonconvergent behavior may occur from time to time. While the usual stabilization techniques (such as contact pair stabilization and static stabilization) can be used to overcome some convergence difficulties, localized damping is included for VCCT or enhanced VCCT by using the viscous regularization technique. Viscous regularization damping causes the tangent stiffness matrix of the softening material to be positive for sufficiently small time increments. Input File Usage: Use one of following options: *FRACTURE CRITERION, TYPE=VCCT, VISCOSITY= *FRACTURE CRITERION, TYPE=ENHANCED VCCT, VISCOSITY= Linear scaling to accelerate convergence for VCCT in Abaqus/Standard For most crack propagation simulations using VCCT or the enhanced VCCT criterion, the deformation can be nearly linear up to the point of the onset of crack growth; past this point the analysis becomes very nonlinear. In this case a linear scaling method can be used to effectively reduce the solution time to reach the onset of crack growth. Suppose that an applied “trial” load at increment is just a fraction of the critical load at the . The following algorithm is used in Abaqus/Standard to quickly onset time of crack growth, converge to the critical load state: where initially would be set between 0.7 and 0.9 depending on the degree of nonlinearity (the default value is 0.9). When becomes smaller than 0.5% (indicating that the load is within 0.5% of its critical value), the next is automatically set to 1.0 to cause the most critical crack-tip node to precisely reach the critical value at the next increment. After the first crack-tip node releases, the linear scaling calculations are no longer valid and the time increment is set to the default value. Cutback is then allowed. *CONTROLS, TYPE=VCCT LINEAR SCALING Input File Usage: Tips for using the VCCT or enhanced VCCT criterion in Abaqus/Standard Crack propagation problems using the VCCT or enhanced VCCT criterion are numerically challenging. The following tips will help you create a successful Abaqus/Standard model: • An analysis with the VCCT or enhanced VCCT criterion requires small time increments. Abaqus/Standard tracks the location of the active crack front node by node when the VCCT or enhanced VCCT criterion is used. Therefore, the crack front is allowed to advance only a single node forward in any single increment (although such an advance may take place across the entire crack front in three-dimensional problems). Because an analysis using the VCCT or enhanced VCCT criterion provides detailed results of the growth of the crack, you will need small time increments, especially if the mesh is highly refined. • Three different types of damping can be used to aid convergence for a model using the VCCT or enhanced VCCT criterion: contact stabilization, automatic or static stabilization, and viscous regularization. Contact and automatic stabilization are not specific to VCCT; they are built into Abaqus/Standard and are compatible with VCCT. Setting the value of the damping parameters is often an iterative procedure. If your VCCT model fails to converge due to unstable crack propagation, set the damping parameters to relatively high values and rerun the analysis. If the parameters are high enough, stable incrementation should return. However, the crack propagation behavior may have been modified by the damping forces and may not be physically correct. To monitor the energy absorbed by viscous damping, plot the damping energy and compare the results to the total strain energy in the model (ALLSE). When set properly, the value of the damping energy should be a small fraction of the total energy. Monitor the damping energy to ensure that the results of the VCCT simulation are reasonable in the presence of damping. When you use contact or automatic stabilization, Abaqus writes the damping energy to the variable ALLSD in the output database (.odb) file. When you use viscous regularization, Abaqus writes the damping energy to the variable ALLVD. • To maximize the accuracy of the debonding simulation, try to use matched meshes between the slave and master surfaces of the debonding contact pair. • If you do use a mismatched mesh, you can maximize the accuracy of the simulation by using the small-sliding, surface-to-surface formulation for the contact pair . • Printing contact constraint information to the data (.dat) file allows you to review the status of the debonding contact pair at the beginning of the analysis. By printing detailed contact conditions to the message (.msg) file, you can track the incremental behavior of the advancing crack front during the analysis. For more information about these output requests, see “Output,” Section 4.1.1. • You can add a small clearance to the initially unbonded portion of the debonding contact pair (“Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 35.3.5). The small clearance will help to eliminate unnecessary severe discontinuity iterations during incrementation as the crack begins to progress. • Do not use tie MPCs (“General multi-point constraints,” Section 34.2.2) for the slave surface in a debonding contact pair. Abaqus is unable to resolve the overconstraint presented by the MPC and the debonded contact state. • You must have continuous master debonding surfaces. • You may be able to help the analysis converge by adding geometric nonlinearity (even if small- sliding is used for the debonding contact pair). For more information, see “Geometric nonlinearity” in “General and linear perturbation procedures,” Section 6.1.3. • For two-dimensional models with contact pairs involving higher-order underlying elements, the initially unbonded portion must extend over complete element faces. In other words, the crack tip in a two-dimensional, higher-order model must start at a corner node on the quadratic slave surfaces. The crack tip must not start at a midside node. Tips for using the VCCT criterion in Abaqus/Explicit Crack propagation problems using the VCCT criterion analyzed in Abaqus/Explicit benefit from the robustness of the general contact algorithm in the context of an explicit time integrator. Nevertheless, as is the case in Abaqus/Standard, these analyses remain challenging given the discontinuous nature of the fracture phenomenon. The following tips will help you create a successful Abaqus/Explicit model: • Dynamic effects are of utmost relevance when assessing the results from a debonding analysis using the VCCT criterion. In most cases experimental and/or theoretical data are available in quasi-static settings. You must ensure that the Abaqus/Explicit analysis generates low ratios of kinetic energy to internal energy (1% or less). In practical terms this requirement often translates into avoiding the use of mass scaling in the model. Use smooth amplitudes to drive the loading to help reduce the kinetic energy in the model. Running the analysis over a longer period of time will not help in most cases because bond breakage is an inherently fast and localized process. • If appropriate, use damping-like behavior in the materials associated with the debonding plates to reduce dynamic vibrations. Unlike Abaqus/Standard, where a pure static equilibrium is achieved at the end of a converged increment, in Abaqus/Explicit the bond breakage at a given location is associated with a dynamic overshoot beyond the static equilibrium position. If the vibrations are significant (kinetic energy is clearly observable), the dynamic overshoot at nodes behind the crack tip may lead to premature debonding of the crack tip. • To maximize the accuracy of the debonding simulation, use quad meshes between the slave and master surfaces of the debonding surfaces. Avoid using elements with aspect ratios greater than 2. In most cases mesh refinement will help with obtaining a realistic result. • Highly mismatched critical energy values between modes tend to induce crack propagation in continuously changing directions in a manner that may be unstable and unrealistic, particularly for modes II and III. Do not use such values unless experimental data suggest so. • Use frequent field output requests to evaluate the debonding evolution as the analysis progresses. In some cases this can point to nontrivial modeling deficiencies that are difficult to identify from a simple data check analysis. • Avoid the use of other constraints involving nodes on both surfaces of the debonding interface because the cohesive contact forces will compete with the constraint forces to achieve global equilibrium. Bond breakage might be hard to interpret in these cases. Comparing VCCT and cohesive elements Using VCCT to solve delamination problems is very similar to using cohesive elements in Abaqus. Table 11.4.3–2 describes the advantages and disadvantages of the two approaches. For an example of the use of cohesive elements, see “Delamination analysis of laminated composites,” Section 2.7.1 of the Abaqus Benchmarks Manual. This example also shows the effect of viscous regularization on the predicted force-displacement response. Table 11.4.3–2 Comparing VCCT and cohesive elements. VCCT Cohesive Elements Simulation (mechanics)-driven crack propagation along a known crack surface. Models brittle fracture using LEFM only. Uses a surface-based framework. Does not require additional elements. Requires a pre-existing flaw at the beginning of the crack surface. Cannot model crack initiation from a surface that is not already cracked. Crack propagates when strain energy release rate exceeds fracture toughness. Multiple crack fronts/surfaces can be included. In Abaqus/Standard crack surfaces are rigidly bonded when uncracked. Requires user-specified fracture toughness of the bond. Simulation (mechanics)-driven crack propagation along a known crack surface. However, cohesive elements can also be placed between element faces as a mechanism for allowing individual elements to separate. Model brittle or ductile fracture for LEFM or EPFM. Very general interaction modeling capability is possible. Require definition of the connectivity and interconnectivity of cohesive elements with the rest of the structure. For accuracy, the mesh of cohesive elements may need to be smaller than the surrounding structural mesh and the associated “cohesive zone.” As a result, cohesive elements may be more expensive. Can model crack initiation from initially uncracked surfaces. The crack initiates when the cohesive traction stress exceeds a critical value. Crack propagates according to cohesive damage model, usually calibrated so that the energy released when the crack is fully open equals the critical strain energy release rate. Multiple crack fronts/surfaces can be included. Crack surfaces are joined elastically when uncracked in Abaqus/Standard. Require user-specified critical traction value and fracture toughness of the bond, as well as elasticity of the bonded surface. Measuring the critical strain energy release properties for VCCT You must obtain the critical strain energy release properties of the bonded surfaces for VCCT. The procedure to obtain the critical strain energy release properties is beyond the scope of this manual; however, you can refer to the following ASTM test specifications for guidance: • ASTM D 5528-94a, “Standard Test Method for Mode I Interlaminar Fracture Toughness of Unidirectional Fiber-Reinforced Polymer Matrix Composites” • ASTM D 6671-01, “Standard Test Method for Mixed Mode I-Mode II Interlaminar Fracture Toughness of Unidirectional Fiber-Reinforced Polymer Matrix Composites” • ASTM D 6115-97, “Standard Test Method for Mode I Fatigue Delamination Growth Onset of Unidirectional Fiber-Reinforced Polymer Matrix Composites” These test specifications can be found in the Annual Book of ASTM Standards, American Society for Testing and Materials, vol. 15.03, 2000. Initial conditions Initial contact conditions are used to identify which part of the slave surface is initially bonded, as explained earlier. Boundary conditions Boundary conditions should not be applied to any of the nodes on the master or slave crack surfaces, but they can be used to load the structure and cause crack propagation. Boundary conditions can be applied to any of the displacement degrees of freedom in a crack propagation analysis (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). In a low-cycle fatigue analysis, prescribed boundary conditions must have an amplitude definition that is cyclic over the step: the start value must be equal to the end value . Loads The following types of loading can be prescribed in a crack propagation analysis: • Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 33.4.2. • Distributed pressure forces or body forces can be applied; see “Distributed loads,” Section 33.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” For a low-cycle fatigue analysis each load must have an amplitude definition that is cyclic over the step: the start value must be equal to the end value . Predefined fields The following predefined fields can be specified in a crack propagation analysis, as described in “Predefined fields,” Section 33.6.1: • Although temperature is not a degree of freedom in stress/displacement elements, nodal The specified temperature affects if temperatures can be specified as predefined fields. temperature-dependent critical stress and crack opening displacement specified. failure criteria, • The values of user-defined field variables can be specified. These values affect field-variable- dependent critical stress and crack opening displacement failure criteria, if specified. The temperatures and user-defined field variables on slave and master surfaces are averaged to determine the critical stresses and crack opening displacements. In a low-cycle fatigue analysis, the temperature values specified must be cyclic over the step: the start value must be equal to the end value . If the temperatures are read from the results file, you should specify initial temperature conditions equal to the temperature values at the end of the step . Alternatively, you can ramp the temperatures back to their initial condition values, as described in “Predefined fields,” Section 33.6.1. Material options Any of the mechanical constitutive models in Abaqus/Standard can be used to model the mechanical behavior of the cracking material. See Part V, “Materials.” Elements Regular, rectangular meshes give the best results in crack propagation analyses. Results with nonlinear materials are more sensitive to meshing than results with small-strain linear elasticity. First-order elements generally work best for crack propagation analysis. Line spring elements cannot be used in crack propagation analysis. The VCCT, enhanced VCCT, and low-cycle fatigue criteria not only support two-dimensional models (planar and axisymmetric) but also three-dimensional models with contact pairs involving first-order underlying elements (solids, shells, and continuum shells). In Abaqus/Standard use of the VCCT or enhanced VCCT criterion in two-dimensional models with contact pairs involving higher-order underlying elements is limited to crack fronts that are aligned with the corner nodes of the higher-order element faces. Use of the low-cycle fatigue criterion with contact pairs involving higher-order underlying elements is not supported. Output Unless otherwise stated, the following discussions in this section are applied only to the critical stress, critical crack opening displacement, and crack length versus time criteria. At the start of an analysis Abaqus/Standard will scan the partially bonded surfaces and identify all of the crack tips that are present in the model. The initial contact status of all of the slave surface nodes is printed in the data (.dat) file. At this stage Abaqus/Standard will explicitly identify all the crack tips and mark them as crack 1, crack 2, etc. The slave and master surfaces that are associated with these cracks are also identified. The initial contact status of all of the slave surface nodes is also printed in the data (.dat) file for the VCCT, enhanced VCCT, and low-cycle fatigue criteria. Printing crack propagation information to the data file By default, crack propagation information will be printed to the data file during the analysis. For each crack that is identified Abaqus/Standard will print out the initial and current crack-tip node numbers, accumulated incremental crack length (distance from the initial crack tip to the current crack tip, measured along the slave surface), and the current value of the user-specified fracture criterion used. Crack propagation information cannot be printed to the data file in Abaqus/Explicit. Input File Usage: *DEBOND, SLAVE=slave, MASTER=master For example, if the crack opening displacement criterion is used, the printed output during the analysis will appear as follows in the data file: CRACK TIP LOCATION AND ASSOCIATED QUANTITIES INITIAL CRACK NUMBER SURFACE SURFACE CRACKTIP CRACKTIP INCREMENTAL COD CUMULATIVE CURRENT MASTER SLAVE CRITICAL ... ... ... NODE # ... NODE # ... LENGTH ... ... Writing crack propagation information to the results file In Abaqus/Standard you can choose to write the crack propagation information to the results (.fil) file. Input File Usage: *DEBOND, SLAVE=slave, MASTER=master, OUTPUT=FILE Writing crack propagation information to both the data file and the results file In Abaqus/Standard you can write the crack propagation information to both the data and the results files. Input File Usage: *DEBOND, SLAVE=slave, MASTER=master, OUTPUT=BOTH Controlling the output frequency In Abaqus/Standard you can control the output frequency in increments. By default, the crack-tip location and associated quantities will be printed every increment. Specify an output frequency of 0 to suppress crack propagation output. Input File Usage: *DEBOND, SLAVE=slave, MASTER=master, FREQUENCY=f Output variables The following bond failure quantities can be requested as surface output for all fracture criteria: DBT DBSF The time when bond failure occurred. For the VCCT, enhanced VCCT, and low- cycle fatigue criteria, this is the time when debonding initiates. Fraction of stress at bond failure that still remains. DBS DBS1i All components of remaining stress in the failed bond. 1i component of stress in the failed bond that remains ( ). For the VCCT, enhanced VCCT, and low-cycle fatigue criteria, the following additional variables can be also requested as surface output : CSDMG BDSTAT OPENBC CRSTS CRSTS1i ENRRT ENRRT1i EFENRRTR Overall value of the scalar damage variable. Bond state. The bond state varies between 1.0 (fully bonded) and 0.0 (fully unbonded). Relative displacement behind crack when the fracture criterion is met. All components of critical stress at failure 1i component of critical stress at failure ( All components of strain energy release rate. 1i component of strain energy release rate ( . Effective energy release rate ratio, ). ). Surface output requests provide the usual output of contact variables in addition to the above quantities. The bond failure quantities must be requested explicitly; otherwise, only the default output for contact will be given. Abaqus/CAE provides support for the visualization of time-history plots and X–Y plots of the variables that are written to the output database. Contour integrals Contour integrals can be requested for two-dimensional crack propagation analyses performed using the critical stress, critical crack opening displacement, or crack length versus time fracture criteria. If the contours are chosen so that the crack tip passes through the contour, the contour value will go to zero (as it should). Therefore, in crack propagation analysis contour integrals should be requested far enough from the crack tip that the crack tip does not pass through the contour, which is easily done by including all nodes along the bond surface in the crack-tip node set specified. See “Contour integral evaluation,” Section 11.4.2, for details on contour integral output. Input file template Abaqus/Standard analysis *HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions *INITIAL CONDITIONS, TYPE=CONTACT (, NORMAL) Data lines to specify initial conditions *SURFACE, NAME=slave Data lines to define slave surface *SURFACE, NAME=master Data lines to define master surface ** *CONTACT PAIR slave, master ** *STEP (, NLGEOM) *STATIC or *VISCO or *COUPLED TEMPERATURE-DISPLACEMENT *DEBOND, SLAVE=slave, MASTER=master Data lines to define debonding amplitude curve *FRACTURE CRITERION, TYPE=type, DISTANCE or NSET Data lines to define fracture criterion *BOUNDARY Data lines to define zero-valued or nonzero boundary conditions *CLOAD and/or *DLOAD and/or *TEMPERATURE and/or *FIELD Data lines to define loading ** *CONTOUR INTEGRAL, CONTOURS=n, TYPE=type **Contour integrals can be requested in a two-dimensional crack propagation analysis *CONTACT PRINT DBT, DBSF, DBS *EL PRINT JK, *END STEP ** *STEP *DIRECT CYCLIC, FATIGUE *DEBOND, SLAVE=slave, MASTER=master *FRACTURE CRITERION, TYPE=FATIGUE Data lines to define material constants used in Paris law and fracture criterion *BOUNDARY Data lines to define zero-valued or nonzero cyclic boundary conditions *CLOAD and/or *DLOAD and/or *TEMPERATURE and/or *FIELD Data lines to define cyclic loading ** *END STEP ** Abaqus/Explicit analysis *HEADING … *BOUNDARY Data lines to specify zero-valued boundary conditions *SURFACE, NAME=slave Data lines to define slave surface *SURFACE, NAME=master Data lines to define master surface ** *CONTACT CLEARANCE, NAME=clearance_name, SEARCH NSET=initially_bonded_nodeset_name *SURFACE INTERACTION, NAME=interaction_name *COHESIVE BEHAVIOR Data lines to specify elastic behavior *FRACTURE CRITERION, TYPE=VCCT, MIXED MODE BEHAVIOR=BK ** *STEP *DYNAMIC, EXPLICIT *CONTACT *CONTACT CLEARANCE ASSIGNMENT Data lines to assign a clearance name to a surface pair *CONTACT PROPERTY ASSIGNMENT Data lines to assign a surface interaction to a surface pair *END STEP ** Additional references • Benzeggagh, M., and M. Kenane, “Measurement of Mixed-Mode Delamination Fracture Toughness of Unidirectional Glass/Epoxy Composites with Mixed-Mode Bending Apparatus,” Composite Science and Technology, vol. 56, p. 439, 1996. • Reeder, J., S. Kyongchan, “Postbuckling and and D. R.. Ambur, Growth of Delaminations in Composite Plates Subjected to Axial Compression” 43rd AIAA/ASME/ASCE/AHS/ASC Structures, Structural Dynamics, and Materials Conference, Denver, Colorado, vol. 1746, p. 10, 2002. P. B. Chunchu, • Wu, E. M., and R. C. Reuter Jr., “Crack Extension in Fiberglass Reinforced Plastics,” T and M Report, University of Illinois, vol. 275, 1965. 11.5 Surface-based fluid modeling • “Surface-based fluid cavities: overview,” Section 11.5.1 • “Fluid cavity definition,” Section 11.5.2 • “Fluid exchange definition,” Section 11.5.3 • “Inflator definition,” Section 11.5.4 11.5.1 SURFACE-BASED FLUID CAVITIES: OVERVIEW Products: Abaqus/Standard Abaqus/Explicit References • “Fluid cavity definition,” Section 11.5.2 • “Fluid exchange definition,” Section 11.5.3 • “Inflator definition,” Section 11.5.4 Overview Surface-based fluid-filled cavities are modeled by: • using standard finite elements to model the fluid-filled structure; • using a surface definition to provide the coupling between the deformation of the fluid-filled structure and the pressure exerted by the contained fluid on the cavity boundary of the structure; • defining the fluid behavior; • using fluid exchange definitions to model the transfer of fluid between a cavity and the environment or between multiple cavities; and • using inflator definitions to infuse a gas mixture into a fluid cavity to simulate the inflation of an automotive airbag. The surface-based fluid cavity capability can be used to model a liquid or gas-filled structure. It supersedes the element-based hydrostatic fluid cavity capability in functionality and does not require the user to define fluid or fluid link elements. Introduction In certain applications it may be necessary to predict the mechanical response of a liquid-filled or a gas-filled structure. Examples include pressure vessels, hydraulic or pneumatic driving mechanisms, and automotive airbags. A primary difficulty in addressing such applications is the coupling between the deformation of the structure and the pressure exerted by the contained fluid on the structure. Figure 11.5.1–1 illustrates a simple example of a fluid-filled structure subjected to a system of external loads. The response of the structure depends not only on the external loads but also on the pressure exerted by the fluid, which, in turn, is affected by the deformation of the structure. The surface-based fluid cavity capability provides the coupling needed to analyze situations in which the cavity can be assumed completely filled by fluid with uniform properties and state. Applications with significant spatial variation within cavities cannot be modeled with this feature. For example, consider the fluid-structure interaction and coupled Eulerian-Lagrangian capabilities for applications involving sloshing and wave propagation through a fluid . fluid Figure 11.5.1–1 Fluid-filled structure. Discretizing the fluid cavity The boundary of the fluid cavity is defined by an element-based surface with normals pointing to the inside of the cavity. The underlying elements can be standard solid or structural elements as well as surface elements. Surface elements can be used to model holes in the structure or to fill in rigid regions where rigid or other load-carrying elements do not exist . Care must be taken when using surface elements such that nodes completely surrounded by only surface elements have proper boundary conditions. Consider the example presented in Figure 11.5.1–1. Solid elements are defined on the top and side of the cavity as indicated in Figure 11.5.1–2. A surface element is defined on the bottom rigid boundary of the cavity where no standard elements exist. The node located at the intersection of the axis of symmetry and the lower rigid boundary of the cavity must be restrained in the r- and z-directions because it is connected only to a surface element. The surface defining the cavity is based on the underlying solid and surface elements. In Abaqus/Explicit an additional user-defined volume can be added to the actual or geometric volume of the cavity. If the boundary of the cavity is not defined by an element-based surface, the fluid cavity is assumed to have a fixed volume that is equal to the added volume. axis of symmetry standard elements cavity reference node surface to define cavity surface element Figure 11.5.1–2 Axisymmetric model of fluid-filled structure. Defining the location of the cavity reference node A single node, known as the cavity reference node, is associated with a fluid cavity. This cavity reference node has a single degree of freedom representing the pressure inside the fluid cavity. The cavity reference node is also used in calculating the cavity volume. If the cavity is not bounded by symmetry planes, the surface defining the cavity must completely enclose the cavity to ensure proper calculation of its volume. In this case the location of the cavity reference node is arbitrary and does not have to lie inside the cavity. If, as a result of symmetry, only a portion of the cavity boundary is modeled with standard elements, the cavity reference node must be located on the symmetry plane or axis (Figure 11.5.1–2). If multiple symmetry planes exist, the cavity reference node must be located on the intersection of the symmetry planes (Figure 11.5.1–3). For an axisymmetric analysis the cavity reference node must be located on the axis of symmetry. These requirements are a consequence of the fluid cavity not being fully enclosed by the surface defining the cavity. Finite element calculations The finite element calculations for surface-based cavities are performed using volume elements as described in “Hydrostatic fluid calculations,” Section 3.8.1 of the Abaqus Theory Manual. The volume elements for a cavity are created internally by Abaqus using the surface facet geometry and the cavity reference node that you define. In Abaqus/Standard the surface facets are represented with the following element types: FAX2 and F2D2 (which are linear, 2-node, axisymmetric and planar elements, respectively) and F3D3 and F3D4 (which are linear, 3-node and 4-node three-dimensional elements, axis of symmetry cavity reference node symmetry plane Figure 11.5.1–3 Axisymmetric model with additional symmetry plane. respectively). Second-order facets in Abaqus are subdivided further into multiple linear facets or elements. Fluid cavity behavior The behavior of the fluid within the fluid-filled cavity can be based either on a hydraulic or a pneumatic model. The hydraulic model can simulate nearly incompressible fluid behavior and fully incompressible behavior in Abaqus/Standard. The compressibility is introduced by defining a bulk modulus. The pneumatic model is based on an ideal gas. The gas can be defined by multiple species in Abaqus/Explicit, and you can specify the temperature of the gas or have it calculated based on the assumption of adiabatic behavior. A multi-species ideal gas with an adiabatic temperature update is an appropriate model for automotive airbags. Modeling flow into or out of a cavity There are many ways in Abaqus to model the transfer of fluid into or out of a cavity. The flow can be specified as a prescribed mass or volume flux history or can model physical mechanisms due to a pressure differential such as venting through an exhaust orifice or leakage through a porous fabric. Fluid exchange definitions are used for this purpose and can model flow between a fluid cavity and its environment or between two fluid cavities . In addition, Abaqus/Explicit has the capability to model inflators used for the deployment of automotive airbags. Conditions at the inflator can be specified directly, or tank test data can be used . Modeling multiple chambers Many fluid-filled systems such as airbags have multiple chambers with fluid flowing between chambers through holes or fabric leakage. In other cases it is advantageous to divide a single physical chamber into multiple chambers with fictitious walls to model a gradient in pressure across the physical chamber. Some fictitious leakage mechanisms through inter-chamber walls can be defined to obtain reasonable behavior. This can be a useful modeling technique when simulating the complex unfolding of an airbag. To model multiple chambers, define a fluid cavity for each chamber and link the fluid cavities together with the appropriate fluid exchange definitions. Averaged properties for the multi-chambered model can be output if requested . Defining the fluid inertia in a dynamic procedure The inertia of the fluid inside a fluid cavity or fluid exchanged between cavities is not automatically taken into account. To add the effect of inertia, use MASS elements on the boundary of the cavity. You should make sure that the total added mass corresponds to the mass of the fluid in the cavity and that the distribution of the MASS elements is a reasonable representation of the distributed fluid mass for the type of loading to which the structure is subjected. Only the overall effect of the fluid inertia can be modeled; the uniform pressure assumption in the cavity makes it impossible to model any pressure gradient-driven fluid motions. Thus, the approach assumes that the time scale of the excitation is very long compared to typical response times for the fluid. Modeling contact involving the cavity boundary If a large amount of fluid is removed from a cavity or the material surrounding the cavity is very flexible, the cavity may partially collapse and portions of the cavity walls may contact each other. Self-contact of the cavity walls and contact with surrounding structures can be handled effectively by using the standard techniques available in Abaqus for modeling contact. Abaqus/Explicit can also account for the blockage of flow out of a cavity due to contacting surfaces . Interpreting negative eigenvalue messages In some applications in Abaqus/Standard, negative eigenvalues may be encountered during the solution. These negative eigenvalues do not necessarily indicate that a bifurcation or buckling load has been exceeded. If the predicted response otherwise appears to be reasonable, these messages can be ignored. A detailed description of how negative eigenvalues can develop during the solution of hydrostatic fluid element problems is presented in “Hydrostatic fluid calculations,” Section 3.8.1 of the Abaqus Theory Manual. Procedures The surface-based fluid cavity capability can be used in all procedures except coupled pore fluid diffusion/stress analysis . Initial conditions The initial fluid pressure and temperature can be specified . For an ideal gas the initial pressure represents the gauge pressure over and above the ambient pressure. The initial temperature should be given in the temperature scale used. Absolute zero in that temperature scale is specified separately for an ideal gas . If membrane elements are used as the underlying elements for the fluid cavity, the reference mesh (initial metric) can also be specified . Boundary conditions The pressure degree of freedom at the cavity reference node (degree of freedom number 8) is a primary variable in the problem. Thus, it can be prescribed by defining a boundary condition , similar to the way displacements of structural nodes can be prescribed. Prescribing the pressure at the cavity reference node is equivalent to applying a uniform pressure to the cavity boundary using a distributed load definition . If the pressure is prescribed with a boundary condition, the fluid volume is adjusted automatically to fill the cavity (that is, fluid is assumed to enter and leave the cavity as needed to maintain the prescribed pressure). This behavior is useful in situations where a cavity is deformed prior to the introduction of the effect of the fluid. In a subsequent step you can remove the boundary condition on the pressure degree of freedom , thus “sealing” the cavity with the current fluid volume. Loads Distributed pressures and body forces, as well as concentrated nodal forces, can be applied to the fluid-filled structure, as described in “Concentrated loads,” Section 33.4.2, and “Distributed loads,” Section 33.4.3. Predefined fields Predefined temperature fields and user-defined field variables can be defined for both fluid-filled structures and the enclosed fluids, as described in “Predefined fields,” Section 33.6.1. Temperatures Fluid temperatures can be specified at all cavity reference nodes as predefined fields , unless an adiabatic process is specified or a coupled temperature-displacement procedure is used. Any difference between the applied and initial temperatures will cause thermal expansion for a pneumatic fluid and for a hydraulic fluid if a thermal expansion coefficient is given. A specified temperature field can also affect temperature-dependent material properties, if any exist, for both fluid-filled structures and enclosed fluids. Field variables The values of user-defined field variables can be specified at all cavity reference nodes . These values will affect field-variable-dependent material properties for the enclosed fluid. Output The state of the fluid inside the cavity is available for history output using the nodal output variables PCAV and CVOL, which represent the gauge fluid pressure and cavity volume, respectively. In steady- state dynamic procedures the magnitude and phase angle of the fluid pressure can be obtained as nodal variable PPOR. Abaqus/Explicit also provides output for the cavity temperature, cavity surface area, and mass of the fluid (nodal output variables CTEMP, CSAREA, and CMASS, respectively). Output variable CTEMP is available only when an ideal gas model is used under adiabatic conditions. If the node set for which the output request is made contains more than one fluid cavity, the time histories of the average fluid pressure, total volume, average fluid temperature, sum of all the external cavity surface areas, and total mass of these cavities will also be output by using the nodal output variables APCAV, TCVOL, ACTEMP, TCSAREA, and TCMASS, respectively. In Abaqus/Explicit, when the model includes fluid exchange definitions, use nodal output variables CMFL and CMFLT to obtain history output of the total mass flow rate and total accumulated mass flow out of a cavity and CEFL and CEFLT to obtain history output of the total heat energy flow rate and total accumulated heat energy flow out of a cavity. If more than one fluid exchange is defined for a cavity, time histories of the mass or heat energy flow rate and accumulated mass or heat energy flow out of the cavity for each fluid exchange will also be output. If the fluid cavity is modeled by a mixture of ideal gases, time histories of the molecular mass fraction of each fluid species inside the fluid cavity can be obtained by using nodal output variable CMF. If inflators are used, use nodal output variables MINFL, MINFLT, and TINFL to obtain time histories of mass flow rate, accumulated mass flow, and inflator temperature for each inflator definition . Input file template An analysis with hydrostatic fluid: *HEADING … *FLUID CAVITY, NAME=cavity_name, BEHAVIOR=behavior_name, REF NODE=cavity_reference_node, SURFACE=surface_name *FLUID BEHAVIOR, NAME=behavior_name *FLUID DENSITY Data line to define density *FLUID BULK MODULUS Data line to define bulk modulus *FLUID EXPANSION Data line to define thermal expansion ** *FLUID EXCHANGE, NAME=exchange_name, PROPERTY=exchange_property_name cavity_reference_node *FLUID EXCHANGE PROPERTY, NAME=exchange_property_name, TYPE=MASS FLUX Data line to define mass flow rate per unit area ** *INITIAL CONDITIONS, TYPE=TEMPERATURE Data line to define initial temperature *INITIAL CONDITIONS, TYPE=FLUID PRESSURE Data line to define initial pressure ** *STEP ** *TEMPERATURE Data line to define temperature *FLUID EXCHANGE ACTIVATION exchange_name ** *END STEP An airbag analysis with a mixture of ideal gases: *HEADING … *FLUID CAVITY, NAME=chamber_1, MIXTURE=MOLAR FRACTION, ADIABATIC, REF NODE=chamber_1_reference_node, SURFACE=surface_name_1 blank line Oxygen, 0.2 Nitrogen, 0.75 Carbon_dioxide, 0.05 ** *FLUID CAVITY, NAME=chamber_2, BEHAVIOR=Air, ADIABATIC, REF NODE=chamber_2_reference_node, SURFACE=surface_name_2 blank line ** *FLUID BEHAVIOR, NAME=Air *CAPACITY, TYPE=POLYNOMIAL Data line to define heat capacity coefficient *MOLECULAR WEIGHT Data line to define molecular weight ** *FLUID BEHAVIOR, NAME=Oxygen *CAPACITY, TYPE=POLYNOMIAL Data line to define heat capacity coefficient *MOLECULAR WEIGHT Data line to define molecular weight ** *FLUID BEHAVIOR, NAME=Nitrogen *CAPACITY, TYPE=POLYNOMIAL Data line to define heat capacity coefficient *MOLECULAR WEIGHT Data line to define molecular weight ** *FLUID BEHAVIOR, NAME=Carbon_dioxide *CAPACITY, TYPE=POLYNOMIAL Data line to define heat capacity coefficient *MOLECULAR WEIGHT Data line to define molecular weight ** *FLUID INFLATOR, NAME=inflator, PROPERTY=inflator_property chamber_1_reference_node *FLUID INFLATOR PROPERTY, NAME=inflator_property, TYPE=TEMPERATURE AND MASS Data lines to define mass flow rate and gas temperature *FLUID INFLATOR MIXTURE, TYPE=MOLAR FRACTION, NUMBER SPECIES=2 Carbon_dioxide, Nitrogen Table to define molecular mass fraction ** *FLUID EXCHANGE, NAME=exhaust, PROPERTY=exhaust_behavior chamber_1_reference_node *FLUID EXCHANGE PROPERTY, NAME=exhaust_behavior, TYPE=ORIFICE Data line to specify orifice behavior *FLUID EXCHANGE, NAME=leakage_1, PROPERTY=fabric_behavior chamber_1_reference_node *FLUID EXCHANGE, NAME=leakage_2, PROPERTY=fabric_behavior chamber_2_reference_node *FLUID EXCHANGE PROPERTY, NAME=fabric_behavior, TYPE=FABRIC LEAKAGE Data line to specify fabric leakage behavior ** *FLUID EXCHANGE, NAME=chamber_wall, PROPERTY=wall_behavior, EFFECTIVE AREA= chamber_1_reference_node, chamber_2_reference_node *FLUID EXCHANGE PROPERTY, NAME=wall_behavior, TYPE=ORIFICE Data line to specify orifice behavior ** *AMPLITUDE, NAME=amplitude_name Data line to define amplitude variations *PHYSICAL CONSTANTS, UNIVERSAL GAS CONSTANT= ** *INITIAL CONDITIONS, TYPE=FLUID PRESSURE Data line to define initial pressure *INITIAL CONDITIONS, TYPE=TEMPERATURE Data line to define initial temperature ** *STEP ** *FLUID EXCHANGE ACTIVATION exhaust, leakage_1, leakage_2, chamber_wall *FLUID INFLATOR ACTIVATION, INFLATION TIME AMPLITUDE=amplitude_name inflator ** *END STEP 11.5.2 FLUID CAVITY DEFINITION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Surface-based fluid cavities: overview,” Section 11.5.1 • “Fluid exchange definition,” Section 11.5.3 • *CAPACITY • *FLUID BEHAVIOR • *FLUID BULK MODULUS • *FLUID CAVITY • *FLUID DENSITY • *MOLECULAR WEIGHT • “Defining a fluid cavity interaction,” Section 15.13.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a fluid cavity interaction property,” Section 15.14.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A surface-based fluid cavity: • can be used to model a liquid-filled or gas-filled structure; • is associated with a node known as the cavity reference node; • is defined by specifying a surface that fully encloses the cavity; • is applicable only for situations where the pressure and temperature of the fluid in a particular cavity are uniform at any point in time; • can be used to model an airbag using the assumptions of an ideal gas mixture under adiabatic conditions; and • has a name that can be used to identify history output associated with the cavity. Defining the fluid cavity You must associate a name with each fluid cavity. Input File Usage: Abaqus/CAE Usage: *FLUID CAVITY, NAME=name Interaction module: Create Interaction: Fluid cavity, Name: name Specifying the cavity reference node Every fluid cavity must have an associated cavity reference node. Along with the fluid cavity name, the reference node is used to identify the fluid cavity. In addition, it may be referenced by fluid exchange and inflator definitions. The reference node should not be connected to any elements in the model. Input File Usage: Abaqus/CAE Usage: *FLUID CAVITY, REF NODE=n Interaction module: Create Interaction: Fluid cavity: select the fluid cavity reference node Specifying the boundary of the fluid cavity The fluid cavity must be completely enclosed by finite elements unless symmetry planes are modeled . Surface elements can be used for portions of the cavity surface that are not structural. The boundary of the cavity is specified using an element-based surface covering the elements that surround the cavity with surface normals pointing inward. By default, an error message is issued if the underlying elements of the surface do not have consistent normals. Alternatively, you can skip the consistency checking for the surface normals. Input File Usage: Use the following option to define the surface with consistent normal checking: *FLUID CAVITY, SURFACE=surface_name, CHECK NORMALS=YES Use the following option to define the surface without consistent normal checking: *FLUID CAVITY, SURFACE=surface_name, CHECK NORMALS=NO Interaction module: Create Interaction: Fluid cavity: select the fluid cavity boundary surface; toggle on or off Check surface normals Abaqus/CAE Usage: Specifying additional volume in a fluid cavity An additional volume can be specified for a fluid cavity in Abaqus/Explicit. The additional volume will be added to the actual volume when the boundary of the cavity is defined by a specified surface. If you do not specify a surface forming the boundary of the fluid cavity, the fluid cavity is assumed to have a fixed volume that is equal to the added volume. Input File Usage: Abaqus/CAE Usage: *FLUID CAVITY, ADDED VOLUME=r Specification of additional volume is not supported in Abaqus/CAE. Specifying the minimum volume When the volume of a fluid cavity is extremely small, transients in an explicit dynamic procedure can cause the volume to go to zero or even negative causing the effective cavity stiffness values to tend to infinity. To avoid numerical problems, you can specify a minimum volume for the fluid in Abaqus/Explicit. If the volume of the cavity (which is equal to the actual volume plus the added volume) drops below the minimum, the minimum value is used to evaluate the fluid pressure. You can specify the minimum volume either directly or as the initial volume of the fluid cavity. If the latter method is used and the initial volume of the fluid cavity is a negative value, the minimum volume is set equal to zero. Input File Usage: Use the following option to specify the minimum volume directly: *FLUID CAVITY, MINIMUM VOLUME=minimum volume Use the following option to specify the minimum volume to be equal to the initial volume: Abaqus/CAE Usage: *FLUID CAVITY, MINIMUM VOLUME=INITIAL VOLUME Specification of a minimum volume is not supported in Abaqus/CAE. Defining the fluid cavity behavior The fluid cavity behavior governs the relationship between cavity pressure, volume, and temperature. A fluid cavity in Abaqus/Standard can contain only a single fluid. In Abaqus/Explicit a cavity can contain a single fluid or a mixture of ideal gases. Fluid behavior with a homogeneous fluid To define a fluid cavity behavior made of a single fluid, specify a single fluid behavior to define the fluid properties. You must associate the fluid behavior with a name. This name can then be used to associate a certain behavior with a fluid cavity definition. Input File Usage: Use the following options: Abaqus/CAE Usage: *FLUID CAVITY, NAME=fluid_cavity_name, BEHAVIOR=behavior_name *FLUID BEHAVIOR, NAME=behavior_name Interaction module: Create Interaction Property: Fluid cavity, Name: behavior_name Fluid behavior with a mixture of ideal gases in Abaqus/Explicit In Abaqus/Explicit you can define a fluid cavity behavior made of multiple gas species. To define a fluid cavity behavior made of multiple gas species, you specify multiple fluid behaviors to define the fluid properties. Specify the names of the fluid behaviors and the initial mass or molar fractions defining the mixture to associate a certain group of behaviors with a fluid cavity definition. Input File Usage: Use the following options to define the fluid cavity mixture in terms of the initial mass fraction: *FLUID BEHAVIOR, NAME=behavior_name *FLUID CAVITY, NAME=fluid_cavity_name, MIXTURE=MASS FRACTION out-of-plane surface thickness (if required; otherwise, blank) behavior_name, initial mass fraction ... Use the following options to define the fluid cavity mixture in terms of the initial molar fraction: *FLUID BEHAVIOR, NAME=behavior_name *FLUID CAVITY, NAME=fluid_cavity_name, MIXTURE=MOLAR FRACTION out-of-plane surface thickness (if required; otherwise, blank) behavior_name, initial molar fraction ... Abaqus/CAE Usage: Specification of ideal gas mixtures is not supported in Abaqus/CAE. User-defined fluid behavior in Abaqus/Standard In Abaqus/Standard the fluid behavior can be defined in user subroutine UFIELD. *FLUID BEHAVIOR, USER User subroutine UFIELD is not supported in Abaqus/CAE. Abaqus/CAE Usage: Input File Usage: Defining the ambient pressure for a fluid cavity For pneumatic fluids the equilibrium problem is generally expressed in terms of the “gauge” pressure in the fluid cavity (that is, ambient atmospheric pressure does not contribute to the loading of the solid and structural parts of the system). You can choose to convert gauge pressure to absolute pressure as used in the constitutive law. For hydraulic fluids you can define the ambient pressure, which can be used to calculate the pressure difference in the fluid exchange between a fluid cavity and its environment. The pressure value given as degree of freedom 8 at the cavity reference node is the value of the gauge pressure. The ambient pressure, , is assumed to be zero if you do not specify it. Input File Usage: Abaqus/CAE Usage: *FLUID CAVITY, AMBIENT PRESSURE= Interaction module: Create Interaction: Fluid cavity: toggle on Specify ambient pressure: Isothermal process For hydraulic fluids and pneumatic fluids in problems of long time duration, it is reasonable to assume that the temperature is constant or a known function of the environment surrounding the cavity. In this case the temperature of the fluid can be defined by specifying initial conditions and predefined temperature fields at the cavity reference node. For a pneumatic fluid the pressure and density of the gas are calculated from the ideal gas law, conservation of mass, and the predefined temperature field. Defining the ambient temperature for a fluid cavity For pneumatic fluids with adiabatic behavior the ambient temperature is needed when the heat energy flow is defined between a single cavity and its environment and the flow definition is based on analysis conditions. The ambient temperature, , is assumed to be zero if you do not specify it. Input File Usage: Abaqus/CAE Usage: *FLUID CAVITY, AMBIENT TEMPERATURE= Specification of ambient temperature is not supported in Abaqus/CAE. Hydraulic fluids The hydraulic fluid model is used to model nearly incompressible fluid behavior and fully incompressible fluid behavior in Abaqus/Standard. Compressibility is introduced by assuming a linear pressure-volume relationship. The required parameters for compressible behavior are the bulk modulus and the reference density. You omit the bulk modulus to specify fully incompressible behavior in Abaqus/Standard. Temperature dependence of the density can be modeled as a thermal expansion of the fluid. Input File Usage: Abaqus/CAE Usage: *FLUID CAVITY, BEHAVIOR=behavior_name Interaction module: Create Interaction Property: Fluid cavity: Definition: Hydraulic Defining the reference fluid density The reference fluid density, , is specified at zero pressure and the initial temperature, : Input File Usage: Abaqus/CAE Usage: *FLUID DENSITY Interaction module: Create Interaction Property: Fluid cavity: Definition: Hydraulic: Fluid density: density Defining the fluid bulk modulus for compressibility The compressibility is described by the bulk modulus of the fluid: where is the current pressure, is the current temperature, is the fluid bulk modulus, is the current fluid volume, is the density at current pressure and temperature, is the fluid volume at zero pressure and current temperature, is the fluid volume at zero pressure and initial temperature, and is the density at zero pressure and current temperature. It is assumed that the bulk modulus is independent of the change in fluid density. However, the bulk Input File Usage: modulus can be specified as a function of temperature or predefined field variables. *FLUID BULK MODULUS Interaction module: Create Interaction Property: Fluid cavity: Definition: Hydraulic: Fluid Bulk Modulus tabbed page: toggle on Specify fluid bulk modulus, and enter the modulus value in the table Abaqus/CAE Usage: Use the following options to include temperature and field variable dependence: Toggle on Use temperature-dependent data, Number of field variables: n Defining the fluid expansion The thermal expansion coefficients are interpreted as total expansion coefficients from a reference temperature, which can be specified as a function of temperature or predefined field variables. The change in fluid volume due to thermal expansion is determined as follows: where (secant) coefficient of thermal expansion. is the reference temperature for the coefficient of thermal expansion and is the mean of If the coefficient of thermal expansion is not a function of temperature or field variables, the value is not needed. Thermal expansion can also be expressed in terms of the fluid density: Input File Usage: Abaqus/CAE Usage: *FLUID EXPANSION, ZERO= Interaction module: Create Interaction Property: Fluid cavity: Definition: Hydraulic: Fluid Expansion tabbed page: toggle on Specify fluid thermal expansion coefficients, and enter the mean coefficient of thermal expansion in the table Use the following options to include temperature and field variable dependence: Toggle on Use temperature-dependent data, Reference temperature: , Number of field variables: n Pneumatic fluids Compressible or pneumatic fluids are modeled as an ideal gas . The equation of state for an ideal gas (or the ideal gas law) is given as where the absolute (or total) pressure is defined as is the ambient pressure, p is the gauge pressure, R is the gas constant, is the current temperature, is absolute zero on the temperature scale being used. The gas constant, R, can also be determined and and from the universal gas constant, , and the molecular weight, , as follows: Conservation of mass gives the change of mass in the fluid cavity as where m is the mass of the fluid, flow rate out of the fluid cavity. Defining the molecular weight is the mass flow rate into the fluid cavity, and is the mass You must specify the value of the molecular weight of the ideal gas, . Input File Usage: *MOLECULAR WEIGHT Abaqus/CAE Usage: Interaction module: Create Interaction Property: Fluid cavity: Definition: Pneumatic, Ideal gas molecular weight: Specifying the value of the universal gas constant You can specify the value of the universal gas constant, . *PHYSICAL CONSTANTS, UNIVERSAL GAS CONSTANT= All modules: Model→Edit attributes→model name: Physical Constants: toggle on Universal gas constant: Input File Usage: Abaqus/CAE Usage: Specifying the value of absolute zero You can specify the value of absolute zero temperature, . Input File Usage: Abaqus/CAE Usage: *PHYSICAL CONSTANTS, ABSOLUTE ZERO= All modules: Model→Edit attributes→model name: Physical Constants: toggle on Absolute zero temperature: Adiabatic process By default, the fluid temperature is defined by the predefined temperature field at the cavity reference node. However, for rapid events the fluid temperature in Abaqus/Explicit can be determined from the conservation of energy assumed in an adiabatic process. With this assumption, no heat is added or removed from the cavity except by transport through fluid exchange definitions or inflators. An adiabatic process is typically well suited for modeling the deployment of an airbag. During deployment, the gas jets out of the inflator at high pressure and cools as it expands at atmospheric pressure. The expansion is so quick that no significant amount of heat can diffuse out of the cavity. The energy equation can be obtained from the first law of thermodynamics. By neglecting the kinetic and potential energy, the energy equation for a fluid cavity is given by where the work done by the fluid cavity expansion is given as is the heat energy flow rate due to the heat transfer through the surface of the fluid cavity. A will generate the heat energy flow out of the primary fluid cavity. The specific and positive value for energy is given by is the initial specific energy at the initial temperature where is the specific heat at constant volume (or the constant volume heat capacity), which depends only upon temperature for an ideal gas, is the specific enthalpy, and V is the volume occupied by the gas. By definition, the specific enthalpy , is is the initial specific enthalpy at the initial (or reference) temperature where is the specific heat at constant pressure, which depends only upon temperature for an ideal gas. The pressure, temperature, and density of the gas are obtained by solving the ideal gas law, the energy balance, and mass conservation. and Adiabatic behavior will always be used for the fluid cavity if an adiabatic or coupled procedure is used. Input File Usage: Abaqus/CAE Usage: *FLUID CAVITY, ADIABATIC Interaction module: Create Interaction: Fluid cavity: Property definition: Pneumatic, toggle on Use adiabatic behavior Defining the heat capacity at constant pressure The heat capacity at constant pressure must be specified when modeling an adiabatic process for the ideal gas. It can be defined either in polynomial or tabular form. The polynomial form is based on the Shomate equation according to the National Institute of Standards and Technology. The constant pressure molar heat capacity can be expressed as are gas constants. These gas constants together with molecular where the coefficients weight are listed in Table 11.5.2–1 for some gases that are often used in airbag simulations. The constant pressure heat capacity can then be obtained by , and , , , The constant volume heat capacity, , can be determined by Table 11.5.2–1 Properties of some commonly used gases (SI units). Gas MW (× 10−3 ) (× 10−6) (× 10−9 ) (× 106 ) (kelvin) Air 0.0289 28.110 Nitrogen 0.028 26.092 Oxygen 0.032 29.659 1.967 8.218 6.137 Hydrogen 0.00202 33.066 −11.36 0.028 25.567 6.096 4.802 –1.976 –1.186 11.432 4.054 −1.966 0.1592 0.0957 –2.772 −2.671 0.0 273–1800 0.0444 298–6000 –0.219 298–6000 –0.158 273–1000 0.131 298–1300 0.044 24.997 55.186 −33.691 7.948 –0.136 298–1200 0.0180 32.240 1.923 0.105 −3.595 0.0 273–1800 Carbon monoxide Carbon dioxide Water vapor You can use the polynomial form for specifying the heat capacity at constant pressure, in which , and . Alternatively, you can define a table of constant pressure case you enter the coefficients , , heat capacity versus temperature and any predefined field variables. , Input File Usage: Use the following option to specify the heat capacity in polynomial form: *CAPACITY, TYPE=POLYNOMIAL , , , , Use the following option to specify the heat capacity in tabular form: *CAPACITY, TYPE=TABULAR, DEPENDENCIES=n , temperature, field_variable_1, etc... ... Abaqus/CAE Usage: Use the following option to specify the heat capacity in polynomial form: Interaction module: Create Interaction Property: Fluid cavity: Definition: Pneumatic, toggle on Specify molar heat capacity: Polynomial, Polynomial Coefficients: , , , , Use the following option to specify the heat capacity in tabular form: Interaction module: Create Interaction Property: Fluid cavity: Definition: Pneumatic: toggle on Specify molar heat capacity: Tabular: enter the molar heat capacity Use the following options to include temperature and field variable dependence in the table: Toggle on Use temperature-dependent data, Number of field variables: n A mixture of ideal gases Abaqus/Explicit can model a mixture of ideal gases in the fluid cavity. For ideal gas mixtures the Amagat- Leduc rule of partial volumes is used to obtain an estimate of the molar-averaged thermal properties (Van Wylen and Sonntag, 1985). Let each species have constant pressure and volume heat capacities, and . The constant pressure and volume heat capacities ; and mass fraction, ; molecular weight, for the mixed gas are then given by and the molecular weight is given by The specific energy and enthalpy for the mixed gas are then given by The energy flow entering the fluid cavity is given by and the energy flow out of the fluid cavity is given by Using the properties of a mixture of ideal gases as given above, the pressure and temperature can be obtained from the ideal gas law and the energy equation. Averaged properties for multiple fluid cavities If the output of the state of the fluid inside the cavity is requested for a node set that contains more than one fluid cavity, the averaged properties of the multiple fluid cavities will also be output automatically. The average pressure is calculated by volume weighting cavity pressure contributions. The average temperature for an adiabatic ideal gas is obtained by mass weighting cavity temperature contributions. Let each fluid cavity have pressure . The average pressure of the fluid cavity cluster is then defined as , gas constant , temperature , and mass , volume and the average temperature is Additional reference • Van Wylen, G. J., and R. E. Sonntag, Fundamentals of Classical Thermodynamics, Wiley, New York, 1985. 11.5.3 FLUID EXCHANGE DEFINITION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Surface-based fluid cavities: overview,” Section 11.5.1 • “Fluid cavity definition,” Section 11.5.2 • *FLUID EXCHANGE • *FLUID EXCHANGE PROPERTY • *FLUID EXCHANGE ACTIVATION • “VUFLUIDEXCH,” Section 1.2.12 of the Abaqus User Subroutines Reference Manual • “VUFLUIDEXCHEFFAREA,” Section 1.2.13 of the Abaqus User Subroutines Reference Manual • “Defining a fluid exchange interaction,” Section 15.13.12 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a fluid exchange interaction property,” Section 15.14.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A fluid exchange definition: • can be used to model flow between a single fluid cavity and its environment or flow between two fluid cavities; • can be used to prescribe mass- or volume-based flux into or out of a cavity; • can model the venting of a cavity through an exhaust orifice; • can model flow through cavity walls such as leakage through a porous fabric; • can be used to prescribe heat loss through a cavity surface due to heat transfer; • can take the local material state into account; • can account for blockage due to contacting boundary surfaces; and • has a name that can be used to identify history output of mass flow rates out of a cavity. Defining fluid exchange The fluid exchange capability is very general and can be used to define flow in and out of a cavity either as a prescribed function or based on the pressure difference arising from analysis conditions. The flow behavior in Abaqus/Standard is based on mass fluid flow, and the behavior in Abaqus/Explicit can be based on mass fluid flow or heat energy flow. You must associate the fluid exchange definition with a name. Input File Usage: *FLUID EXCHANGE, NAME=name Abaqus/CAE Usage: Interaction module: Create Interaction: Fluid exchange, Name: name Flow between a single cavity and its environment To define flow between a fluid cavity and its environment, specify the single reference node associated with the fluid cavity. In the discussion that follows this fluid cavity is referred to as the primary cavity. When the flow is defined as a prescribed function, the flow can either be into or out of the primary cavity. If the flow is into the cavity, the properties of the material flowing in are assumed to be the instantaneous properties of the material in the cavity itself. When the flow behavior is based on analysis conditions, the mass flow can occur only out of the primary cavity but the heat energy flow can be either into or out of the primary cavity. For the case of mass flow Abaqus will use the fluid cavity pressure and the specified constant ambient pressure to calculate the pressure difference used to determine the mass flow rate. For the case of heat energy flow Abaqus/Explicit will use the fluid cavity temperature and the specified constant ambient temperature to calculate the temperature difference used to determine the heat energy flow rate. Input File Usage: Use the following options: *FLUID CAVITY, NAME=primary_cavity_name, REF NODE=primary_cavity_reference_node *FLUID EXCHANGE, NAME=fluid_exchange_name primary_cavity_reference_node Abaqus/CAE Usage: Interaction module: Create Interaction: Fluid exchange: Definition: To environment, Fluid cavity interaction: name, Fluid exchange property: name Flow between two fluid cavities To define flow between two fluid cavities, specify the reference nodes associated with the primary and secondary fluid cavities. When the flow is based on analysis conditions, the fluid will flow from the high pressure or upstream cavity to the low pressure or downstream cavity and the heat energy will flow from the high temperature to the low temperature. Input File Usage: Use the following options: *FLUID CAVITY, NAME=primary_cavity_name, REF NODE=primary_cavity_reference_node *FLUID CAVITY, NAME=secondary_cavity_name, REF NODE=secondary_cavity_reference_node *FLUID EXCHANGE, NAME=fluid_exchange_name primary_cavity_reference_node, secondary_cavity_reference_node Abaqus/CAE Usage: Interaction module: Create Interaction: Fluid exchange: Definition: Between cavities, Fluid cavity interaction 1: name, Fluid cavity interaction 2: name, Fluid exchange property: name Specifying the effective area The flow rate from the primary cavity for any fluid exchange property is proportional to the effective leakage area. The leakage area may represent the size of an exhaust orifice, the area of a porous fabric enclosing the cavity, or the size of a pipe between cavities. You can specify the value of the effective leakage area directly. Alternatively, in Abaqus/Explicit you can define a surface that represents the leakage area by specifying the name of the surface on the boundary enclosing the primary fluid cavity. The effective area for fluid exchange is based on the area of the surface unless you specify the area directly or define the effective area with user subroutine VUFLUIDEXCHEFFAREA. If both the effective area and a surface are specified, the area of the surface is used only to determine blockage; see “Accounting for blockage due to contacting boundary surfaces,” below. If neither area is specified, the effective area defaults to 1.0. You can also define the effective leakage area with user subroutine VUFLUIDEXCHEFFAREA if leakage needs to be modeled as a function of the material state in the underlying elements of the specified surface. For example, this subroutine can be used to define the leakage area at an element level for modeling fabric permeability in uncoated airbags where the leakage can vary locally depending on the strains in the yarn directions and the angle between the fabric yarns. Only membrane elements are supported for use with VUFLUIDEXCHEFFAREA. Input File Usage: Use the following option to specify the effective leakage area directly and to specify a surface that represents the leakage area: *FLUID EXCHANGE, EFFECTIVE AREA=effective_area, SURFACE=surface_name Use the following option to define the effective leakage area with a user subroutine: *FLUID EXCHANGE, EFFECTIVE AREA=USER, SURFACE=surface_name Abaqus/CAE Usage: Interaction module: Create Interaction: Fluid exchange: Effective exchange area: effective_area User subroutine VUFLUIDEXCHEFFAREA is not supported in Abaqus/CAE. Application of fluid cavity pressure on a fluid exchange surface You can control how the effect of the cavity pressure on a fluid exchange surface is accounted for in Abaqus/Explicit. By default, the cavity pressure generates forces at all of the fluid exchange surface nodes, using the same method as for other portions of the fluid cavity. Optionally, the resultant force of the cavity pressure on the fluid exchange surface can be distributed only among the perimeter nodes of the fluid exchange surface; this option can be used to avoid local bulging of a vent surface that can cause inaccurate computation of the leakage area. Input File Usage: Use the following option (default) to indicate that the fluid pressure should generate forces on all nodes of a fluid exchange surface: *FLUID EXCHANGE, CAVITY PRESSURE=SURFACE, SURFACE=surface_name Use the following option to indicate that the fluid pressure should generate force only on perimeter nodes of a fluid exchange: *FLUID EXCHANGE, CAVITY PRESSURE=PERIMETER, SURFACE=surface_name Abaqus/CAE Usage: You cannot change the default pressure application in Abaqus/CAE. The pressure is always applied to all of the fluid exchange surface nodes. Defining the fluid exchange property There are several different types of fluid exchange properties available in Abaqus to define the rate flow from a fluid cavity to the environment or between two cavities. The fluid exchange property can be as simple as prescribing the mass or volume flow rate directly. More complex leakage mechanisms such as those found on automotive airbags can be modeled by defining the mass or volume leakage rate as a function of the pressure difference, . The heat loss ; the absolute pressure, due to heat transfer through the surface of the cavity can be modeled in Abaqus/Explicit by prescribing the heat energy flow rate directly or by defining the heat energy flow rate as a function of the temperature difference, . Alternatively, in Abaqus/Explicit the ; and the temperature, mass flow rate and/or heat energy flow rate can be specified in user subroutine VUFLUIDEXCH. ; the absolute pressure, ; and the temperature, For the purposes of evaluating the mass flow rate between two cavities, the absolute pressure and temperature are taken from the high pressure or upstream cavity. The mass flow is always in the direction from the high pressure cavity to the low pressure or downstream cavity, and the heat energy flow is always in the direction from the high temperature cavity to the low temperature cavity. The cavity absolute pressure and temperature are always used to calculate the flow between a cavity and the environment. You must associate the fluid exchange property with a name. This name can then be used to associate a certain property with a fluid exchange definition. Input File Usage: Use the following options: Abaqus/CAE Usage: *FLUID EXCHANGE, NAME=fluid_exchange_name, PROPERTY=property_name *FLUID EXCHANGE PROPERTY, NAME=property_name Interaction module: Create Interaction Property: Fluid exchange, Name: property_name Specifying a mass or volume flux Fluid flux into or out of the primary fluid cavity can be defined directly by prescribing the mass flow rate per unit area, . The mass flow rate is where A is the effective area. . The mass flow rate is FLUID EXCHANGE where is the density. A negative value for or will generate flux into the primary fluid cavity. When a second fluid cavity is not defined, the state of the fluid flowing into the primary cavity is assumed to be that of the fluid already present in the primary cavity. Input File Usage: Abaqus/CAE Usage: To prescribe a flux based on mass flow rate: *FLUID EXCHANGE PROPERTY, TYPE=MASS FLUX To prescribe a flux based on volumetric flow rate: *FLUID EXCHANGE PROPERTY, TYPE=VOLUME FLUX Interaction module: Create Interaction Property: Fluid exchange: Definition: Mass flux or Volume flux Specifying the flow rate using the viscous and hydrodynamic resistance coefficients The mass flow rate, coefficients such as , can be related to pressure difference by both viscous and hydrodynamic resistance where is the pressure difference, A is the effective area, is the viscous resistance coefficient, and is the hydrodynamic resistance coefficient. The resistance coefficients can be functions of the average absolute pressure, average temperature, and average of any user-defined field variables. A positive value of corresponds to flow out of the first cavity. Input File Usage: *FLUID EXCHANGE PROPERTY, TYPE=BULK VISCOSITY, DEPENDENCIES=n viscous resistance coefficient ( ), hydrodynamic resistance coefficient ( ) Abaqus/CAE Usage: Interaction module: Create Interaction Property: Fluid exchange: Definition: Bulk viscosity: Viscous coefficient: : Hydrodynamic coefficient: Use the following options to include pressure, temperature, and field variable dependence: Toggle on Use pressure-dependent data, toggle on Use temperature-dependent data, Number of field variables: n Specifying the flow rate through a vent or exhaust orifice The mass flow rate through a vent or exhaust orifice that can be approximated by one-dimensional, quasi- steady, and isentropic flow is given (Bird, Stewart and Lightfoot, 2002) by where C is the dimensionless discharge coefficient, A is the vent or exhaust orifice area, temperature in the upstream fluid cavity, and is the is the absolute zero on the temperature scale being used, is the absolute pressure in the upstream fluid cavity. The pressure ratio, q, is defined as is the absolute pressure in the orifice. The critical pressure, where occurs is defined as , at which choked or sonic flow where is the ratio of the constant pressure heat capacity, , and the constant volume heat capacity, : The orifice pressure, , is then given by where pressure for flow between two fluid cavities. is equal to the ambient pressure for flow out of a single fluid cavity or the downstream cavity The value of the discharge coefficient can be a function of the absolute upstream pressure, upstream temperature, and any user-defined field variables. Fluid exchange through a vent or exhaust orifice is valid only for pneumatic fluids. Input File Usage: *FLUID EXCHANGE PROPERTY, TYPE=ORIFICE, DEPENDENCIES=n discharge coefficient Abaqus/CAE Usage: Fluid exchange through vents or orifices is not supported in Abaqus/CAE. Specifying the flow rate due to fabric leakage The mass flow rate due to leakage through fabric can be expressed as where C is the dimensionless fabric leakage or discharge coefficient and A is the effective fabric leakage area. The value of the discharge coefficient can be a function of absolute upstream pressure, upstream temperature, and any user-defined field variables. Input File Usage: *FLUID EXCHANGE PROPERTY, TYPE=FABRIC LEAKAGE, DEPENDENCIES=n discharge coefficient Abaqus/CAE Usage: Defining fluid exchange due to fabric leakage is not supported in Abaqus/CAE. Specifying a table of mass flow rate versus pressure difference The overall mass flow rate can be calculated from a specified mass flow rate per unit area, , by where A is the effective area. In this case you can define the mass flow rate per unit area in a table depending on the absolute value of pressure difference and, optionally, on the average absolute pressure, average temperature, and average value of any user-defined field variables. Values for must be positive and start from zero. and Input File Usage: *FLUID EXCHANGE PROPERTY, TYPE=MASS RATE LEAKAGE, DEPENDENCIES=n 0, 0 , ... Abaqus/CAE Usage: Interaction module: Create Interaction Property: Fluid exchange: Definition: Mass rate leakage: Mass Flow Rate: , Pressure Difference: Use the following options to include pressure, temperature, and field variable dependence: Toggle on Use pressure-dependent data, toggle on Use temperature-dependent data, Number of field variables: n Specifying a table of volumetric flow rate versus pressure difference The overall mass flow rate can be calculated from a specified volumetric flow rate per unit area, , by where A is the effective area and is the density. In this case you can define the volumetric flow rate per unit area in a table depending on the absolute value of pressure difference and, optionally, on the average absolute pressure, average temperature, and average value of any user-defined field variables. Values for must be positive and start from zero. and Input File Usage: *FLUID EXCHANGE PROPERTY, TYPE=VOLUME RATE LEAKAGE, DEPENDENCIES=n 0, 0 , ... Abaqus/CAE Usage: Interaction module: Create Interaction Property: Fluid exchange: Definition: Volume rate leakage: Volumetric Flow Rate: , Pressure Difference: Use the following options to include pressure, temperature, and field variable dependence: Toggle on Use pressure-dependent data, toggle on Use temperature-dependent data, Number of field variables: n Specifying a heat energy flux In Abaqus/Explicit heat energy flux into or out of the primary fluid cavity can be defined directly by prescribing the heat energy flow rate per unit area, . The heat energy flow rate is where A is the effective area. A positive value for generates heat flux out of the primary fluid cavity. Input File Usage: Abaqus/CAE Usage: *FLUID EXCHANGE PROPERTY, TYPE=ENERGY FLUX Defining fluid exchange by specifying the heat energy flow rate explicitly is not supported in Abaqus/CAE. Specifying a table of heat energy flow rate versus temperature difference The overall heat energy flow rate can be calculated from a specified heat energy flow rate per unit area, , by where A is the effective area. In this case in Abaqus/Explicit you can define the heat energy flow rate per unit area in a table depending on the absolute value of temperature difference and, optionally, on the average absolute pressure, average temperature, and average value of any user-defined field variables. Values for and must be positive and start from zero. Input File Usage: *FLUID EXCHANGE PROPERTY, TYPE=ENERGY RATE LEAKAGE, DEPENDENCIES=n 0, 0 , ... Abaqus/CAE Usage: Defining fluid exchange by specifying the heat energy flow rate as a function of temperature difference and pressure is not supported in Abaqus/CAE. Specifying mass flow rate and/or heat energy flow rate with a user subroutine The mass flow rate, , can be defined in Abaqus/Explicit using user subroutine VUFLUIDEXCH . , or the overall heat energy flow rate, Input File Usage: *FLUID EXCHANGE PROPERTY, TYPE=USER Abaqus/CAE Usage: User subroutine VUFLUIDEXCH is not supported in Abaqus/CAE. Activating the fluid exchange definition Fluid exchange will not occur in Abaqus/Explicit unless the fluid exchange definition is activated in an analysis step. Input File Usage: Use the following options to activate a fluid exchange for a given analysis step: *FLUID EXCHANGE, NAME=fluid_exchange_name *FLUID EXCHANGE ACTIVATION fluid_exchange_name Abaqus/CAE Usage: Fluid exchange is activated automatically for Abaqus/Explicit steps in Abaqus/CAE. Varying the magnitude of the flow By default, the magnitude of the flow is based on the specified flow behavior. A time variation of flow magnitude during a step can be introduced by an amplitude curve. The magnitude based on the specified flow behavior is multiplied by the amplitude value to obtain the actual mass or heat energy flow rate. For example, a time variation of prescribed mass or volumetric flux can be defined. An amplitude curve may be used to trigger an event for fluid exchange in the middle of a step. For example, an airbag may deploy at some predetermined time during a step, and it may be desirable to close off all exhaust orifices until the actual deployment. A step amplitude curve that starts at zero and steps up at deployment time could be used for this purpose. Input File Usage: Use the following options: Abaqus/CAE Usage: *AMPLITUDE, NAME=amplitude_name *FLUID EXCHANGE ACTIVATION, AMPLITUDE=amplitude_name The use of an amplitude to activate a fluid exchange is not supported in Abaqus/CAE. Accounting for blockage due to contacting boundary surfaces Abaqus/Explicit can account for the blockage of flow out of a cavity due to an obstruction caused by contacting surfaces. For example, flow out of an exhaust orifice may be fully or partially blocked because it is covered by another contacting surface. Blockage can be considered for any fluid exchange property. However, a surface must be defined on the boundary of the fluid cavity to be checked for contact obstruction. Abaqus/Explicit will calculate the area fraction of the surface not blocked by contacting surfaces and apply this fraction to the mass or energy flow rate out of the cavity. You can control the combination of surfaces that can cause blockage. Abaqus/Explicit will not consider contacting surfaces to cause blockage unless you specify that they can potentially cause blockage . Input File Usage: Abaqus/CAE Usage: *FLUID EXCHANGE ACTIVATION, BLOCKAGE=YES Accounting for blockage due to contacting boundary surfaces is not supported in Abaqus/CAE. Limiting the flow direction By default, flow can occur both in and out of the primary fluid cavity when a second node is included in the fluid exchange definition. In addition, heat energy flow can occur in both directions when flow is defined between a single cavity and its environment. You can limit the flow direction in Abaqus/Explicit in these cases such that fluid or heat energy flows only out of the primary fluid cavity. This method is relevant only for a fluid exchange definition based on analysis conditions and not on prescribed mass, volume, or heat energy flux. Input File Usage: Abaqus/CAE Usage: *FLUID EXCHANGE ACTIVATION, OUTFLOW ONLY Limiting the flow direction is not supported by Abaqus/CAE. Activating the fluid exchange based on the change in the leakage area The flow between cavities can be activated in Abaqus/Explicit based on a change in the area of the surface defining the effective area. You need to specify the ratio of the actual surface area to the initial effective area, which represents the threshold value for triggering the fluid exchange. The effective area used for the fluid exchange between the cavities (or between the cavity and the ambient) is the area difference between the actual area and the initial area. Input File Usage: Use the following options: *FLUID EXCHANGE, SURFACE=surface_name *FLUID EXCHANGE ACTIVATION, DELTA LEAKAGE AREA=surface_ratio Abaqus/CAE Usage: Activating the fluid exchange based on the change in the leakage area is not supported by Abaqus/CAE. Activation in multiple steps By default, when you modify the activation of a fluid exchange definition or activate a new fluid exchange definition, all existing fluid exchange activations in the step remain. When modifying an existing activation, all applicable data must be respecified. Activated fluid exchange definitions remain active in subsequent steps unless deactivated. You can choose to deactivate all fluid exchange definitions in the model and optionally reactivate new ones. If you deactivate any fluid exchange definition in a step, all fluid exchange definitions must be respecified. Input File Usage: Use the following option to modify an existing fluid exchange activation or to specify an additional fluid exchange activation (default): *FLUID EXCHANGE ACTIVATION, OP=MOD Use the following option to deactivate all fluid exchange definitions in the model and optionally reactivate new ones: *FLUID EXCHANGE ACTIVATION, OP=NEW Fluid exchange activation is automatic for all fluid exchange interactions in all steps in Abaqus/CAE. No modifications or additions are allowed. Abaqus/CAE Usage: Additional reference • Bird, R. B., W. E. Stewart, and E. N. Lightfoot, Transport Phenomena, Wiley, New York, 2002. 11.5.4 INFLATOR DEFINITION Product: Abaqus/Explicit References • “Surface-based fluid cavities: overview,” Section 11.5.1 • “Fluid cavity definition,” Section 11.5.2 • “Fluid exchange definition,” Section 11.5.3 • *FLUID INFLATOR • *FLUID INFLATOR PROPERTY • *FLUID INFLATOR ACTIVATION Overview An inflator definition: • can be used to inflate a fluid cavity to simulate actual inflators used for airbag supplemental restraint systems; • can inflate a fluid cavity with an ideal gas mixture different from that present in the fluid cavity; • can be specified directly or by defining data from a tank test; • has a name that can be used to identify history output of mass flow rates; and • can be activated at any time during the analysis. Defining an inflator The inflator capability in Abaqus/Explicit is suited for modeling the flow characteristics of inflators used for airbag systems. You must associate the inflator definition with a name. You specify the reference node of the fluid cavity that the inflator will fill with gas. A single fluid cavity can have any number of inflators. Input File Usage: *FLUID INFLATOR, NAME=name fluid_cavity_reference_node Defining the inflator property The inflator property defines the mass flow rate and temperature as a function of inflation time either directly or by entering tank test data. It also defines the mixture of gases entering the fluid cavity. You must associate the inflator property with a name. This name can then be used to associate a certain property with an inflator definition. Input File Usage: Use the following options: *FLUID INFLATOR, NAME=fluid_inflator_name, PROPERTY=property_name *FLUID INFLATOR PROPERTY, NAME=property_name Specifying the gas temperature and mass flow rate directly The temperature and the mass flow rate of the gas entering the fluid cavity can be given directly as functions of inflation time. Enter a table of mass flow rate and temperature versus inflation time. Input File Usage: *FLUID INFLATOR PROPERTY, TYPE=TEMPERATURE AND MASS inflation time, inflator gas temperature, inflator mass flow rate ... Using tank test data The mass flow rate and the temperature of the gas entering the fluid cavity can be determined by the results of a tank test. In the test the inflator is discharged into a closed, fixed volume tank, and the time history of pressure in the tank is measured. The inflator mass flow rate can then be calculated from the pressure history using the equations of gas dynamics. For an ideal gas, conservation of energy for an adiabatic process is given by where and is the temperature, is the absolute zero on the temperature scale being used, and the subscripts refer to quantities in the inflator and the rigid tank, respectively. Using mass balance and the equation of state for an ideal gas with constant volume gives The mass flow rate can be found by combining the above equations where is the ratio of the constant pressure heat capacity, , and the constant volume heat capacity, : To calculate the mass flow rate using the results of a tank test, enter a table of tank pressure and inflator temperature versus inflation time, and specify the volume of the tank. Input File Usage: *FLUID INFLATOR PROPERTY, TYPE=TANK TEST, TANK VOLUME= inflation time, inflator gas temperature, tank pressure ... Using the dual pressure method If both the inflator pressure, , time history curves can be measured during a tank test, the inflator mass flow rate and temperature can then be calculated using the assumption of isentropic flow (Wang and Nefske, 1988). The mass flow rate through the inflator orifice can be described by , and tank pressure, where C is the discharge coefficient, A is the effective area, and the coefficient assuming choked or sonic flow as is determined by Comparing the expression for inflator mass flow rate obtained in a rigid tank with that given above, the inflator temperature is given by and the inflator mass flow rate is To calculate the inflator mass flow rate and temperature using the dual pressure method, enter a table of tank pressure and inflator pressure versus inflation time; and specify the volume of the tank, the effective area, and the discharge coefficient. The tank volume and effective area must be specified. The discharge coefficient has a default value of 0.4. Input File Usage: *FLUID INFLATOR PROPERTY, TYPE=DUAL PRESSURE, TANK VOLUME= DISCHARGE COEFFICIENT=C inflation time, inflator pressure, tank pressure ... , EFFECTIVE AREA=A, Specifying the inflator pressure and mass flow rate directly You can enter a table of the mass flow rate and inflator pressure versus inflation time and specify the effective area and discharge coefficient. The gas temperature in the inflator will be calculated by using the assumption of isentropic flow. The effective area must be specified. The discharge coefficient has a default value of 0.4. Input File Usage: *FLUID INFLATOR PROPERTY, TYPE=PRESSURE AND MASS, EFFECTIVE AREA=A, DISCHARGE COEFFICIENT=C inflation time, inflator pressure, inflator mass flow rate ... Specifying the gas mixture To define the inflator gas mixture, specify the number of gas species used for the inflator, and enter a list of names of fluid behaviors and a table of the mass fraction or molar fraction of the species. The mass fraction or molar fraction of the species may be a function of inflation time. The sum of the mass fractions or molar fractions for the species should be equal to one at any given time. Input File Usage: Use the following options to specify the gas mixture in terms of the mass fractions: *FLUID INFLATOR PROPERTY *FLUID INFLATOR MIXTURE, NUMBER SPECIES=k, TYPE=MASS FRACTION fluid_behavior_name_1, fluid_behavior_name_2, etc. inflation time, mass fraction 1, mass fraction 2, etc. ... Use the following options to specify the gas mixture in terms of the molar fractions: *FLUID INFLATOR PROPERTY *FLUID INFLATOR MIXTURE, NUMBER SPECIES=k, TYPE=MOLAR FRACTION fluid_behavior_name_1, fluid_behavior_name_2, etc. inflation time, molar fraction 1, molar fraction 2, etc. ... Activating the inflator definition Inflation will not occur unless the inflation definition is activated in an analysis step. Input File Usage: Use the following options to activate a fluid inflator for a given analysis step: *FLUID INFLATOR, NAME=fluid_inflator_name *FLUID INFLATOR ACTIVATION fluid_inflator_name Relating inflation time to analysis time Inflator property definition consists of specifying tables of gas variables versus inflation time. Abaqus/Explicit the inflation time, , is related to the value of an amplitude curve by In Typically the amplitude variation is a step function stepping from zero to one at the time the airbag should be deployed. This amplitude variation has the effect of offsetting the inflation time from the analysis time. Input File Usage: Use the following options: *AMPLITUDE, NAME=amplitude_name *FLUID INFLATOR ACTIVATION, INFLATION TIME AMPLITUDE=amplitude_name Modifying the mass flow rate If the mass flow rate is prescribed directly in the inflator property definition, you can modify it by specifying an amplitude definition during a step. However, if the mass flow rate is calculated by using tank test data or the dual pressure method, the amplitude definition will be ignored. Input File Usage: Use the following options: *AMPLITUDE, NAME=amplitude_name *FLUID INFLATOR ACTIVATION, MASS FLOW AMPLITUDE=amplitude_name Activation in multiple steps By default, when you modify the activation of a fluid inflator definition or activate a new fluid inflator definition, all existing fluid inflator activations in the step remain. When modifying an existing activation, all applicable parameters must be respecified. Activated inflator definitions remain active in subsequent steps unless deactivated. You can choose If you to deactivate all fluid inflator definitions in the model and optionally reactivate new ones. deactivate any fluid inflator definition in a step, all fluid inflator definitions must be respecified. Input File Usage: Use the following option to modify an existing fluid inflator activation or to specify an additional fluid inflator activation (default): *FLUID INFLATOR ACTIVATION, OP=MOD Use the following option to deactivate all fluid inflator definitions in the model and optionally reactivate new ones: *FLUID INFLATOR ACTIVATION, OP=NEW Additional reference • Wang, J. T., and O. J. Nefske, “A New CAL3D Airbag Inflation Model,” SAE paper 880654, 1988. 11.6 Mass scaling • “Mass scaling,” Section 11.6.1 11.6.1 MASS SCALING Products: Abaqus/Explicit Abaqus/CAE References • “Explicit dynamic analysis,” Section 6.3.3 • “Adjust and/or redistribute mass of an element set,” Section 2.6.1 • “Output,” Section 4.1.1 • *FIXED MASS SCALING • *VARIABLE MASS SCALING • “Configuring a dynamic, explicit procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Configuring a dynamic fully coupled thermal-stress procedure using explicit integration” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Mass scaling is often used in Abaqus/Explicit for computational efficiency in quasi-static analyses and in some dynamic analyses that contain a few very small elements that control the stable time increment. Mass scaling can be used to: • scale the mass of the entire model or scale the masses of individual elements and/or element sets; • scale the mass on a per step basis in a multistep analysis; and • scale the mass at the beginning of the step and/or throughout the step. Mass scaling can be performed by: • scaling the masses of all specified elements by a user-supplied constant factor; • scaling the masses of all specified elements by the same value so that the minimum stable time increment for any element in the element set is equal to a user-supplied time increment; • scaling the masses of only the elements in the element set whose element stable time increments are less than a user-supplied time increment so that the element stable time increment for these elements becomes equal to the user-supplied time increment; • scaling the masses of all specified elements so that their element stable time increments each become equal to the user-supplied time increment; and • scaling automatically based on mesh geometry and initial conditions for bulk metal rolling analyses. Introduction The explicit dynamics procedure is typically used to solve two classes of problems: transient dynamic response calculations and quasi-static simulations involving complex nonlinear effects (most commonly problems involving complex contact conditions). Because the explicit central difference method is used to integrate the equations in time , the discrete mass matrix used in the equilibrium equations plays a crucial role in both computational efficiency and accuracy for both classes of problems. When used appropriately, mass scaling can often improve the computational efficiency while retaining the necessary degree of accuracy required for a particular problem class. However, the mass scaling techniques most appropriate for quasi-static simulations may be very different from those that should be used for dynamic analyses. Quasi-static analysis For quasi-static simulations incorporating rate-independent material behavior, the natural time scale is generally not important. To achieve an economical solution, it is often useful to reduce the time period of the analysis or to increase the mass of the model artificially (“mass scaling”). Both alternatives yield similar results for rate-independent materials, although mass scaling is the preferred means of reducing the solution time if rate dependencies are included in the model because the natural time scale is preserved. Mass scaling for quasi-static analysis is usually performed on the entire model. However, when different parts of a model have different stiffness and mass properties, it may be useful to scale only selected parts of the model or to scale each of the parts independently. In any case, it is never necessary to reduce the mass of the model from its physical value, and it is generally not possible to increase the mass arbitrarily without degrading accuracy. A limited amount of mass scaling is usually possible for most quasi-static cases and will result in a corresponding increase in the time increment used by Abaqus/Explicit and a corresponding reduction in computational time. However, you must ensure that changes in the mass and consequent increases in the inertial forces do not alter the solution significantly. Although mass scaling can be achieved by modifying the densities of the materials in the model, the methods described in this section offer much more flexibility, especially in multistep analyses. See “Rolling of thick plates,” Section 1.3.6 of the Abaqus Example Problems Manual, for a discussion of using mass scaling in a quasi-static analysis. Dynamic analysis The natural time scale is always important in dynamic analysis, and an accurate representation of the physical mass and inertia in the model is required to capture the transient response. However, many complex dynamic models contain a few very small elements, which will force Abaqus/Explicit to use a small time increment to integrate the entire model in time. These small elements are often the result of a difficult mesh generation task. By scaling the masses of these controlling elements at the beginning of the step, the stable time increment can be increased significantly, yet the effect on the overall dynamic behavior of the model may be negligible. During an impact analysis, elements near the impact zone typically experience large amounts of deformation. The reduced characteristic lengths of these elements result in a smaller global time increment. Scaling the mass of these elements as required throughout the simulation can significantly decrease the computation time. For cases in which the compressed elements are impacting a stationary rigid body, increases in mass for these small elements during the simulation will have very little effect on the overall dynamic response. Mass scaling for truly dynamic events should almost always occur only for a limited number of elements and should never significantly increase the overall mass properties of the model, which would degrade the accuracy of the dynamic solution. See “Impact of a copper rod,” Section 1.3.10 of the Abaqus Benchmarks Manual, for a discussion of using mass scaling in a dynamic analysis. Stable time increments Throughout this section the term “element stable time increment” refers to the stable time increment of a single element. The term “element-by-element stable time increment” refers to the minimum element stable time increment within a specific element set. The term “stable time increment” refers to the stable time increment of the entire model, regardless of whether the global estimator or the element-by-element estimator is used. Introducing mass scaling into a model Two types of mass scaling are available in Abaqus/Explicit: fixed mass scaling and variable mass scaling. These two types of mass scaling can be applied separately, or they can be applied together to define an overall mass scaling strategy. The mass scaling can also apply globally to the entire model or, alternatively, on an element set by element set basis. Fixed mass scaling Fixed mass scaling is performed once at the beginning of the step for which it is specified. Two basic approaches are available for fixed mass scaling: you can define a mass scaling factor directly, or you can define a desired minimum stable time increment for which the mass scaling factors are determined by Abaqus/Explicit. If both variable mass scaling and fixed mass scaling are specified in a step, the element original mass is scaled once at beginning of that step based on the specified fixed mass scaling. It is then further scaled at the beginning and periodically during that step based on the specified variable mass scaling. Fixed mass scaling provides a simple means to modify the mass properties of a quasi-static model at the beginning of an analysis or to modify the masses of a few small elements in a dynamic model so that they do not control the stable time increment size. Since the scaling operation is performed only once at the beginning of the step for which the mass scaling is defined, fixed mass scaling is computationally efficient. Input File Usage: Abaqus/CAE Usage: *FIXED MASS SCALING Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: At beginning of step Variable mass scaling Variable mass scaling is used to scale the mass of elements at the beginning of a step and periodically during that step. When using this type of mass scaling, you define a desired minimum stable time increment: mass scaling factors will be calculated automatically and applied, as required, throughout the step. If both variable mass scaling and fixed mass scaling are specified in a step, the element original mass is scaled once at beginning of that step based on the specified fixed mass scaling. It is then further scaled at the beginning and periodically during that step based on the specified variable mass scaling. Variable mass scaling is most useful when the stiffness properties that control the stable time increment change drastically during a step. This situation can occur in both quasi-static bulk forming and dynamic simulations in which elements are highly compressed or crushed. Input File Usage: Abaqus/CAE Usage: *VARIABLE MASS SCALING Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: Throughout step Defining a scale factor directly Defining a scale factor directly is useful for quasi-static analyses in which the kinetic energy in the model should remain small. You can define a fixed mass scaling factor that is applied to the original mass of all elements in a specified element set. The masses of the elements will be scaled at the beginning of the step and held fixed throughout the step unless further modified by variable mass scaling. Input File Usage: Abaqus/CAE Usage: *FIXED MASS SCALING, FACTOR=scale_factor For example, the following option scales the masses of elements contained in element set elset by a factor of 10: *FIXED MASS SCALING, FACTOR=10., ELSET=elset Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: At beginning of step, Scale by factor: scale_factor Defining a desired element-by-element stable time increment You can define a desired element-by-element stable time increment for an element set for fixed or variable mass scaling. Abaqus/Explicit will then determine the necessary mass scaling factors. There are three mutually exclusive methods available to scale the mass of the model when a desired element-by-element stable time increment is defined. Each method is described in detail later in this section. To determine the stable time increment used during an increment, Abaqus/Explicit first determines the smallest stable time increment on an element-by-element basis. Then, a global estimation algorithm determines a stable time increment based on the highest frequency of the model. The larger of the two estimates determines the stable time increment used. In general, the stable time increment determined by the global estimator will be greater than the stable time increment determined by the element-by- element estimator. When fixed or variable mass scaling is used with a specified element-by-element stable time increment to scale the mass of a set of elements, the element-by-element stable time increment estimate is being affected directly. If all of the elements in the model are being scaled by a single mass scaling definition, the element-by-element estimate will equal the value assigned to the element-by- element stable time increment unless the penalty method is being used to enforce contact constraints. Penalty contact can cause the element-by-element estimate to be slightly below the value assigned to the element-by-element stable time increment . The actual stable time increment used may be greater than the value assigned to the element-by-element stable time increment because of the use of the global estimator. If mass scaling is performed on only a portion of the model, the elements that are not scaled may have element stable time increments that are less than the value assigned to the element-by-element stable time increment and in that case will control the element-by-element stable time increment estimate. As a result, if only portions of the model are being scaled, the time increment used will generally not equal the value assigned to the element-by-element stable time increment. If the fixed time increment size for the explicit dynamic step is based on the initial element-by- element stability limit or is specified directly, the time increment used will be calculated according to the rules described in “Explicit dynamic analysis,” Section 6.3.3. Scaling the mass uniformly Scaling the mass uniformly is useful for quasi-static analyses in which the kinetic energy in the model should remain small. This approach is similar to defining a scale factor directly. In both cases the masses of all the elements specified are scaled uniformly by a single factor. However, with this method the mass scaling factor is determined by Abaqus/Explicit instead of being user specified. A single mass scaling factor is applied uniformly to all the elements so that the minimum stable time increment within these elements is equal to the value assigned to the element-by-element stable time increment, dt. Input File Usage: Use either of the following options: Abaqus/CAE Usage: *FIXED MASS SCALING, TYPE=UNIFORM, DT=dt *VARIABLE MASS SCALING, TYPE=UNIFORM, DT=dt Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: At beginning of step or Throughout step, Scale to target time increment of: dt, Scale element mass: Uniformly to satisfy target Scaling only elements with element stable time increments below the specified element-by-element stable time increment Scaling elements with element stable time increments below a user-specified value is appropriate for both quasi-static and dynamic analyses. It is useful for increasing the element stable time increment of the most critical elements. When the mesh at the beginning of an analysis or a step contains a few very small elements that control the stable time increment size, use fixed mass scaling to scale the masses of those elements and start the step with a desired time increment value. Increasing the mass of only these controlling elements means that the stable time increment can be increased significantly, yet the effect on the overall behavior of the model may be negligible. For analyses in which evolving deformation creates a limited number of small elements, use variable mass scaling to scale the masses of those elements, thereby limiting the reduction in the stable time increment. Input File Usage: Abaqus/CAE Usage: Use either of the following options: *FIXED MASS SCALING, TYPE=BELOW MIN, DT=dt *VARIABLE MASS SCALING, TYPE=BELOW MIN, DT=dt Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: At beginning of step or Throughout step, Scale to target time increment of: dt, Scale element mass: If below minimum target Scaling all elements to have equal element stable time increments Scaling all elements such that they have the same stable time increment effectively contracts the eigenspectrum of the model; that is, it reduces the range between the lowest and highest natural frequency of the model. Because of the drastic change in mass properties, this approach is appropriate only for quasi-static analyses. It implies that some elements may have mass scaling factors that are less than one. Input File Usage: Abaqus/CAE Usage: Use either of the following options: *FIXED MASS SCALING, TYPE=SET EQUAL DT, DT=dt *VARIABLE MASS SCALING, TYPE=SET EQUAL DT, DT=dt Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: At beginning of step or Throughout step, Scale to target time increment of: dt, Scale element mass: Nonuniformly to equal target Global and local mass scaling Specifying an element set for either fixed or variable mass scaling scales the mass of a localized region of the model. Omitting an element set implies that mass scaling will be performed for all elements. A global definition can be overwritten by a local definition for a given element set by repeating the mass scaling definition with an element set specified. Input File Usage: Use either of the following options: *FIXED MASS SCALING, ELSET=elset *VARIABLE MASS SCALING, ELSET=elset Abaqus/CAE Usage: Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: At beginning of step or Throughout step, Region: Set: elset Example 1 Different mass scaling factors may be useful when materials with vastly different wave speeds or mesh refinements are present in an analysis. In this example a scale factor of 50 may be desirable for the masses of all elements in a quasi-static analysis, except for a few elements for which a mass scaling factor of 500 is used. *FIXED MASS SCALING, FACTOR=50.0 *FIXED MASS SCALING, FACTOR=500.0, ELSET=elset1 The first fixed mass scaling definition scales the masses of all elements in the model by a factor of 50. The second fixed mass scaling definition overrides the first definition for the elements contained in element set elset1 by scaling their masses by a factor of 500. Example 2 An alternative method of scaling the masses of elements in elset1 is to assign a stable time increment to them and allow Abaqus/Explicit to determine the mass scaling factors. *FIXED MASS SCALING, FACTOR=50.0 *FIXED MASS SCALING, DT=.5E-6, TYPE=BELOW MIN, ELSET=elset1 The first fixed mass scaling definition scales the masses in the entire model by a factor of 50. The second fixed mass scaling definition overrides the first definition by scaling the masses of any elements in elset1 whose stable time increments are less than .5 × 10−6 . Mass scaling at the beginning of the step Fixed mass scaling is used to prescribe mass scaling only at the beginning of a step and always scales the original element masses. When the scale factor is defined directly, the mass is scaled by the value assigned to the scale factor. If the element-by-element stable time increment, dt, is specified, the mass scaling is based on this value. If both the scale factor and the element-by-element stable time increment are specified, the mass is first scaled by the value assigned to the scale factor and then possibly scaled again, depending on the value assigned to the element-by-element stable time increment and the type of fixed mass scaling chosen. Local mass scaling can be defined for a specific element set. If no element set is specified, the fixed mass scaling definition will apply to all elements in the model. Only one fixed mass scaling definition is permitted per element set. Multiple fixed mass scaling definitions cannot contain overlapping element sets. Local mass scaling definitions will overwrite global definitions for the specified element sets. Input File Usage: *FIXED MASS SCALING, FACTOR=factor, DT=dt, TYPE=type, ELSET=elset Abaqus/CAE Usage: Example Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: At beginning of step, Scale by factor: factor, Scale to target time increment of: dt Assume that for a quasi-static analysis a mass scaling factor of 50 is applied to all the elements in the model. Furthermore, assume that even after being scaled by a factor of 50, a few extremely small or poorly shaped elements are causing the stable time increment to be less than a desired minimum. To increase the stable time increment, the following option is used: *FIXED MASS SCALING, FACTOR=50., TYPE=BELOW MIN, DT=.5E-6 The specified scale factor causes the masses of all the elements in the model to be scaled by a factor of 50. If any element’s stable time increment is still below 0.5 × 10−6 after being scaled by a factor of 50.0, its mass will be scaled such that its stable time increment is equal to 0.5 × 10−6 . Mass scaling throughout the step Variable mass scaling with a specified element-by-element stable time increment is used to define mass scaling that is to be performed at the beginning and throughout the step. Either the frequency in increments or the number of intervals must be specified to define how frequently mass scaling is to be performed. In increments other than those in which mass scaling is performed, the time increment used will generally be different from the value assigned to the element-by-element stable time increment. Local mass scaling can be defined for a specific element set. If no element set is specified, the variable mass scaling definition will apply to all elements in the model. Only one variable mass scaling definition is permitted per element set. Multiple variable mass scaling definitions cannot contain overlapping element sets. Local mass scaling definitions will overwrite global definitions for the specified element sets. Input File Usage: Abaqus/CAE Usage: *VARIABLE MASS SCALING, DT=dt, TYPE=type, ELSET=elset Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: Throughout step, Scale to target time increment of: dt Calculating the mass scaling at equally spaced increments You can specify the number of increments between mass scaling calculations. For example, specifying a frequency of 5 will cause mass scaling to be performed at the beginning of the step and at increments 5, 10, 15, etc. Care should be taken when choosing the value of the frequency, since performing mass scaling every few increments during an analysis may result in noticeable additional computational cost per increment. Input File Usage: *VARIABLE MASS SCALING, TYPE=type, DT=dt, FREQUENCY=n Abaqus/CAE Usage: Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: Throughout step, Scale to target time increment of: dt, Scale: Every n increments Calculating the mass scaling at equally spaced time intervals Alternatively, you can specify the number of equally spaced time intervals at which the mass scaling calculations are to be performed. For example, specifying 5 intervals in a step with a duration of one second will cause mass scaling to be performed at the beginning of the step and at times of .2 , .4, .6, .8, and 1.0 seconds. Input File Usage: *VARIABLE MASS SCALING, TYPE=type, DT=dt, NUMBER INTERVAL=n Abaqus/CAE Usage: Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: Throughout step, Scale to target time increment of: dt, Scale: At n equal intervals Different mass scaling at the beginning and during the step There are cases where it is desirable to include mass scaling at the beginning of a step that may be modified further throughout the step. Input File Usage: Use both of the following options: *FIXED MASS SCALING, FACTOR=factor, TYPE=type, DT=dt_init *VARIABLE MASS SCALING, TYPE=type, DT=dt_min, FREQUENCY=n or NUMBER INTERVAL=n Abaqus/CAE Usage: Create both of the following mass scaling definitions: Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Semi-automatic mass scaling, Scale: At beginning of step Semi-automatic mass scaling, Scale: Throughout step Example Assume that in a dynamic impact analysis, a few extremely small or poorly shaped elements exist in the mesh and consequently control the stable time increment. To prevent these elements from controlling the stable time increment, it is desirable to scale their masses at the beginning of the step. In addition, elements in a region of the mesh will develop severe distortions as a result of impact with a fixed rigid surface. Consequently, elements in the impact zone may eventually control the stable time increment. Since the elements in the impact zone are essentially stationary against the rigid surface, selectively scaling their masses will guarantee that the overall dynamic response is not adversely affected. Mass scaling these elements by prescribing a time increment to limit the reduction in the element-by-element stable time increment may decrease run time substantially. For example, specify fixed mass scaling for all elements in the model with stable time increments below a value of 1.0 × 10−6 . In addition, specify variable mass scaling for the elements in the impact zone (elset1) with stable time increments below a value of 0.5 × 10−6. In this case all the elements in the model are checked at the beginning of the step. If any have stable time increments less than 1.0 × 10−6 , their masses are scaled (independently) such that the element-by-element stable time increment equals 1.0 × 10−6 . This scaling remains in effect throughout the step and is not further modified, except for those elements in elset1. The variable mass scaling definition causes the elements contained in elset1 to be scaled throughout the step so that their stable time increments do not become less than 0.5 × 10−6 . Because only elements in elset1 are scaled during the step, it is possible that a stable time increment less than 0.5 × 10−6 may result. Mass scaling in a multiple step analysis The scaled element masses at the end of one step and any variable mass scaling methods specified in that step are carried forward automatically to the subsequent step, ensuring continuity in the mass matrix at the step boundaries and continued application of the variable mass scaling methods. However, you can reset the element masses to their original values or recompute the element masses by using a new fixed mass scaling method at the beginning of the subsequent step. You can also remove the variable mass scaling methods inherited from the prior step or replace an inherited method with a new variable mass scaling method. To reset the initial mass matrix, specify a fixed mass scaling method in the subsequent step. Similarly, specify a variable mass scaling method in the subsequent step to discontinue all of the variable mass scaling methods of the prior step. The examples below illustrate the following special cases: (a) continuous mass matrix with no further mass scaling, and (b) reverting the mass matrix to the original state with no further mass scaling. Very large changes in element mass across the steps due to mass scaling may lead to precision problems in the mass calculations. These precision problems may give rise to erroneous or misleading results. When large changes in element masses are desired in such situations, it is recommended that fixed mass scaling be used in the new step to reset the element masses to their original values before using additional mass scaling definitions, as required, to scale the element masses to their desired values. Continuous mass matrix with no further scaling To define a continuous mass matrix with no further scaling, remove any variable mass scaling definitions inherited from the prior step by redefining a new variable mass scaling definition. Input File Usage: Abaqus/CAE Usage: Example Use the following option without any parameters in a new step: *VARIABLE MASS SCALING Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Disable mass scaling throughout step Assume that during the first step of a quasi-static analysis, elements will experience distortions that will cause the stable time increment to decrease dramatically. Furthermore, assume that the deformation during the second step will not be large enough to have any further effect on the stable time increment. *HEADING … *STEP … *FIXED MASS SCALING, FACTOR=1.1 *VARIABLE MASS SCALING, TYPE=BELOW MIN, DT=1.E-5, FREQUENCY=10 … *END STEP *STEP … *VARIABLE MASS SCALING … *END STEP During the first step the fixed mass scaling increases the element mass by the factor 1.1. The variable mass scaling definition scales the mass of the entire model at the beginning of the step and every tenth increment such that the element-by-element stable time increment equals at least 1 × 10−5 . The variable mass scaling definition in the second step replaces the one continued from the first step. This particular definition of variable mass scaling without any parameters in the second step also prevents any further mass scaling during the second step. The scaled mass matrix from the first step is carried over to be used during the entire second step. Reverting the mass matrix to the original state You can introduce a fixed mass scaling method in the subsequent step to discontinue all of the mass scaling methods of the prior step. Further, if the default specification of fixed mass scaling is used, element masses revert to their original values at the beginning of the subsequent step. Thus, specify just the default fixed mass scaling method to prevent the scaled mass of the previous step from being used in a new step. This is useful going from a quasi-static simulation step where mass scaling is appropriate to a dynamic step in which no scaling is desired. Input File Usage: Abaqus/CAE Usage: Use both of the following options without any parameters: *FIXED MASS SCALING *VARIABLE MASS SCALING Create both of the following mass scaling definitions: Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Reinitialize mass Disable mass scaling throughout step Example Assume that an analysis contains a quasi-static step followed by a dynamic step. Mass scaling can be performed during the quasi-static step but turned off during the dynamic step. *HEADING *STEP … *FIXED MASS SCALING, FACTOR=1.1 *VARIABLE MASS SCALING, TYPE=BELOW MIN, DT=1.E-5, FREQUENCY=10 *END STEP *STEP *FIXED MASS SCALING *VARIABLE MASS SCALING *END STEP During the first step the fixed mass scaling increases the element mass by the factor 1.1. The variable mass scaling definition scales the mass of the entire model at the beginning of the step and every tenth increment such that the element-by-element stable time increment equals at least 1 × 10−5 . The new fixed mass scaling definition without any parameters in the second step then reverts the mass matrix back to the original state. The new variable mass scaling definition replaces all the variable mass scaling definitions inherited from the first step. Further, since the new variable mass scaling definition has no parameters, no mass scaling is applied during the second step. Thus, the mass matrix for the second step reverts to that of the original state. Mass contribution from external programs connected to Abaqus via co-simulation Co-simulation can lead to mass and/or rotary inertia from external programs being added to the Abaqus model during a step. However, that contribution along with other quantities imported from the external program must be removed once the co-simulation step is completed. If co-simulation is expected to add mass and/or rotary inertia to the Abaqus model, Abaqus automatically reverts the mass matrix back to the original state once such a co-simulation step is completed. You need to respecify any mass scaling that must be continued beyond the co-simulation step. When mass scaling is or is not used The following entities are not affected by mass scaling: • Thermal solution response in a fully coupled thermal-stress analysis • Gravity loads, viscous pressure loads • Adiabatic heat calculations • Equation of state materials • Fluid and fluid link elements • Surface-based fluid cavities • Spring and dashpot elements Densities associated with any of the relevant items in this list will remain unscaled. Mass, rotary inertia, infinite, and rigid elements can be scaled. However, because none of the elements has an associated stable time increment, they can be scaled only using either a user-specified scale factor or an element- by-element stable time increment applied uniformly. If the element-by-element stable time increment is specified, at least one element with a stable time increment must be included in the mass scaling definition. Rotary inertia in shell, beam, and pipe elements is based on the scaled mass. The mass of infinite elements can be scaled; however, the infinite elements will not act as quiet boundaries unless the densities of each adjacent deformable element are scaled by the same factor. The mass of both elements will be scaled by the same factor if they are both included in the same fixed or variable mass scaling definition. Automatic mass scaling for analysis of bulk metal rolling Bulk metal rolling is generally considered a quasi-static process, but the process is often modeled with Abaqus/Explicit because of its ability to handle the contact problem well. To achieve an economical solution with Abaqus/Explicit, it is often useful to increase the mass of the product artificially. However, the mass scaling factor must be chosen such that the changes in the mass and the corresponding changes in the inertial forces do not alter the solutions significantly. Choosing too high a scaling factor will not produce quasi-static results. Choosing too low a scaling factor, while conservative, will result in long run times. Rolling variable mass scaling can be used to make the choice of the optimal scaling factor automatic for this process. The automatic strategy is based on the semi-automatic method of scaling all elements to have equal element stable time increments. The method is made automatic by determining the appropriate value for the target stable time increment from several parameters of the rolling process. The value used for the target stable time increment, ; the feed rate, V; and the number of nodes in the cross-section of the product, n. The feed rate is defined as the average velocity of the product in the rolling direction during steady-state conditions. The value of is adjusted during the analysis to account for the actual value of the feed rate. You must specify estimated values for the average velocity, the average element length in the rolling direction, and the number of nodes in the cross-section of the product. , is based on the average element length in the rolling direction, The mass of any element will never drop below its original mass. This is different from the method of scaling all elements to have equal element stable time increments. Imposing this restriction means that rolling problems that have significant inertial effects will not have their mass adjusted automatically when they are analyzed as quasi-static. To achieve a good result, it is recommended that: • the product be meshed by extruding a two-dimensional cross-section of the product; • the average element length in the rolling direction not vary significantly along the length of the product; • the product have an initial velocity in the rolling direction approximately equal to the steady-state feed rate; • the element size in the cross-section be equal to or less than the size in the rolling direction; and • no other mass scaling be used on elements scaled with rolling automatic variable mass scaling. Input File Usage: *VARIABLE MASS SCALING, ELSET=elset1, FREQUENCY=n, TYPE=ROLLING, FEED RATE=V, EXTRUDED LENGTH= CROSS SECTION NODES=n , Abaqus/CAE Usage: Output Step module: Create Step: General, Dynamic, Explicit or Dynamic, Temp-disp, Explicit: Mass scaling: Use scaling definitions below: Create: Automatic mass scaling, Feed rate: V, Extruded , Nodes in cross section: n element length: Output variable EMSF provides the element mass scaling factor. Abaqus/CAE can be used to obtain contour and history plots of EMSF. Output variable DMASS provides the total percent change in mass of the model as a result of mass scaling and is available for history plotting in Abaqus/CAE. Output variable DMASS is not available on an element set basis. Output variable EDT provides the element stable time increment. The element stable time increment includes the effect of mass scaling. Abaqus/CAE can be used to obtain history plots of EDT. 11.7 Selective subcycling • “Selective subcycling,” Section 11.7.1 11.7.1 SELECTIVE SUBCYCLING Product: Abaqus/Explicit References • “Explicit dynamic analysis,” Section 6.3.3 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • *SUBCYCLING Overview Selective subcycling: • allows different time increments to be used for different groups of elements; • reduces run time for an analysis when a small region of elements in the model controls the stable time increment; and • is invoked by defining the subcycling zones. Introduction The selective subcycling method in Abaqus/Explicit is based on domain decomposition. In this method subcycling zones are defined that remain unchanged during the analysis. The domain-level parallelization method (“Parallel execution in Abaqus/Explicit,” Section 3.5.3) is invoked automatically when subcycling zones are defined. Each subcycling zone, as well as the non-subcycling zone, is independently decomposed into the user-specified number of parallel domains. The “master” domains are defined as the parallel domains that are derived from the non-subcycling zone and are integrated with the largest stable time increment. The remaining parallel domains derived from the subcycling zones are integrated using smaller time increments, or “subcycles.” The subcycle time increment sizes are chosen as integer divisors of the time increment used in the master parallel domains. Therefore, all parallel domains exactly reach the same time points as the master parallel domains. During subcycling, nodes that lie on the interface with the non-subcycling zone require special treatment. The velocity at the interface nodes is taken from the non-subcycling zone and is constant during subcycles. This produces an interface node displacement field that varies linearly during the subcycles. Defining subcycling zones Subcycling zones are defined by element sets. You can include all element types in these sets except Eulerian element types EC3D8R and EC3D8RT. However, all parallel domains must have at least one deformable element to provide the stable time increment. Abaqus/Explicit issues an error message if there is no deformable element in a parallel domain. You can define an arbitrary number of subcycling zones. However, some modeling features cannot be split between subcycling zones. Abaqus/Explicit automatically merges subcycling zones that contain features that cannot be split. Subcycling zones are merged together when: • the zones overlap; • the zones share the same nodes; • a node is in one subcycling zone, but its adjacent nodes are in a different subcycling zone; • subcycling zones are involved in the same constraint equation, connector, or rigid body; or • general contact is specified in the analysis. When subcycling zones are merged, the smallest stable time increment among the merged zones is used. The constraint, connector, or rigid body is always assigned to the subcycling zone if any one of its nodes is involved in that subcycling zone. Since the domain-level parallelization method is used, all restrictions on parallel domain decomposition apply to subcycling zones. These restrictions prevent certain features from being split across master parallel domains, as well as parallel domains that contain the subcycling zones . Analytical rigid surfaces cannot be included in the general contact domain when a subcycling zone is defined. Efficient selective subcycling requires proper choice of subcycling zones. For each subcycling zone, the time increment size should be small compared to the non-subcycling zone, producing a large number of subcycles. The number of subcycles is the ratio of the stable time increment size in the non-subcycling zone to the stable time increment sizes in the subcycling zones. In addition to a large number of subcycles, the number of elements in a subcycling zone should generally be small compared to the total number of elements in the model for optimal performance benefit. If a majority of elements in the model are in subcycling zones, there will not be much performance benefit. Input File Usage: Use the following option to define a subcycling zone: *SUBCYCLING, ELSET=element_set_name Accuracy of results The subcycling algorithm used in Abaqus/Explicit provides sufficient accuracy for most complex dynamic models. However, because of the relatively large time increment size used in the non-subcycling zone and the interpolation used on zone interface nodes, subcycling solutions can introduce a truncation error, which may slightly alter results compared with traditional solutions. This error should not affect the overall dynamic behavior of the model. Special attention should be given to the interface between the subcycling zone and non-subcycling zone when general contact is involved. surfaces that have the potential for contacting each other within the same zone. However, to minimize truncation errors, it is highly recommended that a single surface that has the potential for contacting others not be split across the zones. Output and mass scaling Output and mass scaling are always performed at the same time points reached by all parallel domains. Input file template *HEADING … *ELSET, ELSET=ZONE1 … *SUBCYCLING, ELSET=ZONE1 ************************* *STEP *DYNAMIC, EXPLICIT Data line to specify the time period of the step ... *END STEP 11.8 Steady-state detection • “Steady-state detection,” Section 11.8.1 11.8.1 STEADY-STATE DETECTION Product: Abaqus/Explicit References • “Output,” Section 4.1.1 • *STEADY STATE DETECTION • *STEADY STATE CRITERIA Overview Steady-state detection: • can be used to detect the time in a quasi-static uni-directional Abaqus/Explicit simulation when a steady-state condition has been reached and then terminate the simulation; • can be used to output quantities that are useful in tracking the progress of a uni-directional Abaqus/Explicit simulation; and • is available only for three-dimensional analysis. Introduction Many types of uni-directional processes are used to transform preformed shapes into forms more suitable for further processing. The most common examples are rolling, wire drawing, and extrusion processes. Since the processes are usually carried out at low speeds, explicit dynamic procedures such as those in Abaqus/Explicit are often used to model the processes as quasi-static. The analyses usually consist of a workpiece that is formed into a desired shape by any number of rollers or other forming surfaces along a primary direction. The forming surfaces are usually modeled as rigid bodies. For rolling simulations the rigid body reference node is usually defined at the center of the roller. The mesh of the workpiece is often extruded and may be constructed of multiple layers of material. As the workpiece progresses through the forming surfaces, the shape eventually reaches a constant state. The position where the workpiece exits the final forming surface is referred to as the exit plane and is usually aligned with the rigid body reference node of the final forming surface. As soon as this constant shape is reached, the analysis is considered to have reached steady state. The force and torque on the final forming surfaces at this steady-state condition have also reached constant values or oscillate about constant values. A significant computational savings can be achieved by detecting the steady-state condition and halting the analysis either immediately or as soon as the steady-state cross-section progresses beyond the exit plane to a position referred to as the cutting plane. Mesh requirements The workpiece mesh is required to meet certain conditions for use with the steady-state detection capability. First, the mesh must be topologically regular in the primary direction. In other words, the mesh should consist of multiple planes of elements with each plane being similar to its adjacent leading and trailing planes in that it contains the same number of elements and the same element topology in the cross-section. Furthermore, each element in a plane is connected to elements in leading and trailing planes that reference the same material and section properties. Therefore, meshes with multiple materials and section properties are permitted, but any row of elements in the primary direction must be of the same type and must reference the same material and section properties . rolling direction exit plane cutting plane Figure 11.8.1–1 Acceptable multiple-material extruded mesh for a rolling analysis. material 1 material 2 Steady-state detection criteria sampling To determine if steady state has been reached, steady-state detection “norms” are calculated, which represent an averaged value of a variable of interest over the cross-section of the workpiece as material passes through a given position along the primary direction. This position is referred to as the exit plane and usually coincides with the position of the last rigid forming tool (e.g., roller) that the workpiece passes through. The normal of the exit plane is by definition coincident with the primary direction. The time intervals at which the norms are sampled vary depending on whether the rolling analysis is modeled in an Eulerian or Lagrangian manner. Sampling in a Lagrangian analysis In a Lagrangian-based analysis (which may include adaptive meshing employed on a Lagrangian domain) the steady-state norms are calculated as the trailing control node of each plane of elements passes the exit plane. Figure 11.8.1–2 illustrates the control node definitions. first steady-state rolling plane trailing control node of the first plane leading control node of the first plane Figure 11.8.1–2 Control node positioning. The time period of norm sampling is, therefore, based on the frequency at which the planes of elements cross the exit plane. For output purposes the values of the norms are assumed to remain constant between the times at which successive control nodes pass the exit plane. Sampling in an Eulerian analysis An Eulerian analysis employs a control volume approach in which material is drawn from an inflow Eulerian boundary and is pushed or pulled out through an outflow boundary. Adaptive mesh domains are defined on the workpiece, and sliding boundary regions are defined to model contact between the workpiece and forming tools such as rollers. See “ALE adaptive meshing: overview,” Section 12.2.1, for details of adaptive meshing techniques. The mesh remains relatively stationary while the material moves through the exit plane. The time period between sampling is, therefore, based on the progress of the material moving through the exit plane. To determine a time period in a manner consistent with the Lagrangian case, the sampling period is determined by dividing the characteristic element length of the workpiece by the speed of the material flow. This period is roughly the time it takes for material to pass through an element of typical size. Steady-state detection norm definitions An individual norm is considered to have achieved steady state if its relative change in value over three consecutive planes does not exceed a tolerance. You can provide the norm tolerances when you define the steady-state criteria, or default values of tolerances can be chosen by Abaqus/Explicit. The norms can be output by requesting their identifiers listed in the definitions below. Equivalent plastic strain norm The plastic strain norm of a plane of elements is defined by summing the product of the equivalent plastic strain and the element volume of each element on the plane, then dividing by the total volume of the elements on the plane. This norm provides a weighted average of the equivalent plastic strain for the plane. The identifier for the equivalent plastic strain norm is SSPEEQ. Spread norm The spread norm of a plane of elements is computed as the largest of the area moments of inertia of the cross-section of the plane. In determining the spread norm, the cross-section of the plane of elements is determined by projecting the element faces whose normals originally coincided with the primary direction onto the exit plane. The area moments of inertia are then determined about the centroid of the section in the directions of the original principal axes of the cross-section. The identifier for the spread norm is SSSPRD. Force norm The force norm is computed by averaging the magnitude of the force at the rigid body reference node of a forming tool, such as the exit roller, over the time period between sampling points. You provide the rigid body reference node and force direction. The identifier for the force norm is SSFORC. Torque norm The torque norm is computed by averaging the magnitude of the torque at the rigid body reference node of a forming tool, such as the exit roller, over the time period between sampling points. You provide the rigid body reference node and torque direction. The identifier for the torque norm is SSTORQ. Requesting steady-state detection during an analysis You must define the criteria that are used to determine if steady state has been reached. Abaqus/Explicit will halt the analysis based on the achievement of steady state. Steady-state detection A steady-state detection definition is used to define the elements in the workpiece, the primary direction of the workpiece, the cutting position, and the type of sampling used. The primary direction is defined by specifying the direction cosines with respect to the global Cartesian coordinate system. The cutting position is defined by specifying the global coordinates of a point lying in the cutting plane. The normal to the cutting plane is assumed to coincide with the primary direction. Once steady state has been detected, the analysis is terminated when the plane of the workpiece that was first detected to have reached steady state has progressed to the cutting plane. You can choose the sampling method used, as described below. Requesting sampling as elements pass the exit plane for a Lagrangian analysis You can request that all steady-state norms be calculated as each plane of elements crosses the exit plane. *STEADY STATE DETECTION, ELSET=elset, SAMPLING=PLANE BY PLANE Input File Usage: Requesting sampling at uniform intervals for an Eulerian analysis Alternatively, you can request that all steady-state norms be calculated at an interval based on the time required for material to progress the length of an average element. Input File Usage: *STEADY STATE DETECTION, ELSET=elset, SAMPLING=UNIFORM Steady-state criteria Any number of steady-state criteria definitions can be specified. Only when all of the criteria specified under any one steady-state criteria definition have been satisfied will the analysis be considered to have reached steady state. To define the criteria, you specify the norm type identifier, the norm tolerance, and the global coordinates of a point on the exit plane. For force and torque norms, you also specify the rigid body reference node of the forming tool at the exit plane and the direction cosines of the force or torque. Exit planes can be defined separately for each norm definition. Input File Usage: Use the following options to define the criteria needed to achieve steady state: *STEADY STATE DETECTION, ELSET=elset, SAMPLING=PLANE BY PLANE or UNIFORM *STEADY STATE CRITERIA *STEADY STATE CRITERIA ... 6.0, 0.0, 0.0 For example, assume that two sets of criteria are of interest and that the analysis can be terminated as soon as either is satisfied. The input might be as follows: *STEADY STATE DETECTION, ELSET=sheet, SAMPLING=PLANE BY PLANE 1.0, 0.0, 0.0, *STEADY STATE CRITERIA SSPEEQ,.002, SSSPRD,.002, SSFORC,.005, SSFORC,.005, SSTORQ,.005, *STEADY STATE CRITERIA SSPEEQ,.001, SSSPRD,.001, SSFORC,.010, 5.0, 0.0, 0.0 5.0, 0.0, 0.0 5.0, 0.0, 0.0, 1000, 1.0, 0.0, 0.0 5.0, 0.0, 0.0, 1000, 0.0, 1.0, 0.0 5.0, 0.0, 0.0, 1000, 0.0, 0.0, 1.0 5.0, 0.0, 0.0 5.0, 0.0, 0.0 5.0, 0.0, 0.0, 1000, 0.0, 1.0, 0.0 Materials Steady-state detection is intended to be used with plasticity-based materials since the equivalent plastic strain norm would be zero for nonplasticity-based material models. Procedures One steady-state detection definition is allowed per analysis. The definition can be entered in any step and is continued through subsequent steps in an analysis. A steady-state detection definition cannot be entered in an annealing step or continued through an annealing step. Elements The current steady-state detection capabilities support the use of C3D8R and C3D8RT elements only. Output The output variables SSPEEQn, SSSPRDn, SSFORCn, and SSTORQn are used to output the equivalent plastic strain, spread, force, and torque norms, respectively. Abaqus/CAE can be used to obtain history plots of each of the steady-state detection norm variables. Individual norms can be output by requesting the norm number n, which is based on the order in which the norms are specified. Referring to the example above, if the force norm of the second steady-state criteria definition were to be requested, the output identifier would be SSFORC3. If a steady-state detection norm is requested that does not include a norm number, SSFORC for example, all norms of that type are output. Once steady state has been detected, an element set is created automatically by Abaqus/Explicit and written to the output database consisting of the plane of elements that first satisfied the steady-state criteria. The element set created is named SteadyStatePlane and can be viewed with Abaqus/CAE. If no output requests are made to the output database, the element set SteadyStatePlane will not be created. Input file template *HEADING … *ELSET, ELSET=WORKPIECE ************************* *STEP *DYNAMIC, EXPLICIT Data line to specify the time period of the step ... *STEADY STATE DETECTION, ELSET=WORKPIECE, SAMPLING=PLANE BY PLANE Data line specifying rolling direction and cutting plane position *STEADY STATE CRITERIA Data lines specifying steady-state detection norm criteria ... *OUTPUT, HISTORY, TIME INTERVAL=1.E-6 *INCREMENTATION OUTPUT SSPEEQ, SSSPRD, SSFORC, SSTORQ ... *END STEP Adaptivity Techniques Adaptivity techniques: overview ALE adaptive meshing Adaptive remeshing Analysis continuation after mesh replacement ADAPTIVITY TECHNIQUES 12.1 12.2 12.3 12.1 Adaptivity techniques: overview • “Adaptivity techniques,” Section 12.1.1 12.1.1 ADAPTIVITY TECHNIQUES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “ALE adaptive meshing: overview,” Section 12.2.1 • “Adaptive remeshing: overview,” Section 12.3.1 • “Mesh-to-mesh solution mapping,” Section 12.4.1 • *ADAPTIVE MESH • “Understanding adaptive remeshing,” Section 17.13 of the Abaqus/CAE User’s Manual Overview The finite element discretization that results from suboptimal meshing of models can limit your ability to obtain adequate analysis results at a reasonable CPU cost. This section provides an overview of the adaptivity techniques available in Abaqus that help you optimize a mesh and, therefore, obtain quality solutions while controlling the cost of your analysis. The term “adaptivity” reflects the adaptive, or solution-dependent, processes that Abaqus uses to adapt your mesh to meet your analysis goals. Selecting an adaptivity technique Three adaptivity techniques are available in Abaqus: Arbitrary Lagrangian-Eulerian (ALE) adaptive meshing; varying topology adaptive remeshing (this functionality is not applicable to V6); and mesh-to- mesh solution mapping, to enable rezoning analysis. Table 12.1.1–1 shows that the adaptivity techniques can be classified according to • their applicability to achieving particular goals, either accuracy or control of mesh distortion; • their impact on mesh definitions, either through smoothing a single mesh or through generating multiple dissimilar meshes; and • when adaptivity occurs with respect to analysis steps. Table 12.1.1–1 The characteristics of the adaptivity techniques. Accuracy Distortion control Single mesh Multiple meshes Adaptivity occurs ALE adaptive meshing Adaptive remeshing (not applicable to V6) Mesh-to-mesh solution mapping ALE adaptive meshing Throughout a step Separately from analysis steps Between analysis steps Arbitrary Lagrangian-Eulerian (ALE) adaptive meshing provides control of mesh distortion. ALE adaptive meshing uses a single mesh definition that is gradually smoothed within analysis steps. ALE adaptive meshing is available for limited applications in Abaqus/Standard and is more generally applicable in Abaqus/Explicit. The term ALE implies a broad range of analysis approaches, from purely Lagrangian analysis, in which the node motion corresponds to material motion, to purely Eulerian analysis, in which the nodes remain fixed in space and material “flows” through the elements. Typically ALE analyses use an approach between these two extremes. The ALE feature is distinct from the Eulerian analysis capability in Abaqus/Explicit, which is described in “Eulerian analysis,” Section 14.1.1. You can use adaptive meshing to control element distortion in cases where large deformation or loss of material occurs. Figure 12.1.1–1 illustrates a case where adaptive meshing limits mesh distortion in a bulk forming simulation. rigid die rigid die symmetry plane without ALE adaptive meshing with ALE adaptive meshing Figure 12.1.1–1 Use of ALE adaptive meshing to control element distortion. Unlike other adaptivity techniques, adaptive meshing operates on your original mesh definition and is, therefore, useful only when a single mesh can be effective for the duration of a simulation. The mesh is adapted through smoothing of the mesh nodes. This smoothing is typically applied frequently within analysis steps. ALE adaptive meshing requires only one analysis job. See “ALE adaptive meshing: overview,” Section 12.2.1, for details. Adaptive remeshing (varying topology adaptivity) Adaptive remeshing is typically used for accuracy control, although it can also be used for distortion control in some situations. The adaptive remeshing process involves the iterative generation of multiple dissimilar meshes to determine a single, optimized mesh that is used throughout an analysis. Adaptive remeshing is available only for Abaqus/Standard analyses submitted from Abaqus/CAE. The goal of adaptive remeshing is to obtain a solution that satisfies mesh discretization error indicator targets that you set, while minimizing the number of elements and, hence, the cost of your analysis. You can use adaptive remeshing to obtain a mesh that provides a balance between solution cost and desired accuracy. Figure 12.1.1–2 illustrates a case where adaptive remeshing improves the quality of the stress result around a fillet with targeted mesh refinement. Figure 12.1.1–2 Use of adaptive remeshing to improve the quality of a stress result. Adaptive remeshing involves an iterative process to determine a single, optimized mesh that is used through an analysis. The iterative process and the remeshing are controlled in Abaqus/CAE. Each successive analysis job covers the same simulation history time period but uses a different mesh. Once the adaptive remeshing process is complete, a single mesh and a single analysis job represent your entire analysis history. See “Adaptive remeshing: overview,” Section 12.3.1, and “Understanding adaptive remeshing,” Section 17.13 of the Abaqus/CAE User’s Manual. Mesh-to-mesh solution mapping Mesh-to-mesh solution mapping is available only in Abaqus/Standard. You can use this technique to control element distortion in cases where large deformation occurs by replacing the mesh and continuing the analysis. Figure 12.1.1–3 illustrates a case where solution mapping is used in conjunction with a new mesh to overcome difficulties associated with element distortion. Figure 12.1.1–3 Use of mesh-to-mesh solution mapping as a component of a rezoning technique. Mesh replacement, or rezoning, involves the creation of multiple Abaqus jobs, each of which represents the configuration of the model in distinct, sequential periods of the simulation history. You use mesh replacement when a single mesh cannot be effective for the duration of a simulation. Each mesh subsequent to the initial configuration reflects a solution-dependent deformed configuration of the model. Therefore, analyses that use mesh replacement are sequentially dependent, and Abaqus uses In mesh-to-mesh solution mapping to propagate solution variables from one analysis to the next. contrast to adaptive remeshing, each mesh replacement job represents a component of the overall analysis history—no single mesh and no single analysis job represent your entire analysis. See “Mesh-to-mesh solution mapping,” Section 12.4.1, for details. 12.2 ALE adaptive meshing • “ALE adaptive meshing: overview,” Section 12.2.1 • “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2 • “ALE adaptive meshing and remapping in Abaqus/Explicit,” Section 12.2.3 • “Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit,” Section 12.2.4 • “Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit,” Section 12.2.5 • “Defining ALE adaptive mesh domains in Abaqus/Standard,” Section 12.2.6 • “ALE adaptive meshing and remapping in Abaqus/Standard,” Section 12.2.7 ALE ADAPTIVE MESHING: OVERVIEW ALE ADAPTIVE MESHING: OVERVIEW The adaptive meshing technique in Abaqus combines the features of pure Lagrangian analysis and pure Eulerian analysis. This type of adaptive meshing is often referred to as Arbitrary Lagrangian-Eulerian (ALE) analysis. The Abaqus documentation often refers to “ALE adaptive meshing” simply as “adaptive meshing.” ALE adaptive meshing is a tool that makes it possible to maintain a high-quality mesh throughout an analysis, even when large deformation or loss of material occurs, by allowing the mesh to move independently of the material. ALE adaptive meshing does not alter the topology (elements and connectivity) of the mesh, which implies some limitations on the ability of this method to maintain a high-quality mesh upon extreme deformation. Refer to “Adaptivity techniques,” Section 12.1.1, for a comparison between ALE adaptive meshing and other Abaqus adaptivity methods. ALE adaptive meshing is distinct from the pure Eulerian analysis capability in Abaqus/Explicit. The pure Eulerian capability supports multiple materials and voids within a single element, which allows effective handling of analyses involving extreme deformation (such as fluid flow). In contrast, ALE elements are always 100% full of a single material; while this formulation limits the deformation of material in the model to the deformation of the elements, it allows more precise definitions of material boundaries and more complex contact interactions. For more information on pure Eulerian analysis, see “Eulerian analysis,” Section 14.1.1. Although the adaptive meshing techniques and the user interface are similar in Abaqus/Explicit and Abaqus/Standard, the use-cases and the level of functionality are different. Adaptive meshing in Abaqus/Explicit is intended to model large-deformation problems. It does not attempt to minimize discretization errors in small-deformation analyses. Adaptive meshing in Abaqus/Standard is intended for use in acoustic domains and for modeling the effects of ablation, or wear, of material. A comparison between the adaptive remeshing functionality in Abaqus/Explicit and Abaqus/Standard is provided in this section. Features of ALE adaptive meshing ALE adaptive meshing: • can often maintain a high-quality mesh under severe material deformation by allowing the mesh to move independently of the underlying material; and • maintains a topologically similar mesh throughout the analysis (i.e., elements are not created or destroyed). In Abaqus/Explicit ALE adaptive meshing: • can be used to analyze Lagrangian problems (in which no material leaves the mesh) and Eulerian problems (in which material flows through the mesh); • can be used as a continuous adaptive meshing tool for transient analysis problems undergoing large deformations (such as dynamic impact, penetration, and forging problems); • can be used as a solution technique to model steady-state processes (such as extrusion or rolling); • can be used as a tool to analyze the transient phase in a steady-state process; and • can be used in explicit dynamics (including adiabatic thermal analysis) and fully coupled thermal- stress procedures. In Abaqus/Standard ALE adaptive meshing: • can be used to solve Lagrangian problems (in which no material leaves the mesh) and to model effects of ablation, or wear (in which material is eroded at the boundary); • can be used to update the acoustic mesh when structural preloading causes significant geometric changes in the acoustic domain; and • can be used in geometrically nonlinear static, steady-state transport, coupled pore fluid flow and stress, and coupled temperature-displacement procedures. Activating ALE adaptive meshing Adaptive meshing can be applied to an entire model or to individual parts of a model. A Lagrangian adaptive mesh domain will be created, so that the domain as a whole will follow the material originally inside it, which is the proper physical interpretation for most structural analyses. Additional options are provided for controlling the mesh. In Abaqus/Explicit analyses you can define Eulerian boundaries to allow material to flow into or out of the domain modeled. The subsequent sections of “ALE adaptive meshing,” Section 12.2, describe the various options that can be used with adaptive meshing. Although these options give you the ability to exercise detailed control over adaptive meshing, they are not necessary for many Lagrangian problems. • To take full advantage of all the adaptive mesh features in Abaqus, it is important to understand the concepts of adaptive mesh domains, boundary regions, boundary edges, geometric features, and mesh constraints. These concepts are explained in “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2, and “Defining ALE adaptive mesh domains in Abaqus/Standard,” Section 12.2.6. Instructions for applying boundary conditions, loads, and surfaces to adaptive mesh boundaries are also provided in those sections. • “ALE adaptive meshing and remapping in Abaqus/Explicit,” Section 12.2.3, and “ALE adaptive meshing and remapping in Abaqus/Standard,” Section 12.2.7, outline the methods used to move the mesh and to remap solution variables to the new mesh. These sections also present options for controlling these algorithms. Although the default methods have been chosen to work well for a wide variety of problems, you may wish to override the defaults to balance the robustness and efficiency of adaptive meshing or to extend the use of adaptive meshing to relatively difficult or unusual applications. • Various output and diagnostics are available for verifying the formation of adaptive mesh domains and for interpreting the results of an analysis. These options are explained in “Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit,” Section 12.2.5. • “Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit,” Section 12.2.4, gives advice, in the form of examples and modeling hints, on setting up and interpreting Eulerian problems in Abaqus/Explicit using adaptive meshing. Input File Usage: Abaqus/CAE Usage: *ADAPTIVE MESH, ELSET=elset_name Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on Use the ALE adaptive mesh domain below, and click Edit to select the region Uses for ALE adaptive meshing Adaptive meshing is of great value in a variety of problems. Abaqus/Explicit and Abaqus/Standard each employ adaptive meshing in ways that provide the greatest value within the particular solver. Uses in Abaqus/Explicit In problems where large deformation is anticipated the improved mesh quality resulting from adaptive meshing can prevent the analysis from terminating as a result of severe mesh distortion. In these situations you can use adaptive meshing to obtain faster, more accurate, and more robust solutions than with pure Lagrangian analyses. Adaptive meshing is particularly effective for simulations of metal forming processes such as forging, extrusion, and rolling because these types of problems usually involve large amounts of nonrecoverable deformation. Because the final shape of the product can be drastically different from the original shape, a mesh that is optimal for the original product geometry can become unsuitable in later stages of the process when large material deformation leads to severe element distortion and entanglement. Element aspect ratios can also degrade in zones with high strain concentrations. Both of these factors can lead to a loss of accuracy, a reduction in the size of the stable time increment, or even termination of the problem. Uses in Abaqus/Standard You can use adaptive meshing to enable acoustic domain meshes to follow the large deformations of the bounding structure. In other applications you can use adaptive meshing and adaptive mesh constraints to model arbitrarily large amounts of ablation of material away from the domain. Adaptive meshing of acoustic regions greatly extends the utility of acoustic analysis procedures. Abaqus can be used to model the response of a coupled structural-acoustic system subjected to structural preloads. By default, the structural-acoustic calculations are based on the original configuration of the acoustic domain. This approximation is adequate as long as the boundary between the fluid and structure does not experience large deformation during application of the preload. However, when the geometry of the acoustic domain changes significantly as a result of structural loading, the original acoustic configuration must be updated. An example is the interior cavity of a tire subjected to inflation, rim mounting, and footprint pressure loads. The acoustic elements in Abaqus do not have mechanical behavior and, therefore, cannot model the deformation of the fluid when the structure undergoes large deformation. Abaqus/Standard solves the problem of computing the current configuration of the acoustic domain by periodically creating a new acoustic mesh that uses the same topology as the original mesh but with the nodal locations adjusted so that the deformation of the structural-acoustic boundary does not lead to severe distortion of the acoustic elements. The geometric changes associated with the new acoustic mesh are then taken into account in a subsequent coupled structural-acoustic analysis. However, it is assumed that the material properties of the fluid, such as the density, do not change as a result of mesh smoothing. Adaptive meshing can also model effects of ablation, or wear, by enabling you to define boundary mesh motions independent of the underlying material motion. An example is the wearing of a tire during its life, an effect that can significantly affect the performance of the structure. Comparison of ALE adaptive meshing in Abaqus/Explicit and Abaqus/Standard Adaptive meshing in Abaqus/Explicit is generally more robust and provides more features for controlling the mesh than does adaptive meshing in Abaqus/Standard. ALE adaptive meshing in Abaqus/Explicit Adaptive meshing in Abaqus/Explicit is designed to handle a large variety of problem classes, and employs a variety of smoothing methods, with controls that you can use to tailor the adaptivity to specific problems. The Abaqus/Explicit implementation allows you to do the following: • to create entirely Eulerian models; • to improve the quality of the mesh initially, before deformation begins; and • to define tracer particles, which enable tracking and output of material-based results quantities. ALE adaptive meshing in Abaqus/Standard Adaptive meshing in Abaqus/Standard uses a single smoothing algorithm that works well for structural acoustic analyses and the modeling of ablation processes. The Abaqus/Standard implementation of adaptive meshing has the following limitations: • Initial mesh sweeps cannot be used to improve the quality of the initial mesh definition. • The method is not intended to be used in general classes of large-deformation problems, such as bulk forming. • Diagnostics capabilities are currently limited. Illustrative examples To illustrate the value of adaptive meshing, simple examples of transient and steady-state forming applications follow. For simplicity, two-dimensional cases are shown. In each case Abaqus/Explicit is used in the simulation. Axisymmetric forging In this example a well-lubricated rigid die of sinusoidal shape moves down to deform a blank of rectangular cross-section . The indentation depth is 80% of the original blank thickness. Material extrudes upward and outward (radially) as the blank is indented. The die is modeled with an analytical rigid surface, and the blank is modeled with axisymmetric continuum elements in a regular mesh configuration. The blank is assumed to have elastic-plastic material properties. A pure Lagrangian analysis of this problem does not run to completion because of excessive distortion in several elements, as shown in Figure 12.2.1–2. The contact surface cannot be treated correctly because of the gross distortion of the elements at the troughs of the sinusoidal rigid surface. rigid die plane of symmetry Figure 12.2.1–1 A blank and a sinusoidal die. Figure 12.2.1–2 Eventually, the purely Lagrangian analysis will terminate because of excessive element distortion. Adaptive meshing allows the problem to run to completion. A Lagrangian adaptive mesh domain is created for the entire blank. Abaqus/Explicit automatically chooses suitable defaults for adaptive meshing; hence, the adaptive mesh approach requires only two additional input lines: *HEADING ... *ELSET, ELSET=BLANK *************************** *STEP *DYNAMIC, EXPLICIT ... *ADAPTIVE MESH, ELSET=BLANK ... *END STEP Figure 12.2.1–3 and Figure 12.2.1–4 show the deformed mesh at various stages of the forming analysis. Because the mesh refinement is maintained on the areas of the slave surface that contact the die troughs as the material flows radially, contact conditions are resolved correctly throughout the analysis. Figure 12.2.1–3 Deformed configuration at an intermediate stage of the analysis. Figure 12.2.1–4 Deformed configuration upon completion of the analysis. Steady-state rolling example This example shows how adaptive meshing can be used in a steady-state simulation to allow the flow of material through Eulerian boundaries on the problem domain. A steel plate is passed through a symmetric roll stand to reduce its height by 50%. This simulation is run until it reaches steady-state conditions. Figure 12.2.1–5 and Figure 12.2.1–6 show the initial and final (steady-state) configurations in a purely Lagrangian model of this problem. rigid roller plane of symmetry Figure 12.2.1–5 The initial configuration of the roller and the undeformed blank in the pure Lagrangian model. Figure 12.2.1–6 The final steady-state configuration in the pure Lagrangian model. Figure 12.2.1–7 shows this problem modeled using an Eulerian adaptive mesh domain, where material flows through the mesh. Only the region near the roller is modeled. The exact location of the free surface does not need to be known to set up the problem: it is created in a likely location, and the final steady-state position is found as part of the solution. Although not shown, a focused mesh can be free surface 100 INFLOW OUTFLOW Figure 12.2.1–7 The initial Eulerian adaptive mesh domain. used to capture steep strain gradients directly beneath the roller. The Eulerian domain reaches the same steady-state solution as obtained with the Lagrangian approach. The Eulerian adaptive mesh domain is created by defining an inflow and an outflow boundary on the adaptive mesh domain. Adaptive mesh constraints are applied normal to these boundaries so that material will flow through the mesh . Frictional contact between the roller and the blank pulls material through the adaptive mesh domain. The problem is set up by making the following modifications to the input file for the pure Lagrangian analysis: *HEADING ... *ELSET, ELSET=BILLET ... *ELSET, ELSET=INFLOW ... *ELSET, ELSET=OUTFLOW ... *NSET, NSET=INFLOW ... *NSET, NSET=OUTFLOW ... *SURFACE, NAME=INFLOW, REGION TYPE=EULERIAN INFLOW, S1 *SURFACE, NAME=OUTFLOW, REGION TYPE=EULERIAN OUTFLOW, S2 *************************** *STEP *DYNAMIC, EXPLICIT Data line to specify the time period of the step ... *ADAPTIVE MESH, ELSET=BILLET, CONTROLS=ADAPT *ADAPTIVE MESH CONTROLS, NAME=ADAPT *ADAPTIVE MESH CONSTRAINT, TYPE=DISPLACEMENT INFLOW, 1, 1, 0.0 100, 2, 2, 0.0 OUTFLOW, 1, 1, 0.0 ... *END STEP Adaptive mesh controls were not required to solve this problem; they were included for illustrative purposes . 12.2.2 DEFINING ALE ADAPTIVE MESH DOMAINS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “ALE adaptive meshing: overview,” Section 12.2.1 • “ALE adaptive meshing and remapping in Abaqus/Explicit,” Section 12.2.3 • *ADAPTIVE MESH • “Understanding ALE adaptive meshing,” Section 14.6 of the Abaqus/CAE User’s Manual Overview Arbitrary Lagrangian-Eulerian (ALE) adaptive mesh domains: • define the portions of a finite element model where mesh movement is independent of material deformation; • can be used to analyze Lagrangian or Eulerian problems; • can contain only first-order, reduced-integration, solid elements (4-node quadrilaterals, 3-node triangles, 8-node hexahedra, 6-node wedges, and 4-node tetrahedra); • can be used in planar, axisymmetric, and three-dimensional geometries; • have boundary regions where loads, boundary conditions, and surfaces can be defined; and • are active only for geometrically nonlinear steps. Defining an ALE adaptive mesh domain ALE adaptive meshing is performed in adaptive mesh domains, which can be either Lagrangian or Eulerian. Within either type of adaptive mesh domain the mesh will move independently of the material. Lagrangian adaptive mesh domains are usually used to analyze transient problems with large deformations. On the boundary of a Lagrangian domain the mesh will follow the material in the direction normal to the boundary, so that the mesh covers the same material domain at all times. Eulerian adaptive mesh domains are usually used to analyze steady-state processes involving material flow. On certain user-defined boundaries of an Eulerian domain, material can flow into or out of the mesh. By default, the mesh is not fixed spatially on these boundaries; mesh constraints must be applied to prevent the mesh from moving with the material, as described in “Mesh constraints,” presented later in this section. There can never be any “empty” elements; all elements in the domain must be filled completely with material at all times. You must specify the region of the original mesh that will be subject to adaptive meshing. Input File Usage: *ADAPTIVE MESH, ELSET=name Multiple adaptive mesh domains can be defined in a step by reusing the *ADAPTIVE MESH option (for example, to prevent material from flowing from one domain to another or to apply adaptive meshing to unconnected domains). The element sets used to create adaptive mesh domains cannot overlap. Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on Use the ALE adaptive mesh domain below, and click Edit to select the region Only one adaptive mesh domain can be defined in Abaqus/CAE for any particular step. Modifying an ALE adaptive mesh domain By default, all adaptive mesh domains defined in the previous analysis step remain unchanged in the subsequent step. You define the adaptive mesh domains in effect for a given step relative to the preexisting adaptive mesh domains. At each new step the existing adaptive mesh domains can be modified and additional adaptive mesh domains can be specified (except in Abaqus/CAE, where only one adaptive mesh domain can be in effect for a given step). Input File Usage: Use either of the following options to modify an existing adaptive mesh domain or to specify an additional adaptive mesh domain: Abaqus/CAE Usage: *ADAPTIVE MESH, ELSET=name *ADAPTIVE MESH, ELSET=name, OP=MOD Step module: Other→ALE Adaptive Mesh Domain→Edit Removing an ALE adaptive mesh domain If you choose to remove any adaptive mesh domain in a step, no adaptive mesh domains will be propagated from the previous step. Therefore, all adaptive mesh domains that are in effect during this step must be respecified. Input File Usage: Use the following option to remove all previously defined adaptive mesh domains and to specify new adaptive mesh domains: Abaqus/CAE Usage: *ADAPTIVE MESH, ELSET=name, OP=NEW If the OP=NEW parameter is used on any *ADAPTIVE MESH option within a step, it must be used on all *ADAPTIVE MESH options in the step. Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on No adaptive mesh domain for this step Splitting ALE adaptive mesh domains User-defined adaptive mesh domains are examined by Abaqus/Explicit. The user-defined domain will be modeled using a single adaptive mesh if the domain: • consists of a single element type; • consists of a single connected region; • consists of a single material; • is subject to a uniform body force (including zero body force); and • has identical section controls. The user-defined domain will be split into multiple adaptive mesh domains, separated by boundary regions, if the domain: • consists of multiple element types; • spans part instances; • consists of multiple regions (including regions that are connected by less than a single element face, only by contact conditions, or only by connectors such as MPCs); • consists of multiple materials; • is subject to multiple body force definitions; or • is subject to multiple section control definitions. In this documentation the term “adaptive mesh domain” refers to a single domain after splitting by Abaqus/Explicit. On the rare occasion that a reference is made to an adaptive mesh domain prior to the automatic splitting, it is referred to as a “user-defined adaptive mesh domain.” Since adaptive mesh domains are split across element types, degenerate elements should be used for mixed domains that include both triangles and quadrilaterals (or tetrahedron and bricks). For example, when defining a mixed plane strain domain with quadrilateral and triangular elements, the CPE4R element type should be used to define both quadrilaterals and degenerated quadrilaterals. Using the CPE3 element will result in split domains, which is generally not desirable. ALE adaptive mesh boundary regions Each ALE adaptive mesh domain has a boundary, which can consist of one or more regions. (Regions, in this context, are surfaces in three-dimensional models or lines in two-dimensional or axisymmetric models.) A boundary region can be either Lagrangian, sliding, or Eulerian. Some boundary regions are created automatically by Abaqus/Explicit; others can be created by defining boundary conditions, loads, and surfaces. Adaptive mesh boundary regions are separated by edges in three dimensions and by corners in two dimensions. Both edges and corners are referred to as “boundary region edges” throughout this documentation. Boundary region edges Two types of boundary region edges can exist: Lagrangian and sliding. Lagrangian edges are always associated with a material line. Material can never flow past a Lagrangian edge, and nodes can move only along a Lagrangian edge (like beads on a string). Sliding edges are associated only with the mesh. Material can flow past a sliding edge (that is, sliding edges are free to slide over the underlying material). Lagrangian edges can be viewed with Abaqus/CAE; see “Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit,” Section 12.2.5. Lagrangian boundary regions Lagrangian boundary regions are the most common boundary regions in structural finite element analysis; therefore, with the exception of contact surfaces, they are always the default in Abaqus/Explicit. A Lagrangian boundary region has the most constraints of all the boundary region types. The mesh is constrained to move with the material in the direction normal to the surface of the boundary region and in the directions perpendicular to the boundary region edges. Lagrangian boundary regions have Lagrangian edges: the edges follow the material. On the interior of a Lagrangian boundary region, the mesh can move independently of the material in the surface of the boundary region. Thus, a Lagrangian boundary region can be thought of as a “mesh patch” that follows the material. Nodes are free to move within and along the edges of the patch but cannot leave the patch. Lagrangian corners A Lagrangian corner is formed where two Lagrangian edges meet. The node at a Lagrangian corner is constrained to move with the material in all directions; it is nonadaptive. Sliding boundary regions A sliding boundary region is the same as a Lagrangian boundary region except that it has a sliding edge. Sliding boundary regions are created by default when you define a surface on the boundary of an adaptive mesh domain . The mesh is constrained to move with the material in the direction normal to the boundary region, but it is completely unconstrained in the directions tangential to the boundary region. Thus, a sliding boundary region can be thought of as a “mesh patch” that moves independently of the underlying material. Sliding boundary regions can be created by defining a surface, boundary condition, or load on the boundary of an adaptive mesh domain (as explained later in this section). Since the mesh is totally unconstrained in the directions tangential to a sliding boundary region, the location of an applied boundary condition or load may not be physically meaningful as the mesh moves over the material. Therefore, to retain the spatial meaning of an applied boundary condition or load, spatial mesh constraints (described in “Mesh constraints,” presented later in this section) are usually applied tangential to sliding boundary regions. Eulerian boundary regions Eulerian boundary regions can be defined on the exterior of a model where it makes physical sense to let material flow across the boundary (for example, at the inlet and outlet of a steady-state extrusion or rolling problem). This flow across the boundary distinguishes Eulerian boundary regions from Lagrangian or sliding boundary regions. Eulerian boundary regions have sliding edges and must lie completely on an exterior surface of a model. It makes no physical sense to allow material flow to originate on an interior surface. You must explicitly define Eulerian boundary regions since, by default, Abaqus/Explicit assumes that no material flows into or out of an adaptive mesh domain. Eulerian boundary regions are created by defining a surface, a boundary condition, or a load on the boundary of an adaptive mesh domain. On Eulerian boundary regions the mesh motion usually should be constrained in the direction normal to the material motion; therefore, the surface mesh should be fixed in space using spatial mesh constraints (described in “Mesh constraints,” presented later in this section). Applying these constraints normal to an Eulerian boundary region allows material to flow into or out of the mesh, as in a fluid flow problem, while allowing adaptive meshing to occur on the surface of the boundary region to maximize mesh quality. The material flowing into an Eulerian boundary region is assumed to have the same properties as the material that is inside the adaptive mesh domain. Techniques for modeling Eulerian domains are presented in “Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit,” Section 12.2.4. Creation of boundary regions Abaqus/Explicit will create adaptive mesh boundary regions automatically on • the exterior of a model, • the boundary between different adaptive mesh domains, or • the boundary between an adaptive mesh domain and a nonadaptive domain. By default, a boundary region on the exterior of a model will be Lagrangian, so that the boundary region follows the material, and loads, boundary conditions, etc. will retain their Lagrangian interpretation. A boundary region between different adaptive mesh domains is always Lagrangian: no material can flow through such a boundary region. An additional constraint is applied when the model contains multiple parallel domains . In this case the boundary region is nonadaptive: no material can flow through the boundary region, and the nodes on this boundary are constrained to move exactly with the underlying material in all directions. A boundary region between an adaptive mesh domain and a nonadaptive domain is always nonadaptive. The only exception to this occurs if an Eulerian boundary region is defined on the boundary between an adaptive mesh domain and a nonadaptive domain that comprises displacement-based infinite elements. In this case the nodes on the boundary behave as in Eulerian boundary regions , and the mesh motion at the boundary nodes can be constrained using spatial mesh constraints. The boundary between two different materials can never “flow” through the mesh; such a physical boundary is always associated with a Lagrangian boundary region or a nonadaptive mesh boundary. Figure 12.2.2–1 shows that will be created automatically by Abaqus/Explicit. In the model shown in this figure Abaqus/Explicit splits the user-defined adaptive mesh domain into two adaptive mesh domains because the original domain is composed of two different materials. some boundary regions In addition to the boundary regions created automatically by Abaqus/Explicit, Lagrangian, sliding, and Eulerian boundary regions can be created by the definition of surfaces, boundary conditions, and loads, as described later in this section. Geometric features Many models include distinct geometric kinks that take the form of geometric edges or corners. It is usually not desirable to perform adaptive meshing across such geometric features unless they flatten. nonadaptive domain adaptive mesh domain material 1 nonadaptive boundary region Lagrangian boundary region adaptive mesh domain material 2 user-defined adaptive mesh domain: right half of box Figure 12.2.2–1 Automatic splitting of mesh domains and creation of boundary regions. Once a geometric feature does flatten, it is usually best if the feature is deactivated so that adaptive meshing will occur across it. This is especially true when adaptive mesh domains are subject to large deformation. The adaptive meshing algorithm in Abaqus/Explicit will respect geometric features on Lagrangian and sliding boundaries. In three dimensions geometric features consist of edges and corners , while in two dimensions they consist of only corners. If a geometric edge coincides with the edge of a Lagrangian boundary region, the presence of the geometric feature has no effect on the treatment of the edge: material cannot flow perpendicular to a Lagrangian edge. Geometric features are not detected or tracked on Eulerian boundary regions because they generally are not physically meaningful. Output options are available for viewing the formation of geometric edges and corners—see “Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit,” Section 12.2.5. Controlling the detection of geometric edges and corners Geometric features are identified initially as edges on boundary regions where the angle between the normals on adjacent element faces is greater than the initial geometric feature angle, ). See Figure 12.2.2–3. The default value for the initial geometric feature angle is ( . z-symmetry crack front x-symmetry geometric corner Lagrangian corner plus geometric corner geometric edge Lagrangian edge y-symmetry Figure 12.2.2–2 Geometric features formed on a solid block with a crack. θ > θ θ ≤ θ Initial mesh with a geometric feature: no mesh flow is permitted past the corner. The geometric feature is deactivated during simulation. Figure 12.2.2–3 Detection and deactivation of geometric features. You can change the value of the angle that will be used to recognize geometric features. Setting will ensure that no geometric edges or corners are formed on the boundary of the adaptive mesh domain. Input File Usage: *ADAPTIVE MESH CONTROLS, NAME=name, INITIAL FEATURE ANGLE= Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Initial feature angle: Controlling the deactivation of geometric edges and corners Geometric features affect only Lagrangian and sliding boundary regions, where they act as temporary Lagrangian edges. During each mesh sweep in an adaptive mesh increment, nodes along a geometric edge are positioned by applying the basic smoothing methods . The nodes are constrained to lie along the discrete geometric edge unless the angle forming the geometric edge becomes less than the transition geometric feature angle, . If the angle across the geometric edge becomes less than , the boundary surface is considered to be flattened sufficiently for the feature to be deactivated, and the mesh is allowed to slide freely over the material (unconstrained by the deactivated geometric edge). Geometric corners are allowed to flatten in a similar fashion. This logic allows great flexibility in mesh adaptation while preserving geometric features in the model. ). The default value for the transition feature angle is ( You can change the transition feature angle. Setting will ensure that no geometric edges or corners are ever deactivated. Input File Usage: *ADAPTIVE MESH CONTROLS, NAME=name, TRANSITION FEATURE ANGLE= Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Transition feature angle: Mesh constraints In most adaptive mesh problems the motion of nodes in the mesh is determined by the meshing algorithm, with constraints imposed by the domain boundary and the boundary region edges. However, there are cases when you must explicitly define the motion of the nodes. As explained earlier, Eulerian and sliding boundary regions generally require mesh constraints for the regions to be physically meaningful. In some problems you may wish to keep certain nodes fixed, to move nodes in a particular direction, or to force certain nodes to move with the material. In other problems you may desire a node or particular set of nodes to follow the material motion. Adaptive mesh constraints allow full control over the mesh movement and act independently of any boundary conditions or loads applied to the underlying material. Applying spatial mesh constraints Use a spatial mesh constraint (the default) to prescribe spatial mesh motion that is independent of the material motion. You specify the nodes to which the constraint is applied, the directions of the prescribed motion, and the amplitude of the prescribed motion. You can prescribe either a displacement or a velocity for the spatial mesh motion. Input File Usage: Use the following option to define the mesh constraints explicitly: *ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=SPATIAL, TYPE=DISPLACEMENT or VELOCITY Abaqus/CAE Usage: To define the mesh constraints explicitly: Step module: Other→ALE Adaptive Mesh Constraint→Create: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Independent of underlying material Rules for applying spatial mesh constraints Spatial mesh constraints can be applied without restriction to nodes on an Eulerian boundary region or in the interior of an adaptive mesh domain. In both two and three dimensions nodes at Lagrangian and active geometric corners are fully constrained to move with the underlying material. No mesh constraints can be applied at such corners. Adaptive mesh constraints must not conflict with other mesh constraints inherent to Lagrangian and sliding boundary regions; therefore, adaptive mesh constraints can be applied only tangentially to a Lagrangian or sliding boundary region. This restriction implies that adaptive mesh constraints can be applied only in two directions in a three-dimensional boundary region, in one direction in a two- dimensional boundary region, or in one direction on a Lagrangian or active geometric edge. It may not always be feasible to adhere to this rule, particularly if the boundary experiences finite rotation. Therefore, if the normal to a boundary region is not perpendicular to a prescribed mesh constraint at a node, it is always moved along the current surface of the boundary region so that the projection of the mesh motion in the direction of the prescribed constraint is correct . If the normal to the boundary region approaches the direction of the applied mesh constraint, large mesh motions will be required to satisfy the constraint. By default, an analysis is terminated if the angle between the normal to the boundary region and the direction of the prescribed constraint becomes less than . This cutoff angle is referred to as the mesh constraint angle, and its default value is 60°. The mesh constraint angle, , is also used when adaptive mesh constraints are applied to nodes along a Lagrangian or active geometric edge. Since independent mesh motion cannot be prescribed perpendicular to these edges, an analysis is terminated if the angle between the prescribed constraint and the plane perpendicular to the edge falls below the specified mesh constraint angle. You can change the value of the mesh constraint angle ( is not recommended because it may cause errors in determining the free surface geometry, especially for curved surfaces. ). Setting Input File Usage: Abaqus/CAE Usage: *ADAPTIVE MESH CONTROLS, MESH CONSTRAINT ANGLE= Step module: Other→ALE Adaptive Mesh Controls→Create: Mesh constraint angle: Defining mesh constraints that vary with time The prescribed magnitude of a nonzero mesh constraint can vary with time during a step according to an amplitude definition . Input File Usage: Use both of the following options: *AMPLITUDE, NAME=name *ADAPTIVE MESH CONSTRAINT, AMPLITUDE=name t = t1 zero-displacement adaptive mesh constraint applied at node 3 in direction 1 direction of applied constraint Θ < Θ c, analysis is terminated movement of node 3 without mesh constraint motion of node 3 along surface to satisfy constraint boundary region t = t0 projection of mesh motion in prescribed direction Figure 12.2.2–4 Enforcing a spatial mesh constraint. Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Constraint→Create: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Independent of underlying material: Amplitude: amplitude Applying spatial mesh constraints in local directions Spatial mesh constraints are applied in local directions if a local coordinate system is defined at a node ; otherwise, they are applied in global directions. Applying Lagrangian mesh constraints Lagrangian mesh constraints on a node are used to indicate that mesh smoothing should not be applied; i.e., the node must follow the material. Input File Usage: *ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=LAGRANGIAN Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Constraint→Create: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Follow underlying material Modifying ALE adaptive mesh constraints By default, all adaptive mesh constraints defined in the previous analysis step remain unchanged in the subsequent step. You define the adaptive mesh constraints in effect for a given step relative to the preexisting adaptive mesh constraints. At each new step the existing adaptive mesh constraints can be modified and additional adaptive mesh constraints can be specified. Input File Usage: Use either of the following options to modify an existing adaptive mesh constraint or to specify an additional adaptive mesh constraint: Abaqus/CAE Usage: *ADAPTIVE MESH CONSTRAINT, *ADAPTIVE MESH CONSTRAINT, OP=MOD Step module: Other→ALE Adaptive Mesh Constraint→Manager: select the desired step and mesh constraint: Edit Removing ALE adaptive mesh constraints If you choose to remove any adaptive mesh constraint in a step, no adaptive mesh constraints will be propagated from the previous step. Therefore, all adaptive mesh constraints that are in effect during this step must be respecified. Input File Usage: Use the following option to remove all previously defined adaptive mesh constraints and to specify new adaptive mesh constraints: *ADAPTIVE MESH CONSTRAINT, OP=NEW If the OP=NEW parameter is used on any *ADAPTIVE MESH CONSTRAINT option within a step, it must be used on all *ADAPTIVE MESH CONSTRAINT options in the step. Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Constraint→Manager: select the desired step and mesh constraint: Deactivate Initial conditions There are no initial conditions specific to adaptive meshing; initial conditions can be defined in the same way as in nonadaptive problems. If initial mesh sweeps are performed to smooth the mesh at the beginning of a step , all initial conditions (except temperatures and field variables, which are discussed in “Predefined fields,” presented later in this section) are remapped to the new mesh. Initial temperatures are remapped during adaptive meshing in an adiabatic analysis. Initial conditions prescribed near an inflow Eulerian boundary region will affect the state of the material flowing into the domain throughout the analysis. See “Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit,” Section 12.2.4, for a discussion of the proper treatment of inflow boundaries. Defining surfaces on ALE adaptive mesh boundaries When you define a surface on the boundary of an adaptive mesh domain , Abaqus creates a boundary region coinciding with the surface. By default, a sliding boundary region is created. You can choose to create a Lagrangian or Eulerian boundary region instead. A surface defined in the interior of an adaptive mesh domain will move independently of the material (unless constrained by mesh constraints). Defining a sliding boundary region using a surface By default, the boundary region created by a surface definition will be sliding (the surface edge will slide freely over the material). Input File Usage: Abaqus/CAE Usage: *SURFACE, REGION TYPE=SLIDING Boundary regions defined using surfaces are not supported in Abaqus/CAE. Defining a Lagrangian boundary region using a surface To force the surface edge to follow the material, create a Lagrangian boundary region. Input File Usage: Abaqus/CAE Usage: *SURFACE, REGION TYPE=LAGRANGIAN Boundary regions defined using surfaces are not supported in Abaqus/CAE. Defining an Eulerian boundary region using a surface To decouple the surface from the material motion, create an Eulerian boundary region and apply spatial mesh constraints normal to the surface. If no mesh constraints are applied, the surface will behave like a sliding boundary region (no material will flow through the surface). As an example, it is often assumed that there is no normal or shear stress in the material at the outflow boundary of an Eulerian domain. This condition can be modeled by defining an Eulerian boundary region using a surface and applying spatial mesh constraints perpendicular to the surface, as shown in Figure 12.2.2–5. Input File Usage: Abaqus/CAE Usage: *SURFACE, REGION TYPE=EULERIAN Boundary regions defined using surfaces are not supported in Abaqus/CAE. Contact Lagrangian and sliding boundary regions created using surfaces can be used in contact pairs; they have the same meaning as surfaces defined on nonadaptive regions. Since contact generally involves relative sliding between bodies, sliding boundary regions are typically appropriate for contact surfaces. Surfaces defined on Eulerian boundary regions cannot be used in contact pairs. free surface Lagrangian boundary region (automatic) flow node set OUT Eulerian boundary region (defined using a surface) symmetry Lagrangian boundary region (automatic) zero-displacement adaptive mesh constraint applied to node set OUT in direction 1 Figure 12.2.2–5 Modeling the outflow boundary of an Eulerian adaptive mesh domain. If the small-sliding formulation is used for a contact pair, all the nodes on both surfaces are nonadaptive . The nodes of an element-based surface in a no-separation contact pair are nonadaptive . All nodes in a general contact domain are nonadaptive . Similarly, the nodes at which spot welds are defined are nonadaptive Distributed loads When a distributed pressure load is applied to the boundary of an adaptive mesh domain, Abaqus/Explicit creates a boundary region that coincides with the area of the load application. The characteristics of boundary regions created in this way are identical to those of boundary regions created by defining surfaces. If a pressure load is applied to a surface in the interior of an adaptive mesh domain, the nodes on the surface will move with the material in all directions (i.e., they will be nonadaptive). Boundary regions created by different pressure loads may overlap. If pressure loads with the same magnitude and amplitude definition are applied to adjacent regions, the regions will be merged into a single boundary region to minimize the number of Lagrangian edges and corners formed . If a nonuniform pressure is applied (for example, a pressure that varies linearly over a surface) or if a pressure load is defined in user subroutine VDLOAD, each element face or edge becomes a separate Lagrangian boundary region. Since Lagrangian corners are formed where Lagrangian edges meet, all If these distributed loads have identical magnitudes and amplitude definitions, they will be combined into one Lagrangian boundary region. Overlapping distributed loads result in three Lagrangian boundary regions. This node is adaptive because the sliding boundary region does not create a Lagrangian corner. L = Lagrangian boundary region created by pressure load S = Sliding boundary region created by pressure load = Lagrangian corner Figure 12.2.2–6 Applying distributed pressure loads to an adaptive mesh domain. nodes will follow the material in every direction, and each region becomes nonadaptive. Likewise, if a nonuniform body force is applied to an adaptive mesh domain, the domain is split into multiple domains, each with a uniform body force. If this splitting results in one-element domains, the region becomes nonadaptive. Defining a Lagrangian boundary region with a pressure load By default, the boundary region created to coincide with a pressure load will be Lagrangian. Pressure loads applied to Lagrangian regions are identical to pressure loads applied to nonadaptive regions, except that the mesh can move inside the boundary region. Input File Usage: Abaqus/CAE Usage: *DLOAD, REGION TYPE=LAGRANGIAN Boundary regions defined using pressure loads are not supported in Abaqus/CAE. Defining a sliding boundary region with a pressure load A pressure load can be applied to a sliding boundary region to simulate a load that is fixed in space while material moves past it . A sliding edge is unconstrained in the direction tangential to the boundary region; therefore, unless adaptive mesh constraints are applied, the area of the load application will move according to the adaptive meshing algorithm, which is probably not physically meaningful. To allow a pressure load to slide over the material, create a sliding boundary region. Input File Usage: Abaqus/CAE Usage: *DLOAD, REGION TYPE=SLIDING Boundary regions defined using pressure loads are not supported in Abaqus/CAE. P0 flow flow flow Lagrangian interpretation Spatial (sliding) interpretation t = t0 t = t1 t = t1 = sliding boundary region created by pressure load = zero-displacement adaptive mesh constraints applied to nodes 1 and 4 in direction 1 Figure 12.2.2–7 Applying a sliding distributed pressure load to an adaptive mesh domain. Defining an Eulerian boundary region with a pressure load To decouple the area of pressure application from the material motion, create an Eulerian boundary region and apply spatial mesh constraints normal to the surface. If no mesh constraints are applied, the mesh will behave like a sliding boundary region (no material will flow through the surface). As an example, it is often assumed that a uniform ambient pressure exists at the outflow boundary of an Eulerian domain. This condition can be modeled by defining the pressure at an Eulerian boundary region using a distributed load and applying spatial mesh constraints perpendicular to the surface, as shown in Figure 12.2.2–8. Input File Usage: Abaqus/CAE Usage: *DLOAD, REGION TYPE=EULERIAN Boundary regions defined using pressure loads are not supported in Abaqus/CAE. Distributed surface fluxes and thermal conditions In coupled thermal-stress analysis Abaqus/Explicit also creates boundary regions for distributed surface fluxes, convective film conditions, and radiation conditions. The rules governing boundary regions for free surface flow node set OUT symmetry = Eulerian boundary region created by pressure load = zero-displacement adaptive mesh constraint applied to node set OUT in direction 1 Figure 12.2.2–8 Modeling an ambient pressure at the outflow boundary of an Eulerian adaptive mesh domain. these loads are identical to those discussed for distributed loads. The ability to specify the boundary region type is also the same. Concentrated loads When a concentrated load is applied to the boundary of an adaptive mesh domain, Abaqus/Explicit creates a boundary region to coincide with the load. Every node to which a concentrated load is applied will be considered its own boundary region because it is not possible to identify a surface area associated with a concentrated load. However, you can control the behavior of each one-node region. If concentrated loads are applied to nodes in the interior of an adaptive mesh domain, those nodes will move with the material in all directions (i.e., they will be nonadaptive). Defining a Lagrangian boundary region with a concentrated load By default, the boundary region created by a concentrated load will be Lagrangian. Each one-node Lagrangian boundary region will follow the material in every direction (the nodes will be nonadaptive). Input File Usage: Abaqus/CAE Usage: *CLOAD, REGION TYPE=LAGRANGIAN Boundary regions defined using concentrated loads are not supported in Abaqus/CAE. Defining a sliding boundary region with a concentrated load A concentrated load can be applied to a sliding boundary region to simulate a load that is fixed in space while material moves past it . A sliding node is unconstrained in the direction Lagrangian interpretation material slides past this node zero-displacement adaptive mesh constraint applied to node N in direction 1 Sliding interpretation t = t0 flow t = t1 flow t = t1 flow Figure 12.2.2–9 Applying a concentrated sliding load to an adaptive mesh domain. tangential to the boundary region; therefore, unless adaptive mesh constraints are applied, the point of load application will move according to the adaptive meshing algorithm, which is probably not physically meaningful. To allow the concentrated load to slide freely over the material, create a sliding boundary region. Input File Usage: Abaqus/CAE Usage: *CLOAD, REGION TYPE=SLIDING Boundary regions defined using concentrated loads are not supported in Abaqus/CAE. Defining an Eulerian boundary region with a concentrated load To decouple the concentrated load from the material motion, create an Eulerian boundary region and apply spatial mesh constraints normal to the surface. If no mesh constraints are applied, each one-node boundary region will behave like a sliding boundary region. Input File Usage: *CLOAD, REGION TYPE=EULERIAN Abaqus/CAE Usage: Boundary regions defined using concentrated loads are not supported in Abaqus/CAE. Concentrated fluxes and thermal conditions In coupled thermal-stress analysis Abaqus/Explicit also creates boundary regions for concentrated heat fluxes, film conditions, and radiation conditions. The rules governing boundary regions for these loads are identical to those discussed for concentrated loads. The ability to specify the boundary region type is also the same. Boundary conditions Lagrangian, sliding, and Eulerian boundary regions can be created by applying kinematic constraints to the boundary of an adaptive mesh domain. If kinematic boundary conditions are applied to nodes in the interior of an adaptive mesh domain, those nodes will move with the material in all directions (i.e., they will be nonadaptive), regardless of the specified boundary region type. Defining a Lagrangian boundary region using a boundary condition By default, the boundary region created by a kinematic boundary condition will be Lagrangian. Abaqus/Explicit will recognize surface-type and point or edge constraints automatically and will create an appropriate Lagrangian boundary region for each type, as explained in the following subsections. *BOUNDARY, REGION TYPE=LAGRANGIAN Boundary regions defined using boundary conditions are not supported in Abaqus/CAE. Abaqus/CAE Usage: Input File Usage: Surface-type constraints applied using boundary conditions Although boundary conditions are always applied to individual nodes in Abaqus/Explicit, they often represent physical constraints on surfaces. For example, symmetry conditions, where nodes are constrained to move in a plane, are actually surface constraints. A fully clamped (ENCASTRE) condition along a boundary can also be considered a surface constraint. (During adaptive meshing it is meaningful to allow nodes to move along a fully clamped edge.) Abaqus/Explicit will examine an adaptive mesh boundary and try to create regions that are coincident with the applied boundary conditions. Currently, Abaqus/Explicit can create boundary regions for surface-based constraints on: • symmetry planes, • fully clamped planes, and • planes on which a uniform motion is prescribed. Figure 12.2.2–2 shows an example in which boundary regions are created by applying surface-type boundary conditions. This figure shows a block of material with a crack and three symmetry planes (therefore, three Lagrangian boundary regions). Material will not flow across any symmetry plane, yet adaptive meshing can be performed within each Lagrangian boundary region. This flexibility is often helpful in problems that have significant deformation. Point or edge constraints applied using boundary conditions Some boundary conditions represent point or edge constraints. For example, a displacement can be prescribed at a node. The boundary regions associated with such nodes are exactly the same as those created by concentrated loads. Defining a sliding boundary region using a boundary condition A sliding boundary region associated with a boundary condition can move according to the adaptive meshing algorithm. Since this behavior is probably not physically meaningful, the edges of a sliding boundary region are usually fixed in the direction tangential to the surface using adaptive mesh constraints. This approach can be used, for example, to simulate frictionless contact between a rigid punch and a deformable body, as shown in Figure 12.2.2–10. = node set CONTACT zero-displacement adaptive mesh constraint applied to node N in direction 1 sliding boundary region created by velocity-type boundary condition applied to node set CONTACT material flows past node N (a) effect of punch modeled with contact (b) effect of punch modeled with boundary conditions applied to sliding boundary region Figure 12.2.2–10 Contact simulation using a sliding boundary region. In this example the punch is replaced by a sliding boundary region with a constant velocity boundary condition applied in the area of “contact.” A tangential mesh constraint is applied to the edge of the boundary region at node N (the other edge is constrained by the Lagrangian boundary region created automatically on the symmetry plane). This problem definition allows material to flow radially underneath the “punch” while retaining the original size and location of the “contact” area. Abaqus/Explicit makes no distinction between surface-type constraints and point or edge constraints for sliding boundary regions. To allow the boundary condition to slide freely over the material, create a sliding boundary region. Input File Usage: Abaqus/CAE Usage: *BOUNDARY, REGION TYPE=SLIDING Boundary regions defined using boundary conditions are not supported in Abaqus/CAE. Defining an Eulerian boundary region using a boundary condition To decouple the boundary region from the material motion, create an Eulerian boundary region and apply spatial mesh constraints normal to the surface. If no mesh constraints are applied, the mesh will behave like a sliding boundary region (no material will flow through the surface). As an example, the mass flow rate at an Eulerian inflow boundary can be prescribed by defining an Eulerian boundary region using a boundary condition. Abaqus/Explicit makes no distinction between surface-type constraints and point or edge constraints for Eulerian boundary regions. Input File Usage: Abaqus/CAE Usage: *BOUNDARY, REGION TYPE=EULERIAN Boundary regions defined using boundary conditions are not supported in Abaqus/CAE. Overlapping boundary regions A Lagrangian boundary region can overlap any number of other Lagrangian or sliding boundary regions . If two boundary regions partially overlap, three regions are formed: the overlapping region and the two initial regions minus the overlapping region. A sliding boundary region is formed when a Lagrangian and a sliding boundary region overlap. An Eulerian boundary region can never overlap a Lagrangian or sliding boundary region. Furthermore, an Eulerian boundary region can never share a boundary with or overlap a nonadaptive region. Because infinite elements are nonadaptive, this latter restriction implies that infinite elements cannot be used to simulate ambient conditions at an outflow boundary. Coincident edges Edges shared by different types of boundary regions are subject to the following rules: • An edge shared between a Lagrangian and a sliding boundary region will be Lagrangian. • An edge shared between a Lagrangian and an Eulerian boundary region will be sliding. • An edge shared between a Lagrangian and a nonadaptive boundary region will be nonadaptive. • An edge shared between a sliding and a nonadaptive boundary region will be nonadaptive. • An edge of an Eulerian boundary region can never be coincident with an edge of a nonadaptive region. Predefined fields There are no restrictions on applying prescribed temperatures or field variables in an adaptive mesh domain, but these nodal values are not remapped when adaptive meshing is performed. Therefore, predefined fields that are not spatially uniform may not be meaningful within an adaptive mesh domain. Lagrangian edge Sliding edge Lagrangian corner L = Lagrangian boundary region S = Sliding boundary region E = Eulerian boundary region Figure 12.2.2–11 Overlapping boundary regions. (Time-varying, spatially uniform predefined fields are acceptable, since adaptive meshing is applied at discrete instances in time.) However, if temperature or field variable data are collected from a spatial frame of reference, it may make physical sense to apply a spatially varying field for an Eulerian domain in which the mesh does not move. Abaqus/Explicit does not perform any checks or calculations on predefined fields for adaptive meshing; you must ensure that the predefined fields are meaningful. Materials All material models and behaviors, except brittle cracking (“Cracking model Section 23.6.2), (“Low-density foams,” Section 22.9.1) materials, can be used in an adaptive mesh domain. fabric (“Fabric material behavior,” Section 23.4.1), for concrete,” and low-density foam For domains modeled with hyperelastic or hyperfoam materials the usefulness of adaptive meshing is limited. The recommended enhanced hourglass method (“Section controls,” Section 27.1.4), which will generally predict a much better return to the original configuration for these materials when loading is removed, cannot be used in an adaptive mesh domain. Therefore, for hyperelastic or hyperfoam materials it is recommended that the analysis be run without adaptive meshing but with enhanced hourglass control. If the porous failure model (“Failure criteria in Abaqus/Explicit” in “Porous metal plasticity,” Section 23.2.9), shear failure model (“Shear failure model” in “Dynamic failure models,” Section 23.2.8), tensile failure model (“Tensile failure model” in “Dynamic failure models,” Section 23.2.8), or one of the progressive damage models (Chapter 24, “Progressive Damage and Failure”) is specified within an adaptive mesh domain, Abaqus/Explicit will continuously monitor the status of elements while performing adaptive meshing. When elements within the domain fail, the nodes along the interface between the failed and unfailed elements will become nonadaptive. This has the effect of creating a material boundary between the failed and unfailed zones. When failure occurs in elements that use the shear failure, the tensile failure, or the progressive damage models without element deletion, elements in the failure zone will not be deleted; they can carry some states of stress. Adaptive meshing will occur within the failure zone but not along the interface with the unfailed material. Elements An adaptive mesh domain can contain only first-order, reduced-integration, solid elements. All elements within an adaptive mesh domain must have the same geometry (all two-dimensional, three-dimensional, axisymmetric, or plane strain, etc.). Since adaptive mesh domains are split across element types, degenerate elements should be used for mixed domains that include both triangles and quadrilaterals (or tetrahedron and bricks). All elements other than first-order, reduced-integration, solid elements—including mass, rotary inertia, and infinite elements—are nonadaptive. These elements can be connected to an adaptive mesh domain, but their nodes are nonadaptive. All nodes and elements on a rigid body are nonadaptive. Rebar are not supported within an adaptive mesh domain. Multi-point constraints and equations As with boundary conditions, multi-point constraints (“General multi-point constraints,” Section 34.2.2) and equations (“Linear constraint equations,” Section 34.2.1) are always applied to nodes but sometimes represent constraints on surfaces. Abaqus/Explicit will recognize surface-type constraints when the following conditions are satisfied: • an equation, PIN MPC, or TIE MPC ties a node set to a single node; and • all the nodes involved in the MPC or equation are coplanar and lie within the boundary region. If these conditions are satisfied, a boundary region will be associated with the node set in the MPC or equation. If the MPC is applied within a Lagrangian or sliding boundary region, a Lagrangian edge will be created. If the MPC is applied within an Eulerian boundary region, no edge will be created. If the above conditions are not satisfied, all nodes connected to the MPC or equation will be nonadaptive. As an example, a constraint can be applied to force a plane section to remain plane in a Lagrangian adaptive mesh domain, as shown in Figure 12.2.2–12(a). In this case all nodes are constrained by an equation to lie in the same plane throughout the analysis, but adaptive meshing is allowed within the plane. As another example, consider the outflow boundary of an Eulerian domain, as shown in Figure 12.2.2–12(b). The outflow boundary of an Eulerian domain is often assumed to be far enough downstream that the velocity is uniform but unknown. To model this condition, an Eulerian boundary region is created at the outflow boundary using a surface. An adaptive mesh constraint is used to fix the mesh perpendicular to the boundary, and all nodes on the plane are constrained by an equation to have the same velocity orthogonal to the plane. For surface-based tie constraints , all nodes on the tied surfaces will be nonadaptive. Lagrangian boundary region node set PLANE Linear constraint equation 1.0u 1.0u = 0 PLANE (a) Using an equation to force a plane section to remain a plane. zero-displacement adaptive mesh constraints applied to node 1 and to node set OUTFLOW in direction 1 material flow element set OUTFLOW node set OUTFLOW Linear constraint equation 1.0u = 0 1.0u OUTFLOW Eulerian boundary region created using a surface defined on the S4 faces of element set OUTFLOW (b) Using an equation to prescribe a uniform velocity outflow condition. Figure 12.2.2–12 Using equations with adaptive meshing. Procedures During an adiabatic analysis temperatures will be remapped properly in adaptive mesh domains. Adaptive meshing is not used during annealing procedures or during geometrically linear analyses. The definitions of adaptive mesh domains, boundary regions, mesh constraints, and controls (as explained in “ALE adaptive meshing and remapping in Abaqus/Explicit,” Section 12.2.3) will propagate from step to step. User subroutines Solution-dependent state variables defined in user subroutine VUMAT will be remapped to the new mesh when adaptive meshing is performed. Solution-dependent state variables that are defined on a slave surface in user subroutines VFRIC, VUINTER, VFRICTION, and VUINTERACTION will not be remapped to the new mesh when adaptive meshing is performed. Therefore, to ensure physically meaningful results, a Lagrangian adaptive mesh constraint should be used for nodes on the contact slave surfaces with solution-dependent state variables where the contact constraint is defined using these user subroutines. Output Since the mesh is no longer constrained to the material when adaptive meshing is performed, output at elements and nodes must be interpreted differently than in a pure Lagrangian problem. See “Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit,” Section 12.2.5, for details. Input file template To create a Lagrangian adaptive mesh domain: *HEADING … *ELSET, ELSET=ADAPT ************************* *STEP *DYNAMIC, EXPLICIT Data line to specify the time period of the step *ADAPTIVE MESH, ELSET=ADAPT ... *END STEP To create an Eulerian adaptive mesh domain with a prescribed velocity inflow condition and a prescribed pressure outflow condition (both in the global x-direction): *HEADING... *ELSET, ELSET=ADAPT ... *ELSET, ELSET=OUT ... *NSET, NSET=INFLOW ... *NSET, NSET=OUTFLOW ... *SURFACE, NAME=INSURF, REGION TYPE=EULERIAN Data lines to define the surface *SURFACE, NAME=OUTSURF, REGION TYPE=EULERIAN Data lines to define the surface ... *EQUATION Data lines specifying uniform velocity at the inflow ************************* *STEP *DYNAMIC, EXPLICIT Data line to specify the time period of the step *ADAPTIVE MESH, ELSET=ADAPT *ADAPTIVE MESH CONSTRAINT INFLOW, 1, 1, 0 OUTFLOW, 1, 1, 0 *BOUNDARY, TYPE=VELOCITY, REGION TYPE=EULERIAN INFLOW, 1, 1, 10.0 *DLOAD, REGION TYPE=EULERIAN OUT, P2, 15.0 ... *END STEP 12.2.3 ALE ADAPTIVE MESHING AND REMAPPING IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “ALE adaptive meshing: overview,” Section 12.2.1 • “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2 • “Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit,” Section 12.2.5 • *ADAPTIVE MESH • *ADAPTIVE MESH CONSTRAINT • *ADAPTIVE MESH CONTROLS • “Customizing ALE adaptive meshing,” Section 14.14 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview ALE adaptive meshing consists of two fundamental tasks: • creating a new mesh, and • remapping solution variables from the old mesh to the new mesh with a process called advection. The success of the adaptive meshing technique depends on the choice of the methods used for each of these tasks. The default methods for creating a new mesh and for remapping solution variables have been chosen carefully to work for a wide variety of problems. However, you may wish to override the default choices to balance the robustness and efficiency of adaptive meshing or to extend the use of adaptive meshing to more difficult or unusual applications. Meshing A new mesh: • is created at a specified frequency for each adaptive domain; • is found by sweeping iteratively over the adaptive mesh domain and moving nodes to smooth the mesh; and • can retain the initial gradation of the original mesh. Remapping The methods used for advecting solution variables to the new mesh: • are consistent, monotonic, and (by default) accurate to the second order; and • conserve mass, momentum, and energy. Controlling the frequency of ALE adaptive meshing In most cases the frequency of adaptive meshing is the parameter that most affects the mesh quality and the computational efficiency of adaptive meshing. A typical adaptive mesh application without Eulerian boundaries will require adaptive meshing every 5–100 increments. In contrast, adaptive meshing should generally be performed much more frequently in a steady-state process simulation using Eulerian boundaries. Thus, if a spatial adaptive mesh constraint or an Eulerian boundary region is defined on an adaptive mesh domain, the default frequency is 1; otherwise, the default frequency is 10. Input File Usage: Use the following option to change the frequency of adaptive meshing: Abaqus/CAE Usage: *ADAPTIVE MESH, FREQUENCY=number of increments Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on Use the ALE adaptive mesh domain below, Frequency: number of increments Controlling the intensity of ALE adaptive meshing During each adaptive meshing increment, the new mesh is created by performing one or more mesh sweeps and then advecting the solution variables to the new mesh. Mesh sweeps In an adaptive meshing increment, a new, smoother mesh is created by sweeping iteratively over the adaptive mesh domain. During each mesh sweep, nodes in the domain are relocated—based on the current positions of neighboring nodes and elements—to reduce element distortion. In a typical sweep a node is moved a fraction of the characteristic length of any element surrounding the node. Increasing the number of sweeps increases the intensity of adaptive meshing in each adaptive meshing increment. The default number of mesh sweeps is one. Input File Usage: Use the following option to change the number of mesh sweeps to be performed in each adaptive mesh increment: Abaqus/CAE Usage: *ADAPTIVE MESH, MESH SWEEPS=number of sweeps Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on Use the ALE adaptive mesh domain below, Remeshing sweeps per increment: number of sweeps Advection sweeps The process of mapping solution variables from an old mesh to a new mesh is referred to as an advection sweep. At least one advection sweep is performed in every adaptive mesh increment. Ideally, an advection sweep will be performed only once, after all mesh sweeps for the increment are complete. However, numerical stability of the advection sweep is maintained only if the difference between the old mesh and the new mesh is small. Therefore, if after a mesh sweep the total accumulated movement of any node in the domain is greater than 50% of the characteristic length of any adjacent element, an advection sweep is performed to remap the solution variables from the old mesh to the intermediate mesh. Mesh sweeps will continue until the specified number is reached or until the movement of any node again exceeds the 50% threshold. At this time an advection sweep is performed again to map variables from the last intermediate mesh to the new intermediate mesh. The cycle will continue until the number of mesh sweeps reaches the specified number. The number of advection sweeps per adaptive mesh increment required for each adaptive mesh domain is determined automatically by Abaqus/Explicit; you cannot override this automatic calculation. The number of advection sweeps is printed by default to the message (.msg) file . The computational cost of ALE adaptive meshing The cost of adaptive meshing depends on the frequency of remeshing, the number of mesh and advection sweeps performed, and the size of the adaptive mesh domains. When compared to a purely Lagrangian analysis, additional computational cost is incurred only within adaptive mesh increments. Generally, the cost of one advection sweep is several times greater than the cost of one mesh sweep. Multiple advection sweeps are triggered when adaptive meshing is performed too infrequently and/or a high number of mesh sweeps is specified. Performing adaptive meshing more frequently and doing 1–5 mesh sweeps in each adaptive mesh increment will usually generate only one advection sweep, minimizing the computational cost. The relatively smooth mesh and improved element aspect ratios that result from adaptive meshing may increase the stable time increment compared to a similar pure Lagrangian analysis. In some cases this increase can offset the cost of adaptive meshing completely. Although computational cost can vary greatly with the type of application, performing adaptive meshing on the entire problem domain in every increment will typically increase the cost of the analysis by 3–5 times that of a similar Lagrangian analysis. Defining adaptive mesh domains that cover only a fraction of the entire problem domain will reduce the cost proportionally. Changing the frequency to every 10–25 increments will result in CPU times that are only moderately higher than those for a pure Lagrangian analysis. Guidelines for controlling ALE adaptive meshing frequency and intensity Although the default values work well for many problems, difficult analyses may require a more frequent adaptive meshing frequency or meshing with a higher intensity. Guidelines for transient analysis For problems without spatial adaptive mesh constraints or Eulerian boundary regions, the default frequency for adaptive meshing is 10, and the default number of mesh sweeps is 1. The default values are usually adequate for low- to moderate-rate dynamic problems and for quasi-static process If the frequency or number of mesh sweeps is too simulations undergoing moderate deformation. low, excess element distortion may cause the analysis to terminate before the mesh is adapted; or, if a solution can be obtained, it may not be as accurate as the solution that could be obtained with a higher quality mesh. In virtually all cases, however, performing adaptive meshing at any frequency will reduce the distortion of elements (and, thus, improve the quality of the solution) compared to a pure Lagrangian analysis. For high-rate impact problems undergoing large amounts of deformation, it may be necessary to increase the frequency of adaptive meshing or the number of mesh sweeps. It is generally less expensive to increase the number of mesh sweeps slightly before increasing the frequency, as long as the number of advection sweeps remains small. For problems involving explosions taking place over just a few hundred increments, adaptive meshing is usually required at every increment. It may also be necessary to increase the frequency of adaptive meshing for quasi-static process simulations that involve large amounts of flow per increment. For problems in which the deformation per increment is small, a high-quality mesh can be maintained by performing adaptive meshing only every 25–100 increments. For these problems the additional cost of adaptive meshing is negligible. Guidelines for steady-state analysis When an adaptive mesh domain contains Eulerian boundary regions or has spatial adaptive mesh constraints, the default frequency of adaptive meshing is 1. This default frequency is conservative and is chosen primarily because spatial mesh constraints are applied only during adaptive mesh increments. Thus, between adaptive mesh increments the mesh may drift from its prescribed location, which may affect the solution. However, drift from adaptive mesh constraints will always be eliminated in the next adaptive mesh increment: it will not accumulate. For problems in which the speed of deformation or the speed of material flow from element to element is much less than the material wave speed, the frequency typically can be increased to 5 or higher. This class of problems includes most steady-state process simulations, where the drift of the mesh from the prescribed location is negligible over a few increments. By performing adaptive meshing less often, steady-state simulations become competitive with their corresponding transient simulations. For Eulerian domains in which the speed of the deformation or material flow is high, such as in dynamic shock problems, the default frequency of 1 should be used. Mesh smoothing methods The determination of the new mesh in Abaqus/Explicit is based on four aspects. You can control each of these aspects by defining adaptive mesh controls. Defaults have been chosen so that the overall algorithm works well for most problems. First, the calculation of the new mesh in Abaqus/Explicit is based on some combination of three basic smoothing methods: volume smoothing, Laplacian smoothing, and equipotential smoothing. The smoothing methods are applied at each node in the adaptive mesh domain to determine the new location of the node based on the locations of surrounding nodes or elements. Although all the smoothing methods tend to smooth the mesh and reduce element distortion, the resulting meshes will differ depending on the methods used. Second, initial element gradation can be maintained at the expense of element distortion if desired. Third, optimal positioning of the nodes before the basic smoothing methods are applied can improve mesh quality and minimize the frequency of adaptive meshing required. Finally, solution-dependent meshing is used to concentrate mesh refinement near areas of evolving boundary curvature. This counteracts the tendency of the basic smoothing methods to reduce the mesh refinement near concave boundaries where solution accuracy is important. Volume smoothing Volume smoothing relocates a node by computing a volume-weighted average of the element centers in the elements surrounding the node. In Figure 12.2.3–1 the new position of node M is determined by a volume-weighted average of the positions of the element centers, C, of the four surrounding elements. The volume weighting will tend to push the node away from element center C1 and toward element center C3, thus reducing element distortion. L3 C4 C3 L4 C1 C2 L1 L2 Figure 12.2.3–1 Relocation of a node during a mesh sweep. Volume smoothing is very robust and is the default method in Abaqus/Explicit. It works well for both structured and highly unstructured domains. (A structured domain is one that contains no degenerate elements and where every node is surrounded by four elements in two dimensions or eight elements in three dimensions.) Laplacian smoothing Laplacian smoothing relocates a node by calculating the average of the positions of each of the adjacent nodes connected by an element edge to the node in question. In Figure 12.2.3–1 the new position of node M is determined by averaging the positions of the four nodes, L, connected to M by element edges. The locations of nodes L2 and L3 will pull node M up and to the right to reduce element distortion. Laplacian smoothing is the least expensive smoothing algorithm and is commonly used in mesh preprocessors. For low to moderately distorted mesh domains, the results of Laplacian smoothing are similar to volume smoothing. For domains with boundaries of complex curvature, volume smoothing generally results in a more balanced mesh. Equipotential smoothing Equipotential smoothing is a higher-order method that relocates a node by calculating a higher-order, weighted average of the positions of the node’s eight nearest neighbor nodes in two dimensions (or its eighteen nearest neighbor nodes in three dimensions). In Figure 12.2.3–1 the new position of node M is based on the position of all the surrounding nodes, L and E. The weighted averaging for the equipotential smoothing method is fairly complex and is based on the solution of the Laplace equation. Equipotential smoothing tends to minimize the local curvature of lines running across a mesh over several elements. Although this tendency can be desirable for gently curving domains, it can inhibit the ability of equipotential smoothing to reduce element distortion in highly deformed and locally curved domains. Equipotential smoothing can be performed only for nodes that are surrounded by a locally structured mesh. Nodes that are surrounded by an unstructured mesh are moved with an equivalent amount of volume smoothing when equipotential smoothing is chosen. Combining smoothing methods The default smoothing method in Abaqus/Explicit is volume smoothing. To choose an alternate smoothing method or to combine smoothing methods, you specify the weighting factor for each method. When more than one smoothing method is used, a node is relocated by computing a weighted average of the locations predicted by each chosen method. All weights must be positive, and their sum should typically be 1.0. If the sum of the chosen weights is less than 1.0, the mesh smoothing algorithm will be less aggressive at each adaptive mesh increment. If the sum of the chosen weights is greater than 1.0, their values are normalized so that their sum is 1.0. Input File Usage: *ADAPTIVE MESH CONTROLS, NAME=name volume smoothing weight, Laplacian smoothing weight, equipotential smoothing weight Abaqus/CAE Usage: For example, the following option could be used to define an equal blend of volume and equipotential smoothing, with no Laplacian smoothing: *ADAPTIVE MESH CONTROLS, NAME=name 0.5, 0.0, 0.5 Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Volumetric: volume smoothing weight, Laplacian: Laplacian smoothing weight, Equipotential: equipotential smoothing weight Geometric enhancements to the basic smoothing methods The conventional forms of the basic smoothing methods do not perform well in highly distorted domains. To ensure the robustness of adaptive meshing, Abaqus/Explicit uses geometrically enhanced forms of the basic smoothing algorithms by default. The enhanced forms are recommended for all adaptive mesh applications. However, since the basic smoothing algorithms are used by many finite element preprocessors, their conventional forms are provided as an option. Input File Usage: Use the following option to use the conventional forms of the volume, Laplacian, or equipotential smoothing algorithms: *ADAPTIVE MESH CONTROLS, NAME=name, GEOMETRIC ENHANCEMENT=NO Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, toggle off Use enhanced algorithm based on evolving element geometry Specifying a uniform mesh smoothing objective For adaptive mesh domains without any Eulerian boundary regions, the default objective of the mesh smoothing methods is to minimize mesh distortion while improving element aspect ratios, at the expense of diffusing initial mesh gradation. The uniform mesh smoothing objective is recommended for problems with moderate to large overall deformation. Input File Usage: Use the following option to specify the uniform mesh smoothing objective: *ADAPTIVE MESH CONTROLS, NAME=name, SMOOTHING OBJECTIVE=UNIFORM Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Priority: Improve aspect ratio Specifying a graded mesh smoothing objective Alternatively, the smoothing methods can attempt to preserve initial mesh gradation while reducing element distortion as the analysis evolves. This objective is the default for adaptive mesh domains with one or more Eulerian boundary regions. The graded mesh smoothing objective is recommended only for adaptive mesh domains with reasonably structured graded meshes undergoing low to moderate overall deformation. Element distortion will be minimized, but the aspect ratios of adjacent elements will be maintained approximately. Mesh gradation is particularly useful in steady-state problems where overall deformations are small and a focused mesh is used in a specific area to capture high solution gradients. Input File Usage: Use the following option to specify the graded mesh smoothing objective: *ADAPTIVE MESH CONTROLS, NAME=name, SMOOTHING OBJECTIVE=GRADED Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Priority: Preserve initial mesh grading Positioning nodes in Lagrangian domains If an adaptive mesh domain has no Eulerian boundary regions, then, by default, the mesh sweeps are based on current nodal locations, which account for material motion accumulated since the last adaptive mesh increment. This approach is generally the best for Lagrangian problems that undergo large overall deformation. Input File Usage: Use the following option to request that the current deformed positions of nodes be used as the starting locations for mesh smoothing: *ADAPTIVE MESH CONTROLS, NAME=name, MESHING PREDICTOR=CURRENT Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Meshing predictor: Current deformed position Positioning nodes in Eulerian domains Mesh sweeps can be based on the locations of nodes at the end of the previous adaptive mesh increment. This technique is recommended for problems that are Eulerian in nature, where material flow is significant compared to overall deformation. Therefore, it is the default for adaptive mesh domains with one or more Eulerian boundary regions. This approach will result in a virtually stationary mesh. Input File Usage: Use the following option to use the position of the nodes at the end of the previous adaptive mesh increment as a starting location for mesh smoothing: *ADAPTIVE MESH CONTROLS, NAME=name, MESHING PREDICTOR=PREVIOUS Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Meshing predictor: Position from previous adaptive mesh increment Solution-dependent meshing based on concave boundary curvature Mesh smoothing algorithms based only on minimizing element distortion tend to reduce the mesh refinement in areas of concave curvature, especially as the curvature evolves. Having sufficient mesh refinement near highly curved boundaries is often important to model both the shape and volume of the domain. To prevent the natural reduction in mesh refinement of areas near evolving concave curvature, Abaqus/Explicit uses solution-dependent meshing to focus mesh gradation toward these areas automatically. Although solution-dependent meshing may “pull” more elements into areas of high curvature, its primary purpose is to retain the nominal refinement in these zones. Therefore, a fine mesh should always be used when and where highly curved boundaries are expected and solution-dependent meshing should generally not be used as a direct substitute for more elements. . By default, The aggressiveness of the solution-dependent meshing is governed by the curvature refinement weight, , which correponds to an aggressivity level that has been chosen to work well on a wide variety of problems. You can change the curvature refinement weight. A value of zero indicates no solution dependence due to evolving boundary curvature, and a value greater than one increases the aggressivity from the default. Input File Usage: *ADAPTIVE MESH CONTROLS, NAME=name, CURVATURE REFINEMENT= Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Curvature refinement: Smoothing a distorted mesh at the beginning of a step When an adaptive mesh domain contains a structured mesh of uniform density, the mesh will move independently from the material only when the domain deforms. If the mesh is initially nonuniform, the meshing algorithms in Abaqus/Explicit will smooth the mesh even in the absence of deformation or material transport. When the initial mesh contains highly distorted elements, it is often useful to smooth the mesh before the step begins so that the best possible mesh is used throughout the step. When a uniform smoothing objective is used, five mesh sweeps are performed by default at the beginning of the step in which the adaptive mesh domain is defined. For a graded smoothing objective, two mesh sweeps are performed by default at the beginning of the step without acccounting for gradation. The aspect ratios used for gradation in all subsequent mesh sweeps are based on this locally smoothed mesh. Initial conditions are advected to the new mesh when initial mesh sweeps are performed. Input File Usage: Use the following option to change the number of mesh sweeps that will be performed at the beginning of the first step in which the adaptive mesh definition is active: *ADAPTIVE MESH, INITIAL MESH SWEEPS=number of initial sweeps For example, the following option would smooth a badly distorted mesh with 15 mesh sweeps at the beginning of the step, before performing adaptive meshing with three mesh sweeps every 20 increments throughout the step: *ADAPTIVE MESH, FREQUENCY=20, MESH SWEEPS=3, INITIAL MESH SWEEPS=15 Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on Use the ALE adaptive mesh domain below, Initial remeshing sweeps: Value: number of initial sweeps Meshing on boundary regions Adaptive meshing on Lagrangian and sliding boundary regions is subject to the constraint that the mesh and material must move together in the direction normal to the boundary. Nodes on the interior of such a boundary are allowed to slide freely over the material within the boundary region, which maximizes the amount of mesh smoothing that can be performed. Nodes are positioned in each mesh sweep by applying the basic smoothing methods while constraining the nodes to lie on the boundary region. In three dimensions some nodes on Lagrangian boundary regions will be on a Lagrangian edge. In each mesh sweep these nodes are positioned by applying the basic smoothing methods while constraining the node to lie along the discrete Lagrangian edge. For problems in which the flow of material from element to element along the boundary is significant compared to the deformation, oscillations in the boundary mesh can result if these constraints are applied symmetrically with respect to the upstream and downstream directions of material flow. Abaqus/Explicit uses a Petrov-Galerkin weighting of the free boundary constraint to suppress any oscillations. The algorithm is volume preserving, and the degree of upwinding is chosen automatically. Advecting solution variables to the new mesh The framework for adaptive meshing in Abaqus/Explicit is the Arbitrary Lagrangian-Eulerian method, which introduces advective terms into the momentum balance and mass conservation equations to account for independent mesh and material motion. There are two basic ways to solve these modified equations: solve the nonsymmetric system of equations directly, or decouple the Lagrangian (material) motion from the additional mesh motion using an operator split. The operator split method is used in Abaqus/Explicit because of its computational efficiency. Furthermore, this technique is appropriate in an explicit setting because small time increments limit the amount of motion within a single increment. In an adaptive meshing increment the element formulations, boundary conditions, external loads, contact conditions, etc. are handled first in a manner consistent with a pure Lagrangian analysis. Once the Lagrangian motion is updated and mesh sweeps have been performed to find the new mesh, the solution variables are remapped by performing an advection sweep. The advection sweep accounts for the advective terms in the momentum balance and continuity equations. Advection methods for element variables Element and material state variables must be transferred from the old mesh to the new mesh in each advection sweep. The number of variables to be advected depends on the material model and element formulation; however, stress, history variables, density, and internal energy are always solution variables. Two methods are available for the advection of element variables: the default second-order method based on the work of Van Leer (Van Leer, 1977) and a first-order method based on donor cell differencing. Both advection methods incorporate the concept of upwinding. They also conserve the element variables in an integral sense when mapping from the old mesh to the new mesh (that is, the value of any solution variable integrated over the domain is unchanged by adaptive meshing). Using a conservative algorithm to advect the element density and the internal energy automatically ensures conservation of mass and energy for an adaptive mesh domain without Eulerian boundary regions. Both advection methods are also monotonic and consistent. A method is monotonic if an element quantity with a monotonic, increasing spatial distribution over a portion of the old mesh remains as such in the new mesh. A method is consistent if, when solution variables are advected to a new mesh that is identical to the old mesh, all element quantities remain unchanged. Second-order advection Second-order advection is used by default for all adaptive mesh domains. It is recommended for all problems, ranging from quasi-static to transient dynamic shock. An element variable, , is remapped from the old mesh to the new mesh by first determining a linear distribution of the variable in each old element, as illustrated in Figure 12.2.3–2 for a simple one-dimensional mesh. The linear distribution of in the two adjacent elements. To construct the linear in the middle element depends on the values of distribution: constant quadratic trial limited element 1 element 2 element 3 Figure 12.2.3–2 Second-order advection. 1. A quadratic interpolation is constructed from the constant values of at the integration points of the middle element and in its adjacent elements. 2. A trial linear distribution, , is found by differentiating the quadratic function to find the slope at the integration point of the middle element. 3. The trial linear distribution in the middle element is limited by reducing its slope until its minimum and maximum values are within the range of the original constant values in the adjacent elements. This process is referred to as flux-limiting and is essential to ensure that the advection is monotonic. Once the flux-limited linear distributions are determined for all elements in the old mesh, these distributions are integrated over each new element. The new value of the variable is found by dividing the value of each integral by the new element volume. Input File Usage: Use the following option to specify that the second-order advection method should be used to remap element variables: *ADAPTIVE MESH CONTROLS, NAME=name, ADVECTION=SECOND ORDER old mesh new mesh φnew = φold φnew φold value on old mesh value on new mesh φnew = φold φold la 1 la lb + lb+ la lb Figure 12.2.3–3 First-order advection. Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, toggle on Second order First-order advection First-order advection is simple and computationally efficient; however, it tends to diffuse sharp gradients over time, especially in transient dynamic analyses or other problems that require fairly frequent adaptive meshing. Therefore, this technique should be used only as a computationally efficient alternative for quasi-static simulations that do not require frequent adaptive meshing. Figure 12.2.3–3 illustrates the first-order method for a portion of a one-dimensional mesh. An element variable, , is remapped from the old mesh to the new mesh by first assuming a constant value of the variable for each old element. These values are then integrated over each new element. The new value of the variable is found by dividing the value of each integral by the new element volume. Input File Usage: Use the following option to specify that the first-order advection method should be used to remap element variables: *ADAPTIVE MESH CONTROLS, NAME=name, ADVECTION=FIRST ORDER Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, toggle on First order Momentum advection Nodal velocities are computed on a new mesh by first advecting momentum, then using the mass distribution on the new mesh to calculate the velocity field. Advecting momentum directly ensures that momentum is conserved properly in the adaptive mesh domain during remapping. Two methods are available for advecting momentum: the default element center projection method and the half-index shift method (Benson, 1992). Both methods are applicable for all adaptive mesh applications. Element center projection method The element center projection method is the default method used to advect momentum and requires the fewest numerical operations. The element momentum is calculated first for the old mesh based on the mass and velocity of the element nodes. The element momentum is then advected from the old mesh to the new mesh by the same first- or second-order algorithms used for advecting element variables. Finally, the element momentum on the new mesh is assembled at the nodes using a projection. The element center projection method requires the advection of only two or three extra variables in two dimensions or three dimensions, respectively. Input File Usage: Use the following option to request momentum advection method: the most computationally efficient *ADAPTIVE MESH CONTROLS, NAME=name, MOMENTUM ADVECTION=ELEMENT CENTER PROJECTION Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Momentum advection: Element center projection Half-index shift method The half-index shift method is computationally more intensive than the element center projection method, but it may result in less wave dispersion for some problems. This method first shifts each of the nodal momentum variables from the nodes surrounding an element to the element center. The shifted momentum variables are then advected from the old mesh to the new mesh by the same first- or second-order algorithms used for advecting element variables, providing momentum variables at the center of the new elements. Finally, the momentum variables at the element centers in the new mesh are shifted back to the nodes. The half-index shift method requires the advection of 8 or 24 extra variables in two or three dimensions, respectively, which can increase the cost of each advection sweep significantly. Input File Usage: Use the following option to specify that the half-index shift method should be used for momentum advection: *ADAPTIVE MESH CONTROLS, NAME=name, MOMENTUM ADVECTION=HALF INDEX SHIFT Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Momentum advection: Half-index shift Additional references • Benson, D. J., “Momentum Advection on a Staggered Mesh,” Journal of Computational Physics, vol. 100, pp. 143–162, 1992. • Van Leer, B., “Towards the Ultimate Conservative Difference Scheme III. Upstream-centered Finite-Difference Schemes for Ideal Compressible Flow,” Journal of Computational Physics, vol. 23, pp. 263–275, 1977. • Van Leer, B., “Towards the Ultimate Conservative Difference Scheme IV. A New Approach to Numerical Convection,” Journal of Computational Physics, vol. 23, pp. 276–299, 1977. 12.2.4 MODELING TECHNIQUES FOR EULERIAN ADAPTIVE MESH DOMAINS IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “ALE adaptive meshing: overview,” Section 12.2.1 • “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2 • *ADAPTIVE MESH CONSTRAINT • “Understanding ALE adaptive meshing,” Section 14.6 of the Abaqus/CAE User’s Manual Overview An Eulerian adaptive mesh domain: • is used to model material flowing through the mesh; and • typically has two Eulerian boundary regions, one inflow and one outflow, connected by Lagrangian and/or sliding boundary regions. The correct combination of mesh constraints and material boundary conditions applied to an Eulerian boundary region depends on whether the region acts as an inflow or an outflow boundary. The region types and mesh constraints assigned to the boundary regions that are connected to the Eulerian boundary regions must be chosen to simulate the correct physical behavior as well. The adaptive meshing technique in Abaqus/Explicit is robust if the mesh is underconstrained: the modeling techniques presented in this section are intended to provide guidance in properly defining Eulerian models. ALE adaptive mesh constraints on Eulerian boundaries ALE adaptive mesh constraints should be applied normal to an Eulerian boundary region; otherwise, the motion of the mesh on the boundary is ambiguous. If no mesh constraints are applied normal to the boundary, Abaqus/Explicit will treat the region as if it were sliding, and the mesh will follow the material normal to the boundary. Although there are no restrictions on specifying adaptive mesh constraints at nodes on an Eulerian boundary region, the following guidelines should be followed in most cases: • Mesh constraints should be applied to every node on the Eulerian boundary region, including the corners and edges. • Mesh constraints should be applied either only normal to the Eulerian boundary region or in every direction. Mesh constraints should not be specified in only the direction tangential to an Eulerian boundary region; such constraints are ambiguous and may result in undesirable motion of the mesh at the boundary. Loads and boundary conditions on Eulerian boundaries act on the material that instantaneously coincides with the mesh at the surface. When used in combination with spatial adaptive mesh constraints, physically meaningful Eulerian flow conditions can be defined. Defining inflow Eulerian boundaries The material flowing into an adaptive mesh domain through an Eulerian boundary will have the same stress and material state as the material in the elements immediately adjacent to the boundary. Therefore, it is important to maintain the stress and material state in those elements at the desired values (which in many cases will be zero, to simulate stress-free material entering the Eulerian domain). To accomplish this goal: • position the inflow boundary far enough upstream from high solution gradients to ensure that the response at the inflow boundary is smooth, and • apply sufficient mesh and material constraints at the boundary (as described later in this section). To be physically meaningful, the size and shape of the inflow boundary region must be maintained. For example, applying sufficient constraints is crucial for steady-state process simulations where the cross-section of the workpiece entering the adaptive mesh domain is known and affects the response downstream. The types of constraints appropriate for an inflow boundary depend on whether the precise location of the inflow boundary region is known or whether it is part of the solution. Known inflow boundary location In many problems the area, shape, and position of the inflow boundary are known a priori. For example, in the steady-state analysis of a forward extrusion process, an inflow Eulerian boundary can be used to model the flow of material into the adaptive mesh domain. The size of the inflow boundary is based on the known billet cross-section, and the location of the inflow boundary is fixed because of the confined conditions on the material. When the area, shape, and location of the inflow boundary are known, both material and mesh constraints should be applied. Figure 12.2.4–1 shows a typical model setup for a two-dimensional forward extrusion problem where either a prescribed mass flow rate or a prescribed uniform pressure is applied to a known inflow boundary. Apply boundary conditions at all nodes on the inflow boundary region to prescribe material constraints in the directions tangential to the boundary surface. Preventing motion of the material tangential to the inflow boundary helps to maintain the stress and material state of the elements adjacent to the Eulerian boundary. Apply adaptive mesh constraints in the normal direction at all nodes on the inflow boundary. In addition, apply mesh constraints in all tangential directions at the edges and corners surrounding the Eulerian boundary region. These constraints fix the location and size of the cross-sectional area at the inflow boundary. If a nonuniform boundary condition or load is applied to the material at the inflow boundary or if the initial material state in the elements adjacent to the boundary is nonuniform in the tangential direction, apply tangential mesh constraints to the nodes strictly in the interior of the Eulerian boundary region. node set TOP contact surface node set INFLOW element set INFLOW flow node set BOTTOM symmetry , zero-displacement adaptive mesh constraints applied to node set INFLOW in direction 1 and to node sets TOP and BOTTOM in direction 2 Eulerian boundary region defined by a zero-displacement boundary condition applied to node set INFLOW in direction 2 Prescribed inflow velocity: or Prescribed inflow pressure: Eulerian boundary region defined by a Eulerian boundary region defined by a velocity-type boundary condition applied to node set INFLOW in direction 1 pressure load applied to element set INFLOW in direction 1 Figure 12.2.4–1 Known inflow boundary. Although the application of mesh and material constraints tangential to and along the edges and corners of an inflow Eulerian boundary may appear to be redundant, they are actually independent. For example, consider a long billet with a variable cross-section, as shown in Figure 12.2.4–2. v0 symmetry outflow boundary; node set OUTFLOW; element set OUTFLOW inflow boundary; node set INFLOW Eulerian boundary region created by a surface defined on the S3 faces of element set OUTFLOW zero-displacement adaptive mesh constraints applied to node sets INFLOW and OUTFLOW in direction 1 velocity-type adaptive mesh constraint with amplitude INCOMING applied to node N in direction 2 Eulerian boundary region defined by a zero-displacement boundary condition applied to node set INFLOW in direction 2 Eulerian boundary region defined by a velocity-type boundary condition with a variable amplitude applied to node set INFLOW in direction 1 Figure 12.2.4–2 Modeling a billet with a variable cross-section. The adaptive mesh domain, with its inflow and outflow Eulerian boundary regions, is assumed to represent a portion of the billet along its length. The entire billet moves with a rigid body velocity along its length (x-direction) so that material flows into one Eulerian boundary and out the other. Boundary conditions are applied to the material at the inflow boundary to maintain this velocity. Mesh constraints are applied normal to the inflow and outflow boundary regions. The mesh constraint applied in the y-direction at node N is used to prescribe the known variable incoming cross-section of the material. The motion of this node does not affect the velocity field of the material entering the domain. Unknown inflow boundary location Sometimes, the location of the inflow boundary region is known only approximately; its precise location will be determined from the solution. For these problems, apply adaptive mesh constraints In the absence of tangential mesh only in the direction normal to the Eulerian boundary region. constraints at the edges and corners of the Eulerian boundary region, Abaqus/Explicit will move these edges and corners with the material in the tangential direction but with the mesh constraints in the normal direction. Therefore, material constraints should be applied using multi-point constraints or linear constraint equations to preserve the cross-sectional area of the inflow boundary. For example, consider a steady-state rolling simulation with multiple rollers in an asymmetric configuration, as shown in Figure 12.2.4–3. billet is free to move node set INFLOW free surface flow of material free surface zero-displacement adaptive mesh constraints applied to node 1 and node set INFLOW in direction 1 PIN-type multi-point constraints applied to node set INFLOW and node 1 Figure 12.2.4–3 Unknown inflow boundary location. It may be impractical to extend the analysis domain as far as the guides on the upstream side, but spatially fixing the inflow boundary at an arbitrary position in the y- and z-directions may cause unrealistic stress on the workpiece as it finds an equilibrium position between the rollers. Mesh constraints are applied normal to the Eulerian boundary region to fix the position of the inflow boundary relative to the rollers in the x-direction. Material constraints (applied with a PIN MPC) are used to ensure that material enters the domain at a uniform velocity and that the cross-section does not rotate. The material constraints will maintain the cross-sectional shape of the section while allowing it to move laterally to the correct equilibrium position. Since tangential mesh constraints are not used, the mesh will follow the material in the directions tangential to the Eulerian boundary region. Defining outflow Eulerian boundaries Typically, adaptive mesh constraints should be applied only in the direction normal to the surface on an Eulerian boundary region that acts as an outflow boundary. No tangential mesh constraints should be applied to the edges or corners of an outflow boundary adjacent to a Lagrangian (or sliding) boundary region acting as a free surface. In contrast to inflow boundaries, the cross-section of an outflow boundary adjacent to a free surface is determined by the solution in the domain. At the edge or corner where an Eulerian boundary region meets a Lagrangian or sliding boundary region, Abaqus/Explicit will satisfy the applied mesh constraint normal to the Eulerian boundary region and the inherent mesh constraint normal to the Lagrangian or sliding boundary region simultaneously, thus correctly handling the evolution of the free surface adjacent to the outflow boundary. Figure 12.2.4–4 shows the evolution of an outflow boundary from to , where material continues to flow through the outflow boundary. free surface v0 symmetry position of free surface at time t0 position of free surface at time t1 Eulerian boundary region created by a surface defined on the S2 faces of element set OUTFLOW zero-displacement adaptive mesh constraint applied to node set OUTFLOW in direction 1 motion of node N to satisfy constraint Figure 12.2.4–4 Abaqus/Explicit will respect the free surface at an Eulerian outflow boundary. The mesh constraint normal to the Eulerian outflow boundary is applied by moving node N along the free surface of the material, so that the outflow boundary “expands” with the material arriving from upstream. Although not shown in the figure, mesh smoothing causes all other nodes on the outflow boundary, with the exception of the node on the symmetry plane, to move up toward node N as the boundary expands. No special material boundary conditions are required at outflow Eulerian boundaries. Boundary conditions tangential to the outflow boundary are recommended only if they are the same as those defined upstream (e.g., a symmetry plane running along the length of an Eulerian domain). However, to improve convergence to the steady-state solution in steady-state process simulations, it is often useful to constrain the material velocity to be uniform normal to the outflow boundary using multi-point constraints or linear constraint equations. Defining Eulerian boundary regions that act as both inflow and outflow boundaries Although it is rarely appropriate, an Eulerian boundary region can act as both an inflow and an outflow boundary at different times during the same analysis step. Adaptive mesh constraints and material boundary conditions at such a boundary should be chosen to be physically meaningful for both inflow and outflow situations. For each node on the edges and corners of an Eulerian boundary region that does not have mesh constraints tangential to the boundary surface, Abaqus/Explicit will determine in each adaptive mesh increment whether the boundary at the node is acting as an inflow or an outflow boundary. If an inflow condition is detected, the node will move with the material in the tangential direction but with the mesh constraints in the normal direction. If an outflow condition is detected, the movement of the node will both follow the adjacent Lagrangian boundary region and satisfy the mesh constraint normal to the Eulerian boundary region. Lagrangian versus sliding boundary regions on Eulerian domains Many applications using Eulerian adaptive mesh domains, including the simulation of steady-state processes, have a primary direction of material flow and use a control volume approach to model the process zone. These problems usually include two Eulerian boundary regions, representing an inflow boundary and outflow boundary. The remaining surfaces between the Eulerian boundaries can be either Lagrangian or sliding boundary regions. Determining which type of boundary region to use between the two Eulerian boundary regions depends on the type of load or boundary condition that is required: • Use a sliding boundary region to define boundary conditions or loads that act at a spatial location on a portion of the surface along the length of the control volume. Apply adaptive mesh constraints to fix the mesh spatially in the flow direction (and possibly in the direction transverse to the flow). For example, a distributed pressure can be applied around the circumference of the control volume, as shown in Figure 12.2.4–5. The distributed pressure load is defined using a sliding boundary region. Mesh constraints are applied to fix the boundary region spatially in the flow direction. Similarly, a concentrated load could be applied to a specific spatial location to model the effect of a very sharp body pressing into the workpiece at a known location with a known force. • Use a sliding boundary region to define boundary conditions or loads that act along the entire length of the Eulerian control volume between the inflow and outflow boundaries and act in a spatial manner transversely to the flow. If the load acts on only a portion of the surface in the transverse direction, it may be necessary to apply mesh constraints in the direction transverse to the flow. For example, a boundary condition that acts as a knife edge along the length of the domain is shown in Figure 12.2.4–6. Mesh constraints are applied in the transverse direction (and, if the line of application is curved, along the line) to keep the boundary condition fixed spatially. • Use a Lagrangian boundary region (default) to define boundary conditions or loads that act along the entire length of the surface of the Eulerian control volume between the inflow and sliding edge Lagrangian edge geometric edge node set BACK node set BOTTOM flo element set LOAD zero-displacement adaptive mesh constraint applied to node set LOADEDGE in direction 3 sliding boundary region defined by a pressure load applied to element set LOAD in direction 1 Lagrangian boundary region defined by symmetry boundary conditions applied to node set BACK about the x-direction and node set BOTTOM about the y-direction Figure 12.2.4–5 Applying a spatial pressure load to a portion of the surface along the length of an Eulerian control volume. sliding edge sliding boundary region defined by a boundary condition adaptive mesh constraint flow Figure 12.2.4–6 Applying a boundary condition along the entire length of the Eulerian control volume. outflow boundary and act in a Lagrangian manner transversely to the flow. In three dimensions, symmetry conditions should typically act in a Lagrangian manner transverse to the flow direction. In many cases geometric edges will prevent material from flowing off the symmetry plane and onto the free surface. However, since geometric edges can be deactivated as surfaces flatten, Lagrangian boundary regions should be used to define the symmetry planes for these types of problems. In Figure 12.2.4–5 quarter-symmetry is assumed, and the symmetry planes are defined using Lagrangian boundary regions. The resulting Lagrangian edges that run from one Eulerian boundary to the other separate the symmetry planes from the free surface. • Boundary conditions or loads that act on only a specific portion of the material between the inflow and outflow boundaries cannot usually be modeled for problems utilizing Eulerian control volumes. Since the mesh underneath the load or boundary condition must follow the material, it will eventually be restricted by the Eulerian boundary. This treatment of loads and boundary conditions is not usually consistent with a steady-state model and should not arise in practical simulations using Eulerian adaptive mesh domains. 12.2.5 OUTPUT AND DIAGNOSTICS FOR ALE ADAPTIVE MESHING IN Abaqus/Explicit Products: Abaqus/Explicit Abaqus/CAE References • “Output to the output database,” Section 4.1.3 • “ALE adaptive meshing: overview,” Section 12.2.1 • “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2 • *ADAPTIVE MESH • *ADAPTIVE MESH CONTROLS • *DIAGNOSTICS • *TRACER PARTICLE • Chapter 78, “Using display groups to display subsets of your model,” of the Abaqus/CAE User’s Manual Overview Output for ALE adaptive meshing: • can be used to verify the automatic splitting of user-defined domains, the formation of Lagrangian the formation of geometric edges and corners, and the determination of edges and corners, nonadaptive nodes; • must be interpreted carefully, since the values of output variables at specific locations in the mesh are no longer linked to values at particular material points; • can include the definition of tracer particles, which follow material points and allow you to examine the trajectory of those points and plot material time histories of all element and nodal variables at those points; and • can include diagnostic information on the efficiency of adaptive meshing and the accuracy of advection. Verifying the model Output that can be used to verify adaptive meshing models is available in the data (.dat) file and in the output database (.odb) . Element sets When user-defined adaptive mesh domains are split by Abaqus/Explicit, the elements that compose the new subdivided domains are printed to the data (.dat) file. New element sets are created and written to the output database (.odb) for all adaptive mesh domains. The name of the element set created for each domain is the user-defined name, plus the number of the subdivision (1 if no subdivisions were created), plus the step number. For example, if the user-defined adaptive mesh domain specified for the element set domain_name spanned three disjoint parts, Abaqus/Explicit would subdivide the user-defined domain into three domains and create three element sets in the output database (.odb) for the first step: domain_name-1-1, domain_name-2-1, and domain_name-3-1. Abaqus/CAE can be used to verify the creation of the subdivided domains. Edges and nonadaptive nodes Abaqus/Explicit automatically forms Lagrangian edges and corners and identifies nonadaptive nodes based on the topology of the adaptive mesh domains, connections to nonadaptive domains, and user-specified boundary regions. Furthermore, geometric edges and corners are formed automatically based on the initial geometry and the value of the initial feature angle. See “Defining ALE adaptive mesh domains in Abaqus/Explicit,” Section 12.2.2. Lagrangian edges, geometric edges and corners, and nonadaptive nodes (including Lagrangian corners) are output to the data (.dat) file for each adaptive mesh domain. This information can be obtained by requesting a history definition summary printout to the data file or by monitoring the progress of the adaptive meshing . In addition, up to three node sets are created in the output database (.odb) for each adaptive mesh domain in each step. The names of the node sets are created by concatenating the following information: • the domain element set name; • the number of the subdivision (1 if no subdivisions were created); • the letters LE for Lagrangian edge, GE for geometric edge or corner, or NA for nonadaptive nodes (including Lagrangian corners); and • the step number. For example, if a user-defined three-dimensional adaptive mesh domain specified for element set domain_name is subdivided automatically into two adaptive mesh domains, Abaqus/Explicit will generate up to six node sets in the output database for the first step: domain_name-1-LE-1, domain_name-1-GE-1, domain_name-1-NA-1, domain_name-2-LE-1, domain_name-2-GE-1, and domain_name-2-NA-1. Since boundary regions are separated by corners, not edges, in two dimensions, node sets will not be created for Lagrangian edges in two-dimensional adaptive mesh domains. The Lagrangian corners are included in the nonadaptive (NA) node set, as for three-dimensional domains. Abaqus/CAE can be used to verify the creation of Lagrangian edges and corners, geometric edges and corners, and nonadaptive nodes. Interpreting results When adaptive meshing is not performed, the finite element mesh follows the material, which enables a straightforward interpretation of analysis results. You can visualize deformation and material motion by studying the motion of the mesh. Each nodal and element output variable corresponds to a specific material location, because the mesh is fixed to the same material point throughout time. Once adaptive meshing takes place, the locations of mesh and material points deviate, and analysis results must be interpreted accordingly. The motion of the mesh on the interior of an adaptive mesh domain represents the composite effects of the material motion and adaptive meshing. The motion of the mesh and the motion of the material on Lagrangian and sliding boundary regions is identical in the direction normal to the boundary but not in the direction tangential to it. Nodal variables When adaptive meshing is performed, a material point that is coincident with a node at the beginning of the step may not remain coincident with that node throughout the step. Values of displacement and current coordinates represent the motion of the node, not necessarily the motion of the material. All other nodal variables—including velocity, acceleration, and reaction forces—represent the value of the variable for the material particle at the current location of the node. Contour or vector plots of these variables will show their correct spatial distribution and are, therefore, meaningful. However, time histories of nodal variables for nodes that undergo adaptive meshing are generally not meaningful. In steady-state problems, though, a velocity or acceleration time history based at a fixed spatial location rather than at a specific material point may be useful. Element variables Similarly, when adaptive meshing is performed, a material particle that is coincident with an element integration point at the beginning of a step may not remain so throughout the step. Therefore, element integration point variables do not necessarily represent values at the same material point throughout the step. Contour or vector plots of element integration point variables are meaningful for the same reasons described for nodal variables. However, time histories are based at the spatial location of the element integration point and not at a specific material point. Whole element variables have a similar interpretation. Tracking nodal or element variables at material points Tracer particles can be defined to track material points in an adaptive mesh domain. These particles can also be used to obtain time histories of nodal or element integration point variables that correspond to the time variation of the variable at a specific material point. Tracer particles are defined as described below . Node and element variable output can be requested for tracer particle sets to examine the trajectory of material particles or to obtain material time histories. Output for tracer particles can be written only to the output database (.odb). Using tracer particles in Lagrangian domains In most adaptive meshing simulations using Lagrangian domains, the nodes and elements in the domain correspond neither to a specific spatial location nor to a specific material point or volume. Thus, time histories of variables at nodes and at element integration points are often physically meaningless in a Lagrangian adaptive mesh domain. Tracer particles should be defined to view time history information. Tracer particles can also be used to visualize the motion of the material. The initial location of a tracer particle is defined to be coincident with a node, termed the parent node. Tracer particles are defined in sets by defining multiple parent nodes or node sets. You indicate the nodes whose current locations correspond to the initial location of the tracer particles and assign a name to the tracer particle set to identify it for use in output requests. Tracer particles are released from their parent nodes repeatedly at specified intervals during the step in which they are defined. The particles follow material points for the remainder of that step and in all subsequent steps. Tracer particles are typically defined only on adaptive mesh domains, although they can be defined on nodes connected to any low-order solid element in the model. For analyses in which adaptive meshing is not performed until later steps, tracer particles can be defined on nonadaptive domains at the beginning of an analysis and will be tracked continuously as the domain becomes adaptive. Similarly, tracer particles will be tracked from domain to domain if adaptive mesh domain topologies change from step to step. Input File Usage: Use the following option to define a tracer particle set: *TRACER PARTICLE, TRACER SET=tracer_set_name list of tracer particle parent nodes Abaqus/CAE Usage: Tracer particles are not supported in Abaqus/CAE. Using tracer particles in Eulerian domains Time histories at nodes and element integration points in an Eulerian domain may have physical meaning at points where spatial adaptive mesh constraints are applied. For example, the time variation of equivalent plastic strain in elements along an outflow Eulerian boundary acts as a spatial time history of that variable and can be used to evaluate whether the process has reached a steady-state solution. Tracer particles can be defined to evaluate the material time history of variables at a material point as it flows through the Eulerian domain. Tracer particles can also be used to evaluate the trajectory and path of material points as they pass through the domain. Tracer particles can be assigned to any parent node in an Eulerian adaptive mesh domain. If a tracer particle reaches an outflow boundary and material continues to flow out, the tracer particle will no longer be tracked and all output history variables associated with the tracer particle will be zero after deactivation. When material flow through the mesh domain is significant, sets of tracer particles can be released from the current locations of the parent nodes at multiple times during the step. Each release of tracer particles is referred to as particle birth. After particle birth the tracer particles follow the motion of the material regardless of the motion of the mesh. You can indicate the number of particle birth stages in a step. These stages will be evenly spaced throughout the time period of the step. For example, a tracer particle set can be defined such that all nodes along an inflow Eulerian boundary are parent nodes. Multiple birth stages can be specified so that a set of tracer particles is released from the mesh at the inflow boundary periodically during the step. If enough birth stages are defined, the domain will eventually be spanned with tracer particles as material flows from the inflow boundary to the outflow boundary. Input File Usage: Use the following option to define a tracer particle set with multiple birth stages: *TRACER PARTICLE, TRACER SET=tracer_set_name, PARTICLE BIRTH STAGES=n list of tracer particle parent nodes Abaqus/CAE Usage: Tracer particles are not supported in Abaqus/CAE. Monitoring the progress of ALE adaptive meshing Diagnostic information can be written to the message (.msg) file to track the efficiency and accuracy of adaptive meshing. You can select the level of diagnostic output that is written. Obtaining a summary at the end of a step By default, a summary of adaptive meshing information for each adaptive mesh domain will be written to the message (.msg) file at the end of each step. This summary information includes: • the average percentage of nodes moved, • the maximum percentage of nodes moved, • the minimum percentage of nodes moved, and • the average number of advection sweeps. Each value is calculated for a single adaptive mesh domain over all adaptive mesh increments. The cost of advection is approximately proportional to the percentage of nodes moved, since variables are not advected for elements that have not been relocated during adaptive meshing. Input File Usage: Abaqus/CAE Usage: Use the following option to request a summary for each adaptive mesh domain at the end of each step: *DIAGNOSTICS, ADAPTIVE MESH=STEP SUMMARY Adaptive mesh diagnostics are not supported in Abaqus/CAE. Obtaining a summary for every ALE adaptive mesh increment In addition to the step summary information, the following diagnostics can be obtained for each adaptive mesh domain at every adaptive mesh increment: • the percentage of nodes moved, and • the number of advection sweeps. Input File Usage: Abaqus/CAE Usage: Use the following option to obtain summary information at the end of the step and at every adaptive mesh increment: *DIAGNOSTICS, ADAPTIVE MESH=SUMMARY Adaptive mesh diagnostics are not supported in Abaqus/CAE. Obtaining details of advection accuracy for every ALE adaptive mesh increment The following detailed diagnostic information can also be written to the message (.msg) file to track the accuracy of the advection: • mass and momentum before and after advection, and • percentage volume change. Input File Usage: Use the following option to request the most detailed diagnostics, which include advection accuracy measures and summary information for each adaptive mesh domain, reported at every adaptive mesh increment: Abaqus/CAE Usage: *DIAGNOSTICS, ADAPTIVE MESH=DETAIL Adaptive mesh diagnostics are not supported in Abaqus/CAE. Suppressing ALE adaptive mesh diagnostics You can suppress output of all adaptive mesh diagnostic information. Input File Usage: Abaqus/CAE Usage: *DIAGNOSTICS, ADAPTIVE MESH=OFF Adaptive mesh diagnostics are not supported in Abaqus/CAE. 12.2.6 DEFINING ALE ADAPTIVE MESH DOMAINS IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “ALE adaptive meshing: overview,” Section 12.2.1 • “ALE adaptive meshing and remapping in Abaqus/Standard,” Section 12.2.7 • *ADAPTIVE MESH • *ADAPTIVE MESH CONSTRAINT • *ADAPTIVE MESH CONTROLS • “Customizing ALE adaptive meshing,” Section 14.14 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview ALE adaptive meshing in Abaqus/Standard: • maintains a topologically similar mesh; • can be used to solve Lagrangian problems (in which no material leaves the mesh) and to model effects of ablation, or wear (in which material is eroded at the boundary); • can be used in static stress/displacement analysis, steady-state transport analysis, coupled pore fluid flow and stress analysis, and coupled temperature-displacement analysis; • can be used only in geometrically nonlinear general analysis steps; and • is available only for acoustic elements and a subset of the solid elements. Defining an ALE adaptive mesh domain You can apply ALE adaptive mesh smoothing to an entire model or to individual parts of the model as a step-dependent feature. Adaptive meshing for solid elements in Abaqus/Standard uses a subset of the adaptive meshing functionality available in Abaqus/Explicit. You must specify the portion of the original mesh that will be subject to adaptive meshing. Input File Usage: Abaqus/CAE Usage: *ADAPTIVE MESH, ELSET=name Multiple adaptive mesh domains can be defined in a step by reusing the *ADAPTIVE MESH option, but each element set must refer to a unique set of elements. Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on Use the ALE adaptive mesh domain below, and click Edit to select the region Only one adaptive mesh domain can be defined in Abaqus/CAE for any particular step. Modifying an ALE adaptive mesh domain By default, all adaptive mesh domains defined in the previous analysis step remain unchanged in the subsequent step. You define the adaptive mesh domains in effect for a given step relative to the preexisting adaptive mesh domains. At each new step the existing adaptive mesh domains can be modified and additional adaptive mesh domains can be specified (except in Abaqus/CAE, where only one adaptive mesh domain can be in effect for a given step). Input File Usage: Abaqus/CAE Usage: Use either of the following options to modify an existing adaptive mesh domain or to specify an additional adaptive mesh domain: *ADAPTIVE MESH, ELSET=name *ADAPTIVE MESH, ELSET=name, OP=MOD Step module: Other→ALE Adaptive Mesh Domain→Edit Removing an ALE adaptive mesh domain If you choose to remove any adaptive mesh domain in a step, no adaptive mesh domains will be propagated from the previous step. Therefore, all adaptive mesh domains that are in effect during this step must be respecified. Input File Usage: Abaqus/CAE Usage: Use the following option to remove all previously defined adaptive mesh domains and to specify new adaptive mesh domains: *ADAPTIVE MESH, ELSET=name, OP=NEW If the OP=NEW parameter is used on any *ADAPTIVE MESH option within a step, it must be used on all *ADAPTIVE MESH options in the step. Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on No ALE adaptive mesh domain for this step Splitting ALE adaptive mesh domains Abaqus/Standard may subdivide each adaptive mesh domain that you specify such that • all elements in an adaptive domain refer to one element property definition; and • all elements in an adaptive domain are of similar type (such as hybrid elements with linear pressure). If Abaqus/Standard subdivides the adaptive mesh domains that you specified, each of the adaptive mesh domain subdivisions will have a new name, which will be used for output and diagnostic purposes. The new names will be formed by concatenating the name of the user-specified element set, a number identifying the subdivision, and the step number. Each of the subdivisions will be further examined to ensure that all the elements in a subdivision are subjected to the same body forces. You may be asked to modify the definition of the adaptive mesh domain to satisfy this requirement. ALE adaptive mesh regions Each adaptive mesh domain has an interior region and a boundary region. The boundary region may include distinct kinks that take the form of geometric edges or corners. The nodes on the boundary region are, therefore, further separated into free surface nodes, edge nodes, and constrained nodes. Different updating rules are applied to nodes in these different regions. These regions are created automatically by Abaqus/Standard. You can control the detection of the geometric features. In addition, mesh constraints can be applied to any node in the adaptive mesh domain. Since acoustic elements do not have displacement degrees of freedom, their treatment for adaptive meshing includes some additional considerations. The acoustic adaptive domain must be connected to the structural domain using a surface-based tie constraint with the slave surface defined on the acoustic domain. Thus, an acoustic adaptive domain has an additional boundary region that is connected to the structural domain. These slave surface nodes are updated based on the displaced configuration of the master surface nodes on the structural domain, without permitting relative sliding between the surfaces. The displacements of the master surface defined on the structural domain, together with nonzero adaptive mesh constraints, serve as the forcing function that drives adaptive mesh smoothing of an acoustic adaptive domain. The mesh smoothing algorithm will produce no changes in the acoustic adaptive domain if these displacements are zero. Options for controlling the mesh smoothing algorithm are described in “ALE adaptive meshing and remapping in Abaqus/Standard,” Section 12.2.7. ALE adaptive mesh interior regions Nodes in the interior region are defined as nodes that are surrounded entirely by elements in the adaptive mesh domain. By default, the new position of an interior node is computed from the positions of the adjacent nodes that are connected through element edges to the node in question. These nodes can move in any direction. To control the displacement of these nodes, you can apply an adaptive mesh constraint in any direction. ALE adaptive mesh boundary regions The boundary region is that part of the surface of the adaptive mesh domain that is not constrained to other elements in the mesh. The nodes on the boundary region are further separated into surface nodes, edge nodes, corner nodes, and constrained nodes. Surface, edge, and corner nodes Surface nodes are defined as nodes at which the surrounding surface facets have the same normal vector within a user-defined angle. These nodes are constrained against movement in the normal direction, but sliding in any tangential direction is permitted. The new position of a surface node is computed from the positions of the adjacent nodes that are connected through the edges of the surface facets to the node in question. Edge nodes are nodes in a three-dimensional model at which the surrounding surface facets have two different normals and where the vectors along two of the surface edges are colinear. Nodes on an edge can slide only along the edge. The new position of an edge node is computed from the positions of the two adjacent nodes along the edge. Corner nodes are nodes at which all the surrounding surface facet normals are different. These nodes are constrained against all mesh smoothing movement. You can control the displacement of these node types on the boundary region by applying an adaptive mesh constraint in any direction. Constrained nodes in an acoustic adaptive domain A surface-based tie constraint can be used to connect two acoustic surfaces together. When both the master and slave nodes of the tie constraint belong to the same adaptive mesh domain, the master surface nodes are updated according to the rules for surface, edge, and corner nodes. An adaptive mesh constraint can be applied at master surface nodes. Slave nodes are updated by applying a tie constraint. Adaptive mesh constraints cannot be applied at slave surface nodes. Mesh smoothing is not applied to these nodes when the master and slave nodes belong to different acoustic adaptive mesh domains. Constrained nodes in a solid adaptive domain Mesh smoothing is not applied to nodes that are involved in multi-point constraints , equations , or kinematic coupling constraints ( “Coupling constraints,” Section 34.3.2). Geometric features The classification of boundary region nodes as surface, edge, and corner nodes is performed based on the identification of geometric features in the mesh’s configuration at the start of a step where adaptive mesh domains are defined and is updated as the analysis proceeds and the configuration changes. You can define the criteria that Abaqus/Standard uses in classifying geometric features through adaptive mesh controls. Controlling the detection of geometric edges and corners Geometric features are identified initially as edges on boundary regions where the angle between the normals on adjacent element faces is greater than the initial geometric feature angle, ( ), as shown in Figure 12.2.6–1. The default value for the initial geometric feature angle is . Setting will ensure that no geometric edges or corners are formed on the boundary of the adaptive mesh domain. You can define adaptive mesh controls to change the value of the angle that will be used to recognize geometric features. Input File Usage: *ADAPTIVE MESH CONTROLS, NAME=name, INITIAL FEATURE ANGLE= Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Initial feature angle: Controlling the activation and deactivation of geometric edges and corners Abaqus/Standard allows geometric features, and consequently the updating rules applied at a node, to change during the analysis. For example, nodes are constrained to lie along a discrete geometric edge unless the angle forming the geometric edge becomes less than the transition geometric feature angle, θ > θ θ ≤ θ Initial mesh with a geometric feature: no mesh flow is permitted past the corner. The geometric feature is deactivated during simulation. Figure 12.2.6–1 Detection and deactivation of geometric features. ). The default value for the transition feature angle is ( . If the angle across the geometric edge becomes less than , the boundary surface is considered to be flattened sufficiently for the feature to be deactivated, and the mesh is allowed to slide freely on the surface. Geometric corners are allowed to flatten in a similar fashion. In addition, surfaces that are initially flat may develop edges or corners during the simulation. This logic allows great flexibility in mesh adaptation while preserving geometric features in the model. Setting will ensure that no geometric edges or corners are ever deactivated. You can change the transition feature angle using adaptive mesh controls. Abaqus/Standard will issue a warning message when geometric features are activated or deactivated. Input File Usage: *ADAPTIVE MESH CONTROLS, NAME=name, TRANSITION FEATURE ANGLE= Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Transition feature angle: Mesh constraints In most adaptive mesh problems the motion of nodes in the mesh is determined by the mesh smoothing algorithm, with constraints imposed by the domain boundary and the boundary region edges. However, there may be cases when you will want to define the motion of the nodes explicitly. You may also wish to keep certain nodes fixed, to move nodes in a particular direction, or to force certain nodes to move with the material. Adaptive mesh constraints give you the flexibility to define the motion of the node explicitly. Input File Usage: Abaqus/CAE Usage: *ADAPTIVE MESH CONSTRAINT Step module: Other→ALE Adaptive Mesh Constraint→Create Applying spatial mesh constraints Spatial mesh constraints are applied to define the motion of the nodes explicitly. Spatial mesh constraints allow full control over the mesh movement and can be applied to any node except those that have Lagrangian mesh constraints applied to them. You can also prescribe the spatial mesh constraints via user subroutine UMESHMOTION. The user subroutine allows you to let the spatial mesh constraints depend on available nodal or material point information. Input File Usage: Use the following option to define the mesh constraints explicitly: *ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=SPATIAL, TYPE=DISPLACEMENT or VELOCITY Use the following option to define the mesh constraints in user subroutine UMESHMOTION: *ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=SPATIAL, TYPE=DISPLACEMENT or VELOCITY, USER Abaqus/CAE Usage: To define the mesh constraints explicitly: Step module: Other→ALE Adaptive Mesh Constraint→Create: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Independent of underlying material To define the mesh motion in user subroutine UMESHMOTION: Step module: Other→ALE Adaptive Mesh Constraint→Create: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: User-defined Defining mesh constraints that vary with time The prescribed magnitude of a nonzero mesh constraint can vary with time during a step according to an amplitude definition . Input File Usage: Use both of the following options: Abaqus/CAE Usage: *AMPLITUDE, NAME=name *ADAPTIVE MESH CONSTRAINT, AMPLITUDE=name Step module: Other→ALE Adaptive Mesh Constraint→Create: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Independent of underlying material: Amplitude: amplitude Applying spatial mesh constraints in local directions Mesh constraints are applied in local directions if a transformed coordinate system is used at a node (“Transformed coordinate systems,” Section 2.1.5); otherwise, they are applied in global directions. Applying Lagrangian mesh constraints Lagrangian mesh constraints on a node are used to indicate that mesh smoothing should not be applied; i.e., the node must follow the material. Input File Usage: *ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=LAGRANGIAN Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Constraint→Create: Types for selected step: Displacement/Rotation or Velocity/Angular velocity: select region: Motion: Follow underlying material Spatial mesh constraint considerations When you decide on the type of spatial adaptive mesh constraint, (displacement, velocity, or specified with a user subroutine), you should consider the guidelines below. Choosing between displacement and velocity adaptive mesh constraints Displacement and velocity mesh constraints differ in their application. Displacement constraints define a node’s displacement relative to its original coordinates, while velocity constraints define a node’s velocity relative to the motion of the material. You will use a displacement constraint to control a node’s motion to a specific coordinate location, while you will use a velocity constraint to control a node’s motion relative to the Lagrangian motion. Therefore, a constant velocity adaptive mesh constraint does not in general lead to a constant velocity of the node relative to it’s original coordinates. Applying spatial adaptive mesh constraints to model material ablation Your spatial mesh constraint is applied without regard to the current material displacement at the node. This behavior allows you to prescribe mesh motion that differs from the current material displacement at the free surface of the adaptive mesh domain, effectively eroding, or adding, material at the boundary. Using adaptive mesh constraints this way is an effective technique for modeling wear or ablation processes. As described above, in common ablation modeling cases you will use the velocity form of the constraint. In addition, for general boundary shapes the most effective interface for ablation is user subroutine UMESHMOTION, where you can apply spatial mesh constraints to the nodes on the free surface in general ways according to solution-dependent variables, if needed. The user subroutine interface provides a local coordinate system that is normal to the free surface at the surface node, enabling you to describe mesh motions in this local system. Modifying ALE adaptive mesh constraints By default, all adaptive mesh constraints defined in the previous analysis step remain unchanged in the subsequent step. You define the adaptive mesh constraints in effect for a given step relative to the preexisting adaptive mesh constraints. At each new step the existing adaptive mesh constraints can be modified and additional adaptive mesh constraints can be specified. Input File Usage: Use either of the following options to modify an existing adaptive mesh constraint or to specify an additional adaptive mesh constraint: Abaqus/CAE Usage: *ADAPTIVE MESH CONSTRAINT, *ADAPTIVE MESH CONSTRAINT, OP=MOD Step module: Other→ALE Adaptive Mesh Constraint→Manager: select the desired step and mesh constraint: Edit Removing ALE adaptive mesh constraints If you choose to remove any adaptive mesh constraint in a step, no adaptive mesh constraints will be propagated from the previous step. Therefore, all adaptive mesh constraints that are in effect during this step must be respecified. Input File Usage: Use the following option to remove all previously defined adaptive mesh constraints and to specify new adaptive mesh constraints: *ADAPTIVE MESH CONSTRAINT, OP=NEW If the OP=NEW parameter is used on any *ADAPTIVE MESH CONSTRAINT option within a step, it must be used on all *ADAPTIVE MESH CONSTRAINT options in the step. Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Constraint→Manager: select the desired step and mesh constraint: Deactivate Contact When surfaces are defined for large-sliding contact, adaptive meshing may relocate the nodes on the surfaces. If the bodies in contact are sliding or deforming considerably, you may want to use Lagrangian mesh constraints on the boundary of the surfaces to prevent the surfaces from sliding from their intended place. For small-sliding contact Abaqus/Standard assumes that the reference configuration does not change significantly. If the reference configuration does not change significantly, the amount of adaptive meshing on these surfaces should be small and the contact quantities computed based on the reference configuration should continue to remain valid (Abaqus/Standard updates the tangent planes if nodes change positions). Hence, Abaqus/Standard will allow the nodes on the contact surface to move as needed by the mesh smoothing. You should apply Lagrangian mesh constraints in cases where nodes are intended to remain nonadaptive. Initial conditions Initial temperatures and field variables can be defined on any region subjected to adaptive mesh smoothing. However, to the updated configuration. these variables will not be remapped from the original Loads For elements with displacement degrees of freedom, no restrictions are made to loads applied to adaptive In cases where loads are intended to follow the material motion, Lagrangian mesh mesh domains. constraints must be applied to the nodes on the boundary of the surface on which distributed loads are applied to prevent the surface from sliding. This will allow adaptive meshing to occur inside the surface while maintaining the location of the distributed load. All the nodes on which concentrated loads are applied become nonadaptive. The loads that can be applied to an acoustic domain are described in “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1. These loads cannot be applied in procedures in which mesh smoothing can be performed. Boundary conditions Special consideration is given to nodes on which boundary conditions are applied. No adaptive meshing is done in the direction in which the boundary condition is applied, but adaptive meshing is carried out in other directions. When a boundary condition is removed in a step, the same restriction applies since Abaqus/Standard will ramp off the contribution of the boundary condition over the duration of the step. The boundary conditions that can be applied to an acoustic domain are described in “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1. These boundary conditions cannot be applied in any analysis procedure in which mesh smoothing can be performed. Predefined fields There are no restrictions on applying prescribed temperatures or field variables in an adaptive mesh domain, but these nodal values are not remapped when adaptive meshing is performed. Therefore, predefined fields that are not constant may not be meaningful in an adaptive mesh domain. Material options For elements with displacement degrees of freedom all material models that are isotropic and homogeneous can be used in an adaptive domain. Material options that have anisotropic behavior such as anisotropic materials , jointed material models , and concrete material models cannot be used in an adaptive mesh domain. For acoustic elements the relevant material models are described in “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1. Mesh smoothing assumes that the geometric changes in the acoustic domain do not lead to changes in material properties, such as fluid density. Elements Adaptive mesh domains can be defined for all acoustic first-order and second-order planar, axisymmetric, and three-dimensional elements in Abaqus/Standard and for a limited number of other elements. Table 12.2.6–1 provides a list of supported elements. Table 12.2.6–1 Elements supported for adaptive meshing. AC1D2, AC1D3, AC2D3, AC2D4, AC2D6, AC2D8, AC3D4, AC3D6, AC3D8, AC3D10, AC3D15, AC3D20, ACAX3, ACAX4, ACAX6, ACAX8 CPS4, CPS4T, CPS3 CPE4, CPE4H, CPE4T, CPE4HT, CPE4P, CPE4PH, CPE3, CPE3H CAX4, CAX4H, CAX4T, CAX4HT, CAX4P, CAX4PH, CAX3, CAX3H C3D8, C3D8R, C3D8H, C3D8RH, C3D8T, C3D8HT, C3D8RT, C3D8RHT, C3D8P, C3D8PH, C3D8RP, C3D8RPH Procedures Adaptive meshing can be used only in geometrically nonlinear general steps that invoke one of the following procedures: • Static stress/displacement analysis (“Static stress analysis procedures: overview,” Section 6.2.1) • Steady-state transport analysis (“Steady-state transport analysis,” Section 6.4.1) • Coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.3) • Coupled pore fluid flow and stress analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1) Acoustic elements will typically undergo adaptive meshing during static procedures and then participate in subsequent acoustic procedures in their updated configuration. Limitations • Elements within the adaptive domain cannot be removed or added (“Element and contact pair removal and reactivation,” Section 11.2.1). • Deformable elements that are declared rigid cannot be part of adaptive mesh domains. • Elements in the adaptive domain cannot contain embedded elements or rebars. • Symmetric results transfer cannot be done from an axisymmetric model that had solid elements in an adaptive domain. • Import cannot be done from a model that had solid elements in the adaptive domain. • It is not meaningful to drive a submodel using the nodes from a global model that were part of an adaptive mesh domain. • Only enhanced hourglass control can be used with reduced-integration elements. • When used with acoustic elements, adaptive mesh smoothing must be applied in steps prior to a coupled structural-acoustic analysis. It cannot be applied during a large-displacement dynamic analysis. • Mesh smoothing assumes that the geometric changes in the acoustic domain do not lead to changes in material properties, such as fluid density. • The coupling between the fluid and structure must be defined using a surface-based tie constraint with the slave surface defined on the acoustic domain. • Nodes in the adaptive domain that are involved in constraints such as multi-point constraints (“General multi-point constraints,” Section 34.2.2) and equations (“Linear constraint equations,” Section 34.2.1) should be made non-adaptive by applying Lagrangian constraints. Input file template Applying ALE adaptive meshing for acoustic analysis *HEADING … *ELEMENT, TYPE=…, ELSET=ACOUSTIC Data lines to define acoustic elements *ELEMENT, TYPE=…, ELSET=SOLID Data lines to define structural elements *SURFACE, NAME=TIE_ACOUSTIC Data lines to define the acoustic surface interface with the structural mesh *SURFACE, NAME=TIE_SOLID Data lines to define the solid surface interface with the acoustic mesh *TIE, NAME=COUPLING TIE_ACOUSTIC, TIE_SOLID … *STEP *STATIC *ADAPTIVE MESH, ELSET=ACOUSTIC, MESH SWEEPS=10 … *END STEP ** *STEP *STEADY STATE DYNAMICS, DIRECT … *END STEP Applying ALE adaptive meshing in other uses *HEADING … *ELEMENT, TYPE=C3D8, ELSET=.. Data lines to define solid elements *NSET, NSET=LAG Data lines to define nodes that should be nonadaptive *NSET, NSET=SPATIAL Data lines to define nodes that will have spatial adaptive mesh constraints applied *ELEMENT, TYPE=…, ELSET=SOLID Data lines to define structural elements *STEP, NLGEOM=YES *STATIC *ADAPTIVE MESH, ELSET=SOLID, MESH SWEEPS=10 *ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=LAGRANGIAN LAG *ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=SPATIAL, USER SPATIAL *END STEP 12.2.7 ALE ADAPTIVE MESHING AND REMAPPING IN Abaqus/Standard Products: Abaqus/Standard Abaqus/CAE References • “Defining ALE adaptive mesh domains in Abaqus/Standard,” Section 12.2.6 • *ADAPTIVE MESH • *ADAPTIVE MESH CONSTRAINT • *ADAPTIVE MESH CONTROLS • “Customizing ALE adaptive meshing,” Section 14.14 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview ALE adaptive meshing consists of two fundamental tasks: • creating a new mesh through a process called sweeping, and • remapping solution variables from the old mesh to the new mesh with a process called advection. You can control the process of mesh sweeping after which, if necessary, Abaqus/Standard will automatically perform advection. The default methods for creating a new mesh have been chosen carefully to work for acoustic analysis and for modeling the effects of ablation, or wear, of material. However, you may need to override the default choices to balance the robustness and efficiency of adaptive meshing or to extend the use of adaptive meshing for other types of applications. Adaptive mesh smoothing is defined as part of a step definition. The adaptive meshing in Abaqus/Standard uses an operator split method wherein each analysis increment consists of a Lagrangian phase followed by an Eulerian phase. The Lagrangian phase is the typical Abaqus/Standard solution increment where neither mesh sweeps nor advection occur. Once the equilibrium equations have converged, mesh smoothing is applied. Following the adjustment of nodes through the mesh sweeping process, material point quantities are advected in an Eulerian phase to account for the revised meshing of the model in its current configuration. This operator split method is chosen to avoid unsymmetric Jacobian terms that would result when the advection and material straining occur simultaneously. Advection is not required for, and is not applied to, acoustic elements. The ALE adaptive mesh sweeping algorithm Adaptive mesh smoothing is performed after the structural equilibrium equations have converged. The mesh smoothing equations are solved explicitly by sweeping iteratively over the adaptive mesh domain. During each mesh sweep, nodes in the domain are relocated—based on the positions of neighboring nodes obtained during the previous mesh sweep—to reduce element distortion. The new position, , of a node is obtained as is the original position of the node, are the neighboring where nodal positions obtained during the previous mesh sweep, and are weight functions obtained from one or a weighted mixture of the following methods. The displacements applied during sweeps are not associated with mechanical behavior. is the nodal displacement, Original configuration projection Original configuration projection is the default in Abaqus/Standard and determines the weight function from a least squares minimization procedure that minimizes node displacement in a projection of the mesh back to the original configuration. This method of smoothing affects only deformations of the mesh and not the original mesh. Volume smoothing Volume smoothing determines the weight function by computing a volume-weighted average of the element centers in the elements surrounding the node. In Figure 12.2.7–1 the new position of node M is determined by a volume-weighted average of the positions of the element centers, C, of the four surrounding elements. The volume weighting will tend to push the node away from element center C1 and toward element center C3, thus reducing element distortion. L3 C4 C3 L4 C1 C2 L1 L2 Figure 12.2.7–1 Relocation of a node during a mesh sweep. Volume smoothing is supported in structured domains, where every node is surrounded by four elements in two dimensions or eight elements in three dimensions. Combining smoothing methods The default smoothing method in Abaqus/Standard is original configuration projection. To choose an alternate smoothing method or to combine the smoothing methods, you specify the weighting factor for each method. When more than one smoothing method is used, a node is relocated by computing a weighted average of the locations predicted by each chosen method. All weights must be zero or positive, and their sum must be nonzero. The weights are significant only in a relative sense; their values are normalized so that their sum is 1.0. Input File Usage: *ADAPTIVE MESH CONTROLS, NAME=name original configuration projection weight, volume smoothing weight Abaqus/CAE Usage: For example, the following option could be used to define an equal blend of original configuration projection and volume smoothing: *ADAPTIVE MESH CONTROLS, NAME=name 0.5, 0.5 Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, Original configuration projection: original configuration projection weight, Volumetric: volume smoothing weight Geometric enhancements to the basic smoothing methods The conventional forms of the basic smoothing methods may not perform well in highly distorted domains. You can use geometrically enhanced forms of the basic smoothing algorithms as a technique to mitigate distortion. These forms are heuristic and based on nodal locations only. Due to their heuristic nature, geometric enhancements may not always improve the mesh smoothing. Input File Usage: Use the following option to apply geometric enhancements to the smoothing algorithm: *ADAPTIVE MESH CONTROLS, NAME=name, GEOMETRIC ENHANCEMENT=YES Abaqus/CAE Usage: Step module: Other→ALE Adaptive Mesh Controls→Create: Name: name, toggle on Use enhanced algorithm based on evolving element geometry Application of the sweeping algorithm The mesh smoothing process begins with the mesh in its current displaced equilibrium configuration. Nodes that have no displacement degrees of freedom, such as those connected to acoustic elements, are maintained at their most recent configuration. Mesh smoothing is then driven by distortions in the current configuration and by boundary constraints. These boundary constraints can be described directly through adaptive mesh constraints. In the case of structural-acoustic boundaries the structural mesh boundary provides a constraint that controls the smoothing of adjacent acoustic element regions. When these boundary constraints are much larger than the characteristic element length in the adaptive mesh domain, significant geometric changes, such as the development of corners, can occur. To prevent such changes, the constraints are applied gradually over a series of “sub-increments” onto the domain boundary. The number of sub-increments used is determined on the basis of the magnitude of the maximum surface displacement and the characteristic element dimension. The remaining nodes (nodes not driven by constraints) are identified as interior nodes, free surface nodes, edge nodes, or corner nodes. These nodes are treated as described in “Defining ALE adaptive mesh domains in Abaqus/Standard,” Section 12.2.6. At the end of mesh sweeping the new geometry is checked to ensure that elements did not become severely distorted during mesh smoothing. Abaqus/Standard responds to severe distortion in different ways, depending on the elements and procedures used. When adaptive meshing is used with acoustic elements, the current analysis increment is repeated with a reduced time increment, followed by another adaptive mesh smoothing attempt. When adaptive meshing is used with other elements, severe distortion results in abandonment of mesh smoothing for that increment. In cases where adaptive mesh constraints are also defined, Abaqus/Standard aborts since the constraints cannot be satisfied. Controlling the frequency of ALE adaptive mesh smoothing In most cases the frequency of adaptive meshing is the parameter that most affects the mesh quality. By default, mesh smoothing will be performed after each converged structural analysis increment. You can change the frequency of adaptive meshing, except when adaptive mesh constraints are defined. Input File Usage: Abaqus/CAE Usage: *ADAPTIVE MESH, FREQUENCY=number of increments Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on Use the adaptive mesh domain below, Frequency: number of increments Controlling convergence of ALE adaptive mesh smoothing The adaptive mesh smoothing equations are solved explicitly by sweeping iteratively over the adaptive mesh domain. During each mesh sweep, nodes in the domain are relocated based on the current positions of neighboring nodes to reduce element distortion. Mesh smoothing is performed following the end of a converged increment. You can control the intensity of the mesh smoothing by defining the number of mesh sweeps required. When the displacements are large, more iterations are usually required. When used in acoustic analyses, more iterations are usually required when the volume of the elements in the acoustic domain decreases compared to the case when the volume increases during structural loading. You can specify the number of mesh sweeps to be performed in each adaptive mesh increment. The default number of mesh sweeps is one. By applying the mesh sweeping algorithm repeatedly, the mesh will converge; in other words, nodal positions are obtained that do not change with further mesh sweeping. However, it is usually not necessary to apply mesh smoothing until a converged mesh is obtained; the main objective is to reduce element distortion. Input File Usage: Abaqus/CAE Usage: *ADAPTIVE MESH, MESH SWEEPS=number of sweeps Step module: Other→ALE Adaptive Mesh Domain→Edit: toggle on Use the adaptive mesh domain below, Remeshing sweeps per increment: number of sweeps The ALE adaptive mesh advection algorithm Abaqus/Standard applies an explicit method, based on the Lax-Wendroff method, to integrate the advection equation. The key principle of the Lax-Wendroff method is replacement of the time derivatives of the material point quantities with the spatial derivatives using the classical relationship between the material time derivative, the referential derivative, and the spatial derivative. The update scheme is second-order accurate and provides some upwinding. Nodal quantities are advected by first converting them to the material point quantities. Advection of the material quantities will generally result in loss of equilibrium, for two main reasons. The first reason is the errors in the advection process itself. To minimize the errors in advection, Abaqus/Standard imposes restrictions on the magnitude of the advection velocity by requiring that the Courant number for every element in the adaptive domain be less than one. In cases where the Courant number is greater than one you will be informed and Abaqus/Standard will generate multiple advection passes per increment. The second reason for the loss of equilibrium is changes in the representation of the underlying material quantities by the changed mesh. For example, consider a region of the structure having some stress gradients spanned initially by two elements. After mesh smoothing, the same region might have more than two elements. This will lead to slightly different volume integration while computing the internal force even when there are no errors in advection. These sources of error in equilibrium are significant only when the mesh is too coarse to provide a good solution and mesh smoothing is carried out with such small frequency that the mesh motion is larger than the average element size. In practical applications these errors are typically insignificant, the resulting loss of equilibrium is generally small, and the residuals generated by the loss of the equilibrium fall within the limits of the Abaqus/Standard convergence criterion. Any loss of equilibrium is not propagated since equilibrium will again be satisfied at the end of the Lagrangian phase of the next increment. Impact of advection on subsequent steps To ensure that the results are output only for the configuration that satisfies equilibrium, Abaqus/Standard always outputs the results at the end of the Lagrangian phase. The Eulerian phase that follows the Lagrangian phase will leave the structure out of equilibrium for the next increment. This sequence has a consequence that after the last Eulerian phase is carried out at the end of the step, equilibrium will not be satisfied exactly at the beginning of the next step and the solution at the end of the step will differ slightly from the solution at the zero increment of the following step. Equilibrium can again be established by following the step that had adaptive meshing by a step that removes all the adaptive mesh domains and allows the structure to equilibrate. A one-increment step will usually suffice. This is particularly important when the following step is a perturbation procedure that uses the solution from the previous step as the base state. Frequency steps that follow adaptive mesh steps will also be impacted, because element mass is not advected during mesh smoothing. This impact on the element mass can be significant, depending on the extent of adaptive mesh motion and change in element size due to mesh smoothing. Abaqus will provide a warning message in cases where adaptive meshing precedes a frequency step; you should evaluate the impact of your updated mesh configuration when interpreting results from a frequency step in these cases. Output In adaptive meshing the integration point of an element will generally not refer to the same material point throughout the analysis. Contour plots of material variables will show correct spatial distribution, but history plots are not meaningful. The displacement of the nodes contains the material displacement as well as the displacement due to mesh motion. You can obtain measures of the volume lost due to adaptive mesh constraints with the partial model variable VOLC, which is useful when using adaptive mesh constraints to model ablation. A summary of the adaptive meshing in each adaptive mesh domain is written to the message (.msg) file. This summary includes the total number of load increments over which the structural displacement is transferred to the fluid, the total number of mesh sweeps performed, the magnitude of the maximum displacement increment, and the node and degree of freedom at which the maximum displacement increment is measured. Warning messages are issued when geometric features change during mesh smoothing. More detailed diagnostic output for adaptive mesh smoothing can be requested; see “The Abaqus/Standard message file” in “Output,” Section 4.1.1. This output provides the magnitude of the maximum displacement and the node and degree of freedom where the maximum displacement increment occurs during each mesh sweep. In addition, the nodes experiencing changes in geometric features are listed. Additional references • Lax, P. D., and B. Wendroff, “Difference Schemes for Hyperbolic Equations with High-Order Accuracy,” Communications on Pure and Applied Mathematics, vol. 17, p. 381, 1964. • Lax, P. D., and B. Wendroff, “Systems of Conservations Laws,” Communications on Pure and Applied Mathematics, vol. 13, pp. 217–237, 1960. 12.3 Adaptive remeshing • “Adaptive remeshing: overview,” Section 12.3.1 • “Selection of error indicators influencing adaptive remeshing,” Section 12.3.2 • “Solution-based mesh sizing,” Section 12.3.3 12.3.1 ADAPTIVE REMESHING: OVERVIEW Abaqus/CAE provides an automated process to remesh your model adaptively. The goal of the adaptive remeshing process is to approach or reach targets on selected error indicators for a specified model and its accompanying load history. See “Adaptivity techniques,” Section 12.1.1, for a comparison of this process to other Abaqus adaptivity methods. Overview The following steps are required to incorporate adaptive remeshing into your Abaqus/CAE model: • You identify regions of the model where you wish to apply one or more adaptive remeshing rules. A remeshing rule defines the step during which it will be applied, the error indicator output variables and targets for those error indicators, the sizing method, and any constraints on element size. See “What are remeshing rules?,” Section 17.13.1 of the Abaqus/CAE User’s Manual. • You define a succession of analysis jobs, an “adaptivity process,” that will be run as Abaqus/CAE attempts to meet your remeshing rule targets. See “What is an adaptivity process?,” Section 19.3.1 of the Abaqus/CAE User’s Manual. Based on these remeshing rules and your adaptivity process definition, Abaqus/CAE iteratively: • executes an Abaqus/Standard analysis, which will write selected error indicator output variables based on your remeshing rule settings , • uses the error indicator variables in a sizing function to compute element sizes for a new mesh, respecting any size constraints you might specify , and • generates a new mesh in the regions specified, based on the computed element sizes. The neighboring regions will also be remeshed. These iterations continue until either: • all remeshing rule targets are satisfied, or • a maximum number of remesh iterations is reached. See “When will my mesh adaptivity stop iterating?,” Section 19.3.2 of the Abaqus/CAE User’s Manual, for more details. Figure 12.3.1–1 shows the interaction of Abaqus products and files in this process. Typical applications Adaptive remeshing can improve the quality of your simulation results. Adaptive remeshing can be helpful when: • you are unsure how refined a mesh needs to be to reach a particular level of accuracy or how coarse the mesh can be without unacceptably impacting solution accuracy; • it is difficult to design an adequately refined mesh near a region of interest, such as near a stress riser; or Automated Abaqus/CAE Actions Figure 12.3.1–1 User actions and automated Abaqus/CAE actions in the adaptive remeshing process. • you do not know a location of interest, such as with formation of a plastic zone, a priori. An example of using adaptive remeshing to study the thermal and stress behavior of a bolted vessel is provided in “Thermal-stress analysis of a reactor pressure vessel bolted closure,” Section 5.1.6 of the Abaqus Example Problems Manual. The example includes a Python script that you can run from Abaqus/CAE to create the model and the remeshing rules. A second script allows you to submit the adaptivity process and to view the changing mesh as Abaqus/CAE computes new element sizes. Example: stress riser Figure 12.3.1–2 shows how adaptive remeshing generates a high-quality mesh for a typical notched specimen subjected to axial loading. Figure 12.3.1–2 Stress riser mesh before and after refinement. Figure 12.3.1–3 shows the effect of these mesh changes on solution accuracy in comparison to the effect of uniform mesh refinement on solution accuracy. Adaptive mesh refinement is much more efficient than uniform mesh refinement at reducing solution error. Example: plastic hinge This example, a doubly-notched specimen axially strained until a plastic hinge or band forms, is used to demonstrate how adaptive remeshing will focus a mesh on a plastic hinge. It illustrates the value of adaptive remeshing in cases where the region of interest may not be known a priori. Figure 12.3.1–4 shows the specimen and the region of active yielding. Figure 12.3.1–5 shows the original mesh and the adapted mesh after three adaptive remeshing iterations. Figure 12.3.1–3 Comparison of adaptive remeshing to uniform mesh refinement based on boundary seeding. Figure 12.3.1–4 Region of active yielding in a doubly-notched specimen. Figure 12.3.1–5 Mesh of doubly-notched specimen before and after adaptive remeshing. Preparing your model for adaptive remeshing You use Abaqus/CAE to do the following when performing adaptive remeshing: • create the model and specify the boundary conditions and loading history, • create remeshing rules, • create an adaptivity process, and • start and monitor the progress of the adaptivity process. Creating the model You do not have to consider adaptive remeshing when you create the model and specify the boundary conditions and loading history; however, before using adaptive remeshing you must do the following: • create the geometry of the model—you cannot use an orphan mesh part—and • provide an initial, nominal, mesh. This mesh can be fairly coarse. Providing an extremely coarse mesh, however, can result in more adaptive remesh iterations due to the poor quality of early remesh iteration error indicator calculations. You can, in typical cases, define a reasonable initial mesh by using the default part instance mesh seeding in Abaqus/CAE. Creating a remeshing rule You create and configure a remeshing rule using the Mesh module in Abaqus/CAE. See “Creating a remeshing rule,” Section 17.21.1 of the Abaqus/CAE User’s Manual, for details on defining remesh rules. Refer to “Selection of error indicators influencing adaptive remeshing,” Section 12.3.2, and “Solution- based mesh sizing,” Section 12.3.3, for details on the methods used to determine revised mesh size distributions. Abaqus/CAE Usage: Mesh module: Adaptivity→Remeshing Rule→Create Creating an adaptivity process You create and configure an adaptivity process using the Job module in Abaqus/CAE. When you create an adaptivity process, you can specify the maximum number of remesh iterations to be performed and set various system resource parameters. See “Creating, editing, and manipulating jobs,” Section 19.7 of the Abaqus/CAE User’s Manual, for details. Abaqus/CAE Usage: Job module: Adaptivity→Create Performing adaptive remeshing with a provisional analysis In some cases you will want to determine an adequate mesh for your model prior to conducting a fully detailed analysis, which might include many steps and complex behavior. A “provisional” analysis can often be used, along with adaptive remeshing, to efficiently determine a good mesh for a model. The provisional analysis may include various simplifications of your fully detailed analyis, such as • replacing your steps with a single linear perturbation step with loading that adequately reflects your more general loading cases, • removing plasticity and other material nonlinearities, and • disabling geometric nonlinearity. The provisional analysis approach may result in a mesh that is not ideally suited to your ultimate choice of loading. However, the cost for obtaining a mesh from a provisional model may be significantly lower than the case where your adaptivity process considers all of the complexity in the fully detailed analysis, and you may find the refined mesh adequate for use in a variety of analysis situations. Special considerations In general, the Abaqus adaptive remeshing process iterates automatically toward a better quality mesh; however, you should be aware of certain considerations. Singularities Stress singularities frequently result from geometric abstractions, such as reentrant corners and contact of a sharp edge in elastic materials, and from point loads or abruptly ended distributed load regions. In these situations the stress field near the singularity is unbounded, and no amount of mesh refinement will enable resolution of the correct solution. If you apply the adaptive remeshing process to regions of your model that include singularities, the process will drive elements near the singularity to very small sizes. The end result may be unacceptably expensive analyses. You can prevent excessively expensive analyses of models with singularities using the following techniques: • Exclude the region of the singularity from consideration in the remeshing process. You exclude a region by partitioning the model and assigning remeshing rules only to regions away from the singularity. • Apply a minimum element size constraint in the remeshing rule. Abaqus/CAE does assign a minimum element size by default, which is a fraction of the default part instance mesh seed. You can modify this constraint to achieve a quality solution near the singularity while avoiding an excessively refined mesh. You can also use the remeshing rule to control the rate at which Abaqus/CAE refines the size of the elements. Element size constraints may prevent an adaptivity process from achieving specified error indicator targets. • Specify a maximum number of elements for a remeshing rule region. Abaqus/CAE adjusts the mesh sizing such that the generated total number of elements approximately satisfies this constraint. Convergence issues Figure 12.3.1–6 shows a typical history of an error indicator and the computational cost, Abaqus/Standard, versus remesh iteration. in Error Indicator Computational Cost 50% 25% 3x 2x 1x Remesh Iteration Figure 12.3.1–6 Error indicator and computational cost versus iteration for a model with a 25% error indicator target. The example in Figure 12.3.1–6 shows a desirable convergence profile. The solution error indicator decreases monotonically and quickly to the desired 25% error indicator target. Accompanying this error indicator decrease is a moderate increase in computational cost, measured either in model degrees of freedom or time in Abaqus/Standard. Certain situations can interfere with this desirable convergence profile, as follows: • If your initial mesh is too coarse, the error indicator variables may be of insufficient quality to result in a mesh that is sufficiently improved in the next iteration. The adaptive remeshing process typically creates a high-quality mesh eventually even if the initial mesh is quite coarse. However, some mesh iterations can be avoided with a reasonably refined initial mesh. • Minimum element size constraints and constraints on the maximum number of elements that you specify when creating the remeshing rule can prevent the mesh from achieving sufficient refinement (in the extreme case of singularities this will always be the case) to satisfy your error indicator targets. You may be able to satisfy your targets by relaxing these constraints; for example, by decreasing the minimum element size. For more information, see “What are remeshing rules?,” Section 17.13.1 of the Abaqus/CAE User’s Manual. • In addition to producing small mesh sizes resulting in a large number of elements, singularities can cause an adaptivity process to fail in achieving the error target or to require more remeshing iterations. As described in “Singularities,” above, you can control the computational cost by specifying a minimum element size constraint or the maximum number of elements. In any case where a singularity exists within a remeshing rule region, you may see poor convergence in the error indicator results. • Linear elements (C3D4, CPS4, etc.) and modified elements (C3D10M, CPS6M, etc.) converge slowly compared to quadratic elements (C3D10, CPS6, etc.) requiring a relatively large number of elements to achieve a given error target. Hence, you should use quadratic elements whenever possible. Continuing a stopped adaptive remeshing process The adaptive remeshing process is designed to be automatic—Abaqus/CAE performs a sequence of analyses as it continues to refine your mesh. However, there are occasions where the process will stop and you will want to continue adaptive remeshing from your most recent mesh: • when you want to change remeshing rules for later remesh iterations, or • when the adaptive remesh process fails to complete due to machine resource problems. You can continue the adaptive remeshing process by resubmitting an existing adaptivity process, creating and submitting a new adaptivity process, or performing manual remeshing. See “Manually resizing and remeshing,” Section 17.21.6 of the Abaqus/CAE User’s Manual. Limitations Adaptive remeshing requires the use of Abaqus/CAE, and only Abaqus/Standard procedures are supported. Other specific limitations also apply. Element types Abaqus/CAE can perform adaptive remeshing only with elements of the following shapes : • Planar continuum triangles and quadrilaterals • Shell triangles and quadrilaterals • Tetrahedrals Procedures Abaqus/CAE can perform remeshing with the following Abaqus/Standard procedures: • “Static stress analysis,” Section 6.2.2 (general and linear perturbation). • “Quasi-static analysis,” Section 6.2.5. • “Uncoupled heat transfer analysis,” Section 6.5.2. • “Fully coupled thermal-stress analysis,” Section 6.5.3. • “Coupled thermal-electrical analysis,” Section 6.7.3. • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1. 12.3.2 SELECTION OF ERROR INDICATORS INFLUENCING ADAPTIVE REMESHING Products: Abaqus/Standard Abaqus/CAE References • “Error indicator output,” Section 4.1.4 • “Adaptive remeshing: overview,” Section 12.3.1 • “Abaqus/Standard output variable identifiers,” Section 4.2.1 • *CONTACT OUTPUT • *ELEMENT OUTPUT • “Understanding adaptive remeshing,” Section 17.13 of the Abaqus/CAE User’s Manual • “Controlling adaptive remeshing,” Section 17.21 of the Abaqus/CAE User’s Manual Overview Your selection of which error indicator variables to use in adaptive remeshing rules for a particular analysis should take into consideration: • characteristics of the error indicator variables; • which fields exist and are of interest; and • the nature of the loading. Error indicator characteristics Error indicator output variables provide estimates of solution accuracy . In the context of adaptive remeshing, error indicators help determine where the mesh should be refined or coarsened to achieve the specified accuracy targets . This Section discusses additional characteristics of error indicators in the context of how well-suited they are for influencing adaptive remeshing in various analysis types. Which fields exist and are of interest Certain variables apply naturally to certain types of analyses. For example, the heat flux indicator (HFLERI) is used in analyses with temperature degrees of freedom. When selecting error indicator variables in the Remeshing Rule editor in Abaqus/CAE , your choices will be restricted to variables available for the selected procedure type. The nature of the loading Some error indicator variables only indicate discretization error at the current analysis time—the particular increment in a step. Other error indicator variables provide a record of the solution history up to the current analysis time. For example, if your simulation involves non-proportional loading or a significantly nonlinear response, you will typically see better adaptive remeshing results when using error indicator variables that record the solution history. Table 12.3.2–1 lists the error indicator variables applicable to adaptive remeshing and indicates whether they record the solution history. Table 12.3.2–1 Error indicator variables applicable to adaptive remeshing that record the solution history. Solution Quantity Error indicator Element energy density Mises stress Equivalent plastic strain Plastic strain Creep strain Heat flux Electric flux Electric potential gradient variable ( ) ENDENERI MISESERI PEEQERI PEERI CEERI HFLERI EFLERI EPGERI Records the solution history? Yes No Yes No No No No No By default, when you create a remeshing rule, error indicators are specified for the final increment of the final step of your analysis and adaptive remeshing is based on error indicators in this final increment. When you select an error indicator that records the solution history, this default error indicator specification is appropriate for almost all analyses. However, for other error indicator variables that do not record the solution history, you may find it appropriate (for multistep cases with non-proportional loading, for example) to define mutiple remeshing rules for the same region, with each rule applied to a different step. The examples that follow provide simple illustrations of typical cases and show appropriate choices of error indicator output variables. Linear response example Figure 12.3.2–1 illustrates the simplest load case, where the load is proportional to the step time and the model’s response is linear. In this case the solution at the final increment would be proportional to any other increment. Therefore, it is appropriate to base the remeshing on the value of the error indicator in the last increment for any choice of error indicator variable. Monotonic response example Figure 12.3.2–2 illustrates a more general case, where the model has a nonlinear response—in this case resulting from a geometric nonlinearity—and the loading is monotonic but not generally proportional to the step time. The response of the model is slightly more general because the solution at a particular increment is not proportional to the solution at the final increment. However, the value of the error indicator output in the final increment still reflects the extreme of the model’s response to the load history. Figure 12.3.2–1 Proportional-loading, linear-response example: small deflection of a cantilever. Figure 12.3.2–2 Monotonic response example: large deflection of a cantilever. Therefore, it is appropriate to base the remeshing on the value of the error indicator in the last increment for any choice of error indicator variable. General response example Figure 12.3.2–3 illustrates a case where the loading characteristics change dramatically during the analysis. Your choice of error indicator in this case will depend on the material model. The element energy density error indicator, ENDENERI, will account for the complexity of load history (and lead to an adapted mesh that provides an accurate solution through the analysis) regardless of the material type. If plastic deformation occurs, you also have the option to use the equivalent plastic strain, PEEQERI, or plastic strain, PEERI, error indicators. Plastic strain and the plastic strain error indicator generally do not capture history effects; for example, they do not account for peak straining in models undergoing symmetric strain reversals. This example, however, involves no strain reversals; therefore, PEERI would be a valid error indicator choice. Figure 12.3.2–3 General response example: block subjected to a rigid indenter. General multistep response example: die forming and springback Figure 12.3.2–4 illustrates a further generalization of a general response. Here, a forming operation is simulated, and different steps are used for different stages of the operation. Figure 12.3.2–4 General multistep response example. In this case the response of the model varies from step to step. You will typically want the error indicator to capture the extreme of the model’s response to the load history adequately. However, you do not know if any particular increment captures this extreme. Therefore, you should select an error indicator variable that records the solution history. 12.3.3 SOLUTION-BASED MESH SIZING Products: Abaqus/Standard Abaqus/CAE References • “Adaptive remeshing: overview,” Section 12.3.1 • “Selection of error indicators influencing adaptive remeshing,” Section 12.3.2 • “Understanding ALE adaptive meshing,” Section 14.6 of the Abaqus/CAE User’s Manual • “Advanced meshing techniques,” Section 17.14 of the Abaqus/CAE User’s Manual Overview Solution-based mesh sizing: • is performed in Abaqus/CAE; and • operates on error indicator output variables and your remeshing rule parameters to determine an improved element size distribution for your mesh. Basic operation of the sizing method The sizing method calculates new element sizes during the adaptive remeshing process. Abaqus/CAE applies the sizing method to a field of error indicator variables and their corresponding base solution variables over the region defined by the remeshing rule. The output of a sizing method is a set of scalar sizes located at the nodes in the region defined by the remeshing rule. Figure 12.3.3–1 illustrates the sizing operation. Figure 12.3.3–1 shows the base solution and error indicator distributions after the first remesh iteration. The sizing method determines that the element size should be reduced in the region of greatest error indicator and increased in the region of the lowest error indicator. The mesh that is generated from these target element sizes is illustrated. Characteristics of error indicators The sizing method and parameter settings that you select have a significant impact on how adaptive remeshing changes the error indicator distribution in your model. You may, for example, choose a sizing method that aggressively reduces error indicators only near a stress riser. In other cases, where the global response of your structure is more important than local effects, you may choose a sizing method that attempts to reduce the error indicators to a uniform level throughout the region. To understand how the sizing methods affect the error indicators, you should first understand typical characteristics of the error indicator variables. Figure 12.3.3–2 provides an illustration of an error indicator and corresponding base solution distribution on a generalized slice through a model. Lowest base solution Figure 12.3.3–1 Sizing method operation and interaction with meshing. Figure 12.3.3–2 illustrates the following error indicator characteristics: • In regions where the value of the base solution is high, such as for element “i” in Figure 12.3.3–2, error indicator values can be low relative to local values of the base solution. In many cases you may want to use mesh refinement to drive these error indicators even lower. error indicator solution cb ce SOLUTION-BASED MESH SIZING maximum base solution ce cb minimum base solution position element i element j Figure 12.3.3–2 Error indicator and base solution distribution. • In regions where the base solution is low, such as for element “j” in Figure 12.3.3–2, error indicator values can be high relative to the local values of the base solution. In many cases you may not be interested in obtaining an accurate solution in these regions. These characteristics can affect your decision on which sizing method to use and what parameters to set in the sizing method. Sizing methods Sizing methods employ the concept of an error target, form and which defines a general goal , which is expressed in a normalized percentage is a measure of the error indicator and where is a measure of the base solution. Based on your definition of the error targets when you created the remeshing rule, Abaqus/CAE creates a size distribution that attempts to meet your error target in the subsequent analysis job using the remeshed model. The specific meaning of an error target depends on your choice of the sizing method. Abaqus/CAE provides two fundamental sizing methods: Minimum/maximum control and Uniform error distribution. You can also choose a third method, Default method and parameters, which results in Abaqus/CAE choosing one of the fundamental sizing methods for you, based on your choice of error indicator variable. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Sizing Method Minimum/maximum control The minimum/maximum control method provides the most flexibility in the remeshing of your model. This method has the following characteristics: • Two error indicator targets for controlling the sizing. the base solution (such as stress) is highest, and solution is lowest. controls the sizing in regions where controls the sizing in regions where the base • A continuous variation in error targets between regions of high and low base solution values, with a bias factor parameter provided to control the variation. • To avoid excessive refinement at elements with a small base solution, a global averaged element base is chosen when the element base solution is smaller than the global averaged element base. • If singularities are present in the remeshing rule region, this method will fail to satisfy the error target because the maximum base solution, which occurs at the location of the singularity, is unbounded. You can either allow Abaqus to choose the targets automatically, or you can specify the error targets. Similarly, you can accept the default bias factor displayed by Abaqus/CAE, or you can specify a qualitative bias factor. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Sizing Method: Method: choose Minimum/Maximum control Allowing Abaqus/CAE to choose the error targets If you specify the minimum/maximum error control method without setting error targets, Abaqus/CAE automatically chooses the error targets, . Both targets are computed as a fraction of the error indicator result in the previous remesh iteration analysis. Automatic error target reduction is a good choice for mesh refinement studies, where you have no specific error target goal but want to see the impact of mesh refinement on your results. and Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Sizing Method: Error Targets; choose Automatic error target reduction Specifying the error targets As an alternative to automatic error target reduction, you can specify the two error targets, . Figure 12.3.3–2 illustrates these two locations. is applied to element , and and is applied to element . Using the value of the two error targets, Abaqus/CAE applies a sizing method that attempts to meet both and at their respective locations. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Sizing Method: Error Targets; choose Fixed error targets; enter the maximum base solution error indicator target, , and the minimum base solution error indicator target, . Bias factor You can use the bias factor definition in the remeshing rule to further tune the distribution of sizing between maximum and minimum base solution locations. The bias factor defines the gradient of the size distribution between these two extremes in your remesh region, as shown in Figure 12.3.3–3. Figure 12.3.3–3 The impact of the bias factor on the element size distribution. You can set this factor between two qualitative extremes, “weak” and “strong.” At the weak extreme, element sizes will increase most quickly at locations moving away from the maximum base solution. At the strong extreme, element sizes will increase most slowly. The default setting is a bias toward the strong extreme. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Sizing Method: Mesh Bias; drag the slider to a setting between Weak and Strong Uniform error distribution The uniform error distribution method provides a single error indicator target, , for controlling the sizing. Abaqus/CAE applies a sizing method such that the total error in the remeshing rule region is distributed uniformly across all the elements and satisfies the given error indicator target. This method attempts to satisfy the error indicator target collectively for the whole remeshing rule region but not at every element. Therefore, the presence of singularities will not prevent the adaptivity process from achieving the error target. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Sizing Method: Method: choose Uniform error distribution Allowing Abaqus/CAE to choose the error target If you specify the uniform error distribution method without setting an error target, Abaqus/CAE automatically chooses the error target, . The target is computed as a fraction of the error indicator result in the previous remesh iteration analysis. Automatic error target reduction is a good choice for mesh refinement studies, where you have no specific error target goal but want to see the impact of mesh refinement on your results. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Sizing Method: Error Targets; choose Automatic error target reduction Specifying the error target As an alternative to the automatic error target reduction, you can specify the single error target, . When you use the uniform error distribution method, Abaqus/CAE compares the error target to a global norm of a normalized form of the error indicator. Such an approach ensures a globally converging mesh within the region. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Sizing Method: Error Targets: choose Fixed error target; enter the error indicator target, Default sizing methods and parameters This method results in application of the Automatic error target reduction form of either the Minimum/maximum control or Uniform error distribution method, with the method applied based on the error indicator variable according to Table 12.3.3–1. Table 12.3.3–1 Default sizing method for each error indicator. Solution Quantity Error indicator variable Default sizing method Element energy density ENDENERI Uniform error distribution Mises stress MISESERI Minimum/maximum control Equivalent plastic strain PEEQERI Minimum/maximum control Plastic strain Creep strain Heat flux Electric flux Electric potential gradient PEERI CEERI HFLERI EFLERI EPGERI Minimum/maximum control Minimum/maximum control Uniform error distribution Minimum/maximum control Minimum/maximum control When your remeshing rule refers to multiple error indicators, sizing methods will be applied independently to each error indicator variable with the resulting local size based on the smallest size calculated from each sizing method. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Sizing Method: Method: choose Default methods and parameters Example: Plate with a circular stress riser The difference between the basic behavior of the minimum/maximum control and the uniform error distribution methods is illustrated by a simple example. Figure 12.3.3–4 shows the stress result for a simple loading of a plate with a hole. Figure 12.3.3–4 Initial mesh and Mises stress distribution for a plane stress plate with a hole, subjected to a uniform horizontal boundary traction. Minimum/maximum control Figure 12.3.3–5 illustrates the adaptive mesh that was generated by Abaqus/CAE when the user selected the minimum/maximum control method and specified the two error targets ( ). In this example =1%, and the mesh bias is set to the default setting. These settings result in a mesh that focuses tightly around the hole, the stress riser, while transitioning smoothly to a relatively coarse mesh away from the hole. =5% and and Uniform error distribution Figure 12.3.3–6 illustrates the adaptive mesh that was generated by Abaqus/CAE when the user selected the uniform error distribution method and specified the single uniform error indicator target ( ). In this example =1%. This setting results in a mesh that focuses around the hole, the stress riser, while also refining the mesh in less stressed regions. Impact of additional remeshing rule settings You specify the sizing method when you create a remeshing rule, and the sizing method calculates new element sizes during the adaptive remeshing process. However, the following additional settings in the remeshing rule can affect the mesh generated by Abaqus/CAE, regardless of the sizing method that you selected: • region selection, • step and frame selection, Figure 12.3.3–5 Adaptive remesh resulting from the minimum/maximum control sizing method. Figure 12.3.3–6 Adaptive remesh resulting from the uniform error distribution sizing method. • size constraints, • approximate maximum number of elements, and • refinement and coarsening rate factors. Region selection Sizing methods are defined across sets of elements, corresponding to the regions over which the remeshing rules were applied in Abaqus/CAE. Within each set of elements, Abaqus/CAE applies the sizing operation to the error indicator variables specified in the remeshing rule. The results of the sizing operation are based on the extrapolation of whole element calculations to the nearest nodes, and the results are node based. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Edit Region Step and frame selection Abaqus applies sizing operations to error indicator variables from only the last available frame in a specified step. See “Error indicator characteristics” in “Selection of error indicators influencing adaptive remeshing,” Section 12.3.2, for a discussion of how your selection of the step, frame, and error indicator can affect your ability to capture the response in transient analyses. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Step and Indicator: Step; select the step to which the rule is applied and Mesh module: Create Remeshing Rule: Step and Indicator: Output Frequency; choose either Last increment of step or All increments of step Size constraints When you create the remeshing rule, you can constrain the sizing operation from specifying elements greater than or less than size constraints that you define for the remesh rule region. Abaqus/CAE provides default settings for these constraints. • The default minimum element size constraint is 1% of the default boundary seed size for the part instance to which the remeshing rule is applied. • The default maximum element size constraint is 10 times the default boundary seed size for the part instance to which the remeshing rule is applied. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Constraints: Element Size Approximate maximum number of elements For a remeshing rule you can specify an approximate limit for the maximum number of elements. By using this constraint, you can control the cost of your analysis and ensure that unreasonably large meshes are not created. If the target error requires more elements than the specified limit when this constraint is defined, Abaqus/CAE will reduce the target error internally so that the generated elements approximately satisfy the specified element count. The use of this constraint may prevent an adaptivity process from achieving the error targets. By default, this constraint is not active. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Constraints: Approximate maximum number of elements Refinement and coarsening rate factors The refinement and coarsening factors that you specify define a constraint on the mesh size in terms of iteration to iteration changes to the mesh. These factors modulate the aggressivity of the sizing methods. The refinement factor controls the refinement of the mesh or the introduction of smaller elements. The coarsening factor controls the coarsening of the mesh or the introduction of larger elements. Abaqus/CAE provides default settings for these rate factors, which are designed to prevent excessive coarsening or prohibitively expensive refinement in a single remesh iteration. The refinement factor can have a significant effect on the convergence of the adaptive meshing procedure. Once you have settled on sizing method parameters that work well for your application, you may be able to achieve faster and more efficient mesh convergence by increasing the refinement factor. In cases where your adaptivity process is not converging well, however, an increased refinement factor could result in an excessive increase in elements in a remesh iteration. Abaqus/CAE Usage: Mesh module: Create Remeshing Rule: Constraints: Rate Limits Reconciling overlapping remeshing rules Abaqus/CAE imposes no restrictions on the region or the steps associated with your remeshing rules. You can apply multiple remeshing rules and, hence, sizing functions to the same region at the same time. Similarly, you can specify remeshing rules that overlap one another. When Abaqus/CAE generates the new mesh, it considers all of the remeshing rules at all of the locations and uses the smallest calculated element size to drive the meshing algorithm. 12.3 Adaptive remeshing This Abaqus functionality is not applicable to V6. 12.4 Analysis continuation after mesh replacement • “Mesh-to-mesh solution mapping,” Section 12.4.1 12.4.1 MESH-TO-MESH SOLUTION MAPPING Product: Abaqus/Standard Reference • *MAP SOLUTION Overview Mapping a solution from one mesh to another is a step in a remeshing analysis technique, where a mesh that has deformed significantly from its original configuration is replaced by a mesh of better quality and the analysis continues. The solution mapping technique: • is used when elements become so severely distorted during an analysis that they no longer provide a good discretization of the problem; • maps the solution from an old, deformed mesh to a new mesh so that the analysis can continue; and • can be used only with continuum elements. Refer to “Adaptivity techniques,” Section 12.1.1 for a high-level discussion comparing this and other Abaqus adaptivity methods. When to remesh Abaqus/Standard uses a Lagrangian formulation: the mesh is attached to the material and, thus, deforms with the material. When the strains become large in geometrically nonlinear analyses, the elements may become so severely distorted that they no longer provide a good discretization of the problem. Severe distortion may occur in rubber elasticity problems or in plastic or viscoplastic calculations, especially when modeling manufacturing processes. When severe distortion occurs, it is necessary to remesh: to create a new mesh better designed to continue the analysis and to map the old-model solution onto this mesh. You must decide when remeshing is needed. This decision can be assisted by looking at the magnitude of strains that have occurred during the phase of the analysis using a particular mesh, as discussed later. When remeshing is required, a new mesh for the deformed object must be generated using the mesh generation capability in Abaqus or an external mesh generator. The analysis is then In most cases it will be desirable to transfer the continued as a new problem using the new mesh. solution from the old mesh to the new mesh. Discontinuity in the solution Whenever the solution is mapped from another mesh, you can expect that there will be some discontinuity in the solution because of the change in the mesh and as a consequence of the solution mapping algorithm. If the discontinuity is significant, it is an indication that the meshes are too coarse or that the remeshing should have been done at an earlier stage before too much distortion occurred. The remeshing technique works well, provided that the meshes are sufficiently fine for the problem and that the remeshing is done before the elements become too distorted. Remeshing criterion The first requirement for remeshing is some indication that the mesh is becoming distorted in regions where this distortion could cause the solution to be inaccurate. One possible criterion for remeshing would be extreme element distortion in areas where high strain gradients need to be resolved accurately. Inaccuracy is less of a concern if the distorted elements have moved into an area where further changes in the strain field are uniform; the elements can represent states of constant strain accurately no matter how distorted they are. Ultimately, however, the decision to remesh is a matter of judgment. Generating a new mesh Once you have decided that the current mesh is inadequate, a new mesh that is more suitable to the current state of the problem must be generated by using the mesh generation capabilities in Abaqus or an external mesh generator. Deformed configuration plots may be useful to provide data about the current shape of the object being modeled. Usually the external surface can be defined for use in a mesh generator from the results file output at the sets of nodes that form the surfaces of the body. See “Erosion of material (sand production) in an oil wellbore,” Section 1.1.22 of the Abaqus Example Problems Manual and “Upsetting of a cylindrical billet: quasi-static analysis with mesh-to-mesh solution mapping (Abaqus/Standard) and adaptive meshing (Abaqus/Explicit),” Section 1.3.1 of the Abaqus Example Problems Manual. Remeshing a contact problem In a region of contact the new mesh must conform closely to the shape of the surface from the old analysis. This requirement is especially important for problems involving contact between two deformable bodies; if the surfaces defined by the new mesh are even slightly different from the surfaces in the old analysis, the contact algorithms may fail to converge. Specifying the solution to be interpolated onto the new mesh The simulation is continued by interpolating the solution onto the new mesh from the output databases generated with the old mesh. Specifying the time at which the solution must be read Solution transfer will occur, by default, from the latest step and increment for which solution variables are available. Alternatively, you can specify the step and increment at which the old solution will be read. Input File Usage: *MAP SOLUTION, STEP=step, INC=increment Obtaining equilibrium An initial step should be included to allow Abaqus/Standard to check for equilibrium after this interpolation has been done. By default, Abaqus/Standard resolves the stress unbalance linearly over the step . You can choose to have the stress unbalance resolved in the first increment instead. Input File Usage: Use the following option to have Abaqus/Standard resolve the stress unbalance linearly over the step: *MAP SOLUTION, UNBALANCED STRESS=RAMP Use the following option to have Abaqus/Standard resolve the stress unbalance in the first increment of the step: *MAP SOLUTION, UNBALANCED STRESS=STEP Translating and rotating the old-job mesh The mesh from the old job can be repositioned prior to performing the mapping by giving a translation and/or rotation relative to the global origin. Specify a translation by giving a translation vector. Specify a rotation by giving two points to define a rotation axis plus a right-handed angular rotation around that axis. Input File Usage: *MAP SOLUTION, STEP=step, INC=increment translation vector data rotation axis and angular rotation data Required output from the old job The files required for restart and the output database must be requested for the old job. Nodal displacement results are not output automatically from the old job; you must explicitly request output of the displacement variable U for all nodes, as described in “Node output” in “Output to the output database,” Section 4.1.3. Alternatively, you can request preselected field output and obtain node displacement output sufficient for solution mapping. In fully coupled procedures you must request nodal output of the coupled field variable to the output database . Table 12.4.1–1 Output database nodal output requirements for fully coupled procedures. Procedure Nodal output variable “Fully coupled thermal-stress analysis,” Section 6.5.3 “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 “Geostatic stress state,” Section 6.8.2 NT11 POR POR Identifying the old job Specify the name of the old job from which restart and results data will be obtained by using the oldjob parameter in the command for running Abaqus or by answering a request made by the command procedure . The files required from the old job include: the restart file (.res), the output database (.odb), the model database (.mdl), the state database (.stt), and the part (.prt) file. Solution mapping algorithm Solution mapping operates by interpolating results from nodes in the old mesh to points (either nodes or integration points) in the new mesh. The first step, therefore, involves associating solution variables with nodes in the old mesh. For nodal solution variables, such as nodal temperature or pore pressure, the association is already made. For integration point variables Abaqus obtains the solution variables at the nodes of the old mesh by extrapolating values from the integration points to the nodes of each element and then averaging these values over all similar elements abutting each node. Next, the location of each point in the new mesh is obtained with respect to the old mesh. The new mesh points include integration points in all cases and nodes in procedures that record nodal state in addition to displacements (for example, nodal temperatures in coupled temperature-displacement procedures). 1. The element (in the old mesh) in which the point lies is found, and the point’s location in that element is obtained. (This procedure assumes that all points in the new mesh lie within the bounds of the old mesh: warning messages are issued if this is not so, and the values of the variables are set to zero.) 2. The variables are then interpolated from the nodes of the old element to the points in the new model. All necessary variables are interpolated automatically in this way so that the solution can proceed with the new mesh. Solution diffusion This algorithm introduces some diffusion in the mapped solution. The effect of the diffusion scales with the solution gradient in the old mesh; hence, even for regions of the model where the mesh does not change from the old to the new model, diffusion due to the mapping can result in significantly different mapped quantities when the old-mesh solution gradient is high. You can moderate this effect by refining the old mesh in regions where solution gradients are high or by remeshing earlier. Procedures The solution mapping capability is supported for the following procedures: • “Static stress analysis,” Section 6.2.2 • “Quasi-static analysis,” Section 6.2.5 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 • “Geostatic stress state,” Section 6.8.2 Initial conditions The solution mapped from the initial analysis forms the initial conditions for the remeshed analysis. Initial conditions such as temperature for a pure stress/displacement analysis can be specified. Any other specified initial conditions will be ignored. Boundary conditions Boundary conditions are not carried over from the old mesh to the new mesh. The boundary conditions applied at the beginning of the remeshed analysis should normally be the same as those in effect at the step and increment selected from the initial analysis. Although boundary conditions can be changed, the problem may fail to converge if the structure is far from an equilibrium state. There are no restrictions on applying boundary conditions in a mapped solution analysis. Boundary conditions can be applied to all available degrees of freedom in the same way as they are applied in an analysis without a mapped solution . Loads There are no restrictions on applying loads in a mapped solution analysis. Loads can be applied in the same way as they are applied in an analysis without a mapped solution. The loads applied at the beginning of the remeshed analysis should normally be the same as those in effect at the end of the initial analysis. Although the loads can be changed, the problem may fail to converge if the structure is far from an equilibrium state. Predefined fields Temperature and field variables are mapped from the old mesh to the new mesh. If the number of field variables is changed in the remeshed analysis, the number common to both analyses will be transferred. Predefined fields can be modified in the same way as they are modified in an analysis without solution mapping . Material options Any of the mechanical constitutive models available in Abaqus can be used in a mapped solution analysis . There is no restriction on agreement between material models in the old and new analyses. The solution mapping algorithm will transfer those variables common to both models. You must ensure that the material models are compatible. Elements The solution mapping capability can be used only with continuum elements elements,” Section 28.1.1). Output There is no output specific to a mapped solution analysis. Output can be requested in the same way as in an analysis without a mapped solution. The output variables available in Abaqus are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Input file template *HEADING *NODE Data lines to define the new-model nodes occupying the space of the old model in its deformed configuration *ELEMENT Data lines to define the new-model elements occupying the space of the old model in its deformed configuration … *MAP SOLUTION, STEP=step, INC=inc translation and rotation data *STEP *STATIC (or *COUPLED TEMPERATURE-DISPLACEMENT or *GEOSTATIC or *SOILS or *VISCO) … *END STEP 13. Optimization Techniques Structural optimization: overview Optimization models 13.1 13.1 Structural optimization: overview • “Structural optimization: overview,” Section 13.1.1 13.1.1 STRUCTURAL OPTIMIZATION: OVERVIEW Structural optimization using Abaqus is an iterative process that helps you refine your designs. The result of a well-designed structural optimization is a component that is lightweight, rigid, and durable. Abaqus provides two approaches to structural optimization—topology optimization and shape optimization. Topology optimization starts with an initial model and determines an optimum design by modifying the properties of the material in selected elements, effectively removing elements from the analysis. Shape optimization further refines the model by modifying the surface of the component by moving the surface nodes to reduce local stress concentrations. Both topology and shape optimization are governed by a set of objectives and constraints. Optimization is a tool for shortening the development process by adding value to a designer’s experience and intuition with an automated procedure. To optimize your model, you need to know what to optimize. It is not sufficient to say that you want to minimize stresses or maximize eigenvalues, your statements must be more specific. For example, you might want to minimize the maximal nodal stresses experienced during two load cases. Similarly, you might want to maximize the sum of the first five eigenvalues. The goal of an optimization is called the objective function. In addition, you can enforce certain values during the optimization. For example, you can specify that the displacement of a given node must not exceed a certain value. An enforced value is called a constraint. You use Abaqus/CAE to create the model to be optimized and to define, configure, and execute the structural optimization. For more information, see Chapter 18, “The Optimization module,” of the Abaqus/CAE User’s Manual. Terminology Structural optimization introduces its own terminology. The following terms are used throughout the Abaqus documentation and the Abaqus/CAE user interface: • Design area: The design area is the region of your model that the structural optimization modifies. The design area can be the whole model, or it can be a subset of the model containing only selected regions. Given the prescribed conditions (such as boundary conditions, loads, and manufacturing constraints), • a topology optimization process removes and adds material from elements in the design area while it attempts to reach an optimal design, and • a shape optimization modifies the surface of the design area by moving surface nodes. • Design variables: For an optimization problem, the design variables represent the parameters to be changed during the optimization. For a topology optimization, the densities of the elements in the design area are the design variables. The Abaqus Topology Optimization Module changes the density during each iteration In effect, the of the optimization and couples the stiffness of each element with the density. optimization removes elements from your model by giving them a mass and stiffness that is small enough to ensure they no longer participate in the overall response of the structure. The model with the revised material properties is then analyzed by Abaqus. For a shape optimization, the displacements of the surface nodes in the design area are the design variables. During the optimization, the Abaqus Topology Optimization Module either moves a node outward (growth) or inward (shrinkage) or leaves the position unchanged (neutral). Restrictions influence the amount a surface node can move and the direction in which it can move. The optimization directly modifies only the position of the corner nodes of elements; the Abaqus Topology Optimization Module interpolates the displacement of midside nodes from the movement of the corner nodes. • Design cycle: Optimization is an iterative design process that updates the design variables, executes an Abaqus analysis of the modified model, and reviews the results to determine if an optimized solution has been reached. Each optimization iteration is called a design cycle. • Optimization task: An optimization task contains the definition of your optimization, such as the design responses, objectives, constraints, and geometric restrictions. To run an optimization, you execute an optimization process. An optimization process refers to an optimization task. • Design responses: The inputs to the optimization are called the design responses. Design responses can be read directly from the Abaqus output database (.odb) file; for example, the Abaqus Topology Optimization Module can read data from the output database file and calculate the design responses from your model; for example, its weight, center of mass, or relative displacements. stress, eigenfrequencies, and displacements. Alternatively, stiffness, A design response is associated with a region of your model; however, it consists of a single In scalar value, such as the maximum stress within a region or the total volume of the model. addition, a design response can be associated with a particular step or load case. • Objective functions: Objective functions define the objective of the optimization. An objective function is a single scalar value extracted from a design response, such as the maximum displacement or the maximum stress. An objective function can be formulated from multiple If you specify that the objective functions minimize or maximize the design design responses. responses, the Abaqus Topology Optimization Module calculates the objective function by adding each of the values determined from the design responses. In addition, if you have multiple objective functions, you can use a weighting factor to scale their influence on the optimization. • Constraints: Constraints are also a single scalar value extracted from a design response; however, a constraint cannot be derived from a combination of design responses. Constraints restrict the value of a design response; for example, you can specify that the volume must be reduced by 45% or the absolute displacement in a region must not exceed 1 mm. You can also apply manufacturing and geometric constraints that are independent of the optimization; for example, a structure must be able to be cast or stamped or the diameter of a bearing surface cannot be changed. • Stop conditions: A global stop condition defines the maximum number of iterations an optimization can perform. A local stop condition specifies that the optimization should end when a local minimum (or maximum) has been reached. Structural optimization with Abaqus/CAE The following steps are required to incorporate structural optimization into your Abaqus/CAE model: • You create an Abaqus model that can be optimized. For example, the design area must include only supported elements and materials. See “Creating Abaqus optimization models,” Section 13.2.3. • You create an optimization task. See “Creating and configuring an optimization task,” Section 18.6 of the Abaqus/CAE User’s Manual. • You create design responses. See “Design responses,” Section 13.2.1. • You use the design responses to create objective functions and constraints. See “Objectives and constraints,” Section 13.2.2. • You create an optimization process and submit it for analysis. See “What is an optimization process?,” Section 19.5.1 of the Abaqus/CAE User’s Manual. Based on the definition of the optimization task and the optimization process, the Abaqus Topology Optimization Module iteratively: • prepares the design variables (element densities or surface node positions) and updates the Abaqus finite element model, and • executes an Abaqus/Standard analysis. These iterations or design cycles continue until either: • the maximum number of design cycles is reached, or • the specified stop conditions are reached. Figure 13.1.1–1 shows the interaction of Abaqus and the optimization process. Topology optimization Topology optimization starts with an initial design (the original design area), which also contains any prescribed conditions (such as boundary conditions and loads). The optimization process determines a new material distribution by changing the density and the stiffness of the elements in the initial design while continuing to satisfy the optimization constraints, such as the minimum volume or the maximum displacement of a region. Figure 13.1.1–2 show the progression of a topology optimization of an automotive control arm during 17 design cycles. The objective function in the optimization is trying to minimize the maximum strain energy calculated from all the elements in the arm, in effect maximizing the structural stiffness of the arm. The constraint is forcing the optimization to reduce the volume by 57% from the initial value. During the optimization the density and the stiffness of the elements in the center of the arm are reduced so that the elements are, in effect, “removed” from the analysis. However, the elements are still present, and they could play a role in the analysis if their density and stiffness increase as the optimization continues. A geometry restriction forces the optimization to create a model that could be cast and removed from a mold—the Abaqus Topology Optimization Module cannot create voids and undercuts. Abaqus can apply the following objectives to a topology optimization process: • strain energy (a measure of structural stiffness), • eigenfrequencies, • internal and reaction forces, Create model Create optimization task User actions Automated optimization actions Setup optimization Create design responses Create objective functions Create constraints Create optimization process Submit optimization process Perform optimization Prepare design variables and update finite element model Monitor optimization progress Design cycle iteration Abaqus analysis Monitor job progress No Optimization complete? Yes Optimization process is finished Review results Figure 13.1.1–1 User actions and automated Abaqus/CAE actions in the optimization process. Start 100% volume After 5 cycles 85% volume After 10 cycles 77% volume After 15 cycles 61% volume After 17 cycles 57% volume Figure 13.1.1–2 The progression of a topology optimization. • weight and volume, • center of gravity, and • moment of inertia. You can apply the same variables as constraints to a topology optimization process. In addition, you can apply a number of manufacturing constraints that ensure the proposed design can be created using standard production processes, such as casting and stamping. You can also freeze selected regions and apply member size, symmetry, and coupling constraints. An example of using topology optimization is provided in “Topology optimization of an automotive control arm,” Section 11.1.1 of the Abaqus Example Problems Manual. The example includes a Python script that you can run from Abaqus/CAE to create the model and configure the optimization. General versus condition-based topology optimization Topology optimization supports two algorithms—the general algorithm, which is more flexible and can be applied to most problems, and the condition-based algorithm, which is more efficient but has limited capabilities. By default, the Abaqus Topology Optimization Module uses the general algorithm; however, you can choose which algorithm to use when you create the optimization task. Each algorithm has a different approach for determining the optimized solution. Algorithms General topology optimization uses an algorithm that adjusts the density and stiffness of the design variables while trying to satisfy the objective function and the constraints. The general algorithm is partly described in Bendsøe and Sigmund (2003). In contrast, condition-based topology optimization uses a more efficient algorithm that uses the strain energy and the stresses at the nodes as input data and does not need to calculate the local stiffness of the design variables. The condition-based algorithm was developed at the University of Karlsruhe, Germany and is described in Bakhtiary (1996). Elements with intermediate densities The general algorithm generates intermediate elements in the final design (their relative density is between zero and one). In contrast, the condition-based optimization algorithm generates elements in the final design that are either void (their relative density is very close to zero) or solid (their relative density is equal to one). Number of optimization design cycles The number of design cycles used by the general optimization algorithm is unknown before the optimization starts, but normally the number of design cycles is between 30 and 45. The condition-based optimization algorithm is more efficient and searches for a solution until it reaches the maximum number of optimization design cycles (15 by default). Analysis types The general algorithm supports the responses of linear and nonlinear static and linear eigenfrequency finite element analyses. Both algorithms support geometrical nonlinearities and contact, and many nonlinear materials are also supported. Furthermore, prescribed displacements are allowed in the Abaqus model for static topology optimization. However, prescribed displacements are not allowed for modal analysis. You can use topology optimization on a structure that uses a composite material; however, the individual laminates of a composite material cannot be modified using topology optimization. For example, you cannot change the orientation of the fibers. Objective functions and constraints The general topology optimization algorithm can use one objective function and several constraints, where the constraints are all inequality constraints. A variety of design responses can be used to define the objective and the constraints, such as strain energy, displacements and rotations, reaction and internal forces, eigenfrequencies, and material volume and weight. The condition-based topology optimization algorithm is more efficient; however, it is less flexible and supports only strain energy (a measure of stiffness) as the objective function and the material volume as an equality constraint. Shape optimization Shape optimization uses an algorithm that is similar to the algorithm used by condition-based topology optimization. You use shape optimization at the end of the design process when the general layout of a component is fixed, and only minor changes are allowed by repositioning surface nodes in selected regions. A shape optimization starts with a finite element model that needs minor improvement or with the finite element model generated by a topology optimization. Typically, the objective of a shape optimization is to minimize stress concentrations using the results of a stress analysis to modify the surface geometry of a component until the required stress level is reached. Shape optimization tries to position the surface nodes of the selected region until the stress across the region is constant (stress homogenization). Figure 13.1.1–3 shows a region at the base of a connecting rod where the surface nodes have been moved by shape optimization to reduce the effect of a stress concentration. Original model After shape optimization Figure 13.1.1–3 The effect of shape optimization. You can apply the following objectives to a shape optimization process: • stresses and contact stresses, • selected natural frequencies, and • elastic, plastic, and total strain and strain energy density. You can apply only a volume constraint to a shape optimization. In addition, you can apply a number of manufacturing geometric restrictions that ensure the proposed design can continue to be produced using casting or stamping processes. You can also freeze selected regions and apply member size, symmetry, and coupling restrictions. An example of using shape optimization is provided in “Shape optimization of a connecting rod,” Section 11.2.1 of the Abaqus Example Problems Manual. The example includes a Python script that you can run from Abaqus/CAE to create the model and configure the optimization. Applying mesh smoothing to a shape optimization During a shape optimization, the Abaqus Topology Optimization Module modifies the surface of your model. If the Abaqus Topology Optimization Module modifies only the surface nodes without adjusting the inner nodes, the layer of surface elements becomes distorted. Therefore, the results of the Abaqus analysis are no longer reliable, and the quality of the optimization suffers. To maintain the quality of the surface elements, the Abaqus Topology Optimization Module can apply mesh smoothing to selected regions, which adjusts the position of the inner nodes in relation to the movement of the surface nodes. You must have a good quality finite element mesh before you start the shape optimization, especially in areas where you expect the shape to change. The Abaqus Topology Optimization Module can apply mesh smoothing to the standard continuum elements, such as triangular, quadrilateral, and tetrahedral elements. Other element types are ignored during the mesh smoothing. You can specify the relative quality of the smoothed mesh, and you can specify the range of angles (quadrilateral and triangular elements) or the range of aspect ratios (tetrahedral elements) that define an element that is considered good quality. Elements that are considered poor are given a quality rating. The poorer an element is rated, the greater the consideration it will be given in improving the element quality. Mesh smoothing can be computationally expensive. The mesh smoothing algorithm is element- based; and computing time increases in regions with many elements with limited degrees of freedom, such as regions with small tetrahedral elements. You should apply mesh smoothing only to regions where you expect the surface nodes to move—regions that will benefit from mesh smoothing. The nodes in the regions to which you apply mesh smoothing must be free to move. For example, you should not apply mesh smoothing to fixed nodes or to frozen regions. You can apply limits to the result of mesh smoothing by applying minimum and maximum growth restrictions to the selected region. See “Creating a growth restriction” in “Creating a geometric restriction in a shape optimization,” Section 18.10.3 of the Abaqus/CAE User’s Manual, for more information. Mesh smoothing can be applied to regions that are included in the design region and to regions that are outside the design region. In particular, you can prevent element distortion by applying mesh smoothing to the region of transition between the design region and the rest of your model. However, the design region must be contained within the region to which you apply mesh smoothing. Free surface nodes are defined as the nodes that lie outside the design area and are not included in a geometric restriction. By default, the Abaqus Topology Optimization Module fixes all degrees of freedom of all of the free surface nodes, and they are not modified during the mesh smoothing operation. Alternatively, you can choose to allow the free surface nodes to move along with a specified number of layers of nodes adjacent to the nodes in the design area. (A “layer” of nodes is created from only corner nodes; midside nodes are not taken into consideration.) You should allow free surface nodes to move in regions that are adjacent to the design area to create a smooth transition between optimized and non-optimized regions. However, in some cases you will want free surface nodes to remain fixed; for example, on a planar face that does not play a role in your optimized model and must remain planar. By default, a constrained Laplacian mesh smoothing algorithm is used. Alternatively, if you have a relatively small model (less than 1000 nodes in the mesh smooth area), you can select a local gradient mesh smoothing algorithm. In each iteration the local gradient mesh smoothing algorithm identifies the elements with the worst element quality and improves them by displacing the nodes. Local gradient mesh smoothing usually generates elements having the optimal shape, where the optimal is defined as the ratio of the element volume (area for shell elements) to the corresponding power of its diameter. For larger models the local gradient mesh smoothing algorithm tends to stop before the optimal mesh quality is reached because the computation time becomes excessive. When the mesh smoothing ends prematurely, only the elements with the worst element quality will be smoothed. 13.2 Optimization models • “Design responses,” Section 13.2.1 • “Objectives and constraints,” Section 13.2.2 • “Creating Abaqus optimization models,” Section 13.2.3 13.2.1 DESIGN RESPONSES Product: Abaqus/CAE References • “Structural optimization: overview,” Section 13.1.1 • “Configuring design responses,” Section 18.7 of the Abaqus/CAE User’s Manual Overview A design response: • is a single scalar value, such as the volume of your structure; • is calculated by the Abaqus Topology Optimization Module by reading results and model data from the output database file; • can be referred to from objective functions and constraints (for example, you can create an objective function that tries to minimize the displacement at a node or a constraint that forces the weight of the structure to be reduced by at least 50%); and • is available only for certain analysis procedures (for example, you must perform an tries to maximize the eigenvalue extraction analysis if you select a design response that lowest eigenfrequencies). Design response operators You must specify the operation that the Abaqus Topology Optimization Module will use to arrive at a single scalar value for the design response, although some restrictions apply. For example, a volume design response can only use the sum of the volume within the design area. A design response that calculates the von Mises stress must use the maximum value of the stress within a region of the model. (None of the operators are relevant when the Abaqus Topology Optimization Module calculates a dynamic frequency design response.) The following design response operators are provided by the Abaqus Topology Optimization Module: • Minimum or maximum: The minimum or maximum value within the selected region. The Abaqus Topology Optimization Module allows only the maximum operator for stress, contact stress, and strain design responses. • Sum: The sum of all the values within the selected area. The Abaqus Topology Optimization Module allows only the sum operator for volume, weight, moment of inertia, and gravity design responses. Design responses for condition-based topology optimization The Abaqus Topology Optimization Module provides strain energy and volume design responses for condition-based topology optimization. Strain energy for linear models, where The compliance of a structure is a measure of its overall flexibility or stiffness and is defined as the sum of the strain energy of all the elements, is the global stiffness matrix. Compliance is the reciprocal of stiffness, and minimizing the compliance is equivalent to maximizing the global stiffness. If a load case is driven by forces or pressures, you should choose to minimize the strain energy to maximize the global stiffness. However, if a load case is driven by a thermal field, strain energy decreases when the optimization modifies the structure to make it softer. As a result, you should always choose to maximize the strain energy because attempting to minimize the strain energy can result in a stiff structure. In addition, you should always choose to maximize the strain energy if prescribed displacements are applied to your model. is the displacement vector and Topology optimization considers the total strain energy for all of the elements; therefore, if you choose strain energy as an objective function, you must apply the objective to the entire model. You cannot use strain energy as a constraint in your optimization. Abaqus/CAE Usage: Optimization module: Task→condition-based topology task, Design Response→Create: Single-term, Variable Strain energy Volume The volume is defined as the sum of the volume of the elements in the design area, is the element volume. During a topology optimization, the elements are scaled with the current relative density defined in your Abaqus model. For most optimization problems, you must apply a volume constraint. For example, if you are trying to minimize the strain energy (maximize the stiffness) and do not apply a volume constraint, the Abaqus Topology Optimization Module simply fills the entire design area with material. , where Abaqus/CAE Usage: Optimization module: Task→condition-based topology task, Design Response→Create: Single-term, Variable: Volume Design responses for general topology optimization The Abaqus Topology Optimization Module provides center of gravity, displacement, rotation, eigenfrequency, moment of inertia, internal and reaction forces and moments, strain energy, volume, and weight design responses for general topology optimization. Center of gravity You can use the center of gravity of a selected region as a design response in an optimization. You can choose the center of gravity in the three principal directions: When the Abaqus Topology Optimization Module calculates the center of gravity, the elements are scaled with the current relative density defined in your Abaqus model. For example, you might want to constrain the center of gravity in the Y-direction so that it remains within a minimum and maximum range during the optimization. The design response can consider the center of gravity of the whole model or a region of the model. If you select a local coordinate system, the Abaqus Topology Optimization Module uses both the direction of the axes and the position of the origin to recalculate the center of gravity. The Abaqus Topology Optimization Module applies the global coordinate system if you do not select a local coordinate system. When the Abaqus Topology Optimization Module calculates the center of gravity, it treats shell and membrane regions as three-dimensional regions by applying the thickness of the region. The Abaqus Topology Optimization Module calculates the center of gravity using only the element types that are supported by topology optimization. As a result, the center of gravity calculated by the Abaqus Topology Optimization Module might not be the same as the center of gravity calculated by Abaqus/Standard or Abaqus/Explicit; for example, if your model contains wire regions. Abaqus/CAE Usage: Optimization module: Task→general topology task, Design Response→Create: Single-term, Variable: Center of gravity Displacement and rotation In most optimization problems you will use displacement and/or rotation to define your objective function or constraints. For example, the maximum displacement of a vertex could be either an objective or a constraint of an optimization. The performance of the optimization is improved if you apply displacements and rotations to only vertices or to small regions. In addition, performance is improved if you assign regions that are used to define displacements or reactions as frozen regions (the Abaqus Topology Optimization Module will not remove elements from frozen regions during the optimization). Table 13.2.1–1 lists the available displacement and rotation variables. Abaqus/CAE Usage: Optimization module: Task→general topology task, Design Response→Create: Single-term, Variable: Displacement Modal eigenfrequency analysis Modal eigenvalues are the simplest dynamic responses in structural analysis. Typical uses of data from an eigenfrequency analysis during a topology optimization include the following: Table 13.2.1–1 Displacement and rotation variables for a general topology optimization. Displacement Rotation i-direction Absolute Absolute in i-direction • maximize the lowest eigenfrequencies, • maximize a selected eigenfrequency, • constrain an eigenfrequency to be higher or lower than a given value, • maximize or minimize an eigenfrequency at a certain mode, and • perform a bandgap optimization that force modes away from a certain frequency. The Abaqus Topology Optimization Module supports two approaches for evaluating the eigenfrequencies: • single eigenfrequencies from modal analysis and • the Kreisselmaier-Steinhauser formulation. The Kreisselmaier-Steinhauser formulation is the more efficient of the two approaches and should be used whenever possible. The only advantage of evaluating single eigenfrequencies is that you can use the sum of the eigenfrequencies as a constraint in a general topology optimization. You cannot use the sum of the eigenfrequencies from the Kreisselmaier-Steinhauser formulation as a constraint in a general topology optimization. When you are trying to maximize the lowest eigenfrequency, it is recommended that you consider not only the first eigenfrequency but also at least the next two highest natural frequencies. During the optimization, the various natural frequencies are weighted by their distance from the lowest natural frequency—the closer a natural frequency approaches the first natural frequency during the optimization, the more it is weighted. You should use the Kreisselmaier-Steinhauser eigenvalue formulation if you are trying to maximize the lowest eigenfrequency or, in particular, if you are trying to maximize more than one of the lowest eigenfrequencies. You do not need to use mode tracking if you are using the Kreisselmaier-Steinhauser formulation to maximize the lowest eigenfrequency, but you should use mode tracking for the higher modes because the modes might switch. For example, while the model is being optimized, the frequency of the first mode is maximized and the second eigenmode can become the mode with the lowest frequency. Abaqus/CAE Usage: Optimization module: Task→general topology task, Design Response→Create: Single-term, Variable: Eigenfrequency from modal analysis or Eigenfrequency calculated with Kreisselmaier-Steinhauser formula Moment of inertia You can use a moment of inertia design response in an optimization to minimize the rotational inertia about a selected axis. You can use the sum of the moment of inertia of the whole model or a region of the model as an objective function or a constraint in a general topology optimization. You can choose the moment of inertia in the three principal directions or the three principal planes: If you select a local coordinate system, the Abaqus Topology Optimization Module uses the direction of the axes to recalculate the center of gravity. The Abaqus Topology Optimization Module applies the global coordinate system if you do not select a local coordinate system. When the Abaqus Topology Optimization Module calculates the moment of inertia, it treats shell and membrane regions as three-dimensional regions by applying the thickness of the region. The Abaqus Topology Optimization Module calculates the moment of inertia using only the element types that are supported by topology optimization. As a result, the moment of inertia calculated by the Abaqus Topology Optimization Module might not be the same as the moment of inertia calculated by Abaqus/Standard or Abaqus/Explicit; for example, if your model contains wire regions. The moment of inertia with respect to any two orthogonal axes is zero if you have selected either of the axes to be an axis of symmetry. Abaqus/CAE Usage: Optimization module: Task→general topology task, Design Response→Create: Single-term, Variable: Moment of inertia Internal forces and moments You can use nodal internal forces and moments of the whole model or a region of the model as an objective function or a constraint in a general topology optimization. Table 13.2.1–2 lists the available nodal internal force and moment variables. Table 13.2.1–2 Nodal internal force and moment variables for a general topology optimization. Nodal internal force Nodal internal moment i-direction Absolute Absolute in i-direction You cannot use a reference coordinate system with absolute internal force or with absolute internal moment. Your structure must have stiffness in the direction of the force used in the optimization; otherwise, the internal force will be zero in this direction. Abaqus/CAE Usage: Optimization module: Task→general topology task, Design Response→Create: Single-term, Variable: Internal force or Internal moment Reaction forces and moments Nodal reaction forces and moments can be used as a design response only in general topology optimization. As with displacements, the performance of the optimization is improved if you apply reaction forces or moments to only vertices or to small regions and assign those regions as frozen regions (the Abaqus Topology Optimization Module will not remove elements during the optimization). Table 13.2.1–3 lists the available nodal reaction force and moment variables. Table 13.2.1–3 Nodal reaction force and moment variables for a general topology optimization. Nodal reaction force Nodal reaction moment i-direction Absolute Absolute in i-direction You cannot use a reference coordinate system with an absolute reaction force or with an absolute reaction moment. Your structure must have stiffness in the direction of the force used in the optimization; otherwise, the reaction force will be zero in this direction. Abaqus/CAE Usage: Optimization module: Task→general topology task, Design Response→Create: Single-term, Variable: Reaction force or Reaction moment Strain energy The compliance of a structure is a measure of its overall stiffness and is defined as the sum of the strain energy of all the elements, is the global stiffness matrix. Compliance is the reciprocal of stiffness, and minimizing the compliance is equivalent to maximizing the global stiffness. If a load case is driven by a thermal field, strain energy decreases when the structure is made softer. As a result, attempting to minimize strain energy can result in a stiff structure. In addition, you should always choose to maximize the strain energy if prescribed displacements are applied to your model. is the displacement vector and for linear models, where Topology optimization considers the total strain energy for all of the elements; therefore, if you choose strain energy as an objective function, you must apply the objective to the entire model. Abaqus/CAE Usage: Optimization module: Task→general topology task, Design Response→Create: Single-term, Variable: Strain energy Volume The volume is defined as the sum of the volume of all the elements in the design area, , where is the element volume. For most optimization problems, you must apply a volume constraint. For example, if you are trying to minimize the strain energy (maximize the stiffness) and do not apply a volume constraint, the Abaqus Topology Optimization Module simply fills the design area with material. Abaqus/CAE Usage: Optimization module: Task→general topology task, Design Response→Create: Single-term, Variable: Volume Weight The weight is defined as the sum of the weight of all the elements in the design area, is the element weight. The Abaqus Topology Optimization Module scales elements using the current relative density. For most optimization problems, you must apply either a volume or a weight constraint. Using weight instead of volume allows you to constrain the optimized model to a specified physical weight. The Abaqus Topology Optimization Module uses only supported element types when calculating the weight. , where Abaqus/CAE Usage: Optimization module: Task→general topology task, Design Response→Create: Single-term, Variable: Weight Design responses for shape optimization The Abaqus Topology Optimization Module provides eigenfrequency, stress, contact stress, strain, nodal strain energy density, and volume design responses for shape optimization. Only a volume design response can be used to define a constraint; all other design responses are used to define objective functions. Eigenfrequency from the Kreisselmaier-Steinhauser formulation You should use the Kreisselmaier-Steinhauser formulation of the eigenvalues as an objective function in a shape optimization if you are trying to maximize the first eigenfrequency or, in particular, if you are trying to maximize more than one of the first eigenfrequencies. You do not need to use mode tracking if you are using the Kreisselmaier-Steinhauser formulation of the eigenvalues. Abaqus/CAE Usage: Optimization module: Task→shape task, Design Response→Create: Single-term, Variable: Eigenfrequency calculated with Kreisselmaier-Steinhauser formula Stress and contact stress Equivalent stresses are the most commonly used objective function of a shape optimization. All of the stress values that are calculated by the Abaqus Topology Optimization Module, whether nodal or from Gauss points or elements, are interpolated to the nodes. For example, you can try to optimize your model with an objective function that tries to minimize the maximum von Mises stresses in a region with stress concentrations or tries to minimize contact pressure in a region with contact. The Abaqus Topology Optimization Module considers only the maximum value of an equivalent stress within a region. The Abaqus Topology Optimization Module issues warnings for nodes that do not have the appropriate stress values. For example, if you select an objective response of contact stress, the Abaqus Topology Optimization Module issues warnings about nodes of elements that are not in contact. If your Abaqus model contains multiple load cases, the design response is evaluated by summing the stress values from each load case. You can choose from the following equivalent stresses: • von Mises • Maximum principal and absolute maximum principal • Minimum principal and absolute minimum principal • Second principal • Beltrami • Drucker Prager • Galilei • Kuhn • Mariotte • Sandel • Sauter • Tresca You can choose from the following equivalent contact stresses: • Contact stress pressure • Total shear contact stress • Shear contact stress in the 1-direction • Shear contact stress in the 2-direction • Total contact stress You can create a design response that uses stress or contact stress only in shape optimization, and it can be used only as an objective function. Abaqus/CAE Usage: Optimization module: Task→shape task, Design Response→Create: Single-term, Variable: Stress or Contact stress Strain If your model is undergoing large deformations, a measure of the stress is not always a good indicator of the model’s response. For example, a structure undergoing plastic deformation will, for an ideal plastic material, experience a large constant stress over the plastic area. In these circumstances a measure of the strain is a more reliable indicator of the model’s response. You can choose from the following equivalent strains: • Elastic • Plastic • Total (the sum of the elastic and plastic) You can create a design response that uses strain only in shape optimization, and it can be used only as an objective function. Abaqus/CAE Usage: Optimization module: Task→shape task, Design Response→Create: Single-term, Variable: Strain Nodal strain energy density The nodal strain energy density, representation of failure than stresses in nonlinear materials. , is a local point-wise strain energy that can provide a better Abaqus/CAE Usage: Optimization module: Task→shape task, Design Response→Create: Single-term, Variable: Strain energy density Volume Volume is the only constraint allowed for a shape optimization. The volume is defined as the sum of the volume of all the elements in the design area, is the element volume. , where For most optimization problems, you must apply a volume constraint to a region of your model. For example, if you are trying to minimize the strain energy (maximize the stiffness) and do not apply a volume constraint, Abaqus simply fills the design area with material. Abaqus/CAE Usage: Optimization module: Task→shape task, Design Response→Create: Single-term, Variable: Volume Operating on design responses You can define a design response that is a combination of the single values generated by multiple design responses; for example, you can add values or find the maximum of several values. You can also define a design response that is the result of an operation on another design response; for example, the difference between the value of the design response at different nodes. For example, you can create two design responses that correspond to the displacement in the 1- direction of two selected vertices. Alternatively, you can create a design response that is the difference between the displacement in the 1-direction of two selected vertices. You can then define a constraint that forces the design response to be close to zero. In effect, the constraint forces the two selected vertices to move together in the 1-direction. Abaqus/CAE Usage: Optimization module: Design Response→Create: Combined-term Additional references • Bakhtiary, N., P. Allinger, M. Friedrich, F. Mulfinger, J. Sauter, O. Müller, and J. Puchinger, “A New Approach for Size, Shape and Topology Optimization,” SAE International Congress and Exposition, Detroit, Michigan, USA, February 26–29, 1996. • Bendsøe, M. P., E. Lund, N. Ohloff, and O. Sigmund, “Topology Optimization - Broadening the Areas of Application,” Control and Cybernetics, vol. 34, pp. 7–35, 2005. • Bendsøe, M. P., and O. Sigmund, Topology Optimization: Theory, Methods and Applications, Springer-Verlag, Berlin Heidelberg New York, 2003. • Bendsøe, M. P., and O. Sigmund, “Material Interpolations in Topology Optimization,” Archive of Applied Mechanics, vol. 69, pp. 635–654, 1999. • Clausen, P. M., and C. B. W. Pedersen, Non-Parametric Large Scale Structural Optimization, ECCM 2006 III European Conference on Computational Mechanics, Lisbon, Portugal, June 5–9, 2006. • Cook, R. D., D. S. Malkus, and M. E. Plesha, Concepts and Applications of Finite Element Analysis, John Wiley & Sons Inc., 1989. • Hansen, L. V., “Topology Optimization of Free Vibrations of Fiber Laser Packages,” Structural and Multidisciplinary Optimization, vol. 29(5), pp. 341–348, 2005. • Olhoff, N., and J. Du, Topology Optimization of Vibrating Bi-Material Plate Structures with Respect to Sound Radiation, IUTUAM Symposium on Topological Design Optimization of Structures, Machines and Materials: Status and Perspectives, M. P. Bendsøe, N. Olhoff, and O. Sigmund, eds., pp. 147–156, Springer, 2006. • Pedersen, C. B. W., and P. Allinger, Industrial Implementation and Applications of Topology Optimization and Future Needs, IUTUAM Symposium on Topological Design Optimization of Structures, Machines and Materials: Status and Perspectives, M. P. Bendsøe, N. Olhoff, and O. Sigmund, eds., pp. 147–156, Springer, 2006. • Sigmund, O., and J. S. Jensen, “Systematic Design of Phononic Band Gap Materials and Structures by Topology Optimization,” Philosophical Transactions of the Royal Society: Mathematical, Physical and Engineering Sciences, vol. 361, pp. 1001–1019, 2003. • Stolpe, M., and K. Svanberg, “An Alternative Interpolation Scheme for Minimum Compliance Optimization,” Structural and Multidisciplinary Optimization, vol. 22, pp. 116–124, 2001. • Svanberg, K., “The Method of Moving Asymptotes—A New Method for Structural Optimization,” International Journal for Numerical Methods in Engineering, vol. 24, pp. 359–373, 1987. 13.2.2 OBJECTIVES AND CONSTRAINTS Product: Abaqus/CAE References • “Structural optimization: overview,” Section 13.1.1 • “Creating objective functions,” Section 18.8 of the Abaqus/CAE User’s Manual • “Creating constraints,” Section 18.9 of the Abaqus/CAE User’s Manual • “Configuring geometric restrictions,” Section 18.10 of the Abaqus/CAE User’s Manual • “Creating local stop conditions,” Section 18.11 of the Abaqus/CAE User’s Manual Overview For an optimization problem: • an objective function defines the objective of the optimization; • a constraint imposes limitations on the optimization and defines a feasible design; • geometric restrictions impose limitations on the topology or shape of the structure that can be generated by the optimization; and • stop conditions define when an optimization task is considered complete. Objective functions Objective functions define the objective of the optimization. An objective function is a single scalar value that is formulated from a set of design responses. For example, if the design responses are defined from the strain energy of the nodes in a region, the objective function could minimize the sum of the design responses; i.e., minimize the sum of the strain energy, in effect maximizing the stiffness of the region. An optimization problem can be stated as: where is the objective function that depends on the state variables, , and the design variables, . The formula for the objective function that tries to minimize design responses can be stated as: where each design response, objective function that tries to maximize , is given a weight, , and a reference value, . The formula for the design responses can be stated as: For a topology optimization the default is 1.0. for a shape optimization the default reference The default weighting factor reference value is calculated by the value is 0.0; Abaqus Topology Optimization Module. For the most common optimization problems you do not need to change the default values of the weighting factor and the reference value. However, in some cases you may have to change the weighting factor to balance the effect of an objective function that is dominating the optimization. You should be aware that changing the weighting factor can have a significant impact on the final design. In addition, a design response that is dominant at the start of the optimization may have less effect as the Abaqus Topology Optimization Module modifies your model. An objective function that tries to minimize the maximum design response is an important optimization formulation. During each design cycle the Abaqus Topology Optimization Module first determines which of the set of weighted design responses has the maximum value and then tries to minimize that design response. In many problems, minimizing the maximum design response provides a satisfactory solution because it reduces the maximum of a number of design responses. For example, if your design responses are defined from the stress in multiple regions of your model, minimizing the maximum design response attempts to minimize the stress in the region that is exhibiting the maximum stress. The formula can be stated as: The design responses provided with the Abaqus Topology Optimization Module are listed in “Design responses,” Section 13.2.1. Defining the target of an objective function The target of an objective function can be minimized or maximized. Alternatively, the target of an objective function can be set to minimize the maximum, such that the design response targets the maximum value, and the objective attempts to minimize that maximum value. In all cases, the weighting and reference values of the design responses are accounted for. Abaqus/CAE Usage: Optimization module: Objective Function→Create: Target Constraints As outlined in the previous section, an optimization problem can be stated as: where Constraints, design variables: is the objective function that depends on the state variables, , can be applied to the optimization problem, and constraints, , and the design variables, . , can be applied to the where , where and . In addition, is an expression for the layout of the design variables, such as manufacturability, is the design response that is constrained by the value and is the constraint on the design variables. The Abaqus Topology Optimization Module can arrive at a solution that optimizes the objective function; however, if the constraints are not satisfied, the result of the optimization may not be a feasible design. A constraint is based on a design response and, similar to a design response, is formulated from a single scalar value. Most optimizations have constraints that prevent the optimization from arriving at a trivial solution. For example, if you are trying to maximize the stiffness of a structure, the Abaqus Topology Optimization Module will simply fill the entire design area if you do not apply any constraints. However, if you apply a weight constraint that limits the weight to 50% of its initial value, the Abaqus Topology Optimization Module is forced to seek an optimum solution that both optimizes the stiffness objective and satisfies the weight constraint. You can apply only volume constraints to both topology optimization and to shape optimization; you cannot use volume as an objective function. You cannot apply multiple constraints of the same type, such as volume, to the whole model or to a single region. Abaqus/CAE Usage: Optimization module: Constraint→Create Applying constraints to regions You can apply different constraints to different regions of your model. In addition, those regions can have different material properties or a material property can vary within a region. When the Abaqus Topology Optimization Module calculates the design response, it considers varying material properties within the region. You cannot apply multiple volume constraints to the whole model or to a single region. Geometric restrictions Geometric restrictions are constraints that are applied directly to the design variables. Geometric restrictions allow you to model design limitations and manufacturing limitations. Defining a frozen area You can specify that a region within the optimization region is excluded from the optimization by freezing the region. For example, you could exclude a circular shaft that forms a bearing surface or a boss that is used to attach the structure to a rigid surface. You must freeze regions that are used to apply prescribed conditions. To simplify this operation, you can request that the Abaqus Topology Optimization Module automatically freeze regions that are used to apply prescribed conditions and loads when you create an optimization process. Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Frozen area Specifying minimum and maximum member size In most cases you should try to avoid the generation of thin trusses in the structure by defining a minimum member size. However, the Abaqus Topology Optimization Module cannot ensure that the optimized structure will not contain regions with a diameter that is smaller than the minimum member size. The minimum member size must be larger than the average element edge length. The maximum member size must be larger than twice the element length; otherwise, the optimization algorithm may experience issues with element connectivity. A coarse mesh and a fine mesh lead to an optimization with the topological equivalent result if you specify the same minimum member size for both cases. The Abaqus Topology Optimization Module will not generate a thin region where prescribed conditions have been applied to the structure. Removing material from these regions may result in the structure collapsing. If your structure will be cast, you may want to avoid the generation of overly thick parts by specifying a region with a maximum member size. The optimization process will avoid creating a thick region by generating several thinner regions. You do not need to specify both a maximum and a minimum member size. The Abaqus Topology Optimization Module assumes the value that you enter for the maximum member size also applies to the minimum member size and will generate trusses of the specified size. The combination of a maximum member size constraint with a restraint that imposes a pull direction, such as a moldable or stampable manufacturing constraint, is allowed only for a general topology optimization. (The “pull direction” is the direction in which the two halves of a mold separate or the direction in which a stamping tool moves.) Computational time increases significantly when you specify regions with a minimum or maximum member size. Therefore, you should apply the member size restrictions only to regions where thin or thick members must be avoided. You should run an optimization without member size restrictions to identify such regions. Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Member size Applying manufacturing restrictions The topology optimization process always creates a structural layout that satisfies the objective function and the constraints; however, the design may be impossible to create using standard manufacturing techniques, such as casting and forging. You can apply geometric restrictions that force the topology optimization process to consider only designs that can be manufactured. For example, when you are using topology optimization you can force the Abaqus Topology Optimization Module to create a castable shape that can be extracted from a mold or a stampable shape that can be created with a tool and die. Maintaining a moldable structure In cases where bending and torsion loads are applied, topology optimization is likely to generate a model with hollow areas or with undercuts that cannot be manufactured. You can prevent the topology optimization from generating cavities and undercuts by specifying the following: • A forgeable structure that can be removed from the forging die, as shown in Figure 13.2.2–1. Pull direction Back plane Figure 13.2.2–1 A forgable part. • A moldable structure that can be removed from two halves of a mold, as shown in Figure 13.2.2–2. Pull directions Center plane Pull direction (normal to every surface) Figure 13.2.2–2 A moldable part. In contrast, Figure 13.2.2–3 illustrates parts with a cavity and an undercut that are not moldable. Pull directions Pull directions Center plane Center plane Figure 13.2.2–3 Cavities and undercuts prevent a part from being moldable. Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Demold control; Demold technique, Demolding with a central plane Optimization module: Geometric Restriction→Create: Demold control; Demold technique, Demolding at the region surface Optimization module: Geometric Restriction→Create: Demold control; Demold technique, Forging Maintaining a stampable structure You can specify that the structure is to be manufactured by a stamping process. If the optimization process removes one element from the structure, it also removes all elements positioned either behind or in front of the element (with respect to the pull direction), as shown in Figure 13.2.2–4. Elements removed during optimization Pull directions Center plane Figure 13.2.2–4 A stampable structure. The rate at which the Abaqus Topology Optimization Module modifies the element properties should not be set too high if the stamping restriction is activated in a condition-based topology optimization; otherwise, supports or trusses generated by the optimization may become unattached from the rest of the structure. Abaqus/CAE Usage: Use the following option to create a stamping geometric restriction in a topology optimization: Optimization module: Geometric Restriction→Create: Demold control; Demold technique, Stamping Use the following option to create a stamping geometric restriction in a shape optimization: Optimization module: Geometric Restriction→Create: Stamp control the Use at which to Abaqus Topology Optimization Module modifies the element properties: following specify option rate the the Optimization module: Task→Create: Advanced , Size of increment for volume modification Specifying a symmetric structure Introducing symmetry constraints into your model can significantly increase the speed at which the Abaqus Topology Optimization Module calculates the optimized structure. You can use the Abaqus Topology Optimization Module to apply the following symmetry constraints: • Symmetry about an axis or plane (reflection symmetry) • Symmetry about a point • Rotational symmetry • Cyclic symmetry (replication of an area with a given distance) You can apply a symmetry restriction to unstructured meshes or to tetrahedron meshes in a topology optimization. The elements should be approximately the same size because the resulting symmetry is based on the resolution of the coarsest part of the mesh. In addition, the Abaqus Topology Optimization Module may fail to create the symmetric conditions if the difference in the element size is too large. To define symmetry for a shape optimization, the Abaqus Topology Optimization Module assembles nodes that are approximately symmetric into a symmetry group (normally there are two symmetric nodes in each symmetry group). The Abaqus Topology Optimization Module then determines the master node of the symmetry group and calculates the design displacements of the client nodes in such a way that they move symmetrically to the plane of the master node. If you are performing a topology optimization, your meshed Abaqus model does not have to be symmetric before the optimization starts. Conversely, if you are performing a shape optimization, your meshed Abaqus model should be symmetric before the optimization starts to allow the Abaqus Topology Optimization Module to identify symmetric nodes and maintain their symmetry when the surface nodes are moved. Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Planar symmetry, Point symmetry, Rotational symmetry, or Cyclic symmetry Applying additional restrictions during a shape optimization the displacement of Shape optimization determines to homogenize the stress on the surface and satisfy the objective function and any constraints. The Abaqus Topology Optimization Module does not couple the displacement of neighboring nodes; each of the design nodes can move independently of the other design nodes. For example, during the optimization a planar surface can develop into a nonplanar free-form surface. By coupling the design nodes you can force the optimization to maintain the regularity of a plane. each surface node in an effort Coupling conditions restrict the range of solutions for the system and reduce the optimization potential. In addition, defining the appropriate coupling conditions can be very time consuming. To simplify your optimization, you should start with an optimization with as few restrictions as possible and only a few coupling conditions and introduce additional coupling conditions only if they are required. You can apply additional restrictions while the Abaqus Topology Optimization Module is moving surface nodes during a shape optimization: • The optimized shape can be manufactured by a tool on a lathe cutting into the model along a specified direction. • The optimized shape can be manufactured by a tool drilling into the model along a specified direction. The hole created by the tool is symmetric about the axis of the tool. In addition, the tool can be withdrawn from the hole. • Selected faces in the optimized shape can slide along each other and/or cannot penetrate each other. • Nodes are restricted to move: – along a specified vector, – a specified distance either inward or outward (shrinkage or growth), – along a specified direction, – only along selected degrees of freedom, and – only in the direction of applied loads. Abaqus/CAE Usage: Optimization module: Geometric Restriction→Create: Turn control, Drill control, Penetration check, Slide region control, or Vector Combining geometric constraints Each geometric constraint that you apply reduces the possibility of Abaqus arriving at an optimized solution. In addition, if you apply too many geometric restrictions, the solution that Abaqus generates may not be the most optimal solution available. Therefore, you should start by allowing Abaqus to perform an optimization with no geometric restrictions applied or with only a limited number. After you have studied the results of the unrestricted, or less-restricted, optimization, you should apply only the restrictions that are required to solve the problem. You can combine geometric constraints; however, only certain combinations are permissible. Abaqus processes geometrical constraints in the following order: • Minimum member size • Symmetry constraints • Manufacturing constraints • Maximum member size Applying one constraint may weaken the effect of another constraint. For example, you cannot define symmetry about a plane in conjunction with a demold pull direction that is not parallel with the axis or plane of symmetry. The following manufacturing restriction combinations are permissible: • You can combine symmetry about a plane with a pull direction provided the pull direction is perpendicular or parallel to the plane of symmetry. • You can combine rotational symmetry with a pull direction provided the pull direction is parallel to the axis of rotation. • You can combine two symmetries about a plane provided the planes are perpendicular. • When you first run a condition-based topology optimization, you should not use a combination of a maximum member size and a pull direction because the optimization may not converge, depending on the finite element mesh. When you are confident the optimization will converge, you can introduce this combination of geometric constraints. • You can specify a minimum member size that is greater than the maximum member size. Abaqus first processes the minimum member size requirement and creates relatively thick supports. The thick supports are subsequently divided into smaller parallel members when Abaqus processes the maximum size requirement. Stop conditions Stop conditions are examined after each design cycle and determine whether an optimization should end because the maximum number of design cycles has been reached or because the optimization has converged on an optimal solution. The Abaqus Topology Optimization Module provides both global and local stop conditions; however, local stop conditions are rarely required. Global stop conditions The global convergence stop condition defines the maximum number of design cycles that should be performed. To limit the number of design cycles, you must define a global stop condition for each optimization task. The default value for the maximum number of design cycles depends on the type of optimization, as shown in Table 13.2.2–1. Abaqus/CAE Usage: Job module: Optimization→Create: Maximum cycles Local stop conditions Local stop conditions indicate if a general topology optimization has converged on an optimal solution. Local stop conditions apply to the displacements or stresses in a region of your model and define when the goals of an optimization have been reached. A local stop condition compares a single scalar value of displacement or equivalent stress to a reference value. The single scalar value can be either the maximum Table 13.2.2–1 Default maximum number of design cycles. Optimization Type Default maximum number of design cycles Condition-based topology optimization General topology optimization Shape optimization 15 50 10 or minimum value over a region or the sum of all the values. The reference value can be taken from the value of the single scalar value after the previous iteration or after the first iteration. In addition, you can modify the reference value by a fixed amount or by a percentage. For example, you can specify a local stop condition that ends the optimization if the sum of the displacements within a region is smaller than 1% of the sum of the displacements after the first optimization cycle. You can define one or two local stop conditions, and you can specify if either or both (default) of the local stop conditions must be met for the Abaqus Topology Optimization Module to end the optimization. Examples of local stop conditions include the following: • If you have specified that the displacement or stress should be minimized (or maximized), a local stop condition can end the optimization if the value of the displacement or stress increases (or decreases) after an optimization cycle. • When the optimization approaches the optimum solution, you can expect only small changes in the value of the displacement or stress. A local stop condition can end the optimization if the relative change in the displacement or stress falls below a tolerance limit after an optimization cycle. • When the optimization approaches the optimum solution, you can expect only small changes in the sum of the displacements and, therefore, only minor modifications to the model. A local stop condition can end the optimization if the change in the sum of the displacements falls below a tolerance limit after an optimization cycle. You can use the sum of the displacements as a stop condition for optimizations with and without constraints. In addition, this stop condition is suitable for a variety of objective functions, such as stress or frequency. Abaqus/CAE Usage: Optimization module: Stop Condition→Create 13.2.3 CREATING Abaqus OPTIMIZATION MODELS Product: Abaqus/CAE References • “Structural optimization: overview,” Section 13.1.1 • “Understanding optimization,” Section 18.3 of the Abaqus/CAE User’s Manual Overview For each design cycle the optimization process: • generates new material and element properties during topology optimization; • modifies nodal coordinates during shape optimization; • sends the modified model to an Abaqus analysis; and • reads the results of the analysis. Preparing the Abaqus model You should take care to ensure that your Abaqus model is supported by structural optimization. Any restrictions imposed by the use of structural optimization, such as the supported element types, apply only to the design area; regions outside the design area do not play a role in the optimization. • You must ensure that your Abaqus model can be analyzed and produces the expected mechanical results before you attempt to optimize your model. • You should account for nonlinearities only if your model is truly nonlinear; the optimization will be significantly less expensive computationally if your Abaqus model is linear. You may want to ensure that an optimization of a linear version of your model produces reasonable results before you introduce geometric or material nonlinearities. • An optimization takes multiple design cycles to complete, and the time required to reach an optimized solution can be significant. As a result, you must configure your Abaqus model to minimize computational time; for example, by removing small details that are not important to the optimization. • The Abaqus Topology Optimization Module does not support the use of parts and assemblies in the Abaqus input file. When you run an optimization task, the Abaqus Topology Optimization Module generates a flattened input file that does not use parts and assemblies. • The Abaqus Topology Optimization Module reads data from the output database (.odb) file. The Abaqus Topology Optimization Module requests data only from the end of each step. To minimize the size of the output database file, you should also request data only from the end of each step. Support for analysis types The following Abaqus analysis types are supported by both topology and shape optimization: • Static stress/displacement, general analysis • Static stress/displacement, linear perturbation analysis • Extract natural frequencies and modal vectors Support for geometric nonlinearities You can specify that geometric nonlinearity should be accounted for only during static stress/displacement analyses. Elements that have limited stiffness, such as elements with hyperelastic material properties, can deform excessively during topology optimization in a nonlinear analysis. This deformation can lead to an adverse effect on the convergence and result in the termination of the analysis. You should be aware of this potential issue when applying topology optimization using hyperelastic materials. Support for multiple load cases If your model is undergoing a sequence of loads, you can significantly reduce the computational cost by defining a multiple load case analysis within a single step. Support for acceleration loading General topology optimization supports prescribed acceleration loading from • gravity, • rotational body forces, and • centrifugal forces. Coriolis forces are not supported. Support for contact during the optimization You can avoid contact in optimized regions of your model by defining geometric restrictions, such as casting or minimum member size restrictions. In some cases, you cannot specify the exact boundary conditions early in the design phase. In addition, nonlinear boundary conditions, such as contact definitions, can change if the Abaqus Topology Optimization Module changes the topology of the model. The optimization process is more efficient if you create an Abaqus model with the appropriate contact definitions and allow Abaqus to calculate the contact. The contact conditions are included in the optimization through the forces at the nodes and the stresses in the elements, and both topology and shape optimization permit contact conditions in the Abaqus model. You can define a contact surface directly on the edge of the design space in topology optimization. However, if the design edge belongs to a contact surface in shape optimization, you must invert the shape optimization algorithm by entering a negative growth scale factor. You may encounter convergence difficulties in your Abaqus model if you have a complex contact problem or if the optimization results in large changes in the model. Restrictions on an Abaqus model used for topology optimization Topology optimization determines the optimal material distribution in the design space, given the prescribed conditions applied to the model along with the objective function and constraints. Your optimization must apply appropriate constraints and restrictions; otherwise, the Abaqus Topology Optimization Module can extensively alter the topology of the component. The resolution of the structure that has been optimized with topology optimization is very dependent on the discretization. A fine mesh produces a structure with a higher resolution than a coarse mesh; however, it will also substantially increase the processing time required. You must determine the appropriate compromise between structural resolution and processing time. During topology optimization the Abaqus Topology Optimization Module modifies the material definition of the elements in the design area. As a result, you must provide the initial density of the materials in the design area, even if it is not required by the Abaqus analysis. Restrictions on an Abaqus model used for shape optimization Abaqus performs a shape optimization by modifying the boundaries or surfaces of a component. The optimization uses the stress condition to calculate new coordinates for nodes on the surface of the component and then adjusts the underlying mesh accordingly. The mesh quality must be sufficient to ensure that the analysis results are mostly unchanged by the movement of the surface nodes. High stress gradients must not be present within an element. When the Abaqus Topology Optimization Module is performing a shape optimization on a shell structure, it optimizes the form of the shell structure and not its thickness. The nodal position along shell edges can be modified; however, Abaqus does not modify the shell definition. Supported materials in the design area The material models supported by structural optimization in the elements in the design area depend on the type of optimization—condition-based topology optimization, general topology optimization, or shape optimization. Materials supported by condition-based topology optimization Condition-based topology optimization in Abaqus supports linear elastic, plastic, and hyperelastic material models. Support for linear elastic material models The following linear elastic material models are supported by condition-based topology optimization: • Linear elastic materials with isotropic behavior. • Linear elastic materials with fully anisotropic behavior. • Linear elastic materials with orthotropic behavior. All of the behavior models are supported, except for orthotropic shear behavior for warping elements and coupled and uncoupled traction behavior for cohesive elements. Support for plastic material models Metal plasticity material properties—the plastic part of the material model for elastic-plastic materials that use the Mises or Hill yield surface—are supported by condition-based topology optimization. Isotropic hardening is supported; however, cyclic loading is not supported—each material point can be unloaded only once and should not become elastoplastic again. Support for hyperelastic material models All of the hyperelastic material models are supported by condition-based topology optimization, except for the Marlow material model and the hyperelastic material models with test data. Support for temperature and field variable dependency Condition-based topology optimization supports materials that have temperature and field variable dependency. Materials supported by general topology optimization General topology optimization in Abaqus supports linear elastic, plastic, and hyperelastic material models. Support for linear elastic material models The following linear elastic material models are supported by general topology optimization: • Linear elastic materials with isotropic behavior. • Linear elastic materials with fully anisotropic behavior. • Linear elastic materials with orthotropic behavior. All of the behavior models are supported, except for orthotropic shear behavior for warping elements and coupled and uncoupled traction behavior for cohesive elements. Support for plastic material models Metal plasticity material properties—the plastic part of the material model for elastic-plastic materials that use the Mises or Hill yield surface—are supported by general topology optimization. Isotropic hardening is supported; however, cyclic loading is not supported—each material point can be unloaded only once and should not become elastoplastic again. Support for hyperelastic material models All of the hyperelastic material models are supported by general topology optimization, except for the Marlow material model and the hyperelastic material models with test data. Support for temperature and field variable dependency General topology optimization supports materials that have temperature and field variable dependency. Material support in shape optimization Shape optimization in Abaqus supports all of the Abaqus material models. Support for coordinate systems In most cases, you will use the same coordinate system to define your model and the optimization task. However, the Abaqus Topology Optimization Module allows you refer to a different coordinate system when you are defining a design response. Supported element types The Abaqus elements that are supported as design elements by topology and shape optimization are listed in Table 13.2.3–1 through Table 13.2.3–4. The tables also list the Abaqus elements that support the reaction and internal force design responses. Unsupported elements are ignored during optimization and remain unchanged. Structural optimization does not place any restrictions on the type of elements that you use outside the design area. Supported two-dimensional solid elements Topology optimization (both condition-based and general) and shape optimization support two-dimensional solid elements listed in Table 13.2.3–1. the Table 13.2.3–1 Supported two-dimensional solid elements. CPE31, CPE3H, CPE41 , CPE4H, CPE4I, CPE4IH, CPE4R1 , CPE4RH, CPE6H, CPE6M, CPE6MH CPE81, CPE8H, CPE8R1 , CPE8RH CPS31 , CPS41 , CPS4I, CPS4R1, CPS61 , CPS6M, CPS6MT, CPS81. CPS8R1 CPEG3, CPEG3H, CPEG4, CPEG4H, CPEG4I, CPEG4IH, CPEG4R, CPEG4RH, CPEG6, CPEG6H, CPEG6M, CPEG6MH, CPEG8, CPEG8H, CPEG8R, CPEG8RH CPE3T, CPE4T, CPE4HT, CPE4RT, CPE4RHT, CPE6MT, CPE6MHT, CPE8T, CPE8HT, CPE8RT, CPE8RHT CPS3T, CPS4T, CPS4RT, CPS8T, CPS8RT CPEG3T, CPEG3HT, CPEG4T, CPEG4RT, CPEG4RHT, CPEG6MT, CPEG6MHT, CPEG8T, CPEG8HT, CPEG8RHT 1 Can include reaction and internal force design responses. Supported three-dimensional solid elements Topology optimization (both condition-based and general) and shape optimization support the three- dimensional solid elements listed in Table 13.2.3–2. Table 13.2.3–2 Supported three-dimensional solid elements. C3D41, C3D4H, C3D81 C3D61, C3D6H C3D8H, C3D8I, C3D8IH, C3D8R1 , C3D8RH C3D101 , C3D10H, C3D10M, C3D10MH C3D151 , C3D15H C3D201 , C3D20H, C3D20R1 , C3D20RH C3D4T, C3D6T, C3D8T, C3D8HT, C3DHRT, C3D8RHT, C3D10MT, C3D10MHT, C3D20T, C3D20HT, C3D20RT, C3D20RHT 1 Can include reaction and internal force design responses. Supported axisymmetric solid elements Topology optimization (both condition-based and general) and shape optimization support axisymmetric solid elements listed in Table 13.2.3–3. the Table 13.2.3–3 Supported axisymmetric solid elements. CAX31, CAX3H, CAX41 , CAX4H, CAX4I, CAX4IH, CAX4R1, CAX4RH CAX81, CAX8H, CAX8R1 , CAX8RH CGAX3, CGAX3H, CGAX4, CGAX4H, CGAX4R, CGAX4RH, CGAX8, CGAX8H, CGAX8R, CGAX8RH CAX3T, CAX4T, CAX4HT, CAX4RT, CAX4RHT, CAX8T, CAX8HT, CAX8RT, CAX8RHT CGAX3T, CGAX3HT, CGAX4T, CGAX4HT, CGAX4RT, CGAX4RHT, CGAX8T, CGAX8HT, CGAX8RT, CGAX8RHT 1 Can include reaction and internal force design responses. Additional supported elements Table 13.2.3–4 lists the general membrane, three-dimensional conventional shell, and beam elements that are supported by optimization. Table 13.2.3–4 Additional supported elements General membrane elements (topology and shape optimization) M3D31, M3D41, M3D4R1, M3D61, M3D81 , M3D8R1 Three-dimensional conventional shell elements (topology optimization only) STRI3, S3, S3R, STRI65, S4, S4R, S4R5, S8R, S8R5, S8RT Three-dimensional conventional shell elements (shape optimization only) STRI31 , S31, S3R1 , S41, S4R1 , S8R1 Beam elements (shape optimization only) B212 , B21H2, B312 , B31H2 1 Can include reaction and internal force design responses. 2 You can include beam elements in shape optimization only to define a neighboring component that is used to restrict the movement of nodes in the optimized region. 13. Optimization Techniques 14. Eulerian Analysis Eulerian analysis 14.1 Eulerian analysis • “Eulerian analysis,” Section 14.1.1 • “Defining Eulerian boundaries,” Section 14.1.2 • “Eulerian mesh motion,” Section 14.1.3 • “Defining adaptive mesh refinement in the Eulerian domain,” Section 14.1.4 14.1.1 EULERIAN ANALYSIS Products: Abaqus/Explicit Abaqus/CAE References • “Eulerian surface definition,” Section 2.3.5 • “Eulerian elements,” Section 32.14.1 • *EULERIAN SECTION • *INITIAL CONDITIONS • *SURFACE • “Creating Eulerian sections,” Section 12.13.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a material assignment field,” Section 16.11.10 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • Chapter 28, “Eulerian analyses,” of the Abaqus/CAE User’s Manual Overview In a traditional Lagrangian analysis nodes are fixed within the material, and elements deform as the material deforms. Lagrangian elements are always 100% full of a single material, so the material boundary coincides with an element boundary. By contrast, in an Eulerian analysis nodes are fixed in space, and material flows through elements that do not deform. Eulerian elements may not always be 100% full of material—many may be partially or completely void. The Eulerian material boundary must, therefore, be computed during each time increment and generally does not correspond to an element boundary. The Eulerian mesh is typically a simple rectangular grid of elements constructed to extend well beyond the Eulerian material boundaries, giving the material space in which to move and deform. If any Eulerian material moves outside the Eulerian mesh, it is lost from the simulation. Eulerian material can interact with Lagrangian elements through Eulerian-Lagrangian contact; simulations that include this type of contact are often referred to as coupled Eulerian-Lagrangian (CEL) analyses. This powerful, easy-to-use feature of Abaqus/Explicit general contact enables fully coupled multi-physics simulation such as fluid-structure interaction. Applications Eulerian analyses are effective for applications involving extreme deformation, up to and including In these applications, traditional Lagrangian elements become highly distorted and lose fluid flow. accuracy. Liquid sloshing, gas flow, and penetration problems can all be handled effectively using Eulerian analysis. Eulerian-Lagrangian contact allows the Eulerian materials to be combined with traditional nonlinear Lagrangian analyses. An example of using Eulerian analysis for a severe deformation analysis is discussed in “Rivet forming,” Section 2.3.1 of the Abaqus Example Problems Manual; using coupled Eulerian-Lagrangian contact for a fluid-structure interaction application is illustrated in “Impact of a water-filled bottle,” Section 2.3.2 of the Abaqus Example Problems Manual. Eulerian volume fraction The Eulerian implementation in Abaqus/Explicit is based on the volume-of-fluid method. In this method, material is tracked as it flows through the mesh by computing its Eulerian volume fraction (EVF) within each element. By definition, if a material completely fills an element, its volume fraction is one; if no material is present in an element, its volume fraction is zero. Eulerian elements may simultaneously contain more than one material. If the sum of all material volume fractions in an element is less than one, the remainder of the element is automatically filled with “void” material. Void material has neither mass nor strength. Material interfaces Volume fraction data are computed for each Eulerian material in an element. Within each time increment, the boundaries of each Eulerian material are reconstructed using these data. The interface reconstruction algorithm approximates the material boundaries within an element as simple planar facets (the Eulerian method is implemented only for three-dimensional elements). This assumption produces a simple, approximate material surface that may be discontinuous between neighboring elements. Therefore, accurate determination of a material’s location within an element is possible only for simple geometries, and fine grid resolution is required in most Eulerian analyses. The discontinuities in an Eulerian material surface can lead to physically unrealistic configurations when visualizing the results of an Eulerian analysis. Abaqus/CAE can apply a nodal averaging algorithm to estimate a more realistic, continuous surface during visualization. For more information on visualizing the material interfaces in an Eulerian model, see “Viewing output from Eulerian analyses,” Section 28.7 of the Abaqus/CAE User’s Manual. Eulerian section definition An Eulerian section definition lists all of the materials that may appear within an Eulerian element. Void material is automatically included in this list. The material list supports an optional material instance name. Material instance names are required to uniquely identify materials that you use more than once. Repeated materials are useful, for example, in mixing simulations where the motion of a material interface is to be computed: the water in a tank could be divided by creating water material instances named “water_left” and “water_right,” and the evolution of the interface between these materials could be simulated. By default, all Eulerian elements are initially filled with void material, regardless of the section assignment. You must introduce nonvoid material into your Eulerian mesh using an initial condition . Eulerian mesh deformation The Eulerian time incrementation algorithm is based on an operator split of the governing equations, resulting in a traditional Lagrangian phase followed by an Eulerian, or transport, phase. This formulation is known as “Lagrange-plus-remap.” During the Lagrangian phase of the time increment nodes are assumed to be temporarily fixed within the material, and elements deform with the material. During the Eulerian phase of the time increment deformation is suspended, elements with significant deformation are automatically remeshed, and the corresponding material flow between neighboring elements is computed. At the end of the Lagrangian phase of each time increment, a tolerance is used to determine which elements are significantly deformed. This test improves performance by allowing those elements with little or no deformation to remain inactive during the Eulerian phase. The inactive elements typically have no impact on the visualization of an Eulerian analysis; however, plotting an Eulerian mesh using a very large deformation scale factor may reveal slight deformations for elements within the deformation tolerance. Eulerian material advection As material flows through an Eulerian mesh, state variables are transferred between elements by advection. The variables are assumed to be linear or constant in each old element, then these values are integrated over the new elements after remeshing. The new value of the variable is found by dividing the value of each integral by the material volume or mass in the new element. Second-order advection Second-order advection assumes a linear distribution of the variable in each old element. To construct the linear distribution, a quadratic interpolation is constructed from the constant values at the integration points of the middle element and its adjacent elements. A trial linear distribution is found by differentiating the quadratic function to find the slope at the integration point of the middle element. The trial linear distribution in the middle element is limited by reducing its slope until its minimum and maximum values are within the range of the original constant values in the adjacent elements. This process is referred to as flux limiting and is essential to ensure that the advection is monotonic. Second-order advection is used by default, and it is recommended for all problems, ranging from quasi-static to transient dynamic shock. Input File Usage: Abaqus/CAE Usage: *EULERIAN SECTION, ADVECTION=SECOND ORDER The second-order advection method is used by default in Abaqus/CAE. First-order advection First-order advection assumes a constant value of the variable in each old element. This method is simple and computationally efficient; however, it tends to diffuse sharp gradients over time. Therefore, this technique should be used only as a computationally efficient alternative for quasi-static simulations. Input File Usage: *EULERIAN SECTION, ADVECTION=FIRST ORDER Abaqus/CAE Usage: The first-order advection method cannot be specified in Abaqus/CAE. Reducing the stable time increment based on the advection speed The stable time increment size is adjusted automatically to prevent material from flowing across more than one element in each increment. When the material velocity approaches the speed of sound (for example, in simulations involving blast and shocks), further restrictions on the time increment size may be needed to maintain accuracy and stability. You can specify a flux limit ratio to restrict the stable time increment size such that material can flow across only a fraction of an element in each increment. The default flux limit ratio is 1.0, and recommended values range from 0.1 to 1.0. Input File Usage: Abaqus/CAE Usage: *EULERIAN SECTION, FLUX LIMIT RATIO=maximum ratio The flux limit ratio cannot be modified in Abaqus/CAE. Initial conditions You can apply initial conditions to Eulerian nodes and elements in the same way that they are used for Lagrangian nodes and elements. Initial stress, temperature, and velocity are common examples. In addition, most Eulerian analyses require the initialization of Eulerian material. By default, all Eulerian elements are initially void. You can use initial conditions to fill Eulerian elements with one or more of the materials listed in the Eulerian section definition. By selectively filling elements, you can create the initial shape of each Eulerian material. To fill an Eulerian element, you must define an initial volume fraction for each available material instance. Material is filled until a volume fraction of 1.0 is reached; any excess material is ignored. The initial conditions apply only at the beginning of an analysis; during the analysis the materials deform according to the applied loads, and the volume fractions are recalculated accordingly. *INITIAL CONDITIONS, TYPE=VOLUME FRACTION Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Material Assignment for the Types for Selected Step Abaqus/CAE Usage: Input File Usage: Boundary conditions By default, Eulerian material can flow freely into and out of the Eulerian domain through mesh boundaries. You can constrain degrees of freedom at Eulerian nodes to restrict material flow. For example, you can define typical fluid “stick” or “sliding” walls using constraints normal and/or tangential to the boundary. Since Eulerian nodes are automatically repositioned during the Eulerian transport phase, you cannot apply prescribed displacement boundary conditions to them. You can use prescribed velocity or acceleration conditions on Eulerian nodes to control material flow. Prescribed velocity or acceleration is implemented in an Eulerian frame, so material velocity will reach the prescribed value as the material passes the Eulerian node. If velocity is directed outward at an Eulerian mesh boundary, either by prescribed condition or naturally as a result of dynamic equilibrium, material may flow out of the Eulerian domain. This material is lost from the simulation, and corresponding decreases in total mass and energy will occur. Similarly, if velocity is directed inward at a boundary, inflow of material into the Eulerian domain will occur. When materials flow into an element through a boundary face, the material content and the state of each inflowing material are equal to that which presently exists within the element. For example, if a boundary element contains 60% hot water and 40% cold air and the interface normal is parallel to the boundary face, inflow velocity will introduce a mixture of 60% hot water and 40% cold air. In this case corresponding increases in total mass and energy will occur. You can also define inflow and outflow conditions at an Eulerian domain boundary, as described in “Defining Eulerian boundaries,” Section 14.1.2. Loads You can apply loads to Eulerian nodes, elements, and faces in the same way as to their Lagrangian counterparts. Eulerian loads act in an Eulerian frame: they affect Eulerian material as it passes the point of load application. Material options You can define material properties for Eulerian analysis in the same way as for Lagrangian analysis. Liquids and gases can be modeled using equation of state materials . Anisotropic materials are not supported because of inaccuracies introduced to orientation data during material transport. Brittle cracking is not supported because the failure mode is anisotropic. Hyperelastic materials can be used in an Eulerian analysis, but due to inaccuracies introduced to the deformation gradient during material transport, these materials might not fully recover their original configuration after loads are removed; the same inaccuracies also affect user-defined materials. The low-density foam material model (“Low-density foams,” Section 22.9.1) is not supported. Eulerian analysis allows materials to undergo extreme strain without the mesh distortion limitations of Lagrangian analysis. Therefore, it is especially important to define your material behavior through the entire strain range, which often requires definition of a failure behavior. Isotropic material failure is supported using a damage variable to characterize the failure level. Element deletion is suppressed for Eulerian sections because undamaged material may flow into “failed” elements. Shear failure models are not supported. Rayleigh mass proportional damping is not supported. Elements The Eulerian method is implemented in the multi-material element type EC3D8R and the multi-material thermally coupled element type EC3D8RT. The underlying mechanical response formulation of these elements is based on the Lagrangian C3D8R element with extensions to allow multiple materials and to support the Eulerian transport phase. The formulation applies the same strain to each material in the element, then allows the stress and other state data to evolve independently within each material. These stresses are combined using volume fraction data to create element averaged values, which are integrated to obtain nodal forces. Similarly, the thermal response formulation for the thermally coupled element is based on the Lagrangian element C3D8RT with the extension to allow multiple materials with different thermal properties and to support temperature advection. All the materials have the same temperature, and the thermal properties (such as thermal conductivity and thermal capacitance) are volume averaged before being used in solving one single heat transfer equation for the multi-material model. Element averaged values of other state data are computed similarly for output purposes. The Eulerian EC3D8R and EC3D8RT elements require eight nodes. Degenerate elements are not supported. The Eulerian method is not implemented for two-dimensional elements. Axisymmetry can be simulated using a wedge-shaped mesh and symmetry boundary conditions. By default, the Eulerian elements use viscous hourglass control. Hourglass control is disabled by default for incompressible liquids modeled using equation of state material types. These choices can be modified using section controls . Constraints Since Eulerian nodes are automatically repositioned during the Eulerian transport phase, you cannot use Eulerian nodes in Lagrangian modeling features such as elements, connectors, and constraints. However, constraints between Eulerian materials and Lagrangian parts can be modeled using tied contact interfaces. Interactions Eulerian material instances interact with each other with a sticky behavior. This sticking occurs because of the kinematic assumption that a single strain field is applied to all materials within an element. Tensile stress can be transmitted across an interface between two Eulerian materials, and no slip occurs at these interfaces. This Eulerian-to-Eulerian contact behavior can be reasonable in some situations, such as in a simulation of a lead bullet penetrating a steel plate. Ablation of the bullet surface against the steel is captured by the sticky behavior within the Eulerian elements at the bullet-steel interface. Relative motion along this interface will occur only due to shearing of the lead material. Eulerian-to-Eulerian contact occurs by default in an Eulerian analysis; you do not need to define contact interactions between Eulerian materials. More complex contact interactions can be simulated when one of the contacting bodies is modeled using Lagrangian elements. This powerful capability supports applications such as fluid-structure interaction, where an Eulerian fluid contacts a Lagrangian structure. is an extension of general contact The implementation of Eulerian-Lagrangian contact in Abaqus/Explicit. The general contact property models and defaults apply to Eulerian-Lagrangian contact . For example, by default, tensile stresses are not transmitted across an Eulerian-Lagrangian contact interface, and the interface friction coefficient is zero. Specifying automatic contact for an entire Eulerian-Lagrangian model allows for interactions between all Lagrangian structures and all Eulerian materials in the model. You can also use Eulerian surfaces to create material-specific interactions or to exclude contact between particular Lagrangian surfaces and Eulerian materials. Input File Usage: Use both of the following options to define contact between all Lagrangian bodies and all Eulerian materials: *CONTACT *CONTACT INCLUSIONS, ALL EXTERIOR Use the following options to include or exclude contact between particular Lagrangian surfaces and Eulerian materials: *CONTACT *CONTACT INCLUSIONS Lagrangian_surface, Eulerian_surface *CONTACT EXCLUSIONS Lagrangian_surface, Eulerian_surface Abaqus/CAE Usage: Use the following option to define contact between all Lagrangian bodies and all Eulerian materials: Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: All* with self Use the following options to include contact between particular Lagrangian surfaces and Eulerian materials: Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: Selected surface pairs: Edit, select the Lagrangian surface in the left column and the Eulerian material instance in the right column, then click the arrows to transfer them to the list of included pairs Use the following options to exclude contact between particular Lagrangian surfaces and Eulerian materials: Interaction module: Create Interaction: General contact (Explicit): Excluded surface pairs: Edit, select the Lagrangian surface in the left column and the Eulerian material instance in the right column, then click the arrows to transfer them to the list of excluded pairs Formulation of Eulerian-Lagrangian contact The Eulerian-Lagrangian contact formulation is based on an enhanced immersed boundary method. In this method the Lagrangian structure occupies void regions inside the Eulerian mesh. The contact algorithm automatically computes and tracks the interface between the Lagrangian structure and the Eulerian materials. A great benefit of this method is that there is no need to generate a conforming mesh for the Eulerian domain. In fact, a simple regular grid of Eulerian elements often yields the best accuracy. If the Lagrangian body is initially positioned inside the Eulerian mesh, you must make sure that the underlying Eulerian elements contain void after material initialization. During the analysis the Lagrangian body pushes material out of the Eulerian elements that it passes through, and they become filled with void. Similarly, Eulerian material flowing toward the Lagrangian body is prevented from entering the underlying Eulerian elements. This formulation ensures that two materials never occupy the same physical space. If the Lagrangian body is initially positioned outside the Eulerian mesh, at least one layer of void Eulerian elements must be present at the Eulerian mesh boundary. This creates a free surface on the Eulerian material inside the Eulerian mesh boundary and provides a source for void material to replace Eulerian material that is driven out of interior elements. Several layers of void elements are typically used above free surfaces to allow simulation of crater formation and backsplashing before this material leaves the Eulerian domain. Eulerian-Lagrangian contact also supports failure and erosion in the Lagrangian body. Lagrangian element failure can open holes in a surface through which Eulerian material may flow. When modeling erosion of a solid Lagrangian body, the interior faces of the solid body must be included in the contact surface definition . Eulerian-Lagrangian contact constraints are enforced using a penalty method, where the default penalty stiffness parameter is automatically maximized subject to stability limits. Eulerian-Lagrangian contact supports thermal interactions when using coupled temperature- displacement Eulerian element EC3D8RT in a dynamic coupled thermal-stress analysis. However, gap radiation and gap conductance as a function of clearance are not supported. Output The set of element output variables EVF gives the Eulerian volume fraction for each material in the Eulerian section definition, including void. It is important to request output for EVF in all Eulerian analyses because visualization of Eulerian material boundaries is based on the material volume fractions. Material-specific Eulerian field output variables are distinguished by appending material names to the base field name. For example, if you request output variable S (stress components) in an Eulerian analysis involving material instances named “steel” and “tin,” you will see results for individual material stresses named “S_steel” and “S_tin.” Several volume fraction averaged field data are also available for output. For example, output variable SVAVG gives a single value of stress for each element computed as a volume fraction average of stress over all materials present in the element. Use of these volume fraction averaged output data has the advantage of substantially reducing the size of the output database for the case where several materials are defined in the Eulerian section. See “Abaqus/Explicit output variable identifiers,” Section 4.2.2, for a complete list of Eulerian-specific output variables. Output variables EVF and SVAVG are included in the PRESELECT variable list when Eulerian elements appear in the model. You can also request integrated volume (VOLEUL) and integrated mass (MASSEUL) over a particular Eulerian element set. These output variables are material specific and are distingushed by having the material names appended to the variable name. Limitations Eulerian analyses are subject to the following limitations: • Boundary conditions: You cannot apply prescribed nonzero displacement boundary conditions to Eulerian nodes. • Lagrangian attachments: You cannot attach Lagrangian elements to Eulerian nodes. Use tied contact interfaces instead. • Constraints: You cannot apply Lagrangian constraints (MPCs, etc.) to Eulerian nodes. Use tied contact interfaces instead. • Materials: Materials with orientation (anisotropic, etc.) are not supported for Eulerian elements. Brittle cracking and shear failure models are also not supported. Rayleigh mass proportional damping is not supported. • Elements: The Eulerian formulation is implemented only for EC3D8R and EC3D8RT elements. • Element import: Eulerian elements are not available for import. • Double-sided contact: Penetration of Eulerian material through the contact interface can occur in some cases involving Eulerian material contacting Lagrangian shell or membrane elements. This type of contact introduces complexity because the sign of the outward normal direction must be determined on the fly as material approaches the Lagrangian element; contact with either side of the element is potentially allowable. You should simplify the contact problem wherever possible by using Lagrangian solid elements instead of shell or membrane elements, since the outward normal direction at solid element faces is unique. For example, if a model involves Eulerian material flowing around a rigid Lagrangian obstacle, mesh the obstacle with solid elements rather than shell elements. • Contact penetration: In some cases Eulerian material may penetrate through the Lagrangian contact surface near corners. This penetration should be limited to an area equal to the local Eulerian element size. Penetration can be minimized by refining the Eulerian mesh or adding a fillet to the Lagrangian mesh with radius equal to the local Eulerian element size. • Contact types: Eulerian-Lagrangian contact does not support Lagrangian beam elements, Lagrangian pipe elements, Lagrangian truss elements, or analytical rigid surfaces. Thermal contact is also not supported. • Contact import: Import of the Eulerian-Lagrangian contact states is not supported. • Thermal contact: Gap radiation and gap conductance as a function of clearance are not supported. • Contact output: Contact variables are output only for the Lagrangian side of Eulerian-Lagrangian interfaces. • Surface loads: You cannot use the Eulerian material surface type for general surface loading. However, distributed loads such as pressure can be applied to surfaces defined on Eulerian element faces. • Mass scaling: You cannot apply mass scaling to Eulerian elements. • Heat transfer: Use coupled temperature-displacement EC3D8RT Eulerian elements to model a fully coupled thermal-stress analysis. Adiabatic conditions are assumed in Eulerian materials when EC3D8R elements are used. • Output: Total strain (LE) is not available for Eulerian elements in field or history output, but it can be accessed via the utility routine VGETVRM. • Subcycling: You cannot include Eulerian elements in subcycling zones. Input file template The following example illustrates a coupled Eulerian-Lagrangian analysis of a Lagrangian boat floating on Eulerian water. A conforming mesh is assumed, so Eulerian material initialization is achieved by whole element filling. Material-specific interactions between the Lagragian body and the Eulerian materials are implemented: a contact interaction is defined between the boat and water, but contact between the boat and air is ignored. Output is requested for Eulerian volume fractions, Eulerian element-averaged stress, and material stress. *HEADING … *ELEMENT, TYPE=C3D8R, ELSET=BOAT_ELSET element definitions for Lagrangian boat *ELEMENT, TYPE=EC3D8R, ELSET=ALL_EULERIAN element definitions for whole Eulerian mesh *ELSET, NAME=AIR_ELSET data lines giving Eulerian elements that are initially filled with air *ELSET, NAME=WATER_ELSET data lines giving Eulerian elements that are initially filled with water ** *MATERIAL, NAME=AIR material definition for air *MATERIAL, NAME=WATER material definition for water ** *EULERIAN SECTION, ELSET=ALL_EULERIAN AIR WATER ** *INITIAL CONDITIONS, TYPE=VOLUME FRACTION AIR_ELSET, AIR, 1.0 WATER_ELSET, WATER, 1.0 *INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC data lines to define water pressure due to gravity ** *SURFACE, NAME=WATER_SURFACE, TYPE=EULERIAN MATERIAL WATER *SURFACE, NAME=BOAT_SURFACE BOAT_ELSET ** *STEP *DYNAMIC, EXPLICIT *DLOAD data lines to define gravity load ** *CONTACT *CONTACT INCLUSIONS BOAT_SURFACE, WATER_SURFACE ** *OUTPUT, FIELD *ELEMENT OUTPUT EVF, SVAVG, PEEQVAVG *END STEP Additional references • Benson, D. J., “Computational Methods in Lagrangian and Eulerian Hydrocodes,” Computer Methods in Applied Mechanics and Engineering, vol. 99, pp. 235–394, 1992. • Benson, D. J., “Contact in a Multi-Material Eulerian Finite Element Formulation,” Computer Methods in Applied Mechanics and Engineering, vol. 193, pp. 4277–4298, 2004. • Peery, J. S., and D. E. Carroll, “Multi-Material ALE methods in Unstructured Grids,” Computer Methods in Applied Mechanics and Engineering, vol. 187, pp. 591–619, 2000. 14.1.2 DEFINING EULERIAN BOUNDARIES Products: Abaqus/Explicit Abaqus/CAE References • “Eulerian analysis,” Section 14.1.1 • “Eulerian elements,” Section 32.14.1 • *EULERIAN BOUNDARY • “Defining an Eulerian boundary condition,” Section 16.10.21 of the Abaqus/CAE User’s Manual Overview In an Eulerian analysis you can define independent inflow and outflow conditions at an Eulerian boundary. An Eulerian boundary condition: • can be used to control the flow of material into the Eulerian domain; • can be used to define a pressure field at the boundary of an Eulerian domain; • can be used to apply a nonreflecting boundary condition at the truncated artificial boundary to simulate an infinite domain; and • is associated with a surface defined on the Eulerian mesh boundary where inflow or outflow occurs. Defining the Eulerian boundary Eulerian boundaries must be defined at surfaces on the Eulerian mesh boundary. You cannot define multiple Eulerian boundaries at the same surface. Input File Usage: *EULERIAN BOUNDARY surface name Abaqus/CAE Usage: Load module: Create Boundary Condition: Category: Other, Types for Selected Step: Eulerian boundary: select region Defining the inflow condition You can use the inflow condition to control the flow of material into the Eulerian domain. Free inflow If no Eulerian boundary is defined, material can flow into the Eulerian domain freely; and the material content and the state of each inflow material are equal to that which presently exists within the element. If an Eulerian boundary is defined, free inflow is the default inflow condition. Input File Usage: Abaqus/CAE Usage: *EULERIAN BOUNDARY, INFLOW=FREE Eulerian boundary condition editor: Flow type: Inflow, Inflow: Free No inflow You can specify an Eulerian boundary where no inflow can occur—no material or void can flow into the Eulerian domain through the specified boundary. The normal component of the velocity is set to zero if the velocity is directed inward at the boundary, while the tangential component of the velocity remains unchanged. Input File Usage: Abaqus/CAE Usage: *EULERIAN BOUNDARY, INFLOW=NONE Eulerian boundary condition editor: Flow type: Inflow, Inflow: None Void inflow You can also specify a boundary through which inflow can occur but the influx volume contains only void. Due to the inflow of void, an Eulerian domain that is initially completely full of material might become partially full during the analysis. Input File Usage: Abaqus/CAE Usage: *EULERIAN BOUNDARY, INFLOW=VOID Eulerian boundary condition editor: Flow type: Inflow, Inflow: Void Defining the outflow condition The outflow condition can be used to simulate an unbounded domain by reducing reflection at the outflow boundary or to prescribe a pressure field at the boundary. Free outflow If no Eulerian boundary condition is specified, material can flow out of the Eulerian domain freely; and the material content and the state of each outflow material are equal to that which presently exists within the element. If an Eulerian boundary condition is defined, free outflow is the default behavior if the void inflow condition is specified at the same surface. Input File Usage: Abaqus/CAE Usage: *EULERIAN BOUNDARY, OUTFLOW=FREE Eulerian boundary condition editor: Flow type: Outflow, Outflow: Free Nonreflecting outflow A nonreflecting outflow condition can be used in boundary value problems defined in unbounded domains or problems in which the region of interest is small in size compared to the surrounding medium. Like the infinite element formulation described in “Using solid medium infinite elements in dynamic analyses” in “Infinite elements,” Section 28.3.1, the nonreflecting outflow condition introduces additional normal and shear tractions on the domain boundary that are proportional to the normal and shear components of the velocity of the boundary. These boundary damping constants are chosen to minimize the reflection of dilatational and shear wave energy back into the finite element mesh. This condition does not provide perfect transmission of energy out of the mesh except in the case of plane body waves impinging orthogonally on the boundary in an isotropic medium. However, it usually provides acceptable modeling for most practical cases. An exception is the case when significant material transport occurs through the boundary, in which case this condition is not suitable to be used. Input File Usage: Abaqus/CAE Usage: *EULERIAN BOUNDARY, OUTFLOW=NONREFLECTING Eulerian boundary condition editor: Flow type: Outflow, Outflow: Nonreflecting Equilibrium outflow Equilibrium outflow is another outflow condition that can effectively reduce spurious reflection at artificial outflow boundaries in unbounded domains. It is assumed that the stress is zero-order continuous across the element faces on the boundary. Traction is applied to these element faces to balance the nodal forces created by the stress in the boundary elements. This condition is usually applied at the outflow boundary where the pressure distribution is unknown. Input File Usage: Abaqus/CAE Usage: *EULERIAN BOUNDARY, OUTFLOW=NONUNIFORM PRESSURE Eulerian boundary condition editor: Flow type: Outflow, Outflow: Equilibrium Zero-pressure outflow It is common in flow problems to specify a zero pressure at the outlet of the flow. Since the normal traction on the boundary contains the contribution from both the pressure and the shear stress, the natural boundary condition, also known as the “do-nothing condition,” is not sufficient to provide such a condition if the shear behavior of the flow is also considered. The zero pressure outflow condition applies a traction that counteracts the shear contribution and, thus, generates a uniformly distributed pressure field on the boundary. You can apply a distributed surface load on the same boundary to specify a nonzero pressure. This is the default outflow condition if the inflow condition is not specified. Input File Usage: Abaqus/CAE Usage: *EULERIAN BOUNDARY, OUTFLOW=ZERO PRESSURE Eulerian boundary condition editor: Flow type: Outflow, Outflow: Zero pressure Using Eulerian boundaries in restart analyses You can define a new Eulerian boundary in a restart analysis, but you cannot specify a void inflow condition at this boundary. In addition, you cannot change the inflow condition at an existing Eulerian boundary to the void inflow condition in a restart analysis. 14.1.3 EULERIAN MESH MOTION Products: Abaqus/Explicit Abaqus/CAE References • “Eulerian surface definition,” Section 2.3.5 • “Eulerian analysis,” Section 14.1.1 • *EULERIAN MESH MOTION • *EULERIAN SECTION • *SURFACE • “Defining an Eulerian mesh motion boundary condition,” Section 16.10.22 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview In a traditional Eulerian analysis, material flows through an Eulerian mesh that is fixed in space. Since it is stationary, the Eulerian mesh must be large enough to enclose the entire trajectory of interest. In some simulations, such as a tumbling liquid-filled bottle, this trajectory can be long, requiring a large Eulerian mesh whose elements are mostly empty. The Eulerian mesh motion feature allows the Eulerian mesh to move in space, following, expanding, and contracting to enclose a target object. This can greatly reduce mesh size and, hence, simulation cost. Mesh motion can also simplify modeling by ensuring that the entire trajectory of interest, which may be unpredictable, is indeed covered by the Eulerian mesh. Activating mesh motion You can independently activate mesh motion for each Eulerian section in a model. The motion applies to all of the elements in the section. Input File Usage: Abaqus/CAE Usage: *EULERIAN MESH MOTION, ELSET=name Load module: BC→Create, Category: Other, Types for Selected Step: Eulerian mesh motion: select an Eulerian part instance Computing mesh motion The motion of the Eulerian mesh is computed using an internally constructed bounding box that encloses the entire Eulerian section. The bounding box has six degrees of freedom: translation of the box center and scaling of each of the three box dimensions. The bounding box is constructed in a local coordinate system. Its six degrees of freedom are also defined in this local system. The local coordinate directions remain fixed in space during the simulation. If no local coordinate system is specified, the local system coincides with the global system. Input File Usage: *EULERIAN MESH MOTION, ORIENTATION= name Abaqus/CAE Usage: Load module: Eulerian mesh motion editor: Bounding Box Csys: Edit or Create Defining the target object You use a surface to define the target object that the Eulerian mesh will follow. By default, the Eulerian mesh bounding box (and, hence, the Eulerian mesh) moves to enclose the surface at all times, subject to any constraints specified on the mesh motion. If the surface type is Lagrangian, the Eulerian mesh bounding box moves to enclose the surface nodes . If the surface type is Eulerian, the Eulerian mesh bounding box moves to enclose the Eulerian material named in the surface definition . Figure 14.1.3–1 Mesh motion, where the target object is the Lagrangian bottle. Figure 14.1.3–2 Mesh motion, where the target object is the Eulerian liquid. The Eulerian mesh may not fully enclose the target object due to: • constraints on the bounding box motion; • a misalignment of the bounding box local orientation; • a mismatch between the shape of the mesh boundary and the bounding box (i.e., the Eulerian mesh is not a rectangular box); or • an inadequately sized or positioned initial Eulerian mesh. Input File Usage: Abaqus/CAE Usage: *EULERIAN MESH MOTION, SURFACE=name Load module: Eulerian mesh motion editor: Object to Follow: name Constraining Eulerian mesh motion Once the motion of the bounding box is computed, the translations and scaling factors are applied directly to the Eulerian mesh. Several types of constraints are available to restrict these motions. Conflicts between competing constraints are resolved in the following order of precedence: 1. constraining the center and faces of the mesh bounding box, 2. limiting the rate of mesh motion, 3. turning off mesh contraction, 4. centering the mesh bounding box on the target’s center of mass or bounding box center, 5. preventing mesh expansion or contraction outside the scale factor limits, 6. limiting aspect ratio changes, and 7. maintaining a buffer between the mesh and target. Constraining mesh expansion and contraction By default, the Eulerian mesh may expand or contract by an unlimited amount in each direction, as necessary to contain the target object. This can be undesirable: expansion creates large Eulerian elements that crudely approximate the shape of Eulerian objects, while contraction leads to decreased stable time increment sizes. You can apply constraints to limit the expansion and contraction independently in each local direction by specifying lower and/or upper limits on the bounding box size scale factors. For example, a maximum scale factor of 1.0 constrains the box dimension to be no larger than 1.0 times the initial box dimension, effectively prohibiting any expansion, while a minimum scale factor of 0.5 limits the box dimension to be no smaller than half its initial dimension. Input File Usage: *EULERIAN MESH MOTION scaling factor limits Abaqus/CAE Usage: Load module: Eulerian mesh motion editor: Axis n: Expansion ratio, Contraction ratio Preventing mesh contraction An additional control is available to prevent incremental contraction. If specified, the box dimensions may increase, but at no point during the simulation may they decrease below their current values. This option prevents oscillations in mesh size during simulations where the mesh is nominally expanding. Input File Usage: Abaqus/CAE Usage: *EULERIAN MESH MOTION, CONTRACT=NO Load module: Eulerian mesh motion editor: Controls: toggle off Allow mesh contraction Constraining mesh translation You can specify the motion of the center of the bounding box to be either free (default) or fixed in each of the local directions. You can also independently specify free (default) or fixed normal motion of the positive and negative box faces in the local coordinate directions. Input File Usage: Abaqus/CAE Usage: *EULERIAN MESH MOTION , face constraints center constraints Load module: Eulerian mesh motion editor: Axis n: Center position, Positive plane position, Negative plane position Centering the mesh bounding box If the motion of the mesh bounding box is unconstrained, the center of the bounding box is aligned with the center of a box enclosing the target surface. If the target surface fragments or “emits” low density material, aligning the center of the bounding box with the center of mass of the target may be advantageous. Input File Usage: Use the following option to center the mesh bounding box on the center of mass of the target object: *EULERIAN MESH MOTION, CENTER=MASS Use the following option to center the mesh bounding box on the center of the target object’s bounding box: *EULERIAN MESH MOTION, CENTER=BOUNDING BOX The center of the mesh bounding box cannot be changed in Abaqus/CAE; the center of the mesh bounding box corresponds to the center of the target object’s bounding box. Abaqus/CAE Usage: Controlling the mesh buffer around the target object The mesh moves to maintain a buffer of Eulerian elements between the target object and the bounding box. By default, this buffer is equal to twice the maximum Eulerian element size in the mesh. You can specify the buffer size as a multiple of the maximum Eulerian element size. You can also specify that the initial spacing between the target object and the mesh (set to zero where the target initially extends outside of the mesh) is used to compute the buffer size. Input File Usage: Use the following option to use a buffer equal to the initial spacing between the target object and the mesh: *EULERIAN MESH MOTION, BUFFER=INITIAL Use the following option to specify a buffer as a multiple of the maximum Eulerian element size: Abaqus/CAE Usage: *EULERIAN MESH MOTION, BUFFER= value Load module: Eulerian mesh motion editor: Controls: Buffer size: Initial or Specify Limiting aspect ratio changes Excessive mesh motion in a single direction can produce badly shaped Eulerian elements. An optional parameter is available to limit the change in maximum aspect ratio of the bounding box. By default, this limit is 10. When the aspect ratio limit is reached, motion in one local direction will induce motion in the other directions to preserve the box aspect ratio. This aspect ratio limit applies to the bounding box dimensions, not the underlying Eulerian element dimensions. Input File Usage: Abaqus/CAE Usage: *EULERIAN MESH MOTION, ASPECT RATIO MAX= value Load module: Eulerian mesh motion editor: Controls: Aspect ratio limit: value Limiting the rate of mesh motion The Eulerian mesh must not be allowed to move abruptly. A hard limit on its motion is given by the advective Courant condition, which prohibits mesh velocity larger than the material wave speed. In addition you can limit the mesh velocity to a multiple of the maximum velocity in the target object. By default, this limit is set to 1.01. Input File Usage: Abaqus/CAE Usage: *EULERIAN MESH MOTION, VMAX FACTOR= value Load module: Eulerian mesh motion editor: Controls: Mesh velocity factor: value Ignoring fragments of Eulerian material When the target object is an Eulerian material, tiny fragments can drive excessive mesh motion. You can specify a minimum Eulerian volume fraction below which Eulerian material is ignored during the mesh motion calculation. This can be particularly useful for impact calculations, where tiny fragments of an impacting, splattering projectile may be allowed to leave the Eulerian domain. The default minimum volume fraction is 0.5. Input File Usage: Abaqus/CAE Usage: *EULERIAN MESH MOTION, VOLFRAC MIN= value Load module: Eulerian mesh motion editor: Controls: Volume fraction threshold: value Limitations An Eulerian mesh can move only according to the available Eulerian mesh motion options. You cannot apply prescribed displacement boundary conditions to Eulerian nodes. DEFINING ADAPTIVE MESH REFINEMENT IN THE EULERIAN DOMAIN EULERIAN ADAPTIVE MESH REFINEMENT Product: Abaqus/Explicit References • “Eulerian analysis,” Section 14.1.1 • *ADAPTIVE MESH REFINEMENT • *EULERIAN SECTION • *EULERIAN MESH MOTION Overview The adaptive mesh refinement feature: • can refine elements locally inside an Eulerian mesh; • allows the user to define various criteria for refinement; • can remove the refinement automatically once the refinement criteria are no longer met; and • is available for Eulerian elements only. Adaptive mesh refinement In a traditional Eulerian analysis the topology of the Eulerian mesh does not change during the analysis. Although the Eulerian mesh motion feature allows the Eulerian mesh to move in space to cover areas of interest, its ability to create a nonuniformly refined mesh that changes with time is limited. The adaptive mesh refinement feature can locally refine the mesh by subdividing elements identified by user-defined criteria. This refinement can be removed automatically during the analysis once the criteria are no longer satisfied. This feature offers great savings in computational cost over an equivalent uniformly refined mesh. Activating adaptive mesh refinement You can independently activate adaptive mesh refinement for each Eulerian section in a model. The feature applies to all of the elements in the section, and these elements are equally divided into eight subelements when refined. Input File Usage: *ADAPTIVE MESH REFINEMENT, ELSET=name Setting the refinement limit When adaptive mesh refinement occurs, more elements are added to the Eulerian mesh. You can set a limit on the maximum increase in the number of elements. The default ratio of the increment is 8.0. Input File Usage: *ADAPTIVE MESH REFINEMENT, RATIO=maximum increase in number of elements/original number of elements Defining refinement criteria You must specify at least one refinement criterion. An element will be selected for refinement if any of the criteria are met. To reduce the numerical artifacts at the mesh transition boundaries (where a fine mesh meets a coarse mesh), the elements adjacent to the selected elements are also refined. The elements are coarsened once the refinement criteria are no longer met. Table 14.1.4–1 lists all the refinement criteria available in Abaqus/Explicit. Table 14.1.4–1 Refinement criteria. Refinement criteria description Refinement criteria label User-specified values Refine elements containing material interfaces VF Refine elements that are in contact with Lagrangian bodies Refine elements in which plastic deformation occurs. Not supported for the critical state (clay) plasticity model. CONT PEEQ Refine elements near a sharp density gradient DENSITY N/A N/A Critical value of the equivalent plastic strain Critical value of the density gradient, computed as the ratio between the change of density across element faces and the density of the material inside the element Input File Usage: *ADAPTIVE MESH REFINEMENT, refinement criteria label, value of the criteria 15. Particle Methods Smoothed particle hydrodynamic analyses 15.1 Smoothed particle hydrodynamic analyses • “Smoothed particle hydrodynamic analysis,” Section 15.1.1 • “Finite element conversion to SPH particles,” Section 15.1.2 SMOOTHED PARTICLE HYDRODYNAMIC ANALYSIS SPH ANALYSIS Product: Abaqus/Explicit References • “Particle elements,” Section 28.5.1 • *SOLID SECTION • *SECTION CONTROLS • *INITIAL CONDITIONS Overview Smoothed particle hydrodynamics (SPH) is a numerical method that is part of the larger family of meshless (or mesh-free) methods. For these methods you do not define nodes and elements as you would normally define in a finite element analysis; instead, only a collection of points are necessary to represent a given body. In smoothed particle hydrodynamics these nodes are commonly referred to as particles or pseudo-particles. Smoothed particle hydrodynamics is a fully Lagrangian modeling scheme permitting the discretization of a prescribed set of continuum equations by interpolating the properties directly at a discrete set of points distributed over the solution domain without the need to define a spatial mesh. The method’s Lagrangian nature, associated with the absence of a fixed mesh, is its main strength. Difficulties associated with fluid flow and structural problems involving large deformations and free surfaces are resolved in a relatively natural way. The method has received substantial theoretical support since its inception (Gingold and Monaghan, 1977), and the number of publications related to the method is now very large. A number of references are listed below. At its core, the method is not based on discrete particles (spheres) colliding with each other in compression or exhibiting cohesive-like behavior in tension as the word particle might suggest. Rather, it is simply a clever discretization method of continuum partial differential equations. In that respect, smoothed particle hydrodynamics is quite similar to the finite element method. The method can use any of the materials available in Abaqus/Explicit (including user materials). You can specify initial conditions and boundary conditions as for any other Lagrangian model. Contact interactions with other Lagrangian bodies are also allowed, thus expanding the range of applications for which this method can be used. The method is less accurate in general than Lagrangian finite element analyses when the deformation is not too severe and than coupled Eulerian-Lagrangian analyses in higher deformation regimes. If a large percentage of all nodes in the model are associated with smoothed particle hydrodynamics, the analysis may not scale well if multiple CPUs are used. Applications Smoothed particle hydrodynamic analyses are effective for applications involving extreme deformation. Fluid sloshing, wave engineering, ballistics, spraying (as in paint spraying), gas flow, and obliteration and fragmentation followed by secondary impacts are a few examples. There are many applications for which both the coupled Eulerian-Lagrangian and the smoothed particle hydrodynamic methods can be used. In many coupled Eulerian-Lagrangian analyses the material to void ratio is small and, consequently, the computational effort may be prohibitively high. In these cases, the smoothed particle hydrodynamic method is preferred. For example, tracking fragments from primary impacts through a large volume until secondary impact occurs can be very expensive in a coupled Eulerian-Lagrangian analysis but comes at no additional cost in a smoothed particle hydrodynamic analysis. “Impact of a water-filled bottle,” Section 2.3.2 of the Abaqus Example Problems Manual, includes an example of using the smoothed particle hydrodynamic method to model the violent sloshing associated with the impact. Artificial viscosity Artificial viscosity in smoothed particle hydrodynamics has the same meaning as bulk viscosity for finite elements. Similar to other Lagrangian elements, particle elements use linear and quadratic viscous contributions to dampen high frequency noise from the computed response. In rare cases when the default values are not appropriate, you can control the amount of artificial viscosity included in a smoothed particle hydrodynamic analysis. Input File Usage: Use the following options to specify scale factors for the linear and quadratic artificial viscosities: *SECTION CONTROLS , , , scale factor for linear artificial viscosity, scale factor for quadratic artificial viscosity Initial conditions “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, describes all of the initial conditions that are available for an explicit dynamic analysis. Initial conditions pertinent to mechanical analyses can be used in a smoothed particle hydrodynamic analysis. Boundary conditions Boundary conditions are defined as described in “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Loads The loading types available for an explicit dynamic analysis are explained in “Applying loads: overview,” Section 33.4.1. Concentrated nodal loads can be applied as usual. Gravity loads are the only distributed loads allowed in a smoothed particle hydrodynamic analysis. Material options Any of the material models in Abaqus/Explicit can be used in a smoothed particle hydrodynamic analysis. Elements The smoothed particle hydrodynamic method is implemented via the formulation associated with PC3D elements. These 1-node elements are simply a means of defining particles in space that model a particular body or bodies. These particle elements utilize existing functionality in Abaqus to reference element- related features such as materials, initial conditions, distributed loads, and visualization. You define these elements in a similar fashion as you would define point masses. The coordinates of these points lie either on the surface or in the interior of the body being modeled, similar to the nodes of a body meshed with brick elements. For more accurate results, you should strive to space the nodal coordinates of these particles as uniformly as possible in all directions. An alternative to directly defining PC3D elements is to define conventional continuum finite element types C3D8R, C3D6, or C3D4 and automatically convert them to particle elements at the beginning of the analysis or during the analysis, as discussed in “Finite element conversion to SPH particles,” Section 15.1.2. The smoothed particle hydrodynamic method implemented in Abaqus/Explicit uses a cubic spline as the interpolation polynomial and is based on the classical smoothed particle hydrodynamic theory as outlined in the references below. The smoothed particle hydrodynamic method is not implemented for two-dimensional elements. Axisymmetry can be simulated using a wedge-shaped sector and symmetry boundary conditions. There are no hourglass or distortion control forces associated with PC3D elements. These elements do not have faces or edges associated with them. SPH kernel interpolator By default, the smoothed particle hydrodynamic method implemented in Abaqus/Explicit uses a cubic spline as the interpolation polynomial. Alternatively, you can choose a quadratic (Johnson et al, 1996) or quintic (Wendland, 1995) interpolator. The implementation is based on the classical smoothed particle hydrodynamic theory as outlined in the references below. You also have the option of using a mean flow correction configuration update, commonly referred to in the literature as the XSPH method , as well as the corrected kernel of Randles and Libersky, 1997, also referred to as the normalized SPH (NSPH) method. You can control these settings as discussed in “Using section controls for smoothed particle hydrodynamics (SPH)” in “Section controls,” Section 27.1.4. Computing the particle volume There is currently no capability to automatically compute the volume associated with these particles. Hence, you need to supply a characteristic length that will be used to compute the particle volume, which in turn is used to compute the mass associated with the particle. It is assumed that the nodes are distributed uniformly in space and that each particle is associated with a small cube centered at the particle. When stacked together, these cubes will fill the overall volume of the body with some minor approximation at the free surface of the body. The characteristic length is half the length of the cube side. From a practical perspective, once you have created the nodes, you can use the half-distance between two nodes as the characteristic length. Alternatively, if you know the mass and density of the part, you can compute the volume of the part and divide it by the total number of particles in the part to obtain the volume of the small cube associated with each particle. Half of the cubic root of this small volume is a reasonable characteristic length for this particle set. You can check the mass of individual sets in the model if you request that model definition data be printed to the data (.dat) file . Input File Usage: Use the following options to define a smoothed particle hydrodynamic body: *ELEMENT, TYPE=PC3D, ELSET=particle_body element number, node number Repeat the data line as often as necessary. *SOLID SECTION, ELSET=particle_body, MATERIAL=material_name characteristic length associated with particle volume Smoothing length calculation Even though particle elements are defined in the model using one node per element, the smoothed particle hydrodynamic method computes contributions for each element based on neighboring particles that are within a sphere of influence. The radius of this sphere of influence is referred to in the literature as the smoothing length. The smoothing length is independent of the characteristic length discussed above and governs the interpolation properties of the method. By default, the smoothing length is computed automatically. As the deformation progresses, particles move with respect to each other and, hence, the neighbors of a given particle can (and typically do) change. Every increment Abaqus/Explicit recomputes this local connectivity internally and computes kinematic quantities (such as normal and shear strains, deformation gradients, etc.) based on contributions from this cloud of particles centered at the particle of interest. Stresses are then computed in a similar fashion as for reduced-integration brick elements, which are in turn used to compute element nodal forces for the particles in the cloud based on the smoothed particle hydrodynamic formulation. By default, Abaqus/Explicit computes a smoothing length at the beginning of the analysis such that the average number of particles associated with an element is roughly between 30 and 50. The smoothing length is kept constant during the analysis. Therefore, the average number of particles per element can either decrease or increase during the analysis depending on whether the average behavior in the model is expansive or compressive, respectively. If the analysis is mostly compressive in nature, the total number of particles associated with a given element might exceed the maximum allowed and the analysis will be stopped. By default, the maximum number of allowed particles associated with one element is 140. You can control most of these settings as discussed in “Using section controls for smoothed particle hydrodynamics (SPH)” in “Section controls,” Section 27.1.4. Smoothed particle hydrodynamic domain A rectangular region is computed at the beginning of the analysis as the bounding box within which the particles will be tracked. This fixed rectangular box is 10% larger than the overall dimensions of the whole model, and it is centered at the geometric center of the model. As the analysis progresses, if a particle is outside this box, it behaves like a free-flying point mass and does not contribute to smoothed particle hydrodynamic calculations. If the particle reenters the box at a later stage, it is once again included in the calculations. You can modify the size of the bounding box as discussed in “Using section controls for smoothed particle hydrodynamics (SPH)” in “Section controls,” Section 27.1.4. Constraints Since the PC3D elements are Lagrangian elements, their nodes can be involved in other features, such as other elements, connectors, or constraints. Since these elements do not have faces or edges, an element- based surface cannot be defined using PC3D elements. Consequently, constraints that require element- based surfaces (such as fasteners) cannot be defined for particles. Interactions Bodies modeled with particles can interact with other finite element meshed bodies via contact. The contact interaction is the same as any contact interaction between a node-based surface (associated with the particles) and an element-based or analytical surface. Both general contact and contact pairs can be used. All interaction types and formulations available for contact involving a node-based surface are allowed, including cohesive behavior. Different contact properties can be assigned via the usual options. By default, the particles are not part of the general contact domain similar to other 1-node elements (such as point masses). The default contact thickness for particles is the same value specified as the characteristic length on the section definition; thus, for contact purposes, particles behave as spheres with radii equal to the radius of a sphere inscribed in the small cube associated with the particle volume as described above. You should not specify a contact thickness of zero for the nodes associated with PC3D elements or contact may not be resolved robustly. The recommended approach is to use the default or specify a reasonable contact thickness. Interaction between different bodies all modeled with PC3D elements is allowed. However, this interaction is meaningful only in cases when the colliding smoothed particle hydrodynamic bodies are made of the same fluid-like material, such as a water drop falling in a bucket partially filled with water. In solids-related applications, such as modeling a bullet perforating an armor plate, one of the bodies must be modeled using regular finite elements. Contact interactions cannot be defined between particles and Eulerian regions. Input File Usage: Output Use the following options to define contact between a meshed or analytical surface with a particle-based surface: *CONTACT *CONTACT INCLUSIONS node-based particle surface, element-based/analytical_surface The element output available for PC3D elements includes all mechanics-related output for continuum elements: stress; strain; energies; and the values of state, field, and user-defined variables. The nodal output includes all output variables generally available in Abaqus/Explicit analyses. Particles can be visualized in Abaqus/CAE via circular discs. In contour plots the values of field output variables are shown as circular patches of color. Symbol plots are also available. Limitations Smoothed particle hydrodynamic analyses are subject to the following limitations: • They are less accurate in general than Lagrangian finite element analyses when the deformation is not too severe and the elements are not distorted. In higher deformation regimes coupled Eulerian- Lagrangian analyses are also generally more accurate. The smoothed particle dynamic method should be used primarily in cases when the conventional finite element method or the coupled Eulerian-Lagrangian method have reached their inherent limitations or are prohibitively expensive to perform. • When the material is in a state of tensile stress, the particle motion may become unstable leading to the so-called tensile instability. This instability, which is strictly related to the interpolation technique of the standard smoothed particle dynamic method, is especially noticeable when simulating the stretched state of a solid. As a consequence, particles tend to clump together and show fracture-like behavior. • Mass distribution in a body defined with particle elements is somewhat different when compared to the mass distribution of the same body defined with continuum elements, such as C3D8R elements. When particle elements are used, the volume of all particles in that body are the same. Consequently, the nodal mass associated with all particles in that body is the same. If the nodes are not placed in a regular cubic arrangement, the mass distribution is somewhat inexact, particularly at the free surface of the body being modeled. • Surface loads cannot be specified on PC3D elements. However, distributed loads, such as pressure, can be applied to other finite element surfaces that can apply a pressure onto the particle elements via contact interactions. • Bodies modeled with particles that were not defined using the same section definition do not interact with each other. Hence, you cannot use smoothed particle hydrodynamics to model the mixing of bodies with dissimilar materials. • The functionality is not supported in Abaqus/CAE. You can use the existing functionality in Abaqus/CAE to generate mass elements, write an input file, and then manually edit the input file to convert the mass elements to particles. Alternatively, you can create a mesh using C3D8R elements, write an input file, and then use a script to convert these elements to particles as described in “Generating particle elements from a solid mesh” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com. • If a large percentage of all nodes in the model are associated with smoothed particle hydrodynamics, the analysis may not scale well if multiple CPUs are used. • Within a given body (part) defined via one solid section definition, gravity loads and mass scaling cannot be specified selectively on a subset of elements referenced by this definition. Instead, the two features must be applied to all the elements in the element set associated with the solid section definition. Input file template The following example illustrates a smoothed particle hydrodynamic analysis of a bottle filled with fluid being dropped on the floor. The plastic bottle and the floor are modeled with conventional shell elements. The fluid is modeled via smoothed particle hydrodynamics using PC3D elements. The nodal coordinates of the particles are defined such they are all located inside the bottle. Material property definitions are defined as usual for both the fluid and the bottle. Contact interaction is defined between the smoothed particle hydrodynamic particles representing the water (node-based surface) and the interior walls of the bottle and also between the bottle exterior and the floor using element-based surfaces (not shown). Output is requested for stresses (pressure) and density in the fluid. *HEADING … *ELEMENT, TYPE=PC3D, ELSET=Fluid_Inside_The_Bottle Element number, node number … *SOLID SECTION, ELSET=Fluid_Inside_The_Bottle, MATERIAL=Water Element characteristic length associated with particle volume *MATERIAL, NAME=Water Material definition for water, such as an EOS material *ELEMENT, TYPE=S4R, ELSET=Plastic_Bottle Element definitions for the shells ** *INITIAL CONDITIONS, TYPE=VELOCITY Data lines to define velocity initial conditions *NSET, NSET=Water_Nodes, ELSET=Fluid_Inside_The_Bottle *SURFACE, NAME=Water_Surface, TYPE=NODE Water_Nodes, *SURFACE, NAME=Bottle_Interior Plastic_Bottle, SNEG ** *STEP *DYNAMIC, EXPLICIT *DLOAD Data lines to define gravity load ** *CONTACT *CONTACT INCLUSIONS Water_Surface, Bottle_Interior ** *OUTPUT, FIELD *ELEMENT OUTPUT, ELSET=Fluid_Inside_The_Bottle S, DENSITY *END STEP Additional references • Gingold, R. A., and J. J. Monaghan, “Smoothed Particle Hydrodynamics: Theory and Application to Non-Spherical Stars,” Royal Astronomical Society, Monthly Notices, vol. 181, pp. 375–389, 1977. • Johnson, J., R. Stryk, and S. Beissel, “SPH for High Velocity Impact Calculations,” Computer Methods in Applied Mechanics and Engineering, 1996. • Libersky, L. D., and A. G. Petschek, “High Strain Lagrangian Hydrodynamics,” Journal of Computational Physics, vol. 109, pp. 67–75, 1993. • Monaghan, Astrophysics, 1992. J., “Smoothed Particle Hydrodynamics,” Annual Review of Astronomy and • Munjiza, A., and K. R. F. Andrews, “NBS Contact Detection Algorithm for Bodies of Similar Size,” International Journal for Numerical Methods in Engineering, vol. 43, pp. 131–149, 1998. • Randles, P. W., and L. D. Libersky, “Recent Improvements in SPH Modeling of Hypervelocity Impact,” International Journal of Impact Engineering, 1997. • Swegle, J. W., and S. W. Attaway, “An Analysis of Smoothed Particle Hydrodynamics,” Sandia National Lab Report SAND93–2513, 1994. • Wendland, H., “Piecewise Polynomial, Positive Definite and Compactly Supported Radial Functions of Minimal Degree,” Advances in Computational Mathematics, 1995. 15.1.2 FINITE ELEMENT CONVERSION TO SPH PARTICLES Products: Abaqus/Explicit Abaqus/CAE References • “Particle elements,” Section 28.5.1 • *CONTACT • *INITIAL CONDITIONS • *OUTPUT • *SECTION CONTROLS • *SOLID SECTION Overview You can take advantage of the intrinsic strengths of both Lagrangian finite element and SPH methods when modeling a body. You can define the model with Lagrangian finite elements and convert them to SPH particles either at the beginning of an analysis or after the deformation becomes significant. It is sometimes easier to create the mesh with Lagrangian finite elements, and Lagrangian finite elements are often more accurate for small deformations. SPH methods are well suited for large deformation. You start by defining a part as usual. You mesh the part with C3D8R, C3D6, or C3D4 reduced- integration elements or a combination of these elements. You then specify that these “parent” elements are to convert to internally generated SPH particles when a user-specified criterion is met. Gravity loads, contact interactions, initial conditions, mass scaling, and output requests associated with the parent elements or nodes of the parent elements will be transferred appropriately to the generated particles upon conversion in an intuitive way as explained below. A special formulation is used to ensure the smoothest possible transition between the two modeling methods. The technique can use any of the materials available in Abaqus/Explicit (including user materials). Activating the conversion to SPH particles functionality The element conversion to particles functionality is not active by default. The conversion functionality is intended to be used when the deformations in the original finite element mesh are significant and elements may distort. Traditionally, in such cases deletion of the soon-to-be distorted Lagrangian elements would be the only choice to allow the analysis to continue. Converting to SPH particles offers an improvement over the element deletion option because the generated particles are able to provide resistance to deformation beyond finite element distortion levels. Consequently, element deletion cannot be used together with element conversion. You can control the number of particles generated per parent element and choose between one of four criteria to specify when the conversion is to be triggered. Input File Usage: *SECTION CONTROLS, ELEMENT CONVERSION=YES Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Conversion to particles: Yes Specifying the number of particles to be generated By default, one particle is generated per parent element. You can control the number of particles generated per element by specifying the number of particles to be generated per parent element isoparametric direction. The total number of particles generated per element depends on the element type that is being converted. For example, if you specify 3 particles to be generated per isoparametric direction, upon conversion 27 particles would be generated from a C3D8R element, 18 from a C3D6 element, and 10 from a C3D4 element, as illustrated in Figure 15.1.2–1. A maximum value of seven particles per direction can be specified. The particles are evenly spaced inside the parent element such that they fill the volume as uniformly as possible. For example, if cubic parent elements are stacked in the user-defined mesh, the particles would be evenly spaced throughout the part. You can control the number of particles generated per isoparametric direction as discussed in “Using section controls to convert continuum elements to particles” in “Section controls,” Section 27.1.4. Figure 15.1.2–1 Internally generated particles per parent element illustrated for three particles per isoparametric direction. Time-based criterion You can specify the time when the conversion of all the elements in the affected element set is to take place regardless of the deformation levels. This option is intended for applications where the SPH functionality is the preferred modeling method, such as fluid sloshing in a tank or a synthetic bird strike on an aircraft. If the conversion time is specified as zero, the conversion takes place at the beginning of the analysis. For example, fluid sloshing is a good candidate for using a time-based criterion if sloshing is expected to start at the beginning of the analysis. You can specify a later time at which the conversion takes place if extreme deformations do not occur until later in the analysis. A bird strike analysis is a potential candidate as the bird might travel for some time without any deformation prior to hitting the intended target. You can control the time when the conversion is to occur as discussed in “Using section controls to convert continuum elements to particles” in “Section controls,” Section 27.1.4. Strain-based criterion You can specify the absolute value of the maximum principal strain when the conversion of a given element is to take place. As elements deform, if the absolute value of the maximum principal strain is greater than the specified threshold, the parent elements will convert progressively to SPH particles. This option is intended for applications where the finite element method is the preferred modeling method but severe deformations could occur in certain regions. Examples include blast applications and crushing. You can control the strain-based threshold upon which conversion is to occur as discussed in “Using section controls to convert continuum elements to particles” in “Section controls,” Section 27.1.4. Stress-based criterion You can specify the absolute value of the maximum principal stress value at which the conversion of a given element takes place. As elements deform, if the absolute value of the maximum principal stress is greater than the specified threshold, the parent elements will convert progressively to SPH particles. This option is intended for the same candidate applications as those discussed for the strain-based criterion. You can control the stress-based threshold upon which conversion is to occur as discussed in “Using section controls to convert continuum elements to particles” in “Section controls,” Section 27.1.4. User subroutine–based criterion The user subroutine–based criterion provides the flexibility of a user subroutine implementation that allows you to implement your own conversion criterion. Element conversion can be controlled during the course of an Abaqus/Explicit analysis through any of the user subroutines that can actively modify state variables associated with a material point, such as VUSDFLD and VUMAT. You specify the state variable number controlling the element conversion flag. For example, specifying a state variable number of two indicates that the second state variable is the conversion flag in the user subroutine. The conversion state variable should be set to a value of one or zero. A value of one indicates that the element is active, while a value of zero indicates that Abaqus/Explicit should convert the element to particles. Since user subroutines have access via arguments (or in the case of the VUSDFLD subroutine via utility routines) to material point state data, the functionality provides a comprehensive means to define the conversion state variable. Input File Usage: Use the following options to define a user subroutine–based conversion criterion: *SECTION CONTROLS, ELEMENT CONVERSION=YES, CONVERSION CRITERION=USER ... *MATERIAL *DEPVAR, CONVERT=variable number Abaqus/CAE Usage: Specifying a user subroutine–based criterion for element conversion is not supported in Abaqus/CAE. Conversion to particles formulation When using the conversion technique, particles are generated internally at the beginning of the preprocessing phase of the analysis, and they are placed in an inactive or dormant state. The particles are attached to the parent elements in a similar fashion as the nodes of embedded elements are attached , and they follow the motion of the parent element nodes in an average sense. The inertial properties of the particles in this inactive state (while the parent finite elements are active) are automatically disregarded to avoid doubling the momentum at a given location. Similar to SPH particles defined directly as PC3D elements, particles generated from parent element sets associated with different section definitions will not interact with each other. Upon conversion a number of internally generated particles per parent element are activated, as illustrated for various element types in Figure 15.1.2–1. The computational cost of the analysis can increase significantly after conversion takes place if a large number of particles are generated per element since a larger number of active elements needs to be processed. In addition, the computational cost increases because the stable time increment associated with the internally generated particles decreases as the particle density increases. Upon conversion the state information (such as stress or equivalent plastic strain) associated with the element being converted is transferred to the generated particles to ensure the smoothest possible transition. The activated particles will interact via the SPH formalism with both the previously activated particles and the neighboring inactive particles that are still embedded in active parent elements. Automatically generated sets and surfaces Since the particles are generated internally, you do not have the ability to define element sets, node sets, or surfaces associated with these particles. Consequently, a number of sets and surfaces are created internally for convenience. You can visualize these internal sets and surfaces via the usual techniques. Table 15.1.2–1, Table 15.1.2–2, and Table 15.1.2–3 describe the internally generated sets and surfaces. Table 15.1.2–1 Internally generated element sets. Internally generated element set Description ALL_GENERATED_ELEMENTS_SPH All generated SPH particles in the entire model ALL_PARENT_ELEMENTS_SPH All parent elements in the entire model Internally generated element set Description UserDefinedElsetName_SECT_SPH UserDefined_AElsetName_SPH All generated particles associated with the UserDefinedElsetName element set used in the section definition All generated particles associated with the element set UserDefined_AElsetName Table 15.1.2–2 Internally generated node sets. Internally generated node set Description ALL_PARENT_ELEMENT_NODES_E_SPH ALL_GENERATED_NODES_SPH UserDefinedElsetName_SECT_E_SPH UserDefined_ANsetName_SPH All nodes of all parent elements in the entire model All nodes of all generated particles in the entire model All nodes of generated particles associated with the UserDefinedElsetName element set used in the section definition Nodes of generated particles from parent elements touching nodes of the UserDefined_ANsetName node set Table 15.1.2–3 Internally generated surfaces. Internally generated surfaces Description UserDefinedElsetName_PARENT_EE_SPH UserDefinedElsetName_SECT_NE_SPH UserDefinedSurfaceName_NS_SPH Element-based surface containing all facets of all elements associated with the UserDefinedElsetName element set used in the section definition Node-based surface with all nodes of all generated particles associated with the UserDefinedElsetName element set used in the section definition Node-based surface containing all nodes of generated particles associated with the elements used in the definition of the UserDefinedSurfaceName element-based surface These sets and surfaces are used by features that are automatically generated internally, such as loads, initial conditions, mass scaling, contact definitions, and output requests. These internally generated features extend the features that you have defined for the associated parent sets and surfaces to internally generated particles. In all cases the internally generated features preserve the attributes that you have defined. Initial conditions Initial conditions cannot be specified directly for the generated particles. However, a subset of the possible initial conditions (stresses, velocity and rotating velocity) is applied to the generated particles automatically. You specify these initial conditions on the original element or node set you have defined in the model, and they are applied appropriately to the associated generated particles. The initial conditions are applied via the internally created sets described above; hence, you must use an element or node set rather than element or node numbers when applying initial conditions. Initial stresses specified on parent elements are applied to the generated particles. This feature is leveraged in cases where parent elements convert to particles at the very beginning of the analysis (time zero). All other initial conditions associated with elements are taken into account for the generated particles as long as the parent elements convert to particles after the first increment in the analysis. The state transfer mechanism described above appropriately transfers the information to particles and, hence, initial conditions are accounted for correctly in the particles. Boundary conditions cannot be applied directly to the generated particles. Boundary conditions applied to nodes of the parent elements are not transferred to the generated particles. However, you can use contact interactions to enforce boundary conditions as explained in “Interactions.” Temperature and field variables specified on node sets that include parent element nodes are extended to the generated particles. Abaqus/Explicit generates corresponding temperature and field variables definitions internally via the internal node sets described in “Automatically generated sets and surfaces.” If all of the nodes of a particular parent element have the same value at a given time, the generated particles would have that same value as well. If different values are specified, no interpolation occurs. Instead, the value of the last definition is used. Loads The loading types available for an explicit dynamic analysis are explained in “Applying loads: overview,” Section 33.4.1. Concentrated nodal loads cannot be applied to generated particles. Gravity loads specified on the parent elements are the only distributed loads that are transferred upon conversion to the generated particles. Material options Any of the material models in Abaqus/Explicit can be used with the conversion technique. Elements When using the conversion technique and C3D8R, C3D6, and/or C3D4 reduced-integration parent elements to define the part, PC3D elements are generated internally at the beginning of the analysis; the parent elements are active, and the PC3D elements are inactive. Upon conversion the active status switches. At no time are a parent element and the associated generated particles both active. By default, the Visualization module automatically displays only the elements that are active at any given time. Particle mass (and volume) is computed automatically from the mass (volume) of the parent element. All particles associated with a specific parent element will have the same mass (volume). The SPH smoothing length and domain required for the SPH formalism are computed in the same fashion as in the case when you define PC3D elements directly . If mass scaling is defined on element sets containing parent elements, Abaqus/Explicit internally generates mass scaling definitions associated with the corresponding internal element sets described in “Automatically generated sets and surfaces.” Constraints Constraints such as couplings or ties cannot be applied directly to the generated particles. However, constraints can be defined on nodes and surfaces associated with the parent element nodes and faces. If such constraints are used to attach parent elements to other Lagrangian bodies or they are used to drive the motion of a part, care must be exercised when the parent element faces involved in such constraints convert to particles. The constraint may be nullified upon parent element conversion and, consequently, the connection to other parts (in the case of tie constraints) or to the driving feature (in the case of coupling constraints) would no longer be realized. Hence, in certain cases you may need to place these constraints far enough from the parent elements that can convert for the constraints to be active throughout the analysis. Element sets that are marked for possible conversion to particles but that are also part of the rigid body definition will never convert because the rigid body constraint is always enforced on the parent elements. Interactions Bodies modeled with elements that may convert to particles can interact with other finite element–meshed or analytical bodies via contact. Upon conversion the internally generated particles may also interact via contact with these bodies but only via the general contact functionality. By default, if general contact interactions are included in your model, contact inclusions and exclusions involving internal node-based surfaces associated with the internal particles are generated. inclusions and exclusions referencing element-based surfaces that include User-specified contact convertible elements will also be reflected in internally generated requests. Table 15.1.2–4 and Table 15.1.2–5 show all correspondences. The naming convention used for the internally generated surfaces is explained in “Automatically generated sets and surfaces” above. Table 15.1.2–4 Internally generated contact inclusions. User-defined contact inclusion Internally generated contact inclusions *CONTACT INCLUSIONS, ALL EXTERIOR blank, AllUserElsets_SECT_NE_SPH blank, UserElemBased blank, UserElemBased_NS_SPH UserElemBased, None UserElemBased1, UserElemBased2 UserElemBased1, UserElemBased2_NS_SPH and UserElemBased2, UserElemBased1_NS_SPH Table 15.1.2–5 Internally generated contact exclusions. User-defined contact exclusion Internally generated contact exclusions Always, regardless of user definitions UserElemBased_PARENT_EE_SPH, UserElemBased_SECT_NE_SPH blank, UserElemBased blank, UserElemBased_NS_SPH UserElemBased, None UserElemBased1, UserElemBased2 UserElemBased1, UserElemBased2_NS_SPH and UserElemBased2, UserElemBased1_NS_SPH As shown in the second row of Table 15.1.2–5, contact between the generated particles and the faces of the associated parent elements is always excluded from the general contact domain. The activated internal particles will interact with the neighboring yet inactive particles still attached to parent elements with exposed faces via the SPH formalism. The contact interaction for the generated particles is the same as any contact interaction between a node-based surface (associated with the internal particles) and an element-based or analytical surface. All interaction types and formulations available for contact involving a node-based surface are allowed, including cohesive behavior. Different contact properties can be assigned via the usual options. The contact control and property assignment options used for pairs of surfaces that involve parent elements that can convert to particles will be reflected in internally generated assignments for the internal particle- based surfaces. Table 15.1.2–6 shows the internally generated assignments associated with user-defined requests. Table 15.1.2–6 Internally generated contact control and property assignments. User-defined contact inclusion Internally generated contact inclusions blank, blank blank, AllUserElsets_SECT_NE_SPH blank, UserElemBased blank, UserElemBased_NS_SPH UserElemBased, UserElemBased, UserElemBased_NS_SPH UserElemBased1, UserElemBased2 UserElemBased1, UserElemBased2_NS_SPH and UserElemBased2, UserElemBased1_NS_SPH The generated particles may have different contact thicknesses since they are computed automatically at the beginning of the analysis. If one or two particles per isoparametric direction are requested to be generated upon conversion, all generated particles will have a contact thickness such that they are barely touching the closest face of the parent element. If three or more particles per direction are requested, some of the particles will not be touching the faces of the parent element. For these particles, the contact thickness will be the minimum thickness of all of the particles that are touching the parent element faces on that parent element. You can specify the contact thickness of the generated particles by using the surface property assignment option for an element-based surface that includes the faces of the parent elements. This modeling choice affects contact interactions on parent elements before they convert. Output Output requests associated with parent elements, nodes of parent elements, or contact involving faces of parent elements trigger the creation of output requests associated with the corresponding internally generated particles. For example, if you request element output for an element set that contains parent elements, Abaqus/Explicit automatically creates an additional element output request using the corresponding internal element set containing generated particles, as described in “Automatically generated sets and surfaces.” A field output request for the STATUS output variable is created automatically for all parent elements and generated particles. The value of the STATUS output variable is toggled automatically between a value of zero and one upon conversion for both parent and generated particles. By default, only the active elements are displayed in the Visualization module. In addition, contour and vector plots are displayed appropriately on the elements that are currently active. History output requests are also replicated for the generated particles. Since the actual element or node numbers of generated particles are defined internally, you can query the actual number of a particle in the Visualization module before identifying which output curve to display. For example, assume that you requested equivalent plastic strain history output for a small element set containing three C3D8R parent elements and that you requested that two particles per isoparametric direction (eight particles per parent element) are to be generated upon conversion. Before conversion you would have 3 curves to analyze; but after the three elements are converted, there are 24 curves from which to choose. You can query the element number of a particle and then select that curve from the 24 available history curves. Before conversion the curves associated with the particles have a value of zero. Upon conversion there will be a jump to the equivalent plastic strain value at the current time. Limitations Analyses involving finite element conversion to SPH particles are subject to the following limitations: • Only reduced-integration continuum elements C3D8R, C3D6, and C3D4 are available for conversion. • Surface loads specified on the faces of parent elements that convert during the analysis are not applied after conversion to particles. However, distributed loads, such as pressure, can be applied to other finite element surfaces that do not convert (e.g., on a piston surface) that can apply a pressure onto the particle elements (e.g., the fluid pushed by the piston) via contact interactions. • Bodies modeled with elements that may convert to particles that were not defined using the same section definition will not interact with each other between the converted portions of the bodies. For example, body A and body B allow elements to convert to particles, but these elements are associated with different section definitions. After conversion, the particles will not interact. • Within a given body (part) defined via one solid section definition, gravity loads and mass scaling cannot be specified selectively on a subset of elements referenced by this definition. Instead, the two features must be applied to all the elements in the element set associated with the solid section definition. Input file template The following example illustrates a smoothed particle hydrodynamic analysis of a bottle filled with fluid being dropped on the floor using the conversion technique. The plastic bottle and the floor are modeled with conventional shell elements. The fluid is modeled with C3D4 elements that will convert to two particles per isoparametric direction (four particles per element) at the beginning of the analysis based on a time-based criterion. Material property definitions are defined as usual for both the fluid and the bottle. Contact interaction is defined using the default options. Output is requested for stresses (pressure) and density in the fluid. *HEADING … *ELEMENT, TYPE=C3D4, ELSET=Fluid_Inside_The_Bottle … *SOLID SECTION, ELSET=Fluid_Inside_The_Bottle, MATERIAL=Water, CONTROLS=Time_Based_Conversion *SECTION CONTROLS, ELEMENT CONVERSION=YES, CONVERSION CRITERION=TIME, NAME=Time_Based_Conversion First data line Second data line Third data line 2, 0.0 *MATERIAL, NAME=Water Material definition for water, such as an EOS material *ELEMENT, TYPE=S4R, ELSET=Plastic_Bottle Element definitions for the shells ** *INITIAL CONDITIONS, TYPE=VELOCITY Data lines to define velocity initial conditions ** *STEP *DYNAMIC, EXPLICIT *DLOAD Data lines to define gravity load ** *CONTACT *OUTPUT, FIELD *ELEMENT OUTPUT, ELSET=Fluid_Inside_The_Bottle S, DENSITY *END STEP 16. Sequentially Coupled Multiphysics Analyses Sequentially coupled multiphysics analyses 16.1 Sequentially coupled multiphysics analyses • “Predefined fields for sequential coupling,” Section 16.1.1 • “Sequentially coupled thermal-stress analysis,” Section 16.1.2 • “Predefined loads for sequential coupling,” Section 16.1.3 16.1.1 PREDEFINED FIELDS FOR SEQUENTIAL COUPLING Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Sequentially coupled thermal-stress analysis,” Section 16.1.2 • “Predefined fields,” Section 33.6.1 • “Creating and modifying output requests,” Section 14.4.5 of the Abaqus/CAE User’s Manual • “Defining a temperature field,” Section 16.11.9 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The time history of the following nodal output quantities, generated in an Abaqus/Standard analysis, can be read into subsequent Abaqus/Standard analyses as predefined fields for sequentially coupled multiphysics workflows: • Temperature • Normalized concentration • Electric potential A sequentially coupled multiphysics analysis can be used when the coupling between one or more of the physical fields in a model is only important in one direction—a special common case is a sequential thermal-stress analysis (“Sequentially coupled thermal-stress analysis,” Section 16.1.2). While the uncoupled thermal-stress analysis is the most common sequential multiphysics workflow, the predefined field capability in Abaqus/Standard directly supports similar sequential workflows involving normalized concentrations (“Mass diffusion analysis,” Section 6.9.1) and electric potentials (“Coupled thermal-electrical analysis,” Section 6.7.3). As with temperatures, normalized concentrations and electric potentials can be read from the output database (.odb) file into subsequent analyses as predefined fields. When defined by results from a previous analysis, predefined fields typically vary with position and are time dependent—they are predefined because they are not changed by the current analysis. When predefined fields are read from a previous analysis, they are read in at the nodes. They are then interpolated within elements as needed . Any number of predefined fields can be read in, and material properties can be defined to depend on them. In addition, volumetric strain will arise in a stress analysis if thermal expansion (“Thermal expansion,” Section 26.1.2) or field expansion (“Field expansion,” Section 26.1.3) are included in the material property definition. Predefined fields may affect the system response through: • the constitutive behavior, such as the yield stress defined as a function of temperature or field variables; or • volumetric strains when thermal or field expansion behaviors (“Thermal expansion,” Section 26.1.2, and “Field expansion,” Section 26.1.3) are included in the material definition in a stress/displacement analysis. Saving temperatures, normalized concentrations, and electric potentials for predefined fields in subsequent analyses Nodal temperatures, normalized concentrations, and electrical potentials can be stored as functions of time for use in subsequent analyses. Temperatures can be stored in either the results (.fil) file or the output database (.odb) file, but normalized concentrations and electrical potentials can be used only if they are stored in the output database file. Saved values must be read into the new analyses as predefined fields. See “Node output” in “Output to the data and results files,” Section 4.1.2, and “Node output” in “Output to the output database,” Section 4.1.3. Saving temperatures for predefined fields in subsequent analyses To be read as a predefined field, nodal temperatures must be stored as functions of time in the results (.fil) file or output database (.odb) file. You can request nodal temperature output (NT) in an uncoupled heat transfer analysis or in a coupled thermal-electrical analysis. Saving normalized concentrations for predefined fields in subsequent analyses To be read as predefined fields, normalized concentrations must be stored as functions of time in the output database (.odb) file—unlike nodal temperatures they cannot be read directly from a results file. You can request nodal normalized concentrations output (NNC) in a mass diffusion analysis. Saving electric potentials for predefined fields in subsequent analyses To be read as predefined fields, electrical potentials must be stored as functions of time in the output database (.odb) file—unlike nodal temperatures they cannot be read directly from a results file. You can request nodal electric potential output (EPOT) in a coupled thermal-electrical analysis or a piezoelectric analysis. Transferring temperatures as temperature fields To define the temperature field at different times in the current analysis, you read the nodal temperatures stored as a function of time in the heat transfer results or output database file. Nodes can be removed for the current problem; for example, in a sequential thermal-stress analysis elements that represent nonstructural parts of the heat transfer mesh (such as insulation or cooling fluid) can be omitted in the stress analysis. When the heat transfer results file or output database file is read, temperatures at nodes that are not present in the mesh for the current analysis are ignored. You must specify the name of the thermal analysis results file or output database file that contains the required nodal temperatures. The file extension is optional. If the heat transfer model and the current analysis model share the same mesh, the default is the results file. If the heat transfer model and the current analysis model have dissimilar meshes, the output database file must be used. See “Reading the values of a field from a user-specified file” in “Predefined fields,” Section 33.6.1, for more information. If both models contain part and assembly definitions, the part (.prt) files from both analyses are required to transfer temperatures from the thermal analysis to the current analysis. If the thermal model is defined in terms of an assembly of part instances, the current analysis must be as well. The part instance names and local node numbers must be the same in both analyses for the nodes at which temperatures are transferred. Transferring temperatures, normalized concentrations, and electric potentials from the output database to predefined fields To define predefined fields at different times in the current analysis, you can read nodal temperatures, normalized concentrations, or electric potentials stored as a function of time in the output database file. Nodes can be removed for the current problem. When the nodal output variables on the output database file are on nodes that are not present in the mesh for the current analysis, they are ignored. You must specify the name of the output database file that contains the required nodal output variables as well as the nodal output label (NT, NNC, or EPOT) to identify the field that is being read. See “Defining fields using nodal scalar output values from a user-specified output database file” in “Predefined fields,” Section 33.6.1. If both models contain part and assembly definitions, the part (.prt) files from both analyses are required to transfer nodal results from the original analysis to the current analysis. If the original model is defined in terms of an assembly of part instances, the current analysis must be as well. The part instance names and local node numbers must be the same in both analyses for the nodes at which nodal results are transferred. Initial conditions Appropriate initial conditions for Abaqus/Standard procedures are discussed in Chapter 6, “Analysis Procedures.” You can read the nodal temperatures, normalized concentrations, or electric potentials from previous analyses to initialize predefined fields. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, for details. Boundary conditions Appropriate boundary conditions for Abaqus/Standard procedures are discussed in Chapter 6, “Analysis Procedures.” See also “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Loads Appropriate loadings for Abaqus/Standard procedures are discussed in Chapter 6, “Analysis Procedures.” See also “Applying loads: overview,” Section 33.4.1. Predefined fields See “Predefined fields,” Section 33.6.1, for additional details on predefined temperatures and fields. Material options See Part V, “Materials,” for details on the material models available in Abaqus/Standard. Volumetric strain will arise in a stress analysis if thermal expansion (“Thermal expansion,” Section 26.1.2) or field expansion (“Field expansion,” Section 26.1.3) is included in the material property definition. Elements Continuum and structural elements available in Abaqus/Standard are discussed in Chapter 28, “Continuum Elements,” and Chapter 29, “Structural Elements.” Details on how results from a previous analysis can be transferred to a current analysis are discussed in “Predefined fields,” Section 33.6.1. Output Appropriate output variables for Abaqus/Standard are described in Part V, “Materials.” All of the output variables are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Input file template A moisture-stress analysis is an example of a sequentially coupled multiphysics analysis. A typical sequentially coupled moisture-stress analysis consists of two Abaqus/Standard runs: a mass diffusion analysis and a subsequent stress analysis. Normalized concentrations are stored in the output database file for the mass diffusion analysis and read into the subsequent stress analysis as a predefined field. The following template shows the input for the mass diffusion analysis massdiffusion.inp: *HEADING … *ELEMENT, TYPE=DC2D4 (Choose the mass diffusion element type) … *STEP *MASS DIFFUSION … Apply loads and boundary conditions … ** Write all normalized concentrations to the output ** database file, massdiffusion.odb *OUTPUT, FIELD *NODE OUTPUT, NSET=NALL NNC *END STEP The following template shows the input for the subsequent static structural analysis: *HEADING … *ELEMENT, TYPE=CPE4R (Choose the continuum element type compatible with the mass diffusion element type used) *MATERIAL *EXPANSION, FIELD=1 (Define field expansion for field 1 so that the normalized concentration causes volumetric strain in the stress analysis) … *STEP *STATIC … Apply structural loads and boundary conditions … *FIELD, FILE=massdiffusion.odb, OUTPUT VARIABLE=NNC, FIELD=1 Read in all normalized concentrations from the output database file into field variable 1 … *END STEP 16.1.2 SEQUENTIALLY COUPLED THERMAL-STRESS ANALYSIS Products: Abaqus/Standard Abaqus/CAE References • “Defining an analysis,” Section 6.1.2 • “Heat transfer analysis procedures: overview,” Section 6.5.1 • “Predefined fields for sequential coupling,” Section 16.1.1 • “Creating and modifying output requests,” Section 14.4.5 of the Abaqus/CAE User’s Manual • “Defining a temperature field,” Section 16.11.9 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A sequentially coupled heat transfer analysis: • is used when the stress/deformation field in a structure depends on the temperature field in that structure, but the temperature field can be found without knowledge of the stress/deformation response; and • is usually performed by first conducting an uncoupled heat stress/deformation analysis. transfer analysis and then a A thermal-stress analysis in which the temperature field does not depend on the stress field is a common example of a sequential multiphysics workflow and is one case of the more general workflow described in “Predefined fields for sequential coupling,” Section 16.1.1. In such thermal-stress analyses, temperature is calculated in an uncoupled heat transfer analysis (“Uncoupled heat transfer analysis,” Section 6.5.2) or in a coupled thermal-electrical analysis (“Coupled thermal-electrical analysis,” Section 6.7.3). Saving the nodal temperatures Nodal temperatures are stored as a function of time in the heat transfer results (.fil) file or output database (.odb) file by requesting output variable NT as nodal output to the results or output database file. See “Node output” in “Output to the data and results files,” Section 4.1.2, and “Node output” in “Output to the output database,” Section 4.1.3. Transferring the heat transfer results to the stress analysis The temperatures are read into the stress analysis as a predefined field; the temperature varies with position and is usually time dependent. It is predefined because it is not changed by the stress analysis solution. Such predefined fields are always read into Abaqus/Standard at the nodes. They are then interpolated to the calculation points within elements as needed . The temperature interpolation in the stress elements is usually approximate and one order lower than the displacement interpolation to obtain a compatible variation of thermal and mechanical strain. Any number of predefined fields can be read in, and material properties can be defined to depend on them. For more information, see “Transferring temperatures as temperature fields” in “Predefined fields for sequential coupling,” Section 16.1.1. Initial conditions Appropriate initial conditions for the thermal and stress analysis problems are described in the heat transfer and stress analysis sections—for example, see “Heat transfer analysis procedures: overview,” Section 6.5.1; “Coupled thermal-electrical analysis,” Section 6.7.3; “Static stress analysis procedures: overview,” Section 6.2.1; and “Dynamic analysis procedures: overview,” Section 6.3.1. See also “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1. Boundary conditions Appropriate boundary conditions for the thermal and stress analysis problems are described in the heat transfer and stress analysis sections—for example, see “Heat transfer analysis procedures: overview,” Section 6.5.1; “Coupled thermal-electrical analysis,” Section 6.7.3; “Static stress analysis procedures: overview,” Section 6.2.1; and “Dynamic analysis procedures: overview,” Section 6.3.1. See also “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1. Loads Appropriate loading for the thermal and stress analysis problems is described in the heat transfer and stress analysis sections—for example, see “Heat transfer analysis procedures: overview,” Section 6.5.1; “Coupled thermal-electrical analysis,” Section 6.7.3; “Static stress analysis procedures: overview,” Section 6.2.1; and “Dynamic analysis procedures: overview,” Section 6.3.1. See also “Applying loads: overview,” Section 33.4.1. Predefined fields In addition to the temperatures read in from the heat transfer analysis, user-defined field variables can be specified; these values only affect field-variable-dependent material properties, if any. See “Predefined fields,” Section 33.6.1. Material options The materials in the thermal analysis must have thermal properties such as conductivity defined . Any mechanical properties such as elasticity will be ignored in the thermal analysis, but they must be defined for the stress analysis procedure. See Part V, “Materials,” for details on the material models available in Abaqus/Standard. Thermal strain will arise in the stress analysis if thermal expansion (“Thermal expansion,” Section 26.1.2) is included in the material property definition. Elements Any of the heat transfer elements in Abaqus/Standard can be used in the thermal analysis. In the stress analysis the corresponding continuum or structural elements must be chosen. For example, if heat transfer shell element type DS4 is defined by nodes 100, 101, 102, and 103 in the heat transfer analysis, three-dimensional shell element type S4R or S4R5 must be defined by these nodes in the stress analysis procedure. For continuum elements heat transfer results from a mesh using first-order elements can be transferred to a stress analysis with a mesh using second-order elements ” in “Predefined fields,” Section 33.6.1). Output The nodal temperatures must be written to the heat transfer analysis results or output database file by requesting the output variable NT . These temperatures will be read into the stress analysis procedure. Appropriate output variables are described in the heat transfer and stress analysis sections. All of the output variables are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1. Input file template A typical sequentially coupled thermal-stress analysis consists of two Abaqus/Standard runs: a heat transfer analysis and a subsequent stress analysis. The following template shows the input for the heat transfer analysis heat.inp: *HEADING … *ELEMENT, TYPE=DC2D4 (Choose the heat transfer element type) … *STEP *HEAT TRANSFER … Apply thermal loads and boundary conditions … ** Write all nodal temperatures to the results or ** output database file, heat.fil/heat.odb *NODE FILE, NSET=NALL NT *OUTPUT, FIELD *NODE OUTPUT, NSET=NALL NT *END STEP The following template shows the input for the subsequent static structural analysis: *HEADING … *ELEMENT, TYPE=CPE4R (Choose the continuum element type compatible with the heat transfer element type used) … *STEP *STATIC … Apply structural loads and boundary conditions … *TEMPERATURE, FILE=heat Read in all nodal temperatures from the results or output database file, heat.fil/heat.odb … *END STEP 16.1.3 PREDEFINED LOADS FOR SEQUENTIAL COUPLING Product: Abaqus/Standard References • “Mapping thermal and magnetic loads,” Section 3.2.22 • “Defining an analysis,” Section 6.1.2 • “Eddy current analysis,” Section 6.7.5 • “Concentrated loads,” Section 33.4.2 Overview The values of the following whole element output quantities, generated in an Abaqus/Standard time- harmonic eddy current analysis, can be read into subsequent Abaqus/Standard analyses as point loads for sequentially coupled multiphysics workflows: • Rate of Joule heat dissipation • Magnetic body force intensity A sequentially coupled multiphysics analysis can be used to apply electromagnetically generated loads (from a time-harmonic eddy current analysis) in a heat transfer, coupled temperature-displacement, or stress/displacement analysis. In many cases coupling is important only from the time-harmonic eddy current analysis; the impact of loading on the structure’s mechanical or thermal response is not great enough to affect the validity of the original time-harmonic eddy current analysis. Saving Joule heat dissipation or magnetic body force intensity for use in subsequent analyses You can request Joule heat dissipation output (EMJH) or magnetic body force intensity output (EMBF) in a time-harmonic eddy current analysis. Only values stored in the output database (.odb) file are available for use with sequential coupling. Converting results for subsequent use The whole element quantities are converted to nodal load quantities using the abaqus emloads utility. The utility converts Joule heat dissipation output to concentrated heat flux and magnetic body force intensity output to point loads. This utility also enables conversion of results between dissimilar meshes. For more information, see “Mapping thermal and magnetic loads,” Section 3.2.22. Conversion limitations When converting results values between dissimilar meshes, global conservation of the net flux is ensured provided that the model domain in the heat transfer, coupled temperature-displacement, or stress/displacement analysis matches the model domain in the time-harmonic eddy current analysis. The conservative mapping algorithm used in the abaqus emloads utility also provides a locally smooth distribution of point flux values (either body force or concentrated heat flux) in cases where the mesh in the time-harmonic eddy current analysis is finer than the “target” representative mesh. In situations where this is not the case and the “target” representative mesh is finer or of similar size to the mesh in the time-harmonic eddy current analysis, you may observe nodal locations with zero converted flux values. In these cases you will still observe global conservation of the flux, but your solution may be adversely affected locally. You can correct for these situations by always performing the time-harmonic eddy current analysis with a finer mesh. Transferring nodal loads from the output database to concentrated loads To define loads in a heat transfer, coupled temperature-displacement, or stress/displacement analysis, you can read nodal concentrated heat fluxes and point loads from the output database (.odb) file created by the abaqus emloads utility. Input file template In this example heat flux values are stored in the output database from a time-harmonic eddy current analysis. These values, after conversion to point heat fluxes, are read into a subsequent analysis as a concentrated flux. The following template shows the input for the time-harmonic eddy current analysis electromagnetic.inp: *HEADING … *ELEMENT, TYPE=EMC3D8 (Choose the electromagnetic element type) … *STEP *ELECTROMAGNETIC, LOW FREQUENCY, TIME HARMONIC … Apply loads and boundary conditions … ** Write element Joule heat dissipation results to the output ** database file, electromagnetic.odb *OUTPUT, FIELD *ELEMENT OUTPUT, ELSET=CONDUCTOR EMJH *END STEP The following template shows the input for the heat transfer analysis, heattransfer.inp, which refers to an output database, pointflux.odb, created using the abaqus emloads utility, and which has mapped quantities from the results of the time-harmonic eddy current analysis, stored in electromagnetic.odb: *HEADING … *ELEMENT, TYPE=DC3D8 (Choose the heat transfer continuum element type) … *STEP *HEAT TRANSFER, STEADY STATE … Apply heat transfer loads and boundary conditions … *CFLUX, FILE=pointflux.odb Read in all nodal heat flux values from the output database and apply as concentrated nodal fluxes … *END STEP Co-simulation Co-simulation Preparing an Abaqus analysis for co-simulation Co-simulation between Abaqus solvers CO-SIMULATION 17.1 17.2 17.1 Co-simulation • “Co-simulation: overview,” Section 17.1.1 17.1.1 CO-SIMULATION: OVERVIEW The co-simulation technique is a capability for run-time coupling of Abaqus and another analysis program. An Abaqus analysis can be coupled to another Abaqus analysis or to a third-party analysis program to perform multiphysics simulations and multidomain (multimodel) coupling. Abaqus provides built-in procedures to solve multiphysics simulations as described in “Multiphysics analyses” in “Solving analysis problems: overview,” Section 6.1.1. For multiphysics problems for which Abaqus does not provide a built-in solution procedure or where the solution procedure is limited in functionality, you can use the co-simulation technique to couple Abaqus with a third-party analysis program; for example, fluid-structure interaction (FSI) simulation in conjunction with computational fluid dynamics (CFD) analysis programs. Co-simulation between Abaqus/Standard and Abaqus/Explicit illustrates a multiple domain analysis approach, where each Abaqus analysis operates on a complementary section of the model domain where it is expected to provide the more computationally efficient solution. For example, Abaqus/Standard provides a more efficient solution for light and stiff components, while Abaqus/Explicit is more efficient for solving complex contact interactions. Another application area is solving complex problems where the model is divided into multiple domains and different analysis programs are used to obtain solutions for each domain; for example, crash safety simulation performed in conjunction with the occupant simulation program MADYMO. Features of the Abaqus co-simulation technique The Abaqus co-simulation technique: • can be used to solve complex fluid-structure interactions by coupling Abaqus with CFD analysis programs, including Abaqus/CFD analyses; • can be used to solve conjugate heat transfer problems by coupling Abaqus/Standard with CFD analysis programs, including Abaqus/CFD analyses; • can be used to solve complex analyses more effectively by coupling Abaqus/Standard to Abaqus/Explicit; • can be used for multiphysics simulations by coupling Abaqus with third-party analysis programs; • can be used to couple Abaqus with in-house codes using the SIMULIA Co-Simulation Engine or the multiphysics code coupling interface, MpCCI; • can be used for crash safety simulations by coupling Abaqus/Explicit with the occupant simulation program MADYMO; • is intended for advanced users with in-depth knowledge of Abaqus and the third-party analysis program; • allows for both unidirectional and bidirectional transfer of data; • can be used with Abaqus models having linear or nonlinear structural response; and • supports both steady-state and transient simulations. Interaction between domains modeled with different analysis programs In a co-simulation the interaction between the domains is through a common physical interface region over which data are exchanged in a synchronized manner between Abaqus and the coupled analysis program. One domain may affect the response of another domain through one or more of the following: • the constitutive behavior, such as the yield stress defined as a function of temperature or stress defined as a function of other solution fields, such as thermal strains or the piezoelectric effect; • surface tractions/fluxes, such as a fluid exerting pressure on a structure; • body forces/fluxes, such as heat generation due to flow of current in a coupled thermal-electrical simulation; • contact forces, such as the forces due to contact between a vehicle and an occupant/pedestrian modeled as separate domains; and • kinematics, such as fluid in contact with a compliant structure where the interface motion affects the fluid flow. Abaqus offers two approaches to couple Abaqus with another analysis program: • Direct coupling using SIMULIA Co-Simulation methods. • Coupling using MpCCI, a third-party connectivity middleware. Coupling Abaqus using SIMULIA Co-Simulation methods SIMULIA Co-Simulation methods provide direct coupling between two Abaqus analyses or between Abaqus and third-party analysis programs, without any third-party communication tool. These methods are used for fluid-structure simulations, conjugate heat transfer, coupling Abaqus/Standard to Abaqus/Explicit for interaction between implicit dynamic and explicit dynamic domains, and coupling Abaqus to MADYMO for vehicle-occupant/pedestrian interaction. Fluid-structure interaction You can perform complex fluid-structure interaction (FSI) problems by coupling Abaqus/Standard or Abaqus/Explicit to a computational fluid dynamics (CFD) analysis program. Abaqus/Standard and Abaqus/Explicit solve the structural domain, and the CFD analysis program solves the fluid domain. Abaqus/Standard and Abaqus/Explicit can be coupled with Abaqus/CFD as well as with several third-party CFD analysis programs. For detailed information on coupling Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit, see “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1, and “Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 17.3.2. For a complete list of qualified partner products, see www.simulia.com. Conjugate heat transfer You can perform conjugate heat transfer problems involving fluids and structures by coupling Abaqus/Standard to a computational fluid dynamics (CFD) analysis program. Abaqus/Standard models heat transfer within the structure , and the CFD analysis program solves the energy equation for the fluid flow surrounding the structure. Abaqus/Standard can be coupled with Abaqus/CFD as well as with several third-party CFD analysis programs. For an example of Abaqus/CFD to Abaqus/Standard co-simulation, refer to “Conjugate heat transfer analysis of a component-mounted electronic circuit board,” Section 6.1.1 of the Abaqus Example Problems Manual. For detailed information on coupling Abaqus/CFD to Abaqus/Standard, see “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1, and “Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 17.3.2. For a complete list of qualified partner products, see www.simulia.com. Interaction between an implicit transient analysis and an explicit dynamics analysis In certain cases you can realize significant computational cost savings by partitioning a model and combining the Abaqus/Standard and Abaqus/Explicit solutions, such as • when the simulation is principally a candidate for Abaqus/Explicit, but where certain parts of the model can be idealized using substructures in Abaqus/Standard, or • when the simulation is principally a candidate for Abaqus/Standard, but where complex contact conditions would be handled more effectively by Abaqus/Explicit. For an example of Abaqus/Standard to Abaqus/Explicit co-simulation, refer to “Dynamic impact of a scooter with a bump,” Section 2.4.1 of the Abaqus Example Problems Manual. For detailed information on coupling Abaqus/Standard and Abaqus/Explicit, see “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1, and “Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 17.3.1. Vehicle-occupant/pedestrian interaction Crash safety simulation generally includes interaction between a vehicle and its occupant or a vehicle and a pedestrian. Abaqus/Explicit is used to model the vehicle, and MADYMO is used to model the occupant or the pedestrian. In some cases the influence of the human response on the structural response of the vehicle is so small as to be negligible. In these cases only a part of the vehicle surrounding the human is used in a coupled analysis. The vehicle analysis is performed without the human, and the motion from a portion of the vehicle immediately surrounding the human is extracted as a submodel of the full vehicle response. The co-simulation technique is used to perform a coupled analysis with the human model and the vehicle submodel. For an example of co-simulation with MADYMO, refer to “Rigid body dynamics with Abaqus/Explicit,” Section 1.3.7 of the Abaqus Benchmarks Manual. The coupling between Abaqus/Explicit and MADYMO is actively supported and tested by both SIMULIA and TNO MADYMO BV. For detailed information, refer to “Using coupling between Abaqus/Explicit and MADYMO in Abaqus” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge- base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com. Coupling using MpCCI MpCCI, the multiphysics code coupling interface developed and distributed by the Fraunhofer-Institute for Algorithms and Scientific Computing (SCAI), provides an open system approach for general multidisciplinary simulations between Abaqus and any third-party analysis program that supports MpCCI. MpCCI provides a scalable communication infrastructure and mapping algorithms for multiple physics domains. In a co-simulation using MpCCI, Abaqus communicates in real time with the MpCCI coupling server to exchange fields with the third-party analysis program while each analysis advances its simulation time. Coupling through MpCCI may occur between Abaqus and any third-party analysis program that supports the MpCCI interface. This includes in-house codes that have the MpCCI adapter embedded. SIMULIA actively supports and qualifies a link between Abaqus and FLUENT for fluid-structure interaction. For more information, refer to “Abaqus User’s Guide for Fluid-Structure Interaction (FSI)” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com. Strength of physics coupling You will typically apply co-simulation techniques to problems where the most complex physics occurs within domains that are handled exclusively within an analysis program (e.g., Abaqus or a CFD analysis program). Due to the comparative numerical simplicity of the numerical techniques applied at the co-simulation interface, the physics controlling the interaction at the interface of the separate analysis domains (the strength of the physics coupling) must be relatively weak for the co-simulation technique to be applied effectively. Coupling to third-party analysis programs In a fluid-structure interaction (FSI) co-simulation the analysis domains are coupled in a staggered approach in a globally explicit manner; that is, the equations for each domain are solved separately, and loads and boundary conditions are exchanged at the common interface. Similarly, in a crash safety simulation with the vehicle modeled in Abaqus/Explicit and the dummy modeled in MADYMO, the interaction of the domains is resolved by application of the forces resulting from the contact condition between the interface of the two domains. The staggered approach is applicable to many problems that exhibit weak to moderate physics coupling. In cases where the coupling is sufficiently weak, the coupling may be required only in one direction (such as when a temperature field contributes to the structural response, but a reverse coupling provides no significant impact on the simulation results). The staggered approach may not be effective for problems that exhibit strong physics coupling. Figure 17.1.1–1 illustrates the coupling strength with an analogy in the frequency domain. Consider a lumped parameter dynamic system with a coupling impedance directly related to a response frequency In a staggered solution approach each domain is solved by temporarily ignoring the coupling terms represented by the gray spring and dashpot in Figure 17.1.1–1. When the response frequency and coupling impedance are low, a staggered approach will likely provide adequate solution . ks Fs ms Ff mf cf structure coupling fluid Figure 17.1.1–1 Mechanical impedance analogy. accuracy and performance. However, when the response frequency is high, such that the coupling impedance is relatively large compared to the structure or fluid, you may encounter solution stability issues with the staggered approach. Coupling in Abaqus/Standard to Abaqus/Explicit co-simulation The strength of the physics coupling can generally be greater in the coupling of Abaqus/Standard to Abaqus/Explicit using the co-simulation technique. Through communication of “right-hand-side” and “left-hand-side” terms, Abaqus/Standard to Abaqus/Explicit co-simulation provides a robust interface solution across a wide range of problem parameters. In many cases you can choose to have Abaqus/Standard and Abaqus/Explicit each advance their solutions according to their own automatic time incrementation scheme without adversely affecting the interface solution stability. References For the latest support information and tips on running FSI simulations and crash safety simulations, see the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com. 17.2 Preparing an Abaqus analysis for co-simulation • “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1 17.2.1 PREPARING AN Abaqus ANALYSIS FOR CO-SIMULATION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD References • “Co-simulation: overview,” Section 17.1.1 • “Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 17.3.1 • “Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 17.3.2 • *CO-SIMULATION • *CO-SIMULATION REGION • *CO-SIMULATION CONTROLS Overview This section provides an overview of preparing an Abaqus analysis for a co-simulation. The discussion in this section is general and may not apply to every product pairing. “Co-simulation between Abaqus solvers,” Section 17.3, provides setup, execution, and limitation details for co-simulation between Abaqus solvers. For co-simulation between Abaqus and third-party analysis programs, consult the appropriate User’s Guide. Preparing an Abaqus analysis for co-simulation involves the following: • identifying the Abaqus analysis step for a co-simulation analysis; • identifying the analysis program, which may be another Abaqus analysis, that is communicating with Abaqus during the co-simulation analysis; • identifying the co-simulation interface regions in the Abaqus model; • identifying the fields exchanged during the co-simulation; and • defining the coupling and rendezvousing schemes. Each of these steps is described in detail below. Identifying the Abaqus step for the co-simulation analysis The co-simulation event need not begin at the start of the first step in an Abaqus analysis. However, it does need to start with the beginning of an analysis step and end within that analysis step. Hence, you need to define the step durations in Abaqus such that the start of the co-simulation event falls at the beginning of an Abaqus analysis step and to define that particular step so that the co-simulation event ends by the end of that step. Regular loads and boundary conditions for the Abaqus model, particularly away from the interface regions, are specified as usual. Communication with the coupled analysis is initiated as the co-simulation event begins and is terminated when the co-simulation event is ended by either program. Abaqus may terminate the co-simulation event when the end of the analysis step is reached or when the analysis cannot proceed any further; for example, due to convergence problems. Co-simulation is supported by the following Abaqus procedures: • “Static stress analysis,” Section 6.2.2 • “Quasi-static analysis,” Section 6.2.5 • “Implicit dynamic analysis using direct integration,” Section 6.3.2 • “Explicit dynamic analysis,” Section 6.3.3 • “Uncoupled heat transfer analysis,” Section 6.5.2 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Incompressible fluid dynamic analysis,” Section 6.6.2 • “Piezoelectric analysis,” Section 6.7.2 • “Coupled thermal-electrical analysis,” Section 6.7.3 • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 Input File Usage: Use the following option within a step definition to indicate the beginning of a co-simulation event: *CO-SIMULATION, NAME=name Identifying the analysis program communicating with Abaqus during the co-simulation The Abaqus co-simulation technique provides several interfaces, such as the SIMULIA Co-Simulation Engine for coupling Abaqus-to-Abaqus and Abaqus to third-party analysis programs; an interface for coupling Abaqus/Standard to Abaqus/Explicit; a general open interface through the multiphysics code coupling interface, MpCCI; and an interface coupling Abaqus to MADYMO. Coupling using the SIMULIA Co-Simulation Engine You can couple Abaqus with another Abaqus analysis or Abaqus with certain third-party analysis programs using the SIMULIA Co-Simulation Engine. For details on coupling with third-party analysis programs, see the respective User’s Guides. Input File Usage: *CO-SIMULATION, NAME=name, PROGRAM=MULTIPHYSICS Coupling Abaqus/Standard and Abaqus/Explicit You can couple an Abaqus/Standard analysis to an Abaqus/Explicit analysis. Input File Usage: *CO-SIMULATION, NAME=name, PROGRAM=ABAQUS Coupling using MpCCI You can use MpCCI to communicate with any third-party analysis program that is MpCCI compliant. MpCCI is a third-party connectivity program for general multidisciplinary simulation and is distributed by the Fraunhofer-Institute for Algorithms and Scientific Computing. In this case Abaqus communicates with the MpCCI server, which in turn communicates with the third-party analysis program. For more information on coupling using MpCCI, refer to “Abaqus User’s Guide for Fluid-Structure Interaction (FSI)” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com. Input File Usage: *CO-SIMULATION, NAME=name, PROGRAM=MPCCI Coupling Abaqus/Explicit and MADYMO For information on coupling using MADYMO, refer to “Using coupling between Abaqus/Explicit and MADYMO in Abaqus” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge- base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com. Identifying the co-simulation interface region Interaction between two Abaqus models or between an Abaqus model and a third-party analysis model takes place through a common interface region referred to as the co-simulation interface region. The co-simulation interface region may be a set of discrete points, a surface region, or a volume region. You must be consistent in your interface region definition; if you define a surface co-simulation region in one analysis, then you must define a surface co-simulation region in the other analysis. Furthermore, these co-simulation regions need to be co-located and have the same region boundaries. Interacting through discrete points Interaction can occur through a set of discrete points where only nodal position information without element topology information (e.g., tributary area) defines the co-simulation interface region. In this case the spatial mapping is limited to point-to-point mapping, and you must ensure that there are matching nodes between the models. In Abaqus you can use a node set or a node-based surface to define a co-simulation interface region consisting of discrete points. Input File Usage: Use the following option to define a node set as a co-simulation region in an Abaqus model: *CO-SIMULATION REGION, TYPE=NODE nodeset_A Use the following options to define a node-based surface as a co-simulation region in an Abaqus model: *SURFACE, TYPE=NODE nodeset_A *CO-SIMULATION REGION, TYPE=SURFACE node-based surface name Interacting through a surface Interaction between distinct domains occurs through a common interface surface. For example, when a fluid interacts with a solid without penetrating it, the fluid-solid interface is defined through a surface. In this case both nodal position and element topology information define the co-simulation interface, and appropriate spatial mapping between dissimilar surface meshes is performed to conservatively map fields. Input File Usage: Use the following option to define an element-based surface as a co-simulation region in an Abaqus model: *CO-SIMULATION REGION, TYPE=SURFACE (default) element-based surface name Interacting through a volume Interaction between overlapping domains occurs through a volume. In this case both nodal position and element topology information define the co-simulation region, and appropriate spatial mapping between dissimilar volume meshes is performed to conservatively map fields. The interface region is defined by an element set. Input File Usage: Use the following option to define a volume as a co-simulation region in an Abaqus model: *CO-SIMULATION REGION, TYPE=VOLUME elset_A Identifying the fields exchanged across a co-simulation interface The coupling of the domain models can be through loads and/or boundary conditions prescribed at the co- simulation interface. In addition, mass, rotary inertia, and heat capacitance terms can also be exchanged. Based on the physics and the interaction type and its enforcement, you must specify the fields that are imported and/or exported in an Abaqus analysis during the co-simulation. The co-simulation interface can consist of a group of discrete points (nodes), a surface region, or a volume region. Not all fields can be exchanged across all region types. This section provides a general overview of all fields available in Abaqus. For detailed information on the fields exchanged between two Abaqus solvers, see “Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 17.3.1, and “Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 17.3.2. For detailed information on fields exchanged by Abaqus and a third-party analysis program, see the respective User’s Guides. Input File Usage: Use the following option to import field data over a region into Abaqus: *CO-SIMULATION REGION, IMPORT region_A, import_field_1 region_A, import_field_2 Use the following option to export data from Abaqus: *CO-SIMULATION REGION, EXPORT region_A, export_field_1 region_A, export_field_2 When using the SIMULIA Co-Simulation Engine, only a single region can be specified. If multiple regions are involved, you must combine these regions into a single region. For example, you can use the *SURFACE, COMBINE option to create a combined surface region. Procedures involving mechanical degrees of freedom Table 17.2.1–1 lists the fields that can be exchanged for procedures supporting mechanical degrees of freedom (degrees of freedom 1–6), their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values. Table 17.2.1–1 Exchanging fields for procedures supporting mechanical degrees of freedom. Field ID Fields Interface Type1 Abaqus Solver2 Import Export Units UT or U Displacement P, S, V S, E, C S, E VT or V AT or A UR VR AR Velocity (transient procedures) Acceleration (transient procedures) Rotations Angular velocity (transient procedures) Angular acceleration (transient procedures) COORD Current coordinates CF CM Concentrated forces Concentrated moments TRSHR Traction vector PRESS Pressure normal to element surface P, S, V P, S, V P, S P, S P, S P, S, V P, S, V P, S S, E S, E S, E radians S, E radians S, E radians S, E S, E S, E S, E 1 P (points), S (surface region), V (volume region) 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) The following procedures support co-simulation using mechanical degrees of freedom: • “Static stress analysis,” Section 6.2.2 • “Quasi-static analysis,” Section 6.2.5 • “Implicit dynamic analysis using direct integration,” Section 6.3.2 • “Explicit dynamic analysis,” Section 6.3.3 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Incompressible fluid dynamic analysis,” Section 6.6.2 • “Piezoelectric analysis,” Section 6.7.2 • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 Displacements Displacements (field ID UT or U) for the translational degrees of freedom can be exported by Abaqus/Standard and Abaqus/Explicit. Displacements can be imported by Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD. When imported, displacements are ramped from the values of the previous exchange time point to those of the next target time point. The displacements are exported in the global coordinate system. Displacements are available for points, surface regions, and volume regions in Abaqus/Standard and for surface regions in Abaqus/Explicit and Abaqus/CFD. Displacements can be viewed in the Visualization module of Abaqus/CAE. Velocity and acceleration Velocity (field ID VT or V) and acceleration (field ID AT or A) for the translational degrees of freedom can be exported by Abaqus/Standard for transient procedures and by Abaqus/Explicit. Velocity can be imported by Abaqus/CFD. Velocity and acceleration are in the global coordinate system. Velocity is available for points and surface regions in Abaqus/Standard and Abaqus/Explicit and for surface regions in Abaqus/CFD. Rotations Rotations (field ID UR) can be exported by Abaqus/Standard and Abaqus/Explicit and imported by Abaqus/Explicit. Rotations are in the global coordinate system. Rotations are available for points and surface regions. Rotations can be viewed in the Visualization module of Abaqus/CAE. Rotational velocity and rotational acceleration Rotational velocity (field ID VR) and rotational acceleration (field ID AR) can be exported by Abaqus/Standard for transient procedures and by Abaqus/Explicit. Rotational velocity and rotational acceleration are in the global coordinate system. Rotational velocity and rotational acceleration are available for points and surface regions. Current coordinates Current nodal coordinates (field ID COORD) can be exported by Abaqus/Standard and Abaqus/Explicit. The coordinates are the current coordinates of small- or is preferred to export displacements large-displacement analysis is performed. (field ID UT or U) rather than current coordinates when results are mapped between dissimilar interface regions. In cases where the partner client does not retain the original coordinates, it may be necessary to send current coordinate values rather than displacements. Current coordinates are available for points, Abaqus/Standard and for surface regions in Abaqus/Explicit. the deformed structure whether and volume regions surface regions, In general, in it Concentrated forces Concentrated forces (field ID CF), if imported, are ramped from the values of the previous exchange time point to those of the next target time point in Abaqus/Standard and are kept constant over the exchange interval in Abaqus/Explicit. The concentrated forces are in the global coordinate system. When exporting concentrated forces, Abaqus/Standard transfers reaction forces at interface nodes that have prescribed displacements. The reaction forces are exported in the global coordinate system. Concentrated forces are available for points, surface regions, and, in Abaqus/Standard only, volume regions. Concentrated normal forces can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CF. Concentrated moments Concentrated moments (field ID CM), if imported, are ramped from the values of the previous exchange time point to those of the next target time point in Abaqus/Standard and are kept constant over the exchange interval in Abaqus/Explicit. The concentrated moments are in the global coordinate system. Concentrated moments are available for points, surface regions, and, in Abaqus/Standard only, volume regions. Concentrated normal moments can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CM. Traction vector The traction vector (field ID TRSHR), supported by Abaqus/CFD, exports the fluid total traction (normal and shear components) on the interface surface. Usually, the exported traction vector is integrated to concentrated forces (field ID CF) when imported into Abaqus/Standard or Abaqus/Explicit in a fluid- structure simulation. The traction vector is a force vector in the global Cartesian coordinate system. The traction vector is available for surface regions in Abaqus/CFD. Normal pressure Normal pressure (field ID PRESS), supported for import by Abaqus/Standard, is the traction normal component to the surface. Pressure values are ramped from the values of the previous exchange time point to those of the next target time point when imported into Abaqus/Standard. In most cases it is preferred to import concentrated forces (field ID CF) since these contain both the normal and shear traction components. For membrane-like structures it might be preferable to import pressures. Normal pressure can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable P. Procedures involving thermal degrees of freedom Table 17.2.1–2 lists the thermal fields available for co-simulation exchange, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values. Table 17.2.1–2 Exchanging fields for procedures supporting thermal degrees of freedom. Interface Type1 Abaqus Solver2 Import Export Units P, S, V S, E P, S, V S, E Fields Temperature as a nodal degree of freedom Concentrated heat flux at a node Heat flux normal to element surface Film properties Film properties (MpCCI only) 17.2.1–8 Field ID NT CFL HFL CFILM Field ID TEMP LUMPEDHEATCAPACITANCE Fields Temperature as a nodal degree of freedom Lumped heat capacitance Interface Type1 Abaqus Solver2 Import Export Units P, S, V P, S, V S, E 1 P (points), S (surface region), V (volume region) 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) The following procedures support co-simulation using thermal degrees of freedom: • “Uncoupled heat transfer analysis,” Section 6.5.2 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Incompressible fluid dynamic analysis,” Section 6.6.2 • “Coupled thermal-electrical analysis,” Section 6.7.3 Nodal temperature Nodal temperature (field ID NT) can be exported by Abaqus/Standard and Abaqus/Explicit and imported by Abaqus/CFD (as field ID TEMP). Temperature values are ramped from the values of the previous exchange time point to those of the next target time point when imported into Abaqus/Standard and Abaqus/CFD. Temperature values can be imported either on the top surface (SPOS) or the bottom surface (SNEG) of structural elements. Temperatures cannot be exchanged on double-sided surfaces where both the SPOS and the SNEG facets have the same underlying shell element. For volume regions, only degree of freedom NT11 is exported, and it should not be used for exchanging temperature values over volumes discretized with structural elements. Nodal temperature values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable NT. Heat flux Use concentrated heat flux (field ID CFL) for heat entering at a node in Abaqus/Standard and Abaqus/Explicit. Concentrated heat flux is available for points, surface regions, and, in Abaqus/Standard only, volume regions. Concentrated heat flux values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CFL. Use surface heat flux (field ID HFL) for a distributed heat flux entering the surface in Abaqus/Standard or distributed heat flux leaving a surface in Abaqus/CFD. Distributed heat flux is available only for surface regions. Film properties Use surface film properties (field ID FILM) or concentrated (nodal) film properties (field ID CFILM) to model convection governed by where q is the heat flux entering the surface, h is a film coefficient, is the wall temperature, and is the fluid or ambient temperature. The film coefficient is computed from the heat flux and fluid temperature obtained from the computational fluid dynamics analysis and the wall temperature from the Abaqus analysis computed during the previous exchange interval, according to Both the film coefficient and fluid temperature are passed into Abaqus/Standard and are kept constant over the subsequent exchange interval. When the fluid and wall temperatures coincide, an arbitrary small value for the heat transfer coefficient is passed into Abaqus. To obtain reasonable film properties for the first exchange interval, you should ensure that the wall temperatures are initialized properly in Abaqus and that you provide a good estimate for the initial fluid temperature. Film properties are available only for surface regions in Abaqus/Standard. Heat capacitance Nodal (lumped) heat capacitance (field ID LUMPEDHEATCAPACITANCE) can be exported by Abaqus/CFD in models in which heat capacitance is defined. Nodal heat capacitance can be imported into Abaqus/Standard and Abaqus/Explicit. Procedures involving pore fluid pressure Table 17.2.1–3 lists additional fields that can be exchanged for a coupled pore fluid diffusion/stress analysis, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values. Table 17.2.1–3 Exchanging fields for a coupled pore fluid diffusion/stress analysis. Field ID Fields POR CFF Pore fluid pressure at a node Concentrated fluid flow at a node Interface Type1 Abaqus Solver2 Import Export Units P, S, V P, S, V Field ID Fields RVF Reaction fluid volume flux due to prescribed pressure Interface Type1 Abaqus Solver2 Import Export Units P, S, V 1 P (points), S (surface region), V (volume region) 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) The following procedure involving pore fluid pressure supports co-simulation: • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 Pore pressure Nodal pore pressure (field ID POR) can be imported and exported by Abaqus/Standard for points, surface regions, and volume regions. Nodal pore pressure values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable POR. Concentrated fluid flow Fluid flow (field ID CFF) defines the seepage flow at a node. Concentrated fluid flow can be imported by Abaqus/Standard for points, surface regions, and volume regions. Concentrated fluid flow values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CFF. Reaction fluid volume flow Reaction fluid volume flux (field ID RVF) defines the rate at which fluid volume is entering or leaving the model through the node to maintain the prescribed pore pressure. Reaction fluid volume flux can be exported by Abaqus/Standard for points, surface regions, and volume regions. Temperature and independent field variables Field variables are time-dependent, predefined fields that exist over the spatial domain of the model . Field variables in conjunction with the co-simulation technique extend the possibilities of multiphysics by allowing material point dependencies on an external field defined by another application. Field variables must be numbered consecutively starting with one. Field variables can be defined: • by entering the data directly, • by reading an Abaqus results file or output database file, • in an Abaqus/Standard user subroutine, and • through the co-simulation interface. If field variables are defined by multiple methods, Abaqus processes them in the order defined above. Care needs be taken when field variables are used with structural elements, such as membranes and shells. In this case only the top or bottom face forming the interface region receives a value. Table 17.2.1–4 lists the temperature and independent field variables available for co-simulation exchange, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values. Table 17.2.1–4 Exchanging temperature and independent field variables. Field ID Fields Interface Type1 Abaqus Solver2 Import Export Units TEMP FV1 FV2 FV3 Temperature as field variable Field variable 1 Field variable 2 Field variable 3 1 P (points), S (surface region), V (volume region) 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) The following Abaqus/Standard procedures support import of temperature and independent field variables: • “Static stress analysis,” Section 6.2.2 • “Quasi-static analysis,” Section 6.2.5 • “Implicit dynamic analysis using direct integration,” Section 6.3.2 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Piezoelectric analysis,” Section 6.7.2 • “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 Temperature Temperature (field ID TEMP) can be imported by Abaqus/Standard for procedures that allow material properties to be defined as a function of an external temperature field. When imported, temperature values are ramped from the values of the previous exchange time point to those of the next target time point. Use field ID NT instead of field ID TEMP to import temperature values for thermal procedures (procedures using degrees of freedom 11, 12, etc.). Temperature can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting element output variable TEMP. Independent field variables Independent field variables (field IDs FV1, FV2, and FV3) can be imported by Abaqus/Standard, allowing material properties to be defined as a function of the external fields. When imported, independent field variable values are ramped from the values of the previous exchange time point to those of the next target time point. Field variables can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variables FV1, FV2, and/or FV3. Miscellaneous fields Table 17.2.1–5 lists miscellaneous fields available for co-simulation exchange, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values. Table 17.2.1–5 Exchanging miscellaneous fields. Field ID Fields MASS or LUMPEDMASS Mass RI Rotary inertia Interface Type1 Abaqus Solver2 Import Export Units P, S P, S S, E S, E, C 1 P (points), S (surface region), V (volume region) 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) Lumped mass Lumped mass values (field ID MASS or LUMPEDMASS) at nodes can be exported by Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD and can be imported by Abaqus/Standard and Abaqus/Explicit. Lumped mass is available for points and surface regions. Rotary inertia Nodal (lumped) rotary inertia (field ID RI) can be imported by Abaqus/Standard and exported by Abaqus/Explicit over points or surface regions for models using structural elements. Defining the rendezvousing scheme Different types of analyses have different time integration requirements that will influence or dictate the frequency of interaction between the analyses in a co-simulation to obtain an accurate and robust solution. For example, consider the difference in time integration between an implicit and an explicit dynamic analysis. Furthermore, Abaqus/Standard can adjust the increment sizes automatically to obtain an economical and accurate solution for transient problems (see “Incrementation” in “Defining an analysis,” Section 6.1.2). For example, consider a transient heat transfer analysis modeling a diffusive process; here the analysis may use small time increments at the beginning of the analysis where there is a high gradient in the solution and large time increments toward the end of the analysis when steady state is reached. Co-simulation controls are used to control the frequency of exchange between the analyses in a co-simulation and to control the time incrementation process in Abaqus. Input File Usage: Use both of the following options to specify co-simulation controls using the SIMULIA Co-Simulation Engine: *CO-SIMULATION, CONTROLS=name *CO-SIMULATION CONTROLS, NAME=name Defining the coupling scheme The coupling scheme defines the sequence of exchanges between analysis programs and also defines whether a coupled simulation can be run in a serial, parallel, or iterative manner. When deciding on the coupling scheme, you should consider solution stability issues as well as the utilization impact on your computing resources. When coupling through the SIMULIA Co-Simulation Engine, you have the choice between a parallel explicit coupling scheme (referred to as the Jacobi coupling algorithm), a sequential explicit coupling scheme (referred to as the Gauss-Seidel coupling algorithm), or an iterative scheme. Parallel explicit coupling scheme (Jacobi) In a parallel explicit coupling scheme, both simulations are executed concurrently, exchanging fields to update the respective solutions at the next target time. The parallel coupling scheme may make more efficient use of computing resources; however, it is considered less stable than the sequential scheme and should be employed only for weakly coupled physics simulations. The co-simulation partner analysis must also specify a Jacobi coupling algorithm. Input File Usage: *CO-SIMULATION CONTROLS, COUPLING SCHEME=JACOBI Sequential explicit coupling scheme (Gauss-Seidel) In a sequential explicit coupling scheme, the simulations are executed in sequential order. One analysis leads while the other analysis lags the co-simulation. The co-simulation partner analysis must also specify a Gauss-Seidel coupling algorithm. Input File Usage: Use the following option to specify that Abaqus leads the co-simulation: *CO-SIMULATION CONTROLS, COUPLING SCHEME=GAUSS- SEIDEL, SCHEME MODIFIER=LEAD The partner analysis must lag the co-simulation. Use the following option to specify that Abaqus lag the co-simulation: *CO-SIMULATION CONTROLS, COUPLING SCHEME=GAUSS- SEIDEL, SCHEME MODIFIER=LAG The partner analysis must lead the co-simulation. Iterative coupling scheme In an iterative coupling scheme, the simulations are executed in sequential order. One analysis leads while the other analysis lags the co-simulation. Multiple exchanges per coupling step are performed until termination criteria are met. The co-simulation partner analysis must also specify an iterative coupling algorithm. The termination criteria depend on the analyses in the co-simulation; for co-simulation between Abaqus and third-party analysis products, consult the appropriate User’s Guide. Input File Usage: Use the following option to specify that Abaqus leads the co-simulation: *CO-SIMULATION CONTROLS, COUPLING SCHEME=ITERATIVE, SCHEME MODIFIER=LEAD The partner analysis must lag the co-simulation. Use the following option to specify that Abaqus lag the co-simulation: *CO-SIMULATION CONTROLS, COUPLING SCHEME=ITERATIVE, SCHEME MODIFIER=LAG The partner analysis must lead the co-simulation. Coupling step size The coupling step is the period between two consecutive exchanges and consequently defines the frequency of exchange between the analyses in a co-simulation. The coupling step size is established at the beginning of each coupling step and is used to compute the target time (the time when the next synchronized exchange occurs). When you use the SIMULIA Co-Simulation Engine, several methods are available for computing the coupling step size. The methods available in Abaqus are described in the sections below. To determine the methods available for a co-simulation partner analysis, consult the appropriate third-party program documentation. Using a constant coupling step size A constant user-defined coupling step size is the most basic method of defining a coupling step size. Both analyses advance while exchanging data at target points according to where is a value that defines the coupling step size to be used throughout the coupled simulation, is the time at the start of the coupling step. For this method both Abaqus is the target time, and and the co-simulation partner analysis need to specify the same value for the coupling step size. Input File Usage: *CO-SIMULATION CONTROLS, STEP SIZE= Selecting the minimum coupling step size This method selects the minimum of the coupling step sizes suggested by each analysis. Abaqus always uses the next increment suggested by its automatic incrementation as its suggested coupling step size. For this method both Abaqus and the co-simulation partner analysis need to specify the minimum coupling step size method. Input File Usage: *CO-SIMULATION CONTROLS, STEP SIZE=MIN Selecting the maximum coupling step size This method selects the maximum of the coupling step sizes suggested by each analysis. Abaqus always uses the next increment suggested by its automatic incrementation as its suggested coupling step size. For this method both Abaqus and the co-simulation partner analysis need to specify the maximum coupling step size method. Input File Usage: *CO-SIMULATION CONTROLS, STEP SIZE=MAX Importing the coupling step size Abaqus can import a coupling step size suggested by the co-simulation partner analysis. For this method the co-simulation partner analysis needs to export a coupling step size. Input File Usage: *CO-SIMULATION CONTROLS, STEP SIZE=IMPORT Exporting the coupling step size Abaqus can export a suggested coupling step size to the co-simulation partner analysis. For this method the co-simulation partner analysis needs to import a coupling step size determined by Abaqus. Abaqus exports the next increment suggested by its automatic incrementation scheme. Input File Usage: *CO-SIMULATION CONTROLS, STEP SIZE=EXPORT Time incrementation scheme Abaqus may take multiple increments per coupling step, or you can force Abaqus to use a single increment per coupling step. Allowing Abaqus to subcycle By default, Abaqus may perform several increments (referred to as “subcycling”) during the coupling step. During subcycling, Abaqus/Standard ramps the loads and boundary conditions (with the exception of film properties) from the values at the end of the previous coupling step to the values at the target time, while in Abaqus/Explicit the loads are applied at the start of the coupling step and kept constant over the coupling step. Subcycling allows Abaqus to use its own time incrementation to reach the target coupling time; specifically, it allows Abaqus to cut back the increment size if there are nonlinear events that require the increment size to be reduced. Input File Usage: *CO-SIMULATION CONTROLS, TIME INCREMENTATION=SUBCYCLE Forcing Abaqus to use a single increment per coupling step In certain cases you may force Abaqus to use a time increment size dictated by the coupling step size (i.e., no subcycling). This allows both solvers to use the same time incrementation and avoid interpolation of quantities during the coupling step. When proceeding in this manner, Abaqus will not be able to reduce the time increment to resolve nonlinear events and, consequently, will terminate the simulation in cases where the nonlinear events require that the increment size be reduced. Input File Usage: *CO-SIMULATION CONTROLS, TIME INCREMENTATION=LOCKSTEP Reaching target times The Abaqus target times can be reached in an exact or loose manner. Reaching target times in an exact manner By default, Abaqus exchanges the data in an exact manner; that is, Abaqus temporarily reduces the time increment so that the solution exchange occurs exactly at the target time. Input File Usage: *CO-SIMULATION CONTROLS, TIME MARKS=YES Reaching target times in a loose manner When subcycling Abaqus may reach the target time in a loose manner; that is, when the current simulation time, t, is within half of an Abaqus increment size away from the target time, In this case performance is selected over solution accuracy. Loose coupling should be employed only for cases where Abaqus uses more increments than the third-party analysis program; for example, when coupling an explicit solver with an implicit solver. Input File Usage: *CO-SIMULATION CONTROLS, TIME MARKS=NO Model dimension and coordinate systems Three-dimensional Abaqus models are fully supported. Two-dimensional and axisymmetric Abaqus models are supported only for Abaqus/Standard to Abaqus/Explicit co-simulation and coupling using MpCCI. For co-simulations that do not support two-dimensional and axisymmetric models, you can represent these models as a three-dimensional slice of unit thickness (or wedge element) with the appropriate boundary conditions applied. Vector quantities are defined according to Abaqus conventions; the first component represents the quantity along the x-axis, the second quantity represents the quantity along the y-axis, and the third quantity represents the quantity along the -axis (for three-dimensional models). For axisymmetric models in Abaqus the axis of revolution is about the y-axis. These conventions apply to both the exported and the imported vector quantities. All exported vector quantities are expressed in the global coordinate system of the Abaqus model, ignoring any transformation definitions. Similarly, the third-party program must provide vector quantities that are imported into Abaqus in the global coordinate system of the Abaqus model. The third-party analysis program may use different conventions, please refer to the appropriate third-party program documentation for further modeling details and/or limitations. Unit system Abaqus does not require that the analysis be run with a particular unit system. In general, the unit system used in creating the Abaqus model may not be the same as that used with the third-party program model. When the two unit systems differ, the fields exchanged between the two programs must go through a transformation of units. Refer to the appropriate third-party program documentation for further modeling details. For the coupling with MADYMO you can specify a set of conversion factors for the basic units of mass, length, and time. If a field with the units of length is exported, Abaqus multiplies this quantity by the length unit conversion factor prior to exporting the value to the third-party program. Similarly, if a field with the units of length is imported, Abaqus divides this quantity from the third-party program by the length unit conversion factor prior to using the field in the Abaqus model. The conversion factors are constructed for the various fields that are exchanged based on the conversion factors for the basic units. Input File Usage: Use the following option to specify unit conversion factors when there is a mismatch in unit systems between the Abaqus/Explicit model and the MADYMO model: *CO-SIMULATION, PROGRAM=MADYMO mass unit conversion factor, length unit conversion factor, time unit conversion factor Restarting a co-simulation Interface loads imported into Abaqus/Standard, Abaqus/Explicit, or Abaqus/CFD are not saved to the Abaqus restart database. Thus, to restart a co-simulation, the coupled analysis must send the loads at the start of the restart analysis. These loads must balance the current deformation of the Abaqus analysis such that the structure is in equilibrium. You must synchronize the restart information written between the analyses to ensure that the simulation is restarted at the same solution (step) time. For more information, see “Synchronizing restart information written in a co-simulation” in “Restarting an analysis,” Section 9.1.1. For example, to restart an FSI co-simulation, the solution time for the particular step/increment number from which Abaqus is restarted must correspond to the coupled analysis solution. Limitations The following limitations apply: • The steps in the Abaqus model must be defined such that the co-simulation fits entirely within a single Abaqus step. Further, there can be only one co-simulation in the Abaqus job. You can use the restart capability to perform multiple co-simulations for an analysis . • A co-simulation surface or volume defined over beam, pipe, and truss elements or defined over the edges of three-dimensional elements cannot be used as an interface region. You should use discrete points to transfer loads and boundary conditions. • A co-simulation surface or volume defined over modified triangular elements or modified tetrahedral elements cannot be used as an interface region. There may be further limitations depending on the third-party analysis program being used. For more information, refer to the appropriate third-party program documentation. 17.3 Co-simulation between Abaqus solvers • “Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 17.3.1 • “Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 17.3.2 17.3.1 Abaqus/Standard TO Abaqus/Explicit CO-SIMULATION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution,” Section 3.2.4 • “Co-simulation: overview,” Section 17.1.1 • “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1 • *CO-SIMULATION • *CO-SIMULATION CONTROLS • “Defining a Standard-Explicit co-simulation interaction,” Section 15.13.14 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • Chapter 26, “Co-simulation,” of the Abaqus/CAE User’s Manual Overview This section discusses analysis setup, execution, and limitation details specific to Abaqus/Standard to Abaqus/Explicit co-simulation. Refer to “Dynamic impact of a scooter with a bump,” Section 2.4.1 of the Abaqus Example Problems Manual, for an example of Abaqus/Standard to Abaqus/Explicit co-simulation. Identifying the Abaqus step for the co-simulation analysis The following Abaqus/Standard analysis procedures can be used for an Abaqus/Standard to Abaqus/Explicit co-simulation: • “Static stress analysis,” Section 6.2.2 • “Implicit dynamic analysis using direct integration,” Section 6.3.2 The following Abaqus/Explicit analysis procedure can be used for an Abaqus/Standard to Abaqus/Explicit co-simulation: • “Explicit dynamic analysis,” Section 6.3.3 Input File Usage: Use the following option within a step definition for an Abaqus/Standard to Abaqus/Explicit co-simulation: Abaqus/CAE Usage: *CO-SIMULATION, PROGRAM=ABAQUS Use the following option for an Abaqus/Standard to Abaqus/Explicit co-simulation: Interaction module: Create Interaction: Standard-Explicit co-simulation Identifying the co-simulation interface region Interaction between the Abaqus/Standard and Abaqus/Explicit models takes place through a common interface region. You can specify an interface region using either node sets or surfaces when coupling Abaqus/Standard to Abaqus/Explicit. You must, however, be consistent in your region definition in Abaqus/Standard and Abaqus/Explicit; if you define a co-simulation region with a node set or node-based surface in one analysis, you must use the same type of co-simulation region definition in the other analysis. Likewise, if you define a co-simulation region with an element-based surface in one analysis, you must define your co-simulation region with an element-based surface in the other analysis. You may have dissimilar meshes in regions shared in the Abaqus/Standard and Abaqus/Explicit model definitions. In some cases, however, you can improve solution stability and accuracy by ensuring that you have matching nodes at the interface . In these cases you can use the modeling practice described in “Ensuring matching nodes at the interface regions,” Section 26.4 of the Abaqus/CAE User’s Manual, to ensure these matching nodes. Input File Usage: Use the following option to define an element-based or node-based surface as a co-simulation region in an Abaqus model: *CO-SIMULATION REGION, TYPE=SURFACE (default) surface_A Use the following option to define a node set as a co-simulation region in an Abaqus model: *CO-SIMULATION REGION, TYPE=NODE nodeset_A Only one *CO-SIMULATION REGION option can be defined in each Abaqus analysis. In addition, only one node set or surface can be defined. Abaqus/CAE Usage: Interaction module: Create Interaction: Standard-Explicit co-simulation: Surface or Node Region: select region Identifying the fields exchanged across a co-simulation interface For Abaqus/Standard to Abaqus/Explicit co-simulation, you do not define the fields exchanged; they are determined automatically according to the procedures and co-simulation parameters used. Defining the rendezvousing scheme Co-simulation controls are used to control the time incrementation process and the frequency of exchange between the two Abaqus analyses. Input File Usage: Abaqus/CAE Usage: Use both of the following options to specify co-simulation controls: *CO-SIMULATION, PROGRAM=ABAQUS, CONTROLS=name *CO-SIMULATION CONTROLS, NAME=name Interaction module: Create Interaction: Standard-Explicit co-simulation Time incrementation scheme You can force Abaqus/Standard to use the same increment size as Abaqus/Explicit, or you can allow the increment sizes in Abaqus/Standard to differ from those in Abaqus/Explicit (subcycling). The time incrementation scheme that you choose for coupling affects the solution computational cost and accuracy but not the solution stability. The subcycling scheme is frequently the most cost effective since Abaqus/Standard time increments, free of any forced co-simulation time incrementation constraints, are commonly much longer than Abaqus/Explicit time increments. The subcycling scheme, however, may be less cost effective when a large portion of the nodes in the model are at the co-simulation interface. This is because Abaqus/Standard performs a set of stabilization operations at the interface (a “free solve”) for each increment in the Abaqus/Explicit analysis. These free-solve operations require an implicit solution of a dense system of equations that scale with the number of interface nodes. In cases of a large number of interface nodes the computational cost of this interface solve can exceed any cost savings seen due to subcycling. Hence, for a model where a significant share of the nodes are at the co-simulation interface performance may be poorer with the subcycling scheme. Forcing Abaqus to use a single increment per coupling step You can force Abaqus/Standard to match the increment size of Abaqus/Explicit, and fields will be exchanged at each of the shared increments. Input File Usage: Use the following option in the Abaqus/Standard analysis and in the Abaqus/Explicit analysis: Abaqus/CAE Usage: *CO-SIMULATION CONTROLS, TIME INCREMENTATION=LOCKSTEP Use the following input in the Abaqus/Standard analysis and in the Abaqus/Explicit analysis: Interaction module: Create Interaction: Standard-Explicit co-simulation: Incrementation control: Lock time steps Allowing Abaqus to subcycle You can allow the Abaqus/Standard increment size to differ from those in Abaqus/Explicit. In this case fields will be exchanged as needed. Input File Usage: Use the following option in the Abaqus/Standard analysis and in the Abaqus/Explicit analysis: *CO-SIMULATION CONTROLS, TIME INCREMENTATION=SUBCYCLE Abaqus/CAE Usage: Use the following input Abaqus/Explicit analysis: in the Abaqus/Standard analysis and in the Interaction module: Create Interaction: Standard-Explicit co-simulation: Incrementation control: Allow subcycling Controlling interface matrix factorization frequency For the subcycling time incrementation scheme an interface solve is performed, by default, in Abaqus/Standard for every Abaqus/Explicit increment. This solve can be significantly costly for two reasons. First, the interface matrix used for the interface solve is dense and its size scales with the number of interface nodes. Second, the interface matrix changes every Abaqus/Explicit increment, requiring factorization in Abaqus/Standard for every Abaqus/Explicit increment. You can reduce the impact of this cost by approximating the interface matrix and factorizing it typically once for the duration of an Abaqus/Standard increment, rather than for each Abaqus/Explicit increment. However, if the Abaqus/Explicit stable time increment changes significantly, the interface matrix is refactored for stability reasons. Allowing Abaqus/Standard to factorize the interface matrix every Abaqus/Explicit increment Factorizing the interface matrix every Abaqus/Explicit increment is the default approach. Input File Usage: Use the following option in the Abaqus/Standard analysis: *CO-SIMULATION CONTROLS, FACTORIZATION FREQUENCY=EXPLICIT INCREMENT Abaqus/CAE Usage: Factorizing the interface matrix every Abaqus/Explicit increment is used by default in Abaqus/CAE. Forcing Abaqus/Standard to factorize the interface matrix once per Abaqus/Standard increment When the number of interface nodes is large, the cost of the interface factorization can be significantly reduced by using this approach. Only the interface matrix factorization is performed once per Abaqus/Standard increment; the interface solve is performed every Abaqus/Explicit increment using this factorized interface matrix. Since this approach approximates the interface matrix, it may slightly increase the drift in the displacement solution at the co-simulation interface. The performance gain with this method depends on the number of interface nodes, the subcycling ratio (which is the ratio between Abaqus/Standard and Abaqus/Explicit increments), and the size of the models. For models with greater than 100 interface nodes and a subcycling ratio greater than 50, this method typically reduces the analysis time by a factor between 1.2 and 3.0. The performance gain increases for larger subcycling ratios and decreases for larger models. Input File Usage: Use the following option in the Abaqus/Standard analysis: *CO-SIMULATION CONTROLS, FACTORIZATION FREQUENCY=STANDARD INCREMENT Abaqus/CAE Usage: Factorizing the interface matrix once per Abaqus/Standard increment is not supported in Abaqus/CAE. Coupling step size The coupling step size is the period between two consecutive co-simulation data exchanges between Abaqus/Standard and Abaqus/Explicit and always equals the current Abaqus/Explicit increment size. When using the subcycling method, this data exchange does not represent a constraint on Abaqus/Standard incrementation; the Abaqus/Standard analysis advances in time using its normal time incrementation logic, but performs data exchanges as needed at the coupling step size intervals. Variable coupling step size If you do not specify a constant coupling step size, Abaqus/Standard and Abaqus/Explicit use the next Abaqus/Explicit increment size as the coupling step size. Input File Usage: Abaqus/CAE Usage: Use the following option in either or both of the Abaqus/Standard and Abaqus/Explicit analyses: *CO-SIMULATION CONTROLS (omit the STEP SIZE parameter) Use the following input in the Abaqus/Standard and Abaqus/Explicit analyses: Interaction module: Create Interaction: Standard-Explicit co-simulation: Coupling step period: Determined by analysis Constant user-defined coupling step size A constant user-defined coupling step size can be specified. Since data exchange occurs at every Abaqus/Explicit increment, the Abaqus/Explicit increment will be set equal to the user-defined coupling step size. This is functionally equivalent to specifying direct user control on the increment size in Abaqus/Explicit. In Abaqus/Standard the step size parameter is ignored for Abaqus/Standard to Abaqus/Explicit co-simulation. Input File Usage: Abaqus/CAE Usage: In the Abaqus/Explicit analysis you may optionally specify a step size: *CO-SIMULATION CONTROLS, STEP SIZE=coupling_step_size Use the following input in the Abaqus/Explicit analysis: Interaction module: Create Interaction: Standard-Explicit co-simulation: Coupling step period: Specified: coupling_step_size Executing the coupled analysis jobs as described in “Abaqus/Standard, You execute the Abaqus/Standard and Abaqus/Explicit Abaqus/Explicit, and Abaqus/CFD co-simulation execution,” Section 3.2.4. the Abaqus/Explicit packager and analysis are both run in double precision to avoid numerical instabilities. You can execute the coupled analysis interactively in Abaqus/CAE as described in “Understanding By default, co-executions,” Section 19.4 of the Abaqus/CAE User’s Manual. Input File Usage: Enter the following input on the command line: Abaqus/CAE Usage: abaqus cosimulation cosimjob=cosim-job-name job=job-name-A,job-name-B Job module: Co-execution→Create: select the Abaqus/Standard model and the Abaqus/Explicit model; Communication time out: timeout-value Co-execution→Manager: Submit Considerations for using the timeout parameter The timeout execution parameter specifies the amount of time in seconds that each analysis waits to receive the co-simulation message expected from the other analysis that is running. The default timeout value is 60 minutes when submitting jobs using the command line options and 10 minutes when executing the jobs in Abaqus/CAE. When the timeout period is large compared to typical analysis increment wallclock times, you have greater flexibility in starting jobs and performing operations that precede the co-simulation analysis step. Examples where this flexibility is needed include: job submission using queues, analyses where steps that precede the co-simulation step have long run times, and cases where one job is resubmitted because of an input error. However, a large timeout period can cause problems when one of the co-simulation jobs fails (for reasons such as convergence issues or availability of computer resources) before the initial co-simulation communication is established. In these cases you may prefer to kill the job left running rather than have it wait the entire timeout period. Command usage example Use the following command to submit a co-simulation between an Abaqus/Standard analysis called “std” and an Abaqus/Explicit analysis called “xpl”: abaqus cosimulation cosimjob=beam job=std,xpl Diagnostics information The Abaqus/Standard job provides detailed descriptions of co-simulation operations in the message (.msg) file. For the subcycling scheme the status (.sta) file provides summary information indicating when the interface calculations followed by re-solve of the increment are made, as shown in the following example status file. The E suffix in the attempt-count entry (column 3) indicates an increment performing interface calculations. An increment without the E suffix indicates re-solve of the increment. SUMMARY OF JOB INFORMATION: STEP INC ATT SEVERE EQUIL TOTAL DISCON ITERS ITERS ITERS 1E 1E 1E 1E TOTAL TIME/ FREQ 0.000 0.00100 0.00100 0.00200 0.00200 0.00300 0.00300 0.00400 STEP TIME/LPF INC OF TIME/LPF DOF IF MONITOR RIKS 0.000 0.00100 0.00100 0.00200 0.00200 0.00300 0.00300 0.00400 0.001000 0.001000 0.001000 0.001000 0.001000 0.001000 0.001000 0.001000 The Abaqus/Explicit job provides summary descriptions of co-simulation operations in the status (.sta) file. Limitations The following limitations apply to Abaqus/Standard to Abaqus/Explicit co-simulation in addition to the limitations discussed in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1. General limitations • Displacement compatibility at the co-simulation interface is not maintained when you allow the Abaqus/Standard increment size to differ from that in Abaqus/Explicit (i.e., when you specify subcycling as a co-simulation time incrementation control). In this case velocity compatibility is maintained, but you may see small amounts of displacement mismatch between Abaqus/Standard and Abaqus/Explicit as the simulation advances in time. This “drift” is more pronounced if severe nonlinearity such as plastic deformation occurs at the co-simulation interface. You can control this drift by adjusting Abaqus/Standard solution parameters so that the Abaqus/Standard increment size is reduced (e.g., by limiting the maximum time increment size or specifying a smaller half-increment residual tolerance for implicit dynamic analyses). • Nodal transformations are not permitted on the co-simulation region nodes. • The ALE technique may not be used in elements attached to co-simulation region nodes. • Fully coupled temperature-displacement elements can be used, but no temperature quantities are exchanged. • An Abaqus/Standard static stress analysis cannot be used with the lockstep time incrementation scheme in Abaqus/Standard to Abaqus/Explicit co-simulation. Dissimilar mesh-related limitations When your Abaqus/Standard and Abaqus/Explicit co-simulation region meshes differ, the following limitations apply: • Solution accuracy may be affected when your co-simulation region meshes are not uniform in the presence or absence of rotational degrees of freedom; for example, if a continuum element mesh is locally reinforced with beam or shell elements at the co-simulation region interface. • In cases where the stress state near the co-simulation interface is significant (approaching 1% or more) relative to the material stiffness, you may observe appreciable irregular mesh distortion if the mesh density adjacent to the co-simulation region differs greatly between the Abaqus/Explicit and Abaqus/Standard models. For example, this effect is common with large deformation of hyperelastic materials. You can minimize this effect by choosing a similar or finer mesh at the Abaqus/Standard co-simulation region when using the subcycling time integration scheme or by choosing a similar or finer mesh at the Abaqus/Explicit co-simulation region when using the lockstep time integration scheme. Abaqus/Standard analysis limitations Abaqus/Standard elements that have no equivalent degree-of-freedom counterpart in Abaqus/Explicit cannot be connected to co-simulation region nodes. These elements include • Axisymmetric elements with twist degrees of freedom (the CGAX element family) • Axisymmetric solid elements with asymmetric deformation (the CAXA element family) • Generalized plane strain elements (the CPEG element family) • Coupled pore pressure-displacement elements • Heat transfer and thermal-electrical elements • Acoustic elements • Piezoelectric elements The following specific limitations also apply: • A co-simulation region node cannot be a slave node in a tie constraint, an MPC constraint, or a kinematic coupling constraint. Abaqus/Explicit analysis limitations Stability and accuracy of the co-simulation solution may be adversely affected when the following model features are defined at or near the co-simulation region: • Connector elements connected to co-simulation region nodes. • Co-simulation region nodes that participate in a tie constraint, an MPC constraint, or a kinematic coupling constraint. When using these features, you should compare the Abaqus/Standard and Abaqus/Explicit solutions (e.g., compatibility of the displacement history) at the co-simulation interface as an indicator of solution accuracy. 17.3.2 Abaqus/CFD TO Abaqus/Standard OR TO Abaqus/Explicit CO-SIMULATION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution,” Section 3.2.4 • “Co-simulation: overview,” Section 17.1.1 • “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1 • *CO-SIMULATION • *CO-SIMULATION CONTROLS • “Defining a fluid-structure co-simulation interaction,” Section 15.13.15 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • Chapter 26, “Co-simulation,” of the Abaqus/CAE User’s Manual Overview This section discusses analysis setup, execution, and limitation details specific to Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation for fluid-structure interaction and conjugate heat transfer. Refer to “Conjugate heat transfer analysis of a component-mounted electronic circuit board,” for an example of Abaqus/CFD to Section 6.1.1 of the Abaqus Example Problems Manual, Abaqus/Standard co-simulation. Identifying the Abaqus step for the co-simulation analysis The following Abaqus/CFD analysis procedure can be used for co-simulation with Abaqus/Standard or Abaqus/Explicit: • “Incompressible fluid dynamic analysis,” Section 6.6.2 The following Abaqus/Standard analysis procedures can be used for co-simulation with Abaqus/CFD: • “Implicit dynamic analysis using direct integration,” Section 6.3.2 • “Uncoupled heat transfer analysis,” Section 6.5.2 The following Abaqus/Explicit analysis procedures can be used for co-simulation with Abaqus/CFD: • “Explicit dynamic analysis,” Section 6.3.3 • “Fully coupled thermal-stress analysis in Abaqus/Explicit” in “Fully coupled thermal-stress analysis,” Section 6.5.3 Input File Usage: Use the following option within a step definition for an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation: *CO-SIMULATION, PROGRAM=MULTIPHYSICS Abaqus/CAE Usage: Use the following option for an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation: Interaction module: Create Interaction: Fluid-Structure Co-simulation boundary Identifying the co-simulation interface region You specify an interface region using surfaces when coupling Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit. You must define an element-based surface, and you can specify only one surface to be used as the interface region in the analysis. You may have dissimilar meshes in regions shared in the model definitions. Input File Usage: Use the following option to define an element-based surface as a co-simulation region: *CO-SIMULATION REGION, TYPE=SURFACE surface_A Abaqus/CAE Usage: Interaction module: Create Interaction: Fluid-Structure Co-simulation boundary: select surface region Identifying the fields exchanged across a co-simulation interface For Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation, see the tables in “Identifying the fields exchanged across a co-simulation interface” in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1, for lists of fields that are available for co-simulation exchange. When using Abaqus/CAE, the fields exchanged are determined automatically by Abaqus/CAE. Defining the rendezvousing scheme Co-simulation controls are used to control the time incrementation process and the frequency of exchange between the two Abaqus analyses. These controls are specified automatically in Abaqus/CAE. Input File Usage: Abaqus/CAE Usage: Use both of the following options to specify co-simulation controls: *CO-SIMULATION, PROGRAM=MULTIPHYSICS, CONTROLS=name *CO-SIMULATION CONTROLS, NAME=name Interaction module: Create Interaction: Fluid-Structure Co-simulation boundary Defining the coupling scheme The sequential explicit coupling scheme (also referred to as the Gauss-Seidel coupling algorithm) is the only coupling scheme available for Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation. By default, the Abaqus/CFD analysis lags the co-simulation and the Abaqus/Standard or Abaqus/Explicit analysis leads the co-simulation. For conjugate heat transfer, the Abaqus/CFD analysis can either lag or lead the co-simulation. For fluid-structure interaction, the Abaqus/CFD analysis must lag the co-simulation and the Abaqus/Standard or Abaqus/Explicit analysis must lead the co-simulation. Input File Usage: Use the following option to specify that the analysis leads the co-simulation: *CO-SIMULATION CONTROLS, SCHEME MODIFIER=LEAD Use the following option to specify that the analysis lags the co-simulation: *CO-SIMULATION CONTROLS, SCHEME MODIFIER=LAG The coupling scheme is specified automatically in Abaqus/CAE when you define a fluid-structure co-simulation interaction. Abaqus/CAE Usage: Coupling step size The coupling step size is the period between two consecutive co-simulation data exchanges. The coupling step size is determined automatically based on the type of analysis and is used to obtain time-accurate solutions for the coupled physics problem. For fluid-structure interaction (FSI) and conjugate heat transfer (CHT) analyses that couple Abaqus/CFD and Abaqus/Standard, the coupling step size is the minimum of the time step sizes determined by the automatic time incrementation schemes of the individual analyses. For FSI problems that couple Abaqus/CFD and Abaqus/Explicit, Abaqus/Explicit imports the coupling step size from Abaqus/CFD; consequently, Abaqus/CFD exports the coupling step size to Abaqus/Explicit. Time incrementation scheme Depending on the type of analysis, Abaqus may either perform one increment (referred to as “lockstep”) or several increments (referred to as “subcycling”) per coupling step. By default, for FSI and CHT analyses that couple Abaqus/CFD and Abaqus/Standard, there is no subcycling involved because the coupling step size is based on the minimum of the individual analyses. For FSI analyses that couple Abaqus/CFD and Abaqus/Explicit, Abaqus/Explicit typically uses subcycling while Abaqus/CFD uses lockstep behavior. Input File Usage: Use the following option to allow the analysis to subcycle: *CO-SIMULATION CONTROLS, TIME INCREMENTATION=SUBCYCLE Use the following option to force the analysis to use a single increment per coupling step: *CO-SIMULATION CONTROLS, TIME INCREMENTATION=LOCKSTEP The time incrementation scheme is specified automatically in Abaqus/CAE when you define a fluid-structure co-simulation interaction. Abaqus/CAE Usage: Reaching target times The Abaqus target times can be reached in an exact or loose manner. By default, Abaqus exchanges the data in an exact manner; that is, Abaqus temporarily reduces the time increment so that the solution exchange occurs exactly at the target time. When subcycling Abaqus may reach the target time in a loose manner; that is, when the current simulation time, t, is within half of an Abaqus increment size away from the target time, Input File Usage: Use the following option to reach target times in an exact manner: *CO-SIMULATION CONTROLS, TIME MARKS=YES (default) Use the following option to reach target times in a loose manner: Abaqus/CAE Usage: *CO-SIMULATION CONTROLS, TIME MARKS=NO The manner is which target times are reached is specified automatically in Abaqus/CAE when you define a fluid-structure co-simulation interaction. Executing the coupled analysis You execute the Abaqus/CFD and Abaqus/Standard or Abaqus/Explicit jobs as described in “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution,” Section 3.2.4. By default, when coupling Abaqus/CFD to Abaqus/Explicit, the Abaqus/Explicit packager and analysis are both run in single precision. You can execute the coupled analysis interactively in Abaqus/CAE as described in “Understanding co-executions,” Section 19.4 of the Abaqus/CAE User’s Manual. Input File Usage: Enter the following input on the command line: Abaqus/CAE Usage: abaqus cosimulation cosimjob=cosim-job-name job=job-name-A,job-name-B Job module: Co-execution→Create: select the models and define initial job parameter settings Co-execution→Manager: Submit Considerations for using the timeout parameter The timeout execution parameter specifies the amount of time in seconds that each analysis waits to receive the co-simulation message expected from the other analysis that is running. The default timeout value is 60 minutes when submitting jobs using the command line options and 10 minutes when executing the jobs in Abaqus/CAE. When the timeout period is large compared to typical analysis increment wallclock times, you have greater flexibility in starting jobs and performing operations that precede the co-simulation analysis step. Examples where this flexibility is needed include: job submission using queues, analyses where steps that precede the co-simulation step have long run times, and cases where one job is resubmitted because of an input error. However, a large timeout period can cause problems when one of the co-simulation jobs fails (for reasons such as convergence issues or availability of computer resources) before the initial co-simulation communication is established. In these cases you may prefer to kill the job left running rather than have it wait the entire timeout period. Command usage example Use the following command to run a co-simulation between a heat transfer analysis called “solid_heat” and a fluids analysis called “fluid”, interactively: abaqus cosimulation cosimjob=cosim_cht job=solid_heat,fluid interactive Limitations The following limitations apply to Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation in addition to the limitations discussed in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1. General limitation An interface region can be used for fluid-structure interaction or conjugate heat transfer but not both. Abaqus/Standard analysis limitations Abaqus/Standard elements that have no equivalent degree-of-freedom counterpart in Abaqus/CFD cannot be connected to co-simulation region nodes. These elements include the following: • Axisymmetric elements with twist degrees of freedom (the CGAX element family) • Axisymmetric solid elements with asymmetric deformation (the CAXA element family) • Generalized plane strain elements (the CPEG element family) • Coupled pore pressure-displacement elements • Acoustic elements • Piezoelectric elements 18. Extending Abaqus Analysis Functionality User subroutines and utilities 18.1 User subroutines and utilities • “User subroutines: overview,” Section 18.1.1 • “Available user subroutines,” Section 18.1.2 • “Available utility routines,” Section 18.1.3 18.1.1 USER SUBROUTINES: OVERVIEW References • “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2 • Abaqus User Subroutines Reference Manual Overview User subroutines: • are provided to increase the functionality of several Abaqus capabilities for which the usual data input methods alone may be too restrictive; • provide an extremely powerful and flexible tool for analysis; • are typically written as FORTRAN code and must be included in a model when you execute the analysis, as discussed below; • must be included and, if desired, can be revised in a restarted run, since they are not saved to the restart files ; • cannot be called one from another; and • can in some cases call utility routines that are also available in Abaqus . Including user subroutines in a model You can include one or more user subroutines in a model by specifying the name of a FORTRAN source or object file that contains the subroutines. Details are provided in “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2. Input File Usage: Enter the following input on the command line: Abaqus/CAE Usage: Job module: job editor: General: User subroutine file abaqus job=job-name user={source-file | object-file} Managing external databases in Abaqus/Standard and exchanging information with other software In Abaqus/Standard it is sometimes desirable to set up the FORTRAN environment and manage interactions with external data files that are used in conjunction with user subroutines. For example, there may be history-dependent quantities to be computed externally, once per increment, for use during the analysis; or output quantities that are accumulated over multiple elements in COMMON block variables within user subroutines may need to be written to external files at the end of a converged increment for postprocessing. Such operations can be performed with user subroutine UEXTERNALDB. This user interface can potentially be used to exchange data with another code, allowing for “stagger” between Abaqus/Standard and another code. Writing a user subroutine User subroutines should be written with great care. To ensure their successful implementation, the rules and guidelines below should be followed. For a detailed discussion of the individual subroutines, including coding interfaces and requirements, refer to the Abaqus User Subroutines Reference Manual. Required INCLUDE statement Every Abaqus/Standard user subroutine must include the statement include 'aba_param.inc' as the first statement after the argument list. Every Abaqus/Explicit user subroutine must include the statement include 'vaba_param.inc' as the first statement after the argument list. If variables are exchanged between the main user subroutine and subsequent subroutines, the user should specify the above include statement in all the subroutines to preserve precision. The files aba_param.inc and vaba_param.inc are installed on the system by the Abaqus installation procedure and contain important installation parameters. These statements tell the Abaqus execution procedure, which compiles and links the user subroutine with the rest of Abaqus, to include the aba_param.inc or vaba_param.inc file automatically. It is not necessary to find the file and copy it to any particular directory; Abaqus will know where to find it. Naming convention If user subroutines call other subroutines or use COMMON blocks to pass information, such subroutines or COMMON blocks should begin with the letter K since this letter is never used to start the name of any subroutine or COMMON block in Abaqus. Redefining variables User subroutines must perform their intended function without overwriting other parts of Abaqus. In particular, you should redefine only those variables identified in this chapter as “variables to be defined.” Redefining “variables passed in for information” will have unpredictable effects. Compilation and linking problems If problems are encountered during compilation or linking of the subroutine, make sure that the Abaqus environment file (the default location for this file is the site subdirectory of the Abaqus installation) contains the correct compile and link commands as specified in the Abaqus Installation and Licensing Guide. These commands should have been set up by the Abaqus site manager during installation. The number and type of arguments must correspond to what is specified in the documentation. Mismatches in type or number of arguments may lead to platform-dependent linking or runtime errors. Memory allocation considerations Your user subroutine will share memory resources with Abaqus. When you need to use large arrays or other large data structures, you should allocate their memory dynamically, so that memory is allocated from the heap and not the stack. Failure to dynamically allocate large arrays may result in stack overflow errors and an abort of your Abaqus analysis. For an example of dynamic allocation of an array in a FORTRAN program, refer to “Creation of a data file to facilitate the postprocessing of elbow element results: FELBOW,” Section 14.1.6 of the Abaqus Example Problems Manual. Testing and debugging When developing user subroutines, test them thoroughly on smaller examples in which the user subroutine is the only complicated aspect of the model before attempting to use them in production analysis work. If needed, debug output can be written to the Abaqus/Standard message (.msg) file using FORTRAN unit 7 or to the Abaqus/Standard data (.dat) file or the Abaqus/Explicit status (.sta) file using FORTRAN unit 6; these units should not be opened by your routines since they are already opened by Abaqus. FORTRAN units 15 through 18 or units greater than 100 can be used to read or write other user- specified information. The use of other FORTRAN units may interfere with Abaqus file operations; see “FORTRAN unit numbers used by Abaqus,” Section 3.7.1. You must open these FORTRAN units; and because of the use of scratch directories, the full pathname for the file must be used in the OPEN statement. Terminating an analysis Utility routine XIT (Abaqus/Standard) or XPLB_EXIT (Abaqus/Explicit) should be used instead of STOP when terminating an analysis from within a user subroutine. This will ensure that all files associated with the analysis are closed properly (“Terminating an analysis,” Section 2.1.15 of the Abaqus User Subroutines Reference Manual). Models defined in terms of an assembly of part instances An Abaqus model can be defined in terms of an assembly of part instances . Reference coordinate system Although a local coordinate system can be defined for each part instance, all variables (such as current coordinates) are passed to a user subroutine in the global coordinate system, not in a part-local coordinate system. The only exception to this rule is when the user subroutine interface specifically indicates that a variable is in a user-defined local coordinate system (“Orientations,” Section 2.2.5, or “Transformed coordinate systems,” Section 2.1.5). The local coordinate system originally may have been defined relative to a part coordinate system, but it was transformed according to the positioning data given for the part instance. As a result, a new local coordinate system was created relative to the assembly (global) coordinate system. This new coordinate system definition is the one used for local orientations in user subroutines. Node and element numbers The node and element numbers passed to a user subroutine are internal numbers generated by Abaqus. These numbers are global in nature; all internal node and element numbers are unique. If the original number and the part instance name are required, call the utility subroutine GETPARTINFO (Abaqus/Standard) or VGETPARTINFO (Abaqus/Explicit) from within your user subroutine . The expense of calling these routines is not trivial, so minimal use of them is recommended. utility Another or VGETINTERNAL (Abaqus/Explicit), can be used to retrieve the internal node or element number corresponding to a given part instance name and local number. GETINTERNAL (Abaqus/Standard) subroutine, Set and surface names Set and surface names passed to user subroutines are always prefixed by the assembly and part instance names, separated by underscores. For example, a surface named surf1 belonging to part instance Part1-1 in assembly Assembly1 will be passed to a user subroutine as Assembly1_Part1-1_surf1 Solution-dependent state variables Solution-dependent state variables are values that can be defined to evolve with the solution of an analysis. Defining and updating Any number of solution-dependent state variables can be used in the following user subroutines: • CREEP • FRIC • HETVAL • UANISOHYPER_INV • UANISOHYPER_STRAIN • UEL • UEXPAN • UGENS • UHARD • UHYPER • UINTER • UMAT • UMATHT • UMULLINS • USDFLD • UTRS • VFABRIC • VFRIC • VFRICTION • VUANISOHYPER_INV • VUANISOHYPER_STRAIN • VUFLUIDEXCH • VUHARD • VUINTER • VUINTERACTION • VUMAT • VUMULLINS • VUSDFLD • VUTRS • VUVISCOSITY • VWAVE The state variables can be defined as a function of any other variables appearing in these subroutines and can be updated accordingly. Solution-dependent state variables should not be confused with field variables, which may also be needed in the constitutive routines and can vary with time; field variables are discussed in detail in “Predefined fields,” Section 33.6.1. state and VUINTERACTION are defined as state variables at slave nodes and are updated with other contact variables. in VFRIC, VUINTER, VFRICTION, Solution-dependent variables used Allocating space You must allocate space for each of the solution-dependent state variables at every applicable integration point or contact slave node. Separate user subroutine groups have been identified that differ in the way the number of solution-dependent state variables is defined. These groups are described below. Solution-dependent state variables can be shared by subroutines within the same group; they cannot be shared between subroutines belonging to different groups. Input File Usage: For most subroutines the number of such variables required at the points or nodes is entered as the only value on the data line of the *DEPVAR option, Abaqus/CAE Usage: which should be included as part of the material definition for every material in which solution-dependent state variables are to be considered: *DEPVAR For subroutines that do not use the material behavior defined with the *MATERIAL option, the *DEPVAR option is not used. For subroutine UEL: *USER ELEMENT, VARIABLES=number of variables For subroutine UGENS: *SHELL GENERAL SECTION, USER, VARIABLES=number of variables For subroutines FRIC and VFRIC: *FRICTION, USER, DEPVAR=number of variables For subroutines UINTER and VUINTER: *SURFACE INTERACTION, USER, DEPVAR=number of variables For subroutine VFRICTION: *FRICTION, USER=FRICTION, DEPVAR=number of variables For subroutine VUFLUIDEXCH: *FLUID EXCHANGE PROPERTY, TYPE=USER, DEPVAR=number of variables For subroutine VUINTERACTION: *SURFACE INTERACTION, USER=INTERACTION, DEPVAR=number of variables For subroutine VWAVE: *WAVE, TYPE=USER, DEPVAR=number of variables For most subroutines the number of such variables required at the points or nodes is entered as part of the material definition for every material in which solution-dependent state variables are to be considered: Property module: material editor: General→Depvar: Number of solution-dependent state variables Defining initial values You can define the initial values of solution-dependent state variable fields directly or in Abaqus/Standard through a user subroutine. The initial values of solution-dependent state variables for contact or for user subroutine VWAVE in Abaqus/Explicit are assigned as zero internally. Defining initial values directly You can define the initial values in a tabular format for elements and/or element sets. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1, for additional details. Input File Usage: *INITIAL CONDITIONS, TYPE=SOLUTION Defining initial values in a user subroutine in Abaqus/Standard For complicated cases in Abaqus/Standard you can call user subroutine SDVINI so that dependencies on coordinates, element numbers, etc. can be used in the definition of the variable field. Input File Usage: *INITIAL CONDITIONS, TYPE=SOLUTION, USER Output User-defined, solution-dependent state variables can be written to the data (.dat) file, the output database (.odb) file, and the results (.fil) file; the output identifiers SDV and SDVn are available as element integration variables . Output of these variables is not available for user subroutines VFRIC, VUINTER, VFRICTION, VUINTERACTION, and VWAVE. Alphanumeric data Alphanumeric data, such as labels (names) of surfaces or materials, are always passed into user subroutines in the upper case. As a result, direct comparison of these labels with corresponding lower-case characters will fail. Upper case must be used for all such comparisons. An example of such a comparison can be found in “UMAT,” Section 1.1.40 of the Abaqus User Subroutines Reference It illustrates the code setup inside user subroutine UMAT when more than one user-defined Manual. material model needs to be defined. The variable CMNAME is compared against MAT1 and MAT2 (even in situations where the material names may have been defined as mat1 and mat2, respectively.) Precision in Abaqus/Explicit Abaqus/Explicit is installed with both single precision and double precision executables. To use the double precision executable, you must specify double precision when you run the analysis . All variables in the user subroutines that start with the letters a to h and o to z will automatically be defined in the precision of the executable that you run. The precision of the executable is defined in the vaba_param.inc file, and it is not necessary to define the precision of the variables explicitly. Vectorization in Abaqus/Explicit Abaqus/Explicit user subroutines are written with a vector interface, which means that blocks of data are passed to the user subroutines. For example, the vectorized user material routines (VFABRIC and VUMAT) are passed stresses, strains, state variables, etc. for nblock material points. One of the parameters defined by vaba_param.inc is maxblk, the maximum block size. If the user subroutine requires the dimensioning of temporary arrays, they can be dimensioned by maxblk. Parallelization User subroutines can be used when running jobs in parallel. However, the use of common block statements in the user subroutines or in subroutines called by the user subroutines must be avoided since it will result in unpredictable behavior of the executable. User subroutine calls Most of the user subroutines available in Abaqus are called at least once for each increment during an analysis step. However, as discussed below, many subroutines are called more or less often. Subroutines that define material, element, or interface behavior Most user subroutines that are used to define material, element, or interface behavior are called twice per material point, element, or slave surface node in the first iteration of every increment such that the model’s initial stiffness matrix can be formulated appropriately for the step procedure chosen. The subroutines are called only once per material point, element, or slave surface node in each succeeding iteration within the increment. By default, in transient implicit dynamic analyses (“Implicit dynamic analysis using direct integration,” Section 6.3.2) Abaqus/Standard calculates accelerations at the beginning of each dynamic step. Abaqus/Standard must call user subroutines that are used to define material, element, or interface behavior two extra times for each material point, element, or slave surface node prior to the zero increment. The extra calls to the user subroutines are not made if the initial acceleration calculations If the half-increment residual tolerances are being checked in a transient implicit are suppressed. dynamic step, Abaqus/Standard must call these user subroutines (except UVARM) one extra time for each material point, element, or slave surface node at the end of each increment. If the calculation of the half-increment residual is suppressed, the extra call to the user subroutines is not made. User subroutines UHARD, UHYPEL, UHYPER, and UMULLINS, when used in plane stress analyses, are called more often. Subroutines that define initial conditions or orientations User subroutines that are used to define initial conditions or orientations are called before the first iteration of the first step’s initial increment within an analysis. Subroutines that define predefined fields User subroutines that are used to define predefined fields are called prior to the first iteration of the relevant step’s first increment for all iterations of all increments whenever the current field variable is needed. Verification of subroutine calls If there is any doubt as to how often a user subroutine is called, this information can be obtained upon testing the subroutine on a small example, as suggested earlier. The current step and increment numbers are commonly passed into these subroutines, and they can be printed out as debug output (also discussed earlier). The iteration number for which the subroutine is called may not be passed into the user subroutine; however, if printed output is sent from the subroutine to the message (.msg) file (“Output,” Section 4.1.1), the location of the output within this file will give the iteration number, provided that the output to the message file is written at every increment. Utility routines A variety of utility routines are available to assist in the coding of user subroutines. You include the utility routine inside a user subroutine. When called, the utility routine will perform a predefined function or action whose output or results can be integrated into the user subroutine. Some utility routines are only applicable to particular user subroutines. Each utility routine is discussed in detail in “Utility routines,” Section 2.1 of the Abaqus User Subroutines Reference Manual. Variables provided for use in utility routines The following utility routines require the use of Abaqus-provided variables passed into the user subroutines from which they are called: • GETNODETOELEMCONN • GETVRM • GETVRMAVGATNODE • GETVRN • IGETSENSORID • IVGETSENSORID • MATERIAL_LIB_MECH • MATERIAL_LIB_HT These variables will be defined properly when passed into your user subroutine; you cannot modify the variables or create alternative variables for use in the utility routines. For example, the GETVRM utility routine requires the variable JMAC, which is passed from Abaqus/Standard into user subroutine UVARM and other user subroutines for which GETVRM is a supported utility. The variable JMAC represents an Abaqus data structure that requires no further manipulation on your part. If you use the GETVRM utility routine from within user subroutine UVARM, you will pass the JMAC variable from UVARM into GETVRM. 18.1.2 AVAILABLE USER SUBROUTINES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/Aqua References • “User subroutines: overview,” Section 18.1.1 • Abaqus User Subroutines Reference Manual Overview User subroutines allow advanced users to customize a wide variety of Abaqus capabilities. Information on writing user subroutines and detailed descriptions of each subroutine appear online in the Abaqus User Subroutines Reference Manual. A listing and explanations of associated utility routines also appear in that manual. Available user subroutines for Abaqus/Standard The available user subroutines for Abaqus/Standard are as follows: • CREEP: Define time-dependent, viscoplastic behavior (creep and swelling). • DFLOW: Define nonuniform pore fluid velocity in a consolidation analysis. • DFLUX: Define nonuniform distributed flux in a heat transfer or mass diffusion analysis. • DISP: Specify prescribed boundary conditions. • DLOAD: Specify nonuniform distributed loads. • FILM: Define nonuniform film coefficient and associated sink temperatures for heat transfer analysis. • FLOW: Define nonuniform seepage coefficient and associated sink pore pressure for consolidation analysis. • FRIC: Define frictional behavior for contact surfaces. • FRIC_COEF: Define frictional coefficient for contact surfaces. • GAPCON: Define conductance between contact surfaces or nodes in a fully coupled temperature- displacement analysis, a fully coupled thermal-electrical-structural analysis, or a pure heat transfer analysis. • GAPELECTR: Define electrical conductance between surfaces in a coupled thermal-electric analysis or a fully coupled thermal-electrical-structural analysis. • HARDINI: Define initial equivalent plastic strain and initial backstress tensor. • HETVAL: Provide internal heat generation in heat transfer analysis. • MPC: Define multi-point constraints. • ORIENT: Provide an orientation for defining local material directions or local directions for kinematic coupling constraints or local rigid body directions for inertia relief. • RSURFU: Define a rigid surface. • SDVINI: Define initial solution-dependent state variable fields. • SIGINI: Define an initial stress field. • UAMP: Specify amplitudes. • UANISOHYPER_INV: Define anisotropic hyperelastic material behavior using the invariant formulation. • UANISOHYPER_STRAIN: Define anisotropic hyperelastic material behavior based on Green strain. • UCORR: Define cross-correlation properties for random response loading. • UDECURRENT: Define nonuniform volume current density in an eddy current or magnetostatic analysis. • UDEMPOTENTIAL: Define nonuniform magnetic vector potential on a surface in an eddy current or magnetostatic analysis. • UDMGINI: Define the damage initiation criterion. • UDSECURRENT: Define nonuniform surface current density in an eddy current or magnetostatic analysis. • UEL: Define an element. • UELMAT: Define an element with access to Abaqus materials • UEXPAN: Define incremental thermal strains. • UEXTERNALDB: Manage user-defined external databases and calculate model-independent history information. • UFIELD: Specify predefined field variables. • UFLUID: Define fluid density and fluid compliance for hydrostatic fluid elements. • UFLUIDLEAKOFF: Define the fluid leak-off coefficients for pore pressure cohesive elements. • UGENS: Define the mechanical behavior of a shell section. • UHARD: Define the yield surface size and hardening parameters for isotropic plasticity or combined hardening models. • UHYPEL: Define a hypoelastic stress-strain relation. • UHYPER: Define a hyperelastic material. • UINTER: Define surface interaction behavior for contact surfaces. • UMASFL: Specify prescribed mass flow rate conditions for a convection/diffusion heat transfer analysis. • UMAT: Define a material’s mechanical behavior. • UMATHT: Define a material’s thermal behavior. • UMESHMOTION: Specify mesh motion constraints during adaptive meshing. • UMOTION: Specify motions during cavity radiation heat transfer analysis or steady-state transport analysis. • UMULLINS: Define damage variable for the Mullins effect material model. • UPOREP: Define initial fluid pore pressure. • UPRESS: Specify prescribed equivalent pressure stress conditions. • UPSD: Define the frequency dependence for random response loading. • URDFIL: Read the results file. • USDFLD: Redefine field variables at a material point. • UTEMP: Specify prescribed temperatures. • UTRACLOAD: Specify nonuniform traction loads. • UTRS: Define a reduced time shift function for a viscoelastic material. • UVARM: Generate element output. • UWAVE: Define wave kinematics for an Abaqus/Aqua analysis. • VOIDRI: Define initial void ratios. Available user subroutines for Abaqus/Explicit The available user subroutines for Abaqus/Explicit are as follows: • VDISP: Specify prescribed boundary conditions. • VDLOAD: Specify nonuniform distributed loads. • VFABRIC: Define fabric material behavior. • VFRIC: Define contact frictional behavior between surfaces defined with the contact pair algorithm. • VFRIC_COEF: Define contact frictional coefficient between surfaces defined with the general contact algorithm. • VFRICTION: Define contact frictional behavior between surfaces defined with the general contact algorithm. • VUAMP: Specify amplitudes. • VUANISOHYPER_INV: Define anisotropic hyperelastic material behavior using the invariant formulation. • VUANISOHYPER_STRAIN: Define anisotropic hyperelastic material behavior based on Green strain. • VUEL: Define an element. • VUFIELD: Specify predefined field variables. • VUFLUIDEXCH: Define mass/heat energy flow rates for fluid exchange. • VUFLUIDEXCHEFFAREA: Define effective area for fluid exchange. • VUHARD: Define the yield surface size and hardening parameters for isotropic plasticity or combined hardening models. • VUINTER: Define the contact interaction between surfaces defined with the contact pair algorithm. • VUINTERACTION: Define the contact interaction between surfaces defined with the general contact algorithm. • VUMAT: Define material behavior. • VUMULLINS: Define damage variable for the Mullins effect material model. • VUSDFLD: Redefine field variables at a material point. • VUTRS: Define a reduced time shift function for a viscoelastic material. • VUVISCOSITY: Define the shear viscosity for equation of state models. • VWAVE: Define wave kinematics for an Abaqus/Aqua analysis. Available user subroutines for Abaqus/CFD The available user subroutines for Abaqus/CFD are as follows: • SMACfdUserPressureBC: Specify prescribed pressure boundary conditions. • SMACfdUserVelocityBC: Specify prescribed velocity boundary conditions. 18.1.3 AVAILABLE UTILITY ROUTINES Products: Abaqus/Standard Abaqus/Explicit Abaqus/Aqua References • “User subroutines: overview,” Section 18.1.1 • “Utility routines,” Section 2.1 of the Abaqus User Subroutines Reference Manual Overview A variety of utility routines are available to assist in the coding of user subroutines. When called, the utility routine will perform a predefined function or action whose output or results can be integrated into the user subroutine. Available utility routines The following utility routines are available for use in coding user subroutines in Abaqus: • GETENVVAR or VGETENVVAR can be called from any Abaqus/Standard or Abaqus/Explicit user subroutine, respectively, to obtain the value of an environment variable (“Obtaining Abaqus environment variables,” Section 2.1.1 of the Abaqus User Subroutines Reference Manual). • GETJOBNAME or VGETJOBNAME can be called from any Abaqus/Standard or Abaqus/Explicit user subroutine, respectively, to obtain the name of the current analysis job (“Obtaining the Abaqus job name,” Section 2.1.2 of the Abaqus User Subroutines Reference Manual). • GETOUTDIR or VGETOUTDIR can be called from any Abaqus/Standard or Abaqus/Explicit user subroutine, respectively, to obtain the name of the directory where analysis job output is being placed (“Obtaining the Abaqus output directory name,” Section 2.1.3 of the Abaqus User Subroutines Reference Manual). • GETNUMCPUS can be called from any Abaqus/Standard user subroutine to obtain the number of MPI processes; VGETNUMCPUS can be called from any Abaqus/Explicit user subroutine in a domain-parallel run to obtain the number of processes used for the parallel run (“Obtaining parallel processes information,” Section 2.1.4 of the Abaqus User Subroutines Reference Manual). • GETRANK can be called from any Abaqus/Standard user subroutine to obtain the rank of the MPI process from which the function is called; VGETRANK can be called from any Abaqus/Explicit user subroutine in a domain-parallel run to obtain the individual process rank (“Obtaining parallel processes information,” Section 2.1.4 of the Abaqus User Subroutines Reference Manual). • GETPARTINFO or VGETPARTINFO can be called from any Abaqus/Standard or Abaqus/Explicit user subroutine, respectively, to retrieve the part instance name and local node or element number corresponding to an internal node or element number. GETINTERNAL or VGETINTERNAL can be called from any Abaqus/Standard or Abaqus/Explicit user subroutine, respectively, to retrieve the internal node or element number corresponding to a given part instance name and local number (“Obtaining part information,” Section 2.1.5 of the Abaqus User Subroutines Reference Manual.) • GETVRM provides access to material point information for Abaqus/Standard user subroutines UVARM and/or USDFLD (“Obtaining material point information in an Abaqus/Standard analysis,” Section 2.1.6 of the Abaqus User Subroutines Reference Manual). • VGETVRM provides access to selected output variables at material points for Abaqus/Explicit user subroutine VUSDFLD (“Obtaining material point information in an Abaqus/Explicit analysis,” Section 2.1.7 of the Abaqus User Subroutines Reference Manual). • GETVRMAVGATNODE provides access to material point information, extrapolated to and averaged at a node, for Abaqus/Standard user subroutine UMESHMOTION (“Obtaining material point information averaged at a node,” Section 2.1.8 of the Abaqus User Subroutines Reference Manual). information for Abaqus/Standard user subroutine the Abaqus User information,” Section 2.1.9 of • GETVRN provides access to node point UMESHMOTION (“Obtaining node point Subroutines Reference Manual). • GETNODETOELEMCONN can be called from user subroutine UMESHMOTION to retrieve a list of elements connected to a specific node. This element list can then be used with utility routine GETVRMAVGATNODE (“Obtaining node to element connectivity,” Section 2.1.10 of the Abaqus User Subroutines Reference Manual). • SINV determines the first and second stress in Abaqus/Standard (“Obtaining stress invariants, principal stress/strain values and directions, and rotating tensors in an Abaqus/Standard analysis,” Section 2.1.11 of the Abaqus User Subroutines Reference Manual). for a given stress invariants tensor • SPRINC or VSPRINC determines the principal values for a given stress or strain tensor in Abaqus/Standard or Abaqus/Explicit, respectively (“Obtaining stress invariants, principal stress/strain values and directions, and rotating tensors in an Abaqus/Standard analysis,” Section 2.1.11 of the Abaqus User Subroutines Reference Manual, and “Obtaining principal stress/strain values and directions in an Abaqus/Explicit analysis,” Section 2.1.12 of the Abaqus User Subroutines Reference Manual). • SPRIND or VSPRIND determines both the principal values and principal directions for a given stress or strain tensor in Abaqus/Standard or Abaqus/Explicit, respectively (“Obtaining stress invariants, principal stress/strain values and directions, and rotating tensors in an Abaqus/Standard analysis,” Section 2.1.11 of the Abaqus User Subroutines Reference Manual, and “Obtaining principal stress/strain values and directions in an Abaqus/Explicit analysis,” Section 2.1.12 of the Abaqus User Subroutines Reference Manual). • ROTSIG can be called from Abaqus/Standard user subroutine UMAT to perform the rotation of tensors when large-strain calculations are performed (“Obtaining stress invariants, principal stress/strain values and directions, and rotating tensors in an Abaqus/Standard analysis,” Section 2.1.11 of the Abaqus User Subroutines Reference Manual). • GETWAVE determines wave kinematic data associated with the applied wave theory in an Abaqus/Aqua analysis (“Obtaining wave kinematic data in an Abaqus/Aqua analysis,” Section 2.1.13 of the Abaqus User Subroutines Reference Manual). • GETWAVEVEL, GETWINDVEL, and GETCURRVEL are used to obtain the wave, wind, and steady current velocity components, respectively, for a given point in an Abaqus/Aqua analysis (“Obtaining wave kinematic data in an Abaqus/Aqua analysis,” Section 2.1.13 of the Abaqus User Subroutines Reference Manual). • STDB_ABQERR or XPLB_ABQERR can be called from any Abaqus/Standard or Abaqus/Explicit user subroutine, respectively, to print an informational, warning, or error message to the message file in Abaqus/Standard or the status file in Abaqus/Explicit (“Printing messages to the message or status file,” Section 2.1.14 of the Abaqus User Subroutines Reference Manual). • XIT or XPLB_EXIT can be called from any Abaqus/Standard or Abaqus/Explicit user subroutine, respectively, to terminate an analysis (“Terminating an analysis,” Section 2.1.15 of the Abaqus User Subroutines Reference Manual). • IGETSENSORID or IVGETSENSORID can be called from Abaqus/Standard user subroutine UAMP or Abaqus/Explicit user subroutine VUAMP, respectively, to obtain the ID of a user-defined sensor. GETSENSORVALUE or VGETSENSORVALUE can be called from Abaqus/Standard user subroutine UAMP or Abaqus/Explicit user subroutine VUAMP, respectively, to obtain the value of a user-defined sensor (“Obtaining sensor information,” Section 2.1.16 of the Abaqus User Subroutines Reference Manual). • MATERIAL_LIB_MECH can be called from Abaqus/Standard user subroutine UELMAT to access the Abaqus material library (“Accessing Abaqus materials,” Section 2.1.17 of the Abaqus User Subroutines Reference Manual). • MATERIAL_LIB_HT can be called from Abaqus/Standard user subroutine UELMAT to access the Abaqus thermal material library (“Accessing Abaqus thermal materials,” Section 2.1.18 of the Abaqus User Subroutines Reference Manual). • SMACfdUserSubroutineGetScalar can be called from any Abaqus/CFD user subroutine to access selected output variables for elements or surface facets that are part of a boundary condition definition (“Obtaining scalar state information in an Abaqus/CFD analysis,” Section 2.1.19 of the Abaqus User Subroutines Reference Manual). • SMACfdUserSubroutineGetVector can be called from any Abaqus/CFD user subroutine to access selected output variables for elements and surface facets that are part of a boundary condition definition (“Obtaining vector state information in an Abaqus/CFD analysis,” Section 2.1.20 of the Abaqus User Subroutines Reference Manual). • SMACfdUserSubroutineGetMpiComm can be called from within any Abaqus/CFD user subroutine to obtain the MPI communicator used in a parallel analysis job (“Obtaining the MPI communicator in an Abaqus/CFD analysis,” Section 2.1.21 of the Abaqus User Subroutines Reference Manual). 19. Design Sensitivity Analysis Design sensitivity analysis 19.1 Design sensitivity analysis • “Design sensitivity analysis,” Section 19.1.1 19.1.1 DESIGN SENSITIVITY ANALYSIS Product: Abaqus/Design References • “Parametric input,” Section 1.4.1 • “Parametric shape variation,” Section 2.1.2 • *STEP • *DESIGN PARAMETER • *DESIGN RESPONSE Overview Design sensitivity analysis (DSA): • is performed with Abaqus/Design, an add-on option for Abaqus/Standard; • provides the sensitivities of responses with respect to specified design parameters; • is available for static stress and frequency analysis using models that have only stress/displacement elements; and • can include design parameters affecting: material properties (elastic, hyperelastic, and hyperfoam models); section properties; concentrated forces and moments; and nodal coordinates (and beam and shell normals if applicable). Design sensitivity analysis The design sensitivity analysis (DSA) capability provides the derivatives of certain output variables with respect to specified design parameters. These derivatives are commonly referred to as sensitivities, because they provide a first-order measure of how sensitive the output variable is to a change in the design parameter. The output variables for which sensitivities are computed are called design responses or simply responses. Design parameters are chosen from a set of existing analysis parameters. As an example, you can choose to obtain the derivatives of stresses with respect to Young’s modulus; stress is the response, and Young’s modulus is the design parameter. The sensitivities are computed based on the direct differentiation method used in conjunction with the semi-analytical computational technique. In the semi-analytical technique some derivatives are computed using numerical (finite) differencing, thus requiring perturbations of the design parameters. For these derivatives by default Abaqus/Design will use a central differencing scheme and automatically determine appropriate perturbation sizes based on a heuristic algorithm. You can override these defaults by specifying the numerical differencing method and the perturbation sizes directly. A full discussion of DSA theory is given in “Design sensitivity analysis,” Section 2.18.1 of the Abaqus Theory Manual. Activating DSA You activate DSA on a step-by-step basis. Input File Usage: Use the following option to activate DSA in a particular step: *STEP, DSA=YES Activating DSA in multiple steps Once DSA is activated in a general step, it remains active in all subsequent general steps until it is deactivated in a subsequent general step. Once DSA is activated in a perturbation step, it remains active in all subsequent consecutive perturbation steps until it is deactivated in a subsequent consecutive perturbation step. However, if DSA is activated in a step whose procedure is not supported for DSA, DSA will be deactivated until it is activated again. Input File Usage: Use the following option to deactivate DSA in a particular step: *STEP, DSA=NO Specifying design parameters You can define multiple parameters to be used in place of Abaqus input quantities for an analysis. You must indicate which of these parameters are to be considered as design parameters. Input File Usage: Use the following option to define analysis parameters: *PARAMETER par1=x par2=y Use the following option to specify the design parameters: *DESIGN PARAMETER par1, par2, Restrictions on design parameters The following are restrictions on design parameters: • Design parameters can be associated only with floating point data. The following analysis components can include design-dependent data: – Beam sections integrated during analysis (“Using a beam section integrated during the analysis to define the section behavior,” Section 29.3.6) – Concentrated loads (“Concentrated loads,” Section 33.4.2) – Elastic materials (“Linear elastic behavior,” Section 22.2.1) – Friction (“Frictional behavior,” Section 36.1.5) – Gasket sections (“Gasket elements: overview,” Section 32.6.1) – Hyperelastic materials (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1) – Hyperfoam materials (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2) – Membrane sections (“Membrane elements,” Section 29.1.1) – Local orientations (“Orientations,” Section 2.2.5) – Shell sections integrated during analysis (“Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5) – Solid sections (“Solid (continuum) elements,” Section 28.1.1) – Transverse shear stiffnesses (“Choosing a beam element,” Section 29.3.3, or “Shell section behavior,” Section 29.6.4) • Shape design parameters (i.e., design parameters that affect nodal coordinates and beam and/or shell normals) can be used only in conjunction with parametric shape variations . • Design parameters must be mutually independent. • Design parameters cannot be tabularly dependent . Specifying responses Response requests are specified using a syntax analogous to that for specifying output requests to the output database. Except for eigenvalues and eigenfrequencies, there are no default responses—if no responses are requested, no response sensitivities will be output. If DSA is active in a frequency step, eigenvalue and eigenfrequency sensitivities will be output automatically. Specifying a response will cause output of both the response and the response sensitivities. Input File Usage: Use the following options to request design responses: *DESIGN RESPONSE, FREQUENCY=interval, MODE LIST *CONTACT RESPONSE, MASTER=master name, NSET=nset name, SLAVE=slave name *ELEMENT RESPONSE, ELSET=elset name *NODE RESPONSE, NSET=nset name Requesting responses in multiple steps Unless respecified, response requests defined in a step propagate to subsequent steps according to the following rules: 1. Requests in general steps propagate to subsequent general steps. 2. Requests in linear perturbation steps propagate to subsequent consecutive linear perturbation steps. 3. When a non-DSA step appears between DSA steps, the responses must be respecified in the DSA step following the non-DSA step. Restrictions on responses The available responses are a subset of the existing output variables. The valid responses based on procedure type are described below. • For static steps the valid responses are: – Node responses: U and RF – Element responses: S, SF, SINV, SP, E, SE, EP, EE, EEP, LE, LEP, NE, NEP, ENER, ELEN, EVOL, and MASS – Contact responses: CSTRESS and CDISP • For frequency steps the valid responses are: – Node responses: None – Element responses: MASS – Contact responses: None – Eigenvalue (EIGVAL) and eigenfrequency (EIGFREQ) sensitivities are output automatically. Specifying design gradients of design-dependent input data The DSA calculations require the gradients of the design-dependent input data with respect to the design parameters. For example, if Poisson’s ratio, , is made dependent on a design parameter, say h, the gradient is required. Design gradients with respect to shape design parameters are specified differently than those with respect to other design parameters. Specifying design gradients with respect to shape design parameters Gradients with respect to shape design parameters must be specified using a parametric shape variation definition . For the purposes of DSA if the parameter to which the shape variation data refer is a design parameter, the shape variation data are interpreted as the gradients of the nodal coordinates with respect to the design parameter. If a nonzero value is given for the shape parameter, Abaqus/Design will also perturb the base coordinates. Input File Usage: Use the following option to specify the design gradients for shape design parameters: *PARAMETER SHAPE VARIATION, PARAMETER=design parameter Specifying gradients for non-shape design parameters For non-shape design parameters, by default Abaqus/Design will use numerical differentiation to calculate design gradients based on the information you provide. However, you can override this default behavior by specifying the gradients directly using Python expressions . You specify a design parameter as the independent parameter and a list of the parameters that depend on that design parameter. Only one independent (design) parameter can be given for each design gradient definition. Input File Usage: Use the following option to specify the design gradients for non-shape design parameters: *DESIGN GRADIENT, INDEPENDENT=design parameter, DEPENDENT=(list of dependent parameters) History dependence and formulation type in a multi-increment analysis Both total and incremental formulations are implemented for DSA. The choice of formulation depends on whether or not an analysis is history dependent. Below is a brief description of these formulation types. A more detailed discussion can be found in “Design sensitivity analysis,” Section 2.18.1 of the Abaqus Theory Manual. By default, the incremental DSA formulation is used. You can specify the DSA formulation only for the entire model; this specification is ignored if given as part of a step definition. Incremental DSA formulation In the incremental formulation the problem is assumed to be history dependent. Abaqus/Design solves for the incremental displacement sensitivities, and the total displacement sensitivity is updated at the end of the increment. Due to the history dependence, the incremental displacement sensitivities for the current increment depend on the sensitivities of the state variables at the beginning of the increment, in the same sense that incremental displacements depend on the state variables at the beginning of the increment for equilibrium analyses. Thus, Abaqus/Design must also compute and update state variable sensitivities in each increment. Consequently, DSA must be activated for all steps up to the last step in which DSA is active, and the DSA calculations will be done at all increments in these steps, regardless of whether or not a design response is requested for a given step. If a response is requested for a step, the specified response frequency is ignored for the purposes of the DSA calculations (the frequency at which the output is written will still be governed by the specified response frequency). The disadvantage of the incremental DSA formulation is its cost, due to the necessity of computing both state variable and incremental displacement sensitivities at each increment prior to the last DSA increment. This increased cost is unavoidable if the problem is history dependent but is unnecessary if the problem is history independent. Thus, the total DSA formulation should be chosen for problems that are not history dependent. Input File Usage: *DSA CONTROLS, FORMULATION=INCREMENTAL Total DSA formulation In the total displacement formulation the total displacement sensitivities are calculated directly based on the assumption that the problem is not history dependent. In other words, the displacement sensitivities do not depend on sensitivity results calculated in previous increments. Thus, the advantage of the total formulation is that the sensitivity calculations need only be done at increments of interest. You can control when DSA calculations are done by activating DSA for only the desired steps and specifying the desired frequency for each design response request. You may choose to use the total DSA formulation in problems that are known to be history dependent. However, in this case the DSA solution is approximate, with the degree of approximation increasing as the problem becomes more strongly history dependent. To assess the validity of using the total DSA formulation, it is recommended that you run both an incremental and total sensitivity analysis for a typical problem and compare the results. Input File Usage: *DSA CONTROLS, FORMULATION=TOTAL DSA in linear perturbation steps The sensitivity of the perturbation response can be calculated in a linear perturbation step . The perturbation response will include the effects of stress and load stiffening in the base state if geometric nonlinearity is considered. Since we need to calculate the sensitivity of an incremental (perturbation) response, the sensitivity of the stress and load stiffening effects must be known at the end of the base step. Thus, if geometric nonlinearity is considered in the base step, DSA must also be active in the base step, irrespective of the type of formulation (total or incremental). Determination of design parameter perturbation sizes The basis of the semi-analytic technique is the use of numerical differencing to obtain derivatives of certain element vectors and matrices . Abaqus/Design will automatically determine appropriate perturbation sizes to be used in the semi-analytic technique unless you specify them directly. Abaqus/Design determines the perturbation sizes using a heuristic perturbation sizing algorithm based on the behavior of a scalar s associated with an element. By default, the perturbation sizing algorithm is applied only for the first increment (static procedure) or first mode (frequency procedure) in each step for which DSA is active. The perturbation sizes are then reused for the remaining increments or modes in the step for which DSA calculations are done. The goal of the algorithm is to find perturbation sizes that are optimal for numerical differencing. Differencing formulas are based on Taylor series expansions, and the order of approximation of the derivative to be computed is reflected in the terms that are neglected in the series. The accuracy of the approximated derivatives often depends strongly on the perturbation size used in the differencing formula. Choosing a perturbation size that is too large will cause a truncation error, which occurs when the order of approximation is no longer valid (i.e., as a result of truncating higher-order terms in the Taylor series). A perturbation size that is too small will lead to inaccuracies in the differencing operations due to round-off, typically referred to as a cancellation error. The algorithm attempts to find perturbation sizes giving the best compromise between cancellation and truncation errors by observing the behavior of s. For each design parameter s is computed for perturbation sizes spanning several orders of magnitude. The error in s between consecutive perturbation sizes is calculated as , is chosen as the best perturbation size. . The perturbation size yielding an acceptable error, This scalar s is selected as follows: • Static procedure. For static steps s is chosen as the norm of the element pseudoload (the partial derivative of the element residual with respect to the design parameters). • Frequency procedure. For frequency steps s is computed from the element contribution to a matrix , where involving the derivatives of the mass and stiffness matrices (namely is the stiffness, is the mass, h is the design parameter, and scalar s is taken as the projection of this matrix onto an eigenvector algorithm is applied to a mode with a distinct eigenvalue, is an eigenvalue). The . If the perturbation sizing is taken as the eigenvector associated with this mode. However, if a mode happens to be associated with a repeated eigenvalue, is taken as the sum of all the eigenvectors associated with the repeated eigenvalue. Thus, the entire set of modes associated with a repeated eigenvalue will be treated simultaneously by the perturbation sizing algorithm (the eigenvalue sensitivities of a repeated eigenvalue are obtained simultaneously from the same reduced eigenvalue system). See “Design sensitivity analysis,” Section 2.18.1 of the Abaqus Theory Manual, for further details on the selection of s. Controlling the numerical differencing behavior You can control various aspects of the numerical differencing operations. These aspects are described in detail in the following sections. You can specify DSA controls for the entire model and/or for individual steps. Specifying these controls for the entire model has the effect of creating new default values for the various settings. When you specify these controls for individual steps, the following propagation rules are enforced: • Once DSA controls are specified in a non-perturbation step, they remain in effect for all subsequent non-perturbation steps, unless they are respecified or reset. • Once DSA controls are specified in a perturbation step, they remain in effect for all subsequent consecutive perturbation steps, unless they are respecified or reset. Resetting DSA controls You can reset DSA controls only for individual steps. If DSA controls are specified for the entire model, resetting them in a particular step will reset the numerical differencing behavior to the behavior specified for the entire model; otherwise, the behavior will be reset to the original default values. Any additional changes specified will be applied after the behavior is reset. Input File Usage: Use the following option to reset the DSA controls for a particular step: *DSA CONTROLS, RESET Changing the defaults for the heuristic perturbation sizing algorithm The following two sections describe how certain parameters associated with the perturbation sizing algorithm can be changed from their default values for purposes of computational efficiency and accuracy. Changing the default tolerance is set to 1.0 × 10−4. Warning messages are written to the message file for By default, the tolerance elements for which this tolerance is not achieved. These elements are collected in element sets and can be viewed in the Visualization module of Abaqus/CAE. It is important to understand that this tolerance controls the effort expended in obtaining an optimum perturbation size; it is not a direct measure of the accuracy of the numerical differentiation. Input File Usage: Use the following option to override the default tolerance: *DSA CONTROLS, TOLERANCE=tolerance Changing the frequency at which the perturbation sizing algorithm is used Determining perturbation sizes using the heuristic algorithm is computationally intensive. You can specify the frequency at which the perturbation sizes are recalculated. For example, specifying a sizing frequency of n will cause Abaqus/Design to determine new perturbation sizes at every n increments or eigenmodes. The perturbation size will always be recalculated at the first increment or eigenmode in each step for which DSA is active, which is equivalent to specifiying a sizing frequency of 0. Since the perturbation sizing algorithm is computationally intensive, care should be exercised to ensure that the sizing frequency is as large as possible (or zero). As discussed above, the perturbation sizing algorithm is applied simultaneously to all modes associated with a repeated eigenvalue. Thus, the actual number of modes associated with a repeated eigenvalue that are “hit” based on the sizing frequency is irrelevant, so long as it is at least one. Input File Usage: Use the following option to specify the frequency at which the perturbation sizes are recalculated: *DSA CONTROLS, SIZING FREQUENCY=frequency Overriding the default heuristic perturbation sizing algorithm If an appropriate perturbation size is already known for a particular design parameter (from previous analyses of similar problems, for example), economy can be gained by applying this perturbation size directly rather than having Abaqus/Design automatically find the perturbation size. You can specify either forward differencing or central differencing directly together with an absolute perturbation size for each design parameter. If you override the default algorithm, it is up to you to choose perturbation sizes that will lead to accurate sensitivities. Input File Usage: Use the following option to override the default heuristic perturbation sizing algorithm for a given design parameter: *DSA CONTROLS design parameter, FD (forward differencing) or CD (central differencing), absolute perturbation size For example, to specify an absolute perturbation size of 0.001 and forward differencing for design parameter despar use the following input: *DSA CONTROLS despar, FD, 0.001 This data line is specified for each design parameter for which the default scheme is to be overridden. Accuracy of the DSA solution As can be seen in “Design sensitivity analysis,” Section 2.18.1 of the Abaqus Theory Manual, the accuracy of the DSA solution is dictated by both the accuracy of the numerically computed derivatives and, for nonlinear static analysis, the accuracy of the tangent stiffness matrix. The accuracy of the numerically computed derivatives is governed by the semi-analytic DSA algorithm; you can control it by specifying DSA controls. In nonlinear static analysis DSA uses the tangent stiffness matrix formed It is possible that the accuracy of the tangent stiffness matrix during the last equilibrium iteration. needed to achieve an accurate equilibrium solution may be insufficient to achieve an accurate DSA solution. In such cases you can tighten the convergence tolerances during the equilibrium analysis so that a more accurate tangent stiffness matrix is obtained . Furthermore, an accurate equilibrium solution often can be obtained when unsymmetric terms in the tangent stiffness are ignored (i.e., the unsymmetric matrix storage and solution scheme is not used; see “Defining an analysis,” Section 6.1.2). However, even if mildly unsymmetric stiffness terms are neglected, the DSA solution may be inaccurate. Therefore, it is recommended that the unsymmetric solution scheme be used for DSA when the tangent stiffness matrix is known to be unsymmetric. In some cases a response at a certain instant in time may be discontinuous with respect to a design parameter. For example, at this point of discontinuity a variation in the design parameter may cause a node to come into contact, frictional behavior to change from sticking to sliding, or a material point to transition from elastic to inelastic behavior. Since the DSA calculations make use of numerical differencing, it is possible that the perturbation of the design parameter used in the differencing scheme may result in values of the response to be differenced that lie on opposite sides of the discontinuity. If this occurs, the accuracy of the computed derivative cannot be guaranteed. Mathematically speaking, the derivative (sensitivity) of the response with respect to the design parameter does not exist at the point of discontinuity. Practically speaking, it is unlikely that the response at any given instant will lie precisely on the discontinuity. In cases where the response is near a discontinuity, if you choose to use the default perturbation sizing algorithm, the algorithm will attempt to choose design parameter perturbation sizes such that the values of the perturbed responses remain on the same side of the discontinuity. In addition, for contact elements DSA calculations are not performed in increments in which the associated contact node is open. Typically, the global results in any increment are not affected by a few discontinuous points in the model. Design dependence and supported features Responses depend on design parameters explicitly and implicitly. Implicit design dependence is the dependence on the design parameter through the solution variables; therefore, this type of dependence can be quantified only after the DSA solution is obtained (recall that the DSA solution is the total displacement sensitivity for the total formulation and the incremental displacement sensitivity for the incremental formulation). All other design dependencies are explicit, meaning that they can be resolved without knowing the DSA solution. The types of dependencies can be identified by looking at the form of the sensitivity of a response, say r, with respect to a design parameter, say h. This sensitivity is expressed as for the total formulation and for the incremental formulation, where represents state variables at the beginning of the increment . The state variables include the displacements at the beginning of the increment. In both cases the last term on the right-hand side represents the implicit design dependence through the solution variables. is a displacement degree of freedom and It is observed from the incremental equation above that the explicit design dependence consists of two terms. The first of these, , represents a direct design dependence, because this term arises from the direct dependence of the response on the design parameter. The second explicit term, , represents the dependence on the design parameter through the state variables at the beginning of the increment. For the total formulation, it is seen that the explicit term involves only direct design dependence. Any feature for which direct design dependence calculations are implemented in Abaqus will be referred to as supported for DSA. Supported and unsupported features can be mixed in an analysis, unless the supported features cause unsupported features to become directly design dependent (an example of this would be making the Young’s modulus for a frame element design dependent, since frames are not supported for DSA). To make a clearer distinction between the types of design dependencies, consider the more concrete example of a linear elastic truss element, fixed at one end and pulled with a concentrated load at the other end. Let represent the displacement at the free end, E represent Young’s modulus, and L represent the length of the truss. Consider the axial stress as the response. Although it is clear in this simple example that the stress can be computed easily as the load divided by the cross-sectional area, the finite element analysis computes the stress equivalently as . Choosing Young’s modulus, E, as the design parameter, the stress sensitivity is given by for the total formulation and for the incremental formulation. This example is a valid analysis since elastic materials and truss elements are supported for DSA. Suppose now that a frame element is added, extending the length of the structure. If the frame element shares the same Young’s modulus, the analysis becomes invalid since the dependency on the design parameter E causes the frame element, which is unsupported, to become directly design dependent (i.e., the term would need to be computed). On the other hand, if the frame uses a different modulus, say that is not a design parameter, the analysis again becomes valid, since the frame no longer depends directly on the design parameter E. Contact interactions Surface-based contact between deformable and rigid surfaces with small- or finite-sliding relative surface motion including friction is supported in a design sensitivity analysis. In all the friction models only the friction coefficients (no test data input) can be made design dependent. Shape design parameters are not valid for rigid surfaces. Contact between deformable surfaces is not supported. Restarting a design sensitivity analysis A design sensitivity analysis can be restarted . However, DSA must have been active in the base analysis, and no design parameter or gradient data can be modified in the restart run. The restarted analysis will follow all the DSA propagation rules that are applicable to a regular analysis. For total formulation DSA, you may choose to activate or deactivate DSA in any new step that is added to the restart run. However, for the incremental formulation DSA must have been active in the step at which restart is attempted for you to continue doing DSA in the restarted analysis. Procedures DSA is available in the following analysis procedures: • Frequency analysis • Static stress analysis (including nonlinear geometric effects and contact) The following analysis procedures and techniques are not supported: • Static stress analysis with the Riks method • Substructuring • Mesh modification or replacement • Importing and transferring results • Symmetric model generation and results transfer • Contour integrals • Cyclic symmetry in frequency procedures Submodeling limitations Design sensitivity analysis can be performed in both the global model and submodel, with the limitation that the DSA solution will not be interpolated from the global model to the submodel. This means that DSA is valid in the submodel only if the global solution that is interpolated onto the boundary of the submodel can be considered independent of the design parameters chosen for the submodel sensitivity analysis. Material options The following material models are supported: • Isotropic, orthotropic, and anisotropic elasticity • Hyperelasticity • Hyperfoam In these models only directly input material coefficients (not test data) can be made design dependent. If test data are specified, that material definition can be replaced by specifying the material coefficients calculated by Abaqus/Design directly. Supported and unsupported material models can be mixed in the same analysis. Elements Solid, truss, shell, beam, gasket, and membrane stress/displacement elements are supported. Shell elements with five degrees of freedom per node cannot be used in a total DSA formulation. Supported and unsupported elements can be mixed in the same analysis. Output The responses and response sensitivities are output only to the output database (sensitivity output to the data file and results file is not supported). The names of the sensitivities are related to the names of the responses as follows: d response name design parameter name For example, if the name of the response is S and the name of the design parameter is Young, the name of the sensitivity is d_S_Young. Input file template *HEADING … *PARAMETER Python expressions defining parameters. *DESIGN PARAMETER List of independent parameters to be considered as design parameters. … *NODE, NSET=nset Data lines to define the nodes. *PARAMETER SHAPE VARIATION, PARAMETER=parameter Data lines to define the gradients of coordinates with respect to the parameter. … *ELEMENT, TYPE=solid element type, ELSET=elset_elastic Data lines to define the elements. *ELEMENT, TYPE=solid element type, ELSET=elset_hyper Data lines to define the elements. *SOLID SECTION, ELSET=elset_elastic, MATERIAL=elastic *SOLID SECTION, ELSET=elset_hyper, MATERIAL=hyper *MATERIAL, NAME=elastic *ELASTIC Data lines to define the elastic properties. *MATERIAL, NAME=hyper *HYPERELASTIC Data lines to define the hyperelastic properties. … *STEP,DSA *STATIC … *DESIGN RESPONSE, FREQUENCY=interval *ELEMENT RESPONSE, ELSET=elset Data lines to specify the element response identifier keys. *NODE RESPONSE, NSET=nset Data lines to specify the nodal response identifier keys. *END STEP Parametric Studies Scripting parametric studies Parametric studies: commands PARAMETRIC STUDIES 20.1 20.1 Scripting parametric studies • “Scripting parametric studies,” Section 20.1.1 20.1.1 SCRIPTING PARAMETRIC STUDIES Products: Abaqus/Standard Abaqus/Explicit References • “Parametric input,” Section 1.4.1 • “Parametric shape variation,” Section 2.1.2 • “Parametric studies,” Section 3.2.8 Overview Parametric studies allow you to generate, execute, and gather the results of multiple analyses that differ only in the values of some of the parameters used in place of input quantities. Parametric studies can be performed by: • Creating a “template” parametrized input file from which the different parametric variations are generated. • Preparing a script (a file with the .psf extension) that contains Python (Lutz, 1996) instructions to generate, execute, and gather output for the parametric variations of the parametrized input file. The Python commands for scripting parametric studies are discussed in this section. Introduction Parametric studies require that multiple analyses be performed to provide information about the behavior of a structure or component at different design points in a design space. The inputs for these analyses differ only in the values assigned to the parameters of a parametrized keyword input file (identified with the .inp extension). Parametric studies in Abaqus require a user-developed Python script in a file (identified with the .psf extension) that contains Python commands to define the parametric study. For example, consider a case where you wish to perform a parametric study in which the thickness of a shell is varied. You need to create a parametrized input file (in this example, a file named shell.inp) containing the parameter definition *PARAMETER thick1 = 5. and the parameter usage: *SHELL SECTION,ELSET=name, MATERIAL=name You create the parametric study by developing a .psf file that contains a script of Python instructions specifying the different designs that are to be analyzed, as follows: thick = ParStudy(par='thick1', name='shell') thick.define(CONTINUOUS, par='thick1', domain=(10., 20.)) thick.sample(NUMBER, par='thick1', number=5) thick.combine(MESH) These scripting commands create five designs with corresponding section thicknesses of 10., 12.5, 15., 17.5, and 20.0. Each of these thicknesses will, in turn, replace the value of 5. specified in the parameter definition in shell.inp. You may then provide additional Python scripting commands in the .psf file instructing Abaqus to do the following: • Generate a number of shell_id.inp files and corresponding Abaqus jobs using the shell.inp file as a template. (The identifier id that is appended to the input file name is unique to each design in the parametric study.) An example of the Python command for this is thick.generate(template='shell') In this example the shell_id.inp files will differ only in the value to be used for the shell thickness. • Execute all the Abaqus jobs representing the different variations of the parametric study. The Python command for this is thick.execute(ALL) You generally want to review certain key results from the large amount of data that is generated by a parametric study. Abaqus provides the following capabilities for this purpose: • A command specifying the source from which the results of a parametric study will be gathered. For example: thick.output(file=ODB, step=1, inc=LAST) The command above sets the output location to the last frame of the first step in the output database (.odb) file. The default behavior is to gather results from the last frame of a given step in the results (.fil) file. • Commands to gather the required results from the multiple analyses generated by the parametric study and report them in a file or table. For example, the sequence of Python scripting commands used to gather and report the value of a displacement at a key node for each of the designs is: thick.gather(results='n33_u', variable='U', node=33, step=1) thick.report(PRINT, par='thick1', results=('n33_u.2')) The commands above gather the results record ’n33_u’ (the displacement vector of node 33 at the end of Step 1 of the analysis) for each of the designs and then print a table of the U2 component (the second component of the results record) of displacement for all designs. • The ability to visualize X–Y plot data gathered across multiple analyses using the Visualization module of Abaqus/CAE. A typical example is to obtain an X–Y plot of the value of the displacement at a key node versus the value of the shell thickness. This is done by gathering the appropriate parametric study results in an ASCII file that can be read into the Visualization module to display the plot. Organization of parametric studies A parametric study in Abaqus is associated with a particular set of parameters that define the design space. Only the values of the parameters can change in a parametric study. A new parametric study must be created if you wish to consider a different set of parameters. Having selected the parameters to be considered in a parametric study, you must specify how each parameter is defined. Parameters are distinguished as either continuous or discrete in nature and may have a domain and reference value. The design points in the design space that are to be analyzed are created by specifying sample values for each parameter (sampling) and by combining the parameter samples to create sets of design points. A few simple commands are provided for parameter value sampling and for combining the sampled parameter values; these commands are described in detail later. An initial definition and sampling of the parameters in the parametric study must be given before any combinations of parameter samples can be specified. After the first combination the initial definition and/or sampling of any individual parameter can be changed before the next combination is specified, thus providing a great deal of flexibility within one parametric study. The domain of possible values and the reference value for a parameter given in the parameter definition can be temporarily redefined in any sampling of that parameter by specifying them differently during the sampling. You need not specify the parameter domain and reference value in the parameter definition so long as these are specified during sampling. Design constraints can be imposed on all of the designs. A design that violates any of the constraints will be eliminated. Finally, after all parametric study variations have been analyzed, you can gather and report results across all or some of the designs of the parametric study. In summary, parametric studies in Abaqus are organized as follows: • Create parametric study. • Define parameters: define parameter type (continuous or discrete valued) and possibly the parameter domain and reference value. • Sample parameters: parameter domain and reference value. specify sampling option and data and possibly temporarily redefine the • Combine parameter samples to create sets of designs. • Constrain designs (optional). • Generate designs and analysis job data. • Execute the analysis jobs for selected designs of the study. • Gather key results for selected designs of the study. • Report gathered results. Note: The sequence of steps—define, sample, and combine—can be repeated as often as is necessary to create all the required design sets. Multiple parametric studies can be performed on a model contained in one input file. In general, more parameters will be defined and used in place of input quantities in the input file than those involved in any particular parametric study. In these cases parameters not involved in a particular parametric study will retain their values defined in the input file for the purposes of that parametric study. Therefore, we can think of the parameter values defined in the input file as representing a nominal design; parametric studies create modified designs by overwriting the values of some (or all) parameters. Defining the design space The design space is defined by the selection of the parameters to be varied in the study as well as the specification of the parameter types and possible values they can have. Parametric study creation Use the aStudy=ParStudy scripting command to create a parametric study and select the independent parameters to be considered for variation. aStudy is the Python variable name assigned by you to the parametric study object created by the command. The methods of the parametric study object are used to carry out all the actions of the parametric study. Input File Usage: aStudy=ParStudy (par=, name=, verbose=, directory=) Parameter definition Use the aStudy.define command to specify the parameter type (choose the CONTINUOUS or the DISCRETE token; a token is a symbolic constant used to select an option within a specific command) and, optionally, to specify the domain of possible parameter values and a reference value for the parameter. If the domain and/or reference value are not specified in this command, they can be specified in the parameter sampling. Redefinitions of a parameter are treated as complete redefinitions; that is, no information is retained from the previous definition of that parameter. Input File Usage: aStudy.define (token, par=, domain=, reference=) CONTINUOUS parameter type In this case the parameter can take any value in a continuous domain specified by minimum and maximum values; for example, domain=(3., 10.). DISCRETE parameter type In this case the parameter can take only the values specified in a list that defines the discrete domain; for example, domain=(1, 4, 9, 16). Sampling and combining parameter values to create sets of design points Each parameter in the parametric study must be sampled before the combination operation is used to create the first set of design points. Any parameter in the parametric study can be redefined or resampled before a subsequent combination operation is performed. Parameter sampling Use the aStudy.sample command and choose one of the available tokens (INTERVAL, NUMBER, REFERENCE, or VALUES) to select how the sampling is done. The sampling data that must be given depend on how the sampling is done, as described next. Sampling by INTERVAL This sampling command assumes that you specify a domain of possible parameter values and wish to sample parameter values at fixed intervals in the domain. Sampling of the extreme values of the parameter is always done. The number of parameter values sampled depends on the interval and the domain. Because the extreme values are sampled, the last sampling interval will generally be smaller than the interval you specify. The domain specification in this sampling command is optional: • If a domain is specified in this command, it temporarily redefines a domain specified in the define command. • If a domain is not specified in this command, the domain specification from the define command is used for sampling. • An error is flagged when a domain is not specified in this command or in the define command. The sampling interval is interpreted differently for continuous and discrete parameters: • For continuously valued parameters the interval at which the samples are spaced is based on For example, specifying interval=10. for a continuous parameter with a numerical value. domain=(10., 35.) will sample values of 10., 20., 30., and 35. for this parameter. • For discrete valued parameters the interval at which the samples are spaced is based on the index of the list of values. The index means the position of the entry in the list, starting at position 0 and continuing with positions 1, 2, 3, etc. In this case interval must be an integer number. For example, specifying interval=−2 for a discrete parameter with domain=(1., 2., 3., 5., 7., 10.) will create sample values of 10., 5., 2., and 1. for this parameter. The interval can have a positive or negative value (zero is not permitted). A positive interval indicates that sampling starts at the minimum value for a continuous parameter or at the first value in the list of values for a discrete parameter (forward sampling). A negative interval indicates that sampling starts at the maximum value for a continuous parameter or at the last value in the list of values for a discrete parameter (reverse sampling). Reverse sampling is useful when the TUPLE combination operation is used . Two special cases of the INTERVAL option are noteworthy: • A positive interval value larger than the range of continuous parameter values or the number of discrete parameter values will sample the minimum and maximum values of the continuous parameter or the first and last values in the discrete parameter list. • A negative interval value larger (in absolute terms) than the range of continuous parameter values or the number of discrete parameter values will sample the maximum and minimum values of the continuous parameter or the last and first values in the discrete parameter list. Input File Usage: aStudy.sample (INTERVAL, par=, interval=, domain=) Sampling by NUMBER This sampling option assumes that you specify a domain of possible parameter values and wish to sample a fixed number of parameter values in the domain. Except for a special case documented below, sampling of the extreme values of the parameter is always done. The parameter is sampled at equally spaced intervals (with some exceptions for discrete parameters, as discussed below) and the size of the interval depends on the number of values sampled as well as the domain. The domain specification in this sampling command is optional: • If a domain is specified in this command, it temporarily redefines the domain specified in the define command. • If a domain is not specified in this command, the domain specification from the define command is used for sampling. • An error is flagged when a domain is not specified in this command or in the define command. The sampling interval is calculated and interpreted differently for continuous and discrete parameters: • For continuous valued parameters the interval at which the samples are spaced is based on For example, specifying number=4 for a continuous parameter with a numerical value. domain=(10., 25.) will sample values of 10., 15., 20., and 25. for this parameter. • For discrete valued parameters the interval at which the samples are spaced is based on the index of the list of values (indexing starts at zero). For example, specifying number=3 for a discrete parameter with domain=(1., 2., 3., 5., 7., 10., 12.) will create sample values of 1., 5., and 12. for this parameter. The number of discrete parameter samples specified by you may not allow equally spaced sampling; for example, specifying number=5 or number=6 for the discrete parameter above does not allow equally spaced sampling. This is resolved by sampling the parameter values that are closest to being equally spaced by rounding the sampling index to the closest index in the list of values. For example, specifying number=5 for the discrete parameter above will create sample values of 1., 3., 5., 10., and 12. The values 1. and 12. are sampled because they are the extreme values. The explanation for the second sampled value being the third value in the list (the value 3.) is as follows: the sampling interval is (highest index − lowest index)/(number − 1) = (6 − 0)/(5 − 1) = 1.5; the second sampled value should then be the one with index = 0 + 1.5 = 1.5 in the list; since the index has to be an integer number, we round off to index = 2 and, thus, sample the third value in the list. The other sampled values can be explained similarly. The same rule is used for character string type discrete parameters. For example, specifying number=3 for a discrete parameter with domain=(’C3D8’, ’C3D8R’, ’C3D8I’, ’C3D8H’) will create sample values of ’C3D8’, ’C3D8I’, and ’C3D8H’. Three special cases of the NUMBER option are noteworthy: • Specifying number=1 will sample the central value of a parameter, which is useful when the center of the design space is of interest. It is the only case in which the use of the NUMBER option does not sample the extreme values of the parameter. • Specifying number=2 will sample the extreme values of a parameter, which is useful when the boundaries of the design space are of interest. • Specifying number=3 will sample the central and the extreme values of a parameter, which is useful when the center and the boundaries of the design space are of interest. Specification of number=0 is not permitted. A negative value for number is permitted; this indicates that the sampling is to be in reverse order. For continuous parameters reverse order means that the first sampled value is the largest and the last sampled value is the smallest. For discrete parameters reverse order means that the first sampled value is the last in the list of values and the last sampled value is the first in the list of values. Sampling in reverse order is useful when the TUPLE combination operation is used . Input File Usage: aStudy.sample (NUMBER, par=, number=, domain=) Sampling by REFERENCE This sampling option allows you to specify a reference value for the parameter and to sample parameter values with respect to this reference value. It is useful for studying alternate designs with respect to an existing (reference) design. This sampling command creates sample values symmetrically about the reference value at multiples of a given interval; in addition, the reference value is also sampled. The number of parameter values in the sample depends on the number of symmetrical pairs of values you specify. The reference value specification in this sampling option is optional: • If a reference value is specified in this command, it temporarily redefines the reference specified in the define command. • If a reference value is not specified in this command, the reference specification from the define command is used for sampling. • An error is flagged when a reference value is not specified in this command or in the define command. The reference value is interpreted differently for continuous and discrete parameters: • For continuous valued parameters reference is the parameter’s numerical value about which a symmetrical sample will be created. • For discrete valued parameters reference is the index of the list of values about which a symmetrical sample will be created. A reference value that falls outside the domain definition for the parameter is flagged as an error. The sampling interval is interpreted differently for continuous and discrete parameters: • For continuous valued parameters the interval at which the samples are taken is based on a numerical value. For example, specifying reference=50., interval=10., and numSymPairs=2 for a continuous parameter will create sample values of 30., 40., 50., 60., and 70. for this parameter. • For discrete valued parameters the interval at which the samples are spaced is based on the index of the list of values (indexing starts at zero); in this case interval must be an integer value. For example, specifying reference=5, interval=−2 and numSymPairs=2 for a discrete parameter with domain=[1, 2, 3, 5, 7, 10, 12, 15, 20, 25] will create sample values of 25, 15, 10, 5, and 2 for this parameter. The specified interval can have a positive or negative value, but a value of zero is not permitted. A positive interval indicates that the list of sampled values starts with the smallest sampled value for a continuous parameter or with the sampled value closest to the beginning of the list of values for a discrete parameter (forward sampling). A negative interval indicates that the list of sampled values starts with the largest sampled value for a continuous parameter or with the sampled value closest to the end of the list of values for a discrete parameter (reverse sampling). Reverse sampling is useful when the TUPLE combination operation is used . The number of symmetrical pairs you specify must be zero or a positive integer; setting the number of symmetrical pairs equal to zero indicates that only the reference value is sampled. The domain specification in this command is optional: • If a domain is specified in this command, it temporarily redefines the domain specified in the define command. • If a domain is not specified in this command, the domain specification from the define command is used for sampling. • An error is flagged in the case of discrete valued parameters when a domain is not specified in this command or in the define command. A domain specification (either in this command or in the define command) is required for discrete valued parameters because the possible discrete values that can be sampled must be known. Although a domain specification is not required for continuous valued parameters, it may be given. In either the case of discrete parameters or the case of continuous parameters, a domain specification can be used to limit the number of values sampled using the REFERENCE option since the domain is treated as a bound on the possible sampling values. For example, specifying reference=50., interval=10., and numSymPairs=3 for a continuous parameter with domain=(35., 100.) will sample values of 40., 50., 60., 70., and 80. for this parameter. The minimum value of the domain acts as a bound in this sampling. Input File Usage: aStudy.sample (REFERENCE, par=, reference=, interval=, numSymPairs=, domain=) Sampling by VALUES This sampling option assumes that you wish to create the parameter sample values directly. You must specify the actual parameter values, irrespective of whether the parameter is continuous or discrete. A parameter domain specified in the define command does not affect the values sampled for the parameter when this option is used. Input File Usage: aStudy.sample (VALUES, par=, values=) Combination of parameter samples Use the aStudy.combine command to create sets of design points from the parameter samples. Choose how the combining is done using one of the following tokens: MESH, TUPLE, or CROSS. The use of each combination command results in the creation of a number of design points, which are grouped into design sets. If a combine operation creates a design that duplicates a design in an existing design set, the duplicate design is deleted immediately. The total number of designs in a parametric study (before the application of any design constraints) is the sum of the number of designs in each design set. You can name a design set; if you do not, it is named by default. The default naming convention is p1 for the first non-user-named design set in the parametric study, p2 for the second non-user-named design set, and so on. The design set name is used to help identify individual designs. A design set named by you with a name identical to a previously specified design set name indicates that it is a respecification of the design set and, thus, overwrites the previously existing one. Input File Usage: aStudy.combine (token, name=) MESH combination This combine option indicates that every sampled value for a parameter is to be combined with every sampled value of every other parameter in the parametric study. The following examples illustrate the use of the MESH combine option. In a two-parameter study with the parameters defined and sampled as study=ParStudy(par=('par1', 'par2')) study.define(DISCRETE, par='par1', domain=(1, 3, 5, 7, 9, 11, 13)) study.sample(REFERENCE, par='par1', reference=0, interval=2, numSymPairs=2) study.define(CONTINUOUS, par='par2', domain=(10., 60.)) study.sample(INTERVAL, par='par2', interval=20.) the combine command study.combine(MESH, name='dSet1') creates the following 12 design points (par1, par2): (1, 10.), (5, 10.), (9, 10.), (1, 30.), (5, 30.), (9, 30.), (1, 50.), (5, 50.), (9, 50.), (1, 60.), (5, 60.), and (9, 60.) . A second use of the combine command preceded by a respecification of the parameter sampling study.sample(NUMBER, par='par1', number=3) study.sample(NUMBER, par='par2', number=3) study.combine(MESH, name='dSet2') par2 60. 50. 40. 30. 20. 10. 9 11 13 par1 Figure 20.1.1–1 Design points in design set dSet1 created with the MESH option of the combine command. creates designs at the following nine points: (1, 10.), (7, 10.), (13, 10.), (1, 35.), (7, 35.), (13, 35.), (1, 60.), (7, 60.), and (13, 60.) . The extreme and center values of both parameters are combined. par2 60. 50. 40. 30. 20. 10. 9 11 13 par1 Figure 20.1.1–2 Design points in design set dSet2 created with the MESH option of the combine command after the parameter sampling is redefined. TUPLE combination This combine option creates design sets consisting of n-tuples of the sampled parameter values, where n is the number of parameters in the parametric study. Each n-tuple consists of one sampled value for each parameter. For example, in a three-parameter study the first sampled value of each of the three parameters makes up the first 3-tuple, the second sampled value of each of the three parameters makes up the second 3-tuple, and so on. The creation of tuples ceases when any of the parameter samples runs out of sampled values. The following examples illustrate the use of the TUPLE combination operation. For a two-parameter study with the parameters defined and sampled as study=ParStudy(par=('par1', 'par2')) study.define(DISCRETE, par='par1', domain=(1, 3, 5, 7, 9, 11, 13)) study.define(CONTINUOUS, par='par2', domain=(10., 60.)) study.sample(INTERVAL, par='par1', interval=1) study.sample(INTERVAL, par='par2', interval=10.) the combination operation study.combine(TUPLE, name='dSet3') creates designs at the following 6 points: (1, 10.), (3, 20.), (5, 30.), (7, 40.), (9, 50.), and (11, 60.) . This represents a diagonal pattern in the two-parameter space. We see that all par2 values are used in the tuple combination but the last par1 value is not used because there are no more par2 sample values to form additional tuples. par2 60. 50. 40. 30. 20. 10. 9 11 13 par1 Figure 20.1.1–3 Design points in design set dSet3 created with the TUPLE option of the combine command. A second invocation of the above combine command after respecifying the par2 sampling as study.sample(INTERVAL, par='par2', interval=-10.) study.combine(TUPLE, name='dSet4') creates designs at the following 6 points: (1, 60.), (3, 50.), (5, 40.), (7, 30.), (9, 20.), and (11, 10.) . This represents the other diagonal in the two-parameter space. par2 60. 50. 40. 30. 20. 10. 9 11 13 par1 Figure 20.1.1–4 Design points in design set dSet4 created with the TUPLE option of the combine command after the parameter sampling is redefined. CROSS combination This combine option creates designs in the form of “cross-shaped” patterns as follows: each value sampled for an individual parameter is combined with the reference value, as specified in the define command, of all the other parameters used in the parametric study. To use the CROSS combine option, it is necessary to specify a reference value in the define command for all parameters in the parametric study. The reference value specified for a parameter in the define command does not have to coincide with a value sampled by that parameter’s sampling rule. However, if the reference value does not coincide with a sampled value, the reference parameter value is not added to the list of sampled values for that parameter; it is used only to form the CROSS combination. The following examples illustrate the use of the CROSS combine option. For a two-parameter study with the parameters defined and sampled as study=ParStudy(par=('par1', 'par2')) study.define(DISCRETE, par='par1', domain=(1, 3, 5, 7, 9, 11, 13), reference=3) study.define(CONTINUOUS, par='par2', domain=(10., 60.), reference=40.) study.sample(REFERENCE, par='par1', interval=1, numSymPairs=3) study.sample(INTERVAL, par='par2', interval=10.) the combine cross option study.combine(CROSS, name='dSet5') creates designs at the following 12 points: (1, 40.), (3, 40.), (5, 40.), (7, 40.), (9, 40.), (11, 40.), (13, 40.), (7, 10.), (7, 20.), (7, 30.), (7, 50.), and (7, 60.) . This combination is a cross-shaped pattern where the cross intersection is at (7, 40.) as specified [7 is the fourth value (reference=3) of the discrete parameter par1]. par2 60. 50. 40. 30. 20. 10. 9 11 13 par1 Figure 20.1.1–5 Design points in design set dSet5 created with the CROSS option of the combine command. A second invocation of the above combine command after respecifying par2 as study.define(CONTINUOUS, par='par2', domain=(10., 60.), reference=45.) study.combine(CROSS, name='dSet6') creates designs at the following 13 design points: (1, 45.), (3, 45.), (5, 45.), (7, 45.), (9, 45.), (11, 45.), (13, 45.), (7, 10.), (7, 20.), (7, 30.), (7, 40.), (7, 50.), and (7, 60.) . Constraining designs A constraint that determines the allowable design points in the parametric study can be specified using the aStudy.constrain scripting command . When such a constraint is specified, existing designs that violate the constraint are eliminated immediately. For example, the constrain command aStudy.constrain('height*width < 12.') where height and width are parameters in the parametric study, can be used to enforce that the cross- sectional area of a rectangular beam must be less than 12.0 in all designs. Input File Usage: aStudy.constrain ('constraint expression') par2 60. 50. 40. 30. 20. 10. 9 11 13 par1 Figure 20.1.1–6 Design points in design set dSet6 created with the CROSS option of the combine command when the parameter par2 is redefined. Generation and execution of the designs of a parametric study Once the required design points have been specified, it is necessary to generate the corresponding analysis job data and execute the analyses. Generation of analysis job data Use the aStudy.generate scripting command to generate an input file for each design. The name of the parametrized template input file from which the input files of each design are generated must be specified. The naming convention for the input files generated by the parametric study is as follows: • The name of each analysis job will start with the template input file name; for example, shell. • The name of the parametric study (specified by you in the ParStudy command using the name= option) is appended, preceded by an underscore (_); for example, shell_thickness for a parametric study defined with the study = ParStudy(name=’thickness’) command. (If no parametric study name has been given, the parametric study name defaults to the name of the Python script file in which the study is defined.) If the template input file name and parametric study name are the same, the name is not repeated. • The name of the design set (specified or created by default in the combine command) is appended, preceded by an underscore (_); for example, shell_thickness_p1 for the first design set (named by default) of the above parametric study. • The design name (created automatically in the combine command) is appended, preceded by an underscore (_); for example, shell_thickness_p1_c1 for the first design in the first design set of the above parametric study. As usual, the input files each have the extension .inp. You can examine and/or edit these input files before execution. The generate command creates a file with the .var extension that contains a description of the parametric study. This file is given the parametric study name—for example, studyName.var—and contains a list of all the designs generated, together with the parameter values associated with each design. You can examine and/or edit this file; however, editing this file will affect the gathering of results across the designs of the parametric study . Each time the generate command is used, new versions of the studyName.var files are created reflecting the designs specified by all previous combine commands. The define, sample, and combine steps are performed before the generate command is executed. It is, thus, possible for you to refer to parameters that do not exist or are not independent parameters in the template input file. These errors are detected and flagged by the generate command. Input File Usage: aStudy.generate (template) Execution of the analysis of the designs of a parametric study Use the aStudy.execute command to execute the analysis of the designs of the study. The command will submit a number of analysis jobs for execution under the control of a Python process. All designs can be evaluated without further user interaction by specifying the ALL or DISTRIBUTED options of this command, or you can control the execution of the analyses interactively by specifying the INTERACTIVE option. In the interactive case you are prompted for further execution instructions. The prompt allows you to: • Specify a number of analyses to be executed before the process pauses and prompts you again. • Execute the remaining analyses without further user interaction. • Specify a number of analyses whose execution is to be skipped before the process pauses and prompts you again. • Stop execution. The interactive option is useful because it provides the opportunity to: • Study the results of the analyses already executed. • Delete unnecessary files generated by the analyses to conserve disk space when many designs are being analyzed. • Analyze only certain designs of the parametric study. The ALL and INTERACTIVE tokens are used for sequential execution of the Abaqus analyses on your machine. The DISTRIBUTED token can be used to schedule analysis jobs on multiple machines or multiple CPUs of one machine. The DISTRIBUTED option is available only on variants of the UNIX operating system. In particular the implementation depends on the operating system for support of the rsh, rcp, and xhost UNIX commands. Because of the use of these commands, it is necessary that for distributed execution of parametric studies the parametric study must itself be executed on your local computer. If binary results are output during the analyses, both the local and remote computers must be binary compatible. Before the distributed execution capability can be used, it is necessary to configure the appropriate queue interfaces in the Abaqus environment file. Each analysis of a design of the parametric study that is executed when you issue the execute command is, by default, executed by Abaqus in background mode, irrespective of the command option used. Files created by the Abaqus analysis of each design will overwrite any existing files of the same name without you being prompted. You can add any necessary Abaqus execution options (refer to “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2) to the execution command for each of the analyses by specifying them with the execOptions option. Input File Usage: aStudy.execute (token, files= , queues= , execOptions= ) Parametric study results Once the analyses associated with a parametric study have been executed, the variation of key results across the different designs can be examined. First, results must be gathered from the results file or output database of each of the analyses; then, these results must be reported. the specification of the file, The aStudy.output command can be used to specify the source of the results to be gathered. All arguments to the aStudy.output the analysis step, and the increment (for command are optional: non-frequency steps) or the mode (for frequency steps) from which the results are to be gathered. If the file is not specified, the results (.fil) file will be used. If the step is not specified, it must be specified in the gather command . The defaults of the increment (for non-frequency steps) or the mode (for frequency steps) are the last increment of the step and the first mode calculated in the step unless specified in the gather command. Some arguments are applicable only to the output (.odb) database: the instance name, the request type (field or history), the frame value where the results are to be gathered, and whether the memory used to access an output database should be overlayed when a different output database is accessed. The specification of the source of the gathered results remains in effect for all subsequent gather commands until the source is respecified. Respecification of the gathering source is treated as a complete respecification; that is, nothing is retained from the previous specification of the gathering source. Input File Usage: aStudy.output (file=, instance=, overlay=, request=, step=, frameValue= | inc= | mode=) Gathering results Use the aStudy.gather command to gather results from the results file or output database of each of the analyses. In each use of the gather command you must specify a name that is associated with the gathered result record. This label is used to refer to the results record in the report commands. When gathering results from the results (.fil) file, each result record to be gathered must be chosen by specifying one of the available output variable identifier keys appearing under the .fil column heading in “Abaqus/Standard output variable identifiers,” Section 4.2.1, or “Abaqus/Explicit output variable identifiers,” Section 4.2.2. For example, the U or S variable identifier keys can be specified, but the U1 or S11 variable identifier keys cannot be specified. In addition, the MODAL variable identifier key can be specified to gather eigenvalue results records (those written to the results file with the record key 1980); in this case, no variable location data are required. When gathering results from the output (.odb) database, each result record to be gathered is chosen by specifying one of the available output variable identifier keys appearing under the .odb column heading in “Abaqus/Standard output variable identifiers,” Section 4.2.1, or “Abaqus/Explicit output variable identifiers,” Section 4.2.2. For field output the component must not be specified, while for history output the component number is required; for example, the U or S variable identifier keys can be specified for field output, while the U1 or S11 variable identifier keys can be specified for history output. Unless the output is at the assembly level, an instance name must be provided as an argument to the gather command. An exception to this instance-name requirement is the case where the output (.odb) database is generated from a model not defined as an assembly of part instances, which is inferred from the presence in the output database of a single assembly named Assembly-1 and a single part instance named PART–1–1. In this case you need not explicitly refer to the instance PART–1–1. The names of components of the result records are created automatically. For example, the command myStudy.gather(results='e52_stress', variable='S', element=52) creates a result record e52_stress whose six components (in the case of a three-dimensional solid element) are named: e52_stress.1 (the S11 stress component), e52_stress.2 (the S22 stress component), e52_stress.3 (the S33 stress component), e52_stress.4 (the S12 stress component), e52_stress.5 (the S13 stress component), and e52_stress.6 (the S23 stress component). The variable location data that must be given depend on the output variable identifier key specified. (Refer to “Gather the results of a parametric study.,” Section 20.2.5, for a description of the location data.) Enough variable location data must be given to define a unique result record. Input File Usage: aStudy.gather (request=, results=, step=, frameValue= | inc= | mode=, variable=, additional location data) Reporting results Use the aStudy.report scripting command to report results gathered from the results files of the parametric study. Use the PRINT, FILE, or XYPLOT options to specify the kind of report to be produced: • PRINT indicates that a table of results (with headings) is to be printed to the default output device (the screen). You may wish to limit the number of columns in a table so as to make the table readable. • FILE indicates that a table of results (with headings) is to be written to an ASCII file. • XYPLOT indicates that a table of results (without headings) is to be written to an ASCII file that can later be read into the Visualization module in Abaqus/CAE to display X–Y plots. Each row in a table represents a design in the parametric study. A column in a table can represent values of a parameter, values of a gathered result, or design names. One or more parameters can be specified in the report command. If no parameters are specified, the default is that all parameters in the parametric study are included in the table. The column corresponding to each parameter shows the value of that parameter in each of the designs included in the table. A design set name can be specified to restrict the rows in the table to designs that are part of the set (refer to the combine command described earlier). If a design set is not specified, the default is that all designs are included in the table. Use variations=ON to specify that the first column in a table must show the design names. If variations=ON is not specified or variations=OFF is included, the column of design names is not included in the table. The names of the results to be reported must be specified as a sequence; for example, the Mises stress of element 33, the S22 stress of element 52, and the U3 displacement of node 10 are gathered in the following three separate commands: myStudy.gather(results='e33_sinv', variable='SINV', element=33) myStudy.gather(results='e52_s', variable='S', element=52) myStudy.gather(results='n10_u', variable='U', node=10) These results can be printed in a single table using the following report command: myStudy.report(PRINT, results=('e33_sinv.1', 'e52_s.2', 'n10_u.3')) This example shows not only how gathered results of different types (element, nodal, etc.) can be collected in a single table but also how to refer to components of results records (the Mises stress is the first component of SINV, S22 is the second component of S, and U3 is the third component of U—refer to “Results file output format,” Section 5.1.2, or the Abaqus Scripting User’s Manual for a description of how the results are stored in the results file and the output database, respectively). When either the FILE token or the XYPLOT token is used, a file name must be given to specify the file to which the results are to be written. A subsequent report command issued in the same session using the same file name will append the new results to the file. However, a subsequent report command issued in a different session using the same file name overwrites the existing file. Input File Usage: aStudy.report (token, results=, par=, designSet=, variations=, file=) Execution of parametric studies To carry out a parametric study, you must prepare a parametrized input file (inputFile.inp). This input file is the template used for the generation of the parametric variations of the study and must contain the parameter definitions necessary to use parameters in place of input quantities. The parameters must be defined in the template file; they cannot be defined in any include files that are referred to by the template file. In addition, you must prepare a Python scripting file, scriptFile.psf, containing instructions that script the actions of the parametric study. Typically, you prepare the Python scripting file using an editor and then invoke execution of this file using the Abaqus execution command abaqus script=scriptFile. This command starts the Python interpreter and executes the instructions in the scripting file. Alternatively, you simply start the Python interpreter, without giving a scripting file, with the Abaqus execution command abaqus script. In this case the Python interpreter remains active, and you can execute additional commands interactively or execute additional commands contained in a file (for example, fileName) using the Python command execfile(’fileName’). The Python interpreter can be terminated using [Ctrl]+d on a UNIX machine or [Ctrl]+z on a Windows machine. It is normally preferable to execute a previously prepared scripting file because it is likely that you will want to develop the script iteratively; in this case you simply have to go back and edit the scripting file and re-execute it until satisfied with the result. You can monitor the progress of the parametric variation analyses using normal operating system commands. Execution in more than one session You may want to gather and report results multiple times, after the parametric variations of the study have been executed. It is possible to define, generate, and execute a parametric study in one session and gather and report results in a separate session. Only the command used to create the parametric study needs to be reissued when you start a new session. Visualization of parametric study results The results of the analysis of a particular parametric study variation can be visualized like any other results of a single analysis. Visualization of results gathered across designs of a parametric study requires gathering of results. For visualization the results must be reported in ASCII files (using the XYPLOT option in the gather command), which can be read by the Visualization module in Abaqus/CAE to produce X–Y plots of results versus parameter values or design names. Scripting commands Parametric studies are scripted in files with the .psf extension using the Python language (Lutz, 1996). A parametric study object, constructed from the ParStudy class, is provided whose methods make scripting of parametric studies straightforward; these methods are described in this chapter. Syntax of scripting commands Scripting commands generally have the following form: aStudy.method (token, data) aStudy is the parametric study object to which the method applies; this object is constructed using the parametric study constructor command. method is the method to be used; for example, define, sample, or execute. Most (but not all) commands have a token that selects an option of the command; for example, aStudy.define (CONTINUOUS, par= ) indicates that one or more continuous parameters are being defined in a parametric study. Tokens are always given in capital letters and are mutually exclusive. For most (but not all) commands additional data must be specified. Python language rules The parametric study scripts contained in scripting files must follow the syntax and semantics of the Python language. Some important aspects of this language are described here (more general Python language rules are discussed in “Parametric input,” Section 1.4.1). Comments Comments must be preceded by the # symbol. The comment is understood to continue to the end of the line. For example, # # This parametric study ... # studyTempEffects.generate(template='shell') #use shell input file Case sensitivity All variable and method names, tokens, and character string literals are case sensitive across all operating systems. For example, study.execute( ) # is valid study.Execute( ) # is not valid because of the capital E study.sample(NUMBER, ...) # uses the valid token NUMBER study.sample(number, ...) # lower case token is not valid study.generate(template='aFile') # 'aFile' is different study.generate(template='afile') # from 'afile' Character strings Character strings are indicated by using paired single (’ ’) or double (” ”) quotation marks. Backward single quotation marks (‘ ‘) cannot be used for this purpose. For example, "double quoted string" 'single quoted string' Printing The Python print command can be used to obtain a printed representation of any Python object. For example, print 'MY TEXT' will print MY TEXT on the standard output device. Lists and tuples The scripting methods for parametric studies accept integer, real, and character string types. These primitive types can, in many cases, optionally be contained within tuple or list structures. Although there are some differences between lists and tuples in Python, they can be used interchangeably in the parametric study scripting commands; they simply represent ordered sequences of items. Items in lists or tuples must be separated by commas and enclosed in parentheses or brackets. For example, aStudy.define(CONTINUOUS, par=('xCoord',))# tuple contains a # single string item aStudy.define(CONTINUOUS, par=['xCoord']) # list contains a # single string item aStudy.define(CONTINUOUS, par=('xCoord', 'yCoord')) # tuple aStudy.define(CONTINUOUS, par=['xCoord', 'yCoord']) # list Indentation Python uses indentation to group blocks of statements. Therefore, a Python statement should begin in the same column as the preceding statement except where grouping of statements is required by Python. Accessing the data of a parametric study In some cases it is desirable to have direct programmatic access to the data of a parametric study. Therefore, all of the important data of the study are stored in repositories that can be accessed as data members of the parametric study object. The repositories have a similar interface and similar behavior to that of Python dictionaries. Repository data are stored as key, value pairs; and methods are provided for accessing the repository keys and values. The syntax aValue = aRepository[aKey] is used to retrieve the value associated with a repository key. A list of the keys of the repository is obtained using the keys() method of the repository; for example, allKeys = aRepository.keys(). Similarly, a list of the values of the repository is obtained using the values() method of the repository; for example, allValues = aRepository.values(). The following parametric study script shows an example of how the parameter repository of a parametric study can be accessed and how a list of the parameter names and a list of the sample values for the parameter t1 can be obtained: studyTempEffect = ParStudy(par=('t1', 't2')) studyTempEffect.define(CONTINUOUS, par=('t1', 't2')) studyTempEffect.sample(VALUES, par='t1', values=(200.,300.,400.)) studyTempEffect.sample(VALUES, par='t2', values=(250.,350.,450.)) parRepository = studyTempEffect.parameter listOfParameters = parRepository.keys() t1Sample = parRepository['t1'].sample The script results in the following assignments: listOfParameters = [’t1’, ’t2’] and t1Sample = [200.0, 300.0, 400.0]. The Python print command can be used to obtain information on the contents of a repository. Parametric study repositories A parametric study has the following repositories and objects as data members: • aStudy.parameter: A repository for parameter objects keyed by parameter name. Each parameter object has a name, type, domain, reference, and sample data member. • aStudy.designSet: A repository for design sets keyed by design set name. Each design set is represented as a list of design points. • aStudy.job: A repository for analysis job objects keyed by the name of the corresponding analysis input file name (without the .inp extension). Each job object has a design, status, root, designSet, and designName data member. • aStudy.resultData: A repository for result records keyed by a name constructed by successively appending the result name, the underscore character (_), and the design name. For results retrieved from the result (.fil) file, each result record is in the format of the result (.fil) file record for the corresponding output variable. For field results retrieved from the output (.odb) database, each result record will be a tuple containing the components of the results. The result record for history results from the output (.odb) database, which can only be retrieved for a single component, will be a tuple containing a single value. • aStudy.table: A table object containing a representation of the table formatted by the last use of the report command. The table object has title, variation, designs, and results data members. Additional reference • Lutz, M., Programming Python, O’Reilly & Associates, Inc., 1996. 20.2 Parametric studies: commands • “Combine parameter samples for parametric studies.,” Section 20.2.1 • “Constrain parameter value combinations in parametric studies.,” Section 20.2.2 • “Define parameters for parametric studies.,” Section 20.2.3 • “Execute the analysis of parametric study designs.,” Section 20.2.4 • “Gather the results of a parametric study.,” Section 20.2.5 • “Generate the analysis job data for a parametric study.,” Section 20.2.6 • “Specify the source of parametric study results.,” Section 20.2.7 • “Create a parametric study.,” Section 20.2.8 • “Report parametric study results.,” Section 20.2.9 • “Sample parameters for parametric studies.,” Section 20.2.10 20.2.1 aStudy.combine(): Combine parameter samples for parametric studies. Products: Abaqus/Standard Abaqus/Explicit This command is used to combine the sampled parameter values in a parametric study. Reference: • “Scripting parametric studies,” Section 20.1.1 Command: aStudy.combine (token, additional data) Tokens: CROSS Use this token to create designs in a “cross-shaped” pattern from the sampled values of the parameters in the parametric study. MESH Use this token to create designs in a “mesh” pattern in which every sampled value of a parameter is combined with every sampled value of every other parameter in the parametric study. PRINT Use this token to print the design points created for the parametric study. TUPLE Use this token to create designs in a “tuple” pattern consisting of tuples of sampled values of the parameters in the parametric study. Additional data for CROSS, MESH, and TUPLE: Optional data: name Set name equal to the name of the design set being defined; this name must be enclosed by quotation marks. A default design set name is created if a name is not specified. Additional data for PRINT: Optional data: name Set name equal to the name of the design set for which information is being printed; this name must be enclosed by quotation marks. If a design set name is not specified, information is printed for all the design sets in the parametric study. 20.2.2 aStudy.constrain(): Constrain parameter value combinations in parametric studies. Products: Abaqus/Standard Abaqus/Explicit This command is used to define constraints on parameter value combinations; combinations that violate any of the constraints are eliminated from the parametric study. Reference: • “Scripting parametric studies,” Section 20.1.1 Command: aStudy.constrain (constraint expression) Required data: constraint expression Provide a constraint expression enclosed by matching quotation marks. This expression may involve operations among parameters, numbers, and previously defined Python variables; for example, ’height*width < maxArea-2.0’. The constraint can be an equality or an inequality. 20.2.3 aStudy.define(): Define parameters for parametric studies. Products: Abaqus/Standard Abaqus/Explicit This command is used to define the parameters specified for a parametric study. Reference: • “Scripting parametric studies,” Section 20.1.1 Command: aStudy.define (token, additional data) Tokens: CONTINUOUS Use this token to indicate that the parameter is continuous valued. DISCRETE Use this token to indicate that the parameter is discrete valued. PRINT Use this token to print parameter definitions. Additional data for CONTINUOUS: Required data: par Set par equal to the name of the parameter or the sequence of parameters being defined. If a single parameter is specified, it must be enclosed by matching quotation marks; for example, ’par1’. If a list of parameters is specified, it must be given inside parentheses or brackets and must contain parameter names enclosed by matching quotation marks and separated by commas; for example, (’par1’, ’par2’, ’par3’) or [’par1’, ’par2’, ’par3’]. Optional data: domain Set domain equal to the minimum and maximum values of the parameter separated by a comma and enclosed by parentheses or brackets; for example, (10., 20.) or [10., 20.]. If domain is omitted from this command and the parameter is later sampled using a method that requires a domain definition, the domain must be specified in the sample command. reference Set reference equal to the reference value of the parameter. If reference is omitted from this command and the parameter is later sampled using a method that requires a reference definition, the reference must be specified in the sample command. Additional data for DISCRETE: Required data: par Set par equal to the name of the parameter or the list of parameters being defined. If a single parameter is specified, it must be enclosed by matching quotation marks; for example, ’par1’. If a list of parameters is specified, it must be given inside parentheses or brackets and must contain parameter names enclosed by matching quotation marks and separated by commas; for example, (’par1’, ’par2’, ’par3’) or [’par1’, ’par2’, ’par3’]. Optional data: domain Set domain equal to the sequence of values that the parameter may have. The values must be separated by commas and enclosed by parentheses or brackets; for example, (1., 2., 5., 3.) or [1., 2., 5., 3.]. If domain is omitted from this command and the parameter is later sampled using a method that requires a domain definition, the domain must be specified in the sample command. reference Set reference equal to the index in the sequence of parameter values. Indexing starts at zero, so that the first value of the sequence corresponds to index zero and the last value of the sequence corresponds to an index equal to the number of values in the sequence minus one. If reference is omitted from this command and the parameter is later sampled using a method that requires a reference definition, the reference must be specified in the sample command. Additional data for PRINT: Optional data: par Set par equal to the name of the parameter or the sequence of parameters whose definition is to be printed. If a single parameter is specified, it must be enclosed by matching quotation marks; for example, ’par1’. If a sequence of parameters is specified, it must be given inside parentheses or brackets and must contain parameter names enclosed by matching quotation marks and separated by commas; for example, (’par1’, ’par2’, ’par3’) or [’par1’, ’par2’, ’par3’]. If par is omitted, parameter definitions are printed for all parameters in the parametric study. 20.2.4 aStudy.execute(): Execute the analysis of parametric study designs. Products: Abaqus/Standard Abaqus/Explicit This command is used to execute the analyses of the designs generated by a parametric study. Reference: • “Scripting parametric studies,” Section 20.1.1 Command: aStudy.execute (token, execOptions= , additional data) Tokens: ALL Use this token to sequentially execute the analyses of all the designs of the parametric study. This option is the default. DISTRIBUTED Use this token to execute the analyses of all designs using the specified queue interfaces of the local and/or remote computers. A similar number of analyses will be distributed to each of the specified queues. INTERACTIVE Use this token to sequentially execute the analyses of all the designs of the parametric study in interactive mode. In this case the process pauses to prompt you for further execution instructions. The prompt allows you to specify the number of analyses to be executed, to execute the remaining analyses, to specify the number of analyses whose execution is to be skipped, or to skip all the remaining analyses. Optional data: execOptions Set execOptions equal to a character string of Abaqus execution options (refer to “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2) that are to be added to the Abaqus execution command when executing the analyses of the designs of the parametric study; this string must be enclosed in matching quotation marks. Additional data for DISTRIBUTED: Required data: queues Set queues equal to the queue interface name or a sequence of queue interface names. If a single name is given, it must be enclosed in matching quotation marks. If a sequence of names is given, it must be enclosed in parentheses or brackets and contain queue interface names enclosed in matching quotation marks and separated by commas. Optional data: files Set files equal to the symbolic constant or a sequence of symbolic constants that identifies the file or files that must be returned to the local computer after remote execution. The sequence items must be separated by commas, and the sequence must be enclosed in parentheses or brackets. The allowed symbolic constants are: DAT, LOG, FIL, SEL, MSG, STA, ODB, IPM, RES, ABQ, and PAC. The default value is files = (DAT, FIL, LOG, ODB, SEL). Defining queues and queue interfaces: Before being used for a distributed parametric study, queue interfaces must be defined within the design_startup portion of the Abaqus environment file. For example, to define a queue interface for an existing queue short on the remote computer server, the following entry in the environment file is required: def onDesignStartup(): from session import Queue import os # convenience assignment SCRATCH = '/scratch/' + os.environ['USER'] # create remote queue interface Queue(name='short_interface', hostName='server', driver='abaqus', queueName='short', directory=SCRATCH) If, in addition, a local queue is required, the entry must be expanded to: def onDesignStartup(): from session import Queue import os # convenience assignment SCRATCH = '/scratch/' + os.environ['USER'] # create remote queue interface Queue(name='short_interface', hostName='server', driver='abaqus', queueName='short', directory=SCRATCH) # create local queue interface Queue(name='local_interface', driver='abaqus', queue_name="local" local="echo "./%S 1>%L 2>&1" | batch" aStudy.execute() 20.2.5 aStudy.gather(): Gather the results of a parametric study. Products: Abaqus/Standard Abaqus/Explicit This command is used to gather analysis results across the designs of a parametric study. Reference: • “Scripting parametric studies,” Section 20.1.1 Command: aStudy.gather (request= , results= , step= , frameValue= | inc= | mode= , variable= , additional data) Required data: results Set results equal to a name that will be used to identify the results record gathered by this command. This name must be enclosed in matching quotation marks. variable Set variable equal to an output variable identifier key; this key must be enclosed in matching quotation marks. For gathering results from the results (.fil) file only those output variable identifier keys appearing under the .fil column heading in “Abaqus/Standard output variable identifiers,” Section 4.2.1, or “Abaqus/Explicit output variable identifiers,” Section 4.2.2, are available. For example, the U or S variable identifier keys can be specified, but the U1 or S11 variable identifier keys cannot be specified. In addition, the MODAL variable identifier key can be specified to gather frequency results (those written to the results file with the record key 1980); in this case no additional data are required in this command. When gathering results from the output database (.odb) file, each result record to be gathered is chosen by specifying one of the available output variable identifier keys appearing under the .odb column heading in “Abaqus/Standard output variable identifiers,” Section 4.2.1, or “Abaqus/Explicit output variable identifiers,” Section 4.2.2. For field output the component must not be specified, while for history output the component number is required; for example, the U or S variable identifier keys can be specified for field output, while the U1 or S11 variable identifier keys can be specified for history output. Optional data: request This option is applicable only if the results are to be gathered from the output database file. Set request equal to FIELD or HISTORY to specify whether the results must be gathered from the field data or the history data in the output database file. If request is omitted from this command, the results will be gathered from the field data. step Set step equal to the analysis step number from which the results are to be gathered. If step is specified in this command as well as in the output command, the step specification in this command is used. If step is omitted from this command, it must have been specified in the output command. Optional and mutually exclusive data: frameValue This option is applicable only if the results are to be gathered from the output database file. Set frameValue equal to the step time or frequency value of the analysis increment in the analysis step specified from which the results are to be gathered. frameValue can also be set equal to the symbolic constant LAST to specify that results are to be gathered from the last increment of the step. If no results are available at the frameValue specified, a warning will be issued and the results will be gathered from the closest increment. If frameValue is specified in this command as well as in the output command, the frameValue specification in this command is used for gathering. If frameValue is omitted from this command, the results are gathered for the frameValue specified in the output command or are gathered from the last increment in the step. inc Set inc equal to the number of the analysis increment of the non-frequency analysis step specified from which the results are to be gathered across the parametric study variations. inc can also be set equal to the symbolic constant LAST to specify that results are to be gathered from the last increment of the step. If inc is specified in this command as well as in the output command, the inc specification in this command is used for gathering. If inc is omitted from this command, the results are gathered from the increment specified in the output command or are gathered from the last increment in the step. This option is not valid for gathering history results from the output database file. mode Set mode equal to the number of the mode of the frequency analysis step specified from which the results are to be gathered across the parametric study variations. If mode is specified in this command as well as in the output command, the mode specification in this command is used. If mode is omitted from this command, the results are gathered from the mode specified in the output command or are gathered from the first mode in the step. Additional data for element integration point variables: Required data: element Set element equal to the number of the element for which results are to be gathered. instance This option is required only if results are gathered for an element on a part instance in an output database file generated from a model described as an assembly of part instances. Set instance equal to the name of the part instance for which results are to be gathered. This name must be enclosed in matching quotation marks. If instance is specified in this command as well as in the output command, the instance specification in this command is used. Optional data: centroid Set centroid equal to the symbolic constant ON to indicate that the results are to be gathered at the centroid of the element. This option is valid only when the results have been written to the results file at the centroid of the element. centroid, int, and node are mutually exclusive. If centroid, int, and node are omitted, the default is int=1. int Set int equal to the number of the integration point of the element for which results are to be gathered. This option is valid only when the results have been written to the results file at the integration points of the element. centroid, int, and node are mutually exclusive. If int is omitted, the default is int=1. If centroid, int, and node are omitted, the default is int=1. node Set node equal to the number of the node in the element for which results are to be gathered. This option is valid only when the results have been written to the results file at the nodes of the element. centroid, int, and node are mutually exclusive. If centroid, int, and node are omitted, the default is int=1. rbnum Set rbnum equal to the number of the rebar for which results are to be gathered. The rebar number is consistent with the order, per element, in which you define the rebar . If rbnum is omitted, the default is rbnum=1. Rebar information cannot be gathered from the output database file. rebar Set rebar equal to the name of the rebar for which results are to be gathered (defined as described in “Defining rebar as an element property,” Section 2.2.4). Rebar results can be obtained for continuum and beam elements only at integration points; for shell and membrane elements rebar results can be obtained at integration points and at the centroid of the element. Rebar information cannot be gathered from the output database file. section Set section equal to the number of the section point of the element for which results are to be gathered. This applies to beam, shell, or layered solid elements. section is not relevant for rebar results. If section is omitted, the default is section=1. Additional data for element section variables: Required data: element Set element equal to the number of the element for which results are to be gathered. instance This option is required only if results are gathered for an element on a part instance in an output database file generated from a model described as an assembly of part instances. Set instance equal to the name of the part instance for which results are to be gathered. This name must be enclosed in matching quotation marks. If instance is specified in this command as well as in the output command, the instance specification in this command is used. Optional data: centroid Set centroid equal to the symbolic token ON to indicate that the results are to be gathered at the centroid of the element. This option is valid only when the results have been written to the results file or output database at the centroid of the element. centroid, int, and node are mutually exclusive. If centroid, int, and node are omitted, the default is int=1. int Set int equal to the number of the integration point of the element for which results are to be gathered. This option is valid only when the results have been written to the results file or output database at the integration points of the element. centroid, int, and node are mutually exclusive. If int is omitted, the default is int=1. If centroid, int, and node are omitted, the default is int=1. node Set node equal to the number of the node in the element for which results are to be gathered. This option is valid only when the results have been written to the results file or output database at the nodes of the element. centroid, int, and node are mutually exclusive. If centroid, int, and node are omitted, the default is int=1. Additional data for whole element variables: Required data: element Set element equal to the number of the element for which results are to be gathered. int Set int = –1. instance This option is required only if results are gathered for an element on a part instance in an output database file generated from a model described as an assembly of part instances. Set instance equal to the name of the part instance for which results are to be gathered. This name must be enclosed in matching quotation marks. If instance is specified in this command as well as in the output command, the instance specification in this command is used. Additional data for partial model (element set) or whole model variables: Optional data: elset Set elset equal to the element set name for which results are to be gathered. If elset is omitted, results will be gathered for the whole model. This name must be enclosed in matching quotation marks. instance This option is required only if results are gathered from an output database file and if the element set is defined on an instance. Set instance equal to the name of the instance on which the element set is defined. This name must be enclosed in matching quotation marks. If the element set is defined on the assembly, instance must not be specified in both this command and the output command. If instance is specified in this command as well as in the output command, the instance specification in this command is used. Additional data for nodal variables: Required data: node Set node equal to the number of the node for which results are to be gathered. instance This option is required only if results are gathered for a node on a part instance in an output database file generated from a model described as an assembly of part instances. Set instance equal to the name of the instance for which results are to be gathered. This name must be enclosed in matching quotation marks. If instance is specified in this command as well as in the output command, the instance specification in this command is used. Additional data for modal variables: There are no additional data. Additional data for contact surface variables: Required data: master Set master equal to the name of the master surface of the contact pair for which results are to be gathered. This name must be enclosed in matching quotation marks. slave Set slave equal to the name of the slave surface of the contact pair for which results are to be gathered. This name must be enclosed in matching quotation marks. Optional data: masterInstance This option is required only if results are gathered from an output database file and if the master surface is defined on an instance. Set masterInstance equal to the name of the instance on which the master surface is defined. This name must be enclosed in matching quotation marks. slaveInstance This option is required only if results are gathered from an output database file and if the slave surface is defined on an instance. Set slaveInstance equal to the name of the instance on which the slave surface is defined. This name must be enclosed in matching quotation marks. Required data when slave surface node variable results are requested: node If slave surface node variable results are to be gathered, set node equal to the number of the node for which results are to be gathered. nset and node are mutually exclusive. instance This option is required only if results are gathered for a node on a part instance in an output database file generated from a model described as an assembly of part instances. Set instance equal to the name of the part instance for which results are to be gathered. This name must be enclosed in matching quotation marks. If instance is specified in this command as well as in the output command, the instance specification in this command is used. Optional data when whole surface variable results are requested: nset Set nset equal to the name of the node set for which whole surface variable results are to be gathered. This name must be enclosed in matching quotation marks. If nset is omitted, the default is the whole surface. If the results are collected from the output database file and the node set is defined on an instance, the node set name must be prefixed with the instance name and a period (for example: “PART–1–1.TOP”). nset and node are mutually exclusive. instance This option is required only if results are gathered from an output database file and if the node set is defined on an instance. Set instance equal to the name of the instance on which the node set is defined. This name must be enclosed in matching quotation marks. If the node set is defined on the assembly, instance must not be specified in both this command and the output command. If instance is specified in this command as well as in the output command, the instance specification in this command is used. Additional data for cavity radiation surface variables: Required data: element Set element equal to the number of the element underlying the cavity facet for which results are to be gathered. elface Set elface equal to the face identifier of the face of the element underlying the cavity facet for which results are to be gathered. instance This option is required only if results are gathered from an output database file generated from a model described as an assembly of part instances. Set instance equal to the name of the part instance for which results are to be gathered. This name must be enclosed in matching quotation marks. If instance is specified in this command as well as in the output command, the instance specification in this command is used. Additional data for section file output: Required data: sectionName Set sectionName equal to the name of the section for which results are to be gathered. This name must be enclosed in matching quotation marks . 20.2.6 aStudy.generate(): Generate the analysis job data for a parametric study. Products: Abaqus/Standard Abaqus/Explicit This command is used to generate the analysis input files for a parametric study. Reference: • “Scripting parametric studies,” Section 20.1.1 Command: aStudy.generate (template= ) Required data: template Set template equal to the name of the template input file from which the input files of each of the parametric study variations are to be generated; this name must be enclosed in matching quotation marks. 20.2.7 aStudy.output(): Specify the source of parametric study results. Products: Abaqus/Standard Abaqus/Explicit This command should precede any results gather commands. It is used to specify from where the results of a parametric study will be gathered. Reference: • “Scripting parametric studies,” Section 20.1.1 Command: aStudy.output (file=, instance=, overlay=, request=, step= , frameValue= | inc= | mode= ) Optional data: file Set file equal to FIL or ODB to specify that results must be read from the results (.fil) file or output database (.odb) file. If file is omitted from this command, the results will be read from the results (.fil) file. instance This option is applicable only if results are gathered from an output (.odb) database containing multiple instances. Set instance equal to the name of the part instance for which results are to be gathered. This name must be enclosed in matching quotation marks. If results are gathered for a set defined on the assembly, instance must not be specified in both this command and the gather command. If instance is omitted from this command and an instance name is required to gather the results, it must be specified in the gather command. overlay This option is applicable only if results are gathered from an output (.odb) database. This option is used to control the trade-off between memory usage and execution speed. Set overlay equal to OFF (the default) or ON to specify whether the memory used for an output database should be overwritten. If memory usage is a problem, set overlay equal to ON to specify that the memory used for an output database must be overwritten after a gather is performed for the specific output database. If execution speed is more important than memory usage, set overlay equal to OFF to specify that memory must be allocated for each output database. The overlay option affects your ability to separately manipulate the output database (.odb) file. When you set overlay equal to OFF, the file will remain open after accessing the results from the gather command, which may affect your ability to separately access or manipulate the file (to delete the file, for example). Set overlay equal to ON to separately access the .odb file after accessing the gather based results. request This option is applicable only if the results are to be gathered from the output (.odb) database. Set request equal to FIELD or HISTORY to specify whether the results must be gathered from the field data or the history data in the output database. If request is omitted from this command, the results will be gathered from the field data. step Set step equal to the analysis step number from which the results are to be gathered. If step is omitted from this command, it must be specified in the gather command. Optional and mutually exclusive data: frameValue This option is applicable only if the results are to be gathered from the output (.odb) database. Set frameValue equal to the step time or frequency value of the analysis increment in the analysis step specified from which the results are to be gathered. frameValue can also be set equal to the symbolic constant LAST to specify that results are to be gathered from the last increment of the step. If no results are available at the frameValue specified, a warning will be issued and the results will be gathered from the closest increment. If frameValue is omitted from this command, the results are gathered from the last increment in the step or are gathered from the increment specified in the gather command. inc Set inc equal to the number of the analysis increment of the non-frequency analysis step specified from which the results are to be gathered. inc can also be set equal to the symbolic constant LAST to specify that results are to be gathered from the last increment of the step specified. If inc is omitted from this command, the results are gathered from the last increment in the step or are gathered from the increment specified in the gather command. This option is not valid for gathering history results from the output (.odb) database. mode Set mode equal to the mode number of the frequency analysis step specified from which the results are to be gathered across the parametric study variations. If mode is omitted, the results are gathered from the mode specified in the gather command or are gathered from the first mode in the step. 20.2.8 aStudy=ParStudy(): Create a parametric study. Products: Abaqus/Standard Abaqus/Explicit This command is used to create a parametric study. It must precede any other scripting commands that refer to the parametric study. Reference: • “Scripting parametric studies,” Section 20.1.1 Command: aStudy=ParStudy (par= , name= , verbose= , directory= ) Required data: par Set par equal to the sequence of independent input parameters selected for the parametric study. This sequence must be given inside parentheses or brackets and must contain independent parameter names enclosed by matching quotation marks and separated by commas; for example, (’par1’, ’par2’, ’par3’) or [’par1’, ’par2’, ’par3’]. If only one parameter is to be listed, its name can be given enclosed by matching quotation marks; for example, ’par1’. Optional data: name Set name equal to the name of the parametric study; the name must be enclosed in matching quotation marks. If a name is not specified, its value defaults to the name of the Python script file that contains the parametric study commands. verbose Set verbose equal to the symbolic token OFF to suppress the printing of comment and warning messages. The default is verbose=ON. directory Set directory equal to the symbolic token ON to select that subdirectories of the current directory are used to organize the files of the parametric study. A subdirectory will be created for each design that is analyzed. The default is directory=OFF. aStudy.report(): Report parametric study results. aStudy.report() Products: Abaqus/Standard Abaqus/Explicit This command is used to report results gathered across the designs of a parametric study. Reference: • “Scripting parametric studies,” Section 20.1.1 Command: aStudy.report (token, results= , par= , designSet= , variations=, truncation= , additional data) Tokens: FILE Use this token to specify that results are to be written to an ASCII file as a table with the relevant headings. PRINT Use this token to specify that results are to be printed as a table with the relevant headings. Since the results are printed to the default output device (the screen), you may wish to limit the number of columns in a table so as to make the table readable. XYPLOT Use this token to specify that results are to be written to an ASCII file as a table without headings. This table can subsequently be read by the Visualization module in Abaqus/CAE to display X–Y plots of result and parameter values. Required data: results Set results equal to the sequence of result names to be reported; this sequence must be enclosed For example, results=(’e33_sinv.1’, ’e52_strain’, by parentheses or brackets. ’n25_u.3’), where ’e33_sinv.1’ is the Mises stress of element 33 (Mises is the first component of the SINV record), ’e52_strain’ are all the strain components of element 52, and ’n25_u.3’ is the third component of displacement of node 25. This example assumes that the three results above were gathered in previous gather commands by requesting the SINV, E, and U variable identifier keys, respectively. Optional data: par Set par equal to the name of the parameter or the sequence of parameters to be included in the report table. If a single parameter is specified, it must be enclosed by matching quotation marks; for example, ’par1’. If a sequence of parameters is specified, it must be given inside parentheses or brackets and must contain parameter names enclosed by matching quotation marks and separated by commas; for example, (’par1’, ’par2’, ’par3’) or [’par1’, ’par2’, ’par3’]. If par is omitted, all parameters in the parametric study are included in the report table. designSet Set designSet equal to the name of the design set whose results are to be included in the report table; this name must be enclosed by matching quotation marks. If designSet is omitted, results for all design sets in the parametric study are included in the report table. variations Set variations equal to ON to indicate that the first column of the report table must show the names of the designs being reported. Set variations equal to OFF to indicate that the names of the designs being reported are not to be given in the first column of the report table. If variations is omitted, the column of design names is not included in the report table. truncation Set truncation equal to ON to indicate that the data of the report table must be reported with limited precision. Set truncation equal to OFF to indicate that the data of the report table must be reported with full precision. If truncation is omitted, the data of the report table are reported with limited precision. Additional data for FILE and XYPLOT: Required data: file Set file equal to the name of the file to which the report table is to be written. The file name must be enclosed by matching quotation marks. 20.2.10 aStudy.sample(): Sample parameters for parametric studies. Products: Abaqus/Standard Abaqus/Explicit This command is used to create samples of the values of the parameters of the study. Reference: • “Scripting parametric studies,” Section 20.1.1 Command: aStudy.sample (token, additional data) Tokens: INTERVAL Use this token to sample a parameter at equal intervals. NUMBER Use this token to sample a given number of values of a parameter. PRINT Use this token to print parameter samples. REFERENCE Use this token to sample parameter values specified with respect to a reference parameter value. VALUES Use this token to sample particular values of a parameter. Additional data for INTERVAL: Required data: interval Set interval equal to the sampling interval. For a continuous valued parameter, values are sampled at equally spaced intervals based on the numerical value of the parameter. For a discrete valued parameter, values are sampled at equally spaced intervals based on the indexing of the sequence of parameter values. par Set par equal to the name of the parameter or the sequence of parameters whose samples are to be printed. If a single parameter is specified, it must be enclosed by matching quotation marks; for example, ’par1’. If a sequence of parameters is specified, it must be given inside parentheses or brackets and must contain parameter names enclosed by matching quotation marks and separated by commas; for example, (’par1’, ’par2’, ’par3’) or [’par1’, ’par2’, ’par3’]. Optional data: domain For a continuous valued parameter, set domain equal to the minimum and maximum values of the parameter separated by a comma and enclosed by parentheses or brackets; for example, (10., 20.) or [10., 20.]. For a discrete valued parameter, set domain equal to the sequence of values that the parameter may have separated by commas and enclosed by parentheses or brackets; for example, (1., 2., 5., 3.) or [1., 2., 5., 3.]. If domain is specified in this command as well as in the define command for this parameter, the domain specification in this command is used for sampling. If domain is omitted from this command, it must have been specified in the define command. Additional data for NUMBER: Required data: number Set number equal to the number of equally spaced values to be sampled for the parameter. par Set par equal to the name of the parameter or the sequence of parameters whose samples are to be printed. If a single parameter is specified, it must be enclosed by matching quotation marks; for example, ’par1’. If a sequence of parameters is specified, it must be given inside parentheses or brackets and must contain parameter names enclosed by matching quotation marks and separated by commas; for example, (’par1’, ’par2’, ’par3’) or [’par1’, ’par2’, ’par3’]. Optional data: domain For a continuous valued parameter, set domain equal to the minimum and maximum values of the parameter separated by a comma and enclosed by parentheses or brackets; for example, (10., 20.) or [10., 20.]. For a discrete valued parameter, set domain equal to the sequence of values that the parameter may have separated by commas and enclosed by parentheses or brackets; for example, (1., 2., 5., 3.) or [1., 2., 5., 3.]. If domain is specified in this command as well as in the define command for this parameter, the domain specification in this command is used for sampling. If domain is omitted from this command, it must have been specified in the define command. Additional data for PRINT: Optional data: par Set par equal to the name of the parameter or the sequence of parameters whose samples are to be printed. If a single parameter is specified, it must be enclosed by matching quotation marks; for example, ’par1’. If a sequence of parameters is specified, it must be given inside parentheses or brackets and must contain parameter names enclosed by matching quotation marks and separated by commas; for example, (’par1’, ’par2’, ’par3’) or [’par1’, ’par2’, ’par3’]. If par is omitted, parameter samplings are printed for all parameters in the parametric study. Additional data for REFERENCE: Required data: interval Set interval equal to the sampling interval. For a continuous valued parameter, values are sampled at equally spaced intervals about the reference value based on the numerical value of the parameter. For a discrete valued parameter, values are sampled at equally spaced intervals about the reference value based on the indexing of the sequence of parameter values. numSymPairs Set numSymPairs equal to the number of pairs of parameter values to be sampled symmetrically about the reference value of the parameter. par Set par equal to the name of the parameter being sampled. This name must be enclosed by matching quotation marks; for example, ’par1’. Optional data: domain For a continuous valued parameter, set domain equal to the minimum and maximum values of the parameter separated by a comma and enclosed by parentheses or brackets; for example, (10., 20.) or [10., 20.]. For a discrete valued parameter, set domain equal to the sequence of values that the parameter may have separated by commas and enclosed by parentheses or brackets; for example, (1., 2., 5., 3.) or [1., 2., 5., 3.]. If domain is specified in this command as well as in the define command for this parameter, the domain specification in this command is used for sampling. In the case of a discrete valued parameter if domain is omitted from this command, it must have been specified in the define command. reference For a continuous valued parameter, set reference equal to the reference value of the parameter. For discrete valued parameters, set reference equal to the index in the sequence of parameter values; indexing starts at zero, so that the first value of the sequence corresponds to index zero and the last value of the sequence corresponds to an index equal to the number of values in the sequence minus one. If reference is specified in this command as well as in the define command for this parameter, the reference specification in this command is used for sampling. If reference is omitted from this command, it must have been specified in the define command. Additional data for VALUES: Required data: par Set par equal to the name of the parameter or the sequence of parameters whose samples are to be printed. If a single parameter is specified, it must be enclosed by matching quotation marks; for example, ’par1’. If a sequence of parameters is specified, it must be given inside parentheses or brackets and must contain parameter names enclosed by matching quotation marks and separated by commas; for example, (’par1’, ’par2’, ’par3’) or [’par1’, ’par2’, ’par3’]. values Set values equal to the sequence of parameter values that constitute the sample. This sequence must be given inside parentheses or brackets and must contain values separated by commas; for example, (’CAX4’, ’CAX4R’, ’CAX4H’) or [10., 20., 40.]. SIMULIA is the Dassault Systèmes brand that delivers a scalable portfolio of Realistic Simulation solutions including the Abaqus product suite for Unified Finite Element Analysis; multiphysics solutions for insight into challenging engineering problems; and lifecycle management solutions for managing simulation data, processes, and intellectual property. By building on established technology, respected quality, and superior customer service, SIMULIA makes realistic simulation an integral business practice that improves product performance, reduces physical prototypes, and drives innovation. Headquartered in Providence, RI, USA, with R&D centers in Providence and in Vélizy, France, SIMULIA provides sales, services, and support through a global network of regional offices and distributors. For more information, visit www.simulia.com. About Dassault Systèmes As a world leader in 3D and Product Lifecycle Management (PLM) solutions, Dassault Systèmes brings value to more than 100,000 customers in 80 countries. A pioneer in the 3D software market since 1981, Dassault Systèmes develops and markets PLM application software and services that support industrial processes and provide a 3D vision of the entire lifecycle of products from conception to maintenance to recycling. The Dassault Systèmes portfolio consists of CATIA for designing the virtual product, SolidWorks for 3D mechanical design, DELMIA for virtual production, SIMULIA for virtual testing, ENOVIA for global collaborative lifecycle management, and 3DVIA for online 3D lifelike experiences. Dassault Systèmes’ shares are listed on Euronext Paris (#13065, DSY.PA), and Dassault Systèmes’ ADRs may be traded on the US Over-The-Counter (OTC) market (DASTY). For more information, visit www.3ds.com. fi , , , , , , , , . . , © . , , . / User’s Manual CAUTION: This documentation is intended for qualified users who will exercise sound engineering judgment and expertise in the use of the Abaqus Software. The Abaqus Software is inherently complex, and the examples and procedures in this documentation are not intended to be exhaustive or to apply to any particular situation. Users are cautioned to satisfy themselves as to the accuracy and results of their analyses. Dassault Systèmes and its subsidiaries, including Dassault Systèmes Simulia Corp., shall not be responsible for the accuracy or usefulness of any analysis performed using the Abaqus Software or the procedures, examples, or explanations in this documentation. Dassault Systèmes and its subsidiaries shall not be responsible for the consequences of any errors or omissions that may appear in this documentation. The Abaqus Software is available only under license from Dassault Systèmes or its subsidiary and may be used or reproduced only in accordance with the terms of such license. This documentation is subject to the terms and conditions of either the software license agreement signed by the parties, or, absent such an agreement, the then current software license agreement to which the documentation relates. This documentation and the software described in this documentation are subject to change without prior notice. No part of this documentation may be reproduced or distributed in any form without prior written permission of Dassault Systèmes or its subsidiary. The Abaqus Software is a product of Dassault Systèmes Simulia Corp., Providence, RI, USA. © Dassault Systèmes, 2012 Abaqus, the 3DS logo, SIMULIA, CATIA, and Unified FEA are trademarks or registered trademarks of Dassault Systèmes or its subsidiaries in the United States and/or other countries. Other company, product, and service names may be trademarks or service marks of their respective owners. For additional information concerning SIMULIA European Headquarters Fax: +1 401 276 4408, simulia.support@3ds.com, http://www.simulia.com Stationsplein 8-K, 6221 BT Maastricht, The Netherlands, Tel: +31 43 7999 084, Fax: +31 43 7999 306, simulia.europe.info@3ds.com Locations Dassault Systèmes’ Centers of Simulation Excellence Fremont, CA, Tel: +1 510 794 5891, simulia.west.support@3ds.com West Lafayette, IN, Tel: +1 765 497 1373, simulia.central.support@3ds.com Northville, MI, Tel: +1 248 349 4669, simulia.greatlakes.info@3ds.com Woodbury, MN, Tel: +1 612 424 9044, simulia.central.support@3ds.com Mayfield Heights, OH, Tel: +1 216 378 1070, simulia.erie.info@3ds.com Mason, OH, Tel: +1 513 275 1430, simulia.central.support@3ds.com Warwick, RI, Tel: +1 401 739 3637, simulia.east.support@3ds.com Lewisville, TX, Tel: +1 972 221 6500, simulia.south.info@3ds.com Richmond VIC, Tel: +61 3 9421 2900, simulia.au.support@3ds.com Vienna, Tel: +43 1 22 707 200, simulia.at.info@3ds.com Maarssen, The Netherlands, Tel: +31 346 585 710, simulia.benelux.support@3ds.com Toronto, ON, Tel: +1 416 402 2219, simulia.greatlakes.info@3ds.com Beijing, P. R. China, Tel: +8610 6536 2288, simulia.cn.support@3ds.com Shanghai, P. R. China, Tel: +8621 3856 8000, simulia.cn.support@3ds.com Espoo, Tel: +358 40 902 2973, simulia.nordic.info@3ds.com Velizy Villacoublay Cedex, Tel: +33 1 61 62 72 72, simulia.fr.support@3ds.com Aachen, Tel: +49 241 474 01 0, simulia.de.info@3ds.com Munich, Tel: +49 89 543 48 77 0, simulia.de.info@3ds.com Chennai, Tamil Nadu, Tel: +91 44 43443000, simulia.in.info@3ds.com Lainate MI, Tel: +39 02 3343061, simulia.ity.info@3ds.com Tokyo, Tel: +81 3 5442 6302, simulia.jp.support@3ds.com Osaka, Tel: +81 6 7730 2703, simulia.jp.support@3ds.com Mapo-Gu, Seoul, Tel: +82 2 785 6707/8, simulia.kr.info@3ds.com Puerto Madero, Buenos Aires, Tel: +54 11 4312 8700, Horacio.Burbridge@3ds.com Stockholm, Sweden, Tel: +46 8 68430450, simulia.nordic.info@3ds.com Warrington, Tel: +44 1925 830900, simulia.uk.info@3ds.com Authorized Support Centers SMARTtech Sudamerica SRL, Buenos Aires, Tel: +54 11 4717 2717 KB Engineering, Buenos Aires, Tel: +54 11 4326 7542 Solaer Ingeniería, Buenos Aires, Tel: +54 221 489 1738 SMARTtech Mecânica, Sao Paulo-SP, Tel: +55 11 3168 3388 Synerma s. r. o., Psáry, Prague-West, Tel: +420 603 145 769, abaqus@synerma.cz 3 Dimensional Data Systems, Crete, Tel: +30 2821040012, support@3dds.gr ADCOM, Givataim, Tel: +972 3 7325311, shmulik.keidar@adcomsim.co.il WorleyParsons Services Sdn. Bhd., Kuala Lumpur, Tel: +603 2039 9000, abaqus.my@worleyparsons.com Kimeca.NET SA de CV, Mexico, Tel: +52 55 2459 2635 Matrix Applied Computing Ltd., Auckland, Tel: +64 9 623 1223, abaqus-tech@matrix.co.nz BudSoft Sp. z o.o., Poznań, Tel: +48 61 8508 466, info@budsoft.com.pl TESIS Ltd., Moscow, Tel: +7 495 612 44 22, info@tesis.com.ru WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com Finite Element Analysis Services (Pty) Ltd., Parklands, Tel: +27 21 556 6462, feas@feas.co.za Principia Ingenieros Consultores, S.A., Madrid, Tel: +34 91 209 1482, simulia@principia.es United States Australia Austria Benelux Canada China Finland France Germany India Italy Japan Korea Latin America Scandinavia United Kingdom Argentina Brazil Czech & Slovak Republics Greece Israel Malaysia Mexico New Zealand Poland Russia, Belarus & Ukraine Singapore South Africa Thailand Turkey Simutech Solution Corporation, Taipei, R.O.C., Tel: +886 2 2507 9550, camilla@simutech.com.tw WorleyParsons Pte Ltd., Singapore, Tel: +65 6735 8444, abaqus.sg@worleyparsons.com A-Ztech Ltd., Istanbul, Tel: +90 216 361 8850, info@a-ztech.com.tr Preface Support Both technical engineering support (for problems with creating a model or performing an analysis) and systems support (for installation, licensing, and hardware-related problems) for Abaqus are offered through a network of local support offices. Regional contact information is listed in the front of each Abaqus manual and is accessible from the Locations page at www.simulia.com. Support for SIMULIA products SIMULIA provides a knowledge database of answers and solutions to questions that we have answered, as well as guidelines on how to use Abaqus, SIMULIA Scenario Definition, Isight, and other SIMULIA products. You can also submit new requests for support. All support incidents are tracked. If you contact us by means outside the system to discuss an existing support problem and you know the incident or support request number, please mention it so that we can query the database to see what the latest action has been. Many questions about Abaqus can also be answered by visiting the Products page and the Support page at www.simulia.com. Anonymous ftp site To facilitate data transfer with SIMULIA, an anonymous ftp account is available at ftp.simulia.com. Login as user anonymous, and type your e-mail address as your password. Contact support before placing files on the site. Training All offices and representatives offer regularly scheduled public training classes. The courses are offered in a traditional classroom form and via the Web. We also provide training seminars at customer sites. All training classes and seminars include workshops to provide as much practical experience with Abaqus as possible. For a schedule and descriptions of available classes, see www.simulia.com or call your local office or representative. Feedback We welcome any suggestions for improvements to Abaqus software, the support program, or documentation. We will ensure that any enhancement requests you make are considered for future releases. If you wish to make a suggestion about the service or products, refer to www.simulia.com. Complaints should be made by contacting your local office or through www.simulia.com by visiting the Quality Assurance section of the 1.1.1 1.2.1 1.2.2 1.3.1 1.4.1 2.1.1 2.1.2 2.1.3 2.1.4 2.1.5 2.1.6 2.2.1 2.2.2 2.2.3 2.2.4 2.2.5 2.3.1 2.3.2 2.3.3 2.3.4 Contents Volume I PART I INTRODUCTION, SPATIAL MODELING, AND EXECUTION 1. Introduction Introduction: general Abaqus syntax and conventions Input syntax rules Conventions Abaqus model definition Defining a model in Abaqus Parametric modeling Parametric input 2. Spatial Modeling Node definition Node definition Parametric shape variation Nodal thicknesses Normal definitions at nodes Transformed coordinate systems Adjusting nodal coordinates Element definition Element definition Element foundations Defining reinforcement Defining rebar as an element property Orientations Surface definition Surfaces: overview Element-based surface definition Node-based surface definition Analytical rigid surface definition Eulerian surface definition Operating on surfaces Rigid body definition Rigid body definition Integrated output section definition Integrated output section definition Mass adjustment Adjust and/or redistribute mass of an element set Nonstructural mass definition Nonstructural mass definition Distribution definition Distribution definition Display body definition Display body definition Assembly definition Defining an assembly Matrix definition Defining matrices 3. Job Execution Execution procedures: overview Execution procedure for Abaqus: overview Execution procedures Obtaining information Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution SIMULIA Co-Simulation Engine controller execution Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD co-simulation execution Abaqus/CAE execution Abaqus/Viewer execution Python execution Parametric studies Abaqus documentation Licensing utilities ASCII translation of results (.fil) files Joining results (.fil) files Querying the keyword/problem database ii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 2.3.5 2.3.6 2.4.1 2.5.1 2.6.1 2.7.1 2.8.1 2.9.1 2.10.1 2.11.1 3.1.1 3.2.1 3.2.2 3.2.3 3.2.4 3.2.5 3.2.6 3.2.7 3.2.8 3.2.9 3.2.10 Making user-defined executables and subroutines Input file and output database upgrade utility Generating output database reports Joining output database (.odb) files from restarted analyses Combining output from substructures Combining data from multiple output databases Network output database file connector Mapping thermal and magnetic loads Fixed format conversion utility Translating Nastran bulk data files to Abaqus input files Translating Abaqus files to Nastran bulk data files Translating ANSYS input files to Abaqus input files Translating PAM-CRASH input files to partial Abaqus input files Translating RADIOSS input files to partial Abaqus input files Translating Abaqus output database files to Nastran Output2 results files Translating LS-DYNA data files to Abaqus input files Exchanging Abaqus data with ZAERO Encrypting and decrypting Abaqus input data Job execution control Environment file settings Using the Abaqus environment settings Managing memory and disk resources Managing memory and disk use in Abaqus Parallel execution Parallel execution: overview Parallel execution in Abaqus/Standard Parallel execution in Abaqus/Explicit Parallel execution in Abaqus/CFD File extension definitions File extensions used by Abaqus FORTRAN unit numbers FORTRAN unit numbers used by Abaqus CONTENTS 3.2.14 3.2.15 3.2.16 3.2.17 3.2.18 3.2.19 3.2.20 3.2.21 3.2.22 3.2.23 3.2.24 3.2.25 3.2.26 3.2.27 3.2.28 3.2.29 3.2.30 3.2.31 3.2.32 3.2.33 3.3.1 3.4.1 3.5.1 3.5.2 3.5.3 3.5.4 3.6.1 3.7.1 4.1.2 4.1.3 4.1.4 4.2.1 4.2.2 4.2.3 4.3.1 5.1.1 5.1.2 5.1.3 5.1.4 CONTENTS 4. Output PART II OUTPUT Output Output to the data and results files Output to the output database Error indicator output Output variables Abaqus/Standard output variable identifiers Abaqus/Explicit output variable identifiers Abaqus/CFD output variable identifiers The postprocessing calculator The postprocessing calculator 5. File Output Format Accessing the results file Accessing the results file: overview Results file output format Accessing the results file information Utility routines for accessing the results file OI.1 Abaqus/Standard Output Variable Index OI.2 Abaqus/Explicit Output Variable Index OI.3 Abaqus/CFD Output Variable Index 6.1.1 6.1.2 6.1.3 6.1.4 6.1.5 6.1.6 6.2.1 6.2.2 6.2.3 6.2.4 6.2.5 6.2.6 6.2.7 6.3.1 6.3.2 6.3.3 6.3.4 6.3.5 6.3.6 6.3.7 6.3.8 6.3.9 6.3.10 6.3.11 6.4.1 6.5.1 6.5.2 Volume II PART III ANALYSIS PROCEDURES, SOLUTION, AND CONTROL 6. Analysis Procedures Introduction Solving analysis problems: overview Defining an analysis General and linear perturbation procedures Multiple load case analysis Direct linear equation solver Iterative linear equation solver Static stress/displacement analysis Static stress analysis procedures: overview Static stress analysis Eigenvalue buckling prediction Unstable collapse and postbuckling analysis Quasi-static analysis Direct cyclic analysis Low-cycle fatigue analysis using the direct cyclic approach Dynamic stress/displacement analysis Dynamic analysis procedures: overview Implicit dynamic analysis using direct integration Explicit dynamic analysis Direct-solution steady-state dynamic analysis Natural frequency extraction Complex eigenvalue extraction Transient modal dynamic analysis Mode-based steady-state dynamic analysis Subspace-based steady-state dynamic analysis Response spectrum analysis Random response analysis Steady-state transport analysis Steady-state transport analysis Heat transfer and thermal-stress analysis Heat transfer analysis procedures: overview Uncoupled heat transfer analysis 6.5.4 6.6.1 6.6.2 6.7.1 6.7.2 6.7.3 6.7.4 6.7.5 6.7.6 6.8.1 6.8.2 6.9.1 6.10.1 6.11.1 6.12.1 7.1.1 7.2.1 7.2.2 7.2.3 7.2.4 CONTENTS Fully coupled thermal-stress analysis Adiabatic analysis Fluid dynamic analysis Fluid dynamic analysis procedures: overview Incompressible fluid dynamic analysis Electromagnetic analysis Electromagnetic analysis procedures Piezoelectric analysis Coupled thermal-electrical analysis Fully coupled thermal-electrical-structural analysis Eddy current analysis Magnetostatic analysis Coupled pore fluid flow and stress analysis Coupled pore fluid diffusion and stress analysis Geostatic stress state Mass diffusion analysis Mass diffusion analysis Acoustic and shock analysis Acoustic, shock, and coupled acoustic-structural analysis Abaqus/Aqua analysis Abaqus/Aqua analysis Annealing Annealing procedure 7. Analysis Solution and Control Solving nonlinear problems Solving nonlinear problems Analysis convergence controls Convergence and time integration criteria: overview Commonly used control parameters Convergence criteria for nonlinear problems Time integration accuracy in transient problems ANALYSIS TECHNIQUES 8. Analysis Techniques: Introduction Analysis techniques: overview 9. Analysis Continuation Techniques Restarting an analysis Restarting an analysis Importing and transferring results Transferring results between Abaqus analyses: overview Transferring results between Abaqus/Explicit and Abaqus/Standard Transferring results from one Abaqus/Standard analysis to another Transferring results from one Abaqus/Explicit analysis to another 10. Modeling Abstractions Substructuring Using substructures Defining substructures Submodeling Submodeling: overview Node-based submodeling Surface-based submodeling Generating global matrices Generating matrices CONTENTS 8.1.1 9.1.1 9.2.1 9.2.2 9.2.3 9.2.4 10.1.1 10.1.2 10.2.1 10.2.2 10.2.3 10.3.1 Symmetric model generation, results transfer, and analysis of cyclic symmetry models Symmetric model generation Transferring results from a symmetric mesh or a partial three-dimensional mesh to a full three-dimensional mesh Analysis of models that exhibit cyclic symmetry Periodic media analysis Periodic media analysis Meshed beam cross-sections Meshed beam cross-sections vii 10.4.1 10.4.2 10.4.3 10.5.1 Modeling discontinuities as an enriched feature using the extended finite element method Modeling discontinuities as an enriched feature using the extended finite element 10.7.1 11.1.1 11.2.1 11.3.1 11.4.1 11.4.2 11.4.3 11.5.1 11.5.2 11.5.3 11.5.4 11.6.1 11.7.1 11.8.1 12.1.1 12.2.1 12.2.2 12.2.3 12.2.4 method 11. Special-Purpose Techniques Inertia relief Inertia relief Mesh modification or replacement Element and contact pair removal and reactivation Geometric imperfections Introducing a geometric imperfection into a model Fracture mechanics Fracture mechanics: overview Contour integral evaluation Crack propagation analysis Surface-based fluid modeling Surface-based fluid cavities: overview Fluid cavity definition Fluid exchange definition Inflator definition Mass scaling Mass scaling Selective subcycling Selective subcycling Steady-state detection Steady-state detection 12. Adaptivity Techniques Adaptivity techniques: overview Adaptivity techniques ALE adaptive meshing ALE adaptive meshing: overview Defining ALE adaptive mesh domains in Abaqus/Explicit ALE adaptive meshing and remapping in Abaqus/Explicit Modeling techniques for Eulerian adaptive mesh domains in Abaqus/Explicit 12.2.5 12.2.6 12.2.7 12.3.1 12.3.2 12.3.3 12.4.1 13.1.1 13.2.1 13.2.2 13.2.3 14.1.1 14.1.2 14.1.3 14.1.4 15.1.1 15.1.2 16.1.1 16.1.2 16.1.3 17.1.1 17.2.1 Output and diagnostics for ALE adaptive meshing in Abaqus/Explicit Defining ALE adaptive mesh domains in Abaqus/Standard ALE adaptive meshing and remapping in Abaqus/Standard Adaptive remeshing Adaptive remeshing: overview Selection of error indicators influencing adaptive remeshing Solution-based mesh sizing Analysis continuation after mesh replacement Mesh-to-mesh solution mapping 13. Optimization Techniques Structural optimization: overview Structural optimization: overview Optimization models Design responses Objectives and constraints Creating Abaqus optimization models 14. Eulerian Analysis Eulerian analysis Defining Eulerian boundaries Eulerian mesh motion Defining adaptive mesh refinement in the Eulerian domain 15. Particle Methods Smoothed particle hydrodynamic analyses Smoothed particle hydrodynamic analysis Finite element conversion to SPH particles 16. Sequentially Coupled Multiphysics Analyses Predefined fields for sequential coupling Sequentially coupled thermal-stress analysis Predefined loads for sequential coupling 17. Co-simulation Co-simulation: overview Preparing an Abaqus analysis for co-simulation Preparing an Abaqus analysis for co-simulation Co-simulation between Abaqus solvers Abaqus/Standard to Abaqus/Explicit co-simulation Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation 18. Extending Abaqus Analysis Functionality User subroutines and utilities User subroutines: overview Available user subroutines Available utility routines 19. Design Sensitivity Analysis Design sensitivity analysis 20. Parametric Studies Scripting parametric studies Scripting parametric studies Parametric studies: commands aStudy.combine(): Combine parameter samples for parametric studies. aStudy.constrain(): Constrain parameter value combinations in parametric studies. aStudy.define(): Define parameters for parametric studies. aStudy.execute(): Execute the analysis of parametric study designs. aStudy.gather(): Gather the results of a parametric study. aStudy.generate(): Generate the analysis job data for a parametric study. aStudy.output(): Specify the source of parametric study results. aStudy=ParStudy(): Create a parametric study. aStudy.report(): Report parametric study results. aStudy.sample(): Sample parameters for parametric studies. 17.3.1 17.3.2 18.1.1 18.1.2 18.1.3 19.1.1 20.1.1 20.2.1 20.2.2 20.2.3 20.2.4 20.2.5 20.2.6 20.2.7 20.2.8 20.2.9 20.2.10 21.1.1 21.1.2 21.1.3 21.2.1 22.1.1 22.2.1 22.2.2 22.2.3 22.3.1 22.4.1 22.5.1 22.5.2 22.5.3 22.6.1 22.6.2 22.7.1 22.7.2 Volume III PART V MATERIALS 21. Materials: Introduction Introduction Material library: overview Material data definition Combining material behaviors General properties Density 22. Elastic Mechanical Properties Overview Elastic behavior: overview Linear elasticity Linear elastic behavior No compression or no tension Plane stress orthotropic failure measures Porous elasticity Elastic behavior of porous materials Hypoelasticity Hypoelastic behavior Hyperelasticity Hyperelastic behavior of rubberlike materials Hyperelastic behavior in elastomeric foams Anisotropic hyperelastic behavior Stress softening in elastomers Mullins effect Energy dissipation in elastomeric foams Viscoelasticity Time domain viscoelasticity Frequency domain viscoelasticity Nonlinear viscoelasticity Hysteresis in elastomers Parallel network viscoelastic model Rate sensitive elastomeric foams Low-density foams 23. Inelastic Mechanical Properties Overview Inelastic behavior Metal plasticity Classical metal plasticity Models for metals subjected to cyclic loading Rate-dependent yield Rate-dependent plasticity: creep and swelling Annealing or melting Anisotropic yield/creep Johnson-Cook plasticity Dynamic failure models Porous metal plasticity Cast iron plasticity Two-layer viscoplasticity ORNL – Oak Ridge National Laboratory constitutive model Deformation plasticity Other plasticity models Extended Drucker-Prager models Modified Drucker-Prager/Cap model Mohr-Coulomb plasticity Critical state (clay) plasticity model Crushable foam plasticity models Fabric materials Fabric material behavior Jointed materials Jointed material model Concrete Concrete smeared cracking Cracking model for concrete Concrete damaged plasticity xii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 22.8.1 22.8.2 22.9.1 23.1.1 23.2.1 23.2.2 23.2.3 23.2.4 23.2.5 23.2.6 23.2.7 23.2.8 23.2.9 23.2.10 23.2.11 23.2.12 23.2.13 23.3.1 23.3.2 23.3.3 23.3.4 23.3.5 23.4.1 23.5.1 23.7.1 24.1.1 24.2.1 24.2.2 24.2.3 24.3.1 24.3.2 24.3.3 24.4.1 24.4.2 24.4.3 25.1.1 25.2.1 26.1.1 26.1.2 26.1.3 26.1.4 26.2.1 26.2.2 26.2.3 26.2.4 Permanent set in rubberlike materials Permanent set in rubberlike materials 24. Progressive Damage and Failure Progressive damage and failure: overview Progressive damage and failure Damage and failure for ductile metals Damage and failure for ductile metals: overview Damage initiation for ductile metals Damage evolution and element removal for ductile metals Damage and failure for fiber-reinforced composites Damage and failure for fiber-reinforced composites: overview Damage initiation for fiber-reinforced composites Damage evolution and element removal for fiber-reinforced composites Damage and failure for ductile materials in low-cycle fatigue analysis Damage and failure for ductile materials in low-cycle fatigue analysis: overview Damage initiation for ductile materials in low-cycle fatigue Damage evolution for ductile materials in low-cycle fatigue 25. Hydrodynamic Properties Overview Hydrodynamic behavior: overview Equations of state Equation of state 26. Other Material Properties Mechanical properties Material damping Thermal expansion Field expansion Viscosity Heat transfer properties Thermal properties: overview Conductivity Specific heat Latent heat Acoustic properties Acoustic medium Mass diffusion properties Diffusivity Solubility Electromagnetic properties Electrical conductivity Piezoelectric behavior Magnetic permeability Pore fluid flow properties Pore fluid flow properties Permeability Porous bulk moduli Sorption Swelling gel Moisture swelling User materials User-defined mechanical material behavior User-defined thermal material behavior 26.3.1 26.4.1 26.4.2 26.5.1 26.5.2 26.5.3 26.6.1 26.6.2 26.6.3 26.6.4 26.6.5 26.6.6 26.7.1 26.7.2 27.1.1 27.1.2 27.1.3 27.1.4 28.1.1 28.1.2 28.1.3 28.1.4 28.1.5 28.1.6 28.1.7 28.2.1 28.2.2 28.3.1 28.3.2 28.4.1 28.4.2 28.5.1 28.5.2 29.1.1 29.1.2 29.1.3 Volume IV PART VI ELEMENTS 27. Elements: Introduction Element library: overview Choosing the element’s dimensionality Choosing the appropriate element for an analysis type Section controls 28. Continuum Elements General-purpose continuum elements Solid (continuum) elements One-dimensional solid (link) element library Two-dimensional solid element library Three-dimensional solid element library Cylindrical solid element library Axisymmetric solid element library Axisymmetric solid elements with nonlinear, asymmetric deformation Fluid continuum elements Fluid (continuum) elements Fluid element library Infinite elements Infinite elements Infinite element library Warping elements Warping elements Warping element library Particle elements Particle elements Particle element library 29. Structural Elements Membrane elements Membrane elements General membrane element library Cylindrical membrane element library Axisymmetric membrane element library Truss elements Truss elements Truss element library Beam elements Beam modeling: overview Choosing a beam cross-section Choosing a beam element Beam element cross-section orientation Beam section behavior Using a beam section integrated during the analysis to define the section behavior Using a general beam section to define the section behavior Beam element library Beam cross-section library Frame elements Frame elements Frame section behavior Frame element library Elbow elements Pipes and pipebends with deforming cross-sections: elbow elements Elbow element library Shell elements Shell elements: overview Choosing a shell element Defining the initial geometry of conventional shell elements Shell section behavior Using a shell section integrated during the analysis to define the section behavior Using a general shell section to define the section behavior Three-dimensional conventional shell element library Continuum shell element library Axisymmetric shell element library Axisymmetric shell elements with nonlinear, asymmetric deformation 29.1.4 29.2.1 29.2.2 29.3.1 29.3.2 29.3.3 29.3.4 29.3.5 29.3.6 29.3.7 29.3.8 29.3.9 29.4.1 29.4.2 29.4.3 29.5.1 29.5.2 29.6.1 29.6.2 29.6.3 29.6.4 29.6.5 29.6.6 29.6.7 29.6.8 29.6.9 29.6.10 30.1.1 30.1.2 30.2.1 30.2.2 30.3.1 30.3.2 30.4.1 30.4.2 31.1.1 31.1.2 31.1.3 31.1.4 31.1.5 31.2.1 31.2.2 31.2.3 31.2.4 31.2.5 31.2.6 31.2.7 31.2.8 31.2.9 31.2.10 32.1.1 32.1.2 30. Inertial, Rigid, and Capacitance Elements Point mass elements Point masses Mass element library Rotary inertia elements Rotary inertia Rotary inertia element library Rigid elements Rigid elements Rigid element library Capacitance elements Point capacitance Capacitance element library 31. Connector Elements Connector elements Connectors: overview Connector elements Connector actuation Connector element library Connection-type library Connector element behavior Connector behavior Connector elastic behavior Connector damping behavior Connector functions for coupled behavior Connector friction behavior Connector plastic behavior Connector damage behavior Connector stops and locks Connector failure behavior Connector uniaxial behavior 32. Special-Purpose Elements Spring elements Springs Spring element library Dashpot elements Dashpots Dashpot element library Flexible joint elements Flexible joint element Flexible joint element library Distributing coupling elements Distributing coupling elements Distributing coupling element library Cohesive elements Cohesive elements: overview Choosing a cohesive element Modeling with cohesive elements Defining the cohesive element’s initial geometry Defining the constitutive response of cohesive elements using a continuum approach Defining the constitutive response of cohesive elements using a traction-separation description Defining the constitutive response of fluid within the cohesive element gap Two-dimensional cohesive element library Three-dimensional cohesive element library Axisymmetric cohesive element library Gasket elements Gasket elements: overview Choosing a gasket element Including gasket elements in a model Defining the gasket element’s initial geometry Defining the gasket behavior using a material model Defining the gasket behavior directly using a gasket behavior model Two-dimensional gasket element library Three-dimensional gasket element library Axisymmetric gasket element library Surface elements Surface elements General surface element library Cylindrical surface element library Axisymmetric surface element library 32.2.1 32.2.2 32.3.1 32.3.2 32.4.1 32.4.2 32.5.1 32.5.2 32.5.3 32.5.4 32.5.5 32.5.6 32.5.7 32.5.8 32.5.9 32.5.10 32.6.1 32.6.2 32.6.3 32.6.4 32.6.5 32.6.6 32.6.7 32.6.8 32.6.9 32.7.1 32.7.2 32.7.3 32.7.4 32.8.1 32.8.2 32.9.1 32.9.2 32.10.1 32.10.2 32.11.1 32.11.2 32.12.1 32.12.2 32.13.1 32.13.2 32.14.1 32.14.2 32.15.1 32.15.2 Tube support elements Tube support elements Tube support element library Line spring elements Line spring elements for modeling part-through cracks in shells Line spring element library Elastic-plastic joints Elastic-plastic joints Elastic-plastic joint element library Drag chain elements Drag chains Drag chain element library Pipe-soil elements Pipe-soil interaction elements Pipe-soil interaction element library Acoustic interface elements Acoustic interface elements Acoustic interface element library Eulerian elements Eulerian elements Eulerian element library User-defined elements User-defined elements User-defined element library EI.1 Abaqus/Standard Element Index EI.2 Abaqus/Explicit Element Index EI.3 Abaqus/CFD Element Index Volume V PART VII PRESCRIBED CONDITIONS 33. Prescribed Conditions Overview Prescribed conditions: overview Amplitude curves Initial conditions Initial conditions in Abaqus/Standard and Abaqus/Explicit Initial conditions in Abaqus/CFD Boundary conditions Boundary conditions in Abaqus/Standard and Abaqus/Explicit Boundary conditions in Abaqus/CFD Loads Applying loads: overview Concentrated loads Distributed loads Thermal loads Electromagnetic loads Acoustic and shock loads Pore fluid flow Prescribed assembly loads Prescribed assembly loads Predefined fields Predefined fields PART VIII CONSTRAINTS 34. Constraints Overview Kinematic constraints: overview Multi-point constraints Linear constraint equations xx Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 33.1.1 33.1.2 33.2.1 33.2.2 33.3.1 33.3.2 33.4.1 33.4.2 33.4.3 33.4.4 33.4.5 33.4.6 33.4.7 33.5.1 34.2.2 34.2.3 34.3.1 34.3.2 34.3.3 34.3.4 34.4.1 34.5.1 34.6.1 35.1.1 35.2.1 35.2.2 35.2.3 35.2.4 35.2.5 35.2.6 35.3.1 35.3.2 35.3.3 35.3.4 35.3.5 35.3.6 35.3.7 35.3.8 General multi-point constraints Kinematic coupling constraints Surface-based constraints Mesh tie constraints Coupling constraints Shell-to-solid coupling Mesh-independent fasteners Embedded elements Embedded elements Element end release Element end release Overconstraint checks Overconstraint checks PART IX INTERACTIONS 35. Defining Contact Interactions Overview Contact interaction analysis: overview Defining general contact in Abaqus/Standard Defining general contact interactions in Abaqus/Standard Surface properties for general contact in Abaqus/Standard Contact properties for general contact in Abaqus/Standard Controlling initial contact status in Abaqus/Standard Stabilization for general contact in Abaqus/Standard Numerical controls for general contact in Abaqus/Standard Defining contact pairs in Abaqus/Standard Defining contact pairs in Abaqus/Standard Assigning surface properties for contact pairs in Abaqus/Standard Assigning contact properties for contact pairs in Abaqus/Standard Modeling contact interference fits in Abaqus/Standard Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs Adjusting contact controls in Abaqus/Standard Defining tied contact in Abaqus/Standard Extending master surfaces and slide lines Contact modeling if substructures are present Contact modeling if asymmetric-axisymmetric elements are present Defining general contact in Abaqus/Explicit Defining general contact interactions in Abaqus/Explicit Assigning surface properties for general contact in Abaqus/Explicit Assigning contact properties for general contact in Abaqus/Explicit Controlling initial contact status for general contact in Abaqus/Explicit Contact controls for general contact in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit Defining contact pairs in Abaqus/Explicit Assigning surface properties for contact pairs in Abaqus/Explicit Assigning contact properties for contact pairs in Abaqus/Explicit Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit Contact controls for contact pairs in Abaqus/Explicit 36. Contact Property Models Mechanical contact properties Mechanical contact properties: overview Contact pressure-overclosure relationships Contact damping Contact blockage Frictional behavior User-defined interfacial constitutive behavior Pressure penetration loading Interaction of debonded surfaces Breakable bonds Surface-based cohesive behavior Thermal contact properties Thermal contact properties Electrical contact properties Electrical contact properties Pore fluid contact properties Pore fluid contact properties 37. Contact Formulations and Numerical Methods Contact formulations and numerical methods in Abaqus/Standard Contact formulations in Abaqus/Standard xxii Abaqus ID:usb-toc Printed on: Fri February 3 -- 18:01:12 2012 35.3.9 35.3.10 35.4.1 35.4.2 35.4.3 35.4.4 35.4.5 35.5.1 35.5.2 35.5.3 35.5.4 35.5.5 36.1.1 36.1.2 36.1.3 36.1.4 36.1.5 36.1.6 36.1.7 36.1.8 36.1.9 36.1.10 36.2.1 37.1.2 37.1.3 37.2.1 37.2.2 37.2.3 38.1.1 38.1.2 38.2.1 38.2.2 39.1.1 39.2.1 39.2.2 39.3.1 39.3.2 39.4.1 39.4.2 39.5.1 39.5.2 40.1.1 Contact constraint enforcement methods in Abaqus/Standard Smoothing contact surfaces in Abaqus/Standard Contact formulations and numerical methods in Abaqus/Explicit Contact formulation for general contact in Abaqus/Explicit Contact formulations for contact pairs in Abaqus/Explicit Contact constraint enforcement methods in Abaqus/Explicit 38. Contact Difficulties and Diagnostics Resolving contact difficulties in Abaqus/Standard Contact diagnostics in an Abaqus/Standard analysis Common difficulties associated with contact modeling in Abaqus/Standard Resolving contact difficulties in Abaqus/Explicit Contact diagnostics in an Abaqus/Explicit analysis Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit 39. Contact Elements in Abaqus/Standard Contact modeling with elements Contact modeling with elements Gap contact elements Gap contact elements Gap element library Tube-to-tube contact elements Tube-to-tube contact elements Tube-to-tube contact element library Slide line contact elements Slide line contact elements Axisymmetric slide line element library Rigid surface contact elements Rigid surface contact elements Axisymmetric rigid surface contact element library 40. Defining Cavity Radiation in Abaqus/Standard Cavity radiation Printed on: • Chapter 27, “Elements: Introduction” • Chapter 28, “Continuum Elements” • Chapter 29, “Structural Elements” • Chapter 30, “Inertial, Rigid, and Capacitance Elements” • Chapter 31, “Connector Elements” 27. Elements: Introduction Introduction 27.1 Introduction • “Element library: overview,” Section 27.1.1 • “Choosing the element’s dimensionality,” Section 27.1.2 • “Choosing the appropriate element for an analysis type,” Section 27.1.3 • “Section controls,” Section 27.1.4 27.1.1 ELEMENT LIBRARY: OVERVIEW Abaqus has an extensive element library to provide a powerful set of tools for solving many different problems. Characterizing elements Five aspects of an element characterize its behavior: • Family • Degrees of freedom (directly related to the element family) • Number of nodes • Formulation • Integration Each element in Abaqus has a unique name, such as T2D2, S4R, C3D8I, or C3D8R. The element name identifies each of the five aspects of an element. For details on defining elements, see “Element definition,” Section 2.2.1. Family Figure 27.1.1–1 shows the element families that are used most commonly in a stress analysis; in addition, continuum (fluid) elements are used in a fluid analysis. One of the major distinctions between different element families is the geometry type that each family assumes. Continuum (solid and fluid) elements Shell elements Beam elements Rigid elements Membrane elements Infinite elements Connector elements such as springs and dashpots Truss elements Figure 27.1.1–1 Commonly used element families. The first letter or letters of an element’s name indicate to which family the element belongs. For example, S4R is a shell element, CINPE4 is an infinite element, and C3D8I is a continuum element. Degrees of freedom The degrees of freedom are the fundamental variables calculated during the analysis. For a stress/displacement simulation the degrees of freedom are the translations and, for shell, pipe, and beam elements, the rotations at each node. For a heat transfer simulation the degrees of freedom are the temperatures at each node; for a coupled thermal-stress analysis temperature degrees of freedom exist in addition to displacement degrees of freedom at each node. Heat transfer analyses and coupled thermal-stress analyses therefore require the use of different elements than does a stress analysis since the degrees of freedom are not the same. See “Conventions,” Section 1.2.2, for a summary of the degrees of freedom available in Abaqus for various element and analysis types. Number of nodes and order of interpolation Displacements or other degrees of freedom are calculated at the nodes of the element. At any other point in the element, the displacements are obtained by interpolating from the nodal displacements. Usually the interpolation order is determined by the number of nodes used in the element. • Elements that have nodes only at their corners, such as the 8-node brick shown in Figure 27.1.1–2(a), use linear interpolation in each direction and are often called linear elements or first-order elements. • In Abaqus/Standard elements with midside nodes, such as the 20-node brick shown in Figure 27.1.1–2(b), use quadratic interpolation and are often called quadratic elements or second-order elements. • Modified triangular or tetrahedral elements with midside nodes, such as the 10-node tetrahedron shown in Figure 27.1.1–2(c), use a modified second-order interpolation and are often called modified or modified second-order elements. (a) Linear element (8-node brick, C3D8) (b) Quadratic element (20-node brick, C3D20) (c) Modified second-order element (10-node tetrahedron, C3D10M) Figure 27.1.1–2 Linear brick, quadratic brick, and modified tetrahedral elements. Typically, the number of nodes in an element is clearly identified in its name. The 8-node brick element is called C3D8, and the 4-node shell element is called S4R. The beam element family uses a slightly different convention: the order of interpolation is identified in the name. Thus, a first-order, three-dimensional beam element is called B31, whereas a second-order, three-dimensional beam element is called B32. A similar convention is used for axisymmetric shell and membrane elements. Formulation An element’s formulation refers to the mathematical theory used to define the element’s behavior. In the Lagrangian, or material, description of behavior the element deforms with the material. In the alternative Eulerian, or spatial, description elements are fixed in space as the material flows through them. Eulerian methods are used commonly in fluid mechanics simulations. Abaqus/Standard uses Eulerian elements to model convective heat transfer. Abaqus/Explicit also offers multimaterial Eulerian elements for use in stress/displacement analyses. Adaptive meshing in Abaqus/Explicit combines the features of pure Lagrangian and Eulerian analyses and allows the motion of the element to be independent of the material . All other stress/displacement elements in Abaqus are based on the Lagrangian formulation. In Abaqus/Explicit the Eulerian elements can interact with Lagrangian elements through general contact . To accommodate different types of behavior, some element families in Abaqus include elements with several different formulations. For example, the conventional shell element family has three classes: one suitable for general-purpose shell analysis, another for thin shells, and yet another for thick shells. In addition, Abaqus also offers continuum shell elements, which have nodal connectivities like continuum elements but are formulated to model shell behavior with as few as one element through the shell thickness. Some Abaqus/Standard element families have a standard formulation as well as some alternative formulations. Elements with alternative formulations are identified by an additional character at the end of the element name. For example, the continuum, beam, and truss element families include members with a hybrid formulation (to deal with incompressible or inextensible behavior); these elements are identified by the letter H at the end of the name (C3D8H or B31H). Abaqus/Standard uses the lumped mass formulation for low-order elements; Abaqus/Explicit uses the lumped mass formulation for all elements. As a consequence, the second mass moments of inertia can deviate from the theoretical values, especially for coarse meshes. Abaqus/CFD uses hybrid elements to circumvent well known div-stability issues for incompressible flow. Abaqus/CFD also permits the addition of degrees of freedom based on procedure settings such as the optional energy equation and turbulence models. Integration Abaqus uses numerical techniques to integrate various quantities over the volume of each element, thus allowing complete generality in material behavior. Using Gaussian quadrature for most elements, Abaqus evaluates the material response at each integration point in each element. Some continuum elements in Abaqus can use full or reduced integration, a choice that can have a significant effect on the accuracy of the element for a given problem. Abaqus uses the letter R at the end of the element name to label reduced-integration elements. For example, CAX4R is the 4-node, reduced-integration, axisymmetric, solid element. Shell, pipe, and beam element properties can be defined as general section behaviors; or each cross- section of the element can be integrated numerically, so that nonlinear response associated with nonlinear material behavior can be tracked accurately when needed. In addition, a composite layered section can be specified for shells and, in Abaqus/Standard, three-dimensional bricks, with different materials for each layer through the section. Combining elements The element library is intended to provide a complete modeling capability for all geometries. Thus, any combination of elements can be used to make up the model; multi-point constraints (“General multi-point constraints,” Section 34.2.2) are sometimes helpful in applying the necessary kinematic relations to form the model (for example, to model part of a shell surface with solid elements and part with shell elements or to use a beam element as a shell stiffener). Heat transfer and thermal-stress analysis In cases where heat transfer analysis is to be followed by thermal-stress analysis, corresponding heat transfer and stress elements are provided in Abaqus/Standard. See “Sequentially coupled thermal-stress analysis,” Section 16.1.2, for additional details. Information available for element libraries The complete element library in Abaqus is subdivided into a number of smaller libraries. Each library is presented as a separate section in this manual. In each of these sections, information regarding the following topics is provided where applicable: • conventions; • element types; • degrees of freedom; • nodal coordinates required; • element property definition; • element faces; • element output; • loading (general loading, distributed loads, foundations, distributed heat fluxes, film conditions, radiation types, distributed flows, distributed impedances, electrical fluxes, distributed electric current densities, and distributed concentration fluxes); • nodes associated with the element; • node ordering and face ordering on elements; and • numbering of integration points for output. For element libraries that are available in both Abaqus/Standard and Abaqus/Explicit, individual element or load types that are available only in Abaqus/Standard are designated with an (S) ; similarly, individual element or load types that are available only in Abaqus/Explicit are designated with an (E) . Element or load types that are available in Abaqus/Aqua are designated with an (A) . Most of the element output variables available for an element are discussed. Additional variables may be available depending on the material model or the analysis procedure that is used. Some elements have solution variables that do not pertain to other elements of the same type; these variables are specified explicitly. 27.1.2 CHOOSING THE ELEMENT’S DIMENSIONALITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Element library: overview,” Section 27.1.1 • “Part modeling space,” Section 11.4.1 of the Abaqus/CAE User’s Manual • “Assigning Abaqus element types,” Section 17.5 of the Abaqus/CAE User’s Manual Overview The Abaqus element library contains the following for modeling a wide range of spatial dimensionality: • one-dimensional elements; • two-dimensional elements; • three-dimensional elements; • cylindrical elements; • axisymmetric elements; and • axisymmetric elements with nonlinear, asymmetric deformation. One-dimensional (link) elements One-dimensional heat transfer, coupled thermal/electrical, and acoustic elements are available only in Abaqus/Standard. In addition, structural link (truss) elements are available in both Abaqus/Standard and Abaqus/Explicit. These elements can be used in two- or three-dimensional space to transmit loads or fluxes along the length of the element. Two-dimensional elements Abaqus provides several different types of two-dimensional elements. For structural applications these include plane stress elements and plane strain elements. Abaqus/Standard also provides generalized plane strain elements for structural applications. Plane stress elements Plane stress elements can be used when the thickness of a body or domain is small relative to its lateral (in-plane) dimensions. The stresses are functions of planar coordinates alone, and the out-of-plane normal and shear stresses are equal to zero. Plane stress elements must be defined in the X–Y plane, and all loading and deformation are also restricted to this plane. This modeling method generally applies to thin, flat bodies. For anisotropic materials the Z-axis must be a principal material direction. Plane strain elements Plane strain elements can be used when it can be assumed that the strains in a loaded body or domain are functions of planar coordinates alone and the out-of-plane normal and shear strains are equal to zero. Plane strain elements must be defined in the X–Y plane, and all loading and deformation are also restricted to this plane. This modeling method is generally used for bodies that are very thick relative to their lateral dimensions, such as shafts, concrete dams, or walls. Plane strain theory might also apply to a typical slice of an underground tunnel that lies along the Z-axis. For anisotropic materials the Z-axis must be a principal material direction. Since plane strain theory assumes zero strain in the thickness direction, isotropic thermal expansion may cause large stresses in the thickness direction. Generalized plane strain elements Generalized plane strain elements provide for the modeling of cases in Abaqus/Standard where the structure has constant curvature (and, hence, no gradients of solution variables) with respect to one material direction—the “axial” direction of the model. The formulation, thus, involves a model that lies between two planes that can move with respect to each other and, hence, cause strain in the axial direction of the model that varies linearly with respect to position in the planes, the variation being due to the change in curvature. In the initial configuration the bounding planes can be parallel or at an angle to each other, the latter case allowing the modeling of initial curvature of the model in the axial direction. The concept is illustrated in Figure 27.1.2–1. Generalized plane strain elements are typically used to model a section of a long structure that is free to expand axially or is subjected to axial loading. Each generalized plane strain element has three, four, six, or eight conventional nodes, at each of which x- and y-coordinates, displacements, etc. are stored. These nodes determine the position and motion of the element in the two bounding planes. Each element also has a reference node, which is usually the same node for all of the generalized plane strain elements in the model. The reference node of a generalized plane strain element should not be used as a conventional node in any element in the model. The reference node has three degrees of freedom 3, 4, and 5: ( ). The first degree of freedom ( ) is the change in length of the axial material fiber connecting this node and its image in the other bounding plane. This displacement is positive as the planes move apart; therefore, there is a tensile strain in the axial fiber. The second and third degrees of freedom ( ) are the components of the relative rotation of one bounding plane with respect to the other. The values stored are the two components of rotation about the X- and Y-axes in the bounding planes (that is, in the cross-section of the model). Positive rotation about the X-axis causes increasing axial strain with respect to the y-coordinate in the cross-section; positive rotation about the Y-axis causes decreasing axial strain with respect to the x-coordinate in the cross-section. The x- and y-coordinates of a generalized plane strain element reference node ( discussed below) remain fixed throughout all steps of an analysis. From the degrees of freedom of the reference node, the length of the axial material fiber passing through the point with current coordinates (x, y) in a bounding plane is defined as , and and , , Bounding planes (x,y) (X ,Y ) 0 0 Reference node Conventional element node Length of line through the thickness at (x,y) is t0 + Δuz + Δφ x (y - Y0) - Δφ y (x - X0) where quantities are defined in the text. Figure 27.1.2–1 Generalized plane strain model. where and is the current length of the fiber, is the initial length of the fiber passing through the reference node (given as part of the element section definition), is the displacement at the reference node (stored as degree of freedom 3 at the reference node), are the total values of the components of the angle between the bounding planes (the original values of are given as part of the element section definition—see “Defining the element’s section properties” in “Solid , (continuum) elements,” Section 28.1.1: degrees of freedom 4 and 5 of the reference node), and are the coordinates of the reference node in a bounding plane. the changes in these values are the and The strain in the axial direction is defined immediately from this axial fiber length. The strain components in the cross-section of the model are computed from the displacements of the regular nodes of the elements in the usual way. Since the solution is assumed to be independent of the axial position, there are no transverse shear strains. Three-dimensional elements Three-dimensional elements are defined in the global X, Y, Z space. These elements are used when the geometry and/or the applied loading are too complex for any other element type with fewer spatial dimensions. Cylindrical elements Cylindrical elements are three-dimensional elements defined in the global X, Y, Z space. These elements are used to model bodies with circular or axisymmetric geometry subjected to general, nonaxisymmetric loading. Cylindrical elements are available only in Abaqus/Standard. Cylindrical elements are useful in situations where the expected solution over a relatively large angle is nearly axisymmetric. In this case a very coarse mesh of cylindrical elements is often sufficient. Footprint and steady-state rolling analyses of tires are good examples of where cylindrical elements have distinct advantages over conventional continuum elements . If, however, the expected solution has significant non-axisymmetric components, a finer mesh of cylindrical elements will be needed and it may be more economical to use conventional continuum elements. Axisymmetric elements Axisymmetric elements provide for the modeling of bodies of revolution under axially symmetric loading conditions. A body of revolution is generated by revolving a plane cross-section about an axis (the symmetry axis) and is readily described in cylindrical polar coordinates r, z, and . Figure 27.1.2–2 shows a typical reference cross-section at . The radial and axial coordinates of a point on this cross-section are denoted by r and z, respectively. At , the radial and axial coordinates coincide with the global Cartesian X- and Y-coordinates. Abaqus does not apply boundary conditions automatically to nodes that are located on the symmetry axis in axisymmetric models. If required, you should apply them directly. Radial boundary conditions at nodes located on the z-axis are appropriate for most problems because without them nodes may displace across the symmetry axis, violating the principle of compatibility. However, there are some analyses, such as penetration calculations, where nodes along the symmetry axis should be free to move; boundary conditions should be omitted in these cases. If the loading and material properties are independent of , the solution in any r–z plane completely defines the solution in the body. Consequently, axisymmetric elements can be used to analyze the z (Y) cross-section at θ = 0 i r (X) Figure 27.1.2–2 Reference cross-section and element in an axisymmetric solid. problem by discretizing the reference cross-section at . Figure 27.1.2–2 shows an element of an axisymmetric body. The nodes i, j, k, and l are actually nodal “circles,” and the volume of material associated with the element is that of a body of revolution, as shown in the figure. The value of a prescribed nodal load or reaction force is the total value on the ring; that is, the value integrated around the circumference. Regular axisymmetric elements Regular axisymmetric elements for structural applications allow for only radial and axial loading and have isotropic or orthotropic material properties, with being a principal direction. Any radial displacement in such an element will induce a strain in the circumferential direction (“hoop” strain); and since the displacement must also be purely axisymmetric, there are only four possible nonzero components of strain ( , and ). , , Generalized axisymmetric stress/displacement elements with twist Axisymmetric solid elements with twist are available only in Abaqus/Standard for the analysis of structures that are axially symmetric but can twist about their symmetry axis. This element family is similar to the axisymmetric elements discussed above, except that it allows for a circumferential loading component (which is independent of ) and for general material anisotropy. Under these conditions, there may be displacements in the -direction that vary with r and z but not with . The problem remains axisymmetric because the solution does not vary as a function of so that the deformation of any r–z plane characterizes the deformation in the entire body. Initially the elements define an axisymmetric reference geometry with respect to the r–z plane at , where the r-direction corresponds to the global X-direction and the z-direction corresponds to the global Y-direction. Figure 27.1.2–3 shows an axisymmetric model consisting of two elements. The figure also shows the local cylindrical coordinate system at node 100. Y (z at θ = 0) e z e θ 100 e r φ100 e z e θ 100 e r X (r at θ = 0) (a) (b) Figure 27.1.2–3 Reference and deformed cross-section in an axisymmetric solid with twist. , the axial displacement The motion at a node of an axisymmetric element with twist is described by the radial displacement (in radians) about the z-axis, each of which is constant in the circumferential direction, so that the deformed geometry remains axisymmetric. Figure 27.1.2–3(b) shows the deformed geometry of the reference model shown in Figure 27.1.2–3(a) and the local cylindrical coordinate system at the displaced location of node 100, for a twist , and the twist . The formulation of these elements is discussed in “Axisymmetric elements,” Section 3.2.8 of the Abaqus Theory Manual. Generalized axisymmetric elements with twist cannot be used in contour integral calculations and in dynamic analysis. Elastic foundations are applied only to degrees of freedom and . These elements should not be mixed with three-dimensional elements. Axisymmetric elements with twist and the nodes of these elements should be used with caution within rigid bodies. If the rigid body undergoes large rotations, incorrect results may be obtained. It is recommended that rigid constraints on axisymmetric elements with twist be modeled with kinematic coupling . Stabilization should not be used with these elements if the deformation is dominated by twist, since stabilization is applied only to the in-plane deformation. Axisymmetric elements with nonlinear, asymmetric deformation These elements are intended for the linear or nonlinear analysis of structures that are initially axisymmetric but undergo nonlinear, nonaxisymmetric deformation. They are available only in Abaqus/Standard. The elements use standard isoparametric interpolation in the r–z plane, combined with Fourier interpolation with respect to . The deformation is assumed to be symmetric with respect to the r–z plane at . Up to four Fourier modes are allowed. For more general cases, full three-dimensional modeling or cylindrical element modeling is probably more economical because of the complete coupling between all deformation modes. These elements use a set of nodes in each of several r–z planes: the number of such planes depends on the order N of Fourier interpolation used with respect to , as follows: Number of Fourier modes N Number of nodal planes Nodal plane locations with respect to Each element type is defined by a name such as CAXA8RN (continuum elements) or SAXA1N (shell elements). The number N should be given as the number of Fourier modes to be used with the element (N=1, 2, 3, or 4). For example, element type CAXA8R2 is a quadrilateral in the r–z plane with biquadratic interpolation in this plane and two Fourier modes for interpolation with respect to . The nodal planes associated with various Fourier modes are illustrated in Figure 27.1.2–4. Y (z at θ = 0) e z e θ e r (a) 2π (b) 3π X (r at θ = 0) (c) (d) Figure 27.1.2–4 Nodal planes of a second-order axisymmetric element with nonlinear, asymmetric deformation and (a) 1, (b) 2, (c) 3, or (d) 4 Fourier modes. 27.1.3 CHOOSING THE APPROPRIATE ELEMENT FOR AN ANALYSIS TYPE Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE References • “Element library: overview,” Section 27.1.1 • “Element type assignment,” Section 17.5.3 of the Abaqus/CAE User’s Manual Overview The Abaqus element library contains the following: • stress/displacement elements, including contact elements, connector elements such as springs, and special-purpose elements such as Eulerian elements and surface elements; • pore pressure elements; • coupled temperature-displacement elements; • coupled thermal-electrical-structural elements; • coupled temperature–pore pressure displacement elements; • heat transfer or mass diffusion elements; • forced convection heat transfer elements; • incompressible flow elements; • coupled thermal-electrical elements; • piezoelectric elements; • electromagnetic elements; • acoustic elements; and • user-defined elements. Each of these element types is described below. Within Abaqus/Standard or Abaqus/Explicit, a model can contain elements that are not appropriate for the particular analysis type chosen; such elements will be ignored. However, an Abaqus/Standard model cannot contain elements that are not available in Abaqus/Standard; likewise, an Abaqus/Explicit model cannot contain elements that are not available in Abaqus/Explicit. The same rule applies to Abaqus/CFD. Stress/displacement elements Stress/displacement elements are used in the modeling of linear or complex nonlinear mechanical analyses that possibly involve contact, plasticity, and/or large deformations. Stress/displacement elements can also be used for thermal-stress analysis, where the temperature history can be obtained from a heat transfer analysis carried out with diffusive elements. Analysis types Stress/displacement elements can be used in the following analysis types: • static and quasi-static analysis (“Static stress analysis procedures: overview,” Section 6.2.1); • implicit transient dynamic, explicit transient dynamic, modal dynamic, and steady-state dynamic analysis (“Dynamic analysis procedures: overview,” Section 6.3.1); • “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1; and • “Fracture mechanics: overview,” Section 11.4.1. Active degrees of freedom Stress/displacement elements have only displacement degrees of freedom. Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. See “Conventions,” Choosing a stress/displacement element Stress/displacement elements are available in several different element families. Continuum elements • “Solid (continuum) elements,” Section 28.1.1; and • “Infinite elements,” Section 28.3.1. Structural elements • “Membrane elements,” Section 29.1.1; • “Truss elements,” Section 29.2.1; • “Beam modeling: overview,” Section 29.3.1; • “Frame elements,” Section 29.4.1; • “Pipes and pipebends with deforming cross-sections: elbow elements,” Section 29.5.1; and • “Shell elements: overview,” Section 29.6.1. Rigid elements • “Point masses,” Section 30.1.1; • “Rotary inertia,” Section 30.2.1; and • “Rigid elements,” Section 30.3.1. Connector elements • “Connector elements,” Section 31.1.2; • “Springs,” Section 32.1.1; • “Dashpots,” Section 32.2.1; • “Flexible joint element,” Section 32.3.1; • “Tube support elements,” Section 32.8.1; and • “Drag chains,” Section 32.11.1. Special-purpose elements • “Cohesive elements: overview,” Section 32.5.1; • “Gasket elements: overview,” Section 32.6.1; • “Surface elements,” Section 32.7.1; • “Line spring elements for modeling part-through cracks in shells,” Section 32.9.1; • “Elastic-plastic joints,” Section 32.10.1; and • “Eulerian elements,” Section 32.14.1. Contact elements • “Gap contact elements,” Section 39.2.1; • “Tube-to-tube contact elements,” Section 39.3.1; • “Slide line contact elements,” Section 39.4.1; and • “Rigid surface contact elements,” Section 39.5.1. Pore pressure elements Pore pressure elements are provided in Abaqus/Standard for modeling fully or partially saturated fluid flow through a deforming porous medium. The names of all pore pressure elements include the letter P (pore pressure). These elements cannot be used with hydrostatic fluid elements. Analysis types Pore pressure elements can be used in the following analysis types: • soils analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1); and • geostatic analysis (“Geostatic stress state,” Section 6.8.2). Active degrees of freedom Pore pressure elements have both displacement and pore pressure degrees of freedom. In second-order elements the pore pressure degrees of freedom are active only at the corner nodes. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. Interpolation These elements use either linear- or second-order (quadratic) interpolation for the geometry and displacements in two or three directions. The pore pressure is interpolated linearly from the corner nodes. Curved element edges should be avoided; exact linear spatial pore pressure variations cannot be obtained with curved edges. For output purposes the pore pressure at the midside nodes of second-order elements is determined by linear interpolation from the corner nodes. Choosing a pore pressure element Pore pressure elements are available only in the following element family: • “Solid (continuum) elements,” Section 28.1.1. Coupled temperature-displacement elements Coupled temperature-displacement elements are used in problems for which the stress analysis depends on the temperature solution and the thermal analysis depends on the displacement solution. An example is the heating of a deforming body whose properties are temperature dependent by plastic dissipation or friction. The names of all coupled temperature-displacement elements include the letter T. Analysis types Coupled temperature-displacement elements are for use in fully coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.3). Active degrees of freedom Coupled temperature-displacement elements have both displacement and temperature degrees of freedom. In second-order elements the temperature degrees of freedom are active at the corner nodes. In modified triangle and tetrahedron elements the temperature degrees of freedom are active at every node. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. Interpolation Coupled temperature-displacement elements use either linear or parabolic interpolation for the geometry and displacements. The temperature is always interpolated linearly. In second-order elements curved edges should be avoided; exact linear spatial temperature variations for these elements cannot be obtained with curved edges. For output purposes the temperature at the midside nodes of second-order elements is determined by linear interpolation from the corner nodes. Choosing a coupled temperature-displacement element Coupled temperature-displacement elements are available in the following element families: • “Solid (continuum) elements,” Section 28.1.1; • “Truss elements,” Section 29.2.1; • “Shell elements: overview,” Section 29.6.1; • “Gap contact elements,” Section 39.2.1; and • “Slide line contact elements,” Section 39.4.1. Coupled thermal-electrical-structural elements Coupled thermal-electrical-structural elements are used when a solution for the displacement, electrical potential, and temperature degrees of freedom must be obtained simultaneously. In these types of problems, coupling between the temperature and displacement degrees of freedom arises from temperature-dependent material properties, thermal expansion, and internal heat generation, which is a function of inelastic deformation of the material. The coupling between the temperature and electrical degrees of freedom arises from temperature-dependent electrical conductivity and internal heat generation (Joule heating), which is a function of the electrical current density. The names of the coupled thermal-electrical-structural elements begin with the letter Q. Analysis types Coupled thermal-electrical-structural elements are for use in a fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4). Active degrees of freedom Coupled thermal-electrical-structural elements have displacement, electrical potential, and temperature degrees of freedom. In second-order elements the electrical potential and temperature degrees of freedom are active at the corner nodes. In modified tetrahedron elements the electrical potential and temperature degrees of freedom are active at every node. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. Interpolation Coupled thermal-electrical-structural elements use either linear or parabolic interpolation for the geometry and displacements. The electrical potential and temperature are always interpolated linearly. In second-order elements curved edges should be avoided; exact linear spatial electrical potential and temperature variations for these elements cannot be obtained with curved edges. For output purposes the electrical potential and temperature at the midside nodes of second-order elements are determined by linear interpolation from the corner nodes. Choosing a coupled thermal-electrical-structural element Coupled thermal-electrical-structural elements are available only in the following element family: • “Solid (continuum) elements,” Section 28.1.1; Coupled temperature–pore pressure elements Coupled temperature–pore pressure elements are used in Abaqus/Standard for modeling fully or partially saturated fluid flow through a deforming porous medium in which the stress, fluid pore pressure, and temperature fields are fully coupled to one another. The names of all coupled temperature–pore pressure elements include the letters T and P. These elements cannot be used with hydrostatic fluid elements. Analysis types Coupled temperature–pore pressure elements are for use in fully coupled temperature–pore pressure analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). Active degrees of freedom Coupled temperature–pore pressure elements have displacement, pore pressure, and temperature degrees of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. Interpolation These elements use either linear- or second-order (quadratic) interpolation for the geometry and displacements. The temperature and pore pressure are always interpolated linearly. Choosing a coupled temperature–pore pressure element Coupled temperature–pore pressure elements are available in the following element family: • “Solid (continuum) elements,” Section 28.1.1; Diffusive (heat transfer) elements Diffusive elements are provided in Abaqus/Standard for use in heat transfer analysis (“Uncoupled heat transfer analysis,” Section 6.5.2), where they allow for heat storage (specific heat and latent heat effects) and heat conduction. They provide temperature output that can be used directly as input to the equivalent stress elements. The names of all diffusive heat transfer elements begin with the letter D. Analysis types The diffusive elements can be used in mass diffusion analysis (“Mass diffusion analysis,” Section 6.9.1) as well as in heat transfer analysis. Active degrees of freedom When used for heat transfer analysis, the diffusive elements have only temperature degrees of freedom. When they are used in a mass diffusion analysis, they have normalized concentration, instead of temperature, degrees of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. Interpolation The diffusive elements use either first-order interpolation in one, two, or three dimensions. (linear) interpolation or second-order (quadratic) Choosing a diffusive element Diffusive elements are available in the following element families: • “Solid (continuum) elements,” Section 28.1.1; • “Shell elements: overview,” Section 29.6.1 (these elements cannot be used in a mass diffusion analysis); and • “Gap contact elements,” Section 39.2.1. Forced convection heat transfer elements Forced convection heat transfer elements are provided in Abaqus/Standard to allow for heat storage (specific heat) and heat conduction, as well as the convection of heat by a fluid flowing through the mesh (forced convection). All forced convection heat transfer elements provide temperature output, which can be used directly as input to the equivalent stress elements. The names of all forced convection heat transfer elements begin with the letters DCC. Analysis types transfer analysis,” Section 6.5.2), The forced convection heat transfer elements can be used in heat transfer analyses (“Uncoupled heat including cavity radiation modeling (“Cavity radiation,” Section 40.1.1). The forced convection heat transfer elements can be used together with the diffusive elements. Active degrees of freedom The forced convection heat transfer elements have temperature degrees of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. Interpolation The forced convection heat transfer elements use only first-order (linear) interpolation in one, two, or three dimensions. Choosing a forced convection heat transfer element Forced convection heat transfer elements are available only in the following element family: • “Solid (continuum) elements,” Section 28.1.1. Incompressible flow elements Hybrid elements suitable for incompressible flow are available in Abaqus/CFD. These elements permit the automatic addition of degrees of freedom for the optional energy equation and turbulence models. The names of all fluid elements begin with the letters FC. Analysis types The incompressible flow elements can be used in a variety of flow analyses (“Incompressible fluid dynamic analysis,” Section 6.6.2), including laminar or turbulent flows, heat transfer, and fluid-solid interaction. Active degrees of freedom The incompressible flow elements provide primarily pressure and velocity degrees of freedom. See “Fluid element library,” Section 28.2.2, for more information on the degrees of freedom in Abaqus/CFD. Interpolation The incompressible flow elements use only first-order (linear) interpolation in one, two, or three dimensions. Choosing an incompressible flow element The incompressible flow elements are available only in the following element family: • “Fluid (continuum) elements,” Section 28.2.1. Coupled thermal-electrical elements Coupled thermal-electrical elements are provided in Abaqus/Standard for use in modeling heating that arises when an electrical current flows through a conductor (Joule heating). Analysis types the thermal and electrical problems . temperature-dependent electrical conductivity and the heat generated in the thermal problem by electric conduction. These elements can also be used to perform uncoupled electric conduction analysis in all or part of the model. In such analysis only the electric potential degree of freedom is activated, and all heat transfer effects are ignored. This capability is available by omitting the thermal conductivity from the material definition. The coupled thermal-electrical elements can also be used in heat transfer analysis (“Uncoupled heat transfer analysis,” Section 6.5.2), in which case all electric conduction effects are ignored. This feature is quite useful if a coupled thermal-electrical analysis is followed by a pure heat conduction analysis (such as a welding simulation followed by cool down). The elements cannot be used in any of the stress/displacement analysis procedures. Active degrees of freedom Coupled thermal-electrical elements have both temperature and electrical potential degrees of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. Interpolation Coupled thermal-electrical elements are provided with first- or second-order interpolation of the temperature and electrical potential. Choosing a coupled thermal-electrical element Coupled thermal-electrical elements are available only in the following element family: • “Solid (continuum) elements,” Section 28.1.1. Piezoelectric elements Piezoelectric elements are provided in Abaqus/Standard for problems in which a coupling between the stress and electrical potential (the piezoelectric effect) must be modeled. Analysis types Piezoelectric elements are for use in piezoelectric analysis (“Piezoelectric analysis,” Section 6.7.2). Active degrees of freedom The piezoelectric elements have both displacement and electric potential degrees of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. The piezoelectric effect is discussed further in “Piezoelectric analysis,” Section 6.7.2. Interpolation Piezoelectric elements are available with first- or second-order interpolation of displacement and electrical potential. Choosing a piezoelectric element Piezoelectric elements are available in the following element families: • “Solid (continuum) elements,” Section 28.1.1; and • “Truss elements,” Section 29.2.1. Electromagnetic elements Electromagnetic elements are provided in Abaqus/Standard for problems that require the computation of the magnetic fields (such as a magnetostatic analysis) or for problems in which a coupling between electric and magnetic fields must be modeled (such as an eddy current analysis). Analysis types Electromagnetic elements are for use in magnetostatic and eddy current analyses (“Magnetostatic analysis,” Section 6.7.6, and “Eddy current analysis,” Section 6.7.5). Active degrees of freedom Electromagnetic elements have magnetic vector potential as the degree of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. Magnetostatic analysis is discussed further in “Magnetostatic analysis,” Section 6.7.6, while the electromagnetic coupling that occurs in an eddy current analysis is discussed further in “Eddy current analysis,” Section 6.7.5. Interpolation Electromagnetic elements are available with zero-order element edge–based interpolation of the magnetic vector potential. Choosing an electromagnetic element Electromagnetic elements are available in the following element family: • “Solid (continuum) elements,” Section 28.1.1. Acoustic elements Acoustic elements are used for modeling an acoustic medium undergoing small pressure changes. The solution in the acoustic medium is defined by a single pressure variable. Impedance boundary conditions representing absorbing surfaces or radiation to an infinite exterior are available on the surfaces of these acoustic elements. Acoustic infinite elements, which improve the accuracy of analyses involving exterior domains, and acoustic-structural interface elements, which couple an acoustic medium to a structural model, are also provided. Analysis types Acoustic elements are for use in acoustic and coupled acoustic-structural analysis (“Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1). Active degrees of freedom Acoustic elements have acoustic pressure as a degree of freedom. Coupled acoustic-structural elements also have displacement degrees of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus. Choosing an acoustic element Acoustic elements are available in the following element families: • “Solid (continuum) elements,” Section 28.1.1; • “Infinite elements,” Section 28.3.1; and • “Acoustic interface elements,” Section 32.13.1. The acoustic elements can be used alone but are often used with a structural model in a coupled analysis. “Acoustic interface elements,” Section 32.13.1, describes interface elements that allow this acoustic pressure field to be coupled to the displacements of the surface of the structure. Acoustic elements can also interact with solid elements through the use of surface-based tie constraints; see “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1. Using the same mesh with different analysis or element types You may want to use the same mesh with different analysis or element types. This may occur, for example, if both stress and heat transfer analyses are intended for a particular geometry or if the effect of using either reduced- or full-integration elements is being investigated. Care should be taken when doing this since unexpected error messages may result for one of the two element types if the mesh is distorted. For example, a stress analysis with C3D10 elements may run successfully, but a heat transfer analysis using the same mesh with DC3D10 elements may terminate during the datacheck portion of the analysis with an error message stating that the elements are excessively distorted or have negative volumes. This apparent inconsistency is caused by the different integration locations for the different element types. Such problems can be avoided by ensuring that the mesh is not distorted excessively. 27.1.4 SECTION CONTROLS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • *SECTION CONTROLS • *HOURGLASS STIFFNESS • “Element type assignment,” Section 17.5.3 of the Abaqus/CAE User’s Manual Overview Section controls in Abaqus/Standard: • choose the hourglass control formulation for most first-order elements with reduced integration; • define the distortion control for C3D10I elements; • select the hourglass control scale factors for all elements with reduced integration; and • select the choice of element deletion and the value of maximum degradation for cohesive elements, connector elements, elements with plane stress formulations (plane stress, shell, continuum shell, and membrane elements) with constitutive behavior that includes damage evolution, any element that can be used with damage evolution models for ductile metals, and any element that can be used with the damage evolution law in a low-cycle fatigue analysis. Section controls in Abaqus/Explicit: • choose the hourglass control formulation or scale factors for all elements with reduced integration; • define the distortion control for solid elements; • select the scale factors for the drill stiffness of shell elements or deactivate the drill stiffness for small-strain shell elements S3RS and S4RS; • select an amplitude for ramping of any initial stresses in membrane elements; • select the kinematic formulation for hexahedron solid elements; • select the accuracy order of the formulation for solid and shell elements; • select the scale factors for linear and quadratic bulk viscosity parameters; • select the choice of element deletion and the value of maximum degradation for elements with constitutive behavior that includes damage evolution; and • control many aspects related to a smoothed particle hydrodynamic (SPH) analysis. In Abaqus/CAE section controls are specified when you assign an element type to particular mesh regions and are referred to as element controls. Using section controls In Abaqus/Standard section controls are used to select the enhanced hourglass control formulation for solid, shell, and membrane elements. This formulation provides improved coarse mesh accuracy with slightly higher computational cost and performs better for nonlinear material response at high strain levels when compared with the default total stiffness formulation. Section controls can also be used to select some element formulations that may be relevant for a subsequent Abaqus/Explicit analysis. In Abaqus/Explicit the default formulations for solid, shell, and membrane elements have been chosen to perform satisfactorily on a wide class of quasi-static and explicit dynamic simulations. However, certain formulations give rise to some trade-off between accuracy and performance. Abaqus/Explicit provides section controls to modify these element formulations so that you can optimize these objectives for a specific application. Section controls can also be used in Abaqus/Explicit to specify scale factors for linear and quadratic bulk viscosity parameters. You can also control the initial stresses in membrane elements for applications such as airbags in crash simulations and introduce the initial stresses gradually based on an amplitude definition. In addition, section controls are used to specify the maximum stiffness degradation and to choose the behavior upon complete failure of an element, once the material stiffness is fully degraded, including the removal of failed elements from the mesh. This functionality applies only to elements with a material definition that includes progressive damage . In Abaqus/Standard this functionality is limited to • cohesive elements with a traction-separation constitutive response that includes damage evolution, • any element with a plane stress formulation that can be used with the damage evolution model for fiber-reinforced composites, • any element that can be used with the damage evolution models for ductile metals, • any element that can be used with the damage evolution law in a low-cycle fatigue analysis, and • connector elements with a constitutive response that includes damage evolution. Input File Usage: Use the following option to specify a section controls definition: *SECTION CONTROLS, NAME=name This option is used in conjunction with one or more of the following options to associate the section control definition with an element section definition: *COHESIVE SECTION, CONTROLS=name *CONNECTOR SECTION, CONTROLS=name *EULERIAN SECTION, CONTROLS=name *MEMBRANE SECTION, CONTROLS=name *SHELL GENERAL SECTION, CONTROLS=name *SHELL SECTION, CONTROLS=name *SOLID SECTION, CONTROLS=name You can apply a single section control definition to several element section definitions. Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Element Controls Methods for suppressing hourglass modes The formulation for reduced-integration elements considers only the linearly varying part of the incremental displacement field in the element for the calculation of the increment of physical strain. The remaining part of the nodal incremental displacement field is the hourglass field and can be expressed in terms of hourglass modes. Excitation of these modes may lead to severe mesh distortion, with no stresses resisting the deformation. Similarly, the formulation for element type C3D4H considers in the constraint equations only the constant part of the incremental pressure Lagrange multiplier field. The remaining part of the nodal incremental pressure Lagrange multiplier interpolation is comprised of hourglass modes. Hourglass control attempts to minimize these problems without introducing excessive constraints on the element’s physical response. Several methods are available in Abaqus for suppressing the hourglass modes, as described below. Integral viscoelastic approach in Abaqus/Explicit The integral viscoelastic approach available in Abaqus/Explicit generates more resistance to hourglass forces early in the analysis step where sudden dynamic loading is more probable. Let q be an hourglass mode magnitude and Q be the force (or moment) conjugate to q. The integral viscoelastic approach is defined as , , and that you can define (by default, where K is the hourglass stiffness selected by Abaqus/Explicit, and s is one of up to three scaling factors ). The scale factors are dimensionless scales scales the hourglass stiffnesses related to the in-plane scales the hourglass stiffnesses related to the rotational degrees scales the hourglass stiffness related to the transverse displacement for small- and relate to specific displacement degrees of freedom. For solid and membrane elements all hourglass stiffnesses. For shell elements displacement degrees of freedom, and of freedom. In addition, strain shell elements. The integral viscoelastic form of hourglass control is available for all reduced-integration elements and is the default form in Abaqus/Explicit, except for elements modeled with hyperelastic, hyperfoam, and low-density foam materials. It is the most computationally intensive hourglass control method. It is not supported for Eulerian EC3D8R elements. Input File Usage: *SECTION CONTROLS, NAME=name, HOURGLASS=RELAX STIFFNESS , , Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass control: Relax stiffness, Displacement hourglass scaling factor: , Out-of-plane , Rotational hourglass scaling factor: displacement hourglass scaling factor: Kelvin viscoelastic approach in Abaqus/Explicit The Kelvin-type viscoelastic approach available in Abaqus/Explicit is defined as where K is the linear stiffness and C is the linear viscous coefficient. This general form has pure stiffness and pure viscous hourglass control as limiting cases. When the combination is used, the stiffness term acts to maintain a nominal resistance to hourglassing throughout the simulation and the viscous term generates additional resistance to hourglassing under dynamic loading conditions. Three approaches are provided in Abaqus/Explicit for specifying Kelvin viscoelastic hourglass control. Specifying the pure stiffness approach The pure stiffness form of hourglass control is available for all reduced-integration elements and is recommended for both quasi-static and transient dynamic simulations. Input File Usage: *SECTION CONTROLS, NAME=name, HOURGLASS=STIFFNESS , , Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass control: Stiffness, Displacement hourglass scaling factor: hourglass scaling factor: hourglass scaling factor: , Out-of-plane displacement , Rotational Specifying the pure viscous approach The pure viscous form of hourglass control is available only for solid and membrane elements with reduced integration and is the default form in Abaqus/Explicit for Eulerian EC3D8R elements. It is the most computationally efficient form of hourglass control and has been shown to be effective for high-rate dynamic simulations. However, the pure viscous method is not recommended for low frequency dynamic or quasi-static problems since continuous (static) loading in hourglass modes will result in excessive hourglass deformation due to the lack of any nominal stiffness. Input File Usage: *SECTION CONTROLS, NAME=name, HOURGLASS=VISCOUS , , Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass control: Viscous, Displacement hourglass scaling factor: hourglass scaling factor: hourglass scaling factor: , Out-of-plane displacement , Rotational Specifying a combination of stiffness and viscous hourglass control A linear combination of stiffness and viscous hourglass control is available only for solid and membrane elements with reduced integration. You can specify the blending weight factor ) to scale the stiffness and viscous contributions. Specifying a weight factor equal to 0.0 or 1.0 results in the limiting cases of pure stiffness and pure viscous hourglass control, respectively. The default weight factor is 0.5. ( Input File Usage: *SECTION CONTROLS, NAME=name, HOURGLASS=COMBINED, WEIGHT FACTOR= , , Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass control: Combined, Stiffness-viscous weight factor: factor: displacement hourglass scaling factor: , Rotational hourglass scaling factor: , Displacement hourglass scaling , Out-of-plane Total stiffness approach in Abaqus/Standard The total stiffness approach available in Abaqus/Standard is the default hourglass control approach for all first-order, reduced-integration elements in Abaqus/Standard, except for elements modeled with hyperelastic, hyperfoam, or hysteresis materials. It is the only hourglass control approach available in Abaqus/Standard for S8R5, S9R5, and M3D9R elements and the only hourglass control approach available for the pressure Lagrange multiplier interpolation for C3D4H elements. Hourglass stiffness factors for first-order, reduced-integration elements depend on the shear modulus, while factors for C3D4H elements depend on the bulk modulus. A scale factor can be applied to these stiffness factors to increase or decrease the hourglass stiffness. Let q be an hourglass mode magnitude and Q be the force (moment, pressure, or volumetric flux) conjugate to q. The total stiffness approach for hourglass control in membrane or solid elements or membrane hourglass control in shell elements is defined as is a dimensionless scale factor (by default, where with units of stress; ( direction, and for the pressure Lagrange multiplier interpolation for C3D4H elements is defined as is an hourglass stiffness factor ); is the gradient interpolator used to define constant gradients in the element refers to a is a material coordinate); and V is the element volume. Similarly, the hourglass control where the superscript P refers to an element node, the subscript is a volumetric gradient operator; is a dimensionless scale factor (by default, where and is an hourglass stiffness factor with units of stress for compressible hyperelastic and hyperfoam materials and units of stress compliance for all other materials. The total stiffness approach for bending hourglass control in shell elements is defined as ); where of the shell element, and A is the area of the shell element. is the scale factor (by default, ), is the hourglass stiffness factor, t is the thickness Input File Usage: *SECTION CONTROLS, NAME=name, HOURGLASS=STIFFNESS , , , , , Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass control: Stiffness, Displacement hourglass scaling factor: hourglass scaling factor: , Rotational Default hourglass stiffness values Normally the hourglass control stiffness is defined from the elasticity associated with the material. In most cases, the control stiffness of first-order, reduced-integration elements is based on a typical value of the initial shear modulus of the material, which may, for example, be given as part of the elastic material definition (“Linear elastic behavior,” Section 22.2.1). Similarly, hourglass control stiffness of the reduced-integration pressure and volumetric Lagrange multiplier interpolations of C3D4H elements is based on a typical value of the initial bulk modulus. For an isotropic elastic or hyperelastic material G is the shear modulus. For a nonisotropic elastic material average moduli are used to calculate the hourglass stiffness: for orthotropic elasticity defined by specifying the terms in the elastic stiffness matrix or for anisotropic elasticity and for orthotropic elasticity defined by specifying the engineering constants or for orthotropic elasticity in plane stress If the elastic moduli are dependent on temperature or field variables, the first value in the table is used. The default values for the stiffness factors are defined below. For membrane or solid elements For membrane hourglass control in a shell For control of bending hourglass modes in a shell For a general shell section defined by specifying the equivalent section properties directly, t is defined as and an effective shear modulus for the section is used to calculate the hourglass stiffness: where is the section stiffness matrix. User-defined hourglass stiffness When the initial shear modulus is not defined, you must define the hourglass stiffness parameters; an example is when user subroutine UMAT is used to describe the material behavior of elements with hourglassing modes. In some cases the default value provided for the hourglass control stiffness may not be suitable and you should define the value. In some coupled pore fluid diffusion and stress analyses the prevailing pore pressure in the medium may approach the magnitude of the stiffness of the material skeleton, as measured by constitutive parameters such as the elastic modulus. These cases are expected in some partial saturation evaluations of the wetting of relatively compliant materials such as tissues or cloth. When reduced-integration or modified tetrahedral or triangular elements are used in such analyses, the default choice of the hourglass control stiffness parameter, which is based on a scaling of skeleton material constitutive parameters, may not be adequate to control hourglassing in the presence of large pore pressure fields. An appropriate hourglass control stiffness in these cases should scale with the expected magnitude of pore pressure changes over an element. Input File Usage: Use the following option to specify nondefault values for the hourglass stiffness factors: *HOURGLASS STIFFNESS , , , drilling hourglass scaling factor for shells This option must immediately follow one of the following options: *MEMBRANE SECTION *SHELL GENERAL SECTION *SHELL SECTION *SOLID SECTION Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass stiffness: Specify or for shells Membrane hourglass stiffness: Specify , Bending hourglass stiffness: Specify factor: Specify drilling hourglass scaling factor for shells , and Drilling hourglass scaling Enhanced hourglass control approach in Abaqus/Standard and Abaqus/Explicit The enhanced hourglass control approach available in both Abaqus/Standard and Abaqus/Explicit represents a refinement of the pure stiffness method in which the stiffness coefficients are based on It is the default hourglass control the enhanced assumed strain method; no scale factor is required. approach for hyperelastic, hyperfoam, and low-density foam materials in Abaqus/Explicit and for hyperelastic, hyperfoam, and hysteresis materials in Abaqus/Standard. This method gives more accurate displacement solutions for coarse meshes with linear elastic materials as compared to other hourglass control methods. It also provides increased resistance to hourglassing for nonlinear materials. Although generally beneficial, this may give overly stiff response in problems displaying plastic yielding under bending. In Abaqus/Explicit the enhanced hourglass method will generally predict a much better return to the original configuration for hyperelastic or hyperfoam materials when loading is removed. The enhanced hourglass control approach is compatible between Abaqus/Standard and Abaqus/Explicit. It is recommended that enhanced hourglass control be used for both Abaqus/Standard and Abaqus/Explicit for all import analyses. See “Transferring results between Abaqus/Explicit and Abaqus/Standard,” Section 9.2.2. The enhanced hourglass method is not supported for enriched elements . Specifying the enhanced hourglass control approach The enhanced hourglass control method is available for first-order solid, membrane, and finite-strain shell elements with reduced integration. In Abaqus/Explicit it cannot be used for a hyperelastic or hyperfoam material when adaptive meshing is used on that domain . Input File Usage: *SECTION CONTROLS, NAME=name, HOURGLASS=ENHANCED Any scaling factors specified on the data line following this option will be ignored. Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass control: Enhanced Special considerations for hyperelastic and hyperfoam materials in an adaptive mesh domain in Abaqus/Explicit The enhanced hourglass method cannot be used with elements modeled with hyperelastic or hyperfoam materials that are included in an adaptive mesh domain. Thus, if you decide to use hyperelastic or hyperfoam materials in an adaptive mesh domain, you must specify section controls to choose a different hourglass control approach. The use of adaptive meshing in domains modeled with finite-strain elastic materials is not recommended since better results are generally predicted using the enhanced hourglass method and, for solid elements, element distortion control (discussed below). Therefore, for these materials it is recommended that the analysis be run without adaptive meshing but with enhanced hourglass control. Use in coupled pore pressure analysis When first-order, reduced-integration, or modified tetrahedral or triangular elements are used in coupled pore fluid diffusion and stress analyses or coupled temperature–pore pressure analyses with enhanced hourglass control, the hourglass control stiffness, which is based on skeleton material constitutive parameters, may not be adequate to control hourglassing in the presence of large pore pressure fields. Since enhanced hourglass control does not allow you to change the hourglass control stiffness, it is recommended that total stiffness hourglass control be used in these cases with an appropriate hourglass control stiffness scaled with the expected magnitude of pore pressure changes over an element. Controlling element distortion for crushable materials in Abaqus/Explicit Many analyses with volumetrically compacting materials such as crushable foams see large compressive and shear deformations, especially when the crushable materials are used as energy absorbers between stiff or heavy components. The material behavior for crushable materials usually stiffens significantly under high compression. When a finer mesh is used, the stiffening behavior of the material model is enough to prevent excessive negative element volumes or other excessive distortion from occurring under high compressive loads. However, analyses may fail prematurely when the mesh is coarse relative to strain gradients and the amount of compression. Abaqus/Explicit offers distortion control to prevent solid elements from inverting or distorting excessively for these cases. The constraint method used in Abaqus/Explicit prevents each node on an element from punching inward toward the center of the element past a point where the element would become non-convex. Constraints are enforced by using a penalty approach, and you can control the associated distortion length ratio. Distortion control is available only for solid elements and cannot be used when the elements are included in an adaptive mesh domain. Distortion control is activated by default for elements modeled with hyperelastic, hyperfoam, or low-density foam materials. Using adaptive meshing in a domain modeled with hyperelastic or hyperfoam materials is not recommended since better results are generally predicted using the enhanced hourglass method in combination with element distortion control. However, if you decide to use hyperelastic or hyperfoam materials in an adaptive mesh domain, you must specify section controls to deactivate distortion control. If distortion control is used, the energy dissipated by distortion control can be output upon request . Although developed for analyses of energy absorbing, volumetrically compacting materials, distortion control can be used with any material model. However, care must be used in interpreting results since the distortion control constraints may inhibit legitimate deformation modes and lock up the mesh. Distortion control cannot prevent elements from being distorted due to temporal instabilities, hourglass instabilities, or physically unrealistic deformation. Input File Usage: Use the following option to activate distortion control: *SECTION CONTROLS, NAME=name, DISTORTION CONTROL=YES Use the following option to deactivate distortion control: *SECTION CONTROLS, NAME=name, DISTORTION CONTROL=NO Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Distortion control: Yes or No Controlling the distortion length ratio By default, the constraint penalty forces are applied when the node moves to a point a small offset distance away from the actual plane of constraint. This appears to improve the robustness of the method and limits the reduction of time increment due to severe shortening of the element characteristic length. This offset distance is determined by the distortion length ratio times the initial element characteristic length. The default value of the distortion length ratio, r, is 0.1. You can change the distortion length ratio by specifying a value for r, . Input File Usage: *SECTION CONTROLS, NAME=name, DISTORTION CONTROL=YES, LENGTH RATIO=r Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Distortion control: Yes, Length ratio: r Selecting a scale factor for the drill stiffness in Abaqus/Explicit A drill constraint acts to keep the element nodal rotations in the direction of the shell normal consistent with the average in-plane rotation of the element. Lack of such a constraint can lead to large rotations at these element nodes. Section controls can be used to select a scale factor for the default drill stiffness of an individual element set. Input File Usage: Use the following options to specify a scale factor for the drill stiffness: *SECTION CONTROLS, NAME=name , , , , , , , scale factor for drill stiffness Drill constraint in small strain shell elements S3RS and S4RS in Abaqus/Explicit The formulation of small strain shell elements S3RS and S4RS includes a drill constraint and does so by default. Alternatively, you can deactivate the drill constraint for these elements. The drill constraint is always active for the finite strain conventional shell elements such as S4R, but the default value of the drill stiffness can be scaled as mentioned above. Input File Usage: Use the following option to activate the drill constraint (default): *SECTION CONTROLS, DRILL STIFFNESS=ON Use the following option to deactivate the drill constraint: *SECTION CONTROLS, DRILL STIFFNESS=OFF Ramping of initial stresses in membrane elements in Abaqus/Explicit For applications such as airbags in crash simulations the initial strains (hence, the initial stresses) are introduced into the model through a reference configuration that is different from the initial configuration. Often the components that confine the airbag in the initial configuration are excluded from the numerical model causing motion of the airbag under initial stresses at the beginning of the analysis. Abaqus/Explicit provides a technique to introduce the initial stresses in the membrane elements gradually based on an amplitude definition. This amplitude must be defined with its value starting from zero and reaching a final value of one. The initial stresses will not be applied for the duration that the amplitude stays at zero. Input File Usage: Use both of the following options: *AMPLITUDE, NAME=name *SECTION CONTROLS, RAMP INITIAL STRESS=name Defining the kinematic formulation for hexahedron solid elements The default kinematic formulation for reduced-integration solid elements in Abaqus (and the only kinematic formulation available in Abaqus/Standard) is based on the uniform strain operator and the hourglass shape vectors. Details can be found in “Solid isoparametric quadrilaterals and hexahedra,” Section 3.2.4 of the Abaqus Theory Manual. These kinematic assumptions result in elements that pass the constant strain patch test for a general configuration and give zero strain under large rigid body rotation. However, the formulation is relatively expensive, especially in three dimensions. Abaqus/Explicit offers two alternative kinematic formulations for the C3D8R solid element that can reduce the computational cost. The performance for each kinematic formulation on the patch test and under large rigid body rotation for various element configurations is summarized in Table 27.1.4–1. Suitable applications for each kinematic formulation are summarized in Table 27.1.4–2. Table 27.1.4–1 Element performance for patch test and large rigid body rotations for various element configurations. Element configuration Satisfaction of the three-dimensional patch test Parallelepiped General Zero straining under rigid body rotation Parallelepiped General Kinematic formulation type Average strain Yes Yes Yes Yes Orthogonal Centroid Yes No Yes Yes Yes No Yes No You can specify the kinematic formulation for 8-node brick elements. Default formulation The default average strain formulation of uniform strain and hourglass shape vectors is the only formulation available in Abaqus/Standard. This formulation is recommended for all problems and is Table 27.1.4–2 Different element formulations and their suitable applications. The default formulation is highlighted below. Kinematic formulation Order of accuracy Average strain Second-order Average strain First-order Orthogonal Centroid — — Suitable applications All; recommended for problems involving a large number of revolutions (>5). All; except those involving a large number of revolutions (>5). All; except those involving high confinement, very coarse meshes, or highly distorted elements. Problems with little rigid body rotation and reasonable mesh refinement. particularly well suited for applications exhibiting high confinement, such as closed-die forming and bushing analyses. Input File Usage: *SECTION CONTROLS, KINEMATIC SPLIT=AVERAGE STRAIN Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Kinematic split: Average strain Orthogonal formulation in Abaqus/Explicit A noticeable reduction in computational cost can be obtained by using the orthogonal formulation available in Abaqus/Explicit. This formulation is based on the centroidal strain operator and a slight modification to the hourglass shape vectors. The centroidal strain operator requires three times fewer floating point operations than the uniform strain operator. Elements formulated with an orthogonal kinematic split pass the patch test only for rectangular or parallelepiped element configurations. However, numerical experience has shown that the element converges on the exact solution for general element configurations as the mesh is refined. It also performs well for large rigid body motions. This formulation provides a good balance between computational speed and accuracy. It is recommended for all analyses except those involving highly distorted elements, very coarse meshes, or high confinement. Suitable applications for this formulation include elastic drop testing. Input File Usage: *SECTION CONTROLS, NAME=name, KINEMATIC SPLIT=ORTHOGONAL Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Kinematic split: Orthogonal Centroid formulation in Abaqus/Explicit The fastest formulation available in Abaqus/Explicit is specified by selecting the centroid formulation. The centroid formulation is based on the centroidal strain operator and the hourglass base vectors. Using the hourglass base vectors instead of the hourglass shape vectors reduces hourglass mode computations by a factor of three. However, the hourglass base vectors are not orthogonal to rigid body rotation for general element configurations, so that hourglass strain may be generated with large rigid body rotations with this formulation. This formulation should be used only to improve computational performance on problems that have reasonable mesh refinement and no significant amount of rigid body rotation (e.g., transient flat rolling simulation). Input File Usage: *SECTION CONTROLS, NAME=name, KINEMATIC SPLIT=CENTROID Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Kinematic split: Centroid Choosing the order of accuracy in solid and shell element formulations Abaqus/Standard offers only a second-order accurate formulation for all elements. Abaqus/Explicit offers both first- and second-order accurate formulations for solid and shell elements. First-order accuracy is the default and yields sufficient accuracy for nearly all Abaqus/Explicit problems because of the inherently small time increment size. Second-order accuracy is usually required for analyses with components undergoing a large number of revolutions (>5). For three-dimensional solids the second-order accuracy formulation is available only with the default average strain kinematic formulation. First-order accuracy In Abaqus/Explicit the first-order accurate formulation for solid and shell elements is the default. This formulation is not available in Abaqus/Standard. Input File Usage: *SECTION CONTROLS, NAME=name, SECOND ORDER ACCURACY=NO Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Second-order accuracy: No Second-order accuracy The second-order accurate element formulation is appropriate for problems with a large number of revolutions (>5). This is the only formulation available in Abaqus/Standard. “Simulation of propeller rotation,” Section 2.3.15 of the Abaqus Benchmarks Manual, illustrates the performance of second-order accurate shell and solid elements in Abaqus/Explicit as they undergo about 100 revolutions. *SECTION CONTROLS, NAME=name, SECOND ORDER ACCURACY=YES Input File Usage: Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Second-order accuracy: Yes Selecting scale factors for bulk viscosity in Abaqus/Explicit Bulk viscosity introduces damping associated with volumetric straining. Its purpose is to improve the modeling of high-speed dynamic events. Abaqus/Explicit contains two forms of bulk viscosity, linear and quadratic, which can be defined for the whole model at each step of the analysis, as discussed in “Bulk viscosity” in “Explicit dynamic analysis,” Section 6.3.3. Section controls can be used to select scale factors for the linear and quadratic bulk viscosities of an individual element set. The pressure term generated by bulk viscosity may introduce unexpected results in the volumetric response of highly compressible materials; therefore, it is recommended to suppress bulk viscosity for these materials by specifying scale factors equal to zero. Input File Usage: Use the following options to specify scale factors for the linear and quadratic bulk viscosities: *SECTION CONTROLS, NAME=name , , , scale factor for linear bulk viscosity, scale factor for quadratic bulk viscosity Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Linear bulk viscosity scaling factor or Quadratic bulk viscosity scaling factor Controlling element deletion and maximum degradation for materials with damage evolution Abaqus offers a general capability for modeling progressive damage and failure of materials In Abaqus/Standard this capability is available (“Progressive damage and failure,” Section 24.1.1). only for cohesive elements, connector elements, elements with plane stress formulations (plane stress, shell, continuum shell, and membrane elements), any element that can be used with the damage evolution models for ductile metals, and any element that can be used with the damage evolution law In Abaqus/Explicit this capability is available for all elements with in a low-cycle fatigue analysis. progressive damage behavior except connector elements. Section controls are provided to specify the value of the maximum stiffness degradation, , and whether element deletion occurs when the degradation reaches this level. By default, an element is deleted when it is fully damaged (i.e., ). The choice of element deletion also affects how the damage is applied; details can be found in the following sections: • “Maximum degradation and choice of element removal” in “Damage evolution and element removal for ductile metals,” Section 24.2.3; • “Maximum degradation and choice of element removal in Abaqus/Standard” in “Connector damage behavior,” Section 31.2.7; • “Maximum degradation and choice of element removal” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6; • “Maximum degradation and choice of element removal” in “Damage evolution and element removal for fiber-reinforced composites,” Section 24.3.3; and • “Damage evolution for ductile materials in low-cycle fatigue,” Section 24.4.3. Input File Usage: Use the following option to delete the element from the mesh: *SECTION CONTROLS, ELEMENT DELETION=YES Use the following option to keep the element in the computation: *SECTION CONTROLS, ELEMENT DELETION=NO Use the following option to specify : *SECTION CONTROLS, MAX DEGRADATION= . Abaqus/CAE Usage: Use the following option to control whether completely damaged elements remain in the computation: Mesh module: Mesh→Element Type: Element deletion Use the following option to determine when an element completely damaged: is considered Mesh module: Mesh→Element Type: Max degradation Using viscous regularization with cohesive elements, connector elements, and elements that can be used with the damage evolution models for ductile metals and fiber-reinforced composites in Abaqus/Standard Material models exhibiting softening behavior and stiffness degradation often lead to severe convergence difficulties in implicit analysis programs, such as Abaqus/Standard. A common technique to overcome some of these convergence difficulties is the use of viscous regularization of the constitutive equations, which causes the tangent stiffness matrix of the softening material to be positive for sufficiently small time increments. The traction-separation laws used to describe the constitutive behavior of cohesive elements can be regularized in Abaqus/Standard using viscosity, by permitting stresses to be outside the limits defined by the traction-separation law. The details of the regularization procedure are discussed in “Viscous regularization in Abaqus/Standard” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6. The same technique is also used to regularize the following: • damaged (softening) connector response , • damaged response of elements with plane stress formulations when they are used with the damage model for fiber-reinforced materials , and • damage response of elements used with the damage model for ductile metals . You specify the amount of viscosity to be used for the regularization procedure. By default, no viscosity is included so that no viscous regularization is performed. Input File Usage: *SECTION CONTROLS, VISCOSITY= Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Viscosity Using viscous damping with connector elements in Abaqus/Standard Material failure in connector elements often causes convergence problems in Abaqus/Standard. To avoid such convergence problems, you can introduce viscous damping into the connector components by specifying the value of the damping coefficient as discussed in “Connector failure behavior,” Section 31.2.9. By default, no damping is included. Input File Usage: *SECTION CONTROLS, VISCOSITY= Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Viscosity Using section controls in an import analysis The recommended procedure for doing import analysis is to specify the enhanced hourglass control formulation in the original analysis. Once the section controls have been specified in the original analysis, they cannot be modified in subsequent import analyses. This ensures that the enhanced hourglass control formulation is used in the original as well as import analyses. The default values for other section controls are usually appropriate and should not be changed. For further details on using section controls in an import analysis, see “Transferring results between Abaqus/Explicit and Abaqus/Standard,” Section 9.2.2. Using section controls for flexion-torsion type connector When the third axes of the two local coordinate systems for a flexion-torsion type connector are exactly aligned, a numerical singularity occurs that may lead to convergence difficulties. To avoid this, a small perturbation can be applied to the local coordinate system defined at the second connector node. Input File Usage: Abaqus/CAE Usage: *SECTION CONTROLS, PERTURBATION=small angle You cannot specify a perturbation for flexion-torsion type connectors in Abaqus/CAE. Using section controls for smoothed particle hydrodynamics (SPH) You can control many aspects of the smoothed particle hydrodynamic (SPH) formulation implemented in Abaqus/Explicit. Using section controls for specifying the SPH kernel For a smoothed particle hydrodynamic analysis, you can choose the order of the kernel used for interpolation. For a list of references that discuss the various kernels that can be used, see “Smoothed particle hydrodynamic analysis,” Section 15.1.1. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *SECTION CONTROLS, KERNEL=CUBIC *SECTION CONTROLS, KERNEL=QUADRATIC *SECTION CONTROLS, KERNEL=QUINTIC In Abaqus/CAE you can choose the order of the kernel used for interpolation only in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles. Mesh module: Mesh→Element Type: Conversion to particles: Kernel: Cubic, Quadratic, or Quintic Using section controls for specifying other SPH formulation parameters You can control the way the smoothing length is computed . You can specify the smoothing length (units of length) for precise control of the radius of influence associated with a given particle. Alternatively, you can scale the default smoothing length by specifying a dimensionless smoothing length factor. By default, the smoothing length is kept constant throughout the analysis. You can specify a variable smoothing length that will increase or decrease during the analysis depending on the divergence of the velocity field, which is a measure of compressive or expansive behavior. By default, the maximum number of particles associated internally with a PC3D element cannot exceed 140. You can modify this number; however, a large value leads to larger memory requirements and, in most cases, to a significant degradation in performance. You can specify a mean velocity filtering coefficient that is used for the modified coordinate updates for particles. A zero value for this coefficient (default) leads to the classical SPH method. As discussed in “Smoothed particle hydrodynamic analysis,” Section 15.1.1, a nonzero value for this coefficient leads to the XSPH method. By default, the SPH kernels satisfy the zero-order completeness requirement. A first-order complete corrected (normalized) kernel is also available, which is sometimes referred in the literature as the normalized SPH (NSPH) method. In high-deformation solid mechanics analyses the use of this kernel may lead to more accurate results. Input File Usage: Abaqus/CAE Usage: *SECTION CONTROLS first data line smoothing length, smoothing length factor, flag for variable smoothing length, maximum number of neighboring particles, mean velocity filtering coefficient, flag for corrected kernel In Abaqus/CAE you can only specify section controls for SPH parameters in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles. Using section controls for specifying the control box used for SPH particles You can also control the rectangular region within which the particle search (finding all neighbors for all particles) is performed. By default, a region that is 10% larger in all directions than the overall model initial dimensions and is centered at the geometric center of the model is used. When a particle is outside this box, it behaves like a free-flying point mass and does not contribute to the SPH calculations. If necessary, you can enlarge (or shrink) this rectangular region by specifying the coordinates of two opposite corners (lower left and upper right) of this box. Input File Usage: *SECTION CONTROLS first data line second data line X, Y, and Z-coordinates (lower box corner) and X, Y, and Z-coordinates (upper box corner) Abaqus/CAE Usage: In Abaqus/CAE you can only specify section controls for SPH parameters in Abaqus/Explicit analyses involving the conversion of continuum elements to SPH particles. Using section controls to convert continuum elements to particles Reduced-integration continuum elements can convert to particles if a certain criterion is met, as discussed in “Finite element conversion to SPH particles,” Section 15.1.2. You can specify the number of particles per parent element to be generated. Several criteria to trigger the conversion are available. Input File Usage: Use the following option to prevent finite elements from converting to particles: *SECTION CONTROLS, ELEMENT CONVERSION=NO (default) Use the following option to trigger the conversion of finite elements to particles: *SECTION CONTROLS, ELEMENT CONVERSION=YES Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Conversion to particles: No or Yes Specifying the number of particles generated You specify the number of particles to be generated per isoparametric direction. The number of particles can range from 1 to 7. Input File Usage: *SECTION CONTROLS, ELEMENT CONVERSION=YES first data line second data line third data line number of particles to be generated per isoparametric direction Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Conversion to particles: Yes, PPD: number of particles to be generated per isoparametric direction Specifying a time-based criterion The time-based criterion is primarily intended as a modeling tool to allow all particles to convert from the defined finite element mesh at the same time. Input File Usage: *SECTION CONTROLS, ELEMENT CONVERSION=YES, CONVERSION CRITERION=TIME (default) first data line second data line third data line , time of conversion Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Conversion to particles: Yes, Criterion: Time Specifying a strain-based criterion The strain-based criterion is primarily intended for cases in which you want to use a progressive conversion approach. You specify the maximum principle strain (absolute value) when continuum elements are to convert to SPH particles. Input File Usage: *SECTION CONTROLS, ELEMENT CONVERSION=YES, CONVERSION CRITERION=STRAIN first data line second data line third data line , maximum principle strain (absolute value) Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Conversion to particles: Yes, Criterion: Strain Specifying a stress-based criterion Similar to the strain-based criterion, the stress-based criterion is primarily intended for cases in which you want to use a progressive conversion approach. You specify the maximum principle stress (absolute value) when continuum elements are to convert to SPH particles. Input File Usage: *SECTION CONTROLS, ELEMENT CONVERSION=YES, CONVERSION CRITERION=STRESS first data line second data line third data line , maximum principle stress (absolute value) Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Conversion to particles: Yes, Criterion: Stress Specifying a user subroutine–based criterion The user subroutine–based criterion allows you to implement a user-defined conversion criterion. You can control element conversion during the course of an Abaqus/Explicit analysis through any of the user subroutines that can actively modify state variables associated with a material point, such as VUSDFLD and VUMAT. Input File Usage: Use the following option to trigger a user subroutine–based conversion criterion: *SECTION CONTROLS, ELEMENT CONVERSION=YES, CONVERSION CRITERION=USER (no data lines) Abaqus/CAE Usage: Specifying a user subroutine–based criterion for element conversion is not supported in Abaqus/CAE. Continuum Elements General-purpose continuum elements Fluid continuum elements Infinite elements Warping elements Particle elements CONTINUUM ELEMENTS 28.1 28.2 28.3 28.4 28.1 General-purpose continuum elements • “Solid (continuum) elements,” Section 28.1.1 • “One-dimensional solid (link) element library,” Section 28.1.2 • “Two-dimensional solid element library,” Section 28.1.3 • “Three-dimensional solid element library,” Section 28.1.4 • “Cylindrical solid element library,” Section 28.1.5 • “Axisymmetric solid element library,” Section 28.1.6 • “Axisymmetric solid elements with nonlinear, asymmetric deformation,” Section 28.1.7 28.1.1 SOLID (CONTINUUM) ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Choosing the element’s dimensionality,” Section 27.1.2 • “One-dimensional solid (link) element library,” Section 28.1.2 • “Two-dimensional solid element library,” Section 28.1.3 • “Three-dimensional solid element library,” Section 28.1.4 • “Cylindrical solid element library,” Section 28.1.5 • “Axisymmetric solid element library,” Section 28.1.6 • “Axisymmetric solid elements with nonlinear, asymmetric deformation,” Section 28.1.7 • *SOLID SECTION • *HOURGLASS STIFFNESS • “Creating homogeneous solid sections,” Section 12.13.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating composite solid sections,” Section 12.13.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating electromagnetic solid sections,” Section 12.13.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Assigning a material orientation” in “Assigning a material orientation or rebar reference orientation,” Section 12.15.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Manual Overview Solid (continuum) elements: • are the standard volume elements of Abaqus; • do not include structural elements such as beams, shells, membranes, and trusses; special-purpose elements such as gap elements; or connector elements such as connectors, springs, and dashpots; • can be composed of a single homogeneous material or, in Abaqus/Standard, can include several layers of different materials for the analysis of laminated composite solids; and • are more accurate if not distorted, particularly for quadrilaterals and hexahedra. The triangular and tetrahedral elements are less sensitive to distortion. Typical applications The solid (or continuum) elements in Abaqus can be used for linear analysis and for complex nonlinear analyses involving contact, plasticity, and large deformations. They are available for stress, heat transfer, acoustic, coupled thermal-stress, coupled pore fluid-stress, piezoelectric, magnetostatic, electromagnetic, and coupled thermal-electrical analyses . Choosing an appropriate element There are some differences in the solid element Abaqus/Explicit. Abaqus/Standard solid element library libraries available in Abaqus/Standard and The Abaqus/Standard solid element library includes first-order (linear) interpolation elements and second-order (quadratic) interpolation elements in one, two, or three dimensions. Triangles and quadrilaterals are available in two dimensions; and tetrahedra, triangular prisms, and hexahedra (“bricks”) are provided in three dimensions. Modified second-order triangular and tetrahedral elements are also provided. Curved (parabolic) edges can be used on the quadratic elements but are not recommended for pore pressure or coupled temperature-displacement elements. Cylindrical elements are provided for structures with edges that are initially circular. In addition, reduced-integration, hybrid, and incompatible mode elements are available in Abaqus/Standard. Electromagnetic elements, based on an edge-based interpolation of the magnetic vector potential, are provided both in two and three dimensions. Abaqus/Explicit solid element library The Abaqus/Explicit solid element library includes first-order (linear) interpolation elements and modified second-order interpolation elements in two or three dimensions. Triangular and quadrilateral first-order elements are available in two dimensions; and tetrahedral, triangular prism, and hexahedral (“brick”) first-order elements are available in three dimensions. The modified second-order elements are limited to triangles and tetrahedra. The acoustic elements in Abaqus/Explicit are limited to first-order (linear) interpolations. For incompatible mode elements only three-dimensional elements are available. Various two-dimensional models (plane stress, plane strain, axisymmetric) are available in both Abaqus/Standard and Abaqus/Explicit. See “Choosing the element’s dimensionality,” Section 27.1.2, for details. Given the wide variety of element types available, it is important to select the correct element for a particular application. Choosing an element for a particular analysis can be simplified by full or reduced integration; considering specific element characteristics: first- or second-order; hexahedra/quadrilaterals or tetrahedra/triangles; or normal, hybrid, or incompatible mode formulation. By considering each of these aspects carefully, the best element for a given analysis can be selected. Choosing between first- and second-order elements In first-order plane strain, generalized plane strain, axisymmetric quadrilateral, hexahedral solid elements, and cylindrical elements, the strain operator provides constant volumetric strain throughout the element. This constant strain prevents mesh “locking” when the material response is approximately incompressible . Second-order elements provide higher accuracy in Abaqus/Standard than first-order elements for “smooth” problems that do not involve severe element distortions. They capture stress concentrations more effectively and are better for modeling geometric features: they can model a curved surface with fewer elements. Finally, second-order elements are very effective in bending-dominated problems. First-order triangular and tetrahedral elements should be avoided as much as possible in stress analysis problems; the elements are overly stiff and exhibit slow convergence with mesh refinement, which is especially a problem with first-order tetrahedral elements. If they are required, an extremely fine mesh may be needed to obtain results of sufficient accuracy. Choosing between full- and reduced-integration elements Reduced integration uses a lower-order integration to form the element stiffness. The mass matrix and distributed loadings use full integration. Reduced integration reduces running time, especially in three dimensions. For example, element type C3D20 has 27 integration points, while C3D20R has only 8; therefore, element assembly is roughly 3.5 times more costly for C3D20 than for C3D20R. In Abaqus/Standard you can choose between full or reduced integration for quadrilateral and hexahedral (brick) elements. In Abaqus/Explicit you can choose between full or reduced integration for hexahedral (brick) elements. Only reduced-integration first-order elements are available for quadrilateral elements in Abaqus/Explicit; the elements with reduced integration are also referred to as uniform strain or centroid strain elements with hourglass control. Second-order reduced-integration elements in Abaqus/Standard generally yield more accurate results than the corresponding fully integrated elements. However, for first-order elements the accuracy achieved with full versus reduced integration is largely dependent on the nature of the problem. Hourglassing Hourglassing can be a problem with first-order, reduced-integration elements (CPS4R, CAX4R, C3D8R, etc.) in stress/displacement analyses. Since the elements have only one integration point, it is possible for them to distort in such a way that the strains calculated at the integration point are all zero, which, in turn, leads to uncontrolled distortion of the mesh. First-order, reduced-integration elements in Abaqus include hourglass control, but they should be used with reasonably fine meshes. Hourglassing can also be minimized by distributing point loads and boundary conditions over a number of adjacent nodes. In Abaqus/Standard the second-order reduced-integration elements, with the exception of the 27-node C3D27R and C3D27RH elements, do not have the same difficulty and are recommended in all cases when the solution is expected to be smooth. The C3D27R and C3D27RH elements have three unconstrained, propagating hourglass modes when all 27 nodes are present. These elements should not be used with all 27 nodes, unless they are sufficiently constrained through boundary conditions. First-order elements are recommended when large strains or very high strain gradients are expected. Shear and volumetric locking Fully integrated elements in Abaqus/Standard and Abaqus/Explicit do not hourglass but may suffer from “locking” behavior: both shear and volumetric locking. Shear locking occurs in first-order, fully integrated elements (CPS4, CPE4, C3D8, etc.) that are subjected to bending. The numerical formulation of the elements gives rise to shear strains that do not really exist—the so-called parasitic shear. Therefore, these elements are too stiff in bending, in particular if the element length is of the same order of magnitude as or greater than the wall thickness. See “Performance of continuum and shell elements for linear analysis of bending problems,” Section 2.3.5 of the Abaqus Benchmarks Manual, for further discussion of the bending behavior of solid elements. Volumetric locking occurs in fully integrated elements when the material behavior is (almost) incompressible. Spurious pressure stresses develop at the integration points, causing an element to behave too stiffly for deformations that should cause no volume changes. If materials are almost incompressible (elastic-plastic materials for which the plastic strains are incompressible), second-order, fully integrated elements start to develop volumetric locking when the plastic strains are on the order of the elastic strains. However, the first-order, fully integrated quadrilaterals and hexahedra use selectively reduced integration (reduced integration on the volumetric terms). Therefore, these elements do not lock with almost incompressible materials. Reduced-integration, second-order elements develop volumetric locking for almost incompressible materials only after significant straining occurs. In this case, volumetric locking is often accompanied by a mode that looks like hourglassing. Frequently, this problem can be avoided by refining the mesh in regions of large plastic strain. If volumetric locking is suspected, check the pressure stress at the integration points (printed output). If the pressure values show a checkerboard pattern, changing significantly from one integration point to the next, volumetric locking is occurring. Choosing a quilt-style contour plot in the Visualization module of Abaqus/CAE will show the effect. Specifying nondefault section controls You can specify a nondefault hourglass control formulation or scale factor for reduced-integration first-order elements (4-node quadrilaterals and 8-node bricks with one integration point). See “Section controls,” Section 27.1.4, for more information about section controls. In Abaqus/Explicit section controls can also be used to specify a nondefault kinematic formulation for 8-node brick elements, the accuracy order of the element formulation, and distortion control for either 4-node quadrilateral or 8-node brick elements. Section controls are also used with coupled temperature- displacement elements in Abaqus/Explicit to change the default values for the mechanical response analysis. In Abaqus/Standard you can specify nondefault hourglass stiffness factors based on the default total stiffness approach for reduced-integration first-order elements (4-node quadrilaterals and 8-node bricks with one integration point) and modified tetrahedral and triangular elements. There are no hourglass stiffness factors or scale factors for the nondefault enhanced hourglass control formulation. See “Section controls,” Section 27.1.4, for more information about hourglass control. Input File Usage: Use both of the following options to associate a section control definition with the element section definition: *SECTION CONTROLS, NAME=name *SOLID SECTION, CONTROLS=name Use both of the following options in Abaqus/Standard to specify nondefault hourglass stiffness factors for the total stiffness approach: *SOLID SECTION *HOURGLASS STIFFNESS Abaqus/CAE Usage: Mesh module: Element Type: Element Controls Element Type: Hourglass stiffness: Specify Choosing between bricks/quadrilaterals and tetrahedra/triangles Triangular and tetrahedral elements are geometrically versatile and are used in many automatic meshing algorithms. It is very convenient to mesh a complex shape with triangles or tetrahedra, and the second-order and modified triangular and tetrahedral elements (CPE6, CPE6M, C3D10, C3D10M, etc.) in Abaqus are suitable for general usage. However, a good mesh of hexahedral elements usually provides a solution of equivalent accuracy at less cost. Quadrilaterals and hexahedra have a better convergence rate than triangles and tetrahedra, and sensitivity to mesh orientation in regular meshes is not an issue. However, triangles and tetrahedra are less sensitive to initial element shape, whereas first-order quadrilaterals and hexahedra perform better if their shape is approximately rectangular. The elements become much less accurate when they are initially distorted . First-order triangles and tetrahedra are usually overly stiff, and extremely fine meshes are required to obtain accurate results. As mentioned earlier, fully integrated first-order triangles and tetrahedra in Abaqus/Standard also exhibit volumetric locking in incompressible problems. As a rule, these elements should not be used except as filler elements in noncritical areas. Therefore, try to use well-shaped elements in regions of interest. Tetrahedral and wedge elements For stress/displacement analyses the first-order tetrahedral element C3D4 is a constant stress tetrahedron, which should be avoided as much as possible; the element exhibits slow convergence with mesh refinement. This element provides accurate results only in general cases with very fine meshing. Therefore, C3D4 is recommended only for filling in regions of low stress gradient in meshes of C3D8 or C3D8R elements, when the geometry precludes the use of C3D8 or C3D8R elements throughout the model. For tetrahedral element meshes the second-order or the modified tetrahedral elements, C3D10 or C3D10M, should be used. Similarly, the linear version of the wedge element C3D6 should generally be used only when necessary to complete a mesh, and, even then, the element should be far from any areas where accurate results are needed. This element provides accurate results only with very fine meshing. Modified triangular and tetrahedral elements to regular second-order triangular and tetrahedral elements. A family of modified 6-node triangular and 10-node tetrahedral elements is available that provides improved performance over the first-order triangular and tetrahedral elements and that occasionally provides improved behavior In Abaqus/Explicit these modified triangular and tetrahedral elements are the only 6-node triangular and 10-node tetrahedral elements available. Regular second-order triangular and tetrahedral elements are typically preferable in Abaqus/Standard; however, regular second-order triangular and tetrahedral elements may exhibit “volumetric locking” when incompressibility is approached, such as in problems with a large amount of plastic deformation. As discussed in “Three-dimensional surfaces with second-order faces and a node-to-surface formulation” in “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 38.1.2, regular second-order tetrahedral elements cannot underly a slave surface for the node-to-surface contact formulation with strict enforcement of a “hard” contact relationship. This limitation is typically not significant because the surface-to-surface contact formulation and penalty contact enforcement are generally recommended. Modified triangular and tetrahedral elements work well in contact, exhibit minimal shear and volumetric locking, and are robust during finite deformation . These elements use a lumped matrix formulation for dynamic analysis. Modified triangular elements are provided for planar and axisymmetric analysis, and modified tetrahedra are provided for three-dimensional analysis. In addition, hybrid versions of these elements are provided in Abaqus/Standard for use with incompressible and nearly incompressible constitutive models. When the total stiffness approach is chosen, modified tetrahedral and triangular elements (C3D10M, CPS6M, CAX6M, etc.) use hourglass control associated with their internal degrees of freedom. The hourglass modes in these elements do not usually propagate; hence, the hourglass stiffness is usually not as significant as for first-order elements. For most Abaqus/Standard analysis models the same mesh density appropriate for the regular second-order triangular and tetrahedral elements can be used with the modified elements to achieve similar accuracy. For comparative results, see the following: • “Geometrically nonlinear analysis of a cantilever beam,” Section 2.1.2 of the Abaqus Benchmarks Manual • “Performance of continuum and shell elements for linear analysis of bending problems,” Section 2.3.5 of the Abaqus Benchmarks Manual • “LE1: Plane stress elements—elliptic membrane,” Section 4.2.1 of the Abaqus Benchmarks Manual • “LE10: Thick plate under pressure,” Section 4.2.10 of the Abaqus Benchmarks Manual • “FV32: Cantilevered tapered membrane,” Section 4.4.7 of the Abaqus Benchmarks Manual • “FV52: Simply supported “solid” square plate,” Section 4.4.10 of the Abaqus Benchmarks Manual However, in analyses involving thin bending situations with finite deformations and in frequency analyses where high bending modes need to be captured accurately , the mesh has to be more refined for the modified triangular and tetrahedral elements (by at least one and a half times) to attain accuracy comparable to the regular second- order elements. The modified triangular and tetrahedral elements might not be adequate to be used in the coupled pore fluid diffusion and stress analysis in the presence of large pore pressure fields if enhanced hourglass control is used. The modified elements are more expensive computationally than lower-order quadrilaterals and hexahedron and sometimes require a more refined mesh for the same level of accuracy. However, in Abaqus/Explicit they are provided as an attractive alternative to the lower-order triangles and tetrahedron to take advantage of automatic triangular and tetrahedral mesh generators. Compatibility with other elements The modified triangular and tetrahedral elements are incompatible with the regular second-order solid elements in Abaqus/Standard. Thus, they should not be connected with these elements in a mesh. Surface stress output In areas of high stress gradients, stresses extrapolated from the integration points to the nodes are not as accurate for the modified elements as for similar second-order triangles and tetrahedra in Abaqus/Standard. In cases where more accurate surface stresses are needed, the surface can be coated with membrane elements that have a significantly lower stiffness than the underlying material. The stresses in these membrane elements will then reflect more accurately the surface stress and can be used for output purposes. Fully constrained displacements In Abaqus/Standard if all the displacement degrees of freedom on all the nodes of a modified element are constrained with boundary conditions, a similar boundary condition is applied to an internal node in the element. If a distributed load is subsequently applied to this element, the reported reaction forces at the nodes you defined will not sum up to the applied load since some of the applied load is taken by the internal node whose reaction force is not reported. Choosing between regular and hybrid elements Hybrid elements are intended primarily for use with incompressible and almost incompressible material these elements are available only in Abaqus/Standard. When the material response is behavior; incompressible, the solution to a problem cannot be obtained in terms of the displacement history only, since a purely hydrostatic pressure can be added without changing the displacements. Almost incompressible material behavior Near-incompressible behavior occurs when the bulk modulus is very much larger than the shear modulus (for example, in linear elastic materials where the Poisson’s ratio is greater than .48) and exhibits behavior approaching the incompressible limit: a very small change in displacement produces extremely large changes in pressure. Therefore, a purely displacement-based solution is too sensitive to be useful numerically (for example, computer round-off may cause the method to fail). This singular behavior is removed from the system by treating the pressure stress as an independently interpolated basic solution variable, coupled to the displacement solution through the constitutive theory and the compatibility condition. This independent interpolation of pressure stress is the basis of the hybrid elements. Hybrid elements have more internal variables than their nonhybrid counterparts and are slightly more expensive. See “Hybrid incompressible solid element formulation,” Section 3.2.3 of the Abaqus Theory Manual, for further details. Fully incompressible material behavior Hybrid elements must be used if the material is fully incompressible (except in the case of plane stress since the incompressibility constraint can be satisfied by adjusting the thickness). If the material is almost incompressible and hyperelastic, hybrid elements are still recommended. For almost incompressible, elastic-plastic materials and for compressible materials, hybrid elements offer insufficient advantage and, hence, should not be used. For Mises and Hill plasticity the plastic deformation is fully incompressible; therefore, the rate of total deformation becomes incompressible as the plastic deformation starts to dominate the response. All of the quadrilateral and brick elements in Abaqus/Standard can handle this rate-incompressibility condition except for the fully integrated quadrilateral and brick elements without the hybrid formulation: CPE8, CPEG8, CAX8, CGAX8, and C3D20. These elements will “lock” (become overconstrained) as the material becomes more incompressible. Elastic strains in hybrid elements Hybrid elements use an independent interpolation for the hydrostatic pressure, and the elastic volumetric strain is calculated from the pressure. Hence, the elastic strains agree exactly with the stress, but they agree with the total strain only in an element average sense and not pointwise, even if no inelastic strains are present. For isotropic materials this behavior is noticeable only in second-order, fully integrated hybrid elements. In these elements the hydrostatic pressure (and, thus, the volumetric strain) varies linearly over the element, whereas the total strain may exhibit a quadratic variation. For anisotropic materials this behavior also occurs in first-order, fully integrated hybrid elements. In such materials there is typically a strong coupling between volumetric and deviatoric behavior: volumetric strain will give rise to deviatoric stresses and, conversely, deviatoric strains will give rise to hydrostatic pressure. Hence, the constant hydrostatic pressure enforced in the fully integrated, first-order hybrid elements does not generally yield a constant elastic strain; whereas the total volume strain is always constant for these elements, as discussed earlier in this section. Therefore, hybrid elements are not recommended for use with anisotropic materials unless the material is approximately incompressible, which usually implies that the coupling between deviatoric and volume behavior is relatively weak. Using hybrid elements with material models that exhibit volumetric plasticity If the material model exhibits volumetric plasticity, such as the (capped) Drucker-Prager model, slow convergence or convergence problems may occur if second-order hybrid elements are used. In that case good results can usually be obtained with regular (nonhybrid) second-order elements. Determining the need for hybrid elements For nearly incompressible materials a displaced shape plot that shows a more or less homogeneous but nonphysical pattern of deformation is an indication of mesh locking. As previously discussed, fully integrated elements should be changed to reduced-integration elements in this case. If reduced-integration elements are already being used, the mesh density should be increased. Finally, hybrid elements can be used if problems persist. Hybrid triangular and tetrahedral elements The following hybrid, triangular, two-dimensional and axisymmetric elements should be used only for mesh refinement or to fill in regions of meshes of quadrilateral elements: CPE3H, CPEG3H, CAX3H, and CGAX3H. Hybrid, three-dimensional tetrahedral elements C3D4H and prism elements C3D6H should be used only for mesh refinement or to fill in regions of meshes of brick-type elements. Since each C3D6H element introduces a constraint equation in a fully incompressible problem, a mesh containing only these elements will be overconstrained. Abutting regions of C3D4H elements with different material properties should be tied rather than sharing nodes to allow discontinuity jumps in the pressure and volumetric fields. In addition, the second-order three-dimensional hybrid elements C3D10H, C3D10MH, C3D15H, and C3D15VH are significantly more expensive than their nonhybrid counterparts. Multi-purpose, improved surface stress visualization tetrahedra The C3D10I tetrahedron has been developed for improved bending results in coarse meshes while avoiding pressure locking in metal plasticity and quasi-incompressible and incompressible rubber elasticity. These elements are available only in Abaqus/Standard. Internal pressure degrees of freedom are activated automatically for a given element once the material exhibits behavior approaching the incompressible limit (i.e., an effective Poisson’s ratio above .45). This unique feature of C3D10I elements make it especially suitable for modeling metal plasticity, since it activates the pressure degrees of freedom only in the regions of the model where the material is incompressible. Once the internal degrees of freedom are activated, C3D10I elements have more internal variables than either hybrid or nonhybrid elements and, thus, are more expensive. This element also uses a unique 11-point integration scheme, providing a superior stress visualization scheme in coarse meshes as it avoids errors due to the extrapolation of stress components from the integration points to the nodes. Incompatible mode elements Incompatible mode elements (CPS4I, CPE4I, CAX4I, CPEG4I, and C3D8I and the corresponding hybrid elements) are first-order elements that are enhanced by incompatible modes to improve their bending behavior; all of these elements are available in Abaqus/Standard and only element C3D8I is available in Abaqus/Explicit. In addition to the standard displacement degrees of freedom, incompatible deformation modes are added internally to the elements. The primary effect of these modes is to eliminate the parasitic shear stresses that cause the response of the regular first-order displacement elements to be too stiff in bending. In addition, these modes eliminate the artificial stiffening due to Poisson’s effect in bending (which is manifested in regular displacement elements by a linear variation of the stress perpendicular to the bending direction). In the nonhybrid elements—except for the plane stress element, CPS4I—additional incompatible modes are added to prevent locking of the elements with approximately incompressible material behavior. For fully incompressible material behavior the corresponding hybrid elements must be used. Because of the added internal degrees of freedom due to the incompatible modes (4 for CPS4I; 5 for CPE4I, CAX4I, and CPEG4I; and 13 for C3D8I), these elements are somewhat more expensive than the regular first-order displacement elements; however, they are significantly more economical than second- order elements. The incompatible mode elements use full integration and, thus, have no hourglass modes. in “Continuum elements with Incompatible mode elements are discussed in more detail incompatible modes,” Section 3.2.5 of the Abaqus Theory Manual. Shape considerations The incompatible mode elements perform almost as well as second-order elements in many situations if the elements have an approximately rectangular shape. The performance is reduced considerably if the elements have a parallelogram shape. The performance of trapezoidal-shaped incompatible mode elements is not much better than the performance of the regular, fully integrated, first-order interpolation elements; see “Performance of continuum and shell elements for linear analysis of bending problems,” Section 2.3.5 of the Abaqus Benchmarks Manual, which illustrates the loss of accuracy associated with distorted elements. Using incompatible mode elements in large-strain applications Incompatible mode elements should be used with caution in applications involving large compressive strains. Convergence may be slow at times, and inaccuracies may accumulate in hyperelastic applications. Hence, erroneous residual stresses may sometimes appear in hyperelastic elements that are unloaded after having been subjected to a complex deformation history. Using incompatible mode elements with regular elements Incompatible mode elements can be used in the same mesh with regular solid elements. Generally the incompatible mode elements should be used in regions where bending response must be modeled accurately, and they should be of rectangular shape to provide the most accuracy. While these elements often provide accurate response in such cases, it is generally preferable to use structural elements (shells or beams) to model structural components. Variable node elements Variable node elements (such as C3D27 and C3D15V) allow midface nodes to be introduced on any element face (on any rectangular face only for the triangular prism C3D15V). The choice is made by the nodes specified in the element definition. These elements are available only in Abaqus/Standard and can be used quite generally in any three-dimensional model. The C3D27 family of elements is frequently used as the ring of elements around a crack line. Cylindrical elements Cylindrical elements (CCL9, CCL9H, CCL12, CCL12H, CCL18, CCL18H, CCL24, CCL24H, and CCL24RH) are available only in Abaqus/Standard for precise modeling of regions in a structure with circular geometry, such as a tire. The elements make use of trigonometric functions to interpolate displacements along the circumferential direction and use regular isoparametric interpolation in the radial or cross-sectional plane of the element. All the elements use three nodes along the circumferential direction and can span angles between 0 and 180°. Elements with both first-order and second-order interpolation in the cross-sectional plane are available. The geometry of the element is defined by specifying nodal coordinates in a global Cartesian system. The default nodal output is also provided in a global Cartesian system. Output of stress, strain, and other material point output quantities are done, by default, in a fixed local cylindrical system where direction 1 is the radial direction, direction 2 is the axial direction, and direction 3 is the circumferential direction. This default system is computed from the reference configuration of the element. An alternative local system can be defined . In this case the output of stress, strain, and other material point quantities is done in the oriented system. The cylindrical elements can be used in the same mesh with regular elements. In particular, regular solid elements can be connected directly to the nodes on the cross-sectional plane of cylindrical elements. For example, any face of a C3D8 element can share nodes with the cross-sectional faces (faces 1 and 2; see “Cylindrical solid element library,” Section 28.1.5, for a description of the element faces) of a CCL12 element. Regular elements can also be connected along the circular edges of cylindrical elements by using a surface-based tie constraint (“Mesh tie constraints,” Section 34.3.1) provided that the cylindrical elements do not span a large segment. However, such usage may result in spurious oscillations in the solution near the tied surfaces and should be avoided when an accurate solution in this region is required. Compatible membrane elements (“Membrane elements,” Section 29.1.1) and surface elements with rebar (“Surface elements,” Section 32.7.1) are available for use with cylindrical solid elements. All elements with first-order interpolation in the cross-sectional plane use full integration for the deviatoric terms and reduced integration for the volumetric terms and, thus, have no hourglass modes and do not lock with almost incompressible materials. The hybrid elements with first-order and second-order interpolation in the cross-sectional plane use an independent interpolation for hydrostatic pressure. Summary of recommendations for element usage The following recommendations apply to both Abaqus/Standard and Abaqus/Explicit: • Make all elements as “well shaped” as possible to improve convergence and accuracy. • If an automatic tetrahedral mesh generator is used, use the second-order elements C3D10 (in Abaqus/Standard) or C3D10M (in Abaqus/Explicit). Use the modified tetrahedral element C3D10M in Abaqus/Standard in analyses with large amounts of plastic deformation. • If possible, use hexahedral elements in three-dimensional analyses since they give the best results for the minimum cost. Abaqus/Standard users should also consider the following recommendations: • For linear and “smooth” nonlinear problems use reduced-integration, second-order elements if possible. • Use second-order, fully integrated elements close to stress concentrations to capture the severe gradients in these regions. However, avoid these elements in regions of finite strain if the material response is nearly incompressible. • Use first-order quadrilateral or hexahedral elements or the modified triangular and tetrahedral If the mesh distortion is severe, use elements for problems involving large distortions. reduced-integration, first-order elements. • If the problem involves bending and large distortions, use a fine mesh of first-order, reduced-integration elements. • Hybrid elements must be used if the material is fully incompressible (except when using plane stress elements). Hybrid elements should also be used in some cases with nearly incompressible materials. • Incompatible mode elements can give very accurate results in problems dominated by bending. Naming convention The naming conventions for solid elements depend on the element dimensionality. One-dimensional, two-dimensional, three-dimensional, and axisymmetric elements One-dimensional, two-dimensional, three-dimensional, and axisymmetric solid elements in Abaqus are named as follows: 3D 20 R H T Optional: heat transfer convection/diffusion with dispersion control (D), coupled temperature-displacement (T), piezoelectric (E), or pore pressure (P) hybrid (optional) Optional: reduced integration (R), incompatible mode quad/bricks or improved surface stress formulation tets (I), or modified (M) number of nodes link (1D), plane strain (PE), plane stress (PS), generalized plane strain (PEG), two-dimensional (2D), three-dimensional (3D), axisymmetric (AX), or axisymmetric with twist (GAX) continuum stress/displacement (C), heat transfer or mass diffusion (DC), heat transfer convection/diffusion (DCC), acoustic (AC), electromagnetic (EMC), or coupled thermal-electrical-structural (Q) For example, CAX4R is an axisymmetric continuum stress/displacement, 4-node, reduced-integration element; and CPS8RE is an 8-node, reduced-integration, plane stress piezoelectric element. The exception for this naming convention is C3D6 and C3D6T in Abaqus/Explicit, which are 6-node linear triangular prism, reduced integration elements. The pore pressure elements violate this naming convention slightly: the hybrid elements have the letter H after the letter P. For example, CPE8PH is an 8-node, hybrid, plane strain, pore pressure element. Axisymmetric elements with nonlinear asymmetric deformation The axisymmetric solid elements with nonlinear asymmetric deformation in Abaqus/Standard are named as follows: AXA 8 R H P number of Fourier modes pore pressure (optional) hybrid (optional) reduced integration (optional) number of nodes (in the reference plane) axisymmetric with nonlinear, asymmetric deformation continuum stress/displacement For example, CAXA4RH1 is a 4-node, reduced-integration, hybrid, axisymmetric element with nonlinear asymmetric deformation and one Fourier mode . Cylindrical elements The cylindrical elements in Abaqus/Standard are named as follows: CL 24 R H hybrid (optional) reduced integration (optional) number of nodes cylindrical continuum stress/displacement For example, CCL24RH is a 24-node, hybrid, reduced-integration cylindrical element. Defining the element’s section properties A solid section definition is used to define the section properties of solid elements. In Abaqus/Standard solid elements can be composed of a single homogeneous material or In can include several layers of different materials for the analysis of laminated composite solids. Abaqus/Explicit solid elements can be composed only of a single homogeneous material. Defining homogeneous solid elements You must associate a material definition (“Material data definition,” Section 21.1.2) with the solid section definition. In an Abaqus/Standard analysis spatially varying material behavior defined with one or more distributions (“Distribution definition,” Section 2.8.1) can be assigned to the solid section definition. In addition, you must associate the section definition with a region of your model. In Abaqus/Standard if any of the material behaviors assigned to the solid section definition (through the material definition) are defined with distributions, spatially varying material properties are applied to all elements associated with the solid section. Default material behaviors (as defined by the distributions) are applied to any element that is not specifically included in the associated distribution. Input File Usage: *SOLID SECTION, MATERIAL=name, ELSET=name where the ELSET parameter refers to a set of solid elements. Abaqus/CAE Usage: Property module: Create Section: select Solid as the section Category and Homogeneous or Electromagnetic, Solid as the section Type: Material: name Assign→Section: select regions Assigning an orientation definition You can associate a material orientation definition with solid elements . A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be assigned to the solid section definition. If the orientation definition assigned to the solid section definition is defined with distributions, spatially varying local coordinate systems are applied to all elements associated with the solid section. A default local coordinate system (as defined by the distributions) is applied to any element that is not specifically included in the associated distribution. Input File Usage: Abaqus/CAE Usage: *SOLID SECTION, ORIENTATION=name Property module: Assign→Material Orientation Defining the geometric attributes, if required For some element types additional geometric attributes are required, such as the cross-sectional area for one-dimensional elements or the thickness for two-dimensional plane elements. The attributes required for a particular element type are defined in the solid element libraries. These attributes are given as part of the solid section definition. Defining composite solid elements in Abaqus/Standard The use of composite solids is limited to three-dimensional brick elements that have only displacement degrees of freedom (they are not available for coupled temperature-displacement elements, piezoelectric elements, pore pressure elements, and continuum cylindrical elements). Composite solid elements are primarily intended for modeling convenience. They usually do not provide a more accurate solution than composite shell elements. The thickness, the number of section points required for numerical integration through each layer (discussed below), and the material name and orientation associated with each layer are specified as part of the composite solid section definition. In Abaqus/Standard spatially varying orientation angles can be specified on a layer using distributions (“Distribution definition,” Section 2.8.1). The material layers can be stacked in any of the three isoparametric coordinates, parallel to opposite faces of the isoparametric master element as shown in Figure 28.1.1–1. The number of integration points within a layer at any given section point depends on the element type. Figure 28.1.1–1 shows the integration points for a fully integrated element. stack direction = 1 from face 6 to face 4 stack direction = 2 from face 3 to face 5 stack direction = 3 from face 1 to face 2 face 6 face 1 face 3 Figure 28.1.1–1 Stacking direction and associated element faces and positions of element integration point output variables in the layer plane. The element faces are defined by the order in which the nodes are specified when the element is defined. The element matrices are obtained by numerical integration. Gauss quadrature is used in the plane of the lamina, and Simpson’s rule is used in the stacking direction. If one section point through the layer is used, it will be located in the middle of the layer thickness. The location of the section points in the plane of the lamina coincides with the location of the integration points. The number of section points required for the integration through the thickness of each layer is specified as part of the solid section definition; this number must be an odd number. The integration points for a fully integrated second-order composite element are shown in Figure 28.1.1–1, and the numbering of section points that are associated with an arbitrary integration point in a composite solid element is illustrated in Figure 28.1.1–2. 15 stack direction 11 10 layer 3 layer 2 layer 1 (5 section points per layer) Figure 28.1.1–2 Numbering of section points in a three-layered composite element. The thickness of each layer may not be constant from integration point to integration point within an element since the element dimensions in the stack direction may vary. Therefore, it is defined indirectly by specifying the ratio between the thickness and the element length along the stack direction in the solid section definition, as shown in Figure 28.1.1–3. Using the ratios that are defined for all layers, actual thicknesses will be determined at each integration point such that their sum equals the element length in the stack direction. The thickness ratios for the layers need not reflect actual element or model dimensions. 0.05 0.10 0.05 (a) composite solid section with the material layers stacked in direction 3 0.10 0.20 0.10 layer 3 layer 2 layer 1 stack direction 0.25 0.50 0.25 (b) thickness ratios Figure 28.1.1–3 Lamina in (a) real space and (b) isoparametric space. Unless your model is relatively simple, you will find it increasingly difficult to define your model using composite solid sections as you increase the number of layers and as you assign different sections to different regions. It can also be cumbersome to redefine the sections after you add new layers or remove or reposition existing layers. To manage a large number of layers in a typical composite model, you may want to use the composite layup functionality in Abaqus/CAE. For more information, see Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Manual. Input File Usage: *SOLID SECTION, COMPOSITE, STACK DIRECTION=1, 2, or 3, ELSET=name thickness, number of integration points, material name, orientation name Abaqus/CAE Usage: Abaqus/CAE uses a composite layup or a composite solid section to define the layers of a composite solid. Use the following option for a composite layup: Property module: Create Composite Layup: select Solid as the Element Type: specify stacking direction, regions, thicknesses, number of integration points, materials, and orientations Use the following options for a composite solid section: Property module: Create Section: select Solid as the section Category and Composite as the section Type Assign→Material Orientation: select regions: Use Default Orientation or Other Method: Stacking Direction: Element direction 1, Element direction 2, Element direction 3, or From orientation Assign→Section: select regions Output locations for composite solid elements You specify the location of the output variables in the plane of the lamina (layers) when you request output of element variables. For example, you can request values at the centroid of each layer. In addition, you specify the number of output points through the thickness of the layers by providing a list of the “section points.” The default section points for the output are the first and the last section point corresponding to the bottom and the top face, respectively . See “Element output” in “Output to the data and results files,” Section 4.1.2, and “Element output” in “Output to the output database,” Section 4.1.3, for more information. Modeling thick composites with solid elements in Abaqus/Standard While laminated composite solids are typically modeled using shell elements, the following cases require three-dimensional brick elements with one or multiple brick elements per layer: when transverse shear effects are predominant; when the normal stress cannot be ignored; and when accurate interlaminar stresses are required, such as near localized regions of complex loading or geometry. One case in which shell elements perform somewhat better than solid elements is in modeling the transverse shear stress through the thickness. The transverse shear stresses in solid elements usually do not vanish at the free surfaces of the structure and are usually discontinuous at layer interfaces. This deficiency may be present even if several elements are used in the discretization through the section thickness. Since the transverse shear stresses in thick shell elements are calculated by Abaqus on the basis of linear elasticity theory, such stresses are often better estimated by thick shell elements than by solid elements . Defining pressure loads on continuum elements The convention used for pressure loading on a continuum element is that positive pressure is directed into the element; that is, it pushes on the element. In large-strain analyses special consideration is necessary for plane stress elements that are pressure loaded on their edges; this issue is discussed in “Distributed loads,” Section 33.4.3. Using solid elements in a rigid body All solid elements can be included in a rigid body definition. When solid elements are assigned to a rigid body, they are no longer deformable and their motion is governed by the motion of the rigid body reference node . Section properties for solid elements that are part of a rigid body must be defined to properly account for rigid body mass and rotary inertia. All associated material properties will be ignored except for the density. Element output is not available for solid elements assigned to a rigid body. Automatic conversion of certain element types in Abaqus/Standard Element types C3D20 and C3D15 are converted automatically to the corresponding variable node element types C3D27 and C3D15V, respectively, if they are adjacent to a slave surface in a node-to-surface contact pair with strict enforcement of “hard” contact conditions. Special considerations for various element types in Abaqus/Standard The following considerations should be acknowledged in the context of the stress/displacement, coupled temperature-displacement, and heat transfer elements in Abaqus/Standard. Interpolation of temperature and field variables in stress/displacement elements The value of temperatures at the integration points used to compute the thermal stresses depends on whether first-order or second-order elements are used. An average temperature is used at the integration points in (compatible) linear elements so that the thermal strain is constant throughout the element; in the case of elements with incompatible modes the temperatures are interpolated linearly. An approximate linearly varying temperature distribution is used in higher-order elements with full integration. Higher- order reduced-integration elements pose no special problems since the temperatures are interpolated linearly. Field variables in a given stress/displacement element are interpolated using the same scheme used to interpolate temperatures. Interpolation in coupled temperature-displacement elements Coupled temperature-displacement elements use either linear or parabolic interpolation for the geometry and displacements. Temperature is interpolated linearly, but certain rules can apply to the temperature and field variable evaluation at the Gauss points, as discussed below. The elements that use linear interpolation for displacements and temperatures have temperatures at all nodes. The thermal strain is taken as constant throughout the element because it is desirable to have the same interpolation for thermal strains as for total strains so as to avoid spurious hydrostatic stresses. Separate integration schemes are used for the internal energy storage, heat conduction, and plastic dissipation (coupling contribution) terms for the first-order elements. The internal energy storage term is integrated at the nodes, which yields a lumped internal energy matrix and, thereby, improves the accuracy for problems with latent heat effects. In fully integrated elements both the heat conduction and plastic dissipation terms are integrated at the Gauss points. While the plastic dissipation term is integrated at each Gauss point, the heat generated by the mechanical deformation at a Gauss point is applied at the nearest node. The temperature at a Gauss point is assumed to be the temperature of its nearest node to be consistent with the temperature treatment throughout the formulation. In reduced- integration elements the plastic dissipation term is obtained at the centroid and the heat generated by the mechanical deformation is applied as a weighted average at each node. The temperature at the centroid of reduced-integration elements is a weighted average of the nodal temperatures to be consistent with the temperature treatment throughout the formulation. The elements that use parabolic interpolation for displacements and linear interpolation for temperatures have displacement degrees of freedom at all of the nodes, but temperature degrees of freedom exist only at the corner nodes. The temperatures are interpolated linearly so that the thermal strains have the same interpolation as the total strains. Temperatures at the midside nodes are calculated by linear interpolation from the corner nodes for output purposes only. In contrast to the linear coupled elements, all terms in the governing equations are integrated using a conventional Gauss scheme. For these elements the stiffness matrix can be generated using either full integration (3 Gauss points in each parametric direction) or reduced integration (2 Gauss points in each parametric direction). The same integration scheme is always used for the specific heat and conductivity matrices as for the stiffness matrix; however, because of the lower-order interpolation for temperature, this implies that we always use a full integration scheme for the heat transfer matrices, even when the stiffness integration is reduced. Reduced integration uses a lower-order integration to form the element stiffness: the mass matrix and distributed loadings are still integrated exactly. Reduced integration usually provides more accurate results (providing that the elements are not distorted) and significantly reduces running time, especially in three dimensions. Reduced integration for the quadratic displacement elements is recommended in all cases except when very sharp strain gradients are expected (such as in finite-strain metal forming applications); these elements are considered to be the most cost-effective elements of this class. The value of field variables at the integration points depends on whether first-order or second-order coupled temperature-displacement elements are used. An average field variable is used at the integration points in linear elements. An approximate linearly varying field variable distribution is used in higher- order elements with full integration. Higher-order reduced-integration elements pose no special problems since the field variables are interpolated linearly. Modified triangle and tetrahedron elements use a special consistent interpolation scheme for displacement and temperature. Displacement and temperature degrees of freedom are active at all user-defined nodes. Integration in diffusive heat transfer elements In all of the first-order elements (2-node links, 3-node triangles, 4-node quadrilaterals, 4-node tetrahedra, 6-node triangular prisms, and 8-node bricks) the internal energy storage term (associated with specific heat and latent heat storage) is integrated at the nodes. This integration scheme gives a diagonal internal energy matrix and improves the accuracy for problems with latent heat effects. Conduction contributions in these elements and all contributions in second-order elements use conventional Gauss schemes. Second-order elements are preferable for smooth problems without latent heat effects. The one-dimensional element cannot be used in a mass diffusion analysis. Forced convection heat transfer elements These elements are available with linear interpolation only. They use an “upwinding” (Petrov-Galerkin) method to provide accurate solutions for convection-dominated problems . Consequently, the internal energy (associated with specific heat storage) is not integrated at the nodes, which yields a consistent internal energy matrix and may cause oscillatory temperatures if strong temperature gradients occur along boundaries that are parallel to the flow direction. Electromagnetic elements These elements are available with linear edge-based interpolation only. The user-defined nodes define the geometry of the element but do not directly participate in the interpolation of the electromagnetic or, in the case of a magnetostatic analysis, the magnetic fields. However, temperature and predefined field variables are defined at the user-defined nodes and are interpolated to the integration points for evaluating material properties that are temperature and predefined field variable dependent. 28.1.2 ONE-DIMENSIONAL SOLID (LINK) ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/CAE References • “Solid (continuum) elements,” Section 28.1.1 • *SOLID SECTION Overview This section provides a reference to the one-dimensional solid (link) elements available in Abaqus/Standard. For structural link (truss) elements, refer to “Truss elements,” Section 29.2.1. Element types Diffusive heat transfer elements DC1D2 DC1D3 2-node link 3-node link Active degree of freedom 11 Additional solution variables None. Forced convection heat transfer elements DCC1D2 2-node link DCC1D2D 2-node link with dispersion control Active degree of freedom 11 Additional solution variables None. Coupled thermal-electrical elements DC1D2E DC1D3E 2-node link 3-node link Active degrees of freedom 9, 11 Additional solution variables None. Acoustic elements AC1D2 AC1D3 2-node link 3-node link Active degree of freedom Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition You must provide the cross-sectional area of the element; by default, unit area is assumed. Input File Usage: Abaqus/CAE Usage: *SOLID SECTION Property module: Create Section: select Solid as the section Category and Homogeneous as the section Type Element-based loading Distributed heat fluxes Distributed heat fluxes are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DFLUX) BF BFNU Abaqus/CAE Load/Interaction Units Description Body heat flux Body heat flux JL−3 T−1 JL−3 T−1 Heat body flux per unit volume. Nonuniform heat body flux per unit volume with magnitude supplied via user subroutine DFLUX. Heat surface flux per unit area into the first end of the link (node 1). S1 Surface heat flux JL−2 T−1 Abaqus/CAE Load/Interaction Units Description Surface heat flux JL−2 T−1 Load ID (*DFLUX) S2 S1NU Not supported JL−2 T−1 S2NU Not supported JL−2 T−1 Heat surface flux per unit area into the second end of the link (node 2 or node 3). Nonuniform heat surface flux per unit area into the first end of the link (node 1) with magnitude supplied via user subroutine DFLUX. Nonuniform heat surface flux per unit area into the second end of the link (node 2 or node 3) with magnitude supplied via user subroutine DFLUX. Film conditions Film conditions are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*FILM) Abaqus/CAE Load/Interaction Units Description F1 F2 Not supported JL−2 T−1 −1 Not supported JL−2 T−1 −1 F1NU Not supported JL−2 T−1 −1 F2NU Not supported JL−2 T−1 −1 Film coefficient and sink temperature (units of ) at the first end of the link (node 1). Film coefficient and sink temperature (units of ) at the second end of the link (node 2 or node 3). Nonuniform film coefficient and sink temperature (units of ) at the first end of the link (node 1) with magnitude supplied via user subroutine FILM. Nonuniform film coefficient and sink temperature (units of ) at the second end of the link (node 2 or node 3) with magnitude supplied via user subroutine FILM. Radiation types Radiation conditions are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*RADIATE) Abaqus/CAE Load/Interaction Units Description R1 R2 Surface radiation Dimensionless Surface radiation Dimensionless Emissivity and sink temperature (units of ) at the first end of the link (node 1). Emissivity and sink temperature (units of ) at the second end of the link (node 2 or node 3). Distributed impedances Distributed impedances are available for elements with acoustic pressure degrees of freedom. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. Load ID (*IMPEDANCE) Abaqus/CAE Load/Interaction Units Description I1 I2 Not supported None Not supported None Name of the impedance property that defines the impedance at the first end of the link (node 1). Name of the impedance property that defines the impedance at the second end of the link (node 2 or node 3). Distributed electric current densities Distributed electric current densities are available for coupled thermal-electrical elements. They are specified as described in “Coupled thermal-electrical analysis,” Section 6.7.3. Load ID (*DECURRENT) Load/Interaction Abaqus/CAE Units Description CBF CS1 CS2 Body current Surface current CL−3T−1 CL−2T−1 Surface current CL−2T−1 Volumetric current source density. Current density at the first end of the link (node 1). Current density at the second end of the link (node 2 or node 3). Element output Heat flux components Available for elements with temperature degrees of freedom. HFL1 Heat flux along the element axis. Electrical potential gradient Available for coupled thermal-electrical elements. EPG1 Electrical potential gradient along the element axis. Electrical current density components Available for coupled thermal-electrical elements. ECD1 Electrical current density along the element axis. Node ordering and face numbering on elements end 2 end 1 end 1 2 - node element 3 - node element end 2 Numbering of integration points for output 2 - node element 3 - node element 28.1.3 TWO-DIMENSIONAL SOLID ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Solid (continuum) elements,” Section 28.1.1 • *SOLID SECTION Overview This section provides a reference to the two-dimensional solid elements available in Abaqus/Standard and Abaqus/Explicit. Element types Plane strain elements CPE3 CPE3H(S) CPE4(S) CPE4H(S) CPE4I(S) 3-node linear 3-node linear, hybrid with constant pressure 4-node bilinear 4-node bilinear, hybrid with constant pressure 4-node bilinear, incompatible modes CPE4IH(S) 4-node bilinear, incompatible modes, hybrid with linear pressure CPE4R 4-node bilinear, reduced integration with hourglass control CPE4RH(S) CPE6(S) CPE6H(S) CPE6M 4-node bilinear, reduced integration with hourglass control, hybrid with constant pressure 6-node quadratic 6-node quadratic, hybrid with linear pressure 6-node modified, with hourglass control CPE6MH(S) 6-node modified, with hourglass control, hybrid with linear pressure CPE8(S) CPE8H(S) CPE8R(S) 8-node biquadratic 8-node biquadratic, hybrid with linear pressure 8-node biquadratic, reduced integration CPE8RH(S) 8-node biquadratic, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2 Additional solution variables The constant pressure hybrid elements have one additional variable relating to pressure, and the linear pressure hybrid elements have three additional variables relating to pressure. Element types CPE4I and CPE4IH have five additional variables relating to the incompatible modes. Element types CPE6M and CPE6MH have two additional displacement variables. Plane stress elements CPS3 CPS4(S) CPS4I(S) CPS4R CPS6(S) CPS6M CPS8(S) 3-node linear 4-node bilinear 4-node bilinear, incompatible modes 4-node bilinear, reduced integration with hourglass control 6-node quadratic 6-node modified, with hourglass control 8-node biquadratic CPS8R(S) 8-node biquadratic, reduced integration Active degrees of freedom 1, 2 Additional solution variables Element type CPS4I has four additional variables relating to the incompatible modes. Element type CPS6M has two additional displacement variables. Generalized plane strain elements CPEG3(S) CPEG3H(S) CPEG4(S) CPEG4H(S) CPEG4I(S) CPEG4IH(S) CPEG4R(S) CPEG4RH(S) 3-node linear triangle 3-node linear triangle, hybrid with constant pressure 4-node bilinear quadrilateral 4-node bilinear quadrilateral, hybrid with constant pressure 4-node bilinear quadrilateral, incompatible modes 4-node bilinear quadrilateral, incompatible modes, hybrid with linear pressure 4-node bilinear quadrilateral, reduced integration with hourglass control 4-node bilinear quadrilateral, reduced integration with hourglass control, hybrid with constant pressure CPEG6(S) CPEG6H(S) CPEG6M(S) 6-node quadratic triangle 6-node quadratic triangle, hybrid with linear pressure 6-node modified, with hourglass control CPEG6MH(S) 6-node modified, with hourglass control, hybrid with linear pressure CPEG8(S) CPEG8H(S) CPEG8R(S) 8-node biquadratic quadrilateral 8-node biquadratic quadrilateral, hybrid with linear pressure 8-node biquadratic quadrilateral, reduced integration CPEG8RH(S) 8-node biquadratic quadrilateral, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2 at all but the reference node 3, 4, 5 at the reference node Additional solution variables The constant pressure hybrid elements have one additional variable relating to pressure, and the linear pressure hybrid elements have three additional variables relating to pressure. Element types CPEG4I and CPEG4IH have five additional variables relating to the incompatible modes. Element types CPEG6M and CPEG6MH have two additional displacement variables. Coupled temperature-displacement plane strain elements CPE3T CPE4T(S) CPE4HT(S) CPE4RT CPE4RHT(S) 3-node linear displacement and temperature 4-node bilinear displacement and temperature 4-node bilinear displacement and temperature, hybrid with constant pressure 4-node bilinear displacement and temperature, reduced integration with hourglass control 4-node bilinear displacement and temperature, reduced integration with hourglass control, hybrid with constant pressure CPE6MT 6-node modified displacement and temperature, with hourglass control CPE6MHT(S) CPE8T(S) CPE8HT(S) CPE8RT(S) CPE8RHT(S) 6-node modified displacement and temperature, with hourglass control, hybrid with constant pressure 8-node biquadratic displacement, bilinear temperature 8-node biquadratic displacement, bilinear temperature, hybrid with linear pressure 8-node biquadratic displacement, bilinear temperature, reduced integration 8-node biquadratic displacement, bilinear temperature, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 11 at corner nodes 1, 2 at midside nodes of second-order elements in Abaqus/Standard 1, 2, 11 at midside nodes of modified displacement and temperature elements in Abaqus/Standard Additional solution variables The constant pressure hybrid elements have one additional variable relating to pressure, and the linear pressure hybrid elements have three additional variables relating to pressure. Element types CPE6MT and CPE6MHT have two additional displacement variables and one additional temperature variable. Coupled temperature-displacement plane stress elements CPS3T CPS4T(S) CPS4RT CPS6MT CPS8T(S) CPS8RT(S) 3-node linear displacement and temperature 4-node bilinear displacement and temperature 4-node bilinear displacement and temperature, reduced integration with hourglass control 6-node modified displacement and temperature, with hourglass control 8-node biquadratic displacement, bilinear temperature 8-node biquadratic displacement, bilinear temperature, reduced integration Active degrees of freedom 1, 2, 11 at corner nodes 1, 2 at midside nodes of second-order elements in Abaqus/Standard 1, 2, 11 at midside nodes of modified displacement and temperature elements in Abaqus/Standard Additional solution variables Element type CPS6MT has two additional displacement variables and one additional temperature variable. Coupled temperature-displacement generalized plane strain elements CPEG3T(S) CPEG3HT(S) CPEG4T(S) CPEG4HT(S) CPEG4RT(S) 3-node linear displacement and temperature 3-node linear displacement and temperature, hybrid with constant pressure 4-node bilinear displacement and temperature 4-node bilinear displacement and temperature, hybrid with constant pressure 4-node bilinear displacement and temperature, reduced integration with hourglass control CPEG4RHT(S) 4-node bilinear displacement and temperature, reduced integration with hourglass control, hybrid with constant pressure CPEG6MT(S) 6-node modified displacement and temperature, with hourglass control CPEG6MHT(S) CPEG8T(S) CPEG8HT(S) CPEG8RHT(S) 6-node modified displacement and temperature, with hourglass control, hybrid with constant pressure 8-node biquadratic displacement, bilinear temperature 8-node biquadratic displacement, bilinear temperature, hybrid with linear pressure 8-node biquadratic displacement, bilinear temperature, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 11 at corner nodes 1, 2 at midside nodes of second-order elements 1, 2, 11 at midside nodes of modified displacement and temperature elements 3, 4, 5 at the reference node Additional solution variables The constant pressure hybrid elements have one additional variable relating to pressure, and the linear pressure hybrid elements have three additional variables relating to pressure. Element types CPEG6MT and CPEG6MHT have two additional displacement variables and one additional temperature variable. Diffusive heat transfer or mass diffusion elements DC2D3(S) DC2D4(S) DC2D6(S) DC2D8(S) 3-node linear 4-node linear 6-node quadratic 8-node biquadratic Active degree of freedom 11 Additional solution variables None. Forced convection/diffusion elements DCC2D4(S) 4-node DCC2D4D(S) 4-node with dispersion control Active degree of freedom 11 Additional solution variables None. Coupled thermal-electrical elements DC2D3E(S) DC2D4E(S) DC2D6E(S) DC2D8E(S) 3-node linear 4-node linear 6-node quadratic 8-node biquadratic Active degrees of freedom 9, 11 Additional solution variables None. Pore pressure plane strain elements CPE4P(S) CPE4PH(S) CPE4RP(S) CPE4RPH(S) CPE6MP(S) CPE6MPH(S) CPE8P(S) CPE8PH(S) CPE8RP(S) CPE8RPH(S) 4-node bilinear displacement and pore pressure 4-node bilinear displacement and pore pressure, hybrid with constant pressure stress 4-node bilinear displacement and pore pressure, reduced integration with hourglass control 4-node bilinear displacement and pore pressure, reduced integration with hourglass control, hybrid with constant pressure 6-node modified displacement and pore pressure, with hourglass control 6-node modified displacement and pore pressure, with hourglass control, hybrid with linear pressure 8-node biquadratic displacement, bilinear pore pressure 8-node biquadratic displacement, bilinear pore pressure, hybrid with linear pressure stress 8-node biquadratic displacement, bilinear pore pressure, reduced integration 8-node biquadratic displacement, bilinear pore pressure, reduced integration, hybrid with linear pressure stress Active degrees of freedom 1, 2, 8 at corner nodes 1, 2 at midside nodes for all elements except CPE6MP and CPE6MPH, which also have degree of freedom 8 active at midside nodes Additional solution variables The constant pressure hybrid elements have one additional variable relating to the effective pressure stress, and the linear pressure hybrid elements have three additional variables relating to the effective pressure stress to permit fully incompressible material modeling. Element types CPE6MP and CPE6MPH have two additional displacement variables and one additional pore pressure variable. Acoustic elements AC2D3 AC2D4(S) AC2D4R(E) AC2D6(S) AC2D8(S) 3-node linear 4-node bilinear 4-node bilinear, reduced integration with hourglass control 6-node quadratic 8-node biquadratic Active degree of freedom Additional solution variables None. Piezoelectric plane strain elements CPE3E(S) CPE4E(S) CPE6E(S) CPE8E(S) 3-node linear 4-node bilinear 6-node quadratic 8-node biquadratic CPE8RE(S) 8-node biquadratic, reduced integration Active degrees of freedom 1, 2, 9 Additional solution variables None. Piezoelectric plane stress elements CPS3E(S) CPS4E(S) CPS6E(S) 3-node linear 4-node bilinear 6-node quadratic CPS8E(S) CPS8RE(S) 8-node biquadratic 8-node biquadratic, reduced integration Active degrees of freedom 1, 2, 9 Additional solution variables None. Electromagnetic elements EMC2D3(S) EMC2D4(S) 3-node zero-order 4-node zero-order Active degree of freedom Magnetic vector potential (for more information, see “Boundary conditions” in “Eddy current analysis,” Section 6.7.5, and “Boundary conditions” in “Magnetostatic analysis,” Section 6.7.6). Additional solution variables None. Nodal coordinates required X, Y Element property definition For all elements except generalized plane strain elements, you must provide the element thickness; by default, unit thickness is assumed. For generalized plane strain elements, you must provide three values: material fiber through the reference node, the initial value of the initial length of the axial (in radians), and the initial value of (in radians). If you do not provide these values, Abaqus assumes the default values of one unit . In addition, you must define the reference point for and as the initial length and zero for generalized plane strain elements. Input File Usage: Abaqus/CAE Usage: Use the following option to define the element properties for all elements except generalized plane strain elements: *SOLID SECTION Use the following option to define the element properties for generalized plane strain elements: *SOLID SECTION, REF NODE=node number or node set name Property module: Create Section: select Solid as the section Category and Homogeneous, Generalized plane strain, or Electromagnetic, Solid as the section Type Generalized plane strain sections must be assigned to regions of parts that have a reference point associated with them. To define the reference point: Part module: Tools→Reference Point: select reference point Element-based loading Distributed loads Distributed loads are available for all elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BX BY BXNU Body force Body force Body force FL−3 FL−3 FL−3 BYNU Body force FL−3 Body force in global X-direction. Body force in global Y-direction. Nonuniform body force in global X-direction with magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user Nonuniform body force in global Y-direction with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. CENT(S) Not supported FL−4 (ML−3T−2) Centrifugal load (magnitude is input as is the mass density , where per unit volume, is the angular velocity). Not available for pore pressure elements. Centrifugal load (magnitude is input as the angular velocity). , where is Coriolis force (magnitude is input as is the mass density , where per unit volume, is the angular velocity). Not available for pore pressure elements. CENTRIF(S) Rotational body force T−2 CORIO(S) Coriolis force FL−4 T (ML−3 T−1 ) Load ID (*DLOAD) GRAV Abaqus/CAE Load/Interaction Gravity HPn(S) Pn PnNU Not supported Pressure Not supported Units Description LT−2 FL−2 FL−2 FL−2 Gravity loading direction (magnitude is acceleration). in specified input as Hydrostatic pressure on face n, linear in global Y. Pressure on face n. on with user face Nonuniform pressure supplied magnitude subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. ROTA(S) Rotational body force T−2 SBF(E) Not supported FL−5 T2 Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Stagnation body force in global X- and Y-directions. Not supported FL−4 T2 Stagnation pressure on face n. Shear traction on face n. Nonuniform shear traction on face and direction n with magnitude supplied subroutine via UTRACLOAD. user General traction on face n. Nonuniform general traction on face and direction n with magnitude supplied subroutine via UTRACLOAD. user Viscous body force in global X- and Y-directions. Viscous pressure on face n, applying a pressure proportional to the velocity normal to the face and opposing the motion. SPn(E) TRSHRn Surface traction TRSHRnNU(S) Not supported TRVECn Surface traction TRVECnNU(S) Not supported FL−2 FL−2 FL−2 FL−2 VBF(E) VPn(E) Not supported FL−4 T Not supported FL−3 T Foundations Foundations are available for Abaqus/Standard elements with displacement degrees of freedom. They are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE Fn(S) Elastic foundation Distributed heat fluxes Units Description FL−3 Elastic foundation on face n. Distributed heat fluxes are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DFLUX) BF BFNU(S) Abaqus/CAE Load/Interaction Units Description Body heat flux Body heat flux JL−3 T−1 JL−3 T−1 Heat body flux per unit volume. Nonuniform heat body flux per unit volume with magnitude supplied via user subroutine DFLUX. Heat surface flux per unit area into face n. Nonuniform heat surface flux per unit area into face n with magnitude supplied via user subroutine DFLUX. Film coefficient and sink temperature (units of ) provided on face n. Nonuniform film coefficient and sink temperature (units of ) provided on face n with magnitude supplied via user subroutine FILM. Film conditions Film conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Abaqus/CAE Load/Interaction Units Description Sn Surface heat flux JL−2 T−1 SnNU(S) Not supported JL−2 T−1 Load ID (*FILM) Fn Surface film condition JL−2 T−1 −1 FnNU(S) Not supported JL−2 T−1 −1 Radiation types Radiation conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*RADIATE) Abaqus/CAE Load/Interaction Units Description Rn Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided on face n. Distributed flows Distributed flows are available for all elements with pore pressure degrees of freedom. They are specified as described in “Pore fluid flow,” Section 33.4.7. Load ID (*FLOW) Qn(S) Abaqus/CAE Load/Interaction Units Description Not supported F−1 L3T−1 QnD(S) Not supported F−1 L3T−1 QnNU(S) Not supported F−1 L3T−1 Seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on face n. Drainage-only seepage provided on face n. coefficient coefficient Nonuniform seepage and reference sink pore pressure (units of FL−2 ) provided on face n with magnitude supplied via user subroutine FLOW. Load ID (*DFLOW) Sn(S) Abaqus/CAE Load/Interaction Units Description Surface pore fluid LT−1 pore Prescribed effective velocity (outward from the face) on face n. fluid SnNU(S) Not supported LT−1 Nonuniform prescribed pore fluid effective velocity (outward from the face) on face n with magnitude supplied via user subroutine DFLOW. Distributed impedances Distributed impedances are available for all elements with acoustic pressure degrees of freedom. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. Load ID (*IMPEDANCE) Abaqus/CAE Load/Interaction Units Description In Not supported None Name of the impedance property that defines the impedance on face n. Electric fluxes Electric fluxes are available for piezoelectric elements. They are specified as described in “Piezoelectric analysis,” Section 6.7.2. Load ID (*DECHARGE) Abaqus/CAE Load/Interaction Units Description EBF(S) ESn(S) Body charge Surface charge CL−3 CL−2 Body flux per unit volume. Prescribed surface charge on face n. Distributed electric current densities Distributed electric current densities are available for coupled thermal-electrical elements, coupled thermal-electrical-structural elements, and electromagnetic elements. They are specified as described in “Coupled thermal-electrical analysis,” Section 6.7.3; “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4; and “Eddy current analysis,” Section 6.7.5. Load ID (*DECURRENT) Load/Interaction Abaqus/CAE Units Description CBF(S) CSn(S) CJ(S) Body current Surface current CL−3T−1 CL−2T−1 Volumetric current source density. Current density on face n. Body density current CL−2T−1 Volume current density vector in an eddy current analysis. Distributed concentration fluxes Distributed concentration fluxes are available for mass diffusion elements. They are specified as described in “Mass diffusion analysis,” Section 6.9.1. Load ID (*DFLUX) BF(S) BFNU(S) Sn(S) SnNU(S) Surface-based loading Distributed loads Abaqus/CAE Load/Interaction Units Description Body concentration flux Body concentration flux Surface concentration flux Surface concentration flux PT−1 PT−1 PLT−1 PLT−1 Concentration body flux per unit volume. Nonuniform concentration body flux per unit volume with magnitude supplied via user subroutine DFLUX. Concentration surface flux per unit area into face n. Nonuniform concentration surface flux per unit area into face n with magnitude supplied via user subroutine DFLUX. Surface-based distributed loads are available for all elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description HP(S) PNU Pressure Pressure Pressure FL−2 FL−2 FL−2 SP(E) Pressure FL−4 T2 TRSHR Surface traction TRSHRNU(S) Surface traction FL−2 FL−2 Hydrostatic pressure on the element surface, linear in global Y. Pressure on the element surface. Nonuniform pressure on the element surface with magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user Stagnation pressure on the element surface. Shear traction on the element surface. Nonuniform shear traction on the element surface with magnitude and (*DSLOAD) Abaqus/CAE Load/Interaction Units Description 2-D SOLIDS TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 VP(E) Pressure FL−3 T direction supplied via user subroutine UTRACLOAD. General surface. traction on the element Nonuniform general traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. Viscous pressure on the element The viscous pressure is surface. proportional to the velocity normal to the element surface and opposing the motion. Distributed heat fluxes Surface-based heat fluxes are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DSFLUX) Abaqus/CAE Load/Interaction Units Description Surface heat flux JL−2 T−1 SNU(S) Surface heat flux JL−2 T−1 Heat surface flux per unit area into the element surface. Nonuniform heat surface flux per unit area applied on the element surface with magnitude supplied via user subroutine DFLUX. Film conditions Surface-based film conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SFILM) Abaqus/CAE Load/Interaction Units Description Surface film condition JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on the element surface. Load ID (*SFILM) FNU(S) Radiation types Abaqus/CAE Load/Interaction Surface film condition Units Description JL−2 T−1 −1 Nonuniform film coefficient and sink temperature (units of ) provided on the element surface with magnitude supplied via user subroutine FILM. Surface-based radiation conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SRADIATE) Abaqus/CAE Load/Interaction Units Description Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided on the element surface. Distributed flows Surface-based flows are available for all elements with pore pressure degrees of freedom. They are specified as described in “Pore fluid flow,” Section 33.4.7. Load ID (*SFLOW) Q(S) Abaqus/CAE Load/Interaction Units Description Not supported F−1 L3T−1 QD(S) Not supported F−1 L3T−1 QNU(S) Not supported F−1 L3T−1 Seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on the element surface. Drainage-only seepage provided on the element surface. coefficient Nonuniform seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on the element surface with magnitude supplied via user subroutine FLOW. Abaqus/CAE Load/Interaction Units Description Surface pore fluid LT−1 28.1.3–16 pore Prescribed effective velocity outward from the element surface. fluid Load ID (*DSFLOW) Load ID (*DSFLOW) SNU(S) Abaqus/CAE Load/Interaction Units Description Surface pore fluid LT−1 Nonuniform prescribed pore fluid effective velocity outward from the surface with magnitude element supplied via user subroutine DFLOW. Distributed impedances Surface-based impedances are available for all elements with acoustic pressure degrees of freedom. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. Incident wave loading Surface-based incident wave loads are available for all elements with displacement degrees of freedom or acoustic pressure degrees of freedom. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. If the incident wave field includes a reflection off a plane outside the boundaries of the mesh, this effect can be included. Electric fluxes Surface-based electric fluxes are available for piezoelectric elements. They are specified as described in “Piezoelectric analysis,” Section 6.7.2. Load ID (*DSECHARGE) Load/Interaction Abaqus/CAE Units Description ES(S) Surface charge CL−2 Prescribed surface charge on the element surface. Distributed electric current densities Surface-based electric current densities are available for coupled thermal-electrical elements, coupled thermal-electrical-structural elements, and electromagnetic elements. They are specified as described in “Coupled thermal-electrical analysis,” Section 6.7.3; “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4; and “Eddy current analysis,” Section 6.7.5. Load ID (*DSECURRENT) Load/Interaction Abaqus/CAE Units Description CS(S) CK(S) Surface current CL−2T−1 Current density applied on the element surface. Surface density current CL−1T−1 Surface current density vector in an eddy current analysis. Element output For most elements output is in global directions unless a local coordinate system is assigned to the element through the section definition (“Orientations,” Section 2.2.5) in which case output is in the local coordinate system (which rotates with the motion in large-displacement analysis). See “State storage,” Section 1.5.4 of the Abaqus Theory Manual, for details. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S33 S12 , direct stress. , direct stress. , direct stress (not available for plane stress elements). , shear stress. Heat flux components Available for elements with temperature degrees of freedom. HFL1 HFL2 Heat flux in the X-direction. Heat flux in the Y-direction. Pore fluid velocity components Available for elements with pore pressure degrees of freedom. FLVEL1 FLVEL2 Pore fluid effective velocity in the X-direction. Pore fluid effective velocity in the Y-direction. Mass concentration flux components Available for elements with normalized concentration degrees of freedom. MFL1 MFL2 Concentration flux in the X-direction. Concentration flux in the Y-direction. Electrical potential gradient Available for elements with electrical potential degrees of freedom. EPG1 EPG2 Electrical potential gradient in the X-direction. Electrical potential gradient in the Y-direction. Electrical flux components Available for piezoelectric elements. EFLX1 EFLX2 Electrical flux in the X-direction. Electrical flux in the Y-direction. Electrical current density components Available for coupled thermal-electrical elements. ECD1 ECD2 Electrical current density in the X-direction. Electrical current density in the Y-direction. Electrical field components Available for electromagnetic elements in an eddy current analysis. EME1 EME2 Electric field in the X-direction. Electric field in the Y-direction. Magnetic flux density components Available for electromagnetic elements. EMB3 Magnetic flux density in the Z-direction. Magnetic field components Available for electromagnetic elements. EMH3 Magnetic field in the Z-direction. Electrical current density components in an eddy current analysis Available for electromagnetic elements in an eddy current analysis. EMCD1 EMCD2 Electrical current density in the X-direction. Electrical current density in the Y-direction. Node ordering and face numbering on elements face 3 face 3 face 2 face 4 face 2 1 2 face 1 3 - node element face 1 4 - node element face 3 4 7 3 face 3 6 5 face 2 face 4 face 2 1 face 1 6 - node element 2 face 1 8 - node element For generalized plane strain elements, the reference node associated with each element (where the generalized plane strain degrees of freedom are stored) is not shown. The reference node should be the same for all elements in any given connected region so that the bounding planes are the same for that region. Different regions may have different reference nodes. The number of the reference node is not incremented when the elements are generated incrementally . Triangular element faces Face 1 Face 2 Face 3 1 – 2 face 2 – 3 face 3 – 1 face Quadrilateral element faces Face 1 Face 2 Face 3 Face 4 1 – 2 face 2 – 3 face 3 – 4 face 4 – 1 face 2-D SOLIDS 6 5 1 2 1 2 3 - node element 6 - node element 4 - node element 4-node reduced integration element 4 7 3 4 7 3 8 - node element 8-node reduced integration element For heat transfer applications a different integration scheme is used for triangular elements, as described in “Triangular, tetrahedral, and wedge elements,” Section 3.2.6 of the Abaqus Theory Manual. 28.1.4 THREE-DIMENSIONAL SOLID ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Solid (continuum) elements,” Section 28.1.1 • *SOLID SECTION Overview This section provides a reference to the three-dimensional solid elements available in Abaqus/Standard and Abaqus/Explicit. Element types Stress/displacement elements C3D4 C3D4H(S) C3D6(S) C3D6(E) C3D6H(S) C3D8 C3D8H(S) C3D8I 4-node linear tetrahedron 4-node linear tetrahedron, hybrid with linear pressure 6-node linear triangular prism 6-node linear triangular prism, reduced integration with hourglass control 6-node linear triangular prism, hybrid with constant pressure 8-node linear brick 8-node linear brick, hybrid with constant pressure 8-node linear brick, incompatible modes C3D8IH(S) 8-node linear brick, incompatible modes, hybrid with linear pressure C3D8R 8-node linear brick, reduced integration with hourglass control C3D8RH(S) C3D10(S) C3D10H(S) C3D10I(S) C3D10M 8-node linear brick, reduced integration with hourglass control, hybrid with constant pressure 10-node quadratic tetrahedron 10-node quadratic tetrahedron, hybrid with constant pressure 10-node general-purpose quadratic tetrahedron, improved surface stress visualization 10-node modified tetrahedron, with hourglass control C3D10MH(S) 10-node modified tetrahedron, with hourglass control, hybrid with linear pressure C3D15(S) 15-node quadratic triangular prism C3D15H(S) C3D20(S) C3D20H(S) C3D20R(S) 15-node quadratic triangular prism, hybrid with linear pressure 20-node quadratic brick 20-node quadratic brick, hybrid with linear pressure 20-node quadratic brick, reduced integration C3D20RH(S) 20-node quadratic brick, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 3 Additional solution variables The constant pressure hybrid elements have one additional variable relating to pressure, and the linear pressure hybrid elements have four additional variables relating to pressure. Element types C3D8I and C3D8IH have thirteen additional variables relating to the incompatible modes. Element types C3D10M and C3D10MH have three additional displacement variables. Stress/displacement variable node elements C3D15V(S) C3D15VH(S) C3D27(S) C3D27H(S) C3D27R(S) 15 to 18-node triangular prism 15 to 18-node triangular prism, hybrid with linear pressure 21 to 27-node brick 21 to 27-node brick, hybrid with linear pressure 21 to 27-node brick, reduced integration C3D27RH(S) 21 to 27-node brick, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 3 Additional solution variables The hybrid elements have four additional variables relating to pressure. Coupled temperature-displacement elements C3D4T C3D6T(S) C3D6T(E) C3D8T C3D8HT(S) C3D8RT 4-node linear displacement and temperature 6-node linear displacement and temperature 6-node linear displacement and temperature, reduced integration with hourglass control 8-node trilinear displacement and temperature 8-node trilinear displacement and temperature, hybrid with constant pressure 8-node trilinear displacement and temperature, reduced integration with hourglass control C3D8RHT(S) 8-node trilinear displacement and temperature, reduced integration with hourglass control, hybrid with constant pressure C3D10MT 10-node modified displacement and temperature tetrahedron, with hourglass control C3D10MHT(S) C3D20T(S) C3D20HT(S) C3D20RT(S) C3D20RHT(S) 10-node modified displacement and temperature tetrahedron, with hourglass control, hybrid with linear pressure 20-node triquadratic displacement, trilinear temperature 20-node triquadratic displacement, trilinear temperature, hybrid with linear pressure 20-node triquadratic displacement, trilinear temperature, reduced integration 20-node triquadratic displacement, trilinear temperature, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 3, 11 at corner nodes 1, 2, 3 at midside nodes of second-order elements in Abaqus/Standard 1, 2, 3, 11 at midside nodes of modified displacement and temperature elements in Abaqus/Standard Additional solution variables The constant pressure hybrid element has one additional variable relating to pressure, and the linear pressure hybrid elements have four additional variables relating to pressure. Element types C3D10MT and C3D10MHT have three additional displacement variables and one additional temperature variable. Coupled thermal-electrical-structural elements Q3D4(S) Q3D6(S) Q3D8(S) Q3D8H(S) Q3D8R(S) Q3D8RH(S) Q3D10M(S) Q3D10MH(S) 4-node linear displacement, electric potential and temperature 6-node linear displacement, electric potential and temperature 8-node trilinear displacement, electric potential and temperature 8-node trilinear displacement, electric potential and temperature, hybrid with constant pressure 8-node trilinear displacement, electric potential and temperature, reduced integration with hourglass control 8-node trilinear displacement, electric potential and temperature, reduced integration with hourglass control, hybrid with constant pressure 10-node modified displacement, electric potential and temperature tetrahedron, with hourglass control 10-node modified displacement, electric potential and temperature tetrahedron, with hourglass control, hybrid with linear pressure Q3D20(S) Q3D20H(S) Q3D20R(S) Q3D20RH(S) 20-node triquadratic displacement, trilinear electric potential and trilinear temperature 20-node triquadratic displacement, trilinear electric potential, trilinear temperature, hybrid with linear pressure 20-node triquadratic displacement, trilinear electric potential, trilinear temperature, reduced integration 20-node triquadratic displacement, trilinear electric potential, trilinear temperature, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 3, 9, 11 at corner nodes 1, 2, 3 at midside nodes of second-order elements in Abaqus/Standard 1, 2, 3, 9, 11 at midside nodes of modified displacement and temperature elements in Abaqus/Standard Additional solution variables The constant pressure hybrid element has one additional variable relating to pressure, and the linear pressure hybrid elements have four additional variables relating to pressure. Element types Q3D10M and Q3D10MH have three additional displacement variables, one additional electric potential variable, and one additional temperature variable. Diffusive heat transfer or mass diffusion elements DC3D4(S) DC3D6(S) DC3D8(S) DC3D10(S) DC3D15(S) DC3D20(S) 4-node linear tetrahedron 6-node linear triangular prism 8-node linear brick 10-node quadratic tetrahedron 15-node quadratic triangular prism 20-node quadratic brick Active degree of freedom 11 Additional solution variables None. Forced convection/diffusion elements DCC3D8(S) 8-node DCC3D8D(S) 8-node with dispersion control Active degree of freedom 11 Additional solution variables None. Coupled thermal-electrical elements DC3D4E(S) DC3D6E(S) DC3D8E(S) 4-node linear tetrahedron 6-node linear triangular prism 8-node linear brick DC3D10E(S) 10-node quadratic tetrahedron DC3D15E(S) 15-node quadratic triangular prism DC3D20E(S) 20-node quadratic brick Active degrees of freedom 9, 11 Additional solution variables None. Pore pressure elements C3D4P(S) C3D6P(S) C3D8P(S) C3D8PH(S) C3D8RP(S) C3D8RPH(S) C3D10MP(S) C3D10MPH(S) C3D20P(S) C3D20PH(S) C3D20RP(S) C3D20RPH(S) 4-node linear displacement and pore pressure 6-node linear displacement and pore pressure 8-node trilinear displacement and pore pressure 8-node trilinear displacement and pore pressure, hybrid with constant pressure 8-node trilinear displacement and pore pressure, reduced integration 8-node trilinear displacement and pore pressure, reduced integration, hybrid with constant pressure 10-node modified displacement and pore pressure tetrahedron, with hourglass control 10-node modified displacement and pore pressure tetrahedron, with hourglass control, hybrid with linear pressure 20-node triquadratic displacement, trilinear pore pressure 20-node triquadratic displacement, trilinear pore pressure, hybrid with linear pressure 20-node triquadratic displacement, trilinear pore pressure, reduced integration 20-node triquadratic displacement, trilinear pore pressure, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 3 at midside nodes for all elements except C3D10MP and C3D10MPH, which also have degree of freedom 8 active at midside nodes 1, 2, 3, 8 at corner nodes Additional solution variables The constant pressure hybrid elements have one additional variable relating to the effective pressure stress, and the linear pressure hybrid elements have four additional variables relating to the effective pressure stress to permit fully incompressible material modeling. Element types C3D10MP and C3D10MPH have three additional displacement variables and one additional pore pressure variable. Coupled temperature–pore pressure elements C3D8PT(S) C3D8PHT(S) C3D8RPT(S) C3D8RPHT(S) C3D10MPT(S) 8-node trilinear displacement, pore pressure, and temperature. 8-node trilinear displacement, pore pressure, and temperature; hybrid with constant pressure 8-node trilinear displacement, pore pressure, and temperature; reduced integration 8-node trilinear displacement, pore pressure, and temperature; reduced integration, hybrid with constant pressure 10-node modified displacement, pore pressure, and temperature tetrahedron, with hourglass control Active degrees of freedom 1, 2, 3, 8, 11 Additional solution variables The constant pressure hybrid elements have one additional variable relating to the effective pressure stress to permit fully incompressible material modeling. Element type C3D10MPT has three additional displacement variables, one additional pore pressure variable, and one additional temperature variable. Acoustic elements AC3D4 AC3D6 AC3D8(S) AC3D8R(E) AC3D10(S) 4-node linear tetrahedron 6-node linear triangular prism 8-node linear brick 8-node linear brick, reduced integration with hourglass control 10-node quadratic tetrahedron AC3D15(S) AC3D20(S) 15-node quadratic triangular prism 20-node quadratic brick Active degree of freedom Additional solution variables None. Piezoelectric elements C3D4E(S) C3D6E(S) C3D8E(S) C3D10E(S) C3D15E(S) C3D20E(S) 4-node linear tetrahedron 6-node linear triangular prism 8-node linear brick 10-node quadratic tetrahedron 15-node quadratic triangular prism 20-node quadratic brick C3D20RE(S) 20-node quadratic brick, reduced integration Active degrees of freedom 1, 2, 3, 9 Additional solution variables None. Electromagnetic elements EMC3D4(S) EMC3D8(S) 4-node zero-order 8-node zero-order Active degree of freedom Magnetic vector potential (for more information, see “Boundary conditions” in “Eddy current analysis,” Section 6.7.5, and “Boundary conditions” in “Magnetostatic analysis,” Section 6.7.6). Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition Input File Usage: *SOLID SECTION Abaqus/CAE Usage: Property module: Create Section: select Solid as the section Category and Homogeneous or Electromagnetic, Solid as the section Type Element-based loading Distributed loads Distributed loads are available for all elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BX BY BZ BXNU Body force Body force Body force Body force FL−3 FL−3 FL−3 FL−3 BYNU Body force FL−3 Body force in global X-direction. Body force in global Y-direction. Body force in global Z-direction. Nonuniform body force in global X-direction with magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user Nonuniform body force in global Y-direction with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. BZNU Body force CENT(S) Not supported FL−3 Nonuniform body force in global Z-direction with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. FL−4 (ML−3T−2) Centrifugal load (magnitude is input as is the mass density , where per unit volume, is the angular velocity). Not available for pore pressure elements. CENTRIF(S) Rotational body force T−2 Centrifugal load (magnitude is input as the angular velocity). , where is CORIO(S) Coriolis force FL−4 T (ML−3 T−1 ) Coriolis force (magnitude is input is the mass density as , where (*DLOAD) Abaqus/CAE Load/Interaction Units Description 3-D SOLIDS GRAV Gravity HPn(S) Pn PnNU Not supported Pressure Not supported LT−2 FL−2 FL−2 FL−2 is the angular per unit volume, velocity). Not available for pore pressure elements. Gravity loading direction (magnitude is acceleration). in specified input as Hydrostatic pressure on face n, linear in global Z. Pressure on face n. on with user face Nonuniform pressure supplied magnitude subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. ROTA(S) Rotational body force T−2 ROTDYNF(S) Not supported T−1 SBF(E) Not supported FL−5 T2 Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Rotordynamic load (magnitude is input as is the angular velocity). , where Stagnation body force in global X-, Y-, and Z-directions. Not supported FL−4 T2 Stagnation pressure on face n. Shear traction on face n. Nonuniform shear traction on face and direction n with magnitude subroutine via supplied UTRACLOAD. user General traction on face n. Nonuniform general traction on face and direction n with magnitude supplied subroutine via UTRACLOAD. user FL−2 FL−2 FL−2 FL−2 28.1.4–9 SPn(E) TRSHRn Surface traction TRSHRnNU(S) Not supported TRVECn Surface traction TRVECnNU(S) Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description VBF(E) VPn(E) Not supported FL−4 T Not supported FL−3 T Viscous body force in global X-, Y-, and Z-directions. Viscous pressure on face n, applying a pressure proportional to the velocity normal to the face and opposing the motion. Foundations Foundations are available for Abaqus/Standard elements with displacement degrees of freedom. They are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE Fn(S) Elastic foundation Distributed heat fluxes Units Description FL−3 Elastic foundation on face n. Distributed heat fluxes are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DFLUX) BF BFNU(S) Abaqus/CAE Load/Interaction Units Description Body heat flux Body heat flux JL−3 T−1 JL−3 T−1 Sn Surface heat flux JL−2 T−1 SnNU(S) Not supported JL−2 T−1 Heat body flux per unit volume. Nonuniform heat body flux per unit volume with magnitude supplied via user subroutine DFLUX. Heat surface flux per unit area into face n. Nonuniform heat surface flux per unit area into face n with magnitude supplied via user subroutine DFLUX. Film conditions Film conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*FILM) Fn Abaqus/CAE Load/Interaction Units Description Surface film condition JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on face n. FnNU(S) Not supported JL−2 T−1 −1 Nonuniform film coefficient and sink temperature (units of ) provided on face n with magnitude supplied via user subroutine FILM. Radiation types Radiation conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*RADIATE) Abaqus/CAE Load/Interaction Units Description Rn Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided on face n. Distributed flows Distributed flows are available for all elements with pore pressure degrees of freedom. They are specified as described in “Pore fluid flow,” Section 33.4.7. Load ID (*FLOW) Qn(S) Abaqus/CAE Load/Interaction Units Description Not supported F−1 L3T−1 Seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on face n. Drainage-only seepage provided on face n. coefficient Nonuniform seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on face n with magnitude supplied via user subroutine FLOW. QnD(S) Not supported F−1 L3T−1 QnNU(S) Not supported F−1 L3T−1 Load ID (*DFLOW) Sn(S) Abaqus/CAE Load/Interaction Units Description Surface pore fluid LT−1 pore Prescribed effective velocity (outward from the face) on face n. fluid SnNU(S) Not supported LT−1 Nonuniform prescribed pore fluid effective velocity (outward from the face) on face n with magnitude supplied via user subroutine DFLOW. Distributed impedances Distributed impedances are available for all elements with acoustic pressure degrees of freedom. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. Load ID (*IMPEDANCE) Abaqus/CAE Load/Interaction Units Description In Not supported None Name of the impedance property that defines the impedance on face n. Electric fluxes Electric fluxes are available for piezoelectric elements. They are specified as described in “Piezoelectric analysis,” Section 6.7.2. Load ID (*DECHARGE) Abaqus/CAE Load/Interaction Units Description EBF(S) ESn(S) Body charge Surface charge CL−3 CL−2 Body flux per unit volume. Prescribed surface charge on face n. Distributed electric current densities Distributed electric current densities are available for coupled thermal-electrical, coupled thermal-electrical-structural elements, and electromagnetic elements. They are specified as described in “Coupled thermal-electrical analysis,” Section 6.7.3; “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4; and “Eddy current analysis,” Section 6.7.5. Load ID (*DECURRENT) Load/Interaction Abaqus/CAE Units Description CBF(S) CSn(S) Body current Surface current CL−3T−1 CL−2T−1 Volumetric current source density. Current density on face n. Load ID (*DECURRENT) Load/Interaction CJ(S) current Body density 3-D SOLIDS Units Description CL−2T−1 Volume current density vector in an eddy current analysis. Distributed concentration fluxes Distributed concentration fluxes are available for mass diffusion elements. They are specified as described in “Mass diffusion analysis,” Section 6.9.1. Load ID (*DFLUX) BF(S) BFNU(S) Sn(S) SnNU(S) Abaqus/CAE Load/Interaction Units Description Body concentration flux Body concentration flux Surface concentration flux Surface concentration flux PT−1 PT−1 PLT−1 PLT−1 Concentration body flux per unit volume. Nonuniform concentration body flux per unit volume with magnitude supplied via user subroutine DFLUX. Concentration surface flux per unit area into face n. Nonuniform concentration surface flux per unit area into face n with magnitude supplied via user subroutine DFLUX. Surface-based loading Distributed loads Surface-based distributed loads are available for all elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description HP(S) PNU Pressure Pressure Pressure FL−2 FL−2 FL−2 Hydrostatic pressure on the element surface, linear in global Z. Pressure on the element surface. Nonuniform pressure on the element supplied surface with magnitude Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description SP(E) Pressure FL−4 T2 TRSHR Surface traction TRSHRNU(S) Surface traction FL−2 FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 VP(E) Pressure FL−3 T user subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. Stagnation pressure on the element surface. Shear traction on the element surface. Nonuniform shear traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. General surface. traction on the element Nonuniform general traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. Viscous pressure applied on the element surface. The viscous pressure is proportional to the velocity normal to the element face and opposing the motion. Distributed heat fluxes Surface-based heat fluxes are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DSFLUX) Abaqus/CAE Load/Interaction Units Description Surface heat flux JL−2 T−1 SNU(S) Surface heat flux JL−2 T−1 Heat surface flux per unit area into the element surface. Nonuniform heat surface flux per unit area into the element surface with magnitude supplied via user subroutine DFLUX. Film conditions Surface-based film conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SFILM) FNU(S) Radiation types Abaqus/CAE Load/Interaction Units Description Surface film condition Surface film condition JL−2 T−1 −1 JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on the element surface. Nonuniform film coefficient and sink temperature (units of ) provided on the element surface with magnitude supplied via user subroutine FILM. Surface-based radiation conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SRADIATE) Abaqus/CAE Load/Interaction Units Description Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided on the element surface. Distributed flows Surface-based flows are available for all elements with pore pressure degrees of freedom. They are specified as described in “Pore fluid flow,” Section 33.4.7. Load ID (*SFLOW) Q(S) Abaqus/CAE Load/Interaction Units Description Not supported F−1 L3T−1 Seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on the element surface. Drainage-only seepage provided on the element surface. coefficient Nonuniform seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on the element QD(S) Not supported F−1 L3T−1 QNU(S) Not supported F−1 L3T−1 Load ID (*SFLOW) Abaqus/CAE Load/Interaction Units Description Load ID (*DSFLOW) S(S) SNU(S) surface with magnitude supplied via user subroutine FLOW. Abaqus/CAE Load/Interaction Units Description Surface pore fluid Surface pore fluid LT−1 LT−1 pore Prescribed effective velocity outward from the element surface. fluid Nonuniform prescribed pore fluid effective velocity outward from the surface with magnitude element supplied via user subroutine DFLOW. Distributed impedances Surface-based impedances are available for all elements with acoustic pressure degrees of freedom. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. Incident wave loading Surface-based incident wave loads are available for all elements with displacement degrees of freedom or acoustic pressure degrees of freedom. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. If the incident wave field includes a reflection off a plane outside the boundaries of the mesh, this effect can be included. Electric fluxes Surface-based electric fluxes are available for piezoelectric elements. They are specified as described in “Piezoelectric analysis,” Section 6.7.2. Load ID (*DSECHARGE) Load/Interaction Abaqus/CAE Units Description ES(S) Surface charge CL−2 Prescribed surface charge on the element surface. Distributed electric current densities Surface-based electric current densities are available for coupled thermal-electrical, coupled thermal- electrical-structural, and electromagnetic elements. They are specified as described in “Coupled thermal- electrical analysis,” Section 6.7.3, “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4, and “Eddy current analysis,” Section 6.7.5. Load ID (*DSECURRENT) Load/Interaction Abaqus/CAE Units Description CS(S) CK(S) Surface current CL−2T−1 Surface density current CL−1T−1 Current density on the surface. element Surface current density vector in an eddy current analysis. Element output For most elements output is in global directions unless a local coordinate system is assigned to the element through the section definition (“Orientations,” Section 2.2.5) in which case output is in the local coordinate system (which rotates with the motion in large-displacement analysis). See “State storage,” Section 1.5.4 of the Abaqus Theory Manual, for details. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S33 S12 S13 S23 , direct stress. , direct stress. , direct stress. , shear stress. , shear stress. , shear stress. Note: the order shown above is not the same as that used in user subroutine VUMAT. Heat flux components Available for elements with temperature degrees of freedom. HFL1 HFL2 HFL3 Heat flux in the X-direction. Heat flux in the Y-direction. Heat flux in the Z-direction. Pore fluid velocity components Available for elements with pore pressure degrees of freedom. FLVEL1 FLVEL2 FLVEL3 Pore fluid effective velocity in the X-direction. Pore fluid effective velocity in the Y-direction. Pore fluid effective velocity in the Z-direction. Mass concentration flux components Available for elements with normalized concentration degrees of freedom. MFL1 MFL2 MFL3 Concentration flux in the X-direction. Concentration flux in the Y-direction. Concentration flux in the Z-direction. Electrical potential gradient Available for elements with electrical potential degrees of freedom. EPG1 EPG2 EPG3 Electrical potential gradient in the X-direction. Electrical potential gradient in the Y-direction. Electrical potential gradient in the Z-direction. Electrical flux components Available for piezoelectric elements. EFLX1 EFLX2 EFLX3 Electrical flux in the X-direction. Electrical flux in the Y-direction. Electrical flux in the Z-direction. Electrical current density components Available for coupled thermal-electrical and coupled thermal-electrical-structural elements. ECD1 ECD2 ECD3 Electrical current density in the X-direction. -direction. Electrical current density in the Electrical current density in the Z-direction. Electrical field components Available for electromagnetic elements in an eddy current analysis. EME1 EME2 EME3 Electric field in the X-direction. Electric field in the Y-direction. Electric field in the Z-direction. Magnetic flux density components Available for electromagnetic elements. EMB1 EMB2 EMB3 Magnetic flux density in the X-direction. Magnetic flux density in the Y-direction. Magnetic flux density in the Z-direction. Magnetic field components Available for electromagnetic elements. EMH1 EMH2 EMH3 Magnetic field in the X-direction. Magnetic field in the Y-direction. Magnetic field in the Z-direction. Electrical current density components in an eddy current analysis Available for electromagnetic elements in an eddy current analysis. EMCD1 EMCD2 EMCD3 Electrical current density in the X-direction. Electrical current density in the Y-direction. Electrical current density in the Z-direction. Node ordering and face numbering on elements All elements except variable node elements face 4 face 4 face 3 face 2 face 2 face 3 face 1 4 - node element face 2 face 5 face 4 face 1 6 - node element face 2 face 5 face 6 face 4 10 face 3 face 1 face 3 13 10 - node element face 2 12 face 5 10 11 14 15 - node element 15 face 4 face 1 face 6 17 face 2 16 13 20 12 18 face 5 15 19 face 4 14 11 10 face 1 face 3 face 3 face 1 8 - node element 20 - node element Tetrahedral element faces Face 1 Face 2 Face 3 Face 4 1 – 2 – 3 face 1 – 4 – 2 face 2 – 4 – 3 face 3 – 4 – 1 face Wedge (triangular prism) element faces Face 1 Face 2 Face 3 Face 4 Face 5 1 – 2 – 3 face 4 – 6 – 5 face 1 – 4 – 5 – 2 face 2 – 5 – 6 – 3 face 3 – 6 – 4 – 1 face Hexahedron (brick) element faces Face 1 Face 2 Face 3 Face 4 Face 5 Face 6 1 – 2 – 3 – 4 face 5 – 8 – 7 – 6 face 1 – 5 – 6 – 2 face 2 – 6 – 7 – 3 face 3 – 7 – 8 – 4 face 4 – 8 – 5 – 1 face Variable node elements 13 15 11 17 12 10 18 16 14 15 to 18 - node element 16–18 are midface nodes on the three rectangular faces . These nodes can be omitted from an element by entering a zero or blank in the corresponding position when giving the nodes on the element. Only nodes 16–18 can be omitted. Face location of nodes 16 to 18 Face node number Corner nodes on face 16 17 18 1 – 4 – 5 – 2 2 – 5 – 6 – 3 3 – 6 – 4 – 1 15 14 26 25 10 23 20 18 11 21 22 19 16 13 27 17 24 12 21 to 27 - node element Node 21 is located at the centroid of the element. (nodes 22–27) are midface nodes on the six faces . These nodes can be deleted from an element by entering a zero or blank in the corresponding position when giving the nodes on the element. Only nodes 22–27 can be omitted. Face location of nodes 22 to 27 Face node number Corner nodes on face 1 – 2 – 3 – 4 5 – 8 – 7 – 6 1 – 5 – 6 – 2 2 – 6 – 7 – 3 3 – 7 – 8 – 4 4 – 8 – 5 – 1 28.1.4–23 22 23 24 25 26 Numbering of integration points for output All elements except variable node elements 4 - node element 10 - node element 10 1 2 6 - node element 8 - node element 15 - node element 8 - node reduced integration element 4 11 3 4 11 3 12 10 2 0 - node element 12 2 0 - node reduced integration element 10 This shows the scheme in the layer closest to the 1–2–3 and 1–2–3–4 faces. The integration points in the second and third layers are numbered consecutively. Multiple layers are used for composite solid elements. For heat transfer applications a different integration scheme is used for tetrahedral and wedge elements, as described in “Triangular, tetrahedral, and wedge elements,” Section 3.2.6 of the Abaqus Theory Manual. For linear triangular prisms in Abaqus/Explicit reduced integration is used; therefore, a C3D6 element and a C3D6T element have only one integration point. For the general-purpose C3D10I 10-node tetrahedra in Abaqus/Standard improved stress visualization is obtained through an 11-point integration rule, consisting of 10 integration points at the elements’ nodes and one integration point at their centroid. For acoustic tetrahedra and wedges in Abaqus/Standard full integration is used; therefore, an AC3D4 element has 4 integration points, an AC3D6 element has 6 integration points, an AC3D10 element has 10 integration points, and an AC3D15 element has 18 integration points. Variable node elements 4 11 3 10 12 15 to 18 - node element 21 to 27 - node element This shows the scheme in the layer closest to the 1–2–3 and 1–2–3–4 faces. The integration points in the second and third layers are numbered consecutively. Multiple layers are used for composite solid elements. The face nodes do not appear. 14 11 10 12 13 21 to 27 - node reduced integration element Node 21 is located at the centroid of the element. 28.1.5 CYLINDRICAL SOLID ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/CAE References • “Solid (continuum) elements,” Section 28.1.1 • *SOLID SECTION Overview This section provides a reference to the cylindrical solid elements available in Abaqus/Standard. Element types CCL9 CCL9H CCL12 CCL12H CCL18 CCL18H CCL24 CCL24H 9-node cylindrical prism, linear interpolation in the radial plane and trigonometric interpolation along the circumferential direction 9-node cylindrical prism, linear interpolation in the radial plane and trigonometric interpolation along the circumferential direction, hybrid with constant pressure in plane and linear pressure in the circumferential direction 12-node cylindrical brick, linear interpolation in the radial plane and trigonometric interpolation along the circumferential direction 12-node cylindrical brick, linear interpolation in the radial plane and trigonometric interpolation along the circumferential direction, hybrid with constant pressure in plane and linear pressure in circumferential direction 18-node cylindrical prism, quadratic interpolation in the radial plane and trigonometric interpolation along the circumferential direction 18-node cylindrical prism, quadratic interpolation in the radial plane and trigonometric interpolation along the circumferential direction, hybrid with linear pressure in plane and linear pressure in the circumferential direction 24-node cylindrical brick, quadratic interpolation in the radial plane and trigonometric interpolation along the circumferential direction 24-node cylindrical brick, quadratic interpolation in the radial plane and trigonometric interpolation along the circumferential direction, hybrid with linear pressure in plane and linear pressure in circumferential direction CCL24R 24-node cylindrical brick, reduced integration, quadratic interpolation in the radial plane and trigonometric interpolation along the circumferential direction CCL24RH 24-node cylindrical brick, reduced integration, quadratic interpolation in the radial plane and trigonometric interpolation along the circumferential direction, hybrid with linear pressure in plane and linear pressure in circumferential direction Active degrees of freedom 1, 2, 3 Additional solution variables The hybrid elements with constant pressure in plane have two additional variables relating to pressure, and the linear pressure hybrid elements have six additional variables relating to pressure. Nodal coordinates required X, Y, Z Element property definition Input File Usage: Abaqus/CAE Usage: *SOLID SECTION Property module: Create Section: select Solid as the section Category and Homogeneous as the section Type Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Units Description FL−3 FL−3 FL−3 FL−3 FL−3 FL−3 Body force in global X-direction. Body force in global Y-direction. Body force in global Z-direction. Nonuniform body force in global X- direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in global Y- direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in global Z- direction with magnitude supplied via user subroutine DLOAD. 28.1.5–2 Load ID (*DLOAD) BX BY BZ BXNU BYNU Units Description Load ID (*DLOAD) CENT FL−4 (ML−3T−2) CENTRIF FL−4 (ML−3T−1) CORIO FL−4 T (ML−3 T−1 ) GRAV HPn Pn ROTA LT−2 FL−2 FL−2 T−2 ROTDYNF(S) T−1 TRSHRn TRSHRnNU(S) TRVECn TRVECnNU(S) FL−2 FL−2 FL−2 FL−2 Centrifugal load (magnitude is input as where , is the mass density per unit volume, is the angular velocity). Centrifugal load (magnitude is input as where is the angular velocity). , Coriolis force (magnitude is input as where , is the mass density per unit volume, is the angular velocity). Gravity loading in a specified direction (magnitude is input as acceleration). Hydrostatic pressure on face n, linear in global Z. Pressure on face n. Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Rotordynamic load (magnitude is input as , where is the angular velocity). Shear traction on face n. Nonuniform shear traction on face n with magnitude and direction supplied via user subroutine UTRACLOAD. General traction on face n. Nonuniform general traction on face n with magnitude and direction supplied via user subroutine UTRACLOAD. Foundations Foundations are available for all cylindrical elements. They are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Units Description Fn FL−3 Elastic foundation on face n. Surface-based loading Distributed loads Surface-based distributed loads are available for elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) HP Pn PnNU TRSHR TRSHRNU(S) TRVEC TRVECNU(S) Element output Units Description FL−2 FL−2 FL−2 FL−2 FL−2 FL−2 FL−2 Hydrostatic pressure on the element surface, linear in global Z. Pressure on the element surface. Nonuniform pressure on the element surface with magnitude supplied via user subroutine DLOAD. Shear traction on the element surface. Nonuniform shear traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. General traction on the element surface. Nonuniform general traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. Output is in a fixed cylindrical system (1=radial, 2=axial, 3=circumferential) unless a local coordinate system is assigned to the element through the section definition (“Orientations,” Section 2.2.5) in which case output is in the local coordinate system (which rotates with the motion in large-displacement analysis). See “State storage,” Section 1.5.4 of the Abaqus Theory Manual, for details. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S33 S12 Local 11 direct stress. Local 22 direct stress. Local 33 direct stress. Local 12 shear stress. S23 Local 13 shear stress. Local 23 shear stress. Node ordering and face numbering on elements face 1 14 23 15 12 13 16 12 face 1 face 6 face 5 11 10 face 4 face 3 face 6 24 21 20 face 2 face 3 face 2 CYLINDRICAL SOLIDS 11 face 5 22 10 19 17 face 4 18 12-node element 12-node element 24-node element face 1 face 3 face 1 12 face 4 face 5 10 face 2 face 3 face 5 11 18 16 face 4 17 15 14 13 face 2 9-node element 18-node element 12-node and 24-node cylindrical element faces Face 1 Face 2 1 – 2 – 3 – 4 face 5 – 8 – 7 – 6 face Face 3 Face 4 Face 5 Face 6 1 – 5 – 6 – 2 face 2 – 6 – 7 – 3 face 3 – 7 – 8 – 4 face 4 – 8 – 5 – 1 face 9-node and 18-node cylindrical element faces Face 1 Face 2 Face 3 Face 4 Face 5 1 – 2 – 3 face 4 – 6 – 5 face 1 – 4 – 5 – 2 face 2 – 5 – 6 – 3 face 3 – 6 – 4 – 1 face Numbering of integration points for output 15 7 8 9 16 4 5 6 14 1 2 3 13 24-node full integration element 16 12-node element 15 14 13 24-node reduced integration element This shows the scheme in the layer closest to the 1–2–3–4 face. The integration points in the second and third layers are numbered consecutively. 28.1.6 AXISYMMETRIC SOLID ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Solid (continuum) elements,” Section 28.1.1 • *SOLID SECTION Overview This section provides a reference to the axisymmetric solid elements available in Abaqus/Standard and Abaqus/Explicit. Conventions Coordinate 1 is , coordinate 2 is the r-direction corresponds to the global x-direction and the z-direction corresponds to the global y-direction. This is important when data must be given in global directions. Coordinate 1 must be greater than or equal to zero. . At Degree of freedom 1 is have an additional degree of freedom, 5, corresponding to the twist angle , degree of freedom 2 is . Generalized axisymmetric elements with twist (in radians). Abaqus does not automatically apply any boundary conditions to nodes located along the symmetry axis. You must apply radial or symmetry boundary conditions on these nodes if desired. In certain situations in Abaqus/Standard it may become necessary to apply radial boundary conditions on nodes that are located on the symmetry axis to obtain convergence in nonlinear problems. Therefore, the application of radial boundary conditions on nodes on the symmetry axis is recommended for nonlinear problems. Point loads and moments, concentrated (nodal) fluxes, electrical currents, and seepage should be given as the value integrated around the circumference (that is, the total value on the ring). Element types Stress/displacement elements without twist CAX3 CAX3H(S) CAX4(S) CAX4H(S) CAX4I(S) 3-node linear 3-node linear, hybrid with constant pressure 4-node bilinear 4-node bilinear, hybrid with constant pressure 4-node bilinear, incompatible modes CAX4IH(S) 4-node bilinear, incompatible modes, hybrid with linear pressure CAX4R 4-node bilinear, reduced integration with hourglass control CAX4RH(S) CAX6(S) CAX6H(S) 4-node bilinear, reduced integration with hourglass control, hybrid with constant pressure 6-node quadratic 6-node quadratic, hybrid with linear pressure CAX6M 6-node modified, with hourglass control CAX6MH(S) 6-node modified, with hourglass control, hybrid with linear pressure CAX8(S) CAX8H(S) CAX8R(S) 8-node biquadratic 8-node biquadratic, hybrid with linear pressure 8-node biquadratic, reduced integration CAX8RH(S) 8-node biquadratic, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2 Additional solution variables The constant pressure hybrid elements have one additional variable and the linear pressure elements have three additional variables relating to pressure. Element types CAX4I and CAX4IH have five additional variables relating to the incompatible modes. Element types CAX6M and CAX6MH have two additional displacement variables. Stress/displacement elements with twist CGAX3(S) 3-node linear CGAX3H(S) 3-node linear, hybrid with constant pressure CGAX4(S) 4-node bilinear CGAX4H(S) CGAX4R(S) CGAX4RH(S) 4-node bilinear, hybrid with constant pressure 4-node bilinear, reduced integration with hourglass control 4-node bilinear, reduced integration with hourglass control, hybrid with constant pressure CGAX6(S) 6-node quadratic CGAX6H(S) CGAX6M(S) 6-node quadratic, hybrid with linear pressure 6-node modified, with hourglass control CGAX6MH(S) 6-node modified, with hourglass control, hybrid with linear pressure CGAX8(S) 8-node biquadratic CGAX8H(S) CGAX8R(S) 8-node biquadratic, hybrid with linear pressure 8-node biquadratic, reduced integration CGAX8RH(S) 8-node biquadratic, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 5 Additional solution variables The constant pressure hybrid elements have one additional variable and the linear pressure elements have three additional variables relating to pressure. Element types CGAX6M and CGAX6MH have three additional displacement variables. Diffusive heat transfer or mass diffusion elements DCAX3(S) DCAX4(S) DCAX6(S) DCAX8(S) 3-node linear 4-node linear 6-node quadratic 8-node quadratic Active degree of freedom 11 Additional solution variables None. Forced convection/diffusion elements DCCAX2(S) 2-node DCCAX2D(S) 2-node with dispersion control DCCAX4(S) 4-node DCCAX4D(S) 4-node with dispersion control Active degree of freedom 11 Additional solution variables None. Coupled thermal-electrical elements DCAX3E(S) DCAX4E(S) DCAX6E(S) 3-node linear 4-node linear 6-node quadratic DCAX8E(S) 8-node quadratic Active degrees of freedom 9, 11 Additional solution variables None. Coupled temperature-displacement elements without twist CAX3T CAX4T(S) CAX4HT(S) CAX4RT 3-node linear displacement and temperature 4-node bilinear displacement and temperature 4-node bilinear displacement and temperature, hybrid with constant pressure 4-node bilinear displacement and temperature, reduced integration with hourglass control CAX4RHT(S) 4-node bilinear displacement and temperature, reduced integration with hourglass control, hybrid with constant pressure CAX6MT 6-node modified displacement and temperature, with hourglass control CAX6MHT(S) CAX8T(S) CAX8HT(S) CAX8RT(S) CAX8RHT(S) 6-node modified displacement and temperature, with hourglass control, hybrid with linear pressure 8-node biquadratic displacement, bilinear temperature 8-node biquadratic displacement, bilinear temperature, hybrid with linear pressure 8-node biquadratic displacement, bilinear temperature, reduced integration 8-node biquadratic displacement, bilinear temperature, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 11 at corner nodes 1, 2 at midside nodes of second-order elements in Abaqus/Standard 1, 2, 11 at midside nodes of the modified displacement and temperature elements in Abaqus/Standard Additional solution variables The constant pressure hybrid elements have one additional variable and the linear pressure elements have three additional variables relating to pressure. Element types CAX6MT and CAX6MHT have two additional displacement variables and one additional temperature variable. Coupled temperature-displacement elements with twist CGAX3T(S) 3-node linear displacement and temperature CGAX3HT(S) 3-node linear displacement and temperature, hybrid with constant pressure CGAX4T(S) 4-node bilinear displacement and temperature CGAX4HT(S) CGAX4RT(S) 4-node bilinear displacement and temperature, hybrid with constant pressure 4-node bilinear displacement and temperature, reduced integration with hourglass control CGAX4RHT(S) 4-node bilinear displacement and temperature, reduced integration with hourglass control, hybrid with constant pressure CGAX6MT(S) 6-node modified displacement and temperature, with hourglass control CGAX6MHT(S) 6-node modified displacement and temperature, with hourglass control, hybrid with constant pressure CGAX8T(S) 8-node biquadratic displacement, bilinear temperature CGAX8HT(S) CGAX8RT(S) 8-node biquadratic displacement, bilinear temperature, hybrid with linear pressure 8-node biquadratic displacement, bilinear temperature, reduced integration CGAX8RHT(S) 8-node biquadratic displacement, bilinear temperature, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 5, 11 at corner nodes 1, 2, 5 at midside nodes of second-order elements 1, 2, 5, 11 at midside nodes of the modified displacement and temperature elements Additional solution variables The constant pressure hybrid elements have one additional variable and the linear pressure elements have three additional variables relating to pressure. Element types CGAX6MT and CGAX6MHT have two additional displacement variables and one additional temperature variable. Pore pressure elements CAX4P(S) CAX4PH(S) CAX4RP(S) CAX4RPH(S) 4-node bilinear displacement and pore pressure 4-node bilinear displacement and pore pressure, hybrid with constant pressure 4-node bilinear displacement and pore pressure, reduced integration with hourglass control 4-node bilinear displacement and pore pressure, reduced integration with hourglass control, hybrid with constant pressure CAX6MP(S) 6-node modified displacement and pore pressure, with hourglass control CAX6MPH(S) CAX8P(S) CAX8PH(S) CAX8RP(S) CAX8RPH(S) 6-node modified displacement and pore pressure, with hourglass control, hybrid with linear pressure 8-node biquadratic displacement, bilinear pore pressure 8-node biquadratic displacement, bilinear pore pressure, hybrid with linear pressure 8-node biquadratic displacement, bilinear pore pressure, reduced integration 8-node biquadratic displacement, bilinear pore pressure, reduced integration, hybrid with linear pressure Active degrees of freedom 1, 2, 8 at corner nodes 1, 2 at midside nodes Additional solution variables The constant pressure hybrid elements have one additional variable relating to the effective pressure stress, and the linear pressure hybrid elements have three additional variables relating to the effective pressure stress to permit fully incompressible material modeling. Element types CAX6MP and CAX6MPH have two additional displacement variables and one additional pore pressure variable. Coupled temperature–pore pressure elements CAX4PT(S) CAX4RPT(S) 4-node bilinear displacement, pore pressure, and temperature 4-node bilinear displacement, pore pressure, and temperature; reduced integration with hourglass control CAX4RPHT(S) 4-node bilinear displacement, pore pressure, and temperature; reduced integration with hourglass control, hybrid with constant pressure Active degrees of freedom 1, 2, 8, 11 Additional solution variables The constant pressure hybrid elements have one additional variable relating to the effective pressure stress to permit fully incompressible material modeling. Acoustic elements ACAX3 3-node linear ACAX4R(E) 4-node linear, reduced integration with hourglass control ACAX4(S) ACAX6(S) ACAX8(S) 4-node linear 6-node quadratic 8-node quadratic Active degree of freedom Additional solution variables None. Piezoelectric elements CAX3E(S) CAX4E(S) CAX6E(S) CAX8E(S) 3-node linear 4-node bilinear 6-node quadratic 8-node biquadratic CAX8RE(S) 8-node biquadratic, reduced integration Active degrees of freedom 1, 2, 9 Additional solution variables None. Nodal coordinates required r, z at Element property definition For element types DCCAX2 and DCCAX2D, you must specify the channel thickness of the element in the (r–z) plane. The default is unit thickness if no thickness is given. For all other elements, you do not need to specify the thickness. Input File Usage: Abaqus/CAE Usage: *SOLID SECTION Property module: Create Section: select Solid as the section Category and Homogeneous as the section Type Element-based loading Distributed loads Distributed loads are available for all elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Distributed load magnitudes are per unit area or per unit volume. They do not need to be multiplied by . Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BR BZ BRNU Body force Body force Body force FL−3 FL−3 FL−3 BZNU Body force FL−3 CENT(S) Not supported FL−4 M−3 T−2 CENTRIF(S) Rotational body force T−2 Body force in radial direction. Body force in axial direction. Nonuniform body force in radial direction with magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user Nonuniform body force in axial direction with magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user , where load (magnitude input Centrifugal as is the mass density per unit volume, is the angular velocity). Not available for pore pressure elements. Centrifugal load (magnitude is input as the angular velocity). , where is GRAV Gravity Not supported Pressure Not supported LT−2 FL−2 FL−2 FL−2 loading Gravity direction (magnitude is acceleration). in specified input as Hydrostatic pressure on face n, linear in global Y. Pressure on face n. on with user face Nonuniform pressure supplied magnitude subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. Not supported FL−5 T2 Stagnation body force in radial and axial directions. Not supported FL−4 T2 Stagnation pressure on face n. 28.1.6–8 HPn(S) Pn PnNU SBF(E) Units Description Load ID (*DLOAD) TRSHRn Abaqus/CAE Load/Interaction Surface traction TRSHRnNU(S) Not supported TRVECn Surface traction TRVECnNU(S) Not supported FL−2 FL−2 FL−2 FL−2 VBF(E) VPn(E) Not supported FL−4 T Not supported FL−3 T Shear traction on face n. Nonuniform shear traction on face and direction n with magnitude supplied subroutine via UTRACLOAD. user General traction on face n. Nonuniform general traction on face and direction n with magnitude supplied subroutine via UTRACLOAD. user Viscous body force in radial and axial directions. Viscous pressure on face n, applying a pressure proportional to the velocity normal to the face and opposing the motion. Foundations Foundations are available for Abaqus/Standard elements with displacement degrees of freedom. They are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE Units Description Fn(S) Elastic foundation FL−3 on foundation face n. Elastic the elastic For CGAX elements foundations are applied to degrees of freedom only. and Distributed heat fluxes Distributed heat fluxes are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Distributed heat flux magnitudes are per unit area or per unit volume. They do not need to be multiplied by . Load ID (*DFLUX) BF Abaqus/CAE Load/Interaction Units Description Body heat flux JL−3 T−1 Heat body flux per unit volume. Load ID (*DFLUX) BFNU(S) Abaqus/CAE Load/Interaction Units Description Body heat flux JL−3 T−1 Sn Surface heat flux JL−2 T−1 SnNU(S) Not supported JL−2 T−1 Nonuniform heat body flux per unit volume with magnitude supplied via user subroutine DFLUX. Heat surface flux per unit area into face n. Nonuniform heat surface flux per unit area into face n with magnitude supplied via user subroutine DFLUX. Film conditions Film conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Abaqus/CAE Load/Interaction Units Description Load ID (*FILM) Fn Surface film condition JL−2 T−1 −1 FnNU(S) Not supported JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on face n. Nonuniform film coefficient and sink temperature (units of ) provided on face n with magnitude supplied via user subroutine FILM. Radiation types Radiation conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*RADIATE) Abaqus/CAE Load/Interaction Units Description Rn Surface radiation Dimensionless Emissivity and sink temperature provided for face n. Distributed flows Distributed flows are available for all elements with pore pressure degrees of freedom. They are specified as described in “Pore fluid flow,” Section 33.4.7. Distributed flow magnitudes are per unit area or per unit volume. They do not need to be multiplied by . Abaqus/CAE Load/Interaction Units Description Not supported F−1 L3T−1 Load ID (*FLOW) Qn(S) QnD(S) Not supported F−1 L3T−1 QnNU(S) Not supported F−1 L3T−1 Seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on face n. Drainage-only seepage provided on face n. coefficient Nonuniform seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on face n with magnitude supplied via user subroutine FLOW. Load ID (*DFLOW) Sn(S) Abaqus/CAE Load/Interaction Units Description Surface pore fluid LT−1 pore Prescribed effective velocity (outward from the face) on face n. fluid SnNU(S) Not supported LT−1 Nonuniform prescribed pore fluid effective velocity (outward from the face) on face n with magnitude supplied via user subroutine DFLOW. Distributed impedances Distributed impedances are available for all elements with acoustic pressure degrees of freedom. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. Load ID (*IMPEDANCE) Abaqus/CAE Load/Interaction Units Description In Not supported None Name of the impedance property that defines the impedance on face n. Electric fluxes Electric fluxes are available for piezoelectric elements. They are specified as described in “Piezoelectric analysis,” Section 6.7.2. Load ID (*DECHARGE) Abaqus/CAE Load/Interaction Units Description EBF(S) ESn(S) Body charge Surface charge CL−3 CL−2 Body flux per unit volume. Prescribed surface charge on face n. Distributed electric current densities Distributed electric current densities are available for coupled thermal-electrical elements. They are specified as described in “Coupled thermal-electrical analysis,” Section 6.7.3. Load ID (*DECURRENT) Load/Interaction Abaqus/CAE Units Description CBF(S) CSn(S) Body current CL−3T−1 Volumetric current source density. Surface current CL−2T−1 Current density on face n. Distributed concentration fluxes Distributed concentration fluxes are available for mass diffusion elements. They are specified as described in “Mass diffusion analysis,” Section 6.9.1. Load ID (*DFLUX) BF(S) BFNU(S) Sn(S) SnNU(S) Abaqus/CAE Load/Interaction Units Description Body concentration flux Body concentration flux Surface concentration flux Surface concentration flux PT−1 PT−1 PLT−1 PLT−1 28.1.6–12 Concentration body flux per unit volume. Nonuniform concentration body flux per unit volume with magnitude supplied via user subroutine DFLUX. Concentration surface flux per unit area into face n. Nonuniform concentration surface flux per unit area into face n with magnitude supplied via user Surface-based loading Distributed loads Surface-based distributed loads are available for all elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Distributed load magnitudes are per unit area or per unit volume. They do not need to be multiplied by . Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description HP(S) PNU Pressure Pressure Pressure FL−2 FL−2 FL−2 SP(E) Pressure FL−4 T2 TRSHR Surface traction TRSHRNU(S) Surface traction FL−2 FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 VP(E) Pressure FL−3 T 28.1.6–13 Hydrostatic pressure on the element surface, linear in global Y. Pressure on the element surface. Nonuniform pressure on the element supplied surface with magnitude subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user Stagnation pressure on the element surface. Shear traction on the element surface. Nonuniform shear traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. General surface. traction on the element Nonuniform general traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. Viscous pressure applied on the element surface. The viscous pressure is proportional to the velocity normal Distributed heat fluxes Surface-based heat fluxes are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Distributed heat flux magnitudes are per unit area or per unit volume. They do not need to be multiplied by . Load ID (*DSFLUX) Abaqus/CAE Load/Interaction Units Description Surface heat flux JL−2 T−1 SNU(S) Surface heat flux JL−2 T−1 Heat surface flux per unit area into the element surface. Nonuniform heat surface flux per unit area into the element surface with magnitude supplied via user subroutine DFLUX. Film conditions Surface-based film conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SFILM) FNU(S) Radiation types Abaqus/CAE Load/Interaction Units Description Surface film condition Surface film condition JL−2 T−1 −1 JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on the element surface. Nonuniform film coefficient and sink temperature (units of ) provided on the element surface with magnitude supplied via user subroutine FILM. Surface-based radiation conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SRADIATE) Abaqus/CAE Load/Interaction Units Description Surface radiation Dimensionless Emissivity and sink temperature provided for the element surface. Distributed flows Surface-based distributed flows are available for all elements with pore pressure degrees of freedom. They are specified as described in “Pore fluid flow,” Section 33.4.7. Distributed flow magnitudes are per unit area or per unit volume. They do not need to be multiplied by . Load ID (*SFLOW) Abaqus/CAE Load/Interaction Units Description Q(S) Not supported F−1 L3T−1 QD(S) Not supported F−1 L3T−1 QNU(S) Not supported F−1 L3T−1 Seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on the element surface. Drainage-only seepage provided on the element surface. coefficient Nonuniform seepage coefficient and reference sink pore pressure (units of FL−2 ) provided on the element surface with magnitude supplied via user subroutine FLOW. Load ID (*DSFLOW) S(S) SNU(S) Abaqus/CAE Load/Interaction Units Description Surface pore fluid Surface pore fluid LT−1 LT−1 pore Prescribed effective velocity outward from the element surface. fluid Nonuniform prescribed pore fluid effective velocity outward from the element surface with magnitude supplied via user subroutine DFLOW. Distributed impedances Surface-based impedances are available for all elements with acoustic pressure degrees of freedom. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. Incident wave loading Surface-based incident wave loads are available for all elements with displacement degrees of freedom or acoustic pressure degrees of freedom. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. If the incident wave field includes a reflection off a plane outside the boundaries of the mesh, this effect can be included. Electric fluxes Surface-based electric fluxes are available for piezoelectric elements. They are specified as described in “Piezoelectric analysis,” Section 6.7.2. Load ID (*DSECHARGE) Load/Interaction Abaqus/CAE Units Description ES(S) Surface charge CL−2 Prescribed surface charge on the element surface. Distributed electric current densities Surface-based electric current densities are available for coupled thermal-electrical elements. They are specified as described in “Coupled thermal-electrical analysis,” Section 6.7.3. Load ID (*DSECURRENT) Load/Interaction Abaqus/CAE Units Description CS(S) Surface current CL−2T−1 Current density on the surface. element Element output Output is in global directions unless a local coordinate system is assigned to the element through the section definition (“Orientations,” Section 2.2.5) in which case output is in the local coordinate system (which rotates with the motion in large-displacement analysis). See “State storage,” Section 1.5.4 of the Abaqus Theory Manual, for details. For regular axisymmetric elements, the local orientation must be in the –z plane with being a principal direction. For generalized axisymmetric elements with twist, the local orientation can be arbitrary. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: For elements with displacement degrees of freedom without twist: S11 S22 S33 S12 Stress in the radial direction or in the local 1-direction. Stress in the axial direction or in the local 2-direction. Hoop direct stress. Shear stress. For elements with displacement degrees of freedom with twist: S11 S22 Stress in the radial direction or in the local 1-direction. Stress in the axial direction or in the local 2-direction. S33 S12 S13 S23 Stress in the circumferential direction or in the local 3-direction. Shear stress. Shear stress. Shear stress. Heat flux components Available for elements with temperature degrees of freedom. HFL1 HFL2 Heat flux in the radial direction or in the local 1-direction. Heat flux in the axial direction or in the local 2-direction. Pore fluid velocity components Available for elements with pore pressure degrees of freedom, except for acoustic elements. FLVEL1 FLVEL2 Pore fluid effective velocity in the radial direction or in the local 1-direction. Pore fluid effective velocity in the axial direction or in the local 2-direction. Mass concentration flux components Available for elements with normalized concentration degrees of freedom. MFL1 MFL2 Concentration flux in the radial direction or in the local 1-direction. Concentration flux in the axial direction or in the local 2-direction. Electrical potential gradient Available for elements with electrical potential degrees of freedom. EPG1 EPG2 Electrical potential gradient in the 1-direction. Electrical potential gradient in the 2-direction. Electrical flux components Available for piezoelectric elements. EFLX1 EFLX2 Electrical flux in the 1-direction. Electrical flux in the 2-direction. Electrical current density components Available for coupled thermal-electrical elements. ECD1 ECD2 Electrical current density in the 1-direction. Electrical current density in the 2-direction. Node ordering and face numbering on elements face 2 face 1 2 - node element face 3 face 3 face 2 face 4 face 2 1 2 face 1 face 1 3 - node element 4 - node element face 3 4 7 3 face 3 6 5 face 2 face 4 face 2 1 face 1 2 face 1 6 - node element 8 - node element 2-node element faces Face 1 Face 2 Section at node 1 Section at node 2 Triangular element faces Face 1 Face 2 Face 3 1 – 2 face 2 – 3 face 3 – 1 face Quadrilateral element faces Face 1 Face 2 Face 3 Face 4 1 – 2 face 2 – 3 face 3 – 4 face 4 – 1 face Numbering of integration points for output 2 - node element 4 - node element 1 2 3 - node element 4 - node reduced integration element 6 5 1 2 6 - node element 4 7 3 4 7 3 8 - node element 8 - node reduced integration element For heat transfer applications a different integration scheme is used for triangular elements, as described in “Triangular, tetrahedral, and wedge elements,” Section 3.2.6 of the Abaqus Theory Manual. 28.1.7 AXISYMMETRIC SOLID ELEMENTS WITH NONLINEAR, ASYMMETRIC DEFORMATION Product: Abaqus/Standard References • “Choosing the element’s dimensionality,” Section 27.1.2 • “Solid (continuum) elements,” Section 28.1.1 • *SOLID SECTION Overview This section provides a reference to the axisymmetric solid elements available in Abaqus/Standard. These elements are intended for analysis of hollow bodies, such as pipes and pressure vessels. They can also be used to model solid bodies, but spurious stresses may occur at zero radius, particularly if transverse shear loads are applied. Conventions Coordinate 1 is r, coordinate 2 is z. Referring to the figures shown in “Choosing the element’s dimensionality,” Section 27.1.2, the r-direction corresponds to the global X-direction in the plane and the negative global Z-direction in the global Y-direction. Coordinate 1 must be greater than or equal to zero. plane, and the z-direction corresponds to the Degree of freedom 1 is you cannot control it. Element types , degree of freedom 2 is . The degree of freedom is an internal variable: Stress/displacement elements CAXA4N Bilinear, Fourier quadrilateral with 4 nodes per r–z plane CAXA4HN CAXA4RN Bilinear, Fourier quadrilateral with 4 nodes per r–z plane, hybrid with constant Fourier pressure Bilinear, Fourier quadrilateral with 4 nodes per r–z plane, reduced integration in r–z planes with hourglass control CAXA4RHN Bilinear, Fourier quadrilateral with 4 nodes per r–z plane, reduced integration in r–z planes, hybrid with constant Fourier pressure CAXA8N Biquadratic, Fourier quadrilateral with 8 nodes per r–z plane CAXA8HN Biquadratic, Fourier quadrilateral with 8 nodes per –z plane, hybrid with linear Fourier pressure CAXA8RN Biquadratic, Fourier quadrilateral with 8 nodes per r–z plane, reduced integration in r–z planes CAXA8RHN Biquadratic, Fourier quadrilateral with 8 nodes per r–z plane, reduced integration in r–z planes, hybrid with linear Fourier pressure Active degrees of freedom 1, 2 Additional solution variables The bilinear elements have 4N and the biquadratic elements 8N additional variables relating to . Element types CAXA4HN and CAXA4RHN have stress. Element types CAXA8HN and CAXA8RHN have stress. additional variables relating to the pressure additional variables relating to the pressure Pore pressure elements CAXA8PN Biquadratic, Fourier quadrilateral with 8 nodes per r–z plane, bilinear Fourier pore pressure CAXA8RPN Biquadratic, Fourier quadrilateral with 8 nodes per r–z plane, bilinear Fourier pore pressure, reduced integration in r–z planes Active degrees of freedom 1, 2, 8 at corner nodes 1, 2 at midside nodes Additional solution variables 8N additional variables relating to . Nodal coordinates required r, z Element property definition Input File Usage: *SOLID SECTION Element-based loading Even though the symmetry in the r–z plane at allows the modeling of half of the initially axisymmetric structure, the loading must be specified as the total load on the full axisymmetric body. Consider, for example, a cylindrical shell loaded by a unit uniform axial force. To produce a unit load on a CAXA element with 4 modes, the nodal forces are 1/8, 1/4, 1/4, 1/4, and 1/8 at , , , , and , respectively. Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Units Description BX BZ BXNU BZNU Pn PnNU HPn FL−3 FL−3 FL−3 FL−3 FL−2 FL−2 FL−2 Body force per unit volume in the global X- direction. Body force per unit volume z-direction. in the Nonuniform body force in the global X-direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in the z-direction with magnitude supplied via user subroutine DLOAD. Pressure on face n. Nonuniform pressure on face n with magnitude supplied via user subroutine DLOAD. Hydrostatic pressure on face n, linear in the global Y-direction. Foundations Foundations are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Units Description Fn FL−3 Elastic foundation on face n. Distributed flows Distributed flows are available for elements with pore pressure degrees of freedom. They are specified as described in “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1. Load ID (*FLOW/ *DFLOW) Units Description Qn F−1 L3T−1 QnD F−1 L3T−1 QnNU F−1 L3T−1 Sn SnNU LT−1 LT−1 Element output (outward flow) normal Seepage proportional to the difference between surface pore pressure and a reference sink pore pressure on face n (units of FL−2 ). Drainage-only seepage (outward normal flow) proportional to the surface pore pressure on face n only when that pressure is positive. Nonuniform seepage (outward normal flow) proportional to the difference between surface pore pressure and a reference sink pore pressure on face n (units of FL−2 ) with magnitude supplied via user subroutine FLOW. Prescribed pore fluid velocity (outward from the face) on face n. Nonuniform prescribed pore fluid velocity (outward from the face) on face n with magnitude supplied via user subroutine DFLOW. equally The numerical integration with respect to spaced integration planes in the element, including the planes, with N being the number of Fourier modes. Consequently, the radial nodal forces corresponding to pressure loads applied in the circumferential direction are distributed in this direction in the ratio of in the 1 Fourier mode element, in the 4 Fourier mode element. The sum of these consistent nodal forces is equal to the integral of the applied pressure over employs the trapezoidal rule. There are and in the 2 Fourier mode element, and . Output is as defined below unless a local coordinate system in the r–z plane is assigned to the element through the section definition (“Orientations,” Section 2.2.5) in which case the components are in the local directions. These local directions rotate with the motion in large-displacement analysis. See “State storage,” Section 1.5.4 of the Abaqus Theory Manual, for details. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S33 S12 S13 S23 Stress in the radial direction or in the local 1-direction. Stress in the axial direction or in the local 2-direction. Hoop direct stress. Shear stress. Shear stress. Shear stress. Node ordering and face numbering on elements The node ordering in the first r–z plane of each element, at , is shown below. Each element must have N more planes of nodes defined, where N is the number of Fourier modes. The node ordering is the same in each plane. You can specify the nodes in each plane. Alternatively, you can specify the node ordering in the first r–z plane of an element, and Abaqus/Standard will generate all other nodes for the element by adding successively a constant offset to each node for each of the N planes of the element. By default, Abaqus/Standard uses an offset of 100000 . face 3 face 4 face 2 face 1 face 3 4 3 face 4 face 1 face 2 4 - node element 8 - node element Element faces Face 1 Face 2 Face 3 Face 4 1 – 2 face 2 – 3 face 3 – 4 face 4 – 1 face Numbering of integration points for output The integration points in the first r–z plane of integration, at points follow in sequence at the r–z integration planes in ascending order of , are shown below. The integration location. 4 - node element 4 - node reduced integration element 4 7 3 4 7 3 8 - node element 8 - node reduced integration element 28.2 Fluid continuum elements • “Fluid (continuum) elements,” Section 28.2.1 • “Fluid element library,” Section 28.2.2 28.2.1 FLUID (CONTINUUM) ELEMENTS Products: Abaqus/CFD Abaqus/CAE References • “Fluid element library,” Section 28.2.2 • “Creating homogeneous fluid sections,” Section 12.13.13 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Fluid elements are provided to discretize the fluid domain. Choosing an appropriate element Three-dimensional fluid elements are available. Naming convention Fluid elements in Abaqus are named as follows: FC 3D 4 number of nodes three-dimensional fluid continuum For example, FC3D8 is a three-dimensional, 8-node brick fluid element. Active fields for fluid elements The fields active in a fluid flow analysis are not determined by the element type but by the analysis procedure and its options. The sole purpose of the element type is to define the shape of the element used to discretize the continuum. 28.2.2 FLUID ELEMENT LIBRARY Products: Abaqus/CFD Abaqus/CAE Reference • “Fluid (continuum) elements,” Section 28.2.1 Overview This section provides a reference to the fluid elements available in Abaqus/CFD. Element types Fluid elements FC3D4 FC3D6 FC3D8 4-node tetrahedron 6-node prism 8-node brick Active degrees of freedom The active degrees of freedom depend on the analysis procedure and options, such as the energy equation and turbulence model. For more information, see “Active degrees of freedom” in “Boundary conditions in Abaqus/CFD,” Section 33.3.2. Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition Input File Usage: Use either of the following options: Abaqus/CAE Usage: *FLUID SECTION *SOLID SECTION Property module: Create Section: select Fluid as the section Element-based loading Distributed loads Distributed loads are available for all fluid element types. They are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BX BY BZ Body force Body force Body force GRAV Gravity FL−3 FL−3 FL−3 LT−2 Body force in global X-direction. Body force in global Y-direction. Body force in global Z-direction. Gravity loading direction (magnitude is acceleration). in specified input as PDBF Porous body force drag None Porous drag body force load (specify porosity as the input). Distributed heat fluxes Distributed heat fluxes are available when the temperature equation is activated on the analysis procedure. They are specified as described in “Thermal loads,” Section 33.4.4. Abaqus/CAE Load/Interaction Units Description Body heat flux JL−3 T−1 Heat body flux per unit volume. Load ID (*DFLUX) BF Surface-based loading Distributed heat fluxes Surface-based heat fluxes are available for all elements when the temperature equation is activated on the analysis procedure. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DSFLUX) Abaqus/CAE Load/Interaction Units Description Surface heat flux JL−2 T−1 Heat surface flux per unit area into the element surface. face 2 face 5 6 - node element face 4 face 1 Element output Element output is always in the global directions. Node ordering and face numbering on elements All elements face 4 face 2 face 3 face 3 face 1 4 - node element face 2 face 5 face 6 face 4 face 1 face 3 8 - node element 28.2.2–3 Tetrahedral element faces Face 1 Face 2 Face 3 Face 4 1 – 3 – 2 face 1 – 2 – 4 face 2 – 3 – 4 face Wedge (triangular prism) element faces Face 1 Face 2 Face 3 Face 4 Face 5 1 – 3 – 2 face 4 – 5 – 6 face 1 – 2 – 5 – 4 face 2 – 3 – 6 – 5 face 1 – 4 – 6 – 3 face Hexahedron (brick) element faces Face 1 Face 2 Face 3 Face 4 Face 5 Face 6 1 – 4 – 3 – 2 face 5 – 6 – 7 – 8 face 1 – 2 – 6 – 5 face 2 – 3 – 7 – 6 face 3 – 4 – 8 – 7 face 1 – 5 – 8 – 4 face 28.3 Infinite elements • “Infinite elements,” Section 28.3.1 • “Infinite element library,” Section 28.3.2 28.3.1 INFINITE ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Infinite element library,” Section 28.3.2 • *SOLID SECTION • “Creating acoustic infinite sections,” Section 12.13.17 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Infinite elements: • are used in boundary value problems defined in unbounded domains or problems in which the region of interest is small in size compared to the surrounding medium; • are usually used in conjunction with finite elements; • can have linear behavior only; • provide stiffness in static solid continuum analyses; and • provide “quiet” boundaries to the finite element model in dynamic analyses. A solid section definition is used to define the section properties of infinite elements. Typical applications The analyst is sometimes faced with boundary value problems defined in unbounded domains or problems in which the region of interest is small in size compared to the surrounding medium. Infinite elements are intended to be used for such cases in conjunction with first- and second-order planar, axisymmetric, and three-dimensional finite elements. Standard finite elements should be used to model the region of interest, with the infinite elements modeling the far-field region. Choosing an appropriate element Plane stress, plane strain, three-dimensional, and axisymmetric infinite elements are available. Reduced- integration elements are also available in Abaqus/Standard. Element type CIN3D18R is intended for use with the three-dimensional variable-number-of-node solids C3D15V, C3D27, and C3D27R in Abaqus/Standard. Acoustic infinite elements are also available in Abaqus. Naming convention Infinite elements in Abaqus are named as follows: CIN PS 5 R reduced integration (optional) number of user nodes plane strain (PE), plane stress (PS), two-dimensional (2D) three-dimensional (3D), or axisymmetric (AX) continuum infinite element acoustic (optional) For example, CINAX4 is a 4-node, axisymmetric, infinite element. Defining the element’s section properties You use a solid section definition to define the section properties. You must associate these properties with a region of your model. Input File Usage: *SOLID SECTION, ELSET=name where the ELSET parameter refers to a set of infinite elements. Abaqus/CAE Usage: Only acoustic infinite sections are supported in Abaqus/CAE. Property module: Create Section: select Other as the section Category and Acoustic infinite as the section Type Assign→Section: select regions Defining the thickness for plane strain and plane stress elements You define the thickness for plane strain and plane stress elements as part of the section definition. If you do not specify a thickness, unit thickness is assumed. Input File Usage: *SOLID SECTION thickness Abaqus/CAE Usage: Structural infinite sections are not supported in Abaqus/CAE. Defining the reference point and thickness for acoustic infinite elements For acoustic infinite elements you specify the thickness and the reference point. The thickness is ignored in three-dimensional and axisymmetric elements. You can prescribe the reference point either as a reference node on the section definition or directly by giving its coordinates on the data line following the thickness value. If both methods are used, the former takes precedence. If you do not define the reference point at all, an error message is issued. acoustic infinite elements, as shown in Figure 28.3.1–1. INFINITE ELEMENTS reference point (X ) radius (R ) node (X ) node ray (n ) Figure 28.3.1–1 Reference point and node rays for acoustic infinite elements. Each node ray is a unit vector in the direction of the line between the reference point and the node. These radii and rays are used in the formulation of acoustic infinite elements. The placement of the reference point is not extremely critical as long as it is near the center of the finite region enclosed by the infinite elements. If acoustic infinite elements are placed on the surface of a sphere, the optimal location for the reference point is the center of the sphere. Acoustic infinite elements whose section properties are defined using a particular solid section definition should not have any nodes in common with acoustic infinite elements associated with a different solid section definition. This is to ensure a unique reference point (and, therefore, a unique “radius” and “node ray”) for each acoustic infinite element node. The node rays are used to compute “cosine” values at each node of the infinite element interface. The “cosine” is equal to the smallest dot product of the unit node ray and the unit normals of all acoustic infinite element faces surrounding the node . An error message is issued for negative values of “cosine.” Both the “radius” and “cosine” for all nodes of acoustic infinite elements are printed to the data (.dat) file as nodal (model) data. For details of how these quantities are used in the formulation, see “Acoustic infinite elements,” Section 3.3.2 of the Abaqus Theory Manual. Input File Usage: *SOLID SECTION, REF NODE=node number or node set name thickness nj n2 n3 n1 X R nj n2 n3 n1 cosine Figure 28.3.1–2 Defining the cosine for acoustic infinite elements. Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Acoustic infinite as the section Type: Plane stress/strain thickness: thickness Acoustic infinite sections must be assigned to regions of parts that have a reference point associated with them. To define the reference point: Part module or Property module: Tools→Reference Point: select reference point Defining the order of interpolation for acoustic infinite elements For acoustic infinite elements the variation of the acoustic field in the infinite direction is given by functions that are members of a set of 10 ninth-order polynomials (for further details, see “Acoustic infinite elements,” Section 3.3.2 of the Abaqus Theory Manual). The members of this set are constructed to correspond to the Legendre modes of a sphere; that is, if infinite elements are placed on a sphere and if tangential refinement is adequate, an ith order acoustic infinite element will absorb waves associated with the ( )th Legendre mode. The computational cost involved in using all 10 members in this set of polynomials to resolve the variation of the acoustic field in the infinite direction may be significant in certain applications in Abaqus/Explicit. In such cases you may wish to include only the first few members of the set, although you should be aware of the possibility of degraded accuracy (i.e., increased reflection at acoustic infinite elements) due to using a reduced set of polynomials. In Abaqus/Explicit you can specify the number, N, of ninth-order polynomials to be used. By default, all 10 members of the set will be used; all 10 are always used in Abaqus/Standard. Specifying a value less than 10 would result in the first N members of the set being used to model the variation of the acoustic field in the infinite direction. Input File Usage: Abaqus/CAE Usage: *SOLID SECTION, ORDER=N Property module: Create Section: select Other as the section Category and Acoustic infinite as the section Type: Order: N Assigning a material definition to a set of infinite elements You must associate a material definition with each infinite element section definition. Optionally, you can associate a material orientation definition with the section . The solution in the far field is assumed to be linear, so that only linear behavior can be associated with infinite elements (“Linear elastic behavior,” Section 22.2.1). In dynamic analysis the material response in the infinite elements is also assumed to be isotropic. In Abaqus/Explicit the material properties assigned to the infinite elements must match the material properties of the adjacent finite elements in the linear domain. Only an acoustic medium material (“Acoustic medium,” Section 26.3.1) is valid for acoustic infinite elements. Input File Usage: Abaqus/CAE Usage: *SOLID SECTION, MATERIAL=name, ORIENTATION=name Only acoustic infinite sections are supported in Abaqus/CAE. Property module: Create Section: select Other as the section Category and Acoustic infinite as the section Type: Material: name Assign→Material Orientation: select regions Assign→Section: select regions Defining nodes for solid medium infinite elements The node numbering for infinite elements must be defined such that the first face is the face that is connected to the finite element part of the mesh. The infinite element nodes that are not part of the first face are treated differently in explicit dynamic analysis than in other procedures. These nodes are located away from the finite element mesh in the infinite direction. The location of these nodes is not meaningful for explicit analysis, and loads and boundary conditions must not be specified using these nodes in explicit dynamic procedures. In other procedures these outer nodes are important in the element definition and can be used in load and boundary condition definitions. Except for explicit procedures, the basis of the formulation of the solid medium elements is that the far-field solution along each element edge that stretches to infinity is centered about an origin, called the “pole.” For example, the solution for a point load applied to the boundary of a half-space has its pole at the point of application of the load. It is important to choose the position of the nodes in the infinite direction appropriately with respect to the pole. The second node along each edge pointing in the infinite direction must be positioned so that it is twice as far from the pole as the node on the same edge at the boundary between the finite and the infinite elements. Three examples of this are shown in Figure 28.3.1–3, Figure 28.3.1–4, and Figure 28.3.1–5. In addition to this length consideration, you must specify the second nodes in the infinite direction such that the element edges in the infinite direction do not cross over, which would give nonunique mappings . Abaqus will stop with an error message if such problems occur. A convenient way of defining these second nodes in the infinite direction is to project the original nodes from a pole node; see “Projecting the nodes in the old set from a pole node” in “Node definition,” Section 2.1.1. The positions of the pole and of the nodes on the boundary between the finite and the infinite elements are used. CAX8R CINAX5R CL Figure 28.3.1–3 Point load on elastic half-space. CPE4R CINPE4 CL Figure 28.3.1–4 Strip footing on infinitely extending layer of soil. CPS4 CINPS4 Figure 28.3.1–5 Quarter plate with square hole. Figure 28.3.1–6 Examples of an acceptable and an unacceptable two-dimensional infinite element. Defining nodes for acoustic infinite elements The nodes of acoustic infinite elements need to be defined only for the face that is connected to the finite element part of the mesh. Additional nodes are generated internally by Abaqus in the direction of the “node ray” . The node rays, which are discussed earlier in this section in the context of defining the reference point, define the sides of the acoustic infinite elements. Using solid medium infinite elements in plane stress and plane strain analyses the far-field In plane stress and plane strain analyses when the loading is not self-equilibrating, displacements typically have the form , where r is distance from the origin. This form implies that the displacement approaches infinity as . Infinite elements will not provide a unique displacement solution for such cases. Experience shows, however, that they can still be used, provided that the displacement results are treated as having an arbitrary reference value. Thus, strain, stress, and relative displacements within the finite element part of the model will converge to unique values as the model is refined; the total displacements will depend on the size of the region modeled with finite If the loading is self-equilibrating, the total displacements will also converge to a unique elements. solution. Using solid medium infinite elements in dynamic analyses In direct-integration implicit dynamic response analysis (“Implicit dynamic analysis using direct integration,” Section 6.3.2), steady-state dynamic frequency domain analysis (“Direct-solution steady-state dynamic analysis,” Section 6.3.4), matrix generation (“Generating matrices,” Section 10.3.1), superelement generation (“Using substructures,” Section 10.1.1), and explicit infinite elements provide “quiet” dynamic analysis (“Explicit dynamic analysis,” Section 6.3.3), boundaries to the finite element model through the effect of a damping matrix; the stiffness matrix of the element is suppressed. The elements do not provide any contribution to the eigenmodes of the system. The elements maintain the static force that was present at the start of the dynamic response analysis on this boundary; as a consequence, the far-field nodes in the infinite elements will not displace during the dynamic response. During dynamic steps the infinite elements introduce additional normal and shear tractions on the finite element boundary that are proportional to the normal and shear components of the velocity of the boundary. These boundary damping constants are chosen to minimize the reflection of dilatational and shear wave energy back into the finite element mesh. This formulation does not provide perfect transmission of energy out of the mesh except in the case of plane body waves impinging orthogonally on the boundary in an isotropic medium. However, it usually provides acceptable modeling for most practical cases. During dynamic response analysis the infinite elements hold the static stress on the boundary constant but do not provide any stiffness. Therefore, some rigid body motion of the region modeled will generally occur. This effect is usually small. Optimizing the transmission of energy out of the finite element mesh For dynamic cases the ability of the infinite elements to transmit energy out of the finite element mesh, without trapping or reflecting it, is optimized by making the boundary between the finite and infinite elements as close as possible to being orthogonal to the direction from which the waves will impinge on this boundary. Close to a free surface, where Rayleigh waves may be important, or close to a material interface, where Love waves may be important, the infinite elements are most effective if they are orthogonal to the surface. (Rayleigh and Love waves are surface waves that decay with distance from the surface.) For acoustic medium infinite elements, these general guidelines apply as well. Defining an initial stress field and corresponding body force field In many applications, especially geotechnical problems, an initial stress field and a corresponding body force field must be defined. For standard elements you define the initial stress field as an initial condition (“Defining initial stresses” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1) and the corresponding body force field as a distributed load (“Distributed loads,” Section 33.4.3). The body force cannot be defined for infinite elements since the elements are of infinite extent. Therefore, Abaqus automatically inserts forces at the nodes of the infinite elements that cause those nodes to be in static equilibrium at the start of the analysis. These forces remain constant throughout the analysis. This capability allows the initial geostatic stress field to be defined in the infinite elements, but it does not check whether or not the geostatic stress field is reasonable. If the initial stress field is due to a body force loading (such as gravity loading), this loading must be held constant during the step. In multistep analyses it must be maintained constant over all steps. You must remember that when infinite elements are used in conjunction with an initial stress condition, it is essential that the initial stress field be in equilibrium. In Abaqus/Standard any procedure that determines the initial static (steady-state) equilibrium conditions is suitable as the first step of the analysis; for example, static (“Static stress analysis,” Section 6.2.2); geostatic stress field (“Geostatic stress state,” Section 6.8.2); coupled pore fluid diffusion/stress (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1); and steady-state fully coupled thermal-stress (“Fully coupled thermal-stress analysis,” Section 6.5.3) steps can be used. To check for equilibrium in Abaqus/Explicit, perform an initial step with no loading (except for the body forces that created the initial stress field) and verify that the accelerations are small. 28.3.2 INFINITE ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Infinite elements,” Section 28.3.1 • *SOLID SECTION Overview This section provides a reference to the infinite elements available in Abaqus/Standard and Abaqus/Explicit. Element types Plane strain solid continuum infinite elements CINPE4 4-node linear, one-way infinite CINPE5R(S) 5-node quadratic, one-way infinite Active degrees of freedom 1, 2 Additional solution variables None. Plane stress solid continuum infinite elements CINPS4 4-node linear, one-way infinite CINPS5R(S) 5-node quadratic, one-way infinite Active degrees of freedom 1, 2 Additional solution variables None. 3-D solid continuum infinite elements CIN3D8 8-node linear, one-way infinite CIN3D12R(S) 12-node quadratic, one-way infinite CIN3D18R(S) 18-node quadratic, one-way infinite Active degrees of freedom 1, 2, 3 Additional solution variables None. Axisymmetric solid continuum infinite elements CINAX4 4-node linear, one-way infinite CINAX5R(S) 5-node quadratic, one-way infinite Active degrees of freedom 1, 2 Additional solution variables None. 2-D acoustic infinite elements ACIN2D2 2-node linear, acoustic infinite ACIN2D3(S) 3-node quadratic, acoustic infinite Active degree of freedom 3-D acoustic infinite elements ACIN3D3 3-node linear, acoustic infinite triangular element ACIN3D4 4-node linear, acoustic infinite quadrilateral element ACIN3D6(S) ACIN3D8(S) 6-node quadratic, acoustic infinite triangular element 8-node quadratic, acoustic infinite quadrilateral element Active degree of freedom Axisymmetric acoustic infinite elements ACINAX2 2-node linear, acoustic infinite ACINAX3(S) 3-node quadratic, acoustic infinite Active degree of freedom Nodal coordinates required Plane stress and plane strain solid continuum elements: X, Y 2-D acoustic elements: X, Y 3-D solid continuum and acoustic elements: X, Y, Z Axisymmetric solid continuum and acoustic elements: r, z Normal directions are not specified at nodes used in acoustic infinite elements; they will be computed automatically. See “Infinite elements,” Section 28.3.1, for details. Element property definition For two-dimensional, plane strain, and plane stress elements, you must provide the thickness of the elements; by default, unit thickness is assumed. For three-dimensional and axisymmetric solid elements, you do not need to specify a thickness. For acoustic elements, you must specify the reference point in addition to the thickness. Input File Usage: Abaqus/CAE Usage: *SOLID SECTION Only acoustic infinite sections are supported in Abaqus/CAE. Property module: Create Section: select Other as the section Category and Acoustic infinite as the section Type Element-based loading None. Element output Stress, strain, and other tensor components No output is available from Abaqus/Explicit for infinite elements. Stress and other tensors (including strain tensors) are available from Abaqus/Standard for infinite elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S33 S12 S13 S23 direct stress or radial stress for axisymmetric elements. direct stress or axial stress for axisymmetric elements. direct stress (not available for plane stress elements) or hoop stress for axisymmetric elements. shear stress or shear stress for axisymmetric elements. shear stress (not available for plane stress, plane strain, and axisymmetric elements). shear stress (not available for plane stress, plane strain, and axisymmetric elements). Node ordering and face numbering on elements Plane stress and plane strain solid continuum elements CINPS4 CINPE4 CINPS5R CINPE5R Axisymmetric solid continuum elements CINAX4 CINAX5R INFINITE ELEMENTS CIN3D8 12 11 10 CIN3D12R 16 13 12 15 18 17 11 14 10 CIN3D18R Two-dimensional and axisymmetric acoustic infinite elements E1 E2 SPOS E1 SPOS E2 ACIN2D2 ACIN2D3 E1 E1 E2 SPOS ACINAX2 SPOS ACINAX3 E2 INFINITE ELEMENTS E3 SPOS E2 E1 ACIN3D3 E3 SPOS E2 E1 ACIN3D6 E3 E4 SPOS E2 E1 ACIN3D4 E3 E2 E4 SPOS E1 ACIN3D8 Numbering of integration points for output Plane stress and plane strain solid continuum elements CINPS4 CINPE4 CINPS5R CINPE5R Axisymmetric solid continuum elements CINAX4 CINAX5R Three-dimensional solid continuum elements 4 7 3 CIN3D8 CIN3D12R 4 7 3 CIN3D18R This shows the scheme in the layer closest to the 1–2–3–4 face. The integration points in the second layer are numbered consecutively. 28.4 Warping elements • “Warping elements,” Section 28.4.1 • “Warping element library,” Section 28.4.2 28.4.1 WARPING ELEMENTS Product: Abaqus/Standard References • “Meshed beam cross-sections,” Section 10.6.1 • *SOLID SECTION Overview Warping elements: • are used to model an arbitrarily shaped beam cross-section profile for use with Timoshenko beams; • are used in conjunction with the beam section generation procedure described in “Meshed beam cross-sections,” Section 10.6.1; and • model linear elastic behavior only. Typical applications Warping elements are special-purpose elements that are used to discretize a two-dimensional model of a beam cross-section. This two-dimensional cross-section model is used in Abaqus/Standard to calculate the out-of-plane component of the warping function, as well as relevant sectional stiffness and mass properties that are required in a subsequent beam analysis in either Abaqus/Standard or Abaqus/Explicit. Applications include any structure whose overall behavior is beam-like, yet the cross-section is non- standard or includes multiple materials. Examples include the cross-section of a ship for performing whipping analysis, a beam model of an airfoil-shaped rotor blade or wing, a laminated I-beam, etc. Choosing an appropriate element To mesh an arbitrarily shaped solid beam cross-section Abaqus/Standard offers two elements: a 3-node linear triangle, WARP2D3, and a 4-node bilinear quadrilateral, WARP2D4. Adjacent elements in the cross-sectional mesh must share common nodes; mesh refinement using multi-point constraints is not allowed. Naming convention Warping elements are named as follows: WARP 2D 3 number of nodes two-dimensional warping elements For example, WARP2D4 is 4-node warping element in two dimensions. Defining the element’s section properties You use a solid section definition to define the section properties. You must associate these properties with a region of your model. No additional data are necessary. Input File Usage: *SOLID SECTION, ELSET=name where the ELSET parameter refers to a set of warping elements. Assigning a material definition to a set of warping elements You must associate a linear elastic material definition with each warping element section definition. Optionally, you can associate a material orientation definition with the section . Only isotropic linear elasticity (“Defining isotropic elasticity” in “Linear elastic behavior,” Section 22.2.1) or orthotropic linear elasticity for warping elements (“Defining orthotropic elasticity for warping elements” in “Linear elastic behavior,” Section 22.2.1) are valid material models for warping elements. Input File Usage: *SOLID SECTION, ELSET=name, MATERIAL=name, ORIENTATION=name 28.4.2 WARPING ELEMENT LIBRARY Product: Abaqus/Standard References • “Meshed beam cross-sections,” Section 10.6.1 • *SOLID SECTION Overview This section provides a reference to the warping elements available in Abaqus/Standard. Element types WARP2D3 3-node linear two-dimensional warping element WARP2D4 4-node bilinear two-dimensional warping element Active degree of freedom 3, representing the out-of-plane warping function Additional solution variables None. Nodal coordinates required X, Y Element property definition Input File Usage: *SOLID SECTION Element-based loading There is no loading for these element types. Element output No output is available for these element types. The two-dimensional warping elements are used to calculate the out-of-plane warping function for beams using a meshed cross-section. This warping function can be viewed in the Visualization module of Abaqus/CAE. The derivatives of the warping function are used to calculate the shear strain and stress at the integration points of the elements due to torsion. Node ordering on elements 1 2 3 - node element 4 - node element Numbering of integration points for output 1 2 3 - node element 4 - node element 28.5 Particle elements • “Particle elements,” Section 28.5.1 • “Particle element library,” Section 28.5.2 28.5.1 PARTICLE ELEMENTS Product: Abaqus/Explicit References • “Smoothed particle hydrodynamic analysis,” Section 15.1.1 • “Particle element library,” Section 28.5.2 • *SOLID SECTION Overview Continuum particle elements: • can be used only in explicit dynamic analyses; • must have one node only; • have one integration point; • can be initialized similarly to continuum elements; and • are fully filled with material. Typical applications Continuum particle elements (PC3D) are useful for simulations involving material that undergoes extreme deformation such as open-surface fluid flow or obliteration/fragmentation of solid structures. They are defined using only one node; however, the element centered at a given node (particle) receives contributions from all particles within a sphere of influence whose radius is commonly referred to as the smoothing length. The smoothed particle hydrodynamic (SPH) formulation determines at every increment of the analysis the connectivity associated with a given particle. Since nodal connectivity is not fixed, severe element distortion is avoided and, hence, the formulation allows for very high strain gradients. The 1-node PC3D element is used to define points both on the surface and in the interior of the body to be modeled. You define these nodes similarly to mass elements, and the nodes can be placed in space the same as the nodes of a regular brick mesh. A smoothed particle hydrodynamic mesh is typically a uniformly spaced grid of elements that conforms to the shape of the body being modeled. For more information, see “Smoothed particle hydrodynamic analysis,” Section 15.1.1. Defining the element’s section properties You must associate a solid section definition with a set of continuum particle elements. The section definition provides the material associated with the PC3D elements. As part of the solid section definition, you can define a characteristic length. This characteristic length, not to be confused with the smoothing length, is used to compute the particle volume. The volume is assumed to be a cube whose sides are equal to twice the specified characteristic length. Input File Usage: *SOLID SECTION, ELSET=element_set_name characteristic length associated with the particle volume where the ELSET parameter refers to a set of particle elements. 28.5.2 PARTICLE ELEMENT LIBRARY Product: Abaqus/Explicit References • “Smoothed particle hydrodynamic analysis,” Section 15.1.1 • “Particle elements,” Section 28.5.1 • *SOLID SECTION Overview This section provides a reference to the particle elements available in Abaqus/Explicit. Element type Stress/displacement element PC3D 1-node continuum particle Active degrees of freedom 1, 2, 3 Nodal coordinates required X, Y, Z Element property definition Input File Usage: *SOLID SECTION Element-based loading Distributed loads Gravity loads as described in “Distributed loads,” Section 33.4.3, are the only distributed loads that are available for particle elements. You define gravity loading in a specified direction, and the magnitude is input as acceleration. Element output Output is in global directions unless a local coordinate system is assigned to the element through the section definition (“Orientations,” Section 2.2.5), in which case output is in the local coordinate system (which rotates with the motion in large-displacement analysis). See “State storage,” Section 1.5.4 of the Abaqus Theory Manual, for details. Stress, strain, and other tensor components Stress, strain, and other tensors are available. All tensors have the same components. For example, the stress components are as follows: S11 S22 S33 S12 S13 S23 , direct stress. , direct stress. , direct stress. , shear stress. , shear stress. , shear stress. Note: the order shown above is not the same as that used in user subroutine VUMAT. Nodes associated with the element 1 node. Structural Elements Membrane elements Truss elements Beam elements Frame elements Elbow elements Shell elements STRUCTURAL ELEMENTS 29.1 29.2 29.3 29.4 29.5 29.1 Membrane elements • “Membrane elements,” Section 29.1.1 • “General membrane element library,” Section 29.1.2 • “Cylindrical membrane element library,” Section 29.1.3 • “Axisymmetric membrane element library,” Section 29.1.4 29.1.1 MEMBRANE ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “General membrane element library,” Section 29.1.2 • “Cylindrical membrane element library,” Section 29.1.3 • “Axisymmetric membrane element library,” Section 29.1.4 • *MEMBRANE SECTION • *NODAL THICKNESS • *DISTRIBUTION • *HOURGLASS STIFFNESS • “Creating membrane sections,” Section 12.13.8 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Membrane elements: • are surface elements that transmit in-plane forces only (no moments); and • have no bending stiffness. Typical applications Membrane elements are used to represent thin surfaces in space that offer strength in the plane of the element but have no bending stiffness; for example, the thin rubber sheet that forms a balloon. In addition, they are often used to represent thin stiffening components in solid structures, such as a reinforcing layer in a continuum. (If the reinforcing layer is made up of chords, rebar should be used. See “Defining rebar as an element property,” Section 2.2.4.) Choosing an appropriate element In addition to the general membrane elements available in both Abaqus/Standard and Abaqus/Explicit, cylindrical membrane elements and axisymmetric membrane elements are available in Abaqus/Standard only. General membrane elements General membrane elements should be used in three-dimensional models in which the deformation of the structure can evolve in three dimensions. Cylindrical membrane elements Cylindrical membrane elements are available in Abaqus/Standard for precise modeling of regions in a structure with circular geometry, such as a tire. The elements make use of trigonometric functions to interpolate displacements along the circumferential direction and use regular isoparametric interpolation in the radial or cross-sectional plane. They use three nodes along the circumferential direction and can span a 0 to 180° segment. Elements with both first-order and second-order interpolation in the cross- sectional plane are available. The geometry of the element is defined by specifying nodal coordinates in a global Cartesian system. The default nodal output is also provided in a global Cartesian system. Output of stress, strain, and other material point quantities is done in a corotational system that rotates with the average material rotation. The cylindrical elements can be used in the same mesh with regular elements. In particular, regular membrane elements can be connected directly to the nodes on the cross-sectional edge of cylindrical elements. For example, any edge of an M3D4 element can share nodes with the cross-sectional edges of an MCL6 element. Compatible cylindrical solid elements (“Cylindrical solid element library,” Section 28.1.5) and surface elements with rebar (“Surface elements,” Section 32.7.1) are available for use with cylindrical membrane elements. Axisymmetric membrane elements The axisymmetric membrane elements available in Abaqus/Standard are divided into two categories: those that do not allow twist about the symmetry axis and those that do. These elements are referred to as the regular and generalized axisymmetric membrane elements, respectively. The generalized axisymmetric membrane elements (axisymmetric membrane elements with twist) allow a circumferential component of loading or material anisotropy, which may cause twist about the symmetry axis. Both the circumferential load component and material anisotropy are independent of the circumferential coordinate . Since there is no dependence of the loading or the material on the circumferential coordinate, the deformation is axisymmetric. The generalized axisymmetric membrane elements cannot be used in dynamic or eigenfrequency extraction procedures. Naming convention The naming convention for membrane elements depends on the element dimensionality. General membrane elements General membrane elements in Abaqus are named as follows: 3D 4 R reduced integration (optional) number of nodes three-dimensional membrane For example, M3D4R is a three-dimensional, 4-node membrane element with reduced integration. Cylindrical membrane elements Cylindrical membrane elements in Abaqus/Standard are named as follows: M CL 6 number of nodes cylindrical membrane For example, MCL6 is a 6-node cylindrical membrane element with circumferential interpolation. Axisymmetric membrane elements Axisymmetric membrane elements in Abaqus/Standard are named as follows: G AX 2 order of interpolation axisymmetric generalized (optional) membrane For example, MAX2 is a regular axisymmetric, quadratic-interpolation membrane element. Element normal definition The “top” surface of a membrane is the surface in the positive normal direction (defined below) and is called the SPOS face for contact definition. The “bottom” surface is in the negative direction along the normal and is called the SNEG face for contact definition. General membrane elements For general membrane elements the positive normal direction is defined by the right-hand rule going around the nodes of the element in the order that they are specified in the element definition. See Figure 29.1.1–1. face SPOS face SNEG Figure 29.1.1–1 Positive normals for general membranes. Cylindrical membrane elements For cylindrical membrane elements the positive normal direction is defined by the right-hand rule going around the nodes of the element in the order that they are specified in the element definition. See Figure 29.1.1–2. Axisymmetric membrane elements For axisymmetric membrane elements the positive normal is defined by a 90° counterclockwise rotation from the direction going from node 1 to node 2. See Figure 29.1.1–3. Defining the element’s section properties You use a membrane section definition to define the section properties. You must associate these properties with a region of your model. Input File Usage: *MEMBRANE SECTION, ELSET=name where the ELSET parameter refers to a set of membrane elements. Abaqus/CAE Usage: Property module: Create Section: select Shell as the section Category and Membrane as the section Type Assign→Section: select regions face SNEG face SPOS Figure 29.1.1–2 Positive normals for cylindrical membranes. face SPOS face SNEG Figure 29.1.1–3 Positive normals for axisymmetric membranes. Defining a constant section thickness You can define a constant section thickness as part of the section definition. Input File Usage: *MEMBRANE SECTION, ELSET=name thickness Abaqus/CAE Usage: Property module: Create Section: select Shell as the section Category and Membrane as the section Type: Membrane thickness: thickness Defining a variable thickness using distributions In Abaqus/Standard you can define a spatially varying thickness for membranes using a distribution (“Distribution definition,” Section 2.8.1). The distribution used to define membrane thickness must have a default value. The default thickness is used by any membrane element assigned to the membrane section that is not specifically assigned a value in the distribution. If the membrane thickness is defined for a membrane section with a distribution, nodal thicknesses cannot be used for that section definition. Input File Usage: Use the following option to define a spatially varying thickness: *MEMBRANE SECTION, MEMBRANE THICKNESS=distribution name Defining a continuously varying thickness Alternatively, you can define a continuously varying thickness over the element. In this case any constant section thickness you specify will be ignored, and the section thickness will be interpolated from the specified nodal values . The thickness must be defined at all nodes connected to the element. If the membrane thickness is defined for a membrane section with a distribution, nodal thicknesses cannot be used for that section definition. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *MEMBRANE SECTION, NODAL THICKNESS *NODAL THICKNESS Continuously varying membrane Abaqus/CAE. thicknesses are not supported in Assigning a material definition to a set of membrane elements You must associate a material definition with each membrane section definition. Optionally, you can associate a material orientation definition with the section . An arbitrary material orientation is valid only for general membrane elements and axisymmetric membrane elements with twist. You can define other directions by defining a local orientation, except for MAX1 and MAX2 elements (“Axisymmetric membrane element library,” Section 29.1.4), which do not support orientations. In Abaqus/Standard if the orientation assigned to a membrane section is defined with distributions, spatially varying local coordinate systems are applied to all membrane elements associated with the membrane section. A default local coordinate system (as defined by the distributions) is applied to any membrane element that is not specifically included in the associated distribution. Input File Usage: Abaqus/CAE Usage: *MEMBRANE SECTION, MATERIAL=name, ORIENTATION=name Property module: Create Section: select Shell as the section Category and Membrane as the section Type: Material: name Assign→Material Orientation Specifying how the membrane thickness changes with deformation You can define how the membrane thickness will change with deformation by specifying a nonzero value for the section Poisson’s ratio that will allow for a change in the thickness of the membrane as a function of the in-plane strains in geometrically nonlinear analysis . Alternatively in Abaqus/Explicit, you can choose to have the thickness change computed through integration of the thickness-direction strain that is based on the element material definition and the plane stress condition. The value of the effective Poisson’s ratio for the section must be between −1.0 and 0.5. By default, the section Poisson’s ratio is 0.5 in Abaqus/Standard to enforce incompressibility of the element; in Abaqus/Explicit the default thickness change is based on the element material definition. A section Poisson’s ratio of 0.0 means that the thickness will not change. Values between 0.0 and 0.5 mean that the thickness changes proportionally between the limits of no thickness change and incompressibility, respectively. A negative value of the section Poisson’s ratio will result in an increase of the section thickness in response to tensile strains. Input File Usage: Use one of the following options: *MEMBRANE SECTION, POISSON= *MEMBRANE SECTION, POISSON=MATERIAL (available in Abaqus/Explicit only) Abaqus/CAE Usage: Property module: Create Section: select Shell as the section Category and Membrane as the section Type: Section Poisson's ratio: Use analysis default or Specify value: Specifying nondefault hourglass control parameters for reduced-integration membrane elements See “Methods for suppressing hourglass modes” in “Section controls,” Section 27.1.4, for more information about hourglass control. Specifying a nondefault hourglass control formulation or scale factors You can specify a nondefault hourglass control formulation or scale factors for reduced-integration membrane elements. The nondefault enhanced hourglass control formulation is available only for M3D4R elements. Input File Usage: Use the following option to specify a nondefault hourglass control formulation in a section control definition: *SECTION CONTROLS, NAME=name, HOURGLASS=hourglass_control_formulation Use the following option to associate the section control definition with the membrane section: *MEMBRANE SECTION, CONTROLS=name Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass control: hourglass_control_formulation Specifying nondefault hourglass stiffness factors In Abaqus/Standard you can specify nondefault hourglass stiffness factors based on the default total stiffness approach for reduced-integration general membrane elements. These stiffness factors are ignored for axisymmetric membrane elements. There are no hourglass stiffness factors or scale factors for the nondefault enhanced hourglass control formulation. Input File Usage: Use both of the following options: *MEMBRANE SECTION *HOURGLASS STIFFNESS Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Hourglass stiffness: Specify Using membrane elements in large-displacement implicit analyses Buckling can occur in Abaqus/Standard if a membrane structure is subject to compressive loading in a large-displacement analysis, causing out-of-plane deformation. Since a stress-free flat membrane has no stiffness perpendicular to its plane, out-of-plane loading will cause numerical singularities and convergence difficulties. Once some out-of-plane deformation has developed, the membrane will be able to resist out-of-plane loading. In some cases loading the membrane elements in tension or adding initial tensile stress can overcome the numerical singularities and convergence difficulties associated with out-of-plane loading. However, you must choose the magnitude of the loading or initial stress such that the final solution is unaffected. Using membrane elements in Abaqus/Standard contact analyses Element types M3D8 and M3D8R are converted automatically to element types M3D9 and M3D9R, respectively, if a slave surface on a contact pair is attached to the element. 29.1.2 GENERAL MEMBRANE ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Membrane elements,” Section 29.1.1 • *NODAL THICKNESS • *MEMBRANE SECTION Overview This section provides a reference to the general membrane elements available in Abaqus/Standard and Abaqus/Explicit. Element types M3D3 M3D4 M3D4R M3D6(S) M3D8(S) M3D8R(S) M3D9(S) M3D9R(S) 3-node triangle 4-node quadrilateral 4-node quadrilateral, reduced integration, hourglass control 6-node triangle 8-node quadrilateral 8-node quadrilateral, reduced integration 9-node quadrilateral 9-node quadrilateral, reduced integration, hourglass control Active degrees of freedom 1, 2, 3 Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition Input File Usage: *MEMBRANE SECTION In addition, use the following option for variable thickness membranes: Abaqus/CAE Usage: *NODAL THICKNESS Property module: Create Section: select Shell as the section Category and Membrane as the section Type You cannot define variable thickness membranes in Abaqus/CAE. Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BX BY BZ BXNU Body force Body force Body force Body force FL−3 FL−3 FL−3 FL−3 BYNU Body force FL−3 BZNU Body force FL−3 Body force in the global X-direction. Body force in the global Y-direction. Body force in the global Z-direction. in force Nonuniform body the global X-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. in force Nonuniform body the global Y-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. in force the Nonuniform body global Z-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. CENT(S) Not supported FL−4 (ML−3 T−2 ) , where Centrifugal load (magnitude is input is the mass density as per unit volume, is the angular velocity). Centrifugal load (magnitude is input as the angular velocity). , where is CENTRIF(S) Rotational body force T−2 Units Description Load ID (*DLOAD) CORIO(S) Abaqus/CAE Load/Interaction Coriolis force FL−4 T (ML−3 T−1 ) GRAV Gravity LT−2 HP(S) Not supported FL−2 Pressure FL−2 PNU Not supported FL−2 Coriolis force (magnitude is input is the mass density as , where per unit volume, is the angular velocity). The load stiffness due to Coriolis loading is not accounted for in direct steady-state dynamic analysis. Gravity loading direction (magnitude is acceleration). in specified input as Hydrostatic pressure applied to the element reference surface and linear in global Z. The pressure is positive in the direction of the positive element normal. Pressure applied to the element reference surface. The pressure is positive in the direction of the positive element normal. applied reference to Nonuniform pressure surface element the supplied via with magnitude DLOAD in user subroutine and VDLOAD Abaqus/Standard The pressure in Abaqus/Explicit. is positive in the direction of the positive element normal. ROTA(S) Rotational body force T−2 ROTDYNF(S) Not supported T−1 SBF(E) Not supported FL−5 T2 Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Rotordynamic load (magnitude is input as is the angular velocity). , where Stagnation body force in global X-, Y-, and Z-directions. Load ID (*DLOAD) SP(E) Abaqus/CAE Load/Interaction Units Description Not supported FL−4 T2 TRSHR Surface traction FL−2 TRSHRNU(S) Not supported FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Not supported FL−2 VBF(E) VP(E) Not supported FL−4 T Not supported FL−3 T Stagnation pressure applied to the element reference surface. traction Shear reference surface. on the element traction on the Nonuniform shear surface with reference element magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction Nonuniform general on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. Viscous body force in global X-, Y-, and Z-directions. surface pressure applied Viscous to the element reference surface. The pressure is proportional to the velocity normal to the element face and opposing the motion. Foundations Foundations are available only in Abaqus/Standard and are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE F(S) Elastic foundation Units Description FL−3 Elastic foundation. Surface-based loading Distributed loads Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description HP(S) Pressure FL−2 Pressure FL−2 PNU Pressure FL−2 SP(E) Pressure FL−4 T2 TRSHR Surface traction FL−2 TRSHRNU(S) Surface traction FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 VP(E) Pressure FL−3 T 29.1.2–5 Hydrostatic pressure on the element reference surface and linear in global Z. The pressure is positive in the direction opposite to the surface normal. Pressure on the element reference surface. The pressure is positive in the direction opposite to the surface normal. Nonuniform pressure on the element reference surface with magnitude supplied via user subroutine DLOAD and VDLOAD in Abaqus/Standard in Abaqus/Explicit. The pressure is positive in the direction opposite to the surface normal. Stagnation pressure applied to the element reference surface. traction Shear reference surface. on the element traction on the Nonuniform shear element surface with reference magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction Nonuniform general on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. Viscous surface pressure applied to the element reference surface. The pressure is proportional to the velocity normal to the element surface and Incident wave loading Surface-based incident wave loads are available. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. If the incident wave field includes a reflection off a plane outside the boundaries of the mesh, this effect can be included. Element output If a local orientation (“Orientations,” Section 2.2.5) is not used with the element, the stress/strain components are in the default directions on the surface defined by the convention given in “Conventions,” Section 1.2.2. If a local orientation is used with the element, the stress/strain components are in the surface directions defined by the orientation. In large-displacement problems the local directions defined in the reference configuration are rotated into the current configuration by the average material rotation. See “State storage,” Section 1.5.4 of the Abaqus Theory Manual, for details. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S12 Local 11 direct stress. Local 22 direct stress. Local 12 shear stress. Section thickness STH Current thickness. Node ordering on elements 1 2 3 - node element 4 - node element 6 5 1 2 4 7 3 6 - node element 8 - node element 4 7 3 9 - node element Numbering of integration points for output 6 5 1 2 1 2 3 - node element 6 - node element 4 - node element 4 - node reduced integration element 4 7 3 4 7 3 8 - node element 8 - node reduced integration element 4 7 3 4 7 3 9 - node element 9 - node reduced integration element 29.1.3 CYLINDRICAL MEMBRANE ELEMENT LIBRARY Product: Abaqus/Standard References • “Membrane elements,” Section 29.1.1 • *MEMBRANE SECTION Overview This section provides a reference to the cylindrical membrane elements available in Abaqus/Standard. Element types MCL6 MCL9 6-node cylindrical membrane 9-node cylindrical membrane Active degrees of freedom 1, 2, 3 Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition Input File Usage: *MEMBRANE SECTION Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) BX BY BZ Units Description FL−3 FL−3 FL−3 Body force in the global X-direction. Body force in the global Y-direction. Body force in the global Z-direction. Description CYLINDRICAL MEMBRANES Load ID (*DLOAD) BXNU BYNU BZNU FL−3 FL−3 FL−3 CENT FL−4 (ML−3 T−2 ) CENTRIF T−2 CORIO FL−4 T (ML−3 T−1 ) GRAV HP PNU ROTA ROTDYNF(S) LT−2 FL−2 FL−2 FL−2 T−2 T−1 Abaqus ID: Printed on: Nonuniform body force in the global X-direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in the global Y-direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in the global Z-direction with magnitude supplied via user subroutine DLOAD. Centrifugal load (magnitude is input as where , is the mass density per unit volume, is the angular velocity). Centrifugal load (magnitude is input as where is the angular velocity). , Coriolis force (magnitude is input as where , is the mass density per unit volume, is the angular velocity). Gravity loading in a specified direction (magnitude is input as acceleration). Hydrostatic pressure applied to the element reference surface and linear in global Z. The pressure is positive in the direction of the positive element normal. Pressure applied to the element reference surface. The pressure is positive in the direction of the positive element normal. Nonuniform pressure applied to the element reference surface with magnitude supplied via user subroutine DLOAD. The pressure is positive in the direction of the positive element normal. Rotary acceleration load (magnitude is input as is the rotary acceleration. , where Rotordynamic load (magnitude is input as Load ID (*DLOAD) TRSHR Units FL−2 TRSHRNU(S) FL−2 TRVEC FL−2 TRVECNU(S) FL−2 Description Shear traction on the element reference surface. Nonuniform shear traction on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. General traction on the element reference surface. Nonuniform general traction on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. Foundations Foundations are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Units Description FL−3 Elastic foundation. Surface-based loading Distributed loads Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Units Description on pressure Hydrostatic element reference surface and linear in global Z. The pressure is positive in the direction opposite to the surface normal. the Pressure on the element reference surface. The pressure is positive in the direction opposite to the surface normal. Nonuniform pressure on the element reference surface with magnitude supplied 29.1.3–3 HP PNU FL−2 FL−2 Load ID (*DSLOAD) Units Description TRSHR FL−2 TRSHRNU(S) FL−2 TRVEC FL−2 TRVECNU(S) FL−2 via user subroutine DLOAD. The pressure is positive in the direction opposite to the surface normal. Shear traction on the element reference surface. Nonuniform shear traction on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. General traction on the element reference surface. Nonuniform general traction on the element reference surface with magnitude and subroutine direction supplied via user UTRACLOAD. Element output If a local orientation (“Orientations,” Section 2.2.5) is not used with the element, the stress/strain components are expressed in the default directions on the surface defined by the convention given in “Conventions,” Section 1.2.2. If a local orientation is used with the element, the stress/strain components are in the surface directions defined by the orientation. In large-displacement problems the local directions defined in the reference configuration are rotated into the current configuration by the average material rotation. See “State storage,” Section 1.5.4 of the Abaqus Theory Manual, for details. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S12 Local Local Local direct stress. direct stress. shear stress. Section thickness STH Current thickness. Node ordering and face numbering on elements 6-node element 9-node element Numbering of integration points for output 6-node element 9-node element AXISYMMETRIC MEMBRANE ELEMENT LIBRARY AXISYMMETRIC MEMBRANE LIBRARY Products: Abaqus/Standard Abaqus/CAE References • “Membrane elements,” Section 29.1.1 • *MEMBRANE SECTION • *NODAL THICKNESS Overview This section provides a reference to the axisymmetric membrane elements available in Abaqus/Standard. Conventions Coordinate 1 is r, coordinate 2 is z. At , the r-direction corresponds to the global X-direction and the z-direction corresponds to the global Y-direction. This is important when data are required in global directions. Coordinate 1 should be greater than or equal to zero. Degree of freedom 1 is have an additional degree of freedom, 5, corresponding to the twist angle , degree of freedom 2 is . Generalized axisymmetric elements with twist (in radians). Abaqus/Standard does not automatically apply any boundary conditions to nodes located along the symmetry axis. You must apply radial or symmetry boundary conditions on these nodes if desired. Point loads and moments should be given as the value integrated around the circumference; that is, the total value on the ring. Element types Regular axisymmetric membranes MAX1 MAX2 2-node linear, without twist 3-node quadratic, without twist Active degrees of freedom 1, 2 Additional solution variables None. Generalized axisymmetric membranes MGAX1 MGAX2 2-node linear, with twist 3-node quadratic, with twist Active degrees of freedom 1, 2, 5 Additional solution variables None. Nodal coordinates required R, Z Element property definition Input File Usage: *MEMBRANE SECTION In addition, use the following option for variable thickness membranes: Abaqus/CAE Usage: *NODAL THICKNESS Property module: Create Section: select Shell as the section Category and Membrane as the section Type You cannot define variable thickness membranes in Abaqus/CAE. Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BR BZ Body force Body force BRNU Body force FL−3 FL−3 FL−3 BZNU Body force FL−3 CENT Not supported FL−4 (ML−3 T−2 ) 29.1.4–2 Body force in the radial (1 or r) direction. Body force in the axial (2 or z) direction. Nonuniform body force in the radial direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in the axial direction with magnitude supplied via user subroutine DLOAD. Centrifugal load (magnitude is input is the mass density as per unit volume, is the angular Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description velocity). Since only axisymmetric deformation is allowed, the spin axis must be the z-axis. CENTRIF Rotational body force T−2 GRAV Gravity LT−2 HP Not supported FL−2 Pressure FL−2 PNU Not supported FL−2 , where Centrifugal load (magnitude is input as the angular velocity). Since only axisymmetric deformation is allowed, the spin axis must be the z-axis. is Gravity direction acceleration). loading in (magnitude specified as input Hydrostatic pressure applied to the element reference surface and linear in global Z. The pressure is positive in the direction of the positive element normal. Pressure applied to the element reference surface. The pressure is positive in the direction of the positive element normal. applied reference to Nonuniform pressure surface element the with magnitude supplied via user subroutine DLOAD. The pressure is positive in the direction of the positive element normal. TRSHR Surface traction FL−2 TRSHRNU(S) Not supported FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Not supported FL−2 traction Shear reference surface. on the element Nonuniform shear traction on the surface with reference element magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element Nonuniform general on the element reference surface with traction Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description magnitude and direction supplied via user subroutine UTRACLOAD. Foundations Foundations are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE Units Description Elastic foundation FL−3 Elastic foundation. For MGAX elements the elastic foundations are applied to degrees of freedom and only. Surface-based loading Distributed loads Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description HP Pressure FL−2 Pressure FL−2 PNU Pressure FL−2 TRSHR Surface traction FL−2 29.1.4–4 Hydrostatic pressure on the element reference surface and linear in global Z. The pressure is positive in the direction opposite to the surface normal. Pressure on the element reference surface. The pressure is positive in the direction opposite to the surface normal. Nonuniform pressure on the element reference surface with magnitude supplied via user subroutine DLOAD. The pressure is positive in the the surface direction opposite of normal. traction Shear reference surface. on the Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description TRSHRNU(S) Surface traction FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 traction on the Nonuniform shear element surface with reference magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction Nonuniform general on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. Incident wave loading Surface-based incident wave loads are available. They are specified as described in “Acoustic and shock loads,” Section 33.4.6. If the incident wave field includes a reflection off a plane outside the boundaries of the mesh, this effect can be included. Element output The default local material directions are such that local material direction 1 lies along the line of the element and local material direction 2 is the hoop direction. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S12 Local direct stress. Local direct stress. Local elements. shear stress. Only available for generalized axisymmetric membrane Section thickness STH Current thickness. Node ordering on elements 2 - node element 3 - node element Numbering of integration points for output 2 - node element 3 - node element 29.2 Truss elements • “Truss elements,” Section 29.2.1 • “Truss element library,” Section 29.2.2 29.2.1 TRUSS ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Truss element library,” Section 29.2.2 • *SOLID SECTION • “Creating truss sections,” Section 12.13.12 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Truss elements: • are long, slender structural members that can transmit only axial force (nonstructural link elements are presented in “One-dimensional solid (link) element library,” Section 28.1.2); and • do not transmit moments. Typical applications Truss elements are used in two and three dimensions to model slender, line-like structures that support loading only along the axis or the centerline of the element. No moments or forces perpendicular to the centerline are supported. The two-dimensional truss elements can be used in axisymmetric models to represent components, such as bolts or connectors, where the strain is computed from the change in length in the r–z plane only. Two-dimensional trusses can also be used to define master surfaces for contact applications in Abaqus/Standard . In this case the direction of the master surface’s outward normal is critical for proper detection of contact. The 3-node truss element available in Abaqus/Standard is often useful for modeling curved reinforcing cables in structures, such as prestressed tendons in reinforced concrete or long slender pipelines used in the off-shore industry. Choosing an appropriate element A 2-node straight truss element, which uses linear interpolation for position and displacement and has a constant stress, is available in both Abaqus/Standard and Abaqus/Explicit. In addition, a 3-node curved truss element, which uses quadratic interpolation for position and displacement so that the strain varies linearly along the element, is available in Abaqus/Standard. Hybrid versions of the stress/displacement trusses, coupled temperature-displacement trusses, and piezoelectric trusses are available in Abaqus/Standard. Hybrid stress/displacement truss elements Hybrid (mixed) versions of the stress/displacement trusses, in which the axial force is treated as an additional unknown, are available in two and three dimensions in Abaqus/Standard. These elements are useful (to offset the effects of numerical ill-conditioning on governing equations) when a truss represents a very rigid link whose stiffness is much larger than that of the overall structural model. In such a case a hybrid truss provides an alternative to a truly rigid link, modeled with multi-point constraints or rigid elements . Coupled temperature-displacement truss elements truss elements are available in two and three dimensions in Coupled temperature-displacement Abaqus/Standard. These elements have temperature as an additional degree of freedom (11). See “Fully coupled thermal-stress analysis,” Section 6.5.3, for information about fully coupled temperature-displacement analysis in Abaqus/Standard. Piezoelectric truss elements Piezoelectric truss elements are available in two and three dimensions in Abaqus/Standard. These elements have electric potential as an additional degree of freedom (9). See “Piezoelectric analysis,” Section 6.7.2, for information about piezoelectric analysis. Naming convention Truss elements in Abaqus are named as follows: 3D 2 H Optional: hybrid (H), coupled temperature-displacement (T), or piezoelectric (E) number of nodes two-dimensional (2D) or three-dimensional (3D) truss For example, T2D3E is a two-dimensional, 3-node piezoelectric truss element. Element normal definition For two-dimensional trusses the positive outward normal, rotation from the direction going from node 1 to node 2 or node 3 of the element, as shown. , is defined by a 90° counterclockwise Defining the element’s section properties You use a solid section definition to define the section properties. You must associate these properties with a region of your model. Input File Usage: *SOLID SECTION, ELSET=name where the ELSET parameter refers to a set of truss elements. Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category and Truss as the section Type Assign→Section: select regions Defining the cross-sectional area of a truss element You can define the cross-sectional area associated with the truss element as part of the section definition. If you do not specify a value for the cross-sectional area, unit area is assumed. When truss elements are used in large-displacement analysis, the updated cross-sectional area is calculated by assuming that the truss is made of an incompressible material, regardless of the actual material definition. This assumption affects cases only where the strains are large. It is adopted because the most common applications of trusses at large strains involve yielding metal behavior or rubber elasticity, in which cases the material is effectively incompressible. Therefore, a linear elastic truss element does not provide the same force-displacement response as a linear SPRINGA spring element when the axial strain is not infinitesimal. Input File Usage: *SOLID SECTION, ELSET=name cross-sectional area Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category and Truss as the section Type: Cross-sectional area: cross-sectional area Assigning a material definition to a set of truss elements You must associate a material definition with each solid section definition. No material orientation is permitted with truss elements. Input File Usage: *SOLID SECTION, MATERIAL=name Any value given to the ORIENTATION parameter on the *SOLID SECTION option will be ignored by truss elements. Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category and Truss as the section Type: Material: name Using truss elements in large-displacement implicit analysis Truss elements have no initial stiffness to resist loading perpendicular to their axis. If a stress-free line of trusses is loaded perpendicular to its axis in Abaqus/Standard, numerical singularities and lack of convergence can result. After the first iteration in a large-displacement implicit analysis, stiffness perpendicular to the initial line of the elements develops, sometimes allowing an analysis to overcome numerical problems. In some cases loading the truss elements along their axis first or including initial tensile stress can overcome these numerical singularities. However, you must choose the magnitude of the loading or initial stress such that the final solution is unaffected. 29.2.2 TRUSS ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Truss elements,” Section 29.2.1 • *SOLID SECTION Overview This section provides a reference to the truss elements available in Abaqus/Standard and Abaqus/Explicit. Element types 2-D stress/displacement truss elements T2D2 T2D2H(S) T2D3(S) T2D3H(S) 2-node linear displacement 2-node linear displacement, hybrid 3-node quadratic displacement 3-node quadratic displacement, hybrid Active degrees of freedom 1, 2 Additional solution variables Element type T2D2H has one additional variable and element type T2D3H has two additional variables relating to axial force. 3-D stress/displacement truss elements T3D2 T3D2H(S) T3D3(S) T3D3H(S) 2-node linear displacement 2-node linear displacement, hybrid 3-node quadratic displacement 3-node quadratic displacement, hybrid Active degrees of freedom 1, 2, 3 Additional solution variables Element type T3D2H has one additional variable and element type T3D3H has two additional variables relating to axial force. 2-D coupled temperature-displacement truss elements T2D2T(S) T2D3T(S) 2-node, linear displacement, linear temperature 3-node, quadratic displacement, linear temperature Active degrees of freedom 1, 2 at middle node for T2D3T 1, 2, 11 at all other nodes Additional solution variables None. 3-D coupled temperature-displacement truss elements T3D2T(S) T3D3T(S) 2-node, linear displacement, linear temperature 3-node, quadratic displacement, linear temperature Active degrees of freedom 1, 2, 3 at middle node for T3D3T 1, 2, 3, 11 at all other nodes Additional solution variables None. 2-D piezoelectric truss elements T2D2E(S) T2D3E(S) 2-node, linear displacement, linear electric potential 3-node, quadratic displacement, quadratic electric potential Active degrees of freedom 1, 2, 9 Additional solution variables None. 3-D piezoelectric truss elements T3D2E(S) T3D3E(S) 2-node, linear displacement, linear electric potential 3-node, quadratic displacement, quadratic electric potential Active degrees of freedom 1, 2, 3, 9 Additional solution variables None. Nodal coordinates required 2-D: X, Y 3-D: X, Y, Z Element property definition You must provide the cross-sectional area of the element. If no area is given, Abaqus assumes unit area. Input File Usage: Abaqus/CAE Usage: *SOLID SECTION Property module: Create Section: select Beam as the section Category and Truss as the section Type Element-based loading Distributed loads Distributed loads are available for elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BX BY BZ Body force Body force Body force BXNU Body force FL−3 FL−3 FL−3 FL−3 BYNU Body force FL−3 BZNU Body force FL−3 Body force in global X-direction. Body force in global Y-direction. Body force in global Z-direction. (Only for 3-D trusses.) Nonuniform body force in global X-direction with magnitude supplied subroutine DLOAD in user via and VDLOAD in Abaqus/Standard Abaqus/Explicit. Nonuniform body force in global Y-direction with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. Nonuniform body force in global Z-direction with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description CENT(S) Not supported FL−4 (ML−3 T−2 ) CENTRIF(S) Rotational body force T−2 CORIO(S) Coriolis force FL−4 T (ML−3 T−1 ) GRAV Gravity LT−2 ROTA(S) Rotational body force T−2 Abaqus/Explicit. trusses.) (Only for 3-D , where Centrifugal load (magnitude is input is the mass density as per unit volume, is the angular velocity). Centrifugal load (magnitude is input as the angular velocity). , where is Coriolis force (magnitude is input is the mass density as , where per unit volume, is the angular velocity). loading Gravity direction (magnitude is acceleration). in specified input as Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Abaqus/Aqua loads Abaqus/Aqua loads are specified as described in “Abaqus/Aqua analysis,” Section 6.11.1. They are available only for stress/displacement trusses. Load ID (*CLOAD/ *DLOAD) FDD(A) FD1(A) FD2(A) FDT(A) FI(A) Abaqus/CAE Load/Interaction Units Description Not supported FL−1 Transverse fluid drag load. Not supported Not supported Not supported Not supported FL−1 FL−1 Fluid drag force on the first end of the truss (node 1). Fluid drag force on the second end of the truss (node 2 or node 3). Tangential fluid drag load. Fluid inertia load. Load ID (*CLOAD/ *DLOAD) FI1(A) FI2(A) PB(A) WDD(A) WD1(A) WD2(A) Abaqus/CAE Load/Interaction Units Description Not supported Not supported Not supported Not supported Not supported Not supported FL−1 FL−1 Fluid inertia force on the first end of the truss (node 1). Fluid inertia force on the second end of the truss (node 2 or node 3). Buoyancy load (with closed end condition). Transverse wind drag load. Wind drag force on the first end of the truss (node 1). Wind drag force on the second end of the truss (node 2 or node 3). Distributed heat fluxes Distributed heat fluxes are available for coupled temperature-displacement trusses. They are specified as described in “Thermal loads,” Section 33.4.4. Abaqus/CAE Load/Interaction Units Description Load ID (*DFLUX) BF(S) BFNU(S) S1(S) S2(S) Body heat flux Body heat flux JL−3 T−1 JL−3 T−1 Surface heat flux JL−2 T−1 Surface heat flux JL−2 T−1 Heat body flux per unit volume. Nonuniform heat body flux per unit volume with magnitude supplied via user subroutine DFLUX. Heat surface flux per unit area into the first end of the truss (node 1). Heat surface flux per unit area into the second end of the truss (node 2 or node 3). Nonuniform heat surface flux per unit area into the first end of the truss (node 1) with magnitude supplied via user subroutine DFLUX. Nonuniform heat surface flux per unit area into the second end of the truss S1NU(S) Not supported JL−2 T−1 S2NU(S) Not supported JL−2 T−1 Load ID (*DFLUX) Abaqus/CAE Load/Interaction Units Description (node 2 or node 3) with magnitude supplied via user subroutine DFLUX. Film conditions Film conditions are available for coupled temperature-displacement trusses. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*FILM) F1(S) F2(S) Abaqus/CAE Load/Interaction Units Description Not supported JL−2 T−1 −1 Not supported JL−2 T−1 −1 F1NU(S) Not supported JL−2 T−1 −1 F2NU(S) Not supported JL−2 T−1 −1 Film coefficient and sink temperature at the first end of the truss (node 1). Film coefficient and sink temperature at the second end of the truss (node 2 or node 3). Nonuniform film coefficient and sink temperature at the first end of the truss (node 1) with magnitude supplied via user subroutine FILM. Nonuniform film coefficient and sink temperature at the second end of the truss (node 2 or node 3) with magnitude supplied via user subroutine FILM. Radiation types Radiation conditions are available for coupled temperature-displacement trusses. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*RADIATE) Abaqus/CAE Load/Interaction Units Description R1(S) R2(S) Surface radiation Dimensionless Surface radiation Dimensionless Emissivity and sink temperature at the first end of the truss (node 1). Emissivity and sink temperature at the second end of the truss (node 2 or node 3). Electric fluxes Electric fluxes are available for piezoelectric trusses. They are specified as described in “Piezoelectric analysis,” Section 6.7.2. Load ID (*DECHARGE) Abaqus/CAE Load/Interaction Units Description EBF(S) Body charge CL−3 Body flux per unit volume. Element output Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 Axial stress. Heat flux components Available for coupled temperature-displacement trusses. HFL1 Heat flux along the element axis. Node ordering on elements end 2 end 1 end 1 2 - node element 3 - node element end 2 Numbering of integration points for output 2 - node element 3 - node element 29.3 Beam elements • “Beam modeling: overview,” Section 29.3.1 • “Choosing a beam cross-section,” Section 29.3.2 • “Choosing a beam element,” Section 29.3.3 • “Beam element cross-section orientation,” Section 29.3.4 • “Beam section behavior,” Section 29.3.5 • “Using a beam section integrated during the analysis to define the section behavior,” Section 29.3.6 • “Using a general beam section to define the section behavior,” Section 29.3.7 • “Beam element library,” Section 29.3.8 • “Beam cross-section library,” Section 29.3.9 29.3.1 BEAM MODELING: OVERVIEW Abaqus offers a wide range of beam modeling options. Overview Beam modeling consists of: • choosing a beam cross-section (“Choosing a beam cross-section,” Section 29.3.2, and “Beam cross- section library,” Section 29.3.9); • choosing the appropriate beam element type (“Choosing a beam element,” Section 29.3.3, and “Beam element library,” Section 29.3.8); • defining the beam cross-section orientation (“Beam element cross-section orientation,” Section 29.3.4); • determining whether or not numerical integration is needed to define the beam section behavior (“Beam section behavior,” Section 29.3.5); and • defining the beam section behavior (“Using a beam section integrated during the analysis to define the section behavior,” Section 29.3.6, or “Using a general beam section to define the section behavior,” Section 29.3.7). Determining whether beam modeling is appropriate Beam theory is the one-dimensional approximation of a three-dimensional continuum. The reduction in dimensionality is a direct result of slenderness assumptions; that is, the dimensions of the cross-section are small compared to typical dimensions along the axis of the beam. The axial dimension must be interpreted as a global dimension (not the element length), such as • distance between supports, • distance between gross changes in cross-section, or • wavelength of the highest vibration mode of interest. In Abaqus a beam element is a one-dimensional line element in three-dimensional space or in the X–Y plane that has stiffness associated with deformation of the line (the beam’s “axis”). These deformations consist of axial stretch; curvature change (bending); and, torsion. (“Truss elements,” Section 29.2.1, are one-dimensional line elements that have only axial stiffness.) Beam elements offer additional flexibility associated with transverse shear deformation between the beam’s axis and its cross-section directions. Some beam elements in Abaqus/Standard also include warping—nonuniform out-of-plane deformation of the beam’s cross-section—as a nodal variable. The main advantage of beam elements is that they are geometrically simple and have few degrees of freedom. This simplicity is achieved by assuming that the member’s deformation can be estimated entirely from variables that are functions of position along the beam axis only. Thus, a key issue in using beam elements is to judge whether such one-dimensional modeling is appropriate. in space, The fundamental assumption used is that the beam section (the intersection of the beam with a plane that is perpendicular to the beam axis; see the discussion in “Choosing a beam cross-section,” Section 29.3.2) cannot deform in its own plane (except for a constant change in cross-sectional area, which may be introduced in geometrically nonlinear analysis and causes a strain that is the same in all directions in the plane of the section). The implications of this assumption should be considered carefully in any use of beam elements, especially for cases involving large amounts of bending or axial tension/compression of non-solid cross-sections such as pipes, I-beams, and U-beams. Section collapse may occur and result in very weak behavior that is not predicted by beam theory. Similarly, thin-walled, curved pipes exhibit much softer bending behavior than would be predicted by beam theory because the pipe wall readily bends in its own section—another effect precluded by this basic assumption of beam theory. This effect, which must generally be considered when designing piping elbows, can be modeled by using shell elements to model the pipe as a three-dimensional shell or, in Abaqus/Standard, by using elbow elements . In addition to beam elements, frame elements are provided in Abaqus/Standard. These elements provide efficient modeling for design calculations of frame-like structures composed of initially straight, slender members. They operate directly in terms of axial force, bending moments, and torque at the element’s end nodes. They are implemented for small or large displacements (large rotations with small strains) and permit the formation of plastic hinges at their ends through a “lumped” plasticity model that includes kinematic hardening. See “Frame elements,” Section 29.4.1, for details. In addition to the various beam elements, Abaqus also provides pipe elements to model beams with pipe cross-sections that are subject to internal stress due to internal and/or external pressure loading. Abaqus provides a choice of two formulations for pipe elements: • the thin-walled formulation, where the hoop stress is assumed to be constant and the radial stress is neglected, is available in Abaqus/Explicit and Abaqus/Standard; and • the thick-walled formulation, where the hoop and radial stress vary through the cross-section, is available only in Abaqus/Standard. The pipe elements are a specialized form of the corresponding beam elements that allow for internal and/or external pressure load specification and take the resulting hoop stress (as well as radial stress for thick-walled pipes) into account for the material constitutive calculations. Usage of the pipe elements is identical to that of the corresponding beam elements with respect to the section definition, boundary conditions at the element nodes, surface definitions, interactions such as tie constraints, etc. Using beam elements in dynamic and eigenfrequency analysis The rotary inertia of a beam cross-section is usually insignificant for slender beam structures, except for twist around the beam axis. Therefore, Abaqus/Standard ignores rotary inertia of the cross-section for Euler-Bernoulli beam elements in bending. For thicker beams the rotary inertia plays a role in dynamic analysis, but to a lesser extent than shear deformation effects. For Timoshenko beams the inertia properties are calculated from the cross-section geometry. The rotary inertia associated with torsional modes is different from that of flexural modes. For unsymmetric cross-sections the rotary inertia is different in each direction of bending. Abaqus allows you to choose the rotary inertia formulation for Timoshenko beams. When an approximate isotropic formulation is requested, the rotary inertia associated with the torsional mode is used for all rotational degrees of freedom in Abaqus/Standard, and a scaled flexural inertia with a scaling factor chosen to maximize the stable time increment is used for all rotational degrees of freedom in Abaqus/Explicit. The center of mass of the cross-section is taken to be located at the beam node. When the exact (anisotropic) formulation is requested, the rotary inertia associated with bending and torsion differ and the coupling between the translational and rotational degrees of freedom is included for beam cross-section definitions where the beam node is not located at the center of mass of the cross-section. For Timoshenko beams with the exact (default) rotary inertia formulation, you can define an additional mass and rotary inertia contribution to the beam’s inertia response that does not add to its structural stiffness; see “Adding inertia to the beam section behavior for Timoshenko beams” in “Beam section behavior,” Section 29.3.5. 29.3.2 CHOOSING A BEAM CROSS-SECTION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Beam modeling: overview,” Section 29.3.1 • “Beam cross-section library,” Section 29.3.9 • “Meshed beam cross-sections,” Section 10.6.1 • “Defining profiles,” Section 12.2.2 of the Abaqus/CAE User’s Manual Overview The choice of cross-section is determined by the geometry of the cross-section and its behavior. A beam’s cross-section: • can be solid or thin-walled; • if thin-walled, can be open or closed; and • can be defined by choosing from the Abaqus cross-section library; by specifying geometric quantities such as area, moments of inertia, and torsional constant; or by using a mesh of special two-dimensional elements, for which geometric quantities are calculated numerically. You must consider whether the section should be treated as a solid cross-section or as a thin-walled cross-section. This choice determines the basis upon which Abaqus computes the axial and shear strains at each point in the section. Solid cross-sections For solid sections under bending, plane (beam) sections remain plane. Under torsional loading any noncircular beam section will warp: the beam section will not remain planar. However, for solid sections the warping of the section is small enough so that the axial strain due to warping of the section can be neglected and St. Venant warping theory can be used to construct a single component of shear strain at each integration point in the section. This is done automatically for the rectangular and trapezoidal sections in the beam section library. The St. Venant warping functions are used to define the shear strain even when the response in the section is no longer purely elastic. This limits the accuracy of the modeling for cases involving noncircular solid beam sections subjected to torsional loadings that cause large amounts of inelastic deformation. When using a meshed beam profile, two shear strain components are available for output in the user-specified material system. The thick pipe section is treated as a solid cross-section. Nonsolid (“thin-walled”) cross-sections In Abaqus nonsolid sections are treated as “thin-walled” sections; that is, in the plane of the section, the thickness of a branch of the section is assumed to be small compared to its length. Thin-walled beam theory determines the shear in the wall of the section depending on whether the section is closed or open. Closed sections A closed section is a nonsolid section whose branches form closed loops. Closed sections offer significant resistance to torsion and do not warp significantly. Abaqus ignores warping effects for closed sections. In Abaqus predefined beam sections can model only one closed loop. Sections with multiple loops must be modeled with a meshed beam section or with shells. For sufficiently small thickness of the section walls, the variation of shear stress across the thickness is negligible; the formulation of the closed sections available in Abaqus is based on this assumption. Open sections An open section is a nonsolid section with branches that do not form closed loops, such as an I-section or a U-section. In such sections the shear stress is assumed to vary linearly over the wall thickness and to vanish at the center of the wall. Open sections can warp significantly and generally require the use of open-section warping theory (available with beam element types BxxOS in Abaqus/Standard) with suitable warping constraints (applied to degree of freedom 7) at supports or joints. Such warping constraints may significantly increase the torsional stiffness of the beam. Open, thin-walled sections whose branches are straight lines that meet at a single point (such as the L-section in the Abaqus beam element section library, T-sections, or X-sections) do not warp; therefore, warping constraints have no effect. Such sections always have very little torsional stiffness. If an open section is used with a regular beam element type (not BxxOS), the open section is assumed to be free to warp and the axial strain due to warping is neglected. Consequently, the section will have very little torsional stiffness. Section property calculations Thin-walled assumptions are used when calculating nonsolid section properties. Properties for sections comprised of intersecting straight segments (arbitrary, box, hexagonal, I-, and L-sections) also include an approximation of the intersection geometry. Available beam cross-sections You can specify any of the following types of beam cross-sections: an Abaqus library cross-section, a generalized cross-section for which you specify the geometric quantities directly, or a meshed cross- section. The Abaqus beam cross-section library The Abaqus beam cross-section library contains solid sections (circular, rectangular, and trapezoidal), closed thin-walled sections (box, hexagonal, and pipe), open thin-walled sections (I-shaped, T-shaped, or L-shaped), and a thick-walled pipe section. Abaqus also provides an arbitrary thin-walled section definition; Abaqus will treat this section type as a closed or open section, depending on how the section is defined. Trapezoidal, I, and arbitrary library sections allow you to define the location of the origin of the local coordinate system. Other section types—such as rectangular, circular, L, or pipe—have preset origins. Input File Usage: Use the following option to define a beam section integrated during the analysis: *BEAM SECTION, SECTION=name where name can be ARBITRARY, BOX, CIRC, HEX, I, L, PIPE, RECT, THICK PIPE, or TRAPEZOID. A T-section is defined by specifying geometric data for only one flange of an I-section. Use the following option to define a general beam section: *BEAM GENERAL SECTION, SECTION=name where name can be ARBITRARY, BOX, CIRC, HEX, I, L, PIPE, RECT, or TRAPEZOID. A T-section is defined by specifying geometric data for only one flange of an I-section. Abaqus/CAE Usage: Property module: Create Profile: choose Box, Pipe, Circular, Rectangular, Hexagonal, Trapezoidal, I, L, T, or Arbitrary Generalized cross-sections Abaqus also allows you to specify “generalized” cross-sections by specifying the geometric quantities necessary to define the section. Such generalized sections can be used only with linear material behavior although the section response can be linear or nonlinear. Input File Usage: Use the following option to define a linear generalized cross-section: *BEAM GENERAL SECTION, SECTION=GENERAL Use the following option to define a nonlinear generalized cross-section: Abaqus/CAE Usage: *BEAM GENERAL SECTION, SECTION=NONLINEAR GENERAL Property module: Create Profile: choose Generalized Nonlinear generalized cross-sections are not supported in Abaqus/CAE. Meshed cross-sections Abaqus allows you to mesh an arbitrarily shaped solid cross-section by using warping elements in a two-dimensional analysis to generate beam cross-section properties that can be used in a subsequent two- or three-dimensional beam analysis. Such sections permit only linear, elastic material behavior. Therefore, a meshed cross-section can be used only with a general beam section definition; for details, see “Meshed beam cross-sections,” Section 10.6.1. Input File Usage: *BEAM GENERAL SECTION, SECTION=MESHED Abaqus/CAE Usage: Meshed cross-sections are not supported in Abaqus/CAE. CHOOSING A BEAM ELEMENT BEAM ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Beam modeling: overview,” Section 29.3.1 • “Beam element library,” Section 29.3.8 • *TRANSVERSE SHEAR STIFFNESS • “Creating beam sections,” Section 12.13.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Abaqus offers a wide range of beam elements, “Timoshenko”-type beams with solid, thin-walled closed and thin-walled open sections. including “Euler-Bernoulli”-type beams and The Abaqus/Standard beam element library includes: • Euler-Bernoulli (slender) beams in a plane and in space; • Timoshenko (shear flexible) beams in a plane and in space; • linear, quadratic, and cubic interpolation formulations; • warping (open section) beams; • pipe elements; and • hybrid formulation beams, typically used for very stiff beams that rotate significantly (applications in robotics or in very flexible structures such as offshore pipelines). The Abaqus/Explicit beam element library includes: • Timoshenko (shear flexible) beams in a plane and in space; • linear and quadratic interpolation formulations; and • linear pipe elements. Naming convention Beam elements in Abaqus are named as follows: 1 OS H hybrid (optional) open section (optional) linear (1), quadratic (2), cubic (3), or initially straight cubic (4) beam or pipe in plane (2) or beam or pipe in space (3) beam (B) or pipe (PIPE) element For example, B21H is a planar beam that uses linear interpolation and a hybrid formulation. Euler-Bernoulli (slender) beams Euler-Bernoulli beams (B23, B23H, B33, and B33H) are available only in Abaqus/Standard. These elements do not allow for transverse shear deformation; plane sections initially normal to the beam’s axis remain plane (if there is no warping) and normal to the beam axis. They should be used only to model slender beams: the beam’s cross-sectional dimensions should be small compared to typical distances along its axis (such as the distance between support points or the wavelength of the highest mode that participates in a dynamic response). For beams made of uniform material, typical dimensions in the cross-section should be less than about 1/15 of typical axial distances for transverse shear flexibility to be negligible. (The ratio of cross-section dimension to typical axial distance is called the slenderness ratio.) Load stiffness for pressure loads is not included for these elements. Interpolation The Euler-Bernoulli beam elements use cubic interpolation functions, which makes them reasonably accurate for cases involving distributed loading along the beam. Therefore, they are well suited for dynamic vibration studies, where the d’Alembert (inertia) forces provide such distributed loading. The cubic beam elements are written for small-strain, large-rotation analysis. They may not be appropriate for torsional stability problems due to the approximations in the underlying formulation and cannot be used in analyses involving very large rotations (of the order 180°); quadratic or linear beam elements should be used instead. Mass formulation The Euler-Bernoulli beam elements use a consistent mass formulation. Rotary inertia for twist around the beam axis is the same as for Timoshenko beams. For details, see “Mass and inertia for Timoshenko beams,” Section 3.5.5 of the Abaqus Theory Manual. Any additional inertia defined for these elements is ignored. Timoshenko (shear flexible) beams Timoshenko beams (B21, B22, B31, B31OS, B32, B32OS, PIPE21, PIPE22, PIPE31, PIPE32, and their “hybrid” equivalents) allow for transverse shear deformation. They can be used for thick (“stout”) as well as slender beams. For beams made from uniform material, shear flexible beam theory can provide useful results for cross-sectional dimensions up to 1/8 of typical axial distances or the wavelength of the highest natural mode that contributes significantly to the response. Beyond this ratio the approximations that allow the member’s behavior to be described solely as a function of axial position no longer provide adequate accuracy. Abaqus assumes that the transverse shear behavior of Timoshenko beams is linear elastic with a fixed modulus and, thus, independent of the response of the beam section to axial stretch and bending. For most beam sections Abaqus will calculate the transverse shear stiffness values required in the element formulation. You can override these default values as described below in “Defining the transverse shear stiffness and the slenderness compensation factor.” The default shear stiffness values are not calculated in some cases if estimates of shear moduli are unavailable during the preprocessing stage of input; for example, when the material behavior is defined by user subroutine UMAT, UHYPEL, UHYPER, or VUMAT. In such cases you must define the transverse shear stiffnesses as described below. The Timoshenko beams can be subjected to large axial strains. The axial strains due to torsion are assumed to be small. In combined axial-torsion loading, torsional shear strains are calculated accurately only when the axial strain is not large. Transverse shear stiffness definition The effective transverse shear stiffness of the section of a shear flexible beam is defined in Abaqus as is the section shear stiffness in the where the shear stiffness from becoming too large in slender beam elements; of the section; and are the local directions of the cross-section. The -direction; is a dimensionless factor used to prevent is the actual shear stiffness have units of force. The dimensionless factors are always included in the calculation of transverse shear stiffness and are defined as is the inertia in the -direction, is a constant of value where l is the length of the element, A is the cross-sectional area, is the slenderness compensation factor (with a default value of 0.25), and 1.0 for first-order elements and 10−4 for second-order elements. For meshed cross-sections the above expressions change to You can define the or as described below. If you do not specify them, they are defined by or where G is the elastic shear modulus or moduli and A is the cross-sectional area of the beam section. Temperature and field variable dependencies of G are not taken into account when calculating and . The shear factor k (Cowper, 1966) is defined as: Section type Shear factor, k Arbitrary Box Circular Elbow Generalized Hexagonal I (and T) Meshed Nonlinear generalized Pipe Rectangular Thick pipe Trapezoidal 1.0 0.44 0.89 0.85 1.0 0.53 0.44 1.0 1.0 1.0 0.53 0.85 0.53–0.89 0.822 When a beam section definition integrated during the analysis is used , G is calculated from the elastic material definition used with the section. When a general beam section definition is used (see “Using a general beam section to define the section behavior,” Section 29.3.7), you provide G as part of the beam section data. Defining the transverse shear stiffness and the slenderness compensation factor You can define the transverse shear stiffness for beam sections integrated during the analysis and general beam sections. In the case of two-dimensional beams, you can input a single value of transverse shear stiffness, namely is omitted or given as zero, the nonzero value will be used for both. . If either value of You can also define the slenderness compensation factor. The default value for the slenderness If a slenderness compensation factor value is provided, you must also compensation factor is 0.25. provide the values of the shear stiffness . In the case of first-order elements, you may define the slenderness compensation factor by including , and any values values are calculated from the elastic material the label SCF. Abaqus will then use a slenderness compensation factor of of definition. that you specify are ignored. Instead, the The transverse shear stiffness is not relevant to Euler-Bernoulli beam elements for which the transverse shear constraints are satisfied exactly. Input File Usage: Abaqus/CAE Usage: Use both of the following options to define the transverse shear stiffness for beam sections integrated during the analysis: *BEAM SECTION *TRANSVERSE SHEAR STIFFNESS Use both of the following options to define the transverse shear stiffness for general beam sections: *BEAM GENERAL SECTION *TRANSVERSE SHEAR STIFFNESS To define transverse shear stiffness for beam sections integrated during the analysis: Property module: beam section editor: Section integration: During analysis: Stiffness: toggle on Specify transverse shear To define transverse shear stiffness for general beam sections: Property module: beam section editor: Section integration: Before analysis: Stiffness, toggle on Specify transverse shear Interpolation Abaqus provides finite axial strain, shear flexible beams with linear and quadratic interpolations. Their formulation is described in “Beam element formulation,” Section 3.5.2 of the Abaqus Theory Manual. Element types B21, B31, B31OS, PIPE21, PIPE31, and their hybrid equivalents use linear interpolation. These elements are well suited for cases involving contact, such as the laying of a pipeline in a trench or on the seabed or the contact between a drill string and a well hole, and for dynamic versions of similar problems (impact). Element types B22, B32, B32OS, PIPE22, PIPE32, and their hybrid equivalents use quadratic interpolation. Mass formulation The linear Timoshenko beam elements use a lumped mass formulation by default. The quadratic Timoshenko beam elements in Abaqus/Standard use a consistent mass formulation, except in dynamic procedures in which a lumped mass formulation with a 1/6, 2/3, 1/6 distribution is used. For details, see “Mass and inertia for Timoshenko beams,” Section 3.5.5 of the Abaqus Theory Manual. The quadratic Timoshenko beam elements in Abaqus/Explicit use a lumped mass formulation with a 1/6, 2/3, 1/6 distribution. Using a consistent mass matrix in Abaqus/Standard Alternatively, in Abaqus/Standard you can use the McCalley-Archer consistent mass matrix based on the cubic interpolation of deflections and quadratic interpolation of rotations. Input File Usage: Abaqus/CAE Usage: Use the following option for linear Timoshenko beam elements with beam sections integrated during the analysis: *BEAM SECTION, LUMPED=NO Use the following option for linear Timoshenko beam elements with general beam sections: *BEAM GENERAL SECTION, LUMPED=NO Use the following option for linear Timoshenko beam elements with beam sections integrated during the analysis: Property module: beam section editor: Section integration: During analysis: Stiffness tabbed page: toggle on Use consistent mass matrix formulation Use the following option for linear Timoshenko beam elements with general beam sections: Property module: beam section editor: Section integration: Before analysis: Stiffness tabbed page: toggle on Use consistent mass matrix formulation Rotary inertia treatment and additional beam inertia the exact (anisotropic with displacement-rotation coupling) rotary inertia is used for By default, Timoshenko beams. Optionally, an uncoupled isotropic approximation to the rotary inertia can be used. See “Rotary inertia for Timoshenko beams” in “Beam section behavior,” Section 29.3.5, for further details. The exception to this rule is the static procedure with automatic stabilization , where the mass matrix for Timoshenko beams is always calculated assuming isotropic rotary inertia, regardless of the type of rotary inertia specified for the beam section definition . In some structural applications the beam element may be a one-dimensional approximation of a structure with complex cross-sectional geometry and mass distribution. In such a cross-section there may be inertia contributions that represent heavy machinery, cargo loaded in a ship compartment, fluid-filled ballast tanks, or any other mass distributed along the length of the beam that is not part of the beam’s structural stiffness. In such cases you can define additional mass and rotary inertia associated with the beam section properties. Multiple masses per unit length (with location other than the origin of the beam cross-section) and rotary inertias per unit length can be specified. Mass proportional damping (alpha or composite damping) associated with this additional inertia can also be specified. Abaqus will use the mass weighted average (based on the material damping and the added inertial damping) for the element mass proportional damping. See “Material damping,” Section 26.1.1, for details. Additional inertia due to immersion in fluid When a beam is fully or partially submerged, the effect of the surrounding fluid can be modeled as an additional distributed inertia on the beam. See “Additional inertia due to immersion in fluid” in “Beam section behavior,” Section 29.3.5, for details. Warping (open-section) beams When modeling beams in space, a further consideration arises from the possible warping of the beam’s cross-section under torsional loading. For all but circular sections the beam’s cross-section will deform out of its original plane when subject to torsion. This warping deformation will modify the shear strain distribution throughout the section. Open sections will typically twist very easily if warping is not prevented, especially if the walls that form the beam section are thin. Constraint of this warping at certain points along the beam (such as where the beam is built into some other member, Figure 29.3.3–1, or into a wall) is then a major determinant of the beam’s overall torsional response. Figure 29.3.3–1 Intersection of open section beams. Element types B31OS, B32OS (and their “hybrid” equivalents) have the warping magnitude, w, as a degree of freedom at each node; they are available only in Abaqus/Standard. In these elements Abaqus/Standard assumes that the warping of the cross-section follows a certain pattern as a function of position in the cross-section (Abaqus will calculate this warping pattern if you have specified a standard library section or an “arbitrary” section): only the warping magnitude varies with position along the beam’s axis. These elements are meant for the analysis of thin-walled open sections in which warping constraints play a role and the axial strains due to warping cannot be neglected. Examples of such open sections that may warp in this fashion are the I-section and any open arbitrary section. In the other beam element types warping is considered unconstrained and any axial stress due to warping is neglected; torsional behavior will not be represented adequately when these element types are used with thin-walled, open sections. In general, the warping magnitude can be continuous only when the beam axis is continuous through a node and the beam cross-section is the same on both sides of the node. Thus, if open-section members intersect at a node (such as the cross-member of a vehicle chassis abutting a longitudinal member, Figure 29.3.3–1), separate nodes may have to be used for the intersecting members with different axial directions and appropriate constraints must be chosen for the warping amplitudes in each member at this point. The choice of these constraints is a matter of detail of the local construction. For example, if the joint is reinforced, warping may be prevented; therefore, degree of freedom 7 should be fully constrained with a boundary condition on the appropriate members at the joint. “Pipe” elements The pipe elements in Abaqus assume a hollow circular section. The internal stress caused by internal or external pressure loading in the pipe is included in these elements so that on the pipe cross-section a point under tension will have different yield than a point under compression (Figure 29.3.3–2), thus causing an asymmetry in the section’s response to inelastic bending. Two formulations are available for pipe elements in Abaqus. The thin-walled pipe formulation assumes constant hoop stress across the cross- section and neglects the radial stress, whereas thick-walled pipes (available only in Abaqus/Standard) allow the hoop and radial stress components to vary across the cross-section. The hoop stress in thin-walled pipe elements is computed as the average stress in equilibrium with the internal and external pressure loading on the pipe section. For the thin-walled formulation, an integration rule with one point through the thickness suffices to obtain an accurate solution. For thick-walled pipes, the hoop stress and radial stress variation under applied internal and/or external pressure are calculated using Lamé’s equations. The constitutive calculations at each material point take into account the imposed hoop and radial stress values to determine the structural response. A two-dimensional integration rule is used for thick-walled pipes to capture the effect of stress variation across the section accurately. “Hybrid” beams Hybrid beam element types (B21H, B33H, etc.) are provided in Abaqus/Standard for use in cases where it is numerically difficult to compute the axial and shear forces in the beam by the usual finite element displacement method. This problem arises most commonly in geometrically nonlinear analysis when the beam undergoes large rotations and is very rigid in axial and transverse shear deformation, such as a link in a vehicle’s suspension system or a flexing long pipe or cable. The problem in such cases is that slight differences in nodal positions can cause very large forces, which, in turn, cause large motions in other directions. The hybrid elements overcome this difficulty by using a more general formulation in which the axial and transverse shear forces in the elements are included, along with the nodal displacements and rotations, as primary variables. Although this formulation makes these elements more expensive, they generally converge much faster when the beam’s rotations are large and, therefore, are more efficient overall in such cases. Additional references • Archer, J. S., “Consistent Matrix Formulations for Structural Analysis using Finite-Element Techniques,” American Institute of Aeronautics and Astronautics Journal, vol. 3, pp. 1910–1918, 1965. • Cowper, R. G., “The Shear Coefficient in Timoshenko’s Beam Theory,” Journal of Applied Mechanics, vol. 33, pp. 335–340, 1966. σ hoop hoop stress caused by pressurization σ axial asymmetric stress limits in tension and compression Mises yield surface Figure 29.3.3–2 Yield behavior in thin-walled PIPE elements. 29.3.4 BEAM ELEMENT CROSS-SECTION ORIENTATION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Beam modeling: overview,” Section 29.3.1 • “Beam cross-section library,” Section 29.3.9 • “Beam section behavior,” Section 29.3.5 • “Assigning a beam orientation,” Section 12.15.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The orientation of a beam cross-section: • is defined in terms of a local, right-handed axis system; and • can be user-defined or calculated by Abaqus. Beam cross-sectional axis system The orientation of a beam cross-section is defined in Abaqus in terms of a local, right-handed ( , axis system, where the second node of the element, and of the cross-section. to the beam. This beam cross-sectional axis system is illustrated in Figure 29.3.4–1. ) is the tangent to the axis of the element, positive in the direction from the first to are basis vectors that define the local 1- and 2-directions is referred to as the normal is referred to as the first beam section axis, and and , Defining the n1 -direction For beams in a plane the motion occurs. Therefore, planar beams can bend only about the first beam-section axis. -direction is always (0.0, 0.0, −1.0); that is, normal to the plane in which the For beams in space the approximate direction of must be defined directly as part of the beam section definition or by specifying an additional node off the beam axis as part of the element definition . This additional node is included in the element’s connectivity list. • If an additional node is specified, the approximate direction of from the first node of the element to the additional node. is defined by the vector extending • If is defined directly for the section and an additional node is specified, the direction calculated by using the additional node will take precedence. • If the approximate direction is not defined by either of the above methods, the default value is (0.0, 0.0, −1.0). n2 n1 Figure 29.3.4–1 Local axis definition for beam-type elements. This approximate -direction may be used to determine the -direction has been defined or calculated, the actual -direction (discussed below). Once the , possibly -direction will be calculated as resulting in a direction that is different from the specified direction. Input File Usage: Use the following option to specify the integrated during the analysis: *BEAM SECTION -direction directly for a beam section -direction (the data line number depends on the value of the SECTION parameter) Use the following option to specify the section: *BEAM GENERAL SECTION -direction directly for a general beam -direction (the data line number depends on the value of the SECTION parameter) -direction: Use the following option to specify an additional node off the beam axis to define the *ELEMENT Property module: Assign→Beam Section Orientation: select region and enter the -direction Specifying an additional node off Abaqus/CAE. the beam axis is not supported in 29.3.4–2 Defining nodal normals For beams in space you can define the nodal normal ( -direction) by giving its direction cosines as the fourth, fifth, and sixth coordinates of each node definition or by giving them in a user-specified normal definition; see “Normal definitions at nodes,” Section 2.1.4, for details. Otherwise, the nodal normal will be calculated by Abaqus, as described below. If the nodal normal is defined as part of the node definition, this normal is used for all of the structural elements attached to the node except those for which a user-specified normal is defined. If a user-specified normal is defined at a node for a particular element, this normal definition takes precedence over the normal defined as part of the node definition. If the specified normal subtends an angle that is greater than 20° with the plane perpendicular to the element axis, a warning message is issued in the data (.dat) file. If the angle between the normal defined as part of the node definition or the user-specified normal and is greater than 90°, the reverse of the specified normal is used. Input File Usage: Abaqus/CAE Usage: Use the following option to specify the definition: *NODE node number, nodal coordinates, nodal normal coordinates -direction as part of the node Use the following option to define a user-specified normal: *NORMAL Defining the nodal normal is not supported in Abaqus/CAE; the nodal normal calculated by Abaqus is always used. Calculation of the average nodal normals by Abaqus If the nodal normal is not defined as part of the node definition, element normal directions at the node are calculated for all shell and beam elements for which a user-specified normal is not defined (the “remaining” elements). For shell elements the normal direction is orthogonal to the shell midsurface, as described in “Shell elements: overview,” Section 29.6.1. For beam elements the normal direction is the second cross-section direction, as described in “Beam element cross-section orientation,” Section 29.3.4. The following algorithm is then used to obtain an average normal (or multiple averaged normals) for the remaining elements that need a normal defined: 1. If a node is connected to more than 30 remaining elements, no averaging occurs and each element is assigned its own normal at the node. The first nodal normal is stored as the normal defined as part of the node definition. Each subsequent normal is stored as a user-specified normal. 2. If a node is shared by 30 or fewer remaining elements, the normals for all the elements connected to the node are computed. Abaqus takes one of these elements and puts it in a set with all the other elements that have normals within 20° of it. Then: a. Each element whose normal is within 20° of the added elements is also added to this set (if it is not yet included). b. This process is repeated until the set contains for each element in the set all the other elements whose normals are within 20°. c. If all the normals in the final set are within 20° of each other, an average normal is computed for all the elements in the set. If any of the normals in the set are more than 20° out of line from even a single other normal in the set, no averaging occurs for elements in the set and a separate normal is stored for each element. d. This process is repeated until all the elements connected to the node have had normals computed for them. e. The first nodal normal is stored as the normal defined as part of the node definition. Each subsequently generated nodal normal is stored as a user-specified normal. This algorithm ensures that the nodal averaging scheme has no element order dependence. A simple example illustrating this process is included below. Example: beam normal averaging Consider the three beam element model in Figure 29.3.4–2. Elements 1, 2, and 3 share a common node 10, with no user-specified normal defined. 10 20 40 30 Figure 29.3.4–2 Three-element example for nodal averaging algorithm. In the first scenario, suppose that at node 10 the normal for element 2 is within 20° of both elements 1 and 3, but the normals for elements 1 and 3 are not within 20° of each other. In this case, each element is assigned its own normal: one is stored as part of the node definition and two are stored as user-specified normals. In the second scenario, suppose that at node 10 the normal for element 2 is within 20° of both elements 1 and 3 and the normals for elements 1 and 3 are within 20° of each other. In this case, a single average normal for elements 1, 2, and 3 would be computed and stored as part of the node definition. In the last scenario, suppose that at node 10 the normal for element 2 is within 20° of element 1 but the normal of element 3 is not within 20° of either element 1 or 2. In this case, an average normal is computed and stored for elements 1, and 2 and the normal for element 3 is stored by itself: one is stored as part of the node definition and the other is stored as a user-specified normal. Appropriate beam normals To ensure proper application of loads that act normal to the beam cross-section, it is important to have beam normals that correctly define the plane of the cross-section. When linear beams are used to model a curved geometry, appropriate beam normals are the normals that are averaged at the nodes. For such cases it is preferable to define the cross-sectional axis system such that beam normals lie in the plane of curvature and are properly averaged at the nodes. Initial curvature and initial twist In Abaqus/Standard normal direction definitions can result in a beam element having an initial curvature or an initial twist, which will affect the behavior of some elements. • When the normal to an element is not perpendicular to the beam axis (obtained by interpolation using the nodes of the element), the beam element is curved. Initial curvature can result when you define the normal directly (as part of the node definition or as a user-specified normal) or can result when beams intersect at a node and the normals to the beams are averaged as described above. The effect of this initial curvature is considered in cubic beam elements. Initial curvature resulting from normal definitions is not considered in quadratic beam elements; however, these elements do properly account for any initial curvature represented by the node positions. • Similarly, nodal-normal directions that are in different orientations about the beam axis at different nodes imply a twist. The effect of an initial twist, which could result from normal averaging or user-defined normal definitions, is considered in quadratic beam elements. Since the behavior of initially curved or initially twisted beams is quite different from straight beams, the changes caused by averaging the normals may result in changes in the deformation of some beam elements. You should always check the model to ensure that the changes caused by averaging the normals are intended. If the normal directions at successive nodes subtend an angle that is greater than 20°, a warning message is issued in the data (.dat) file. In addition, a warning message will be issued during input file preprocessing if the average curvature computed for a beam differs by more than 0.1 degrees per unit length or if the approximate integrated curvature for the entire beam differs by more than 5 degrees as compared to the curvature computed without nodal averaging and without user-defined normals. In Abaqus/Explicit initial curvature of the beam is not taken into account: all beam elements are assumed to be initially straight. The element’s cross-section orientation is calculated by averaging the -directions associated with its nodes. These two vectors are then projected onto the plane that are made orthogonal is perpendicular to the beam element’s axis. These projected directions to each other by rotating in this plane by an equal and opposite angle. - and and 29.3.5 BEAM SECTION BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Beam modeling: overview,” Section 29.3.1 • *BEAM GENERAL SECTION • *BEAM SECTION • “Creating beam sections,” Section 12.13.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The beam section behavior: • is defined in terms of the response of the beam section to stretching, bending, shear, and torsion; • may or may not require numerical integration over the section; and • can be linear or nonlinear (as a result of nonlinear material response). Beam section behavior Defining a beam section’s response to stretching, bending, shear, and torsion of the beam’s axis requires a suitable definition of the axial force, N; bending moments, ; and torque, T, as functions and of the axial strain, . Here the subscripts 1 and 2 refer to ; curvature changes, local, orthogonal axes in the beam section. ; and twist, and If open-section beam types are used, the section behavior must also define the warping bimoment, W, and the generalized strain measures include the warping amplitude, w, and the bicurvature of the beam, , which is the gradient of the warping amplitude with respect to position along the beam: . The type of section definition you choose determines whether the beam section properties are recomputed during the progression of the analysis or established in the preprocessor for the duration If a general beam section definition is used , the cross-section properties are computed once, during preprocessing. Alternatively, a beam section definition that is integrated during the analysis can be used , in which case Abaqus will use numerical integration of the stress over the cross-section to define the beam’s response as the analysis proceeds. Since planar beams deform only in the X–Y plane, only N and , , and w are assumed to be zero. the response in these elements: , and and , contribute to In Abaqus bending moments in beam sections are always measured about the centroid of the beam section, while torque is measured with respect to the shear center. The beam axis (defined as the line joining the nodes that define the beam element) need not pass through the centroid of the beam section. coordinate system defined in the cross-section of the beam; that is, the line of the element connecting the element’s nodes passes through the origin of the cross-section’s local coordinate system. The degrees of freedom of the beam element are at the origin of the local Determining whether to use a beam section integrated during the analysis or a general beam section When a beam section integrated during the analysis is used , Abaqus integrates numerically over the section as the beam deforms, evaluating the material behavior independently at each point on the section. This type of beam section should be used when the section nonlinearity is caused only by nonlinear material response. When a general beam section is used , Abaqus precomputes the beam cross-section quantities and performs all section computations during the analysis in terms of the precomputed values. This method combines the functions of beam section and material descriptions (a material definition is not needed). The precomputed section properties may be specified in a variety of ways, including quite complex geometries defined with a two-dimensional finite element mesh . A general beam section should be used when the beam section response is linear or when it is nonlinear and the nonlinearity arises from more than just material nonlinearity, such as in cases when section collapse occurs. Input File Usage: Use the following option to define a beam section integrated during the analysis: *BEAM SECTION Use the following option to define a general beam section: *BEAM GENERAL SECTION To define a beam section integrated during the analysis: Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: During analysis To define a general beam section: Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: Before analysis Geometric section quantities The section quantities described below are needed to define the behavior of a general beam section. Moments of inertia The moments of inertia with respect to the centroid are defined as and where ( position of the centroid of the cross-sectional area. ) is the position of the point in the local beam section axis system and ( ) is the Bending stiffness and rotary inertia contributions for a meshed section profile are calculated using the two-dimensional cross-section model. The following integrated properties are defined for the entire cross-section model meshed with warping elements: and where ( ) is the center of mass of the cross section. Torsional constant The torsional constant, J, depends on the shape of the cross section. The torsional constant of a circular section is the polar moment of inertia, . The torsional constant for the rectangular and trapezoidal library sections is calculated numerically by Abaqus using the Prandtl stress function approach. A local finite element model of the cross-section is created internally for this purpose. The number of integration points selected for the cross-section determines the accuracy of this finite element model. For increased accuracy specify a higher-order rule by selecting nondefault integration. The above rule is also applied to both the thin-walled box section and the arbitrary section to increase the accuracy of the model. If the thickness for each segment making up the section varies significantly, more integration points for the box section or smaller segments for the arbitrary section should be specified in the area where the thickness varies. The torsional stiffness for a meshed section is calculated over the two-dimensional region meshed with warping elements. The accuracy of the integration depends on the number of elements in the model: where denotes the derivative of the warping function with respect to the cross-section (1, 2) axis and is the position of the shear center of the cross-sectional area. All indices take values 1, 2. For more details, see “Meshed beam cross-sections,” Section 3.5.6 of the Abaqus Theory Manual. For closed thin-walled sections the torsional constant is calculated from where t is the thickness of the section, is the area enclosed by the median line of the section, and s is the length of the median line, measured along the circumference of the section in a counterclockwise direction. For open, built-up, thin-walled sections, Abaqus will check if a built-up section is closed or not and will use the appropriate torsional constant. Sectorial moment and warping constant For open, thin-walled sections the sectorial moment is defined as and the warping constant is defined as where is the sectorial area at a point in the section with the shear center as its pole. Rotary inertia for Timoshenko beams In general, the rotary inertia associated with torsional modes is different from that of flexural modes. For unsymmetric cross-sections the rotary inertia is different in each direction of bending. For cross-sections where the beam node is not located at the center of mass, coupling exists between the translational and rotational degrees of freedom. By default, the exact (anisotropic and coupled) rotary inertia is used for Timoshenko beams. In Abaqus/Standard the anisotropic rotary inertia introduces unsymmetric terms in the Jacobian operator during geometrically nonlinear, transient, direct-integration dynamic simulations. If the rotary inertia effects are significant in the geometrically nonlinear dynamic response and the exact rotary inertia is used, the unsymmetric solver should be used for better convergence. Optionally, an approximate isotropic and uncoupled rotary inertia can be selected. In Abaqus/Standard this means that the rotary inertia associated with the torsional mode only is used for all rotational degrees of freedom; potentially destabilizing rotary inertia effects in impact problems due to the anisotropy or displacement-rotation coupling will not be introduced. In Abaqus/Explicit this means a scaled flexural inertia with a scaling factor chosen to maximize the stable element time increment is used for all rotational degrees of freedom; i.e., the stable time increment will not be determined by the flexural response of the beam. In some slender beam analyses an isotropic approximation to the rotary inertia may be accurate enough. If beam elements are used to model plate-type structures in Abaqus/Explicit (i.e., if the moment of inertia about one section axis of the beam is more than a thousand times greater than the moment of inertia about the other axis), the exact rotary inertia formulation may lead to a sharp cut-back in the stable time increment. In this case it is recommended that you either use the isotropic approximation or alternatively consider modeling the structure with shell elements, which might be better suited to this type of analysis. For a definition of rotary inertia for the beam’s cross-section, see “Mass and inertia for Timoshenko beams,” Section 3.5.5 of the Abaqus Theory Manual. Input File Usage: Use the following option to specify isotropic rotary inertia for a beam section integrated during the analysis: *BEAM SECTION, ROTARY INERTIA=ISOTROPIC Use the following option to specify isotropic rotary inertia for a general beam section: Abaqus/CAE Usage: *BEAM GENERAL SECTION, ROTARY INERTIA=ISOTROPIC Isotropic rotary inertia for beam sections is not supported in Abaqus/CAE. The default exact rotary inertia is always used. Adding inertia to the beam section behavior for Timoshenko beams Additional mass and rotary inertia properties for Timoshenko beams (including PIPE elements) can be defined. This added inertia defined within the cross-section per unit length along the beam contributes to the inertia response of the beam without contributing to the structural stiffness. Additional beam inertia cannot be defined for a section if isotropic rotary inertia is used. To specify additional beam inertia, you define the mass (per unit length) with the mass center in the local (1, 2) beam cross-section axis system. To include rotary inertia (in degrees) within the cross-section local (1, 2) system relative to the local 1-direction positioned at point (per unit length), you can also define the angle that positions the first axis of the rotary inertia coordinate system in the beam cross-section axis system. See Figure 29.3.5–1 for an illustration. x 2 x 1 Figure 29.3.5–1 Beam element with added inertia. The rotary inertia components relative to the rotary inertia coordinate system are defined as and where A is the area, measured from is the mass density, and X and Y are the local rotary inertia system coordinates , the center of the added mass contribution. As many point masses and rotary inertia contributions as are needed to define the added inertia can be specified. Mass proportional damping associated with the added inertia can be specified by assigning a value to the mass proportional Rayleigh damping coefficient, , or the composite damping coefficient, . Abaqus will use the mass weighted average (based on the material damping and the added inertia damping) for the element mass proportional damping. Input File Usage: Use the following option in conjunction with the beam section definition to specify additional inertia properties: *BEAM ADDED INERTIA, ALPHA= mass per unit length, , , , , , COMPOSITE= , Abaqus/CAE Usage: Additional inertia properties are not supported in Abaqus/CAE. Additional inertia due to immersion in fluid When a beam is fully or partially submerged, the effect of the surrounding fluid can be modeled as an additional distributed inertia on the beam . By default, the beam is assumed to be fully submerged. Alternatively, you can specify that the added inertia per unit length should be reduced by a factor of one-half to model a partially submerged beam. You specify the fluid mass density, (per unit volume); beam local x and y coordinates of the wetted cross-section centroid; wetted section effective radius, r; and empirical drag or flow coefficients, and . The inertia added per unit length to a fully immersed beam cross-section is given by Because the beam cross-section origin may not be coincident with the centroid of the wetted cross-section, the additional fluid inertia may include rotary effects. Nonzero values for the x- and y-offsets of the wetted cross-section centroid will produce rotation-displacement coupling in the inertia formulation. The default model for the added inertia derives from inviscid flow around a cylindrical cross-section ( , that models flow around a different cross-section geometry. ); you can specify a coefficient, An immersed beam also experiences an additional added mass effect at its free ends. If a beam element’s end node is not attached to any other element and additional fluid inertia is defined for this element, an additional mass may be added in the form: For this added mass corresponds to that of a hemispherical cap; the default value is can be changed to model other geometries. If the beam is partially submerged, the end inertia is automatically reduced by one-half. However, the added mass at the free ends is always isotropic: axial and transverse motions experience the same additional inertia. . The coefficient The “virtual mass” added to a submerged or partially submerged beam is not included in the total mass, center of mass, moments, or products of inertia reported in the data (.dat) file. Input File Usage: Use the following option in conjunction with the beam section definition to define a fully immersed beam: *BEAM FLUID INERTIA, FULL , x, y, r, , Use the following option in conjunction with the beam section definition to define a partially immersed beam: *BEAM FLUID INERTIA, HALF , x, y, r, , Abaqus/CAE Usage: To define a fully immersed beam: Property module: beam section editor: Fluid Inertia: toggle on Specify fluid inertia effects: Fully submerged To define a partially immersed beam: Property module: beam section editor: Fluid Inertia: toggle on Specify fluid inertia effects: Half submerged Additional reference • Blevins, R. D., Formulas for Natural Frequency and Mode Shape, R. E. Krieger Publishing Co., Inc., 1987. 29.3.6 USING A BEAM SECTION INTEGRATED DURING THE ANALYSIS TO DEFINE THE SECTION BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Beam modeling: overview,” Section 29.3.1 • “Beam section behavior,” Section 29.3.5 • *BEAM SECTION • “Specifying properties for beam sections integrated during analysis” in “Creating beam sections,” Section 12.13.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A beam section integrated during the analysis: • is used when section properties must be recomputed as the beam deforms over the course of the analysis; and • can be associated with linear or nonlinear material behavior. Defining the behavior of a beam section integrated during the analysis Use a beam section integrated during the analysis to define the section behavior when numerical integration over the section is required as the beam deforms. You can choose a section shape from the library of beam section shapes provided and define the section’s dimensions. In addition, you can specify the number of section points to use for integration. The default number of section points is adequate for monotonic loading that causes plasticity. If reversed plasticity will occur, more section points are required. Use a material definition (“Material data definition,” Section 21.1.2) to define the material properties of the section, and associate these properties with the section definition. Linear or nonlinear material behavior can be associated with the section definition. However, if the material response is linear, the more economic approach is to use a general beam section . You must associate the section properties with a region of your model. Input File Usage: *BEAM SECTION, ELSET=name, SECTION=library_section, MATERIAL=name The ELSET parameter is used to associate the section properties with a set of beam elements. Abaqus/CAE Usage: Property module: Create Profile: Name: library_section Create Section: select Beam as the section Category and Beam as the section Type: Section integration: During analysis, Profile name: library_section, Material name: name Assign→Section: select regions Defining a change in cross-sectional area due to straining In the shear flexible elements Abaqus provides for a possible uniform cross-sectional area change by allowing you to specify an effective Poisson’s ratio for the section. This effect is considered only in geometrically nonlinear analysis and is provided to model the reduction or increase in the cross-sectional area for a beam subjected to large axial stretch. The value of the effective Poisson’s ratio must be between −1.0 and 0.5. By default, this effective Poisson’s ratio for the section is set to 0.0 so that this effect is ignored. Setting the effective Poisson’s ratio to 0.5 implies that the overall response of the section is incompressible. This behavior is appropriate if the beam is made of a typical metal whose overall response at large deformation is essentially incompressible (because it is dominated by plasticity). Values between 0.0 and 0.5 mean that the cross-sectional area changes proportionally between no change and incompressibility, respectively. A negative value of the effective Poisson’s ratio will result in an increase in the cross-sectional area in response to tensile axial strains. This effective Poisson’s ratio is not available for use with Euler-Bernoulli beam elements. Input File Usage: Abaqus/CAE Usage: *BEAM SECTION, POISSON= Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: During analysis, Section Poisson's ratio: Defining material damping When a beam section integrated during the analysis is used, damping can be introduced through the material behavior definition. See “Material damping,” Section 26.1.1, for more information about the material damping types available in Abaqus. Specifying temperature and field variables Temperature and field variables can be specified at specific points through the section or by defining the value at the origin of the cross-section and specifying the gradients in the local 1- and 2-directions. The actual values of the temperature and field variables are specified as either predefined fields or initial conditions . In any element it is assumed that the temperature definitions at all the nodes of the element are compatible with the temperature definition method chosen for the element. For cases in which the temperature definition method changes from one element to the next, separate nodes must be used on the interface between elements with different temperature definition methods and MPCs must be applied to make the displacements and rotations the same at the nodes. By defining the value at the origin and the gradients in the 1- and 2-directions Temperatures and field variables can be defined by giving the value at the origin of the cross-section and the gradients in the 2- and 1-directions of the cross-section (that is, give in the predefined field or initial condition definition). For beams in a plane only and need be given; gradients in the 1-direction are ignored in this case. and Input File Usage: Abaqus/CAE Usage: *BEAM SECTION, TEMPERATURE=GRADIENTS Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: During analysis, Linear by gradients By defining the values at points through the section Temperatures and field variables can be defined at a set of points on the section, as indicated for each cross-section in “Beam cross-section library,” Section 29.3.9. This technique cannot be used for any beam element that is adjacent to a general beam section element, as it can lead to incorrect temperature distributions at the shared cross-section. If you cannot avoid this modeling scenario, you must define the adjacent elements using separate nodes connected by MPCs, as discussed above. Input File Usage: Abaqus/CAE Usage: *BEAM SECTION, TEMPERATURE=VALUES Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: During analysis, Interpolated from temperature points Output Beam section properties such as cross-sectional area, moments of inertia, etc. are printed in the model data output. When a beam section integrated during the analysis is used, section forces, moments, and transverse shear forces and section strains, curvatures, and transverse shear strains can be output for the section . In addition, stress and strain can be output at each section point. “Beam element library,” Section 29.3.8, lists some of the element output quantities that are available for beam elements. Axial strains due to warping are included in the stress/strain output from Abaqus/Standard if a beam section integrated during the analysis is used. Temperature output at the section points can be obtained using the element variable TEMP. If the temperatures are given at specific points through the section, output at the temperature points can be obtained using the nodal variable NTxx. The nodal variable NTxx should not be used for output at the temperature points if the temperatures are specified by defining the value at the origin of the cross-section and specifying the gradients in the local 1- and 2-directions. In this case output variable NT should be requested; NT11 (the reference temperature value) and NT12 and NT13 (the temperature gradients in the local 1- and 2-directions, respectively) will be output automatically. Beam normals are written to the output database automatically for all frames that include field output of nodal displacements. The normal directions can be visualized in the Visualization module of Abaqus/CAE. 29.3.7 USING A GENERAL BEAM SECTION TO DEFINE THE SECTION BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Beam modeling: overview,” Section 29.3.1 • “Beam section behavior,” Section 29.3.5 • *BEAM GENERAL SECTION • “Specifying properties for general beam sections” in “Creating beam sections,” Section 12.13.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview A general beam section: • is used to define beam section properties that are computed once and held constant for the entire analysis; • can be used to define linear or nonlinear section behavior; • for linear section behavior can be associated only with linear material behavior • enables the use of meshed cross-sections (“Meshed beam cross-sections,” Section 10.6.1); and • enables the use of tapered cross-sections (Abaqus/Standard only). Linear section behavior Linear section response is calculated as follows. At each point in the cross-section the axial stress, and the shear stress, , are given by , where and is Young’s modulus (which may depend on the temperature, beam axis); is the shear modulus (which may also depend on the temperature and field variables at the beam axis); is the axial strain; is the shear caused by twist; and is the thermal expansion strain. , and field variables, , at the The thermal expansion strain is given by where is the thermal expansion coefficient, is the current temperature at a point in the beam section, are field variables, is the reference temperature for is the initial temperature at this point , and are the initial values of the field variables at this point . , If the thermal expansion coefficient is temperature or field-variable dependent, it is evaluated at the temperature and field variables at the beam axis. Therefore, since we assume that varies linearly over the section, also varies linearly over the section. The temperature is defined from the temperature of the beam axis and the gradients of temperature with respect to the local - and -axes: The axial force, N; bending moments, and T; and bimoment, W, are defined in terms of the axial stress formulation,” Section 3.5.2 of the Abaqus Theory Manual). These terms are about the 1 and 2 beam section local axes; torque, (see “Beam element and the shear stress is the area of the section, is the moment of inertia for bending about the 1-axis of the section, is the moment of inertia for cross-bending, is the moment of inertia for bending about the 2-axis of the section, is the torsional constant, is the sectorial moment of the section, is the warping constant of the section, is the axial strain measured at the centroid of the section, 29.3.7–2 where is the thermal axial strain, is the curvature change about the first beam section local axis, is the curvature change about the second beam section local axis, is the twist, is the bicurvature defining the axial strain in the section due to the twist of the beam, and is the difference between the unconstrained warping amplitude, warping amplitude, w. , and the actual , , , and are nonzero only for open-section beam elements. Defining linear section behavior for library cross-sections or linear generalized cross-sections Linear beam section response is defined geometrically by A, , , , J, and—if necessary— and . You can input these geometric quantities directly or specify a standard library section and Abaqus will calculate these quantities. In either case define the orientation of the beam section ; give Young’s modulus, the torsional shear modulus, and the coefficient of thermal expansion, as functions of temperature; and associate the section properties with a region of your model. If the thermal expansion coefficient is temperature dependent, the reference temperature for thermal expansion must also be defined as described later in this section. Specifying the geometric quantities directly , J, and—if You can define “generalized” linear section behavior by specifying A, necessary— and directly. In this case you can specify the location of the centroid, thus allowing the bending axis of the beam to be offset from the line of its nodes. In addition, you can specify the location of the shear center. , , , , , , J, Use the following option to define generalized linear beam section properties: *BEAM GENERAL SECTION, SECTION=GENERAL, ELSET=name A, If necessary, use the following option to specify the location of the centroid: *CENTROID If necessary, use the following option to specify the location of the shear center: *SHEAR CENTER Property module: Create Profile: Name: generalized_section, Generalized Create Section: select Beam as the section Category and Beam as the section Type: Section integration: Before analysis, Profile name: generalized_section: Centroid and Shear Center Assign→Section: select regions 29.3.7–3 Input File Usage: Specifying a standard library section and allowing Abaqus to calculate the geometric quantities You can select one of the standard library sections and specify the geometric input data needed to define the shape of the cross-section. Abaqus will then calculate the geometric quantities needed to define the section behavior automatically. Input File Usage: Abaqus/CAE Usage: *BEAM GENERAL SECTION, SECTION=library_section, ELSET=name Property module: Create Profile: Name: library_section Create Section: select Beam as the section Category and Beam as the section Type: Section integration: Before analysis, Profile name: library_section Assign→Section: select regions Defining linear section behavior for meshed cross-sections Linear beam section response for a meshed section profile is obtained by numerical integration from the two-dimensional model. The numerical integration is performed once, determining the beam stiffness and inertia quantities, as well as the coordinates of the centroid and shear center, for the duration of the analysis. These beam section properties are calculated during the beam section generation and are written to the text file jobname.bsp. This text file can be included in the beam model. See “Meshed beam cross-sections,” Section 10.6.1, for a detailed description of the properties defining the linear beam section response for a meshed section, as well as for how a typical meshed section is analyzed. Input File Usage: Use the following options: *BEAM GENERAL SECTION, SECTION=MESHED, ELSET=name *INCLUDE, INPUT=jobname.bsp Abaqus/CAE Usage: Meshed cross-sections are not supported in Abaqus/CAE. Defining linear section behavior for tapered cross-sections in Abaqus/Standard In Abaqus/Standard you can define Timoshenko beams with linearly tapered cross-sections. General beam sections with linear response and standard library sections are supported, with the exception of arbitrary sections. The section parameters are defined at the two end nodes of each beam element. The effective beam area and moment of inertia for bending about the 1- and 2-axis of the section used in the calculation of the beam stiffness matrix, section forces, and stresses are eff eff eff and where the superscripts refer to the two end nodes of the beam. The remaining effective geometric quantities are calculated as the average between the values at the two end nodes. This approximation suffices for mild tapering along each element, but it can lead to large errors if the tapering is not gradual. Abaqus/Standard issues a warning message during input file preprocessing if the area or inertia ratio is larger than 2.0 and an error message if the ratio is larger than 10.0. The effective area and inertia are not used in the computation of the mass matrix. Instead, terms on the diagonal quadrants use the properties from the respective nodes, while off-diagonal quadrants use averaged quantities. For example, the axial inertia a linear element would have the diagonal term coming from node , while node and the two off-diagonal contributions equal . Mild tapering is assumed in this formulation, since the total mass of the element totals contributes with of . Note: When you apply a tapered beam section to geometry in Abaqus/CAE, the full tapering is applied to each element along the beam’s length. For beams that include multiple elements, this modeling style can create a “sawtooth” pattern along the length of the beam. If you want to model gradual tapering along the entire length of the beam in Abaqus/CAE, you must calculate the size and shape of the beam profiles at the intermediate nodes, then apply different tapered beam sections to each beam element along the length. Input File Usage: Use the following option to define linear section behavior of tapered cross- sections: Abaqus/CAE Usage: *BEAM GENERAL SECTION, TAPER, ELSET=name Property module: Create Profile: Name: library_section Create Section: select Beam as the section Category and Beam as the section Type: Section integration: Before analysis, Beam shape along length: Tapered: Beam start and Beam end options: Profile name: library_section Assign→Section: select regions Nonlinear section behavior Typically nonlinear section behavior is used to include the experimentally measured nonlinear response of a beam-like component whose section distorts in its plane. When the section behaves according to beam theory (that is, the section does not distort in its plane) but the material has nonlinear response, it is usually better to use a beam section integrated during the analysis to define the section geometrically , in association with a material definition. Nonlinear section behavior can also be used to model beam section collapse in an approximate sense: “Nonlinear dynamic analysis of a structure with local inelastic collapse,” Section 2.1.1 of the Abaqus Example Problems Manual, illustrates this for the case of a pipe section that may suffer inelastic collapse due to the application of a large bending moment. In following this approach you should recognize that such unstable section collapse, like any unstable behavior, typically involves localization of the deformation: results will, therefore, be strongly mesh sensitive. Calculation of nonlinear section response Nonlinear section response is assumed to be defined by means a functional dependence on the conjugate variables: , where etc. For example, , the temperature of the beam axis; and of , any predefined field variables at the beam axis. When the section behavior is defined in this way, only the temperature and field variables of the beam axis are used: any temperature or field-variable gradients given across the beam section are ignored. means that N is a function of: ; , These nonlinear responses may be purely elastic (that is, fully reversible—the loading and unloading responses are the same, even though the behavior is nonlinear) or may be elastic-plastic and, therefore, irreversible. The assumption that these nonlinear responses are uncoupled is restrictive; in general, there is some interaction between these four behaviors, and the responses are coupled. You must determine if this approximation is reasonable for a particular case. The approach works well if the response is dominated by one behavior, such as bending about one axis. However, it may introduce additional errors if the response involves combined loadings. Defining nonlinear section behavior You can define “generalized” nonlinear section behavior by specifying the area, A; moments of inertia, for bending about the 1-axis of the section, for bending about the 2-axis of the section, and for cross-bending; and torsional constant, J. These values are used only to calculate the transverse shear stiffness; and, if needed, A is used to compute the mass density of the element. In addition, you can define the orientation and the axial, bending, and torsional behavior of the beam section (N, , T), as well as the thermal expansion coefficient. If the thermal expansion coefficient is temperature dependent, the reference temperature for thermal expansion must also be defined as described below. , Nonlinear generalized beam section behavior cannot be used with beam elements with warping degrees of freedom. The axial, bending, and torsional behavior of the beam section and the thermal expansion coefficient are defined by tables. See “Material data definition,” Section 21.1.2, for a detailed discussion of the tabular input conventions. In particular, you must ensure that the range of values given for the variables is sufficient for the application since Abaqus assumes a constant value of the dependent variable outside this range. Input File Usage: Abaqus/CAE Usage: , , J Use the following options to define generalized nonlinear beam section properties: *BEAM GENERAL SECTION, SECTION=NONLINEAR GENERAL, ELSET=name A, , *AXIAL for N *M1 for *M2 for *TORQUE for T *THERMAL EXPANSION for the thermal expansion coefficient Nonlinear generalized cross-sections are not supported in Abaqus/CAE. Defining linear response for N, M1 , M2 , and T If the particular behavior is linear, N, and predefined field variables, if appropriate. As an example of axial behavior, if , , and T should be specified as functions of the temperature where as a function of temperature and field variables. is constant for a given temperature, the value of is entered. can still be varied Input File Usage: Abaqus/CAE Usage: Use the following options to define linear axial, bending, and torsional behavior: *AXIAL, LINEAR *M1, LINEAR *M2, LINEAR *TORQUE, LINEAR Nonlinear generalized cross-sections are not supported in Abaqus/CAE. Defining nonlinear elastic response for N, M1 , M2 , and T If the particular behavior is nonlinear but elastic, the data should be given from the most negative value of the kinematic variable to the most positive value, always giving a point at the origin. See Figure 29.3.7–1 for an example. Input File Usage: Abaqus/CAE Usage: Use the following options to define nonlinear elastic axial, bending, and torsional behavior: *AXIAL, ELASTIC *M1, ELASTIC *M2, ELASTIC *TORQUE, ELASTIC Nonlinear generalized cross-sections are not supported in Abaqus/CAE. Bending moment, M M 5 M 4 The origin should be included in the data M=M6 for K K6 K 2 K 3 K4 K5 K6 Curvature, K M 3 M 2 M 1 M=M1 for K K1 Figure 29.3.7–1 Example of elastic nonlinear beam section behavior definition. Defining elastic-plastic response for N, M1 , M2 , and T By default, elastic-plastic response is assumed for N, , , and T. The inelastic model is based on assuming linear elasticity and isotropic hardening (or softening) plasticity. The data in this case must begin with the point and proceed to give positive values of the kinematic variable at increasing positive values of the conjugate force or moment. Strain softening is allowed. The elastic modulus is defined by the slope of the initial line segment, so that straining beyond the point that terminates that initial line segment will be partially inelastic. If strain reversal occurs in that part of the response, it will be elastic initially. See Figure 29.3.7–2 for an example. Input File Usage: Use the following options to define elastic-plastic axial, bending, and torsional behavior: *AXIAL *M1 *M2 *TORQUE Nonlinear generalized cross-sections are not supported in Abaqus/CAE. Abaqus/CAE Usage: Bending moment, M Elastic-plastic response for continued straining beyond here Elastic modulus defined by first line segment The origin must be the first data point Curvature, K Elastic unloading behavior Response to opposite curvature of the response given Figure 29.3.7–2 Example of inelastic nonlinear beam section behavior definition. Defining the reference temperature for thermal expansion The thermal expansion coefficient may be temperature dependent. In this case the reference temperature for thermal expansion, , must be defined. *BEAM GENERAL SECTION, ZERO= Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: Before analysis: Basic: Specify reference temperature: Input File Usage: Abaqus/CAE Usage: Defining the initial section forces and moments You can define initial stresses for general beam sections that will be applied as initial section forces and moments. Initial conditions can be specified only for the axial force, the bending moments, and the twisting moment. Initial conditions cannot be prescribed for the transverse shear forces. Defining a change in cross-sectional area due to straining In the shear flexible elements Abaqus provides for a possible uniform cross-sectional area change by allowing you to specify an effective Poisson’s ratio for the section. This effect is considered only in geometrically nonlinear analysis and is provided to model the reduction or increase in the cross-sectional area for a beam subjected to large axial stretch. The value of the effective Poisson’s ratio must be between −1.0 and 0.5. By default, this effective Poisson’s ratio for the section is set to 0.0 so that this effect is ignored. Setting the effective Poisson’s ratio to 0.5 implies that the overall response of the section is incompressible. This behavior is appropriate if the beam is made of rubber or if it is made of a typical metal whose overall response at large deformation is essentially incompressible (because it is dominated by plasticity). Values between 0.0 and 0.5 mean that the cross-sectional area changes proportionally between no change and incompressibility, respectively. A negative value of the effective Poisson’s ratio will result in an increase in the cross-sectional area in response to tensile axial strains. This effective Poisson’s ratio is not available for use with Euler-Bernoulli beam elements. Input File Usage: Abaqus/CAE Usage: *BEAM GENERAL SECTION, POISSON= Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: Before analysis: Basic: Section Poisson's ratio: Defining damping When the beam section and material behavior are defined by a general beam section, you can include mass and viscous stiffness proportional damping in the dynamic response (calculated in Abaqus/Standard with the direct time integration procedure, “Implicit dynamic analysis using direct integration,” Section 6.3.2). See “Material damping,” Section 26.1.1, for more information about the material damping types available in Abaqus. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *BEAM GENERAL SECTION *DAMPING Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: Before analysis: Damping: Alpha, Beta, Structural, and Composite Specifying temperature and field variables Define temperatures and field variables by giving the values at the origin of the cross-section as either predefined fields or initial conditions . Temperature gradients can be specified in the local 1- and 2-directions; other field-variable gradients defined through the cross-section will be ignored in the response of beam elements that use a general beam section definition. Output Only the section forces, moments, and transverse shear forces and section strains, curvatures, and transverse shear strains can be output . You can output stress and strain at particular points in the section. For linear section behavior defined using a standard library section or a generalized section, only axial stress and axial strain values are available. For linear section behavior defined using a meshed section, axial and shear stress and strain are available. For nonlinear generalized section behavior, axial strain output only is provided. Specifying the output section points for standard library sections and generalized sections To locate points in the section at which output of axial strain (and, for linear section behavior, axial stress) is required, specify the local coordinates of the point in the cross-section: Abaqus numbers the points 1, 2, … in the order that they are given. The variation of over the section is given by where changes of curvature for the section. are the local coordinates of the centroid of the beam section and and are the For open-section beam element types, the variation of over the section has an additional term of the form is the warping function. The warping function itself is undefined in the general beam section definition. Therefore, Abaqus will not take into account the axial strain due to warping when calculating section points output. Axial strains due to warping are included in the stress/strain output if a beam section integrated during the analysis is used. , where Abaqus uses St. Venant torsion theory for noncircular solid sections. The torsion function and its derivatives are necessary to calculate shear stresses in the plane of the cross-section. The function and its derivatives are not stored for a general beam section. Therefore, you can request output of axial components of stress/strain only. A beam section integrated during the analysis must be used to obtain output of shear stresses. Input File Usage: Use both of the following options to specify the output section points for general beam sections: *BEAM GENERAL SECTION *SECTION POINTS , , ... Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: Before analysis: Output Points: x1, x2, ... Requesting output of maximum axial stress/strain in Abaqus/Standard If you specify the output section points to obtain the maximum axial stress/strain (MAXSS) for a linear generalized section, the output value will be the maximum of the values at the user-specified section points. You must select enough section points to ensure that this is the true maximum. MAXSS output is not available for nonlinear generalized sections or for an Abaqus/Explicit analysis. Specifying the output section points for meshed cross-sections For meshed cross-sections you can indicate in the two-dimensional cross-section analysis the elements and integration points where the stress and strain will be calculated during the subsequent beam analysis. Abaqus will then add the section points specification to the resulting jobname.bsp text file. This text file is then included as the data for the general beam section definition in the subsequent beam analysis. See “Meshed beam cross-sections,” Section 10.6.1, for details. The variation of the axial strain over the meshed section is given by where changes of curvature for the section. are the local coordinates of the centroid of the beam section and and are the The variations of shear components and over the meshed section are given by where beam axis, shear forces. are the local coordinates of the shear center of the beam section, is the twist of the are shear strains due to the transverse is the warping function, and and For the case of an orthotropic composite beam material, the axial stress and the two shear components and are calculated in the beam section (1, 2) axis as follows: where determines the material orientation. Input File Usage: Use both of the following options in the two-dimensional meshed cross-section analysis to specify the output section points for the subsequent beam analysis: *BEAM SECTION GENERATE *SECTION POINTS section_point_label, element_number, integration_point_number Abaqus/CAE Usage: Meshed cross-sections are not supported in Abaqus/CAE. 29.3.8 BEAM ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Beam modeling: overview,” Section 29.3.1 • “Choosing a beam element,” Section 29.3.3 • *BEAM GENERAL SECTION • *BEAM SECTION Overview This section provides a reference to the beam elements available in Abaqus/Standard and Abaqus/Explicit. Element types Beams in a plane B21 B21H(S) B22 B22H(S) B23(S) B23H(S) PIPE21 2-node linear beam 2-node linear beam, hybrid formulation 3-node quadratic beam 3-node quadratic beam, hybrid formulation 2-node cubic beam 2-node cubic beam, hybrid formulation 2-node linear pipe PIPE21H(S) PIPE22(S) PIPE22H(S) 2-node linear pipe, hybrid formulation 3-node quadratic pipe 3-node quadratic pipe, hybrid formulation Active degrees of freedom 1, 2, 6 Additional solution variables All of the cubic beam elements have two additional variables relating to axial strain. The linear thin-walled pipe elements have one additional variable, and the quadratic thin-walled pipe elements have two additional variables relating to the hoop strain. The linear thick-walled pipe elements have two additional variables, and the quadratic thick-walled pipe elements have four additional variables relating to the hoop and radial strain components. The hybrid beam and pipe elements have additional variables relating to the axial force and transverse shear force. The linear elements have two, the quadratic elements have four, and the cubic elements have three additional variables. Beams in space B31 B31H(S) B32 B32H(S) B33(S) B33H(S) PIPE31 2-node linear beam 2-node linear beam, hybrid formulation 3-node quadratic beam 3-node quadratic beam, hybrid formulation 2-node cubic beam 2-node cubic beam, hybrid formulation 2-node linear pipe PIPE31H(S) PIPE32(S) PIPE32H(S) 2-node linear pipe, hybrid formulation 3-node quadratic pipe 3-node quadratic pipe, hybrid formulation Active degrees of freedom 1, 2, 3, 4, 5, 6 Additional solution variables All of the cubic beam elements have two additional variables relating to axial strain. The linear thin-walled pipe elements have one additional variable, and the quadratic thin-walled pipe elements have two additional variables relating to the hoop strain. The linear thick-walled pipe elements have two additional variables, and the quadratic thick-walled pipe elements have four additional variables relating to the hoop and radial strain components. The hybrid beam and pipe elements have additional variables relating to the axial force and transverse shear force in the linear and quadratic elements and to the axial force only in the cubic elements. The linear and cubic elements have three and the quadratic elements have six additional variables. Open-section beams in space B31OS(S) B31OSH(S) B32OS(S) B32OSH(S) 2-node linear beam 2-node linear beam, hybrid formulation 3-node quadratic beam 3-node quadratic beam, hybrid formulation Active degrees of freedom 1, 2, 3, 4, 5, 6, 7 Additional solution variables Element type B31OSH has three additional variables and element type B32OSH has six additional variables relating to the axial force and transverse shear force. Nodal coordinates required Beams in a plane: X, Y, also (optional) , , the direction cosines of the normal. Beams in space: X, Y, Z, also (optional) section axis. , , , the direction cosines of the second local cross- Element property definition For PIPE elements use the pipe section type to specify the thin-walled pipe formulation or the thick pipe section type to specify the thick-walled pipe formulation. No other section types can be used with PIPE elements. For open-section elements use only the arbitrary, I, L, and linear generalized section types. Local orientations defined as described in “Orientations,” Section 2.2.5, cannot be used with beam elements to define local material directions. The orientation of the local beam section axes in space is discussed in “Beam element cross-section orientation,” Section 29.3.4. Input File Usage: Use either of the following options: *BEAM SECTION *BEAM GENERAL SECTION Property module: Create Section: select Beam as the section Category and Beam as the section Type Abaqus/CAE Usage: Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) CENT(S) Abaqus/CAE Load/Interaction Not supported Units Description FL−2 (ML−1 T−2 ) Centrifugal force (magnitude is input , where m is the mass per unit as length and is the angular velocity). Load ID (*DLOAD) CENTRIF(S) Abaqus/CAE Load/Interaction Units Description Rotational body force T−2 Centrifugal load (magnitude is input as the angular velocity). , where is CORIO(S) Coriolis force FL−2 T (ML−1 T−1 ) GRAV Gravity PX PY PZ Line load Line load Line load PXNU Line load LT−2 FL−1 FL−1 FL−1 FL−1 PYNU Line load FL−1 PZNU Line load FL−1 P1 Line load FL−1 29.3.8–4 Coriolis force (magnitude is input as , where m is the mass per unit length and is the angular velocity). The load stiffness due to Coriolis loading is not accounted for in direct steady-state dynamics analysis. Gravity loading direction (magnitude is acceleration). in specified input as Force per unit length in global X- direction. Force per unit length in global Y- direction. Force per unit length in global Z-direction (only for beams in space). Nonuniform force per unit length in global X-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. Nonuniform force per unit length in global Y-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. Nonuniform force per unit length in global Z-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. (Only for beams in space.) Force per unit length in beam local (*DLOAD) P2 Abaqus/CAE Load/Interaction Line load P1NU Line load BEAM ELEMENT LIBRARY Units Description FL−1 FL−1 Force per unit length in beam local 2-direction. per unit force Nonuniform length in beam local 1-direction via with magnitude user in subroutine VDLOAD Abaqus/Standard in Abaqus/Explicit. (Only for beams in space.) supplied DLOAD and P2NU Line load FL−1 ROTA(S) Rotational body force T−2 ROTDYNF(S) Not supported T−1 per Nonuniform unit force length in beam local 2-direction supplied via with magnitude DLOAD user in subroutine and VDLOAD Abaqus/Standard in Abaqus/Explicit. Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Rotordynamic load (magnitude is input as is the angular velocity). , where The following load types are available only for PIPE elements: Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description HPI HPE PI PE Pipe pressure FL−2 Pipe pressure FL−2 Pipe pressure Pipe pressure FL−2 FL−2 Hydrostatic internal pressure (closed- end condition), varying linearly with the global Z-coordinate. Hydrostatic external pressure (closed- end condition), varying linearly with the global Z-coordinate. Uniform internal pressure (closed-end condition). Uniform external pressure (closed- end condition). Load ID (*DLOAD) PENU Abaqus/CAE Load/Interaction Units Description Pipe pressure FL−2 Nonuniform (closed-end magnitude subroutine DLOAD. external condition) supplied via pressure with user PINU Pipe pressure FL−2 Nonuniform (closed-end magnitude subroutine DLOAD. internal condition) supplied via pressure with user Abaqus/Aqua loads Abaqus/Aqua loads are specified as described in “Abaqus/Aqua analysis,” Section 6.11.1. They are not available for open-section beams and do not apply to beams that are defined to have additional inertia due to immersion in fluid . Abaqus/CAE Load/Interaction Units Description Not supported FL−1 Transverse fluid drag load. Not supported Not supported Not supported Not supported Not supported Not supported Not supported Not supported Not supported FL−1 FL−1 FL−1 FL−1 29.3.8–6 Fluid drag force on the first end of the beam (node 1). Fluid drag force on the second end of the beam (node 2 or node 3). Tangential fluid drag load. Transverse fluid inertia load. Fluid inertia force on the first end of the beam (node 1). Fluid inertia force on the second end of the beam (node 2 or node 3). Buoyancy load (closed-end condition). Transverse wind drag load. Wind drag force on the first end of the beam (node 1). Load ID (*CLOAD/ *DLOAD) FDD(A) FD1(A) FD2(A) FDT(A) FI(A) FI1(A) FI2(A) PB(A) WDD(A) Load ID (*CLOAD/ *DLOAD) WD2(A) Foundations Abaqus/CAE Load/Interaction Units Description Not supported Wind drag force on the second end of the beam (node 2 or node 3). Foundations are available only in Abaqus/Standard and are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE Units Description FX(S) FY(S) FZ(S) F1(S) F2(S) Not supported Not supported Not supported Not supported Not supported FL−2 FL−2 FL−2 FL−2 FL−2 Stiffness per unit length in global X- direction. Stiffness per unit length in global Y- direction. Stiffness per unit length in global Z- direction (only for beams in space). Stiffness per unit length in beam local 1-direction (only for beams in space). Stiffness per unit length in beam local 2-direction. Surface-based loading Distributed loads Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description Force per unit length in beam local 2-direction. The distributed surface force is positive in the direction opposite to the surface normal. per unit force Nonuniform length in beam local 2-direction via with magnitude in subroutine user supplied DLOAD Pressure FL−1 PNU Pressure FL−1 Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description and VDLOAD Abaqus/Standard in Abaqus/Explicit. The distributed surface force is positive in the direction opposite to the surface normal. Incident wave loading Incident wave loading is also available for these elements, with some restrictions. See “Acoustic and shock loads,” Section 33.4.6. Element output See “Beam cross-section library,” Section 29.3.9, for a description of the beam element output locations. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors, except for meshed sections, have the same components. For example, the stress components are as follows: S11 S22 S33 S12 Axial stress. Hoop stress (available only for pipe elements). Radial stress (available only for thick-walled pipe elements). Shear stress caused by torsion (available only for beam-type elements in space). This component is not available when thin-walled, open sections are employed (I-section, L-section, and arbitrary open section). Stress and strain for section points for meshed sections S11 S12 S13 Axial stress. Shear stress along the second cross-section axis caused by shear force and, for beam elements in space, torsion. Shear stress along the first cross-section axis caused by shear force and torsion (available only for beams in space). Section forces, moments, and transverse shear forces SF1 SF2 SF3 Axial force. Transverse shear force in the local 2-direction (not available for B23, B23H, B33, B33H). Transverse shear force in the local 1-direction (available only for beams in space, not available for B33, B33H). SM1 SM2 SM3 BIMOM ESF1 Bending moment about the local 1-axis. Bending moment about the local 2-axis (available only for beams in space). Twisting moment about the beam axis (available only for beams in space). Bimoment due to warping (available only for open-section beams in space). Effective axial force for beams subjected to pressure loading (available for all Abaqus/Standard stress/displacement analysis types except response spectrum and random response). See “Beam element formulation,” Section 3.5.2 of the Abaqus Theory Manual, for the definitions of the section forces and moments. The effective axial section force for beams subjected to pressure loading is defined as and are the external and the internal pressures, respectively, and where are the external and the internal pipe areas as defined in the load definition. The pressure loadings (with a closed- end condition) that are relevant to the effective axial force are external/internal pressure (load types PE, PI, PENU, and PINU); external/internal hydrostatic pressure (load types HPE and HPI); and, in an Abaqus/Aqua environment, buoyancy pressure, PB, which includes dynamic pressure if waves are present. and For beams that are not subjected to pressure loading, the effective axial force ESF1 is equal to the usual axial force SF1. Section strains, curvatures, and transverse shear strains SE1 SE2 SE3 SK1 SK2 SK3 Axial strain. Transverse shear strain in the local 2-direction (not available for B23, B23H, B33, and B33H). Transverse shear strain in the local 1-direction (available only for beams in space, not available for B33 and B33H). Curvature change about the local 1-axis. Curvature change about the local 2-axis (available only for beams in space). Twist of the beam (available only for beams in space). BICURV Bicurvature due to warping (available only for open-section beams in space). Node ordering on elements 2 - node element 3 - node element For beams in space an additional node may be given after a beam element’s connectivity (in the element definition—see “Element definition,” Section 2.2.1) to define the approximate direction of the first cross- section axis, . See “Beam element cross-section orientation,” Section 29.3.4, for details. Numbering of integration points for output 2 - node element 3 - node quadratic element 2 - node cubic element 29.3.9 BEAM CROSS-SECTION LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Beam modeling: overview,” Section 29.3.1 • “Choosing a beam cross-section,” Section 29.3.2 • “Frame elements,” Section 29.4.1 • “Defining profiles,” Section 12.2.2 of the Abaqus/CAE User’s Manual Overview This section describes the standard beam sections that are available in Abaqus/Standard and Abaqus/Explicit for use with beam elements. A subset of the standard beam sections are available for use with frame elements in Abaqus/Standard. General (nonstandard) beam cross-sections can be defined as described in “Choosing a beam cross-section,” Section 29.3.2. Arbitrary, thin-walled, open and closed sections t AB t BC t CD Example of arbitrary section The arbitrary section type is provided to permit modeling of simple, arbitrary, thin-walled, open and closed sections. You specify the section by defining a series of points in the thin-walled cross-section of the beam; these points are then linked by straight line segments, each of which is integrated numerically along the axis of the section so that the section can be used together with nonlinear material behavior. An independent thickness is associated with each of the segments making up the arbitrary section. Warping effects are included when an arbitrary section is used with open-section beam elements (available only in Abaqus/Standard). Input File Usage: Use either of the following options: *BEAM SECTION, SECTION=ARBITRARY *BEAM GENERAL SECTION, SECTION=ARBITRARY Property module: Create Profile: Arbitrary Abaqus/CAE Usage: Restrictions • An arbitrary section can be used only with beams in space (three-dimensional models). • An arbitrary section should not be used to define closed sections with branches, multiply connected closed sections, or open sections with disconnected regions. • For each individual segment of an arbitrary section there is no bending stiffness about the line joining the end points of the segment. Thus, an arbitrary section cannot be made up of only one segment. Geometric input data First, give the number of segments, the local coordinates of points A and B, and the thickness of the segment connecting these two vertices. Then, proceed by giving the local coordinates of point C and the thickness of the segment between points B and C, followed by the local coordinates of point D and the thickness of the segment between points C and D, and so on. An arbitrary section can contain as many segments as needed. All coordinates of section definition points are given in the local 1–2 axis system of the section. The origin of the local 1–2 axis system is the beam node, and the position of this node used to define the section is arbitrary: it does not have to be the centroid. Defining a closed section A closed section is defined by making the starting and end points coincident. Only single-cell closed sections can be modeled accurately. Closed sections with fins (single branches attached to the cell) cannot be modeled with the capability in Abaqus. Defining an arbitrary section with discontinuous branches If the arbitrary section contains discontinuous sections (branches), a section with zero thickness should be used to return from the ending point of the branch to the starting point of the subsequent section. This zero thickness section should always coincide with a nonzero thickness section. For an example of an I-section defined using this method, see “Buckling analysis of beams,” Section 1.2.1 of the Abaqus Benchmarks Manual. Default integration A three-point Simpson integration scheme is used for each segment making up the section. For more detailed integration, specify several segments along each straight portion of the section. Default stress output points if a beam section integrated during the analysis is used The vertices of the section. Temperature and field variable input at specific points through beam sections integrated during the analysis Give the value at each vertex of the section (points A, B, C, D in the figure). Box section Input File Usage: Use one of the following options: *BEAM SECTION, SECTION=BOX *BEAM GENERAL SECTION, SECTION=BOX *FRAME SECTION, SECTION=BOX Property module: Create Profile: Box Abaqus/CAE Usage: t 2 t 4 t 3 14 15 t 1 16 Default integration, beam in space t 2 t 4 t 3 t 1 10 11 12 13 Default integration, beam in a plane Geometric input data a, b, , , , Default integration (Simpson) Beam in a plane: 5 points Beam in space: 5 points in each wall (16 total) Nondefault integration input for a beam section integrated during the analysis Beam in a plane: Give the number of points in each wall that is parallel to the 2-axis. This number must be odd and greater than or equal to three. Beam in space: Give the number of points in each wall that is parallel to the 2-axis, then the number of points in each wall that is parallel to the 1-axis. Both numbers must be odd and greater than or equal to three. Default stress output points if a beam section integrated during the analysis is used Beam in a plane: Bottom and top (points 1 and 5 above for default integration). Beam in space: 4 corners (points 1, 5, 9, and 13 above for default integration). Temperature and field variable input at specific points for beam sections integrated during the analysis Give the value at each of the points shown below. Beam in a plane Beam in space Temperature input for a frame section Constant temperature throughout the element cross-section is assumed; therefore, only one temperature value per node is required. Circular section Input File Usage: Use one of the following options: *BEAM SECTION, SECTION=CIRC *BEAM GENERAL SECTION, SECTION=CIRC *FRAME SECTION, SECTION=CIRC Property module: Create Profile: Circular Abaqus/CAE Usage: 11 10 8 9 15 13 12 14 16 17 Default integration, beam in a plane Default integration, beam in space Geometric input data Radius Default integration Beam in a plane: 5 points Beam in space: 3 points radially, 8 circumferentially (17 total; trapezoidal rule). Integration point 1 is situated at the center of the beam and is used for output purposes only. It makes no contribution to the stiffness of the element; therefore, the integration point volume (IVOL) associated with this point is zero. Nondefault integration input for a beam section integrated during the analysis Beam in a plane: A maximum of 9 points are permitted. Beam in space: Give an odd number of points in the radial direction, then an even number of points in the circumferential direction. Default stress output points if a beam section integrated during the analysis is used Beam in a plane: Bottom and top (points 1 and 5 above for default integration). Beam in space: On the intersection of the surface with the 1- and 2-axes (points 3, 7, 11, and 15 above for default integration). Temperature and field variable input at specific points for beam sections integrated during the analysis Give the value at each of the points shown below. Beam in a plane Beam in space Temperature input for a frame section Constant temperature throughout the element cross-section is assumed; therefore, only one temperature value per node is required. Hexagonal section Input File Usage: Abaqus/CAE Usage: Use either of the following options: *BEAM SECTION, SECTION=HEX *BEAM GENERAL SECTION, SECTION=HEX Property module: Create Profile: Hexagonal 12 10 11 Default integration, beam in a plane Default integration, beam in space Geometric input data d (circumscribing radius), t (wall thickness) Default integration (Simpson) Beam in a plane: 5 points Beam in space: 3 points in each wall segment (12 total) Nondefault integration input for a beam section integrated during the analysis Beam in a plane: Give the number of points along the section wall, moving in the second beam section axis direction. This number must be odd and greater than or equal to three. Beam in space: Give the number of points in each wall segment. This number must be odd and greater than or equal to three. Default stress output points if a beam section integrated during the analysis is used Beam in a plane: Bottom and top (points 1 and 5 above for default integration). Beam in space: Vertices (points 1, 3, 5, 7, 9, and 11 above for default integration). Temperature and field variable input at specific points for beam sections integrated during the analysis Give the value at each of the points shown below. Beam in a plane Beam in space I-section Input File Usage: Use one of the following options: *BEAM SECTION, SECTION=I *BEAM GENERAL SECTION, SECTION=I *FRAME SECTION, SECTION=I Property module: Create Profile: I Abaqus/CAE Usage: t 3 t 2 t 1 b 1 Default integration, beam in a plane Geometric input data l, h, , , , , 10 11 12 13 t 2 t 1 t 3 b1 Default integration, beam in space By allowing you to specify l, the origin of the local cross-section axis can be placed anywhere on the symmetry line (the local 2-axis). In the above figures a negative value of l implies that the origin of the local cross-section axis is below the lower edge of the bottom flange, which may be needed when constraining a beam stiffener to a shell. Defining a T-section Input File Usage: Set and or and to zero to model a T-section. Abaqus/CAE Usage: Property module: Create Profile: T Default integration (Simpson) Beam in a plane: 5 points (one in each flange plus 3 in web) Beam in space: 5 points in web, 5 in each flange (13 total) Nondefault integration input for a beam section integrated during the analysis Beam in a plane: Give the number of points in the second beam section axis direction. This number must be odd and greater than or equal to three. Beam in space: Give the number of points in the lower flange first, then in the web, and then in the upper flange. These numbers must be odd and greater than or equal to three in each nonvanishing section. Default stress output points if a beam section integrated during the analysis is used Beam in a plane: Flanges (points 1 and 5 above for default integration). Beam in space: Ends of flanges (points 1, 5, 9, and 13 above for default integration). Temperature and field variable input at specific points for beam sections integrated during the analysis Give the value at each of the points shown below. Beam in a plane Beam in space For a beam in space the temperature is first interpolated linearly through the flanges based on the temperature at points 1 and 2, and then 4 and 5, respectively. It is then interpolated parabolically through the web. Temperature input for a frame section Constant temperature throughout the element cross-section is assumed; therefore, only one temperature value per node is required. L-section Input File Usage: Use either of the following options: Abaqus/CAE Usage: *BEAM SECTION, SECTION=L *BEAM GENERAL SECTION, SECTION=L Property module: Create Profile: L t 2 t 2 t 1 t 1 Default integration, beam in a plane Default integration, beam in space Geometric input data a, b, , Default integration (Simpson) Beam in a plane: 5 points Beam in space: 5 points in each flange (9 total) Nondefault integration input for a beam section integrated during the analysis Beam in a plane: Give the number of points in the second beam section axis direction. This number must be odd and greater than or equal to three. Beam in space: Give the number of points in the first beam section axis direction, then the number of points in the second beam section axis direction. These numbers must be odd and greater than or equal to three. Default stress output points if a beam section integrated during the analysis is used Beam in a plane: Bottom and top (points 1 and 5 above for default integration). Beam in space: End of flange along positive local 1-axis; section corner; end of flange along positive local 2-axis (points 1, 5, and 9 above for default integration). Temperature and field variable input at specific points for beam sections integrated during the analysis Give the value at each of the points shown below. Beam in a plane Beam in space Pipe section (thin-walled) Pipe cross-sections can be associated with beam, pipe, or frame elements. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *BEAM SECTION, SECTION=PIPE *BEAM GENERAL SECTION, SECTION=PIPE *FRAME SECTION, SECTION=PIPE Property module: Create Profile: Pipe: Thin walled Default integration, beam in a plane Default integration, beam in space Geometric input data r (outside radius), t (wall thickness) Default integration Beam in a plane: 5 points (Simpson’s rule) Beam in space: 8 points (trapezoidal rule) Nondefault integration input for a beam section integrated during the analysis Beam in a plane: Give an odd number of points. This number must be greater than or equal to five. Beam in space: Give an even number of points. This number must be greater than or equal to eight. Default stress output points if a beam section integrated during the analysis is used Beam in a plane: Bottom and top (points 1 and 5 above for default integration). Beam in space: On the intersection of the surface with the 1- and 2-axes (points 1, 3, 5, and 7 above for default integration). Temperature and field variable input at specific points for beam sections integrated during the analysis Give the value at each of the points shown below. Beam in a plane Beam in space Temperature input for a frame section Constant temperature throughout the element cross-section is assumed; therefore, only one temperature value per node is required. Pipe section (thick-walled) Thick-walled pipe cross-sections can be associated with beam or pipe elements. Input File Usage: Use the following option: Abaqus/CAE Usage: *BEAM SECTION, SECTION=THICK PIPE Property module: Create Profile: Pipe: Thick walled 12 11 10 9 8 15 14 13 12 11 10 18 17 16 98 21 20 19 22 23 24 15 14 13 12 11 10 98 Default integration, beam in a plane Default integration, beam in space Geometric input data r (outside radius), t (wall thickness) Default integration Beam in a plane: 3 points radially (Simpson’s rule), 5 circumferentially (trapezoidal rule) Beam in space: 3 points radially (Simpson’s rule), 8 circumferentially (trapezoidal rule) Nondefault integration input for a beam section integrated during the analysis Beam in a plane: Give an odd number of points in the radial direction, then an odd number of points (greater than or equal to 5) in the circumferential direction. Beam in space: Give an odd number of points in the radial direction, then an even number of points (greater than or equal to 8) in the circumferential direction. Default stress output points if a beam section integrated during the analysis is used Beam in a plane: Bottom and top on the pipe midsurface (points 2 and 14 above for default integration). Beam in space: On the intersection of the pipe midsurface with the 1- and 2-axes (points 2, 8, 14, and 20 above for default integration). Temperature and field variable input at specific points for beam sections integrated during the analysis Give the value at each of the points shown below. Beam in a plane Beam in space Rectangular section Input File Usage: Abaqus/CAE Usage: Use one of the following options: *BEAM SECTION, SECTION=RECT *BEAM GENERAL SECTION, SECTION=RECT *FRAME SECTION, SECTION=RECT Property module: Create Profile: Rectangular 21 16 11 23 18 13 22 17 12 24 19 14 25 20 15 10 Default integration, beam in a plane Default integration, beam in space Geometric input data a, b Default integration (Simpson) Beam in a plane: 5 points Beam in space: 5 × 5 (25 total) Nondefault integration input for a beam section integrated during the analysis Beam in a plane: Give the number of points in the second beam section axis direction. This number must be odd and greater than or equal to five. Beam in space: Give the number of points in the first beam section axis direction, then the number of points in the second beam section axis direction. These numbers must be odd and greater than or equal to five. Default stress output points if a beam section integrated during the analysis is used Beam in a plane: Bottom and top (points 1 and 5 above for default integration). Beam in space: Corners (points 1, 5, 21, and 25 above for default integration). Temperature and field variable input at specific points for beam sections integrated during the analysis Give the value at each of the points shown below. Beam in a plane Beam in space Temperature input for a frame section Constant temperature throughout the element cross-section is assumed; therefore, only one temperature value per node is required. Trapezoidal section Input File Usage: Use either of the following options: Abaqus/CAE Usage: *BEAM SECTION, SECTION=TRAPEZOID *BEAM GENERAL SECTION, SECTION=TRAPEZOID Property module: Create Profile: Trapezoidal 21 22 16 17 11 12 23 18 13 24 25 19 20 14 15 10 Default integration, beam in a plane Default integration, beam in space Geometric input data a, b, c, d By allowing you to specify d, the origin of the local cross-section axes can be placed anywhere on the symmetry line (the local 2-axis). In the above figures a negative value of d implies that the origin of the local cross-section axis is below the lower edge of the section. This may be needed when constraining a beam stiffener to a shell. Default integration (Simpson) Beam in a plane: 5 points Beam in space: 5 × 5 (25 total) Nondefault integration input for a beam section integrated during the analysis Beam in a plane: Give the number of points in the second beam section axis direction. This number must be odd and greater than or equal to five. Beam in space: Give the number of points in the first beam section axis direction, then the number of points in the second beam section axis direction. These numbers must be odd and greater than or equal to five. Default stress output points if a beam section integrated during the analysis is used Beam in a plane: Bottom and top (points 1 and 5 above for default integration). Beam in space: Corners (points 1, 5, 21, and 25 above for default integration). Temperature and field variable input at specific points for beam sections integrated during the analysis Give the value at each of the points shown below. b/2 b/2 Beam in a plane Beam in space 29.4 Frame elements • “Frame elements,” Section 29.4.1 • “Frame section behavior,” Section 29.4.2 • “Frame element library,” Section 29.4.3 29.4.1 FRAME ELEMENTS Product: Abaqus/Standard References • “Beam modeling: overview,” Section 29.3.1 • “Frame section behavior,” Section 29.4.2 • “Frame element library,” Section 29.4.3 • *FRAME SECTION Overview Frame elements: • are 2-node, initially straight, slender beam elements intended for use in the elastic or elastic-plastic analysis of frame-like structures; • are available in two or three dimensions; • have elastic response that follows Euler-Bernoulli beam theory with fourth-order interpolation for the transverse displacements; • have plastic response that is concentrated at the element ends (plastic hinges) and is modeled with a lumped plasticity model that includes nonlinear kinematic hardening; • are implemented for small or large displacements (large rotations with small strains); • output forces and moments at the element ends and midpoint; • output elastic axial strain and curvatures at the element ends and midpoint and plastic displacements and rotations at the element ends only; • admit, optionally, a uniaxial “buckling strut” response where the axial response of the element is governed by a damaged elasticity model in compression and an isotropic hardening plasticity model in tension and where all transverse forces and moments are zero; • can switch to buckling strut response during the analysis (for pipe sections only); and • can be used in static, implicit dynamic, and eigenfrequency extraction analyses only. Typical applications Frame elements are designed to be used for small-strain elastic or elastic-plastic analysis of frame-like structures composed of slender, initially straight beams. Typically, a single frame element will represent the entire structural member connecting two joints. A frame element’s elastic response is governed by Euler-Bernoulli beam theory with fourth-order interpolations for the transverse displacement field; hence, the element’s kinematics include the exact (Euler-Bernoulli) solution to concentrated end forces and moments and constant distributed loads. The elements can be used to solve a wide variety of civil engineering design applications, such as truss structures, bridges, internal frame structures of buildings, off-shore platforms, and jackets, etc. A frame element’s plastic response is modeled with a lumped plasticity model at the element ends that simulates the formation of plastic hinges. The lumped plasticity model includes nonlinear kinematic hardening. The elements can, thus, be used for collapse load prediction based on the formation of plastic hinges. Slender, frame-like members loaded in compression often buckle in such a way that only axial force is supported by the member; all other forces and moments are negligibly small. Frame elements offer optional buckling strut response whereby the element only carries axial force, which is calculated based on a damaged elasticity model in compression and an isotropic hardening plasticity model in tension. This model provides a simple phenomenological approximation to the highly nonlinear geometric and material response that takes place during buckling and postbuckling deformation of slender members loaded in compression. For pipe sections only, frame elements allow switching to optional uniaxial buckling strut response during the analysis. The criterion for switching is the “ISO” equation together with the “strength” equation . When the ISO and strength equations are satisfied, the elastic or elastic-plastic frame element undergoes a one-time-only switch in behavior to buckling strut response. Element cross-sectional axis system , ) axis system, where The orientation of the frame element’s cross-section is defined in Abaqus/Standard in terms of a local, right-handed ( , is the tangent to the axis of the element, positive in the direction from the first to the second node of the element, and are basis vectors that define the local 1- and 2-directions of the cross-section. is referred to as the normal to the element. Since these elements are initially straight and assume small strains, the cross-section directions are constant along each element and possibly discontinuous between elements. is referred to as the first axis direction, and and Defining the n1 -direction at the nodes For frame elements in a plane the -direction is always (0.0, 0.0, −1.0); that is, normal to the plane in which the motion occurs. Therefore, planar frame elements can bend only about the first axis direction. must be defined directly as part of the element section definition or by specifying an additional node off the element’s axis. This additional node is included in the element’s connectivity list . For frame elements in space the approximate direction of • If an additional node is specified, the approximate direction of from the first node of the element to the additional node. is defined by the vector extending • If both input methods are used, the direction calculated by using the additional node will take precedence. • If the approximate direction is not defined by either of the above methods, the default value is (0.0, 0.0, −1.0). -direction is then the normal to the element’s axis that lies in the plane defined by the element’s The axis and this approximate -direction. The -direction is defined as . Large-displacement assumptions The frame element’s formulation includes the effect of large rigid body motions (displacements and rotations) when geometrically nonlinear analysis is selected . Strains in these elements are assumed to remain small. Material response (section properties) of frame elements For frame elements the geometric and material properties are specified together as part of the frame section definition. No separate material definition is required. You can choose one of the section shapes that is valid for frame elements from the beam cross-section library . The valid section shapes depend upon whether elastic or elastic-plastic material response is specified or whether buckling strut response is included. See “Frame section behavior,” Section 29.4.2, for a complete discussion of specifying the geometric and material section properties. Input File Usage: *FRAME SECTION, SECTION=section_type Mechanical response and mass formulation The mechanical response of a frame element includes elastic and plastic behavior. Optionally, uniaxial buckling strut response is available. Elastic response The elastic response of a frame element is governed by Euler-Bernoulli beam theory. The displacement interpolations for the deflections transverse to the frame element’s axis (the local 1- and 2-directions in three dimensions; the local 2-direction in two dimensions) are fourth-order polynomials, allowing quadratic variation of the curvature along the element’s axis. Thus, each single frame element exactly models the static, elastic solution to force and moment loading at its ends and constant distributed loading along its axis (such as gravity loading). The displacement interpolation along an element’s axis is a second-order polynomial, allowing linear variation of the axial strain. In three dimensions the twist rotation interpolation along an element’s axis is linear, allowing constant twist strain. The elastic stiffness matrix is integrated numerically and used to calculate 15 nodal forces and moments in three dimensions: an axial force, two shear forces, two bending moments, and a twist moment at each end node, and an axial force and two shear forces at the midpoint node. In two dimensions 8 nodal forces and moments exist: an axial force, a shear force, and a moment at each end, and an axial force and a shear force at the midpoint. The forces and moments are illustrated in Figure 29.4.1–1. Elastic-plastic response The plastic response of the element is treated with a “lumped” plasticity model such that plastic deformations can develop only at the element’s ends through plastic rotations (hinges) and plastic axial displacement. The growth of the plastic zone through the element’s cross-section from initial yield to a fully yielded plastic hinge is modeled with nonlinear kinematic hardening. It is assumed that the plastic deformation at an end node is influenced by the moments and axial force at that node only. Hence, the N2 N1 N2 N1 N2 N1 n2 n1 M1 M2 M1 M2 Figure 29.4.1–1 Forces and moments on a frame element in space. yield function at each node, also called the plastic interaction surface, is assumed to be a function of that node’s axial force and three moment components only. No length is associated with the plastic hinge. In reality, the plastic hinge will have a finite size determined by the element’s length and the specific loading that causes yielding; the hinge size will influence the hardening rate but not the ultimate load. Hence, if the rate of hardening and, thus, the plastic deformation for a given load are important, the lumped plasticity model should be calibrated with the element’s length and the loading situation taken into account. For details on the elastic-plastic element formulation, see “Frame elements with lumped plasticity,” Section 3.9.2 of the Abaqus Theory Manual. Uniaxial linear elastic and buckling strut response with tensile yield You can obtain a frame element’s response to uniaxial force only, based on linear elasticity, buckling strut response, and tensile yield. In that case all transverse forces and moments in the element are zero. For linear elastic response the element behaves like an axial spring with constant stiffness. For buckling strut response if the tensile axial force in the element does not exceed the yield force, the axial force in the element is constrained to remain inside a buckling envelope. See “Frame section behavior,” Section 29.4.2, for a description of this envelope. Inside the envelope the force is related to strain by a damaged elastic modulus. The cyclic, hysteretic response of this model is phenomenological and approximates the response of thin-walled, pipe-like members. When the element is loaded in tension beyond the yield force, the force response is governed by isotropic hardening plasticity. In reverse loading the response is governed by the buckling envelope translated along the strain axis by an amount equal to the axial plastic strain. For details of the buckling strut formulation, see “Buckling strut response for frame elements,” Section 3.9.3 of the Abaqus Theory Manual. Mass formulation The frame element uses a lumped mass formulation for both dynamic analysis and gravity loading. The mass matrix for the translational degrees of freedom is derived from a quadratic interpolation of the axial and transverse displacement components. The rotary inertia for the element is isotropic and concentrated at the two ends. For buckling strut response a lumped mass scheme is used, where the element’s mass is concentrated at the two ends; no rotary inertia is included. Using frame elements in contact problems When contact conditions play a role in a structure’s behavior, frame elements have to be used with caution. A frame element has one additional internal node, located in the middle of the element. No contact constraint is imposed on this node, so this internal node may penetrate the surface in contact, resulting in a sagging effect. Output The forces and moments, elastic strains, and plastic displacements and rotations in a frame element are reported relative to a corotational coordinate system. The local coordinate directions are the axial direction and the two cross-sectional directions. Output of section forces and moments as well as elastic strains and curvatures is available at the element ends and midpoint. Output of plastic displacement and rotations is available only at the element ends. You can request output to the output database (at the integration points only), to the data file, or to the results file . Since frame elements are formulated in terms of section properties, stress output is not available. 29.4.2 FRAME SECTION BEHAVIOR Product: Abaqus/Standard References • “Frame elements,” Section 29.4.1 • *FRAME SECTION Overview The frame section behavior: • requires definition of the section’s shape and its material response; • uses linear elastic behavior in the interior of the frame element; • can include “lumped” plasticity at the element ends to model the formation of plastic hinges; • can be uniaxial only, with response governed by a phenomenological buckling strut model, together with linear elasticity and tensile plastic yielding; and • for pipe sections only, can switch to buckling strut response during the analysis. Defining elastic section behavior The elastic response of the frame elements is formulated in terms of Young’s modulus, E; the torsional shear modulus, G; coefficient of thermal expansion, ; and cross-section shape. Geometric properties such as the cross-sectional area, A, or bending moments of inertia are constant along the element and during the analysis. If present, thermal strains are constant over the cross-section, which is equivalent to assuming that the temperature does not vary in the cross-section. As a result of this assumption only the axial force, N, depends on the thermal strain where defines the total axial strain, including any initial elastic strain caused by a user-defined nonzero initial axial force, and defines the thermal expansion strain given by where is the thermal expansion coefficient, is the current temperature at the section, is the reference temperature for , is the user-defined initial temperature at this point (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1), are field variables, and are the user-defined initial values of field variables at this point (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). The bending moment and twist torque responses are defined by the constitutive relations where is the moment of inertia for bending about the 1-axis of the section, is the moment of inertia for bending about the 2-axis of the section, is the moment of inertia for cross-bending, is the torsional constant, is the curvature change about the first beam section local axis, including any elastic curvature change associated with a user-defined nonzero initial moment (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1), is the curvature change about the second beam section local axis, including any elastic curvature change associated with a user-defined nonzero initial moment (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1), and is the twist, including any elastic twist associated with a user-defined nonzero initial twisting moment (torque) T (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). Defining temperature and field-variable-dependent section properties The temperature and predefined field variables may vary linearly over the element’s length. Material constants such as Young’s modulus, , and the coefficient of thermal expansion, . You must associate the section definition with an element set. , can also depend on the temperature, , the torsional shear modulus, , and field variables Input File Usage: *FRAME SECTION, ELSET=name Specifying a standard library section and allowing Abaqus/Standard to calculate the cross-section’s parameters Select one of the following section profiles from the standard library of cross-sections : box, circular, I, pipe, or rectangular. Specify the geometric input data needed to define the shape of the cross-section. Abaqus/Standard will then calculate the geometric quantities needed to define the section behavior automatically. Input File Usage: *FRAME SECTION, SECTION=library_section, ELSET=name Specifying the geometric quantities directly Specify a general cross-section to define the area of the cross-section, moments of inertia, and torsional constant directly. These data are sufficient for defining the elastic section behavior since the axial stretching, bending response, and torsional behavior are assumed to be uncoupled. Input File Usage: *FRAME SECTION, SECTION=GENERAL, ELSET=name Specifying the elastic behavior Specify the elastic modulus, the torsional shear modulus, and the coefficient of thermal expansion as functions of temperature and field variables. Input File Usage: *FRAME SECTION, SECTION=section_type, ELSET=name first_data_line second_data_line elastic_modulus, torsional_shear_modulus, coefficient_of_thermal_expansion, temperature, fv_1, fv_2, etc. Defining elastic-plastic section behavior , , , and T directly as functions of their conjugate To include elastic-plastic response, specify N, plastic deformation variables or use the default plastic response for N, , and T based on the material yield stress. Abaqus/Standard uses the specified or default values to define a nonlinear kinematic hardening model that is “lumped” into plastic hinges at the element ends. Since the plasticity is lumped at the element ends, no length dimension is associated with the hinge. Generalized forces are related to generalized plastic displacements, not strains. In reality, the plastic hinge will have a finite size determined by the structural member’s length and the loading, which will affect the hardening rate but not the ultimate load. For example, yielding under pure bending (a constant moment over the member) will produce a hinge length equal to the member length, whereas yielding of a cantilever with transverse tip load (a linearly varying moment over the member) will produce a much more localized hinge. Hence, if the rate of hardening and, thus, the plastic deformation at a given load are of importance, you should calibrate the plastic response appropriately for different lengths and different loading situations. In the plastic range the only plastic surface available is an ellipsoid. This yield surface is only reasonably accurate for the pipe cross-section. Box, circular, I, and rectangular cross-sections can be used at your discretion with the understanding that the elliptic yield surface may not approximate the elastic-plastic response accurately. The general cross-section type cannot be used with plasticity. Defining N, M1 , M2 , and T directly , You can define N, , and T directly. Abaqus/Standard will fit an exponential curve to the user-supplied data as discussed below (see “Elastic-plastic data curve fit and calculation of default values” below). The plastic data describe the response to axial force, moment about the cross-sectional 1- and 2-directions, and torque. You must specify pairs of data relating the generalized force component to the appropriate plastic variable. Since the plasticity is concentrated at the element ends, the overall plastic response is dependent on the length of the element; hence, members with different lengths might require different hardening data. The plasticity model for frame elements is intended for frame-like structures: each member between structural joints is modeled with a single frame element where plastic hinges are allowed to develop at the end connections. At least three data pairs for each plastic variable are required to describe the elastic-plastic section hardening behavior. If fewer than three data pairs are given, Abaqus/Standard will issue an error message. Input File Usage: Use the following options: *FRAME SECTION, SECTION=PIPE, ELSET=name *PLASTIC AXIAL for N *PLASTIC M1 for *PLASTIC M2 for *PLASTIC TORQUE for T Allowing Abaqus/Standard to calculate default values for N, M1 , M2 , and T You can use the default elastic-plastic material response for the plastic variables based on the yield stress for the material. The default elastic-plastic material response differs for each of the plastic variables: the plastic axial force, first plastic bending moment, second plastic bending moment, and plastic torsional moment. Specific default values are given below. If you define the plastic variables directly and specify that the default response should be used, the data defined by you will take precedence over the default values. Input File Usage: Use the following options: *FRAME SECTION, SECTION=PIPE, ELSET=name, PLASTIC DEFAULTS, YIELD STRESS= plastic options if user-defined values are necessary for a particular generalized force Elastic-plastic data curve fit and calculation of default values The elastic-plastic response is a nonlinear kinematic hardening plasticity model. See “Models for metals subjected to cyclic loading,” Section 23.2.2, for a discussion of the nonlinear kinematic hardening formulation. Nonlinear kinematic hardening with N, M1 , M2 , and T defined directly For each of the four plastic material variables Abaqus/Standard uses an exponential curve fit of the user-supplied generalized force versus generalized plastic displacement to define the limits on the elastic range. The curve-fit procedure generates a hardening curve from the user-supplied data. It requires at least three data pairs. The nonlinear kinematic hardening model describes the translation of the yield surface in generalized force space through a generalized backstress, . The kinematic hardening is defined to be an additive combination of a purely kinematic linear hardening term and a relaxation (recall) term such that the backstress evolution is defined by sign where F is a component of generalized force, and C and based on the user-defined or default hardening data. C is the initial hardening modulus, and determines the rate at which the kinematic hardening modulus decreases with increasing backstress, are material parameters that are calibrated . The saturation value of ( ), called , is See Figure 29.4.2–1 for an illustration of the elastic range for the nonlinear kinematic hardening model. F0 F0 F = F0+ qpl Figure 29.4.2–1 Nonlinear kinematic hardening model: yield . surface for positive loading and the center of the yield surface, Allowing Abaqus/Standard to generate the default nonlinear kinematic hardening model To define the default plastic response, three data points are generated from the yield stress value and the cross-section shape. These three data points relate generalized force to generalized plastic displacement per unit length of the element. Since the model is calibrated per unit element length, the generated default plastic response is different for different element lengths. The generalized force levels for these , and , and three points are is the generalized force at zero plastic generalized displacement. are generalized force magnitudes that characterize the ultimate load-carrying capacity. The ) characterize the hardening slopes between the data points (i.e., the generalized plastic moduli response. See Figure 29.4.2–2 for an illustration of the default nonlinear kinematic hardening model. and . F2 F1 F0 D1 D2 qpl Figure 29.4.2–2 Data points generated for the default nonlinear kinematic hardening model. For the plastic axial force, is the axial force that causes initial yielding. For the plastic bending moments about the first and second axes, is the moment about the first and second cross-sectional directions, respectively, that produces first fiber yielding. For the plastic torsional moment, is the torque about the axis that produces first fiber yielding. The generalized force levels and , along with the connecting slopes , are chosen to approximate the response of a pipe cross-section made of a typical structural steel, with mild work hardening, from initial yielding to the development of a fully plastic hinge. The work hardening of the material corresponds to the default hardening of the section during axial loading. For different loading situations the size of the plastic hinge will vary; hence, the default model should be checked for validity against all anticipated loading situations. Default values for corresponding to each plastic variable are listed in Table 29.4.2–1. These default values are available for pipe, box, and I cross-section types with the values for the coefficients , and as shown in Table 29.4.2–2. , and and , , , Table 29.4.2–1 Default values for generalized forces and connecting slopes for corresponding plastic variables. Plastic axial force First plastic bending moment Second plastic bending moment Plastic torsional moment (for box and pipe sections) Plastic torsional moment (for I-sections) Table 29.4.2–2 Coefficients , , and . Cross-section type Pipe Box I (strong) I (weak) 0.30 0.17 0.10 0.43 0.07 0.02 0.02 0.10 1.35 1.20 1.12 1.50 Defining optional uniaxial strut behavior Frame elements optionally allow only uniaxial response (strut behavior). In this case neither end of the element supports moments or forces transverse to the axis; hence, only a force along the axis of the element exists. Furthermore, this axial force is constant along the length of the element, even if a distributed load is applied tangentially to the element axis. The uniaxial response of the element is linear elastic or nonlinear, in which case it includes buckling and postbuckling in compression and isotropic hardening plasticity in tension. Defining linear elastic uniaxial behavior , where A linear elastic uniaxial frame element behaves like an axial spring with constant stiffness E is Young’s modulus, A is the cross-sectional area, and L is the original element length. The strain measure is the change in length of the element divided by the element’s original length. Input File Usage: *FRAME SECTION, SECTION=library_section, ELSET=name, PINNED Defining buckling, postbuckling, and plastic uniaxial behavior: buckling strut response If uniaxial buckling and postbuckling in compression and isotropic hardening plasticity in tension are modeled (buckling strut response), the buckling envelope must be defined. The buckling envelope defines the force versus axial strain (change in length divided by the original length) response of the element. It is illustrated in Figure 29.4.2–3. force Py ζPy EA κPcr Pcr γEA strain βEA αEA Figure 29.4.2–3 Buckling envelope for uniaxial buckling response. The buckling envelope derives from Marshall Strut theory, which is developed for pipe cross-section profiles only. No other cross-section types are permitted with buckling strut response. Seven coefficients determine the buckling envelope as follows (the default values are listed, where D is the pipe outer diameter and t is the pipe wall thickness): ). is the yield stress. Elastic limit force ( Isotropic hardening slope ( Critical compressive buckling force predicted by the ISO equation, defined in “Buckling strut response for frame elements,” Section 3.9.3 of the Abaqus Theory Manual. Slope of a segment on the buckling envelope, and ). ( ). Corner on the buckling envelope ( ). Slope of a segment on the buckling envelope ( Corner on the buckling envelope ( ). ). The axial force in the element is required to stay inside or on the buckling envelope. When tension yielding occurs, the enclosed part of the envelope translates along the strain axis by an amount equal to the plastic strain. When reverse loading occurs for points on the boundary of the enclosed part of the envelope, the strut exhibits “damaged elastic” behavior. This damaged elastic response is determined by drawing a line from the point on the envelope to the tension yield point (force value ). As long as the force and axial strain remain inside the enclosed part of the envelope, the force response is linear elastic with a modulus equal to the damaged elastic modulus. At any time that the compressive strain is greater in magnitude than the negative extreme strain point of the envelope, the force is constant with a value of zero. The value of yield stress value. is a function of an element’s geometrical and material properties, including the Buckling strut response cannot be used with elastic-plastic frame section behavior; the strut’s plastic behavior is defined by and the isotropic hardening slope . Defining the buckling envelope You can specify that the default buckling envelope should be used, or you can define the buckling envelope. If you define the buckling envelope directly and specify that the default envelope should be used, the values defined by you will take precedence. In either case you must provide the yield stress value, which will be used to determine the yield force in tension and the critical compressive buckling load (through the ISO equation described later in this section). Input File Usage: To specify the default buckling envelope, use the following option: *FRAME SECTION, SECTION=PIPE, ELSET=name, BUCKLING, PINNED, YIELD STRESS= To specify a user-defined buckling envelope, use both of the following options: *FRAME SECTION, SECTION=PIPE, ELSET=name, PINNED, YIELD STRESS= *BUCKLING ENVELOPE Defining the critical buckling load The critical buckling load, , is determined by the ISO equation, which is an empirical relationship determined by the International Organization for Standardization based on experimental results for pipe- like or tubular structural members. Within the ISO equation, four variables can be changed from their default values: the effective length factors, , in the first and second sectional directions (the default values are 1.0) and the added length, , in the first and second sectional directions and (the default values are 0). These variables account for the buckling member’s end connectivity. The effective element length in the transverse direction i ( . For details on the ISO equation, see “Buckling strut response for frame elements,” Section 3.9.3 of the Abaqus Theory Manual. and ) is Input File Usage: To define nondefault coefficients for the ISO equation with the default buckling envelope, use both of the following options: *FRAME SECTION, SECTION=PIPE, ELSET=name, BUCKLING, PINNED, YIELD STRESS= *BUCKLING LENGTH To define nondefault coefficients for the ISO equation with a user-defined buckling envelope, use all of the following options: *FRAME SECTION, SECTION=PIPE, ELSET=name, PINNED, YIELD STRESS= *BUCKLING ENVELOPE *BUCKLING LENGTH Switching to optional uniaxial strut behavior during an analysis Frame elements allow switching to uniaxial buckling strut response during the analysis. The criterion for switching is the “ISO” equation together with the “strength” equation . When the ISO equation is satisfied, the elastic or elastic-plastic frame element undergoes a one-time-only switch in behavior to buckling strut response. The strength equation is introduced to prevent switching in the absence of significant axial forces. When the frame element switches to buckling strut response, a dramatic loss of structural stiffness If the global occurs. The switched element no longer supports bending, torsion, or shear loading. structure is unstable as a result of the switch (that is, the structure would collapse under the applied loading), the analysis may fail to converge. To permit switching of the element response, use the default buckling envelope or define a buckling envelope and provide a yield stress, but do not activate linear elastic uniaxial behavior for the frame element. The ISO equation is an empirical relationship based on experiments with slender, pipe-like (tubular) members. Since the equation is written explicitly in terms of the pipe outer diameter and thickness, only pipe sections are permitted with buckling strut response. The ISO equation incorporates several factors that you can define. Effective and added length factors account for element end fixity, and buckling reduction factors account for bending moment influence on buckling. You can define nondefault values for these factors in each local cross-section direction. Input File Usage: To allow switching to buckling strut response with default coefficients for the ISO equation and the default buckling envelope, use the following option: *FRAME SECTION, SECTION=PIPE, ELSET=name, BUCKLING, YIELD STRESS= To allow switching to buckling strut response with nondefault coefficients for the ISO equation and the default buckling envelope, use all of the following options: *FRAME SECTION, SECTION=PIPE, ELSET=name, BUCKLING, YIELD STRESS= *BUCKLING LENGTH *BUCKLING REDUCTION FACTORS To allow switching to buckling strut response with nondefault coefficients for the ISO equation and a user-defined buckling envelope, use all of the following options: *FRAME SECTION, SECTION=PIPE, ELSET=name, YIELD STRESS= *BUCKLING ENVELOPE *BUCKLING LENGTH *BUCKLING REDUCTION FACTORS Defining the reference temperature for thermal expansion You can define a thermal expansion coefficient for the frame section. The thermal expansion coefficient may be temperature dependent. In this case you must define the reference temperature for thermal expansion, . Input File Usage: Use both of the following options: *FRAME SECTION, ZERO= *THERMAL EXPANSION Specifying temperature and field variables Define temperatures and field variables by giving the value at the origin of the cross-section (i.e., only one temperature or field-variable value is given). Input File Usage: Use one or more of the following options: *TEMPERATURE *FIELD *INITIAL CONDITIONS, TYPE=TEMPERATURE *INITIAL CONDITIONS, TYPE=FIELD 29.4.3 FRAME ELEMENT LIBRARY Product: Abaqus/Standard References • “Frame elements,” Section 29.4.1 • *FRAME SECTION Overview This section provides a reference to the frame elements available in Abaqus/Standard. Element types Frame in a plane FRAME2D 2-node straight frame element Active degrees of freedom 1, 2, 6 Additional solution variables Two additional variables relating to the axial and lateral displacements. Frame in space FRAME3D 2-node straight frame element Active degrees of freedom 1, 2, 3, 4, 5, 6 Additional solution variables Three additional variables relating to the axial and lateral displacements. Nodal coordinates required Frame in a plane: X, Y (Direction cosines of the normal are not used; any values given are ignored.) Frame in space: X, Y, Z (Direction cosines of the normal are not used; any values given are ignored.) Element property definition Local orientations defined as described in “Orientations,” Section 2.2.5, cannot be used with frame elements to define local material directions. The orientation of the local section axes in space is discussed in “Frame elements,” Section 29.4.1. Input File Usage: *FRAME SECTION Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) GRAV PX PY PZ P1 P2 Units Description LT−2 FL−1 FL−1 FL−1 FL−1 FL−1 Gravity loading in a specified direction (magnitude is input as acceleration). Force per unit length in global X-direction. Force per unit length in global Y-direction. Force per unit length in global Z-direction (only for frames in space). Force per unit 1-direction (only for frames in space). length in frame local Force per unit 2-direction. length in frame local Abaqus/Aqua loads Abaqus/Aqua loads are specified as described in “Abaqus/Aqua analysis,” Section 6.11.1. Units Description FL−1 FL−1 FL−1 Transverse fluid drag load. Fluid drag force on the first end of the frame (node 1). Fluid drag force on the second end of the frame (node 2). Tangential fluid drag load. Transverse fluid inertia load. Fluid inertia force on the first end of the frame (node 1). Fluid inertia force on the second end of the frame (node 2). 29.4.3–2 Load ID (*CLOAD/ *DLOAD) FDD(A) FD1(A) FD2(A) FDT(A) FI(A) FI1(A) Load ID (*CLOAD/ *DLOAD) PB(A) WDD(A) WD1(A) WD2(A) Foundations Units Description FL−1 FL−1 Buoyancy load (closed-end condition). Transverse wind drag load. Wind drag force on the first end of the frame (node 1). Wind drag force on the second end of the frame (node 2). Foundations are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Units Description FX FY FZ F1 F2 FL−2 FL−2 FL−2 FL−2 FL−2 Stiffness per unit direction. Stiffness per unit direction. length in global X- length in global Y- Stiffness per unit direction (only for frames in space). length in global Z- Stiffness per unit length in frame local 1- direction (only for frames in space). Stiffness per unit 2-direction. length in frame local Element output All element output variables are given at the element ends (nodes 1 and 2) and midpoint (node 3). Section forces and moments SF1 SF2 SF3 SM1 SM2 SM3 Axial force. Transverse shear force in the local 2-direction. Transverse shear force in the local 1-direction (only available for frames in space). Bending moment about the local 1-axis. Bending moment about the local 2-axis (only available for frames in space). Twisting moment about the frame axis (only available for frames in space). See “Frame elements with lumped plasticity,” Section 3.9.2 of the Abaqus Theory Manual, for a discussion of the section forces and moments. Section elastic strains and curvatures SEE1 SKE1 SKE2 SKE3 Elastic axial strain. Elastic curvature change about the local 1-axis. Elastic curvature change about the local 2-axis (only available for frames in space). Elastic twist of the beam (only available for frames in space). Plastic displacements and rotations in the element coordinate system SEP1 SKP1 SKP2 SKP3 Plastic axial displacement. Plastic rotation about the local 1-axis. Plastic rotation about the local 2-axis (only available for frames in space). Plastic rotation about the beam axis (only available for frames in space). Section force and moment backstresses SALPHA1 SALPHA2 SALPHA3 SALPHA4 Axial force backstress. Bending moment backstress about the local 1-axis. Bending moment backstress about the local 2-axis (only available for frames in space). Twisting moment backstress about the beam axis (only available for frames in space). Node ordering on elements end 2 end 1 2 - node element For frames in space an additional node may be given after a frame element’s connectivity (in the element definition—see “Element definition,” Section 2.2.1) to define the approximate direction of the first cross- section axis, . See “Frame elements,” Section 29.4.1, for details. 29.5 Elbow elements • “Pipes and pipebends with deforming cross-sections: elbow elements,” Section 29.5.1 • “Elbow element library,” Section 29.5.2 PIPES AND PIPEBENDS WITH DEFORMING CROSS-SECTIONS: ELBOW ELEMENTS ELBOW ELEMENTS Product: Abaqus/Standard References • “Elbow element library,” Section 29.5.2 • *BEAM SECTION Overview Elbow elements: • are intended to provide accurate modeling of the nonlinear response of initially circular pipes and pipebends when distortion of the cross-section by ovalization and warping dominates the behavior; • appear as beams but are shells with quite complex deformation patterns allowed; • use plane stress theory to model the deformation through the pipe wall; and • cannot provide nodal values of stress, strain, and other constitutive results. Typical applications In the usual approach to linear analysis of elbows, the response prediction is based on semianalytical results, used as “flexibility factors” to correct results obtained with simple beam theory. Such factors do not apply in nonlinear cases, and the pipeline must be modeled as a shell to predict the response accurately (for example, see “Parametric study of a linear elastic pipeline under in-plane bending,” Section 1.1.3 of the Abaqus Example Problems Manual). Although the elbow elements appear as beams, they are, in fact, shells, with quite complex deformation patterns allowed. In thin-walled elbows the interaction of elbows and adjacent straight segments is an important aspect of elbow modeling, as are the large rotations that readily occur in the cross-sectional deformation, even at small relative rotations of the pipe axis itself. All of these effects (including the stiffening effect of internal pressure) can be modeled with these elements. Elbow elements are intended to provide accurate modeling of the nonlinear response of initially circular pipes and pipebends when distortion of the cross-section by ovalization and warping dominates the behavior. Such behavior arises in two circumstances: in pipebends, where the initial curvature of the pipe, together with the thinness of the wall of the pipe, causes ovalization to dominate the response, and in straight pipe sections, where excessive bending can lead to a buckling collapse of the thin-walled circular section (“Brazier buckling”). Because the elbow elements use a full shell formulation around the circumference, the number of degrees of freedom per element is high. Elbow elements that use all Fourier modes (discussed below) to model ovalization and warping are considerably more expensive computationally than beam elements, but their cost is comparable to that of coarse shell models, which can be used to model the section. If an analysis requires connecting pipe elements to a pipebend, it is easier to connect elbow elements to pipe elements than it is to connect shell elements to pipe elements. Choosing an appropriate element Elbow elements use polynomial interpolation along their length (linear or quadratic depending on the element type), together with Fourier interpolation around the pipe to model the ovalization and warping of the section. Shell theory is then used to model the behavior. Two types of elbow elements are provided. ELBOW31 and ELBOW32 Element types ELBOW31 and ELBOW32 are the most complete elbow elements. In these elements the ovalization of the pipe wall is made continuous from one element to the next, thus modeling such effects as the interaction between pipe bends (elbows) and adjacent straight segments of the pipeline. ELBOW31 and ELBOW32 should not be used for the analysis of unconnected straight pipes unless the warping and ovalization are restrained at some point in the pipe. ELBOW31B and ELBOW31C Element types ELBOW31B and ELBOW31C use a simplified version of the formulation, in which ovalization only is considered (no warping) and axial gradients of the ovalization are neglected. These approximations are often satisfactory, and indeed they form the basis of the standard flexibility factor approach used in linear analysis of piping systems. They provide a considerably less expensive capability. ELBOW31C includes the further approximation that the odd numbered terms in the Fourier interpolation around the pipe, except the first term, are neglected. This formulation provides a slightly less expensive model for cases where the radius of the pipe is small compared to the radius of curvature of the pipe axis. Defining the element’s section properties You use a beam section definition integrated during the analysis to define the section properties of elbow elements. Give the outside radius of the pipe, r; pipe wall thickness, t; and elbow torus radius, measured to the pipe axis, R. For a straight pipe, set R to zero. You must associate these properties with a set of elbow elements. Input File Usage: *BEAM SECTION, SECTION=ELBOW, ELSET=name r, t, R Defining the section orientation For all elbow elements the section must be oriented in space by specifying a point that, together with the nodes of the element, defines the plane of the -axis in Figure 29.5.1–1. For bent pipes this point should lie outside the bend (the side of the pipe on the outside of the bend is referred to as the extrados). For pipebends of less than 180° this point can be set to be the point of intersection of the tangents to the adjacent straight pipe runs. If a pipebend subtends an angle greater than or equal to 180°, the bend should be partitioned into sections of less than 180° and a separate beam section should be defined for each partition so that the point used to define the plane of the When the elements are used to model straight pipes, the point can be any point off the pipe axis. -axis can lie outside of the extrados. Second cross-sectional direction a = a x a a - positive from 1st to 2nd node torus radius Figure 29.5.1–1 Elbow element geometry. When ovalization modeling is extended onto straight runs adjacent to a pipebend by using ELBOW31 or ELBOW32 elements for the pipebend and for the straight pipe, you must ensure that the -axis is defined so that its orientation about the axis of the pipe is the same between the pipebend and each of the straight segments. When possible, the -axis should also be the same between adjacent pipebends. In some cases, such as adjacent pipebends in different planes, the -axes are necessarily discontinuous. In such cases separate nodes must be introduced at the point where the -axis changes orientation, and MPC type ELBOW must be invoked to impose the appropriate constraints to ensure continuity of displacements. See Figure 29.5.1–2. Use two coincident nodes with MPC type ELBOW to allow for change in direction of a2 a2 a2 x x xx a2 a2 a2 a2 a2 a2 Figure 29.5.1–2 Use of MPC type ELBOW with ELBOW31 or ELBOW32. Input File Usage: *BEAM SECTION, SECTION=ELBOW first data line coordinates of orientation point Defining the number of integration points and Fourier modes You can specify the number of integration points and Fourier modes for an elbow section. Experience suggests that for relatively thick-walled cases 4 Fourier modes with 12 integration points around the pipe are sufficient. For thin-walled elbows 6 Fourier modes and 18 integration points around the pipe are needed. As a general rule, the number of integration points around the pipe should not be less than three times the number of Fourier modes used; otherwise, singularities may arise in the stiffness matrix. When used with zero Fourier modes, the elements become simple pipe elements with hoop strain and stress included: when Poisson’s ratio is set to zero, they show similar behavior to the PIPE elements in Abaqus . Input File Usage: *BEAM SECTION, SECTION=ELBOW first data line second data line number of int. pts. through thickness, number of int. pts. around pipe, number of Fourier modes Assigning a material definition to a set of elbow elements You must associate a material definition with each elbow section definition. Input File Usage: *BEAM SECTION, SECTION=ELBOW, MATERIAL=name Specifying temperature and field variables Temperature and field variables can be specified by defining the values at specific points through the section or by defining the value at the middle of the pipe wall and specifying the gradient through the pipe thickness. By defining the values at points through the section You can define temperatures and field variables by giving the values at each of the three points shown below. outside inside 3 points through thickness No matter how many section points there are through the thickness of the elbow, specify the values at only these three points. These three values are applied to all integration points around the circumference so that the only admissible variation is in the radial direction. Input File Usage: *BEAM SECTION, SECTION=ELBOW, TEMPERATURE=VALUES By defining the value at the middle of the pipe wall and the gradient through the thickness Alternatively, you can define temperatures and field variables by giving the value on the middle surface of the pipe wall and the gradient of temperature with respect to position through the pipe wall thickness, positive when the outside surface is hotter than the inside surface. Input File Usage: *BEAM SECTION, SECTION=ELBOW, TEMPERATURE=GRADIENTS Using elbow elements in large-displacement analysis When elbow elements are subjected to pipe pressure loads (load types PI, PE, HPI, or HPE) in large- displacement analysis (“General and linear perturbation procedures,” Section 6.1.3), the most significant contributions to the load stiffness are taken into account. Defining kinematic boundary conditions on elbow elements Kinematic boundary conditions on the standard degrees of freedom at the nodes of elbow elements (that is, degrees of freedom 1–6) should be treated in the usual way. In addition, the elements have ovalization and warping terms stored internally. For ELBOW31B and ELBOW31C elements this requires no additional consideration. For ELBOW31 or ELBOW32 elements you may often need to provide kinematic boundary conditions on these additional degrees of freedom. For example, it is common to model a pipeline with ovalization and warping allowed in the elbows and adjacent straight pipe segments but no ovalization in the middle segments of long, straight pipe runs . (The latter is usually accomplished by specifying ELBOW31 elements with zero modes or PIPE31 elements so that the usual bending terms and the uniform radial expansion term, associated with pressure in the pipe, are included; if internal pressure is not important, a simple beam element, B31, can be used instead.) Where the segments with ovalization and warping end, the warping must be restrained; and if a stiff flange or vessel exists at that point, the ovalization should also be restrained. To do so, specify NOWARP and/or NOOVAL or NODEFORM boundary conditions for that node (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.3.1). NOWARP means that no warping is allowed at the node, but ovalization and uniform radial expansion are allowed; NOOVAL means that there can be no ovalization at the node, but warping and uniform radial expansion are allowed; NODEFORM means that there can be no cross-section deformation at all—no warping, ovalization, or uniform radial expansion. Typically, NOWARP will be specified at the end of a pipebend segment modeled with ELBOW31 adjacent to a straight pipe run, while NOWARP and NOOVAL would be specified at a stiff flange or vessel attachment point. NODEFORM restrains all cross-sectional deformation, including the uniform radial expansion term: this will result in large stresses if thermal expansion occurs. NODEFORM should be used, for example, at a built-in end. Visualizing the cross-section deformation The current release of Abaqus/Standard does not provide a direct way of visualizing the cross-section the utility routine felbow.f (“Creation of a data file to facilitate the ovalization. However, postprocessing of elbow element results: FELBOW,” Section 14.1.6 of the Abaqus Example Problems Manual) creates a data file that can be used in Abaqus/CAE to plot the current coordinates of the integration points around the circumference of the elbow section of interest. The routine uses output variable COORD (“Abaqus/Standard output variable identifiers,” Section 4.2.1) to obtain the current coordinates of the integration points. These values are available only if geometric nonlinearity is considered in the step. You will have to ensure that the variable COORD is written to the results (.fil) file for this purpose. The routine is suitable for elbow elements oriented arbitrarily in space: the integration points of the elbow section are projected appropriately to a coordinate system suitable for plotting the cross- section. The input data for plotting are written to a file that can be read into Abaqus/CAE. An X–Y plot of the elbow element’s deformed cross-section can be displayed using the XY Data Manager in the Visualization module. a. Typical pipeline b. Sections modeled with continuous ovalization Figure 29.5.1–3 Pipeline schematic. In addition to facilitating the visualization of the cross-section ovalization, the program also allows you to create data files to plot the variation of a variable along a line of elbow elements and around the circumference of a given elbow element. Similar C++ and Python utility routines, felbow.C (“A C++ version of FELBOW,” Section 10.15.6 of the Abaqus Scripting User’s Manual) and felbow.py (“An Abaqus Scripting Interface version of FELBOW,” Section 9.10.12 of the Abaqus Scripting User’s Manual), are provided to process the pertinent elbow element results output written to the output database (.odb) file. When these programs are executed, they write data to an ASCII format file and/or an output database file that can be used in Abaqus/CAE to plot the current coordinates of the integration points around the circumference of the elbow section. Both these routines can also be used to visualize the variation of an output variable around the circumference of the elbow section. 29.5.2 ELBOW ELEMENT LIBRARY Product: Abaqus/Standard References • “Pipes and pipebends with deforming cross-sections: elbow elements,” Section 29.5.1 • *BEAM SECTION Overview This section provides a reference to the elbow elements available in Abaqus/Standard. Element types ELBOW31 2-node pipe in space with deforming section, linear interpolation along the pipe ELBOW32 3-node pipe in space with deforming section, quadratic interpolation along the pipe ELBOW31B 2-node pipe in space with ovalization only, axial gradients of ovalization neglected ELBOW31C 2-node pipe in space with ovalization only, axial gradients of ovalization neglected. This formulation is the same as that for element type ELBOW31B, with the exception that all odd numbered terms in the Fourier interpolation around the pipe but the first term are neglected. Active degrees of freedom 1, 2, 3, 4, 5, 6 Additional solution variables Elbow elements have numerous variables to model cross-sectional ovalization and warping. The number of variables depends on the type of elbow element, the number of nodes, and the number of Fourier modes chosen. In the following table p is the number of Fourier modes: Element type Number of variables ELBOW31 ELBOW32 ELBOW31B 16, if p=0 (16p+8), if p 24, if p=0 (24p+12), if 13+2p, if p=0,1 11+4p, if Element type Number of variables ELBOW31C 13+2p, if p=0,1,3,5 15+2p, if p=2,4,6 Nodal coordinates required Element property definition Input File Usage: *BEAM SECTION, SECTION=ELBOW Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Units Description BX BY BZ BXNU BYNU BZNU FL−3 FL−3 FL−3 FL−3 FL−3 FL−3 CENT FL−4 (ML−3T−2) Body force per unit volume in global X- direction. Body force per unit volume in global Y- direction. Body force per unit volume in global Z- direction. Nonuniform body force in global X- direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in global Y- direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in global Z- direction with magnitude supplied via user subroutine DLOAD. , is the mass density per unit volume Centrifugal load (magnitude is input as where and is the angular velocity). Units Description T−2 LT−2 FL−2 FL−2 FL−2 FL−2 FL−2 FL−2 T−2 Centrifugal load (magnitude is input as where is the angular velocity). , Gravity loading in a specified direction (magnitude is input as acceleration). Hydrostatic external pressure, with linear variation in global Z (closed-end condition). Hydrostatic internal pressure, with linear variation in global Z (closed-end condition). Uniform external pressure condition). (closed-end Uniform internal pressure condition). (closed-end pressure with Nonuniform external magnitude supplied via user subroutine DLOAD (closed-end condition). Nonuniform internal with magnitude supplied via user subroutine DLOAD (closed-end condition). pressure Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Load ID (*DLOAD) CENTRIF GRAV HPE HPI PE PI PENU PINU ROTA Abaqus/Aqua loads Abaqus/Aqua loads are specified as described in “Abaqus/Aqua analysis,” Section 6.11.1. Units Description FL−1 FL−1 FL−1 Transverse fluid drag load. Fluid drag force on the first end of the elbow (node 1). Fluid drag force on the second end of the elbow (node 2 or node 3). Tangential fluid drag load. Transverse fluid inertia load. 29.5.2–3 Load ID (*CLOAD/ *DLOAD) FDD(A) FD1(A) FD2(A) FDT(A) Load ID (*CLOAD/ *DLOAD) FI1(A) FI2(A) PB(A) WDD(A) WD1(A) WD2(A) Element output Units Description FL−1 FL−1 Fluid inertia force on the first end of the elbow (node 1). Fluid inertia force on the second end of the elbow (node 2 or node 3). Buoyancy force (closed-end condition). Transverse wind drag load. Wind drag force on the first end of the elbow (node 1). Wind drag force on the second end of the elbow (node 2 or node 3). The default stress output points are on the inside surface and the outside surface at all integration stations around the pipe. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S12 Direct stress along the pipe. Direct stress around the pipe section. Shear stress in the pipe wall. Section forces and moments SF1 SM1 SM2 SM3 Axial force. Bending moment about the local 1-axis. Bending moment about the local 2-axis. Twisting moment about the elbow axis. Node ordering on elements 2-node element 3-node element Numbering of integration points for output 13 14 15 16 17 18 19 12 11 10 extrados 20 intrados outside inside x x x The extrados is the side of the pipebend that is furthest away from the center of the torus defining the pipebend; that is, the side of the pipebend to which the -axis points. The intrados is the side of the pipebend closest to the center of the torus. The middle surface integration points around a section are shown above. There is a default of five thickness direction integration points at each such point, with point 1 on the inside surface of the pipe and point 5 on the outside surface. For ELBOW31 and ELBOW31B only one integration station is used along the axis of the element. For ELBOW32 two integration stations are used along the axis of the elbow and the point numbers on the second section are a continuation of those on the first section (e.g., 21, 22, …, 40 in the default case), located around the pipe as shown above. 29.6 Shell elements • “Shell elements: overview,” Section 29.6.1 • “Choosing a shell element,” Section 29.6.2 • “Defining the initial geometry of conventional shell elements,” Section 29.6.3 • “Shell section behavior,” Section 29.6.4 • “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5 • “Using a general shell section to define the section behavior,” Section 29.6.6 • “Three-dimensional conventional shell element library,” Section 29.6.7 • “Continuum shell element library,” Section 29.6.8 • “Axisymmetric shell element library,” Section 29.6.9 • “Axisymmetric shell elements with nonlinear, asymmetric deformation,” Section 29.6.10 29.6.1 SHELL ELEMENTS: OVERVIEW Abaqus offers a wide variety of shell modeling options. Overview Shell modeling consists of: • choosing the appropriate shell element type (“Choosing a shell element,” Section 29.6.2); • defining the initial geometry of the surface (“Defining the initial geometry of conventional shell elements,” Section 29.6.3); • determining whether or not numerical integration is needed to define the shell section behavior (“Shell section behavior,” Section 29.6.4); and • defining the shell section behavior (“Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, or “Using a general shell section to define the section behavior,” Section 29.6.6). Conventional shell versus continuum shell Shell elements are used to model structures in which one dimension, the thickness, is significantly smaller than the other dimensions. Conventional shell elements use this condition to discretize a body by defining the geometry at a reference surface. In this case the thickness is defined through the section property definition. Conventional shell elements have displacement and rotational degrees of freedom. In contrast, continuum shell elements discretize an entire three-dimensional body. The thickness is determined from the element nodal geometry. Continuum shell elements have only displacement degrees of freedom. From a modeling point of view continuum shell elements look like three-dimensional continuum solids, but their kinematic and constitutive behavior is similar to conventional shell elements. Figure 29.6.1–1 illustrates the differences between a conventional shell and a continuum shell element. Conventions The conventions that are used for shell elements are defined below. Definition of local directions on the surface of a shell in space The default local directions used on the surface of a shell for definition of anisotropic material properties and for reporting stress and strain components are defined in “Conventions,” Section 1.2.2. You can define other directions by defining a local orientation , except for SAX1, SAX2, and SAX2T elements (“Axisymmetric shell element library,” Section 29.6.9), which do not support orientations. A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be assigned to shell elements. For SAXA elements structural body being modeled Conventional shell model - geometry is specified at the reference surface; thickness is defined by section property. displacement and rotation degrees of freedom Finite Element Model Element displacement degrees of freedom only Continuum shell model - full 3-D geometry is specified; element thickness is defined by nodal geometry. Figure 29.6.1–1 Conventional versus continuum shell element. (“Axisymmetric shell elements with nonlinear, asymmetric deformation,” Section 29.6.10) any anisotropic material definition must be symmetric with respect to the r–z plane at and . In large-deformation (geometrically nonlinear) analysis these local directions rotate with the average rotation of the surface at that point. They are output as directions in the current configuration except in the shell elements in Abaqus/Standard that provide only large rotation but small strain (element types STRI3, STRI65, S4R5, S8R, S8RT, S8R5, S9R5—see “Choosing a shell element,” Section 29.6.2), where they are output as directions in the reference configuration. Therefore, in geometrically nonlinear analysis, when displaying these directions or when displaying principal values of stress, strain, or section forces or moments in Abaqus/CAE, the current (deformed) configuration should be used except for the small-strain elements in Abaqus/Standard, for which the reference configuration should be used. Positive normal definition for conventional shell elements The “top” surface of a conventional shell element is the surface in the positive normal direction and is referred to as the positive (SPOS) face for contact definition. The “bottom” surface is in the negative direction along the normal and is referred to as the negative (SNEG) face for contact definition. Positive and negative are also used to designate top and bottom surfaces when specifying offsets of the reference surface from the shell’s midsurface. The positive normal direction defines the convention for pressure load application and output of quantities that vary through the thickness of the shell. A positive pressure load applied to a shell element produces a load that acts in the direction of the positive normal. Three-dimensional conventional shells For shells in space the positive normal is given by the right-hand rule going around the nodes of the element in the order that they are specified in the element definition. See Figure 29.6.1–2. face SPOS face SNEG Figure 29.6.1–2 Positive normals for three-dimensional conventional shells. Axisymmetric conventional shells For axisymmetric conventional shells (including the SAXA1n and SAXA2n elements that allow for nonsymmetric deformation) the positive normal direction is defined by a 90° counterclockwise rotation from the direction going from node 1 to node 2. See Figure 29.6.1–3. face SPOS face SNEG Figure 29.6.1–3 Positive normal for conventional axisymmetric shells. Normal definition for continuum shell elements Figure 29.6.1–4 illustrates the key geometrical features of continuum shells. It is important that the continuum shells are oriented properly, since the behavior in the thickness direction is different from that in the in-plane directions. By default, the element top and bottom faces and, hence, the element normal, stacking direction, and thickness direction are defined by the nodal connectivity. For the triangular in- plane continuum shell element (SC6R) the face with corner nodes 1, 2, and 3 is the bottom face; and the face with corner nodes 4, 5, and 6 is the top face. For the quadrilateral continuum shell element (SC8R) thickness direction top face bottom face thickness direction Figure 29.6.1–4 Default normals and thickness direction for continuum shell elements. the face with corner nodes 1, 2, 3, and 4 is the bottom face; and the face with corner nodes 5, 6, 7, and 8 is the top face. The stacking direction and thickness direction are both defined to be the direction from the bottom face to the top face. Additional options for defining the element thickness direction, including one option that is independent of nodal connectivity, are presented below. Surfaces on continuum shells can be defined by specifying the face identifiers S1–S6 identifying the individual faces as defined in “Continuum shell element library,” Section 29.6.8. Free surface generation can also be used. Pressure loads applied to faces P1–P6 are defined similar to continuum elements, with a positive pressure directed into the element. Defining the stacking and thickness direction By default, the continuum shell stacking direction and thickness direction are defined by the nodal connectivity as illustrated in Figure 29.6.1–4. Alternatively, you can define the element stacking direction and thickness direction by either selecting one of the element’s isoparametric directions or by using an orientation definition. Defining the stacking and thickness direction based on the element isoparametric direction You can define the element stacking direction to be along one of the element’s isoparametric directions . The 8-node hexahedron continuum shell has three possible stacking directions; the 6-node in-plane triangular continuum shell has only one stack direction, which is in the element 3-isoparametric direction. The default stacking direction is 3, providing the same thickness and stacking direction as outlined in the previous section. To obtain a desired thickness direction, the choice of the isoparametric direction depends on the element connectivity. For a mesh-independent specification, use an orientation-based method as described below. Input File Usage: Use one of the following options to define the element stacking direction based on the element’s isoparametric directions: F6 F2 F5 F4 F3 F1 Stack direction F2 F5 F3 F1 F4 Stack direction Stack direction = 1 from face 6 to face 4 Stack direction = 2 from face 3 to face 5 Stack direction = 3 from face 1 to face 2 Stack direction = 3 from face 1 to face 2 Figure 29.6.1–5 Stack directions for SC6R and SC8R elements. Abaqus/CAE Usage: *SHELL SECTION, STACK DIRECTION=n *SHELL GENERAL SECTION, STACK DIRECTION=n where n = 1, 2, or 3. Use the following option to define the stacking direction based on the element’s isoparametric directions if the continuum shell is defined using a composite layup: Property module: Create Composite Layup: select Continuum Shell as the Element Type: Stacking Direction: Element direction 1, Element direction 2, or Element direction 3 Use the following option to define the stacking direction based on the element’s isoparametric directions if the continuum shell is defined using a composite shell section: Assign→Material Orientation: select regions: Use Default Orientation or Other Method: Stacking Direction: Element isoparametric direction 1, Element isoparametric direction 2, or Element isoparametric direction 3 Defining the stacking and thickness direction based on an orientation definition Alternatively, you can define the element stacking direction based on a local orientation definition. For shell elements the orientation definition defines an axis about which the local 1 and 2 material directions may be rotated. This axis also defines an approximate normal direction. The element stacking and thickness directions are defined to be the element isoparametric direction that is closest to this approximate normal . “The pinched cylinder problem,” Section 2.3.2 of the Abaqus Benchmarks Manual, and “LE3: Hemispherical shell with point loads,” Section 4.2.3 of the Abaqus Benchmarks Manual, illustrate the use Cohesive section, stack direction based on cylor1 ' (10, 0, 0) Local cylindrical orientation cylor1: a = 0, 0, 0 b = 10, 0, 0 ' 2 Global (0, 0, 0) Abaqus selects the isoparametric direction  that is closest to the 1st (i.e., x , or radial) axis, at the center. Figure 29.6.1–6 Example illustrating the use of a cylindrical system to define the stacking direction. of a cylindrical and spherical orientation system, respectively, to define the stack and thickness direction independent of nodal connectivity. Input File Usage: Use one of the following options to define the element stacking direction based on a user-defined orientation: *SHELL SECTION, STACK DIRECTION=ORIENTATION, ORIENTATION=name *SHELL GENERAL SECTION, STACK DIRECTION=ORIENTATION, ORIENTATION=name Abaqus/CAE Usage: Use the following option to define the stacking direction based on a user-defined orientation if the continuum shell is defined using a composite layup: Property module: Create Composite Layup: select Continuum Shell as the Element Type: Stacking Direction: Layup orientation Use the following option to define the stacking direction based on a user-defined orientation if the continuum shell is defined using a composite shell section: Assign→Material Orientation: select regions: Use Default Orientation or Other Method: Stacking Direction: Normal direction of material orientation Verifying the element stack and thickness direction You can verify the element stack and thickness direction visually in Abaqus/CAE by either contouring the element section thickness or plotting the material axis. Generally, the in-plane dimensions are significantly larger than the element thickness. By contouring the shell section thickness, output variable STH, you can easily verify that all elements are oriented appropriately and have the correct thickness. If the element is oriented improperly, one of the in-plane dimensions will become the element section thickness, resulting in a discontinuous contour plot. Alternatively, you can plot the material axis to verify that the 3-axis points in the desired normal direction. If the element is oriented improperly, one of the in-plane axes (either the 1- or 2-axis) would point in the normal direction. Numbering of section points through the shell thickness The section points through the thickness of the shell are numbered consecutively, starting with point 1. For shell sections integrated during the analysis, section point 1 is exactly on the bottom surface of the shell if Simpson’s rule is used, and it is the point that is closest to the bottom surface if Gauss quadrature is used. For general shell sections, section point 1 is always on the bottom surface of the shell. For a homogeneous section the total number of section points is defined by the number of integration points through the thickness. For shell sections integrated during the analysis, you can define the number of integration points through the thickness. The default is five for Simpson’s rule and three for Gauss quadrature. For general shell sections, output can be obtained at three section points. For a composite section the total number of section points is defined by adding the number of integration points per layer for all of the layers. For shell sections integrated during the analysis, you can define the number of integration points per layer. The default is three for Simpson’s rule and two for Gauss quadrature. For general shell sections, the number of section points for output per layer is three. Default output points In Abaqus/Standard the default output points through the thickness of a shell section are the points that are on the bottom and top surfaces of the shell section (for integration with Simpson’s rule) or the points that are closest to the bottom and top surfaces (for Gauss quadrature). For example, if five integration points are used through a single layer shell, output will be provided for section points 1 (bottom) and 5 (top). In Abaqus/Explicit all section points through the thickness of a shell section are written to the results file for element output requests. 29.6.2 CHOOSING A SHELL ELEMENT Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Shell elements: overview,” Section 29.6.1 • “Three-dimensional conventional shell element library,” Section 29.6.7 • “Continuum shell element library,” Section 29.6.8 • “Axisymmetric shell element library,” Section 29.6.9 • “Axisymmetric shell elements with nonlinear, asymmetric deformation,” Section 29.6.10 • “Creating homogeneous shell sections,” Section 12.13.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating composite shell sections,” Section 12.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The Abaqus/Standard shell element library includes: • elements for three-dimensional shell geometries; • elements for axisymmetric geometries with axisymmetric deformation; • elements for axisymmetric geometries with general deformation that is symmetric about one plane; • elements for stress/displacement, heat transfer, and fully coupled temperature-displacement analysis; • general-purpose elements, as well as elements specifically suitable for the analysis of “thick” or “thin” shells; • general-purpose, three-dimensional, first-order elements that use reduced or full integration; • elements that account for finite membrane strain; • elements that use five degrees of freedom per node where possible, as well as elements that always use six degrees of freedom per node; and • continuum shell elements. The Abaqus/Explicit shell element library includes: • general-purpose three-dimensional elements to model “thick” or “thin” shells that account for finite membrane strains; • small-strain elements; • fully coupled temperature-displacement analysis elements; • an element for axisymmetric geometries with axisymmetric deformation; and • continuum shell elements. Naming convention The naming convention for shell elements depends on the element dimensionality. Three-dimensional shell elements Three-dimensional shell elements in Abaqus are named as follows: 8 R 5 W warping considered in small-strain formulation in ABAQUS/Explicit (optional) optional: 5 dof (5); coupled temperature-displacement (T); small-strain formulation in ABAQUS/Explicit (S) reduced integration (optional) number of nodes conventional stress/displacement shell (S); continuum stress/displacement shell (SC); triangular stress/displacement thin shell (STRI); heat transfer shell (DS) For example, S4R is a 4-node, quadrilateral, stress/displacement shell element with reduced integration and a large-strain formulation; and SC8R is an 8-node, quadrilateral, first-order interpolation, stress/displacement continuum shell element with reduced integration. Axisymmetric shell elements Axisymmetric shell elements in Abaqus are named as follows: AX 2 Optional: coupled temperature-displacement (T); number of Fourier modes (1, 2, 3, or 4) order of interpolation axisymmetric (AX); axisymmetric with nonlinear, asymmetric deformation (AXA) stress/displacement shell (S); heat transfer shell (DS) For example, DSAX1 is an axisymmetric, heat transfer shell element with first-order interpolation. Conventional stress/displacement shell elements The conventional stress/displacement shell elements in Abaqus can be used in three-dimensional or axisymmetric analysis. In Abaqus/Standard they use linear or quadratic interpolation and allow mechanical and/or thermal (uncoupled) loading; in Abaqus/Explicit they use linear interpolation and allow mechanical loading. These elements can be used in static or dynamic procedures. Some elements include the effect of transverse shear deformation and thickness change, while others do not. Some elements allow large rotations and finite membrane deformation, while others allow large rotations but small strains. Interpolation of temperature and field variables in stress/displacement shell elements The value of temperatures at the integration locations in the surface of the shell used to compute the thermal stresses depends on whether first-order or second-order elements are used. An average temperature is used at the integration location in linear elements so that the thermal strain is constant throughout the shell surface. A linearly varying temperature distribution is used in higher-order shell elements. Field variables in stress/displacement shell elements are interpolated the same way as temperatures. Stress/displacement continuum shell elements The stress/displacement continuum shell elements in Abaqus can be used in three-dimensional analysis. Continuum shells discretize an entire three-dimensional body, unlike conventional shells which discretize a reference surface . These elements have displacement degrees of freedom only, use linear interpolation, and allow mechanical and/or thermal (uncoupled) loading for static and dynamic procedures. The continuum shell elements are general-purpose shells that allow finite membrane deformation and large rotations and, thus, are suitable for nonlinear geometric analysis. These elements include the effects of transverse shear deformation and thickness change. Continuum shell elements employ first-order layer-wise composite theory, and estimate through- thickness section forces from the initial elastic moduli. Unlike conventional shells, continuum shell elements can be stacked to provide more refined through-thickness response. Stacking continuum shell elements allows for a richer transverse shear stress and force prediction. Although continuum shell elements discretize a three-dimensional body, care should be taken to verify whether the overall deformation sustained by these elements is consistent with their layer-wise plane stress assumption; that is, the response is bending dominated and no significant thickness change is observed (i.e., approximately less than 10% thickness change). Otherwise, regular three-dimensional solid elements (“Three-dimensional solid element library,” Section 28.1.4) should be used. Furthermore, the thickness strain mode may yield a small stable time increment for thin continuum shell elements in Abaqus/Explicit . Coupled temperature-displacement continuum shell elements The coupled temperature-displacement continuum shell elements in Abaqus have continuum shell geometry and use linear interpolation for the geometry and displacements. The temperature is interpolated linearly as well. The thermal formulation is similar to that used for three-dimensional coupled temperature-displacement solid elements with reduced integration, for which the temperature variation is trilinear elements,” Section 28.1.1). The temperatures at the section points through the thickness are interpolated linearly from the temperatures at the nodes. Heat transfer shell elements These elements, available only in Abaqus/Standard and only with conventional shell element geometry, are intended to model heat transfer in shell-type structures. They provide the values of temperature at a number of points through the thickness at each shell node. This output can be input directly to the equivalent stress analysis shell element for sequentially coupled thermal-stress analysis (“Sequentially coupled thermal-stress analysis,” Section 16.1.2). Temperature variation through the shell thickness The temperature variation is assumed to be piecewise quadratic through the thickness, while the interpolation on the reference surface of the shell is the same as that of the corresponding stress elements. For shell sections integrated during the analysis (“Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5) you can specify the number of section points used for cross-section integration and thickness-direction temperature interpolation at each node. Only Simpson’s rule can be used for integration through the shell thickness. The temperature on the bottom surface of the shell (the surface in the negative direction along the shell normal—see “Defining the initial geometry of conventional shell elements,” Section 29.6.3) is degree of freedom 11. The temperature on the top surface is degree of freedom . A maximum of 20 temperature degrees of freedom can exist at a node. For a single-layer shell is the total number of integration points used through the shell section. If a single section point is used for the cross-section integration, there is no temperature variation through the thickness of the shell and the temperature of the entire shell cross-section is degree of freedom 11. For a multi-layered shell the temperature at the top of each layer is the same as the temperature at the bottom of the next layer. Therefore, ( > 1) is the number of integration points used in layer l. If where is equal to the number of composite layers. In this case, there is no temperature variation through the thickness of the shell, and the temperature of the entire composite is degree of freedom 11. The internal energy storage and heat conduction terms for shells are integrated in the same way as in the corresponding continuum elements elements,” Section 28.1.1). =1, Using shells in a thermal-stress analysis To use the temperatures that are saved in the Abaqus/Standard results file directly as input to a thermal- stress analysis, the mesh and the specification of the number of temperature points in the shell sections must be the same in the heat transfer and the stress analysis models. In addition, multi-layered heat transfer shell elements must have the same number of integration points in each layer. Coupled temperature-displacement shell elements The coupled temperature-displacement shell elements available in Abaqus have conventional shell element geometry and use linear or quadratic interpolation for the geometry and displacements. The temperature is interpolated linearly from the corner or end nodes; the lower-order temperature interpolation in quadratic shells is chosen to give the same interpolation order for thermal strain, which is proportional to temperature, as for total strain. All terms in the governing equations are integrated in the reference surface of the shell using a conventional Gauss scheme; Simpson’s rule is used to integrate through the shell thickness. Temperature variation through the shell thickness The temperature variation through the shell thickness is assumed to be piecewise quadratic and is interpolated from temperatures at a series of points through the thickness of the shell at each node. The number of temperature values to be used at each node is determined by the number of integration points that you specify in the shell section definition . Up to a maximum of 20 temperature values are stored as degrees of freedom 11, 12, 13, etc. (up to degree of freedom 30) in a manner that is identical to that used for heat transfer shell elements . “Thick” versus “thin” conventional shell elements Abaqus includes general-purpose, conventional shell elements as well as conventional shell elements that are valid for thick and thin shell problems. See below for a discussion of what constitutes a “thick” or “thin” shell problem. This concept is relevant only for elements with displacement degrees of freedom. The general-purpose, conventional shell elements provide robust and accurate solutions to most applications and will be used for most applications. However, in certain cases, for specific applications in Abaqus/Standard, enhanced performance may be obtained with the thin or thick conventional shell elements; for example, if only small strains occur and five degrees of freedom per node are desired. The continuum shell elements can be used for any thickness; however, thin continuum shell elements may result in a small stable time increment in Abaqus/Explicit. General-purpose conventional shell elements These elements allow transverse shear deformation. They use thick shell theory as the shell thickness increases and become discrete Kirchhoff thin shell elements as the thickness decreases; the transverse shear deformation becomes very small as the shell thickness decreases. Element types S3/S3R, S3RS, S4, S4R, S4RS, S4RSW, SAX1, SAX2, SAX2T, SC6R, and SC8R are general-purpose shells. Thick conventional shell elements In Abaqus/Standard thick shells are needed in cases where transverse shear flexibility is important and second-order interpolation is desired. When a shell is made of the same material throughout its thickness, this occurs when the thickness is more than about 1/15 of a characteristic length on the surface of the shell, such as the distance between supports for a static case or the wavelength of a significant natural mode in dynamic analysis. Abaqus/Standard provides element types S8R and S8RT for use only in thick shell problems. Thin conventional shell elements In Abaqus/Standard thin shells are needed in cases where transverse shear flexibility is negligible and the Kirchhoff constraint must be satisfied accurately (i.e., the shell normal remains orthogonal to the shell reference surface). For homogeneous shells this occurs when the thickness is less than about 1/15 of a characteristic length on the surface of the shell, such as the distance between supports or the wave length of a significant eigenmode. However, the thickness may be larger than 1/15 of the element length. Abaqus/Standard has two types of thin shell elements: those that solve thin shell theory (the Kirchhoff constraint is satisfied analytically) and those that converge to thin shell theory as the thickness decreases (the Kirchhoff constraint is satisfied numerically). • The element that solves thin shell theory is STRI3. STRI3 has six degrees of freedom at the nodes and is a flat, faceted element (initial curvature is ignored). If STRI3 is used to model a thick shell problem, the element will always predict a thin shell solution. • The elements that impose the Kirchhoff constraint numerically are S4R5, STRI65, S8R5, S9R5, SAXA1n, and SAXA2n. These elements should not be used for applications in which transverse shear deformation is important. If these elements are used to model a thick shell problem, the elements may predict inaccurate results. Finite-strain versus small-strain shell elements Abaqus has both finite-strain and small-strain shell elements. This concept is relevant only for elements with displacement degrees of freedom. Finite-strain shell elements Element types S3/S3R, S4, S4R, SAX1, SAX2, SAX2T, SAXA1n, and SAXA2n account for finite membrane strains and arbitrarily large rotations; therefore, they are suitable for large-strain analysis. The underlying formulation is described in “Axisymmetric shell elements,” Section 3.6.2 of the Abaqus Theory Manual; “Finite-strain shell element formulation,” Section 3.6.5 of the Abaqus Theory Manual; and “Axisymmetric shell element allowing asymmetric loading,” Section 3.6.7 of the Abaqus Theory Manual. Continuum shell elements SC6R and SC8R account for finite membrane strains, arbitrary large rotation, and allow for changes in thickness, making them suitable for large-strain analysis. Computation of the change in thickness is based on the element nodal displacements, which in turn are computed from an effective elastic modulus defined at the beginning of an analysis. Small-strain shell elements In Abaqus/Standard the three-dimensional “thick” and “thin” element types STRI3, S4R5, STRI65, S8R, S8RT, S8R5, and S9R5 provide for arbitrarily large rotations but only small strains. The change in thickness with deformation is ignored in these elements. In Abaqus/Explicit element types S3RS, S4RS, and S4RSW are provided for shell problems with small membrane strains and arbitrarily large rotations. Many impact dynamics analyses fall within this class of problems, including those of shell structures undergoing large-scale buckling behavior but relatively small amounts of membrane stretching and compression. Although solution the small-strain shell elements in accuracy may degrade as membrane strains become large, Abaqus/Explicit provide a computationally efficient alternative to the finite-membrane-strain elements for appropriate applications. The underlying formulation is described in “Small-strain shell elements in Abaqus/Explicit,” Section 3.6.6 of the Abaqus Theory Manual. Change of shell thickness Thickness change is considered only in geometrically nonlinear analyses. For conventional shells, stress in the thickness direction is zero and the strain results only from the Poisson’s effect. For continuum shells, the stress in the thickness direction may not be zero and may cause additional strain beyond that due to Poisson’s effect. The thickness strain due to Poisson’s effect is referred as the “Poisson strain,” and any additional strain beyond the “Poisson strain” is referred to as the “effective thickness strain.” For shell elements in Abaqus/Explicit defined by integrating the section during the analysis, the Poisson strain is calculated by enforcing the plane stress condition either at the individual material points in the section and then integrating the Poisson strain from these material points, or at the integration station for the whole section using a “section Poisson’s ratio.” For shell elements in Abaqus/Standard only the section Poisson’s ratio method is available. For shell elements defined by general shell sections, only the section Poisson’s ratio method is applicable. See “Defining the Poisson strain in shell elements in the thickness direction” in “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, and “Defining the Poisson strain in shell elements in the thickness direction” in “Using a general shell section to define the section behavior,” Section 29.6.6, for details. Thickness direction stress in continuum shell elements The thickness direction stress is computed by penalizing the effective thickness strain with a constant “thickness modulus.” The thickness modulus used for a single layer shell element with an elastic or elastic-plastic material is twice the in-plane elastic shear modulus. In the case of a composite shell with each layer either an elastic or elastic-plastic material, the thickness modulus is computed as the thickness- weighted harmonic mean of the contributions from the individual layers: where thickness of layer the material definition for layer is the thickness modulus, , and in the initial configuration. is the layer index, is the relative is the number of layers, is twice the initial in-plane elastic shear modulus based on See “Defining the thickness modulus in continuum shell elements” in “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, and “Defining the thickness modulus in continuum shell elements” in “Using a general shell section to define the section behavior,” Section 29.6.6, for details. Five degree of freedom shells versus six degree of freedom shells Two types of three-dimensional conventional shell elements are provided in Abaqus/Standard: ones that use five degrees of freedom (three displacement components and two in-surface rotation components) where possible and ones that use six degrees of freedom (three displacement components and three rotation components) at all nodes. The elements that use five degrees of freedom (S4R5, STRI65, S8R5, S9R5) can be more economical. However, they are available only as “thin” shells (they cannot be used as “thick” shells) and cannot be used for finite-strain applications (although they model large rotations with small strains accurately). In addition, output for the five degree of freedom shell elements is restricted as follows: • At nodes that use the two in-surface rotation components, the values of these in-surface rotations are not available for output. • When output variable NFORC is requested, moments corresponding to the in-surface rotations are not available for output. When five degree of freedom shell elements are used, Abaqus/Standard will automatically switch to using three global rotation components at any node that: • has kinematic boundary conditions applied to rotational degrees of freedom, • is used in a multi-point constraint (“General multi-point constraints,” Section 34.2.2) that involves rotational degrees of freedom, • is shared with a beam element or a shell element that uses the three global rotation components at all nodes, • is on a fold line in the shell (that is, on a line where shells with different surface normals come together), or • is loaded with moments. In all elements that use three global rotation components at all nodes (whether activated as described above or always present), a singularity exists at any node where the surface is assumed to be continuously curved: three rotation components are used, but only two are actively associated with stiffness. A small stiffness is associated with the rotation about the normal to avoid this difficulty. The default stiffness values used are sufficiently small such that the artificial energy content is negligible. In some rare cases this stiffness may need to be altered. You can define a scaling factor for this stiffness, as described in “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, and “Using a general shell section to define the section behavior,” Section 29.6.6. Reduced integration Many shell element types in Abaqus use reduced (lower-order) integration to form the element stiffness. The mass matrix and distributed loadings are still integrated exactly. Reduced integration usually provides more accurate results (provided the elements are not distorted or loaded in in-plane bending) and significantly reduces running time, especially in three dimensions. When reduced integration is used with first-order (linear) elements, hourglass control is required. Therefore, when using first-order reduced-integration elements, you must check if hourglassing is occurring; if it is, a finer mesh may be required or concentrated loads must be distributed over multiple nodes. The second-order reduced-integration elements available in Abaqus/Standard generally do not have the same difficulty and are recommended in cases when the solution is expected to be smooth. First-order elements are recommended when large strains or very high strain gradients are expected. Specifying section controls for shell elements In Abaqus/Standard you can specify nondefault hourglass control parameters for shell elements. In Abaqus/Explicit you can specify second-order accuracy in the element formulation, nondefault hourglass control parameters for S4R, S4RS, and S4RSW elements, or deactivate the drill constraint for S3RS and S4RS elements. See “Section controls,” Section 27.1.4, for more information. Input File Usage: Use the following options in Abaqus/Standard: *SHELL SECTION or *SHELL GENERAL SECTION *HOURGLASS STIFFNESS Use one of the following options in Abaqus/Explicit: *SHELL SECTION, CONTROLS=name *SHELL GENERAL SECTION, CONTROLS=name Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Element Controls Modeling issues A number of modeling issues must be considered when using shell elements. Using S3/S3R and S3RS elements Both S3 and S3R refer to the same 3-node triangular shell element. This element is a degenerated version of S4R that is fully compatible with S4R and, in Abaqus/Standard, S4. Element S3RS, available in Abaqus/Explicit, is a degenerated version of S4RS that is fully compatible with S4RS. S3/S3R and S3RS provide accurate results in most loading situations. However, because of their constant bending and membrane strain approximations, high mesh refinement may be required to capture pure bending deformations or solutions to problems involving high strain gradients. A consequence of the degenerated element formulation is that the solution changes slightly when the element connectivity is permuted. Degenerating elements Element types S4, S4R, S4R5, S4RS, S8R5, and S9R5 can be degenerated to triangles. However, for elements S4 (element S4 degenerated to a triangle may exhibit overly stiff response in membrane deformation), S4R, and S4RS it is recommended that S3R and S3RS be used instead. The quarter-point technique (moving the midside nodes to the quarter points to give a singularity for elastic fracture mechanics applications) can be used with the quadratic element types S8R5 and S9R5 . The accuracy of the element is very significantly reduced when it is degenerated to a triangle; therefore, this is not recommended except for special applications, such as fracture. Element types S8R and S8RT cannot be degenerated to triangles. Element types DS4 and DS8 can be degenerated to triangles, but it is recommended that DS3 and DS6 elements be used instead. Modeling with continuum shell elements Continuum shell elements are similar to continuum solids from a modeling point of view. The element geometries for the SC6R and SC8R elements are a triangular prism and hexahedron, respectively, with displacement degrees of freedom only. Continuum shell elements must be oriented correctly, since these elements have a thickness direction associated with them. See “Shell elements: overview,” Section 29.6.1, for further details on element connectivity and orientation. When classical shell structures (structures in which only the midsurface geometry and kinematic constraints are provided) are analyzed, care must be taken that appropriate moments and rotations are specified. For example, a moment may be applied as a force-couple system at the corresponding nodes on the top and bottom faces. A rotation boundary condition may be specified through a kinematic constraint to yield the appropriate displacement boundary conditions on the edge of the continuum shell. Continuum shell elements can be connected directly to first-order continuum solids without any kinematic transition. An appropriate kinematic transition needs to be provided when conventional shell elements are connected to continuum shell elements to correctly transfer the moment/rotation at the reference surface of a conventional shell. Such a transition can be defined with a shell-to-solid coupling constraint or any other kinematic constraint, such as a surface-based coupling constraint, a multi-point constraint, or a linear constraint equation. Using the SC6R element The SC6R element is a degenerated version of the SC8R element. The SC6R element provides accurate results in most loading situations. However, because of its constant bending and membrane strain approximations, high mesh refinement may be required to capture pure bending deformations or solutions to problems involving high strain gradients. Modeling contact with continuum shell elements Continuum shell elements, SC6R and SC8R, allow two-sided contact with changes in the thickness and are thus suitable for modeling contact. Stable time increment in Abaqus/Explicit In Abaqus/Explicit the element stable time increment can be controlled by the continuum shell element thickness, particularly for thin shell applications. This may increase significantly the number of increments taken to complete the analysis when compared to the same problem modeled with conventional shell elements. The small stable time increment size may be mitigated by specifying a lower stiffness in the thickness direction when appropriate. Limitations with continuum shell elements Continuum shell elements cannot be used with the hyperfoam material definitions, nor can they be used with general shell sections where the section stiffness is provided directly. Modeling a “sandwich” shell For a “sandwich” shell, in which parts of the cross-section are made of a softer material (especially when the layers are nonisotropic so that some layers are weak in particular directions), the transverse shear flexibility can be important even when the shell is rather thin. Use of general-purpose shell elements or stacking continuum shell elements is recommended in such cases. See “Shell section behavior,” Section 29.6.4, for a discussion of transverse shear stiffness in shell elements. Modeling bending of a thin curved shell in Abaqus/Standard In Abaqus/Standard curved elements (STRI65, S8R5, S9R5) are preferable for modeling bending of a thin curved shell. Element type STRI3 is a flat facet element. If this element is used to model bending of a curved shell, a dense mesh may be required to obtain accurate results. Modeling buckling of doubly curved shells in Abaqus/Standard Element type S8R5 may give inaccurate results for buckling problems of doubly curved shells due to the fact that the internally defined center node may not be positioned on the actual shell surface. Element type S9R5 should be used instead. Using S8R5 in contact analyses Element type S8R5 is converted automatically to element type S9R5 if a slave surface in a contact pair is attached to the element. Applying moments to S9R5 elements Moments should not be applied to the center node of S9R5 elements. Using S4 elements Element type S4 is a fully integrated, general-purpose, finite-membrane-strain shell element. The element’s membrane response is treated with an assumed strain formulation that gives accurate solutions to in-plane bending problems, is not sensitive to element distortion, and avoids parasitic locking. Element type S4 does not have hourglass modes in either the membrane or bending response of the element; hence, the element does not require hourglass control. The element has four integration locations per element compared with one integration location for S4R, which makes the element computationally more expensive. S4 is compatible with both S4R and S3R. S4 can be used for problems prone to membrane- or bending-mode hourglassing, in areas where greater solution accuracy In all of these situations S4 will is required, or for problems where in-plane bending is expected. outperform element type S4R. S4 cannot be used with the hyperelastic or hyperfoam material definitions in Abaqus/Standard. 29.6.3 DEFINING THE INITIAL GEOMETRY OF CONVENTIONAL SHELL ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Shell elements: overview,” Section 29.6.1 • “Assigning a section,” Section 12.15.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Assigning shell/membrane normal directions,” Section 12.15.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The initial shell geometry: • must be defined accurately since most shell elements are true curved shell elements; • is defined by initial normal directions, which can be user-defined or calculated by Abaqus; • requires that sufficient mesh refinement be used so that the discretized surface accurately represents the actual surface; and • can include an offset of the reference surface from the shell’s midsurface. Defining nodal normals This discussion applies to conventional shell elements only. The normals of a continuum shell element are defined by the position of the top and bottom nodes along the shell corner edge . Conventional shell elements in Abaqus (with the exception of element types S3/S3R, S3RS, S4R, S4RS, S4RSW, and STRI3) are true curved shell elements; true curved shell elements require special attention to accurate calculation of the initial curvature of the surface. Shell normals can be defined by giving the direction cosines of the normal to the surface at all nodes attached to shell elements. These direction cosines can be entered as the fourth, fifth, and sixth coordinates of each node definition or in a user-specified normal definition, as described below; see “Normal definitions at nodes,” Section 2.1.4, for more information. If the user-defined normal differs from the midsurface normal by more than 20°, a warning message is issued to the data (.dat) file. However, if the angle is more than 160°, the direction of the midsurface normal is reversed and no warning message is issued. An additional warning message is issued if the nodal normal deviates more than 10° from the average element normal. Specifying the same normal at a node for all shell elements attached to the node creates a smooth shell surface at the node. Define a user-specified normal to introduce a fold line. If the normals are not defined as part of the node definition or by a user-specified normal, Abaqus will calculate the normal using the algorithm given below. Since the only information available for this calculation is the nodal coordinates, it may not define the normal directions accurately. Accurate definition can be important on edges of the model, especially if they are also symmetry planes, or on lines where the curvature of the shell changes discontinuously. It is also important when relatively coarse meshing is used on highly curved shells, since Abaqus may estimate that the change in direction from one element to its neighbor is so large that it represents a fold line, not a smoothly curving surface. You are, therefore, advised to enter the direction cosines whenever the shell normal is defined ambiguously by the nodal coordinates. Failure to do so may lead to inaccurate results. The normal direction at a node is needed for temperature input and nodal stress output. The direction is taken from the definitions below for the elements adjacent to the nodes. If this leads to a conflict at a node, the positive normal direction used at that node will be the one defined by the lowest numbered element at the node. Calculation of average nodal normals by Abaqus If the nodal normal is not defined as part of the node definition, element normal directions at the node are calculated for all shell and beam elements for which a user-specified normal is not defined (the “remaining” elements). For shell elements the normal direction is orthogonal to the shell midsurface, as described in “Shell elements: overview,” Section 29.6.1. For beam elements the normal direction is the second cross-section direction, as described in “Beam element cross-section orientation,” Section 29.3.4. The following algorithm is then used to obtain an average normal (or multiple averaged normals) for the remaining elements that need a normal defined: 1. If a node is connected to more than 30 remaining elements, no averaging occurs and each element is assigned its own normal at the node. The first nodal normal is stored as the normal defined as part of the node definition. Each subsequent normal is stored as a user-specified normal. 2. If a node is shared by 30 or fewer remaining elements, the normals for all the elements connected to the node are computed. Abaqus takes one of these elements and puts it in a set with all the other elements that have normals within 20° of it. Then: a. Each element whose normal is within 20° of the added elements is also added to this set (if it is not yet included). b. This process is repeated until the set contains for each element in the set all the other elements whose normals are within 20°. c. If all the normals in the final set are within 20° of each other, an average normal is computed for all the elements in the set. If any of the normals in the set are more than 20° out of line from even a single other normal in the set, no averaging occurs for elements in the set and a separate normal is stored for each element. d. This process is repeated until all the elements connected to the node have had normals computed for them. e. The first nodal normal is stored as the normal defined as part of the node definition. Each subsequently generated nodal normal is stored as a user-specified normal. This algorithm ensures that the nodal averaging scheme has no element order dependence. A simple example illustrating this process is included below. Example: shell normal averaging Consider the three element model in Figure 29.6.3–1. Elements 1, 2, and 3 share a common node, node 10, with no user-specified normal defined. 10 20 50 30 40 Figure 29.6.3–1 Three element example for nodal averaging algorithm. In the first scenario, suppose that at node 10 the normal for element 2 is within 20° of both elements 1 and 3, but the normals for elements 1 and 3 are not within 20° of each other. In this case, each element is assigned its own normal: one is stored as part of the node definition and two are stored as user-specified normals. In the second scenario, suppose that at node 10 the normal for element 2 is within 20° of both elements 1 and 3 and the normals for elements 1 and 3 are within 20° of each other. In this case, a single average normal for elements 1, 2, and 3 would be computed and stored as part of the node definition. In the last scenario, suppose that at node 10 the normal for element 2 is within 20° of element 1 but the normal of element 3 is not within 20° of either element 1 or 2. In this case, an average normal is computed and stored for elements 1, and 2 and the normal for element 3 is stored by itself: one is stored as part of the node definition and the other is stored as a user-specified normal. Meshing concerns In a coarse mesh this algorithm may introduce fold lines where the shell is smooth, or it may create a smooth shell where there should be a fold if the angle of the fold line is less than 20°. Difficulties in large- displacement shell analysis are sometimes caused by false fold lines introduced by coarse meshing. To model a smooth shell, the mesh should be refined enough to create unique nodal normals or the normals must be defined as part of the node definition or by a user-specified normal. To model plates or shells with fold lines, you should define user-specified normals. Verifying the normal definitions Normal definitions can be checked by examining the analysis input file processor output. The direction cosines of the reference normal associated with a node are listed under the NODE DEFINITIONS output in the data (.dat) file. User-specified normals are listed under the NORMAL DEFINITIONS output in the data file. Offset: reference surface versus midsurface This discussion applies to conventional shell elements only. Continuum shell elements define a top and bottom surface around the structural body being modeled. The notion of a shell reference surface is not applicable for these types of elements. The reference surface for conventional shell elements is defined by the shell’s nodes and normal definitions. When modeling with shell elements, the reference surface is typically coincident with the shell’s midsurface. However, many situations arise in which it is more convenient to define the reference surface as offset from the shell’s midsurface. For example, CAD surfaces usually represent either the top or bottom surface of the shell. In this case it may be easier to define the reference surface to be coincident with the CAD surface and, therefore, offset from the shell’s midsurface. Shell offsets can also be used to define a more precise surface geometry for contact problems where shell thickness is important. Another situation where the offset from the midsurface may be important is when a shell with continuously varying thickness is modeled. In this case if one surface of the shell is smooth while the other surface is rough, as in some aircraft structures, using the smooth surface as the reference surface, with an offset of half the shell’s thickness from the midsurface, will represent the physical geometry more accurately. The use of the midsurface as the reference surface for this case is much more complicated and may result in an inaccurate model. You can introduce offsets in the section definitions for both shell sections integrated during the analysis and general shell sections. The offset value is defined as a fraction of the shell thickness measured from the shell’s midsurface to the shell’s reference surface. See “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, and “Using a general shell section to define the section behavior,” Section 29.6.6, for details. The degrees of freedom for the shell are associated with the reference surface. All kinematic quantities, including the element’s area, are calculated there. Any loading in the plane of the reference surface will, therefore, cause both membrane forces and bending moments when a nonzero offset value is used. Large offset values for curved shells may also lead to a surface integration error, affecting the stiffness, mass, and rotary inertia for the shell section. For stability purposes Abaqus/Explicit also automatically scales the rotary inertia used for shell elements by a factor proportional to the offset squared, which may result in errors for large offsets. When a large offset from the shell’s midsurface is necessary, use multi-point constraints instead . 29.6.4 SHELL SECTION BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Shell elements: overview,” Section 29.6.1 • “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5 • “Using a general shell section to define the section behavior,” Section 29.6.6 • *SHELL GENERAL SECTION • *SHELL SECTION • “Creating homogeneous shell sections,” Section 12.13.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating composite shell sections,” Section 12.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The shell section behavior: • may or may not require numerical integration over the section; • can be linear or nonlinear; and • can be homogeneous or composed of layers of different material. Methods for defining the shell section behavior Two methods are provided to define the cross-sectional behavior of a shell. • Linear moment-bending and force-membrane strain relationships can be defined by using a general shell section . In this case all calculations are done in terms of section forces and moments. In Abaqus/Standard when section properties are given directly (i.e., the section is not associated with one or more material definitions), strains and stresses are not available for output. However, when section properties are specified by one or more elastic material layers, strains and stresses are available when requested for output. In Abaqus/Explicit stresses and strains are not available for output at the section points whenever a general shell section is used; only section forces, section moments, and section strains are available for output. In Abaqus/Standard nonlinear behavior of the shell section, formulated in terms of forces and moments, can be defined by using a general shell section in conjunction with user subroutine UGENS. • Alternatively, a shell section integrated during the analysis allows the cross-sectional behavior to be calculated by numerical integration through the shell thickness, thus providing complete generality in material modeling. With this type of section any number of material points can be defined through the thickness and the material response can vary from point to point. Both general shell sections and shell sections integrated during the analysis allow layers of different materials, in different orientations, to be used through the cross-section. In these cases the section definition provides the shell thickness, material, and orientation per layer. For conventional shell elements you can specify an offset of the reference surface from the shell’s midsurface when the section properties are specified by one or more material layers. When the section properties are given directly, you cannot directly specify an offset; however, an offset can be included implicitly in the section properties. A nonzero offset cannot be specified for continuum shell elements. If a nonzero offset is specified for a continuum shell element, an error message is issued during input file preprocessing. Determining whether to use a shell section integrated during the analysis or a general shell section When a shell section integrated during the analysis is used, Abaqus uses numerical integration through the thickness of the shell to calculate the section properties. This type of shell section is generally used with nonlinear material behavior in the section. It must be used with shells that provide for heat transfer, since general shell sections do not allow the definition of heat transfer properties. Use a general shell section if the response of the shell is linear elastic and its behavior is not dependent on changes in temperature or predefined field variables or, in Abaqus/Standard, if nonlinear behavior in terms of forces and moments is to be defined in user subroutine UGENS. Transverse shear stiffness For all shell elements in Abaqus/Standard that use transverse shear stiffness and for the finite-strain shell elements in Abaqus/Explicit, the transverse shear stiffness is computed by matching the shear response for the shell to that of a three-dimensional solid for the case of bending about one axis. For the small- strain shell elements in Abaqus/Explicit the transverse shear stiffness is based on the effective shear modulus. Transverse shear stiffness for shell elements in Abaqus/Standard and finite-strain shell elements in Abaqus/Explicit In all shell elements in Abaqus/Standard that are valid for thick shell problems or that enforce the Kirchhoff constraint numerically (i.e., all shell elements except STRI3) and in the finite-strain shell elements in Abaqus/Explicit (S3R, S4, S4R, SAX1, SC6R, and SC8R), Abaqus computes the transverse shear stiffness by matching the shear response for the case of the shell bending about one axis, using a parabolic variation of transverse shear stress in each layer. The approach is described in “Transverse shear stiffness in composite shells and offsets from the midsurface,” Section 3.6.8 of the Abaqus Theory Manual, and generally provides a reasonable estimate of the shear flexibility of the shell. It also provides estimates of interlaminar shear stresses in composite shells. In calculating the transverse shear stiffness, Abaqus assumes that the shell section directions are the principal bending directions (bending about one principal direction does not require a restraining moment about the other direction). For composite shells with orthotropic layers that are not symmetric about the shell midsurface, the shell section directions may not be the principal bending directions. In such cases the transverse shear stiffness is a less accurate approximation and will change if different shell section directions are used. Abaqus computes the transverse shear stiffness only once at the begining of the analysis based on initial elastic properties given in the model data. Any changes to the transverse shear stiffness that occur due to changes in the material stiffness during the analysis are ignored. Axisymmetric shell elements SAX1 and SAX2; three-dimensional shell elements S3/S3R, S4, S4R, S8R, and S8RT; and continuum shell elements SC6R and SC8R are based on a first-order shear deformation theory. Other shell elements—such as S4R5, S8R5, S9R5, STRI65, and SAXAmn—use the transverse shear stiffness to enforce the Kirchhoff constraints numerically in the thin shell limit. The transverse shear stiffness is not relevant for shells without displacement degrees of freedom nor is it relevant for element type STRI3. Although element type S4 has four integration points, the transverse shear calculation is assumed constant over the element. Higher resolution of the transverse shear may be obtained by stacking continuum shell elements. For most shell sections, including layered composite or sandwich shell sections, Abaqus will calculate the transverse shear stiffness values required in the element formulation. You can override these default values. The default shear stiffness values are not calculated in some cases if estimates of shear moduli are unavailable during the preprocessing stage of input; for example, when the material behavior is defined by user subroutine UMAT, UHYPEL, UHYPER, or VUMAT or, in Abaqus/Standard, when the section behavior is defined in UGENS. You must define the transverse shear stiffnesses in such cases. Transverse shear stiffness definition The transverse shear stiffness of the section of a shear flexible shell element is defined in Abaqus as where are the components of the section shear stiffness ( refer to the default surface directions on the shell, as defined in “Conventions,” Section 1.2.2, or to the local directions associated with the shell section definition); is a dimensionless factor that is used to prevent the shear stiffness from becoming too large in thin shells; and is the actual shear stiffness of the section (calculated by Abaqus or user-defined). You can specify all three shear stiffness terms ( the default values defined below. The dimensionless factor transverse shear stiffness, regardless of the way ); otherwise, they will take is always included in the calculation of is obtained. For shell elements of type S4R5, S8R5, , and , S9R5, STRI65, or SAXAn the average of of force per length. The dimensionless factor is defined as and is used and is ignored. The have units where A is the area of the element and t is the thickness of the shell. When a general shell section definition not associated with one or more material definitions is used to define the shell section stiffness, the thickness of the shell, t, is estimated as If you do not specify the , they are calculated as follows. For laminated plates and sandwich constructions the are estimated by matching the elastic strain energy associated with shear deformation of the shell section with that based on piecewise quadratic variation of the transverse shear stress across the section, under conditions of bending about one axis. For unsymmetric lay-ups the coupling term can be nonzero. When a general shell section is used and the section stiffness is given directly, the are defined as where is the section stiffness matrix and Y is the initial scaling modulus. When a user subroutine (for example, UMAT, UHYPEL, UHYPER, or VUMAT) is used to define a shell element’s material response, you must define the transverse shear stiffness. The definition of an appropriate stiffness depends on the shell’s material composition and its lay-up; that is, how material is distributed through the thickness of the cross-section. The transverse shear stiffness should be specified as the initial, linear elastic stiffness of the shell in response to pure transverse shear strains. For a homogeneous shell made of a linear, orthotropic elastic material, where the strong material direction aligns with the element’s local 1-direction, the transverse shear stiffness should be and and are the material’s shear moduli in the out-of-plane direction. The number 5/6 is the shear correction coefficient that results from matching the transverse shear energy to that for a three-dimensional structure in pure bending. For composite shells the shear correction coefficient will be different from the value for homogeneous ones; see “Transverse shear stiffness in composite shells and offsets from the midsurface,” Section 3.6.8 of the Abaqus Theory Manual, for a discussion of how the effective shear stiffness for elastic materials is obtained in Abaqus. Checking the validity of using shell theory For linear elastic materials the slenderness ratio, , where =1 or 2 (no sum on ) and l is a characteristic length on the surface of the shell, can be used as a guideline to decide if the assumption that plane sections must remain plane is satisfied and, hence, shell theory is adequate. Generally, if shell theory will be adequate; for smaller values the membrane strains will not vary linearly through the section, and shell theory will probably not give sufficiently accurate results. The characteristic length, l, is independent of the element length and should not be confused with the element’s characteristic length, . To obtain the , you must run a data check analysis using a composite general and shell section definition. The will be printed under the title “TRANSVERSE SHEAR STIFFNESS FOR THE SECTION” in the data (.dat) file if you request model definition data . The will be printed out under the title “SECTION STIFFNESS MATRIX.” Transverse shear stiffness for small-strain shell elements in Abaqus/Explicit When a shell section integrated during the analysis is used, the transverse shear stresses for the small- strain shells in Abaqus/Explicit are assumed to have a piecewise constant distribution in each layer. The transverse shear force will converge to the correct solution for single or multilayer isotropic sections and single-layer orthotropic sections. The transverse shear stiffness is approximate for multilayer orthotropic sections where convergence to the proper transverse shear behavior may not be obtained as shells become thick and principal material directions deviate from the principal section directions. The finite-strain S4R element should be used with a shell section integrated during the analysis if accurate through-thickness transverse shear stress distributions are required for the analysis of composite shells. The same transverse shear stiffness described for the finite-strain shells is used to calculate the transverse shear force for the small-strain shells in Abaqus/Explicit when a general shell section is used. Thus, for this case the transverse shear force for multilayer composite shells will converge to the correct value for both thin and thick sections. Bending strain measures All three-dimensional shell elements in Abaqus use bending strain measures that are approximations to those of Koiter-Sanders shell theory . As per the Koiter-Sanders theory the displacement field normal to the shell surface does not produce any bending moments. For example, a purely radial expansion of a cylinder will result in only membrane stress and strains—there are no variations through the thickness and, hence, no bending. This applies to both the incremental strain measures for linear elastic materials and the deformation gradient for hyperelastic materials. Nodal mass and rotary inertia for composite sections For composite shell sections Abaqus computes the nodal masses based on an average density through the section, weighted with respect to the layer thicknesses. This average density is used to compute an average rotary inertia as if the section were homogeneous. As a consequence, Abaqus does not account for an unsymmetric distribution of mass: the center of mass is assumed to be at the reference surface of the shell. For continuum shells the mass is equally distributed to the top and bottom surface nodes. 29.6.5 USING A SHELL SECTION INTEGRATED DURING THE ANALYSIS TO DEFINE THE SECTION BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Shell elements: overview,” Section 29.6.1 • “Shell section behavior,” Section 29.6.4 • *DISTRIBUTION • *HOURGLASS STIFFNESS • *SHELL SECTION • *TRANSVERSE SHEAR STIFFNESS • “Creating homogeneous shell sections,” Section 12.13.6 of the Abaqus/CAE User’s Manual • “Creating composite shell sections,” Section 12.13.7 of the Abaqus/CAE User’s Manual • Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Manual Overview A shell section integrated during the analysis: • is used when numerical integration through the thickness of the shell is required; and • can be associated with linear or nonlinear material behavior. Defining a homogeneous shell section To define a shell made of a single material, use a material definition (“Material data definition,” Section 21.1.2) to define the material properties of the section and associate these properties with the section definition. Optionally, you can refer to an orientation (“Orientations,” Section 2.2.5) to be associated with this material definition. A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be assigned to the shell section definition. Linear or nonlinear material behavior can be associated with the section definition. However, if the material response is linear, the more economic approach is to use a general shell section . You specify the shell thickness and the number of integration points to be used through the shell section . For continuum shell elements the specified shell thickness is used to estimate certain section properties, such as hourglass stiffness, which are later computed using the actual thickness computed from the element geometry. You must associate the section properties with a region of your model. If the orientation definition assigned to a shell section definition is defined with distributions, spatially varying local coordinate systems are applied to all shell elements associated with the shell section. A default local coordinate system (as defined by the distributions) is applied to any shell element that is not specifically included in the associated distribution. Input File Usage: *SHELL SECTION, ELSET=name, MATERIAL=name, ORIENTATION=name Abaqus/CAE Usage: where the ELSET parameter refers to a set of shell elements. Property module: Create Section: select Shell as the section Category and Homogeneous as the section Type: Section integration: During analysis; Basic: Material: name Assign→Material Orientation: select regions Assign→Section: select regions Defining a composite shell section You can define a laminated (layered) shell made of one or more materials. You specify the thickness, the number of integration points , the material, and the orientation (either as a reference to an orientation definition or as an angle measured relative to the overall orientation definition) for each layer of the shell. The order of the laminated shell layers with respect to the positive direction of the shell normal is defined by the order in which the layers are specified. Optionally, you can specify an overall orientation definition for the layers of a composite shell. A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be used to specify the overall orientation definition for the layers of a composite shell. For continuum shell elements the thickness is determined from the element geometry and may vary through the model for a given section definition. Hence, the specified thicknesses are only relative thicknesses for each layer. The actual thickness of a layer is the element thickness times the fraction of the total thickness that is accounted for by each layer. The thickness ratios for the layers need not be given in physical units, nor do the sum of the layer relative thicknesses need to add to one. The specified shell thickness is used to estimate certain section properties, such as hourglass stiffness, which are later computed using the actual thickness computed from the element geometry. Spatially varying thicknesses can be specified on the layers of conventional shell elements using distributions (“Distribution definition,” Section 2.8.1). A distribution that is used to define layer thickness must have a default value. The default layer thickness is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution. An example of a section with three layers and three section points per layer is shown in Figure 29.6.5–1. The material name specified for each layer refers to a material definition (“Material data definition,” Section 21.1.2). The material behavior can be linear or nonlinear. The orientation for each layer is specified by either the name of the orientation (“Orientations,” Section 2.2.5) associated with the layer or the orientation angle in degrees for the layer. Spatially varying orientation angles can be specified on a layer using distributions (“Distribution definition,” Section 2.8.1). Orientation angles, , are measured positive counterclockwise around the normal and relative to the overall section orientation. If either of the two local directions from the overall section orientation is t3 t2 t1 Layer 3 (material 1, orientation 3) Layer 2 (material 2, orientation 2) Layer 1 (material 1, orientation 1) Layers 1 & 3 use the same material in different orientations n, shell normal Specify 3 temperature values read per layer for stress analysis Use default of 3 section points per layer (also define temperature degrees of freedom for heat transfer) Figure 29.6.5–1 Example of composite shell section definition. not in the surface of the shell, surface. If you do not specify an overall section orientation, shell directions . is applied after the section orientation has been projected onto the shell is measured relative to the default local You must associate the section properties with a region of your model. If the orientation definition assigned to a shell section definition is defined with distributions, spatially varying local coordinate systems are applied to all shell elements associated with the shell section. A default local coordinate system (as defined by the distributions) is applied to any shell element that is not specifically included in the associated distribution. Unless your model is relatively simple, you will find it increasingly difficult to define your model using composite shell sections as you increase the number of layers and as you assign different sections to different regions. It can also be cumbersome to redefine the sections after you add new layers or remove or reposition existing layers. To manage a large number of layers in a typical composite model, you may want to use the composite layup functionality in Abaqus/CAE. For more information, see Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Manual. Input File Usage: *SHELL SECTION, ELSET=name, COMPOSITE, ORIENTATION=name where the ELSET parameter refers to a set of shell elements. Abaqus/CAE Usage: Abaqus/CAE uses a composite layup or a composite shell section to define the layers of a composite shell. Use the following option for a composite layup: Property module: Create Composite Layup: select Conventional Shell or Continuum Shell as the Element Type: Section integration: During analysis: specify orientations, regions, and materials Use the following options for a composite shell section: Property module: Create Section: select Shell as the section Category and Composite as the section Type: Section integration: During analysis Assign→Material Orientation: select regions Assign→Section: select regions Defining the shell section integration Simpson’s rule and Gauss quadrature are provided to calculate the cross-sectional behavior of a shell. You can specify the number of section points through the thickness of each layer and the integration method as described below. The default integration method is Simpson’s rule with five points for a homogeneous section and Simpson’s rule with three points in each layer for a composite section. The three-point Simpson’s rule and the two-point Gauss quadrature are exact for linear problems. The default number of section points should be sufficient for routine thermal-stress calculations and nonlinear applications (such as predicting the response of an elastic-plastic shell up to limit load). For more severe thermal shock cases or for more complex nonlinear calculations involving strain reversals, more section points may be required; normally no more than nine section points (using Simpson’s rule) are required. Gaussian integration normally requires no more than five section points. Gauss quadrature provides greater accuracy than Simpson’s rule when the same number of section points are used. Therefore, to obtain comparable levels of accuracy, Gauss quadrature requires fewer section points than Simpson’s rule does and, thus, requires less computational time and storage space. Using Simpson’s rule By default, Simpson’s rule will be used for the shell section integration. The default number of section points is five for a homogeneous section and three in each layer for a composite section. Simpson’s integration rule should be used if results output on the shell surfaces or transverse shear stress at the interface between two layers of a composite shell is required and must be used for heat transfer and coupled temperature-displacement shell elements. Input File Usage: Abaqus/CAE Usage: *SHELL SECTION, SECTION INTEGRATION=SIMPSON Use the following option for a composite layup: Property module: composite layup editor: Section integration: During analysis, Thickness integration rule: Simpson Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: During analysis; Basic: Thickness integration rule: Simpson Using Gauss quadrature If you use Gauss quadrature for the shell section integration, the default number of section points is three for a homogeneous section and two in each layer for a composite section. In Gauss quadrature there are no section points on the shell surfaces; therefore, Gauss quadrature should be used only in cases where results on the shell surfaces are not required. Gauss quadrature cannot be used for heat transfer and coupled temperature-displacement shell elements. Input File Usage: Abaqus/CAE Usage: *SHELL SECTION, SECTION INTEGRATION=GAUSS Use the following option for a composite layup: Property module: composite layup editor: Section integration: During analysis, Thickness integration rule: Gauss Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: During analysis; Basic: Thickness integration rule: Gauss Defining a shell offset value for conventional shells You can define the distance (measured as a fraction of the shell’s thickness) from the shell’s midsurface to the reference surface containing the element’s nodes . Positive values of the offset are in the positive normal direction . When the offset is set equal to 0.5, the top surface of the shell is the reference surface. When the offset is set equal to −0.5, the bottom surface is the reference surface. The default offset is 0, which indicates that the middle surface of the shell is the reference surface. You can specify an offset value that is greater in magnitude than 0.5. However, this technique should be used with caution in regions of high curvature. All kinematic quantities, including the element’s area, are calculated relative to the reference surface, which may lead to a surface area integration error, affecting the stiffness and mass of the shell. In an Abaqus/Standard analysis a spatially varying offset can be defined for conventional shells using a distribution (“Distribution definition,” Section 2.8.1). The distribution used to define the shell offset must have a default value. The default offset is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution. An offset to the shell’s top surface is illustrated in Figure 29.6.5–2. The shell offset value is ignored for continuum shell elements. Input File Usage: Use the following option to specify a value for the shell offset: *SHELL SECTION, OFFSET=offset The OFFSET parameter accepts a value, a label (SPOS or SNEG), or in an Abaqus/Standard analysis the name of a distribution that is used to define a spatially varying offset. Specifying SPOS is equivalent to specifying a value of 0.5; specifying SNEG is equivalent to specifying a value of −0.5. SPOS SPOS SPOS SNEG SNEG SNEG Mid surface a) OFFSET= 0 Reference surface and midsurface are coincident b) OFFSET= −0.5 (SNEG) Reference surface is the bottom surface c) OFFSET= +0.5 (SPOS) Reference surface is the top surface Figure 29.6.5–2 Schematic of shell offset for an offset value of 0.5. Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: During analysis; Offset: choose a reference surface, specify an offset, or select a scalar discrete field Use the following option for a shell section assignment: Property module: Assign→Section: select regions: Section: select a homogeneous or composite shell section: Definition: select a reference surface, specify an offset, or select a scalar discrete field Defining a variable thickness for conventional shells using distributions You can define a spatially varying thickness for conventional shells using a distribution (“Distribution definition,” Section 2.8.1). The thickness of continuum shell elements is defined by the element geometry. For composite shells the total thickness is defined by the distribution, and the layer thicknesses you specify are scaled proportionally such that the sum of the layer thicknesses is equal to the total thickness (including spatially varying layer thicknesses defined with a distribution). The distribution used to define shell thickness must have a default value. The default thickness is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution. If the shell thickness is defined for a shell section with a distribution, nodal thicknesses cannot be used for that section definition. Input File Usage: Use the following option to define a spatially varying thickness: *SHELL SECTION, SHELL THICKNESS=distribution name Abaqus/CAE Usage: Use the following option for a conventional shell composite layup: Property module: composite layup editor: Section integration: During analysis; Shell Parameters: Shell thickness: Element distribution: select an analytical field or an element-based discrete field Use the following option for a homogeneous shell section: Property module: shell section editor: Section integration: During analysis; Basic: Shell thickness: Element distribution: select an analytical field or an element-based discrete field Use the following option for a composite shell section: Property module: shell section editor: Section integration: During analysis; Advanced: Shell thickness: Element distribution: select an analytical field or an element-based discrete field Defining a variable nodal thickness for conventional shells You can define a conventional shell with continuously varying thickness by specifying the thickness of the shell at the nodes. The thickness of continuum shell elements is defined by the element geometry. If you indicate that the nodal thicknesses will be specified, for homogeneous shells any constant shell thickness you specify will be ignored, and the shell thickness will be interpolated from the nodes. The thickness must be defined at all nodes connected to the element. For composite shells the total thickness is interpolated from the nodes, and the layer thicknesses you specify are scaled proportionally such that the sum of the layer thicknesses is equal to the total thickness (including spatially varying layer thicknesses defined with a distribution). If the shell thickness is defined for a shell section with a distribution, nodal thicknesses cannot be used for that section definition. However, if nodal thicknesses are used, you can still use distributions to define spatially varying thicknesses on the layers of conventional shell elements. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *NODAL THICKNESS *SHELL SECTION, NODAL THICKNESS Use the following option for a conventional shell composite layup: Property module: composite layup editor: Section integration: During analysis; Shell Parameters: Nodal distribution: select an analytical field or a node-based discrete field Use the following option for a homogeneous shell section: Property module: shell section editor: Section integration: During analysis; Basic: Nodal distribution: select an analytical field or a node-based discrete field Use the following option for a composite shell section: Property module: shell section editor: Section integration: During analysis; Advanced: Nodal distribution: select an analytical field or a node-based discrete field Defining the Poisson strain in shell elements in the thickness direction Abaqus allows for a possible uniform change in the shell thickness in a geometrically nonlinear analysis . The Poisson’s strain can be based on a fixed section Poisson’s ratio, either user specified or computed by Abaqus based on the elastic portion of the material definition. Alternatively, in Abaqus/Explicit the Poisson strain can be integrated through the section based on the material response at the individual material points in the section. By default, Abaqus/Standard computes the Poisson’s strain using a fixed section Poisson’s ratio of 0.5; Abaqus/Explicit uses the material response to compute the Poisson’s strain. See “Finite-strain shell element formulation,” Section 3.6.5 of the Abaqus Theory Manual, for details regarding the underlying formulation. Input File Usage: Use the following option to specify a value for the effective Poisson’s ratio: *SHELL SECTION, POISSON= Use the following option to cause the shell thickness to change based on the element initial elastic material definition: *SHELL SECTION, POISSON=ELASTIC Use the following option (available only in Abaqus/Explicit) to cause the thickness direction strain under plane stress conditions to be a function of the membrane strains and the in-plane material properties: Abaqus/CAE Usage: *SHELL SECTION, POISSON=MATERIAL Use the following option for a composite layup: Property module: composite layup editor: Section integration: During analysis; Shell Parameters: Section Poisson's ratio: Use analysis default or Specify value: Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: During analysis; Advanced: Section Poisson's ratio: Use analysis default or Specify value: You cannot specify a shell thickness direction behavior based on the initial elastic material definition in Abaqus/CAE. Defining the thickness modulus in continuum shell elements The thickness modulus is used in computing the stress in the thickness direction . Abaqus computes a thickness modulus value by default based on the elastic portion of the material definitions in the initial configuration. Alternatively, you can provide a value. If the material properties are unavailable during the preprocessing stage of input; for example, when the material behavior is defined by the fabric material model or user subroutine UMAT or VUMAT, you must specify the effective thickness modulus directly. Input File Usage: Use the following option to define an effective thickness modulus directly: Abaqus/CAE Usage: *SHELL SECTION, THICKNESS MODULUS= Use the following option for a composite layup: Property module: composite layup editor: Section integration: During analysis; Shell Parameters: Thickness modulus specify the thickness properties directly to Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: During analysis; Advanced: Thickness modulus to specify the thickness properties directly You cannot specify a shell thickness direction behavior based on the initial elastic material definition in Abaqus/CAE. Defining the transverse shear stiffness You can provide nondefault values of the transverse shear stiffness. You must specify the transverse shear stiffness in Abaqus/Standard if the section is used with shear flexible shells and the material definitions used in the shell section do not include linear elasticity (“Linear elastic behavior,” Section 22.2.1). See “Shell section behavior,” Section 29.6.4, for more information about transverse shear stiffness. If you do not specify the transverse shear stiffness values, Abaqus will integrate through the section to determine them. The transverse shear stiffness is precalculated based on the initial elastic material properties, as defined by the initial temperature and predefined field variables evaluated at the midpoint of each material layer. This stiffness is not recalculated during the analysis. For most shell sections, including layered composite or sandwich shell sections, Abaqus will calculate the transverse shear stiffness values required in the element formulation. You can override these default values. The default shear stiffness values are not calculated in some cases if estimates of shear moduli are unavailable during the preprocessing stage of input; for example, when the material behavior is defined by the fabric material model or by user subroutine UMAT, UHYPEL, UHYPER, or VUMAT. You must define the transverse shear stiffnesses in such cases except for STRI3 elements. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *SHELL SECTION *TRANSVERSE SHEAR STIFFNESS Use the following option for a composite layup: Property module: composite layup editor: Section integration: During analysis; Shell Parameters: toggle on Specify transverse shear Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: During analysis; Advanced: toggle on Specify transverse shear Specifying the order of accuracy in the Abaqus/Explicit shell element formulation In Abaqus/Explicit you can specify second-order accuracy in the shell element formulation. See “Section controls,” Section 27.1.4, for more information. Input File Usage: *SHELL SECTION, CONTROLS=name Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Element Controls Defining density for conventional shells You can define additional mass per unit area for conventional shell elements directly in the section definition. This functionality is similar to the more general functionality of defining a nonstructural mass contribution The only difference between the two definitions is that the nonstructural mass contributes to the rotary inertia terms about the midsurface while the additional mass defined in the section definition does not. Input File Usage: Use the following option to define the density directly: Abaqus/CAE Usage: *SHELL SECTION, ELSET=name, DENSITY= Use the following option for a composite layup: Property module: composite layup editor: Section integration: During analysis; Shell Parameters: toggle on Density, and enter Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: During analysis; Advanced: toggle on Density, and enter Specifying nondefault hourglass control parameters for reduced-integration shell elements You can specify a nondefault hourglass control formulation or scale factors for elements that use reduced integration. See “Section controls,” Section 27.1.4, for more information. In Abaqus/Standard the nondefault enhanced hourglass control formulation is available only for S4R and SC8R elements. When the enhanced hourglass control formulation is used with composite shells, the average value of the bulk material properties and the minimum value of the shear material properties over all the layers are used for computing the hourglass forces and moments. In Abaqus/Standard you can modify the default values for hourglass control stiffness based on the default total stiffness approach for elements that use reduced integration and define a scaling factor for the stiffness associated with the drill degree of freedom (rotation about the surface normal) for elements that use six degrees of freedom at a node. The stiffness associated with the drill degree of freedom is the average of the direct components of the transverse shear stiffness multiplied by a scaling factor. In most cases the default scaling factor is appropriate for constraining the drill rotation to follow the in-plane rotation of the element. If an additional scaling factor is defined, the additional scaling factor should not increase or decrease the drill stiffness by more than a factor of 100.0 for most typical applications. Usually, a scaling factor between 0.1 and 10.0 is appropriate. Continuum shell elements do not use a drill stiffness; hence, the scale factor is ignored. There are no hourglass stiffness factors or scale factors for hourglass stiffness for the nondefault enhanced hourglass control formulation. You can define the scale factor for the drill stiffness for the nondefault enhanced hourglass control formulation. Input File Usage: Use both of the following options to specify a nondefault hourglass control formulation or scale factors for reduced-integration elements: *SECTION CONTROLS, NAME=name *SHELL SECTION, CONTROLS=name Use both of the following options in Abaqus/Standard to modify the default values for hourglass control stiffness based on the default total stiffness approach for reduced-integration elements and to define a scaling factor for the stiffness associated with the drill degree of freedom (rotation about the surface normal) for six degree of freedom elements: *SHELL SECTION *HOURGLASS STIFFNESS Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Element Controls Specifying temperature and field variables You can specify temperatures and field variables for conventional shell elements by defining the value at the reference surface of the shell and the gradient through the shell thickness or by defining the values at equally spaced points through each layer of the shell’s thickness. You can specify a temperature gradient only for elements without temperature degrees of freedom. The temperatures and field variables for continuum shell elements are defined at the nodes and then interpolated to the section points. The actual values of the temperatures and field variables are specified as either predefined fields or initial conditions . If temperature is to be read as a predefined field from the results file or the output database file of a previous analysis, the temperature must be defined at equally spaced points through each layer of the thickness. In addition, the results file must be modified so that the field variable data are stored in record 201. See “Predefined fields,” Section 33.6.1, for additional details. Defining the value at the reference surface and the gradient through the thickness You can define the temperature or predefined field by its magnitude on the reference surface of the shell and the gradient through the thickness. If only one value is given, the magnitude will be constant through the thickness. Input File Usage: Use the following option to specify that the temperatures or predefined fields are defined by a gradient: *SHELL SECTION Use any of the following options to specify the actual values of the temperatures or predefined fields: *TEMPERATURE *FIELD *INITIAL CONDITIONS, TYPE=TEMPERATURE *INITIAL CONDITIONS, TYPE=FIELD Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: During analysis; Shell Parameters; Temperature variation: Linear through thickness Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: During analysis: Advanced; Temperature variation: Linear through thickness Only initial temperatures and predefined temperature fields are supported in Abaqus/CAE. Load module: Create Predefined Field: Step: initial_step or analysis_step: choose Other for the Category and Temperature for the Types for Selected Step Defining the values at equally spaced points through the thickness Alternatively, you can define the temperature and field variable values at equally spaced points through the thickness of a shell or of each layer of a composite shell. For a sequentially coupled thermal-stress analysis in Abaqus/Standard, the number (n) of equally spaced points through the thickness of a layer is an odd number when temperature values are obtained from the results file or the output database file generated by a previous Abaqus/Standard heat transfer analysis (since only Simpson’s rule can be used for integration through the section in heat transfer analysis). n may be even or odd if the values are supplied from some other source. In either case Abaqus/Standard interpolates linearly between the two closest defined temperature points to find the temperature values at the section points. The number of predefined field points through each layer, n, must be the same as the number of integration points used through the same layer in the analysis from which the temperatures are obtained. This requirement implies that in the previous analysis each of the layers must have the same number of integration points. You specify in the shell section and variable value for a given node or node set. ( temperature or field variable values, where =1, you specify > 1) is the value of n. For is the number of layers one temperature or field Input File Usage: Use the following option to specify that the temperatures or predefined fields are defined at equally spaced points: *SHELL SECTION, TEMPERATURE=n Use any of the following options to specify the actual values of the temperatures or predefined fields: *TEMPERATURE *FIELD *INITIAL CONDITIONS, TYPE=TEMPERATURE *INITIAL CONDITIONS, TYPE=FIELD Use the following option for a composite layup: Abaqus/CAE Usage: Property module: composite layup editor: Section integration: During analysis; Shell Parameters; Temperature variation: Piecewise linear over n values Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: During analysis: Advanced; Temperature variation: Piecewise linear over n values Only initial temperatures and predefined temperature fields are supported in Abaqus/CAE. Load module: Create Predefined Field: Step: initial_step or analysis_step: choose Other for the Category and Temperature for the Types for Selected Step Example An example of this scheme is illustrated in Figure 29.6.5–3 and Figure 29.6.5–4. The following Abaqus/Standard heat transfer shell section definition corresponds to this example: *SHELL SECTION, COMPOSITE , 3, MAT1, ORI1 , 3, MAT2, ORI2 , 3, MAT3, ORI3 Composite shell section 9 layer 3 t3 7 layer 2 t2 layer 1 t1 ⎫⎫⎬⎬⎭⎭ Use default of 3 section points per layer ⎫⎫⎬⎬⎭⎭ Specify 3 temperature points per layer, shared at layer intersections, 7 total nT = 3 nl = 3 1 + nl (nT -1) = 7 Figure 29.6.5–3 Defining temperature values at n equally spaced points using Simpson’s rule. This creates degrees of freedom 11–17 in the heat transfer analysis. Temperatures corresponding to these degrees of freedom are then read into the stress analysis at the temperature points shown and interpolated to the section points shown. Defining a continuous temperature field In Abaqus/Standard if an element with temperature degrees of freedom other than a shell abuts the bottom surface of a shell element with temperature degrees of freedom, the temperature field is made continuous when the elements share nodes. If another element with temperature degrees of freedom abuts the top surface, separate nodes must be used and a linear constraint equation (“Linear constraint equations,” Section 34.2.1) must be used to constrain the temperatures to be the same (that is, to give the same value to the top surface degree of freedom on the shell and degree of freedom 11 on the other element). For the same reason you must be careful if a different number of temperature points is used in adjacent shell elements. For compatibility MPCs (“General multi-point constraints,” Section 34.2.2) or equation constraints are also needed in this case. composite shell section layer 3 t3 layer 2 t2 layer 1 t1 ⎫⎫⎬⎬⎭⎭ Use default of 2 section points per layer ⎫⎫⎬⎬⎭⎭ Specify 3 temperature points per layer, shared at layer intersections, 7 total nT = 3 nl = 3 1 + nl (nT -1) = 7 Figure 29.6.5–4 Defining temperature values at n equally spaced points using Gauss integration. In Abaqus/Explicit since no thermal MPCs and no thermal equation constraints are available for degrees of freedom greater than 11, care must be taken when using a different number of temperature points in adjacent shell elements. This should usually have a localized effect on the temperature distribution, but it may affect the overall solution for the cases in which the temperature gradient through the thickness is significant. In both Abaqus/Standard and Abaqus/Explicit be careful in the models in which the shell’s normals are reversed. In this case the temperature at the bottom of the shell becomes the temperature at the top of the adjacent shell. This may have a small impact on the overall solution for the cases in which the thermal gradient through the thickness is negligible and the temperature variation is mainly in plane. However, if the temperature gradient through the thickness is significant, it may lead to incorrect results. Output In an Abaqus/Standard stress analysis temperature output at the section points can be obtained using the element variable TEMP. If the temperature values were specified at equally spaced points through the thickness, output at the temperature points can be obtained in an Abaqus/Standard stress analysis, as in a heat transfer analysis, by using the nodal variable NTxx. This nodal output variable is also available in Abaqus/Explicit for coupled temperature-displacement analyses. The nodal variable NTxx should not be used for output at the temperature points with the default gradient method. In this case output variable NT should be requested; NT11 (the reference temperature value) and NT12 (the temperature gradient) will be output automatically. For continuum shell elements, there is only NT11; all other NTxx are irrelevant. Other output variables that are relevant for shells are listed in each of the library sections describing the specific shell elements. For example, stresses, strains, section forces and moments, average section stresses, section strains, etc. can be output. The section moments are calculated relative to the reference surface. 29.6.6 USING A GENERAL SHELL SECTION TO DEFINE THE SECTION BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Shell elements: overview,” Section 29.6.1 • “Shell section behavior,” Section 29.6.4 • “UGENS,” Section 1.1.34 of the Abaqus User Subroutines Reference Manual • *DISTRIBUTION • *HOURGLASS STIFFNESS • *SHELL GENERAL SECTION • *TRANSVERSE SHEAR STIFFNESS • “Creating homogeneous shell sections,” Section 12.13.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating composite shell sections,” Section 12.13.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating general shell stiffness sections,” Section 12.13.10 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Manual Overview A general shell section: • is used when numerical integration through the thickness of the shell is not required; • can be associated with linear elastic material behavior or, in Abaqus/Standard, can invoke user subroutine UGENS to define nonlinear section properties in terms of forces and moments; • can be used to model an equivalent shell section for some more complex geometry (for example, replacing a corrugated shell with an equivalent smooth plate for global analysis); and • cannot be used with heat transfer and coupled temperature-displacement shells. Defining the shell section behavior A general shell section can be defined as follows: • The section response can be specified by associating the section with a material definition or, in the case of a composite shell, with several different material definitions. • The section properties can be specified directly. • In Abaqus/Standard the section response can be programmed in user subroutine UGENS. Specifying the equivalent section properties by defining the layers (thickness, material, and orientation) You can define the shell section’s mechanical response by specifying the thickness; the material reference; and the orientation of the section or, for a composite shell, the orientation of each of its layers. Abaqus will determine the equivalent section properties. You must associate the section behavior with a region of your model. The linear elastic material behavior is defined with a material definition (“Material data definition,” Section 21.1.2), which may contain linear elastic behavior (“Linear elastic behavior,” Section 22.2.1) and thermal expansion behavior (“Thermal expansion,” Section 26.1.2). The density (“Density,” Section 21.2.1) and damping (“Material damping,” Section 26.1.1) behavior can also be specified as described below; in Abaqus/Explicit the density of the material must be defined. However, no nonlinear material properties, such as plastic behavior, can be included since Abaqus will precompute the section response and will not update that response during the analysis. Dependence of the linear elastic material behavior on temperature or predefined field variables is not allowed. The shell section response is defined by No temperature-dependent scaling of the modulus is included. The section forces and moments caused by thermal strains, , vary linearly with temperature and are defined by are the generalized stresses caused by a fully constrained unit temperature rise that result from where the user-defined thermal expansion, is the initial (stress-free) temperature at this point in the shell (defined by the initial nodal temperatures given as initial conditions; see “Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1). is the temperature, and Defining a shell made of a single linear elastic material To define a shell made of a single linear elastic material, you refer to the name of a material definition (“Material data definition,” Section 21.1.2) as described above. Optionally, you can define an orientation definition to be used with the section (“Orientations,” Section 2.2.5). A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be assigned to the shell In addition, you specify the shell thickness as part of the section definition. For section definition. continuum shell elements the specified thickness is used to estimate certain section properties, such as hourglass stiffness, that are later computed from the element geometry. You must associate this section behavior with a region of your model. You can redefine the thickness, offset, section stiffness, and material orientation specified in the section definition on an element-by-element basis. See “Distribution definition,” Section 2.8.1. If the orientation definition assigned to a shell section definition is defined with distributions, spatially varying local coordinate systems are applied to all shell elements associated with the shell section. A default local coordinate system (as defined by the distributions) is applied to any shell element that is not specifically included in the associated distribution. Input File Usage: *SHELL GENERAL SECTION, ELSET=name, MATERIAL=name, ORIENTATION=name Abaqus/CAE Usage: where the ELSET parameter refers to a set of shell elements. Property module: Create Section: select Shell as the section Category and Homogeneous as the section Type: Section integration: Before analysis; Basic: Material: name Assign→Material Orientation: select regions Assign→Section: select regions Defining a shell made of layers with different linear elastic material behaviors You can define a shell made of layers with different linear elastic material behaviors. Optionally, you can define an orientation definition to be used with the section (“Orientations,” Section 2.2.5). A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be assigned to the shell section definition. You specify the layer thickness; the name of the material forming this layer (as described above); and the orientation angle, , (in degrees) measured positive counterclockwise relative to the specified section orientation definition. Spatially varying orientation angles can be specified on a layer using distributions (“Distribution definition,” Section 2.8.1). If either of the two local directions from the specified section orientation is not in the surface of the shell, is applied after the section orientation has been projected onto the shell surface. If you do not specify a section orientation, is measured relative to the default shell local directions . The order of the laminated shell layers with respect to the positive direction of the shell normal is defined by the order in which the layers are specified. For continuum shell elements the thickness is determined from the element geometry and may vary through the model for a given section definition. Hence, the specified thicknesses are only relative thicknesses for each layer. The actual thickness of a layer is the element thickness times the fraction of the total thickness that is accounted for by each layer. The thickness ratios for the layers need not be given in physical units, nor do the sum of the layer relative thicknesses need to add to one. The specified shell thickness is used to estimate certain section properties, such as hourglass stiffness, that are later computed from the element geometry. Spatially varying thicknesses can be specified on the layers of conventional shell elements (not continuum shell elements) using distributions (“Distribution definition,” Section 2.8.1). A distribution that is used to define layer thickness must have a default value. The default layer thickness is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution. You must associate this section behavior with a region of your model. If the orientation definition assigned to a shell section definition is defined with distributions, spatially varying local coordinate systems are applied to all shell elements associated with the shell section. A default local coordinate system (as defined by the distributions) is applied to any shell element that is not specifically included in the associated distribution. Unless your model is relatively simple, you will find it increasingly difficult to define your model using composite shell sections as you increase the number of layers and as you assign different sections to different regions. It can also be cumbersome to redefine the sections after you add new layers or remove or reposition existing layers. To manage a large number of layers in a typical composite model, you may want to use the composite layup functionality in Abaqus/CAE. For more information, see Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Manual. Input File Usage: *SHELL GENERAL SECTION, ELSET=name, COMPOSITE, ORIENTATION=name where the ELSET parameter refers to a set of shell elements. Abaqus/CAE Usage: Abaqus/CAE uses a composite layup or a composite shell section to define a shell made of layers with different linear elastic material behaviors. Use the following option for a composite layup: Property module: Create Composite Layup: select Conventional Shell or Continuum Shell as the Element Type: Section integration: Before analysis: specify orientations, regions, and materials Use the following options for a composite shell section: Property module: Create Section: select Shell as the section Category and Composite as the section Type: Section integration: Before analysis Assign→Material Orientation: select regions Assign→Section: select regions Specifying the equivalent section properties directly for conventional shells You can define the section’s mechanical response by specifying the general section stiffness and thermal expansion response— , , as defined below—directly. Since this method then provides the complete specification of the section’s mechanical response, no material reference is needed. Optionally, you can define , the reference temperature for thermal expansion. and , You must associate this section behavior with a region of your model. In this case the shell section response is defined by are the forces and moments on the shell section (membrane forces per unit length, bending moments per unit length); are the generalized section strains in the shell (reference surface strains and curvatures); is the section stiffness matrix; is a scaling modulus, which can be used to introduce temperature dependence of the cross-section stiffness; and and field-variable 29.6.6–4 are the section forces and moments (per unit length) caused by thermal strains. These thermal forces and moments in the shell are generated according to the formula where is a scaling factor (the “thermal expansion coefficient”); is the initial (stress-free) temperature at this point in the shell, defined by the initial nodal temperatures given as initial conditions (“Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 33.2.1); and are the user-specified generalized section forces and moments (per unit length) caused by a fully constrained unit temperature rise. If the coefficient of thermal expansion, needed. Note the distinction between temperature, . is not , is not a function of temperature, the value of , the reference value used in defining , and the stress-free initial In these equations the order of the terms is that is, the direct membrane terms come first, then the shear membrane term, then the direct and shear bending terms, with six terms in all. Engineering measures of shear membrane strain ( ) and twist ( ) are used in Abaqus. This method of defining the shell section properties cannot be used with variable thickness shells or continuum shell elements. See “Laminated composite shells: buckling of a cylindrical panel with a circular hole,” Section 1.2.2 of the Abaqus Example Problems Manual, for more information. The stiffness matrix, , can be defined as a constant stiffness for the section or as a spatially varying stiffness by referring to a distribution (“Distribution definition,” Section 2.8.1). If a spatially varying stiffness is used, the distribution must have a default stiffness defined. The default stiffness is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution. Input File Usage: *SHELL GENERAL SECTION, ELSET=name, ZERO= where the ELSET parameter refers to a set of shell elements. Abaqus/CAE Usage: Property module: Create Section: select Shell as the section Category and General shell stiffness as the section Type Assign→Section: select regions Specifying the section properties in user subroutine UGENS In Abaqus/Standard you can define the section response in user subroutine UGENS for the more general case where the section response may be nonlinear. User subroutine UGENS is particularly useful if the nonlinear behavior of the section involves geometric as well as material nonlinearity, such as may occur due to section collapse. If only nonlinear material behavior is present, it is simpler to use a shell section integrated during the analysis with the appropriate nonlinear material model. You must specify a constant section thickness as part of the section definition or a continuously varying thickness by defining the thickness at the nodes as described below. Even though the section’s mechanical behavior is defined in user subroutine UGENS, the thickness of the shell section is required for calculation of the hourglass control stiffness. You must associate this section behavior with a region of your model. Abaqus/Standard calls user subroutine UGENS for each integration point at each iteration of every increment. The subroutine provides the section state at the start of the increment (section forces and moments, ; solution-dependent state variables; temperature; and any predefined field variables); the increments in temperature and predefined field variables; the generalized section strain increments, ; generalized section strains, ; and the time increment. The subroutine must perform two functions: it must update the forces, the moments, and the solution-dependent state variables to their values at the end of the increment; and it must provide the section stiffness matrix, . The complete section response, including the thermal expansion effects, must be programmed in the user subroutine. You should ensure that the strain increment is not used or changed in user subroutine UGENS for linear perturbation analyses. For this case the quantity is undefined. This method of defining the shell section properties cannot be used with continuum shell elements. *SHELL GENERAL SECTION, ELSET=name, USER Input File Usage: Abaqus/CAE Usage: where the ELSET parameter refers to a set of shell elements. User subroutine UGENS is not supported in Abaqus/CAE. Defining whether or not the section stiffness matrices are symmetric If the section stiffness matrices are not symmetric, you can specify that Abaqus/Standard should use its unsymmetric equation solution capability . Input File Usage: Abaqus/CAE Usage: *SHELL GENERAL SECTION, ELSET=name, USER, UNSYMM User subroutine UGENS is not supported in Abaqus/CAE. Defining the section properties Any number of constants can be defined to be used in determining the section behavior. You can specify the number of integer property values required, m, and the number of real (floating point) property values required, n; the total number of values required is the sum of these two numbers. The default number of integer property values required is 0, and the default number of real property values required is 0. Integer property values can be used inside user subroutine UGENS as flags, indices, counters, etc. Examples of real (floating point) property values are material properties, geometric data, and any other information required to calculate the section response in UGENS. The property values are passed into user subroutine UGENS each time the subroutine is called. Input File Usage: *SHELL GENERAL SECTION, ELSET=name, USER, I PROPERTIES=m, PROPERTIES=n To define the property values, enter all floating point values on the data lines first, followed immediately by the integer values. Eight values can be entered per line. User subroutine UGENS is not supported in Abaqus/CAE. Abaqus/CAE Usage: Defining the number of solution-dependent variables that must be stored for the section You can define the number of solution-dependent state variables that must be stored at each integration point within the section. There is no restriction on the number of variables associated with a user-defined section. The default number of variables is 1. Examples of such variables are plastic strains, damage variables, failure indices, user-defined output quantities, etc. These solution-dependent state variables can be calculated and updated in user subroutine UGENS. Input File Usage: Abaqus/CAE Usage: *SHELL GENERAL SECTION, ELSET=name, USER, VARIABLES=n User subroutine UGENS is not supported in Abaqus/CAE. Idealizing the section response Idealizations allow you to modify the stiffness coefficients in a shell section based on assumptions about the shell’s makeup or expected behavior. The following idealizations are available for general shell sections: • Retain only the membrane stiffness for shells whose predominant response will be in-plane stretching. • Retain only the bending stiffness for shells whose predominant response will be pure bending. • Ignore the effects of the material layer stacking sequence for composite shells. The membrane stiffness and bending stiffness idealizations can be applied to homogeneous shell sections, composite shell sections, or shell sections with the stiffness coefficients specified directly. The idealization to ignore stacking effects can be applied only to composite shell sections. Idealizations modify the shell general stiffness coefficients after they have been computed normally, including the effects of offset. • If you use any idealization, all membrane-bending coupling terms are set to zero. • If you retain only the membrane stiffness, off-diagonal terms of the bending submatrix are set to zero, and diagonal bending terms are set to 1 × 10−6 times the largest diagonal membrane coefficient. • If you retain only the bending stiffness, off-diagonal terms of the membrane submatrix are set to zero, and diagonal membrane terms are set to 1 × 10−6 times the largest diagonal bending coefficient. • If you ignore the material layer stacking sequence in a composite shell, each term of the bending submatrix is set equal to T 2 /12 times the corresponding membrane submatrix term, where T is the total thickness of the shell. Input File Usage: Use the following option to retain only the membrane stiffness: *SHELL GENERAL SECTION, MEMBRANE ONLY Use the following option to retain only the bending stiffness: *SHELL GENERAL SECTION, BENDING ONLY Use the following option to ignore the effects of the layer stacking sequence: *SHELL GENERAL SECTION, COMPOSITE, SMEAR ALL LAYERS Multiple idealization options can be used on the same general shell section. Abaqus/CAE Usage: Use any of the following options to apply an idealization to a shell section: Property module: Homogeneous shell section editor: Section integration: Before analysis; Basic: Idealization: Membrane only or Bending only Property module: Composite shell section editor: Section integration: Before analysis; Basic: Idealization: Membrane only, Bending only, or Smear all layers Property module: Shell (conventional or continuum) composite layup editor: Section integration: Before analysis; Basic: Idealization: Membrane only, Bending only, or Smear all layers You cannot apply multiple idealizations to the same shell section in Abaqus/CAE, and you cannot apply idealizations to a general shell stiffness section. Defining a shell offset value for conventional shells You can define the distance (measured as a fraction of the shell’s thickness) from the shell’s midsurface to the reference surface containing the element’s nodes . Positive values of the offset are in the positive normal direction . When the offset is set equal to 0.5, the top surface of the shell is the reference surface. When the offset is set equal to −0.5, the bottom surface is the reference surface. The default offset is 0, which indicates that the middle surface of the shell is the reference surface. You can specify an offset value that is greater in magnitude than 0.5. However, this technique should be used with caution in regions of high curvature. All kinematic quantities, including the element’s area, are calculated relative to the reference surface, which may lead to a surface area integration error, affecting the stiffness and mass of the shell. In an Abaqus/Standard analysis a spatially varying offset can be defined for conventional shells using a distribution (“Distribution definition,” Section 2.8.1). The distribution used to define the shell offset must have a default value. The default offset is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution. An offset to the shell’s top surface is illustrated in Figure 29.6.6–1. SPOS SPOS SPOS SNEG SNEG SNEG Mid surface a) OFFSET= 0 Reference surface and midsurface are coincident b) OFFSET= −0.5 (SNEG) Reference surface is the bottom surface c) OFFSET= +0.5 (SPOS) Reference surface is the top surface Figure 29.6.6–1 Schematic of shell offset for an offset value of 0.5. A shell offset value can be specified only if a material definition is referenced or a composite shell section is defined. The shell offset value is ignored when the section definition is applied to continuum shell elements. Input File Usage: Use the following option to specify a value for the shell offset: *SHELL GENERAL SECTION, OFFSET=offset The OFFSET parameter accepts a value, a label (SPOS or SNEG), or in an Abaqus/Standard analysis the name of a distribution that is used to define a spatially varying offset. Specifying SPOS is equivalent to specifying a value of 0.5; specifying SNEG is equivalent to specifying a value of −0.5. Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: Before analysis; Offset: choose a reference surface, specify an offset, or select a scalar discrete field Use the following option for a shell section assignment: Property module: Assign→Section: select regions: Section: select a homogeneous or composite shell section: Definition: select a reference surface, specify an offset, or select a scalar discrete field Defining a variable thickness for conventional shells using distributions You can define a spatially varying thickness for conventional shells using a distribution (“Distribution definition,” Section 2.8.1). The thickness of continuum shell elements is defined by the element geometry. For composite shells the total thickness is defined by the distribution, and the layer thicknesses you specify are scaled proportionally such that the sum of the layer thicknesses is equal to the total thickness (including spatially varying layer thicknesses defined with a distribution). The distribution used to define shell thickness must have a default value. The default thickness is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution. If the shell thickness is defined for a shell section with a distribution, nodal thicknesses cannot be used for that section definition. Input File Usage: Use the following option to define a spatially varying thickness: Abaqus/CAE Usage: *SHELL SECTION, SHELL THICKNESS=distribution name Use the following option for a conventional shell composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: Shell thickness: Element distribution: select an analytical field or an element-based discrete field Use the following option for a homogeneous shell section: Property module: shell section editor: Section integration: Before analysis; Basic: Shell thickness: Element distribution: select an analytical field or an element-based discrete field Use the following option for a composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: Shell thickness: Element distribution: select an analytical field or an element-based discrete field Defining a variable nodal thickness for conventional shells You can define a conventional shell with continuously varying thickness by specifying the thickness of the shell at the nodes. This method can be used only if the section is defined in terms of material properties; it cannot be used if the section behavior is defined by specifying the equivalent section properties directly. For continuum shell elements a continuously varying thickness can be defined through the element nodal geometry; hence, the nodal thickness is not meaningful. If you indicate that the nodal thicknesses will be specified, for homogeneous shells any constant shell thickness you specify will be ignored, and the shell thickness will be interpolated from the nodes. The thickness must be defined at all nodes connected to the element. For composite shells the total thickness is interpolated from the nodes, and the layer thicknesses you specify are scaled proportionally such that the sum of the layer thicknesses is equal to the total thickness (including spatially varying layer thicknesses defined with a distribution). If the shell thickness is defined for a shell section with a distribution, nodal thicknesses cannot be used for that section definition. However, if nodal thicknesses are used, you can still use distributions to define spatially varying thicknesses on the layers of conventional shell elements. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *NODAL THICKNESS *SHELL GENERAL SECTION, NODAL THICKNESS Use the following option for a conventional shell composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: Nodal distribution: select an analytical field or a node-based discrete field Use the following option for a homogeneous shell section: Property module: shell section editor: Section integration: Before analysis; Basic: Nodal distribution: select an analytical field or a node-based discrete field Use the following option for a composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: Nodal distribution: select an analytical field or a node-based discrete field Defining the Poisson strain in shell elements in the thickness direction Abaqus allows for a possible uniform change in the shell thickness in a geometrically nonlinear analysis . The Poisson’s strain is based on a fixed section Poisson’s ratio, either user specified or computed by Abaqus based on the elastic portion of the material definition. By default, Abaqus computes the Poisson’s strain using a fixed section Poisson’s ratio of 0.5. Input File Usage: Use the following option to specify a value for the effective Poisson’s ratio: *SHELL GENERAL SECTION, POISSON= Use the following option to cause the shell thickness to change based on the initial elastic properties of the material: *SHELL GENERAL SECTION, POISSON=ELASTIC Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: Section Poisson's ratio: Use analysis default or Specify value: Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: Section Poisson's ratio: Use analysis default or Specify value: You cannot specify a shell thickness direction behavior based on the initial elastic material definition in Abaqus/CAE. Defining the thickness modulus in continuum shell elements The thickness modulus is used in computing the stress in the thickness direction . Abaqus computes a thickness modulus value by default based on the elastic portion of the material definitions in the initial configuration. Alternatively, you can provide a value. If the material properties are unavailable during the preprocessing stage of input; for example, when the material behavior is defined by the fabric material model or user subroutine UMAT or VUMAT, you must specify the effective thickness modulus directly. Input File Usage: Abaqus/CAE Usage: Use the following option to define an effective thickness modulus directly: *SHELL GENERAL SECTION, THICKNESS MODULUS= Use the following option for a composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: Thickness modulus specify the thickness properties directly to Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: Thickness modulus specify the thickness properties directly to Defining the transverse shear stiffness You can provide nondefault values of the transverse shear stiffness. You must specify the transverse shear stiffness for shear flexible shells in Abaqus/Standard if the section properties are specified in user subroutine UGENS. If you do not specify the transverse shear stiffness, it will be calculated as described in “Shell section behavior,” Section 29.6.4. Input File Usage: Use both of the following options: *SHELL GENERAL SECTION *TRANSVERSE SHEAR STIFFNESS Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: toggle on Specify transverse shear Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: toggle on Specify transverse shear Defining the initial section forces and moments You can define initial stresses for general shell sections that will be applied as initial section Initial conditions can be specified only for the membrane forces, the bending forces and moments. Initial conditions cannot be prescribed for the transverse shear moments, and the twisting moment. forces. Specifying the order of accuracy in the Abaqus/Explicit shell element formulation In Abaqus/Explicit you can specify second-order accuracy in the shell element formulation. See “Section controls,” Section 27.1.4, for more information. Input File Usage: *SHELL GENERAL SECTION, CONTROLS=name Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Element Controls Specifying nondefault hourglass control parameters for reduced-integration shell elements You can specify a nondefault hourglass control formulation or scale factors for elements that use reduced integration. See “Section controls,” Section 27.1.4, for more information. In Abaqus/Standard the nondefault enhanced hourglass control formulation is available only for S4R and SC8R elements. In Abaqus/Standard you can modify the default values for hourglass control stiffness based on the default total stiffness approach for elements that use hourglass control and define a scaling factor for the stiffness associated with the drill degree of freedom (rotation about the surface normal) for elements that use six degrees of freedom at a node. No default values are available for hourglass control stiffness if the section properties are specified in user subroutine UGENS. Therefore, you must specify the hourglass control stiffness when UGENS is used to specify the section properties for reduced-integration elements. The stiffness associated with the drill degree of freedom is the average of the direct components of the transverse shear stiffness multiplied by a scaling factor. In most cases the default scaling factor is appropriate for constraining the drill rotation to follow the in-plane rotation of the element. If an additional scaling factor is defined, the additional scaling factor should not increase or decrease the drill stiffness by more than a factor of 100.0 for most typical applications. Usually, a scaling factor between 0.1 and 10.0 is appropriate. There are no hourglass stiffness factors or scale factors for hourglass stiffness for the nondefault enhanced hourglass control formulation. You can define the scale factor for the drill stiffness for the nondefault enhanced hourglass control formulation. Input File Usage: Use both of the following options to specify a nondefault hourglass control formulation or scale factors for reduced-integration elements: *SECTION CONTROLS, NAME=name *SHELL GENERAL SECTION, CONTROLS=name Use both of the following options in Abaqus/Standard to modify the default values for hourglass control stiffness based on the default total stiffness approach for reduced-integration elements and to define a scaling factor for the stiffness associated with the drill degree of freedom (rotation about the surface normal) for six degree of freedom elements: *SHELL GENERAL SECTION *HOURGLASS STIFFNESS Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Element Controls Defining density for conventional shells You can define the mass per unit area for conventional shell elements whose section properties are specified directly in terms of the section stiffness (either directly in the section definition or, in Abaqus/Standard, in user subroutine UGENS). The density is required, for example, in a dynamic analysis or for gravity loading. See “Density,” Section 21.2.1, for details. The density is defined as part of the material definition for shells whose section properties include a material definition. This functionality is similar to the more general functionality of defining a nonstructural mass contribution The only difference between the two definitions is that the nonstructural mass contributes to the rotary inertia terms about the midsurface while the additional mass defined in the section definition does not. Input File Usage: Use the following option to define the density directly: *SHELL GENERAL SECTION, ELSET=name, DENSITY= Use the following option in Abaqus/Standard to define the density in user subroutine UGENS: *SHELL GENERAL SECTION, ELSET=name, USER, DENSITY= Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: toggle on Density, and enter Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: toggle on Density, and enter You cannot define the shell section properties in user subroutine UGENS in Abaqus/CAE. Defining damping You can include mass and stiffness proportional damping in a shell section definition. See “Material damping,” Section 26.1.1, for more information about material damping in Abaqus. Specifying temperature and field variables Temperatures and field variables can be specified by defining the value at the reference surface of the shell or by defining the values at the nodes of a continuum shell element. The actual values of the temperatures and field variables are specified as either predefined fields or initial conditions . Output The following output variables are available from Abaqus/Explicit as element output: section forces and moments, section strains, element energies, element stable time increment, and element mass scaling factor. The output that is available from Abaqus/Standard depends on how the section behavior is defined. Output if the section is defined in terms of material properties For shells whose section properties include a material definition (homogeneous or composite), section forces and moments and section strains are available as element output. The section moments are calculated relative to the reference surface. In addition, stress (in-plane and, for certain elements, transverse shear), strain, and orthotropic failure measures can be output. Since the behavior of the material is linear, three section points per layer (the bottom, middle, and top, respectively) are available for output. Stress invariants and principal stresses are not available as output but can be visualized in Abaqus/CAE. Output if the equivalent section properties are specified directly or in UGENS matrix is used to specify the equivalent section properties directly or if user subroutine If the UGENS is used, section point stresses and strains and section strains are not available for output or visualization inAbaqus/CAE; only section forces and moments can be requested for outputor visualized inAbaqus/CAE. THREE-DIMENSIONAL CONVENTIONAL SHELL ELEMENT LIBRARY 3-D CONVENTIONAL SHELL ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Shell elements: overview,” Section 29.6.1 • “Choosing a shell element,” Section 29.6.2 • *NODAL THICKNESS • *SHELL GENERAL SECTION • *SHELL SECTION Overview This section provides a reference to the three-dimensional shell elements available in Abaqus/Standard and Abaqus/Explicit. Element types Stress/displacement elements STRI3(S) 3-node triangular facet thin shell S3 S3R S3RS(E) STRI65(S) S4 S4R S4RS(E) S4RSW(E) S4R5(S) S8R(S) 3-node triangular general-purpose shell, finite membrane strains (identical to element S3R) 3-node triangular general-purpose shell, finite membrane strains (identical to element S3) 3-node triangular shell, small membrane strains 6-node triangular thin shell, using five degrees of freedom per node 4-node general-purpose shell, finite membrane strains 4-node general-purpose shell, membrane strains reduced integration with hourglass control, finite 4-node, reduced integration, shell with hourglass control, small membrane strains 4-node, reduced integration, shell with hourglass control, small membrane strains, warping considered in small-strain formulation 4-node thin shell, reduced integration with hourglass control, using five degrees of freedom per node 8-node doubly curved thick shell, reduced integration S8R5(S) S9R5(S) 8-node doubly curved thin shell, reduced integration, using five degrees of freedom per node 9-node doubly curved thin shell, reduced integration, using five degrees of freedom per node Active degrees of freedom 1, 2, 3, 4, 5, 6 for STRI3, S3R, S3RS, S4, S4R, S4RS, S4RSW, S8R 1, 2, 3 and two in-surface rotations for STRI65, S4R5, S8R5, S9R5 at most nodes 1, 2, 3, 4, 5, 6 for STRI65, S4R5, S8R5, S9R5 at any node that • has a boundary condition on a rotational degree of freedom; • is involved in a multi-point constraint that uses rotational degrees of freedom; • is attached to a beam or to a shell element that uses six degrees of freedom at all nodes (such as S4R, S8R, STRI3, etc.); • is a point where different elements have different surface normals (user-specified normal definitions or normal definitions created by Abaqus because the surface is folded); or • is loaded with moments. Additional solution variables Element type S8R5 has three displacement and two rotation variables at an internally generated midbody node. Heat transfer elements DS3(S) DS4(S) DS6(S) DS8(S) 3-node triangular shell 4-node quadrilateral shell 6-node triangular shell 8-node quadrilateral shell Active degrees of freedom 11, 12, etc. (temperatures through the thickness as described in “Choosing a shell element,” Section 29.6.2) Additional solution variables None. Coupled temperature-displacement elements S3T(S) S3RT 3-node triangular general-purpose shell, finite membrane strains, bilinear temperature in the shell surface (identical to element S3RT) 3-node triangular general-purpose shell, finite membrane strains, bilinear temperature in the shell surface (for Abaqus/Standard it is identical to element S3T ) S4T(S) S4RT 4-node general-purpose shell, finite membrane strains, bilinear temperature in the shell surface 4-node general-purpose shell, membrane strains, bilinear temperature in the shell surface reduced integration with hourglass control, finite S8RT(S) 8-node thick shell, biquadratic displacement, bilinear temperature in the shell surface Active degrees of freedom 1, 2, 3, 4, 5, 6 at all nodes 11, 12, 13, etc. (temperatures through the thickness as described in “Choosing a shell element,” Section 29.6.2) at all nodes for S3T, S3RT, S4T, and S4RT; and at the corner nodes only for S8RT Additional solution variables None. Nodal coordinates required and, optionally for shells with displacement degrees of freedom in Abaqus/Standard, , the direction cosines of the shell normal at the node. Element property definition Input File Usage: Use either of the following options for stress/displacement elements: *SHELL SECTION *SHELL GENERAL SECTION Use the following option for heat transfer or coupled temperature-displacement elements: *SHELL SECTION In addition, use the following option for variable thickness shells: *NODAL THICKNESS Property module: Create Section: select Shell as the section Category and Homogeneous or Composite as the section Type Abaqus/CAE Usage: Element-based loading Distributed loads Distributed loads are available for all elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Body forces, centrifugal loads, and Coriolis forces must be given as force per unit area if the equivalent section properties are specified directly as part of the general shell section definition. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BX BY BZ Body force FL−3 Body force FL−3 Body force FL−3 BXNU Body force FL−3 BYNU Body force FL−3 BZNU Body force FL−3 (give magnitude Body force as force per unit volume) in the global X-direction. (give magnitude Body force as force per unit volume) in the global Y-direction. (give magnitude Body force as force per unit volume) in the global Z-direction. as per force force (give Nonuniform body magnitude unit volume) in the global X-direction, via with magnitude user in subroutine VDLOAD Abaqus/Standard in Abaqus/Explicit. supplied DLOAD and as per force force (give Nonuniform body magnitude unit volume) in the global Y-direction, via with magnitude in subroutine user VDLOAD Abaqus/Standard in Abaqus/Explicit. supplied DLOAD and as per force force Nonuniform body (give unit magnitude volume) in the global Z-direction, supplied via with magnitude DLOAD user in subroutine and VDLOAD Abaqus/Standard in Abaqus/Explicit. CENT(S) Not supported FL−4 (ML−3 T−2 ) CENTRIF(S) Rotational body force T−2 Centrifugal load (magnitude defined is the mass density as and , where is the angular speed). Centrifugal load (magnitude is input as is the angular speed). , where Units Description Coriolis force (magnitude input where , is the mass density and is the angular speed). The load stiffness due to Coriolis loading is not accounted for in direct steady-state dynamics analysis. General traction on edge n. Nonuniform general traction on edge and direction n with magnitude subroutine via supplied UTRACLOAD. user Moment on edge n. Nonuniform moment on edge n with magnitude supplied via user subroutine UTRACLOAD. Normal traction on edge n. Nonuniform normal traction on edge n with magnitude supplied via user subroutine UTRACLOAD. Shear traction on edge n. Nonuniform shear traction on edge n with magnitude supplied via user subroutine UTRACLOAD. Transverse traction on edge n. Nonuniform transverse traction on edge n with magnitude supplied via user subroutine UTRACLOAD. Gravity loading direction (magnitude is acceleration). in specified input as Hydrostatic pressure applied to the element reference surface and linear in global Z. The pressure is positive in Load ID (*DLOAD) CORIO(S) Abaqus/CAE Load/Interaction Coriolis force FL−4 T (ML−3 T−1 ) EDLDn Shell edge load EDLDnNU(S) Not supported EDMOMn Shell edge load EDMOMnNU(S) Not supported EDNORn Shell edge load EDNORnNU(S) Not supported EDSHRn Shell edge load EDSHRnNU(S) Not supported EDTRAn Shell edge load EDTRAnNU(S) Not supported GRAV Gravity FL−1 FL−1 FL−1 FL−1 FL−1 FL−1 FL−1 FL−1 LT−2 HP(S) Not supported FL−2 Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description Pressure FL−2 PNU Not supported FL−2 the direction of the positive element normal. applied to the element Pressure reference surface. The pressure is positive in the direction of the positive element normal. applied reference to Nonuniform pressure surface the element via with magnitude in user subroutine VDLOAD Abaqus/Standard in Abaqus/Explicit. The pressure is positive in the direction of the positive element normal. supplied DLOAD and ROTA(S) Rotational body force T−2 ROTDYNF(S) Not supported T−1 SBF(E) SP(E) Not supported FL−5 T Not supported FL−4 T2 TRSHR Surface traction FL−2 TRSHRNU(S) Not supported FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Not supported FL−2 29.6.7–6 Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Rotordynamic load (magnitude is input as is the angular velocity). , where Stagnation body force in global X-, Y-, and Z-directions. Stagnation pressure applied to the element reference surface. traction Shear reference surface. on the element Nonuniform shear traction on the surface with reference element magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element Nonuniform general on the element reference surface with Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description VBF(E) VP(E) Not supported FL−4 T Not supported FL−3 T magnitude and direction supplied via user subroutine UTRACLOAD. Viscous body force in global X-, Y-, and Z-directions. Viscous surface pressure. The viscous pressure is proportional to the velocity face and normal opposing the motion. to the element Foundations Foundations are available for Abaqus/Standard elements with displacement degrees of freedom. They are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE Units Description F(S) Elastic foundation FL−3 Elastic foundation in the direction of the shell normal. Distributed heat fluxes Distributed heat fluxes are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DFLUX) BF(S) BFNU(S) Abaqus/CAE Load/Interaction Units Description Body heat flux Body heat flux JL−3 T−1 JL−3 T−1 Body heat flux per unit volume. Nonuniform body heat flux per unit volume with magnitude supplied via user subroutine DFLUX. Surface heat flux per unit area into the bottom face of the element. Surface heat flux per unit area into the top face of the element. Nonuniform surface heat flux per unit area into the bottom face of the element with magnitude supplied via user subroutine DFLUX. SNEG(S) Surface heat flux JL−2 T−1 SPOS(S) Surface heat flux JL−2 T−1 SNEGNU(S) Not supported JL−2 T−1 Load ID (*DFLUX) Abaqus/CAE Load/Interaction Units Description SPOSNU(S) Not supported JL−2 T−1 Nonuniform surface heat flux per unit area into the top face of the element with magnitude supplied via user subroutine DFLUX. Film conditions Film conditions are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*FILM) FNEG(S) FPOS(S) Abaqus/CAE Load/Interaction Units Description Surface film condition Surface film condition JL−2 T−1 −1 JL−2 T−1 −1 FNEGNU(S) Not supported JL−2 T−1 −1 FPOSNU(S) Not supported JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on the bottom face of the element. Film coefficient and sink temperature (units of ) provided on the top face of the element. Nonuniform film coefficient and sink temperature (units of ) provided on the bottom face of the element with magnitude supplied via user subroutine FILM. Nonuniform film coefficient and sink temperature (units of ) provided on the top face of the element with magnitude supplied via user subroutine FILM. Radiation types Radiation conditions are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*RADIATE) RNEG(S) Abaqus/CAE Load/Interaction Units Description Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided for the bottom face of the shell. Load ID (*RADIATE) RPOS(S) Abaqus/CAE Load/Interaction Units Description Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided for the top face of the shell. Surface-based loading Distributed loads Surface-based distributed loads are available for all elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description EDLD Shell edge load FL−1 EDLDNU(S) Shell edge load FL−1 EDMOM Shell edge load EDMOMNU(S) Shell edge load EDNOR Shell edge load FL−1 EDNORNU(S) Shell edge load FL−1 EDSHR Shell edge load EDSHRNU(S) Shell edge load FL−1 FL−1 General surface. traction on edge-based traction Nonuniform general on edge-based surface with magnitude and direction supplied via user subroutine UTRACLOAD. Moment on edge-based surface. Nonuniform moment on edge-based surface with magnitude supplied via user subroutine UTRACLOAD. Normal surface. traction on edge-based traction on Nonuniform normal edge-based surface with magnitude supplied subroutine via UTRACLOAD. user Shear traction on edge-based surface. traction Nonuniform shear on edge-based surface with magnitude subroutine via supplied UTRACLOAD. user EDTRA Shell edge load FL−1 Transverse traction on edge-based surface. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description EDTRANU(S) Shell edge load FL−1 HP(S) Pressure FL−2 Pressure FL−2 PNU Pressure FL−2 SP(E) Pressure FL−4 T2 TRSHR Surface traction FL−2 TRSHRNU(S) Surface traction FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 29.6.7–10 Nonuniform transverse traction on edge-based surface with magnitude subroutine via supplied UTRACLOAD. user Hydrostatic pressure on the element reference surface and linear in global Z. The pressure is positive in the direction opposite to the surface normal. Pressure on the element reference surface. The pressure is positive in the direction opposite to the surface normal. Nonuniform pressure on the element reference surface with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. The pressure is positive in the direction opposite to the surface normal. Stagnation pressure applied to the element reference surface. traction Shear reference surface. on the element traction on the Nonuniform shear element surface with reference magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction on Nonuniform general the element reference surface with magnitude and direction supplied via Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description VP(E) Pressure FL−3 T Viscous surface pressure. The viscous pressure is proportional to the velocity face and normal opposing the motion. to the element Distributed heat fluxes Surface-based distributed heat fluxes are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DSFLUX) Abaqus/CAE Load/Interaction Units Description S(S) Surface heat flux JL−2 T−1 SNU(S) Surface heat flux JL−2 T−1 Surface heat flux per unit area into the element surface. Nonuniform surface heat flux per unit area into the element surface with magnitude supplied via user subroutine DFLUX. Film conditions Surface-based film conditions are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SFILM) F(S) FNU(S) Radiation types Abaqus/CAE Load/Interaction Units Description Surface film condition Surface film condition JL−2 T−1 −1 JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on the element surface. Nonuniform film coefficient and sink temperature (units of ) provided on the element surface with magnitude supplied via user subroutine FILM. Surface-based radiation conditions are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SRADIATE) Abaqus/CAE Load/Interaction Units Description R(S) Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided for the element surface. Incident wave loading Surface-based incident wave loads are available. They are specified as described in “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1. If the incident wave field includes a reflection off a plane outside the boundaries of the mesh, this effect can be included. Element output If a local coordinate system is not assigned to the element, the stress/strain components, as well as the section forces/strains, are in the default directions on the surface defined by the convention given in “Conventions,” Section 1.2.2. If a local coordinate system is assigned to the element through the section definition (“Orientations,” Section 2.2.5), the stress/strain components and the section forces/strains are in the surface directions defined by the local coordinate system. In large-displacement problems with elements that allow finite membrane strains in Abaqus/Standard and in all problems in Abaqus/Explicit, the local directions defined in the reference configuration are rotated into the current configuration by the average material rotation. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S12 Local Local Local direct stress. direct stress. shear stress. Section forces, moments, and transverse shear forces Available for elements with displacement degrees of freedom. SF1 SF2 SF3 SF4 SF5 Direct membrane force per unit width in local 1-direction. Direct membrane force per unit width in local 2-direction. Shear membrane force per unit width in local 1–2 plane. Transverse shear force per unit width in local 1-direction (available only for S3/S3R, S3RS, S4, S4R, S4RS, S4RSW, S8R, and S8RT). Transverse shear force per unit width in local 2-direction (available only for S3/S3R, S3RS, S4, S4R, S4RS, S4RSW, S8R, and S8RT). SM1 SM2 SM3 Bending moment force per unit width about local 2-axis. Bending moment force per unit width about local 1-axis. Twisting moment force per unit width in local 1–2 plane. The section force and moment resultants per unit length in the normal basis directions in a given shell section of thickness h can be defined on this basis as where is the offset of the reference surface from the midsurface. The section force SF6, which is the integral of through the shell thickness, is reported only for finite- strain shell elements and is zero because of the plane stress constitutive assumption. The total number of attributes written to the results file for finite-strain shell elements is 9; SF6 is the sixth attribute. Average section stresses Available for elements with displacement degrees of freedom. SSAVG1 SSAVG2 SSAVG3 SSAVG4 SSAVG5 Average membrane stress in local 1-direction. Average membrane stress in local 2-direction. Average membrane stress in local 1–2 plane. Average transverse shear stress in local 1-direction. Average transverse shear stress in local 2-direction. The average section stresses are defined as where h is the current section thickness. Section strains, curvatures, and transverse shear strains Available for elements with displacement degrees of freedom. SE1 SE2 SE3 SE4 Direct membrane strain in local 1-direction. Direct membrane strain in local 2-direction. Shear membrane strain in local 1–2 plane. Transverse shear strain in the local 1-direction (available only for S3/S3R, S3RS, S4, S4R, S4RS, S4RSW, S8R, and S8RT). SE5 SE6 SK1 SK2 SK3 Transverse shear strain in the local 2-direction (available only for S3/S3R, S3RS, S4, S4R, S4RS, S4RSW, S8R, and S8RT). Strain in the thickness direction (available only for S3/S3R, S3RS, S4, S4R, S4RS, and S4RSW). Curvature change about local 2-axis. Curvature change about local 1-axis. Surface twist in local 1–2 plane. The local directions are defined in “Shell elements: overview,” Section 29.6.1. Shell thickness STH Shell thickness, which is the current section thickness for S3/S3R, S3RS, S4, S4R, S4RS, and S4RSW elements. Transverse shear stress estimates Available for S3/S3R, S3RS, S4, S4R, S4RS, S4RSW, S8R, and S8RT elements. TSHR13 TSHR23 13-component of transverse shear stress. 23-component of transverse shear stress. Estimates of the transverse shear stresses are available at section integration points as output variables TSHR13 or TSHR23 for both Simpson’s rule and Gauss quadrature. For Simpson’s rule output of variables TSHR13 or TSHR23 should be requested at nondefault section points, since the default output is at section point 1 of the shell section where the transverse shear stresses vanish. For the small- strain elements in Abaqus/Explicit, transverse shear stress distributions are assumed constant for non- composite sections and piecewise constant for composite sections; therefore, transverse shear stresses at integration points should be interpreted accordingly. For element type S4 the transverse shear calculation is performed at the center of the element and assumed constant over the element. Hence, transverse shear strain, force, and stress will not vary over the area of the element. For numerically integrated shell sections (with the exception of small-strain shells in Abaqus/Explicit), estimates of the interlaminar shear stresses in composite sections—i.e., the transverse shear stresses at the interface between two composite layers—can be obtained only by using Simpson’s rule. With Gauss quadrature no section integration point exists at the interface between composite layers. Unlike the S11, S22, and S12 in-plane stress components, transverse shear stress components TSHR13 and TSHR23 are not calculated from the constitutive behavior at points through the shell section. They are estimated by matching the elastic strain energy associated with shear deformation of the shell section with that based on piecewise quadratic variation of the transverse shear stress across the section, under conditions of bending about one axis . Therefore, interlaminar shear stress calculation is supported only when the elastic material model is used for each layer of the shell section. If you specify the transverse shear stiffness values, interlaminar shear stress output is not available. Heat flux components Available for elements with temperature degrees of freedom. HFL1 HFL2 HFL3 Heat flux in local 1-direction. Heat flux in local 2-direction. Heat flux in local 3-direction. Node ordering on elements face 3 face 2 face 4 face 3 face 2 1 2 face 1 face 1 3-node element 4-node element face 3 4 7 3 face 3 face 2 face 4 6 5 1 face 1 2 face 2 face 1 6-node element 8-node element face 3 4 7 3 face 4 face 2 face 1 9-node element Numbering of integration points for output Stress/displacement analysis 9-node reduced integration element S3R element 4-node reduced integration element STRI3 element 6 6-node element 4-node full integration element 4 8-node reduced integration element Heat transfer analysis DS3 DS4 DS6 DS8 29.6.8 CONTINUUM SHELL ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Shell elements: overview,” Section 29.6.1 • “Choosing a shell element,” Section 29.6.2 • *SHELL GENERAL SECTION • *SHELL SECTION Overview This section provides a reference to the continuum shell elements available in Abaqus/Standard and Abaqus/Explicit. Element types Stress/displacement elements SC6R 6-node triangular in-plane continuum shell wedge, general-purpose, finite membrane strains SC8R 8-node hexahedron, general-purpose, finite membrane strains Active degrees of freedom 1, 2, 3 Additional solution variables None. Coupled temperature-displacement elements SC6RT SC8RT 6-node linear displacement and temperature, wedge, general-purpose, finite membrane strains triangular in-plane continuum shell 8-node linear displacement and temperature, hexahedron, general-purpose, finite membrane strains Active degrees of freedom 1, 2, 3, 11 Additional solution variables None. Nodal coordinates required Element property definition Input File Usage: Abaqus/CAE Usage: Use either of the following options: *SHELL SECTION *SHELL GENERAL SECTION Property module: Create Section: select Shell as the section Category and Homogeneous or Composite as the section Type Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description (give magnitude Body force as force per unit volume) in the global X-direction. (give magnitude Body force as force per unit volume) in the global Y-direction. (give magnitude Body force as force per unit volume) in the global Z-direction. as per force force (give Nonuniform body magnitude unit volume) in the global X-direction, via with magnitude user in subroutine VDLOAD Abaqus/Standard in Abaqus/Explicit. supplied DLOAD and force (give Nonuniform body magnitude unit volume) in the global Y-direction, via with magnitude supplied force per as BX BY BZ Body force FL−3 Body force FL−3 Body force FL−3 BXNU Body force FL−3 BYNU Body force FL−3 Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description subroutine user Abaqus/Standard in Abaqus/Explicit. DLOAD in and VDLOAD as per force force (give Nonuniform body magnitude unit volume) in the global Z-direction, via with magnitude user in subroutine VDLOAD Abaqus/Standard in Abaqus/Explicit. supplied DLOAD and Centrifugal load (magnitude defined as is the mass density and , where is the angular speed). Centrifugal load (magnitude is input as is the angular speed). , where Coriolis force (magnitude input where , is the mass density and is the angular speed). The load stiffness due to Coriolis loading is not accounted for in direct steady-state dynamics analysis. Gravity loading direction (magnitude is acceleration). in specified input as Hydrostatic pressure on face n, linear in global Z. A positive pressure is directed into the element. A positive Pressure on face n. pressure is directed into the element. on with user Nonuniform pressure face magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. A positive pressure is directed into the element. BZNU Body force FL−3 CENT(S) Not supported FL−4 (ML−3 T−2 ) CENTRIF(S) Rotational body force T−2 CORIO(S) Coriolis force FL−4 T (ML−3 T−1 ) GRAV Gravity LT−2 HPn(S) Not supported FL−2 Pn Pressure PnNU Not supported FL−2 FL−2 Load ID (*DLOAD) ROTA(S) Abaqus/CAE Load/Interaction Units Description Rotational body force T−2 Not supported FL−4 T2 Stagnation pressure on face n. ROTDYNF(S) Not supported T−1 SBF(E) Not supported FL−5 T2 SPn(E) TRSHRn Surface traction TRSHRnNU(S) Not supported TRVECn Surface traction TRVECnNU(S) Not supported FL−2 FL−2 FL−2 FL−2 VBF(E) VPn(E) Not supported FL−4 T Not supported FL3T Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Rotordynamic load (magnitude is input as is the angular velocity). , where Stagnation body force in global X-, Y-, and Z-directions. Shear traction on face n. Nonuniform shear traction on face and direction n with magnitude subroutine via supplied UTRACLOAD. user General traction on face n. Nonuniform general traction on face and direction n with magnitude supplied subroutine via UTRACLOAD. user Viscous body force in global X-, Y-, and Z-directions. Viscous pressure on face n, applying a pressure proportional to the velocity normal to the face and opposing the motion. Foundations Foundations are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE Units Description Fn(S) Elastic foundation FL−3 Elastic foundation on face n. A positive pressure is directed into the element. Distributed heat fluxes Distributed heat fluxes are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DFLUX) BF BFNU(S) Abaqus/CAE Load/Interaction Units Description Body heat flux Body heat flux JL−3 T−1 JL−3 T−1 Sn Surface heat flux JL−2 T−1 SnNU(S) Not supported JL−2 T−1 Heat body flux per unit volume. Nonuniform heat body flux per unit volume with magnitude supplied via user subroutine DFLUX. Heat surface flux per unit area into face n. Nonuniform heat surface flux per unit area into face n with magnitude supplied via user subroutine DFLUX. Film conditions Film conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Abaqus/CAE Load/Interaction Units Description Load ID (*FILM) Fn Surface film condition JL−2 T−1 −1 FnNU(S) Not supported JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on face n. Nonuniform film coefficient and sink temperature (units of ) provided on face n with magnitude supplied via user subroutine FILM. Radiation types Radiation conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*RADIATE) Abaqus/CAE Load/Interaction Units Description Rn Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided on face n. Surface-based loading Distributed loads Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description HP(S) Pressure FL−2 Pressure FL−2 PNU Pressure FL−2 SP(E) Pressure FL−4 T2 TRSHR Surface traction FL−2 TRSHRNU(S) Surface traction FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 29.6.8–6 Hydrostatic pressure applied to the element surface, in global Z. The pressure is positive in the direction opposite to the surface normal. linear Pressure applied to the element surface. The pressure is positive in the direction opposite to the surface normal. Nonuniform pressure applied to the element surface with magnitude supplied via user subroutine DLOAD and VDLOAD in Abaqus/Standard in Abaqus/Explicit. The pressure is positive in the direction opposite to the surface normal. Stagnation pressure applied to the element reference surface. traction Shear reference surface. on the element traction on the Nonuniform shear element surface with reference magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction on Nonuniform general the element reference surface with magnitude and direction supplied via Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description VP(E) Pressure FL3T Viscous surface pressure. The viscous pressure is proportional to the velocity face and normal opposing the motion. to the element Distributed heat fluxes Surface-based heat fluxes are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DSFLUX) Abaqus/CAE Load/Interaction Units Description Surface heat flux JL−2 T−1 SNU(S) Surface heat flux JL−2 T−1 Heat surface flux per unit area into the element surface. Nonuniform heat surface flux per unit area into the element surface with magnitude supplied via user subroutine DFLUX. Film conditions Surface-based film conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SFILM) FNU(S) Radiation types Abaqus/CAE Load/Interaction Units Description Surface film condition Surface film condition JL−2 T−1 −1 JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on the element surface. Nonuniform film coefficient and sink temperature (units of ) provided on the element surface with magnitude supplied via user subroutine FILM. Surface-based radiation conditions are available for all elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SRADIATE) Abaqus/CAE Load/Interaction Units Description Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided on the element surface. Element output If a local coordinate system is not assigned to the element, the stress/strain components, as well as the section forces/strains, are in the default directions on the surface defined by the convention given in “Conventions,” Section 1.2.2. If a local coordinate system is assigned to the element through the section definition (“Orientations,” Section 2.2.5), the stress/strain components and the section forces/strains are in the surface directions defined by the local coordinate system. The local directions defined in the reference configuration are rotated into the current configuration by the average material rotation. In the case of composite shells the components of section forces, section strains, and transverse shear stress estimates for stacked continuum shells (CTSHR13 and CTSHR23) are reported in the local orientation defined for the entire section (or the default shell coordinate directions if no section orientation is used). Components of stress, strain, and transverse shear stress (TSHR13 and TSHR23) are given with respect to the individual layer orientations. Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available. All tensors have the same components. For example, the stress components are as follows: S11 S22 S12 Local Local Local direct stress. direct stress. shear stress. The stress in the thickness direction, , is reported as zero to the output database as discussed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. may be obtained through the average section stress variable SSAVG6. Output of in-plane stress components of continuum shell elements does not include Poisson effects due to changes in the thickness direction. Heat flux components Available for elements with temperature degrees of freedom. HFL1 HFL2 HFL3 Heat flux in the X-direction. Heat flux in the Y-direction. Heat flux in the Z-direction. Section forces, moments, and transverse shear forces SF1 SF2 SF3 SF4 SF5 SF6 SM1 SM2 SM3 Direct membrane force per unit width in local 1-direction. Direct membrane force per unit width in local 2-direction. Shear membrane force per unit width in local 1–2 plane. Transverse shear force per unit width in local 1-direction. Transverse shear force per unit width in local 2-direction. Thickness stress integrated over the element thickness. Bending moment force per unit width about local 2-axis. Bending moment force per unit width about local 1-axis. Twisting moment force per unit width in local 1–2 plane. The section force and moment resultants per unit length in the normal basis directions in a given shell section of thickness h can be defined on this basis as where stress in the thickness direction is constant through the thickness. Outputs of in-plane section forces of continuum shell elements do not include Poisson effects due to changes in the thickness direction. Average section stresses SSAVG1 SSAVG2 SSAVG3 SSAVG4 SSAVG5 SSAVG6 Average membrane stress in local 1-direction. Average membrane stress in local 2-direction. Average membrane stress in local 1–2 plane. Average transverse shear stress in local 1-direction. Average transverse shear stress in local 2-direction. Average thickness stress in the local 3-direction. The average section stresses are defined as where and h is the current section thickness. is constant through the thickness. Section strains, curvatures, and transverse shear strains SE1 SE2 SE3 SE4 SE5 SE6 SK1 SK2 SK3 Direct membrane strain in local 1-direction. Direct membrane strain in local 2-direction. Shear membrane strain in local 1–2 plane. Transverse shear strain in the local 1-direction. Transverse shear strain in the local 2-direction. Total strain in the thickness direction. Curvature change about local 1-axis. Curvature change about local 2-axis. Surface twist in local 1–2 plane. The local directions are defined in “Shell elements: overview,” Section 29.6.1. Shell thickness STH Section thickness, which is the current section thickness if geometric nonlinearity is considered; otherwise, it is the initial section thickness. Transverse shear stress estimates TSHR13 TSHR23 13-component of transverse shear stress. 23-component of transverse shear stress. Estimates of the transverse shear stresses are available at section integration points as output variables TSHR13 or TSHR23 for both Simpson’s rule and Gauss quadrature. For Simpson’s rule output of variables TSHR13 or TSHR23 should be requested at nondefault section points, since the default output is at section point 1 of the shell section where the transverse shear stresses vanish. For numerically integrated sections, estimates of the interlaminar shear stresses in composite sections—i.e., the transverse shear stresses at the interface between two composite layers—can be obtained only by using Simpson’s rule. With Gauss quadrature no section integration point exists at the interface between composite layers. Unlike the S11, S22, and S12 in-surface stress components, TSHR13 and TSHR23 are not calculated from the constitutive behavior at points through the shell section. They are estimated by matching the elastic strain energy associated with shear deformation of the shell section with that based on piecewise quadratic variation of the transverse shear stress across the section, under conditions of bending about one axis . Therefore, interlaminar shear stress calculation is supported only when If you specify the transverse the elastic material model is used for each layer of the shell section. shear stiffness values, interlaminar shear stress output is not available. TSHR13 and TSHR23 are valid only for sections that have one element through the thickness direction. For sections with two or more continuum shell elements stacked in the thickness direction, output variables SSAVG4 and SSAVG5 or CTSHR13 and CTSHR23 should be used instead. An example using SSAVG4 and SSAVG5 to estimate the transverse shear stress distribution in stacked continuum shells can be found in “Composite shells in cylindrical bending,” Section 1.1.3 of the Abaqus Benchmarks Manual. Transverse shear stress estimates for stacked continuum shells 13-component of transverse shear stress for stacked continuum shells. 23-component of transverse shear stress for stacked continuum shells. CTSHR13 CTSHR23 Estimates of the transverse shear stresses that take into account the continuity of interlaminar transverse shear stress for stacked continuum shells are available at section integration points as output variables CTSHR13 or CTSHR23 for both Simpson’s rule and Gauss quadrature. CTSHR13 or CTSHR23 are available only in Abaqus/Standard. CTSHR13 and CTSHR23 are not calculated from the constitutive behavior at points through the shell section. They are estimated by assuming a quadratic variation of shear stress across the element section and by enforcing the continuity of interface transverse shear between adjoining continuum elements in a stack. It is also assumed that the transverse shear is zero at the free boundaries of a stack. The intended use case for CTSHR13 and CTSHR23 is to estimate the through-the-thickness transverse shear stress for flat or nearly flat composite plates that are modeled with stacked continuum shell elements where each continuum element in the stack models a single material layer. Central to CTSHR13 and CTSHR23 is the concept of a “stack” of continuum shell elements. During input file preprocessing Abaqus partitions all the continuum shells in a model into stacks. A “stack” is defined as a contiguous set of continuum shells whose first and last elements lie on a free boundary and who are connected through shared nodes on the top and bottom element surfaces (as determined by the elements’ stack directions). In this context a “free boundary” is a top or bottom surface of a continuum shell element that is not connected through its nodes to another continuum shell element. For example, assuming that the stack direction of all the elements in Figure 29.6.8–1 is in the z-direction, elements 1–6 would form a stack. z A stack of continuum shell elements x Figure 29.6.8–1 Composite plate meshed with six stacked continuum shells through the thickness. It is important to emphasize that stacks of continuum shells are connected through shared nodes, not through constraints or other elements. Suppose, for example, that in Figure 29.6.8–1 element pairs 1–2, 2–3, 4–5, and 5–6 are connected to each other through shared nodes, but elements 3 and 4 are connected through a constraint (such as a tied constraint). In that case Abaqus would interpret the bottom surface of element 3 and the top surface of element 4 as free boundaries; therefore, elements 1–3 would form one stack, and elements 4–6 would form a second independent stack. For another example, suppose that element 4 is not a continuum shell element. In this case elements 1–3 would form one stack, and elements 5–6 would form another stack. In a final example, suppose the stack directions of elements 1–5 are in the global z-direction and the stack direction of element 6 is in the global x-direction. In this case elements 1–5 would form a stack separate from element 6. In the three cases just discussed the computed values of CTSHR13 and CTSHR23 would probably not be what you wanted. It is more likely that you want elements 1–6 to be in the same stack. It may be necessary to make changes in your model to achieve this. You can review the partitioning of the continuum shell elements into stacks in the data file by making a model definition data request. The continuum shell elements in a stack must satisfy certain criteria; otherwise, Abaqus marks the stack as invalid with respect to computing CTSHR13 or CTSHR23. If a stack is marked as invalid, CTSHR13 or CTSHR23, if requested, are not computed and are set to zero for all continuum shell elements in that stack. If a continuum shell element does not have an elastic material model, if you specify the transverse shear for any element in the stack, or if the element is specified as rigid, that stack is marked as invalid. A stack is also marked as invalid if the normal of any element in a stack is not within 10° of the average normal for the stack. In addition, if a continuum shell element is removed during the analysis, the stack to which the element belongs is marked as invalid until the element is reactivated. There are several other certain restrictions on CTSHR13 and CTSHR23. CTSHR13 and CTSHR23 are not available in any continuum shell element with a multi-layer composite material definition. However, having a multi-layer composite element in the stack does not invalidate the stack. For the purposes of computing CTSHR13 and CTSHR23, a maximum of 500 continuum shell elements can be put in any individual stack. If more than 500 continuum shell elements are stacked on top of each other, Abaqus issues a warning message during input file preprocessing, and CTSHR13 and CTSHR23 are not computed and are set to zero for all continuum shell elements in the model. CTSHR13 and CTSHR23 are not available if element operations are run in parallel . CTSHR13 or CTSHR23 are currently available only for static and direct-integration dynamic analyses. An example using CTSHR13 and CTSHR23 to estimate the transverse shear stress distribution in stacked continuum shells can be found in “Composite shells in cylindrical bending,” Section 1.1.3 of the Abaqus Benchmarks Manual. Node ordering on elements face 5 face 1 face 3 face 2 face 4 face 2 face 3 face 6 face 1 face 5 face 4 6-node continuum shell 8-node continuum shell Numbering of integration points for output Stress/displacement analysis 6-node continuum shell 8-node continuum shell 29.6.9 AXISYMMETRIC SHELL ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Shell elements: overview,” Section 29.6.1 • “Choosing a shell element,” Section 29.6.2 • *NODAL THICKNESS • *SHELL GENERAL SECTION • *SHELL SECTION Overview This section provides a reference to the axisymmetric shell elements available in Abaqus/Standard and Abaqus/Explicit. For axisymmetric shell geometries in which nonaxisymmetric behavior is expected, use the SAXA elements available in Abaqus/Standard . Conventions Coordinate 1 is r, coordinate 2 is z. The r-direction corresponds to the global X-direction, and the z- direction corresponds to the global Y-direction. Coordinate 1 should be greater than or equal to zero. Degree of freedom 1 is plane. , degree of freedom 2 is , and degree of freedom 6 is rotation in the r–z Abaqus does not automatically apply any boundary conditions to nodes located along the symmetry axis. You should apply radial or symmetry boundary conditions on these nodes if desired. Point loads and concentrated fluxes should be given as the value integrated around the circumference (that is, the load on the complete ring). The meridional direction is the direction that is tangent to the element in the r–z plane; that is, the meridional direction is along the line that is rotated about the axis of symmetry to generate the full three-dimensional body. The circumferential or hoop direction is the direction normal to the r–z plane. Element types Stress/displacement elements SAX1 SAX2(S) 2-node thin or thick linear shell 3-node thin or thick quadratic shell Active degrees of freedom 1, 2, 6 Additional solution variables None. Heat transfer elements DSAX1(S) DSAX2(S) 2-node shell 3-node shell Active degrees of freedom 11, 12, 13, etc. (temperatures through the thickness as described in “Choosing a shell element,” Section 29.6.2) Additional solution variables None. Coupled temperature-displacement element SAX2T(S) 3-node thin or thick shell, quadratic displacement, linear temperature in the shell surface Active degrees of freedom 1, 2, 6 at all three nodes 11, 12, 13, etc. (temperatures through the thickness as described in “Choosing a shell element,” Section 29.6.2) at the end nodes Additional solution variables None. Nodal coordinates required r, z, and optionally for shells with displacement degrees of freedom, shell normal at the node. , , the direction cosines of the Element property definition Input File Usage: Use either of the following options for stress/displacement elements: *SHELL SECTION *SHELL GENERAL SECTION Use the following option for heat transfer or coupled temperature-displacement elements: *SHELL SECTION In addition, use the following option for variable thickness shells: *NODAL THICKNESS Property module: Create Section: select Shell as the section Category and Homogeneous or Composite as the section Type Abaqus/CAE Usage: Element-based loading Distributed loads Distributed loads are available for elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Distributed load magnitudes are per unit area or per unit volume. They do not need to be multiplied by . Body forces and centrifugal loads must be given as force per unit area if a general shell section is used. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BR BZ Body force Body force BRNU Body force FL−3 FL−3 FL−3 BZNU Body force FL−3 Body force per unit volume in the radial direction. Body force per unit volume in the axial direction. in the the magnitude Nonuniform body force per unit radial direction, volume with supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user the magnitude Nonuniform body force per unit volume in the global z-direction, with supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user CENT(S) Not supported FL−4 (ML−3 T−2 ) Centrifugal load (magnitude given as is the mass density and is the angular velocity). Since only , where Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description axisymmetric deformation is allowed, the spin axis must be the z-axis. CENTRIF(S) Rotational body force T−2 GRAV Gravity LT−2 HP(S) Not supported FL−2 Pressure FL−2 PNU Not supported FL−2 , where Centrifugal load (magnitude is input as the angular velocity). Since only axisymmetric deformation is allowed, the spin axis must be the z-axis. is Gravity direction acceleration). loading in (magnitude specified as input Hydrostatic pressure applied to the element reference surface and linear in global Z. The pressure is positive in the direction of the positive element normal. Pressure applied to the element reference surface. The pressure is positive in the direction of the positive element normal. applied reference to Nonuniform pressure surface the element via with magnitude in user subroutine VDLOAD Abaqus/Standard in Abaqus/Explicit. The pressure is positive in the direction of the positive element normal. supplied DLOAD and SBF(E) SP(E) Not supported FL−5 T2 Not supported FL−4 T2 TRSHR Surface traction FL−2 TRSHRNU(S) Not supported FL−2 Stagnation body force in radial and axial directions. Stagnation pressure applied to the element reference surface. traction Shear reference surface. on the element Nonuniform shear reference element traction on the surface with (*DLOAD) Abaqus/CAE Load/Interaction Units Description AXISYMMETRIC SHELLS TRVEC Surface traction FL−2 TRVECNU(S) Not supported FL−2 VBF(E) VP(E) Not supported FL−4 T Not supported FL−3 T magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction Nonuniform general on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. Viscous body force in radial and axial directions. Viscous surface pressure. The viscous pressure is proportional to the velocity normal face and opposing the motion. to the element Foundations Foundations are available for Abaqus/Standard elements with displacement degrees of freedom. They are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE Units Description F(S) Elastic foundation FL−3 Elastic foundation in the direction of the shell normal. Distributed heat fluxes Distributed heat fluxes are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DFLUX) BF(S) BFNU(S) Abaqus/CAE Load/Interaction Units Description Body heat flux Body heat flux JL−3 T−1 JL−3 T−1 Body heat flux per unit volume. Nonuniform body heat flux per unit volume with magnitude supplied via user subroutine DFLUX. Surface heat flux per unit area into the bottom face of the element. SNEG(S) Surface heat flux JL−2 T−1 Load ID (*DFLUX) Abaqus/CAE Load/Interaction Units Description SPOS(S) Surface heat flux JL−2 T−1 SNEGNU(S) Not supported JL−2 T−1 SPOSNU(S) Not supported JL−2 T−1 Surface heat flux per unit area into the top face of the element. Nonuniform surface heat flux per unit area into the bottom face of the element with magnitude supplied via user subroutine DFLUX. Nonuniform surface heat flux per unit area into the top face of the element with magnitude supplied via user subroutine DFLUX. Film conditions Film conditions are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*FILM) FNEG(S) FPOS(S) Abaqus/CAE Load/Interaction Units Description Surface film condition Surface film condition JL−2 T −1 −1 JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on the bottom face of the element. Film coefficient and sink temperature (units of ) provided on the top face of the element. Nonuniform film coefficient and sink temperature (units of ) provided on the bottom face of the element with magnitude supplied via user subroutine FILM. Nonuniform film coefficient and sink temperature (units of ) provided on the top face of the element with magnitude supplied via user subroutine FILM. FNEGNU(S) Not supported JL−2 T−1 −1 FPOSNU(S) Not supported JL−2 T−1 −1 Radiation types Radiation conditions are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*RADIATE) RNEG(S) Abaqus/CAE Load/Interaction Units Description Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided for the bottom face of the shell. Emissivity and sink temperature (units of ) provided for the top face of the shell. RPOS(S) Surface radiation Dimensionless Surface-based loading Distributed loads Surface-based distributed loads are available for elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Distributed load magnitudes are per unit area or per unit volume. They do not need to be multiplied by . Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description HP(S) Pressure FL−2 Pressure FL−2 PNU Pressure FL−2 Hydrostatic pressure on the element reference surface and linear in global Z. The pressure is positive in the direction opposite the surface normal. Pressure on the element reference surface. The pressure is positive in the direction opposite to the surface normal. Nonuniform pressure on the element reference surface with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. The pressure is positive in the direction opposite to the surface normal. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description SP(E) Pressure FL−4 T2 TRSHR Surface traction FL−2 TRSHRNU(S) Surface traction FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 VP(E) Pressure FL−3 T Stagnation pressure applied to the element reference surface. traction Shear reference surface. on the element traction on the Nonuniform shear surface with reference element magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction Nonuniform general on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. Viscous surface pressure. The viscous pressure is proportional to the velocity normal to the element surface and opposing the motion. Distributed heat fluxes Surface-based heat fluxes are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DSFLUX) Abaqus/CAE Load/Interaction Units Description S(S) Surface heat flux JL−2 T−1 SNU(S) Surface heat flux JL−2 T−1 Surface heat flux per unit area into the element surface. Nonuniform surface heat flux per unit area into the element surface with magnitude supplied via user subroutine DFLUX. Film conditions Surface-based film conditions are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SFILM) F(S) FNU(S) Radiation types Abaqus/CAE Load/Interaction Units Description Surface film condition Surface film condition JL−2 T−1 −1 JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on the element surface. Nonuniform film coefficient and sink temperature (units of ) provided on the element surface with magnitude supplied via user subroutine FILM. Surface-based radiation conditions are available for elements with temperature degrees of freedom. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SRADIATE) Abaqus/CAE Load/Interaction Units Description R(S) Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided for the element surface. Incident wave loading Surface-based incident wave loads are available. They are specified as described in “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1. If the incident wave field includes a reflection off a plane outside the boundaries of the mesh, this effect can be included. Element output Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 Meridional stress. Hoop (circumferential) stress. Section forces, moments, and transverse shear forces Available for elements with displacement degrees of freedom. SF1 SF2 Membrane force per unit width in the meridional direction. Membrane force per unit width in the hoop direction. SF3 SF4 SM1 SM2 Transverse shear force per unit width in the meridional direction (available only from Abaqus/Standard). Integrated stress in the thickness direction; always zero (available only from Abaqus/Standard). Bending moment per unit width about the hoop direction. Bending moment per unit width about the meridional direction. Section strains, curvature changes, and transverse shear strains Available for elements with displacement degrees of freedom. SE1 SE2 SE3 SE4 SK1 SK2 Membrane strain in the meridional direction. Membrane strain in the hoop direction. Transverse shear Abaqus/Standard). Strain in the thickness direction (available only from Abaqus/Standard). Curvature change about the hoop direction. Curvature change about the meridional direction. strain in the meridional direction (available only from Shell thickness STH Shell thickness, which is the current thickness for SAX1, SAX2, and SAX2T elements. Heat flux components Available for elements with temperature degrees of freedom. HFL1 HFL2 Heat flux in the meridional direction. Heat flux in the thickness direction. Node ordering on elements 2 - node element 3 - node element Numbering of integration points for output 2 - node element 3 - node element 29.6.10 AXISYMMETRIC SHELL ELEMENTS WITH NONLINEAR, ASYMMETRIC DEFORMATION Product: Abaqus/Standard References • “Shell elements: overview,” Section 29.6.1 • “Choosing a shell element,” Section 29.6.2 • *NODAL THICKNESS • *SHELL GENERAL SECTION • *SHELL SECTION Overview This section provides a reference to the axisymmetric shell elements with nonlinear, asymmetric deformation available in Abaqus/Standard. For an axisymmetric reference geometry where axisymmetric deformation is expected, use regular axisymmetric elements . For an axisymmetric reference geometry where nonaxisymmetric deformation is expected and the thickness to characteristic radius is high or through the thickness detail is required, use CAXA-type elements . Conventions Coordinate 1 is r, coordinate 2 is z. The r-direction corresponds to the global X-direction in the plane and the global Y-direction in the Z-direction. Coordinate 1 should be greater than or equal to zero. plane, and the z-direction corresponds to the global Degree of freedom 1 is , degree of freedom 2 is , degree of freedom 6 is rotation in the r–z plane. allows the modeling of half of the initially Even though the symmetry in the r–z plane at axisymmetric structure, the loading must be specified as the total load on the full axisymmetric body. Consider, for example, a cylindrical shell loaded by a unit uniform axial force. To produce a unit load on a SAXA element with four modes, the nodal forces are 1/8, 1/4, 1/4, 1/4, and 1/8 at , , , , and , respectively. The meridional direction is the direction tangent to the element in the r–z plane; that is, the meridional direction is along the line that is rotated about the axis of symmetry to generate the full three-dimensional body. The circumferential or hoop direction is the direction normal to the r–z plane. Element types SAXA1N SAXA2N Linear interpolation, Fourier shell element with 2 nodes in the meridional direction and N Fourier modes Quadratic interpolation, Fourier shell element with 3 nodes in the meridional direction and N Fourier modes Active degrees of freedom 1, 2, 6 See Figure 29.6.10–1 for the positive nodal displacement and rotation directions. The nodal rotation, is consistent with the SAX elements; however, a positive nodal rotation is in the negative -direction. , uz ur φθ uz φθ ur uz ur φθ Figure 29.6.10–1 Element coordinate system and positive displacement/rotation directions. SAXA22 element shown. Additional solution variables elements have SAXA variables relating to ( SAXA elements have variables relating to ( , , , , ). ). Nodal coordinates required r, z (given in the r–z plane for ) The two direction cosines, or by a user-specified normal definition . , of the nodal normal field can be specified either in the nodal data and Element property definition If a general shell section is used and the section stiffness matrix is given directly, a full 6 × 6 section stiffness should be specified (i.e., 21 constants as for a three-dimensional shell). Input File Usage: Use either of the following options: *SHELL SECTION *SHELL GENERAL SECTION In addition, use the following option for variable thickness shells: *NODAL THICKNESS Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Distributed load magnitudes are per unit area or per unit volume. They do not need to be multiplied by times the radius. Load ID (*DLOAD) Units Description FL−3 FL−3 FL−3 FL−3 FL−2 FL−2 FL−2 Body force per unit volume in the global X- direction. Body force per unit volume in the global Z- direction. Nonuniform body force in the global X-direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in the global Z-direction with magnitude supplied via user subroutine DLOAD. Hydrostatic pressure on the shell surface, linear in the global Z-direction. Pressure on the shell surface. Nonuniform pressure on the shell surface with magnitude supplied via user subroutine DLOAD. 29.6.10–3 BX BZ BXNU BZNU HP Element output employs the trapezoidal rule. There are and equally The numerical integration with respect to spaced integration planes in the element, including the planes, with N being the number of Fourier modes. Consequently, the radial nodal forces corresponding to pressure loads applied in the circumferential direction are distributed in this direction in the ratio of in the 1 Fourier mode element, in the 4 Fourier mode element. The sum of these consistent nodal forces is equal to the integral of the applied pressure over the full circumference ( in the 2 Fourier mode element, and ). Stress, strain, and other tensor components Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows: S11 S22 S12 Meridional stress. Hoop (circumferential) stress. Local 12 shear stress (zero at and ). Section forces SF1 SF2 SF3 SF4 SM1 SM2 SM3 Section strains SE1 SE2 SE3 SE4 SK1 SK2 SK3 Direct membrane force per unit width in local 1-direction. Direct membrane force per unit width in local 2-direction. Shear membrane force per unit width in local 1–2 plane. Integrated stress in the thickness direction; always zero. Bending moment per unit width about local 2-axis. Bending moment per unit width about local 1-axis. Twisting moment per unit width in local 1–2 plane. Direct membrane strain in local 1-direction. Direct membrane strain in local 2-direction. Shear membrane strain in local 1–2 plane. Strain in the thickness direction. Bending strain in local 1-direction. Bending strain in local 2-direction. Twisting strain in local 1–2 plane. The section force and moment resultants per unit length in the normal basis directions for a given layer of thickness h can be defined, in components relative to this basis, as: where is the offset of the reference surface from the midsurface. The local directions are defined in “Defining the initial geometry of conventional shell elements,” Section 29.6.3. Current shell thickness STH Current shell thickness. Node ordering on elements The node ordering in the first generator plane ( ) of each element is shown below. You specify the line or curve of nodes in the generator plane just as with the SAX1 and SAX2 elements. Each element must have N more planes of nodes defined, where N is the number of Fourier modes used. Abaqus/Standard will generate these additional circumferential nodes and number them by adding a constant offset value to the nodes specified in the first plane . 30. Inertial, Rigid, and Capacitance Elements Point mass elements Rotary inertia elements Rigid elements Capacitance elements 30.1 30.2 30.3 30.1 Point mass elements • “Point masses,” Section 30.1.1 • “Mass element library,” Section 30.1.2 30.1.1 POINT MASSES Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Mass element library,” Section 30.1.2 • *MASS • “Defining point mass and rotary inertia,” Section 33.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Mass elements: • allow the introduction of concentrated mass that is either isotropic or anisotropic at a point; • are associated with the three translational degrees of freedom at a node. If rotary inertia is also required (for example, to represent a rigid body), use element type ROTARYI (“Rotary inertia,” Section 30.2.1). In addition to point masses, Abaqus provides a convenient nonstructural mass definition that can be used to smear mass from features that have negligible structural stiffness over a region that is typically adjacent to the nonstructural feature. The nonstructural mass can be specified in the form of a total mass value, a mass per unit volume, a mass per unit area, or a mass per unit length . Defining the isotropic mass value You specify a mass magnitude, which is associated with the three translational degrees of freedom at the node of the element. Specify mass, not weight. You must associate this mass with a region of your model. Input File Usage: *MASS, ELSET=name mass magnitude where the ELSET parameter refers to a set of MASS elements. Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Magnitude: Isotropic: mass magnitude Defining the mass matrix explicitly in Abaqus/Standard You can define a general mass matrix explicitly in Abaqus/Standard if the introduction of individual terms on and off the diagonal of the mass matrix is desired. See “User-defined elements,” Section 32.15.1, for details. Input File Usage: Abaqus/CAE Usage: Use both of the following options: *USER ELEMENT *MATRIX Defining the mass matrix explicitly is not supported in Abaqus/CAE. Defining the anisotropic mass tensor You can specify the mass as anisotropic by giving the three principal values and the principal directions. When the orientation of the principal directions is not specified, they are assumed to coincide with the In a large-displacement analysis the local axes of the anisotropic mass rotate with the global axes. rotation, if active, of the node to which the anisotropic mass is attached. The rotation degree of freedom is active at a node if that node is connected to a beam, a conventional shell, a rotary inertia element, or a rigid body. You can specify mass proportional loads such as gravitation on an anisotropic mass. Damping and mass scaling can also be used with an anisotropic mass. Specify mass, not weight. You must associate this mass with a region of your model. Input File Usage: *MASS, ELSET=name, TYPE=ANISOTROPIC, ORIENTATION=orientation_name , , where the ELSET parameter refers to a set of MASS elements. Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Magnitude: Anisotropic: , , and Defining damping for MASS elements In Abaqus/Standard you can define mass proportional damping for direct-integration dynamic analysis or composite damping for modal dynamic analysis. Although both damping definitions can be specified for a set of MASS elements, only the damping that is relevant to the particular dynamic analysis procedure will be used. In Abaqus/Explicit mass proportional damping can be defined for MASS elements. Dynamics You can define inertia proportional damping for MASS elements in direct-integration dynamic analysis or explicit dynamic analysis. See “Material damping,” Section 26.1.1, for details. Input File Usage: Abaqus/CAE Usage: *MASS, ALPHA= Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Damping: Alpha: Modal dynamics You can define the fraction of critical damping to be used with the MASS elements when calculating composite damping factors for the modes when used in modal dynamic analysis. See “Material damping,” Section 26.1.1, for details. Abaqus/CAE Usage: *MASS, COMPOSITE= Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Damping: Composite: POINT MASSES 30.1.2 MASS ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Point masses,” Section 30.1.1 • *MASS Overview This section provides a reference to the mass elements available in Abaqus/Standard and Abaqus/Explicit. Element type MASS Point mass Active degrees of freedom 1, 2, 3 Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition Input File Usage: Abaqus/CAE Usage: *MASS Not supported Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description Centrifugal load (magnitude is input as the angular velocity). , where is CENTRIF(S) Not supported T−2 Load ID (*DLOAD) GRAV Abaqus/CAE Load/Interaction Units Description Not supported LT−2 ROTA(S) Not supported T−2 Gravity direction. loading in specified Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Element output ELKE Element kinetic energy (available only from Abaqus/Standard). Nodes associated with the element 1 node. 30.2 Rotary inertia elements • “Rotary inertia,” Section 30.2.1 • “Rotary inertia element library,” Section 30.2.2 30.2.1 ROTARY INERTIA Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Rotary inertia element library,” Section 30.2.2 • *ROTARY INERTIA • “Defining point mass and rotary inertia,” Section 33.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Rotary inertia elements: • allow rotary inertia to be included at a node; • are associated with the three rotational degrees of freedom at a node; and • can be paired with a MASS element (“Point masses,” Section 30.1.1) to define the mass and inertia properties of a rigid body directly (“Rigid body definition,” Section 2.4.1). Defining the rotary inertia The ROTARYI element allows rotary inertia to be included at a node. The node is assumed to be the center of mass of the body so that only second moments of inertia are required. If the node is part of a rigid body, the offset between the node and the center of mass of the rigid body is accounted for. All six components of the rotary inertia tensor— , , and —about the global coordinate , system are defined as follows: , , The rotary inertia tensor must be positive semi-definite. You specify the moments of inertia, which should be given in units of ML2 . You must associate these moments of inertia with a region of your model. Optionally, you can refer to a local orientation (“Orientations,” Section 2.2.5) that defines the directions of the local axes for which the rotary inertia values are being given. If you do not specify a local orientation and the rotary inertia element is defined within a part or a part instance , the components of the inertia tensor must be given with respect to the local part axes. If you do not specify a local orientation and the rotary inertia element is not defined within a part or a part instance, the components of the inertia tensor must be given with respect to the global axes. Input File Usage: *ROTARY INERTIA, ELSET=name, ORIENTATION=name , , , , , where the ELSET parameter refers to a set of ROTARYI elements. Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Magnitude: I11: , I33: ; if necessary, toggle on Specify off-diagonal terms: I12: , I13: ; CSYS: Edit , I23: , I22: Defining damping for ROTARYI elements In Abaqus/Standard you can define mass proportional damping for direct-integration dynamic analysis or composite damping for modal dynamic analysis. Although both damping definitions can be specified for a set of ROTARYI elements, only the damping that is relevant to the particular dynamic analysis procedure will be used. In Abaqus/Explicit mass proportional damping can be defined for ROTARYI elements. Dynamics You can define inertia proportional damping for ROTARYI elements in direct-integration dynamic analysis or explicit dynamic analysis. See “Material damping,” Section 26.1.1, for details. Input File Usage: Abaqus/CAE Usage: *ROTARY INERTIA, ALPHA= Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Damping: Alpha: Modal dynamics You can define the fraction of critical damping to be used with the ROTARYI elements when calculating composite damping factors for the modes when used in modal dynamic analysis. See “Material damping,” Section 26.1.1, for details. Input File Usage: Abaqus/CAE Usage: *ROTARY INERTIA, COMPOSITE= Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Damping: Composite: Speeding up convergence in three-dimensional implicit analyses In geometrically nonlinear analysis in Abaqus/Standard, rigid body rotary inertia contributes some unsymmetric terms to the system matrix when the motion is in three dimensions and the rotary inertia is not the same about all three axes. Therefore, in cases when the rotary inertia effects are significant, the solution may converge faster if you use the unsymmetric matrix storage and solution scheme for the step (“Defining an analysis,” Section 6.1.2). 30.2.2 ROTARY INERTIA ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Rotary inertia,” Section 30.2.1 • *ROTARY INERTIA Overview This section provides a reference to the rotary inertia elements available in Abaqus/Standard and Abaqus/Explicit. Element type ROTARYI Rotary inertia at a point Active degrees of freedom 4, 5, 6 Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition Input File Usage: Abaqus/CAE Usage: *ROTARY INERTIA Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Magnitude: Rotary Inertia Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description ROTA(S) Not supported T−2 ROTDYNF(S) Not supported T−1 Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Rotordynamic load (magnitude is input as is the angular velocity). , where Element output ELKE Element kinetic energy (available only from Abaqus/Standard). Nodes associated with the element 1 node. 30.3 Rigid elements • “Rigid elements,” Section 30.3.1 • “Rigid element library,” Section 30.3.2 30.3.1 RIGID ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Rigid body definition,” Section 2.4.1 • “Rigid element library,” Section 30.3.2 • *RIGID BODY • “Defining rigid body constraints,” Section 15.15.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Rigid elements: • can be used to define the surfaces of rigid bodies for contact; • can be used to define rigid bodies for multibody dynamic simulations; • can be attached to deformable elements; • can be used to constrain parts of a model; • are used to apply Abaqus/Aqua loads to rigid structures; and • are associated with a given rigid body and share a common node known as the rigid body reference node. Choosing an appropriate element Use R2D2 elements in plane strain or plane stress analysis, RAX2 elements in axisymmetric planar geometries, and R3D3 and R3D4 elements in three-dimensional analysis. RB2D2 and RB3D2 elements are often used in Abaqus/Standard to model offshore structures that will transmit Abaqus/Aqua loads but will not deform. They can also be used as rigid links between nodes on deformable bodies. Naming convention Rigid elements in Abaqus are named as follows: 3D 2 number of nodes two-dimensional (2D), three-dimensional (3D), or axisymmetric (AX) beam (optional) rigid element For example, R2D2 is a two-dimensional, 2-node, rigid element. Element normal definition For all rigid elements the face on the side of the element with the positive outward normal is referred to as SPOS. The face on the opposite side is referred to as SNEG. The positive normal direction for each element is defined below. R2D2, RAX2, RB2D2, R3D3, and R3D4 rigid elements can be used in Abaqus/Standard to define master surfaces for contact applications. The direction of the master surface’s outward normal is critical for proper detection of contact. See “Defining contact pairs in Abaqus/Standard,” Section 35.3.1, for a more detailed discussion of contact surface definitions. Two-dimensional rigid elements The positive outward normal direction, going from node 1 to node 2 of the element. See Figure 30.3.1–1. , is defined by a 90° counterclockwise rotation from the direction face SPOS face SNEG Y or z X or r Figure 30.3.1–1 Positive normal for two-dimensional rigid elements. Three-dimensional rigid elements The positive normal for R3D3 and R3D4 elements is given by the right-hand rule going around the nodes of the element in the order that they are given in the element’s connectivity. See Figure 30.3.1–2. RB3D2 elements do not have a unique normal definition. face SPOS face SNEG Figure 30.3.1–2 Positive normals for R3D3 and R3D4 elements. Defining rigid elements Rigid elements must always be part of a rigid body. See “Rigid body definition,” Section 2.4.1, for complete details on the definition of a rigid body. Input File Usage: *RIGID BODY, ELSET=name where the ELSET parameter refers to a set of rigid elements. Abaqus/CAE Usage: Interaction module: Create Constraint: Rigid body: Body (elements) Mass distribution In Abaqus/Standard rigid elements do not contribute mass to the rigid body to which they are assigned. The mass distribution on the rigid surface can be accounted for by using point mass (“Point masses,” Section 30.1.1) and rotary inertia elements (“Rotary inertia,” Section 30.2.1) on the nodes connected to the rigid elements. By default in Abaqus/Explicit, rigid elements do not contribute mass to the rigid body to which they are assigned. To define the mass distribution, you can specify the density of all rigid elements in a rigid body. When a nonzero density and thickness are specified, mass and rotary inertia contributions to the rigid body from rigid elements will be computed in an analogous manner to structural elements. Input File Usage: Abaqus/CAE Usage: Use the following option in Abaqus/Explicit to specify the density of rigid elements: *RIGID BODY, DENSITY=density You cannot specify the density of rigid elements in Abaqus/CAE. Geometry in Abaqus/Explicit In Abaqus/Explicit you can specify the cross-sectional area or thickness for all of the rigid elements that are part of a rigid body. Abaqus/Explicit assumes a default zero cross-sectional area or thickness if you do not specify one. To account for a continuously varying thickness of a surface formed by rigid elements in Abaqus/Explicit, you can specify the thickness of the rigid elements at the nodes. Specifying a nonzero thickness for rigid elements that form a rigid surface in a contact pair definition can be used to account for the effect of surface thickness in the contact constraint. It also enables the use of the double-sided surface contact feature with rigid surfaces formed by rigid elements. Input File Usage: Use the following option in Abaqus/Explicit to specify the cross-sectional area or thickness for all rigid elements in a rigid body: *RIGID BODY cross-sectional area or thickness Use both of the following options to specify a continuously varying thickness for a surface formed by rigid elements: *NODAL THICKNESS *RIGID BODY, NODAL THICKNESS You cannot specify the cross-sectional area or thickness of rigid elements in Abaqus/CAE. Abaqus/CAE Usage: Offset in Abaqus/Explicit In Abaqus/Explicit you can define the distance (measured as a fraction of the rigid element’s thickness) from the rigid element’s midsurface to the reference surface containing the element’s nodes. The positive values of the offset are in the direction of the element normal. When the offset distance is 0.5, the top surface is the reference surface. When the offset distance is −0.5, the bottom surface is the reference surface. The default offset distance is 0, which indicates that the middle surface of the rigid element is the reference surface. You can specify a value for the offset distance that is greater in magnitude than half the rigid element’s thickness. Since no element-level calculations are performed for rigid elements, a specified offset affects only the handling of contact pairs with rigid surfaces formed by rigid elements . Mass and rotary inertia contributions to the rigid body from rigid elements defined with an offset are computed as if the offset is zero. Input File Usage: Use the following option in Abaqus/Explicit to specify a surface offset for a rigid element: *RIGID BODY, OFFSET=offset The OFFSET parameter accepts a value or a label (SPOS or SNEG). Specifying SPOS is equivalent to specifying a value of 0.5; specifying SNEG is equivalent to specifying a value of −0.5. Abaqus/CAE Usage: You cannot specify an offset for rigid elements in Abaqus/CAE. 30.3.2 RIGID ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Rigid elements,” Section 30.3.1 • *RIGID BODY Overview This section provides a reference to the rigid elements available in Abaqus/Standard and Abaqus/Explicit. Element types 2-D rigid elements R2D2 RAX2 2-node, linear link (for use in plane strain or plane stress) 2-node, linear link (for use in axisymmetric planar geometries) RB2D2(S) 2-node, rigid beam Slave kinematic variables R2D2 and RAX2: 1, 2 RB2D2: 1, 2, 6 Master degrees of freedom R2D2, RAX2, and RB2D2: 1, 2, 6 at the rigid body reference node Additional solution variables None. 3-D rigid elements R3D3 R3D4 3-node, triangular facet 4-node, bilinear quadrilateral RB3D2(S) 2-node, rigid beam Slave kinematic variables R3D3 and R3D4: 1, 2, 3 RB3D2: 1, 2, 3, 4, 5, 6 Master degrees of freedom 1, 2, 3, 4, 5, 6 at the rigid body reference node Additional solution variables None. Nodal coordinates required R2D2 and RB2D2: X, Y RAX2: r, z R3D3, R3D4, and RB3D2: X, Y, Z Element property definition For R2D2, RB2D2, and RB3D2 elements you can specify the cross-sectional area of the element. In Abaqus/Standard if no area is given, unit area is assumed; the area is required in Abaqus/Explicit. For RAX2, R3D3, and R3D4 elements you can specify the thickness of the element. In Abaqus/Standard if no thickness is given, unit thickness is assumed; the thickness is required in Abaqus/Explicit. The cross-sectional area or element thickness is used for the purpose of defining body forces, which are given in units of force per unit volume, and, in Abaqus/Explicit, determining the total mass. Input File Usage: Abaqus/CAE Usage: *RIGID BODY Interaction module: Create Constraint: Rigid body: Body (elements) Element-based loading Distributed loads Distributed loads are available for elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Available for R2D2 elements only: Load ID (*DLOAD) BX(S) BY(S) BXNU(S) Abaqus/CAE Load/Interaction Units Description Body force Body force Body force FL−3 FL−3 FL−3 Body force in global X-direction. Body force in global Y-direction. Nonuniform body force in global X- direction with magnitude supplied via user subroutine DLOAD. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BYNU(S) Body force FL−3 CENT(S) Not supported CORIO(S) Coriolis force FL−4 (ML−3 T−2 ) FL−4 T (ML−3 T−1 ) P(E) Pressure FL−2 PNU(E) Not supported FL−2 Nonuniform body force in global Y- direction with magnitude supplied via user subroutine DLOAD. Centrifugal load (magnitude is input is the mass density as , where per unit volume and is the angular velocity). Coriolis force (magnitude is input is the mass density as , where per unit volume and is the angular velocity). The load stiffness due to Coriolis loading is not accounted for in direct steady-state dynamics analysis. Pressure on the element surface. The pressure is positive in the direction of the positive element normal. Nonuniform pressure on the element surface with magnitude supplied via user subroutine VDLOAD. The pressure is positive in the direction of the positive element normal. Available for RAX2 elements only: Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BR(S) BZ(S) Body force Body force BRNU(S) Body force FL−3 FL−3 FL−3 Body force per unit volume in the radial direction. Body force per unit volume in the axial direction. Nonuniform body force per unit volume in the radial direction, with the magnitude supplied via user subroutine DLOAD. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BZNU(S) Body force FL−3 CENT(S) Not supported FL−4 3 T−2 ) (ML− HP(S) Not supported FL−2 Pressure FL−2 PNU Not supported FL−2 TRSHR Surface traction TRSHRNU(S) Not supported FL−2 FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Not supported FL−2 30.3.2–4 Nonuniform body force per unit volume z-direction, with the magnitude supplied via user subroutine DLOAD. in the , where Centrifugal load (magnitude given as is the mass density and is the angular speed). Since only axisymmetric deformation is allowed, the spin axis must be the z-axis. Hydrostatic pressure on the element surface and linear in global Z. The pressure is positive in the direction of the positive element normal. Pressure on the element surface. The pressure is positive in the direction of the positive element normal. Nonuniform pressure on the element surface with the magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard The pressure is Abaqus/Explicit. positive in the direction of the positive element normal. Shear traction on the element surface. Nonuniform shear traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. General surface. traction on the element Nonuniform general traction on the element surface with magnitude and direction supplied via user subroutine RIGID ELEMENT LIBRARY Abaqus/CAE Load/Interaction Units Description Load ID (*DLOAD) BX(S) BY(S) BZ(S) BXNU(S) Body force Body force Body force Body force FL−3 FL−3 FL−3 FL−3 Body force in the global X-direction. Body force in the global Y-direction. Body force in the global Z-direction. Nonuniform body force in the global X-direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in the global Y-direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in the global Z-direction with magnitude supplied via user subroutine DLOAD. Centrifugal load (magnitude is input is the mass density as , where per unit volume and is the angular velocity). Coriolis force (magnitude is input as is the mass density , where per unit volume and is the angular velocity). The load stiffness due to Coriolis loading is not accounted for in direct steady-state dynamics analysis. Hydrostatic pressure on the element surface and linear in global Z. The pressure is positive in the direction of the positive element normal. Pressure on the element surface. The pressure is positive in the direction of the positive element normal. Nonuniform pressure on the element surface with magnitude supplied subroutine DLOAD in via user BYNU(S) Body force FL−3 BZNU(S) Body force FL−3 CENT(S) Not supported CORIO(S) Coriolis force FL−4 (ML−3 T−2 ) FL−4 T (ML−3 T−1 ) HP(S) Not supported FL−2 Pressure FL−2 PNU Not supported FL−2 Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description TRSHR Surface traction TRSHRNU(S) Not supported FL−2 FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Not supported FL−2 Abaqus/Standard and VDLOAD in Abaqus/Explicit. The pressure is positive in the direction of the positive element normal. Shear traction on the element surface. Nonuniform shear traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. General surface. traction on the element Nonuniform general traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. Abaqus/Aqua loads Abaqus/Aqua loads are specified as described in “Abaqus/Aqua analysis,” Section 6.11.1. Available for R3D3 and R3D4 elements only: Load ID (*CLOAD/ *DLOAD) Abaqus/CAE Load/Interaction Units Description PB(A) Not supported FL−2 Buoyancy force. Available for RB2D2 and RB3D2 elements only: Load ID (*CLOAD/ *DLOAD) FDD(A) FD1(A) FD2(A) Abaqus/CAE Load/Interaction Units Description Not supported FL−1 Transverse fluid drag force. Not supported Not supported Fluid drag force on the first end of the rigid link (node 1). Fluid drag force on the second end of the rigid link (node 2). Load ID (*CLOAD/ *DLOAD) FDT(A) FI(A) FI1(A) FI2(A) PB(A) WDD(A) WD1(A) WD2(A) Abaqus/CAE Load/Interaction Units Description Not supported Not supported Not supported Not supported Not supported Not supported Not supported Not supported FL−1 FL−1 FL−1 FL−1 Tangential fluid drag load. Transverse fluid inertia load. Fluid inertia load on the first end of the rigid link (node 1). Fluid inertia load on the second end of the rigid link (node 2). Buoyancy force (with closed-end condition). Transverse wind drag force. Wind drag force on the first end of the rigid link (node 1). Wind drag force on the second end of the rigid link (node 2). Surface-based loading Distributed loads Surface-based distributed loads are available for elements with displacement degrees of freedom. They are specified as described in “Distributed loads,” Section 33.4.3. Available for RAX2, R3D3, and R3D4 elements only: Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description HP(S) Pressure FL−2 Pressure PNU Pressure FL−2 FL−2 30.3.2–7 Hydrostatic pressure on the element surface and linear in global Z. The pressure is positive in the direction opposite to the surface normal. Pressure on the element surface. The pressure is positive in the direction opposite to the surface normal. Nonuniform pressure on the element surface with the magnitude supplied subroutine DLOAD in via Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description Abaqus/Standard and VDLOAD in Abaqus/Explicit. The pressure is positive in the direction opposite to the surface normal. Shear traction on the element surface. Nonuniform shear traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. General surface. traction on the element Nonuniform general traction on the element surface with magnitude and direction supplied via user subroutine UTRACLOAD. TRSHR Surface traction TRSHRNU(S) Surface traction FL−2 FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 Element output None. RIGID ELEMENT LIBRARY R2D2, RAX2 RB2D2, RB3D2 R3D3 R3D4 30.4 Capacitance elements • “Point capacitance,” Section 30.4.1 • “Capacitance element library,” Section 30.4.2 30.4.1 POINT CAPACITANCE Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Capacitance element library,” Section 30.4.2 • *HEATCAP • “Defining heat capacitance,” Section 33.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Capacitance elements: • allow the introduction of concentrated heat capacitance at a point; • are associated with the temperature degree of freedom at a node; and • have a capacitance that can be specified as a function of temperature and/or field variables. Defining the capacitance value The heat capacitance is associated with the temperature degree of freedom at the node of the element. You specify the capacitance magnitude, (density × specific heat × volume). Specify capacitance, not specific heat. You must associate this capacitance with a region of your model. Input File Usage: *HEATCAP, ELSET=name Abaqus/CAE Usage: where the ELSET parameter refers to a set of HEATCAP elements. Property or Interaction module: Special→Inertia→Create: Heat capacitance: select points: Capacitance 30.4.2 CAPACITANCE ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Point capacitance,” Section 30.4.1 • *HEATCAP Overview This section provides a reference to the capacitance elements available in Abaqus/Standard and Abaqus/Explicit. Element type HEATCAP Point heat capacitance Active degree of freedom 11 Nodal coordinates required X, Y, Z Element property definition Input File Usage: Abaqus/CAE Usage: *HEATCAP Property or Interaction module: Special→Inertia→Create: Heat capacitance Element-based loading None. Element output None. Nodes associated with the element 1 node. Connector Elements Connector elements Connector element behavior CONNECTOR ELEMENTS 31.1 31.1 Connector elements • “Connectors: overview,” Section 31.1.1 • “Connector elements,” Section 31.1.2 • “Connector actuation,” Section 31.1.3 • “Connector element library,” Section 31.1.4 • “Connection-type library,” Section 31.1.5 31.1.1 CONNECTORS: OVERVIEW Abaqus offers a library of connector types and connector elements to model the behavior of connectors. Overview Connector modeling consists of: • choosing and defining the appropriate connector elements (“Connector elements,” Section 31.1.2); • defining the connector behavior (“Connector behavior,” Section 31.2.1); • defining any connector actuations (“Connector actuation,” Section 31.1.3); and • monitoring connector output (“Connector elements,” Section 31.1.2, and “Connector element library,” Section 31.1.4). Typical applications The analyst is often faced with modeling problems in which two different parts are connected in some way. Sometimes connections are simple, such as two panels of sheet metal spot welded together or a door connected to a frame with a hinge. In other cases the connection may impose more complicated kinematic constraints, such as constant velocity joints, which transmit constant spinning velocity In addition to imposing kinematic constraints, connections between misaligned and moving shafts. may include (nonlinear) force versus displacement (or velocity) behavior in their unconstrained relative motion components, such as a muscle force resisting the rotation of a knee joint in a crash-test occupant model. More complex connections may include the following: • stopping mechanisms, which restrict the range of motion of an otherwise unconstrained relative motion; • internal friction, such as the lateral force or moments on a bolt generating friction in the translation of the bolt along a slot; • failure conditions, where excess force or displacement inside the connection causes the entire connection or a single component of relative motion to break free; and • locking mechanisms that engage after some force or displacement criteria is met, such as a snap-fit connector or a falling-pin locking mechanism on a satellite deployment arm. In many situations the connection can be actuated either through displacement or force control, such as a hydraulic piston or a gear-driven robot arm. In Abaqus/Standard if the two parts being connected are rigid bodies, multi-point constraints cannot be used to connect the bodies at nodes other than the reference nodes, since multi-point constraints use degree-of-freedom elimination and the other nodes on a rigid body do not have independent degrees of freedom. In Abaqus/Explicit this restriction does not apply. See “General multi-point constraints,” Section 34.2.2. Connector elements in Abaqus provide an easy and versatile way to model these and many other types of physical mechanisms whose geometry is discrete (i.e., node-to-node), yet the kinematic and kinetic relationships describing the connection are complex. Connector elements versus multi-point constraints In many instances connector elements perform functions similar to multi-point constraints (“General multi-point constraints,” Section 34.2.2). However, in most cases multi-point constraints eliminate degrees of freedom at one of the nodes involved in the connection. This elimination has the advantage that the problem size is reduced; it has the disadvantage that output and other functionality provided with connector elements is not available. In addition, in Abaqus/Standard the degree of freedom elimination prevents the use of multi-point constraints between nodes without independent degrees of freedom (such as nodes on a rigid body whose degrees of freedom are dependent on the degrees of freedom at the reference node). In contrast, connector elements do not eliminate degrees of freedom; kinematic constraints are enforced with Lagrange multipliers. These Lagrange multipliers are additional solution variables in Abaqus/Standard. The Lagrange multipliers provide constraint force and moment output. Since connector elements do not eliminate degrees of freedom, they can be used in many situations where multi-point constraints cannot be used or do not exist for the function required; for example, to connect two rigid bodies at nodes other than the reference node in Abaqus/Standard. Multi-point constraints are more efficient than connector elements; and if the requirements of the analysis can be satisfied with multi-point constraints, they should be used in place of connector elements. Input file template The following template shows the options used to define and activate the connector elements shown in Figure 31.1.1–1 and Figure 31.1.1–2. In the respective figures on the left is a schematic representation of a connection to be modeled; on the right is a representation of the equivalent finite element model. All options are discussed in detail in the following sections. extensible range 7.5 node 12 1 (local orientation) node 11 Figure 31.1.1–1 Simplified connector model of a shock absorber. 2.0 15.0 body 2 node 120 ⇒ node 110 node 120 1 (local orientation) node 110 45° body 1 global directions Figure 31.1.1–2 A pin-in-slot connection modeled with SLOT and CARDAN connection types. *HEADING ... *ELEMENT, TYPE=CONN3D2, ELSET=shock 101, 11, 12 *ELEMENT, TYPE=CONN3D2, ELSET=pininslot 1010, 110, 120 ... *ORIENTATION, NAME=ori60 0.5, 0.866025, 0.0, -0.866025, 0.5, 0.0 *ORIENTATION, NAME=ori45 0.707, 0.707, 0.0, -0.707, 0.707, 0.0 *CONNECTOR SECTION, ELSET=shock, BEHAVIOR=sbehavior revolute, slot ori60, ... *CONNECTOR BEHAVIOR, NAME=sbehavior *CONNECTOR DAMPING, COMPONENT=1 1500.0 *CONNECTOR LOCK, COMPONENT=3, LOCK=4 , , -500.0, 500.0 *CONNECTOR ELASTICITY, COMPONENT=4, NONLINEAR -900., -0.7 0.0 0.7 0., 1250., *CONNECTOR CONSTITUTIVE REFERENCE , , , 22.5, 0.0 0.45 *CONNECTOR STOP, COMPONENT=1 7.5, 15.0 ... *CONNECTOR FRICTION 0.34, 0.55, 0.34, 0.10, *FRICTION .15 ... *CONNECTOR SECTION, ELSET=pininslot cardan, slot ori45, *CONNECTOR MOTION pininslot, 4 pininslot, 5 ... *STEP ... *CONNECTOR MOTION, TYPE=VELOCITY pininslot, 6, 0.7854 ... *CONNECTOR LOAD pininslot, 1, 1000.0 ... *END STEP 31.1.2 CONNECTOR ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • “Connector element library,” Section 31.1.4 • “Connection-type library,” Section 31.1.5 • *CONNECTOR SECTION • “Creating connector sections,” Section 15.12.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Creating and modifying connector section assignments,” Section 15.12.12 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Connector elements: • are available for two-dimensional, axisymmetric, and three-dimensional analyses; • can define a connection between two nodes (each node can be connected to a rigid part, a deformable part, or not connected to any part); • can define a connection between a node and ground; • have relative displacements and rotations that are local to the element, which are referred to as components of relative motion; • are functionally defined by specifying the connector attributes; • have comprehensive kinematic and kinetic output; and • can be used to monitor kinematics in local coordinate systems. Choosing an appropriate element Two connector elements are provided. The element type to be chosen depends on the dimensionality of the analysis: CONN2D2 for two-dimensional and axisymmetric analyses and CONN3D2 for three- dimensional analyses. Both connector elements have at most two nodes. The position and motion of the second node on the connector element are measured relative to the first node. Naming convention Connector elements in Abaqus are named as follows: CONN 3D 2 number of nodes two-dimensional (2D) or three-dimensional (3D) connector For example, CONN2D2 is a two-dimensional, 2-node connector element. Defining a connection between points A connector element can be used to connect two points. Input File Usage: *ELEMENT, TYPE=name connector element number, node_1, node_2 Abaqus/CAE Usage: Interaction module: Connector→Assignment→Create: select wires Defining a connection between a point and ground A connector element can be connected to ground, and the ground “node” can be the first or second point on the connector element. The initial position of the ground node used for calculating relative position and displacement is the initial position of the other point on the element. All displacements and rotations at the ground node, if they exist, are fixed. Input File Usage: Use one of the following options: *ELEMENT, TYPE=name connector element number, node number on the body *ELEMENT, TYPE=name connector element number, , node number on the body Abaqus/CAE Usage: Interaction module: Connector→Assignment→Create: select wires connected to ground Components of relative motion Connector elements have relative displacements and rotations that are local to the element. These relative displacements and rotations are referred to as components of relative motion. In the three-dimensional case connector elements use 12 nodal degrees of freedom to define six relative motion components: three displacements and three rotations in element local directions. In two dimensions six nodal degrees of freedom define three relative motion components: two displacements and one rotation. The components of relative motion are either constrained or unconstrained (“available”), depending upon the definition of the connector element. Constrained components of relative motion Constrained components of relative motion are displacements and rotations that are fixed by the connector element. In connector elements with constrained components of relative motion, Abaqus/Standard uses Lagrange multipliers to enforce the kinematic constraints. Accordingly, in Abaqus/Standard the constraint forces and moments carried by the element appear as additional solution variables. The number of additional solution variables is equal to the number of constrained components of relative motion. In Abaqus/Explicit the constraints are enforced using an augmented Lagrangian technique for which no additional solution variables are needed. Available components of relative motion Available components of relative motion are displacements and rotations that are not constrained kinematically and, hence, specifying time-dependent motion, applying loading, or assigning complex interactions, such as contact or friction. Many connection types have available components of relative motion, and their meaning is described in “Connection-type library,” Section 31.1.5, for each individual connection type. remain available for defining material-like behavior, Defining the connection attributes The connection attributes define the connector element’s function. In the most general case you specify the following attributes: • the connection type or types, • the local directions associated with the connector’s nodes, • additional data for certain connection types, and • the connector behavior. The connector definition that is defined with these attributes is associated with a set of connector elements. Input File Usage: Abaqus/CAE Usage: *CONNECTOR SECTION, ELSET=name Interaction module: Connector→Geometry→Create Wire Feature Connector→Section→Create: Name: connector section name Connector→Assignment→Create: select wires: Section: connector section name Defining the connection type Abaqus provides a comprehensive library of connection types. See “Connection-type library,” Section 31.1.5, for the available connection types. The connection types are divided into three categories: basic connection components, assembled connections, and complex connections. The basic connection components affect either translations or rotations on the second node. A connector element may include one translational basic connection component and/or one rotational basic connection component. The assembled connections are constructed from the basic connection components. They are provided for convenience and cannot be combined in the same connector element definition with a basic connection component or other assembled connections. Complex connections affect a combination of degrees of freedom at the nodes in the connection and cannot be combined with other connection components. The connection type is specified as: • a single basic connection type (translational or rotational), • one translational and one rotational basic connection type, • one assembled connection type, or • one complex connection type. Input File Usage: Use one of the following options: Abaqus/CAE Usage: *CONNECTOR SECTION, ELSET=name basic connection type, basic connection type *CONNECTOR SECTION, ELSET=name assembled connection or complex connection Interaction module: Connector→Section→Create: Connection Category: Basic, Translational type: translational basic connection type and/or Rotational type: rotational basic connection type or Connector→Section→Create: Connection Category: Assembled/Complex, Assembled/Complex type: assembled connection or complex connection Defining the local connector directions Local directions at the nodes are often required to define the connection types used to define the connector element. The local directions and how they are used to define the connection are described in “Connection-type library,” Section 31.1.5. In the most general case the connection type uses two sets of local directions, which are defined as described in “Orientations,” Section 2.2.5. The names associated with the two orientation definitions must be referred to from the connector section definition. Input File Usage: Use the following options for the most general case: *ORIENTATION, NAME=orientation_1 *ORIENTATION, NAME=orientation_2 *CONNECTOR SECTION, ELSET=name basic connection type(s) or assembled connection orientation_1 for first node (or ground), orientation_2 for second node (or ground) Abaqus/CAE Usage: Interaction module: Connector→Assignment→Create: select wires: Orientation 1, Orientation 2: Edit: select the orientations for the first and second points, respectively, of the selected wires Degree of freedom activation and co-rotation of connection directions Many connection types either require connection directions at the nodes on the element or allow optional directions to be defined. In cases where an orientation definition is permitted for defining connection directions (required or optional), connector elements activate the rotational degrees of freedom at the nodes to which they are attached, if they do not exist already. The only exception is connection type JOIN, for which connection directions are optional at the first node of the element, but rotation degrees of freedom are not activated. The connector element’s orientation directions co-rotate with the rotational degrees of freedom at the corresponding node on the element. If there is no element with rotational degrees of freedom or rotation constraint (such as an equation or a multi-point constraint) attached to the node, you must ensure that sufficient rotational boundary conditions are provided to avoid numerical singularities associated with unconstrained rotational degrees of freedom. Connection type JOIN uses fixed directions when rotational degrees of freedom are not active at the nodes on the connector element. Example Figure 31.1.2–1 illustrates the use of the CONN3D2 element to connect two bodies with a cylindrical- like connector oriented at 60° from the global 1-axis. On the left is a schematic representation of the connection to be modeled; on the right is a representation of the equivalent finite element model. See “Connection-type library,” Section 31.1.5, for a list of connector type names. extensible range 7.5 node 12 1 (local orientation) node 11 Figure 31.1.2–1 Simplified connector model of a shock absorber. The connection requires node b to remain on the line of the shock absorber, which is determined by the position and orientation directions of node a. Furthermore, the two rotation components perpendicular to the line of the shock absorber at node b must be the same as those at node a. Hence, the only relative motion components permitted in the connection are the displacement of node b relative to node a along the line of the shock absorber and the rotation of node b relative to node a about the line of the shock absorber. This displacement and this rotation are the available components of relative motion. The connector is defined using the following lines in the input file: *ELEMENT, TYPE=CONN3D2, ELSET=shock 101, 11, 12 *CONNECTOR SECTION, ELSET=shock slot, revolute ori60, *ORIENTATION, NAME=ori60 **Defines the local 1-direction along the slot (required) **Also defines the rotation axis for the revolute (required) 0.5, 0.866025, 0.0, -0.866025, 0.5, 0.0 Alternatively, you could use the assembled connection type CYLINDRICAL instead of the two basic connection types SLOT and REVOLUTE. Defining additional connection type data Some connection types allow additional data to define the kinematic behavior of the connector. For example, the connection type FLOW-CONVERTER allows you to specify a scaling factor for material flow at node b. See “Connection-type library,” Section 31.1.5, for more information. Defining the connector behavior Abaqus provides comprehensive kinetic behavior modeling in the available components of relative motion. Defining connector behavior is optional and can be used to incorporate spring, dashpot, locking, friction, plasticity-like effects, and failure. The kinetic modeling node-to-node contact, capabilities in connectors are described in detail in “Connector behavior,” Section 31.2.1. Using connector elements in two-dimensional and axisymmetric analysis Not all connection types can be used with element type CONN2D2. The connection-type library contains many connection types whose mechanics are valid for three-dimensional analyses only. In other cases the local directions required in the definition of the connection type conflict with the two-dimensional coordinate system. See “Connection-type library,” Section 31.1.5, for more information. Using multiple connector elements in parallel Connector elements in Abaqus allow most physical connections to be modeled with a single connector element. However, in certain circumstances more complex connections or output considerations may require multiple connector elements to be used in parallel. This is accomplished by defining two or more connector elements between the same nodes. In this case you must ensure that a constrained component of relative motion in one connector element is not constrained (either by a kinematic constraint or through motion specified as described in “Connector actuation,” Section 31.1.3) by one of the other connector elements. Multiple connector elements are sometimes used in parallel to obtain output in different coordinate systems. For a connector element between two bodies, the local directions at the nodes can be determined by the requirements of the connection type. However, output may be needed in a different, possibly co-rotating, coordinate system. For example, the angular acceleration history could be reported in a local, body-fixed coordinate system (other than the one used to define the connector element) by using a second connector element (such as connection type CARDAN) that does not impose kinematic constraints or use connector behavior but aligns with the desired local output directions. Defining connectors in a model that contains parts and an assembly An Abaqus model can be defined in terms of an assembly of part instances . Connector elements can be defined at either the part level or the assembly level in such a model. Using connector elements with nodal transformations Nodal transformations can be defined for either node connected to the connector element. Since these transformations affect only the nodal degrees of freedom, their use does not affect the behavior of the connector element. Connector elements operate on components of motion local to the connection. Using nonlinear connections in geometrically linear analyses If a connector element with a nonlinear kinematic constraint is used in a geometrically linear analysis, the kinematic constraint is linearized. For example, if connection type LINK is used in a geometrically linear analysis, the distance between the two nodes is held constant after projection onto the direction of the line between the original positions of the nodes. The difference should be noticeable only if the magnitudes of the rotations and displacements are not small. Mismatched masses at connector nodes in Abaqus/Explicit If the nodes of a connector element in Abaqus/Explicit have masses that are highly mismatched, the implicit solver may encounter convergence problems due to the resulting ill-conditioned coefficient matrix. To prevent this from happening, if the nodal masses or rotary inertias of a connector element differ by more than three orders of magnitude, Abaqus/Explicit adds mass/rotary inertia to the connector element node that has the smaller mass/rotary inertia. The mass/rotary inertia added is negligibly small (less than three orders of magnitude smaller) compared to the larger of the connector element’s nodal inertias. This additional mass almost never affects the solution significantly. However, in certain situations (for example, for a strongly dynamic analysis that has connector elements with highly mismatched nodal masses) this adjustment may have a noticeable effect. Connector output The connector element force, moment, and kinematic output is defined in “Connector element library,” Section 31.1.4. These output quantities include total, elastic, viscous, and friction forces and moments. In addition, reaction forces and moments caused by connector stops and locks are available as well as connector contact forces used for friction calculation. To obtain accurate reaction force and moment output for connectors from Abaqus/Explicit, it may sometimes be necessary to run the analysis in double precision. In such situations a double precision run will also yield a better estimate of the work done by the reaction forces and moments, thereby providing a more accurate value of the energy due to the external work reported by Abaqus/Explicit. Kinematic output includes relative position, relative displacement, relative velocity, relative acceleration, frictional slip, and constitutive displacements (the displacement used in the elastic force and hysteretic friction calculations defined as the difference between the current relative positions and the reference positions; see “Defining reference lengths and angles for constitutive response” in “Connector behavior,” Section 31.2.1). For relative rotations the Abaqus convention of reporting angles between radians is not used with connector elements. Connector element output of angles and rotational components or relative motion includes accumulated multiple rotations whose magnitudes can be arbitrarily large. Energy output is available, as are output flags to identify whether a connector has failed (in Abaqus/Explicit only), locked, or reached a connector stop. and In a geometrically linear step in Abaqus/Standard the relative position output variable does not change (in the same fashion that the nodal coordinates are output). Therefore, care must be exercised in interpreting output for connector stops and locks since they use updated coordinates. Using connector elements for output only Connector elements defined without kinematic constraints or constitutive behavior can be used to monitor kinematic output in local coordinate systems. Quantities of interest include relative position, displacement, velocity, and acceleration in local coordinate parametrization. Finite rotation parametrizations include Euler and Cardan angles, rotation vector, and flexion-torsion-sweep. For an example that uses a connector element to monitor Euler angles, see “Motion of a rigid body in Abaqus/Standard,” Section 1.3.6 of the Abaqus Benchmarks Manual. In Abaqus/Explicit all such connectors are solved without invoking the implicit solver, which leads to better performance in domain parallel mode (particularly when such connectors nodes overlap with other constraints such as slave nodes of tie constraints). 31.1.3 CONNECTOR ACTUATION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • *CONNECTOR LOAD • *CONNECTOR MOTION • “Defining a connector force,” Section 16.9.13 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a connector moment,” Section 16.9.14 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a connector displacement boundary condition,” Section 16.10.5 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a connector velocity boundary condition,” Section 16.10.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a connector acceleration boundary condition,” Section 16.10.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Connector actuation: • is meant to model situations, such as deployment maneuvers, where a motor attached to the body loads the connection with an internal force or moment history or a hydraulic system imposes a known motion; • can be used to fix available components of relative motion; and • consists of driving an available component of relative motion by a prescribed displacement (rotation) or by a specified force (moment). The prescribed relative motions and loads are in the local directions associated with the available components of relative motion for the connector. Prescribing displacements/rotations for available components of relative motion that also include connector stop or connector lock behaviors may lead to overconstraints. Abaqus will issue a warning message if an overconstraint occurs. Fixing available components of relative motion A common practice is to fix available components of motion. Such fixed motion conditions can be used to customize connection types for specific applications. As an example, the REVOLUTE connection type uses the local 1-direction as the shared revolute axis and, hence, the available component of relative motion. If, for convenience, a revolute connection about the local 3-direction were needed, you could fix the relative rotations about the local 1- and 2-directions in a CARDAN connection type. In doing so, a connection type identical to the REVOLUTE connection type would be created; however, the shared axis would be the local 3-direction instead of the local 1-direction. An example is provided later in this section in which the pin part of a pin-in-slot connection is modeled with a CARDAN connection type with fixed rotations. Input File Usage: Use the following option in the model portion of the input file to fix available connector components of relative motion: Abaqus/CAE Usage: *CONNECTOR MOTION Load module: Create Boundary Condition: Step: Initial: Mechanical: Connector displacement Displacement-controlled actuation You can specify a relative displacement, velocity, or acceleration between two parts in the connector’s local directions in a manner similar to defining a boundary condition . You specify the connector element set name or connector element number; the component number identifying the available component of relative motion being actuated; and the value of the relative displacement, velocity, or acceleration. You cannot specify the motion of connectors in a subspace dynamic analysis. Input File Usage: Use the following option in the history portion of the input file to specify a relative displacement for a connector: *CONNECTOR MOTION, AMPLITUDE=name, OP=MOD or NEW, TYPE=DISPLACEMENT Use the following option in the history portion of the input file to specify a relative velocity for a connector: *CONNECTOR MOTION, AMPLITUDE=name, OP=MOD or NEW, TYPE=VELOCITY Use the following option in the history portion of the input file to specify a relative acceleration for a connector: *CONNECTOR MOTION, AMPLITUDE=name, OP=MOD or NEW, TYPE=ACCELERATION Abaqus/CAE Usage: Load module: Create Boundary Condition: Mechanical: Connector displacement, Connector velocity, or Connector acceleration Example Figure 31.1.3–1 illustrates a pin-in-slot connection oriented at 45° from the global 1-axis modeled with element type CONN3D2. 2.0 15.0 body 2 node 120 ⇒ node 110 node 120 1 (local orientation) node 110 45° body 1 global directions Figure 31.1.3–1 A pin-in-slot connection modeled with SLOT and CARDAN connection types. The figure on the left is a schematic representation of the connection to be modeled, while the figure on the right is the finite element mesh. Displacements in the slot are allowed only along the line of the slot, and connection type SLOT is appropriate for enforcing these kinematics. Assume the pin and slot are constructed in such a way that the only rotation of the pin relative to the slot is along the local 3-direction. This is a revolute constraint; however, basic rotation connection type REVOLUTE uses the local 1-direction as the revolute axis. In this case connection type CARDAN combined with a specified constraint can be used to define a revolute-type connection with the appropriate revolute axis. For illustrative purposes assume the connection is actuated by a rotational velocity of radians per second around the pin’s axis. Using input parametrization for convenience, the following lines are used: *PARAMETER PI = 3.141592 rotangvel = PI/4 ... *ELEMENT, TYPE=CONN3D2, ELSET=pininslot 101, 110, 120 *CONNECTOR SECTION, ELSET=pininslot cardan, slot ori45, *CONNECTOR MOTION pininslot, 4 pininslot, 5 *ORIENTATION, NAME=ori45 0.707, 0.707, 0.0, -0.707, 0.707, 0.0 ... *STEP ... *CONNECTOR MOTION, TYPE=VELOCITY pininslot, 6, ... *END STEP Force-controlled actuation You can specify concentrated loads applied to the available components of relative motion in a manner similar to defining concentrated loads for other elements in Abaqus . However, connector loads are always follower loads that rotate with the rotation of the available components of relative motion as the connector element moves. You specify the connector element set name or connector element number, the component number identifying the available component of relative motion being loaded, and the value of the actuation force or moment. Input File Usage: Abaqus/CAE Usage: Use the following option in the history portion of the input file to specify a concentrated load for a connector: *CONNECTOR LOAD, AMPLITUDE=name, OP=MOD Load module: Create Load: Mechanical: Connector force or Connector moment Example Returning to the example in Figure 31.1.3–1, assume that the pin is pushed along the slot by a constant force of 1000.0 units (for example, through a hydraulic system). The following lines should be added to the input file: *STEP ... *CONNECTOR LOAD pininslot, 1, 1000.0 ... *END STEP Connector actuation in linear perturbation procedures Nonzero magnitude connector motions are allowed only in the eigenvalue buckling, direct-solution steady-state dynamic, and linear static perturbation procedures. Any nonzero magnitude specified during an eigenfrequency extraction procedure is ignored, and the specified available component of relative motion is held fixed. Connector motions cannot be used in any modal-based procedure. In direct-solution steady-state dynamic analyses the real and imaginary parts of any available connector component of relative motion are either restrained or unrestrained simultaneously; it is physically impossible to have one part restrained and the other part unrestrained. Abaqus/Standard will automatically restrain both the real and the imaginary parts of a component of relative motion even when only one part is prescribed specifically. The unspecified part will be assumed to have a perturbation magnitude of zero. A nonzero prescribed connector motion in an eigenvalue buckling step will contribute to the incremental stress and, thus, will contribute to the differential initial stress stiffness. When prescribing nonzero connector motions, you must interpret the resulting eigenproblem carefully. See the discussion for boundary conditions in “Eigenvalue buckling prediction,” Section 6.2.3, for more details. In steady-state dynamic analyses both real and imaginary connector loads can be applied in a manner similar to concentrated loads . Multiple connector load cases can be defined in random response analyses in the same manner as concentrated loads. Connector loads are ignored during an eigenfrequency extraction analysis. 31.1.4 CONNECTOR ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connector elements,” Section 31.1.2 • “Connection-type library,” Section 31.1.5 • *CONNECTOR BEHAVIOR • *CONNECTOR LOAD • *CONNECTOR SECTION Overview This section provides a reference to the connector elements available in Abaqus/Standard and Abaqus/Explicit. Element types Connector in a plane CONN2D2 Connector element between two nodes or ground and a node. Active degrees of freedom 1, 2, 6 for the most general connection types. Additional solution variables In Abaqus/Standard there can be up to three additional constraint variables related to forces and a moment associated with the connector. The number of additional constraint variables depends on the connection type. Connector in space CONN3D2 Connector element between two nodes or ground and a node. Active degrees of freedom 1, 2, 3, 4, 5, 6 for the most general connection types. Additional solution variables In Abaqus/Standard there can be up to six additional constraint variables related to forces and moments associated with the connector. The number of additional constraint variables depends on the connection type. Nodal coordinates required CONN2D2: X, Y CONN3D2: X, Y, Z Element property definition Input File Usage: Abaqus/CAE Usage: *CONNECTOR SECTION Interaction module: Connector→Section→Create Element-based loading Use connector loads to apply loading to the available components of relative motion. Prescribe connector motion to specify relative kinematics (zero or nonzero values) for the available components of relative motion. See “Connector actuation,” Section 31.1.3, for details. Element output Total force components CTF1 CTF2 CTF3 CTM1 CTM2 CTM3 Total force in the 1-direction. Total force in the 2-direction. Total force in the 3-direction. Total moment about the 1-direction. Total moment about the 2-direction. Total moment about the 3-direction. The total force is obtained as CTF = CEF + CVF + CUF + CSF + CRF – CCF. Elastic force components CEF1 CEF2 CEF3 CEM1 CEM2 CEM3 Elastic force in the 1-direction. Elastic force in the 2-direction. Elastic force in the 3-direction. Elastic moment about the 1-direction. Elastic moment about the 2-direction. Elastic moment about the 3-direction. Elastic displacement components CUE1 CUE2 Elastic displacement in the 1-direction. Elastic displacement in the 2-direction. CUE3 CURE1 CURE2 CURE3 Elastic displacement in the 3-direction. Elastic rotation about the 1-direction. Elastic rotation about the 2-direction. Elastic rotation about the 3-direction. Plastic relative displacement components CUP1 CUP2 CUP3 CURP1 CURP2 CURP3 Plastic relative displacement in the 1-direction. Plastic relative displacement in the 2-direction. Plastic relative displacement in the 3-direction. Plastic relative rotation about the 1-direction. Plastic relative rotation about the 2-direction. Plastic relative rotation about the 3-direction. Equivalent plastic relative displacement components CUPEQ1 CUPEQ2 CUPEQ3 CURPEQ1 CURPEQ2 CURPEQ3 CUPEQC Equivalent plastic relative displacement in the 1-direction. Equivalent plastic relative displacement in the 2-direction. Equivalent plastic relative displacement in the 3-direction. Equivalent plastic relative rotation about the 1-direction. Equivalent plastic relative rotation about the 2-direction. Equivalent plastic relative rotation about the 3-direction. Equivalent plastic relative motion for a coupled plasticity definition. Kinematic hardening shift force components CALPHAF1 CALPHAF2 CALPHAF3 CALPHAM1 CALPHAM2 CALPHAM3 Kinematic hardening shift force in the 1-direction. Kinematic hardening shift force in the 2-direction. Kinematic hardening shift force in the 3-direction. Kinematic hardening shift moment about the 1-direction. Kinematic hardening shift moment about the 2-direction. Kinematic hardening shift moment about the 3-direction. Viscous force components CVF1 CVF2 CVF3 CVM1 Viscous force in the 1-direction. Viscous force in the 2-direction. Viscous force in the 3-direction. Viscous moment about the 1-direction. CVM2 CVM3 Viscous moment about the 2-direction. Viscous moment about the 3-direction. Uniaxial force components Connector uniaxial behavior can be defined only in Abaqus/Explicit; therefore, there is no uniaxial force output available in Abaqus/Standard. CUF1 CUF2 CUF3 CUM1 CUM2 CUM3 Uniaxial force in the 1-direction. Uniaxial force in the 2-direction. Uniaxial force in the 3-direction. Uniaxial moment in the 1-direction. Uniaxial moment in the 2-direction. Uniaxial moment in the 3-direction. Friction force components CSF1 CSF2 CSF3 CSM1 CSM2 CSM3 CSFC Force due to frictional stress in the 1-direction. Force due to frictional stress in the 2-direction. Force due to frictional stress in the 3-direction. Frictional moment about the 1-direction. Frictional moment about the 2-direction. Frictional moment about the 3-direction. Force due to frictional stress in the instantaneous slip direction. Available only for predefined or user-defined coupled friction interactions. Contact force components generating friction CNF1 CNF2 CNF3 CNM1 CNM2 CNM3 CNFC Contact force generating friction in the 1-direction. Contact force generating friction in the 2-direction. Contact force generating friction in the 3-direction. Contact moment generating friction about the 1-direction. Contact moment generating friction about the 2-direction. Contact moment generating friction about the 3-direction. Contact force generating friction in the instantaneous slip direction. Total overall damage components CDMG1 CDMG2 CDMG3 CDMGR1 Overall damage variable in the 1-direction. Overall damage variable in the 2-direction. Overall damage variable in the 3-direction. Overall damage variable along the 1-direction. CDMGR2 CDMGR3 Overall damage variable along the 2-direction. Overall damage variable along the 3-direction. Connector force-based damage initiation criteria CDIF1 CDIF2 CDIF3 CDIFR1 CDIFR2 CDIFR3 CDIFC Connector force-based damage initiation criterion in the 1-direction. Connector force-based damage initiation criterion in the 2-direction. Connector force-based damage initiation criterion in the 3-direction. Connector force-based damage initiation criterion along the 1-direction. Connector force-based damage initiation criterion along the 2-direction. Connector force-based damage initiation criterion along the 3-direction. Connector force-based damage initiation criterion in the instantaneous slip direction. Connector motion-based damage initiation criteria CDIM1 CDIM2 CDIM3 CDIMR1 CDIMR2 CDIMR3 CDIMC Connector motion-based damage initiation criterion in the 1-direction. Connector motion-based damage initiation criterion in the 2-direction. Connector motion-based damage initiation criterion in the 3-direction. Connector motion-based damage initiation criterion along the 1-direction. Connector motion-based damage initiation criterion along the 2-direction. Connector motion-based damage initiation criterion along the 3-direction. Connector motion-based damage initiation criterion in the instantaneous slip direction. Connector plastic motion-based damage initiation criteria CDIP1 CDIP2 CDIP3 CDIPR1 CDIPR2 CDIPR3 CDIPC Connector plastic motion-based damage initiation criterion in the 1-direction. Connector plastic motion-based damage initiation criterion in the 2-direction. Connector plastic motion-based damage initiation criterion in the 3-direction. Connector plastic motion-based damage initiation criterion along the 1-direction. Connector plastic motion-based damage initiation criterion along the 2-direction. Connector plastic motion-based damage initiation criterion along the 3-direction. Connector plastic motion-based damage initiation criterion in the instantaneous slip direction. Connector lock or stop status CSLSTi Flags for connector stop and connector lock status . Friction-related accumulated slip CASU1 Accumulated frictional slip in the 1-direction. CASU2 CASU3 CASUR1 CASUR2 CASUR3 CASUC Accumulated frictional slip in the 2-direction. Accumulated frictional slip in the 3-direction. Accumulated frictional rotation about the 1-direction. Accumulated frictional rotation about the 2-direction. Accumulated frictional rotation about the 3-direction. Accumulated frictional slip in the instantaneous slip direction. Frictional instantaneous velocity in the slip direction (available only if friction is defined in the slip direction) CIVC Friction-related instantaneous velocity in the slip direction. Reaction force components due to kinematic constraints, connector locks, connector stops, and prescribed connector motion CRF1 CRF2 CRF3 CRM1 CRM2 CRM3 Connector reaction force in the 1-direction. Connector reaction force in the 2-direction. Connector reaction force in the 3-direction. Connector reaction moment about the 1-direction. Connector reaction moment about the 2-direction. Connector reaction moment about the 3-direction. Connector concentrated force components due to connector loads CCF1 CCF2 CCF3 CCM1 CCM2 CCM3 Connector concentrated force in the 1-direction. Connector concentrated force in the 2-direction. Connector concentrated force in the 3-direction. Connector concentrated moment about the 1-direction. Connector concentrated moment about the 2-direction. Connector concentrated moment about the 3-direction. Relative position components CP1 CP2 CP3 CPR1 CPR2 CPR3 Relative position in the 1-direction. Relative position in the 2-direction. Relative position in the 3-direction. Relative angular position in the 1-direction. Relative angular position in the 2-direction. Relative angular position in the 3-direction. Relative displacement components CU1 CU2 CU3 CUR1 CUR2 CUR3 Relative displacement in the 1-direction. Relative displacement in the 2-direction. Relative displacement in the 3-direction. Relative rotation in the 1-direction. Relative rotation in the 2-direction. Relative rotation in the 3-direction. Constitutive displacement components CCU1 CCU2 CCU3 CCUR1 CCUR2 CCUR3 Constitutive displacement in the 1-direction. Constitutive displacement in the 2-direction. Constitutive displacement in the 3-direction. Constitutive rotation in the 1-direction. Constitutive rotation in the 2-direction. Constitutive rotation in the 3-direction. Relative velocity components CV1 CV2 CV3 CVR1 CVR2 CVR3 Relative velocity in the 1-direction. Relative velocity in the 2-direction. Relative velocity in the 3-direction. Relative angular velocity in the 1-direction. Relative angular velocity in the 2-direction. Relative angular velocity in the 3-direction. Relative acceleration components CA1 CA2 CA3 CAR1 CAR2 CAR3 Relative acceleration in the 1-direction. Relative acceleration in the 2-direction. Relative acceleration in the 3-direction. Relative angular acceleration in the 1-direction. Relative angular acceleration in the 2-direction. Relative angular acceleration in the 3-direction. Connector failure status CFAILSTi Flags for connector failure status . Node ordering on elements or or 31.1.5 CONNECTION-TYPE LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connector elements,” Section 31.1.2 • “Connector element library,” Section 31.1.4 • *CONNECTOR BEHAVIOR • *CONNECTOR SECTION Overview The connection-type library contains: • translational basic connection components, which affect translational degrees of freedom at both nodes and may affect rotational degrees of freedom at the first node or at both nodes on the connector element; • rotational basic connection components, which affect only rotational degrees of freedom at both nodes on the connector element; • specialized rotational basic connection components, which in addition to rotational degrees of freedom affect other degrees of freedom at the nodes on the connector element; • assembled connections, which are predefined combinations of translational and rotational or translational and specialized rotational basic connection components; and • complex connections, which affect a combination of degrees of freedom at the nodes on the connector element and cannot be combined with any other connection component. Using the connection-type library Each connection type is described in the connection-type library. Each library entry includes a figure, which relates the physical behavior to the idealized model and defines the local coordinate directions. Following the figure, each library entry defines kinematic constraints; constraint forces and moments internal to the connection; components of relative motion available for defining the connector behavior, connector motion, or connector loads (called available components); and kinetic forces and moments conjugate to the available components of relative motion. If appropriate, a discussion of the predicted Coulomb-like friction in the connection is included. Finally, the connection type is summarized in a table. Connection figures A schematic drawing of each connection type is included along with the Abaqus idealization of the connection. The idealization indicates in what sense available components of relative motion are measured and how the nodes’ positions and orientation directions define the connection. When orientation directions are used to define the connection, the idealization shows these local directions at the appropriate nodes. If available components of relative motion exist in the connection, they are indicated in the figure as free relative motions. Figure 31.1.5–1 shows the connection figure for the REVOLUTE connection type, which affects only rotations. It has one available component (the rotation about the shared axis), requires an orientation at node a, and allows an optional orientation at node b. eb eb eb ea ea ea ea eb Figure 31.1.5–1 Example connection type: REVOLUTE. Orientation directions , where The orientation directions at node a (the first node on the connector element) are indicated as unit base vectors . When orientation directions are required at a node, you must define them as described in “Orientations,” Section 2.2.5. If orientation directions are optional but not provided at node a, the global directions are used by default. If orientation directions are optional but not provided at node b, the orientation directions from node a are used by default. . Similarly, the orientation directions at node b are indicated as Connector elements activate rotational degrees of freedom at the nodes to which they are attached if they do not exist already and an orientation is permitted at that node. The only exception is connection type JOIN, where an orientation is optional at node a but rotation degrees of freedom are not activated. The orientation directions co-rotate with the rotation of the node to which they are attached (with the exception of connection type JOIN, which uses fixed directions when rotation degrees of freedom are not active at node a). If there are no elements with rotational degrees of freedom attached to the node, rotational multi-point constraints, or rotational equations, you must ensure that sufficient rotational boundary conditions are provided to avoid numerical singularities associated with unconstrained rotational degrees of freedom. Components of relative motion and connector forces and moments The six components of relative motion, denoted , are defined in the description and for each connection, where needed. These components include constrained and available components of relative motion. Forces and moments are denoted and . These quantities are either constraint forces and moments, which enforce the kinematic constraints on the constrained components of relative motion, or kinetic forces and moments, which are the work conjugate variables to the available components of for relative motion. For example, the REVOLUTE connection type has one available component of relative motion, and the local , and two kinematic rotation constraints (equivalent to setting two rotation components, , to zero). Conjugate to the available rotation component is the kinetic moment acting about -direction. In general, kinetic forces and moments include the effects of connector behaviors, such as elastic springs, viscous damping, friction, and reaction forces and moments due to connector stops and locks. For constitutive response defined as a function of displacement or rotation, the initial position may not correspond with the reference position where constitutive forces and moments are zero. You can define reference lengths and angles (given in degrees) for connector behavior as described in “Defining reference lengths and angles for constitutive response” in “Connector behavior,” Section 31.2.1. These reference quantities define , the connector constitutive displacements and rotations. These constitutive displacements and rotations are used only to define constitutive response and differ from the relative displacements and rotations measured in the connector elements only when you define the reference lengths or angles. and As an example, if the REVOLUTE connection included linear spring and dashpot behavior combined with a connector stop, is the spring stiffness, where by the connector stop. In the REVOLUTE connection there are two constraint moment components, about is the dashpot coefficient, and is the reaction moment caused about and . Interpreting connector forces and moments -direction aligned with the global X-direction and the local The kinematic constraint and kinetic forces and moments are always computed as work conjugates of the kinematics in the connector (components of relative motion). In most connection types one direct consequence is that the constraint forces (and moments) in connectors are reported as the forces (and moments) applied at the second node but in the local system associated with the first node. Since the kinematics are complex in many of the connection types, the connector forces and moments can be somewhat surprising upon first inspection. For example, consider the case of a HINGE connection defined with the local -direction aligned with the global Y-direction. Assume that the second connector node is grounded and that the first node is subjected to a concentrated load along the global Y-direction. If the only available relative rotation in the HINGE is constrained with a zero-valued connector motion, the second node does not rotate with respect to the first node and the connector reaction force along the local -direction matches the applied load while the other two connector reaction forces are zero. However, if a nonzero connector motion is specified, the first connector reaction force is still zero while both the second and third connector reaction forces are nonzero and only the vector-norm of these two forces matches the applied load. In both cases the only nonzero nodal reaction force at the second connector node is the one in the global Y-direction, as dictated by the equilibrium in a free body diagram. Hence, the connector reaction forces and nodal reaction forces are not equivalent in most cases. Coulomb-like friction behavior Coulomb-like friction behavior is possible for any connection type that has available components of relative motion; see “Connector friction behavior,” Section 31.2.5, for details. Friction behavior requires a “tangent” direction (the direction in which slipping may occur) and a “normal” direction (the direction perpendicular to the contacting surfaces). In the most general case you define the normal force causing friction in the connector. However, Abaqus predefines friction behavior for a limited number of connection types, as discussed in the connection-type library in this section. In these predefined friction cases you do not have to define the contact normal force. Summary table Each connection library entry includes a table summarizing the connection type. This summary table indicates whether the connection type is basic, assembled, or complex. It gives the kinematic constraints; constraint force or moment components; available components of relative motion; “kinetic” force or moment components following from the constitutive behavior in the available components of relative motion; which orientation directions are required, optional, or ignored; how connector stops limit the available components of relative motion; what reference lengths and angles are used to define the constitutive behavior; what parameters are used for predefined Coulomb-like friction; and how the contact normal forces are defined by Abaqus in association with predefined Coulomb-like friction. Basic connection components Basic connection components are divided into three categories: • Translational basic connection components, which affect translational degrees of freedom at both nodes and may affect rotational degrees of freedom at the first node or at both nodes • Rotational basic connection components, which affect only rotational degrees of freedom at both nodes • Specialized rotational basic connection components, which in addition to rotational degrees of freedom affect other degrees of freedom at the nodes Only one translational basic connection component and one rotational or specialized rotational basic connection component can be used in the definition of a connector element. If a more complicated connection requires more basic connection components than this, use multiple connector elements attached to the same nodes. Translational basic connection components The following basic connection components affect translational degrees of freedom at both node a and node b. Some of these connector components affect rotational degrees of freedom at node a or at both node a and node b. Any basic connection component from this list can be used to define the translational behavior of a connector element. AXIAL CARTESIAN JOIN LINK PROJECTION CARTESIAN RADIAL-THRUST SLIDE-PLANE SLOT CONNECTION-TYPE LIBRARY Provide a connection between two nodes to measure the relative acceleration, velocity, and position of a body in a local coordinate system. This connection type is available only in Abaqus/Explicit. If it is defined in an Abaqus/Standard model, it will be converted internally to a CARTESIAN connector type. Provide a connection between two nodes that acts along the line connecting the nodes. Provide a connection between two nodes that allows independent behavior in three local Cartesian directions that follow the system at node a. Join the position of two nodes. Provide a pinned rigid link between two nodes to keep the distance between the two nodes constant. Provide a connection between two nodes that allows independent behavior in three local Cartesian directions that follow the system at both nodes a and b. Provide a connection between two nodes that allows different behavior for radial and thrust displacements. Provide a slide-plane connection to make the position of the second node remain on a plane defined by the orientation of the first node and the initial position of the second node. Provide a slot connection to make the position of the second node remain on a line defined by the orientation of the first node and the initial position of the second node. Rotational basic connection components The following basic connection components affect only rotational degrees of freedom at the nodes in the connection. Any basic connection component from this list can be used to define the rotational behavior of a connector element. ALIGN CARDAN CONSTANT VELOCITY EULER FLEXION-TORSION Provide a connection between two nodes that aligns their local directions. Provide a rotational connection between two nodes parameterized by Cardan (or Bryant) angles. Provide a constant velocity connection between two nodes. Provide a rotational connection between two nodes parameterized by Euler angles. Provide a connection between two nodes that allows different behavior for flexural and torsional rotations. PROJECTION FLEXION- TORSION REVOLUTE ROTATION Provide a connection between two nodes that allows different behavior for two flexural rotations and one torsional rotation. Provide a revolute connection between two nodes. Provide a rotational connection between two nodes parameterized by the rotation vector. ROTATION-ACCELEROMETER Provide a connection between two nodes to measure the relative angular acceleration, velocity, and position of a body in a local coordinate system. This connection type is available only in Abaqus/Explicit. If it is defined in an Abaqus/Standard model, it will be converted internally to a CARDAN connector type. Provide a universal connection between two nodes. UNIVERSAL Specialized rotational basic connection components The following basic connection component affects rotational and other non-translational degrees of freedom at the nodes in the connection. The specialized rotational basic connection component can be combined with translational basic connection components. FLOW-CONVERTER Provide a means of converting the material flow (degree of freedom 10) at a connector node into a rotation. Assembled connections Assembled connections are included for convenience. Each assembled connection is created by combinations of basic connection components. The equivalent basic connection components used for each assembled connection are listed in parentheses. (JOIN + Provide a rigid beam connection between two nodes. ALIGN) Provide a connection between two nodes that allows independent behavior in three local Cartesian directions that follow the system at both nodes a and b and that allows different behavior in two flexural rotations and one torsional rotation. (PROJECTION CARTESIAN + PROJECTION FLEXION-TORSION) Join the position of two nodes, and provide a constant velocity connection between their rotational degrees of freedom. (JOIN + CONSTANT VELOCITY) Provide a slot connection between two nodes, and constrain the rotations by a revolute connection. (SLOT + REVOLUTE) Join the position of and provide a revolute connection between their rotational degrees of freedom. (JOIN + REVOLUTE) two nodes, 31.1.5–6 BEAM BUSHING CVJOINT CYLINDRICAL Provide a slide-plane connection between two nodes with a revolute connection about the normal direction to the plane. The PLANAR connection creates a local two-dimensional system in three-dimensional analyses. (SLIDE-PLANE + REVOLUTE) Join the position of two nodes, and convert material flow into rotation. (JOIN + FLOW-CONVERTER) Provide a slot connection between two nodes, and align their three local axis directions. (SLOT + ALIGN) Join the position of two nodes, and provide a universal connection between their rotational degrees of freedom at the nodes. (JOIN + UNIVERSAL) Join the position of two nodes, and align their three local axis directions. (JOIN + ALIGN) PLANAR RETRACTOR TRANSLATOR UJOINT WELD Complex connections Complex connections affect a combination of degrees of freedom at the nodes in the connection and cannot be combined with other connection components. They typically model highly coupled physical connections. SLIPRING Model material flow and stretching between two points of a belt system (such as an automotive seat belt). Connection-type library The following descriptions list all the basic connection components and assembled connections in alphabetical order. ACCELEROMETER Connection type ACCELEROMETER provides a convenient way to measure the relative position, velocity, and acceleration of a body in a local coordinate system. These kinematic quantities are measured relative to the motion of node a and are reported in the coordinate system of node b. Each node of the connector can translate and rotate independently, although fixing the first of the two nodes to ground is more common. With the first node fixed, connection type ACCELEROMETER provides a convenient way to measure the local components of the velocity and acceleration in a coordinate system fixed to a moving body (for example, an accelerometer). Connection type ACCELEROMETER is available only in Abaqus/Explicit. It is the translation counterpart relative to connection type ROTATION-ACCELEROMETER, which measures angular position, velocity, and acceleration. ACCELEROMETER connections cannot be used in two-dimensional and axisymmetric analyses in Abaqus/Explicit. ea ea ea Figure 31.1.5–2 Connection type ACCELEROMETER. Description The ACCELEROMETER connection does not impose kinematic constraints. It defines three local directions at node a and three local directions at node b. The ACCELEROMETER connection’s formulation is similar to that for the CARTESIAN connection. The ACCELEROMETER connection measures the position of node b relative to node a and There are no available components of relative motion for the ACCELEROMETER connection. The connector displacement components are where , , and are the initial coordinates of node b relative to node a. The ACCELEROMETER connection measures velocity and acceleration in the local directions In contrast to the CARTESIAN connection, the at node a as if node a were an inertial frame. and ACCELEROMETER connection reports the computed velocity and acceleration in the local directions at node b. Let . Then the ACCELEROMETER connection measures velocity and acceleration as be the transformation from to and where the derivatives above are time derivatives in a system moving with . In two-dimensional and axisymmetric analyses . Summary ACCELEROMETER Basic, assembled, or complex: Kinematic constraints: Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: Constitutive reference lengths: Predefined friction parameters: Contact force for predefined friction: Basic None None None None Optional Optional None None None None ALIGN Connection type ALIGN provides a connection between two nodes where all three local directions are aligned. If both local axes are given and do not align initially, their initial relative angular position is held constant. ea eb eb ea eb ea Figure 31.1.5–3 Connection type ALIGN. Description The ALIGN connection imposes kinematic constraints only. The local directions at node b are set equal to those at node a. If the local directions do not align initially, the ALIGN connection holds fixed the Cardan angles between the local orientation directions at node b, , and those at node a, . These fixed angular positions are the connector position output quantities. See connection type CARDAN for a definition of Cardan angles. The constraint moment enforcing the alignment of the local directions is In two-dimensional analysis . Summary ALIGN Basic, assembled, or complex: Basic Kinematic constraints: Constraint moment output: Available components: Kinetic moment output: Orientation at a: None None Optional ALIGN Orientation at b: Connector stops: Constitutive reference angles: Predefined friction parameters: Contact force for predefined friction: Optional None None None None AXIAL Connection type AXIAL provides a connection between two nodes where the relative displacement is along the line separating the two nodes. It models discrete physical connections such as axial springs, axial dashpots, or node-to-node (gap-like) contact. u1 Figure 31.1.5–4 Connection type AXIAL. Description The AXIAL connection does not constrain any component of relative motion. The distance between nodes a and b is The available component of relative motion, the change in distance separating the two nodes, and is defined as , acts along the line connecting the two nodes, measures where is the initial distance from node a to b. The connector constitutive displacement is The kinetic force is where In Abaqus/Standard an optional orientation can be provided at one of the nodes in an AXIAL connection to provide direction for the force if the nodes are coincident or when one of the nodes is a “ground node.” If the orientation is provided at both of the coincident nodes, the orientation at the first node in the connectivity will be used. The orientation definitions remain fixed during the analysis and will be ignored when the two nodes separate. Rotational degrees of freedom are not activated for connection type AXIAL. Symbol plots in the Visualization module of Abaqus/CAE display vector field output for the AXIAL connector along the 1-direction of the orientation at the first node instead of along the line joining the two nodes. If an orientation is not defined for the first node of the connector, the vector is displayed along the 1-direction of the global coordinate system. Summary AXIAL Basic, assembled, or complex: Kinematic constraints: Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: Basic None None Optional Optional Constitutive reference lengths: Predefined friction parameters: Contact force for predefined friction: None None BEAM Connection type BEAM provides a rigid beam connection between two nodes. eb eb ea eb ea ea Figure 31.1.5–5 Connection type BEAM. Description Connection type BEAM imposes kinematic constraints and uses local orientation definitions equivalent to combining connection types JOIN and ALIGN. Summary BEAM Basic, assembled, or complex: Assembled Kinematic constraints: JOIN + ALIGN Constraint force and moment output: Available components: Kinetic force and moment output: Orientation at a: Orientation at b: Connector stops: Constitutive reference lengths and angles: Predefined friction parameters: Contact force for predefined friction: None None Optional Optional None None None None BUSHING Connection type BUSHING provides a bushing-like connection between two nodes. It cannot be used in two-dimensional or axisymmetric analyses. attached to Part A deformable material attached to Part B deformable material (e.g. rubber) attached to Part A attached to Part B Figure 31.1.5–6 Connection type BUSHING. Description Connection type BUSHING does not constrain any components of relative motion and uses local orientation definitions equivalent to combining connection types PROJECTION CARTESIAN and PROJECTION FLEXION-TORSION. Summary BUSHING Basic, assembled, or complex: Assembled Kinematic constraints: Constraint force and moment output: Available components: None None BUSHING Kinetic force and moment output: Orientation at a: Orientation at b: Connector stops: Required Optional Constitutive reference lengths and angles: Predefined friction parameters: Contact force for predefined friction: None None CARDAN Connection type CARDAN provides a rotational connection between two nodes where the relative rotation between the nodes is parameterized by Cardan (or Bryant) angles. A Cardan-angle parameterization of finite rotations is also called a 1–2–3 or yaw-pitch-roll parameterization. Connection type CARDAN cannot be used in two-dimensional or axisymmetric analysis. When connection type CARDAN is used with connector behavior, the relative rotation axis with the highest resistance to rotational motion should be assigned to the second component of relative rotation (component number 5) to avoid “gimbal lock,” a singularity in the rotation parameterization for relative rotation angles . α rotation ea β rotation ea eb ea ea γ rotation ea eb ea e2 eb ea ea eb Figure 31.1.5–7 Connection type CARDAN. ea Description The CARDAN connection does not impose kinematic constraints. A CARDAN connection is a finite rotation connection where the local directions at node b are parameterized in terms of Cardan (or Bryant) angles relative to the local directions at node a. Local directions are positioned relative to by three successive finite rotations , , and as follows: 1. Rotate by 2. Rotate by 3. Rotate by radians about axis radians about the intermediate 2-axis, radians about axis ; . Rotation angle large (i.e., magnitude greater than should be moderate (magnitude less than ). The Cardan angles are determined by the local directions as ; and ), whereas and may be arbitrarily Here, m and n are integers that account for rotations with a magnitude greater than . The three available components of relative motion in the CARDAN connection are the changes in the Cardan angles positioning the local directions at node b relative to the local directions at node a. Therefore, where , , and are the initial Cardan angles. The connector constitutive rotations are and The kinetic moment in a CARDAN connection is determined from the three component relationships: and Summary CARDAN Basic, assembled, or complex: Kinematic constraints: Constraint moment output: Available components: Kinetic moment output: Orientation at a: Orientation at b: Connector stops: and Basic None None Required Optional Constitutive reference angles: Predefined friction parameters: Contact force for predefined friction: None None CARTESIAN Connection type CARTESIAN provides a connection between two nodes where the change in position is measured in three local connection directions for node a, shown in Figure 31.1.5–8. ea ea ea Figure 31.1.5–8 Connection type CARTESIAN. Description The CARTESIAN connection does not impose kinematic constraints. It defines three local directions at node a and measures the change in position of node b along these local coordinate directions. The local directions at node a follow the rotation of node a. The position of node b relative to node a is The available components of relative motion are and and where The connector constitutive displacements are , and , are the initial coordinates of node b relative to the local coordinate system at node a. The kinetic force is and In two-dimensional analysis , , , and . Summary CARTESIAN Basic, assembled, or complex: Kinematic constraints: Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: Basic None None Optional Ignored Constitutive reference lengths: Predefined friction parameters: Contact force for predefined friction: None None CONSTANT VELOCITY Connection type CONSTANT VELOCITY provides the rotational part of connection type CVJOINT. It cannot be used in two-dimensional or axisymmetric analysis. Furthermore, the connection type does not have available components of relative motion. To include connector behavior in flexural motion, use connection type FLEXION-TORSION with the torsion angle set to zero. This connection type models physical connectors that under certain conditions transmit a constant spinning velocity about misaligned shafts. ea ea eb eb eb ea Figure 31.1.5–9 Connection type CONSTANT VELOCITY. Description The shaft direction at node a is is stated as follows. In any configuration there are two unit length orthogonal vectors plane perpendicular to the shaft at node b. These vectors can be written , and the shaft direction at node b is . The constant velocity constraint in the and The angle is chosen such that and The constant velocity constraint requires that the angle is constant at all times. The constant velocity constraint is equivalent to constraining the torsion angle to be constant in a FLEXION-TORSION connection. The name “constant velocity” for this connection type derives from the following property. If the , have components only along each shaft, respectively, and direction), angular velocities of the two shafts, in the direction of the normal to the plane containing the two shafts (that is, along the the components of angular velocity along the respective shaft directions are equal: and Hence, the “spinning” angular velocity component is the same about each shaft. The constraint moment imposing the constant velocity constraint has a single component about the average shaft direction and is written Summary CONSTANT VELOCITY Basic, assembled, or complex: Basic Kinematic constraints: Constraint moment output: Available components: Kinetic moment output: Orientation at a: Orientation at b: Connector stops: Constitutive reference angles: Predefined friction parameters: Contact force for predefined friction: None None Required Optional None None None None CVJOINT Connection type CVJOINT joins the position of two nodes and provides a constant velocity constraint between their rotational degrees of freedom. Connection type CVJOINT cannot be used in two-dimensional or axisymmetric analysis. ea a, b eb ea eb 1eb ea Figure 31.1.5–10 Connection type CVJOINT. Description Connection type CVJOINT imposes kinematic constraints and uses local orientation definitions equivalent to combining connection types JOIN and CONSTANT VELOCITY. Summary CVJOINT Basic, assembled, or complex: Assembled Kinematic constraints: JOIN + CONSTANT VELOCITY Constraint force and moment output: Available components: Kinetic force and moment output: Orientation at a: Orientation at b: Connector stops: Constitutive reference lengths and angles: Predefined friction parameters: Contact force for predefined friction: None None Required Optional None None None None CYLINDRICAL Connection type CYLINDRICAL provides a slot connection between two nodes and a revolute constraint where the free rotation is about the line of the slot. It cannot be used in two-dimensional or axisymmetric analysis. ea eb ea ea eb ur1 eb u1 Figure 31.1.5–11 Connection type CYLINDRICAL. Description Connection type CYLINDRICAL imposes kinematic constraints and uses local orientation definitions equivalent to combining connection types SLOT and REVOLUTE. The connector constraint forces and moments reported as connector output depend strongly on the order and the location of the nodes in the connector . Since the kinematic constraints are enforced at node b (the second node of the connector element), the reported forces and moments are the constraint forces and moments applied at node b to enforce the CYLINDRICAL constraint. Thus, in most cases the connector output associated with a CYLINDRICAL connection is best interpreted when node b is located at the center of the device enforcing the constraint. This choice is essential when moment-based friction is modeled in the connector since the contact forces are derived on the connector forces and moments, as illustrated below. Proper enforcement of the kinematic constraints is independent of the order or location of the nodes. Friction Predefined Coulomb-like friction in the CYLINDRICAL connection defines the friction force (CSFC) along the instantaneous slip direction on the two contacting cylindrical surfaces (the pin and the sleeve) illustrated above. The table below summarizes the parameters that are used to specify predefined friction in this connection type as discussed in detail next. The frictional effect is formally written as where the potential in a direction tangent to the cylindrical surface on which contact occurs, normal force on the same cylindrical surface, and represents the magnitude of the frictional tangential tractions in the connector is the friction-producing is the friction coefficient. Frictional stick occurs if ; and sliding occurs if , in which case the friction force is . The normal force is the sum of a magnitude measure of friction-producing connector forces, , and a self-equilibrated internal contact force (such as from a press-fit assembly), : The magnitude measure of friction-producing connector contact force, , is defined by summing the following two contributions: • a radial force contribution, constraint): (the magnitude of the constraint forces enforcing the SLOT • a force contribution from “bending,” (the magnitude of the constraint moments enforcing the REVOLUTE constraint), by a length factor, as follows: , obtained by scaling the bending moment, where L represents a characteristic overlapping length between the shaft and the outer sleeve in the 1-direction. If L is 0.0, is ignored. Thus, where . The magnitude of the frictional tangential moment, is computed using where R is an effective radius of the shaft cross-section in the local 2–3 plane. The potential represents the magnitude of connector tangential tractions on the cylindrical contact surface due to simultaneous translation and rotation. The instantaneous slip direction is a result of combined motion in these directions. Summary CYLINDRICAL Basic, assembled, or complex: Assembled Kinematic constraints: SLOT + REVOLUTE Constraint force and moment output: Available components: Kinetic force and moment output: Orientation at a: Orientation at b: Connector stops: , , Required Optional Constitutive reference lengths and angles: , Predefined friction parameters: Required: R; optional: L, Contact force for predefined friction: EULER Connection type EULER provides a rotational connection between two nodes where the total relative rotation between the nodes is parameterized by Euler angles. An Euler-angle parameterization of finite rotations is also called a 3–1–3 or precession-nutation-spin parameterization. Connection type EULER cannot be used in two-dimensional or axisymmetric analysis. α rotation ea β rotation γ rotation ea eb ea eb ea ea ea ea e1 ea Figure 31.1.5–12 Connection type EULER. Description eb ea eb The EULER connection does not impose kinematic constraints. An EULER connection is a finite rotation connection where the local directions at node b are parameterized in terms of Euler angles relative to the local directions at node a. Local directions by three successive finite rotations are positioned relative to as follows: , and , ; 1. Rotate by 2. Rotate by 3. Rotate by ; radians about axis radians about the intermediate 1-axis, radians about axis . The Euler angles are determined by the local directions as Here i, j, and k are integers that account for rotations with magnitudes greater than . Initially, the intermediate rotation angle is chosen in the interval If the intermediate rotation is an even multiple of , . , where , the other two Euler angles become non-unique. In this case Similarly, if the intermediate rotation is an odd multiple of the other two Euler angles become nonunique as well. In this case , , where 0, , In both of these cases a singularity results in the rotation parameterization when the axes align. The EULER connection should be used in such a way that these axes do not align throughout the computation. For a singularity-free condition Abaqus will choose such that a smooth parameterization results for the above values of the intermediate angle . and and The available components of relative motion in the EULER connection are the changes in the Euler angles that position the local directions at node b relative to the local directions at node a. Therefore, where , , and are the initial Euler angles. The connector constitutive rotations are and The kinetic moment in a EULER connection is determined from the three component relationships: and and EULER Basic, assembled, or complex: Kinematic constraints: Constraint moment output: Available components: Basic None None 31.1.5–28 EULER Kinetic moment output: Orientation at a: Orientation at b: Connector stops: Required Optional Constitutive reference angles: Predefined friction parameters: Contact force for predefined friction: None None FLEXION-TORSION Connection type FLEXION-TORSION provides a rotational connection between two nodes. It models the bending and twisting of a cylindrical coupling between two shafts. In this case the response to twist rotations about the shafts may differ from the response to bending of the shafts. Connection type FLEXION-TORSION cannot be used in two-dimensional or axisymmetric analysis. The flexural part of the connection resists angular misalignment of the two shafts, whereas the torsional part of the connection resists relative rotations about the shafts. Connection type FLEXION- TORSION can be used in conjunction with connection type RADIAL-THRUST when resistance to relative radial and thrust displacements is modeled. ea eb ea ea Figure 31.1.5–13 Connection type FLEXION-TORSION. Description The FLEXION-TORSION connection does not TORSION connection describes a finite rotation by three angles: flexion, torsion, and sweep ( , The FLEXION- , and ). However, the flexion, torsion, and sweep angles do not represent three successive rotations. The flexion angle between two shafts measures the angle of misalignment of the two shafts and is always reported as a positive angle. The torsion angle measures the twist of one shaft relative to the other. impose kinematic constraints. – The sweep angle orients the rotation vector, in the plane, for the flexion motion. See Figure 31.1.5–13. Since the flexion angle is never negative, the sweep angle may undergo discontinuous jumps by up to radians when the flexion angle passes through zero. An analysis may give inaccurate results or may not converge if any jump occurs in the sweep angle. In general, the sweep angle is not used as an available component of relative motion for which connector behavior is defined. Rather, it is used to define angular dependence for the elastic constitutive response in flexion deformations (as an independent component in the connector elastic behavior definition). Since the sweep angle is restricted to the interval radians, any dependence on the sweep angle should be periodic, such that the to . Since is the same as behavior for is a singular point for which the sweep angle is not uniquely defined, it is strongly recommended that any connector behavior that defines flexural moment versus flexion angle gives zero moment at zero flexion angle. If connector behavior is defined in the sweep available component, the sweep moment must be zero at flexion angles . The FLEXION-TORSION connection is similar to a finite successive rotation parameterization 3–2–3. However, in terms of the 3–2–3 parameterization, the sweep angle is the first rotation angle, the flexion angle is the second rotation angle, and the torsion angle is the sum of the first and third rotation angles. and The first shaft direction at node a is , and the second shaft direction at node b is . Let the two shafts form an angle , called the flexion angle. Then, The flexion angle is a rotation by about the (unit) rotation vector where The torsion angle between the two shafts is defined as where where positive torsion angles are rotations about the positive The sweep angle measures the angle from to the projection of -direction, and m is an integer. onto the – plane. With this definition It follows that the flexion rotation vector, , can be written where A singularity in the definition of the sweep angles occurs when the flexion angle vanishes. In this ; that is, the torsion and sweep angle axes are coincident, and the two angles are no longer case independent. When , the sweep angle is assumed zero, . The available components of relative motion , , and are the changes in the flexion, torsion, and sweep angles and are defined as where angle and are the initial flexion and torsion angles, respectively. The initial value of the sweep is chosen to be zero if the shafts align initially. The connector constitutive rotations are and The kinetic moment in a FLEXION-TORSION connection is determined from the three component relationships: and Summary FLEXION-TORSION Basic, assembled, or complex: Kinematic constraints: Constraint moment output: Available components: Kinetic moment output: Orientation at a: Orientation at b: Connector stops: and Basic None None Required Optional Constitutive reference angles: Predefined friction parameters: Contact force for predefined friction: None None FLOW-CONVERTER Connection type FLOW-CONVERTER converts the relative rotation about a user-specified axis between the two nodes of the connector into material flow degree of freedom (10) at the second node of a connector element. This connection type can be used to model retractor and pretensioner devices in automotive seat belts or cable drums in winch-like devices. Belt or cable material is considered to be wrapped around an axle or a drum, and material can be spooled either into or out of the connector element. In certain cases, material flow needs to be converted into a displacement rather than a rotation. Examples include pretensioner devices for which experimental force vs. displacement data need to be specified. Although this connection type always converts the material flow into a rotation, the two modeling cases are equivalent. The experimentally available force vs. displacement data can be input directly as moment vs. rotation data for the same end result. This connection type activates degree of freedom 10 at the second node of a connector. As with any other nodal degree of freedom, you must be careful in constraining it. This is typically done by attaching the connector to a SLIPRING connector that is part of the belt system or by applying a boundary condition. FLOW-CONVERTER connections cannot be used in two-dimensional and axisymmetric analyses in Abaqus/Explicit. L W Figure 31.1.5–14 Connection type FLOW-CONVERTER. Description The FLOW-CONVERTER connection constrains the relative rotation between the two nodes about the third local direction, . The constraint can be written as , to the material flow at node b, is the relative nodal rotation between node a andb and where part of the associated connector section definition. By default, with the nodal rotation at node a. is a scaling factor specified as rotates . The local direction There are no available components of relative motion for this connection type; hence, kinetic behavior cannot be specified. However, the following kinematic quantities are available for output: which will be output as CPR1 and CPR2, respectively. The constraint moment is and Limitation At most two FLOW-CONVERTER connectors can share their second node where degree of freedom 10 is active. Summary FLOW-CONVERTER Basic, assembled, or complex: Specialized basic rotational Kinematic constraints: Constraint moment output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: Constitutive reference lengths: Predefined friction parameters: Contact force for predefined friction: None None Required Ignored None None None None HINGE Connection type HINGE joins the position of two nodes and provides a revolute constraint between their rotational degrees of freedom. Connection type HINGE cannot be used in two-dimensional or axisymmetric analysis. ea , eb ea a, b ea eb eb Figure 31.1.5–15 Connection type HINGE. Description Connection type HINGE imposes kinematic constraints and uses local orientation definitions equivalent to combining connection types JOIN and REVOLUTE. The connector constraint forces and moments reported as connector output depend strongly on the order and the location of the nodes in the connector element . Since the kinematic constraints are enforced at node b (the second node of the connector element), the reported forces and moments are the constraint forces and moments applied at node b to enforce the HINGE constraint. Thus, in most cases the connector output associated with a HINGE connection is best interpreted when node b is located at the center of the device enforcing the constraint. This choice is essential when moment-based friction is modeled in the connector since the contact forces are derived from the connector forces and moments, as illustrated below. Proper enforcement of the kinematic constraints is independent of the order or location of the nodes. Friction Predefined Coulomb-like friction in the HINGE connection relates the kinematic constraint forces and moments in the connector to a friction moment (CSM1) in the rotation about the hinge axis. The table below summarizes the parameters that are used to specify predefined friction in this connection type as discussed in detail next. A typical interpretation of the geometric scaling constants is illustrated in Figure 31.1.5–16. Since the rotation about the 1-direction is the only possible relative motion in the connection, the frictional effect is formally written in terms of moments generated by tangential tractions and moments generated by contact forces, as follows: L s Part B Pin 2Ra Part A 2R Contact on this face between Part A and Part B Figure 31.1.5–16 Illustration of the geometric scaling constants for a HINGE connection. where the potential connector in a direction tangent to the cylindrical surface on which contact occurs, producing normal moment on the same cylindrical surface, and stick occurs if ; and sliding occurs if represents the moment magnitude of the frictional tangential tractions in the is the friction- is the friction coefficient. Frictional , in which case the friction moment is is the sum of a magnitude measure of friction-producing connector , and a self-equilibrated internal contact moment (such as from a press-fit The normal moment . moments, assembly), : The magnitude measure of friction-producing connector contact moments, , is defined by summing the following contributions: • a moment from an axial force, is an effective friction arm associated with the constraint force in the axial direction (the radius could be interpreted as an average radius of the outer sleeve cylindrical sections as found in a typical door hinge or as an effective radius associated with the hinge end caps, if they exist; if is ignored); and , where is 0.0, and • a moment from normal forces to the cylindrical face, section in the local 2–3 plane and , where is itself a sum of the following two contributions: is the radius of the pin cross- – a radial force contribution, (the magnitude of the constraint forces enforcing the translation constraints in the local 2–3 plane): – a force contribution from “bending,” , obtained by scaling the bending moment, (the magnitude of the constraint moments enforcing the REVOLUTE constraint), by a length factor, as follows: represents a characteristic overlapping length between the pin and the sleeve. If is ignored. where is 0.0, Thus, where . The moment magnitude of the frictional tangential tractions, . Summary HINGE Basic, assembled, or complex: Assembled Kinematic constraints: JOIN + REVOLUTE Constraint force and moment output: Available components: Kinetic force and moment output: Orientation at a: Orientation at b: Required Optional HINGE Connector stops: Constitutive reference lengths: Predefined friction parameters: Required: ; optional: , , Contact moment for predefined friction: JOIN Connection type JOIN makes the position of two nodes the same. If the two nodes are not co-located initially, the position of node b is fixed relative to that of node a in a Cartesian coordinate system attached to node a. Even though an orientation is optional at node a, connection type JOIN does not activate rotational degrees of freedom at node a. ea a, b ea ea Figure 31.1.5–17 Connection type JOIN. Description The JOIN connection makes the position of node b equal to that of node a. If the two nodes are not coincident initially, the Cartesian coordinates of node b relative to node a are fixed. See connection type CARTESIAN for a definition of the Cartesian coordinates of node b relative to node a. If rotational degrees of freedom exist at node a, the local directions co-rotate with the node. The constraint force in the JOIN connection acts in the three local directions at node a and is where in two-dimensional analysis. Friction When used by itself, there is no predefined Coulomb-like friction in the JOIN connection, since there are no available components of relative motion for which friction can be defined. However, when the JOIN and REVOLUTE connection types are used together, the predefined friction is the same as the HINGE connection. When the JOIN and UNIVERSAL connection types are used together, the predefined friction is the same as the UJOINT connection. Summary JOIN Basic, assembled, or complex: Basic Kinematic constraints: JOIN Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: Constitutive reference lengths: Predefined friction parameters: Contact force for predefined friction: None None Optional Ignored None None None None LINK Connection type LINK maintains a constant distance between two nodes. Rotational degrees of freedom, if they exist, are not affected at either node. Figure 31.1.5–18 Connection type LINK. Description The LINK connection constrains the position of node b, distance between the two nodes is , to a constant distance from node a. The and is constant. The constraint force in the LINK connection acts along the line connecting the two nodes and is where Symbol plots in the Visualization module of Abaqus/CAE display vector field output for the LINK connector along the 1-direction of the orientation at the first node instead of along the line joining the two nodes. If an orientation is not defined for the first node of the connector, the vector is displayed along the 1-direction of the global coordinate system. Summary LINK Basic, assembled, or complex: Basic Kinematic constraints: Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: None None Ignored Ignored None LINK Constitutive reference lengths: Predefined friction parameters: Contact force for predefined friction: None None None PLANAR Connection type PLANAR provides a local two-dimensional system in a three-dimensional analysis. Connection type PLANAR cannot be used in two-dimensional or axisymmetric analysis. ea ea eb ea u2 ur1 u3 eb eb Figure 31.1.5–19 Connection type PLANAR. Description Connection type PLANAR imposes kinematic constraints and uses local orientation definitions equivalent to combining connection types SLIDE-PLANE and REVOLUTE. Friction Predefined Coulomb-like friction in the PLANAR connection relates the kinematic constraint forces and moments in the connector to the friction forces in the translations in the local 2–3 plane and the frictional moment in the rotation about the local 1-direction. These two frictional effects are discussed separately below. A. The frictional effect due to sliding in the 2–3 plane is formally written as where the potential connector in a direction tangent to the local 2–3 plane on which contact occurs, producing normal force on the same plane, and if represents the magnitude of the frictional tangential tractions in the is the friction- is the friction coefficient. Frictional stick occurs ; and sliding occurs if , in which case the friction force (CSFC) is is the sum of a magnitude measure of force-producing connector forces, : , and a self-equilibrated internal contact force, The normal force . The contact force magnitude is defined by summing the following two contributions: • a force contribution, and (the constraint force enforcing the SLIDE-PLANE constraint); • a force contribution from “bending,” , obtained by scaling the bending moment, (the magnitude of the constraint moments enforcing the REVOLUTE constraint), by a length factor, as follows: where R represents a characteristic radius of the “puck” (as illustrated in Figure 31.1.5–20) in the local 2–3 plane. If R is 0.0, is ignored. bend F1 bend 2R bend 2R Figure 31.1.5–20 Illustration of the effective internal friction contact forces. Thus, where . The magnitude of the frictional tangential moment, is computed using B. Since the frictional effects due to rotation about the 1-direction are quantified, the frictional effect is formally written in terms of moments generated by tangential tractions and moments generated by contact forces as where the potential connector about the 1-direction, axis, and occurs if represents the magnitude of the frictional tangential moment in the is the friction-producing normal moment about the same ; and sliding is the friction coefficient. Frictional stick in rotation occurs if . , in which case the friction moment (CSM1) is The normal moment is the sum of a magnitude measure of friction-producing connector moments, , and a self-equilibrated internal contact moment, : The contact moment magnitude is defined by summing the following two contributions: • a moment from a contact force in the 2–3 plane, SLIDE-PLANE constraint): (the constraint moment enforcing the where Figure 31.1.5–20) in the local 2–3 plane (if R is 0.0, from integrating moment contributions from a uniform pressure ( contact patch; and , R represents a characteristic radius of the “puck” (as illustrated in is ignored), and the 2/3 factor comes ) over the circular • a moment contribution from “bending,” enforcing the REVOLUTE constraint): (the magnitude of the constraint moments Thus, The magnitude of the frictional tangential tractions, is computed using Summary PLANAR Basic, assembled, or complex: Assembled Kinematic constraints: SLIDE-PLANE + REVOLUTE Constraint force and moment output: Available components: Kinetic force and moment output: Orientation at a: Orientation at b: Connector stops: Required Optional Constitutive reference lengths and angles: Predefined friction parameters: Optional: R, , Contact forces and moments for predefined friction: , PROJECTION CARTESIAN Connection type PROJECTION CARTESIAN provides a connection between two nodes where the response in three local connection directions (that is, the axes of the local Cartesian coordinate system) is measured. Unlike the CARTESIAN connection, which uses an orthonormal coordinate system that follows node a, the PROJECTION CARTESIAN connection uses an orthonormal system that follows the systems at both nodes a and b. The connector local directions used in the PROJECTION CARTESIAN connection are identical to those used in the PROJECTION FLEXION-TORSION connection. Connection type PROJECTION CARTESIAN is compatible with connection type PROJECTION FLEXION-TORSION and is appropriate for modeling the displacement response of bushing-like or spot-weld-like components. ea e3 eb e1 a, b e2 Figure 31.1.5–21 Connection type PROJECTION CARTESIAN. Description The PROJECTION CARTESIAN connection does not impose kinematic constraints. It defines three local directions as a function of the directions at both nodes a and b. These directions are the projection directions defined by the PROJECTION FLEXION-TORSION connection. The PROJECTION CARTESIAN connection measures the change in position of node b relative to node a along the (projection) coordinate directions . The position of node b relative to node a is The available components of relative motion are and and where directions. The connector constitutive displacements are , and , are the initial coordinates of node b relative to node a along the initial and The local directions in a PROJECTION CARTESIAN connection are “centered” between the systems at the two connector nodes. PROJECTION CARTESIAN connections are appropriate where isotropic or anisotropic material response is modeled and the local material directions evolve as a function of the rotations at both ends of the connection. The kinetic force is In two-dimensional analysis , , , and . Summary PROJECTION CARTESIAN Basic, assembled, or complex: Kinematic constraints: Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: Basic None None Optional Optional Constitutive reference lengths: Predefined friction parameters: Contact force for predefined friction: None None PROJECTION FLEXION-TORSION It models the bending and twisting of a cylindrical coupling between two shafts. Connection type PROJECTION FLEXION-TORSION provides a rotational connection between two nodes. In this case the response to twist rotations about the shafts may differ from the response to bending of the shafts. Connection type PROJECTION FLEXION-TORSION is similar to connection type FLEXION-TORSION. Whereas the FLEXION-TORSION connection has rotation parameterization angles consisting of total flexion, the PROJECTION FLEXION-TORSION connection has rotation parameterization angles consisting of two component flexion angles and a torsion angle. The flexion angle of the FLEXION-TORSION connection is the resultant flexion angle resulting from the two component flexion angles of the PROJECTION FLEXION-TORSION connection. Connection type PROJECTION FLEXION-TORSION cannot be used in two-dimensional or axisymmetric analysis. torsion, and sweep, The flexural part of the connection resists angular misalignment of the two shafts, whereas the torsional part of the connection resists relative rotations about the shafts. Connection type PROJECTION FLEXION-TORSION can be used in conjunction with connection type PROJECTION CARTESIAN when modeling the response of bushing-like or spot-weld-like components. ea e3 eb e1 a, b e2 Figure 31.1.5–22 Connection type PROJECTION FLEXION-TORSION. Description The PROJECTION FLEXION-TORSION connection does not impose kinematic constraints. The PROJECTION FLEXION-TORSION connection describes a finite rotation by three angles: flexion 1, flexion 2, and torsion ( , and ). However, the flexion 1, flexion 2, and torsion angles do not represent three successive rotations. The two component flexion angles ( ) make up the total flexion angle between two shafts and measure the angle of misalignment of the two shafts. The torsion angle measures the twist of one shaft relative to the other. and , The first shaft direction at node a is , and the second shaft direction at node b is . Let the two shafts form an angle , called the total flexion angle. Then, where The flexion angle is a rotation by about the (unit) rotation vector, where The PROJECTION FLEXION-TORSION connection is formulated in terms of the unit vector . See Figure 31.1.5–22. The is referred to as the flexion-torsion plane. The component flexion angles , and two unit vectors spanning this plane, normal to a plane, plane with normal vector and and are determined from and by projection onto the two in-plane directions: and The torsion angle in a PROJECTION FLEXION-TORSION connection can be understood from a finite successive rotation parameterization 3–2–3. In terms of the 3–2–3 parameterization the total flexion angle is the second successive rotation angle, and the torsion angle is the sum of the first and third successive rotation angles. The torsion angle between the two shafts is defined as where positive torsion angles are rotations about the positive -direction and m is an integer. The PROJECTION FLEXION-TORSION connection avoids the singularity that occurs in the sweep angle of the FLEXION-TORSION connection when the total flexion angle vanishes. As a result, the PROJECTION FLEXION-TORSION connection is better suited for defining bushing-like behavior for flexion response that varies with the direction of in the flexion-torsion plane. The available components of relative motion , , and are the changes in the two flexion angles and the torsion angle and are defined as and where , and connector constitutive rotations are , are the initial flexion component angles and torsion angle, respectively. The The kinetic moment in a PROJECTION FLEXION-TORSION connection is and Summary PROJECTION FLEXION-TORSION Basic, assembled, or complex: Kinematic constraints: Constraint moment output: Available components: Kinetic moment output: Orientation at a: Orientation at b: Connector stops: Basic None None Required Optional Constitutive reference angles: Predefined friction parameters: Contact force for predefined friction: None None RADIAL-THRUST Connection type RADIAL-THRUST provides a connection between two nodes where the response differs in the radial and cylindrical axis directions. Connection type RADIAL-THRUST models situations such as a point inside a cylindrical bearing where the response to radial displacements differs from the response to thrusting motions. Connection type RADIAL-THRUST cannot be used in two-dimensional or axisymmetric analysis. If the rotational degrees of freedom at the two nodes are connected through flexural and torsional resistance, connection type FLEXION-TORSION can be used in conjunction with connection type RADIAL-THRUST. ea Figure 31.1.5–23 Connection type RADIAL-THRUST. Description The RADIAL-THRUST connection does not impose kinematic constraints. An orientation at node a is required to define the axis of the rectangular coordinate system, . The position of node b relative to node a is given by the radial and axial-direction distances and The RADIAL-THRUST connection has two available components of relative motion, radial displacement coordinate system and is defined as . The measures the change in distance from node b to the axis of the cylindrical and where change in distance from node a to node b along the cylindrical axis and is defined as is the initial radial distance from node b to the axis. The thrust displacement measures the where displacements are is the initial distance along the axis from node b to node a. The connector constitutive The kinetic force is and where the radial unit vector is – The radial resistance of the RADIAL-THRUST connector is analogous to a single spring in the plane. Loads applied in this plane and perpendicular to the current radial unit vector will initially encounter no resistance and may lead to numerical singularity and/or zero pivot warnings from the solver during static analyses. If the numerical singularities cause convergence difficulties, one modeling option is to overlay the RADIAL-THRUST connector with a CARTESIAN connector with a very small elastic stiffness. Summary RADIAL-THRUST Basic, assembled, or complex: Kinematic constraints: Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: Basic None None Required Ignored Constitutive reference lengths: Predefined friction parameters: Contact force for predefined friction: None None RETRACTOR Connection type RETRACTOR joins the position of two nodes and provides a FLOW-CONVERTER constraint between the material flow degree of freedom (10) at the second node and the rotational degrees of freedom at the first node of the connector. This connection type can be used to model retractor and pretensioner devices in automotive seat belts or cable drums in winch-like devices. RETRACTOR connections cannot be used in two-dimensional and axisymmetric analyses in Abaqus/Explicit. L W Figure 31.1.5–24 Connection type RETRACTOR. Description Connection type RETRACTOR imposes kinematic constraints and uses local orientation definitions equivalent to combining connection types JOIN and FLOW-CONVERTER. Summary RETRACTOR Basic, assembled, or complex: Assembled Kinematic constraints: JOIN + FLOW-CONVERTER Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: None None Required Ignored RETRACTOR Connector stops: Constitutive reference lengths: Predefined friction parameters: None None None Contact force for predefined friction: None REVOLUTE Connection type REVOLUTE provides a connection between two nodes where the rotations are constrained about two local directions and free about a shared axis. The shared axis of rotation is the connector local 1-direction. Connection type REVOLUTE cannot be used in two-dimensional or axisymmetric analysis. Connection type REVOLUTE models the rotational part of a HINGE or CYLINDRICAL joint. eb eb eb ea ea ea ea eb Figure 31.1.5–25 Connection type REVOLUTE. Description A REVOLUTE connection constrains two rotational components of relative motion between two nodes and allows one free rotational component. The two kinematic constraints imposed by the REVOLUTE connection are and which are equivalent to the requirement that . Alternatively, the REVOLUTE constraint is equivalent to setting the second and third Cardan angles to zero in a CARDAN connection. If the shared axes do not align initially, the REVOLUTE constraint will hold the second and third Cardan angles fixed at their initial values. The constraint moment in the REVOLUTE connection is and Node b can rotate about the shared local direction . The relative angular position of the local directions at node b relative to a is is the first Cardan angle measuring a counterclockwise rotation about the -direction of to where . , measures the change in angular position and is defined as CONNECTION-TYPE LIBRARY where shared axis. The connector constitutive rotation is is the initial angular position and n is an integer accounting for multiple rotations about the The kinetic moment in the REVOLUTE connection is Friction When used by itself, there is no predefined Coulomb-like friction in the REVOLUTE connection. However, when the REVOLUTE connection is used in combination with a JOIN, SLIDE-PLANE, or SLOT connection, the predefined friction is the same as the HINGE, PLANAR, and CYLINDRICAL connections, respectively. Summary REVOLUTE Basic, assembled, or complex: Basic Kinematic constraints: Constraint moment output: Available components: Kinetic moment output: Orientation at a: Orientation at b: Connector stops: Constitutive reference angles: Required Optional Predefined friction parameters: None Contact moment for predefined friction: None ROTATION Connection type ROTATION provides a rotational connection between two nodes where the relative rotation between the nodes is parameterized by the rotation vector. In two-dimensional and axisymmetric analyses, the ROTATION connection type involves a single (scalar) relative rotation component. Although available components of relative motion exist for the ROTATION connection type in three-dimensional analysis, the finite rotation parameterization of the connection is not necessarily well-suited for defining connector behavior. If a finite, three-dimensional ROTATION connection with connector behavior is desired, either the CARDAN or EULER connection type typically is more appropriate. When connection type ROTATION is used in a connector element connected to ground at the element’s first node, the rotational components relative to the orientation at ground are identical to the Abaqus convention for nodal rotation degrees of freedom. Hence, connection type ROTATION can be used in conjunction with prescribed connector motion to specify finite rotation boundary conditions in local coordinate directions using the Abaqus convention for finite rotation boundary conditions. eb eb eb ea ea ea Figure 31.1.5–26 Connection type ROTATION. Description The rotation connection does not impose kinematic constraints. The rotation connection is a finite rotation connection where the local directions at node b are parameterized relative to the local directions at node a by the rotation vector. Let relative to be the rotation vector that positions local directions ; that is, for all Section 1.3.1 of the Abaqus Theory Manual, for a discussion of finite rotations. is the skew-symmetric matrix with axial vector , where . See “Rotation variables,” The available components of relative motion in the ROTATION connection are the change in the rotation vector components positioning the local directions at node b relative to the local directions at node a. Therefore, , all vector components are components relative to the local directions is an integer accounting for rotations with magnitude greater . The , and is the initial rotation vector, where than connector constitutive rotations are The kinetic moment in a rotation connection is In two-dimensional and axisymmetric analyses and . Summary ROTATION Basic, assembled, or complex: Kinematic constraints: Constraint moment output: Available components: Kinetic moment output: Orientation at a: Orientation at b: Connector stops: Basic None None Optional Optional Constitutive reference angles: Predefined friction parameters: Contact force for predefined friction: None None ROTATION-ACCELEROMETER Connection type ROTATION-ACCELEROMETER provides a convenient way to measure the relative angular position, velocity, and acceleration of a body in a local coordinate system. These kinematic quantities are measured relative to the motion of node a and are reported in the coordinate system of node b. Each node of the connector can translate and rotate independently, although fixing the first of the two nodes to ground is more common. With the first node fixed, connection type ROTATION- ACCELEROMETER provides a convenient way to measure the local components of the angular velocity and angular acceleration in a coordinate system fixed to a moving body (for example, an accelerometer). Connection type ROTATION-ACCELEROMETER is available only in Abaqus/Explicit. It is the rotation counterpart to connection type ACCELEROMETER, which measures relative translational position, velocity, and acceleration. ROTATION-ACCELEROMETER connectors cannot be used in two-dimensional and axisymmetric analysis in Abaqus/Explicit. eb eb eb ea ea ea Figure 31.1.5–27 Connection type ROTATION-ACCELEROMETER. Description The ROTATION-ACCELEROMETER connection does not It defines three local directions at node a and three local directions at node b. The ROTATION- ACCELEROMETER connection’s formulation is similar to that for the ROTATION connection. The ROTATION-ACCELEROMETER connection measures the finite rotation that takes the local directions at node a into the local directions at node b and parameterizes that finite rotation by the rotation vector. Let be the rotation vector that positions local directions impose kinematic constraints. relative to ; that is, , where . See “Rotation variables,” is the skew-symmetric matrix with axial vector for all Section 1.3.1 of the Abaqus Theory Manual, for a discussion of finite rotations. The connection measures the change in the rotation vector components in the local directions rotating with the body at node b. The rotation vector components are calculated as There are no available components of relative motion for the ROTATION-ACCELEROMETER connection. The connector rotation is where greater than . is the initial rotation vector and is an integer accounting for rotations with magnitude The ROTATION-ACCELEROMETER connection differs from the ROTATION connection in the way angular velocity and acceleration are calculated. The ROTATION-ACCELEROMETER connection measures velocity and acceleration from the nodes as where , , , and are the nodal angular velocities and accelerations at nodes a and b, respectively. In two-dimensional and axisymmetric analyses . and Summary ROTATION-ACCELEROMETER Basic, assembled, or complex: Kinematic constraints: Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: Constitutive reference lengths: Predefined friction parameters: Contact force for predefined friction: Basic None None None None Optional Optional None None None None SLIDE-PLANE Connection type SLIDE-PLANE keeps node b on a plane defined by the orientation of node a and the initial position of node b. Connection type SLIDE-PLANE cannot be used in two-dimensional or axisymmetric analysis. The normal direction defining the plane at node a is . Connection type SLIDE-PLANE models a point confined between parallel plates or a pin-in-slot connection where the pin is free to move normal to the plane of the slot. ea ea x0 ea u2 u3 Figure 31.1.5–28 Connection type SLIDE-PLANE. Description The SLIDE-PLANE connection constrains the position of node b, the local normal direction . The normal direction distance from node a to the plane is constant: , to remain on a plane defined by where connection is is the initial distance from node a to the plane. The constraint force in the SLIDE-PLANE Node b can move in the plane defined by the normal of node a. The position of node b in the plane relative to node a is The two available components of relative motion, and , are and and where displacements are and are the coordinates of the initial position of node b. The connector constitutive The kinetic force in the plane is and Friction Predefined Coulomb-like friction in the SLIDE-PLANE connection relates the kinematic constraint forces in the connector to the friction forces (CSFC) in the translations along the two local directions in the 2–3 plane. The frictional effect is formally written as where the potential in a direction tangent to the 2–3 plane on which contact occurs, on the same plane, and if represents the magnitude of the frictional tangential tractions in the connector is the friction-producing normal force ; and sliding occurs is the friction coefficient. Frictional stick occurs if , in which case the friction force is . The normal force is the sum of a magnitude measure of friction-producing connector forces, , and a self-equilibrated internal contact force, : The force magnitude The magnitude of the frictional tangential tractions, . is computed using The predefined Coulomb-like friction is computed differently when the SLIDE-PLANE connection is used in combination with a REVOLUTE connection. See the description of the PLANAR connection for the predefined friction definition in this case. Summary SLIDE-PLANE Basic, assembled, or complex: Basic Kinematic constraints: Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: Required Ignored Constitutive reference lengths: Predefined friction parameters: Optional: Contact force for predefined friction: SLIPRING Connection type SLIPRING provides a connection between two nodes that models material flow and stretching between two points of a belt system. It can be used to model seat belts , pulley systems, and taut cable systems. The angle between two adjacent belt segments is used only for friction calculations. By default, the angle, and . Alternatively, you can specify the angle between two adjacent belt segments (in radians) as part of the connector section definition. You can use this option to specify wrapping angles larger than . , is computed automatically from the nodal coordinates as an angle between This connection type activates the material flow degree of freedom (10) at both nodes of the connector. As with any other nodal degree of freedom, you must be careful in constraining it. This is typically done by attaching the connector to other SLIPRING connectors that are part of the belt system, attaching it to a RETRACTOR (FLOW-CONVERTER) connector, or applying a boundary condition. SLIPRING connections cannot be used in two-dimensional and axisymmetric analyses in Abaqus/Explicit.  radius ignored  Figure 31.1.5–29 Connection type SLIPRING. Description The SLIPRING connection does not constrain any component of relative motion. Hence, there is no restriction on the position of the connector nodes. The distance between nodes is The belt material can flow and stretch between nodes a and b. Flow can occur with no stretching (such as in a rigid belt), stretching can occur with no flow (such as when the flow is constrained at both nodes of the connector), or both flow and stretching can occur simultaneously (such as in compliant belts). By convention, the material flow at node a is positive if it enters segment and is positive at node b if it exits the segment. A reference length can be defined in incremental fashion as is the reference length at the end of the current increment, where beginning of the current increment, flow at node b. The stretch in the belt can then be defined as is the incremental flow at node a, and is the reference length at the is the incremental and the “strain” in the belt can be computed as At the beginning of the analysis, the reference length at is is the initial stretch of the belt. By default, the initial stretch is where no initial strains in the belt. You can specify initial strains in the belt, constitutive reference. The initial stretch is then computed using meaning that there are , by specifying a connector The second available component of relative motion is simply the material flow past node b, The third component of relative motion is the material flow into node a and is used only for output: The kinetic force is where Symbol plots in the Visualization module of Abaqus/CAE display vector field output for the SLIPRING connector along the 1-direction of the orientation at the first node instead of along the line joining the two nodes. If an orientation is not defined for the first node of the connector, the vector is displayed along the 1-direction of the global coordinate system. Limitations At most two SLIPRING connectors can share a common node. The following limitations apply with respect to the kinetic behavior that can be defined in the SLIPRING connection type: • Only predefined friction can be defined in the second component of relative motion as outlined below. • In Abaqus/Explicit plasticity, damage and lock connector behavior cannot be specified. • The connectivities of the two adjacent SLIPRING connector elements sharing a common node b (Figure 31.1.5–29) should be in the typical order a–b and b–c. In addition, any two adjacent SLIPRING connector elements must refer to the same connector behavior except for the friction data. Friction in component 1) to the tension in the adjacent belt segment Predefined Coulomb-like friction in the SLIPRING connection relates the tension in the belt segment . In the simpler case of (kinetic force frictionless sliding, the two tensions are equal (apart from inertial effects due to the motion of the belt in dynamic analyses). If frictional effects are included as material flows past node b, the two tensions differ by the total friction force (CSF2) over the contact arch between the belt and the ring (angle ). The Coulomb-like frictional effect is a well-known analytical result. In the case when frictional sliding occurs in the direction illustrated in Figure 31.1.5–29, the tensions in the two segments, and , are related as follows: where is the friction coefficient. The friction force is simply the difference More formally, the frictional relationship is modeled by considering the potential function Frictional stick occurs if ; and sliding occurs if . Friction forces do not develop if the kinetic force = , in which case the tension force is compressive. When sliding occurs in the opposite direction, the sign of the exponent in the potential equation changes. The friction force is reported as in this connection type. The friction-generating “contact force” is reported as CNF2= . In Abaqus/Explicit, by default, the distance between the two nodes of the SLIPRING is not allowed to become less then one hundredth of the original distance between the nodes, which prevents the SLIPRING from collapsing to zero length during the analysis. The two nodes of the SLIPRING can move apart after coming to the minimum distance configuration during the analysis. In addition, the belt can continue to slip over the nodes while they are stopped at the minimum distance configuration. This default value of the minimum distance can be overridden by specifying a lower limit of the connector stop in component 1 of the SLIPRING. Output Some of the connector output variables have a somewhat different meaning for this connection type than usual, as follows: • CP1 is the current distance between the nodes; • CP2 is the material flow at node b; • CP3 is the material flow at node a; and • CU1 is the strain (dimensionless) in the segment . Summary SLIPRING Basic, assembled, or complex: Complex Kinematic constraints: Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: None None Ignored Ignored None Constitutive reference lengths: Predefined friction parameters: None Contact force for predefined friction: SLOT Connection type SLOT provides a connection where node b stays on the line defined by the orientation of node a and the initial position of node b. The line of action of the slot is the -direction. In three-dimensional analysis node b cannot move in the direction normal to the slot; i.e., the direction. If node b is free to move in the normal direction, connection type SLIDE-PLANE should be used. ea ea y0 u1 Figure 31.1.5–30 Connection type SLOT. Description The line of the slot is defined by the first local direction at node a, The SLOT connection constrains the position of node b, the relative position of node b is fixed in the directions perpendicular to the slot: , and the initial position of node b. , to remain on the line of the slot. Therefore, where is the initial distance from node a to the slot in the local 2-direction. In three dimensions where the slot is is the initial distance from node a to the slot in the local 3-direction. The constraint force in where in two-dimensional analysis. Node b can move along the line of the slot. The relative position in the slot is the distance between node b and node a along the -direction and is defined as The available component of relative motion is the displacement relative position in length along the slot and is defined as , which measures the change of the where displacement is is the initial distance between node b and node a along the slot. The connector constitutive The kinetic force in the slot is Friction Predefined Coulomb-like friction in the SLOT connection relates the kinematic constraint forces in the connector to the friction force (CSF1) in the translation along the slot. The frictional effect is formally written as where the potential in a direction tangent to the slot axis along which contact occurs, (contact) force in the direction normal to the slot, and if represents the magnitude of the frictional tangential tractions in the connector is the friction-producing normal is the friction coefficient. Frictional stick occurs . , in which case the friction force is ; and sliding occurs if The normal force is the sum of a magnitude measure of the friction-producing connector force, , and a self-equilibrated internal contact force, : The force magnitude is computed using The magnitude of the frictional tangential tractions The predefined Coulomb-like friction is computed differently when the SLOT connection is used in combination with a REVOLUTE or an ALIGN connection. See CYLINDRICAL and TRANSLATOR, respectively, for the predefined friction definition in these cases. . Summary SLOT Basic, assembled, or complex: Basic Kinematic constraints: Constraint force output: Available components: Kinetic force output: Orientation at a: Orientation at b: Connector stops: Required Ignored Constitutive reference lengths: Predefined friction parameters: Optional: Contact force for predefined friction: TRANSLATOR Connection type TRANSLATOR provides a slot constraint between two nodes and aligns their local directions. ea ea eb ea eb eb u1 Figure 31.1.5–31 Connection type TRANSLATOR. Description Connection type TRANSLATOR imposes kinematic constraints and uses local orientation definitions equivalent to combining connection types SLOT and ALIGN. The connector constraint forces and moments reported as connector output depend strongly on the order and location of the nodes in the connector . Since the kinematic constraints are enforced at node b (the second node of the connector element), the reported forces and moments are the constraint forces and moments applied at node b to enforce the TRANSLATOR constraint. Thus, in most cases the connector output associated with a TRANSLATOR connection is best interpreted when node b is located at the center of the device enforcing the constraint. This choice is essential when moment-based friction is modeled in the connector since the contact forces are derived from the connector forces and moments, as illustrated below. Proper enforcement of the kinematic constraints is independent of the order or location of the nodes. Friction Predefined Coulomb-like friction in the TRANSLATOR connection relates the kinematic constraint forces and moments in the connector to the friction force (CSF1) in the translation along the slot. The frictional effect is formally written as where the potential the local 1-direction, slot, and which case the friction force is is the friction coefficient. Frictional stick occurs if . represents the magnitude of the frictional tangential traction in the connector in is the friction-producing normal (contact) force in the direction normal to the , in ; and sliding occurs if is the sum of a magnitude measure of contact friction-producing connector forces, , and a self-equilibrated internal contact force, : CONNECTION-TYPE LIBRARY The contact force magnitude • a force contribution from torque, is defined by summing the following three contributions: , obtained by scaling the torque constraint moment about the 1-direction, , by a length factor, as follows: where 0.0, represents the effective radius of the shaft cross-section in the local 2–3 plane (if is ignored); is • a radial force contribution, constraint): (the magnitude of the constraint forces enforcing the SLOT and • a force contribution from “bending,” , by a length factor, as follows: , obtained by scaling the bending constraint moment, where L represents a characteristic overlapping length in the slot direction. If L is 0.0, ignored. is Thus, where . The magnitude of the frictional tangential tractions, is . Summary TRANSLATOR Basic, assembled, or complex: Assembled Kinematic constraints: SLOT + ALIGN Constraint force and moment output: Available components: Kinetic force and moment output: Orientation at a: Orientation at b: Connector stops: Constitutive reference lengths: Required Optional Predefined friction parameters: Optional: , L, Contact force for predefined friction: UJOINT Connection type UJOINT joins the position of two nodes and provides a universal constraint between their rotational degrees of freedom. Connection type UJOINT cannot be used in two-dimensional or axisymmetric analysis. ea eb ea eb Figure 31.1.5–32 Connection type UJOINT. Description Connection type UJOINT imposes kinematic constraints and uses local orientation definitions equivalent to combining connection types JOIN and UNIVERSAL. The connector constraint forces and moments reported as connector output depend strongly on the order of the nodes and location of the nodes in the connector . Since the kinematic constraints are enforced at node b (the second node of the connector element), the reported forces and moments are the constraint forces and moments applied at node b to enforce the UJOINT constraint. Thus, in most cases the connector output associated with a UJOINT connection is best interpreted when node b is located at the center of the device enforcing the constraint. This choice is essential when moment-based friction is modeled in the connector since the contact forces are derived from the connector forces and moments, as illustrated below. Proper enforcement of the kinematic constraints is independent of the order or location of the nodes. Friction Predefined Coulomb-like friction in the UJOINT connection relates the kinematic constraint forces and moments in the connector to friction moments about the unconstrained rotations (about the two directions of the connection cross). The UJOINT connection type consists of four hinge-like connections placed at the four ends of the connection cross that generate frictional moments about the cross axes. The frictional moments in each of these hinges are computed in a fashion similar to the HINGE connection. The constraint forces and moments are used first to compute a reaction force, of the constraint forces enforcing the JOIN constraint), and a “twisting” constraint moment, magnitude of the constraint moment enforcing the UNIVERSAL connection), as follows: (the magnitude (the and The two cross directions are given by perpendicular to the connection cross given by to be applied at the center of the connection cross. The constraint moment, the four hinges a bending-like moment about . The constraint moment, . Both : and , acts about an axis are considered , produces in each of and a transverse force in the cross plane , where where represents a characteristic length of the cross arm between the center of the cross and the ends of the cross. The scaling factors and are nonlinear functions of the slenderness of the cross axes (the aspect ratio is the average radius of the four pins at the ends of the connection cross): they can be approximated by assuming the cross arm with rigid bodies for infinitely small aspect ratios, with Timoshenko beams for small aspect ratios (less than 20), and with Euler-Bernoulli beams for slender axes (large aspect ratios). Abaqus chooses the appropriate values automatically based on the user-specified geometric constants . Figure 31.1.5–33 illustrates the evolution of the scaling factors as a function of the aspect ratio: as the aspect ratio approaches 0.0, approaches 0.0 and approaches 0.375. , can be decomposed into axial forces along the two axes of the connection cross approaches 0.25; for large aspect ratios, The constraint force, and a “bending” force perpendicular to the connection cross plane: approaches 0.125 and and where axial twist twist axial Figure 31.1.5–33 Scaling factors in the UJOINT connection. Friction in the UJOINT connection is the superposition of four HINGE-like frictional effects due to rotations about the two cross axes. Since the rotations about the local 1- and 3-directions are the only possible relative motions in the connection, the frictional effects (CSM1 and CSM3) are formally written in terms of moments generated by tangential tractions and moments generated by contact forces. In the following equations subscript 1 refers to frictional effects about the local 1-direction, and subscript 3 refers to frictional effects about the local 3-direction. The frictional effects are written as follows: and where the potentials tractions in the connector in directions tangent to the cylindrical surface on which contact occurs, and friction coefficient. Frictional stick occurs in a particular direction if occurs if are the friction-producing normal moments on the same cylindrical surface, and , in which case the friction moments are represent the moment magnitudes of the frictional tangential is the ; and sliding and or or . The normal moments and connector moments, (such as from a press-fit assembly), and are the sums of magnitude measures of force-producing , and self-equilibrated internal contact moments and , respectively: The factor of two in the above equations comes from the fact that there are two hinges on each cross direction. The moment magnitudes and are defined by summing the following contributions: • moment from axial forces, , and constraint force in the axial direction in each of the pins (if ignored); and and , is an average effective friction arm associated with the are is 0.0, , where and • moment from normal forces, following contributions: and , where and are themselves sums of the – transverse force contributions, hinges along the two hinges along the -direction) and -direction): (the magnitude of the total transverse force in the two (the magnitude of the total transverse force in the where , is defined above, , and ; and – force contributions from “bending,” , obtained by scaling the total bending moment, (the magnitude of the total bending moment on each of the four hinges), by a length factor, as follows: where overlapping length between the pins and their sleeves. If is defined above, and , is 0.0, represents a characteristic is ignored. Thus, The moment magnitudes of the frictional tangential tractions are and . Summary UJOINT Basic, assembled, or complex: Assembled Kinematic constraints: JOIN + UNIVERSAL Constraint force and moment output: Available components: Kinetic force and moment output: Orientation at a: Orientation at b: Connector stops: Constitutive reference lengths: Predefined friction parameters: Required Optional Required: , , , ; optional: , Contact moments for predefined friction: , UNIVERSAL Connection type UNIVERSAL provides a connection between two nodes where the rotations are fixed about one local direction and free about two others. Connection type UNIVERSAL provides the rotational part of a UJOINT connection. Connection type UNIVERSAL cannot be used in two-dimensional or axisymmetric analysis. ea ea ea eb eb eb Figure 31.1.5–34 Connection type UNIVERSAL. Description A UNIVERSAL connection constrains the rotation about the shaft directions at two nodes. The shaft directions at nodes a and b are , respectively. A UNIVERSAL connection requires that local direction and . This single constraint is written be perpendicular to This constraint is equivalent to constraining the second Cardan angle to be zero in a Cardan angle parameterization of the local directions at node b relative to those at node a. If the initial orientation directions at node b do not satisfy the above constraint condition, the universal constraint will hold the second Cardan angle fixed at its initial value. The constraint moment imposed by the UNIVERSAL connection is A UNIVERSAL connection allows two free rotational components of relative motion between two nodes. The first and third Cardan angles that position local directions at node b relative to those at node a are and The two available components of relative motion for the UNIVERSAL connection, changes in the two unconstrained Cardan angles when the second Cardan angle is fixed. Therefore, and , are the where and are the initial Cardan angles. The connector constitutive rotations are and The kinetic moment in the UNIVERSAL connection is and Friction When used by itself, there is no predefined Coulomb-like friction in the UNIVERSAL connection. However, when the UNIVERSAL connection is used in combination with the JOIN connection type, the predefined friction is the same as the UJOINT connection. Summary UNIVERSAL Basic, assembled, or complex: Basic Kinematic constraints: Constraint moment output: Available components: Kinetic moment output: Orientation at a: Orientation at b: Connector stops: Required Optional Constitutive reference angles: Predefined friction parameters: Contact force for predefined friction: None None WELD Connection type WELD provides a fully bonded connection between two nodes. ea 2, eb ea 1, eb a, b ea 3, eb Figure 31.1.5–35 Connection type WELD. Description Connection type WELD imposes kinematic constraints and uses local orientation definitions equivalent to combining connection types JOIN and ALIGN. Summary WELD Basic, assembled, or complex: Kinematic constraints: Constraint force and moment output: Available components: Kinetic force and moment output: Orientation at a: Orientation at b: Connector stops: Constitutive reference lengths and angles: Predefined friction parameters: Contact force for predefined friction: Assembled JOIN + ALIGN None None Optional Optional None None None None 31.2 Connector element behavior • “Connector behavior,” Section 31.2.1 • “Connector elastic behavior,” Section 31.2.2 • “Connector damping behavior,” Section 31.2.3 • “Connector functions for coupled behavior,” Section 31.2.4 • “Connector friction behavior,” Section 31.2.5 • “Connector plastic behavior,” Section 31.2.6 • “Connector damage behavior,” Section 31.2.7 • “Connector stops and locks,” Section 31.2.8 • “Connector failure behavior,” Section 31.2.9 • “Connector uniaxial behavior,” Section 31.2.10 31.2.1 CONNECTOR BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • “Connector elastic behavior,” Section 31.2.2 • “Connector damping behavior,” Section 31.2.3 • “Connector functions for coupled behavior,” Section 31.2.4 • “Connector friction behavior,” Section 31.2.5 • “Connector plastic behavior,” Section 31.2.6 • “Connector damage behavior,” Section 31.2.7 • “Connector stops and locks,” Section 31.2.8 • “Connector failure behavior,” Section 31.2.9 • “Connector uniaxial behavior,” Section 31.2.10 • *CONNECTOR BEHAVIOR • *CONNECTOR CONSTITUTIVE REFERENCE • *CONNECTOR SECTION • “Creating connector sections,” Section 15.12.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a reference length,” Section 15.17.12 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining time integration,” Section 15.17.13 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Connector behavior: • can be defined for connection types with available components of relative motion; • can incorporate simple spring, dashpot, and node-to-node contact as particular applications; • may include linear or nonlinear force versus displacement and force versus velocity behavior for the unconstrained relative motion components; • can include uncoupled or coupled behavior specifications; • can allow frictional force in an unconstrained component of relative motion to be generated by any force or moment in the connection; • can allow for plasticity definitions for individual components or coupled plasticity definitions using user-defined yield functions; • can be used to specify sophisticated damage mechanisms with various damage evolution laws; • can provide user-defined locking criteria to lock in the current position all relative motion in the connector element or a single unconstrained component of relative motion; • can be used to specify failure of the connector element; and • can be used to specify complex uniaxial models by specifying the loading and unloading behavior in an available component of relative motion. Assigning a connector behavior to a connector element You can assign the name of a connector behavior to particular connector elements. Input File Usage: Abaqus/CAE Usage: Use the following options to define the connector behavior: *CONNECTOR SECTION, ELSET=name, BEHAVIOR=behavior name *CONNECTOR BEHAVIOR, NAME=behavior name Interaction module: Connector→Section→Create: Name: connector section name: Behavior Options, Add Connector→Assignment→Create: select wires: Section: connector section name Connector behavior models Connector behaviors allow for modeling of the following types of effects: • spring-like elastic behavior; • rigid-like elastic behavior; • dashpot-like (damping) behavior; • friction; • plasticity; • damage; • stops; • locks; • failure; and • uniaxial behavior. Kinetic behavior can be specified only in available components of relative motion. The list of available components of relative motion for each connector type is given in “Connection-type library,” Section 31.1.5. A connector behavior can be specified in any of the following ways: • uncoupled: motion; the behavior is specified separately in individual available components of relative • coupled: all or several of the available components of relative motion are used simultaneously in a coupled manner to define the behavior; or • combined: a combination of both uncoupled and coupled definitions are used simultaneously. A conceptual model illustrating how connector behaviors interact with each other is shown locks, friction) act in parallel. in Figure 31.2.1–1. Most behaviors (elasticity, damping, stops, Plasticity models are always defined in conjunction with spring-like or rigid-like elasticity definitions. Degradation due to damage can be specified either for the elastic-plastic or rigid-plastic response alone or for the entire kinetic response in the connector. The failure behavior will apply to the entire connector response. elastic/rigid plastic damage elastic/rigid plastic first connector node DMG ERP damping stop/lock friction damage failure DMG ALL FAIL second connector node Figure 31.2.1–1 Conceptual illustration of connector behaviors. Multiple definitions for the same behavior type are permitted. For example, if connector elasticity (or damping) is defined several times in an uncoupled fashion for the same available component of relative motion, in a coupled fashion, or in both fashions, the spring-like (or dashpot-like) responses are added together. Multiple definitions of friction, plasticity, and damage behaviors are permitted as long as the rules outlined in the corresponding behavior sections are followed. Multiple uncoupled stop and lock definitions for the same component are permitted, but only one will be enforced at a time. Defining coupled and uncoupled connector behavior In many cases connector behavior is specified in an uncoupled manner in individual available components of relative motion. Coupled behavior can be defined for all or some of the available components of relative motion in a connector. For coupled plasticity, damage, and, in certain situations, friction behavior, additional functions describing the nature of the coupling effects must be defined . These functions do not define a behavior by themselves but are used as tools for building a desired behavior. For example, these functions may be used to define: • sophisticated yield functions in the connector force space for coupled plasticity behavior; • friction-generating contact forces for friction behavior; or • force or relative motion magnitude measures needed for damage behavior specifications. Input File Usage: Use the following input to define uncoupled behavior: *CONNECTOR BEHAVIOR OPTION, COMPONENT=n Use the following input to define coupled behavior: *CONNECTOR BEHAVIOR OPTION Abaqus/CAE Usage: Interaction module: connector section editor: Add→connector behavior: Coupling: Uncoupled or Coupled Defining nonlinear connector behavior properties to depend on relative positions or constitutive displacements/rotations In all nonlinear uncoupled connector kinetic behaviors the independent variable is the connector available component in the direction for which the response is defined. When modeling the following connector behaviors, the properties can also depend on relative positions or constitutive displacements/rotations in several component directions: • connector elasticity, • connector damping, • connector derived components, and • connector friction. When modeling connector uniaxial behavior, displacements/rotations Section 31.2.10, for more information. in several component directions; the properties can also depend on constitutive see “Connector uniaxial behavior,” Input File Usage: Use the following option to specify that the connector behavior properties are dependent on components of relative position included in the behavior definition: *CONNECTOR BEHAVIOR OPTION, INDEPENDENT COMPONENTS=POSITION (default) Use the following option to specify that the connector behavior properties are dependent on components of constitutive relative displacements or rotations included in the behavior definition: *CONNECTOR BEHAVIOR OPTION, INDEPENDENT COMPONENTS=CONSTITUTIVE MOTION In either case the first data line identifies the independent component numbers to be used in determining the dependencies, and the additional data for the connector behavior definition begin on the second data line. Abaqus/CAE Usage: For elasticity or damping behavior, use the following input to specify that connector behavior properties are dependent on relative position or constitutive relative displacements/rotations: Interaction module: connector section editor: Add→Elasticity or Damping: Coupling: Coupled on position or Coupled on motion, select components and enter data For connector derived components, use the following input to specify that connector behavior properties are dependent on relative position or constitutive relative displacements/rotations: Interaction module: connector section editor: Add→Friction, Plasticity, or Damage: Force Potential, Initiation Potential, or Evolution Potential Specify derived component, Use local directions: Independent position components or Independent constitutive motion components, select components and enter data For friction behavior specifying internal contact forces, use the following input to specify that connector behavior properties are dependent on relative position or constitutive relative displacements/rotations: Interaction module: connector section editor: Add→Friction: Friction model: User-defined, Contact Force, Use independent components: Position or Motion, select components and enter data Defining reference lengths and angles for constitutive response In many connector behavior definitions, material-like behavior has a reference position where the force or moment is zero, which is different from the initial position. This is the case, for example, in a spring that has nonzero force or moment in the initial configuration. In these situations the most convenient way to define the connector behavior is relative to the nominal or reference geometry where the forces or moments vanish. You can define the translational or angular positions at which constitutive forces and moments are zero by specifying up to six reference values (one per component of relative motion): three lengths and three angles (in degrees). The reference lengths and angles affect only spring-like elastic connector behavior and, if the friction-generating contact force (moment) is a function of the relative displacement (rotation), connector friction behavior. By default, the reference lengths and angles are the length and angle values determined from the initial geometry. See “Connection-type library,” Section 31.1.5, for the meaning of the reference lengths and angles for each connection type. Input File Usage: *CONNECTOR CONSTITUTIVE REFERENCE length 1, length 2, length 3, angle 1, angle 2, angle 3 Abaqus/CAE Usage: Interaction module: connector section editor: Add→Reference Length: Length associated with CORM Defining precompressed or preextended linear elastic behavior In many cases connectors are precompressed or preextended when installed in assemblies. In such cases the connector force is nonzero in the initial configuration. While nonlinear elasticity could be used to define nonzero force in the initial configuration, it is often more convenient to specify a (linear) spring stiffness plus a reference length or angle at which the force or moment is zero. For example, linear uncoupled elastic behavior defined with the connection type AXIAL would have force given by the equation where constitutive reference length. The connector constitutive displacement quantities, different connection types as described in “Connection-type library,” Section 31.1.5. . l is the current length of the AXIAL connection, and is the user-defined , are defined for Example An input file template for a connector model of the shock absorber in Figure 31.2.1–2 is presented in “Connectors: overview,” Section 31.1.1. A reference angle of 22.5° is defined for the nonlinear torsional spring as the fourth data item (corresponding to the connector’s fourth component of relative motion) in the connector constitutive reference: *CONNECTOR BEHAVIOR, NAME=sbehavior ... *CONNECTOR CONSTITUTIVE REFERENCE , , , 22.5 The effect of this reference angle is that the nonlinear torsional spring has a zero moment at an angle of 22.5°. extensible range 7.5 node 12 1 (local orientation) node 11 Figure 31.2.1–2 Simplified connector model of a shock absorber. Defining the time integration method for constitutive response in Abaqus/Explicit In Abaqus/Explicit kinematic constraints, stops, locks, and actuated motion in connector elements are treated with implicit time integration. By default, connector constitutive behavior (for example, elasticity, damping, and friction) is also integrated implicitly. The advantage of implicit time integration is that elements with these behaviors do not affect the stability or time incrementation of the analysis in any way. When “soft” springs are modeled with connectors, a more traditional explicit time integration for the constitutive response can be used. This explicit time integration may lead to a small improvement in computational performance. However, explicit integration of relatively stiff springs will reduce the global time increment size, since such connector elements are included in the stable time increment size calculation. Input File Usage: Use the following option to specify implicit integration of the constitutive response: *CONNECTOR BEHAVIOR, INTEGRATION=IMPLICIT Use the following option to specify explicit integration of the constitutive response: Abaqus/CAE Usage: *CONNECTOR BEHAVIOR, INTEGRATION=EXPLICIT Interaction module: connector section editor: Add→Integration: Integration: Implicit or Explicit Defining connector behavior in linear perturbation procedures In linear perturbation procedures the connector element kinematics are linearized about the base state. Hence, linearized versions of kinematic constraints are applied, and the connector behavior is linearized about the state at the end of the previous general analysis step. Using several connectors in series or in parallel Connector element behaviors allow for proper modeling of most physical connection behaviors within a single connector element. However, in rare circumstances more complex connection behaviors may require multiple connector elements to be used in parallel or in series. You place connector elements in parallel by defining two or more connector elements between the same nodes. You place connectors in series by specifying additional nodes (most often in the same location as the nodes of interest) and then stringing connector elements between these nodes. For example, assume that you would like to define a connector stop that exhibits elastic-plastic behavior upon contact. Since this is not permitted within the context of one connector behavior definition, you can circumvent the limitation by using two connector elements in series. This concept is illustrated in Figure 31.2.1–3. The first connector defines the stop, and the second defines the elastic-plastic behavior. Since both elements are subject to the same load (because they are in series), the desired behavior is obtained. first connector element second connector element node on the first body stop elastic-plastic additional node node on the second body Figure 31.2.1–3 Conceptual illustration of two connector elements/behaviors in series. Connectors in parallel can be used as well to model complex kinetic behavior. For example, assume that you need to define an elastic-viscous connector with spring-like and dashpot-like behaviors in parallel (for example, the strut in an automotive suspension). Assume that damage can occur only in the dashpot once it is stretched/compressed beyond specified limits. Since this is not permitted within the context of one connector behavior definition, you can circumvent the limitation by using two connector elements in parallel. This concept is illustrated in Figure 31.2.1–4. first connector element elastic node on the first body DMG ALL node on the second body damping second connector element Figure 31.2.1–4 Conceptual illustration of two connector elements/behaviors in parallel. The first connector defines the elastic behavior, and the second defines the dashpot behavior. Since the two connector elements are in parallel, they undergo the same motion (stretching/compression). A motion-based damage behavior can be used to degrade the entire behavior in the second element. Thus, only the dashpot behavior will eventually degrade. Defining connector behavior using tabular data Tabular data are often used to define connector behaviors, such as nonlinear elasticity, isotropic hardening, etc. As shown in Figure 31.2.1–5, the data points make up a nonlinear curve in the constitutive space. Force, F F(0) F1 Linear extrapolation Constant extrapolation Displacement, u Constant extrapolation Linear extrapolation Figure 31.2.1–5 Nonlinear connector behaviors defined as tabular data. The options to define table lookups are described below. Extrapolation options By default, the dependent variables are extrapolated as a constant (with a value corresponding to the endpoints of the curve) outside the specified range of the independent variables. This choice may cause a zero stiffness response, which may lead to convergence problems. You can specify linear extrapolation to extrapolate the dependent variables outside the specified range of the independent variables assuming that the slope given by the end points of the curve remains constant. The extrapolation behavior is illustrated in Figure 31.2.1–5. You define the extrapolation choice globally for all connector behaviors but can redefine the extrapolation choice for the following connector behaviors individually: • connector elasticity; • connector plasticity (connector hardening); • connector damping; • derived components for connector elements; • connector friction; • connector damage (connector damage initiation and evolution); • connector locks; and • connector uniaxial behavior. Tabular data for connector stop and lock behavior options are not supported in Abaqus/CAE. Specifying constant extrapolation for all connector behaviors You can specify constant extrapolation for tabular data for all connector behaviors. Input File Usage: Abaqus/CAE Usage: *CONNECTOR BEHAVIOR, EXTRAPOLATION=CONSTANT (default) Interaction module: connector section editor: Table Options tabbed page: Extrapolation: Constant Specifying linear extrapolation for all connector behaviors You can specify linear extrapolation for tabular data for all connector behaviors. Input File Usage: Abaqus/CAE Usage: *CONNECTOR BEHAVIOR, EXTRAPOLATION=LINEAR Interaction module: connector section editor: Table Options tabbed page: Extrapolation: Linear Redefining the extrapolation choice for individual connector behaviors You can redefine the extrapolation choice for individual connector behaviors. Input File Usage: Use either of the following options: Abaqus/CAE Usage: *CONNECTOR BEHAVIOR OPTION, EXTRAPOLATION=CONSTANT *CONNECTOR BEHAVIOR OPTION, EXTRAPOLATION=LINEAR For example, use the following options to use constant extrapolation for all connector behaviors except for connector elasticity: *CONNECTOR BEHAVIOR, EXTRAPOLATION=CONSTANT *CONNECTOR ELASTICITY, EXTRAPOLATION=LINEAR Use the following input for elasticity, damping, friction, plasticity, and damage behaviors: Interaction module: connector section editor: Behavior Options tabbed page: Table Options button: Extrapolation: toggle off Use behavior settings and choose Constant or Linear Use the following input for connector derived components: Interaction module: derived component editor: Add: Table Options button: Extrapolation: toggle off Use behavior settings and choose Constant or Linear Regularization options for Abaqus/Explicit By default, Abaqus/Explicit regularizes the data into tables that are defined in terms of even intervals of the independent variables since table lookups are most economical if the interpolation is from even intervals of the independent variables. In some cases, where it is necessary to capture sharp changes in connector behavior accurately, you can use the user-defined tabular connector behavior data directly by turning regularization off. However, the table lookups will be more computationally expensive compared to using regular intervals. Therefore, the use of regularization is almost always recommended. Abaqus/Explicit uses an error tolerance to regularize the input data. The number of intervals in the range of each independent variable is chosen such that the error between the piecewise linear regularized data and each of your defined points is less than the tolerance times the range of the dependent variable. The default tolerance is 0.03. In some cases where the dependent quantities are defined at uneven intervals of the independent variables and the range of the independent variable is large compared to the smallest interval, Abaqus/Explicit may fail to obtain an accurate regularization of your data in a reasonable number of intervals. In this case Abaqus/Explicit stops after all data are processed and issues an error message that you must redefine the behavior data. See “Material data definition,” Section 21.1.2, for a more detailed discussion of data regularization. You define the choice of regularization and regularization tolerance globally for all connector behaviors but can redefine the choice of regularization and regularization tolerance for the following connector behaviors individually: • connector elasticity; • connector plasticity (connector hardening) • connector damping; • derived components for connector elements; • connector friction; • connector damage (connector damage initiation and evolution); • connector locks; and • connector uniaxial behavior. Tabular data for connector stop and lock behavior options are not supported in Abaqus/CAE. Specifying the regularization of user-defined tabular data for all connector behaviors You can specify regularization of tabular data and a regularization tolerance to be used globally for all connector behaviors. Input File Usage: *CONNECTOR BEHAVIOR, REGULARIZE=ON (default), RTOL=tolerance Abaqus/CAE Usage: Interaction module: connector section editor: Table Options tabbed page: Regularization: toggle on Regularize data (Explicit only), Specify: tolerance Specifying the use of user-defined tabular data without regularization for all connector behaviors You can specify the use of user-defined tabular data directly by turning regularization off for all connector behaviors. Input File Usage: Abaqus/CAE Usage: *CONNECTOR BEHAVIOR, REGULARIZE=OFF Interaction module: connector section editor: Table Options tabbed page: Regularization: toggle off Regularize data (Explicit only) Redefining the regularization options for individual connector behaviors You can redefine the choice of regularization and regularization tolerance for individual connector behaviors. Input File Usage: Use either of the following options: Abaqus/CAE Usage: *CONNECTOR BEHAVIOR OPTION, REGULARIZE=ON, RTOL=tolerance *CONNECTOR BEHAVIOR OPTION, REGULARIZE=OFF For example, use the following options to regularize the user-defined data for all connector behaviors except for connector elasticity: *CONNECTOR BEHAVIOR, REGULARIZE=ON, RTOL=0.05 *CONNECTOR ELASTICITY, REGULARIZE=OFF Use the following input for elasticity, damping, friction, plasticity, and damage behaviors: Interaction module: connector section editor: Behavior Options tabbed page: Table Options button: Regularization: toggle off Use behavior settings; toggle on Regularize data (Explicit only) and Specify: tolerance, or toggle off Regularize data (Explicit only) Use the following input for connector derived components: Interaction module: derived component editor: Add: Table Options button: Regularization: toggle off Use behavior settings; toggle on Regularize data (Explicit only) and Specify: tolerance, or toggle off Regularize data (Explicit only) Evaluation of rate-dependent data Data for the tabulated isotropic hardening in connector plasticity (“Defining the isotropic hardening component by specifying tabular data” in “Connector plastic behavior,” Section 31.2.6) and plastic motion–based damage initiation criterion (“Plastic motion–based damage initiation criterion” in “Connector damage behavior,” Section 31.2.7) can be specified as dependent on the equivalent relative plastic motion rate. Loading/unloading data for the rate-dependent connector uniaxial behavior model can be specified as dependent on the rate of deformation. Specifying linear intervals for interpolation of rate-dependent data By default, both Abaqus/Standard and Abaqus/Explicit interpolate rate-dependent data using linear intervals of the relative motion rate. Input File Usage: Use the following option to specify linear interpolation for isotropic hardening data: *CONNECTOR HARDENING, RATE INTERPOLATION=LINEAR Use the following option to specify linear interpolation for damage initiation data: *CONNECTOR DAMAGE INITIATION, RATE INTERPOLATION= LINEAR Use both of the following options to specify linear interpolation for uniaxial behavior loading/unloading data: *CONNECTOR UNIAXIAL BEHAVIOR *LOADING DATA, RATE INTERPOLATION=LINEAR Abaqus/Standard always interpolates rate-dependent data using linear intervals of the equivalent relative plastic motion rate. Abaqus/CAE Usage: Use the following input for isotropic hardening data: Interaction module: connector section editor: Add→Plasticity: Isotropic Hardening: Definition: Tabular, Table Options button: Interpolation: Linear Use the following input for damage initiation data: Interaction module: connector section editor: Add→Damage: Initiation: Table Options button: Interpolation: Linear Connector uniaxial behavior cannot be defined in Abaqus/CAE. Specifying logarithmic intervals for interpolation of rate-dependent data in Abaqus/Explicit In Abaqus/Explicit you can specify that logarithmic intervals of the relative motion rate be used for the interpolation of rate-dependent data if the rate dependence of the data is measured at logarithmic intervals. Input File Usage: Use the following option to specify linear interpolation for isotropic hardening data: *CONNECTOR HARDENING, RATE INTERPOLATION=LOGARITHMIC Abaqus/CAE Usage: Use the following option to specify linear interpolation for damage initiation data: *CONNECTOR DAMAGE INITIATION, RATE INTERPOLATION=LOGARITHMIC Use both of the following options to specify linear interpolation for uniaxial behavior loading/unloading data: *CONNECTOR UNIAXIAL BEHAVIOR *LOADING DATA, RATE INTERPOLATION=LOGARITHMIC Use the following input for isotropic hardening data: Interaction module: connector section editor: Add→Plasticity: Isotropic Hardening: Definition: Tabular, Table Options button: Interpolation: Logarithmic Use the following input for damage initiation data: Interaction module: connector section editor: Add→Damage: Initiation: Table Options button: Interpolation: Logarithmic Connector uniaxial behavior cannot be defined in Abaqus/CAE. Filtering the equivalent plastic motion rate in Abaqus/Explicit Rate-sensitive connector constitutive behavior may introduce nonphysical high-frequency oscillations in an explicit dynamic analysis. To overcome this problem, Abaqus/Explicit uses a filtered equivalent plastic motion rate for the evaluation of rate-dependent data. during the time increment of the increment, respectively. The factor associated with rate-dependent connector behavior. You can specify the value of the rate filter factor, directly. The default value is 0.9. A value of is the incremental change in equivalent plastic motion are the plastic motion rates at the beginning and end ) facilitates filtering high-frequency oscillations , provides no filtering and should be used with caution. , and and ( Input File Usage: Use either of the following options: *CONNECTOR HARDENING, RATE FILTER FACTOR= *CONNECTOR DAMAGE INITIATION, RATE FILTER FACTOR= Abaqus/CAE Usage: Use the following input for isotropic hardening data: Interaction module: connector section editor: Add→Plasticity: Isotropic Hardening: Definition: Tabular, Table Options button: Filter factor: Specify: Use the following input for damage initiation data: Interaction module: connector section editor: Add→Damage: Initiation: Table Options button: Filter factor: Specify: 31.2.2 CONNECTOR ELASTIC BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • “Connector behavior,” Section 31.2.1 • *CONNECTOR BEHAVIOR • *CONNECTOR ELASTICITY • “Defining elasticity,” Section 15.17.1 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Spring-like elastic connector behavior: • can be defined in any connector with available components of relative motion; • can be specified for each available component of relative motion independently, in which case the behavior can be linear or nonlinear; • can be specified as dependent on relative positions or constitutive motions in several local directions; and • can be specified for all available components of relative motion as coupled linear elastic behavior. Alternatively, rigid-like behavior can be specified in any of the available components of relative motion using an automatically chosen stiff spring. The directions in which the forces and moments act and the displacements and rotations are measured are determined by the local directions as described in “Connection-type library,” Section 31.1.5, for each connection type. Defining linear uncoupled elastic behavior In the simplest case of linear uncoupled elasticity you define the spring stiffnesses for the selected components (i.e., for component 2, etc.), which are used in the equation for component 1, (no sum on ) is the force or moment in the is the connector where displacement or rotation in the direction. The elastic stiffness can depend on frequency (in Abaqus/Standard), temperature, and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of frequency, temperature, and field variables. component of relative motion and If a frequency-dependent damping behavior is specified in an Abaqus/Standard analysis procedure other than direction-solution steady-state dynamics, the data for the lowest frequency given will be used. Input File Usage: Use the following options to define linear uncoupled elastic connector behavior: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY, COMPONENT=component number, DEPENDENCIES=n Abaqus/CAE Usage: Interaction module: connector section editor: Add→Elasticity: Definition: Linear, Force/Moment: component or components, Coupling: Uncoupled Defining linear coupled elastic behavior In the linear coupled case you define the spring stiffness matrix components, equation , which are used in the where component of relative motion, is the force in the is the coupling between the component, and is the motion of the components. The D matrix is assumed to be symmetric, so only the upper triangle of the matrix is specified. In connectors with kinematic constraints the entries that correspond to the constrained components of relative motion will be ignored. The elastic stiffness can depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and field variables. and Input File Usage: Abaqus/CAE Usage: Use the following options to define linear coupled elastic connector behavior: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY, DEPENDENCIES=n Interaction module: connector section editor: Add→Elasticity: Definition: Linear, Force/Moment: component or components, Coupling: Coupled Modeling coupled unsymmetric linear stiffness By definition, linear elastic behavior should be defined by a symmetric spring stiffness matrix. However, Abaqus/Standard allows you to define an unsymmetric coupled spring stiffness matrix. The intended use case is to approximate fluid film bearings supporting a rotating structure in a rotordynamic analysis . Abaqus/Standard will not check the stability of an unsymmetric spring stiffness matrix; therefore, you must ensure that it is defined properly. In the linear coupled case you define the spring stiffness matrix components, , which are used in the equation component, is the motion of the where and components. The D matrix in this case is assumed to be unsymmetric, so the entire matrix is specified. The entries that correspond to the constrained is the force in the is the coupling between the component of relative motion, and components of relative motion are ignored. When the unsymmetric matrix storage and solution scheme are used, the stiffness can depend on frequency, temperature, and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of frequency, temperature and field variables. Input File Usage: Use the following options to define unsymmetric linear coupled stiffness connector behavior: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY, UNSYMM, FREQUENCY DEPENDENCE=ON Abaqus/CAE Usage: Unsymmetric linear coupled stiffness behavior Abaqus/CAE. is not supported in Defining nonlinear elastic behavior For nonlinear elasticity you specify forces or moments as nonlinear functions of one or more available components of relative motion, . These functions can also depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and field variables. Defining nonlinear elastic behavior that depends on one component direction By default, each nonlinear force or moment function depends only on the displacement or rotation in the direction of the specified component of relative motion. Input File Usage: Use the following options: Abaqus/CAE Usage: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY, COMPONENT=component number, NONLINEAR, DEPENDENCIES=n Interaction module: connector section editor: Add→Elasticity: Definition: Nonlinear, Force/Moment: component or components, Coupling: Uncoupled Defining nonlinear elastic behavior that depends on several component directions Alternatively, the functions can depend on the relative positions or constitutive displacements/rotations in several component directions, as described in “Defining nonlinear connector behavior properties to depend on relative positions or constitutive displacements/rotations” in “Connector behavior,” Section 31.2.1. In this case the operator matrices are unsymmetric when , for , and unsymmetric matrix storage and solution may be needed in Abaqus/Standard to improve convergence. Input File Usage: Use the following options to define nonlinear elastic connector behavior that depends on components of relative position: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY, COMPONENT=component number, NONLINEAR, INDEPENDENT COMPONENTS=POSITION, DEPENDENCIES=n Use the following options to define nonlinear elastic connector behavior that depends on components of constitutive displacements or rotations: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY, COMPONENT=component number, NONLINEAR, INDEPENDENT COMPONENTS=CONSTITUTIVE MOTION, DEPENDENCIES=n Interaction module: connector section editor: Add→Elasticity: Definition: Nonlinear, Force/Moment: component or components, Coupling: Coupled on position or Coupled on motion Abaqus/CAE Usage: Examples The combined connector in Figure 31.2.2–1 has two available components of relative motion: the relative displacement along the 1-direction (from the SLOT connection) and the rotation around the 1-direction (from the REVOLUTE connection)—see “Connection-type library,” Section 31.1.5. Thus, the connector components of relative motion 1 and 4 can be used to specify connector behavior. extensible range 7.5 node 12 1 (local orientation) node 11 Figure 31.2.2–1 Simplified connector model of a shock absorber. To define a nonlinear torsional spring to resist the relative rotation between the top and the bottom connection point around the local 1-direction, use the following input: *CONNECTOR SECTION, ELSET=shock, BEHAVIOR=sbehavior slot, revolute ori, *CONNECTOR BEHAVIOR, NAME=sbehavior *CONNECTOR ELASTICITY, COMPONENT=4, NONLINEAR -900., -0.7 0.0 0.7 0., 1250., Although no elastic coupling is assumed to occur between the two available components of relative motion, you could replace the nonlinear moment versus rotation data with coupled linear elastic behavior to define the rotational stiffness around the shock’s axis coupled to the axial displacement. In another application this same connector may have coupled linear elastic behavior, in the sense that relative rotation and sliding affect each other through a linear coupling. To define a translational stiffness of 2000.0 units, the constant (the 1st entry of a symmetric matrix) is entered in the connector elasticity definition. To define a torsional stiffness of 1000.0 units, the constant (the 10th entry of a symmetric matrix) is entered; and to define a coupling stiffness of 50.0 units between the available rotation and displacement, the constant (the 7th entry) is entered. *CONNECTOR ELASTICITY 2000.0, , , , , , 50.0, 0.0, 1000.0, , , , , , , , , , Defining rigid connector behavior Rigid-like elastic connector behavior can be used to make an otherwise available component of relative motion rigid. Consider a CARTESIAN connector that has no intrinsic kinematic constraints. If rigid behavior is specified in the local 2- and 3-directions, the connector will behave in a similar fashion to a SLOT connector. This technique of using connectors with available components of relative motion for which rigid behavior is specified instead of connectors with intrinsically kinematic constraints is particularly useful when you need to: • customize the constrained components in a connector with available components of relative motion; for example, you can constrain the local 1- and 2-directions in a CARTESIAN connector to define a SLOT-like connector in the 3-direction; • define rigid plastic behavior ; or • define rigid damage behavior . For example, if you use a SLOT connector, plasticity and damage behavior cannot be specified in the intrinsically constrained 2- and 3-directions. To resolve the issue, you can use a CARTESIAN connector with rigid behavior in components 2 and 3 as discussed above and then define rigid plasticity (and/or damage) in these components. See the examples in “Connector plastic behavior,” Section 31.2.6, for illustrations. In Abaqus/Standard an overconstraint may occur if a rigid component is defined in the same local direction as an active connector stop, connector lock, or specified connector motion. Input File Usage: Use the following option to define rigid connector behavior for a specified component of relative motion: *CONNECTOR ELASTICITY, RIGID, COMPONENT=n Use the following option to define rigid connector behavior for multiple specified components of relative motion: *CONNECTOR ELASTICITY, RIGID data line listing components to be made rigid Use the following option to define rigid connector behavior for all available components of relative motion: *CONNECTOR ELASTICITY, RIGID (no data lines) Abaqus/CAE Usage: Interaction module: connector section editor: Add→Elasticity: Definition: Rigid, Components: component or components Enforcing rigid-like elastic behavior Rigid-like elastic behavior in a particular component is enforced by using a stiff, linear elastic spring in that component. The stiffness of the spring is chosen automatically and depends on the circumstances in which the connector is used. In Abaqus/Standard the stiffness is taken to be 10 times larger than the average stiffness of the surrounding elements to which the connector element attaches. If the average stiffness cannot be computed (as would be the case when the connector element does not attach to other elements or attaches to rigid bodies), a stiffness of is used. In Abaqus/Explicit a Courant stiffness is first computed by considering the average mass at the connector element nodes and the stable time increment in the analysis. In most cases the Courant stiffness is then used to calculate the value of the rigid-like elastic behavior using heuristics that depend on modeling circumstances and the precision (single or double) of the analysis. For example, if plasticity is defined in the connector, the rigid-like elastic stiffness in components involved in the plasticity definition does not exceed one thousandth of the initial yield value. If plasticity is not defined, the rigid-like stiffness is computed as a multiple of the Courant stiffness. In most cases, the heuristics used in the computation of the rigid-like stiffness produces a stiffness value that is adequate. If this stiffness does not serve the needs of your application, you can always customize the elastic stiffness by specifying the linear stiffness value directly. Due to the different stiffness values used for rigid-like elastic behavior in Abaqus/Standard and Abaqus/Explicit, you may notice a discontinuity in the behavior when such a model is imported from one solver to the other. Defining elastic connector behavior in linear perturbation procedures Available components of relative motion with connector elasticity use the linearized elastic stiffness from the base state. In direct-solution steady-state dynamic and subspace-based steady-state dynamic analyses, the linear elastic stiffness defined by an uncoupled connector elasticity behavior may be frequency dependent. Output The Abaqus output variables available for connectors are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The following output variables are of particular interest when defining elasticity in connectors: CU CUE CEF Connector relative displacements/rotations. Connector elastic displacements/rotations. Connector elastic forces/moments. Additional reference • Genta, G., Dynamics of Rotating Systems, Springer, 2005. 31.2.3 CONNECTOR DAMPING BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • “Connector behavior,” Section 31.2.1 • *CONNECTOR BEHAVIOR • *CONNECTOR DAMPING • “Defining damping,” Section 15.17.2 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Connector damping behavior: • can be of a dashpot-like viscous nature in transient or steady-state dynamic analyses; • can be of a “structural” nature, related to complex stiffness, for steady-state dynamics procedures that support non-diagonal damping; • can be defined in any connector with available components of relative motion; • can be specified for each available component of relative motion independently, in which case the behavior can be linear or nonlinear for viscous nature damping; • can be specified as dependent on relative positions or constitutive motions in several local directions for viscous nature damping; and • can be specified for all available components of relative motion as coupled damping behavior. The directions in which the forces and moments act and the relative velocities are measured are determined by the local directions as described in “Connection-type library,” Section 31.1.5, for each In dynamic analysis the relative velocities are obtained as part of the integration connection type. operator; in quasi-static analysis in Abaqus/Standard the relative velocities are obtained by dividing the relative displacement increments by the time increment. Defining linear uncoupled viscous damping behavior In the simplest case of linear uncoupled damping you define the damping coefficients for the selected components (i.e., for component 2, etc.), which are used in the equation for component 1, (no sum on ) where velocity in the is the force or moment in the is the velocity or angular direction. The damping coefficient can depend on frequency (in Abaqus/Standard), component of relative motion and temperature, and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of frequency, temperature, and field variables. If frequency-dependent damping behavior is specified in an Abaqus/Standard analysis procedure other than direct solution steady-state dynamics, the data for the lowest frequency given will be used. Input File Usage: Use the following options to define linear uncoupled damping connector behavior: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR DAMPING, COMPONENT=component number, DEPENDENCIES=n Abaqus/CAE Usage: Interaction module: connector section editor: Add→Damping: Definition: Linear, Force/Moment: component or components, Coupling: Uncoupled Defining linear coupled viscous damping behavior In the linear coupled case you define the damping coefficient matrix components, the equation , which are used in where component of relative motion, is the force in the is the coupling between the component, and is the velocity in the components. The C matrix is assumed to be symmetric, so only the upper triangle of the matrix is specified. In connectors with kinematic constraints the entries that correspond to the constrained components of relative motion will be ignored. The damping coefficient can depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and field variables. and Input File Usage: Abaqus/CAE Usage: Use the following options to define linear coupled damping connector behavior: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR DAMPING, DEPENDENCIES=n Interaction module: connector section editor: Add→Damping: Definition: Linear, Force/Moment: component or components, Coupling: Coupled Defining unsymmetric linear coupled viscous damping behavior As with linear coupled elastic behavior (“Connector elastic behavior,” Section 31.2.2), Abaqus/Standard allows you to define an unsymmetric coupled viscous damping matrix. In the linear coupled case you define the damping coefficient matrix components, , which are used in the equation where is the force in the is the coupling between the component, and is the velocity in the components. The C matrix is assumed to be unsymmetric, so the entire matrix is specified. The entries that correspond to the constrained components of relative component of relative motion, and motion are ignored. When the unsymmetric matrix storage and solution scheme are used, the damping coefficients can depend on frequency, temperature, and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of frequency, temperature and field variables. Input File Usage: Use the following options to define unsymmetric linear coupled viscous damping connector behavior: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR DAMPING, UNSYMM, FREQUENCY DEPENDENCE=ON Abaqus/CAE Usage: Unsymmetric linear coupled viscous damping behavior is not supported in Abaqus/CAE. Defining nonlinear viscous damping behavior For nonlinear damping you specify forces or moments as nonlinear functions of the velocity in the available components of relative motion directions, . These functions can also depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and field variables. Defining nonlinear viscous damping behavior that depends on one component direction By default, each nonlinear force or moment function is dependent only on the velocity in the direction of the specified component of relative motion. Input File Usage: Use the following options: Abaqus/CAE Usage: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR DAMPING, COMPONENT=component number, NONLINEAR, DEPENDENCIES=n Interaction module: connector section editor: Add→Damping: Definition: Nonlinear, Force/Moment: component or components, Coupling: Uncoupled Defining nonlinear viscous damping behavior that depends on several component directions Alternatively, the functions can depend on the relative positions or constitutive displacements/rotations in several component directions, as described in “Defining nonlinear connector behavior properties to depend on relative positions or constitutive displacements/rotations” in “Connector behavior,” Section 31.2.1. Input File Usage: Use the following options to define nonlinear damping connector behavior that depends on components of relative position: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR DAMPING, COMPONENT=component number, NONLINEAR, INDEPENDENT COMPONENTS=POSITION, DEPENDENCIES=n Use the following options to define nonlinear damping connector behavior that depends on components of constitutive displacements or rotations: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR DAMPING, COMPONENT=component number, NONLINEAR, INDEPENDENT COMPONENTS=CONSTITUTIVE MOTION, DEPENDENCIES=n Interaction module: connector section editor: Add→Damping: Definition: Nonlinear, Force/Moment: component or components, Coupling: Coupled on position or Coupled on motion Abaqus/CAE Usage: Example Refer to the example in Figure 31.2.3–1. extensible range 7.5 node 12 1 (local orientation) node 11 Figure 31.2.3–1 Simplified connector model of a shock absorber. In addition to the torsional spring resisting relative rotations, the shock absorber damps translational motion along the line of the shock with a dashpot. To include a nonlinear dashpot behavior that is dependent on the relative position between the attachment points, use the following input: *CONNECTOR BEHAVIOR, NAME=sbehavior ... *CONNECTOR DAMPING, COMPONENT=1, INDEPENDENT COMPONENTS=POSITION, NONLINEAR 1500.0, 0.1, 0.0 1625.0, 0.2, 0.0 1750.0, 0.1, 10.0 1925.0, 0.2, 10.0 Defining linear structural damping behavior Structural connector damping is supported in steady-state dynamics and modal transient procedures that support non-diagonal damping (for example, direct solution steady-state dynamics). Defining linear uncoupled structural damping behavior You define the damping coefficients, component 2, etc.), which are used in the equation , for the selected components (i.e., for component 1, for where (no sum on ) is the structural damping matrix, relative motion, coefficient can depend on frequency. is the displacement in the is the imaginary part of the force or moment in the direction of is the stiffness matrix. The damping direction, and Input File Usage: Use the following options: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR DAMPING, COMPONENT=component number, TYPE=STRUCTURAL Abaqus/CAE Usage: Linear uncoupled structural damping behavior Abaqus/CAE. is not supported in Defining linear coupled structural damping behavior You define 21 which are used in the equation damping coefficients (the symmetric half of the 6 × 6 damping coefficient matrix), where (no sum on ) is the structural damping matrix, motion, coefficient matrix cannot depend on frequency. is the displacement in the is the imaginary part of the force in the direction of relative is the stiffness matrix. The damping direction, and Input File Usage: Use the following options: Abaqus/CAE Usage: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR DAMPING, TYPE=STRUCTURAL Linear coupled structural damping behavior is not supported in Abaqus/CAE. Defining connector damping behavior in linear perturbation procedures In both the direct-solution and subspace-based steady-state dynamic procedures, the viscous or structural damping defined using an uncoupled connector damping behavior may be frequency dependent. In other linear perturbation procedures connector damping behavior is ignored. Output The Abaqus output variables available for connectors are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The following output variables are of particular interest when defining damping in connectors: CV CVF Connector relative velocities/angular velocities. Connector viscous forces/moments. 31.2.4 CONNECTOR FUNCTIONS FOR COUPLED BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • “Connector friction behavior,” Section 31.2.5 • “Connector plastic behavior,” Section 31.2.6 • “Connector damage behavior,” Section 31.2.7 • *CONNECTOR BEHAVIOR • *CONNECTOR DERIVED COMPONENT • *CONNECTOR POTENTIAL • “Specifying connector derived components,” Section 15.17.15 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Specifying potential terms,” Section 15.17.16 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview This section describes how to define two special functions used to specify complex coupled behavior for a connector element in Abaqus: derived components and potentials. Connector derived components are user-specified component definitions based on a function of intrinsic (1 through 6) connector components of relative motion. They can be used: • to specify the friction-generating normal force in connectors as a complex combination of connector forces and moments, and • as an intermediate result in a connector potential function. Connector potentials are user-defined functions of intrinsic components of relative motion or derived components. These functions can be quadratic, elliptical, or maximum norms. They can be used to define: • the yield function for connector coupled plasticity when several available components of relative motion are involved simultaneously, • the potential function for coupled user-defined friction when the slip direction is not aligned with an available component of relative motion, • a magnitude measure as a coupled function of connector forces or motions used to detect the initiation of damage in the connector, and • an effective motion measure as a coupled function of connector motions to drive damage evolution in the connector. Defining derived components for connector elements The definition of coupled behavior in connector elements beyond simple linear elasticity or damping often requires the definition of a resultant force involving several intrinsic (1 through 6) components or the definition of a “direction” not aligned with any of the intrinsic components. These user-defined resultants or directions are called derived components. The forces and motions associated with these derived components are functions of the forces and motions in the intrinsic relative components of motion in the connector element. Consider the case of a SLOT connector for which frictional effects are defined in the only available component of relative motion (the 1-direction). The two constraints enforced by this connection type will produce two reaction forces ( ), as shown in Figure 31.2.4–1. Both forces generate friction in the 1-direction in a coupled and fashion. f3 f2 f1 slot housing Figure 31.2.4–1 Resultant contact force in a SLOT connector. A reasonable estimate for the resulting contact force is where is the collection of connector forces and moments in the intrinsic components. The function can be specified as a derived component. Resultant forces that can be defined as derived components may take more complicated forms. Consider a BUSHING connection type for which a tensile (Mode I) damage mechanism with failure is to be specified in the 1-direction. You may wish to include the effects of the axial force and of the resultant of the “flexural” moments in defining an overall resultant force in the axial direction upon which damage initiation (and failure) can be triggered, as shown in Figure 31.2.4–2. One choice would be to define the resultant axial force as and inner cylinder outer cylinder rubber f1 f axial m2 m3 Figure 31.2.4–2 Resultant axial force in a BUSHING connector. where is a geometric factor relating translations to rotations with units of one over length. The function can be specified as a derived component. A derived component can also be interpreted as a user-specified direction that is not aligned with the connector component directions. For example, if the motion-based damage with failure criterion in a CARTESIAN connection with elastic behavior does not align with the intrinsic component directions, the damage criterion can be defined in terms of a derived component representing a different direction, as shown in Figure 31.2.4–3. One possible choice for the direction could be where interpreted as direction cosines ( derived component. is the collection of connector relative motions in the components and , , ). The function , , and can be can be specified as a Functional form of the derived component The functional form of a derived component The derived component is specified as a sum of terms in Abaqus is quite general; you specify its exact form. U transf Figure 31.2.4–3 User-defined direction in a CARTESIAN connector. is a generic name for the connector intrinsic component values (such as forces, where ), are selected depending on the context in which the derived component is used. , or motions, is the number of terms. The appropriate component values for is also a summation term in the sum, and is the of several contributions and can take one of the following three forms: • a norm ( -type) • a direct sum ( -type) • a Macauley sum ( -type) where is the term’s sign (plus or minus), is the Macauley bracket ( , and ). In general, the units of the scaling factors depend on the context. In most cases they are either dimensionless, have units of length, or have units of one over length. The scaling factors should be chosen such that all the terms in the resulting derived component have the same units, and these units must be consistent with the use of the derived component later on in a connector potential or connector contact force. are scaling factors, component of is the Defining a derived component with only one term (NT = 1) Connector derived components are identified by the names given to them. If one term ( to define the derived component g, specify only one connector derived component definition. ) is sufficient Input File Usage: *CONNECTOR DERIVED COMPONENT, NAME=derived_component_name Abaqus/CAE Usage: Connector derived component names are not supported in Abaqus/CAE; you define the individual derived component terms. Use the following input to define a connector derived component term for a friction-generating user-defined contact force: Interaction module: connector section editor: Add→Friction: Friction model: User-defined, Contact Force, Specify component: Derived component, click Edit to display the derived component editor: click Add and select components Use the following input to define a connector derived component term as an intermediate result in a connector potential function: Interaction module: connector section editor: Add→Friction, Plasticity, or Damage: potential contribution editors: Specify derived component, click Edit to display the derived component editor: click Add and select components Defining a derived component containing multiple terms (NT > 1) If several terms ( define the individual terms. , , etc.) are needed in the overall definition of the derived component g, you must Input File Usage: You must specify connector derived component definitions with the same name to define the individual terms. All definitions with the same name will be summed together to produce the desired derived component g. See the spot weld example below for an illustration. *CONNECTOR DERIVED COMPONENT, NAME=derived_component_name *CONNECTOR DERIVED COMPONENT, NAME=derived_component_name ... Abaqus/CAE Usage: Connector derived component names are not supported in Abaqus/CAE; you define the individual derived component terms. Interaction module: derived component editor: click Add and select components. Repeat, adding terms as necessary. Specifying a term in the derived component as a norm By default, a derived component term is computed as the square root of the sum of the squares of each intrinsic component contribution. If the term has only one contribution ( ), the norm has the same meaning as the absolute value. Input File Usage: *CONNECTOR DERIVED COMPONENT, NAME=derived_component_name, OPERATOR=NORM (default) component For example, the following input can be used to define the discussed above: *CONNECTOR DERIVED COMPONENT, NAME=axial 1.0, ** *CONNECTOR DERIVED COMPONENT, NAME=axial 5, 6 , ** Abaqus/CAE Usage: The axial derived component is Interaction module: derived component editor: Add: Term operator: Square root of sum of squares . Specifying a term in the derived component as a direct sum Alternatively, you can choose to compute a derived component term as the direct sum of the intrinsic component contributions. Input File Usage: *CONNECTOR DERIVED COMPONENT, NAME=derived_component_name, OPERATOR=SUM component For example, the following input can be used to define the discussed above: *CONNECTOR DERIVED COMPONENT, NAME=transf, OPERATOR=SUM 1, 2, 3 , , ** The transf derived component is Interaction module: derived component editor: Add: Term operator: Direct sum . 31.2.4–6 Specifying a term in the derived component as a Macauley sum Alternatively, you can choose to compute a derived component term as the Macauley sum of the intrinsic component contributions. Input File Usage: *CONNECTOR DERIVED COMPONENT, NAME=derived_component_name, OPERATOR=MACAULEY SUM For example, the following input can be used to define the first term of the normal component of the force ( ) in the spotweld example discussed below: *CONNECTOR DERIVED COMPONENT, NAME=normal, OPERATOR=MACAULEY SUM 1.0 ** Abaqus/CAE Usage: Interaction module: derived component editor: Add: Term operator: Macauley sum Specifying the sign of a term You can specify whether the sign of a derived component term should be positive or negative. Input File Usage: Abaqus/CAE Usage: Use one of the following options: *CONNECTOR DERIVED COMPONENT, NAME=derived_component_name, SIGN=POSITIVE (default) *CONNECTOR DERIVED COMPONENT, NAME=derived_component_name, SIGN=NEGATIVE Interaction module: derived component editor: Add: Overall term sign: Positive or Negative Defining the derived component contributions to depend on local directions The scaling factors used in the definition of the derived component can depend on the relative positions or constitutive displacements/rotations in several component directions, as described in “Defining nonlinear connector behavior properties to depend on relative positions or constitutive displacements/rotations” in “Connector behavior,” Section 31.2.1. See the first example in “Connector friction behavior,” Section 31.2.5, for an illustration. Input File Usage: Use the following option to define a connector derived component that depends on components of relative position: *CONNECTOR DERIVED COMPONENT, INDEPENDENT COMPONENTS=POSITION Use the following option to define a connector derived component that depends on components of constitutive displacements or rotations: *CONNECTOR DERIVED COMPONENT, INDEPENDENT COMPONENTS=CONSTITUTIVE MOTION Abaqus/CAE Usage: Interaction module: derived component editor: Add: Use local directions: Independent position components or Independent constitutive motion components Requirements for constructing a derived component used in plasticity or friction definitions When a derived component is used to construct the yield function for a plasticity or friction definition, the following simple requirements must be satisfied: • All terms of a derived component must be of a compatible type cannot be mixed with direct sum-type terms -type) in the same derived component definition but can be mixed with Macauley sum-type derived component”); norm-type terms ( ( terms ( -type). • If all terms are norm-type terms, the sign of each term must be positive (the default). is greater than 1, the associated functions (potentials) in which the derived component is used If may become non-smooth. More precisely, the normal to the hyper-surface defined by the potential may experience sudden changes in direction at certain locations. In these cases, Abaqus will automatically smooth-out the defined functions by slightly changing the derived component functional definition. These changes should be transparent to the user as the results of the analysis will change only by a small margin. Example: spot weld The spot weld shown in Figure 31.2.4–4 is subjected to loading in the F-direction. Fn Figure 31.2.4–4 Loading of a spot weld connection. The connector chosen to model the spot weld has six available components of relative motion: three translations (components 1–3) and three rotations (components 4–6). You have chosen this connection type because you are modeling a general deformation state. However, you would like to define inelastic behavior in the connection in terms of a normal and a shear force, as shown in Figure 31.2.4–5, since experimental data are available in this format. plates spot weld Fn Fs Fn f3 m3 m1 m2 f1 Fs f2 Figure 31.2.4–5 Spot weld connection: derived component definitions. Therefore, you want to derive the normal and shear components of the force, for example, as follows: and In these equations have units of length; their interpretation is relatively straightforward if you consider the spot weld as a short beam with the axis along the spot weld axis (3-direction). If the average cross-section area of the spot weld is A and the beam’s second moment of inertia about one of the in-plane axes is ). Furthermore, if the cross-section is considered to be circular, becomes equal to a fraction of the spot weld radius. In all cases can be taken to be can be interpreted as the square root of the ratio (or (or ), . The reasoning above for the interpretation of the calibration constants in the equations is only a suggestion. In general, any combination of constants that would lead to good comparisons with other results (experimental, analytical, etc.) is equally valuable. To define with the same name: , you would specify the following two connector derived component definitions, each *PARAMETER =30.68 A=19.63 =sqrt( = ) *CONNECTOR DERIVED COMPONENT, NAME=normal, OPERATOR=MACAULEY SUM 1.0 *CONNECTOR DERIVED COMPONENT, NAME=normal 4, 5 , symbols denote that The component derived component defines the first term is specified using a parameter definition. The normal force derived . The first connector , while the second defines the second term is defined as the sum of two terms, . Similarly, to define , you would specify the following two connector derived component definitions for the component shear: *CONNECTOR DERIVED COMPONENT, NAME=shear *CONNECTOR DERIVED COMPONENT, NAME=shear 1, 2 1.0, 1.0 Defining connector potentials Connector potentials are user-defined mathematical functions that represent yield surfaces, limiting surfaces, or magnitude measures in the space spanned by the components of relative motion in the connector. The functions can be quadratic, general elliptical, or maximum norms. The connector potential does not define a connector behavior by itself; instead, it is used to define the following coupled connector behaviors: • friction, • plasticity, or • damage. Consider the case of a SLIDE-PLANE connection in which frictional sliding occurs in the connection plane, as shown in Figure 31.2.4–6. The function governing the stick-slip frictional behavior can be written as where is the connector potential defining the pseudo-yield function (the magnitude of the frictional tangential tractions in the connector in a direction tangent to the connection plane on which contact occurs), is the friction coefficient. Frictional stick occurs if . In this case the potential can be defined as the magnitude of the frictional tangential tractions, is the friction-producing normal (contact) force, and , and sliding occurs if fn f2 normal direction f3 sliding with friction in this plane Figure 31.2.4–6 Friction in the SLIDE-PLANE connection. Connector potentials can also be useful in defining connector damage with a force-based coupled damage initiation criterion. For example, in a connection type with six available components of relative motion you could define a potential Damage (with failure) can be initiated when the value of the potential limiting value (usually 1.0). The units of the and final product. For example, if the intended units of while the coefficients have units of one over length. is greater than a user-specified coefficients must be consistent with the units of the coefficients are dimensionless are newtons, the Connector potentials can take more complicated forms. Assume that coupled plasticity is to be defined in a spot weld, in which case a plastic yield criterion can be defined as where potential could be defined as is the connector potential defining the yield function and is the yield force/moment. The could be the named derived components normal and shear defined in the example and where in “Defining derived components for connector elements” above. If also have units of force, are dimensionless. and has units of force and and Input File Usage: Abaqus/CAE Usage: *CONNECTOR POTENTIAL Use the following input to define connector potentials for friction behavior: Interaction module: connector section editor: Add→Friction: Friction model: User-defined, Slip direction: Compute using force potential, Force Potential Use the following input to define connector potentials for plasticity behavior: Interaction module: connector section editor: Add→Plasticity: Coupling: Coupled, Force Potential Use the following input to define connector potentials for damage behavior: Interaction module: connector section editor: Add→Damage: Coupling: Coupled, Initiation Potential or Evolution Potential Functional form of the potential The functional form of the potential potential is specified as one of the following direct functions of several contributions: in Abaqus is quite general; you specify its exact form. The a quadratic form a general elliptical form a maximum form where ), is a generic name for the connector intrinsic component values (such as forces, and is the number of contributions, contribution to the potential, , or motions, are positive is the overall sign of the contribution (1.0 – default, or −1.0). are selected depending on the context in which the potential is ), and 2.0, is the numbers (defaults The appropriate component values for used in. The positive exponents ( yields a real number. , ) and the sign should be chosen such that the contribution is a direct function of either an intrinsic connector component (1 through 6) or a derived connector component. Since derived components are ultimately a function of intrinsic components , the contribution is defined as is ultimately a function of . where is the function used to generate the contribution: • absolute value (default, • Macauley bracket ( • identity (X); ), is the value of the identified component (intrinsic or derived); is a shift factor (default 0.0); and is a scaling factor (default 1.0). ), or can be the identity function only if The function . The units of the various coefficients in the equations above depend on the context in which the potential is used. In most cases the coefficients in the equations above are either dimensionless, have units of length, or have units of one over length. In all cases you must be careful in defining potentials for which the units are consistent. Defining the potential as a quadratic or general elliptical form To define a general elliptical form of the potential, you must specify the inverse of the overall exponent, if they are different from the default value, which is the specified . You can also define the exponents value of . Input File Usage: To define a quadratic form of the potential, you can omit specifying default value is 2.0. Use the following option: *CONNECTOR POTENTIAL component name or number, ... , , , , since its Use the following option to define a general elliptical form of the potential: *CONNECTOR POTENTIAL, OPERATOR=SUM, EXPONENT= component name or number, ... , , , , Abaqus/CAE Usage: Each data line defines one contribution to the potential, can be ABS (absolute value and the default), MACAULEY (Macauley bracket), or NONE (identity). . The function Interaction module: connector section editor: friction, plasticity, or damage behavior option: Force Potential, Initiation Potential, or Evolution Potential: Operator: Sum, Exponent: 2 (for quadratic form) or (for elliptical form), select Add and enter data for the potential contribution. Repeat, adding contributions as necessary. Defining the potential as a maximum form Alternatively, you can define the potential as a maximum form. Input File Usage: *CONNECTOR POTENTIAL, OPERATOR=MAX component name or number, ... Each data line defines one contribution to the potential, can be ABS (absolute value and the default), MACAULEY (Macauley bracket), or NONE (identity). . The function , , , , Abaqus/CAE Usage: Interaction module: connector section editor: friction, plasticity, or damage behavior option: Force Potential, Initiation Potential, or Evolution Potential: Operator: Maximum, select Add and enter data for the potential contribution. Repeat, adding contributions as necessary. Requirements for constructing a potential used in plasticity or friction definitions The connector potential, , can be defined using intrinsic components of relative motion, derived components, or both. A particular contribution to the potential may be one of the following two types: • A norm-type contribution ( ) defined using the absolute value or the Macauley bracket functions or using a combination of norm-type derived components with any of the available functions. and Macauley sum-type • A sum-type contribution ( ) defined using an intrinsic component of relative motion or a derived together with the identity function. When used in the context of connector plasticity or connector friction, the potential must be constructed such that the following requirements are satisfied: • All contributions to the potential must be of the same type. Mixed and contributions are not allowed in the same potential definition. • If all • The positive numbers terms are -type terms, the sign of each term must be positive (the default). and cannot be smaller than 1.0 and must be equal (the default). Example: spot weld Referring to the spot weld shown in Figure 31.2.4–5 and the yield function defined above, you would define this potential using the derived components normal and shear with the following input: *PARAMETER =0.02 =0.05 =1.5 *CONNECTOR POTENTIAL, EXPONENT= normal, , , MACAULEY shear, , , ABS Output The Abaqus/Explicit output variables available for connectors are listed in “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The following variables (available only in Abaqus/Explicit ) are of particular interest when defining connector functions for coupled behavior: CDERF CDERU Connector derived force/moment with the connector derived component name appended to the output variable. If the connector derived component is used with connector plasticity, connector friction, and connector damage initiation (type force), the derived components used to form the potential represent forces and this quantity is available for both field and history output. If connector friction is used with contact force, the derived components are not used to form a potential, and the derived force is in fact the connector normal force CNF (which is available for connector history output.) Connector derived displacement/rotation with the connector derived component name appended to the output variable. If the connector derived component is used with motion type for the connector damage initiation and connector damage evolution, the derived components to form the potential represent displacements and this quantity is available for both field and history output. 31.2.5 CONNECTOR FRICTION BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • “Connector behavior,” Section 31.2.1 • “Connector functions for coupled behavior,” Section 31.2.4 • *CHANGE FRICTION • *CONNECTOR BEHAVIOR • *CONNECTOR DERIVED COMPONENT • *CONNECTOR FRICTION • *CONNECTOR POTENTIAL • *FRICTION • “Defining friction,” Section 15.17.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Frictional effects can be defined in any connector with available components of relative motion. A typical connector might have several pieces that are in relative motion and are contacting with friction. Therefore, both frictional forces and frictional moments may develop in the connector available components of relative motion. To define connector friction in Abaqus, you must specify the following: • the friction law as governed by a friction coefficient; • the contributions to the friction-generating connector contact forces or moments; and • the local “tangent” direction in which the friction forces/moments act. The friction coefficient can be • expressed in a general form in terms of slip rate, contact force, temperature, and field variables; • defined by a static and kinetic term with a smooth transition zone defined by an exponential curve; and • limited by a tangential maximum force, can be carried by the connector before sliding occurs. , which is the maximum value of tangential force that Abaqus provides two alternatives for specifying the other aspects of friction interactions in connectors: • Predefined friction interactions for which you need to specify a set of parameters that are characteristic of the connection type for which friction is modeled. Abaqus automatically defines the contact force contributions and the local “tangent” directions in which friction occurs. Predefined friction interactions represent common cases and are available for many connection types . If desired, known internal contact forces (such as from a press-fit assembly) can be defined as well. • User-defined friction interactions for which you define all friction-generating contact force contributions and the local “tangent” directions along which friction occurs. The user-defined friction interactions can be used if predefined friction is not available for the connection type of interest or if the predefined friction interaction does not adequately describe the mechanism being analyzed. Although more complicated to utilize, user-defined interactions: – are very general in nature due to flexibility in defining arbitrary sliding directions via connector potentials and contact forces via connector derived components; – allow for the specification of sliding directions, contact forces, and additional internal contact forces as functions of connector relative position or motion, temperature, and field variables (the internal contact forces can also be dependent on accumulated slip); and – allow for several friction definitions to be used in the same connection applied in different components of relative motion. Friction formulation in connectors The basic concept of Coulomb friction between two contacting bodies is the relation of the maximum allowable frictional (shear) force across an interface to the contact force between the contacting bodies. In the basic form of the Coulomb friction model, two contacting surfaces can carry shear forces, , up to a certain magnitude across their interface before they start sliding relative to one another; this state is known as sticking. The Coulomb friction model defines this critical shear force as is the coefficient of friction and is the contact force. The stick/slip calculations determine when a point transitions from sticking to slipping or from slipping to sticking. Mathematically, the relationship can be formalized as , where Frictional stick occurs if ; and sliding occurs if , in which case the friction force is . Friction in connectors is based on the analogy that contacting surfaces of various parts inside a connector device transmit tangential as well as normal forces across their interfaces. The normal (contact) forces, , are typically generated by kinematic constraints or by elastic forces/moments in the connector. Connector friction can be used to model tangential (shear) forces, , in the space spanned by the available components of relative motion for both stick and slip conditions. Figure 31.2.5–1 illustrates the simplest frictional mechanism in connectors, a SLOT connector in a two-dimensional analysis. The local tangent direction in which frictional sliding occurs is the 1-direction (tangential traction ), and the normal force is developed by the kinematic constraint enforcing the SLOT constraint in the 2-direction, . The friction model is defined in this case by f2 f1 Figure 31.2.5–1 Friction in a two-dimensional SLOT connection. which in case of slip predicts a friction force as expected. In this case the friction model is straightforward to understand as the slip direction is along an intrinsic (1 through 6) component of relative motion and the normal force is given only by the force in one other single component orthogonal to the sliding direction. In many connectors the definition of the tangential tractions is more complex. For example, friction may develop in a tangent direction that spans two or more available components of relative motion. Consider the case of frictional sliding in a SLIDE-PLANE connection as illustrated in “Connector In this case the friction-generating normal force is functions for coupled behavior,” Section 31.2.4. given by the constraint force in the 1-direction, . However, the magnitude of the tangential tractions is given by thus including contributions from two components of relative motion. The instantaneous direction of frictional slip in the 2–3 plane is not known a priori. In many connectors the normal force may have contributions from several connector components. Consider the case of a three-dimensional SLOT as illustrated in “Connector functions for coupled behavior,” Section 31.2.4. In this case the magnitude of the tangential tractions is given by , but the normal force is generated by constraint forces in both the 2- and 3-directions and can be written as In the most general case both the tangential tractions and the normal force may have contributions from several components. Further, the component directions may include both translations (forces) and rotations (moments). Thus, friction modeling in connectors is defined in a more general form, as follows. First, the function governing the stick-slip condition is defined as where is the connector potential , which represents the magnitude of the frictional is the collection of forces in the connector; tangential tractions in the connector in a direction tangent to the surface on which contact occurs; and is the friction-producing normal (contact) force on the same contact surface. Frictional stick occurs if ; and sliding occurs if , in which case the friction force is . The normal force, , is the sum of a magnitude measure of contact force-producing connector , and a self-equilibrated internal contact force (such as from a press-fit assembly), forces, : is given by a connector derived component definition as illustrated in “Connector The function functions for coupled behavior,” Section 31.2.4. Using this formalism, we can easily reconstruct the examples illustrated above: • In the two-dimensional SLOT case, • In the SLIDE-PLANE case, • In the three-dimensional SLOT case, and and and . . . See the examples at the end of this section for more complex illustrations of friction definitions in connectors. If frictional effects are defined for a rotational component of relative motion (such as in a HINGE connector), it is often more convenient to define “tangential” moments and “normal” moments instead of tangential tractions/forces and normal forces. The pseudo-yield function governing the stick/slip behavior is defined in a similar fashion: where the “normal” moment is written as is the self-equilibrated friction-generating internal “contact” moment (for example, from press fit). See “Specifying friction in a HINGE connection” at the end of this section for an illustration. Predefined friction behavior Predefined friction interactions allow you to model typical frictional mechanisms in commonly used connector types without having to define the mechanics of the frictional response. Instead of specifying the potential, , directly to define the magnitude measure of the tangential tractions and the contact force via a derived component, you specify: • a set of friction-related parameters associated with the connection type, which include geometric or contact parameters specific to the connection type and, optionally, the internal contact force moment ; and • the friction law (governed by the friction coefficient) as described in “Defining the friction coefficient.” Abaqus then automatically generates internally the potential, , based on the connection type and geometric parameters provided. Table 31.2.5–1 shows the connection types for which predefined friction interactions are available and the associated friction-related parameters. The meanings of the geometric parameters as well as the corresponding potentials and derived components automatically generated by Abaqus are described in “Connection-type library,” Section 31.1.5. , and the contact force, Table 31.2.5–1 Predefined friction-related parameters. Connection type Friction-related parameters Geometric parameters Internal contact force/moment CYLINDRICAL R, L HINGE PLANAR SLIDE-PLANE SLOT TRANSLATOR UJOINT SLIPRING , , , None None , L , , , None , None See the examples at the end of this section for illustrations of predefined friction. Input File Usage: *CONNECTOR FRICTION, PREDEFINED friction-related parameters outlined in Table 31.2.5–1 Abaqus/CAE Usage: Interaction module: connector section editor: Add→Friction: Friction model: Predefined, Predefined Friction Parameters, enter the friction-related parameters outlined in Table 31.2.5–1 in the data table User-defined friction behavior User-defined friction behavior can be used if predefined friction is not available for the connection type of interest or if the predefined friction interaction does not describe adequately the mechanism being analyzed. For user-defined friction you must specify: • “tangent” direction information, as follows: – if the slip direction is known, you specify directly the direction in which friction forces/moments act, from which Abaqus constructs the potential ; – if the slip direction is unknown, you specify the potential from which Abaqus computes the instantaneous slip direction; • the friction-producing normal force, following: , or normal moment, , by defining at least one of the – the contact force – the internal contact force or contact moment ; and/or or contact moment ; and • the friction law (governed by the friction coefficient) as described in “Defining the friction coefficient.” Specifying the slip direction aligned with an available component of relative motion The friction tangent direction is identified by specifying an available component (1–6) to define friction forces or moments in a specified intrinsic connector local direction. This is the natural choice in cases when the connector element has only one available component of relative motion (for example, SLOT, REVOLUTE, or TRANSLATOR); in these cases the relative slip between the various parts forming the physical connection occurs in one local direction only. In connections with two or more available components of relative motion, specifying a particular available component of relative motion allows you to specify frictional effects in that direction only, if desired. For example, in the case of a CYLINDRICAL connection, specifying component 1 defines frictional effects only in translation while rotation around the axis is ignored for friction. Abaqus constructs the potential, , automatically as where is the force/moment in the specified component i. Input File Usage: Abaqus/CAE Usage: *CONNECTOR FRICTION, COMPONENT=i Interaction module: connector section editor: Add→Friction: Friction model: User-defined, Slip direction: Specify direction, component Specifying the potential when the slip direction is unknown In connection types with two or more available components of relative motion, frictional slipping is not necessarily solely along one of the available components of relative motion. In such cases the instantaneous slip direction is not known, as illustrated in the SLIDE-PLANE case in “Friction formulation in connectors.” Another example is the CYLINDRICAL connection in which frictional sliding occurs in a direction tangent to the cylindrical surface, thus involving simultaneously a translational slip in the local 1-direction and a rotational slip about the same axis . Thus, frictional slip may occur in a coupled fashion spanning several available components simultaneously. In such cases you must specify the magnitude measure of the tangential tractions on the assumed contact surface using a connector potential definition, . Abaqus then computes the instantaneous slip direction simultaneously with the stick-slip determination similar to the surface-based three-dimensional frictional contact computations described in “Coulomb friction,” Section 5.2.3 of the Abaqus Theory Manual. This procedure is best illustrated for the SLIDE-PLANE case, as follows: • First, the potential is evaluated. • Slipping occurs if the pseudo-yield function • The two vector components (the local 2- and 3-directions) of the instantaneous slip direction are , normalized by the magnitude of the potential. and given by the ratios of the two shear forces, . In general, this strategy is extended to the space spanned by the available components of relative motion associated with the connection type that ultimately participate in the potential definition . For example, up to two components for SLIDE-PLANE or CYLINDRICAL connections, three components for CARDAN connections, and six components for a user-assembled connection using CARTESIAN and CARDAN connections can be included in the potential. See the examples below for several illustrations. Input File Usage: Use the following two options to specify coupled user-defined friction: Abaqus/CAE Usage: *CONNECTOR FRICTION *CONNECTOR POTENTIAL Interaction module: connector section editor: Add→Friction: Friction model: User-defined, Slip direction: Compute using force potential, Force Potential Specifying the contact force You specify the friction-generating user-defined contact force, , or contact moment, , by referring to either an intrinsic component of relative motion number (1 through 6) or a named connector derived component . In the latter case the scaling parameters used in the definition of can be made functions of identified local directions, temperature, and field variables. It is often desirable to include contributions from both connector forces and moments in the definition of the derived component. In these cases the scaling parameters used to define the derived components should have units of length or one over length for meaningful contact force/moment definitions. Input File Usage: Use the following option to define a contact force for connector friction using an intrinsic connector component: Abaqus/CAE Usage: *CONNECTOR FRICTION, CONTACT FORCE=component number (1–6) Use the following options to define a contact force for connector friction using a connector derived component: *CONNECTOR DERIVED COMPONENT, NAME=derived_component_name *CONNECTOR FRICTION, CONTACT FORCE=derived_component_name Interaction module: connector section editor: Add→Friction: Friction model: User-defined, Contact Force, Specify component: Intrinsic component or Derived component, component or specify derived component Connector derived component names are not supported in Abaqus/CAE. Specifying the internal contact force Internal contact forces such as contact interference may occur in connectors during the physical assembly of the various pieces forming the connector (for example, a press-fit shaft into the sleeve of a CYLINDRICAL connection). When relative motion occurs between the connector parts, these self-equilibrating contact stresses will produce contact forces, ; see “Friction formulation in connectors.” , or contact moments, The internal contact forces/moments are created by specifying a contact force/moment curve (positive values only) as a function of accumulated slip, temperature, and field variables. The accumulated slip is computed as the sum of the absolute values of all slip increments in an instantaneous slip direction. Consequently, the accumulated slip is monotonically increasing for oscillatory or periodic motion and can be used to model dependencies related to wear or heat generation in the connection. Input File Usage: Abaqus/CAE Usage: The internal contact forces limiting curve is defined on the data lines of the *CONNECTOR FRICTION option. Interaction module: connector section editor: Add→Friction: Friction model: User-defined, Contact Force, and enter the Internal Contact Force in the data table Specifying the internal contact force to depend on local directions The internal contact force can also be defined as dependent on either connector relative positions or constitutive relative motions. Input File Usage: Abaqus/CAE Usage: Use the following option to define an internal contact force that depends on components of relative position: *CONNECTOR FRICTION, INDEPENDENT COMPONENTS=POSITION Use the following option to define an internal contact force that depends on components of constitutive displacements or rotations: *CONNECTOR FRICTION, INDEPENDENT COMPONENTS=CONSTITUTIVE MOTION Interaction module: connector section editor: Add→Friction: Friction model: User-defined, Contact Force, Use independent components: Position or Motion Defining the friction coefficient The connector friction definition uses the standard friction model described in “Frictional behavior,” Section 36.1.5, to define the friction coefficient. The anisotropic friction and friction data associated with the second contact direction are ignored for connector elements. If the friction coefficients are not specified or are set to zero, the connector friction has no effect on the connector behavior. If the equivalent shear force/moment limit, , is specified , the limiting friction force is replaced by in the pseudo-yield function . Rough, Lagrange, and user-defined friction cannot be used in connector elements. Input File Usage: Use the following options: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR FRICTION *FRICTION Abaqus/CAE Usage: Interaction module: connector section editor: Add→Friction: Tangential Behavior, Friction Coefficient, and enter the Friction Coeff. in the data table Changing the friction coefficients during an Abaqus/Standard analysis In Abaqus/Standard the friction coefficients can be changed during the analysis as for any analysis including friction . Controlling the unsymmetric solver in Abaqus/Standard In Abaqus/Standard friction constraints produce unsymmetric terms when the connector nodes are sliding relative to each other. These terms have a strong effect on the convergence rate if frictional stresses have a substantial influence on the overall displacement field and the magnitude of the frictional stresses is highly solution dependent. Abaqus/Standard will automatically use the unsymmetric solution method if the coefficient of friction is greater than 0.2. If desired, you can turn off the unsymmetric solution method as described in “Defining an analysis,” Section 6.1.2. Defining the stick stiffness Abaqus determines whether the connector is sticking or slipping in a similar fashion as for all contact interactions , as outlined in “Friction formulation in connectors.” If the model is sticking, the elastic stiffness of the response is determined by the optional stick stiffness that is specified as part of the connector friction definition. If the stick stiffness is not specified, Abaqus will compute a usually appropriate stick stiffness. In Abaqus/Standard a maximum allowable elastic slip length (or angle) is first defined using either the value of the slip tolerance, , together with an automatically computed characteristic length (angle) in the model or the absolute magnitude of the allowable elastic slip, , to be used in the stiffness method for sticking friction directly . The elastic stick stiffness is then determined by simply dividing the current connector limiting friction force by this maximum allowable elastic slip length (angle). In Abaqus/Explicit the elastic stick stiffness is determined from the Courant (stability) condition. Input File Usage: Abaqus/CAE Usage: *CONNECTOR FRICTION, STICK STIFFNESS=elastic stiffness Interaction module: connector section editor: Add→Friction: Stick stiffness: Specify: elastic stiffness Using multiple connector friction definitions Multiple connector frictions can be used as part of the same connector behavior definition. However, only one connector friction definition can be used to define friction interactions for each available component of relative motion. If predefined friction is used, only one connector friction definition can be associated with a connector behavior definition. At most one coupled user-defined friction definition can be associated with a connector behavior definition. Additional connector friction definitions are permitted for the same connector behavior definition only if the component relative motion spaces for each definition do not overlap; for example, you could define uncoupled connector friction in components 1, 2, and 6 and coupled connector friction (by defining a potential) using components 3, 4, and 5. All connector friction definitions act in parallel and will be summed if necessary. For a particular connector element there will be as many stick-slip calculations as connector friction definitions. See the examples below. Examples The following examples illustrate how to define friction in connector elements. Equivalent ways of specifying friction behavior in a CYLINDRICAL connection In the example in Figure 31.2.5–2 assume Coulomb-like friction affects the translational motion along the shock and the rotational motion about the shock axis. li 2r Figure 31.2.5–2 Simplified connector model of a shock absorber. The coefficient of friction is , and the overlapping length for the two parts of the shock is length units in the undeformed configuration. An average radius of the two cylinders is considered to be units. It is also assumed that the axial motion in the connection is relatively small so that the overlapping length between the connector parts does not change much. The friction-generating contact force has contributions from two sources: • the normal force from the inner walls pushing against each other (the vector magnitude of the Lagrange multipliers imposing the SLOT constraint), and • the “bending” in the REVOLUTE constraint (the vector magnitude of the Lagrange multipliers imposing the REVOLUTE constraint). See “Connection-type library,” Section 31.1.5, for a detailed discussion of predefined contact forces and tangential tractions in the CYLINDRICAL connection. Two equivalent alternatives to model these frictional effects are shown below: A. Using the Abaqus predefined friction behavior: *PARAMETER r=0.24 =0.55 ... *CONNECTOR FRICTION, PREDEFINED , *FRICTION 0.15 Using a predefined connector friction behavior yields the most compact definition of frictional effects. This definition requires only the specification of the two friction-relevant geometrical scaling constants. B. Using a user-defined frictional behavior: *PARAMETER r=0.24 =0.55 =1.0 =2.0/ ... *CONNECTOR BEHAVIOR, NAME=shock *CONNECTOR DERIVED COMPONENT, NAME=normal 2, 3 , **( ) *CONNECTOR DERIVED COMPONENT, NAME=normal, 5, 6 , ) **( *CONNECTOR FRICTION, CONTACT FORCE=normal *CONNECTOR POTENTIAL 1, 4, *FRICTION 0.15 The contact force “normal” is defined by The connector potential defines the magnitude of the tangential tractions as This force magnitude is tangent to the cylindrical surface of the connector on which contact occurs. The choice of normal force definition and potential in this case ensures that the same frictional effects defined in Case A are modeled. Specifying friction interactions in a CYLINDRICAL connection accounting for position dependencies In the example in Figure 31.2.5–2 assume that large axial motion occurs between the two connector parts and, hence, the overlapping length will change significantly during the analysis. For the sake of discussion, assume that the two connector nodes are specified to be overlapped in the initial configuration. Thus, at CP1=0.0 the initial overlap is as specified above. If during the analysis the connector relative position along the 1-component reaches CP1=0.45 units, the final overlap would be . If the connection is subjected to a “bending-like” loading, one can argue that as the overlapping length decreases, the contact forces developed between the two parts become increasingly higher. Use the following user-defined friction behavior definitions to model this dependence of the contact force on relative positions: *PARAMETER r=0.24 =0.55 =0.1 =1.0 =2.0/ =2.0/ ... *CONNECTOR BEHAVIOR, NAME=shock *CONNECTOR DERIVED COMPONENT, NAME=normal 2, 3 , **( ) *CONNECTOR DERIVED COMPONENT, NAME=normal, INDEPENDENT COMPONENTS=POSITION 5, 6 **( , , , 0 , 0.45 at CP1=0.0) **( *CONNECTOR FRICTION, CONTACT FORCE=normal at CP1=0.45) *CONNECTOR POTENTIAL 1, 4, *FRICTION 0.15 Specifying friction due to assembly contact interference Assume a CYLINDRICAL connector element in which the shaft was press-fit into the sleeve, as shown in the initial configuration (relative motion = 0.0) in Figure 31.2.5–3. 2r Figure 31.2.5–3 CYLINDRICAL connection with slightly conical pin. The shaft is not perfectly cylindrical but slightly conical so that its cross-section diameter is increasing in a linear fashion along the shaft direction. If the relative displacement along the shaft direction becomes positive, the contact forces will increase (more contact interference); if the relative displacements become negative (less interference), they will decrease. An exponential decay model is assumed to model the transition from a static coefficient of friction to a kinetic one. Only the positive contact force versus displacement values need to be specified. The following user-defined friction behavior definitions can be used: *PARAMETER r=0.24 ... *CONNECTOR FRICTION, INDEPENDENT COMPONENTS=CONSTITUTIVE MOTION ** (independent component 1) 0.70, -0.7854 0.85, -0.3927 0.0 1.0 , 0.3927 1.15, 1.30, 0.7854 *CONNECTOR POTENTIAL 1, 4, *FRICTION, EXPONENTIAL DECAY ... 0.25, 0.10, 0.2 The internal contact forces are specified directly on the data lines to model known contact interference forces as a function of the connector constitutive component of relative motion along component 1. Since no intrinsic component of relative motion number or named connector derived component was specified to define the contact force, the only contribution to the contact force is the specified internal contact force. Specifying friction in a HINGE connection This example illustrates the use of a connector friction definition to specify frictional effects in a HINGE connection. The friction behavior defines friction moments about the 1-direction, since there are no other available components of relative motion. As illustrated in “Connection-type library,” Section 31.1.5, the three geometrical scaling constants that need to be specified for predefined friction are the radius of the pin cross-section, =0.14; and the overlapping length between the pin and the sleeve, =0.65. The friction coefficient is assumed to be =0.15. It is assumed that the connector has been assembled with initial known contact interference-producing contact moments of units. The following input could be used to specify the predefined friction behavior in the HINGE connection: =0.12; the effective friction arm in the axial direction, *PARAMETER =0.12 =0.14 =0.65 ... *CONNECTOR FRICTION, PREDEFINED , , , 100.0 *FRICTION 0.15 Alternatively, a user-defined friction behavior could be specified to define identical frictional effects . Moreover, a reduction of the interference contact forces as the pin wears due to accumulated sliding can be modeled in this case by specifying the internal contact forces/moments to be functions of accumulated slip. The following input can be used: *PARAMETER =0.12 =0.14 =0.65 = = =2.0* ... *CONNECTOR DERIVED COMPONENT, NAME=contact_moment 1, , ** ( ) *CONNECTOR DERIVED COMPONENT, NAME=contact_moment 2, 3 , **( *CONNECTOR DERIVED COMPONENT, NAME=contact_moment 5, 6 ) , ) **( *CONNECTOR FRICTION, COMPONENT=4, CONTACT FORCE=contact_moment 100, 0.0 90 , 1000.0 ** interference contact moments decreasing due to wear effects *FRICTION 0.15 The additional friction moments due to contact interference are modeled by specifying decreasing internal contact moments as a function of accumulated rotational slip about the 1-direction. The connector derived component definitions are used to define a contact moment-producing friction in the same direction (component 4). The contact moment is defined by The connector potential is defined automatically by Abaqus as . Specifying friction in a ball-in-socket connection This example illustrates the specification of frictional effects in a ball-in-socket connection. While the first choice in defining a ball-in-socket connection is JOIN and ROTATION, other rotation parameterizations could be used (JOIN and CARDAN, JOIN and EULER, or JOIN and FLEXION-TORSION). Assuming that the radius of the ball is and the coefficient of friction is , the following lines can be used to define the friction interactions: *PARAMETER =0.30 ... *CONNECTOR DERIVED COMPONENT, NAME=normal 1, 2, 3 1.0, 1.0, 1.0 **( ) *CONNECTOR FRICTION, CONTACT FORCE=normal *CONNECTOR POTENTIAL 4, 5, 6, *FRICTION 0.15 The computed connector friction moments and the friction-induced moments at the connector nodes are dependent on the connection type. Defining connector friction behavior in linear perturbation procedures Frictional slipping is not allowed in linear perturbation procedures. If a connector is slipping at the end of the last general analysis step, it will slip freely during the current linear perturbation step. Otherwise, Abaqus will allow the connector to slip elastically with the specified stick stiffness or enforce a sticking condition if a stick stiffness is not specified. Output The Abaqus output variables available for connectors are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The following variables are of particular interest when defining friction in connectors: CSF CNF CASU CIVC In addition to the usual six components Connector friction forces/moments. associated with connector output variables, CSF includes the scalar CSFC, which is the friction force generated by a coupled friction definition. Connector normal forces/moments. CNF includes the scalar CNFC, which is the friction-generating normal force associated with a coupled friction definition. Connector accumulated slip. CASU includes the scalar CASUC, which is the accumulated slip associated with a coupled friction definition. Connector instantaneous velocity associated with a coupled friction definition. 31.2.6 CONNECTOR PLASTIC BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • “Connector behavior,” Section 31.2.1 • “Connector elastic behavior,” Section 31.2.2 • “Connector functions for coupled behavior,” Section 31.2.4 • *CONNECTOR BEHAVIOR • *CONNECTOR DERIVED COMPONENT • *CONNECTOR ELASTICITY • *CONNECTOR HARDENING • *CONNECTOR PLASTICITY • *CONNECTOR POTENTIAL • “Defining plasticity,” Section 15.17.6 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Connector plasticity in Abaqus: • can be used to model plastic/irreversible deformations of parts forming an actual connection device; for example, – the pin or the sleeve in a door hinge may deform plastically if the forces/moments acting on them are large enough; – connection elements in automotive suspension systems may deform irreversibly due to abusive loading; or – spot welds in a car frame and rivets in an airplane could undergo inelastic deformations if the forces acting on the structural members they are a part of are larger than intended; • is defined in terms of resultant forces and moments in the connector; • uses perfect plasticity or isotropic/kinematic hardening behavior models; • can be used when rate-dependent effects are important; • can be specified in any connectors with available components of relative motion; • can be used for available components of relative motion for which either elastic or rigid behavior was specified; • can be used in an uncoupled fashion to define elastic-plastic or rigid plastic response in individual available components of relative motion; and • can be used to specify coupled elastic-plastic or rigid plastic behavior, in which case the responses in several available components of relative motion are involved simultaneously in a coupled fashion to define plasticity effects. To define connector plasticity in Abaqus, the following are necessary: • the elastic or rigid behavior prior to the onset of plasticity; • a yield function upon which plastic flow will be initiated; and • hardening behavior to define the initial yield value and, optionally, the yield value evolution after plastic motion initiation. Plasticity formulation in connectors The plasticity formulation in connectors is similar to the plasticity formulation in metal plasticity . In connectors the stress ( ) corresponds to the force ( ), the strain ( ) corresponds to the constitutive motion ( ), the plastic strain ( ) corresponds to the plastic relative motion ( ) corresponds to the equivalent plastic relative ), and the equivalent plastic strain ( motion ( ). The yield function is defined as is the collection of forces and moments in the available components of relative motion that where ultimately contribute to the yield function; , defines a magnitude of connector tractions similar to defining an equivalent state of stress in Mises plasticity and is either automatically defined by Abaqus or user-defined; and is the yield force/moment. The connector relative motions, ; and when plastic flow occurs, , remain elastic as long as the connector potential, . If yielding occurs, the plastic flow rule is assumed to be associated; thus, the plastic relative motions are defined by where is the rate of plastic relative motion and is the equivalent plastic relative motion rate. Loading and unloading behavior Abaqus allows for the following three types of behaviors associated with a plasticity definition when the connector is not actively yielding: • Linear elastic behavior, shown in Figure 31.2.6–1(a), is the most common case since similar behavior can be modeled in metal plasticity, for example, by specifying the Young’s modulus. Elastic motion occurs prior to plasticity onset, and unloading from a plastic state occurs on a straight line parallel to the initial loading. • Rigid behavior, shown in Figure 31.2.6–1(b), assumes that the slope in the linear elastic behavior is infinite; thus, the elastic motion prior to plasticity onset is zero, and unloading from a plastic state plasticity onset linear elastic unloading/reloading 0 linear elasticity U plasticity onset rigid unloading/reloading U plasticity onset user-specified nonlinear elasticity nonlinear elastic unloading/reloading 0 F 0 Fl0 (a) (b) (c) 0 0 c U Figure 31.2.6–1 Linear elastic-plastic (a), rigid plastic (b), and nonlinear elastic-plastic (c) response. occurs on a vertical line. In practice, the rigid behavior is enforced using an automatically chosen high penalty stiffness. • Nonlinear elastic behavior, shown in Figure 31.2.6–1(c), in which the initial elastic loading occurs along the defined nonlinear path. Elastic unloading occurs along a nonlinear curve (C Oc ) that is simply the user-defined nonlinear elastic curve motion shifted such that it passes through point C. The user-defined nonlinear elastic behavior must be such that the unloading path (C Oc ) does not intersect with the loading path (O C); otherwise, a local instability will occur. Other behaviors (such as damping or friction) can be specified in addition to the elastic/rigid/plastic specifications but will not be considered in the plasticity calculations since they are considered to be in parallel with the elastic-plastic/rigid plastic behavior . Defining elastic-plastic or rigid plastic behavior As is the case with any other connector behavior type, connector plasticity can be defined only for available components of relative motion. For example, you cannot define plastic behavior in a BEAM connector or in components 2 and 3 of a SLOT connector since these components are not available for behavior definitions. The solution to this problem is to: • define a connection type with available components of relative motion that best models the kinematics of your connection device both before and after plasticity onset; • define the desired components as rigid ; and • specify rigid plastic behavior in some or all of these components. For example, to define rigid plasticity for an otherwise rigid beam-like connector, you could use a PROJECTION CARTESIAN connection together with a PROJECTION FLEXION-TORSION connection, define all components as rigid, and proceed with your plasticity definitions. Elastic-plastic behavior is usually specified for available components of relative motion for which spring-like behavior is specified and for which plastic deformation may occur. Input File Usage: Abaqus/CAE Usage: Use the following options to define rigid plasticity in connectors: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY, RIGID *CONNECTOR PLASTICITY *CONNECTOR HARDENING Use the following options to define elastic-plasticity in connectors: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY *CONNECTOR PLASTICITY *CONNECTOR HARDENING Use the following input to define rigid plasticity in connectors: Interaction module: connector section editor: Add→Elasticity, Definition: Rigid; Add→Plasticity Use the following input to define elastic-plasticity in connectors: Interaction module: connector section editor: Add→Elasticity; Add→Plasticity Defining uncoupled plastic behavior Uncoupled elastic-plastic or rigid plastic behavior, specified for each component of relative motion independently, is similar to one-dimensional plasticity. You must define elastic or rigid behavior in the specified component of relative motion. In this case the connector potential function is chosen automatically as where behavior is specified. The associated plastic flow in this case becomes is the force or moment in the available component of relative motion for which plastic where is the rate of plastic relative motion and is the equivalent plastic relative motion rate in the component. Input File Usage: Use the following options to define uncoupled rigid plastic connector behavior: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY, RIGID, COMPONENT=i *CONNECTOR PLASTICITY, COMPONENT=i *CONNECTOR HARDENING Use the following options to define uncoupled elastic-plastic connector behavior: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY, COMPONENT=i *CONNECTOR PLASTICITY, COMPONENT=i *CONNECTOR HARDENING Use the following input to define uncoupled rigid plastic connector behavior: Interaction module: connector section editor: Add→Elasticity, Definition: Rigid; Add→Plasticity, Coupling: Uncoupled Use the following input to define uncoupled elastic-plastic connector behavior: Interaction module: connector section editor: Add→Elasticity, Definition: Linear or Nonlinear, Coupling: Uncoupled; Add→Plasticity, Coupling: Uncoupled 31.2.6–5 Defining coupled plastic behavior You should define coupled plasticity in connectors when several available components of relative motion are involved simultaneously in a coupled fashion in the definition of the yield function . In this case you must define the potential, P, via a connector potential definition. Plastic flow eventually occurs only in the intrinsic components of relative motion that are ultimately involved in the potential. Elastic or rigid behavior should be specified for all components of relative motion that are involved in the potential definition. The elastic/rigid behavior for these components can be specified in an uncoupled fashion, in a coupled fashion, or in a combination of both. All elasticity definitions specified in a connector behavior that are pertinent to the components of relative motion involved in the potential definition are used collectively to define the elasticity for the coupled elastic-plastic or rigid plastic definition. Input File Usage: Use the following options to define coupled elastic-plastic or rigid plastic connector behavior: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR ELASTICITY *CONNECTOR PLASTICITY *CONNECTOR POTENTIAL *CONNECTOR HARDENING Interaction module: connector section editor: Add→Elasticity; Add→Plasticity, Coupling: Coupled, Force Potential Abaqus/CAE Usage: Mode-mix ratio If the coupled plasticity definition includes at least two terms in the associated potential definition , a mode-mix ratio can be defined to reflect the relative weight of the first two terms in their contribution to the potential. The mode-mix ratio can be used in plastic motion-based connector damage definitions to specify dependencies in both damage initiation and damage evolution. It is defined as where the force/moment in the second component specified for the same potential. is the force/moment in the first component specified for the plasticity potential and if is , if , and is somewhere in between −1.0 and 1.0 if neither is 0.0. Defining the plastic hardening behavior Abaqus provides a number of hardening models varying from simple perfect plasticity to nonlinear isotropic/kinematic hardening. Connector hardening is analogous to the hardening models used in Abaqus for metals subjected to cyclic loading and described in “Models for metals subjected to cyclic loading,” Section 23.2.2. Defining perfect plasticity Perfect plasticity means that the yield force does not change with plastic relative motion. Input File Usage: Use the following option to define perfect plasticity: *CONNECTOR HARDENING Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify isotropic hardening, Isotropic Hardening, and enter the Yield Force/Moment in the data table Defining nonlinear isotropic hardening Isotropic hardening behavior defines the evolution of the yield surface size, equivalent plastic relative motion, function of in tabular form or by using the simple exponential law . This evolution can be introduced by specifying , as a function of the directly as a is the yield value at zero plastic relative motion and where is the maximum change in the size of the yield surface, and b defines the rate at which the size of the yield surface changes as plastic deformation develops. When the equivalent force defining the size of the yield surface remains constant ( ), there is no isotropic hardening. and b are material parameters. Defining the isotropic hardening component by specifying tabular data Isotropic hardening can be introduced by specifying the equivalent force defining the size of the yield surface, , and, if required, of the , temperature, and/or other predefined field variables. The equivalent relative plastic motion rate, yield value at a given state is simply interpolated from this table of data. , as a tabular function of the equivalent relative plastic motion, Input File Usage: *CONNECTOR HARDENING, TYPE=ISOTROPIC, DEFINITION=TABULAR (default) Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify isotropic hardening, Isotropic Hardening, Definition: Tabular Defining the isotropic hardening component using the exponential law Specify the material parameters of the exponential law ( , and b) directly if they are already calibrated from test data. These parameters can be specified as functions of temperature and/or field variables. , Input File Usage: *CONNECTOR HARDENING, TYPE=ISOTROPIC, DEFINITION=EXPONENTIAL LAW Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify isotropic hardening, Isotropic Hardening, Definition: Exponential law Defining nonlinear kinematic hardening When nonlinear kinematic hardening is specified, the center of the yield surface is allowed to translate in the force space. The backforce, , is the current center of the yield surface and is interpreted similar to the backstress discussed in “Classical metal plasticity,” Section 23.2.1. The yield surface is defined by the function where is the yield value and is the potential with respect to the backforce . The kinematic hardening component is defined to be an additive combination of a purely kinematic term (the linear Ziegler hardening law) and a relaxation term (the recall term) that introduces the nonlinearity. When temperature and field variable dependencies are omitted, the hardening law is are material parameters that must be calibrated from cyclic test data. C is the initial where C and kinematic hardening modulus, and determines the rate at which the kinematic hardening modulus decreases with increasing plastic deformation. When C and are zero, the model reduces to an isotropic hardening model. When is zero, the linear Ziegler hardening law is recovered. Refer to “Models for metals subjected to cyclic loading,” Section 23.2.2, for a discussion of calibrating the material parameters. Defining the kinematic hardening component by specifying half-cycle test data If limited test data are available, C and can be based on the force-constitutive motion data obtained from the first half cycle of a unidirectional tension or compression experiment. An example of such test data is shown in Figure 31.2.6–2. This approach is usually adequate when the simulation will involve only a few cycles of loading. For each data point ( is obtained from the test data as ) a value of where hardening definition or the initial yield force if the isotropic hardening component is not defined. is the user-defined size of the yield surface at the corresponding plastic motion for the isotropic Integration of the backforce evolution law over a half cycle yields the expression which is used for calibrating C and . When test data are given as functions of temperature and/or field variables, it is recommended that a data check analysis be run first. During the data check run, Abaqus will determine several pairs of material parameters (C, ), where each pair will correspond to a given combination of temperature and/or F3, upl F1, upl F2, upl F upl Figure 31.2.6–2 Half-cycle of force-motion data. to be a constant, the data check analysis will field variables. Since Abaqus requires the parameter terminate with an error message if is not a constant. However, an appropriate constant value of may be determined from the information provided in the data file during the data check run. The values for the parameter C and the constant can then be entered directly as described below. Input File Usage: *CONNECTOR HARDENING, TYPE=KINEMATIC, DEFINITION=HALF CYCLE (default) Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify kinematic hardening, Kinematic Hardening, Definition: Half-cycle Defining the kinematic hardening component by specifying test data from a stabilized cycle Force-constitutive motion data can be obtained from the stabilized cycle of a specimen that is subjected to symmetric cycles. A stabilized cycle is obtained by cycling the specimen over a fixed motion range until a steady-state condition is reached; that is, until the force-motion curve no longer changes shape from one cycle to the next. Such a stabilized cycle is shown in Figure 31.2.6–3. See “Models for metals subjected to cyclic loading,” Section 23.2.2, for information on how the data should be processed before they are specified in the connector hardening definition. Input File Usage: *CONNECTOR HARDENING, TYPE=KINEMATIC, DEFINITION=STABILIZED Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify kinematic hardening, Kinematic Hardening, Definition: Stabilized Defining the kinematic hardening component by specifying the material parameters directly The parameters C and can be specified directly if they are already calibrated from test data. The parameter C can be provided as a function of temperature and/or field variables, but temperature and field variable dependence of is not available. The algorithm currently used to integrate the nonlinear isotropic/kinematic hardening model does not provide accurate solutions if the value of changes significantly in an increment due to temperature and/or field variable dependence. Fn F1 Δu F2 up Fi ui pl ui = ui − i − 0up Figure 31.2.6–3 Force-motion data for a stabilized cycle. Input File Usage: *CONNECTOR HARDENING, TYPE=KINEMATIC, DEFINITION=PARAMETERS Abaqus/CAE Usage: Interaction module: connector section editor: Add→Plasticity: Specify kinematic hardening, Kinematic Hardening, Definition: Parameters Defining nonlinear isotropic/kinematic hardening The evolution law of the combined isotropic/kinematic model consists of two components: an isotropic hardening component, which describes the change in the equivalent force defining the size of the yield surface, , as a function of plastic relative motion, and a nonlinear kinematic hardening component, which describes the translation of the yield surface in force space through the backforce, . At most two connector hardening definitions, one isotropic and one kinematic, can be associated with a connector plasticity definition. If only one connector hardening definition is specified, it can be either isotropic or kinematic. Input File Usage: Abaqus/CAE Usage: Use the following two options to define nonlinear hardening: *CONNECTOR HARDENING, TYPE=KINEMATIC *CONNECTOR HARDENING, TYPE=ISOTROPIC Interaction module: connector section editor: Add→Plasticity: Specify isotropic hardening and Specify kinematic hardening isotropic/kinematic Using multiple plasticity definitions Multiple connector plasticity definitions can be used as part of the same connector behavior definition. However, only one connector plasticity definition can be used to define plasticity for each available component of relative motion. At most one coupled plasticity definition can be associated with a connector behavior definition. Additional connector plasticity definitions are permitted for the same connector behavior definition only if the two spaces do not overlap; for example, you could define uncoupled connector plasticity for components 1, 2, and 6 and have one coupled connector plasticity definition involving components 3, 4, and 5. Each connector plasticity definition must have its own hardening definition. Examples Illustrations of uncoupled and coupled plasticity behaviors are shown in the following examples. Uncoupled plasticity in a SLOT-like connector Consider a SLOT connector that you have used to model a physical device efficiently. You have examined the reaction forces enforcing the SLOT constraint in the local 2- and 3-directions; since they appear to be quite large, you need to assess whether plastic deformations in the device may occur. One option that you have is to create detailed meshes for the slot and the pin in the device, define the contact interactions between them, and use elastic-plastic material definitions for the underlying materials. While this is the most accurate modeling solution, it may be impractical, especially when the device you are modeling is part of a larger model. Alternatively, you can do the following: • use a CARTESIAN connection type instead of the SLOT connection with the first axis aligned with the slot direction; • define components 2 and 3 as rigid; and • define rigid plasticity separately in each of the components. The following input can be used: *CONNECTOR SECTION, BEHAVIOR=slot CARTESIAN orientation at node a *CONNECTOR BEHAVIOR, NAME=slot *CONNECTOR ELASTICITY, RIGID 2, 3 *CONNECTOR PLASTICITY, COMPONENT=2 *CONNECTOR HARDENING, TYPE=ISOTROPIC 100, 0.0 110, 0.12 *CONNECTOR PLASTICITY, COMPONENT=3 *CONNECTOR HARDENING, TYPE=ISOTROPIC 50, 0.0 75, 0.23 The yield forces that you specify in the connector hardening definitions are obtained from an experimental result or are assessed from a “virtual experiment,” as follows: • Use the meshed model of the slot discussed above. • Run two simple separate analyses by constraining the slot part of the device and driving the pin into the slot walls using a boundary condition. • Plot the reaction force at the pin node against its motion. • Use these data to create the force-motion hardening curve to be specified in the connector hardening definition. Coupled plasticity in a spot weld Referring to the spot weld shown in Figure 31.2.6–4 and to the yield function described in “Defining connector potentials” in “Connector functions for coupled behavior,” Section 31.2.4, you could complete the plasticity definition, for example, by specifying tabular isotropic hardening and kinematic hardening via parameters. Fn Figure 31.2.6–4 Spot weld connection. *PARAMETER =0.02 =0.05 *CONNECTOR ELASTICITY, RIGID *CONNECTOR PLASTICITY *CONNECTOR POTENTIAL, EXPONENT=a normal, , , MACAULEY shear, *CONNECTOR HARDENING, TYPE=ISOTROPIC , , ABS , , *CONNECTOR HARDENING, TYPE=KINEMATIC, DEFINITION=PARAMETERS C, Defining plastic connector behavior in linear perturbation procedures Plastic relative motions are not allowed during linear perturbation analyses. Therefore, the connector relative motions will be linear elastic perturbations about the plastically deformed base state, similar to metal plasticity. Output The Abaqus output variables available for connectors are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The following output variables are of particular interest when defining plasticity in connectors: CUE CUP CUPEQ Connector elastic displacements/rotations. Connector plastic displacements/rotations. Connector equivalent plastic relative displacements/rotations. In addition to the usual six components associated with connector output variables, CUPEQ includes the scalar CUPEQC, which is the equivalent plastic relative motion associated with a coupled plasticity definition. CALPHAF Connector kinematic hardening shift forces/moments. 31.2.7 CONNECTOR DAMAGE BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • “Connector behavior,” Section 31.2.1 • *CONNECTOR BEHAVIOR • *CONNECTOR DAMAGE EVOLUTION • *CONNECTOR DAMAGE INITIATION • *CONNECTOR ELASTICITY • *CONNECTOR PLASTICITY • *CONNECTOR POTENTIAL • *SECTION CONTROLS • “Defining damage,” Section 15.17.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Connector damage behavior: • can be specified in any connectors with available components of relative motion; • can be used to degrade the elastic, elastic-plastic, or rigid plastic response in connector elements; • can use a force-based, motion-based, or plastic motion–based damage initiation criterion upon which response degradation may be triggered; • can use either a (plastic) motion-based or an energy-based damage evolution law to degrade the force response in the connector; • can be defined in terms of several competing damage mechanisms; and • can be used only as an indicator of proximity to the damage initiation point without degrading the connector response. Damage formulation in connectors If relative forces or motions in a connection exceed critical values, the connector starts undergoing irreversible damage (degradation). Upon additional loading there is further evolution of damage leading to eventual failure. If damage has occurred, the force response in the connector component i will change according to the following general form: where relative motion i if damage were not present (effective response). is a scalar damage variable and is the response in the available connector component of To define a connector damage mechanism, you specify the following: • a criterion for damage initiation; and • a damage evolution law that specifies how the damage variable d evolves (optional). Prior to damage initiation, d has a value of 0.0; thus, the force response in the connector does not change. Once damage has been initiated, the damage variable will monotonically evolve up to the maximum value of 1.0 if damage evolution is specified. Complete failure occurs when d = 1.0. Abaqus allows you to specify a maximum degradation value (the default value is 1.0); damage evolution will stop when the damage variable reaches this value, and the element will be deleted from the mesh by default. Alternatively, you can specify that the damaged connector elements remain in the analysis with no further damage evolution. The maximum degradation value is used to evaluate the damaged stiffness in the remaining part of the analysis. This functionality is discussed in detail in “Controlling element deletion and maximum degradation for materials with damage evolution” in “Section controls,” Section 27.1.4. Defining connector damage initiation The degradation process in connectors initiates when forces or relative motions in the connector satisfy certain criteria. Three different criteria types can be used to trigger damage in connectors: criteria based on force, plastic motion, or constitutive motion. Connector damage initiation criteria for the available components of relative motion can be specified for each component independently (uncoupled). Alternatively, connector damage initiation criteria that couple all or some of the available components of relative motion in the connector can be defined. The damage initiation criterion can depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and field variables. Force-based damage initiation criterion By default, the damage initiation criterion is specified in terms of forces/moments in the connector. Elastic or rigid connector behavior must be defined for the components involved in the initiation. You provide the lower (compression) limit, , for the force/moment damage initiation values. If the force is outside the range specified by the two limit values, damage is initiated. The output variable CDIF can be used to monitor the proximity to the damage initiation point. , and the upper (tension) limit, Defining uncoupled force-based damage initiation For an uncoupled force-based damage initiation criterion, the connector force in the specified component is compared to the specified limit values. Damage is initiated when the force in the specified component i, , is for the first time outside the range ( or ). Input File Usage: *CONNECTOR DAMAGE INITIATION, COMPONENT=component number, CRITERION=FORCE (default), DEPENDENCIES=n Abaqus/CAE Usage: Interaction module: connector section editor: Add→Damage: Coupling: Uncoupled, Initiation criterion: Force Defining coupled force-based damage initiation For a coupled force-based damage initiation criterion, a connector potential, , must be specified to define an equivalent force magnitude (scalar). The equivalent force magnitude is compared to the specified limit values to assess damage initiation. Damage is initiated when the equivalent force magnitude, , is for the first time outside the range ( or ). Input File Usage: Use the following options: Abaqus/CAE Usage: *CONNECTOR DAMAGE INITIATION, CRITERION=FORCE (default), DEPENDENCIES=n *CONNECTOR POTENTIAL Interaction module: connector section editor: Add→Damage: Coupling: Coupled, Initiation criterion: Force, Initiation Potential Plastic motion–based damage initiation criterion The damage initiation criterion can be specified in terms of an equivalent relative plastic motion in the connector. You provide the relative equivalent plastic displacement/rotation at which damage will be initiated as a function of the relative equivalent plastic rate. The output variable CDIP can be used to monitor the proximity to the damage initiation point. Defining uncoupled plastic damage initiation For an uncoupled elastic-plastic or rigid plastic damage initiation criterion, uncoupled connector plasticity in the specified component of relative motion must be defined . When the equivalent relative plastic motion as defined by the associated plasticity definition is greater than the specified limit value for the first time, damage is initiated. Input File Usage: Use the following options: *CONNECTOR DAMAGE INITIATION, COMPONENT=component number, CRITERION=PLASTIC MOTION, DEPENDENCIES=n *CONNECTOR PLASTICITY, COMPONENT=component number or *CONNECTOR PLASTICITY Interaction module: connector section editor: Add→Damage: Initiation criterion: Plastic motion; Add→Plasticity Abaqus/CAE Usage: Defining coupled plastic damage initiation For a coupled elastic-plastic or rigid plastic damage initiation criterion, coupled connector plasticity must be defined. The connector potential used in the coupled connector plasticity function defines an equivalent relative plastic motion. This equivalent relative plastic motion is compared to the specified limit values to assess damage initiation. The equivalent relative plastic motion at which damage is initiated can be a function of the mode-mix ratio . Input File Usage: Abaqus/CAE Usage: Use the following options: *CONNECTOR DAMAGE INITIATION, CRITERION=PLASTIC MOTION, DEPENDENCIES=n *CONNECTOR PLASTICITY *CONNECTOR POTENTIAL Interaction module: connector section editor: Add→Damage: Coupling: Coupled, Initiation criterion: Plastic motion; Add→Plasticity: Coupling: Coupled, Force Potential Constitutive motion-based damage initiation criterion The damage initiation criterion can be specified in terms of relative constitutive displacements/rotations in the connector. You provide the lower (compression) limit, , for the constitutive displacement/rotation damage initiation values. If the motion is outside the range specified by the two limit values, damage is initiated. The output variable CDIM can be used to monitor the proximity to the damage initiation point. , and the upper (tension) limit, Defining uncoupled constitutive motion-based damage initiation For an uncoupled motion-based damage initiation criterion, the connector relative constitutive motion in the specified component is compared to the specified limit values. Damage is initiated when the relative constitutive displacement/rotation in the specified component i, , is for the first time outside the range ( or ). Input File Usage: *CONNECTOR DAMAGE INITIATION, COMPONENT=component number, CRITERION=MOTION, DEPENDENCIES=n Abaqus/CAE Usage: Interaction module: connector section editor: Add→Damage: Coupling: Uncoupled, Initiation criterion: Motion Defining coupled constitutive motion-based damage initiation , must be specified For a coupled motion-based damage initiation criterion, a connector potential, to define an equivalent motion magnitude (scalar), where is the collection of all available components of relative motion in the connector. The equivalent motion magnitude is compared to the specified limit values to assess damage initiation. Damage is initiated when the equivalent motion magnitude, , is for the first time outside the range ( or ). Input File Usage: Abaqus/CAE Usage: Use the following options: *CONNECTOR DAMAGE INITIATION, CRITERION=MOTION, DEPENDENCIES=n *CONNECTOR POTENTIAL Interaction module: connector section editor: Add→Damage: Coupling: Coupled, Initiation criterion: Motion, Initiation Potential Defining connector damage evolution Connector damage evolution specifies the evolution law for the damage variable. Upon evolution, the connector response will be degraded. The evolution of damage can be based on an energy dissipation criterion or on relative (plastic) motions. In the motion-based criteria the damage variable, d, can be defined as a linear, exponential, or tabular function of relative motions. The damage evolution law can depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and field variables. Specifying the affected components By default (i.e., the affected components are not specified explicitly), only the elastic/rigid or elastic/rigid-plastic response in the connector will be damaged. The response due to friction, damping, and stop/lock behavior will not be degraded. For an uncoupled connector damage mechanism (uncoupled damage initiation criterion), only the specified component of relative motion will undergo damage. For coupled connector damage initiation, the components that will be degraded by default are chosen as follows: • If a force-based or constitutive motion-based damage initiation criterion is used, the intrinsic available components (1 through 6) that ultimately contribute to the connector potential for damage initiation will be affected. • If a plastic motion–based damage initiation criterion is used, the intrinsic available components that ultimately contribute to the connector potential used in the coupled plasticity definition will be affected. Alternatively, you can specify the available components of relative motion that will be affected by the damage evolution law directly. In this case the entire connector response (elasto/rigid-plastic, friction, damping, constraint forces and moments, etc.) in the affected components will be damaged. *CONNECTOR DAMAGE EVOLUTION, AFFECTED COMPONENTS Input File Usage: Abaqus/CAE Usage: The first data line identifies the component numbers that will be damaged, and the additional data for the connector damage evolution definition begins on the second data line. Interaction module: connector section editor: Add→Damage: Specify damage evolution, Evolution, Specify affected components Defining a motion-based linear damage evolution law The linear form of the damage evolution law is illustrated here in the context of linear elasticity, although it can be used in any situation. Assume that the connector response is linear elastic and that after damage initiation a linear damage evolution is desired, as illustrated in Figure 31.2.7–1. Feff Fc linear elastic response (no damage) damage initiation effective response (if damage was not present) d Feff actual current response in the connector with damage F = (1-d) Feff damaged response U o U c Uf (1-d) E unloading/reloading curve Figure 31.2.7–1 Linear damage evolution law for linear elastic connector behavior. If damage were not specified, the response would be linear elastic (a straight line passing through the origin). Assume that damage has initiated at point I as triggered by a force-based or motion-based criterion, for example; the corresponding constitutive motion at this point is If the connector is . loaded further such that the constitutive motion increases to , the connector force response at point C becomes . The response is diminished by . If unloading occurs at point C, the (the elastic response with no damage). Thus, unloading curve of slope , the damage variable, d, stays constant at the value obtained when point C is first reached. If further loading occurs, further damage occurs until the ultimate failure motion, , is reached (d = 1) and the connector component loses the ability to carry any load. Thus, one possible loading/unloading sequence is O I C O C is followed. As long as the constitutive motion does not exceed when compared to the effective response . The linear damage evolution law defines a truly linear damaged force response only in the case of linear elastic or rigid behavior with optional perfect plasticity. If nonlinear elasticity or plasticity with hardening are defined for the damaged components, an approximate linear damaged response is observed. Defining the linear evolution law for a force-based or constitutive motion-based damage initiation criterion If an uncoupled damage initiation criterion is used in component i, you specify the difference between the constitutive relative motion at ultimate failure, , and the constitutive relative motion at damage initiation, , in the specified component ( ). If a coupled damage initiation criterion is used, an equivalent constitutive relative motion, be defined for damage evolution purposes. A connector potential definition is used to define You specify the difference between the equivalent motion at ultimate failure, motion at damage initiation, ). ( , must . , and the equivalent Input File Usage: Use the following options to define a linear evolution law for an uncoupled initiation criterion: *CONNECTOR DAMAGE INITIATION, COMPONENT=component number, CRITERION=FORCE or MOTION *CONNECTOR DAMAGE EVOLUTION, TYPE=MOTION, SOFTENING=LINEAR Use the following options to define a linear evolution law for a coupled initiation criterion: *CONNECTOR DAMAGE INITIATION, CRITERION=FORCE or MOTION *CONNECTOR POTENTIAL *CONNECTOR DAMAGE EVOLUTION, TYPE=MOTION, SOFTENING=LINEAR *CONNECTOR POTENTIAL The second *CONNECTOR POTENTIAL option defines Use the following input to define a linear evolution law for an uncoupled initiation criterion: . Interaction module: connector section editor: Add→Damage: Coupling: Uncoupled, Initiation criterion: Force or Motion; Specify damage evolution, Evolution type: Motion, Evolution softening: Linear Use the following input to define a linear evolution law for a coupled initiation criterion: Interaction module: connector section editor: Add→Damage: Coupling: Coupled, Initiation criterion: Force or Motion; Specify damage evolution, Evolution type: Motion, Evolution softening: Linear; Initiation Potential; Evolution Potential Abaqus/CAE Usage: Defining the linear evolution law for a plastic motion–based damage initiation criterion , and the associated equivalent plastic relative motion at damage initiation, You can specify the difference between the associated equivalent plastic relative motion at ultimate failure, ), as a function of the mode-mix ratio, , defined in “Connector plastic behavior,” Section 31.2.6. The equivalent plastic relative motions are calculated from the associated plasticity definition (either coupled or uncoupled). ( Input File Usage: Use the following options: *CONNECTOR DAMAGE INITIATION, CRITERION=PLASTIC MOTION Abaqus/CAE Usage: *CONNECTOR DAMAGE EVOLUTION, TYPE=MOTION, SOFTENING=LINEAR Interaction module: connector section editor: Add→Damage: Initiation criterion: Plastic motion; Specify damage evolution, Evolution type: Motion, Evolution softening: Linear Defining a motion-based exponential damage evolution law The exponential damage evolution law is illustrated in the context of a linear elastic-plastic response with hardening, although it can be used in any situation. The force response in a particular connector component is shown in Figure 31.2.7–2. plasticity with hardening (no damage) plasticity onset damage initiation Feff elastic response Fc d Feff (1-d) E actual response with damage unloading/reloading curve pl U o pl U c pl Uf Figure 31.2.7–2 Exponential damage evolution law for linear elastic-plastic connector behavior with hardening. Assume that damage is initiated at point I as triggered by a plastic motion–based damage initiation . Unloading from criterion. If further loading occurs until point C, the response is point C occurs along the damaged elastic line of slope . Upon unloading/reloading, the damage variable remains constant until point C is reached again. Further loading (beyond point C) leads to an increasingly damaged response until the ultimate failure point, , is reached (d = 1). The damage variable d is given by the following equation: The damaged response will appear to be truly exponential only if either linear elasticity or perfect plasticity is used. An approximate exponential degradation is obtained if plasticity with hardening is present. You specify the difference between the relative motions at ultimate failure and at damage initiation . The difference between the relative motions is interpreted in the same and the exponential coefficient way as described in “Defining a motion-based linear damage evolution law,” as follows: • If an uncoupled force-based or constitutive motion-based damage initiation criterion is used, the difference between the relative motions at ultimate failure and at damage initiation in the specified component i, , is specified. • If a coupled force-based or constitutive motion-based damage initiation criterion is used, an ). The difference , is specified. equivalent relative motion is defined using a connector potential ( between the relative motions at ultimate failure and at damage initiation, • If a plastic motion–based damage initiation criterion is used, the difference between the equivalent relative plastic motions at ultimate failure and at damage initiation, , is specified. The equivalent plastic relative motion is calculated from the associated plasticity definition. The data can also be functions of the mode-mix ratio . In the first two cases the equation for the damage variable is similar to that given above for plastic motion–based damage initiation except that (equivalent) constitutive relative motions are used instead of equivalent relative plastic motions. Input File Usage: Abaqus/CAE Usage: *CONNECTOR DAMAGE EVOLUTION, TYPE=MOTION, SOFTENING=EXPONENTIAL Interaction module: connector section editor: Add→Damage: Specify damage evolution, Evolution type: Motion, Evolution softening: Exponential Defining a motion-based tabular damage evolution law You can also specify the damage variable directly as a tabular function of the differences between the relative motions at ultimate failure and the relative motions at damage initiation. The differences between the relative motions are interpreted in the same way as described in “Defining a motion-based linear damage evolution law,” as follows: • If an uncoupled force-based or constitutive motion-based damage initiation criterion is used, the differences between the constitutive relative motions at ultimate failure and at damage initiation in the specified component i, , are used to define the tabular data. • If a coupled force-based or constitutive motion-based damage initiation criterion is used, an ). The differences equivalent relative motion is defined using a connector potential ( between the relative motions at ultimate failure and at damage initiation, the tabular data. , are used to define • If a plastic motion–based damage initiation criterion is used, the differences between the equivalent relative plastic motions at ultimate failure and at damage initiation, , are used. The equivalent plastic relative motion is calculated from the associated plasticity definition. The tabular data can also be functions of the mode-mix ratio . Input File Usage: Abaqus/CAE Usage: *CONNECTOR DAMAGE EVOLUTION, TYPE=MOTION, SOFTENING=TABULAR, DEPENDENCIES=n Interaction module: connector section editor: Add→Damage: Specify damage evolution, Evolution type: Motion, Evolution softening: Tabular Defining a damage evolution law using post-damage initiation dissipation energies This damage evolution law is illustrated in the context of nonlinear elasticity, as shown in Figure 31.2.7–3. nonlinear elastic response Feff Fc damage initiation d Feff nonlinear elastic response (no damage) Gc actual response with damage U o U c unloading/reloading curve Figure 31.2.7–3 Post-damage initiation dissipation energy evolution law for nonlinear elastic connector behavior. as triggered by Assume that damage is initiated at point I when the constitutive relative motion is a force-based or a motion-based damage initiation criterion, for example. The response at point C will be . Unloading from point C occurs along the CO curve, which is the original nonlinear elastic response curve (OE) scaled down by the ( ) factor. Damage remains constant on the unloading/reloading curve (C O C), and it increases only if loading increases beyond point C. Instantaneous failure can be specified upon initiation if is specified as 0.0. In all other cases ultimate failure (d = 1) would occur (in theory) at infinite motion since an exponential-like response that asymptotically goes to zero is generated. Abaqus will set d = 1 when the damage dissipated energy reaches 0.99 . You specify the post-damage initiation dissipated energy at ultimate failure, . motion–based initiation criterion is used, can be specified as a function of the mode-mix ratio If a plastic . Input File Usage: *CONNECTOR DAMAGE EVOLUTION, TYPE=ENERGY, DEPENDENCIES=n Abaqus/CAE Usage: Interaction module: connector section editor: Add→Damage: Specify damage evolution, Evolution type: Energy Using multiple damage mechanisms At most three uncoupled damage mechanisms (pairs of connector damage initiation criteria and connector damage evolution laws) can be defined for each available component of relative motion, one for each type of initiation criterion (force, motion, and plastic motion). In addition, three coupled damage mechanisms can be defined (one for each type of initiation criterion). Coupled and uncoupled damage definitions can be combined; only one overall damage variable per component will be used to damage the response in a particular available component of relative motion. Only the overall damage will be output. Specifying the contribution of each damage mechanism When several damage mechanisms are defined for the same connector behavior, you can specify the contribution of each damage mechanism to the overall damage effect for a particular component of relative motion. By default, the damage value associated with a particular mechanism will be compared to the damage values from any other damage mechanisms defined for the connector behavior, and only the maximum value will be considered for the overall damage. Alternatively, you can specify that the damage values for the mechanisms associated with the connector behavior should be combined in a multiplicative fashion to obtain the overall damage. See the last example below for an illustration. Input File Usage: Use the following option to specify that only the maximum damage value associated with a particular connector behavior should contribute to the overall damage effect: *CONNECTOR DAMAGE EVOLUTION, DEGRADATION=MAXIMUM Use the following option to specify that all the damage values associated with a particular connector behavior should contribute in a multiplicative way to the overall damage effect: *CONNECTOR DAMAGE EVOLUTION, DEGRADATION=MULTIPLICATIVE Abaqus/CAE Usage: Interaction module: connector section editor: Add→Damage: Specify damage evolution, Evolution, Degradation: Maximum or Multiplicative Examples The examples that follow illustrate several methods for defining damage mechanisms. Uncoupled damage The following input could be used to define a simple uncoupled damage mechanism: *CONNECTOR ELASTICITY, COMPONENT=1 *CONNECTOR DAMAGE INITIATION, COMPONENT=1, CRITERION=FORCE force_compress, force_tens *CONNECTOR DAMAGE EVOLUTION, TYPE=ENERGY 0.0 Damage will initiate when the elastic force in component 1 is either smaller than force_compress or larger than force_tens. Only the elastic response in component 1 will be damaged. Since the dissipated energy specified for damage evolution is 0.0, the damage evolves catastrophically instantaneously after it has initiated. Coupled rigid plasticity with plasticity-based damage Referring to the spot weld in Figure 31.2.7–4 for which coupled plasticity is defined in “Connector plastic behavior,” Section 31.2.6, a plastic motion–based damage initiation and evolution with dependencies on the mode-mix ratio can be specified as follows: Fn Figure 31.2.7–4 Spot weld connection. 31.2.7–12 *PARAMETER =0.25 =0.35 =0.45 =0.75 =0.78 =0.85 *CONNECTOR DAMAGE INITIATION, CRITERION=PLASTIC MOTION , 0.0 , 0.5 , 1.0 *CONNECTOR DAMAGE EVOLUTION, TYPE=MOTION, SOFTENING=LINEAR , 0.0 , 0.3 , 0.5 , 1.0 The equivalent plastic relative motion on the data lines is defined by the associated coupled plasticity definition illustrated in “Connector plastic behavior,” Section 31.2.6. For the damage evolution the post- damage-initiation equivalent plastic relative motion should be specified. The second column in all the data lines represents the mode-mix ratios as defined in “Connector plastic behavior,” Section 31.2.6. In this particular case the mode-mix ratio is . The data point at 0.0 comes from a pure “shear” experiment, and the data point at 1.0 comes from a pure “normal” experiment. Data for the values in between come from combined “shear-normal” experiments. Coupled rigid plasticity with force-based damage initiation and motion-based damage evolution Referring to the spot weld in Figure 31.2.7–4 and using the derived components normal and shear defined in “Defining derived components for connector elements” in “Connector functions for coupled behavior,” Section 31.2.4, an alternative way to define damage in the spot weld is to use: *PARAMETER =2 =0.85 =120.0 =115.0 *CONNECTOR DAMAGE INITIATION, CRITERION=FORCE , 1.0 *CONNECTOR POTENTIAL normal, shear, ** *CONNECTOR DAMAGE EVOLUTION, TYPE=MOTION, SOFTENING=EXPONENTIAL , *CONNECTOR POTENTIAL ** and Damage will be initiated when the force magnitude defined by the first connector potential definition exceeds the specified value of 1.0. The scale factors in the first potential definition are used in this case to define a force magnitude that would be 1.0 at damage initiation. A motion-based exponential decay damage evolution law is chosen. The second connector potential definition is associated with the connector damage evolution definition and defines an equivalent motion, , in the connection. When the equivalent post-initiation motion, , ultimate failure occurs. All components (1 through 6) are affected in this case since they all ultimately contribute to the first connector potential definition . at damage initiation), reaches (where is Elastic-plasticity with four competing damage mechanisms This example illustrates how to specify the contributions of multiple damage mechanisms to the overall damage effect and the components of relative motion affected by the damage evolution law. Most of the data line entries or parameters are not given for conciseness. ** first damage mechanism: force-based damage initiation ** damage variable *CONNECTOR DAMAGE INITIATION, COMPONENT=4, CRITERION=FORCE *CONNECTOR DAMAGE EVOLUTION, TYPE=MOTION, SOFTENING=EXPONENTIAL, DEGRADATION=MAXIMUM, AFFECTED COMPONENTS 4, 6 ** ** second damage mechanism: motion-based damage initiation ** damage variable *CONNECTOR DAMAGE INITIATION, COMPONENT=4, CRITERION=MOTION *CONNECTOR DAMAGE EVOLUTION, TYPE=MOTION, SOFTENING=LINEAR, DEGRADATION=MULTIPLICATIVE, AFFECTED COMPONENTS 1, 2, 6 ** ** third damage mechanism: plastic motion–based damage initiation ** damage variable *CONNECTOR DAMAGE INITIATION, COMPONENT=4, CRITERION=PLASTIC MOTION *CONNECTOR DAMAGE EVOLUTION, TYPE=MOTION, SOFTENING=TABULAR, DEGRADATION=MULTIPLICATIVE, AFFECTED COMPONENTS 1, 2 ** ** fourth damage mechanism: coupled force-based damage initiation ** damage variable *CONNECTOR DAMAGE INITIATION, CRITERION=FORCE *CONNECTOR POTENTIAL ** using components 1, 2, 3, 4, 5, 6 *CONNECTOR DAMAGE EVOLUTION, TYPE=ENERGY, DEGRADATION=MAXIMUM, AFFECTED COMPONENTS 1, 3, 4, 6 Four damage mechanisms (connector damage initiation/connector damage evolution pairs) are specified: three uncoupled and one coupled. The first line of each damage evolution definition establishes the components that will be damaged by the mechanism. The overall damage in a particular component is determined by contributions from all the mechanisms that affect that component. For example, the overall damage in component 1, , is determined by the second, third, and fourth damage mechanisms as follows: use multiplicative degradation; therefore, they are multiplied first: and uses maximum degradation, so is compared to . and the minimum value is taken. =0.6 (the only one increasing) while For example, assume that at a particular time t, , stay the same. The overall damage variable gets closer to the ultimate damage value faster when all three damage mechanisms are used than if we use only the =0.2 and at time mechanism: =0.3, and =0.5, and while Complete failure occurs when reaches 0.0. available component of relative motion. The overall damage variables for the other components are determined as follows (based on the specified affected components for each damage evolution law): , where i refers to the Maximum degradation and choice of element removal in Abaqus/Standard You have control over how Abaqus/Standard treats connector elements with severe damage. By default, the upper bound to the overall damage variable at a material point is . You can reduce this upper bound as discussed in “Controlling element deletion and maximum degradation for materials with damage evolution” in “Section controls,” Section 27.1.4. By default, once the overall damage variable in at least one component reaches , the connector elements are removed (deleted). See “Controlling element deletion and maximum degradation for materials with damage evolution” in “Section controls,” Section 27.1.4, for details. Once removed, connector elements offer no resistance to subsequent deformation. Alternatively, you can specify that a connector element should remain in the model even after the , . In this case, once the overall damage variable reaches overall damage variable reaches the element stiffness remains constant at times the undamaged stiffness. Viscous regularization in Abaqus/Standard Damage causes a softening response in connector elements, which often leads to convergence difficulties in an implicit code such as Abaqus/Standard. One technique for overcoming convergence difficulties is applying viscous regularization to the constitutive response by introducing a viscous damage variable, , as defined by the evolution equation where representing the relaxation time. The damaged response of the viscous material is given as is the damage variable evaluated in the inviscid backbone model and is the viscosity parameter As a result of viscous regularization, the damped damage variable does not obey the specified evolution law exactly (only the backbone damage variable does). Input File Usage: Abaqus/CAE Usage: *SECTION CONTROLS, NAME=name, VISCOSITY= *CONNECTOR SECTION, CONTROLS=name Viscous regularization is not supported in Abaqus/CAE. Defining connector damage behavior in linear perturbation procedures Damage cannot be initiated and damage variables do not evolve during linear perturbation analyses. Consequently, during a linear perturbation step damage is “frozen” in the state attained at the end of the previous general step. Output The Abaqus output variables available for connectors are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The following variables are of particular interest when damage is defined in connectors: CDMG CDIF CDIM CDIP Connector overall damage variable. Force-based connector damage initiation variable. In addition to the usual six components associated with connector output variables, CDIF includes the scalar CDIFC, which is the damage initiation criterion value associated with a coupled force-based damage initiation criterion. Motion-based connector damage initiation variable. CDIM includes the scalar CDIMC, which is the damage initiation criterion value associated with a coupled motion-based damage initiation criterion. Plastic motion–based connector damage initiation variable. CDIP includes the scalar CDIPC, which is the damage initiation criterion value associated with a coupled plastic motion–based damage initiation criterion. ALLDMD ALLCD Energy dissipated by damage. Energy dissipated by viscous regularization. 31.2.8 CONNECTOR STOPS AND LOCKS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • “Connector behavior,” Section 31.2.1 • *CONNECTOR BEHAVIOR • *CONNECTOR LOCK • *CONNECTOR STOP • “Defining a stop,” Section 15.17.9 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • “Defining a lock,” Section 15.17.10 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Connector stops and locks can be: • specified in any connector with available components of relative motion; • used to specify contact-enforced stops in individual components of relative motion; and • used to lock in position an available component of relative motion when a certain criterion is met. Defining connector stops In the physical construction of most connectors the admissible position of one body relative to the other is limited by a certain range. In Abaqus these limits are modeled as built-in inequality constraints. You specify the available components of relative motion for which the connector stops are to be defined and the lower and upper limit values of the connector’s admissible range of positions in the directions of the components of relative motion. Input File Usage: Use the following options to define a connector stop: Abaqus/CAE Usage: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR STOP, COMPONENT=component number lower limit, upper limit Interaction module: connector section editor: Add→Stop: Components: component or components, Lower bound: lower limit, Upper bound: upper limit Example Since the shock in Figure 31.2.8–1 has finite length, contact with the ends of the shock determines the upper and lower limit values of the distance that node b can be from node a. extensible range 7.5 node 12 1 (local orientation) node 11 Figure 31.2.8–1 Simplified connector model of a shock absorber. Assume that the maximum length of the shock is 15.0 units and that the minimum length is 7.5 units. Modify the input file presented in “Connectors: overview,” Section 31.1.1, that is associated with the example in Figure 31.2.8–1 to include the following lines: *CONNECTOR BEHAVIOR, NAME=sbehavior ... *CONNECTOR STOP, COMPONENT=1 7.5, 15.0 Defining connector locks Connector mechanisms may have devices designed to lock the connector in place once a desired configuration is achieved. For example, a revolute connection might have a falling-pin mechanism that locks the rotational motion after achieving a desired angle. A user-defined connector locking criterion can be defined for connector elements that contain available components of relative motion. You can select the component of relative motion for which the locking criterion is defined. Connector locks can be used to specify connector behavior for constrained as well as available components of relative motion. Limit values for force or moment can be specified for all components of relative motion involved in the connection. The force/moment used in evaluating the criterion is as computed in the output variable CTF. In addition, limit values can be specified for relative position corresponding to the available components of relative motion. If no other behavior is specified for an available component of relative motion, a force locking criterion will not be useful because CTF is zero. In Abaqus/Explicit you can also specify the limiting values of velocity in the available components as a criterion for locking. Velocity-dependent locking criteria are useful in modeling seatbelt systems in automobiles . Moreover, the limiting values can be dependent on temperature and field variables. Field variable dependencies can be used to model time-dependent locks. If the locking criterion specified for the selected component of relative motion is met, either all components lock or a single available component locks in place. By default, all components of relative motion are locked in place upon meeting the locking criterion. In this case the connector element will be completely kinematically locked from that point on. In dynamic analyses this locking may introduce high accelerations. You can specify if only a selected component of relative motion is locked. Input File Usage: Use the following options to define a connector lock: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR LOCK, COMPONENT=component number, LOCK=ALL or component number Abaqus/CAE Usage: Interaction module: connector section editor: Add→Lock: Components: component or components, Lock: All or Specify component Example In the example in Figure 31.2.8–1 assume that relative rotations about the shock will lock if the force in the local 3-direction exceeds 500.0 units of force. *CONNECTOR BEHAVIOR, NAME=sbehavior *CONNECTOR LOCK, COMPONENT=3, LOCK=4 , , -500.0, 500.0 Defining connector stops and locks in linear perturbation procedures The status of connector locks or stops cannot change during a linear perturbation analysis; all connector stop and connector lock definitions remain in the same status as in the base state. Output The Abaqus output variables available for connectors are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The following output variables are of particular interest when defining stops and locks in connectors: CSLST CRF Flags for connector stops and locks. Connector reaction forces/moments. At a given time and for a particular component of relative motion i, the output variable CSLSTi is 1 if the connector is actually stopped or locked in that component (stop or lock criteria are met). In that case, the correspondent CRF output variable will most likely be nonzero and equal to the actual force/moment required to enforce the stop or lock constraint. Since CRF is included in the calculation of CTF, the latter will change as well when the lock or stop is active. If the stop or lock criteria are not met at a given time for a particular component i, the output variable CSLSTi is 0 and in most cases the corespondent reaction force CRF is zero (the only possible exception is when a connector motion is also applied in that component). 31.2.9 CONNECTOR FAILURE BEHAVIOR Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Connectors: overview,” Section 31.1.1 • “Connector behavior,” Section 31.2.1 • *CONNECTOR BEHAVIOR • *CONNECTOR FAILURE • “Defining failure,” Section 15.17.11 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Connector failure behavior: • can be defined in any connector with available components of relative motion in Abaqus/Standard; • can be defined in any connector in Abaqus/Explicit; • can be used in Abaqus/Standard to fail all or specified components of relative motion if a failure criterion is met; • can be used in Abaqus/Explicit to fail all or specified components if a failure criterion is met; • can be triggered if either a connector relative motion or connector force in a specified component is outside a specified range; and • can be replaced in most cases by the more sophisticated connector damage initiation/evolution behavior . Defining connector failure behavior A typical connector might have pieces that break if a relative motion component, force, or moment becomes too large. Abaqus provides a way to define which components of relative motion will break and the criteria used to release these components. You can select the component of relative motion on which the failure criterion is based. In Abaqus/Standard connector failure can be used to specify connector behavior based on available components of relative motion. In Abaqus/Explicit connector failure can be used to specify connector behavior based on constrained as well as available components of relative motion. Limit values for force or moment can be specified for all components of relative motion involved in the connection. In addition, for connectors with available components of relative motion, limit values can be specified for the relative positions corresponding to an available component. In Abaqus/Standard if the failure criterion specified for the selected component of relative motion is met, either all components of relative motion fail or a single available component fails. By default, all components of relative motion are released upon meeting the failure criterion. The nodal force contributions for all released components from the connector element will be removed during the increment when the failure criterion is met. In Abaqus/Explicit if the failure criterion specified for the selected component is met, either all components or a single available component fails. By default, all components are released upon meeting the failure criterion. The nodal force contributions for all released components from the connector element will be removed during the increment when the failure criterion is met. Input File Usage: Use the following options to define connector failure: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR FAILURE, COMPONENT=component number, RELEASE=ALL or component number Abaqus/CAE Usage: Interaction module: connector section editor: Add→Failure: Components: component or components, Release: All or Specify component Viscous damping in Abaqus/Standard In Abaqus/Standard the sudden release of the failed connection may lead to convergence problems. To avoid convergence problems, you can add viscous damping to the components. Damping forces in the component are calculated as is the velocity of the failed component. Viscous damping is applied only if a selected available component of relative motion is released. is the user-defined damping coefficient and , where Input File Usage: Abaqus/CAE Usage: Example Use the following options to add viscous damping to failed components in Abaqus/Standard: *SECTION CONTROLS, NAME=name, VISCOSITY= *CONNECTOR SECTION, CONTROLS=name Viscous regularization is not supported in Abaqus/CAE. In the example in Figure 31.2.9–1 assume that the shock absorber pulls apart if the tensile force in the shock exceeds 800.0 units of force. extensible range 7.5 node 12 1 (local orientation) node 11 Figure 31.2.9–1 Simplified connector model of a shock absorber. ... *CONNECTOR BEHAVIOR, NAME=sbehavior *CONNECTOR FAILURE, COMPONENT=1, RELEASE=ALL , , , 800.0 Output The Abaqus output variables available for connectors are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The following output variables are of particular interest when defining failure in connectors: CFAILST ALLVD Flags for connector failure status. Energy dissipated by viscous damping added to failed components. At any given time and for a particular component of relative motion i, the output variable CFAILSTi is 1 if the connector fails in that particular component of relative motion (failure criteria are met). If the failure criteria are not met at a given time for a particular component i, the output variable CFAILSTi is 0. 31.2.10 CONNECTOR UNIAXIAL BEHAVIOR Product: Abaqus/Explicit References • “Connectors: overview,” Section 31.1.1 • “Connector behavior,” Section 31.2.1 • *CONNECTOR BEHAVIOR • *LOADING DATA • *UNLOADING DATA Overview Connector uniaxial behavior: • can be defined in any connector with available components of relative motion by specifying the loading and unloading behavior; • can be specified for each available component of relative motion independently; • can define separate response in the tensile and compressive directions; • can exhibit nonlinear elastic behavior, damaged elastic behavior, or elastic-plastic type behavior with permanent deformation upon complete unloading; • can have an unloading response specified; and • can be specified as dependent on constitutive motions in several local directions. The local directions for each connection type (as described in “Connection-type library,” Section 31.1.5) determine the directions in which the forces and moments act and in which the displacements and rotations are measured. Specifying uniaxial behavior for an available component of relative motion Uniaxial behavior can be specified for an available component of relative motion by defining the loading and unloading response for that component. For each component, separate loading/unloading response data can be defined for the response in the tensile and compressive directions. The loading and unloading response can be classified according to three available behavior types: • nonlinear elastic behavior; • damaged elastic behavior; and • elastic-plastic type behavior with permanent deformation. To define the loading response, you specify forces or moments as nonlinear functions of the components of relative motion. These functions can also depend on temperature, field variables, and constitutive displacements/rotations in the other component directions. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and field variables. The unloading response can be defined in the following ways: • You can specify several unloading curves that express the forces or moments as nonlinear functions of the components of relative motion; Abaqus interpolates these curves to create an unloading curve that passes through the point of unloading in an analysis. • You can specify an energy dissipation factor (and a permanent deformation factor for models with permanent deformation), from which Abaqus calculates an exponential/quadratic unloading function. • You can specify the forces or moments as nonlinear functions of the components of relative motion, as well as a transition slope; the connector unloads along the specified transition slope until it intersects the specified unloading function, at which point it unloads according to the function. (This unloading definition is referred to as combined unloading.) • You can specify the forces or moments as nonlinear functions of the components of relative motion; Abaqus shifts the specified unloading function along the strain axis so that it passes through the point of unloading in an analysis. The behavior type that is specified for the loading response dictates the type of unloading you can define, as summarized in Table 31.2.10–1. The different behavior types, as well as the associated loading and unloading curves, are discussed in more detail in the sections that follow. Table 31.2.10–1 Available unloading definitions for the uniaxial behavior types. Unloading definition Interpolated Quadratic Exponential Combined Shifted Material behavior type Rate-dependent elastic Damaged elastic Permanent deformation Input File Usage: Use the following options to define connector uniaxial behavior: *CONNECTOR BEHAVIOR, NAME=name *CONNECTOR UNIAXIAL BEHAVIOR, COMPONENT=component number *LOADING DATA, DIRECTION=deformation direction, TYPE=behavior type data lines to define loading data *UNLOADING DATA data lines to define unloading data Defining the deformation direction The loading/unloading data can be defined separately for tension and compression by specifying the deformation direction. If the deformation direction is defined (tension or compression), the tabular values defining tensile or compressive behavior should be specified with positive values of forces/moments and displacements/rotations in the specified component of relative motion and the loading data must start at the origin. If the behavior is not defined in a loading direction, the force response will be zero in that direction (the connector has no resistance in that direction). If the deformation direction is not defined, the data apply to both tension and compression. However, the behavior is then considered to be nonlinear elastic and no damage or permanent deformation can be specified. The response data will be considered to be symmetric about the origin if either tensile or compressive data are omitted. Input File Usage: Use the following option to define tensile behavior: *LOADING DATA, DIRECTION=TENSION Use the following option to define compressive behavior: *LOADING DATA, DIRECTION=COMPRESSION Use the following option to define both tensile compressive behavior in a single table: *LOADING DATA Behavior that depends on relative positions or motions in multiple component directions By default, the loading and unloading functions depend only on the displacement or rotation in the direction of the component of relative motion specified for the connector uniaxial behavior definition . However, it is also possible to define loading and unloading functions that depend on the constitutive displacements and rotations in multiple component directions. Input File Usage: Use the following option to define connector uniaxial behavior that depends on the relative displacements and/or rotations in several component directions: *LOADING DATA, INDEPENDENT COMPONENTS=CONSTITUTIVE MOTION Defining rate-independent nonlinear elastic behavior When the loading response is rate independent, the unloading response is also rate independent and occurs along the same user-specified loading curve as illustrated in Figure 31.2.10–1. An unloading curve does not need to be specified. Loading curve Figure 31.2.10–1 Nonlinear elastic loading. Input File Usage: *LOADING DATA, TYPE=ELASTIC Defining rate-dependent behavior The rate-dependent models require the specification of force-displacement curves at different rates of deformation to describe both loading and unloading behavior. If unloading behavior is not specified, the unloading occurs along the loading curve with the smallest rate of deformation. As the rate of deformation changes, the response is obtained by interpolation of the specified loading/unloading data. Unphysical jumps in the forces due to sudden changes in the rate of deformation are prevented using a technique based on viscoplastic regularization. This technique also helps model relaxation effects in a very simplistic manner, with the relaxation time given as are material parameters and is a linear viscosity parameter that controls the relaxation time when is a nonlinear viscosity parameter that controls the relaxation time at higher values of . The smaller this value, the shorter the relaxation time. controls the sensitivity of the relaxation speed to the stretch in the component of relative motion. Suggested values of these parameters are . Figure 31.2.10–2 , and illustrates the loading/unloading behavior as the connector is loaded at a rate and then unloaded at a rate . Small values of this parameter should be used. is the stretch. , where , and , , . Figure 31.2.10–3 shows the loading/unloading response of a connector element for two different . The larger the relaxation time, the longer it takes to achieve the relaxation times specified loading/unloading response for the applied deformation rate. and with uu uu uu Figure 31.2.10–2 Rate-dependent loading/unloading. Input File Usage: Figure 31.2.10–3 Rate-dependent loading/unloading. Use the following options when the unloading is also rate dependent: *LOADING DATA, TYPE=ELASTIC, RATE DEPENDENT *UNLOADING DATA, DEFINITION=INTERPOLATED CURVE, RATE DEPENDENT Use the following options when the unloading is rate independent: *LOADING DATA, TYPE=ELASTIC, RATE DEPENDENT *UNLOADING DATA, DEFINITION=INTERPOLATED CURVE Defining models with damage The damage models dissipate energy upon unloading, and there is no permanent deformation upon complete unloading. The unloading behavior controls the amount of energy dissipated by damage mechanisms and can be specified in one of the following ways: • an analytical unloading curve (exponential/quadratic); • an unloading curve interpolated from multiple user-specified unloading curves; or • unloading along a transition unloading curve (constant slope specified by user) to the user-specified unloading curve (combined unloading). For an overview of the different available behaviors, see “Specifying uniaxial behavior for an available component of relative motion” above. The various unloading types are discussed in the sections that follow. Defining onset of damage You can specify the onset of damage by defining the displacement below which unloading occurs along the loading curve. Input File Usage: *LOADING DATA, TYPE=DAMAGE, DAMAGE ONSET=value Specifying exponential/quadratic unloading The damage model in Figure 31.2.10–4 is based on an analytical unloading curve that is derived from an energy dissipation factor, (fraction of energy that is dissipated at any displacement level). As the connector is loaded, the force follows the path given by the loading curve. If the connector is unloaded (for example, at point B), the force follows the unloading curve . Reloading after unloading follows the unloading curve , after which the loading path follows the loading curve. The arrows shown in Figure 31.2.10–4 illustrate the loading/unloading paths of this model. until the loading is such that the displacement becomes greater than The unloading response follows the loading curve when the calculated unloading curve lies above the loading curve to prevent energy generation and follows a zero force response when the unloading curve yields a negative response. In such cases the dissipated energy will be less than the value specified by the energy dissipation factor. Input File Usage: Use the following option to define quadratic unloading behavior: *UNLOADING DATA, DEFINITION=QUADRATIC Use the following option to define exponential unloading behavior: *UNLOADING DATA, DEFINITION=EXPONENTIAL Specifying interpolated curve unloading The damage model in Figure 31.2.10–5 illustrates an interpolated unloading response based on multiple unloading curves that intersect the primary loading curve at increasing values of forces/displacements. You can specify as many unloading curves as are necessary to define the unloading response. Each Primary loading curve exponential/quadratic unloading Umax Figure 31.2.10–4 Exponential/quadratic unloading. unloading curve always starts at point O, the point of zero force and zero displacements, since the damage models do not allow any permanent deformation. The unloading curves are stored in normalized form so that they intersect the loading curve at a unit force for a unit displacement, and the interpolation occurs between these normalized curves. If unloading occurs from a maximum displacement for which an unloading curve is not specified, the unloading is interpolated from neighboring unloading curves. As the connector is loaded, the force follows the path given by the loading curve. If the connector is unloaded (for example, at point B), the force follows the unloading curve . Reloading after unloading follows the unloading path , after which the loading path follows the loading curve. until the loading is such that the displacement becomes greater than Primary loading curve Unloading curves Umax Figure 31.2.10–5 Interpolated curve unloading If the loading curve depends on the constitutive displacements/rotations in several component directions, the unloading curves also depend on the same component directions. The unloading curves also have the same temperature and field variable dependencies as the loading curve. Input File Usage: *UNLOADING DATA, DEFINITION=INTERPOLATED CURVE Specifying combined unloading in addition to the loading As illustrated in Figure 31.2.10–6, you can specify an unloading curve curve as well as a constant transition slope that connects the loading curve to the unloading curve. As the connector is loaded, the force follows the path given by the loading curve. If the connector is unloaded (for example, at point B), the force follows the unloading curve is defined by the constant transition slope, and lies on the specified unloading curve. Reloading after unloading follows the unloading path until the loading is such that the displacement becomes greater than , after which the loading path follows the loading curve. . The path Primary loading curve transition curve unloading curve Umax Figure 31.2.10–6 Combined unloading. If the loading curve depends on the constitutive displacements/rotations in several component directions, the unloading curve also depends on the same component directions. The unloading curve also has the same temperature and field variable dependencies as the loading curve. Input File Usage: *UNLOADING DATA, DEFINITION=COMBINED Defining models with permanent deformation These models dissipate energy upon unloading and exhibit permanent deformation upon complete unloading. The unloading behavior controls the amount of energy dissipated as well as the amount of permanent deformation. The unloading behavior can be specified in one of the following ways: • an analytical unloading curve (exponential/quadratic); • an unloading curve interpolated from multiple user-specified unloading curves; or • an unloading curve obtained by shifting the user-specified unloading curve to the point of unloading. For an overview of the different available behaviors, see “Specifying uniaxial behavior for an available component of relative motion” above. The various unloading types are discussed in the sections that follow. Defining the onset of permanent deformation By default, the onset of yield will be obtained as soon as the slope of the loading curve decreases by 10% from the maximum slope recorded up to that point while traversing along the loading curve. To override the default method of determining the onset of yield, you can specify either a value for the decrease in slope of the loading curve other than the default value of 10% (slope drop = 0.1) or by defining the displacement below which unloading occurs along the loading curve. If a slope drop is specified, the onset of yield will be obtained as soon as the slope of the loading curve decreases by the specified factor from the maximum slope recorded up to that point. Input File Usage: Use the following options to specify the onset of yield by defining the displacement below which unloading occurs along the loading curve: *LOADING DATA, TYPE=PERMANENT DEFORMATION, YIELD ONSET=value Use the following options to specify the onset of yield by defining a slope drop for the loading curve: *LOADING DATA, TYPE=PERMANENT DEFORMATION, SLOPE DROP=value Specifying exponential/quadratic unloading The model in Figure 31.2.10–7 illustrates an analytical unloading curve that is derived based on an energy dissipation factor, (fraction of energy that is dissipated at any displacement level) and a permanent deformation factor, . As the connector is loaded, the force follows the path given by the loading curve. If the connector is unloaded (for example, at point B), the force follows the unloading curve . The point D corresponds to the permanent deformation, . Reloading after unloading follows the unloading curve , after which the loading path follows the loading curve. The arrows shown in Figure 31.2.10–7 illustrate the loading/unloading paths of this model. until the loading is such that the displacement becomes greater than The unloading response follows the loading curve when the calculated unloading curve lies above the loading curve to prevent energy generation and follows a zero force response when the unloading curve yields a negative response. In such cases the dissipated energy will be less than the value specified by the energy dissipation factor. Input File Usage: Use the following option to define quadratic unloading behavior: *UNLOADING DATA, DEFINITION=QUADRATIC Use the following option to define exponential unloading behavior: *UNLOADING DATA, DEFINITION=EXPONENTIAL Primary loading curve Umax DpUmax exponential/quadratic unloading Figure 31.2.10–7 Exponential/quadratic unloading. Specifying interpolated curve unloading The model in Figure 31.2.10–8 illustrates an interpolated unloading response based on multiple unloading curves that intersect the primary loading curve at increasing values of forces/displacements. You can specify as many unloading curves as are necessary to define the unloading response. The first point of each unloading curve defines the permanent deformation if the connector is completely unloaded. The unloading curves are stored in normalized form so that they intersect the loading curve at a unit force for a unit displacement, and the interpolation occurs between these normalized curves. If unloading occurs from a maximum displacement for which an unloading curve is not specified, the unloading curve is interpolated from neighboring unloading curves. As the connector is loaded, the force follows the path given by the loading curve. If the connector is unloaded (for example, at point B), the force follows the unloading curve until the loading is such that the displacement becomes greater than , after which the loading path follows the loading curve. . Reloading after unloading follows the unloading path If the loading curve depends on the constitutive displacements/rotations in several component directions, the unloading curves also depends on the same component directions. The unloading curve also has the same temperature and field variable dependencies as the loading curve. Input File Usage: *UNLOADING DATA, DEFINITION=INTERPOLATED CURVE Specifying shifted curve unloading You can specify an unloading curve passing through the origin in addition to the loading curve. The actual unloading curve is obtained by horizontally shifting the user-specified unloading curve to pass through the point of unloading as shown in Figure 31.2.10–9. The permanent deformation upon complete unloading is the horizontal shift applied to the unloading curve. Primary loading curve Unloading curves Umax Figure 31.2.10–8 Interpolated curve unloading. unloading curve Primary loading curve shifted unloading curve Umax Figure 31.2.10–9 Shifted curve unloading. If the loading curve depends on the constitutive displacements/rotations in several component directions, the unloading curve also depends on the same component directions. The unloading curve also has the same temperature and field variable dependencies as the loading curve. *UNLOADING DATA, DEFINITION=SHIFTED CURVE Input File Usage: Using different uniaxial models in tension and compression When appropriate, different uniaxial behavior models can be used in tension and compression. For example, a model with permanent deformation and exponential unloading in tension can be combined with a nonlinear elastic model in compression . Primary loading curve unloading nonlinear elastic Figure 31.2.10–10 Different uniaxial models in tension and compression. Output The Abaqus output variables available for connectors are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2. The following output variables are of particular interest when defining uniaxial behavior in connectors: CU CUF Connector relative displacements/rotations. Connector uniaxial forces/moments. 32. Special-Purpose Elements 32.1 32.2 32.3 32.4 32.5 32.6 32.7 32.8 32.9 32.10 32.11 32.12 32.13 32.14 32.15 Spring elements Dashpot elements Flexible joint elements Distributing coupling elements Cohesive elements Gasket elements Surface elements Tube support elements Line spring elements Elastic-plastic joints Drag chain elements Pipe-soil elements Acoustic interface elements Eulerian elements 32.1 Spring elements • “Springs,” Section 32.1.1 • “Spring element library,” Section 32.1.2 32.1.1 SPRINGS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Spring element library,” Section 32.1.2 • *SPRING • “Defining springs and dashpots,” Section 37.1 of the Abaqus/CAE User’s Manual Overview Spring elements: • can couple a force with a relative displacement; • in Abaqus/Standard can couple a moment with a relative rotation; • can be linear or nonlinear; • if linear, can be dependent on frequency in direct-solution steady-state dynamic analysis; • can be dependent on temperature and field variables; and • can be used to assign a structural damping factor to form the imaginary part of spring stiffness. The terms “force” and “displacement” are used throughout the description of spring elements. When the spring is associated with displacement degrees of freedom, these variables are the force and relative displacement in the spring. If the springs are associated with rotational degrees of freedom, they are torsional springs; these variables will then be the moment transmitted by the spring and the relative rotation across the spring. Viscoelastic spring behavior can be modeled in Abaqus/Standard by combining frequency- dependent springs and frequency-dependent dashpots. Typical applications Spring elements are used to model actual physical springs as well as idealizations of axial or torsional components. They can also model restraints to prevent rigid body motion. They are also used to represent structural dampers by specifying structural damping factors to form the imaginary part of the spring stiffness. Choosing an appropriate element SPRING1 and SPRING2 elements are available only in Abaqus/Standard. SPRING1 is between a node and ground, acting in a fixed direction. SPRING2 is between two nodes, acting in a fixed direction. The SPRINGA element is available in both Abaqus/Standard and Abaqus/Explicit. SPRINGA acts between two nodes, with its line of action being the line joining the two nodes, so that this line of action can rotate in large-displacement analysis. The spring behavior can be linear or nonlinear in any of the spring elements in Abaqus. Element types SPRING1 and SPRING2 can be associated with displacement or rotational degrees of freedom (in the latter case, as torsional springs). However, the use of torsional springs in large- displacement analysis requires careful consideration of the definition of total rotation at a node; therefore, connector elements (“Connectors: overview,” Section 31.1.1) are usually a better approach to providing torsional springs for large-displacement cases. Input File Usage: Use the following option to specify a spring element between a node and ground, acting in a fixed direction: Abaqus/CAE Usage: *ELEMENT, TYPE=SPRING1 Use the following option to specify a spring element between two nodes, acting in a fixed direction: *ELEMENT, TYPE=SPRING2 Use the following option to specify a spring element between two nodes with its line of action being the line joining the two nodes: *ELEMENT, TYPE=SPRINGA Property or Interaction module: Special→Springs/Dashpots→Create, then select one of the following: Connect points to ground: select points: toggle on Spring stiffness (equivalent to SPRING1) Connect two points: select points: Axis: Specify fixed direction: toggle on Spring stiffness (equivalent to SPRING2) Connect two points: select points: Axis: Follow line of action: toggle on Spring stiffness (equivalent to SPRINGA) Stability considerations in Abaqus/Explicit A SPRINGA element introduces a stiffness between two degrees of freedom without introducing an associated mass. In an explicit dynamic procedure this represents an unconditionally unstable element. The nodes to which the spring is attached must have some mass contribution from adjacent elements; if this condition is not satisfied, Abaqus/Explicit will issue an error message. If the spring is not too stiff (relative to the stiffness of the adjacent elements), the stable time increment determined by the explicit dynamics procedure (“Explicit dynamic analysis,” Section 6.3.3) will suffice to ensure stability of the calculations. Abaqus/Explicit does not use the springs in the determination of the stable time increment. During the data check phase of the analysis, Abaqus/Explicit computes the minimum of the stable time increment for all the elements in the mesh except the spring elements. The program then uses this minimum stable time increment and the stiffness of each of the springs to determine the mass required for each spring to give the same stable time increment. If this mass is too large compared to the mass of the model, Abaqus/Explicit will issue an error message that the spring is too stiff compared to the model definition. Relative displacement definition The relative displacement definition depends on the element type. SPRING1 elements The relative displacement across a SPRING1 element is the ith component of displacement of the spring’s node: where i is defined as described below and can be in a local direction . SPRING2 elements The relative displacement across a SPRING2 element is the difference between the ith component of displacement of the spring’s first node and the jth component of displacement of the spring’s second node: where i and j are defined as described below and can be in local directions . It is important to understand how the SPRING2 element will behave according to the above relative displacement equation since the element can produce counterintuitive results. For example, a SPRING2 element set up in the following way will be a “compressive” spring: If the nodes displace so that , the spring appears to be in compression, while the force in the SPRING2 element is positive. To obtain a “tensile” spring, the SPRING2 element should be set up in the following way: and SPRINGA elements For geometrically linear analysis the relative displacement is measured along the direction of the SPRINGA element in the reference configuration: where second node. is the reference position of the first node of the spring and is the reference position of its For geometrically nonlinear analysis the relative displacement across a SPRINGA element is the change in length in the spring between the initial and the current configuration: where configuration. Here is the current length of the spring and is the value of l in the initial and are the current positions of the nodes of the spring. In either case the force in a SPRINGA element is positive in tension. Defining spring behavior The spring behavior can be linear or nonlinear. In either case you must associate the spring behavior with a region of your model. Input File Usage: *SPRING, ELSET=name where the ELSET parameter refers to a set of spring elements. Abaqus/CAE Usage: Property or Interaction module: Special→Springs/Dashpots→Create: select connectivity type: select points Defining linear spring behavior You define linear spring behavior by specifying a constant spring stiffness (force per relative displacement). The spring stiffness can depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and independent field variables. For direct-solution steady-state dynamic analysis the spring stiffness can depend on frequency, as well as on temperature and field variables. If a frequency-dependent spring stiffness is specified for any other analysis procedure in Abaqus/Standard, the data for the lowest frequency given will be used. Input File Usage: *SPRING, DEPENDENCIES=n first data line spring stiffness, frequency, temperature, field variable 1, etc. ... Abaqus/CAE Usage: Property or Interaction module: Special→Springs/Dashpots→Create: select connectivity type: select points: Property: Spring stiffness: spring stiffness Defining the spring stiffness as a function of frequency, temperature, and field variables is not supported in Abaqus/CAE when you define springs as engineering features; instead, you can define connectors that have spring-like elastic behavior . Defining nonlinear spring behavior You define nonlinear spring behavior by giving pairs of force–relative displacement values. These values should be given in ascending order of relative displacement and should be provided over a sufficiently wide range of relative displacement values so that the behavior is defined correctly. Abaqus assumes that the force remains constant (which results in zero stiffness) outside the range given . Force, F F(0) F1 Continuation assumed if u < u1 Continuation assumed if u > u4 Displacement, u Figure 32.1.1–1 Nonlinear spring force–relative displacement relationship. Initial forces in nonlinear springs should be defined as part of the relationship by giving a nonzero force, , at zero relative displacement. The spring stiffness can depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and independent field variables. Abaqus/Explicit will regularize the data into tables that are defined in terms of even intervals of the independent variables. In some cases where the force is defined at uneven intervals of the independent variable (relative displacement) and the range of the independent variable is large compared to the smallest interval, Abaqus/Explicit may fail to obtain an accurate regularization of your data in a reasonable number of intervals. In this case the program will stop after all data are processed with an error message that you must redefine the material data. See “Material data definition,” Section 21.1.2, for a more detailed discussion of data regularization. Input File Usage: Abaqus/CAE Usage: *SPRING, NONLINEAR, DEPENDENCIES=n first data line force, relative displacement, temperature, field variable 1, etc. ... Defining nonlinear spring behavior is not supported in Abaqus/CAE when you define springs as engineering features; instead, you can define connectors that have spring-like elastic behavior . Defining the direction of action for SPRING1 and SPRING2 elements You define the direction of action for SPRING1 and SPRING2 elements by giving the degree of freedom at each node of the element. This degree of freedom may be in a local coordinate system (“Orientations,” Section 2.2.5). The local system is assumed to be fixed: even in large-displacement analysis SPRING1 and SPRING2 elements act in a fixed direction throughout the analysis. Input File Usage: *SPRING, ORIENTATION=name dof at node 1, dof at node 2 Abaqus/CAE Usage: Property or Interaction module: Special→Springs/Dashpots→Create, then select one of the following: Connect points to ground: select points: Orientation: Edit: select orientation Connect two points: select points: Axis: Specify fixed direction: Orientation: Edit: select orientation Defining linear spring behavior with complex stiffness Springs can be used to simulate structural dampers that contribute to the imaginary part of the element stiffness forming an elemental structural damping matrix. You specify both the real part of the spring stiffness for particular degrees of freedom and the structural damping factor, s. The imaginary part of the spring stiffness is calculated as and represents structural damping. These data can be frequency dependent. Input File Usage: *SPRING, COMPLEX STIFFNESS first data line real spring stiffness, structural damping factor, frequency Abaqus/CAE Usage: Linear spring behavior with complex stiffness is not supported in Abaqus/CAE. 32.1.2 SPRING ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Springs,” Section 32.1.1 • *SPRING Overview This section provides a reference to the spring elements available in Abaqus/Standard and Abaqus/Explicit. Element types SPRINGA SPRING1(S) SPRING2(S) Axial spring between two nodes, whose line of action is the line joining the two nodes. This line of action may rotate in large-displacement analysis. Spring between a node and ground, acting in a fixed direction Spring between two nodes, acting in a fixed direction Active degrees of freedom SPRINGA: 1, 2, 3. The translational degree of freedom in the 3-direction is not activated in an Abaqus/Standard analysis if both nodes of the element are connected to two-dimensional entities such as two-dimensional analytical rigid surfaces, two-dimensional beam elements, etc. SPRING1 or SPRING2: 1, 2, 3, 4, 5, or 6. If you specify a local orientation for the spring, these are local degrees of freedom. Otherwise, these are global degrees of freedom. Additional solution variables None. Nodal coordinates required SPRINGA: X, Y, Z. These coordinates are used in the calculation of the action of the element. SPRING1 or SPRING2: None. The element nodes do not need to have coordinates defined since the action associated with these elements is defined by specifying the degrees of freedom involved. Element property definition Input File Usage: Abaqus/CAE Usage: *SPRING Property or Interaction module: Special→Springs/Dashpots→Create Element-based loading None. Element output S11 E11 Force in the spring. Relative displacement across the spring. Node ordering on elements SPRINGA SPRING2 SPRING1 32.2 Dashpot elements • “Dashpots,” Section 32.2.1 • “Dashpot element library,” Section 32.2.2 32.2.1 DASHPOTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Dashpot element library,” Section 32.2.2 • *DASHPOT • “Defining springs and dashpots,” Section 37.1 of the Abaqus/CAE User’s Manual Overview Dashpot elements: • can couple a force with a relative velocity; • in Abaqus/Standard can couple a moment with a relative angular velocity; • can be linear or nonlinear; • if linear, can be dependent on frequency in direct-solution steady-state dynamic analysis; • can be dependent on temperature and field variables; and • can be used in any stress analysis procedure. The terms “force” and “velocity” are used throughout the description of dashpot elements. When the dashpot is associated with displacement degrees of freedom, these variables are the force and relative velocity in the dashpot. If the dashpots are associated with rotational degrees of freedom, they are torsional dashpots; these variables will then be the moment transmitted by the dashpot and the relative angular velocity across the dashpot. In dynamic analysis the velocities are obtained as part of the integration operator; in quasi-static analysis in Abaqus/Standard the velocities are obtained by dividing the displacement increments by the time increment. Typical applications Dashpots are used to model relative velocity-dependent force or torsional resistance. They can also provide viscous energy dissipation mechanisms. Dashpots are often useful in unstable, nonlinear, static analyses where the modified Riks algorithm is not appropriate and where the automatic time stepping algorithm is used because sudden shifts in configuration can be controlled by the forces that arise in the dashpots. In such cases the magnitude of the damping must be chosen in conjunction with the time period so that enough damping is available to control such difficulties but the damping forces are negligible when a stable static response is obtained. See also the contact damping available with contact elements in Abaqus/Standard . Choosing an appropriate element DASHPOT1 and DASHPOT2 elements are available only in Abaqus/Standard. DASHPOT1 is between a specified degree of freedom and ground. DASHPOT2 is between two specified degrees of freedom. The DASHPOTA element is available in both Abaqus/Standard and Abaqus/Explicit. DASHPOTA is between two nodes with its line of action being the line joining the two nodes. The dashpot behavior can be linear or nonlinear in any of these elements. Input File Usage: Use the following option to specify a dashpot element between a specified degree of freedom and ground: Abaqus/CAE Usage: *ELEMENT, TYPE=DASHPOT1 Use the following option to specify a dashpot element between two degrees of freedom: *ELEMENT, TYPE=DASHPOT2 Use the following option to specify a dashpot element between two nodes with its line of action being the line joining the two nodes: *ELEMENT, TYPE=DASHPOTA Property or Interaction module: Special→Springs/Dashpots→Create, then select one of the following: Connect points to ground: select points: toggle on Dashpot coefficient (equivalent to DASHPOT1) Connect two points: select points: Axis: Specify fixed direction: toggle on Dashpot coefficient (equivalent to DASHPOT2) Connect two points: select points: Axis: Follow line of action: toggle on Dashpot coefficient (equivalent to DASHPOTA) Stability considerations in Abaqus/Explicit Abaqus/Explicit does not take dashpots into account when determining the stable time step; therefore, care should be taken when introducing dashpots into the mesh. A DASHPOTA element introduces a damping force between two degrees of freedom without introducing any stiffness between these degrees of freedom and without introducing any mass at the nodes. This can cause a reduction in the stable time increment. For example, consider a simple system of a truss element and a dashpot element as shown in Figure 32.2.1–1. The dynamic equation for this system is or ⇒ k = EA m = ρAL Figure 32.2.1–1 A simple truss and dashpot system. where and The stable time increment for the spring-dashpot system is As the dashpot coefficient c is increased, the stable time increment, , will be reduced. To avoid this reduction in the stable time increment, dashpots should be used in parallel with spring or truss elements, where the stiffness of the spring or truss elements is chosen so that the stable time increment of the dashpot and spring or truss is larger than the stable critical time increment that is calculated by Abaqus/Explicit. If this requires springs or trusses that have unacceptable forces, specify the time increment size directly for the step . Relative velocity definition The relative velocity definition depends on the element type. DASHPOT1 elements The relative velocity across a DASHPOT1 element is the ith component of velocity of the dashpot’s node: where i is defined as described below and can be in a local direction . DASHPOT2 elements The relative velocity across a DASHPOT2 element is the difference between the ith component of velocity at the dashpot’s first node and the jth component of velocity of the dashpot’s second node: where i and j are defined as described below and can be in local directions . It is important to understand how the DASHPOT2 element will behave according to the above relative displacement equation since the element can produce counterintuitive results. For example, a DASHPOT2 element set up in the following way will be a “compressive” dashpot: If the nodes have velocities such that , the dashpot is compressed while the force and in the dashpot is positive. To obtain a “tensile” dashpot, the DASHPOT2 element should be set up in the following way: DASHPOTA elements The relative velocity across a DASHPOTA element is the difference between the velocity of the dashpot’s second node and the dashpot’s first node, taken in the direction of the current axis of the dashpot. For geometrically linear analysis, where second node, and is the reference position of the dashpot’s first node, is the reference length of the dashpot. For geometrically nonlinear analysis, is the reference position of the dashpot’s where second node, and l is the current length of the dashpot. is the current position of the dashpot’s first node, is the current position of the dashpot’s In either case the force in a DASHPOTA element is positive if the dashpot is extending. Defining dashpot behavior The dashpot behavior can be linear or nonlinear. In either case you must associate the dashpot behavior with a region of your model. Input File Usage: *DASHPOT, ELSET=name where the ELSET parameter refers to a set of dashpot elements. Abaqus/CAE Usage: Property or Interaction module: Special→Springs/Dashpots→Create: select connectivity type: select points Linear dashpot behavior You define linear dashpot behavior by specifying a constant dashpot coefficient (force per relative velocity). The dashpot coefficient can depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and independent field variables. For direct-solution steady-state dynamic analysis the dashpot coefficient can depend on frequency, as well as on temperature and field variables. If a frequency-dependent dashpot coefficient is specified for any other analysis procedure in Abaqus/Standard, the data for the lowest frequency given will be used. Input File Usage: Abaqus/CAE Usage: *DASHPOT, DEPENDENCIES=n first data line dashpot coefficient, frequency, temperature, field variable 1, etc. ... Property or Interaction module: Special→Springs/Dashpots→Create: select connectivity type: select points: Property: Dashpot coefficient: dashpot coefficient Defining the dashpot coefficient as a function of frequency, temperature, and field variables is not supported in Abaqus/CAE when you define dashpots as engineering features; instead, you can define connectors that have dashpot-like damping behavior . Nonlinear dashpot behavior You define nonlinear dashpot behavior by giving pairs of force–relative velocity values. These values should be given in ascending order of relative velocity and should be provided over a sufficiently wide range of relative velocity values so that the behavior is defined correctly. Abaqus assumes that the force remains constant outside the range given . In addition, the curve should pass through the origin. That is, the force should be zero at zero relative velocity. Force, F F1 Continuation assumed if v < v1 Continuation assumed if v > v4 Relative velocity, v Figure 32.2.1–2 Nonlinear dashpot force-relative velocity relationship. The dashpot coefficient can depend on temperature and field variables. See “Input syntax rules,” Section 1.2.1, for further information about defining data as functions of temperature and independent field variables. Abaqus/Explicit will regularize the data into tables that are defined in terms of even intervals of the independent variables. In some cases where the force is defined at uneven intervals of the independent variable (relative velocity) and the range of the independent variable is large compared to the smallest interval, Abaqus/Explicit may fail to obtain an accurate regularization of your data in a reasonable number of intervals. In this case the program will stop after all data are processed with an error message that you must redefine the material data. See “Material data definition,” Section 21.1.2, for a more detailed discussion of data regularization. Input File Usage: Abaqus/CAE Usage: *DASHPOT, NONLINEAR, DEPENDENCIES=n first data line force, relative velocity, temperature, field variable 1, etc. ... Defining nonlinear dashpot behavior is not supported in Abaqus/CAE when you define dashpots as engineering features; instead, you can define connectors that have dashpot-like damping behavior . Defining the direction of action for DASHPOT1 and DASHPOT2 elements You define the direction of action for DASHPOT1 and DASHPOT2 elements by giving the degree of freedom at each node of the element. This degree of freedom may be in a local coordinate system (“Orientations,” Section 2.2.5). This local system is assumed to be fixed: even in large-displacement analysis DASHPOT1 and DASHPOT2 elements act in a fixed direction throughout the analysis. Input File Usage: *DASHPOT, ORIENTATION=name dof at node 1, dof at node 2 Abaqus/CAE Usage: Property or Interaction module: Special→Springs/Dashpots→Create, then select one of the following: Connect points to ground: select points: Orientation: Edit: select orientation Connect two points: select points: Axis: Specify fixed direction: Orientation: Edit: select orientation Dashpots within substructures Dashpots cannot be used within substructures. You can define Rayleigh damping within the substructure definition or on the usage level to create damping within a substructure; see “Defining substructure damping” in “Using substructures,” Section 10.1.1, for more information. 32.2.2 DASHPOT ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Dashpots,” Section 32.2.1 • *DASHPOT Overview This section provides a reference to the dashpot elements available in Abaqus/Standard and Abaqus/Explicit. Element types DASHPOTA Axial dashpot between two nodes, whose line of action is the line joining the two nodes DASHPOT1(S) Dashpot between a node and ground, acting in a fixed direction DASHPOT2(S) Dashpot between two nodes, acting in a fixed direction Active degrees of freedom DASHPOTA: 1, 2, 3. The translational degree of freedom in the 3-direction is not activated in an Abaqus/Standard analysis if both nodes of the element are connected to two-dimensional entities such as two-dimensional analytical rigid surfaces, two-dimensional beam elements, etc. DASHPOT1 or DASHPOT2: 1, 2, 3, 4, 5, or 6. If you specify a local orientation for the dashpot, these are local degrees of freedom. Otherwise, these are global degrees of freedom. Additional solution variables None. Nodal coordinates required DASHPOTA: X, Y, Z. These coordinates are used in the calculation of the action of the element. DASHPOT1 or DASHPOT2: None. The element nodes do not need to have coordinates defined since the action associated with these elements is defined by specifying the degrees of freedom involved. Element property definition Input File Usage: Abaqus/CAE Usage: *DASHPOT Property or Interaction module: Special→Springs/Dashpots→Create Element-based loading None. Element output S11 E11 ER11 The force in the dashpot. The relative displacement across the dashpot. The relative velocity across the dashpot (available only from Abaqus/Standard). Node ordering on elements DASHPOTA DASHPOT2 DASHPOT1 32.3 Flexible joint elements • “Flexible joint element,” Section 32.3.1 • “Flexible joint element library,” Section 32.3.2 32.3.1 FLEXIBLE JOINT ELEMENT Product: Abaqus/Standard References • “Flexible joint element library,” Section 32.3.2 • *JOINT • *DASHPOT • *SPRING Overview JOINTC elements: • are used to model joint interactions; and • are made up of translational and rotational springs and parallel dashpots in a local, corotational coordinate system. Details of the element formulation can be found in “Flexible joint element,” Section 3.9.6 of the Abaqus Theory Manual. Typical applications The JOINTC element is provided to model the interaction between two nodes that are (almost) coincident geometrically and that represent a joint with internal stiffness and/or damping (such as a rubber bushing in a car suspension system) so that the second node of the joint can displace and rotate slightly with respect to the first node. Joints that have only one or two axes of rotation and no relative displacement are better modeled by the REVOLUTE- or UNIVERSAL-type MPCs . Similar functionality is available using connectors; see “Connectors: overview,” Section 31.1.1. Defining the joint behavior The joint behavior consists of linear or nonlinear springs and dashpots in parallel, coupling the corresponding components of relative displacement and of relative rotation in the joint. You define the spring and dashpot behavior as described in “Springs,” Section 32.1.1, and “Dashpots,” Section 32.2.1. Each spring or dashpot definition defines the behavior for one of the six local directions; up to six spring and six dashpot definitions can be included. If no specification is given for a particular local relative motion in the joint, the joint is assumed to have no stiffness with respect to that component. The joint behavior can be defined in a local coordinate system that rotates with the motion of the first node of the element (“Orientations,” Section 2.2.5). If a local coordinate system is not defined, the global system is used. You must associate the joint behavior with a set of JOINTC elements. The kinematic behavior of JOINTC elements is described in detail in “Flexible joint element,” Section 3.9.6 of the Abaqus Theory Manual. Input File Usage: Use the following options to define the joint behavior: *JOINT, ELSET=name, ORIENTATION=name *DASHPOT *SPRING Up to six *SPRING and *DASHPOT options can appear. Using JOINTC elements in large-displacement analyses In large-displacement analysis the formulation for the relationship between moments and rotations limits the usefulness of these elements to small relative rotations. The relative rotation across a JOINTC element should be of a magnitude to qualify as a small rotation. 32.3.2 FLEXIBLE JOINT ELEMENT LIBRARY Product: Abaqus/Standard References • “Flexible joint element,” Section 32.3.1 • *JOINT Overview This section provides a reference to the flexible joint elements available in Abaqus/Standard. Element types JOINTC Joint interaction element Active degrees of freedom 1, 2, 3, 4, 5, 6 Additional solution variables None. Nodal coordinates required None. The element nodes do not need to have coordinates defined since the action associated with these elements is defined by specifying the degrees of freedom involved. Element property definition Input File Usage: *JOINT Element-based loading None. Element output S11 S22 S33 S12 S13 S23 Total direct force in the first local direction. Total direct force in the second local direction. Total direct force in the third local direction. Total moment about the first local direction. Total moment about the second local direction. Total moment about the third local direction. The relative displacements and rotations corresponding to the forces and moments above are chosen by requesting the corresponding “strains.” Nodes associated with the element Two nodes. The rotation at the first node of the element defines the rotation of the local axis system. { JOINT C ( local system, defined by a local orientation, attached to node 1 ) 32.4 Distributing coupling elements • “Distributing coupling elements,” Section 32.4.1 • “Distributing coupling element library,” Section 32.4.2 32.4.1 DISTRIBUTING COUPLING ELEMENTS Product: Abaqus/Standard References • “Distributing coupling element library,” Section 32.4.2 • *DISTRIBUTING COUPLING Overview Distributing coupling elements: • can be used to distribute forces and moments on a reference node to a collection of nodes; • can be used to prescribe an average displacement and rotation to a collection of nodes; • can be used to distribute mass to a collection of nodes; • can control the force and mass distribution through the use of weight factors specified for each coupling node; • can be used to create a flexible coupling between structural and solid elements; and • can be used with two- or three-dimensional stress/displacement elements. If distribution of mass is not required, the preferred method for defining a distributing constraint is described in “Coupling constraints,” Section 34.3.2. Typical applications The distributing coupling element constrains the motion of the coupling nodes to the translation and rotation of the element node. This constraint is enforced in an average sense and in a way that enables control of the transmission of loads. These characteristics make the distributing coupling element useful in a number of applications: • The element can be used to prescribe a displacement and rotation condition on a boundary in cases where relative motion among the nodes on the boundary is required. An example of such a case is prescribing a twist on the end of a structure that is expected to warp and/or deform within the end surface . • The element can be used to provide, through the motion of the reference node, a weighted average of the motion of the coupling nodes. • The element can be used to distribute loads, where the load distribution can be described with moment-of-inertia expressions. Examples of such cases include the classic bolt-pattern and weld- pattern load distribution expressions. • The element can be used as a coupling between two parts (structural-solid) to transfer forces and moments. In comparison to MPCs and the kinematic coupling constraint, the distributing coupling element can be considered a more “flexible” connection. DCOUP3D element node (NODE 1) prescribed rotation warping is permitted by the coupling element Group of coupling nodes (COUPLESET) Figure 32.4.1–1 DCOUP3D element used to impart a rotation on the surface of a structure without constraining motion within the surface. Choosing an appropriate element Two- and three-dimensional distributing coupling elements are available. Element DCOUP2D describes behavior only in the global X–Y plane. Element DCOUP2D can be used in an axisymmetric analysis; however, its use requires care in selecting the load distributing weight factors. For example, a uniform axial load distribution to a structure would require specification of load distribution weight factors in proportion to the radius of the coupling nodes. Since the radius of these nodes will change with deformation, this use of DCOUP2D would only approximate the correct load distribution behavior in a large-displacement analysis. Defining the distributing coupling To define a distributing coupling, you specify the coupling nodes to which loads and mass are to be distributed, along with the corresponding weighting of the distribution. A minimum of two coupling nodes is required. Input File Usage: *DISTRIBUTING COUPLING, ELSET=name node number or node set, weight_factor_1 node number or node set, weight_factor_2 ... Example This example illustrates the use of the DCOUP3D element to impart a rotation to the surface of a structure that is expected to deform in a general way. In this case warping and motion within the plane of the end surface are expected to occur. *ELEMENT, TYPE=DCOUP3D, ELSET=ROTATEELEMENT 1001, 1 *DISTRIBUTING COUPLING, ELSET=ROTATEELEMENT COUPLESET, 1.0 … *STEP, NLGEOM … *BOUNDARY 1, 6, 6, 1.0 … *END STEP Defining the load distribution The element distributes loads such that the resultants of the forces on the coupling nodes are equal to the forces and moments on the element node. For cases of more than a few coupling nodes, the distribution of the forces is not determined by equilibrium alone, and the user-specified weight factors are used to define the distribution. The weight factors are dimensionless and are normalized within each element so that the sum of all weight factors is one. As a consequence, the normalized weight factors describe the proportion of the total element force and moment that is transmitted through the particular coupling node. In the case of transmission of forces alone, the proportion of force transmitted through the node is simply the normalized weight factor. In the general case of transmission of forces and moments, the force distribution follows that of a classic bolt-pattern analysis, where the weight factors could be considered the areas of particular bolt cross-sections. Refer to “Distributing coupling elements,” Section 3.9.8 of the Abaqus Theory Manual, for specific details of the load distribution. In the example shown in Figure 32.4.1–1 the weight factor distribution chosen is homogeneous, with a value of 1.0. For the rotation depicted, a more accurate load distribution would reflect the fact that the shear forces on nodes near the edge of the slot will diminish to zero, which could be described by choosing individual weight factors for nodes near the slot edge. If the loading on the element were along the axis of the structure, the homogeneous distribution shown would be appropriate. For cases where different loading modes require different descriptions of the weight factor distribution, multiple distributing coupling elements with different element nodes and different weight factors can be used. Colinear coupling node arrangements The distributing coupling element transmits moments at the element node as a force distribution among the coupling nodes, even if these nodes have rotational degrees of freedom. Thus, when the coupling node arrangement is colinear, the element is not capable of transmitting all components of a moment at the element node. Specifically, the moment component that is parallel to the colinear coupling node arrangement will not be transmitted. When this case arises, a warning message is issued that identifies the axis about which the element will not transmit a moment. Use with nonuniform meshes When the distributing coupling element is used with coupling nodes attached to elements of varying size, care should be taken in selecting the weight factors. The weight factor selected for a node should generally scale with the size of the elements attached to that node. Defining the mass distribution The mass distribution is analogous to the force distribution; the specified element mass is distributed to the coupling nodes in proportion to the weight factors. Input File Usage: *DISTRIBUTING COUPLING, ELSET=name, MASS=total_element_mass node number or node set, weight_factor_1 node number or node set, weight_factor_2 ... Output Element nodal forces (the force the element places on the element and coupling nodes) are available through element variable NFORC. Element kinetic energy is available in dynamic procedures through the whole element variable ELKE. 32.4.2 DISTRIBUTING COUPLING ELEMENT LIBRARY Product: Abaqus/Standard References • “Distributing coupling elements,” Section 32.4.1 • *DISTRIBUTING COUPLING Overview This section provides a reference to the distributing coupling elements available in Abaqus/Standard. Element types DCOUP2D Two-dimensional distributing coupling element DCOUP3D Three-dimensional distributing coupling element Active degrees of freedom DCOUP2D: 1, 2, 6 DCOUP3D: 1, 2, 3, 4, 5, 6 Additional solution variables None. Nodal coordinates required DCOUP2D: X, Y DCOUP3D: X, Y, Z Element property definition You must identify a minimum of two nodes to which the distributing coupling element distributes loads and mass; in addition, you can specify the element mass. *DISTRIBUTING COUPLING Input File Usage: Element-based loading None. Element output ELKE Element kinetic energy. NFORC Element nodal forces. Nodes associated with the element 1 node is defined with the element. Additional nodes forming the coupling are defined in the element property definition. 32.5 Cohesive elements • “Cohesive elements: overview,” Section 32.5.1 • “Choosing a cohesive element,” Section 32.5.2 • “Modeling with cohesive elements,” Section 32.5.3 • “Defining the cohesive element’s initial geometry,” Section 32.5.4 • “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5 • “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6 • “Defining the constitutive response of fluid within the cohesive element gap,” Section 32.5.7 • “Two-dimensional cohesive element library,” Section 32.5.8 • “Three-dimensional cohesive element library,” Section 32.5.9 • “Axisymmetric cohesive element library,” Section 32.5.10 32.5.1 COHESIVE ELEMENTS: OVERVIEW Abaqus offers a library of cohesive elements to model the behavior of adhesive joints, interfaces in composites, and other situations where the integrity and strength of interfaces may be of interest. Overview Modeling with cohesive elements consists of: • choosing the appropriate cohesive element type (“Choosing a cohesive element,” Section 32.5.2); • including the cohesive elements in a finite element model, connecting them to other components, and understanding typical modeling issues that arise during modeling using cohesive elements (“Modeling with cohesive elements,” Section 32.5.3); • defining the initial geometry of the cohesive elements (“Defining the cohesive element’s initial geometry,” Section 32.5.4); and • defining the mechanical, and optionally the fluid, constitutive behavior of the cohesive elements. The mechanical constitutive behavior of the cohesive elements can be defined: • with a continuum-based constitutive model (“Modeling of an adhesive layer of finite thickness” in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5), • with a uniaxial stress-based constitutive model useful in modeling gaskets and/or single adhesive patches (“Modeling of gaskets and/or small adhesive patches” in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5), or • by using a constitutive model specified directly in terms of traction versus separation (“Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6). When pore pressure cohesive elements are used in soils procedures in Abaqus/Standard, the fluid constitutive behavior of the cohesive elements can be defined (“Defining the constitutive response of fluid within the cohesive element gap,” Section 32.5.7): • by defining the tangential fluid flow relationship, and • by defining a fluid leak-off coefficient that accounts for caking or fouling effects in rock fracture. Typical applications Cohesive elements are useful in modeling adhesives, bonded interfaces, gaskets, and rock fracture. The constitutive response of these elements depends on the specific application and is based on certain assumptions about the deformation and stress states that are appropriate for each application area. The nature of the mechanical constitutive response may broadly be classified to be based on: • a continuum description of the material; • a traction-separation description of the interface; or • a uniaxial stress state appropriate for modeling gaskets and/or laterally unconstrained adhesive patches. Each of these constitutive response types is discussed briefly below. Continuum-based modeling The modeling of adhesive joints involves situations where two bodies are connected together by a glue- like material . A continuum-based modeling of the adhesive is appropriate when the glue has a finite thickness. The macroscopic properties, such as stiffness and strength, of the adhesive material can be measured experimentally and used directly for modeling purposes . The adhesive material is generally more compliant than the surrounding material. The cohesive elements model the initial loading, the initiation of damage, and the propagation of damage leading to eventual failure in the material. Figure 32.5.1–1 Typical peel test using cohesive elements to model finite-thickness adhesives. In three-dimensional problems the continuum-based constitutive model assumes one direct (through-thickness) strain, two transverse shear strains, and all (six) stress components to be active at a material point. In two-dimensional problems it assumes one direct (through-thickness) strain, one transverse shear strain, and all (four) stress components to be active at a material point. Traction-separation-based modeling The modeling of bonded interfaces in composite materials often involves situations where the intermediate glue material is very thin and for all practical purposes may be considered to be of zero In this case the macroscopic material properties are not relevant thickness . directly, and the analyst must resort to concepts derived from fracture mechanics—such as the amount of energy required to create new surfaces . The cohesive elements model the stiffener skin debonding bond line Debonding along skin-stringer interface. Figure 32.5.1–2 Debonding along a skin-stringer interface: typical situation for traction-separation-based modeling. initial loading, the initiation of damage, and the propagation of damage leading to eventual failure at the bonded interface. The behavior of the interface prior to initiation of damage is often described as linear elastic in terms of a penalty stiffness that degrades under tensile and/or shear loading but is unaffected by pure compression. You may use the cohesive elements in areas of the model where you expect cracks to develop. However, the model need not have any crack to begin with. In fact, the precise locations (among all areas modeled with cohesive elements) where cracks initiate, as well as the evolution characteristics of such cracks, are determined as part of the solution. The cracks are restricted to propagate along the layer of cohesive elements and will not deflect into the surrounding material. In three-dimensional problems the traction-separation-based model assumes three components of separation—one normal to the interface and two parallel to it; and the corresponding stress components are assumed to be active at a material point. In two-dimensional problems the traction-separation-based model assumes two components of separation—one normal to the interface and the other parallel to it; and the corresponding stress components are assumed to be active at a material point. Modeling of gaskets and/or laterally unconstrained adhesive patches Cohesive elements also provide some limited capabilities for modeling gaskets . The constitutive response of gaskets modeled with cohesive elements can be defined using only macroscopic properties such as stiffness and strength . No specialized gasket behavior (typically defined in terms of pressure versus closure) is available. Compared to the class flanges gasket gasket fasteners Figure 32.5.1–3 Typical application involving gaskets. of gasket elements available in Abaqus/Standard (“Gasket elements: overview,” Section 32.6.1), the cohesive elements • are fully nonlinear (can be used with finite strains and rotations); • can have mass in a dynamic analysis; and • are available in both Abaqus/Standard and Abaqus/Explicit. It is assumed that the gaskets are subjected to a uniaxial stress state. A uniaxial stress state is also appropriate for modeling small adhesive patches that are unconstrained in the lateral direction. Any material model in Abaqus that is available for use with a one-dimensional element (beams, trusses, or rebars)—including, for example, the hyperelastic and the elastomeric foam material models (useful in this context for modeling gaskets, sealants, or shock absorbers made out of poron)—can be used with this approach. Spatial representation of a cohesive element Figure 32.5.1–4 demonstrates the key geometrical features that are used to define cohesive elements. The connectivity of cohesive elements is like that of continuum elements, but it is useful to think of cohesive elements as being composed of two faces separated by a thickness. The relative motion of the bottom and top faces measured along the thickness direction (local 3-direction for three-dimensional elements; local 2-direction for two-dimensional elements—see “Defining the cohesive element’s initial geometry,” Section 32.5.4, for further details on local directions) represents opening or closing of the interface. The relative change in position of the bottom and top faces measured in the plane orthogonal to the thickness thickness direction COHESIVE ELEMENTS: OVERVIEW cohesive element node bottom face midsurface Figure 32.5.1–4 Spatial representation of a three-dimensional cohesive element. direction quantifies the transverse shear behavior of the cohesive element. Stretching and shearing of the midsurface of the element (the surface halfway between the bottom and top faces) are associated with membrane strains in the cohesive element; however, it is assumed that the cohesive elements do not generate any stresses in a purely membrane response. Figure 32.5.1–5 shows the different deformation modes of a cohesive element. cohesive layer through-thickness behavior transverse shear membrane stretch membrane stretch membrane shear Figure 32.5.1–5 Deformation modes of a cohesive element. General issues related to modeling with cohesive elements While using cohesive elements, you should be mindful of important issues that are specific to these elements. Such issues include special considerations associated with using cohesive elements in conjunction with contact interactions, potential degradation of the stable time increment size in Abaqus/Explicit, and potential convergence problems in Abaqus/Standard. These issues are discussed in detail in “Modeling with cohesive elements,” Section 32.5.3. Cohesive elements are typically used to bond components together. “Modeling with cohesive elements,” Section 32.5.3, also discusses methods for connecting a cohesive layer to adjacent components. Procedures with which cohesive elements are allowed Cohesive elements without pore pressure degrees of freedom can be used in all stress/displacement analysis types. Although they do not have any degrees of freedom other than displacement, they can be used in coupled procedures to bond together components made out of coupled temperature-displacement elements, and in Abaqus/Standard coupled pore pressure-displacement elements and/or piezoelectric elements, to simulate mechanical failure of interfaces. The response of the cohesive element in such coupled procedures is mechanical only (for example, no heat transfer occurs across the interface in a coupled temperature-displacement problem). Cohesive elements with pore pressure degrees of freedom can be used in coupled pore fluid diffusion/stress analyses (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). The mechanical response of the coupled pore pressure–displacement element is the same as the equivalent displacement-only element, except that the gap fluid pressure is considered as a traction on open faces. 32.5.2 CHOOSING A COHESIVE ELEMENT Products: Abaqus/Standard Abaqus/Explicit References • “Cohesive elements: overview,” Section 32.5.1 • “Two-dimensional cohesive element library,” Section 32.5.8 • “Three-dimensional cohesive element library,” Section 32.5.9 • “Axisymmetric cohesive element library,” Section 32.5.10 Overview The Abaqus cohesive element library includes: • elements for two-dimensional analyses; • elements for three-dimensional analyses; and • elements for axisymmetric analyses. Naming convention The cohesive elements used in Abaqus are named as follows: COH 3D pore pressure (optional) number of nodes two-dimensional (2D), three-dimensional (3D), or axisymmetric (AX) cohesive element For example, COH2D4 is a 4-node, two-dimensional cohesive element. 32.5.3 MODELING WITH COHESIVE ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Cohesive elements: overview,” Section 32.5.1 • “Choosing a cohesive element,” Section 32.5.2 • *COHESIVE SECTION • Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Manual Overview Cohesive elements: • are used to model adhesives between two components, each of which may be deformable or rigid; • are used to model interfacial debonding using a cohesive zone framework; • are used to model gaskets and/or small adhesive patches; • can be connected to the adjacent components by sharing nodes, by using mesh tie constraints, or by using MPCs type TIE or PIN; and • may interact with other components via contact for gasket applications. This section discusses the techniques that are available to discretize cohesive zones and assemble them in a model representing several components that are bonded to one another. It also discusses several common modeling issues related to cohesive elements. Discretizing cohesive zones using cohesive elements The cohesive zone must be discretized with a single layer of cohesive elements through the thickness. If the cohesive zone represents an adhesive material with a finite thickness, the continuum macroscopic properties of this material can be used directly for modeling the constitutive response of the cohesive zone. Alternatively, if the cohesive zone represents an infinitesimally thin layer of adhesive at a bonded interface, it may be more relevant to define the response of the interface directly in terms of the traction at the interface versus the relative motion across the interface. Finally, if the cohesive zone represents a small adhesive patch or a gasket with no lateral constraint, a uniaxial stress state provides a good approximation to the state of these elements. Abaqus provides modeling capabilities for all the above cases. The details are discussed in later sections. Connecting cohesive elements to other components At least one of either the top or the bottom face of the cohesive element must be constrained to another component. In most applications it is appropriate to have both faces of the cohesive elements tied to neighboring components. If only one face of the cohesive element is constrained and the other face is free, the cohesive element exhibits one or (for three-dimensional elements) more singular modes of deformation due to the lack of membrane stiffness. The singular modes can propagate from one cohesive element to the adjacent one but can be suppressed by constraining the nodes on the side face at the end of a series of cohesive elements. In some cases it may be convenient and appropriate to have cohesive elements share nodes with the elements on the surfaces of the adjacent components. More generally, when the mesh in the cohesive zone is not matched to the mesh of the adjacent components, cohesive elements can be tied to other components. When cohesive elements are used to model gaskets, it may be more appropriate to tie or share nodes on one side and define contact on the other side as discussed below. This will prevent the gaskets from being subjected to tensile stresses. Having cohesive elements share nodes with other elements When the cohesive elements and their neighboring parts have matched meshes, it is straightforward to connect cohesive elements to other components in a model simply by sharing nodes . Explicitly defined node Part 1 pore pressure cohesive elements internally generated nodes Part 2 Figure 32.5.3–1 Cohesive elements sharing nodes with other Abaqus elements. When these elements are used as adhesives or to model debonding, this method can be used to obtain initial results from a model—more accurate local results (in the decohesion zone) would typically be obtained with the cohesive zone more refined than the elements of the surrounding components. When these elements are used to model gaskets, this approach is suitable in situations when no frictional slip occurs between the gaskets and the surrounding components. The method of sharing nodes in gasket applications will lead to tensile stresses in the gasket should the parts connected to the gasket be pulled apart. Defining contact on one side of the cohesive elements will avoid such tensile stresses. Connecting cohesive elements to other components by using surface-based tie constraints If the two neighboring parts do not have matched meshes, such as when the discretization level in the cohesive layer is different (typically finer) from the discretization level in the surrounding structures, the top and/or bottom surfaces of the cohesive layer can be tied to the surrounding structures using a tie constraint (“Mesh tie constraints,” Section 34.3.1). Figure 32.5.3–2 shows an example in which a finer discretization is used for the cohesive layer than for the neighboring parts. tie constraints Part 1 Part 2 cohesive elements Figure 32.5.3–2 Independent meshes with tie constraints. Contact interactions between cohesive elements and other components For some applications involving gaskets it is appropriate to define contact on one side of the cohesive element . Contact can be defined with either the general contact algorithm interactions in Abaqus/Explicit,” Section 35.4.1) in Abaqus/Explicit (“Defining general contact or the contact pair algorithm in Abaqus/Standard (“Defining contact pairs in Abaqus/Standard,” Section 35.3.1) or Abaqus/Explicit (“Defining contact pairs in Abaqus/Explicit,” Section 35.5.1). If pure master-slave contact is used, typically the surface of the cohesive elements should be the slave surface and the surface of the neighboring part should be the master surface. This choice of master and slave is based on the cohesive zone typically being composed of softer materials and having a finer discretization. The second consideration also suggests that mismatched meshes will often be used If mismatched meshes are used, the pressure distribution in analyses involving cohesive elements. contact interaction tie constraints Part 1 Part 2 cohesive elements Figure 32.5.3–3 Contact interaction on one side of a cohesive zone. on the cohesive elements may not be predicted accurately; submodeling (“Submodeling: overview,” Section 10.2.1) may be required to obtain accurate local results. Using cohesive elements in large-displacement analyses Cohesive elements can be used in large-displacement analyses. The assembly containing the cohesive elements can undergo finite displacement as well as finite rotation. Selecting the broad class of the constitutive response of cohesive elements As discussed earlier, cohesive elements can be used to model finite-thickness adhesives, negligibly thin adhesive layers for debonding applications, as well as gaskets and/or small adhesive patches. You must choose one of these broad classes of applications when you define the section properties of cohesive elements. The detailed implications of each choice are discussed in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5, and “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6. Input File Usage: Use the following option to model a finite-thickness adhesive layer using a continuum-based constitutive response: *COHESIVE SECTION, RESPONSE=CONTINUUM Use the following option to model a negligibly (geometrically) thin layer of adhesive using a traction-separation-based response: *COHESIVE SECTION, RESPONSE=TRACTION SEPARATION Use the following option to use cohesive elements as gaskets and/or small adhesive patches: *COHESIVE SECTION, RESPONSE=GASKET Property module: Create Section: select Other as the section Category and Cohesive as the section Type: Response: Continuum, Traction Separation, or Gasket Abaqus/CAE Usage: Assigning a material behavior to a cohesive element You assign the name of a material definition to a particular element set. The constitutive behavior for this element set is defined entirely by the constitutive thickness of the cohesive layer (discussed in “Specifying the constitutive thickness” in “Defining the cohesive element’s initial geometry,” Section 32.5.4) and the material properties referring to the same name. The constitutive behavior of the cohesive elements can be defined either in terms of a material model provided in Abaqus or a user-defined material model . When cohesive elements are used in applications involving a finite-thickness adhesive, any available material model in Abaqus, including material models for progressive damage, can be used. For applications involving gasket and/or small finite-thickness adhesive patches, any material model that can be used with one-dimensional elements (such as beams, trusses, and rebars), including material models for progressive damage, can be used. For further details, see “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5. For applications in which the behavior of cohesive elements is defined directly in terms of traction versus separation, the response can be defined only in terms of a linear elastic relation (between the traction and the separation) along with progressive damage . To define the constitutive behavior of cohesive elements, you assign the name of a material model to a particular element set through the section definition. The actual material model for a user-defined material model is defined in user subroutine UMAT in Abaqus/Standard or VUMAT in Abaqus/Explicit. Input File Usage: Abaqus/CAE Usage: *COHESIVE SECTION, ELSET=name, MATERIAL=name Property module: cohesive section editor: Material: name Using cohesive elements in coupled pore fluid diffusion/stress analyses Cohesive elements with, or without, pore pressure degrees of freedom can be used in coupled pore fluid diffusion/stress analyses. Cohesive elements without pore pressure degrees of freedom will only contribute mechanically, and surfaces exposed when cohesive elements open will be impermeable to fluid flow. Cohesive elements with pore pressure degrees of freedom provide a more general response, including the ability to model tangential flow and leakage flow from the gap into the adjacent material. These elements have additional pore pressure nodes in the gap interior, and you can choose to define these nodes explicitly or have them generated automatically by Abaqus/Standard. In a typical use you will have these gap interior nodes generated for you for the majority of cohesive elements in the model. You invoke automatic node generation as discussed in “By defining the bottom- face element connectivity and an integer offset” in “Defining the cohesive element’s initial geometry,” Section 32.5.4. Defining contact between surrounding components Cohesive elements are used to bond two different components. Often the cohesive elements completely degrade in tension and/or shear as a result of the deformation. Subsequently, the components that are initially bonded together by cohesive elements may come into contact with each other. Approaches for modeling this kind of contact include the following: • In certain situations this kind of contact can be handled by the cohesive element itself. By default, cohesive elements retain their resistance to compression even if their resistance to other deformation modes is completely degraded. As a result, the cohesive elements resist interpenetration of the surrounding components even after the cohesive element has completely degraded in tension and/or shear. This approach works best when the top and the bottom faces of the cohesive element do not displace tangentially by a significant amount relative to each other during the deformation. In other words, to model the situation described above, the deformation of the cohesive elements should be limited to “small sliding.” • Another possible approach is to define contact between the surfaces of the surrounding components that could potentially come into contact and to delete the cohesive elements once they are completely damaged. Thus, contact is modeled throughout the analysis. This approach is not recommended if the geometric thickness of the cohesive elements in the model is very small or zero (the geometric thickness of the cohesive elements may be different from the constitutive thickness you specify while defining the section properties of the cohesive elements—see “Specifying the constitutive thickness” in “Defining the cohesive element’s initial geometry,” Section 32.5.4) because contact will effectively cause nonphysical resistance to compression of the cohesive layer while the cohesive elements are still active. If frictional contact is modeled, there may also be nonphysical shearing forces. This is the behavior that will occur by default with the general contact algorithm in Abaqus/Explicit. Figure 32.5.3–4, Figure 32.5.3–5, and Figure 32.5.3–6 show the default surface for general contact. This surface: – is insensitive to whether the cohesive elements and neighboring elements share nodes, are tied together, or are not connected; and – does not include faces of cohesive elements. tie constraints Part 1 ⇒ cohesive elements Part 2 all element-based surfaces Figure 32.5.3–4 Default surface when cohesive elements share nodes with surrounding elements. tie constraints Part 1 ⇒ cohesive elements Part 2 all element-based surfaces Figure 32.5.3–5 Default surface when cohesive elements are tied to the surrounding elements. contact interaction tie constraints Part 1 ⇒ cohesive elements Part 2 all element- based surfaces Figure 32.5.3–6 Default surface when cohesive elements are tied on one side and interact through contact on the other side. Figure 32.5.3–7 shows the situation when the surfaces of the cohesive elements are also added to the default surface. Abaqus/Explicit generates a contact exclusion automatically so that the general contact algorithm avoids consideration of contact between the bottom surface of the cohesive elements and the top surface of Part 2 since these surfaces are tied together. contact interaction tie constraints Part 1 ⇒ cohesive elements Part 2 all element- based surfaces Figure 32.5.3–7 Top and bottom faces of the cohesive element along with the default surface when cohesive elements are tied on one side and interact through contact on the other side. Input File Usage: Use the following options to add the top and bottom faces of the cohesive elements to the default general contact surface (the cohesive elements are included in the element set COH_ELEMS): *SURFACE, NAME=DEFAULT_PLUS_COH , COH_ELEMS, *CONTACT *CONTACT INCLUSIONS DEFAULT_PLUS_COH, Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: default_plus_coh: pick faces in viewport Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: Selected surface pairs: Edit, select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of included pairs • For general contact in Abaqus/Explicit, yet another approach for modeling contact between the surrounding structures involves activating contact only when the cohesive elements are completely degraded and deleted from the model (see “Maximum degradation and choice of element removal” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6). For this approach the cohesive elements must share nodes with the neighboring element and the general contact definition must include surfaces on the top and bottom faces of the cohesive elements, as shown in Figure 32.5.3–8. Since each surface face of the cohesive elements directly opposes a surface face of a neighboring element, the general contact algorithm does not consider these faces active while both parent elements are active. However, if the cohesive element fails, the opposing surface faces become active. Input File Usage: Use the following options to include the top and bottom faces of the cohesive elements in the general contact definition (the cohesive elements are included in the element set COH_ELEMS): *SURFACE, NAME=gc_surf , COH_ELEMS, *CONTACT *CONTACT INCLUSIONS gc_surf, Abaqus/CAE Usage: Any module except Sketch, Job, and Visualization: Tools→Surface→Create: Name: gc_surf: pick faces in viewport Interaction module: Create Interaction: General contact (Explicit): Included surface pairs: Selected surface pairs: Edit, select the surfaces in the columns on the left, and click the arrows in the middle to transfer them to the list of included pairs Part 1 ⇒ cohesive elements Part 2 ⇒ all element- based surfaces and bottom and top faces of cohesive elements Figure 32.5.3–8 Surfaces that are involved in general contact when cohesive elements are included in the surface definition and erosion is used. Stable time increment in Abaqus/Explicit The stable time increment for a cohesive element in Abaqus/Explicit is equal to the time, for a stress wave to travel across the constitutive thickness, , of the cohesive layer: , required is the wave speed and represent the bulk stiffness and the density, respectively, where of the adhesive material. In terms of the expression for the wave speed, the stable time increment can be written as and For cases in which the constitutive response is defined in terms of traction versus separation, the slope of the traction versus separation relationship is and the density is specified as mass per unit area rather than per unit volume: . Therefore, for traction versus separation the expression for the time increment becomes It is quite common that the time increment of cohesive elements will be significantly less than that of the other elements in the model, unless you take some action to alter one or more of the factors influencing the time increment. This requires some judgement on your part. The following discussions provide some recommendations for controlling the time increment for the different methods of defining the material response. However, Abaqus/Standard may be preferable in some applications where it is necessary to model a thin, stiff cohesive layer without approximations. Constitutive response defined in terms of a continuum or uniaxial stress-state approach For constitutive response defined in terms of a continuum or uniaxial stress-state approach, the ratio of the stable time increment of the cohesive elements to that of the other elements is given by where the subscripts “c” and “e” stand for the cohesive elements and the surrounding elements, respectively. The thickness of the cohesive layer is often smaller than a characteristic length of the other elements in the model, so the quantity is often small. The quantity under the radical will depend on the materials involved. For an epoxy adhesive between steel components, the quantity under the radical is on the order of unity. The stable time increment of the cohesive element can be increased by artificially • increasing the constitutive thickness, • increasing the density, • reducing the stiffness, • some combination of the above. ; ; or ; In many cases the most attractive option will be to increase the density, which is also referred to as mass scaling (“Mass scaling,” Section 11.6.1). However, if the thickness of the cohesive zone is very small, the mass scaling required to achieve a reasonable time increment may affect the results significantly. In such cases it may be necessary to artificially reduce the cohesive stiffness in addition to some mass scaling. This approach involves the use of a stiffness that is different from the measured stiffness of the interface; however, if the peak strength and the fracture energy remain unchanged, the global response will not be affected significantly in many cases. Constitutive response defined in terms of traction versus separation For constitutive response defined in terms of traction versus separation, the ratio of the stable time increment of the cohesive elements to that for the other elements is given by where the subscripts “c” and “e” stand for the cohesive elements and the surrounding elements, respectively. One way to ensure that the cohesive elements will have no adverse effect on the stable time increment is to choose material properties such that , which implies This is accomplished if, for example, the cohesive element stiffness and density per unit area are chosen such that where represents the characteristic length of the neighboring non-cohesive elements. By choosing , the stiffness in the cohesive layer relative to the surrounding elements will be similar to the default stiffness used by penalty contact in Abaqus/Explicit (relative to the equivalent one-dimensional stiffness of the surrounding elements). This approach involves the use of a stiffness that is likely to be different from the measured stiffness of the interface; however, if the peak strength and the fracture energy remain unchanged, the global response will not be affected significantly in many cases. Convergence issues in Abaqus/Standard In many problems cohesive elements are modeled as undergoing progressive damage leading to failure. The modeling of progressive damage involves softening in the material response, which is known to lead to convergence difficulties in an implicit solution procedure, such as in Abaqus/Standard. Convergence difficulties may also occur during unstable crack propagation, when the energy available is higher than the fracture toughness of the material. Several methods are available to help avoid these convergence problems. Using viscous regularization Abaqus/Standard provides a viscous regularization capability that helps in improving the convergence for these kinds of problems. This capability is discussed in detail in “Using viscous regularization with cohesive elements, connector elements, and elements that can be used with the damage evolution models for ductile metals and fiber-reinforced composites in Abaqus/Standard” in “Section controls,” Section 27.1.4, and “Viscous regularization in Abaqus/Standard” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6. Using automatic stabilization Another approach to help convergence behavior is the use of automatic stabilization , which is useful when a problem is unstable due to local instabilities. Generally, if sufficient viscous regularization is used (as measured by the viscosity coefficient—see “Viscous regularization in Abaqus/Standard” in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6, for further details), the use of the automatic stabilization technique is not necessary. In problems where a small amount or no viscous regularization is used, automatic stabilization will improve the convergence characteristics. Using nondefault solution controls The use of nondefault solution controls and activation of the line search technique (“Improving the efficiency of the solution by using the line search algorithm” in “Convergence criteria for nonlinear problems,” Section 7.2.3) may be useful in improving the solution efficiency. DEFINING THE COHESIVE ELEMENT’S INITIAL GEOMETRY COHESIVE GEOMETRY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Cohesive elements: overview,” Section 32.5.1 • Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Manual Overview The initial geometry of a cohesive element is defined: • by the nodal connectivity of the element and the position of these nodes; • by the stack direction, which can be used to specify the top and the bottom faces of the cohesive element independent of the nodal connectivity; and • by the magnitude of the initial constitutive thickness, which can either correspond to the geometric thickness implied by the nodal positions and stack direction or be specified directly. Defining the element connectivity The connectivity of a cohesive element is like that of a continuum element; however, it is useful to think of a cohesive element as being composed of two faces (a bottom and a top face) separated by the cohesive zone thickness. The element has nodes on its bottom face and corresponding nodes on its top face. Pore pressure cohesive elements include a third, middle face, which is used to model fluid flow within the element. Three methods are available to define the element connectivity. By directly defining the element’s complete connectivity The complete connectivity of a cohesive element can be given directly . By defining the bottom-face element connectivity and an integer offset Alternatively, you can specify the connectivity of the bottom face plus a positive integer offset that will be used to determine the remaining cohesive element nodes. Input File Usage: Abaqus/CAE Usage: *ELEMENT, OFFSET=n Element offsets are not supported in Abaqus/CAE. Use with displacement cohesive elements The integer offset will be used to define node numbers of the top face of the cohesive element. Abaqus will automatically position the nodes of the top face to be coincident with those of the bottom face unless the nodes of the top face have already been assigned coordinates directly with a node definition (“Node definition,” Section 2.1.1). Use with pore pressure-displacement cohesive elements When you define only the bottom face nodes, the integer offset will first be used to define the node numbers of the top face of the cohesive element, with the numbering of the top-face nodes offset from the bottom face node numbers. The integer offset will again be used to define the middle surface node numbers offset, with the numbering of the middle-face nodes offset from the top face node numbers. Abaqus will automatically position the nodes of the top and middle faces to be coincident with those of the bottom face unless the nodes of the top face have already been assigned coordinates directly with a node definition (“Node definition,” Section 2.1.1). By defining the bottom- and top-face element connectivities and an integer offset For pore pressure cohesive elements, you also can specify the connectivity of the bottom and top faces plus a positive integer offset that will be used to determine the middle face cohesive element nodes. When you define the bottom and top face nodes, the integer offset will be used to define the node numbers of the middle face, with the numbering of the middle-face nodes offset from the bottom face node numbers. Abaqus will automatically position the nodes of the middle face to be halfway between those of the bottom and top faces unless the nodes of the middle face have already been assigned coordinates directly with a node definition (“Node definition,” Section 2.1.1). *ELEMENT, OFFSET=n Element offsets are not supported in Abaqus/CAE. Abaqus/CAE Usage: Input File Usage: Specifying the out-of-plane thickness for two-dimensional elements For two-dimensional cohesive elements the out-of-plane thickness is required. You specify this additional information in the cohesive section definition; the default value is 1.0. Input File Usage: *COHESIVE SECTION first data line out-of-plane thickness Abaqus/CAE Usage: Property module: cohesive section editor: toggle on Out-of-plane thickness: and specify the out-of-plane thickness Specifying the constitutive thickness You can specify the constitutive thickness of the cohesive element directly or allow Abaqus to compute it based on nodal coordinates such that the constitutive thickness is equal to the geometric thickness. The default behavior depends on the nature of the application. If the geometric thickness of the cohesive element is very small compared to its surface dimensions, the thickness computed from the nodal coordinates may be inaccurate. In such cases you can specify a constant thickness directly when defining the section properties of these elements. The characteristic element length of a cohesive element is equal to its constitutive thickness. The characteristic element length is often useful in defining the evolution of damage in materials . When the cohesive element response is based on a continuum approach When the response of the cohesive elements is based on a continuum approach, by default the constitutive thickness of the element is computed by Abaqus based on the nodal coordinates. You can override this default by specifying the constitutive thickness directly. Input File Usage: Use the following option to have Abaqus compute the thickness based on the nodal coordinates: *COHESIVE SECTION, RESPONSE=CONTINUUM, THICKNESS=GEOMETRY (default) Use the following option to specify the thickness directly: *COHESIVE SECTION, RESPONSE=CONTINUUM, THICKNESS=SPECIFIED thickness (1.0 by default) Abaqus/CAE Usage: Property module: cohesive section editor: Response: Continuum: Initial thickness: Use nodal coordinates, Specify: thickness, or Use analysis default When the cohesive element response is based on a traction-separation approach When the response of the cohesive elements is based on a traction-separation approach, Abaqus assumes by default that the constitutive thickness is equal to one. This default value is motivated by the fact that the geometric thickness of cohesive elements is often equal to (or very close to) zero for the kinds of applications in which a traction-separation-based constitutive response is appropriate. This default choice ensures that nominal strains are equal to the relative separation displacements . You can override this default by specifying another value or specifying that the constitutive thickness should be equal to the geometric thickness. Input File Usage: Use the following option to specify the thickness directly: *COHESIVE SECTION, RESPONSE=TRACTION SEPARATION, THICKNESS=SPECIFIED (default) thickness (1.0 by default) Abaqus/CAE Usage: Use the following option to have Abaqus compute the thickness based on the nodal coordinates: *COHESIVE SECTION, RESPONSE=TRACTION SEPARATION, THICKNESS=GEOMETRY Property module: cohesive section editor: Response: Traction Separation: Initial thickness: Specify: thickness, Use analysis default, or Use nodal coordinates When the cohesive element response is based on a uniaxial stress state When the response of the cohesive elements is based on a uniaxial stress state, there is no default method for computing the constitutive thickness. You must indicate your choice of the method of determining the constitutive thickness. Input File Usage: Use the following option to specify the thickness: *COHESIVE SECTION, RESPONSE=GASKET, THICKNESS=SPECIFIED thickness (1.0 by default) Use the following option to have Abaqus compute the thickness based on the nodal coordinates: *COHESIVE SECTION, RESPONSE=GASKET, THICKNESS=GEOMETRY Abaqus/CAE Usage: Property module: cohesive section editor: Response: Gasket: thickness: Specify: thickness or Use nodal coordinates Initial Element thickness direction definition It is important to define the orientation of cohesive elements correctly, since the behavior of the elements is different in the thickness and in-plane directions. By default, the top and bottom faces of cohesive elements are as shown in Figure 32.5.4–1 for three-dimensional cohesive elements and Figure 32.5.4–2 for two-dimensional and axisymmetric cohesive elements. Options for overriding the default orientation of cohesive elements are discussed below along with an explanation of how the local thickness direction and in-plane direction vectors are established. Setting the stack direction equal to an isoparametric direction The “stack direction” refers to the isoparametric direction along which the top and bottom faces of a cohesive element are stacked. By default, the top and bottom faces are stacked along the third isoparametric direction in three-dimensional cohesive elements and along the second isoparametric direction in two-dimensional and axisymmetric cohesive elements. You can choose to stack the top and bottom faces along an alternate isoparametric direction for most element types (the COH3D6 element can have only the third isoparametric direction as the stack direction). The choice of the isoparametric direction depends on the element connectivity. For a mesh-independent specification, top face bottom face thickness direction thickness direction Figure 32.5.4–1 Default thickness direction for three-dimensional cohesive elements. y (z) x (r) thickness direction Figure 32.5.4–2 Default thickness direction for two-dimensional and axisymmetric cohesive elements. use an orientation-based method as described below. three-dimensional cohesive elements are shown in Figure 32.5.4–3. The isoparametric direction choices for F6 F2 F5 F4 F3 F1 Stack direction F2 F5 F3 F1 F4 Stack direction Stack direction = 1 from face 6 to face 4 Stack direction = 2 from face 3 to face 5 Stack direction = 3 from face 1 to face 2 Stack direction = 3 from face 1 to face 2 Figure 32.5.4–3 Stack directions for COH3D8 (left) and COH3D6 (right) elements. Input File Usage: Use the following option to define the element top and bottom faces based on the element’s isoparametric directions: Abaqus/CAE Usage: *COHESIVE SECTION, STACK DIRECTION=n You cannot define the stack direction based on isoparametric directions in Abaqus/CAE. The stack direction will correspond to the default discussed above. Setting the stack direction based on a user-defined orientation You can also control the orientation of the stack direction through a user-defined local orientation (“Orientations,” Section 2.2.5). When you define an orientation for cohesive elements, you also specify an axis about which the local 1 and 2 material directions may be rotated. This axis also defines an approximate normal direction. The stack direction will be the element isoparametric direction that is closest to this approximate normal . Cohesive section, stack direction based on cylor1 ' (10, 0, 0) Local cylindrical orientation cylor1: a = 0, 0, 0 b = 10, 0, 0 ' Global (0, 0, 0) ABAQUS selects the isoparametric direction  that is closest to the 1st (i.e., x , or radial) axis, at the center. Figure 32.5.4–4 Example illustrating the use of a cylindrical system to define the stack direction. Input File Usage: Use the following option to define the element thickness direction based on a user-defined orientation: Abaqus/CAE Usage: *COHESIVE SECTION, STACK DIRECTION=ORIENTATION, ORIENTATION=name You cannot define the stack direction based on an orientation definition in Abaqus/CAE. The stack direction will correspond to the default discussed above. Verifying the stack direction The stack direction can be verified visually in Abaqus/CAE by using the stack direction query tool . For three-dimensional elements Abaqus/CAE colors the top face purple and the bottom face brown. For two-dimensional and axisymmetric elements, arrows indicate the orientation of the element. In addition, Abaqus/CAE highlights any element faces and edges that have inconsistent orientations. Alternatively, the material axes can be plotted in the Visualization module of Abaqus/CAE to verify that the 3-axis points in the desired normal direction for three-dimensional elements; and if the element is oriented improperly, one of the in-plane axes (either the 1- or 2-axis) will point in the normal direction. For two-dimensional and axisymmetric elements, the stack direction is consistent with the 2-axis material direction. Thickness direction computation for two-dimensional and axisymmetric elements To compute the thickness direction for two-dimensional and axisymmetric elements, Abaqus forms a midsurface by averaging the coordinates of the node pairs forming the bottom and top surfaces of the element. This midsurface passes through the integration points of the element, as shown in Figure 32.5.4–5 for the default choice of the bottom and top surfaces. For each integration point Abaqus computes a tangent whose direction is defined by the sequence of nodes given on the bottom and top surfaces. The thickness direction is then obtained as the cross product of the out-of-plane and tangent directions. n1 t1 midsurface n2 t2 Figure 32.5.4–5 Thickness direction for a two-dimensional or axisymmetric element. Thickness direction computation for three-dimensional elements To compute the thickness direction for three-dimensional elements, Abaqus forms a midsurface by averaging the coordinates of the node pairs forming the bottom and top surfaces of the element. This midsurface passes through the integration points of the element, as shown in Figure 32.5.4–6 for the default choice of the bottom and top surfaces. Abaqus computes the thickness direction as the normal to the midsurface at each integration point; the positive direction is obtained with the right-hand rule going around the nodes of the element on the bottom or top surface. n1 midsurface n4 n2 n3 Figure 32.5.4–6 Thickness direction for a three-dimensional element. Local directions at integration points Abaqus computes default local directions at each integration point. The local directions are used for output of all quantities that describe the current deformation state of a cohesive element. Details of local directions are discussed separately below for cohesive elements with two versus three local directions. Local directions for two-dimensional and axisymmetric cohesive elements The local 2-direction for two-dimensional and axisymmetric cohesive elements corresponds to the thickness direction, which is computed as discussed above in “Element thickness direction definition.” The local 1-direction is defined such that the cross product between the local 1- and 2-directions gives the out-of-plane direction . You cannot modify either local direction for these elements for a given stack orientation. Transverse shear behavior is defined in the 1–2 plane for these elements. Figure 32.5.4–7 Local directions for two-dimensional and axisymmetric cohesive elements. Local directions for three-dimensional cohesive elements The local 3-direction for three-dimensional cohesive elements corresponds to the thickness direction, which is computed as discussed above in “Element thickness direction definition” and cannot be modified for a given stack orientation. The local 1- and 2-directions are normal to the thickness direction and, by Section 1.2.2). The default local directions for a three-dimensional cohesive element are shown in Figure 32.5.4–8. COHESIVE GEOMETRY projection of x-axis onto surface Figure 32.5.4–8 Local directions for three-dimensional cohesive elements. Transverse shear behavior is defined in the local 1–3 and 2–3 planes for these elements. You can modify the local 1- and 2-directions for three-dimensional cohesive elements in the plane normal to the thickness direction by using a local orientation definition (“Orientations,” Section 2.2.5). Input File Usage: Abaqus/CAE Usage: *COHESIVE SECTION, ELSET=name, ORIENTATION=name Property module: Assign→Material Orientation: orientation select region: select 32.5.5 DEFINING THE CONSTITUTIVE RESPONSE OF COHESIVE ELEMENTS USING A CONTINUUM APPROACH Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Cohesive elements: overview,” Section 32.5.1 • “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6 • “Progressive damage and failure,” Section 24.1.1 • *COHESIVE SECTION • *TRANSVERSE SHEAR STIFFNESS • Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Manual Overview The features described in this section are used to model cohesive elements using a continuum approach, which assumes that the cohesive zone contains material of finite thickness that can be modeled using the conventional material models in Abaqus. If the cohesive zone is very thin and for all practical purposes may be considered to be of zero thickness, the constitutive response is commonly described in terms of a traction-separation law; this alternative approach is discussed in “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6. The constitutive response of cohesive elements modeled as a continuum: • can be defined in terms of macroscopic material properties such as stiffness and strength using conventional material models; • can be specified in terms of either a built-in material model or a user-defined material model; • can include the effects of material damage and failure in Abaqus/Explicit; and • can also include the effects of material damage and failure in a low-cycle fatigue analysis in Abaqus/Standard. Behavior of cohesive elements with conventional material models The implementation of the conventional material models (including user-defined models) in Abaqus for cohesive elements is based on certain assumptions regarding the state of the deformation in the cohesive layer. Two different classes of problems are considered: modeling of an adhesive layer of finite thickness and modeling of gaskets. Modeling of damage with cohesive elements for these classes of problems can be carried out only in Abaqus/Explicit . You may need to alter the damage model for an adhesive material to account for the fact that the failure of an adhesive bond may occur at the interface between the adhesive and the adherend rather than within the adhesive material. When used with conventional material models in Abaqus, cohesive elements use true stress and strain measures. When used with a material model that is based on a traction-separation description , cohesive elements use nominal stress and strain measures. The frequency characteristics of cohesive elements are accounted for by the algorithms to automatically choose the time increment (“Explicit dynamic analysis,” Section 6.3.3). In many applications involving adhesives or gaskets cohesive elements may be quite thin compared to the other elements, which tends to decrease the stable time increment. See “Stable time increment in Abaqus/Explicit” in “Modeling with cohesive elements,” Section 32.5.3, for further discussion on this topic, including suggestions on how to avoid significant reductions in the stable time increment when using cohesive elements. in Abaqus/Explicit Modeling of an adhesive layer of finite thickness For adhesive layers with finite thickness it is assumed that the cohesive layer is subjected to only one direct component of strain, which is the through-thickness strain, and to two transverse shear strain components (one transverse shear strain component for two-dimensional problems). The other two direct components of the strain (the direct membrane strains) and the in-plane (membrane) shear strain are assumed to be zero for the constitutive calculations. More specifically, the through-thickness and the transverse shear strains are computed from the element kinematics. However, the membrane strains are not computed based on the element kinematics; they are simply assumed to be zero for the constitutive calculations. These assumptions are appropriate in situations where a relatively thin and compliant layer of adhesive bonds two relatively rigid (compared to the adhesive) parts. The above kinematic assumptions are approximately correct everywhere inside the cohesive layer except around its outer edges. An additional linear elastic transverse shear behavior can be defined to provide more stability to cohesive elements, particularly after damage has occurred. The transverse shear behavior is assumed to be independent of the regular material response and does not undergo any damage. Input File Usage: Abaqus/CAE Usage: Use the following options (the second option is needed only to define uncoupled transverse shear response): *COHESIVE SECTION, RESPONSE=CONTINUUM *TRANSVERSE SHEAR STIFFNESS Property module: Create Section: select Other as the section Category and Cohesive as the section Type: Response: Continuum Transverse shear behavior is not supported in Abaqus/CAE for cohesive sections. Modeling of gaskets and/or small adhesive patches The modeling of gaskets and/or small adhesive patches involves situations where there are no lateral constraints on the cohesive layer. Hence, the layers are free to expand in the lateral direction in a stress- free manner. Application areas include individual spot welds and gaskets. The constitutive calculations assume only one direct stress component, which is the through-thickness normal stress. All other stress components, including the transverse shear stress components, are assumed to be zero. The gasket modeling capability that is offered with this option has some advantages compared to the family of gasket elements in Abaqus/Standard. The cohesive elements are fully nonlinear (the element kinematics properly account for finite strains as well as finite rotations), can contribute mass and damping in a dynamic analysis, and are available in Abaqus/Explicit. The gasket response modeled in the above manner is similar to modeling using the special-purpose gasket elements in Abaqus/Standard with thickness-direction behavior only . Uncoupled, linear-elastic transverse shear behavior, if desired, can be defined. The transverse shear behavior may either define the response of the gasket and/or adhesive patch or provide stability after damage has occurred in the response in the thickness direction. There is no damage associated with the transverse shear response. Input File Usage: Use the following options (the second option is needed only to define uncoupled transverse shear response): *COHESIVE SECTION, RESPONSE=GASKET *TRANSVERSE SHEAR STIFFNESS Property module: Create Section: select Other as the section Category and Cohesive as the section Type: Response: Gasket Transverse shear behavior is not supported in Abaqus/CAE for cohesive sections. Abaqus/CAE Usage: Output All standard output variables in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2) are available for cohesive elements that are used with conventional material models. The stresses due to the additional transverse shear response are reported separately using the output variables TSHR13 and (in three dimensions) TSHR23. These stresses are not added to the usual material point stresses reported using the output variable S. 32.5.6 DEFINING THE CONSTITUTIVE RESPONSE OF COHESIVE ELEMENTS USING A TRACTION-SEPARATION DESCRIPTION Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Cohesive elements: overview,” Section 32.5.1 • “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5 • *COHESIVE SECTION • *DAMAGE EVOLUTION • *DAMAGE INITIATION • “Defining damage,” Section 12.9.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual • Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Manual Overview The features described in this section are primarily intended for bonded interfaces where the interface thickness is negligibly small. In such cases it may be straightforward to define the constitutive response of the cohesive layer directly in terms of traction versus separation. If the interface adhesive layer has a finite thickness and macroscopic properties (such as stiffness and strength) of the adhesive material are available, it may be more appropriate to model the response using conventional material models. The former approach is discussed in this section, while the latter approach is discussed in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5. Cohesive behavior defined directly in terms of a traction-separation law: • can be used to model the delamination at interfaces in composites directly in terms of traction versus separation; • allows specification of material data such as the fracture energy as a function of the ratio of normal to shear deformation (mode mix) at the interface; • assumes a linear elastic traction-separation law prior to damage; • can be used in combination with linear viscoelasticity in Abaqus/Explicit (“Defining viscoelastic behavior for traction-separation elasticity in Abaqus/Explicit” in “Time domain viscoelasticity,” Section 22.7.1) to describe rate-dependent delamination behavior; • assumes that failure of the elements is characterized by progressive degradation of the material stiffness, which is driven by a damage process; • allows multiple damage mechanisms; and • can be used with user subroutine UMAT in Abaqus/Standard or VUMAT in Abaqus/Explicit to specify user-defined traction-separation laws. Defining constitutive response in terms of traction-separation laws To define the constitutive response of the cohesive element directly in terms of traction versus separation, you choose a traction-separation response when defining the section behavior of the cohesive elements. Input File Usage: Abaqus/CAE Usage: *COHESIVE SECTION, RESPONSE=TRACTION SEPARATION Property module: Create Section: select Other as the section Category and Cohesive as the section Type: Response: Traction Separation Linear elastic traction-separation behavior The available traction-separation model in Abaqus assumes initially linear elastic behavior followed by the initiation and evolution of damage. The elastic behavior is written in terms of an elastic constitutive matrix that relates the nominal stresses to the nominal strains across the interface. The nominal stresses are the force components divided by the original area at each integration point, while the nominal strains are the separations divided by the original thickness at each integration point. The default value of the original constitutive thickness is 1.0 if traction-separation response is specified, which ensures that the nominal strain is equal to the separation (i.e., relative displacements of the top and bottom faces). The constitutive thickness used for traction-separation response is typically different from the geometric thickness (which is typically close or equal to zero). See “Specifying the constitutive thickness” in “Defining the cohesive element’s initial geometry,” Section 32.5.4, for a discussion on how to modify the constitutive thickness. The nominal traction stress vector, , , consists of three components (two components in two-dimensional problems): , which represent the normal (along the local 3-direction in three dimensions and along the local 2-direction in two dimensions) and the two shear tractions (along the local 1- and 2-directions in three dimensions and along the local 1-direction in two dimensions), respectively. The corresponding separations are denoted by , and the original thickness of the cohesive element, the nominal strains can be defined as , and (in three-dimensional problems) . Denoting by , The elastic behavior can then be written as The elasticity matrix provides fully coupled behavior between all components of the traction vector and separation vector and can depend on temperature and/or field variables. Set the off-diagonal terms in the elasticity matrix to zero if uncoupled behavior between the normal and shear components is desired. Input File Usage: Use the following option to define uncoupled traction-separation behavior: *ELASTIC, TYPE=TRACTION Use the following option to define coupled traction-separation behavior: Abaqus/CAE Usage: *ELASTIC, TYPE=COUPLED TRACTION Use the following option to define uncoupled traction-separation behavior: Property module: material editor: Mechanical→Elasticity→Elastic: Type: Traction Use the following option to define coupled traction-separation behavior: Property module: material editor: Mechanical→Elasticity→Elastic: Type: Coupled Traction Interpretation of material properties The material parameters, such as the interfacial elastic stiffness, for a traction-separation model can be better understood by studying the equation that represents the displacement of a truss of length L, elastic stiffness E, and original area A, due to an axial load P: This equation can be rewritten as where displacement. Likewise, the total mass of the truss, assuming a density , is given by is the nominal stress and is the stiffness that relates the nominal stress to the The above equations suggest that the actual length L may be replaced with 1.0 (to ensure that the strain is the same as the displacement) if the stiffness and the density are appropriately reinterpreted. In particular, the stiffness is , where the true length of the truss is used in these equations. The density represents mass per unit area instead of mass per unit volume. and the density is and density These ideas can be carried over to a cohesive layer of initial thickness . If the adhesive material has stiffness , the stiffness of the interface (relating the nominal traction to the displacement) is given by . As discussed earlier, and the density of the interface is given by the default choice of the constitutive thickness for modeling the response in terms of traction versus separation is 1.0 regardless of the actual thickness of the cohesive layer. With this choice, the nominal strains are equal to the corresponding separations. When the constitutive thickness of the cohesive layer is “artificially” set to 1.0, ideally you should specify (if needed) as the material stiffness and density, respectively, as calculated with the true thickness of the cohesive layer. and , tends to infinity and the density, The above formulae provide a recipe for estimating the parameters required for modeling the traction-separation behavior of an interface in terms of the material properties of the bulk adhesive material. As the thickness of the interface layer tends to zero, the above equations imply that the stiffness, , tends to zero. This stiffness is often chosen as a penalty parameter. A very large penalty stiffness is detrimental to the stable time increment in Abaqus/Explicit and may result in ill-conditioning of the element operator in Abaqus/Standard. Recommendations for the choice of the stiffness and density of an interface for an Abaqus/Explicit analysis such that the stable time increment is not adversely affected are provided in “Stable time increment in Abaqus/Explicit” in “Modeling with cohesive elements,” Section 32.5.3. Modeling rate-dependent traction-separation behavior in Abaqus/Explicit Time domain viscoelasticity can be used in Abaqus/Explicit to model rate-dependent behavior of cohesive elements with traction-separation elasticity. The evolution equation for the normal and two shear nominal tractions take the form: , , and are the instantaneous nominal tractions at time t in the normal and the two where local shear directions, respectively. The functions represent the dimensionless shear and normal relaxation moduli, respectively. See “Defining viscoelastic behavior for traction-separation elasticity in Abaqus/Explicit” in “Time domain viscoelasticity,” Section 22.7.1, for additional details and usage information. and You can also combine time domain viscoelasticity with the models for progressive damage and failure described in the next sections. This combination allows modeling rate-dependent behavior both during the initial elastic response (prior to damage initiation), as well as during damage progression. Damage modeling Both Abaqus/Standard and Abaqus/Explicit allow modeling of progressive damage and failure in cohesive layers whose response is defined in terms of traction-separation. By comparison, only Abaqus/Explicit allows modeling of progressive damage and failure for cohesive elements modeled with conventional materials (“Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5). Damage of the traction-separation response is defined within the same general framework used for conventional materials . This general framework allows the combination of several damage mechanisms acting simultaneously on the same material. Each failure mechanism consists of three ingredients: a damage initiation criterion, a damage evolution law, and a choice of element removal (or deletion) upon reaching a completely damaged state. While this general framework is the same for traction-separation response and conventional materials, many details of how the various ingredients are defined are different. Therefore, the details of damage modeling for traction-separation response are presented below. The initial response of the cohesive element is assumed to be linear as discussed above. However, once a damage initiation criterion is met, material damage can occur according to a user-defined damage evolution law. Figure 32.5.6–1 shows a typical traction-separation response with a failure mechanism. If the damage initiation criterion is specified without a corresponding damage evolution model, Abaqus will evaluate the damage initiation criterion for output purposes only; there is no effect on the response of the cohesive element (i.e., no damage will occur). The cohesive layer does not undergo damage under pure compression. traction t (t , t ) n s t δ (δ ,δ ) δ (δ ,δ ) separation Figure 32.5.6–1 Typical traction-separation response. Damage initiation As the name implies, damage initiation refers to the beginning of degradation of the response of a material point. The process of degradation begins when the stresses and/or strains satisfy certain damage initiation criteria that you specify. Several damage initiation criteria are available and are discussed below. Each damage initiation criterion also has an output variable associated with it to indicate whether the criterion is met. A value of 1 or higher indicates that the initiation criterion has been met . Damage initiation criteria that do not have an associated evolution law affect only output. Thus, you can use these criteria to evaluate the propensity of the material to undergo damage without actually modeling the damage process (i.e., without actually specifying damage evolution). , , , and , and In the discussion below, represent the peak values of the nominal stress when the deformation is either purely normal to the interface or purely in the first or the second shear direction, respectively. Likewise, represent the peak values of the nominal strain when the deformation is either purely normal to the interface or purely in the first or the second shear direction, respectively. With the initial constitutive thickness , the nominal strain components are equal to the respective components of the relative displacement— , , and —between the top and bottom of the cohesive layer. The symbol used in the discussion below represents the Macaulay bracket with the usual interpretation. The Macaulay brackets are used to signify that a pure compressive deformation or stress state does not initiate damage. Maximum nominal stress criterion Damage is assumed to initiate when the maximum nominal stress ratio (as defined in the expression below) reaches a value of one. This criterion can be represented as Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=MAXS Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Maxs Damage Maximum nominal strain criterion Damage is assumed to initiate when the maximum nominal strain ratio (as defined in the expression below) reaches a value of one. This criterion can be represented as Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=MAXE Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Maxe Damage Quadratic nominal stress criterion Damage is assumed to initiate when a quadratic interaction function involving the nominal stress ratios (as defined in the expression below) reaches a value of one. This criterion can be represented as Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=QUADS Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quads Damage Quadratic nominal strain criterion Damage is assumed to initiate when a quadratic interaction function involving the nominal strain ratios (as defined in the expression below) reaches a value of one. This criterion can be represented as Input File Usage: Abaqus/CAE Usage: *DAMAGE INITIATION, CRITERION=QUADE Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quade Damage Damage evolution The damage evolution law describes the rate at which the material stiffness is degraded once the corresponding initiation criterion is reached. The general framework for describing the evolution of damage in bulk materials (as opposed to interfaces modeled using cohesive elements) is described in “Damage evolution and element removal for ductile metals,” Section 24.2.3. Conceptually, similar ideas apply for describing damage evolution in cohesive elements with a constitutive response that is described in terms of traction versus separation; however, many details are different. A scalar damage variable, D, represents the overall damage in the material and captures the combined effects of all the active mechanisms. It initially has a value of 0. If damage evolution is modeled, D monotonically evolves from 0 to 1 upon further loading after the initiation of damage. The stress components of the traction-separation model are affected by the damage according to otherwise (no damage to compressive stiffness); , where current strains without damage. and are the stress components predicted by the elastic traction-separation behavior for the To describe the evolution of damage under a combination of normal and shear deformation across the interface, it is useful to introduce an effective displacement (Camanho and Davila, 2002) defined as Mixed-mode definition The mode mix of the deformation fields in the cohesive zone quantify the relative proportions of normal and shear deformation. Abaqus uses two measures of mode mix, one based on energies and the other based on tractions. You can choose one of these measures when you specify the mode dependence of the damage evolution process. Denoting by the work done by the tractions and their conjugate relative displacements in the normal, first, and second shear directions, respectively, and defining , the mode-mix definitions based on energies are as follows: , and , Clearly, only two of the three quantities defined above are independent. It is also useful to define the quantity to denote the portion of the total work done by the shear traction and the corresponding relative displacement components. As discussed later, Abaqus requires that you specify material properties related to damage evolution as functions of (or, equivalently, ) and . The corresponding definitions of the mode mix based on traction components are given by where definition (before they are normalized by the factor is a measure of the effective shear traction. The angular measures used in the above ) are illustrated in Figure 32.5.6–2. The mode-mix ratios defined in terms of energies and tractions can be quite different in general. The following example illustrates this point. In terms of energies a deformation in the purely normal direction is one for which , irrespective of the values of the normal and the shear tractions. In particular, for a material with coupled traction-separation behavior both the normal and shear tractions may be nonzero for a deformation in the purely normal direction. For this case the definition of mode mix based on energies would indicate a purely normal deformation, while the definition based on tractions would suggest a mix of both normal and shear deformation. and There are two components to the definition of the evolution of damage. The first component involves specifying either the effective displacement at complete failure, , relative to the effective displacement at the initiation of damage, . The ; or the energy dissipated due to failure, second component to the definition of damage evolution is the specification of the nature of the evolution t~ normal t n t t Shear 2 t s Shear 1 traction Figure 32.5.6–2 Mode mix measures based on traction. δ o δ f separation Figure 32.5.6–3 Linear damage evolution. of the damage variable, D, between initiation of damage and final failure. This can be done by either defining linear or exponential softening laws or specifying D directly as a tabular function of the effective displacement relative to the effective displacement at damage initiation. The material data described above will in general be functions of the mode mix, temperature, and/or field variables. Figure 32.5.6–4 is a schematic representation of the dependence of damage initiation and evolution on the mode mix, for a traction-separation response with isotropic shear behavior. Figure 32.5.6–4 Illustration of mixed-mode response in cohesive elements. The figure shows the traction on the vertical axis and the magnitudes of the normal and the shear separations along the two horizontal axes. The unshaded triangles in the two vertical coordinate planes represent the response under pure normal and pure shear deformation, respectively. All intermediate vertical planes (that contain the vertical axis) represent the damage response under mixed mode conditions with different mode mixes. The dependence of the damage evolution data on the mode mix can be defined either in tabular form or, in the case of an energy-based definition, analytically. The manner in which the damage evolution data are specified as a function of the mode mix is discussed later in this section. Unloading subsequent to damage initiation is always assumed to occur linearly toward the origin of the traction-separation plane, as shown in Figure 32.5.6–3. Reloading subsequent to unloading also occurs along the same linear path until the softening envelope (line AB) is reached. Once the softening envelope is reached, further reloading follows this envelope as indicated by the arrow in Figure 32.5.6–3. Input File Usage: Use the following option to use the mode-mix definition based on energies: Abaqus/CAE Usage: *DAMAGE EVOLUTION, MODE MIX RATIO=ENERGY Use the following option to use the mode-mix definition based on tractions: *DAMAGE EVOLUTION, MODE MIX RATIO=TRACTION Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Suboptions→Damage Evolution: Mode mix ratio: Energy or Traction Evolution based on effective displacement (i.e., the effective displacement at complete failure, , relative to You specify the quantity the effective displacement at damage initiation, , as shown in Figure 32.5.6–3) as a tabular function of the mode mix, temperature, and/or field variables. In addition, you also choose either a linear or an exponential softening law that defines the detailed evolution (between initiation and complete failure) of the damage variable, D, as a function of the effective displacement beyond damage initiation. Alternatively, instead of using linear or exponential softening, you can specify the damage variable, D, directly as a tabular function of the effective displacement after the initiation of damage, ; mode mix; temperature; and/or field variables. Linear damage evolution For linear softening Abaqus uses an evolution of the damage variable, D, that reduces (in the case of damage evolution under a constant mode mix, temperature, and field variables) to the expression proposed by Camanho and Davila (2002), namely: In the preceding expression and in all later references, refers to the maximum value of the effective displacement attained during the loading history. The assumption of a constant mode mix at a material point between initiation of damage and final failure is customary for problems involving monotonic damage (or monotonic fracture). Input File Usage: Use the following option to specify linear damage evolution: Abaqus/CAE Usage: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=LINEAR Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Suboptions→Damage Evolution: Type: Displacement: Softening: Linear Exponential damage evolution For exponential softening Abaqus uses an evolution of the damage variable, D, that reduces (in the case of damage evolution under a constant mode mix, temperature, and field variables) to In the expression above evolution and is the exponential function. is a non-dimensional material parameter that defines the rate of damage traction δ o δ f separation Figure 32.5.6–5 Exponential damage evolution. Input File Usage: Abaqus/CAE Usage: Use the following option to specify exponential softening: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=EXPONENTIAL Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Suboptions→Damage Evolution: Type: Displacement: Softening: Exponential Tabular damage evolution For tabular softening you define the evolution of D directly in tabular form. D must be specified as a function of the effective displacement relative to the effective displacement at initiation, mode mix, temperature, and/or field variables. Input File Usage: Use the following option to define the damage variable directly in tabular form: Abaqus/CAE Usage: *DAMAGE EVOLUTION, TYPE=DISPLACEMENT, SOFTENING=TABULAR Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Suboptions→Damage Evolution: Type: Displacement: Softening: Tabular Evolution based on energy Damage evolution can be defined based on the energy that is dissipated as a result of the damage process, also called the fracture energy. The fracture energy is equal to the area under the traction-separation curve . You specify the fracture energy as a material property and choose either a linear or an exponential softening behavior. Abaqus ensures that the area under the linear or the exponential damaged response is equal to the fracture energy. The dependence of the fracture energy on the mode mix can be specified either directly in tabular form or by using analytical forms as described below. When the analytical forms are used, the mode-mix ratio is assumed to be defined in terms of energies. Tabular form The simplest way to define the dependence of the fracture energy is to specify it directly as a function of the mode mix in tabular form. Input File Usage: Use the following option to specify fracture energy as a function of the mode mix in tabular form: *DAMAGE EVOLUTION, TYPE=ENERGY, MIXED MODE BEHAVIOR=TABULAR Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Suboptions→Damage Evolution: Type: Energy: Mixed mode behavior: Tabular Power law form The dependence of the fracture energy on the mode mix can be defined based on a power law fracture criterion. The power law criterion states that failure under mixed-mode conditions is governed by a power law interaction of the energies required to cause failure in the individual (normal and two shear) modes. It is given by The mixed-mode fracture energy when the above condition is satisfied. In other words, You specify the quantities failure in the normal, the first, and the second shear directions, respectively. , and , , which refer to the critical fracture energies required to cause Input File Usage: Abaqus/CAE Usage: Use the following option to define the fracture energy as a function of the mode mix using the analytical power law fracture criterion: *DAMAGE EVOLUTION, TYPE=ENERGY, MIXED MODE BEHAVIOR=POWER LAW, POWER= Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Suboptions→Damage Evolution: Type: Energy: Mixed mode behavior: Power Law: Toggle on Power and enter the exponent value Benzeggagh-Kenane (BK) form The Benzeggagh-Kenane fracture criterion (Benzeggagh and Kenane, 1996) is particularly useful when the critical fracture energies during deformation purely along the first and the second shear directions are the same; i.e., . It is given by where , , and is a material parameter. You specify , , and . Input File Usage: Abaqus/CAE Usage: Use the following option to define the fracture energy as a function of the mode mix using the analytical BK fracture criterion: *DAMAGE EVOLUTION, TYPE=ENERGY, MIXED MODE BEHAVIOR=BK, POWER= Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Suboptions→Damage Evolution: Type: Energy: Mixed mode behavior: Bk: Toggle on Power and enter the exponent value Linear damage evolution For linear softening Abaqus uses an evolution of the damage variable, D, that reduces to where as the effective traction at damage initiation. maximum value of the effective displacement attained during the loading history. with refers to the Input File Usage: Use the following option to specify linear damage evolution: Abaqus/CAE Usage: *DAMAGE EVOLUTION, TYPE=ENERGY, SOFTENING=LINEAR Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Suboptions→Damage Evolution: Type: Energy: Softening: Linear Exponential damage evolution For exponential softening Abaqus uses an evolution of the damage variable, D, that reduces to In the expression above is the elastic energy at damage initiation. In this case the traction might not drop immediately after damage initiation, which is different from what is seen in Figure 32.5.6–5. are the effective traction and displacement, respectively. and Input File Usage: Use the following option to specify exponential softening: *DAMAGE EVOLUTION, TYPE=ENERGY, SOFTENING=EXPONENTIAL Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Traction- Separation Laws→Quade Damage, Maxe Damage, Quads Damage, or Maxs Damage: Suboptions→Damage Evolution: Type: Energy: Softening: Exponential Defining damage evolution data as a tabular function of mode mix As discussed earlier, the material data defining the evolution of damage can be tabular functions of the mode mix. The manner in which this dependence must be defined in Abaqus is outlined below for mode- mix definitions based on energy and traction, respectively. In the following discussion it is assumed that the evolution is defined in terms of energy. Similar observations can also be made for evolution definitions based on effective displacement. Mode mix based on energy For an energy-based definition of mode mix, in the most general case of a three-dimensional state of deformation with anisotropic shear behavior the fracture energy, , must be defined as a function of is a measure of the fraction of the total deformation that is shear, while is a measure of the fraction of the total shear deformation that is in the second shear direction. Figure 32.5.6–6 shows a schematic of the fracture energy versus mode mix behavior. . The quantity and Modes n-s Modes s-t Modes n-t m + m = ( 2 3 G s G T ( 1.0 1.0 Figure 32.5.6–6 Fracture energy as a function of mode mix. m 3 m + m = ( 2 3 ( G t GS , The limiting cases of pure normal and pure shear deformations in the first and second shear directions are denoted in Figure 32.5.6–6 by , respectively. The lines labeled “Modes n-s,” “Modes n-t,” and “Modes s-t” show the transition in behavior between the pure normal and the pure shear in the first direction, pure normal and pure shear in the second direction, and pure shears in the first and second directions, respectively. In general, at various fixed values of versus as a “data block.” The following guidelines are . In the discussion that follows we refer to a data set of must be specified as a function of corresponding to a fixed , and useful in defining the fracture energy as a function of the mode mix: • For a two-dimensional problem only. The data column corresponding to only one “data block” is needed. needs to be defined as a function of in this case) must be left blank. Hence, essentially ( • For a three-dimensional problem with isotropic shear response, the shear behavior is defined by the . Therefore, in this case a single ) also suffices to define the fracture energy and not by the individual values of and sum “data block” (the “data block” for as a function of the mode mix. • In the most general case of three-dimensional problems with anisotropic shear behavior, several versus can vary between “data blocks” would be needed. As discussed earlier, each “data block” would contain . In each “data block” at a fixed value of . The case (the first data point in any “data block”), which corresponds to 0 and a purely normal mode, can never be achieved when (i.e., the only valid point on line OB in Figure 32.5.6–6 is the point O, which corresponds to a purely normal deformation). However, in the tabular definition of the fracture energy as a function of mode mix, this point simply serves to set a limit that ensures a continuous change in fracture energy as a purely normal state is approached from various combinations of normal and shear deformations. Hence, the fracture energy of the first data point in each “data block” must always be set equal to the fracture energy in a purely normal mode of deformation ( ). As an example of the anisotropic shear case, consider that you want to input three “data blocks” corresponding to fixed values of 0., 0.2, and 1.0, respectively. For each of the three “data blocks,” the first data point must be for the reasons discussed above. The rest of the data points in each “data block” define the variation of the fracture energy with increasing proportions of shear deformation. Mode mix based on traction needs to The fracture energy needs to be specified in tabular form of be specified as a function of . A “data block” in this case corresponds to a set of data for may vary from 0 (purely normal deformation) to 1 (purely shear deformation). An important restriction is that each data block must specify the same value of the fracture energy for . This restriction ensures that the energy required for fracture as the traction vector approaches the normal direction does not depend on the orientation of the projection of the traction vector on the shear plane . at various fixed values of , at a fixed value of . In each “data block” . Thus, versus versus and Evaluating damage when multiple criteria are active When multiple damage initiation criteria and associated evolution definitions are used for the same material, each evolution definition results in its own damage variable, , where the subscript i represents the ith damage system. The overall damage variable, D, is computed based on the individual as explained in “Evaluating overall damage when multiple criteria are active” in “Damage evolution and element removal for ductile metals,” Section 24.2.3, for damage in bulk materials. Maximum degradation and choice of element removal You have control over how Abaqus treats cohesive elements with severe damage. By default, the upper bound to the overall damage variable at a material point is . You can reduce this upper bound as discussed in “Controlling element deletion and maximum degradation for materials with damage evolution” in “Section controls,” Section 27.1.4. You can control what happens to the cohesive element when the damage reaches this limit, as discussed below. By default, once the overall damage variable reaches at all of its material points and none of its material points are in compression, the cohesive elements, except for the pore pressure cohesive elements, are removed (deleted). See “Controlling element deletion and maximum degradation for materials with damage evolution” in “Section controls,” Section 27.1.4, for details. This element removal approach is often appropriate for modeling complete fracture of the bond and separation of components. Once removed, cohesive elements offer no resistance to subsequent penetration of the components, so it may be necessary to model contact between the components as discussed in “Defining contact between surrounding components” in “Modeling with cohesive elements,” Section 32.5.3. Alternatively, you can specify that a cohesive element should remain in the model even after the overall damage variable reaches . In this case the stiffness of the element in tension and/or shear remains constant (degraded by a factor of 1 − over the initial undamaged stiffness). This choice is appropriate if the cohesive elements must resist interpenetration of the surrounding components even after they have completely degraded in tension and/or shear . In Abaqus/Explicit it is recommended that you suppress bulk viscosity in the cohesive elements by setting the scale factors for the linear and quadratic bulk viscosity parameters to zero using section controls . Uncoupled transverse shear response An optional linear elastic transverse shear behavior can be defined to provide additional stability to cohesive elements, particularly after damage has occurred. The transverse shear behavior is assumed to be independent of the regular material response and does not undergo any damage. Input File Usage: Abaqus/CAE Usage: Use the following options: *COHESIVE SECTION, RESPONSE=TRACTION SEPARATION *TRANSVERSE SHEAR STIFFNESS Transverse shear behavior is not supported in Abaqus/CAE for cohesive sections. Viscous regularization in Abaqus/Standard Material models exhibiting softening behavior and stiffness degradation often lead to severe convergence difficulties in implicit analysis programs, such as Abaqus/Standard. A common technique to overcome some of these convergence difficulties is the use of viscous regularization of the constitutive equations, which causes the tangent stiffness matrix of the softening material to be positive for sufficiently small time increments. The traction-separation laws can be regularized in Abaqus/Standard using viscosity by permitting stresses to be outside the limits set by the traction-separation law. The regularization process involves the use of a viscous stiffness degradation variable, , which is defined by the evolution equation: where is the viscosity parameter representing the relaxation time of the viscous system and D is the degradation variable evaluated in the inviscid backbone model. The damaged response of the viscous material is given as Using viscous regularization with a small value of the viscosity parameter (small compared to the characteristic time increment) usually helps improve the rate of convergence of the model in the softening regime, without compromising results. The basic idea is that the solution of the viscous system relaxes to that of the inviscid case as , where t represents time. You can specify the value of the viscosity parameter as part of the section controls definition . If the viscosity parameter is different from zero, output results of the stiffness degradation refer to the viscous value, . The default value of the viscosity parameter is zero so that no viscous regularization is performed. Use of viscous regularization for improving the convergence behavior of delamination and debonding problems is discussed in “Delamination analysis of laminated composites,” Section 2.7.1 of the Abaqus Benchmarks Manual, and “Analysis of skin-stiffener debonding under tension,” Section 1.4.5 of the Abaqus Example Problems Manual. The approximate amount of energy associated with viscous regularization over the whole model or over an element set is available using output variable ALLCD. Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for cohesive elements with traction-separation behavior: STATUS SDEG DMICRT MAXSCRT MAXECRT QUADSCRT QUADECRT ALLCD Status of element (the status of an element is 1.0 if the element is active, 0.0 if the element is not). Overall value of the scalar damage variable, D. All damage initiation criteria components. Maximum value of the nominal stress damage initiation criterion at a material point during the analysis. It is evaluated as Maximum value of the nominal strain damage initiation criterion at a material point during the analysis. It is evaluated as Maximum value of the quadratic nominal stress damage initiation criterion at a material point during the analysis. It is evaluated as Maximum value of the quadratic nominal strain damage initiation criterion at a material point during the analysis. It is evaluated as The approximate amount of energy over the whole model or over an element set that is associated with viscous regularization in Abaqus/Standard. Corresponding output variables (such as CENER, ELCD, and ECDDEN) represent the energy associated with viscous regularization at the integration point level and element level (the last quantity represents the energy per unit volume in the element), respectively. For the variables above that indicate whether a certain damage initiation criterion has been satisfied or not, a value that is less than 1.0 indicates that the criterion has not been satisfied, while a value of 1.0 or higher indicates that the criterion has been satisfied. If damage evolution is specified for this criterion, the maximum value of this variable does not exceed 1.0. However, if damage evolution is not specified for the initiation criterion, this variable can have values higher than 1.0. The extent to which the variable is higher than 1.0 may be considered to be a measure of the extent to which this criterion has been violated. Additional references • Benzeggagh, M. L., and M. Kenane, “Measurement of Mixed-Mode Delamination Fracture Toughness of Unidirectional Glass/Epoxy Composites with Mixed-Mode Bending Apparatus,” Composites Science and Technology, vol. 56, pp. 439–449, 1996. • Camanho, P. P., and C. G. Davila, “Mixed-Mode Decohesion Finite Elements for the Simulation of Delamination in Composite Materials,” NASA/TM-2002–211737, pp. 1–37, 2002. 32.5.7 DEFINING THE CONSTITUTIVE RESPONSE OF FLUID WITHIN THE COHESIVE ELEMENT GAP Products: Abaqus/Standard Abaqus/CAE References • “Cohesive elements: overview,” Section 32.5.1 • “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6 • *FLUID LEAKOFF • *GAP FLOW • Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Manual Overview The cohesive element fluid flow model: • is typically used in geotechnical applications, where fluid flow continuity within the gap and through the interface must be maintained; • enables fluid pressure on the cohesive element surface to contribute to its mechanical behavior, which enables the modeling of hydraulically driven fracture; • enables modeling of an additional resistance layer on the surface of the cohesive element; and • can be used only in conjunction with traction-separation behavior. The features described in this section are used to model fluid flow within and across surfaces of pore pressure cohesive elements. Defining pore fluid flow properties The fluid constitutive response comprises: • Tangential flow within the gap, which can be modeled with either a Newtonian or power law model; and • Normal flow across the gap, which can reflect resistance due to caking or fouling effects. The flow patterns of the pore fluid in the element are shown in Figure 32.5.7–1. The fluid is assumed to be incompressible, and the formulation is based on a statement of flow continuity that considers tangential and normal flow and the rate of opening of the cohesive element. Specifying the fluid flow properties You can assign tangential and normal flow properties separately. cohesive elements tangential flow normal flow Figure 32.5.7–1 Flow within cohesive elements. Tangential flow By default, there is no tangential flow of pore fluid within the cohesive element. To allow tangential flow, define a gap flow property in conjunction with the pore fluid material definition. Newtonian fluid In the case of a Newtonian fluid the volume flow rate density vector is given by the expression is the tangential permeability (the resistance to the fluid flow), is the pressure gradient along where the cohesive element, and In Abaqus the gap opening, is the gap opening. , is defined as where and and are the current and original cohesive element geometrical thicknesses, respectively; is the initial gap opening, which has a default value of 0.002. Abaqus defines the tangential permeability, or the resistance to flow, according to Reynold’s equation: is the fluid viscosity and is the gap opening. You can also specify an upper limit on the value where of . Input File Usage: Abaqus/CAE Usage: Use the following option to define the initial gap opening directly: *SECTION CONTROLS, INITIAL GAP OPENING Use the following option to define the tangential flow in a Newtonian fluid: *GAP FLOW, TYPE=NEWTONIAN, KMAX Initial gap opening is not supported in Abaqus/CAE. Property module: material editor: Other→Pore Fluid→Gap Flow: Type: Newtonian: Toggle on Maximum Permeability and enter the value of Power law fluid In the case of a power law fluid the constitutive relation is defined as is the shear stress, where coefficient. Abaqus defines the tangential volume flow rate density as is the shear strain rate, is the fluid consistency, and is the power law where is the gap opening. Input File Usage: Abaqus/CAE Usage: *GAP FLOW, TYPE=POWER LAW Property module: material editor: Other→Pore Fluid→Gap Flow: Type: Power law Normal flow across gap surfaces You can permit normal flow by defining a fluid leakoff coefficient for the pore fluid material. This coefficient defines a pressure-flow relationship between the cohesive element’s middle nodes and their adjacent surface nodes. The fluid leakoff coefficients can be interpreted as the permeability of a finite layer of material on the cohesive element surfaces, as shown in Figure 32.5.7–2. The normal flow is defined as and where and pressure; and are the flow rates into the top and bottom surfaces, respectively; and are the pore pressures on the top and bottom surfaces, respectively. is the midface Input File Usage: Abaqus/CAE Usage: *FLUID LEAKOFF Property module: material editor: Other→Pore Fluid→Fluid Leakoff: Type: Coefficients Pt Pi Pb permeable layer Figure 32.5.7–2 Leakoff coefficient interpretation as a permeable layer. Defining leakoff coefficients as a function of temperature and field variables Input File Usage: You can optionally define leakoff coefficients as functions of temperature and field variables. *FLUID LEAKOFF, DEPENDENCIES Property module: material editor: Other→Pore Fluid→Fluid Leakoff: Type: Coefficients: Toggle on Use temperature-dependent data and select the number of field variables. Abaqus/CAE Usage: Defining leakoff coefficients in a user subroutine User subroutine UFLUIDLEAKOFF can also be used to define more complex leakoff behavior, including the ability to define a time accumulated resistance, or fouling, through the use of solution-dependent state variables. Input File Usage: Abaqus/CAE Usage: *FLUID LEAKOFF, USER Property module: material editor: Other→Pore Fluid→Fluid Leakoff: Type: User Tangential and normal flow combinations Table 32.5.7–1 shows the permitted combinations of tangential and normal flow and the effects of each combination. Initially open elements When the opening of the cohesive element is driven primarily by entry of fluid into the gap, you will have to define one or more elements as initially open, since tangential flow is possible only in an open element. Identify initially open elements as initial conditions. Input File Usage: Abaqus/CAE Usage: *INITIAL CONDITIONS, TYPE=INITIAL GAP Initial gap definition is not supported in Abaqus/CAE. Table 32.5.7–1 Effects of flow property definition combinations. Normal flow is defined Normal flow is undefined Tangential flow is defined Tangential and normal flow are modeled. Tangential flow is undefined Normal flow is modeled. Tangential flow is modeled. Pore pressure continuity is enforced between facing nodes in the cohesive element only when the element is closed. Otherwise, the surfaces are impermeable in the normal direction. Tangential flow is not modeled. Pore pressure continuity is always enforced between facing nodes in the cohesive element. Use of unsymmetric matrix storage and solution The pore pressure cohesive element matrices are unsymmetric; therefore, unsymmetric matrix storage and solution may be needed to improve convergence . Additional considerations Your use of cohesive element fluid properties and your property values can impact your solution in some cases. Large coefficient values You must make sure that the tangential permeability or fluid leakoff coefficients are not excessively large. If either coefficient is many orders of magnitude higher than the permeability in the adjacent continuum elements, matrix conditioning problems may occur, leading to solver singularities and unreliable results. Use in total pore pressure simulations Definition of tangential flow properties may result in inaccurate results if the total pore pressure formulation is used and the hydrostatic pressure gradient contributes significantly to the tangential flow in the gap. The total pore pressure formulation is invoked if you apply gravity distributed loads to all elements in the model. The results will be accurate if the hydrostatic pressure gradient (i.e., the gravity vector) is perpendicular to the cohesive element. Output The following output variables are available when flow is enabled in pore pressure cohesive elements: GFVR PFOPEN Gap fluid volume rate. Fracture opening. LEAKVRT Leak-off flow rate at element top. ALEAKVRT Accumulated leak-off flow volume at element top. LEAKVRB Leak-off flow rate at element bottom. ALEAKVRB Accumulated leak-off flow volume at element bottom. 32.5.8 TWO-DIMENSIONAL COHESIVE ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Cohesive elements: overview,” Section 32.5.1 • “Choosing a cohesive element,” Section 32.5.2 • *COHESIVE SECTION • Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Manual Overview This section provides a reference to the two-dimensional cohesive elements available in Abaqus/Standard and Abaqus/Explicit. Element types General element COH2D4 4-node two-dimensional cohesive element Active degrees of freedom 1, 2 Additional solution variables None. Pore pressure element COH2D4P(S) 6-node displacement and pore pressure two-dimensional cohesive element Active degrees of freedom 1, 2, 8 at nodes on the top and bottom faces 8 at nodes on the middle face Additional solution variables None. Nodal coordinates required Element property definition You can define the element’s initial constitutive thickness and the out-of-plane width. The default initial constitutive thickness of cohesive elements depends on the response of these elements. For continuum response, the default initial constitutive thickness is computed based on the nodal coordinates. For traction-separation response, the default initial constitutive thickness is assumed to be 1.0. For response based on a uniaxial stress state, there is no default; you must indicate your choice of the method for computing the initial constitutive thickness. See “Specifying the constitutive thickness” in “Defining the cohesive element’s initial geometry,” Section 32.5.4, for details. Abaqus calculates the thickness direction automatically based on the midsurface of the element. Input File Usage: Abaqus/CAE Usage: *COHESIVE SECTION Property module: Create Section: select Other as the section Category and Cohesive as the section Type Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BX BY BXNU Body force Body force Body force FL−3 FL−3 FL−3 BYNU Body force FL−3 Body force in global X-direction. Body force in global Y-direction. Nonuniform body force in global X-direction with magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user Nonuniform body force in global Y-direction with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. CENT(S) Not supported FL−4 (ML−3T−2) Centrifugal load (magnitude is input is the mass density , where is the angular as per unit volume, velocity). (*DLOAD) CENTRIF(S) 2-D COHESIVE ELEMENT LIBRARY Abaqus/CAE Load/Interaction Units Description Rotational body force T−2 Centrifugal load (magnitude is input as the angular velocity). , where is CORIO(S) Coriolis force FL−4 T (ML−3 T−1 ) GRAV Gravity Pn PnNU Pressure Not supported LT−2 FL−2 FL−2 ROTA(S) Rotational body force T−2 SBF(E) SPn(E) VBF(E) VPn(E) Not supported FL−5 T2 Not supported Not supported FL−4 T2 FL−4 T Not supported FL−3 T Coriolis force (magnitude is input is the mass density as , where per unit volume, is the angular velocity). Gravity loading direction (magnitude is acceleration). in specified input as Pressure on face n. on Nonuniform pressure with magnitude via user Abaqus/Standard Abaqus/Explicit. face supplied subroutine DLOAD in and VDLOAD in Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Stagnation body force in global X- and Y-directions. Stagnation pressure on face n. Viscous body force in global X- and Y-directions. Viscous pressure on face n, applying a pressure proportional to the velocity normal to the face and opposing the motion. Surface-based loading Distributed loads Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description PNU SP(E) VP(E) Pressure Pressure FL−2 FL−2 Pressure FL−4 T2 Pressure FL−3 T Pressure on the element surface. Nonuniform pressure on the element surface with magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user Stagnation pressure on the element surface. Viscous pressure applied on the element surface. The viscous pressure is proportional to the velocity normal to the element face and opposing the motion. Element output Stress, strain, and other tensor components available for output depend on whether the cohesive elements are used to model adhesive joints, gaskets, or delamination problems. You indicate the intended usage of the cohesive elements by choosing an appropriate response type when defining the section properties of these elements. The available response types are discussed in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5, and “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6. Cohesive elements using a continuum response Stress and other tensors (including strain tensors) are available for elements with continuum response. Both the stress tensor and the strain tensor contain true values. For the constitutive calculations using a continuum response, only the direct through-thickness and the transverse shear strains are assumed to be nonzero. All the other strain components (i.e., the membrane strains) are assumed to be zero . All tensors have the same number of components. For example, the stress components are as follows: S11 S22 S33 S12 Direct membrane stress. Direct through-thickness stress. Direct membrane stress. Transverse shear stress. Cohesive elements using a uniaxial stress state Stress and other tensors (including strain tensors) are available for cohesive elements with uniaxial stress response. Both the stress tensor and the strain tensor contain true values. For the constitutive calculations using a uniaxial stress response, only the direct through-thickness stress is assumed to be nonzero. All the other stress components (i.e., the membrane and transverse shear stresses) are assumed to be zero . All tensors have the same number of components. For example, the stress components are as follows: S22 Direct through-thickness stress. Cohesive elements using a traction-separation response Stress and other tensors (including strain tensors) are available for elements with traction-separation response. Both the stress tensor and the strain tensor contain nominal values. The output variables E, LE, and NE all contain the nominal strain when the response of cohesive elements is defined in terms of traction versus separation. All tensors have the same number of components. For example, the stress components are as follows: S22 S12 Direct through-thickness stress. Transverse shear stress. Node ordering and face numbering on elements face 3 face 4 face 2 5 face 1 4 - node element 6 - node element Element faces Face 1 Face 2 Face 3 Face 4 1 – 2 face 2 – 3 face 3 – 4 face 4 – 1 face Numbering of integration points for output 5 1 2 6 4 - node element 6 - node element 32.5.9 THREE-DIMENSIONAL COHESIVE ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Cohesive elements: overview,” Section 32.5.1 • “Choosing a cohesive element,” Section 32.5.2 • *COHESIVE SECTION • Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Manual Overview section provides a reference to the three-dimensional cohesive elements available in This Abaqus/Standard and Abaqus/Explicit. Element types General elements COH3D6 COH3D8 6-node three-dimensional cohesive element 8-node three-dimensional cohesive element Active degrees of freedom 1, 2, 3 Additional solution variables None. Pore pressure elements COH3D6P 9-node displacement and pore pressure three-dimensional cohesive element COH3D8P 12-node displacement and pore pressure three-dimensional cohesive element Active degrees of freedom 1, 2, 3, 8 at nodes on the top and bottom faces 8 at nodes on the middle face Additional solution variables None. Nodal coordinates required Element property definition You can define the element’s initial constitutive thickness. The default initial constitutive thickness of cohesive elements depends on the response of these elements. For continuum response, the default initial constitutive thickness is computed based on the nodal coordinates. For traction-separation response, the default initial constitutive thickness is assumed to be 1.0. For response based on a uniaxial stress state, there is no default; you must indicate your choice of the method for computing the initial constitutive thickness. See “Specifying the constitutive thickness” in “Defining the cohesive element’s initial geometry,” Section 32.5.4, for details. Abaqus computes the thickness direction automatically based on the midsurface of the element. Input File Usage: Abaqus/CAE Usage: *COHESIVE SECTION Property module: Create Section: select Other as the section Category and Cohesive as the section Type Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BX BY BZ BXNU Body force Body force Body force Body force FL−3 FL−3 FL−3 FL−3 BYNU Body force FL−3 BZNU Body force FL−3 Body force in global X-direction. Body force in global Y-direction. Body force in global Z-direction. user Nonuniform body force in global X-direction with magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. Nonuniform body force in global Y-direction with magnitude supplied subroutine DLOAD in user via and VDLOAD in Abaqus/Standard Abaqus/Explicit. Nonuniform body force in global Z-direction with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. Load ID (*DLOAD) Abaqus/CAE Load/Interaction CENT(S) Not supported Units Description FL−4 (ML−3T−2) Centrifugal load (magnitude is input is the mass density , where is the angular as per unit volume, velocity). Centrifugal load (magnitude is input as the angular velocity). , where is Coriolis force (magnitude is input is the mass density as , where per unit volume, is the angular velocity). Gravity loading direction (magnitude is acceleration). in specified input as Pressure on face n. on Nonuniform pressure with magnitude via user Abaqus/Standard Abaqus/Explicit. face supplied subroutine DLOAD in and VDLOAD in Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Stagnation body force in global X-, Y-, and Z-directions. Stagnation pressure on face n. Viscous body force in global X-, Y-, and Z-directions. Viscous pressure on face n, applying a pressure proportional to the velocity normal to the face and opposing the motion. CENTRIF(S) Rotational body force T−2 CORIO(S) Coriolis force FL−4 T (ML−3 T−1 ) GRAV Gravity Pn PnNU Pressure Not supported LT−2 FL−2 FL−2 ROTA(S) Rotational body force T−2 SBF(E) SPn(E) VBF(E) VPn(E) Not supported FL−5 T2 Not supported Not supported FL−4 T2 FL−4 T Not supported FL−3 T Surface-based loading Distributed loads Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description PNU SP(E) VP(E) Pressure Pressure FL−2 FL−2 Pressure Pressure FL−4 T2 FL−3 T Pressure on the element surface. Nonuniform pressure on the element surface with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. Stagnation pressure on the element surface. Viscous pressure applied on the element surface. The viscous pressure is proportional to the velocity normal to the element face and opposing the motion. Element output Stress, strain, and other tensor components available for output depend on whether the cohesive elements are used to model adhesive joints, gaskets, or delamination problems. You indicate the intended usage of the cohesive elements by choosing an appropriate response type when defining the section properties of these elements. The available response types are discussed in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5, and “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6. Cohesive elements using a continuum response Stress and other tensors (including strain tensors) are available for elements with continuum response. Both the stress tensor and the strain tensor contain true values. For the constitutive calculations using a continuum response, only the direct through-thickness and the transverse shear strains are assumed to be nonzero. All the other strain components (i.e., the membrane strains) are assumed to be zero . All tensors have the same number of components. For example, the stress components are as follows: S11 Direct membrane stress. S22 S33 S12 S13 S23 Direct membrane stress. Direct through-thickness stress. In-plane membrane shear stress. Transverse shear stress. Transverse shear stress. Cohesive elements using a uniaxial stress state Stress and other tensors (including strain tensors) are available for cohesive elements with uniaxial stress response. Both the stress tensor and the strain tensor contain true values. For the constitutive calculations using a uniaxial stress response, only the direct through-thickness stress is assumed to be nonzero. All the other stress components (i.e., the membrane and transverse shear stresses) are assumed to be zero . All tensors have the same number of components. For example, the stress components are as follows: S33 Direct through-thickness stress. Cohesive elements using a traction-separation response Stress and other tensors (including strain tensors) are available for elements with traction-separation response. Both the stress tensor and the strain tensor contain nominal values. The output variables E, LE, and NE all contain the nominal strain when the response of cohesive elements is defined in terms of traction versus separation. All tensors have the same number of components. For example, the stress components are as follows: S33 S13 S23 Direct through-thickness stress. Transverse shear stress. Transverse shear stress. Node ordering and face numbering on elements face 3 face 2 face 5 face 4 face 1 6 - node element 9 - node element face 2 face 5 face 6 face 4 face 1 face 3 9 10 12 11 8 - node element 1 2 - node element Element faces for COH3D6 Face 1 Face 2 Face 3 Face 4 Face 5 1 – 2 – 3 face 4 – 6 – 5 face 1 – 4 – 5 – 2 face 2 – 5 – 6 – 3 face 3 – 6 – 4 – 1 face Element faces for COH3D8 Face 1 Face 2 Face 3 Face 4 Face 5 Face 6 1 – 2 – 3 – 4 face 5 – 8 – 7 – 6 face 1 – 5 – 6 – 2 face 2 – 6 – 7 – 3 face 3 – 7 – 8 – 4 face 4 – 8 – 5 – 1 face Numbering of integration points for output 7 1 8 2 6 9 3 6 - node element 9 - node element 12 4 11 9 1 10 8 - node element 1 2 - node element 32.5.10 AXISYMMETRIC COHESIVE ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Cohesive elements: overview,” Section 32.5.1 • “Choosing a cohesive element,” Section 32.5.2 • *COHESIVE SECTION • Chapter 21, “Adhesive joints and bonded interfaces,” of the Abaqus/CAE User’s Manual Overview This section provides a reference to the axisymmetric cohesive elements available in Abaqus/Standard and Abaqus/Explicit. Element types General element COHAX4 4-node axisymmetric cohesive element Active degrees of freedom , 1, 2 ( ) Additional solution variables None. Pore pressure element COHAX4P 6-node displacement and pore pressure axisymmetric cohesive element Active degrees of freedom 1, 2, 8 Additional solution variables None. Nodal coordinates required Element property definition You can define the element’s initial constitutive thickness. The default initial constitutive thickness of cohesive elements depends on the response of these elements. For continuum response, the default initial constitutive thickness is computed based on the nodal coordinates. For traction-separation response, the default initial constitutive thickness is assumed to be 1.0. For response based on a uniaxial stress state, there is no default; you must indicate your choice of the method for computing the initial constitutive thickness. See “Specifying the constitutive thickness” in “Defining the cohesive element’s initial geometry,” Section 32.5.4, for details. Abaqus calculates the thickness direction automatically based on the midsurface of the element. Input File Usage: Abaqus/CAE Usage: *COHESIVE SECTION Property module: Create Section: select Other as the section Category and Cohesive as the section Type Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BR BY BRNU Body force Body force Body force FL−3 FL−3 FL−3 BZNU Body force FL−3 Body force in radial direction. Body force in axial direction. Nonuniform body force in radial direction with magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user Nonuniform body force in axial direction with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. CENT(S) Not supported FL−4 (ML−3T−2) Centrifugal load (magnitude is input is the mass density , where is the angular as per unit volume, velocity). Centrifugal load (magnitude is input as the angular velocity). , where is CENTRIF(S) Rotational body force T−2 (*DLOAD) GRAV Abaqus/CAE Load/Interaction Gravity Pressure Not supported AXISYMMETRIC COHESIVE ELEMENT LIBRARY Units Description LT−2 FL−2 FL−2 Gravity loading direction (magnitude is acceleration). in specified input as Pressure on face n. on with user face Nonuniform pressure supplied magnitude subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. Not supported FL−5 T2 Not supported Not supported FL−4 T2 FL−4 T Not supported FL−3 T Stagnation body force in radial and axial directions. Stagnation pressure on face n. Viscous body force in radial and axial directions. Viscous pressure on face n, applying a pressure proportional to the velocity normal to the face and opposing the motion. Pn PnNU SBF(E) SPn(E) VBF(E) VPn(E) Surface-based loading Distributed loads Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description PNU Pressure Pressure FL−2 FL−2 SP(E) Pressure FL−4 T2 32.5.10–3 Pressure on the element surface. Nonuniform pressure on the element surface with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. Stagnation pressure on the element Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description VP(E) Pressure FL−3 T Viscous pressure applied on the element surface. The viscous pressure is proportional to the velocity normal to the element face and opposing the motion. Element output Stress, strain, and other tensor components available for output depend on whether the cohesive elements are used to model adhesive joints, gaskets, or delamination problems. You indicate the intended usage of the cohesive elements by choosing an appropriate response type when defining the section properties of these elements. The available response types are discussed in “Defining the constitutive response of cohesive elements using a continuum approach,” Section 32.5.5, and “Defining the constitutive response of cohesive elements using a traction-separation description,” Section 32.5.6. Cohesive elements using a continuum response Stress and other tensors (including strain tensors) are available for elements with continuum response. Both the stress tensor and the strain tensor contain true values. For the constitutive calculations using a continuum response, only the direct through-thickness and the transverse shear strains are assumed to be nonzero. All the other strain components (i.e., the membrane strains) are assumed to be zero . All tensors have the same number of components. For example, the stress components are as follows: S11 S22 S33 S12 Direct membrane stress. Direct through-thickness stress. Direct membrane stress. Transverse shear stress. Cohesive elements using a uniaxial stress state Stress and other tensors (including strain tensors) are available for cohesive elements with uniaxial stress response. Both the stress tensor and the strain tensor contain true values. For the constitutive calculations using a uniaxial stress response, only the direct through-thickness stress is assumed to be nonzero. All the other stress components (i.e., the membrane and transverse shear stresses) are assumed to be zero . All tensors have the same number of components. For example, the stress components are as follows: S22 Direct through-thickness stress. Cohesive elements using a traction-separation response Stress and other tensors (including strain tensors) are available for elements with traction-separation response. Both the stress tensor and the strain tensor contain nominal values. The output variables E, LE, and NE all contain the nominal strain when the response of cohesive elements is defined in terms of traction versus separation. All tensors have the same number of components. For example, the stress components are as follows: S22 S12 Direct through-thickness stress. Transverse shear stress. Node ordering and face numbering on elements face 3 face 4 face 2 face 1 4 - node element 6 - node element Element faces Face 1 Face 2 Face 3 Face 4 1 – 2 face 2 – 3 face 3 – 4 face 4 – 1 face Numbering of integration points for output 5 1 2 6 4 - node element 6 - node element 32.6 Gasket elements • “Gasket elements: overview,” Section 32.6.1 • “Choosing a gasket element,” Section 32.6.2 • “Including gasket elements in a model,” Section 32.6.3 • “Defining the gasket element’s initial geometry,” Section 32.6.4 • “Defining the gasket behavior using a material model,” Section 32.6.5 • “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6 • “Two-dimensional gasket element library,” Section 32.6.7 • “Three-dimensional gasket element library,” Section 32.6.8 • “Axisymmetric gasket element library,” Section 32.6.9 32.6.1 GASKET ELEMENTS: OVERVIEW Abaqus/Standard offers a library of gasket elements to model the behavior of gaskets. Overview Gasket modeling consists of: • choosing the appropriate gasket element type (“Choosing a gasket element,” Section 32.6.2); • including the gasket elements in a finite element model (“Including gasket elements in a model,” Section 32.6.3); • defining the initial geometry of the gasket (“Defining the gasket element’s initial geometry,” Section 32.6.4); and • defining the gasket behavior with either a material model (“Defining the gasket behavior using a material model,” Section 32.6.5) or a gasket behavior model (“Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6). Motivation for gasket elements Gaskets are constructed in many ways and from many materials. Some types of gaskets consist of several layers of preformed metal, possibly with thin elastomeric coatings or elastomeric inserts . Others use plastics together with elastomeric inserts. Section A−A Figure 32.6.1–1 Typical gasket consisting of several layers of preformed metal. Gaskets are usually very thin and act as sealing components between structural components. They are carefully designed to provide appropriate pressure-closure behaviors through their thickness (the thin direction of the gaskets) so that they maintain their sealing action as the components undergo It is difficult to use solid continuum elements deformations due to thermal and mechanical loads. to model the through-thickness behavior of gaskets with the material library available. Therefore, Abaqus/Standard offers a variety of gasket elements that have through-thickness behaviors specifically designed for the study of gaskets. The gasket behavior models are separate from the models in the material library and assume that the thickness-direction, transverse shear, and membrane behaviors are uncoupled . For a gasket behavior that is not readily addressed by these special behavior models, such as occurs when coupled behaviors or through-thickness tensile behavior must be considered, Abaqus/Standard provides a versatile alternative by allowing a gasket element to use either a built-in or user-defined material model . Spatial representation of a gasket element Figure 32.6.1–2 demonstrates the key geometrical features that are used to define gasket elements. Gasket elements are composed of two surfaces separated by a thickness. The relative motion of the bottom and top surfaces measured along the thickness direction to the gasket quantifies the thickness-direction (local 1-direction) behavior of the gasket element. The relative change in position of the bottom and top surfaces measured in the plane orthogonal to the thickness direction quantifies the transverse shear behavior of the gasket element. The stretching and shearing of the midsurface of the element (the surface halfway between the bottom and top surfaces) quantifies the membrane behavior of the gasket element. top face (SPOS) normal direction gasket element node bottom face (SNEG) midsurface Figure 32.6.1–2 Spatial representation of a gasket element. Local behavior directions defined at the integration points The thickness direction defined at the integration points of gasket elements constitutes the local 1-direction. The transverse shear behavior is defined in the local 1–2 and 1–3 planes. The membrane behavior is defined in the 2–3 plane. The local 2- and 3-directions are not defined for elements that have nodes with only one degree of freedom because these elements consider only the thickness-direction behavior of a gasket. The local directions are used to specify the gasket behavior and for output of all quantities that describe the current deformation state of a gasket. Abaqus/Standard computes the local directions by default. You can also define them for some element types. Default local directions Abaqus/Standard computes the local 1-direction as explained in “Defining the gasket element’s initial geometry,” Section 32.6.4. For two-dimensional and axisymmetric gasket elements, the local 2-direction is defined so that the cross product between the local 1- and 2-directions gives the out-of-plane direction . Figure 32.6.1–3 Local directions for two-dimensional and axisymmetric gasket elements. For three-dimensional area and three-dimensional link elements, the local 2- and 3-directions are normal to the local 1-direction and are defined by the standard Abaqus convention for local directions on surfaces in space . projection of x-axis onto surface Figure 32.6.1–4 Local directions for three-dimensional area and three-dimensional link gasket elements. For three-dimensional line elements, the local 2-direction is obtained by the projection of the tangent to the midsurface of the element onto the plane orthogonal to the local 1-direction . The local 3-direction is then obtained by the cross product of the local 1- and 2-directions. midsurface t = tangent vector Figure 32.6.1–5 Local directions for three-dimensional line gasket elements. Specifying the local directions You can define the local 1-direction as explained in “Defining the gasket element’s initial geometry,” Section 32.6.4. The local 2- and 3-directions can be defined using local orientations (“Orientations,” Section 2.2.5) for three-dimensional area and three-dimensional link elements that consider transverse shear and membrane deformations. Input File Usage: Use the following option to associate a local orientation with a particular gasket element set: Abaqus/CAE Usage: *GASKET SECTION, ELSET=name, ORIENTATION=name Property module: Assign→Material Orientation Procedures with which gasket elements are allowed Gasket elements can be used in static, static perturbation, quasi-static, dynamic, and frequency analyses. However, gasket elements are assumed to have no mass; therefore, the density cannot be defined for gasket elements. 32.6.2 CHOOSING A GASKET ELEMENT Products: Abaqus/Standard Abaqus/CAE References • “Gasket elements: overview,” Section 32.6.1 • “Two-dimensional gasket element library,” Section 32.6.7 • “Three-dimensional gasket element library,” Section 32.6.8 • “Axisymmetric gasket element library,” Section 32.6.9 • Chapter 32, “Gaskets,” of the Abaqus/CAE User’s Manual Overview The Abaqus/Standard gasket element library includes: • elements for two-dimensional analyses; • elements for three-dimensional analyses; • elements for axisymmetric analyses; • elements that account for the thickness-direction behavior of gaskets only; and • elements that account for the thickness-direction, membrane, and transverse shear behaviors of gaskets. Naming convention The gasket elements used in Abaqus/Standard are named as follows: GK 3D 12 M N Optional: thickness-direction behavior only (N) Optional: line element (L), element for use with modified tetrahedral elements (M) number of nodes plane strain (PE), plane stress (PS), two-dimensional (2D), three-dimensional (3D), or axisymmetric (AX) gasket element For example, GKPE4 is a 4-node, plane strain gasket element that accounts for thickness-direction, membrane, and transverse shear behaviors. Elements for general use versus elements with thickness-direction behavior only In both classes material properties can be Abaqus/Standard offers two classes of gasket elements. specified by either special gasket behavior models or built-in material models, including user-defined materials . The first class is a collection of gasket elements that have all displacement degrees of freedom active at their nodes. These elements are necessary when the membrane and/or transverse shear behavior of the gasket is of importance . The thickness-direction, transverse shear, and membrane behaviors can be defined as uncoupled behaviors only, when the elements are used in conjunction with special gasket behavior models. In some cases the membrane effects are only secondary; in such cases it is possible to model only the thickness-direction and transverse shear behaviors. These elements are suited for analyses where both thickness-direction behavior and frictional effects are important. gasket normal behavior transverse shear membrane stretch membrane shear membrane stretch Figure 32.6.2–1 Different deformation modes of gaskets. In the second class of gasket elements deformation is measured only in the thickness direction. The response of the gasket to any other deformation mode is ignored. The nodes of these elements have only one displacement degree of freedom, which lies in the thickness direction of the gasket. This class of elements is intended as a means to reduce the computational cost of an analysis when the thickness- direction behavior of the gasket is the only behavior of importance. This behavior can be specified easily in terms of pressure in the gasket versus gasket closure. Frictional forces cannot be transmitted by such elements, and any thermal expansion or stretching of the gasket in its plane is not accounted for. Elements for two-dimensional, three-dimensional, and axisymmetric analyses For both classes of gasket elements Abaqus/Standard offers a choice of two-dimensional, three-dimensional, and axisymmetric elements. Plane stress and plane strain elements are provided for two-dimensional analyses to represent thin gaskets or thick gaskets in the out-of-plane direction, respectively. Axisymmetric gasket elements are provided for cases where the geometry and loading of the structure are axisymmetric. Abaqus/Standard offers 2-node or link elements for two-dimensional, three-dimensional, and axisymmetric analyses; three-dimensional line elements; and a three-dimensional 12-node element for use with modified tetrahedral elements. These elements have specific characteristics that are useful when modeling gaskets. Link elements Because link gasket elements have two nodes, their geometry defines only one dimension of the gasket—the through-thickness dimension. A link gasket element might typically be used to model a washer used under a bolt, when the bolt itself is modeled with a truss element. For two-dimensional and three-dimensional link elements the cross-section of the gasket is undetermined. For axisymmetric link elements the width of the element is undetermined. The reduction in dimensionality of these elements offers flexibility in the specification of the gasket behavior and can prove to be very efficient in some cases; see “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6, for further details. Three-dimensional line elements Three-dimensional line gasket elements are typically used to model narrow, thicker features in gaskets, such as an elastomeric insert around a hole. Since they are used in three-dimensional analyses, their width is undetermined from the element’s geometry. This reduction in dimensionality offers flexibility in the specification of the gasket behavior and can prove to be very efficient in some cases; see “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6, for further details. 12-node elements for use with modified tetrahedral elements The 12-node gasket elements have the same contact properties as the modified 10-node tetrahedra; these elements have consistent nodal forces at the corner and midside nodes. They are primarily intended for use with the modified tetrahedral elements but can also be used in conjunction with other solid continuum elements by using contact pairs. In the latter case the solution may be noisy for badly mismatched meshes. 32.6.3 INCLUDING GASKET ELEMENTS IN A MODEL Products: Abaqus/Standard Abaqus/CAE References • “Gasket elements: overview,” Section 32.6.1 • “Choosing a gasket element,” Section 32.6.2 • “Contact interaction analysis: overview,” Section 35.1.1 • “General multi-point constraints,” Section 34.2.2 • Chapter 32, “Gaskets,” of the Abaqus/CAE User’s Manual Overview Gasket elements: • are used to model gaskets and other seals between two components, each of which may be deformable or rigid; and • are connected to the adjacent components by sharing nodes, by using surface-based tie constraints, by using MPCs type TIE or PIN, or by using contact pairs. This section discusses the techniques that are available to discretize gaskets and assemble them in a model representing several components, such as an internal combustion engine. The methods described all apply to gasket elements that have all displacement degrees of freedom active at their nodes. For the most part they also apply to gasket elements with only thickness-direction behavior; exceptions are discussed later in this section. Discretizing gaskets using gasket elements Gaskets are generally manufactured as independent components. The gasket behavior is usually measured by performing a compression experiment on the gasket. In this case the gasket can be discretized as a single layer of gasket elements. Gaskets are sometimes made of several layers of materials. If the behavior of the gasket is obtained by compression testing of the entire gasket, the gasket can again be discretized as a single layer of gasket elements. However, if the behavior of the gasket is obtained by compression testing of each layer constituting the gasket, the gasket can be discretized with a corresponding set of layers of gasket elements. Discretizing gaskets with multiple layers If layers of gasket elements are used in the thickness direction and these layers do not have the same element layout in the plane of the gasket, use surface-based tie constraints, mesh refinement MPCs, or tied contact pairs to connect the different layers of the gasket. If tied contact pairs are used, assign a positive value to the adjustment zone depth, a, for the contact pairs (see “Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs,” Section 35.3.5) so that all slave nodes are properly tied at the beginning of the analysis. Assembling gaskets to other components in a model The easiest method to connect gasket elements that use all displacement components at their nodes to other components in a model is to define the mesh so that the gasket elements can share nodes with the elements on the surfaces of the adjacent components. More generally, when the gasket mesh is not matched to the meshing of the surfaces of the adjacent components or when the gasket elements that consider only thickness-direction behavior are used, gasket elements can be connected to other components by using contact pairs. Connecting gaskets to other components by using contact pairs or surface-based constraints Gaskets are usually composed of materials that are softer than the materials that compose the neighboring components. In addition, the discretization of gaskets will usually be finer than the discretization of neighboring parts. These two facts suggest that the contacting surfaces of a gasket should be the slave surfaces and that the contacting surfaces of neighboring parts should be the master surfaces. The second consideration also suggests that mismatched meshes will often be used in analyses involving gaskets. If mismatched meshes are used, the pressure distribution on a compressed gasket may not be predicted accurately; submodeling (“Submodeling: overview,” Section 10.2.1) may be required to obtain accurate local results. Two techniques are available to connect gasket elements to other parts in the model when surface-based constraints are used. Using a regular contact pair and a tied contact pair or a surface-based constraint This technique is required when the gasket membrane behavior is not defined. Use a tied contact pair (“Defining tied contact in Abaqus/Standard,” Section 35.3.7) or a tie constraint (“Mesh tie constraints,” Section 34.3.1) on one side of the gasket and a regular contact pair on the other side, as shown in Figure 32.6.3–1. Because a regular contact pair is used on one side of the gasket, tensile stresses cannot develop in the gasket thickness direction should the components surrounding the gasket be pulled apart. Assign a positive value to the adjustment zone depth, a, for the tied contact pair or, if necessary, specify a position tolerance for the tie constraint so that all slave nodes are properly tied at the beginning of the analysis. This technique allows for frictional slip on only one side of the gasket. Using a regular contact pair and a contact pair that does not allow separation This technique allows for frictional slip to be transmitted on both sides of the gasket. It is recommended when membrane behavior is defined for the gasket since it allows for the gasket membrane to stretch or contract as a result of frictional effects considered on both sides of the gasket. A contact pair or a constraint pair that does not allow for separation of the surfaces (“Contact pressure-overclosure relationships,” Section 36.1.2) should be used on one side of the gasket and a regular contact pair on the other, as shown in Figure 32.6.3–2. or tied constraint pair MODELING WITH GASKET ELEMENTS part 1 contact pair gasket element part 2 Figure 32.6.3–1 Connecting gaskets to other parts using contact pairs. contact pair or constraint pair that does not allow for separation of the surfaces part 1 contact pair gasket element with membrane behavior defined part 2 Figure 32.6.3–2 Connecting gaskets to other parts when the gasket membrane behavior is defined. Assign a positive value to the adjustment zone depth, a, for the contact pair so that the surfaces are in contact at the beginning of the analysis. Use the no separation contact pressure- overclosure relationship so that these surfaces do not separate during the analysis. This technique will prevent rigid body modes of the gasket in its thickness direction. You may still need to prevent rigid body modes in the plane of the gasket until frictional forces develop between the gasket and the adjacent components. Having gasket elements share nodes with other elements When the gaskets and their neighboring parts have matched meshes, it is straightforward to connect gaskets to other components in a model simply by sharing nodes . Part 1 gasket element Part 2 Figure 32.6.3–3 Gasket elements sharing nodes with other Abaqus elements. This method of connecting gaskets to other components is suited for cases when no frictional slip occurs between the gasket and the other components. It can be used whether or not the membrane behavior of the gasket elements is defined; however, if the gasket membrane behavior is defined, using a contact pair approach will lead to more realistic results since the difference in membrane stiffness between the gasket and its neighboring parts may lead to frictional slip. The method of sharing nodes will also lead to some small tensile stresses in the gasket should the parts connected to the gasket be pulled apart, as a result of the numerical stabilization technique added to the gasket thickness-direction behavior . The contact pair approach will avoid such tensile stresses. This node-sharing approach cannot be used with the gasket elements that consider only thickness-direction behavior. Using gasket elements that model thickness-direction behavior only In general, the modeling techniques discussed earlier can be used with gasket elements that model these elements have only one displacement degree thickness-direction behavior only. However, of freedom per node and cannot share nodes with elements that have all displacement degrees of freedom active at a node. They can, however, share nodes with other gasket elements that model thickness-direction behavior only. Discretizing a gasket with gasket elements that model thickness-direction behavior only When discretizing a gasket with several layers of gasket elements along the gasket direction, it is recommended that all the nodes belonging to a cross-section of the gasket have the same thickness direction . An approximate solution will be generated if the thickness direction changes, since only the magnitude of the force is transmitted from one gasket element to the next through the thickness of the gasket. cross section Figure 32.6.3–4 Discretizing a gasket using several layers of elements with thickness-direction behavior only. Connecting gaskets to other components when gasket elements with thickness-direction behavior only are chosen Contact pairs can be used to connect the gasket mesh to adjacent components, as explained above, but only frictionless, small-sliding contact can be used. MPC type PIN or TIE can also be used to connect a one degree of freedom node of a gasket element to another coincident node that has all its displacement degrees of freedom active . Abaqus/Standard automatically constrains the single displacement degree of freedom node to the global displacements of the other node. Surface-based tie constraints cannot be used to connect gasket elements that model thickness-direction behavior only. Additional considerations when using gasket elements Several cases require special consideration when using gasket elements. part 1 gasket elements part 2 1 d.o.f. Use TIE- or PIN-type MPC 2 d.o.f. coincident node Figure 32.6.3–5 Connecting gasket elements with thickness-direction behavior only to other parts by using MPCs. Using gasket elements in large-displacement analyses Gasket elements are small-strain, small-displacement elements. They can be used in large-displacement analyses. However, the local directions of the gasket elements are not updated with the solution, so incorrect results will be generated if the assembly containing the gasket elements undergoes any significant amount of rotation. Using 12-node gasket elements These elements are primarily for use when the adjacent components are modeled with modified 10-node tetrahedral elements (element type C3D10M). When the contact pair approach is used, such elements can also be placed adjacent to other three-dimensional solid continuum elements; however, if the meshes are badly mismatched, the solution may be noisy. Using 18-node gasket elements These elements are intended to share nodes with 21 to 27-node brick elements. They can also be connected to a mesh composed of 21 to 27-node brick elements or a mesh composed of 20-node brick elements when the contact pair approach is used. Abaqus/Standard allows the node numbers and the coordinates of the midface nodes in the 18-node gasket elements to be generated automatically if the faces are part of contact surfaces, similar to the way that midface nodes are generated for 20-node brick element faces on which a contact surface is defined. This feature is invoked by leaving the entries for nodes 17 and 18 in the element connectivity blank. Using the three-dimensional line gasket elements Three-dimensional line gasket elements are typically used to model narrow, thicker features in gaskets, such as an elastomeric insert around a hole. A typical mesh for such a case is presented in Figure 32.6.3–6. The gasket is discretized mainly with three-dimensional area elements. The insert is modeled with three-dimensional line elements that may or may not be connected to the area elements. These gasket elements are connected to surrounding components using two sets of contact pairs, and the area elements will typically have initial gaps specified in the gasket property definition so that the thicker inserts develop pressure on contact before the area elements do. nodes of the line gasket elements three-dimensional line gasket elements area gasket elements Figure 32.6.3–6 Typical use of three-dimensional line gasket elements to model inserts in gaskets. If three-dimensional line gasket elements that have all displacement degrees of freedom active at their nodes are used to discretize a gasket and the local 3-direction is the same at all the nodes of these elements (this is the case when all elements lie in a plane), the nodes of these elements can move in the local 3-direction without creating any strain in the elements . In such a case you should make sure that these elements are restrained properly in the local 3-direction. 32.6.4 DEFINING THE GASKET ELEMENT’S INITIAL GEOMETRY Products: Abaqus/Standard Abaqus/CAE References • “Gasket elements: overview,” Section 32.6.1 • *GASKET SECTION • “Creating gasket sections,” Section 12.13.15 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The initial gasket geometry: • is defined by the nodal coordinates of the element; and • is also defined by the thickness direction and initial thickness, each of which can be calculated by Abaqus/Standard or user-defined. Defining the element geometry A gasket element is basically composed of two surfaces (a bottom and a top surface) separated by the gasket thickness. The element has nodes on its bottom face and corresponding nodes on its top face. Two methods are available to define the element geometry. By defining the element’s nodes You can define the geometry of the gasket element by defining the coordinates of all the element’s nodes. You can define elements with constant or varying thickness. If the gasket element is very thin in comparison to dimensions in its surfaces, the thickness of the element calculated from the nodal coordinates may be inaccurate. In this case you can specify a constant thickness directly. By defining the bottom surface of the element You can specify a list of only the nodes on the bottom surface of the gasket element and the positive offset number that will be used to define the corresponding nodes on the top surface of the gasket element. Abaqus/Standard will create the nodes of the top face coincident with those of the bottom face unless the nodes of the top face have already been assigned coordinates. If the bottom and top nodes coincide, you must specify the thickness of the gasket element. Specifying the element thickness You can specify the gasket element thickness as part of its section property definition. Input File Usage: *GASKET SECTION thickness Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Gasket as the section Type: Initial thickness: Specify: thickness Additional quantities needed to specify the element geometry For three-dimensional area elements, the element geometry is defined entirely by the location of the top and bottom surfaces and the element thickness. For two- and three-dimensional link elements (elements with two nodes, one on each face) you should specify the cross-sectional area of the element. For axisymmetric link elements you should specify the width of the element. For general two-dimensional elements the out-of-plane thickness is required. For three-dimensional line elements you should also specify the width of the element. This additional information is specified as part of the gasket section property definition; if it is not specified but is needed, it is assumed to have a value of 1.0. Input File Usage: *GASKET SECTION , , , additional geometric data (cross-sectional area, width, or out-of-plane thickness) Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Gasket as the section Type: Cross-sectional area, width, or out-of-plane thickness: additional geometric data Default element thickness-direction definition Gaskets are usually manufactured to have a desired behavior in their thickness direction. Therefore, it is important to define the thickness directions of gasket elements accurately. Abaqus/Standard computes these directions by default. The method that Abaqus/Standard uses depends on the gasket element type. Link elements Abaqus/Standard computes the thickness direction for a two-dimensional, three-dimensional, or axisymmetric link element by subtracting the coordinates of node 1 from those of node 2, as shown in Figure 32.6.4–1. The computed thickness direction is then assigned to each node. If the gasket element is very thin, the thickness direction may not be predicted accurately. You can overwrite this direction, as explained below in “Specifying the thickness direction explicitly.” Two-dimensional and axisymmetric elements To compute the thickness direction for two-dimensional and axisymmetric elements, Abaqus/Standard forms a midsurface by averaging the coordinates of the node pairs forming the bottom and top surfaces of the element. This midsurface passes through the integration points of the element, as shown in Figure 32.6.4–2. For each integration point Abaqus/Standard computes a tangent whose direction is defined by the sequence of nodes given on the bottom and top surfaces. The thickness direction is then obtained as the cross product of the out-of-plane and tangent directions. The thickness direction computed at each integration point is then assigned to the nodes on either side of the integration point. Figure 32.6.4–1 Thickness direction for a link element. n2 n2 n2 t2 t1 n1 n1 n1 midsurface n3 n3 t3 n3 Figure 32.6.4–2 Thickness direction for a two-dimensional or axisymmetric element. Three-dimensional area elements To compute the thickness direction for three-dimensional area elements, Abaqus/Standard forms a midsurface by averaging the coordinates of the node pairs forming the bottom and top surfaces of the element. This midsurface passes through the integration points of the element, as shown in Figure 32.6.4–3. Abaqus/Standard computes the thickness direction to the midsurface at each integration point; the positive direction is obtained with the right-hand rule going around the nodes of the element on the bottom or top surface. The thickness direction computed at each integration point is assigned to the nodes on either side of the integration point. Three-dimensional line elements To compute the thickness direction for three-dimensional line elements, Abaqus/Standard computes the thickness direction at each integration point of the line element by differencing the coordinates of the element’s surface nodes associated with the integration point. The thickness direction will point from the node on the bottom face to the node on the top face of the element. The thickness direction computed at each integration point is then assigned to the nodes on either side of the integration point . n1 n1 n1 n4 n4 n4 midsurface n2 n2 n2 n3 n3 n3 Figure 32.6.4–3 Thickness direction for a three-dimensional area element. n1 n1 n1 n2 n2 n2 n3 n3 n3 Figure 32.6.4–4 Thickness direction for a three-dimensional line element. If the gasket element is very thin, the computation of the thickness direction may not be accurate. You can overwrite this definition as explained below in “Specifying the thickness direction explicitly.” Creating a smooth gasket Gasket elements can be used in a single layer or can be stacked in multiple layers . The thickness directions computed at the nodes of gasket elements on an element-by-element basis are averaged at nodes shared by two or more gasket elements. This averaging process ensures that, if the gasket is not planar, it has a thickness direction that varies smoothly even though the gasket has been discretized by elements. You must ensure that the connectivities of the elements are such that the thickness direction does not reverse from one element to the next for this process to work properly. Once the averaging process is complete, the thickness directions at the nodes of a given element may vary significantly along the gasket midsurface and through its thickness, as shown in Figure 32.6.4–5. The thickness directions at any of the nodes of an element should not vary in direction by more than 20°. In addition, the thickness directions of two associated nodes through the thickness direction should not vary in direction by more than 5°. Abaqus/Standard will require that the gasket be remeshed when such conditions are not met. multi-layered gasket thickness direction 20° 5° 5° midsurface Figure 32.6.4–5 Result of the averaging process. Specifying the thickness direction explicitly For cases when the above averaging process is not satisfactory, two methods are provided to specify the thickness direction of gasket elements. Specifying the thickness direction as part of the gasket section definition You can specify the components of the thickness direction as part of the gasket section definition. In this case all nodes of the gasket elements using this section definition are assigned the same thickness direction. The thickness direction specified at the nodes of the element will be averaged at nodes shared by two or more elements. Input File Usage: *GASKET SECTION , , , , component 1, component 2, component 3 Abaqus/CAE Usage: You cannot specify the gasket thickness direction in Abaqus/CAE. Specifying the thickness direction by specifying a normal direction at the nodes You can define the thickness direction at a particular integration point of a gasket element by specifying a normal direction for the node on the bottom face of the element that is associated with the integration point . The thickness direction will not be averaged if this node belongs to more than one element. The thickness direction specified at the bottom node will also be assigned at the top node associated with the same integration point. This thickness direction will not be averaged if the top node belongs to more than one element; however, you can overwrite this thickness direction by specifying a normal at this node if it is the bottom node of another element. This last situation can occur only in cases when gasket elements are stacked up through the thickness direction of the gasket. If this method is used to specify conflicting thickness directions at the same node, Abaqus/Standard will issue an error message. Thickness directions specified using this method will overwrite any thickness directions specified at a gasket node as part of the gasket section definition. Input File Usage: Abaqus/CAE Usage: *NORMAL User-specified nodal normals are not supported in Abaqus/CAE. Creating fold lines It is possible to introduce a fold line in a gasket by creating gaskets with coincident nodes and using MPC type TIE or PIN (“General multi-point constraints,” Section 34.2.2) to constrain the displacement of these nodes. However, fold lines are rarely needed in the analysis of gaskets, since almost all gaskets are manufactured with smoothly varying surfaces. Verifying the thickness direction Thickness direction definitions can be checked by examining the analysis input file processor output. The direction cosines of the thickness directions obtained at the nodes of gasket elements are listed under GASKET THICKNESS DIRECTIONS in the data (.dat) file. Specifying an initial gap and an initial void in the thickness direction of a gasket element The construction of gaskets in their through-thickness direction may be complex; for example, certain automotive gaskets are usually composed of several layers of metal and/or elastomeric inserts, and it is likely that the layers do not all touch until the gasket is compressed. The inter-layer spaces in a gasket are referred to in Abaqus as the initial void. The initial void is used only for calculating thermal strain and creep strain. It is also possible that the gasket surface geometry is such that pressure will not start building up until the gasket has been compressed by a certain amount. The gasket closure that is needed to generate a pressure is referred to in Abaqus as the initial gap. Figure 32.6.4–6 shows a schematic representation of the initial gap and initial void in a typical gasket. You can specify both the initial gap and initial void as part of the gasket section property definition. The initial thickness of the element should include the initial gap and the initial void. Input File Usage: *GASKET SECTION , initial gap, initial void Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Gasket as the section Type: Initial gap: initial gap, Initial void: initial void initial gap metallic plate metallic frame initial void spacers Figure 32.6.4–6 Schematic representation of an initial gap and an initial void in a typical gasket. Stability of unsupported gasket elements Gasket elements that extend outside neighboring components (unsupported gasket elements) can be troublesome and should be avoided. If a gasket element is completely or partially unsupported, incorrect areas can result in an incorrect stiffness, and numerical singularity problems can occur in the equation solver. Minor extensions (caused by numerical roundoff in mesh generation) will not usually cause a problem because Abaqus/Standard automatically extends the master surfaces a small amount beyond the edge of the model. Numerical problems can occur in the direction tangential to the gasket (if general gasket elements are used and no membrane stiffness is specified) as well as in the direction normal to the gasket. The numerical singularity problems normal to the gasket can be treated by stabilizing the elements with a small artificial stiffness. By default, Abaqus/Standard automatically applies a small stabilization stiffness (on the order of 10−9 times the initial compressive stiffness in the thickness direction) to all types of gasket elements except the link elements. For persistent numerical singularity problems in unsupported gasket elements the following treatment methods can be considered. First, make sure that an adequate membrane elasticity is specified. Second, specify a higher value for the artificial stiffness for the gasket section. If problems still persist, consider trimming, “skinning,” and using MPCs . Input File Usage: Use the following option to change the artificial stiffness for a gasket section: Abaqus/CAE Usage: *GASKET SECTION, STABILIZATION STIFFNESS=stiffness_value Use the following option to change the artificial stiffness for a gasket section: Property module: Create Section: select Other as the section Category and Gasket as the section Type: Stabilization stiffness: Specify: stiffness_value 32.6.5 DEFINING THE GASKET BEHAVIOR USING A MATERIAL MODEL Products: Abaqus/Standard Abaqus/CAE References • “Gasket elements: overview,” Section 32.6.1 • “UMAT,” Section 1.1.40 of the Abaqus User Subroutines Reference Manual • “Creating and editing materials,” Section 12.7 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The gasket behavior defined by a material model: • can be specified in terms of a built-in material model or a user-defined small-strain material model; • considers only the thickness behavior and assumes a uniaxial stress state for gasket elements that model thickness-direction behavior only; • admits both compressive and tensile stresses in the thickness direction; • is defined in terms of small-strain measures and, hence, finite-strain material models such as hyperelastic and hyperfoam cannot be used; • is restricted to small-strain elasticity models for line gasket elements that use the built-in material models; • causes Abaqus/Standard to use the reference thickness to convert the relative displacements at the top and bottom surfaces of the gasket to strains and uses these strains in conjunction with the constitutive law to obtain the stresses; and • makes the notions of “initial gap” and “initial void” in the thickness direction irrelevant (consequently, Abaqus/Standard ignores such data specified as part of the gasket section property definition). Assigning a gasket behavior to a gasket element To define the gasket behavior by a material model, you must assign a gasket section definition to a region of your model and assign the name of a material definition to the gasket section definition. The gasket behavior for this region is defined entirely by the gasket thickness and the material properties specified by the material definition referring to the same name. The gasket behavior can be defined in terms of a built-in or a user-defined material model. In the latter case the actual material model is defined in user subroutine UMAT. Input File Usage: Use the following options to define the gasket behavior in terms of a built-in material model: *GASKET SECTION, ELSET=name, MATERIAL=name *MATERIAL, NAME=name Use the following options to define the gasket behavior in terms of a user- defined material model: *GASKET SECTION, ELSET=name, MATERIAL=name *MATERIAL, NAME=name *USER MATERIAL, CONSTANTS=n Property module: Create Material: Name: name, enter data for any materials that are valid for gasket sections except those found under Other→Gasket Create Section: select Other as the section Category and Gasket as the section Type: Material: name Abaqus/CAE Usage: Tensile behavior modeling Tensile behavior modeling can be desirable when gaskets carry (limited) tensile stresses, such as occurs when adhesives are present. Undesired tensile behavior can be avoided by using appropriate contact pairs and/or implementing a user-defined no-tension material model in user subroutine UMAT. Specific output for material definition of gasket behavior The output variables for stresses and strains are the same as those used for solid elements: tensile and compressive stresses/strains are indicated as positive and negative quantities, respectively. However, for all stress/strain output variables the 11-component refers to the through-thickness direction; the 22-, 33-, and 23-components refer to two direct and one shear membrane component, respectively; the remaining 12- and 13-components refer to the transverse shear components. For details about these definitions, see “Gasket elements: overview,” Section 32.6.1. The output variable NE is available to output nominal (effective) strains for gasket elements defined using a material model; however, NE is identical to E in this case. 32.6.6 DEFINING THE GASKET BEHAVIOR DIRECTLY USING A GASKET BEHAVIOR MODEL Products: Abaqus/Standard Abaqus/CAE References • “Gasket elements: overview,” Section 32.6.1 • “Defining the gasket element’s initial geometry,” Section 32.6.4 • “Defining gasket behavior,” Section 12.12.4 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview The gasket behavior defined by a gasket behavior model: • can be specified in terms of uncoupled thickness direction, membrane, and transverse shear behavior only; • can be nonlinear elastic with damage or nonlinear elastic-plastic in the thickness direction; • can consider creep effects in the thickness direction when rate-independent elastic-plastic modeling is used; • can consider the dynamic stiffness and damping characteristics in the thickness direction when elastic-damage modeling is used; • will be linear elastic in the membrane and transverse shear directions; and • can consider thermal effects in the thickness and membrane directions. Assigning a gasket behavior to a gasket element To define the gasket behavior by a gasket behavior model, you must assign a gasket section definition to a region of your model and assign the name of a gasket behavior definition to the gasket section definition. The gasket behavior for this region is defined entirely by the properties specified by the gasket behavior definition referring to the same name. Input File Usage: Abaqus/CAE Usage: Use both of the following options to define the gasket behavior in terms of a gasket behavior model: *GASKET SECTION, ELSET=name, BEHAVIOR=name *GASKET BEHAVIOR, NAME=name Property module: Material editor: Name: name, enter data for any materials found under Other→Gasket Create Section: select Other as the section Category and Gasket as the section Type: Material: name Specifying a gasket behavior The thickness-direction, transverse shear, and membrane behaviors are defined to be uncoupled. Each behavior is specified independently. You must specify the thickness-direction behavior. You can specify multiple thickness-direction behaviors to define the loading and unloading characteristics. You can obtain an average contact pressure output when the thickness-direction behavior is defined as force or force per unit length versus closure. The transverse shear and membrane behaviors are optional for gasket elements that have all displacement degrees of freedom active at their nodes. You can define one or both of these behaviors. When thermal and rate-dependent effects are important, you can define thermal expansion and creep behavior for gaskets; user subroutines UEXPAN and CREEP can be used to define these behaviors. You cannot specify density for gasket elements since they have no mass matrix. Input File Usage: Use the first two options and any of the following options to specify a gasket behavior: *GASKET BEHAVIOR, NAME=name *GASKET THICKNESS BEHAVIOR *GASKET ELASTICITY *GASKET CONTACT AREA *EXPANSION *CREEP *DEPVAR *USER OUTPUT VARIABLES The *GASKET THICKNESS BEHAVIOR option can be repeated to define the loading and unloading characteristics of the thickness-direction behavior. The *GASKET ELASTICITY option can be repeated to define both transverse shear and membrane behaviors. The other options cannot be repeated within a single behavior definition. The order in which these options are specified has no importance, but they must appear immediately after the *GASKET BEHAVIOR option. Abaqus/CAE Usage: Use the first option and any of the following options to specify a gasket behavior: Property module: material editor: Other→Gasket→Gasket Thickness Behavior Other→Gasket→Gasket Transverse Shear Elasticity and/or Gasket Membrane Elasticity Mechanical→Expansion Mechanical→Plasticity→Creep General→Depvar General→User Output Variables Defining the thickness-direction behavior of the gasket To define the thickness-direction behavior of gaskets, Abaqus/Standard offers a nonlinear elastic model with damage and a nonlinear elastic-plastic model with the possibility of considering creep effects. Thermal effects in the thickness direction can also be accounted for. Abaqus/Standard measures the thickness-direction deformation as the closure between the bottom and top faces of the gasket element; therefore, the thickness-direction behavior must always be defined in terms of closure. The closure is the sum of the elastic closure, plastic closure, creep closure, thermal closure, plus any initial gap in the thickness direction. As explained below, the behavior can be defined as pressure versus closure, force versus closure, or force per unit length versus closure. In all cases the thickness-direction behavior can be defined as a function of temperature and/or field variables. Input File Usage: Abaqus/CAE Usage: *GASKET THICKNESS BEHAVIOR, DEPENDENCIES Property module: material editor: Other→Gasket→Gasket Thickness Behavior Choosing a unit system used to define the thickness-direction behavior The thickness-direction behavior can be defined in terms of pressure versus closure, force versus closure, or force per unit length versus closure. Prescribing the thickness-direction behavior as pressure versus closure You can define the thickness-direction behavior in terms of pressure and closure for all gasket element types. The pressure is available for output or visualization. Input File Usage: Abaqus/CAE Usage: *GASKET THICKNESS BEHAVIOR, VARIABLE=STRESS Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Units: Stress Prescribing the thickness-direction behavior as force or force per unit length versus closure You can define the thickness-direction behavior in terms of force or force per unit length and closure only for link elements and three-dimensional line elements. This method is suited for cases where the gasket cross-section in the 1–2 or 1–3 plane varies greatly with deformation because it would be too expensive to model such a deformation with a full two- or three-dimensional model. In such cases a model with link elements or three-dimensional line elements can give meaningful answers as long as the deformation is quantified in terms of force or force per unit length . When using two- or three-dimensional link elements, you must specify the thickness-direction behavior as force versus closure. When using axisymmetric link elements or three-dimensional line elements, you must specify the thickness-direction behavior as force per unit length versus closure. Input File Usage: Abaqus/CAE Usage: *GASKET THICKNESS BEHAVIOR, VARIABLE=FORCE Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Units: Force top block bottom block gasket undeformed configuration deformed configuration bottom block gasket element force or force per unit length top block bottom block model for analysis Figure 32.6.6–1 Modeling complex deformations with link or three-dimensional line elements. Defining a nonlinear elastic model with damage The nonlinear elastic model with damage is illustrated in Figure 32.6.6–2. pressure loading curves unloading curves Cmax closure Cmax Figure 32.6.6–2 Elastic model with damage. As the gasket is compressed, the pressure (or force, or force per unit length) follows the path given by the loading curve. If the gasket is unloaded, for example at point B, the pressure follows the unloading curve until the loading is such that the closure becomes greater than . The arrows shown in the figure illustrate the loading/unloading paths of this model. . Reloading after unloading follows the unloading curve , after which the loading path follows the loading curve Defining the loading curve To define the loading curve in piecewise linear form, you provide data points of pressure versus elastic closure, starting with point A. For negative elastic closures, the model gives zero pressure (or force). For closures larger than the last user-specified closure, the pressure-closure relationship is extrapolated based on the last slope computed from the user-specified data. Input File Usage: *GASKET THICKNESS BEHAVIOR, TYPE=DAMAGE, DIRECTION=LOADING Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Type: Damage, Loading Defining the unloading curve , , and so on), you provide data points of pressure (or force) To define the unloading curves ( versus elastic closure up to a given maximum closure ( , and so on). You can specify as many unloading curves as are necessary. Each unloading curve always starts at point A, the point of zero pressure for zero elastic closure, since the damaged elasticity model does not allow any permanent deformation. If unloading occurs from a maximum closure for which an unloading curve is not specified, the unloading is interpolated from neighboring unloading curves. The unloading curves are stored in normalized form so that they intersect the loading curve at a unit stress (or unit force) for a unit elastic closure, and the interpolation occurs between these normalized curves. If unloading curves are not specified, the loading/unloading will follow the loading curve. , or Input File Usage: *GASKET THICKNESS BEHAVIOR, TYPE=DAMAGE, DIRECTION=UNLOADING Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Type: Damage, Unloading, toggle on Include user-specified unloading curves Defining the behavior for elements with an initial gap For cases when the load in the gasket does not increase as soon as the gasket is compressed , you can specify an initial gap as part of the gasket section property definition and define the loading/unloading curves as if the initial gap were not present (the case of Figure 32.6.6–2). This method is convenient when many gasket elements refer to the same gasket behavior and the only difference is the initial gap. pressure loading curves unloading curves closure initial gap Figure 32.6.6–3 Elastic model with damage and initial gap. Defining a nonlinear elastic-plastic model The nonlinear elastic-plastic model is illustrated in Figure 32.6.6–4. As the gasket is compressed, the pressure (or force) follows the path given by the loading curve . The loading curve is a nonlinear elastic curve until point B is reached. At point B the slope of the loading curves decreases by more than 10%, which is assumed to correspond with the onset of plastic deformation. The value of 10% was chosen as a reasonable minimum value that can be expected at the onset of yield. If yield starts at a point at which no decrease in the slope occurs, numerical difficulties may occur. If the elastic part of the loading curve has a changing slope, the curve should be defined such that the slope does not decrease by more than 10% at any given point. After point B plastic deformation starts taking place. If unloading occurs before point B is reached, unloading will take place along the initial loading curve. Once loading has gone beyond point B, unloading will take place along an unloading curve such as curve . The unloading is assumed to be entirely elastic. The amount of closure at point D represents the plastic closure for the unloading curve until the gasket yields, after which the loading curve is followed. Plastic deformation takes place until the last point M on the loading curve is reached. Beyond point M, the curve is followed for both loading and unloading; this behavior represents the behavior of a crushed gasket, which is assumed to be entirely elastic and can be specified in a piecewise-linear fashion, even beyond point M. The arrows shown in the figure illustrate the loading/unloading paths for the elastic-plastic model. . Reloading after unloading follows the same curve Abaqus/Standard will automatically convert the curves so that the unloading curves become curves of pressure (or force) versus elastic closure for a given plastic closure. The loading curve will be transformed into an elastic loading/unloading curve defined at zero plastic closure (the portion of the curve) and a yield curve (the portion of the curve). By default, the onset of yield (point B) will be obtained as soon as the slope of the loading curve decreases by 10% from the maximum slope recorded up to that point while traveling along the loading curve from point A to point M. pressure closure plastic closure at point D Figure 32.6.6–4 Elastic-plastic model. Abaqus/Standard offers two alternatives to allow you to override this default method of determining the onset of yield as described below. If only a loading curve is provided, the unloading will be based on the curve , independent of the level of plasticity. Defining the loading curve To define the loading curve in piecewise linear form, you provide data points of pressure (or force, or force per unit length) versus closure (where closure represents the elastic plus the plastic closure), starting with point A. The last closure value given represents the closure at which the gasket is assumed crushed (point M in Figure 32.6.6–4); at this point, the maximum permanent deformation is reached. For negative closures the model gives zero pressure (or force). To override the default method of determining the onset of yield, you can specify either a value for the decrease in slope other than the default value of 10% or the closure value at which onset of yield occurs. The specified value must correspond to a point on the loading curve at which the slope decreases. Input File Usage: Use the following option to define the loading curve and use the default method for determining the onset of yield: *GASKET THICKNESS BEHAVIOR, TYPE=ELASTIC-PLASTIC, DIRECTION=LOADING Use the following option to define the loading curve and specify a nondefault value for the decrease in slope that defines the onset of yield: *GASKET THICKNESS BEHAVIOR, TYPE=ELASTIC-PLASTIC, DIRECTION=LOADING, SLOPE DROP=drop Use the following option to define the loading curve and specify the closure value that defines the onset of yield: *GASKET THICKNESS BEHAVIOR, TYPE=ELASTIC-PLASTIC, DIRECTION=LOADING, YIELD ONSET=closure_value Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Type: Elastic-Plastic, Loading, Yield onset method: Relative slope drop drop or Yield onset method: Closure value closure_value Abaqus/CAE Usage: Defining the unloading curve , To define the unloading curves ( , and so on), you provide data points of pressure (or force, or force per unit length) versus closure (elastic plus plastic) for each given plastic closure (closure at points D, F, and so on) in ascending values of closure. You can specify as many unloading curves as are necessary. If unloading occurs at a plastic closure for which an unloading curve is not specified, the unloading curve is interpolated from neighboring unloading curves. If no unloading curves are specified, unloading is assumed to follow a curve similar to the initial nonlinear elastic segment of the loading curve. The unloading curves are stored in normalized form so that they intersect the yield curve at a unit stress (or unit force) for a unit elastic closure, and the interpolation occurs between these normalized curves. If the loading curve includes highly nonlinear behavior after the onset of yield, the interpolated unloading may give unreasonable behavior (such as the interpolated unloading path crossing over the user-defined loading curve). You should specify as many user-defined unloading curves as are needed to create regions for which interpolated unloading response is appropriate. For example, Figure 32.6.6–5 illustrates a loading curve that includes a sharp decrease in the hardening slope well after the onset of yield. In this case it is insufficient to specify only one unloading curve at the gasket crush point (the end of the loading data). If unloading were to take place from point C, the unloading path would cross over the loading path. At least one additional unloading curve is required, after the sharp decrease in hardening slope, to prevent the interpolated unloading path crossing the loading curve. Input File Usage: *GASKET THICKNESS BEHAVIOR, TYPE=ELASTIC-PLASTIC, DIRECTION=UNLOADING Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Type: Elastic-Plastic, Unloading, toggle on Include user-specified unloading curves Defining the behavior for elements with an initial gap For cases when the load in the gasket does not increase as soon as the gasket is compressed , you can specify an initial gap as part of the gasket section property definition and define the loading/unloading curves as if the initial gap were not present (the case of Figure 32.6.6–4). This method is convenient when many gasket elements refer to the same gasket behavior and the only difference is the initial gap. pressure point where user-defined unloading response should be specified gasket crush point interpolated unloading response onset of yield closure Figure 32.6.6–5 Elastic-plastic behavior with complex loading curve. pressure closure initial gap Figure 32.6.6–6 Elastic-plastic model with initial gap. Numerical stabilization of the thickness-direction behavior The damage and elastic-plastic models described above have zero stiffness at zero pressure. To overcome numerical problems caused by this zero stiffness, Abaqus/Standard automatically adds a small stiffness (by default, equal to 10−3 times the initial compressive stiffness) in the thickness direction of the gasket when the pressure obtained from the specified gasket thickness behavior is zero. This numerical stabilization ensures that the gasket element always returns to its stress-free thickness when it is totally unloaded. Hence, if the gasket surfaces are pulled apart, a small force will arise from the stabilization process. You can change the default stiffness. Input File Usage: *GASKET THICKNESS BEHAVIOR, DIRECTION=LOADING, TENSILE STIFFNESS FACTOR=factor Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Loading, Tensile stiffness factor: factor Defining the transverse shear behavior of the gasket You can define the elastic transverse shear stiffness of the gasket. Abaqus/Standard measures the relative displacement between the bottom and top of the gasket element along the local 2- or 3-directions to define the transverse shear in the gasket. Therefore, you should always define the elastic transverse stiffness as stress (or force, or force per unit length) per unit displacement. You can specify the stiffness as a function of temperature and field variables. The same stiffness is used for the shear in the 1–2 plane and the shear in the 1–3 plane. For each set of temperature and/or field variables, the first slope of the initial loading curve for the gasket’s thickness-direction behavior will be used to compute the transverse shear stiffness if the transverse shear behavior is not defined explicitly. Input File Usage: Abaqus/CAE Usage: *GASKET ELASTICITY, COMPONENT=TRANSVERSE SHEAR, DEPENDENCIES Property module: material editor: Other→Gasket→Gasket Transverse Shear Elasticity Choosing a unit system to define the transverse shear behavior The transverse shear stiffness is defined with units of stress per unit displacement, force per unit displacement, or force per unit length per unit displacement. The unit system used to define the transverse shear behavior must be consistent with the unit system used for the thickness-direction behavior. Providing the stiffness with units of stress per unit displacement You can define the transverse shear stiffness in units of stress per unit displacement for all gasket element types. The stiffness will be used to compute transverse shear stresses, which are available for output or visualization. Input File Usage: *GASKET ELASTICITY, COMPONENT=TRANSVERSE SHEAR, VARIABLE=STRESS Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Transverse Shear Elasticity: Units: Stress Providing the stiffness with other units You can define the transverse shear stiffness in units of force (or force per unit length) per unit displacement only for link elements and three-dimensional line elements. This method is suited for cases where the gasket cross-section in the 1–2 or 1–3 plane varies greatly with deformation because it would be too expensive to model such a deformation mechanism with a full two- or three-dimensional model, as explained earlier. When using two- or three-dimensional link elements, you must specify the stiffness in terms of units of force per unit displacement. Abaqus/Standard will use this stiffness to compute transverse shear forces, which are available for output or visualization. When using axisymmetric link elements and three-dimensional line elements, you must specify the stiffness in terms of units of force per unit length per unit displacement. Abaqus/Standard will use this stiffness to compute transverse shear forces per unit length, which are available for output or visualization. Input File Usage: Abaqus/CAE Usage: *GASKET ELASTICITY, COMPONENT=TRANSVERSE SHEAR, VARIABLE=FORCE Property module: material editor: Other→Gasket→Gasket Transverse Shear Elasticity: Units: Force Defining the membrane behavior of the gasket You can define the linear elastic behavior of the gasket by giving Young’s modulus and Poisson’s ratio. These data can be provided as a function of temperature and/or field variables. If you do not specify the linear elastic behavior of the gasket, the gasket has no membrane stiffness. In this case you must ensure that the nodes of the elements are restrained adequately in the directions orthogonal to the thickness direction of the gasket. Input File Usage: Abaqus/CAE Usage: *GASKET ELASTICITY, COMPONENT=MEMBRANE, DEPENDENCIES Property module: material editor: Other→Gasket→Gasket Membrane Elasticity Defining thermal expansion for the membrane and thickness-direction behaviors You can define isotropic thermal expansion to specify the same coefficient of thermal expansion for the membrane and thickness-direction behaviors. Alternatively, you can define orthotropic thermal expansion to specify three different coefficients of thermal expansion. The first coefficient will apply to the thermal expansion of the gasket in the thickness direction; the other two coefficients will apply to the expansion of the gasket in the local 2- and 3-directions, respectively. The membrane thermal strains, , are obtained as explained in “Thermal expansion,” Section 26.1.2. Abaqus/Standard computes the thermal closure for the thickness direction as initial gap initial void initial thickness so that the “mechanical” closure is obtained as You can specify the initial gap and initial void as part of the gasket section definition; the initial thickness is obtained directly from the nodal coordinates of the gasket elements, or you can specify it as part of the gasket section definition . If user subroutine UEXPAN is used to define the thermal expansion of the gasket, the incremental thermal strains must be provided in the subroutine. The thermal closure will be obtained from the thermal strain in the thickness direction, as described above. Input File Usage: Use either of the following options to define the thermal expansion directly: *EXPANSION, TYPE=ISO *EXPANSION, TYPE=ORTHO Use either of the following options to define the thermal expansion in user subroutine UEXPAN: *EXPANSION, TYPE=ISO, USER *EXPANSION, TYPE=ORTHO, USER Property module: material editor: Mechanical→Expansion: Use user subroutine UEXPAN (optional) Abaqus/CAE Usage: Defining creep behavior for the thickness-direction behavior You can define creep behavior in the thickness direction of the gasket only when the elastic-plastic model is used. The creep closure rate will be obtained as initial thickness initial gap initial void where is obtained as explained in “Rate-dependent plasticity: creep and swelling,” Section 23.2.4. You can specify the initial gap and initial void as part of the gasket section definition; the initial thickness is obtained directly from the nodal coordinates of the gasket elements, or you can specify it as part of the gasket section definition . If user subroutine CREEP is used to define the rate-dependent thickness-direction response of the gasket, the compressive creep strain increment must be provided in the subroutine. The creep closure will be obtained from the creep strain, as described above. Input File Usage: Use the following option to define the creep behavior directly: *CREEP Use the following option to define the creep behavior in user subroutine CREEP: Abaqus/CAE Usage: *CREEP, LAW=USER Property module: material editor: Mechanical→Plasticity→Creep: Law: User-defined (optional) Defining viscoelastic behavior for the thickness-direction behavior You can define viscoelastic behavior in the thickness direction of the gasket only when the elastic- damage model is used. Only frequency domain viscoelastic behavior is supported. This behavior is useful for modeling the steady-state dynamic response of automotive components with gaskets about some pre-loaded base state, such as would be obtained at the end of a nonlinear sealing analysis, to determine the noise-vibration-harshness (NVH) characteristics of the system. During the nonlinear sealing analysis step the frequency-domain viscoelastic behavior is ignored, and the material response is determined by the long-term elastic properties of the material. It is generally accepted (Zubeck and Marlow, 2002) that the dynamic stiffness and damping characteristics of automotive components such as gaskets and grommets vary with the frequency of excitation as well as the level of preload. These structural properties also depend on the geometry and the level of confinement of the gasket. This capability allows the direct specification of such dynamic properties as quantified by the effective storage and loss moduli in the thickness-direction, as tabular functions of the frequency of excitation and the level of preload. The preload is quantified by the amount of closure in the base state about which the steady-state dynamic response is desired. In determining the dynamic response of the gasket, the long-term elastic response is assumed to be defined by the nonlinear elastic model with damage. The steady-state dynamic response is assumed to be a perturbation about a base state defined by this elastic damage behavior at a certain value of closure. The viscoelastic response can be specified using two approaches, as discussed below. Direct specification of the properties The first approach involves direct (tabular) specification of the thickness-direction loss and storage moduli as functions of excitation frequency at different levels of closure. Input File Usage: Abaqus/CAE Usage: *VISCOELASTIC, TYPE=TRACTION, PRELOAD=UNIAXIAL Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Frequency and Frequency: Tabular Specification of properties in terms of ratios The second approach allows the specification of the ratio of both the thickness-direction storage and the loss moduli to the long-term thickness-direction elastic modulus. These ratios can be specified as tabular functions of the excitation frequency but are assumed to be independent of the amount of closure. The actual storage or loss modulus at any given level of closure is computed by multiplying the appropriate ratio with the long-term elastic modulus at the current value of closure (of the base state). See “Frequency domain viscoelasticity,” Section 22.7.2, for a summary of the second approach in the context of continuum material viscoelastic properties (the approach used here is just a one-dimensional specialization of the more general approach presented there). Input File Usage: Abaqus/CAE Usage: *VISCOELASTIC, TYPE=TRACTION Property module: material editor: Mechanical→Elasticity→Viscoelastic: Domain: Frequency and Frequency: Tabular Defining the contact area for average contact pressure output When the thickness-direction behavior of the gasket is defined in terms of force or force per unit length versus closure, Abaqus/Standard will provide the thickness-direction force or force per unit length as output variable S11. In this case you can define either a contact width or contact area versus closure curve that will be used to obtain the average “contact” pressure at each integration point as output variable CS11. This average pressure considers the changing contact area that occurs as a result of the deformation of a gasket, as shown in Figure 32.6.6–1. The closure used for input of this curve corresponds to the total mechanical closure, defined as the sum of the elastic, plastic, and creep closures. When two- and three-dimensional link gasket elements are used, you should specify the contact area versus mechanical closure in tabular form. When axisymmetric link and three-dimensional line elements are used, you should specify the contact width versus mechanical closure in tabular form. A typical curve is shown in Figure 32.6.6–7. area mechanical closure Figure 32.6.6–7 Specification of contact area versus mechanical closure for output of average pressure. You must specify the area at zero closure, then the area at increasing closures. The area is constant when the mechanical closure is negative and is extrapolated from the slope computed from the last two user-specified data points if the closure reaches values that are greater than the last user-specified closure. Area versus closure curves can be provided as a function of temperature and field variables. Input File Usage: *GASKET CONTACT AREA, DEPENDENCIES Abaqus/CAE Usage: Property module: material editor: Other→Gasket→Gasket Thickness Behavior: Units: Force, Suboptions→Contact Area Specific output for directly defined gasket behavior Output variable E is usually used in Abaqus/Standard to output strain. For gasket elements with behavior defined by a gasket behavior model this output variable has thickness-direction and transverse shear components with units of displacement and membrane strains. Output variable NE is used to output an effective strain. The effective strain components are computed as follows: NE11 NE11 NE22 NE33 NE12 NE13 NE23 E11 initial thickness initial gap) for perturbation steps; otherwise E11 initial gap initial thickness initial gap)); and E22 E33 E12 initial thickness E13 (initial thickness E23 The output variables THE, PE, or CE can also be used for gasket elements to output generalized thermal strains, plastic strains, or creep strains, respectively. For all stress/strain output variables the 11-component refers to the through-thickness direction; the 22-, 33- and 23-components refer to two direct and one shear membrane component, respectively; the remaining 12- and 13-components refer to the transverse shear components. For details about these definitions, see “Gasket elements: overview,” Section 32.6.1. The output of the elastic strain energy (output variable ALLSE) also contains the energy due to damage or change in elasticity as a function of plasticity. Therefore, this energy is usually not fully recoverable. Additional reference • Zubeck, M. W., and R. S. Marlow, “Local-Global Finite Element Analysis for Cam Cover Noise Reduction,” Society of Automotive Engineering, Inc., no. SAE 2003–01–1725, 2003. 32.6.7 TWO-DIMENSIONAL GASKET ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/CAE References • “Gasket elements: overview,” Section 32.6.1 • “Choosing a gasket element,” Section 32.6.2 • *GASKET SECTION Overview This section provides a reference to the two-dimensional gasket elements available in Abaqus/Standard. Element types Link elements GK2D2 2-node, two-dimensional gasket element GK2D2N 2-node, two-dimensional gasket element with thickness-direction behavior only Active degrees of freedom 1 for gasket elements with thickness-direction behavior only. 1, 2 for other gasket elements. Additional solution variables None. General elements GKPS4 GKPE4 4-node, plane stress gasket element 4-node, plane strain gasket element GKPS4N 4-node, two-dimensional gasket element with thickness-direction behavior only GKPS6 GKPE6 6-node, plane stress gasket element 6-node, plane strain gasket element GKPS6N 6-node, two-dimensional gasket element with thickness-direction behavior only Active degrees of freedom 1 for gasket elements with thickness-direction behavior only. 1, 2 for other gasket elements. Additional solution variables None. Nodal coordinates required Element property definition You must define the element’s cross-sectional area (for link elements) or out-of-plane width (for general elements), initial gap, and initial void. You can specify the thickness direction as part of the gasket section definition or by specifying a normal direction at the nodes; you can specify the element thickness as part of the gasket section definition. Otherwise, Abaqus/Standard will calculate the thickness direction. For link elements the thickness direction is the direction from the first to the second node and the thickness is the distance between the nodes. For general elements the thickness direction is based on the midsurface of the element and the thicknesses at the integration points are based on the nodal positions. See “Defining the gasket element’s initial geometry,” Section 32.6.4, for more details. Input File Usage: Abaqus/CAE Usage: *GASKET SECTION Property module: Create Section: select Other as the section Category and Gasket as the section Type Element-based loading None. Element output GK2D2 elements S11 CS11 S12 E11 E12 NE11 NE12 Pressure or thickness-direction force in the gasket element. Contact pressure in the gasket element (only available if S11 is the force in the gasket element and the gasket response is not defined using a material model). Shear stress or shear force. Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Shear motion if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain in the gasket element. Effective shear strain in the gasket element. GK2D2N elements S11 CS11 E11 NE11 Pressure or thickness-direction force in the gasket element. Contact pressure in the gasket element (only available if S11 is the force in the gasket element and the gasket response is not defined using a material model). Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain in the gasket element. General elements with thickness-direction behavior only S11 E11 Pressure in the gasket element. Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. NE11 Effective thickness-direction strain in the gasket element. Other general elements Pressure in the gasket element. Direct membrane stress. Direct membrane stress (only available for plane strain elements). Shear stress. Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Direct membrane strain. Direct membrane strain (only available for plane strain elements). Shear motion if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain in the gasket element. Direct membrane strain. Direct membrane strain (only available for plane strain elements). Effective shear strain. 32.6.7–3 S11 S22 S33 S12 E11 E22 E33 E12 NE11 NE22 NE33 Node ordering and integration point numbering Link elements 2 - node element General elements 4 - node element 6 - node element THREE-DIMENSIONAL GASKET ELEMENT LIBRARY 3-D GASKET ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/CAE References • “Gasket elements: overview,” Section 32.6.1 • “Choosing a gasket element,” Section 32.6.2 • *GASKET SECTION Overview This section provides a reference to the three-dimensional gasket elements available in Abaqus/Standard. Element types Link elements GK3D2 2-node, three-dimensional gasket element GK3D2N 2-node, three-dimensional gasket element with thickness-direction behavior only Active degrees of freedom 1 for gasket elements with thickness-direction behavior only. 1, 2, 3 for other gasket elements. Additional solution variables None. Line elements GK3D4L 4-node, three-dimensional line gasket element GK3D4LN 4-node, three-dimensional line gasket element with thickness-direction behavior only GK3D6L 6-node, three-dimensional line gasket element GK3D6LN 6-node, three-dimensional line gasket element with thickness-direction behavior only Active degrees of freedom 1 for gasket elements with thickness-direction behavior only. 1, 2, 3 for other gasket elements. Additional solution variables None. Area elements GK3D6 6-node, three-dimensional gasket element GK3D6N 6-node, three-dimensional gasket element with thickness-direction behavior only GK3D8 8-node, three-dimensional gasket element GK3D8N 8-node, three-dimensional gasket element with thickness-direction behavior only GK3D12M 12-node, three-dimensional gasket element GK3D12MN 12-node, three-dimensional gasket element with thickness-direction behavior only GK3D18 18-node, three-dimensional gasket element GK3D18N 18-node, three-dimensional gasket element with thickness-direction behavior only Active degrees of freedom 1 for gasket elements with thickness-direction behavior only. 1, 2, 3 for other gasket elements. Additional solution variables None. Nodal coordinates required Element property definition You must define the element’s initial gap and initial void, as well as the cross-sectional area (for link elements) or width (for line elements). You can specify the thickness direction as part of the gasket section definition or by specifying a normal direction at the nodes; you can specify the element thickness as part of the gasket section definition. Otherwise, Abaqus/Standard will calculate the thickness direction and the thickness. For link elements the thickness direction is the direction from the first to the second node and the thickness is the distance between the nodes. For line elements the thickness direction is the direction from the bottom node to the top node associated with the integration point and the thicknesses are the distances between these same bottom and top nodes. For area elements the thickness direction is based on the midsurface of the element and the thicknesses at the integration points are based on the nodal positions. See “Defining the gasket element’s initial geometry,” Section 32.6.4, for more details. Input File Usage: Abaqus/CAE Usage: *GASKET SECTION Property module: Create Section: select Other as the section Category and Gasket as the section Type Element-based loading None. Element output GK3D2 elements S11 CS11 S12 S13 E11 E12 E13 NE11 NE12 NE13 Pressure or thickness-direction force in the gasket element. Contact pressure in the gasket element (only available if S11 is a force and the gasket response is not defined using a material model). Shear stress or shear force. Shear stress or shear force. Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Shear motion if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Shear motion if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain in the gasket element. Effective shear strain. Effective shear strain. GK3D2N elements S11 CS11 E11 NE11 Pressure or thickness-direction force in the gasket element. Contact pressure in the gasket element (only available if S11 is a force and the gasket response is not defined using a material model.) Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain in the gasket element. Line elements with thickness-direction behavior only S11 CS11 E11 NE11 Pressure or thickness-direction force per unit length in the gasket element. Contact pressure in the gasket element (only available if S11 is a force per unit length and the gasket response is not defined using a material model). Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain in the gasket element. Other line elements S11 CS11 S22 S12 S13 E11 E22 E12 E13 NE11 NE22 NE12 NE13 Pressure or thickness-direction force per unit length in the gasket element. Contact pressure in the gasket element (only available if S11 is a force per unit length and the gasket response is not defined using a material model). Direct membrane stress. Shear stress or shear force per unit length. Shear stress or shear force per unit length. Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Direct membrane strain. Shear motion if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Shear motion if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain in the gasket element. Direct membrane strain. Effective shear strain. Effective shear strain. Area elements with thickness-direction behavior only S11 E11 NE11 Pressure in the gasket element. Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain in the gasket element. Other area elements S11 S22 S33 S12 S13 S23 E11 E22 E33 Pressure in the gasket element. Direct membrane stress. Direct membrane stress. Transverse shear stress. Transverse shear stress. Membrane shear stress. Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Direct membrane strain. Direct membrane strain. Transverse shear motion if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Transverse shear motion if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Membrane shear strain. Effective thickness-direction strain in the gasket element. Direct membrane strain. Direct membrane strain. Effective shear strain. Effective shear strain. Membrane shear strain. E12 E13 E23 NE11 NE22 NE33 NE12 NE13 NE12 Node ordering and integration point numbering Link elements 2 - node element Line elements 4 - node element 6 - node element 32.6.8–5 Area elements 6 - node element 12 10 11 12 - node element 11 12 15 14 16 18 13 17 10 8 - node element 18 - node element Integration points are indicated with an X and have the same numbers as the bottom face nodes, except that the point between nodes 17 and 18 in the 18-node gasket element is integration point number 9. 32.6.9 AXISYMMETRIC GASKET ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/CAE References • “Gasket elements: overview,” Section 32.6.1 • “Choosing a gasket element,” Section 32.6.2 • *GASKET SECTION Overview This section provides a reference to the axisymmetric gasket elements available in Abaqus/Standard. Element types Link elements GKAX2 2-node, axisymmetric gasket element GKAX2N 2-node, axisymmetric gasket element with thickness-direction behavior only Active degrees of freedom 1 for gasket elements with thickness-direction behavior only. 1, 2 for other gasket elements. Additional solution variables None. General elements GKAX4 4-node, axisymmetric gasket element GKAX4N 4-node, axisymmetric gasket element with thickness-direction behavior only GKAX6 6-node, axisymmetric gasket element GKAX6N 6-node, axisymmetric gasket element with thickness-direction behavior only Active degrees of freedom 1 for gasket elements with thickness-direction behavior only. 1, 2 for other gasket elements. Additional solution variables None. Nodal coordinates required Element property definition You must define the element’s initial gap and initial void. In addition, for link elements you must define the element’s width. You can specify the thickness direction as part of the gasket section definition or by specifying a normal direction at the nodes; you can specify the element thickness as part of the gasket section definition. Otherwise, Abaqus/Standard will calculate the thickness direction and the thickness. For link elements the thickness direction is the direction from the first to the second node and the thickness is the distance between the nodes. For general elements the thickness direction is based on the midsurface of the element and the thicknesses at the integration points are based on the nodal positions. See “Defining the gasket element’s initial geometry,” Section 32.6.4, for more details. Input File Usage: Abaqus/CAE Usage: *GASKET SECTION Property module: Create Section: select Other as the section Category and Gasket as the section Type Element-based loading None. Element output GKAX2 elements S11 CS11 S22 S12 E11 E22 E12 NE11 NE22 NE12 Pressure or thickness-direction force per unit length in the gasket element. Contact pressure in the gasket element (only available if S11 is a force per unit length and the gasket response is not defined using a material model). Hoop stress. Shear stress or shear force per unit length. Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Hoop strain. Shear motion if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain. Hoop strain. Effective shear strain. GKAX2N elements S11 CS11 E11 NE11 Pressure or thickness-direction force per unit length in the gasket element. Contact pressure in the gasket element (only available if S11 is a force per unit length and the gasket response is not defined using a material model). Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain. General elements with thickness-direction behavior only S11 E11 Pressure in the gasket element. Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. NE11 Effective thickness-direction strain. Other general elements S11 S22 S33 S12 E11 E22 E33 E12 NE11 NE22 NE33 NE12 Pressure in the gasket element. Direct membrane stress. Hoop stress. Shear stress. Gasket closure if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Direct membrane strain. Hoop strain. Shear motion if the gasket response is defined directly using a gasket behavior model; strain if the gasket response is defined using a material model. Effective thickness-direction strain. Direct membrane strain. Direct membrane strain. Effective shear strain. Node ordering and integration point numbering Link elements 2 - node element General elements 4 - node element 6 - node element 32.7 Surface elements • “Surface elements,” Section 32.7.1 • “General surface element library,” Section 32.7.2 • “Cylindrical surface element library,” Section 32.7.3 • “Axisymmetric surface element library,” Section 32.7.4 32.7.1 SURFACE ELEMENTS Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “General surface element library,” Section 32.7.2 • “Cylindrical surface element library,” Section 32.7.3 • “Axisymmetric surface element library,” Section 32.7.4 • *SURFACE SECTION • “Creating surface sections,” Section 12.13.9 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Surface elements: • are defined just like membrane elements—as surfaces in space; • have no inherent stiffness; • may have mass per unit area; • may be used to define rigid bodies; • may be used in the definition of surfaces and surface-based tie constraints; • behave just like membrane elements with zero thickness; • may be used with rebar layers; • can be embedded in solid elements; • can transmit only in-plane forces; and • have no bending stiffness or transverse shear stiffness. Typical applications Surface elements are useful in several special modeling cases: • They are used to carry rebar layers to represent thin stiffening components in solid structures. The stiffness and mass of the rebar layers are added to the surface elements . The reinforced surface elements can also be embedded in “host” solid elements . • They are used to bring additional mass into the model in the form of a mass per unit area; for example, to spread the mass of fuel in a tank over the tank surface, particularly when the tank is modeled with solid elements. • They are used to specify a surface used in a constraint, when that surface does not have structural properties. • When used in conjunction with a surface-based tie constraint, they are used to specify distributed surface loading, such as incident wave loading, on beam elements. • In Abaqus/Explicit (when used in conjunction with a surface-based tie constraint) they can be used to specify a complex surface on beam elements for use in general contact. The stiffness of the penalty springs used to enforce contact constraints is approximately proportional to the mass of the surface nodes. Contact will not be enforced if the surface nodes have no mass. • In Abaqus/Explicit they can be used to define all or part of the boundary for a surface-based fluid cavity (for example, see “Hydrostatic fluid elements: modeling an airspring,” Section 1.1.9 of the Abaqus Example Problems Manual). Choosing an appropriate element In addition to the general surface elements available in both Abaqus/Standard and Abaqus/Explicit, cylindrical surface elements and axisymmetric surface elements are available in Abaqus/Standard only. General surface elements General surface elements should be used in three-dimensional models in which the deformation of the structure can evolve in three dimensions. Cylindrical surface elements Cylindrical surface elements are available in Abaqus/Standard for precise modeling of regions in a structure with circular geometry, such as a tire. The elements make use of trigonometric functions to interpolate displacements along the circumferential direction and use regular isoparametric interpolation in the in-plane direction. They use three nodes along the circumferential direction and can span a segment between 0° and 180°. Elements with both first-order and second-order interpolation in the in-plane direction are available. The geometry of the element is defined by specifying nodal coordinates in a global Cartesian system. These elements can be used in the same mesh with regular surface elements. They can also be embedded in general solid and cylindrical elements. Axisymmetric surface elements The axisymmetric surface elements available in Abaqus/Standard are divided into two categories: those that do not allow twist about the symmetry axis and those that do. These elements are referred to as the regular and generalized axisymmetric surface elements, respectively. The generalized axisymmetric surface elements (axisymmetric surface elements with twist) allow a circumferential component of loading, which may cause twist about the symmetry axis. The circumferential load component is independent of the circumferential coordinate . Since there is no dependence of the loading on the circumferential coordinate, the deformation is axisymmetric. The generalized axisymmetric surface elements cannot be used in dynamic or eigenfrequency extraction procedures. Naming convention The naming convention for surface elements depends on the element dimensionality. General surface elements General surface elements in Abaqus are named as follows: SF 3D 4 R reduced integration (optional) number of nodes three-dimensional membrane-like surface For example, SFM3D4R is a three-dimensional, 4-node surface element with reduced integration. Cylindrical surface elements Cylindrical surface elements in Abaqus/Standard are named as follows: SF M CL 6 number of nodes cylindrical membrane-like surface For example, SFMCL6 is a 6-node cylindrical surface element with circumferential interpolation. Axisymmetric surface elements Axisymmetric surface elements in Abaqus/Standard are named as follows: SF G AX 2 order of interpolation axisymmetric generalized (optional) membrane-like surface For example, SFMAX2 is a regular axisymmetric, quadratic-interpolation surface element. Element normal definition The “top” surface of a surface element is the surface in the positive normal direction (defined below) and is called the SPOS face for contact definition. The “bottom” surface is in the negative direction along the normal and is called the SNEG face for contact definition. General surface elements For general surface elements the positive normal direction is defined by the right-hand rule going around the nodes of the element in the order that they are specified in the element definition. See Figure 32.7.1–1. face SPOS face SNEG Figure 32.7.1–1 Positive normals for general surface elements. Cylindrical surface elements The positive normal direction is defined by the right-hand rule going around the nodes of the element in the order that they are specified in the element definition. See Figure 32.7.1–2. face SNEG face SPOS Figure 32.7.1–2 Positive normals for cylindrical surface elements. Axisymmetric surface elements For axisymmetric surface elements the positive normal is defined by a 90° counterclockwise rotation from the direction going from node 1 to node 2. See Figure 32.7.1–3. face SPOS face SNEG Figure 32.7.1–3 Positive normals for axisymmetric surface elements. Defining the element’s section properties You must associate the surface section properties with a region of your model. Input File Usage: *SURFACE SECTION, ELSET=name where the ELSET parameter refers to a set of surface elements. Abaqus/CAE Usage: Property module: Create Section: select Shell as the section Category and Surface as the section Type Assign→Section: select regions Using a surface element to carry rebar layers You can define layers of reinforcement that are carried by the surface element. The stiffness and mass due to the rebar layers are added to the surface element. Input File Usage: Use both of the following options: Abaqus/CAE Usage: *SURFACE SECTION, ELSET=name *REBAR LAYER Property module: Create Section: select Shell as the section Category and Surface as the section Type, Rebar Layers Using a surface element to bring additional mass into the model You can define the mass per unit area carried by the surface element. Input File Usage: Abaqus/CAE Usage: *SURFACE SECTION, ELSET=name, DENSITY=number Property module: Create Section: select Shell as the section Category and Surface as the section Type, toggle on Density: number Using a surface element in a constraint Surface elements can be used to define a surface in Abaqus, and this surface can be used in a surface- based tie constraint . Input File Usage: Use the following options: *SURFACE, NAME=surface_name *TIE, NAME=name surface_name, master_name Abaqus/CAE Usage: In Abaqus/CAE you can select one or more faces directly in the viewport when you are prompted to select a surface. In addition, you can define surfaces as collections of faces and edges using the Surface toolset. Interaction module: Create Constraint: Tie 32.7.2 GENERAL SURFACE ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE References • “Surface elements,” Section 32.7.1 • *SURFACE SECTION • *REBAR LAYER Overview This section provides a reference to the surface elements available in Abaqus/Standard and Abaqus/Explicit. Element types SFM3D3 3-node triangle SFM3D4(S) 4-node quadrilateral SFM3D4R 4-node quadrilateral, reduced integration SFM3D6(S) SFM3D8(S) 6-node triangle 8-node quadrilateral SFM3D8R(S) 8-node quadrilateral, reduced integration Active degrees of freedom 1, 2, 3 Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition Input File Usage: Use the following option to define surface element properties: *SURFACE SECTION If rebar are being defined, use the following option in conjunction with the *SURFACE SECTION option: *REBAR LAYER Use the following option to define a mass density per unit area: *SURFACE SECTION, DENSITY=number Property module: Create Section: select Shell as the section Category and Surface as the section Type, Rebar Layers (optional) You cannot define the mass per unit area for a surface section in Abaqus/CAE. Abaqus/CAE Usage: Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Gravity, centrifugal, rotary acceleration, and Coriolis force loads apply only if the surface elements have rebar defined or if the elements have a defined density. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BX BY BZ BXNU Body force Body force Body force Body force FL−2 FL−2 FL−2 FL−2 BYNU Body force FL−2 BZNU Body force FL−2 Body force in the global X-direction. Body force in the global Y-direction. Body force in the global Z-direction. in force Nonuniform body the global X-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. in force the Nonuniform body global Y-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. in force Nonuniform body the global Z-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. CENT(S) Not supported FL−3 (ML−2 T−2 ) CENTRIF(S) Rotational body force T−2 Centrifugal load (magnitude is input is the mass density as per unit area, is the angular speed). , where Centrifugal load (magnitude is input as is the angular speed). , where Units Description Load ID (*DLOAD) CORIO(S) Abaqus/CAE Load/Interaction Coriolis force FL−3 T (ML−2 T−1 ) GRAV Gravity LT−2 HP(S) Not supported FL−2 Pressure FL−2 PNU Not supported FL−2 , where Coriolis force (magnitude is input as is the mass density per unit area, is the angular speed). The load stiffness due to Coriolis loading is not accounted for in direct steady- state dynamics analysis. loading Gravity direction (magnitude is acceleration). in specified input as Hydrostatic pressure applied to the element reference surface and linear in global Z. The pressure is positive in the direction of the positive element normal. Pressure applied to the element reference surface. The pressure is positive in the direction of the positive element normal. applied reference to Nonuniform pressure surface the element via with magnitude in subroutine user VDLOAD Abaqus/Standard in Abaqus/Explicit. The pressure is positive in the direction of the positive element normal. supplied DLOAD and ROTA(S) SBF(E) SP(E) Rotational body force T−2 Not supported FL−5 T2 Not supported FL−4 T2 TRSHR Surface traction FL−2 Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Stagnation body force in global X-, Y-, and Z-directions. Stagnation pressure applied to the element reference surface. traction Shear reference surface. on the element Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description TRSHRNU(S) Not supported FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Not supported FL−2 VBF(E) VP(E) Not supported FL−4 T Not supported FL−3 T traction on the Nonuniform shear element surface with reference magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction Nonuniform general on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. Viscous body force in global X-, Y-, and Z-directions. surface pressure Viscous applied reference surface. to the element The pressure is proportional to the velocity normal to the element face and opposing the motion. Foundations Foundations are available only in Abaqus/Standard and are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE Elastic foundation Units Description FL−2 Elastic foundation. Surface-based loading Distributed loads Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description HP(S) Pressure FL−2 Hydrostatic pressure on the element reference surface and linear in global Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description Pressure FL−2 PNU Pressure FL−2 SP(E) Pressure FL−4 T2 TRSHR Surface traction FL−2 TRSHRNU(S) Surface traction FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 VP(E) Pressure FL−3 T Z. The pressure is positive in the direction opposite to the surface normal. Pressure on the element reference surface. The pressure is positive in the direction opposite to the surface normal. Nonuniform pressure on the element reference surface with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. The pressure is positive in the direction opposite to the surface normal. Stagnation pressure applied to the element reference surface. traction Shear reference surface. on the element traction on the Nonuniform shear element surface with reference magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction on Nonuniform general the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. Viscous surface pressure applied to the element reference surface. The pressure is proportional to the velocity normal to the element surface and opposing the motion. Incident wave loading Surface-based incident wave loading is also available for these elements. See “Acoustic and shock loads,” Section 33.4.6. Element output Output is currently available only when the surface element is used to carry rebar layers. See “Defining reinforcement,” Section 2.2.3, for details. Node ordering on elements 1 2 3 - node element 4 - node element 6 5 1 2 4 7 3 6 - node element 8 - node element Numbering of integration points for output 6 5 1 2 1 2 3 - node element 6 - node element 4 - node element 4 - node reduced integration element 4 7 3 4 7 3 8 - node element 8 - node reduced integration element CYLINDRICAL SURFACE ELEMENT LIBRARY CYLINDRICAL SURFACE ELEMENTS Product: Abaqus/Standard References • “Surface elements,” Section 32.7.1 • *SURFACE SECTION • *REBAR LAYER Overview This section provides a reference to the cylindrical surface elements available in Abaqus/Standard. Element types SFMCL6 6-node cylindrical surface SFMCL9 9-node cylindrical surface Active degrees of freedom 1, 2, 3 Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition Input File Usage: Use the following option to define surface element properties: *SURFACE SECTION If rebar are being defined, use the following option in conjunction with the *SURFACE SECTION option: *REBAR LAYER Use the following option to define a mass density per unit area: *SURFACE SECTION, DENSITY=number Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Gravity, centrifugal, rotary acceleration, and Coriolis force loads apply only if the surface elements have rebar defined or if the elements have a defined density. Units Description Body force in the global X-direction. Body force in the global Y-direction. Body force in the global Z-direction. Nonuniform body force in the global X-direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in the global Y-direction with magnitude supplied via user subroutine DLOAD. Nonuniform body force in the global Z-direction with magnitude supplied via user subroutine DLOAD. Centrifugal load (magnitude is input as where is the angular speed). is the mass density per unit area, Centrifugal load (magnitude is input as where is the angular speed). , , Coriolis force (magnitude is input as where , is the mass density per unit area, is the angular speed). The load stiffness due to Coriolis loading is not accounted for in direct steady-state dynamics analysis. Gravity loading in a specified direction (magnitude is input as acceleration). Hydrostatic pressure applied to the element reference surface and linear in global Z. The 32.7.3–2 Load ID (*DLOAD) BX BY BZ BXNU BYNU BZNU FL−3 FL−2 FL−2 FL−2 FL−2 FL−2 CENT FL−3 (ML−2 T−2 ) CENTRIF T−2 CORIO FL−3 T (ML−2 T−1 ) GRAV HP LT−2 Load ID (*DLOAD) Units Description PNU ROTA TRSHR FL−2 FL−2 T−2 FL−2 TRSHRNU(S) FL−2 TRVEC FL−2 TRVECNU(S) FL−2 pressure is positive in the direction of the positive element normal. Pressure applied to the element reference surface. The pressure is positive in the direction of the positive element normal. Nonuniform pressure applied to the element reference surface with magnitude supplied via user subroutine DLOAD. Rotary acceleration load (magnitude is input as is the rotary acceleration). , where Shear traction on the element reference surface. Nonuniform shear traction on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. General traction on the element reference surface. Nonuniform general traction on the element reference surface with magnitude and subroutine direction supplied via user UTRACLOAD. Foundations Foundations are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Units Description FL−2 Elastic foundation. Surface-based loading Distributed loads Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Units Description HP PNU FL−2 FL−2 FL−2 TRSHR FL−2 TRSHRNU(S) FL−2 TRVEC FL−2 TRVECNU(S) FL−2 on pressure Hydrostatic element reference surface and linear in global Z. The pressure is positive in the direction opposite to the surface normal. the Pressure on the element reference surface. The pressure is positive in the direction opposite to the surface normal. Nonuniform pressure on the element reference surface with magnitude supplied via user subroutine DLOAD. The pressure is positive in the direction opposite to the surface normal. Shear traction on the element reference surface. Nonuniform shear traction on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. General traction on the element reference surface. Nonuniform general traction on the element reference surface with magnitude and subroutine direction supplied via user UTRACLOAD. Incident wave loading Surface-based incident wave loading is also available for these elements. See “Acoustic and shock loads,” Section 33.4.6. Element output Output is currently available only when the surface element is used to carry rebar layers. See “Defining reinforcement,” Section 2.2.3, for details. Node ordering and face numbering on elements 6-node element 9-node element Numbering of integration points for output 6-node element 9-node element AXISYMMETRIC SURFACE ELEMENT LIBRARY AXISYMMETRIC SURFACE LIBRARY Products: Abaqus/Standard Abaqus/CAE References • “Surface elements,” Section 32.7.1 • *SURFACE SECTION • *REBAR LAYER Overview This section provides a reference to the axisymmetric surface elements available in Abaqus/Standard. Conventions Coordinate 1 is r, coordinate 2 is z. At , the r-direction corresponds to the global X-direction and the z-direction corresponds to the global Y-direction. This is important when data must be given in global directions. Coordinate 1 should be greater than or equal to zero. Degree of freedom 1 is have an additional degree of freedom, 5, corresponding to the twist angle , degree of freedom 2 is . Generalized axisymmetric elements with twist (in radians). Abaqus/Standard does not automatically apply any boundary conditions to nodes located along the symmetry axis. You must apply radial or symmetry boundary conditions on these nodes if desired. Point loads and moments should be given as the value integrated around the circumference; that is, the total value on the ring. Element types Regular axisymmetric surface elements SFMAX1 SFMAX2 2-node linear, without twist 3-node quadratic, without twist Active degrees of freedom 1, 2 Additional solution variables None. Generalized axisymmetric surface elements SFMGAX1 2-node linear, with twist SFMGAX2 3-node quadratic, with twist Active degrees of freedom 1, 2, 5 Additional solution variables None. Nodal coordinates required R, Z Element property definition Use the following option to define surface elements: *SURFACE SECTION If rebar are being defined, use the following option in conjunction with the *SURFACE SECTION option: *REBAR LAYER Use the following option to define a mass density per unit area: *SURFACE SECTION, DENSITY=number Property module: Create Section: select Shell as the section Category and Surface as the section Type, Rebar Layers (optional) You cannot define the mass per unit area for a surface section in Abaqus/CAE. Input File Usage: Abaqus/CAE Usage: Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Gravity and centrifugal loads apply only if the surface elements have rebar defined or if the elements have a defined density. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description BR BZ Body force Body force BRNU Body force FL−2 FL−2 FL−2 Body force in the radial (1 or r) direction. Body force in the axial (2 or z) direction. Nonuniform body force in the radial direction with magnitude supplied via user subroutine DLOAD. Abaqus/CAE Load/Interaction Units Description Load ID (*DLOAD) BZNU Body force FL−2 CENT Not supported FL−3 (ML−2 T−2 ) CENTRIF Rotational body force T−2 GRAV Gravity LT−2 HP Not supported FL−2 Pressure FL−2 PNU Not supported FL−2 Nonuniform body force in the axial direction with magnitude supplied via user subroutine DLOAD. Centrifugal load (magnitude is input is the mass density as , where per unit area, is the angular velocity). Since only axisymmetric deformation is allowed, the spin axis must be the z-axis. , where Centrifugal load (magnitude is input as the angular velocity). Since only axisymmetric deformation is allowed, the spin axis must be the z-axis. is Gravity direction acceleration). loading in (magnitude specified as input Hydrostatic pressure applied to the element reference surface and linear in global Z. The pressure is positive in the direction of the positive element normal. Pressure applied to the element reference surface. The pressure is positive in the direction of the positive element normal. applied reference to Nonuniform pressure the surface element with magnitude supplied via user subroutine DLOAD. The pressure is positive in the direction of the positive element normal. TRSHR Surface traction FL−2 TRSHRNU(S) Not supported FL−2 traction Shear reference surface. on the element Nonuniform shear reference element traction on the surface with Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description TRVEC Surface traction FL−2 TRVECNU(S) Not supported FL−2 magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction Nonuniform general on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. Foundations Foundations are specified as described in “Element foundations,” Section 2.2.2. Load ID (*FOUNDATION) Load/Interaction Abaqus/CAE Units Description Elastic foundation FL−2 Surface-based loading Distributed loads Elastic foundation. For SFMGAX1 and SFMGAX2 elements the elastic foundations are applied to degrees of freedom only. and Surface-based distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description Hydrostatic pressure applied to the element reference surface and linear in global Z. The pressure is positive in the direction opposite to the surface normal. Pressure applied to the element reference surface. The pressure is positive in the direction opposite to the surface normal. Nonuniform pressure element the reference applied to surface HP Pressure FL−2 Pressure FL−2 PNU Pressure FL−2 Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description TRSHR Surface traction FL−2 TRSHRNU(S) Surface traction FL−2 TRVEC Surface traction FL−2 TRVECNU(S) Surface traction FL−2 with magnitude supplied via user subroutine DLOAD. The pressure is positive in the direction opposite to the surface normal. traction Shear reference surface. on the element traction on the Nonuniform shear element surface with reference magnitude and direction supplied via user subroutine UTRACLOAD. General reference surface. traction on the element traction Nonuniform general on the element reference surface with magnitude and direction supplied via user subroutine UTRACLOAD. Incident wave loading Surface-based incident wave loading is also available for these elements. See “Acoustic and shock loads,” Section 33.4.6. Element output Output is currently available only when the surface element is used to carry rebar layers. See “Defining reinforcement,” Section 2.2.3, for details. Node ordering on elements 2 - node element 3 - node element Numbering of integration points for output 2 - node element 3 - node element 32.8 Tube support elements • “Tube support elements,” Section 32.8.1 • “Tube support element library,” Section 32.8.2 32.8.1 TUBE SUPPORT ELEMENTS Product: Abaqus/Standard References • “Tube support element library,” Section 32.8.2 • *ITS • *DASHPOT • *FRICTION • *SPRING Overview Tube support elements: • are provided to model the interaction of a tube with a closely adjacent tube support, for cases where intermittent contact between the tube and the support may occur; and • are made up of a spring/friction link (to simulate direct contact between the tube and the support) and a parallel dashpot (to simulate the effect of the fluid in the annulus between the tube and the support), as shown in Figure 32.8.1–1. Details of the element formulations can be found in “Tube support elements,” Section 3.9.4 of the Abaqus Theory Manual. Typical applications An ITSCYL element can be used to model a drilled hole support . Several ITSUNI elements can be attached to the same node of the beam elements representing the tube to model the case of a tube support made up of a series of straight segments, as in an “egg-crate” design . Choosing an appropriate element Two types of tube support elements are provided. ITSUNI elements ITSUNI is a “unidirectional” element, which always acts in a fixed direction in space. One node of the element must be located on the axis of the tube, which is modeled using beam elements; and the other node must be located equidistant between the two parallel support plates. The support plates are built into the ITSUNI element definition. P3 Spring ( linear or nonlinear ) Friction Dashpot ( linear or nonlinear ) P3 Figure 32.8.1–1 Tube support element behavior. ITSCYL elements ITSCYL is a “cylindrical” element, which can be used to simulate the interaction between a circular tube and a circular hole. One node of the element must be located on the axis of the tube, which is modeled using beam elements, and the other node must be located at the center of the hole in the circular tube support plate. The circular hole is built into the ITSCYL element definition. Defining the behavior of ITS elements You define the diameter of the tube and other geometric quantities that define the ITS element. You must associate these quantities with a set of ITS elements. In addition, you must define the behavior of the spring, friction link, and dashpot that make up a tube support element. Tube center Tube C of tube Tube support plate Center of hole ITSCYL element Figure 32.8.1–2 Use of an ITSCYL element for a drilled hole support. The spring behavior of an ITS element is shown in Figure 32.8.1–4. Relative displacements in the element are measured from the position where the tube and the hole in the support plate are aligned exactly—when the nodes of the element are at the same location. As indicated in Figure 32.8.1–4, the spring behavior of an ITS element is modified from that of the assigned spring definition to account for any clearance between the tube and support when the nodes of the element are at the same location. When there is no contact between the tube and the support, no force is transmitted by the spring; when the tube is in contact with the support, the force increases as the tube wall is deformed. This force can be modeled as a linear or a nonlinear function of the relative displacement between the axis of the tube and the center of the hole in the support. Tube ITSUNI elements Parallel support plates for element 2 C of tube n2 n1 Center of opening in support plates Parallel support plates for element 1 Figure 32.8.1–3 Use of ITSUNI elements for an “egg-crate” support. Friction between the tube and support will generate a moment at the tube node if the tube diameter is greater than zero and a moment at the hole node if the hole size is greater than zero. At least one of the following should be true for any node of an ITS element that will have a moment acting on it: • the node should be associated with a beam or other element that can carry a moment; • the nodal rotation should be set to zero with a boundary condition. Input File Usage: Use the following options to define the behavior of ITS elements: *ITS, ELSET=name *DASHPOT *SPRING *FRICTION P3 TUBE SUPPORT Stiffness associated with tube wall flattening -c0 c0 u3 c0 = clearance between tube and support side in fully aligned position P3 ITSCYL Stiffness associated with tube wall flattening c0 u3 c0 = difference between support plate hole radius and tube outside radius Figure 32.8.1–4 Nonlinear spring behavior in ITS elements to model clearance and tube flattening. 32.8.2 TUBE SUPPORT ELEMENT LIBRARY Product: Abaqus/Standard References • “Tube support elements,” Section 32.8.1 • *ITS Overview This section provides a reference to the tube support elements available in Abaqus/Standard. Element types ITSUNI ITSCYL Unidirectional tube support element Cylindrical geometry tube support element Active degrees of freedom 1, 2, 3, 4, 5, 6 Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition Input File Usage: *ITS Element-based loading Total direct force in the element. Tangential (shear) force component, caused by friction, in the plane of the cross- section of the tube. Tangential (shear) force component, caused by friction, parallel to the axis of the tube. 32.8.2–1 None. Element output S11 S12 The force in the spring link and the force in the dashpot are defined as generalized substresses and, therefore, are available as substress selections in the output options, as follows: SS1 SS2 Force in the spring link. Force in the dashpot. The relative axial and tangential displacements corresponding to the forces above are chosen by requesting the corresponding “strains,” except that “strain” component E13 is not defined in element type ITSCYL. The relative tangential (shear) displacement components during slip are available as “plastic strain” components PE12 and PE13. The “equivalent plastic strain” is defined in these elements as where and are the two relative tangential displacement components. Nodes associated with the element ITSUNI: Two nodes—one on the axis of the tube and one equidistant between the two parallel support plates. ITSCYL: Two nodes—one on the axis of the tube and one at the center of the hole in the support plate. 32.9 Line spring elements • “Line spring elements for modeling part-through cracks in shells,” Section 32.9.1 • “Line spring element library,” Section 32.9.2 LINE SPRING ELEMENTS FOR MODELING PART-THROUGH CRACKS IN SHELLS LINE SPRING ELEMENTS Product: Abaqus/Standard References • “Line spring element library,” Section 32.9.2 • *SHELL SECTION • *SURFACE FLAW Overview Line spring elements: • are used to evaluate part-through cracks (flaws) in shells inexpensively; • are used together with shell elements; • can be used with elastic or elastic-plastic (isotropic hardening, Mises yield) material behavior; • do not include thermal strain effects; • are written for small-displacement analysis only (large-rotation effects are not included); • are not available in linear perturbation steps; • use quite significant approximations (especially in the elastic-plastic case) and should, therefore, be used with care; • do not provide useful results for crack depths less than 2% or greater than 95% of the shell thickness; and • will not yield accurate results at the ends of the flaws or locations where the flaw depth varies rapidly with position, due to the three-dimensional nature of the solution in such areas. Typical applications Line spring elements provide inexpensive evaluation of part-through cracks in shells. The basic concept is that these elements introduce the local solution, dominated by the singularity at the crack tip, into a shell model of the uncracked geometry. This is accomplished by allowing an additional freedom in the model along the line of the crack, this freedom being provided by the line spring elements, as indicated in Figure 32.9.1–1. The compliance of the line spring with respect to these additional freedoms embeds the local solution in the global response. From the relative displacements and rotations conjugate to that compliance, Abaqus/Standard computes and prints out the J-integral and, in the linear case, stress intensity factors at integration points in the line spring elements. Because the elements are simple, the analysis is not significantly more expensive than a shell analysis of the uncracked geometry. The results provide acceptable accuracy for many common applications. shell elements typical line spring element Section A-A 'positive' crack (open on +n surface) 'negative' crack (open on -n surface) nodes representing opposite side of crack Figure 32.9.1–1 Line spring models. See “Line spring elements,” Section 3.9.5 of the Abaqus Theory Manual, for details of the theory behind these elements. Choosing an appropriate element Two versions of the element are provided—both are intended for use with the second-order shell elements (S8R, S8R5, S9R5). Line spring element LS6 is for general cases, while line spring element LS3S is for use when the flaw lies on a symmetry plane and only one side of the symmetry plane is modeled. Defining the element’s section properties You must associate the shell section properties with a set of line spring elements. Input File Usage: *SHELL SECTION, ELSET=name Defining a constant section thickness You can define a constant section thickness for the line spring element as part of the shell section definition. Input File Usage: *SHELL SECTION shell thickness Defining a variable section thickness Alternatively, you can define a line spring element with continuously varying thickness and specify the thickness of the line spring element at the nodes. In this case any constant section thickness you specify will be ignored, and the line spring thickness will be interpolated from the nodes . The thickness must be defined at all nodes connected to the element. Input File Usage: Use both of the following options: *SHELL SECTION, NODAL THICKNESS *NODAL THICKNESS Assigning a material definition to a set of line spring elements You must associate a material definition with each shell section definition. Line spring elements can be used with isotropic elastic or elastic-plastic (isotropic hardening, Mises yield) material behavior (“Linear elastic behavior,” Section 22.2.1, and “Classical metal plasticity,” Section 23.2.1); these are the only material behavior definitions that are relevant to these elements. The elastic behavior must be isotropic. Plasticity is included for Mode I (crack opening) response only; an elastic-plastic analysis will be accurate only when Mode I behavior dominates. The same material must be used through the section: a layered section cannot be defined with a line spring. Thermal strain effects are not included in the line spring elements; however, most of the thermal strain occurs in the shell, so this is not important in many cases (it is within the approximation made by line springs). Input File Usage: *SHELL SECTION, ELSET=name, MATERIAL=name Defining the flaw The flaw is defined by specifying its depth at each node along the crack front. You must identify whether the crack originates from the positive or negative surface of the shell (the positive surface is located a positive distance along the surface normal from the shell’s middle surface, as shown in Figure 32.9.1–1). At a point where the surface flaw depth is very small or zero, the compliance of the line spring element is also very small. To avoid numerical problems when a small compliance is inverted to form a stiffness, the minimum surface flaw depth used by Abaqus/Standard is 2% of the thickness specified for the line spring element, even if you specify a smaller surface flaw depth. If you want to constrain the two nodes where the surface flaw depth is zero to have the same displacements, you should tie the nodes together with a linear constraint equation or a multi-point constraint (“Kinematic constraints: overview,” Section 34.1.1). This is normally not required. Input File Usage: *SURFACE FLAW, SIDE=POSITIVE or NEGATIVE node number or node set label, crack depth ... Defining the shell model that contains the flaw You must specify the uncracked thickness of the shell in the section definition. The geometry of the shell at the flaw (coordinates and surface normals) is given in the usual way. Including the effects of pressure loading on the crack faces Cracks often occur on surfaces that are subjected to pressure; to include the effect of such loading on the crack faces, suitable distributed loading types are provided. These loading types are not intended for elastic-plastic line springs because the nodal equivalent forces calculated for the pressures are based on superposition methods that are valid only in the linear elastic case. J -integral output If the material is linear elastic only, the J-integral value and the stress intensity factors are output; for the elastic-plastic case local values of are provided as well as their sum into a single J value. In this case the J values will have acceptable accuracy only if . See “Line spring elements,” Section 3.9.5 of the Abaqus Theory Manual, for further details. is much larger than and 32.9.2 LINE SPRING ELEMENT LIBRARY Product: Abaqus/Standard References • “Line spring elements for modeling part-through cracks in shells,” Section 32.9.1 • *SHELL SECTION • *SURFACE FLAW Overview This section provides a reference to the line spring elements available in Abaqus/Standard. Element types LS6 LS3S 6-node general second-order line spring 3-node second-order line spring for use on a symmetry plane Active degrees of freedom 1, 2, 3, 4, 5, 6 Additional solution variables None. Nodal coordinates required X, Y, Z required at each node and, optionally, at each node. , , (direction cosines of the normal to the shell) A user-defined normal definition can also be used to specify . If these are not specified, they are constructed as for all other shell elements—by averaging over the shell elements attached to each node. , , Element property definition The only element property used is the thickness; the number of integration points is ignored, since the elements work on the basis of section properties. Input File Usage: Use the following option to define line spring element properties: *SHELL SECTION Use the following option to define the depth of the crack as a function of position: *SURFACE FLAW Element-based loading Distributed loads Distributed loads are specified as described in “Distributed loads,” Section 33.4.3. Three Gauss points are used for crack face pressure loading. Load ID (*DLOAD) HP Element output Units Description FL−2 FL−2 Hydrostatic surface pressure on the crack faces, with magnitude varying linearly with the global Z-direction. Surface pressure on the crack faces. Nodes 1, 2, and 3 on the element define side B and nodes 4, 5, and 6 define side A . The sign of the crack is defined by the surface of the shell from which the crack originates, which you identify when you define the depth of the crack . If the crack originates from the positive surface of the shell, sign(crack)=1.0; if the crack originates from the negative surface of the shell, sign(crack)=−1.0. is defined by the right-hand rule from the cross product of the tangent, The vector , which is positive going from node 1 to node 3 of the element, and the normal, , defined when the coordinates are given (or by a user-defined normal definition). For element type LS3S the vector must point into the model (away from the symmetry plane). For element type LS6 the vector must point from side A to side B. “Strains” E11 E22 Mode I opening displacement, Mode I opening rotation, The following strains exist only for LS6: E33 E12 E13 E23 Mode II through thickness shear, Mode II rotation, (this strain plays no role) Mode III anti-plane shear, Mode III opening rotation, The conjugate forces and moments are available by requesting “stress” output. The J-integral is provided at each integration point. If elastic-plastic material behavior is defined, the elastic and plastic parts of J are provided. The stress intensity factors, K, are also provided corresponding to the elastic parts of J. Figure 32.9.2–1 Notation for line spring strains. Nodes associated with the element LS6 LS3S side A side B side B Numbering of integration points for output Three points (these points are at the nodes) are used for integration and element output. LS6 LS3S 32.10 Elastic-plastic joints • “Elastic-plastic joints,” Section 32.10.1 • “Elastic-plastic joint element library,” Section 32.10.2 32.10.1 ELASTIC-PLASTIC JOINTS Product: Abaqus/Aqua References • *EPJOINT • “Elastic-plastic joint element library,” Section 32.10.2 Overview JOINT2D and JOINT3D elements: • are available for use only in Abaqus/Aqua used in conjunction with Abaqus/Standard (“Abaqus/Aqua analysis,” Section 6.11.1); • can be used to model flexible joints between structural members or the interaction between spud cans and the ocean floor; • are valid for small displacements and rotations; and • can be purely elastic or elastic-plastic. Elastic-plastic joint elements Abaqus/Standard provides JOINT2D and JOINT3D elements for modeling a joint between structural members or between a structural member and a fixed support. They can be used in an Abaqus/Aqua analysis to model the interaction between a “spud can” and the sea floor for jack-up foundation analysis in offshore applications. The joint has two nodes. One of these nodes should be constrained fully (by using a boundary condition) if the joint is between a structural member and a fixed support. Kinematics and local coordinate system The deformation of the joint is characterized by joint “strains,” which are relative displacements and rotations between the nodes of the joint. The joint must be associated with a user-defined local orientation system that is defined by three orthonormal directions: . The joint, when strained by relative extension or rotation of the two nodes, responds by applying equal and opposite forces and/or moments to the nodes. These forces and moments, or joint “stresses,” can be a linear (elastic) or nonlinear (elastic-plastic) function of the “strains,” depending on the type of constitutive model used in the joint. , and , The stresses and strains are named as shown in Figure 32.10.1–1. Positive stress indicates tension; positive strain indicates extension. joint between structural members 13 22 23 11 12 33 D0 joint as a spud can joint "stresses": forces and moments shown on node 2 Figure 32.10.1–1 Local axis definition for joint elements. Even when geometrically nonlinear analysis is requested (“Geometric nonlinearity” in “General and linear perturbation procedures,” Section 6.1.3), the element kinematics are defined with the assumption of small relative displacements and small rotations; therefore, these elements should not be used when these assumptions are violated. If large rotations are required and there is no plasticity, JOINTC elements can be used . The “extensional” strains are defined through and the “bending” strains through where are the relative displacements and rotations of the two nodes of the joint, respectively. For two-dimensional elements only the axial strains , , and the bending strain exist. For three-dimensional elements all six components exist. Input File Usage: Use the following option to associate a local orientation system with an elastic- plastic joint element: *EPJOINT, ORIENTATION=name Joint constitutive models The elastic moduli for joint elasticity can be entered in one of two ways. You can specify a general, anisotropic relation between the forces/moments and elastic extensions. Alternatively, you can enter moduli specific for a spud can; the elastic stiffness matrix is diagonal and depends on the diameter of the spud can at the soil surface, D, which can vary if spud can plasticity is defined and the spud can is conical. See “Joint elasticity models” below for details. Three joint plasticity models are provided. Two are specific to spud cans. The third is a parabolic model for structural joints or members. See “Joint plasticity” below for details. If plasticity is included, the plastic straining is assumed to occur in the local 1–2 plane so that the . It is assumed that plasticity in the 3-direction can be only nonzero plastic strains are neglected. In a three-dimensional model strains out of the 1–2 plane produce purely elastic response. , and , If the parabolic plasticity model for structural joints or members is used, the 1-direction is the axial direction along the members, while the 2-direction is the transverse direction . In the spud can plasticity models the 1-direction is the vertical direction, and the 2-direction is the horizontal direction in which plastic extension can take place. In three-dimensional models the 3-direction is the horizontal direction in which only elastic extension can take place. Any combination of elastic and plastic models can be used. For example, usually spud can elastic moduli will be used with spud can plasticity, but the use of general moduli with spud can plasticity is allowed. If plasticity is used in a three-dimensional model, coupling is not allowed through the elastic ) and the remaining, out-of-plane, , modulus between the strains or stresses in the 1–2 plane ( strains ( , ). Thus, in this case many of the general elastic moduli must be set to zero. Input File Usage: Use one or both of the following options immediately after the related *EPJOINT option to define the joint constitutive model: *JOINT ELASTICITY *JOINT PLASTICITY Orientation Care must be taken in defining the local directions and node numbering so that the motion of node 2 Incorrect relative to node 1 in the positive 1-direction of the local axis corresponds to extension. specification of the local directions or element node numbering can produce incorrect results in plastic analysis because compression will be interpreted as extension. If one of the nodes must be fixed to represent the ground, it is most convenient to let this node be the first node of the element; extension is then represented by the motion of node 2 of the element in the positive local 1-direction. If a spud can is being modeled in this way, the local 1-direction should be the outward normal to the ocean floor. For a two-dimensional analysis that uses Abaqus/Aqua structural loads, this direction must be the global y-direction. For a three-dimensional analysis that uses Abaqus/Aqua structural loads, the local 1-direction should point in the global z-direction. If plasticity is being used, the local 2-direction should be set so that the 1–2 plane is the plane of greatest deformation. Input File Usage: Use the following orientation definition to model a spud can with the first node fixed: *ORIENTATION, NAME=name, TYPE=RECTANGULAR 0, 1, 0, −1, 0, 0 Use the following orientation definition for a three-dimensional Abaqus/Aqua analysis with plasticity: *ORIENTATION, NAME=name, TYPE=RECTANGULAR 0, 0, 1, x, y, 0 where (x, y, 0) defines the local 2-direction. Spud can geometry If either spud can elasticity or spud can plasticity is used, you must specify the constants to define the spud can geometry. The entire spud can section definition has no effect if there is neither spud can elasticity nor spud can plasticity. The spud can, illustrated in Figure 32.10.1–1, can be either conical-based or flat-based. The spud , the diameter of the cylindrical portion, and , the planar angle of the . You can specify a flat-based spud can by omitting the specification can geometry is defined by conical portion, where of or by giving a value of 0 or 180 for Input File Usage: . *EPJOINT, SECTION=SPUD CAN , Spud can initial embedment If spud can plasticity is defined or if there is spud can elasticity and the spud can is conical, you must specify the initial embedment of the spud can, . The embedment can be prescribed directly or by specifying a “preload” that produces the embedment, as discussed below. Specification of both embedment and preload is not allowed. If either embedment or preload is given, both embedment and equivalent preload (in the case of plasticity) can be examined in the data file at the start of the analysis. At any time in the analysis the spud can has a total (plastic) embedment of , where is the plastic embedment between the start of the analysis and time t. (The negative sign in this equation reflects the fact that the sign convention for strain in Abaqus is positive for tensile strain. Most often for spud can plasticity, will be compressive, or negative.) The joint can be purely elastic, in which case always. , so The height of the conical portion of the spud can is given by . The effective diameter of the spud can at the soil surface, D, is defined by 1. For a flat-based spud can: 2. For a conical-based spud can: a. Cone portion partially penetrating ( ): b. Penetration beyond cone-cylinder transition ( ): The current spud can area at the soil surface, A, is defined through . The effective diameter can vary throughout the analysis only for a conical spud can with plasticity. The embedment has no effect and is not required if the spud can is cylindrical and spud can plasticity is not defined. Specifying the embedment directly The embedment value can be prescribed directly using initial conditions . Input File Usage: *INITIAL CONDITIONS, TYPE=SPUD EMBEDMENT Specifying the spud can preload If spud can plasticity is defined, you can specify the initial compressive capacity (“preload”), , instead of the embedment. In this case Abaqus/Aqua will use the hardening law to calculate the plastic embedment that follows when the preload is applied vertically. The preload initial condition is used only to calculate the initial plastic embedment; the spud can starts the analysis in a zero strain and stress state at this initial plastic embedment, and the preload is assumed to be removed. You must apply any operational vertical load through loading within the history definition. Input File Usage: *INITIAL CONDITIONS, TYPE=SPUD PRELOAD Embedment in an elastic spud can analysis If the spud can model is purely elastic, the spud can geometry is needed only for calculating the embedded diameter of the spud can for spud can elastic moduli. The embedment is required for this calculation only if the spud can is conical. Output Force and moment output in the element local system is available through the “stress” output variable S. Extension and relative rotation are available through the “strain” output variable E. Elastic and plastic strains are available through the output variables EE and PE. For spud cans the plastic embedment since the start of the analysis is available through the vertical component of plastic strain, PE11, and will usually be negative, indicating compression; the total vertical embedment, , is available through output variable PEEQ. Element nodal force (the force the element places on its nodes, in the global system) is available through element variable NFORC. Joint elasticity models The elastic load-displacement behavior of the JOINT2D and JOINT3D elements is characterized by elastic spring stiffnesses, which are assembled to form the elastic element stiffness matrix. A special diagonal modulus for spud cans can be specified or, alternatively, a fully populated (general) elastic modulus can be specified. Spud can moduli Spud can moduli can be prescribed for either two-dimensional or three-dimensional elements. Two-dimensional spud can moduli The elastic stiffness for a two-dimensional spud can is where is the vertical elastic spring stiffness, is the horizontal elastic spring stiffness, is the elastic spring stiffness in bending, ; ; ; in which , displacements, respectively; clay). , and are equivalent elastic shear moduli for vertical, horizontal, and rotational is the Poisson’s ratio of the soil (suggested value: 0.2 for sand and 0.5 for Input File Usage: *JOINT ELASTICITY, MODULI=SPUD CAN, NDIM=2 Three-dimensional spud can moduli For a three-dimensional spud can the moduli are where is the vertical elastic spring stiffness, is a horizontal elastic spring stiffness, is a horizontal elastic spring stiffness, is an elastic spring stiffness in bending, is an elastic spring stiffness in bending, is the torsional elastic spring stiffness, ; ; ; ; ; ; in which , , , and are as before and is a user-specified torsional stiffness value. Straining out of the 1–2 plane through the strains produces purely elastic response in the three-dimensional model regardless of plasticity. The moduli related to these strains are assumed not to be affected by the plasticity so that are based on the initial embedded diameter, while the other moduli depend on the current embedded diameter. , and , and Input File Usage: *JOINT ELASTICITY, MODULI=SPUD CAN, NDIM=3 General moduli General moduli can be specified for either two-dimensional or three-dimensional elements. Two-dimensional general moduli For the two-dimensional case six independent elastic moduli are needed. The stress-strain relations are as follows: Input File Usage: *JOINT ELASTICITY, MODULI=GENERAL, NDIM=2 Three-dimensional general moduli For the three-dimensional case 21 independent elastic moduli are needed. The stress-strain relations are as follows: Input File Usage: *JOINT ELASTICITY, MODULI=GENERAL, NDIM=3 Joint plasticity In what follows horizontal load in the 1–2 plane, and the bending moment in the local 1–2 plane, respectively. represent the vertical compressive load, the , and If plasticity is defined, the joint can yield axially, horizontally, or rotationally. The stress depends linearly on the elastic strain. The elastic moduli can depend on the plasticity in the case of a conical spud can, through the diameter at the surface, D. The models are rate independent, with a yield equation of the form where f is the yield function and total vertical plastic embedment, model. is a set of hardening parameters, which in these models depend on defines the type of plasticity ; the form of f and the definition of The flow rule requires that the plastic flow direction is normal to the contours of the flow potential, g. Associated flow is assumed in all of these models (except at vertices in the yield surface, as discussed below). Yield surface The three available plasticity models all use parabolic yield surfaces. Each has a compressive and a tensile limit for the stress in the 1-direction, which are termed is zero for the clay model. The sign convention for always obeys is such that they are always positive; thus, , respectively; and and The yield surface is most conveniently drawn in vertical load and is defined as -space, where is normalized compressive where the length of the limiting range for V. The normalized load is, therefore, always within the range is the middle value of the limiting elastic range for V, and is with representing the tensile limit and representing the compressive limit . is the normalized equivalent horizontal load and is defined through where normalized horizontal force are defined through and The normalized yield function in and -space for each model is defined through . are the moment and horizontal yield stresses. The normalized moment and and is a parabola as plotted in Figure 32.10.1–2. The yield surface in the space of the three normalized stresses is the surface of revolution of this parabola. f, g = 0 "tensile" yield (softening) compressive yield (hardening) -1 V1 g = 0 f = 0 .95 Figure 32.10.1–2 Yield surface and flow potential contour. Flow potential The flow potential is the same as the yield function (associated flow) except that some smoothing is done to the flow potential where the yield function has corners. The yield surface has corners and, therefore, nonunique normals at points where it is intersected by -axis. the To avoid problems with the indeterminate flow directions at these corners, Abaqus/Standard uses a flow potential whose contours are rounded in the region of the vertex, as indicated in the detail of a vertex shown in Figure 32.10.1–2. This rounding is achieved by fitting an elliptical segment to the flow potential contour for . Integration of the plasticity equations Abaqus/Aqua uses fully implicit integration for the plasticity equations. The corresponding tangent stiffness is unsymmetric for these plasticity models. By default, the symmetrized tangent is used in the global Newton loop. If the convergence rate seems to be poor, you may get some benefit out of using the unsymmetric matrix storage and solution scheme for the step . Joint plasticity models The three models differ only in the definitions of and in the hardening definitions. , We present the yield function for each model as it is presented in the literature rather than in normalized form. The equivalent normalized form can be obtained by identifying , which are explicit in the given yield functions for clay and member plasticity; for the sand model they are provided for reference. , and and , Sand model A. Yield function: and where The special case of Osborne, et al. are constant coefficients that determine the geometric shape of the yield function. gives the yield function as proposed by and B. Work hardening equations: i. Flat-base spud can: is soil unit weight; where classical bearing capacity factors, which can be calculated as: is an experimentally determined constant; and and are where is the soil friction angle. ii. Conical-base spud can: a. Cone portion partially penetrating: b. Penetration beyond cone-cylinder transition: where is a “cone equivalency coefficient.” The constants centrifuge data: and are based on the following empirical relation, which has been derived from in which the soil friction angle is in degrees. The sand model yield function can be put in normalized form by using and where . For the model of Osborne et al. . This model requires a nonzero initial embedment or equivalent preload. Input File Usage: *JOINT PLASTICITY, TYPE=SAND Clay model A. Yield function: where is the undrained shear strength of clay; and is the elevation area of the embedded portion of the spud can, defined through: i. Flat-base spud can: ii. Conical-base spud can: a. Cone portion penetrating: b. Penetration beyond cone-cylinder transition: B. Work hardening equations: i. Flat-base spud can: ii. Conical-base spud can: where , and c are user-defined empirical constants. This model has zero yield strength in tension and requires a nonzero initial embedment or equivalent preload. Input File Usage: *JOINT PLASTICITY, TYPE=CLAY Parabolic model for structural joints/members A. Yield function: where are horizontal and moment capacities, respectively. B. Work hardening: no work hardening is assumed (the model is perfectly plastic). Input File Usage: *JOINT PLASTICITY, TYPE=MEMBER Plasticity analysis issues Because associated flow is assumed in the spud can plasticity models, tensile vertical plastic strain can occur whenever the yield surface is encountered with . It is not required that the vertical force itself be tensile for tensile plastic yield to occur; tensile plastic yield can occur on any part of the yield surface where . The spud can models soften during this tensile plastic yield; if there is insufficient support from the rest of the model, an instability can occur and the analysis may fail to converge. When this happens, the spud can is likely to be lifting out of the sea floor. To make it easier to diagnose analysis problems that may arise due to these issues, a message is printed to the message file in the following cases: if tensile plastic yield occurs for a spud can, if yield occurs near the top of the parabolic yield surface ( ) where there is very little hardening, or if the embedment of a spud can becomes less than 10% of the initial embedment. These messages are not printed more than once in a given step. The plasticity algorithm can fail in an iteration if the strain increment is excessively large. Some details that may be of help in diagnosing failure in joint elements can be obtained by requesting detailed printout to the message file of problems with the plasticity algorithms . 32.10.2 ELASTIC-PLASTIC JOINT ELEMENT LIBRARY Product: Abaqus/Aqua References • “Elastic-plastic joints,” Section 32.10.1 • *EPJOINT Overview This section provides a reference to the elastic-plastic joint elements available in Abaqus/Aqua. Element types JOINT2D Two-dimensional elastic-plastic joint element JOINT3D Three-dimensional elastic-plastic joint element Active degrees of freedom 1, 2, 6 for JOINT2D 1, 2, 3, 4, 5, 6 for JOINT3D Additional solution variables None. Nodal coordinates required None. Element property definition Input File Usage: *EPJOINT Element-based loading None. Element output The relative displacements and rotations corresponding to the forces and moments below are chosen by requesting the corresponding “strains.” Elastic and plastic strains are available. For a spud can the vertical (plastic) embedment since the start of the analysis is given by PE11; the total vertical embedment is available as PEEQ. JOINT2D S11 S22 S12 JOINT3D S11 S22 S33 S12 S13 S23 Total direct force in the first local direction. Total direct force in the second local direction. Total moment about the third local direction. Total direct force in the first local direction. Total direct force in the second local direction. Total direct force in the third local direction. Total moment about the third local direction. Total moment about the second local direction. Total moment about the first local direction. Nodes associated with the element Two nodes. 32.11 Drag chain elements • “Drag chains,” Section 32.11.1 • “Drag chain element library,” Section 32.11.2 32.11.1 DRAG CHAINS Product: Abaqus/Standard References • “Drag chain element library,” Section 32.11.2 • *DRAG CHAIN • *RIGID SURFACE Overview Drag chain elements: • are used for simulating the effects of drag chains on the seabed for near bottom bending simulation modeling; and • can be used in two-dimensional or three-dimensional problems. Typical applications The drag chain is modeled as a concentrated weight on the seabed, with a chain between it and an attachment point on the pipe . o o oooo ooooooooooooooooooooo o o o o o ° ° °°°°°°°°° ° ° ° ° ° Figure 32.11.1–1 Drag chain model. Given a uniform drag chain of total length , weight per unit length w, and friction coefficient between it and the seabed, attached to the pipeline at height h above the seabed, the length of chain on the seabed at slip, , is given by and the horizontal projection of the suspended length, , is Thus, the equivalent model should have a friction limit of taken as any value from to , can be . Comparison with experiment has shown that taking this length as The horizontal length at slip, is a reasonable choice. When the pipeline attachment point is directly above the weight, there will be no horizontal force or horizontal stiffness offered by a drag chain element; this position is assumed as the initial condition. As the pipe moves relative to the seabed, the horizontal force on the pipeline caused by the drag chain opposes the relative motion and gradually increases (an approximation to the catenary equation is used to relate the force to the offset ) until the drag chain slips when the force reaches the friction limit. The height, h, is assumed to be small compared to . Choosing an appropriate element Two- and three-dimensional drag chain elements are available. Element DRAG2D assumes that the seabed is flat and parallel to the plane in which the pipe is moving; therefore, the seabed does not have to be modeled explicitly. Element DRAG3D requires that the seabed be defined as an analytical rigid surface, which must be flat and parallel to the global (X, Y) plane and is considered to be fixed throughout the analysis. Defining the seabed for three-dimensional drag chains The seabed is defined as an analytical rigid surface. This surface definition is used to determine if the chain touches the seabed, depending on the separation between the pipe node and the position of the seabed surface. See “Analytical rigid surface definition,” Section 2.3.4, for more information. Since the seabed is considered to be fixed, boundary conditions must be applied to the rigid body reference node of the seabed surface, which is also the second node of the DRAG3D element. Input File Usage: Use the following option to define the seabed surface for DRAG3D elements: *RIGID SURFACE In a model defined in terms of an assembly of part instances, the rigid surface definition that defines the seabed must appear inside the same part definition as the drag chain elements. Defining the drag chain behavior For DRAG2D elements you specify the maximum horizontal length, , between the attachment point and the concentrated weight. At this length the weight will start to slip on the seabed. In addition, you specify the horizontal force between the weight and the seabed at slip (that is, the frictional limit). For DRAG3D elements you specify the total length of the chain, the friction coefficient, and the weight per unit length of chain. You must associate the drag chain behavior with a set of drag chain elements. Input File Usage: *DRAG CHAIN, ELSET=name drag chain data 32.11.2 DRAG CHAIN ELEMENT LIBRARY Product: Abaqus/Standard References • “Drag chains,” Section 32.11.1 • *DRAG CHAIN • *RIGID SURFACE Overview This section provides a reference to the drag chain elements available in Abaqus/Standard. Element types DRAG2D Two-dimensional drag chain, for use in cases where only horizontal motion is being studied DRAG3D Three-dimensional drag chain Active degrees of freedom DRAG2D: 1, 2 DRAG3D: At the first node: 1, 2, 3. At the second node: 1, 2, 3, 4, 5, 6. Additional solution variables None. Nodal coordinates required DRAG2D: (X, Y) coordinates of the pipeline attachment node in the horizontal plane. DRAG3D: (X, Y, Z) coordinates of both nodes. Element property definition Input File Usage: Use the following option to define the horizontal length at slip and the friction limit: *DRAG CHAIN Use the following option to define the seabed for DRAG3D elements: *RIGID SURFACE The rigid surface must be flat and parallel to the global (X, Y) plane. Element-based loading None. Element output S11 S12 E11 E12 The horizontal component of force supported by the drag chain in the plane parallel to the seabed. The vertical component of force in the drag chain for DRAG3D elements. The horizontal length of the drag chain for DRAG2D elements. The length of chain on the seabed floor (not suspended) for DRAG3D elements. The orientation of the drag chain (angle from the global X-axis). Nodes associated with the element DRAG2D: One node at the position where the chain attaches to the pipe. DRAG3D: Two nodes. The first node is the node where the chain attaches to the pipe; the second node is the “reference node” of the rigid body containing the rigid surface that defines the seabed. 32.12 Pipe-soil elements • “Pipe-soil interaction elements,” Section 32.12.1 • “Pipe-soil interaction element library,” Section 32.12.2 32.12.1 PIPE-SOIL INTERACTION ELEMENTS Product: Abaqus/Standard References • “Pipe-soil interaction element library,” Section 32.12.2 • *PIPE-SOIL INTERACTION • *PIPE-SOIL STIFFNESS Overview The pipe-soil interaction elements in Abaqus/Standard: • can be used to model the interaction between a buried pipeline and the surrounding soil; • must be used with beam elements, pipe, or elbow elements ; and • can have linear or nonlinear constitutive behavior. Pipe foundation elements Abaqus/Standard provides two-dimensional (PSI24 and PSI26) and three-dimensional (PSI34 and PSI36) pipe-soil interaction elements for modeling the interaction between a buried pipeline and the surrounding soil. The pipeline itself is modeled with any of the beam, pipe, or elbow elements in the Abaqus/Standard element library . The ground behavior and soil-pipe interaction are modeled with the pipe-soil interaction (PSI) elements. These elements have only displacement degrees of freedom at their nodes. One side or edge of the element shares nodes with the underlying beam, pipe, or elbow element that models the pipeline . The nodes on the other edge represent a far-field surface, such as the ground surface, and are used to prescribe the far-field ground motion via boundary conditions together with amplitude references as needed. The far-field side and the side that shares nodes with the pipeline are defined by the element connectivity. Care must be taken in attaching the underlying elements to the correct edge of the PSI element, since the connectivity of the pipe-soil element determines the local coordinate system as defined below, and the depth, H, of the pipeline below the ground surface. The depth below the surface is measured along the edge of the PSI element as shown in Figure 32.12.1–1 and is updated during geometrically nonlinear analysis. It is important to note that PSI elements do not discretize the actual domain of the surrounding soil. The extent of the soil domain is reflected through the stiffness of the elements, which is defined by the constitutive model as described later. far-field edge ground surface PSI element e1 e2 e3 pipe centerline pipeline edge pipeline discretized with beam-type elements Figure 32.12.1–1 Pipe-soil interaction model. The pipe-soil interaction model does not include the density of the surrounding soil medium. Mass can be associated with the model by applying concentrated MASS elements at the nodes of the pipe-soil interaction elements if needed. Assigning the pipe-soil interaction behavior to a PSI element You must assign the pipe-soil interaction behavior to a set of pipe-soil interaction elements. Input File Usage: Use the following option to assign the pipe-soil interaction behavior to a particular element set: *PIPE-SOIL INTERACTION, ELSET=name Use the following option immediately after the*PIPE-SOIL INTERACTION option to define the stiffness behavior for the element set: *PIPE-SOIL STIFFNESS Kinematics and local coordinate system The deformation of the pipe-soil interaction element is characterized by the relative displacements between the two edges of the element. When the element is “strained” by the relative displacements, forces are applied to the pipeline nodes. These forces can be a linear (elastic) or nonlinear (elastic-plastic) function of the “strains,” depending on the type of constitutive model used for the element. Positive “strains” are defined by where are the relative displacements between the two edges ( the pipeline displacements), directions. For two-dimensional elements only the in-plane components of strain three-dimensional elements all three strain components are are local directions, and the index i (=1, 2, 3) refers to the three local exist. For are the far-field displacements, and exist. , and , , The local orientation system is defined by three orthonormal directions: . The default local directions are defined so that is the direction normal to the plane of the element (transverse horizontal direction), and is the direction in the plane of the element that defines the transverse vertical behavior. Positive default directions are defined so that points from the pipeline edge toward the far-field edge, as shown in Figure 32.12.1–1. You can also define these local directions by specifying a local orientation (“Orientations,” Section 2.2.5) for the pipe-soil interaction. is the direction along the pipeline (axial direction), points toward the second pipeline node and , and , In a large-displacement analysis the local coordinate system rotates with the rigid body motion of the underlying pipeline. In a small-displacement analysis the local system is defined by the initial geometry of the PSI element and remains fixed in space during the analysis. Input File Usage: Use the following option to associate a local orientation with a pipe-soil interaction behavior: *PIPE-SOIL INTERACTION, ORIENTATION=name Constitutive models The constitutive behavior for a pipe-soil interaction is defined by the force per unit length, or “stress,” at each point along the pipeline, , between that point and the point on the far-field surface: , caused by relative displacement or “strain,” where are state variables (such as plastic strains), and are temperatures and/or field variables. You can define these relationships quite generally by programming them in user subroutine UMAT. Alternatively, you can define the relationships by specifying the data directly. In this case the assumption is that the foundation behavior is separable: in which case each of the independent relationships must be defined separately. Abaqus/Standard assumes, by default, that these relationships are symmetric about the origin (as is generally appropriate for the axial and transverse horizontal motions). However, you may give a nonsymmetric behavior for any of the three relative motions (this is usually the case in the vertical direction when the pipeline is not buried too deeply). These models assume that positive “strains” give rise to forces on the pipe that act along the positive directions of the local coordinate system. Specifying the constitutive behavior with a user subroutine To define the relationships quite generally, you can program them in user subroutine UMAT. Input File Usage: *PIPE-SOIL STIFFNESS, TYPE=USER Specifying the constitutive behavior directly Two methods are provided for specifying constitutive behavior data directly. One method is to define the relationships directly in tabular (piecewise linear) form. The other method is to use ASCE formulae. Forms of these relationships suitable for use with sands and clays are defined in the ASCE Guidelines for the Seismic Design of Oil and Gas Pipeline Systems. Specifying the constitutive behavior directly using tabular input You can define a linear or nonlinear constitutive model with different behavior in tension and compression using tabular input. Linear model To define a linear constitutive model, you specify the stiffness as a function of temperature and field variables . You can enter different values for positive and negative “strain.” Abaqus/Standard assumes, by default, that the relationship is symmetric about the origin. Input File Usage: *PIPE-SOIL STIFFNESS, TYPE=LINEAR Nonlinear model To define a nonlinear constitutive model, you specify the relationship as a function of positive and negative relative displacement (“strain”), temperature, and field variables . The behavior is assumed symmetric about the origin if only positive or negative data are provided. You must provide the data in ascending order of relative displacement; you should provide it over a sufficiently wide range of relative displacement values so that the behavior is defined correctly. The force remains constant outside the range of data points. You must separate positive and negative data by specifying the data point at the origin of the force-relative displacement diagram. The two data points immediately before and after the data point at the origin define the elastic stiffness, , and the initial elastic limits, , as indicated in Figure 32.12.1–3. and and The model provides linear elastic behavior if where respectively. Inelastic deformation occurs when the relative force exceeds these elastic limits. are the equivalent plastic strains associated with negative and positive deformations, and Kn Kp Figure 32.12.1–2 Linear constitutive model. qi, ε qp Kp 0, 0 q1, ε q2, ε Kn qn Figure 32.12.1–3 Nonlinear constitutive relationship. Hardening of the model is controlled by independent evolution of and . The model assumes that remains constant when the increment in relative displacement is negative, and remains constant when the increment in relative displacement is positive. The response predicted by this model during a full loading cycle is shown in Figure 32.12.1–4 for a simple constitutive law that uses different bilinear behavior associated with positive and negative force. Figure 32.12.1–4 shows that the yield stress associated with positive force is updated to , while the initial yield stress associated with negative force, , remains constant during initial loading. Similarly, during subsequent reversed loading the yield stress associated with negative force is updated to , while the yield stress associated with positive force remains constant. Consequently, yielding occurs at during the next load reversal. Such behavior is appropriate for the directions transverse to the pipeline where it is expected that relative positive motion between the pipe and soil is independent from relative negative motion between the pipe and soil. Kn qn qp Kp Kp Kp Kn qn qn qp Figure 32.12.1–4 Cyclic loading for a bilinear model. An isotropic hardening model is used if the behavior is symmetric about the origin (when only positive or negative data are provided). In this case only one equivalent plastic strain variable, , is used, which is updated when either negative or positive inelastic deformation occurs. Such an evolution model is more appropriate along the axial direction where it is expected that positive inelastic deformation influences subsequent negative inelastic deformation. Input File Usage: *PIPE-SOIL STIFFNESS, TYPE=NONLINEAR Specifying the constitutive behavior directly using ASCE formulae Abaqus/Standard also provides analytical models to describe the pipe-soil interaction. These models define the constant ultimate force that can be exerted on the pipeline. In other words, these models describe elastic, perfectly plastic behavior. Forms of these formulae suitable for use with sands and clays are described in detail in the ASCE Guidelines for the Seismic Design of Oil and Gas Pipeline Systems. The ASCE formulae can be applied in any arbitrary local system by associating an orientation definition with the element. However, these formulae are intended to be used in the default local coordinate system so that the formula for axial behavior is applied along the pipeline axis (the 1-direction), the formula for vertical behavior is applied along the 2-direction, and the formula for horizontal behavior along the 3-direction. You must specify the direction in which the behavior is specified when it is described by ASCE fomulae. You specify all the parameters in the expressions below, except the depth, H, below the surface, which is measured along the edge of the PSI element as shown in Figure 32.12.1–1 and is updated during geometrically nonlinear analysis. Values for the remaining parameters can be found in standard soil mechanics textbooks. Typical values are also provided in the ASCE Guidelines for the Seismic Design of Oil and Gas Pipeline Systems. Axial behavior The ultimate axial load for sand, , is given by where of the pipeline, D is the external diameter of the pipeline, the interface angle of friction. is the coefficient of soil pressure at rest, H is the depth from the ground surface to the center is is the effective unit weight of soil, and The ultimate axial load for clay is given by where S is the undrained soil shear strength and is an empirical adhesion factor that relates the undrained soil shear strength to the cohesion, . The maximum load is reached at an ultimate relative displacement, , of approximately 2.5 to 5.0 mm (0.1 to 0.2 inches) for sand and approximately 2.5 to 10.0 mm (0.2 to 0.4 inches) for clay. A linear elastic response is assumed for . The axial behavior is assumed to be symmetric about the origin. Consequently, only one equivalent , describes the evolution of the model. The equivalent plastic strain is updated plastic strain variable, when either negative or positive inelastic deformation occurs. Input File Usage: Use one of the following options to define the axial behavior: *PIPE-SOIL STIFFNESS, DIRECTION=AXIAL, TYPE=SAND *PIPE-SOIL STIFFNESS, DIRECTION=AXIAL, TYPE=CLAY Transverse vertical behavior The vertical behavior is described by different relationships for “upward” motion (when the pipeline rises with respect to the ground surface) and “downward” motion. Downward motions give rise to positive relative displacements so that positive forces are applied to the pipeline. Similarly, upward motions give rise to negative relative displacements and pipeline forces. The ultimate force for downward motion of the pipe in sand is given by where and downward direction, and section. The ultimate force for downward motion of the pipe in clay is given by are bearing capacity factors for vertical strip footings, vertically loaded in the is the total soil unit weight. Other parameters are defined in the previous where approximately is a bearing capacity factor. The ultimate force is reached at a relative displacement of for both sand and clay. to The ultimate force for upward motion of the pipe in sand is given by and for clay by where and are vertical uplift factors. The ultimate force is reached at a relative displacement of approximately to to for sand and for clay. The transverse vertical behavior is non-symmetric about the origin. Consequently, two equivalent plastic strain variables—one associated with negative relative displacement, , and the other with positive relative displacement, —are used to describe the evolution of the model. The model assumes that remains constant when the increment in relative displacement is positive. remains constant when the increment in relative displacement is negative, and Input File Usage: Use one of the following options to define the vertical behavior: *PIPE-SOIL STIFFNESS, DIRECTION=VERTICAL, TYPE=SAND *PIPE-SOIL STIFFNESS, DIRECTION=VERTICAL, TYPE=CLAY Transverse horizontal behavior The horizontal force-relative displacement relationship for sand is given by and for clay by where sections. The ultimate force is reached at a relative displacement of approximately are horizontal bearing capacity factors. Other variables are defined in the previous , and where between 0.02 to 0.03 for dense sand. is between 0.07 to 0.1 for loose sand, between 0.03 to 0.05 for medium sand and clay, and The transverse horizontal behavior is assumed to be symmetric about the origin. Consequently, only , describes the evolution of the model. The equivalent plastic one equivalent plastic strain variable, strain is updated when either negative or positive inelastic deformation occurs. Input File Usage: Use one of the following options to define the horizontal behavior: *PIPE-SOIL STIFFNESS, DIRECTION=HORIZONTAL, TYPE=SAND *PIPE-SOIL STIFFNESS, DIRECTION=HORIZONTAL, TYPE=CLAY Specifying the directions for which the constitutive behavior is defined If you are defining the constitutive behavior by specifying the data directly, by default an isotropic model is assumed. If the model is not isotropic, you can specify different constitutive relationships in each direction. For two-dimensional nonisotropic models you must specify the behavior in two directions; for three-dimensional nonisotropic models you must specify the behavior in three directions. You must indicate the direction in which the behavior is specified. You can specify the 1-direction, 2-direction, 3-direction, axial direction, vertical direction, or horizontal direction. Abaqus/Standard assumes that the axial direction is equivalent to the 1-direction, the vertical direction is equivalent to the 2-direction, and the horizontal direction is equivalent to the 3-direction. Input File Usage: Use the following option to define an isotropic constitutive model: *PIPE-SOIL STIFFNESS Use the following option to define the constitutive model in a particular direction: *PIPE-SOIL STIFFNESS, DIRECTION=direction where direction can be 1, 2, 3, AXIAL, VERTICAL, or HORIZONTAL. Repeat the *PIPE-SOIL STIFFNESS option with the DIRECTION parameter as many times as necessary to define the behavior in each direction. Output The force per unit length in the element local system is available through the “stress” output variable S. Relative deformation is available through the “strain” output variable E. Elastic and plastic “strains” are available through the output variables EE and PE. Element nodal force (the force the element places on the pipeline nodes, in the global system) is available through element variable NFORC. Additional reference • Audibert, J. M. E., D. J. Nyman, and T. D. O’Rourke, “Differential Ground Movement Effects on Buried Pipelines,” Guidelines for the Seismic Design of Oil and Gas Pipeline Systems, ASCE publication, pp. 151–180, 1984. 32.12.2 PIPE-SOIL INTERACTION ELEMENT LIBRARY Product: Abaqus/Standard References • “Pipe-soil interaction elements,” Section 32.12.1 • *PIPE-SOIL INTERACTION Overview This section provides a reference to the pipe-soil interaction elements available in Abaqus/Standard. Element types 2-D elements PSI24 PSI26 Two-dimensional 4-node pipe-soil interaction element Two-dimensional 6-node pipe-soil interaction element Active degrees of freedom 1, 2 Additional solution variables None. 3-D elements PSI34 PSI36 Three-dimensional 4-node pipe-soil interaction element Three-dimensional 6-node pipe-soil interaction element Active degrees of freedom 1, 2, 3 Additional solution variables None. Nodal coordinates required 2–D: X, Y 3–D: X, Y, Z Element property definition Input File Usage: *PIPE-SOIL INTERACTION Element-based loading None. Element output The relative displacements corresponding to the forces below are chosen by requesting the corresponding “strains.” Elastic and plastic strains are available. Two-dimensional elements S11 S22 Force per unit length in the first local direction. Force per unit length in the second local direction. Three-dimensional elements S11 S22 S33 Force per unit length in the first local direction. Force per unit length in the second local direction. Force per unit length in the third local direction. Node ordering and integration point numbering far-field edge pipeline edge PSI24 and PSI34 far-field edge pipeline edge PSI26 and PSI36 32.13 Acoustic interface elements • “Acoustic interface elements,” Section 32.13.1 • “Acoustic interface element library,” Section 32.13.2 32.13.1 ACOUSTIC INTERFACE ELEMENTS Products: Abaqus/Standard Abaqus/CAE References • “Acoustic interface element library,” Section 32.13.2 • “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1 • *INTERFACE • “Creating acoustic interface sections,” Section 12.13.18 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Acoustic interface elements: • can be used to couple a model of an acoustic fluid to a structural model containing continuum or structural elements; • couple the accelerations of the surface of the structural model to the pressure in the acoustic medium; • can be used in dynamic and steady-state dynamic procedures; • must be defined with the nodes shared by the acoustic elements and the structural (or solid) elements; • can be used only in small-displacement simulations and are not intended for use in nonlinear or hydrostatic fluid-structure interactions; • are ignored in eigenfrequency extraction analyses if the subspace iteration eigensolver is used; and • if necessary, can be degenerated into triangular elements. For most problems the surface-based, structural-acoustic capabilities described in “Mesh tie constraints,” Section 34.3.1, and in “Defining tied contact in Abaqus/Standard,” Section 35.3.7, provide more general and easy to use methods for modeling the interaction between an acoustic fluid and a structure. User- specified acoustic interface elements give you increased control over the coupling specification, at the expense of the convenience of the surface-based procedures. Typical applications The acoustic interface elements are used in simulations where the motion of a solid structure influences the pressure in the acoustic fluid, such as when the vibrations of a car frame produce noise in the passenger compartment; or where the pressure in the fluid affects a neighboring structure, such as when the small- amplitude sloshing of a fluid inside a container affects its response. User-specified acoustic interface elements are also useful in problems involving only an acoustic medium because they allow you to specify displacement, velocity, or acceleration boundary conditions directly on the nodes of the acoustic interface elements. In this application, however, you must be aware that the tangential displacements are not coupled to the fluid. Therefore, zero-energy modes may arise involving the displacement degrees of freedom if these nodes are not constrained in the tangential direction. When acoustic interface elements are used to couple fluid and solid elements, this problem does not arise because of the stiffness and inertia of the solid. Choosing an appropriate element The order of the underlying acoustic and structural elements usually dictates which acoustic interface element should be used. The general acoustic interface element, ASI1, can be used in any coupled acoustic-structural simulation; however, normally it is used only with the acoustic link elements (AC1D2 and AC1D3). Defining the normal direction of the acoustic-structural interface The connectivity of the acoustic interface elements and the right-hand rule define the normal direction of the acoustic-structural interface, as shown in “Acoustic interface element library,” Section 32.13.2. It is very important that this normal point into the acoustic fluid, as shown in Figure 32.13.1–1 and Figure 32.13.1–2. The one exception is the ASI1 acoustic interface element, where you must define the normal direction. fluid solid ASI2D2 ASIAX2 fluid solid ASI2D3 ASIAX3 Figure 32.13.1–1 Normal directions for two-dimensional and axisymmetric acoustic-structural interface elements. Defining the acoustic interface element’s section properties You must associate the acoustic interface section definition with a set of acoustic interface elements. This section definition must be used with three-dimensional and axisymmetric acoustic interface elements, even though there are no user-defined geometric properties for these elements. Input File Usage: Abaqus/CAE Usage: *INTERFACE, ELSET=element_set_name Property module: Create Section: select Other as the section Category and Acoustic interface as the section Type Assign→Section: select regions fluid solid ASI3D4 fluid fluid solid ASI3D3 fluid solid solid ASI3D6 ASI3D8 Figure 32.13.1–2 Normal directions for three-dimensional acoustic-structural interface elements. Defining the geometric properties associated with ASI1 elements The ASI1 elements consist of a single node. Abaqus/Standard cannot calculate the surface area associated with these elements, so you must supply this information. If accurate surface areas are not given, Abaqus/Standard may calculate incorrect accelerations or acoustic fluid pressure at the acoustic-structural interface. In addition, Abaqus/Standard cannot calculate the direction of the interface normal associated with these elements. You must provide the direction cosines, in the global Cartesian coordinate system, of the interface normal for these elements. Input File Usage: Abaqus/CAE Usage: *INTERFACE surface area, X-direction cosine, Y-direction cosine, Z-direction cosine General-use acoustic interface sections are not supported in Abaqus/CAE. Defining the thickness for planar acoustic interface elements You can specify the thickness of planar acoustic interface elements. The default value is unit thickness. Input File Usage: *INTERFACE thickness Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Acoustic interface as the section Type: Plane stress/strain thickness: thickness Using acoustic interface elements when elements with different interpolation orders form the acoustic-structural interface It is normally assumed that the same order of interpolation will be used for both the acoustic fluid mesh and the structural mesh (at least at the interface surfaces). If this is not the case, suitable MPCs must be applied to the nodes along the acoustic-structural interface to maintain the compatibility in the pressure (MPC type P LINEAR) or displacement fields (MPC type LINEAR). 32.13.2 ACOUSTIC INTERFACE ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/CAE References • “Acoustic interface elements,” Section 32.13.1 • *INTERFACE Overview This section provides a reference to the acoustic interface elements available in Abaqus/Standard. Element types Element for general use ASI1 1-node Active degrees of freedom 1, 2, 3, 8 Additional solution variables None. Elements for use in planar models ASI2D2 ASI2D3 2-node linear 3-node quadratic Active degrees of freedom 1, 2, 8 Additional solution variables None. Elements for use in 3-D models ASI3D3 ASI3D4 ASI3D6 ASI3D8 3-node linear 4-node linear 6-node quadratic 8-node quadratic Active degrees of freedom 1, 2, 3, 8 Additional solution variables None. Elements for use in axisymmetric models ASIAX2 ASIAX3 2-node linear 3-node quadratic Active degrees of freedom 1, 2, 8 Additional solution variables None. Nodal coordinates required General use element: None. Planar: X, Y 3-D: X, Y, Z Axisymmetric: r, z Element property definition For general-use elements, you must define the element’s surface area and the direction cosines of the normal to the acoustic fluid-structural interface, pointing into the fluid. For elements for use in planar models, you must specify the thickness (out-of-plane) of the element. The default is unit thickness if no thickness is specified. For elements for use in three-dimensional and axisymmetric models, no additional data are required. Input File Usage: Abaqus/CAE Usage: *INTERFACE Property module: Create Section: select Other as the section Category and Acoustic interface as the section Type General-use acoustic interface sections are not supported in Abaqus/CAE. Element-based loading Distributed impedances cannot be applied. Element output None. Node ordering on elements Planar 3-D ASI2D2 ASI2D3 ASI3D3 ASI3D4 ASI3D6 ASI3D8 Axisymmetric ASIAX2 ASIAX3 32.14 Eulerian elements • “Eulerian elements,” Section 32.14.1 • “Eulerian element library,” Section 32.14.2 32.14.1 EULERIAN ELEMENTS Products: Abaqus/Explicit Abaqus/CAE References • “Eulerian analysis,” Section 14.1.1 • “Eulerian element library,” Section 32.14.2 • *EULERIAN SECTION • “Creating Eulerian sections,” Section 12.13.3 of the Abaqus/CAE User’s Manual, in the online HTML version of this manual Overview Eulerian elements: • can be used only in explicit dynamic analyses; • must have eight unique nodes; • are filled with void material by default; • can be initialized with nonvoid material; • can contain multiple materials simultaneously; and • can be partially filled with material. Typical applications Eulerian elements are useful for simulations involving material that undergoes extreme deformation, up to and including fluid flow. The Eulerian formulation allows material to flow from one element to another, even as the Eulerian mesh remains fixed. Applications that utilize Eulerian elements are discussed in “Eulerian analysis of a collapsing water column,” Section 1.7.1 of the Abaqus Benchmarks Manual, and “Rivet forming,” Section 2.3.1 of the Abaqus Example Problems Manual. For more information on Eulerian analyses, see “Eulerian analysis,” Section 14.1.1. Choosing an appropriate element The available Eulerian elements are the three-dimensional, 8-node element EC3D8R and the three-dimensional, 8-node thermally coupled element EC3D8RT. Two-dimensional simulations can be approximated using a one-element thick mesh or a wedge-shaped mesh with appropriate boundary conditions. The Eulerian mesh is typically a simple rectangular grid of elements that does not conform to the shape of the Eulerian materials. Complex material shapes can be represented inside this mesh using a combination of fully and partially filled elements surrounded by void regions. Defining the Eulerian element’s section properties You must associate the Eulerian section definition with a set of Eulerian elements. This set of elements must not share nodes with other types of elements. The section definition provides a list of materials that may occupy the Eulerian elements. Input File Usage: *EULERIAN SECTION, ELSET=element_set_name data lines giving list of materials Abaqus/CAE Usage: Property module: Create Section: select Solid as the section Category and Eulerian as the section Type Assign→Section: select part 32.14.2 EULERIAN ELEMENT LIBRARY Products: Abaqus/Explicit Abaqus/CAE References • “Eulerian analysis,” Section 14.1.1 • *EULERIAN SECTION Overview This section provides a reference to the Eulerian elements available in Abaqus/Explicit. Element types Eulerian stress/displacement element EC3D8R 8-node linear brick, multimaterial, reduced integration with hourglass control Active degrees of freedom 1, 2, 3 Additional solution variables None. Eulerian thermally coupled element EC3D8RT 8-node thermally coupled linear brick, multimaterial, hourglass control reduced integration with Active degrees of freedom 1, 2, 3,11 Additional solution variables None. Nodal coordinates required X, Y, Z Element property definition You must specify a list of materials that may be present in the Eulerian element. You can also assign a material instance name to each material . Input File Usage: *EULERIAN SECTION Abaqus/CAE Usage: Property module: Create Section: select Solid as the section Category and Eulerian as the section Type Element-based loading Distributed loads Distributed loads are available only for Eulerian elements. They are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description Body force in global X-direction. Body force in global Y-direction. Body force in global Z-direction. Nonuniform body force in global X-direction with magnitude supplied subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user Nonuniform body force in global Y-direction with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. Nonuniform body force in global Z-direction with magnitude supplied subroutine DLOAD in via user and VDLOAD in Abaqus/Standard Abaqus/Explicit. Gravity loading direction (magnitude is acceleration). in specified input as Pressure on face n. Nonuniform pressure on face n via with magnitude user in subroutine VDLOAD Abaqus/Standard in Abaqus/Explicit. supplied DLOAD and BX BY BZ BXNU Body force Body force Body force Body force FL−3 FL−3 FL−3 FL−3 BYNU Body force FL−3 BZNU Body force FL−3 GRAV Gravity Pn PnNU Pressure Not supported LT−2 FL−2 FL−2 Load ID (*DLOAD) Abaqus/CAE Load/Interaction Units Description SBF SPn TRSHRn TRVECn VBF VPn Not supported FL−5 T2 Stagnation body force in global X-, Y-, and Z-directions. Not supported FL−4 T2 Stagnation pressure on face n. Surface traction Surface traction FL−2 FL−2 Not supported FL−4 T Not supported FL−3 T Shear traction on face n. General traction on face n. Viscous body force in global X-, Y-, and Z-directions. Viscous pressure on face n, applying a pressure proportional to the velocity normal to the face and opposing the motion. Distributed heat fluxes Distributed heat fluxes are available only for EC3D8RT elements. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DFLUX) Abaqus/CAE Load/Interaction Units Description BF Sn Body heat flux Surface heat flux JL−3 T−1 JL−2 T−1 Heat body flux per unit volume. Heat surface flux per unit area into face n. Film conditions Film conditions are available only for EC3D8RT elements. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*FILM) Fn Radiation types Abaqus/CAE Load/Interaction Units Description Surface film condition JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on face n. Radiation conditions are available only for EC3D8RT elements. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*RADIATE) Abaqus/CAE Load/Interaction Units Description Rn Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided on face n. Surface-based loading Distributed loads Surface-based distributed loads are available for Eulerian elements. They are specified as described in “Distributed loads,” Section 33.4.3. Load ID (*DSLOAD) Abaqus/CAE Load/Interaction Units Description PNU Pressure Pressure FL−2 FL−2 SP Pressure FL−4 T2 TRSHR TRVEC Surface traction Surface traction FL−2 FL−2 VP Pressure FL−3 T Pressure on the element surface. Nonuniform pressure on the element supplied surface with magnitude subroutine DLOAD in via Abaqus/Standard and VDLOAD in Abaqus/Explicit. user Stagnation pressure on the element surface. Shear traction on the element surface. General surface. traction on the element Viscous pressure applied on the element surface. The viscous pressure is proportional to the velocity normal to the element face and opposing the motion. Distributed heat fluxes Surface-based heat fluxes are available only for EC3D8RT elements. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*DSFLUX) Abaqus/CAE Load/Interaction Units Description Surface heat flux JL−2 T−1 Heat surface flux per unit area into the element surface. Film conditions Surface-based film conditions are available only for EC3D8RT elements. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SFILM) Radiation types Abaqus/CAE Load/Interaction Units Description Surface film condition JL−2 T−1 −1 Film coefficient and sink temperature (units of ) provided on the element surface. Surface-based radiation conditions are available only for EC3D8RT elements. They are specified as described in “Thermal loads,” Section 33.4.4. Load ID (*SRADIATE) Abaqus/CAE Load/Interaction Units Description Surface radiation Dimensionless Emissivity and sink temperature (units of ) provided on the element surface. Element output A set of output variables is written for each Eulerian material instance listed in the Eulerian section definition. The output variable names are automatically appended with the material instance names. For example, if you define material instances named “steel” and “tin” and request stress output, the first stress components will be written to separate output variables named “S11_steel” and “S11_tin.” All output is given in global coordinates. Stress and other tensor components Stress and other tensors (excluding total strain tensors) are available. All tensors have the same components. For example, the stress components are as follows: S11 S22 S33 S12 S13 S23 , direct stress. , direct stress. , direct stress. , shear stress. , shear stress. , shear stress. Element-averaged quantities Several output variables are also available as element-averaged quantities. These variables are computed as a volume fraction weighted average of all materials present in the element. Use of these variables can substantially decrease the size of the output database for models with many Eulerian materials. For example: SVAVG Volume fraction averaged stress. Node ordering and face numbering on elements All elements must have eight nodes. Degenerate elements are not supported. face 2 face 5 face 6 face 4 face 1 face 3 8 - node element Element faces Face 1 Face 2 Face 3 Face 4 Face 5 Face 6 1 – 2 – 3 – 4 face 5 – 8 – 7 – 6 face 1 – 5 – 6 – 2 face 2 – 6 – 7 – 3 face 3 – 7 – 8 – 4 face 4 – 8 – 5 – 1 face Numbering of integration points for output The single integration point is located at the centroid of the element. All materials within the element are evaluated at this integration point. 32.15 User-defined elements • “User-defined elements,” Section 32.15.1 • “User-defined element library,” Section 32.15.2 32.15.1 USER-DEFINED ELEMENTS Products: Abaqus/Standard Abaqus/Explicit References • “User-defined element library,” Section 32.15.2 • “UEL,” Section 1.1.27 of the Abaqus User Subroutines Reference Manual • “UELMAT,” Section 1.1.28 of the Abaqus User Subroutines Reference Manual • “VUEL,” Section 1.2.10 of the Abaqus User Subroutines Reference Manual • “Accessing Abaqus thermal materials,” Section 2.1.18 of the Abaqus User Subroutines Reference Manual • “Accessing Abaqus materials,” Section 2.1.17 of the Abaqus User Subroutines Reference Manual • *MATRIX • *UEL PROPERTY • *USER ELEMENT Overview User-defined elements: • can be finite elements in the usual sense of representing a geometric part of the model; • can be feedback links, supplying forces at some points as functions of values of displacement, velocity, etc. at other points in the model; • can be used to solve equations in terms of nonstandard degrees of freedom; • can be linear or nonlinear; and • can access selected materials from the Abaqus material library. Assigning an element type key to a user-defined element You must assign an element type key to a user-defined element. The element type key must be of the form Un in Abaqus/Standard and VUn in Abaqus/Explicit, where n is a positive integer that identifies the element type uniquely. For example, you can define element types U1, U2, U3, VU1, VU7, etc. In Abaqus/Standard n must be less than 10000; while in Abaqus/Explicit n must be less than 9000. The element type key is used to identify the element in the element definition. For general user elements the integer part of the identifier is provided in user subroutines UEL, UELMAT and VUEL so that you can distinguish between different element types. Input File Usage: *USER ELEMENT, TYPE=element_type Invoking user-defined elements User-defined elements are invoked in the same way as native Abaqus elements: you specify the element type, Un or VUn, and define element numbers and nodes associated with each element . User elements can be assigned to element sets in the usual way, for cross-reference to element property definitions, output requests, distributed load specifications, etc. Material definitions (“Material data definition,” Section 21.1.2) are relevant only to user-defined elements in Abaqus/Standard. If a material is assigned to a user-defined element (“Assigning an Abaqus material to the user element”), user subroutine UELMAT will be used to define the element response. User subroutine UELMAT allows access to selected Abaqus materials. If no material definition is specified, all material behavior must be defined in user subroutines UEL and VUEL, based on user-defined material constants and on solution-dependent state variables associated with the element and calculated in the same subroutines. For linear user elements all material behavior must be defined through a user-defined stiffness matrix. Input File Usage: Use the following options to invoke a user-defined element: *USER ELEMENT, TYPE=element_type *ELEMENT, TYPE=element_type Defining the active degrees of freedom at the nodes Any number of user element types can be defined and used in a model. Each user element can have any number of nodes, at each of which a specified set of degrees of freedom is used by the element. The activated degrees of freedom should follow the Abaqus convention (“Conventions,” Section 1.2.2). In Abaqus/Standard this is important because the convergence criteria are based on the degrees of freedom numbers. In Abaqus/Explicit the activated degrees of freedom must follow the Abaqus convention because these are the only degrees of freedom that can be updated. Abaqus always works in the global system when passing information to or from a user element. Therefore, the user element’s stiffness, mass, etc. should always be defined with respect to global directions at its nodes, even if local transformations (“Transformed coordinate systems,” Section 2.1.5) are applied to some of these nodes. You define the ordering of the variables on a user element. The standard and recommended ordering is such that the degrees of freedom at the first node appear first, followed by the degrees of freedom at the second node, etc. For example, suppose that the user-defined element type is a planar beam with three nodes. The element uses degrees of freedom 1, 2, and 6 ( ) at its first and last node and degrees of freedom 1 and 2 at its second (middle) node. In this case the ordering of variables on the element is: , and , Element variable number Node Degree of freedom Element variable number Node Degree of freedom This ordering will be used in most cases. However, if you define an element matrix that does not have its degrees of freedom ordered in this way, you can change the ordering of the degrees of freedom as outlined below. You specify the active degrees of freedom at each node of the element. If the degrees of freedom are the same at all of the element’s nodes, you specify the list of degrees of freedom only once. Otherwise, you specify a new list of degrees of freedom each time the degrees of freedom at a node are different from those at previous nodes. Thus, different nodes of the element can use different degrees of freedom; this is especially useful when the element is being used in a coupled field problem so that, for example, some of its nodes have displacement degrees of freedom only, while others have displacement and temperature degrees of freedom. This method will produce an ordering of the element variables such that all of the degrees of freedom at the first node appear first, followed by the degrees of freedom at the second node, etc. In Abaqus/Standard there are two ways to define element variable numbers that order the degrees of freedom on the element differently. Since the user element can accept repeated node numbers when defining the nodal connectivity for the element, the element can be declared to have one node per degree of freedom on the element. For example, if the element is a planar, 3-node triangle for stress analysis, it has three nodes, each of which has degrees of freedom 1 and 2. If all degrees of freedom 1 are to appear first in the element variables, the element can be defined with six nodes, the first three of which have degree of freedom 1, while nodes 4–6 have degree of freedom 2. The element variables would be ordered as follows: Element variable number Node Degree of freedom 32.15.1–3 Alternatively, the user element variables can be defined so as to order the degrees of freedom on the element in any arbitrary fashion. You specify a list of degrees of freedom for the first node on the element. All nodes with a nodal connectivity number that is less than the next connectivity number for which a list of degrees of freedom is specified will have the first list of degrees of freedom. The second list of degrees of freedom will be used for all nodes until a new list is defined, etc. If a new list of degrees of freedom is encountered with a nodal connectivity number that is less than or equal to that given with the previous list, the previous list’s degrees of freedom will be assigned through the last node of the element. This generation of degrees of freedom can be stopped before the last node on the element by specifying a nodal connectivity number with an empty (blank) list of degrees of freedom. Example The above procedure continues using this new list to define additional degrees of freedom in accordance with the new node and degrees of freedom. For example, consider a 3-node beam that has degrees of freedom 1, 2, and 6 at nodes 1 and 3 and degrees of freedom 1 and 2 at node 2 (middle node). To order degrees of freedom 1 first, followed by 2, followed by 6, the following input could be used: *USER ELEMENT 1, 2 1, 6 2, 3, 6 In this case the ordering of the variables on the element is: Element variable number Node Degree of freedom Requirements for activated degrees of freedom in Abaqus/Explicit There are the following additional requirements with respect to activated degrees of freedom on a user element of type VUn: • Only degrees of freedom 1 through 6, 8, and 11 can be activated because these are the only degrees of freedom numbers that can be updated in Abaqus/Explicit. (In Abaqus/Standard degrees of freedom 1 through 30 can be used.) • If one translational degree of freedom is activated at a node, all translational degrees of freedom up to the specified maximum number of coordinates must be activated at that node; moreover, the translational degrees of freedom at the node must be in consecutive order. • In three-dimensional analyses, if one rotational degree of freedom is activated at a node, all three rotational degrees of freedom must be activated in consecutive order. For example, if you define a 4-node three-dimensional user element that has translations and rotations active at the first and fourth nodes, temperature only at the second node, and translations and temperature at the third node, the following input could be used: *USER ELEMENT 1,2,3,4,5,6 2,11 3,1,2,3,11 4,1,2,3,4,5,6 Rotation update in geometrically nonlinear analyses If all three rotational degrees of freedom (4, 5, and 6) are used at a node in a geometrically nonlinear analysis, Abaqus assumes that these rotations are finite rotations. In this case the incremental values of these degrees of freedom are not simply added to the total values: the quaternion update formulae are used instead. Similarly, the corrections are not simply added to the incremental values. The update procedure is described in “Rotation variables,” Section 1.3.1 of the Abaqus Theory Manual, and is mentioned in “Conventions,” Section 1.2.2. To avoid the rotation update in a geometrically nonlinear analysis in Abaqus/Standard, you may define repeated node numbers in the nodal connectivity of the element such that at least one of the degrees of freedom 4, 5, or 6 is missing from the degree of freedom list at each node. Visualizing user-defined elements in Abaqus/CAE Plotting of user elements is not supported in Abaqus/CAE. However, if the user elements contain displacement degrees of freedom, they can be overlaid with standard elements; and model plots of these standard elements can be displayed, allowing you to see the shape of the user elements. If deformed mesh plots of the user elements are required, the material properties of the overlaying standard elements must be chosen so that the solution is not changed by including them. If this technique is used, nodes of the user element will be tied to nodes of the standard elements. Therefore, degrees of freedom 1, 2, and 3 in the user element must correspond to the displacement degrees of freedom at the nodes of the standard elements. Defining a linear user element in Abaqus/Standard Linear user elements can be defined only in Abaqus/Standard. In the simplest case a linear user element can be defined as a stiffness matrix and, if required, a mass matrix. In these matrices can be read from a results file or defined directly. Reading the element matrices from an Abaqus/Standard results file To read the element matrices from an Abaqus/Standard results file, you must have written the stiffness and/or mass matrices in a previous analysis to the results file as element matrix output (“Element matrix output in Abaqus/Standard” in “Output,” Section 4.1.1) or substructure matrix output (“Writing the recovery matrix, reduced stiffness matrix, mass matrix, load case vectors, and gravity vectors to a file” in “Defining substructures,” Section 10.1.2). You must specify the element number, n, or substructure identifier, Zn, to which the matrices correspond. For models defined in terms of an assembly of part instances (“Defining an assembly,” Section 2.10.1), the element numbers written to the results file are internal numbers generated by Abaqus/Standard . A map between these internal numbers and the original element numbers and part instance names is provided in the data file of the analysis from which the element matrix output was written. In addition, for element matrix output you must specify the step number and increment number at which the element matrix was written. These items are not required if a substructure whose matrix was output during its generation is used. Input File Usage: *USER ELEMENT, FILE=name, OLD ELEMENT=n or Zn, STEP=n, INCREMENT=n Defining the linear user element by specifying the matrices directly If you define the stiffness and/or mass matrix directly, you must specify the number of nodes associated with the element. Input File Usage: *USER ELEMENT, LINEAR, NODES=n Defining whether or not the element matrices are symmetric If the element matrices are not symmetric, you can request that Abaqus/Standard use its nonsymmetric equation solution capability . Input File Usage: *USER ELEMENT, LINEAR, NODES=n, UNSYMM Defining the mass or stiffness matrix You define the element mass matrix and the element stiffness matrix separately. If the element is a heat transfer element, the “stiffness matrix” is the conductivity matrix and the “mass matrix” is the specific heat matrix. You can define either one matrix for the element (mass or stiffness) or both types of matrices. You can read the mass and/or stiffness matrices from a file or define them directly. In either case Abaqus/Standard reads four values per line, using F20 format. This format ensures that the data are read with adequate precision. Data written in E20.14 format can be read under this format. Start with the first column of the matrix. Start a new line for each column. If you do not specify that the element matrix is unsymmetric, give the matrix entries from the top of each column to the diagonal term only: do not give the terms below the diagonal. If you specify that the element matrix is unsymmetric, give all terms in each column, starting from the top of the column. Input File Usage: Use the following option to define the element mass matrix: *MATRIX, TYPE=MASS Use the following option to define the element stiffness matrix: *MATRIX, TYPE=STIFFNESS Use the following option to read the element mass or stiffness matrix from a file: *MATRIX, TYPE=MASS or STIFFNESS, INPUT=file_name For example, if the matrix is symmetric, the following data lines should be used: Etc. If the matrix is unsymmetric, the following data lines should be used: … …, Etc. where m is the size of the matrix and column j. is the entry in the matrix for row i Geometrically nonlinear analysis When a linear user element is used in a geometrically nonlinear analysis, the stiffness matrix provided will not be updated to account for any nonlinear effects such as finite rotations. Defining the element properties You must associate a property definition with every user element, even though no property values (except Rayleigh damping factors) are associated with linear user elements. Input File Usage: Use the following option to associate a property definition with a user element set: *UEL PROPERTY, ELSET=name Defining Rayleigh damping for direct-integration dynamic analysis You can define the Rayleigh damping factors for direct-integration dynamic analysis (“Implicit dynamic analysis using direct integration,” Section 6.3.2) for linear user elements. The Rayleigh damping factors are defined as is the damping matrix, where are the user-specified damping factors. See “Material damping,” Section 26.1.1, for more information on Rayleigh damping. is the stiffness matrix, and is the mass matrix, and Input File Usage: *UEL PROPERTY, ELSET=name, ALPHA= , BETA= Defining loads to the nodes of linear user-defined elements in the You can apply point loads, moments, fluxes, etc. usual way using concentrated loads and concentrated fluxes (“Concentrated loads,” Section 33.4.2, and “Thermal loads,” Section 33.4.4). Distributed loads and fluxes cannot be defined for linear user-defined elements. Defining a general user element General user elements are defined in user subroutines UEL and UELMAT in Abaqus/Standard and in user subroutine VUEL in Abaqus/Explicit. The implementation of user elements in user subroutines is recommended only for advanced users. Defining the number of nodes associated with the element You must specify the number of nodes associated with a general user element. You can define “internal” nodes that are not connected to other elements. Input File Usage: *USER ELEMENT, NODES=n Defining whether or not the element matrices are symmetric in Abaqus/Standard If the contribution of the element to the Jacobian operator matrix of the overall Newton method is not symmetric (i.e., the element matrices are not symmetric), you can request that Abaqus/Standard use its nonsymmetric equation solution capability . Input File Usage: *USER ELEMENT, NODES=n, UNSYMM Defining the maximum number of coordinates needed at any nodal point You can define the maximum number of coordinates needed in user subroutines UEL, UELMAT, or VUEL at any node point of the element. Abaqus assigns space to store this many coordinate values at all of the nodes associated with elements of this type. The default maximum number of coordinates at each node is 1. Abaqus will change the maximum number of coordinates to be the maximum of the user-specified value or the value of the largest active degree of freedom of the user element that is less than or equal to 3. For example, if you specify a maximum number of coordinates of 1 and the active degrees of freedom of the user element are 2, 3, and 6, the maximum number of coordinates will be changed to 3. If you specify a maximum number of coordinates of 2 and the active degrees of freedom of the user element are 11 and 12, the maximum number of coordinates will remain as 2. Input File Usage: *USER ELEMENT, COORDINATES=n Defining the element properties You can define the number of properties associated with a particular user element and then specify their numerical values. Specifying the number of property values required Any number of properties can be defined to be used in forming a general user element. You can specify the number of integer property values required, n, and the number of real (floating point) property values required, m; the total number of values required is the sum of these two numbers. The default number of integer property values required is 0 and the default number of real property values required is 0. Integer property values can be used inside user subroutines UEL, UELMAT, and VUEL as flags, indices, counters, etc. Examples of real (floating point) property values are the cross-sectional area of a beam or rod, thickness of a shell, and material properties to define the material behavior for the element. Input File Usage: *USER ELEMENT, I PROPERTIES=n, PROPERTIES=m Specifying the numerical values of element properties You must associate a user element property definition with each user-defined element, even if no property values are required. The property values specified in the property definition are passed into user subroutines UEL, UELMAT, and VUEL each time the subroutine is called for the user elements that are in the specified element set. Input File Usage: Use the following option to associate a property definition with a user element set: *UEL PROPERTY, ELSET=name To define the property values, enter all floating point values on the data lines first, followed immediately by the integer values. Eight values should be entered on all data lines except the last one, which may have fewer than eight values. Assigning an Abaqus material to the user element If the Abaqus material library is accessed from a user element, a material must be defined and assigned to the user element. Input File Usage: Use the following option to associate a material with the user element: *UEL PROPERTY, MATERIAL=name If this option is used, user subroutine UELMAT must be used to define the contribution of the element to the model. Otherwise, user subroutine UEL must be used. Assigning an orientation definition If the Abaqus material library is accessed from a user element, you can associate a material orientation definition (“Orientations,” Section 2.2.5) with the user element. The orientation definition specifies a local coordinate system for material calculations in the element. The local coordinate system is assumed to be uniform in a given element and is based on the coordinates at the element centroid. Input File Usage: Use the following option to associate an orientation definition with a user element: *UEL PROPERTY, ORIENTATION=name Specifying the element type If the Abaqus material library is accessed from a user element, the element type must be specified. Input File Usage: Use the following option to define a three-dimensional element in a stress/ displacement or a heat transfer analysis: *USER ELEMENT, TENSOR=THREED Use the following option to define a two-dimensional element in a heat transfer analysis: *USER ELEMENT, TENSOR=TWOD Use the following option to define a plane strain element displacement analysis: *USER ELEMENT, TENSOR=PSTRAIN Use the following option to define a plane stress element displacement analysis: *USER ELEMENT, TENSOR=PSTRESS in a stress/ in a stress/ Specifying the number of integration points If the Abaqus material library is accessed from a user element, the number of integration points must be specified. Input File Usage: Use the following option to specify the number of integration points: *USER ELEMENT, INTEGRATION=n Defining the number of solution-dependent variables that must be stored within the element You can define the number of solution-dependent state variables that must be stored within a general user element. The default number of variables is 1. Examples of such variables are strains, stresses, section forces, and other state variables (for example, hardening measures in plasticity models) used in the calculations within the element. These variables allow quite general nonlinear kinematic and material behavior to be modeled. These solution-dependent state variables must be calculated and updated in user subroutines UEL, UELMAT, and VUEL. As an example, suppose the element has four numerical integration points, at each of which you wish to store strain, stress, inelastic strain, and a scalar hardening variable to define the material state. Assume that the element is a three-dimensional solid, so that there are six components of stress and strain at each integration point. Then, the number of solution-dependent variables associated with each such element is 4 × (6 × 3 + 1) = 76. Input File Usage: *USER ELEMENT, VARIABLES=n Defining the contribution of the element to the model in user subroutine UEL For a general user element in Abaqus/Standard, user subroutine UEL may be coded to define the contribution of the element to the model. Abaqus/Standard calls this routine each time any information about a user-defined element is needed. At each such call Abaqus/Standard provides the values of the nodal coordinates and of all solution-dependent nodal variables (displacements, incremental displacements, velocities, accelerations, etc.) at all degrees of freedom associated with the element, as well as values, at the beginning of the current increment, of the solution-dependent state variables associated with the element. Abaqus/Standard also provides the values of all user-defined properties associated with this element and a control flag array indicating what functions the user subroutine must perform. Depending on this set of control flags, the subroutine must define the contribution of the element to the residual vector, define the contribution of the element to the Jacobian (stiffness) matrix, update the solution-dependent state variables associated with the element, form the mass matrix, and so on. Often, several of these functions must be performed in a single call to the routine. Formulation of an element with user subroutine UEL The element’s principal contribution to the model during general analysis steps is that it provides nodal forces and on the solution-dependent state variables that depend on the values of the nodal variables within the element: geometry, attributes, predefined field variables, distributed loads Here we use the term “force” to mean that quantity in the variational statement that is conjugate to the basic nodal variable: physical force when the associated degree of freedom is physical displacement, moment when the associated degree of freedom is a rotation, heat flux when it is a temperature value, and so on. The signs of the forces in are such that external forces provide positive nodal force values and “internal” forces caused by stresses, internal heat fluxes, etc. in the element provide negative nodal force values. For example, in the case of mechanical equilibrium of a finite element subject to surface tractions and body forces with stress , and with interpolation , In general procedures Abaqus/Standard solves the overall system of equations by Newton’s method: Solve Set Iterate , , where is the residual at degree of freedom N and is the Jacobian matrix. During such iterations you must define , which is the element’s contribution to the residual, , and which is the element’s contribution to the Jacobian we imply that the element’s contribution to of the include terms such as . For example, the on the . By writing the total derivative , should include all direct and indirect dependencies will ; therefore, will generally depend on Use in transient analysis procedures In procedures such as transient heat transfer and dynamic analysis, the problem also involves time integration of rates of change of the nodal degrees of freedom. The time integration schemes used by Abaqus/Standard for the various procedures are described in more detail in the Theory Manual. For example, in transient heat transfer analysis, the backward difference method is used: Therefore, if energy storage), the Jacobian contribution should include the term depends on and (as would be the case if the user element includes thermal where is defined from the time integration procedure as . In all cases where Abaqus/Standard integrates first-order problems in time, the are never stored because they are readily available as . However, for direct, , where implicit integration of dynamic systems Abaqus/Standard requires storage of . These values are, therefore, passed into subroutine UEL. If the user element contains effects that depend on these time derivatives (damping and inertial effects), its Jacobian contribution will include and For the Hilber-Hughes-Taylor scheme and where integration, the same expressions apply with element’s damping matrix, and are the (Newmark) parameters of the integration scheme. For backwark Euler time is the equal to unity. The term and is its mass matrix. The Hilber-Hughes-Taylor scheme writes the overall dynamic equilibrium equations as where is often is the total force at degree of freedom N, excluding d’Alembert (inertia) forces. referred to as the “static residual.” Therefore, if a user element is to be used with Hilber-Hughes-Taylor time integration, the element’s contribution to the overall residual must be formulated in the same way. Since Abaqus/Standard provides information only at the time point at which UEL is called, this implies that each time UEL is called the if half-increment residual calculations are required, where from the beginning of the previous increment) and used to store if half-increment residual calculations are required) for use in the next increment. This complication can be avoided if the numerical damping control parameter, , for the dynamic step is set to zero; i.e., if the trapezoidal rule is used for integration of the dynamic equations . This complication is also avoided with the backward Euler time integration operator because dynamic equilibrium is enforced at the end of the step. array must be used to recover indicates (and (and If solution-dependent state variables ( ) are used in the element, a suitable time integration method must be coded into subroutine UEL for these variables. Any of the associated with the element that are not shared with standard Abaqus/Standard elements may be integrated in time by any , etc. at particular points suitable technique. If, in such cases, it is necessary to store values of in time, the solution-dependent state variable array, , can be used for this purpose. Abaqus/Standard will still compute and store values of using the formulae associated with whatever time integrator it is using, but these values need not be used. To ensure accurate, stable time integration, you can control the size of the time increment used by Abaqus/Standard. and , Constraints defined with Lagrange multipliers Introduction of constraints with Lagrange multipliers should be avoided since Abaqus/Standard cannot detect such variables and avoid eigensolver problems by proper ordering of the equations. Defining the contribution of the element to the model in user subroutine UELMAT Alternatively, for a general user element in Abaqus/Standard, user subroutine UELMAT may be coded to define the contribution of the element to the model. User subroutine UELMAT is an enhanced version of user subroutine UEL; consequently, all the information provided for user subroutine UEL is also valid for user subroutine UELMAT. The enhancement allows you to access some of the material models from the Abaqus material library from UELMAT. UELMAT works only with a subset of procedures for which UEL is available: • static; • direct-integration dynamic; • frequency extraction; • steady-state uncouple heat transfer; and • transient uncouple heat transfer. User subroutine UELMAT will be called if an Abaqus material model is assigned to a user element ; otherwise, user subroutine UEL will be called. Accessing Abaqus materials from user subroutine UELMAT Abaqus allows you to access some of the material models from the Abaqus material library from user subroutine UELMAT. The material models are accessed through the utility routines MATERIAL_LIB_MECH and MATERIAL_LIB_HT (“Accessing Abaqus thermal materials,” Section 2.1.18 of the Abaqus User Subroutines Reference Manual, and “Accessing Abaqus materials,” Section 2.1.17 of the Abaqus User Subroutines Reference Manual). Each time user subroutine UELMAT is called with the flags set to values that require computation of the right-hand-side vector and the element Jacobian, the material library must be called for each integration point, where the number of integration points is specified in the element definition (“Specifying the number of integration points” in “User-defined elements,” Section 32.15.1). The material models that are accessible from user subroutine UELMAT are: • linear elastic model; • hyperelastic model; • Ramberg-Osgood model; • classical metal plasticity models (Mises and Hill); • extended Drucker-Prager model; • modified Drucker-Prager/Cap plasticity model; • porous metal plasticity model; • elastomeric foam material model; and • crushable foam plasticity model. Defining the contribution of the element to the model in user subroutine VUEL For a general user element in Abaqus/Explicit, user subroutine VUEL must be coded to define the contribution of the element to the model. Abaqus/Explicit calls this routine each time any information about a user-defined element is needed. At each such call Abaqus/Explicit provides the values of the nodal coordinates and of all solution-dependent nodal variables (displacements, velocities, accelerations, etc.) at all degrees of freedom associated with the element, as well as values of the solution-dependent state variables associated with the element at the beginning of the current increment. The incremental displacements are those obtained in a previous increment. Abaqus/Explicit also provides the values of all user-defined properties associated with this element and a control flag array indicating what functions the user subroutine must perform. Depending on this set of control flags, the subroutine must define the contribution of the element to the internal or external force/flux vector, form the mass/capacity matrix, update the solution-dependent state variables associated with the element, and so on. The element’s principal contribution to the model is that it provides nodal forces that depend , and on the solution-dependent on the values of the nodal variables state variables within the element: , the rate of nodal variables geometry, attributes, predefined field variables, distributed loads In addition, the element mass matrix external load contribution from the element due to specified distributed loading. Abaqus/Explicit solves for the accelerations at the end of the increment using can be defined. Optionally, you can also define the In each increment where using the central difference method is the applied load vector. The solution (velocity, displacement) is then integrated in time For coupled temperature/displacement elements the temperatures are computed at the beginning of the increment using where vector. The temperature is integrated in time using the explicit forward-difference integration rule, is the lumped capcitance matrix, is the applied nodal source, and is the internal flux More details can be found in “Explicit dynamic analysis,” Section 6.3.3 and “Fully coupled thermal- stress analysis,” Section 6.5.3. The signs of the forces defined in are such that external forces provide positive nodal force values and “internal” forces caused by stresses, damping effects, internal heat fluxes, etc. in the element provide negative nodal force values. Internal forces due to bulk viscosity are dependent on the scaled mass of the element. The necessary information (bulk viscosity constants and mass scaling factors) is passed into the user subroutine for this purpose. Requirements for defining the mass matrix As explained in “Explicit dynamic analysis,” Section 6.3.3, what makes the explicit time integration method efficient is that the mass inversion process is extremely effective. This is due to the fact that most of the nonzero entries in the mass matrix are located on the diagonal positions. The only exception is for rotational degrees of freedom in three-dimensional analyses in which case at each node an anisotropic rotary inertia (symmetric 3 × 3 tensor) can be defined. In these cases some of the nonzero entries in the mass matrix may be off-diagonal; but the inversion process is local and, hence, very effective. The mass matrix defined in user subroutine VUEL must adhere to these requirements as illustrated in detail in “VUEL,” Section 1.2.10 of the Abaqus User Subroutines Reference Manual. If you specify a zero mass matrix or skip the definition of the mass matrix altogether, Abaqus/Explicit issues an error message. The definition of a realistic mass matrix is not mandatory, but it is strongly recommended. If you choose to not define a realistic mass matrix using the user subroutine, you must provide realistic mass, rotary inertia, heat capacity, etc. at all nodes and at all degrees of freedom associated with the user element. This can be accomplished by various means, such as by defining mass and rotary inertia elements at the nodes or by connecting the user element to other elements for which density, heat capacity, etc. was specified. Mass is computed only once at the beginning of the analysis. Consequently, the mass of the user element cannot be changed arbitrarily during the analysis. If necessary, mass scaling is applied accordingly to ensure the requested time incrementation. Definition of the stable time increment Since the central difference operator is conditionally stable, the time increments in Abaqus/Explicit must be somewhat smaller than the stable time increment. You must provide an accurate estimate for the stable time increment associated with the user element. This scalar value is highly dependent on the element formulation, and sophisticated coding may be required inside the user subroutine to obtain a reliable estimate. A conservative estimate will reduce the time increment size for the entire analysis and, hence, lead to longer analysis times. Defining loads You can apply point loads, moments, fluxes, etc. to the nodes of general user-defined elements in the usual way, using concentrated loads and concentrated fluxes (“Concentrated loads,” Section 33.4.2, and “Thermal loads,” Section 33.4.4). You can also define distributed loads and fluxes for general user-defined elements (“Distributed loads,” Section 33.4.3, and “Thermal loads,” Section 33.4.4). These loads require a load type key. For user-defined elements, you can define load type keys of the forms Un and, in Abaqus/Standard, UnNU, where n is any positive integer. If the load type key is of the form Un, the load magnitude is defined directly and follows the standard Abaqus conventions with respect to its amplitude variation as a function of time. In Abaqus/Standard, if the load key is of the form UnNU, all of the load definition will be accomplished inside subroutine UEL and UELMAT. Each time Abaqus/Standard calls subroutine UEL or UELMAT, it tells the subroutine how many distributed loads/fluxes are currently active. For each active load or flux of type Un Abaqus/Standard gives the current magnitude and current increment in magnitude of the load. The coding in subroutine UEL or UELMAT must distribute the loads into consistent equivalent nodal forces and, if necessary, provide their contribution to the Jacobian matrix—the “load stiffness matrix.” In Abaqus/Explicit only load keys of the form Un can be used, and they can be used only for distributed loads (however, thermal fluxes can be defined in the coding in subroutine VUEL). Each time Abaqus/Explicit calls subroutine VUEL, it tells the subroutine which load number is currently active and the current magnitude of the load. The coding in subroutine VUEL must distribute the loads into consistent equivalent nodal forces. Defining output All quantities to be output must be saved as solution-dependent state variables. In Abaqus/Standard, the solution-dependent state variables can be printed or written to the results file using output variable identifier SDV (“Abaqus/Standard output variable identifiers,” Section 4.2.1). The components of solution-dependent state variables that belong to a user element are not available in Abaqus/CAE. You can write output to separate files in a table format that can be accessed in Abaqus/CAE to produce history output. Defining wave kinematic data A utility routine GETWAVE is provided in user subroutine UEL to access the wave kinematic data defined for an Abaqus/Aqua analysis (“Abaqus/Aqua analysis,” Section 6.11.1). This utility is discussed in “Obtaining wave kinematic data in an Abaqus/Aqua analysis,” Section 2.1.13 of the Abaqus User Subroutines Reference Manual, where the arguments to GETWAVE and the syntax for its use are defined. Use in contact Only node-based surfaces (“Node-based surface definition,” Section 2.3.3) can be created on user-defined elements. Hence, these elements can be used to define only slave surfaces in a contact analysis. In Abaqus/Explicit the user elements will not be included in the general contact algorithm automatically. Node-based surfaces can be defined using these nodes and then included in the general contact definition. Import of user elements User elements cannot be imported from an Abaqus/Standard analysis into an Abaqus/Explicit analysis or vice versa. Equivalent user elements can be defined in both products to overcome this limitation. However, the state variables associated with these elements will not be communicated. 32.15.2 USER-DEFINED ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit References • “User-defined elements,” Section 32.15.1 • “UEL,” Section 1.1.27 of the Abaqus User Subroutines Reference Manual • “UELMAT,” Section 1.1.28 of the Abaqus User Subroutines Reference Manual • “VUEL,” Section 1.2.10 of the Abaqus User Subroutines Reference Manual • *MATRIX • *UEL PROPERTY • *USER ELEMENT Overview This section provides a reference to the user-defined elements available in Abaqus/Standard and Abaqus/Explicit. Element types Un VUn n must be a positive integer ( in Abaqus/Standard n must be a positive integer ( in Abaqus/Explicit Active degrees of freedom As defined in the user element definition. Additional solution variables ) that will define the element type uniquely ) that will define the element type uniquely You can define solution variables associated with nodes that are not connected to other elements. However, in Abaqus/Standard, definition of constraints with Lagrange multipliers in user elements should be avoided because of potential equation solver problems. In Abaqus/Explicit definition of constraints with Lagrange multipliers is not possible because the stable time increment would decrease to infinitesimally small values. Nodal coordinates required None required for linear user elements. As needed in user subroutines UEL, UELMAT, or VUEL for general user elements. The maximum number of coordinates per node is specified in the user element definition (see “Defining the maximum number of coordinates needed at any nodal point” in “User-defined elements,” Section 32.15.1). The first coordinate entries at each node should correspond to the standard Abaqus convention (X, Y, Z or r, z for axisymmetric elements). Element property definition For a linear user element the properties are the stiffness and mass, defined via user-defined matrices or read from an Abaqus/Standard results file. If necessary, you can specify Rayleigh damping values for linear user elements in the element property definition. For a general user element defined via user subroutines UEL, UELMAT, or VUEL, you define the number of element properties in the user element definition and provide the numerical values in the element property definition. The definition of these properties depends on your coding in subroutine UEL, UELMAT, or VUEL. Input File Usage: *UEL PROPERTY Element-based loading None for linear user elements. Un: Distributed load or flux whose magnitude is given via distributed load or distributed flux loading definitions for a general user element. n must be a positive integer that is passed into user subroutines UEL, UELMAT, or VUEL to identify the particular load type. UnNU: Available in Abaqus/Standard only. Distributed load or flux that is completely defined as equivalent nodal values inside user subroutine UEL or UELMAT for a general user element. n must be will be passed into subroutine UEL or UELMAT when such a load is active to a positive integer: identify the load type. The minus sign on n indicates that the load is of type NU. Element output For a linear user element there are no stress or strain components since the element only appears as a stiffness and mass. For a general user element any stress, strain, or other solution-dependent variables within the element must be defined as solution-dependent state variables by your coding within subroutine UEL, UELMAT, or VUEL. In Abaqus/Standard, they can be output using output variable SDV. Currently element output to the output database is not supported for user-defined elements. Node ordering on elements As defined in the user element definition. EI.1 Abaqus/Standard ELEMENT INDEX This index provides a reference to all of the element types that are available in Abaqus/Standard. Elements are listed in alphabetical order, where numerical characters precede the letter “A” and two-digit numbers are put in numerical, rather than “alphabetical,” order. Thus, AC1D2 precedes ACAX4, and AC3D20 follows AC3D8. For certain options, such as contact and surface-based distributing coupling, Abaqus may generate internal elements (such as IDCOUP3D for surface-based distributing coupling). These internal element names are not included in the index below but may appear in an output database (.odb) or data (.dat) file. 28.1.2 28.1.2 28.1.3 28.1.3 28.1.3 28.1.3 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.6 28.1.6 28.1.6 28.1.6 28.3.2 28.3.2 28.3.2 28.3.2 28.3.2 28.3.2 28.3.2 28.3.2 32.13.2 2-node acoustic link 3-node acoustic link 3-node linear 2-D acoustic triangle 4-node linear 2-D acoustic quadrilateral 6-node quadratic 2-D acoustic triangular prism 8-node quadratic 2-D acoustic quadrilateral 4-node linear acoustic tetrahedron 6-node linear acoustic triangular prism 8-node linear acoustic brick 10-node quadratic acoustic tetrahedron 15-node quadratic acoustic triangular prism 20-node quadratic acoustic brick 3-node linear axisymmetric acoustic triangle 4-node linear axisymmetric acoustic quadrilateral 6-node quadratic axisymmetric acoustic triangle 8-node quadratic axisymmetric acoustic quadrilateral 2-node linear 2-D acoustic infinite element 3-node quadratic 2-D acoustic infinite element 3-node linear 3-D acoustic infinite element 4-node linear 3-D acoustic infinite element 6-node quadratic 3-D acoustic infinite element 8-node quadratic 3-D acoustic infinite element 2-node linear axisymmetric acoustic infinite element 3-node quadratic axisymmetric acoustic infinite element 1-node acoustic interface element EI.1–1 AC1D2 AC1D3 AC2D3 AC2D4 AC2D6 AC2D8 AC3D4 AC3D6 AC3D8 AC3D10 AC3D15 AC3D20 ACAX3 ACAX4 ACAX6 ACAX8 ACIN2D2 ACIN2D3 ACIN3D3 ACIN3D4 ACIN3D6 ACIN3D8 ACINAX2 ACINAX3 2-node linear 2-D acoustic interface element (this element has been renamed to ASI2D2) 2-node linear axisymmetric acoustic interface element (this element has been renamed to ASIAX2) 2-node linear 2-D acoustic interface element 3-node quadratic 2-D acoustic interface element 3-node quadratic 2-D acoustic interface element (this element has been renamed to ASI2D3) 3-node quadratic axisymmetric acoustic interface element (this element has been renamed to ASIAX3) 3-node linear 3-D acoustic interface element 4-node linear 3-D acoustic interface element 6-node quadratic 3-D acoustic interface element 8-node quadratic 3-D acoustic interface element 4-node linear 3-D acoustic interface element (this element has been renamed to ASI3D4) 8-node quadratic 3-D acoustic interface element (this element has been renamed to ASI3D8) 2-node linear axisymmetric acoustic interface element 3-node quadratic axisymmetric acoustic interface element 2-node linear beam in a plane 2-node linear beam in a plane, hybrid formulation 3-node quadratic beam in a plane 3-node quadratic beam in a plane, hybrid formulation 2-node cubic beam in a plane 2-node cubic beam in a plane, hybrid formulation 2-node linear beam in space 2-node linear beam in space, hybrid formulation 2-node linear open-section beam in space 2-node linear open-section beam in space, hybrid formulation 3-node quadratic beam in space 3-node quadratic beam in space, hybrid formulation 3-node quadratic open-section beam in space 3-node quadratic open-section beam in space, hybrid formulation 2-node cubic beam in space 2-node cubic beam in space, hybrid formulation 4-node linear tetrahedron 32.13.2 32.13.2 32.13.2 32.13.2 32.13.2 32.13.2 32.13.2 32.13.2 32.13.2 32.13.2 32.13.2 32.13.2 32.13.2 32.13.2 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 28.1.4 EI.1–2 ASI2 ASI2A ASI2D2 ASI2D3 ASI3 ASI3A ASI3D3 ASI3D4 ASI3D6 ASI3D8 ASI4 ASI8 ASIAX2 ASIAX3 B21 B21H B22 B22H B23 B23H B31 B31H B31OS B31OSH B32 B32H B32OS B32OSH B33 B33H 4-node linear piezoelectric tetrahedron 4-node linear tetrahedron, hybrid, linear pressure 4-node linear coupled pore pressure element 4-node thermally coupled tetrahedron, linear displacement and temperature 6-node linear triangular prism 6-node linear piezoelectric triangular prism 6-node linear triangular prism, hybrid, constant pressure 6-node linear coupled pore pressure element 6-node thermally coupled triangular prism, linear displacement and temperature 8-node linear brick 8-node linear piezoelectric brick 8-node linear brick, hybrid, constant pressure 8-node thermally coupled brick, trilinear displacement and temperature, hybrid, constant pressure 8-node linear brick, incompatible modes 8-node linear brick, hybrid, linear pressure, incompatible modes 8-node brick, trilinear displacement, trilinear pore pressure 8-node brick, trilinear displacement, trilinear pore pressure, hybrid, constant pressure 8-node brick, trilinear displacement, trilinear pore pressure, trilinear temperature, hybrid, constant pressure 8-node brick, trilinear displacement, trilinear pore pressure, trilinear temperature 8-node linear brick, reduced integration, hourglass control 8-node linear brick, hybrid, constant pressure, reduced integration, hourglass control 8-node thermally coupled brick, trilinear displacement and temperature, reduced integration, hourglass control, hybrid, constant pressure 8-node brick, trilinear displacement, trilinear pore pressure, reduced integration 8-node brick, trilinear displacement, trilinear pore pressure, reduced integration, hybrid, constant pressure 8-node brick, trilinear displacement, trilinear pore pressure, trilinear temperature, reduced integration, hybrid, constant pressure 8-node brick, trilinear displacement, trilinear pore pressure, trilinear temperature, reduced integration 8-node thermally coupled brick, trilinear displacement and temperature, reduced integration, hourglass control 8-node thermally coupled brick, trilinear displacement and temperature 10-node quadratic tetrahedron 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 EI.1–3 C3D4E C3D4H C3D4P C3D4T C3D6 C3D6E C3D6H C3D6P C3D6T C3D8 C3D8E C3D8H C3D8HT C3D8I C3D8IH C3D8P C3D8PH C3D8PHT C3D8PT C3D8R C3D8RH C3D8RHT C3D8RP C3D8RPH C3D8RPHT C3D8RPT C3D8RT C3D8T linear improved surface stress linear pressure, hourglass 10-node quadratic piezoelectric tetrahedron 10-node quadratic tetrahedron, hybrid, constant pressure 10-node general-purpose quadratic tetrahedron, visualization 10-node modified tetrahedron, hourglass control 10-node modified quadratic tetrahedron, hybrid, control 10-node thermally coupled modified quadratic tetrahedron, hybrid, pressure, hourglass control 10-node modified displacement and pore pressure tetrahedron, hourglass control 10-node modified displacement and pore pressure tetrahedron, hybrid, linear pressure, hourglass control 10-node modified displacement, pore pressure, and temperature tetrahedron, linear pressure, hourglass control 10-node thermally coupled modified quadratic tetrahedron, hourglass control 15-node quadratic triangular prism 15-node quadratic piezoelectric triangular prism 15-node quadratic triangular prism, hybrid, linear pressure 15 to 18-node triangular prism 15 to 18-node triangular prism, hybrid, linear pressure 20-node quadratic brick 20-node quadratic piezoelectric brick 20-node quadratic brick, hybrid, linear pressure 20-node thermally coupled brick, temperature, hybrid, linear pressure 20-node brick, triquadratic displacement, trilinear pore pressure 20-node brick, triquadratic displacement, trilinear pore pressure, hybrid, linear pressure 20-node quadratic brick, reduced integration 20-node quadratic piezoelectric brick, reduced integration 20-node quadratic brick, hybrid, linear pressure, reduced integration 20-node triquadratic displacement, temperature, hybrid, linear pressure, reduced integration 20-node brick, integration 20-node brick, triquadratic displacement, trilinear pore pressure, hybrid, linear pressure, reduced integration thermally coupled brick, triquadratic displacement, triquadratic displacement, trilinear pore pressure, trilinear trilinear reduced 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 EI.1–4 C3D10E C3D10H C3D10I C3D10M C3D10MH C3D10MHT C3D10MP C3D10MPH C3D10MPT C3D10MT C3D15 C3D15E C3D15H C3D15V C3D15VH C3D20 C3D20E C3D20H C3D20HT C3D20P C3D20PH C3D20R C3D20RE C3D20RH C3D20RHT C3D20RP thermally coupled brick, 20-node temperature, reduced integration 20-node thermally coupled brick, triquadratic displacement, trilinear temperature triquadratic displacement, trilinear 21 to 27-node brick 21 to 27-node brick, hybrid, linear pressure 21 to 27-node brick, reduced integration 21 to 27-node brick, hybrid, linear pressure, reduced integration 3-node linear axisymmetric triangle 3-node linear axisymmetric piezoelectric triangle 3-node linear axisymmetric triangle, hybrid, constant pressure 3-node axisymmetric thermally coupled triangle, temperature linear displacement and 4-node bilinear axisymmetric quadrilateral 4-node bilinear axisymmetric piezoelectric quadrilateral 4-node bilinear axisymmetric quadrilateral, hybrid, constant pressure 4-node axisymmetric thermally coupled quadrilateral, bilinear displacement and temperature, hybrid, constant pressure 4-node bilinear axisymmetric quadrilateral, incompatible modes 4-node bilinear axisymmetric quadrilateral, hybrid, linear pressure, incompatible modes 4-node axisymmetric quadrilateral, bilinear displacement, bilinear pore pressure 4-node axisymmetric quadrilateral, bilinear displacement, bilinear pore pressure, hybrid, constant pressure 4-node axisymmetric quadrilateral, bilinear displacement, bilinear pore pressure, bilinear temperature reduced integration, hourglass 4-node bilinear axisymmetric quadrilateral, control 4-node bilinear axisymmetric quadrilateral, hybrid, constant pressure, reduced integration, hourglass control 4-node thermally coupled axisymmetric quadrilateral, bilinear displacement and temperature, reduced integration, hourglass control 4-node axisymmetric quadrilateral, bilinear displacement, bilinear pore pressure, reduced integration 4-node axisymmetric quadrilateral, bilinear displacement, bilinear pore pressure, hybrid, constant pressure, reduced integration 4-node axisymmetric quadrilateral, bilinear displacement, bilinear pore pressure, bilinear temperature, hybrid, constant pressure, reduced integration EI.1–5 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 C3D20RT C3D20T C3D27 C3D27H C3D27R C3D27RH CAX3 CAX3E CAX3H CAX3T CAX4 CAX4E CAX4H CAX4HT CAX4I CAX4IH CAX4P CAX4PH CAX4PT CAX4R CAX4RH CAX4RHT CAX4RP CAX4RPH CAX4RPT 4-node axisymmetric quadrilateral, bilinear displacement, bilinear pore pressure, bilinear temperature, reduced integration CAX4RT CAX4T CAX6 CAX6E CAX6H CAX6M CAX6MH CAX6MHT CAX6MP CAX6MPH CAX6MT CAX8 CAX8E CAX8H CAX8HT CAX8P CAX8PH CAX8R CAX8RE CAX8RH 4-node thermally coupled axisymmetric quadrilateral, bilinear displacement and temperature, hybrid, constant pressure, reduced integration, hourglass control 4-node axisymmetric thermally coupled quadrilateral, bilinear displacement and temperature 6-node quadratic axisymmetric triangle 6-node quadratic axisymmetric piezoelectric triangle 6-node quadratic axisymmetric triangle, hybrid, linear pressure 6-node modified axisymmetric triangle, hourglass control 6-node modified quadratic axisymmetric triangle, hybrid, hourglass control linear pressure, 6-node modified axisymmetric thermally coupled triangle, hybrid, pressure, hourglass control linear 28.1.6 6-node modified displacement and pore pressure axisymmetric triangle, hourglass control 6-node modified displacement and pore pressure axisymmetric triangle, hybrid, linear pressure, hourglass control 28.1.6 28.1.6 6-node modified axisymmetric thermally coupled triangle, hourglass control linear pressure, 28.1.6 8-node biquadratic axisymmetric quadrilateral 8-node biquadratic axisymmetric piezoelectric quadrilateral 8-node biquadratic axisymmetric quadrilateral, hybrid, linear pressure 8-node axisymmetric thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, hybrid, linear pressure 8-node axisymmetric quadrilateral, biquadratic displacement, bilinear pore pressure 8-node axisymmetric quadrilateral, biquadratic displacement, bilinear pore pressure, hybrid, linear pressure 8-node biquadratic axisymmetric quadrilateral, reduced integration 8-node biquadratic axisymmetric piezoelectric quadrilateral, reduced integration 8-node biquadratic axisymmetric quadrilateral, hybrid, linear pressure, reduced integration 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 CAX8RHT CAX8RP 8-node axisymmetric thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, hybrid, linear pressure, reduced integration 8-node axisymmetric quadrilateral, biquadratic displacement, bilinear pore pressure, reduced integration CAX8RPH CAX8RT CAX8T CAXA4N CAXA4HN CAXA4RN 8-node axisymmetric quadrilateral, biquadratic displacement, bilinear pore pressure, hybrid, linear pressure, reduced integration 8-node axisymmetric thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, reduced integration 8-node axisymmetric thermally coupled quadrilateral, biquadratic displacement, bilinear temperature Bilinear asymmetric-axisymmetric, Fourier quadrilateral with 4 nodes per r–z plane Bilinear asymmetric-axisymmetric, Fourier quadrilateral with 4 nodes per r–z plane, constant Fourier pressure, hybrid Bilinear asymmetric-axisymmetric, Fourier quadrilateral with 4 nodes per r–z plane, reduced integration in r–z planes, hourglass control 28.1.6 28.1.6 28.1.6 28.1.7 28.1.7 28.1.7 CAXA4RHN Bilinear asymmetric-axisymmetric, Fourier quadrilateral with 4 nodes per r–z 28.1.7 CAXA8N CAXA8HN CAXA8PN CAXA8RN plane, constant Fourier pressure, hybrid, reduced integration in r–z planes Biquadratic asymmetric-axisymmetric, Fourier quadrilateral with 8 nodes per r–z plane Biquadratic asymmetric-axisymmetric, Fourier quadrilateral with 8 nodes per r–z plane, linear Fourier pressure, hybrid Biquadratic asymmetric-axisymmetric, Fourier quadrilateral with 8 nodes per r–z plane, bilinear Fourier pore pressure Biquadratic asymmetric-axisymmetric, Fourier quadrilateral with 8 nodes per r–z plane, reduced integration in r–z planes 28.1.7 28.1.7 28.1.7 28.1.7 CAXA8RHN Biquadratic asymmetric-axisymmetric, Fourier quadrilateral with 8 nodes per r–z 28.1.7 CAXA8RPN CCL9 CCL9H CCL12 CCL12H CCL18 CCL18H CCL24 CCL24H CCL24R CCL24RH CGAX3 CGAX3H plane, linear Fourier pressure, hybrid, reduced integration in r–z planes Biquadratic asymmetric-axisymmetric, Fourier quadrilateral with 8 nodes per r–z plane, bilinear Fourier pore pressure, reduced integration in r–z planes 9-node cylindrical prism 9-node cylindrical hybrid prism 12-node cylindrical brick 12-node cylindrical hybrid brick 18-node cylindrical prism 18-node cylindrical hybrid prism 24-node cylindrical brick 24-node cylindrical hybrid brick 24-node cylindrical brick with reduced integration 24-node cylindrical hybrid brick with reduced integration 3-node generalized linear axisymmetric triangle, twist 3-node generalized linear axisymmetric triangle, hybrid, constant pressure, twist 28.1.7 28.1.5 28.1.5 28.1.5 28.1.5 28.1.5 28.1.5 28.1.5 28.1.5 28.1.5 28.1.5 28.1.6 28.1.6 CGAX3HT CGAX3T CGAX4 CGAX4H CGAX4HT CGAX4R CGAX4RH CGAX4RHT CGAX4RT CGAX4T CGAX6 CGAX6H CGAX6M CGAX6MH 3-node generalized axisymmetric thermally coupled triangle, hybrid, constant pressure, linear displacement and temperature, twist 3-node generalized axisymmetric thermally coupled triangle, linear displacement and temperature, twist 4-node generalized bilinear axisymmetric quadrilateral, twist 4-node generalized bilinear axisymmetric quadrilateral, hybrid, constant pressure, twist 4-node generalized axisymmetric thermally coupled quadrilateral, hybrid, constant pressure, bilinear displacement and temperature, twist 4-node generalized bilinear axisymmetric quadrilateral, reduced integration, hourglass control, twist 4-node generalized bilinear axisymmetric quadrilateral, hybrid, constant pressure, reduced integration, hourglass control, twist 4-node generalized axisymmetric thermally coupled quadrilateral, bilinear displacement and temperature, hybrid, constant pressure, reduced integration, hourglass control, twist 4-node generalized axisymmetric thermally coupled quadrilateral, bilinear displacement and temperature, reduced integration, hourglass control, twist 4-node generalized axisymmetric thermally coupled quadrilateral, bilinear displacement and temperature, twist 6-node generalized quadratic axisymmetric triangle, twist 6-node generalized quadratic axisymmetric triangle, hybrid, linear pressure, twist 6-node generalized modified axisymmetric triangle, twist, hourglass control 6-node generalized modified axisymmetric triangle, pressure, hourglass control twist, hybrid, linear CGAX6MT CGAX8 CGAX8H CGAX6MHT 6-node generalized modified thermally coupled axisymmetric triangle, quadratic displacement, linear temperature, hybrid, linear pressure, twist, hourglass control 6-node generalized modified thermally coupled axisymmetric triangle, quadratic displacement, linear temperature, twist, hourglass control 8-node generalized biquadratic axisymmetric quadrilateral, twist 8-node generalized biquadratic axisymmetric quadrilateral, hybrid, pressure, twist 8-node generalized axisymmetric thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, hybrid, linear pressure, twist 8-node generalized biquadratic axisymmetric quadrilateral, reduced integration, twist 8-node generalized biquadratic axisymmetric quadrilateral, hybrid, pressure, reduced integration, twist CGAX8RH CGAX8HT CGAX8R linear linear 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 8-node generalized axisymmetric thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, hybrid, linear pressure, reduced integration, twist 8-node generalized axisymmetric thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, reduced integration, twist 8-node generalized axisymmetric thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, twist 8-node linear one-way infinite brick 12-node quadratic one-way infinite brick 18-node quadratic one-way infinite brick 4-node linear axisymmetric one-way infinite quadrilateral 5-node quadratic axisymmetric one-way infinite quadrilateral 4-node linear plane strain one-way infinite quadrilateral 5-node quadratic plane strain one-way infinite quadrilateral 4-node linear plane stress one-way infinite quadrilateral 5-node quadratic plane stress one-way infinite quadrilateral 4-node axisymmetric cohesive element 6-node axisymmetric pore pressure cohesive element 4-node two-dimensional cohesive element 6-node two-dimensional pore pressure cohesive element 6-node three-dimensional cohesive element 9-node three-dimensional pore pressure cohesive element 8-node three-dimensional cohesive element 12-node three-dimensional pore pressure cohesive element Connector element in a plane between two nodes or ground and a node Connector element in space between two nodes or ground and a node 3-node linear plane strain triangle 3-node linear plane strain piezoelectric triangle 3-node linear plane strain triangle, hybrid, constant pressure 3-node plane strain thermally coupled triangle, temperature 4-node bilinear plane strain quadrilateral 4-node bilinear plane strain piezoelectric quadrilateral 4-node bilinear plane strain quadrilateral, hybrid, constant pressure 4-node plane strain thermally coupled quadrilateral, bilinear displacement and temperature, hybrid, constant pressure 4-node bilinear plane strain quadrilateral, incompatible modes linear displacement and 28.1.6 28.1.6 28.1.6 28.3.2 28.3.2 28.3.2 28.3.2 28.3.2 28.3.2 28.3.2 28.3.2 28.3.2 32.5.10 32.5.10 32.5.8 32.5.8 32.5.9 32.5.9 32.5.9 32.5.9 31.1.4 31.1.4 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 EI.1–9 CGAX8RHT CGAX8RT CGAX8T CIN3D8 CIN3D12R CIN3D18R CINAX4 CINAX5R CINPE4 CINPE5R CINPS4 CINPS5R COHAX4 COHAX4P COH2D4 COH2D4P COH3D6 COH3D6P COH3D8 COH3D8P CONN2D2 CONN3D2 CPE3 CPE3E CPE3H CPE3T CPE4 CPE4E CPE4H CPE4HT 4-node bilinear plane strain quadrilateral, hybrid, linear pressure, incompatible modes 4-node plane strain quadrilateral, bilinear displacement, bilinear pore pressure 4-node plane strain quadrilateral, bilinear displacement, bilinear pore pressure, hybrid, constant pressure 4-node bilinear plane strain quadrilateral, reduced integration, hourglass control 4-node bilinear plane strain quadrilateral, hybrid, constant pressure, reduced integration, hourglass control 4-node bilinear plane strain thermally coupled quadrilateral, hybrid, constant pressure, reduced integration, hourglass control 4-node plane strain quadrilateral, bilinear displacement, bilinear pore pressure, reduced integration, hourglass control 4-node plane strain quadrilateral, bilinear displacement, bilinear pore pressure, hybrid, constant pressure, reduced integration, hourglass control 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 4-node bilinear plane strain thermally coupled quadrilateral, displacement and temperature, reduced integration, hourglass control bilinear 28.1.3 4-node plane strain thermally coupled quadrilateral, bilinear displacement and temperature 6-node quadratic plane strain triangle 6-node quadratic plane strain piezoelectric triangle 6-node quadratic plane strain triangle, hybrid, linear pressure 6-node modified quadratic plane strain triangle, hourglass control 6-node modified quadratic plane strain triangle, hybrid, linear pressure, hourglass control 6-node modified quadratic plane strain thermally coupled triangle, hybrid, linear pressure, hourglass control 6-node modified displacement and pore pressure plane strain triangle, hourglass control 6-node modified displacement and pore pressure plane strain triangle, hybrid, linear pressure, hourglass control 6-node modified quadratic plane strain thermally coupled triangle, hourglass control 8-node biquadratic plane strain quadrilateral 8-node biquadratic plane strain piezoelectric quadrilateral 8-node biquadratic plane strain quadrilateral, hybrid, linear pressure 8-node plane strain thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, hybrid, linear pressure 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 EI.1–10 CPE4IH CPE4P CPE4PH CPE4R CPE4RH CPE4RHT CPE4RP CPE4RPH CPE4RT CPE4T CPE6 CPE6E CPE6H CPE6M CPE6MH CPE6MHT CPE6MP CPE6MPH CPE6MT CPE8 CPE8E CPE8H 8-node plane strain quadrilateral, biquadratic displacement, bilinear pore pressure 8-node plane strain quadrilateral, biquadratic displacement, bilinear pore pressure, hybrid, linear pressure stress 8-node biquadratic plane strain quadrilateral, reduced integration 8-node biquadratic plane strain piezoelectric quadrilateral, reduced integration 8-node biquadratic plane strain quadrilateral, hybrid, linear pressure, reduced integration 8-node plane strain thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, reduced integration, hybrid, linear pressure 8-node plane strain quadrilateral, biquadratic displacement, bilinear pore pressure, reduced integration 8-node biquadratic displacement, bilinear pore pressure, reduced integration, hybrid, linear pressure 8-node plane strain thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, reduced integration 8-node plane strain thermally coupled quadrilateral, biquadratic displacement, bilinear temperature 3-node linear generalized plane strain triangle 3-node linear generalized plane strain triangle, hybrid, constant pressure 3-node generalized plane strain thermally coupled triangle, linear displacement and temperature, hybrid, constant pressure 3-node generalized plane strain thermally coupled triangle, linear displacement and temperature 4-node bilinear generalized plane strain quadrilateral 4-node bilinear generalized plane strain quadrilateral, hybrid, constant pressure 4-node generalized plane strain thermally coupled quadrilateral, bilinear displacement and temperature, hybrid, constant pressure 4-node bilinear generalized plane strain quadrilateral, incompatible modes 4-node bilinear generalized plane strain quadrilateral, hybrid, linear pressure, incompatible modes 4-node bilinear generalized plane strain quadrilateral, reduced integration, hourglass control 4-node bilinear generalized plane strain quadrilateral, hybrid, constant pressure, reduced integration, hourglass control 4-node generalized plane strain thermally coupled quadrilateral, bilinear displacement and temperature, hybrid, constant pressure, reduced integration, hourglass control 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 EI.1–11 CPE8P CPE8PH CPE8R CPE8RE CPE8RH CPE8RHT CPE8RP CPE8RPH CPE8RT CPE8T CPEG3 CPEG3H CPEG3HT CPEG3T CPEG4 CPEG4H CPEG4HT CPEG4I CPEG4IH CPEG4R CPEG4RH linear pressure, 4-node generalized plane strain thermally coupled quadrilateral, bilinear displacement and temperature, reduced integration, hourglass control 4-node generalized plane strain thermally coupled quadrilateral, bilinear displacement and temperature 6-node quadratic generalized plane strain triangle 6-node quadratic generalized plane strain triangle, hybrid, linear pressure 6-node modified generalized plane strain triangle, hourglass control 6-node modified generalized plane strain triangle, hybrid, hourglass control 6-node modified generalized plane strain thermally coupled triangle, quadratic displacement, linear temperature, hybrid, constant pressure, hourglass control 6-node modified generalized plane strain thermally coupled triangle, quadratic displacement, linear temperature, hourglass control 8-node biquadratic generalized plane strain quadrilateral 8-node biquadratic generalized plane strain quadrilateral, hybrid, linear pressure 8-node generalized plane strain thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, hybrid, linear pressure 8-node biquadratic generalized plane strain quadrilateral, reduced integration 8-node biquadratic generalized plane strain quadrilateral, hybrid, linear pressure, reduced integration 8-node generalized plane strain thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, hybrid, linear pressure, reduced integration 8-node generalized plane strain thermally coupled quadrilateral, biquadratic displacement, bilinear temperature 3-node linear plane stress triangle 3-node linear plane stress piezoelectric triangle 3-node plane stress thermally coupled triangle, temperature 4-node bilinear plane stress quadrilateral 4-node bilinear plane stress piezoelectric quadrilateral 4-node bilinear plane stress quadrilateral, incompatible modes 4-node bilinear plane stress quadrilateral, reduced integration, hourglass control 4-node plane stress thermally coupled quadrilateral, bilinear displacement and temperature, reduced integration, hourglass control 4-node plane stress thermally coupled quadrilateral, bilinear displacement and temperature 6-node quadratic plane stress triangle 6-node quadratic plane stress piezoelectric triangle linear displacement and 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 EI.1–12 CPEG4RT CPEG4T CPEG6 CPEG6H CPEG6M CPEG6MH CPEG6MHT CPEG6MT CPEG8 CPEG8H CPEG8HT CPEG8R CPEG8RH CPEG8RHT CPEG8T CPS3 CPS3E CPS3T CPS4 CPS4E CPS4I CPS4R CPS4RT CPS4T CPS6 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 32.2.2 32.2.2 32.2.2 28.1.2 28.1.2 28.1.2 28.1.2 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 CPS6M CPS6MT CPS8 CPS8E CPS8R CPS8RE CPS8RT CPS8T 6-node modified second-order plane stress triangle, hourglass control 6-node modified second-order plane stress thermally coupled triangle, hourglass control 8-node biquadratic plane stress quadrilateral 8-node biquadratic plane stress piezoelectric quadrilateral 8-node biquadratic plane stress quadrilateral, reduced integration 8-node biquadratic plane stress piezoelectric quadrilateral, reduced integration 8-node plane stress thermally coupled quadrilateral, biquadratic displacement, bilinear temperature, reduced integration 8-node plane stress thermally coupled quadrilateral, biquadratic displacement, bilinear temperature Dashpot between a node and ground, acting in a fixed direction Dashpot between two nodes, acting in a fixed direction DASHPOT1 DASHPOT2 DASHPOTA Axial dashpot between two nodes, whose line of action is the line joining the two nodes 2-node heat transfer link 2-node coupled thermal-electrical link 3-node heat transfer link 3-node coupled thermal-electrical link 3-node linear heat transfer triangle 3-node linear coupled thermal-electrical triangle 4-node linear heat transfer quadrilateral 4-node linear coupled thermal-electrical quadrilateral 6-node quadratic heat transfer triangle 6-node quadratic coupled thermal-electrical triangle 8-node quadratic heat transfer quadrilateral 8-node quadratic coupled thermal-electrical quadrilateral 4-node linear heat transfer tetrahedron 4-node linear coupled thermal-electrical tetrahedron 6-node linear heat transfer triangular prism 6-node linear coupled thermal-electrical triangular prism 8-node linear heat transfer brick 8-node linear coupled thermal-electrical brick 10-node quadratic heat transfer tetrahedron 10-node quadratic coupled thermal-electrical tetrahedron 15-node quadratic heat transfer triangular prism 15-node quadratic coupled thermal-electrical triangular prism EI.1–13 DC1D2 DC1D2E DC1D3 DC1D3E DC2D3 DC2D3E DC2D4 DC2D4E DC2D6 DC2D6E DC2D8 DC2D8E DC3D4 DC3D4E DC3D6 DC3D6E DC3D8 DC3D8E DC3D10 DC3D10E DC3D15 DC3D20 20-node quadratic heat transfer brick DC3D20E 20-node quadratic coupled thermal-electrical brick DCAX3 3-node linear axisymmetric heat transfer triangle DCAX3E 3-node linear axisymmetric coupled thermal-electrical triangle DCAX4 4-node linear axisymmetric heat transfer quadrilateral DCAX4E 4-node linear axisymmetric coupled thermal-electrical quadrilateral DCAX6 6-node quadratic axisymmetric heat transfer triangle DCAX6E 6-node quadratic axisymmetric coupled thermal-electrical triangle DCAX8 DCAX8E DCC1D2 8-node quadratic axisymmetric heat transfer quadrilateral 8-node quadratic axisymmetric coupled thermal-electrical quadrilateral 2-node convection/diffusion link DCC1D2D 2-node convection/diffusion link, dispersion control DCC2D4 4-node convection/diffusion quadrilateral DCC2D4D 4-node convection/diffusion quadrilateral, dispersion control DCC3D8 8-node convection/diffusion brick DCC3D8D 8-node convection/diffusion brick, dispersion control DCCAX2 2-node axisymmetric convection/diffusion link DCCAX2D 2-node axisymmetric convection/diffusion link, dispersion control DCCAX4 4-node axisymmetric convection/diffusion quadrilateral DCCAX4D 4-node axisymmetric convection/diffusion quadrilateral, dispersion control DCOUP2D Two-dimensional distributing coupling element DCOUP3D Three-dimensional distributing coupling element DGAP DRAG2D DRAG3D DS3 DS4 DS6 DS8 Unidirectional thermal interactions between two nodes 2-D drag chain, for use in cases where only horizontal motion is being studied 3-D drag chain 3-node heat transfer triangular shell 4-node heat transfer quadrilateral shell 6-node heat transfer triangular shell 8-node heat transfer quadrilateral shell DSAX1 DSAX2 2-node axisymmetric heat transfer shell 3-node axisymmetric heat transfer shell ELBOW31 2-node pipe in space with deforming section, linear interpolation along the pipe ELBOW31B 2-node pipe in space with ovalization only, axial gradients of ovalization neglected 28.1.4 28.1.4 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.2 28.1.2 28.1.3 28.1.3 28.1.4 28.1.4 28.1.6 28.1.6 28.1.6 28.1.6 32.4.2 32.4.2 39.2.2 32.11.2 32.11.2 29.6.7 29.6.7 29.6.7 29.6.7 29.6.9 29.6.9 29.5.2 29.5.2 29.5.2 29.5.2 28.1.3 28.1.3 28.1.4 28.1.4 29.4.3 29.4.3 39.2.2 39.2.2 39.2.2 39.2.2 32.6.7 32.6.7 32.6.8 32.6.8 32.6.8 32.6.8 32.6.8 32.6.8 32.6.8 32.6.8 32.6.8 32.6.8 32.6.8 32.6.8 32.6.8 32.6.8 32.6.9 ELBOW31C ELBOW32 EMC2D3 EMC2D4 EMC3D4 EMC3D8 FRAME2D FRAME3D GAPCYL GAPSPHER GAPUNI GAPUNIT GK2D2 GK2D2N GK3D2 GK3D2N GK3D4L GK3D4LN GK3D6L GK3D6LN 2-node pipe in space with ovalization only, axial gradients of ovalization neglected. This is the same as element type ELBOW31B except that the odd numbered terms in the Fourier interpolation around the pipe, except the first term, are neglected. 3-node pipe in space with deforming section, quadratic interpolation along the pipe 3-node triangular zero-order electromagnetic element 4-node quadrilateral zero-order electromagnetic element 4-node tetrahedral zero-order electromagnetic element 8-node hexahedral zero-order electromagnetic element 2-node two-dimensional straight frame element 2-node three-dimensional straight frame element Cylindrical gap between two nodes Spherical gap between two nodes Unidirectional gap between two nodes Unidirectional gap and thermal interactions between two nodes 2-node two-dimensional gasket element 2-node two-dimensional gasket element with thickness-direction behavior only 2-node three-dimensional gasket element 2-node three-dimensional gasket element with thickness-direction behavior only 4-node three-dimensional line gasket element 4-node three-dimensional line gasket element with thickness-direction behavior only 6-node three-dimensional line gasket element 6-node three-dimensional line gasket element with thickness-direction behavior only 6-node three-dimensional gasket element 6-node three-dimensional gasket element with thickness-direction behavior only 8-node three-dimensional gasket element 8-node three-dimensional gasket element with thickness-direction behavior only 12-node three-dimensional gasket element GK3D6 GK3D6N GK3D8 GK3D8N GK3D12M GK3D12MN 12-node three-dimensional gasket element with thickness-direction behavior GK3D18 GK3D18N GKAX2 only 18-node three-dimensional gasket element 18-node three-dimensional gasket element with thickness-direction behavior only 2-node axisymmetric gasket element 2-node axisymmetric gasket element with thickness-direction behavior only 4-node axisymmetric gasket element 4-node axisymmetric gasket element with thickness-direction behavior only 6-node axisymmetric gasket element 6-node axisymmetric gasket element with thickness-direction behavior only 4-node plane strain gasket element 6-node plane strain gasket element 4-node plane stress gasket element 4-node two-dimensional gasket element with thickness-direction behavior only 6-node plane stress gasket element 6-node two-dimensional gasket element with thickness-direction behavior only Point heat capacitance Axisymmetric rigid surface element (for use with first-order axisymmetric elements) Axisymmetric rigid surface element (for use with second-order axisymmetric elements) 2-node axisymmetric slide line element (for use with first-order axisymmetric elements) 3-node axisymmetric slide line element (for use with second-order axisymmetric elements) Cylindrical geometry tube support interaction element Unidirectional tube support interaction element Tube-tube element for use with first-order, 2-D beam and pipe elements Tube-tube element for use with first-order, 3-D beam and pipe elements Two-dimensional elastic-plastic joint interaction element. These elements are available only for use in Abaqus/Aqua. Three-dimensional elastic-plastic joint interaction element. These elements are available only for use in Abaqus/Aqua. Three-dimensional joint interaction element 3-node second-order line spring for use on a symmetry plane 6-node general second-order line spring. This element can be used only with linear elastic material behavior. 3-node triangular membrane 4-node quadrilateral membrane 4-node quadrilateral membrane, reduced integration, hourglass control 6-node triangular membrane 8-node quadrilateral membrane 32.6.9 32.6.9 32.6.9 32.6.9 32.6.9 32.6.7 32.6.7 32.6.7 32.6.7 32.6.7 32.6.7 30.4.2 39.5.2 39.5.2 39.4.2 39.4.2 32.8.2 32.8.2 39.3.2 39.3.2 32.10.2 32.10.2 32.3.2 32.9.2 32.9.2 29.1.2 29.1.2 29.1.2 29.1.2 29.1.2 EI.1–16 GKAX2N GKAX4 GKAX4N GKAX6 GKAX6N GKPE4 GKPE6 GKPS4 GKPS4N GKPS6 GKPS6N HEATCAP IRS21A IRS22A ISL21A ISL22A ITSCYL ITSUNI ITT21 ITT31 JOINT2D JOINT3D JOINTC LS3S LS6 M3D3 M3D4 M3D4R M3D6 8-node quadrilateral membrane, reduced integration 9-node quadrilateral membrane 9-node quadrilateral membrane, reduced integration, hourglass control Point mass 2-node linear axisymmetric membrane 3-node quadratic axisymmetric membrane 6-node cylindrical membrane 9-node cylindrical membrane 2-node linear axisymmetric membrane, twist 3-node quadratic axisymmetric membrane, twist 2-node linear pipe in a plane 2-node linear pipe in a plane, hybrid formulation 3-node quadratic pipe in a plane 3-node quadratic pipe in a plane, hybrid formulation 2-node linear pipe in space 2-node linear pipe in space, hybrid formulation 3-node quadratic pipe in space 3-node quadratic pipe in space, hybrid formulation 4-node 2-D pipe-soil interaction element 6-node 2-D pipe-soil interaction element 4-node 3-D pipe-soil interaction element 6-node 3-D pipe-soil interaction element 29.1.2 29.1.2 29.1.2 30.1.2 29.1.4 29.1.4 29.1.3 29.1.3 29.1.4 29.1.4 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 29.3.8 32.12.2 32.12.2 32.12.2 32.12.2 4-node tetrahedron, temperature linear displacement, linear electric potential and linear 28.1.4 6-node linear triangular prism, linear displacement, linear electric potential and linear temperature 8-node brick, trilinear displacement, trilinear electric potential and trilinear temperature 28.1.4 28.1.4 trilinear displacement, 8-node brick, temperature, hybrid, constant pressure 8-node brick, temperature, reduced integration, hourglass control trilinear displacement, trilinear electric potential, trilinear electric potential, trilinear 28.1.4 trilinear 28.1.4 8-node brick, temperature, reduced integration, hourglass control, hybrid, constant pressure trilinear electric potential, trilinear displacement, trilinear 28.1.4 10-node modified displacement, electric potential, tetrahedron, hourglass control temperature quadratic 28.1.4 EI.1–17 M3D8R M3D9 M3D9R MASS MAX1 MAX2 MCL6 MCL9 MGAX1 MGAX2 PIPE21 PIPE21H PIPE22 PIPE22H PIPE31 PIPE31H PIPE32 PIPE32H PSI24 PSI26 PSI34 PSI36 Q3D4 Q3D6 Q3D8 Q3D8H Q3D8R Q3D8RH temperature quadratic 10-node modified displacement, electric potential, tetrahedron, hybrid, linear pressure, hourglass control 20-node quadratic brick, triquadratic displacement, trilinear electric potential, trilinear temperature 20-node quadratic brick, triquadratic displacement, trilinear electric potential, trilinear temperature, hybrid, linear pressure 20-node quadratic brick, triquadratic displacement, trilinear electric potential, trilinear temperature, reduced integration 20-node quadratic brick, triquadratic displacement, trilinear electric potential, trilinear temperature, hybrid, linear pressure, reduced integration 2-node 2-D linear rigid link (for use in plane strain or plane stress) 3-node 3-D rigid triangular facet 4-node 3-D bilinear rigid quadrilateral 2-node linear axisymmetric rigid link (for use in axisymmetric planar geometries) 2-node 2-D rigid beam 2-node 3-D rigid beam Rotary inertia at a point 3-node triangular general-purpose shell, finite membrane strains (identical to element S3R) 3-node thermally coupled triangular general-purpose shell, finite membrane strains (identical to element S3RT) 3-node triangular general-purpose shell, finite membrane strains (identical to element S3) 3-node thermally coupled triangular general-purpose shell, finite membrane strains (identical to element S3T) 4-node general-purpose shell, finite membrane strains 4-node thermally coupled general-purpose shell, finite membrane strains 4-node general-purpose shell, reduced integration, hourglass control, finite membrane strains 4-node thermally coupled general-purpose shell, reduced integration, hourglass control, finite membrane strains 4-node thin shell, reduced integration, hourglass control, using five degrees of freedom per node 8-node doubly curved thick shell, reduced integration 8-node doubly curved thin shell, reduced integration, using five degrees of freedom per node 8-node thermally coupled quadrilateral general displacement, bilinear temperature in the shell surface thick shell, biquadratic 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 30.3.2 30.3.2 30.3.2 30.3.2 30.3.2 30.3.2 30.2.2 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 EI.1–18 Q3D10MH Q3D20 Q3D20H Q3D20R Q3D20RH R2D2 R3D3 R3D4 RAX2 RB2D2 RB3D2 ROTARYI S3 S3T S3R S3RT S4 S4T S4R S4RT S4R5 S8R S8R5 reduced thick shell, quadratic in-plane general-purpose continuum shell, 9-node doubly curved thin shell, reduced integration, using five degrees of freedom per node 2-node linear axisymmetric thin or thick shell 3-node quadratic axisymmetric thin or thick shell 3-node axisymmetric thermally coupled thin or displacement, linear temperature in the shell surface Linear asymmetric-axisymmetric, Fourier shell element with 2 nodes in the generator direction and N Fourier modes Quadratic asymmetric-axisymmetric, Fourier shell element with 3 nodes in the generator direction and N Fourier modes 6-node triangular in-plane continuum shell wedge, general-purpose continuum shell, finite membrane strains. 8-node quadrilateral integration with hourglass control, finite membrane strains. 6-node linear displacement and temperature, triangular in-plane continuum shell wedge, general-purpose continuum shell, finite membrane strains. 8-node linear displacement and temperature, quadrilateral in-plane general- purpose continuum shell, reduced integration with hourglass control, finite membrane strains. 3-node triangular surface element 4-node quadrilateral surface element 4-node quadrilateral surface element, reduced integration 6-node triangular surface element 8-node quadrilateral surface element 8-node quadrilateral surface element, reduced integration 2-node linear axisymmetric surface element 3-node quadratic axisymmetric surface element 6-node cylindrical surface element 9-node cylindrical surface element 2-node linear axisymmetric surface element, twist 3-node quadratic axisymmetric surface element, twist Spring between a node and ground, acting in a fixed direction Spring between two nodes, acting in a fixed direction Axial spring between two nodes, whose line of action is the line joining the two nodes. This line of action may rotate in large-displacement analysis. 3-node triangular facet thin shell 6-node triangular thin shell, using five degrees of freedom per node 2-node linear 2-D truss 29.6.7 29.6.9 29.6.9 29.6.9 29.6.10 29.6.10 29.6.8 29.6.8 29.6.8 29.6.8 32.7.2 32.7.2 32.7.2 32.7.2 32.7.2 32.7.2 32.7.4 32.7.4 32.7.3 32.7.3 32.7.4 32.7.4 32.1.2 32.1.2 32.1.2 29.6.7 29.6.7 29.2.2 EI.1–19 S9R5 SAX1 SAX2 SAX2T SAXA1N SAXA2N SC6R SC8R SC6RT SC8RT SFM3D3 SFM3D4 SFM3D4R SFM3D6 SFM3D8 SFM3D8R SFMAX1 SFMAX2 SFMCL6 SFMCL9 SFMGAX1 SFMGAX2 SPRING1 SPRING2 SPRINGA STRI3 STRI65 T2D2E T2D2H T2D2T T2D3 T2D3E T2D3H T2D3T T3D2 T3D2E T3D2H T3D2T T3D3 T3D3E T3D3H T3D3T 2-node 2-D piezoelectric truss 2-node linear 2-D truss, hybrid 2-node 2-D thermally coupled truss 3-node quadratic 2-D truss 3-node 2-D piezoelectric truss 3-node quadratic 2-D truss, hybrid 3-node 2-D thermally coupled truss 2-node linear 3-D truss 2-node 3-D piezoelectric truss 2-node linear 3-D truss, hybrid 2-node 3-D thermally coupled truss 3-node quadratic 3-D truss 3-node 3-D piezoelectric truss 3-node quadratic 3-D truss, hybrid 3-node 3-D thermally coupled truss WARP2D3 3-node linear 2-D warping element WARP2D4 4-node bilinear 2-D warping element 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 29.2.2 28.4.2 28.4.2 EI.2 Abaqus/Explicit ELEMENT INDEX This index provides a reference to all of the element types that are available in Abaqus/Explicit. Elements are listed in alphabetical order, where numerical characters precede the letter “A” and two-digit numbers are put in numerical, rather than “alphabetical,” order. For example, C3D8R precedes CAX3. For certain options, such as contact and surface-based distributing coupling, Abaqus may generate internal elements (such as IDCOUP3D for surface-based distributing coupling). These internal element names are not included in the index below but may appear in an output database (.odb) or data (.dat) file. 3-node linear 2-D acoustic triangle 4-node linear 2-D acoustic quadrilateral, reduced integration, hourglass control 4-node linear acoustic tetrahedron 6-node linear acoustic triangular prism 8-node linear acoustic brick, reduced integration, hourglass control 3-node linear axisymmetric acoustic triangle 4-node linear axisymmetric acoustic quadrilateral, reduced integration, hourglass control 2-node linear 2-D acoustic infinite element 3-node linear 3-D acoustic infinite element 4-node linear 3-D acoustic infinite element 2-node linear axisymmetric acoustic infinite element 2-node linear beam in a plane 3-node quadratic beam in a plane 2-node linear beam in space 3-node quadratic beam in space 4-node linear tetrahedron 4-node thermally coupled tetrahedron, linear displacement and temperature 6-node linear triangular prism, reduced integration, hourglass control 6-node thermally coupled triangular prism, linear displacement and temperature, reduced integration, hourglass control 8-node linear brick 8-node linear brick, incompatible modes 8-node linear brick, reduced integration, hourglass control 8-node thermally coupled brick, trilinear displacement and temperature 8-node thermally coupled brick, trilinear displacement and temperature, reduced integration, hourglass control 28.1.3 28.1.3 28.1.4 28.1.4 28.1.4 28.1.6 28.1.6 28.3.2 28.3.2 28.3.2 28.3.2 29.3.8 29.3.8 29.3.8 29.3.8 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 28.1.4 EI.2–1 AC2D3 AC2D4R AC3D4 AC3D6 AC3D8R ACAX3 ACAX4R ACIN2D2 ACIN3D3 ACIN3D4 ACINAX2 B21 B22 B31 B32 C3D4 C3D4T C3D6 C3D6T C3D8 C3D8I C3D8R C3D8T linear displacement and reduced integration, hourglass 10-node modified second-order tetrahedron 10-node modified thermally coupled second-order tetrahedron 3-node linear axisymmetric triangle 3-node thermally coupled axisymmetric triangle, temperature 4-node bilinear axisymmetric quadrilateral, control 4-node thermally coupled axisymmetric quadrilateral, bilinear displacement and temperature, hybrid, constant pressure, reduced integration, hourglass control 6-node modified second-order axisymmetric triangle 6-node modified second-order axisymmetric thermally coupled triangle 8-node linear one-way infinite brick 4-node linear axisymmetric one-way infinite quadrilateral 4-node linear plane strain one-way infinite quadrilateral 4-node linear plane stress one-way infinite quadrilateral 4-node axisymmetric cohesive element 4-node two-dimensional cohesive element 6-node three-dimensional cohesive element 8-node three-dimensional cohesive element Connector element in a plane between two nodes or ground and a node Connector element in space between two nodes or ground and a node 3-node linear plane strain triangle 3-node plane strain thermally coupled triangle, temperature 4-node bilinear plane strain quadrilateral, reduced integration, hourglass control 4-node bilinear plane bilinear strain thermally coupled quadrilateral, displacement and temperature, reduced integration, hourglass control 6-node modified second-order plane strain triangle 6-node modified second-order plane strain thermally coupled triangle 3-node linear plane stress triangle 3-node plane stress thermally coupled triangle, temperature 4-node bilinear plane stress quadrilateral, reduced integration, hourglass control 4-node plane stress thermally coupled quadrilateral, bilinear displacement and temperature, reduced integration, hourglass control 6-node modified second-order plane stress triangle 6-node modified second-order plane stress thermally coupled triangle linear displacement and linear displacement and 28.1.4 28.1.4 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.1.6 28.3.2 28.3.2 28.3.2 28.3.2 32.5.10 32.5.8 32.5.9 32.5.9 31.1.4 31.1.4 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 28.1.3 EI.2–2 C3D10M C3D10MT CAX3 CAX3T CAX4R CAX4RT CAX6M CAX6MT CIN3D8 CINAX4 CINPE4 CINPS4 COHAX4 COH2D4 COH3D6 COH3D8 CONN2D2 CONN3D2 CPE3 CPE3T CPE4R CPE4RT CPE6M CPE6MT CPS3 CPS3T CPS4R CPS4RT CPS6M EC3D8R Abaqus/Explicit ELEMENT INDEX reduced 8-node linear multi-material Eulerian brick, reduced integration, hourglass control 8-node thermally coupled linear multi-material Eulerian brick, integration, hourglass control Point heat capacitance 3-node triangular membrane 4-node quadrilateral membrane 4-node quadrilateral membrane, reduced integration, hourglass control Point mass 1-node continuum particle element 2-node linear pipe in a plane 2-node linear pipe in space 2-node 2-D linear rigid link (for use in plane strain or plane stress) 3-node 3-D rigid triangular facet 4-node 3-D bilinear rigid quadrilateral 2-node linear axisymmetric rigid link (for use in axisymmetric geometries) Rotary inertia at a point 3-node triangular shell, finite membrane strains 3-node triangular shell, small membrane strains 3-node thermally-coupled triangular shell, finite membrane strains 4-node general-purpose shell, finite membrane strains 4-node shell, reduced integration, hourglass control, finite membrane strains 4-node shell, reduced integration, hourglass control, small membrane strains 4-node shell, reduced integration, hourglass control, small membrane strains, warping considered in small-strain formulation 4-node thermally-coupled shell, reduced integration, hourglass control, finite membrane strains 2-node linear axisymmetric shell 6-node triangular in-plane continuum shell wedge, general-purpose continuum shell, finite membrane strains. 8-node quadrilateral integration with hourglass control, finite membrane strains. 6-node thermally coupled triangular in-plane continuum shell wedge, general- purpose continuum shell, finite membrane strains. 8-node thermally coupled quadrilateral in-plane general-purpose continuum shell, reduced integration with hourglass control, finite membrane strains. in-plane general-purpose continuum shell, reduced 32.2.2 32.14.1 32.14.1 30.4.2 29.1.2 29.1.2 29.1.2 30.1.2 28.5.2 29.3.8 29.3.8 30.3.2 30.3.2 30.3.2 30.3.2 30.2.2 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.7 29.6.9 29.6.8 29.6.8 29.6.8 29.6.8 EI.2–3 EC3D8RT HEATCAP M3D3 M3D4 M3D4R MASS PC3D PIPE21 PIPE31 R2D2 R3D3 R3D4 RAX2 ROTARYI S3R S3RS S3RT S4 S4R S4RS S4RSW S4RT SAX1 SC6R SC8R SC6RT SFM3D3 3-node triangular surface element SFM3D4R 4-node quadrilateral surface element, reduced integration SPRINGA Axial spring between two nodes T2D2 T3D2 2-node linear 2-D truss 2-node linear 3-D truss 32.7.2 32.7.2 32.1.2 29.2.2 29.2.2 EI.3 Abaqus/CFD ELEMENT INDEX This index provides a reference to all of the element types that are available in Abaqus/CFD. Elements are listed in alphabetical order. FC3D4 FC3D6 FC3D8 4-node tetrahedron 6-node prism 8-node brick 28.2.2 28.2.2 28.2.2 SIMULIA is the Dassault Systèmes brand that delivers a scalable portfolio of Realistic Simulation solutions including the Abaqus product suite for Unified Finite Element Analysis; multiphysics solutions for insight into challenging engineering problems; and lifecycle management solutions for managing simulation data, processes, and intellectual property. By building on established technology, respected quality, and superior customer service, SIMULIA makes realistic simulation an integral business practice that improves product performance, reduces physical prototypes, and drives innovation. Headquartered in Providence, RI, USA, with R&D centers in Providence and in Vélizy, France, SIMULIA provides sales, services, and support through a global network of regional offices and distributors. For more information, visit www.simulia.com. About Dassault Systèmes As a world leader in 3D and Product Lifecycle Management (PLM) solutions, Dassault Systèmes brings value to more than 100,000 customers in 80 countries. A pioneer in the 3D software market since 1981, Dassault Systèmes develops and markets PLM application software and services that support industrial processes and provide a 3D vision of the entire lifecycle of products from conception to maintenance to recycling. The Dassault Systèmes portfolio consists of CATIA for designing the virtual product, SolidWorks for 3D mechanical design, DELMIA for virtual production, SIMULIA for virtual testing, ENOVIA for global collaborative lifecycle management, and 3DVIA for online 3D lifelike experiences. Dassault Systèmes’ shares are listed on Euronext Paris (#13065, DSY.PA), and Dassault Systèmes’ ADRs may be traded on the US Over-The-Counter (OTC) market (DASTY). For more information, visit www.3ds.com. fi , , , , , , , , . . , © . , , . /